Abaqus Example Problems Manual
Abaqus 6.12
Example Problems Manual
Volume I: Static and Dynamic Analyses
Abaqus Version 6.12 ID:
Printed on:
Abaqus
Example Problems Manual
Volume I
Abaqus Version 6.12 ID:
Printed on:
Legal Notices
CAUTION: This documentation is intended for qualified users who will exercise sound engineering judgment and expertise in the use of the Abaqus
Software. The Abaqus Software is inherently complex, and the examples and procedures in this documentation are not intended to be exhaustive or to apply
to any particular situation. Users are cautioned to satisfy themselves as to the accuracy and results of their analyses.
Dassault Systèmes and its subsidiaries, including Dassault Systèmes Simulia Corp., shall not be responsible for the accuracy or usefulness of any analysis
performed using the Abaqus Software or the procedures, examples, or explanations in this documentation. Dassault Systèmes and its subsidiaries shall not
be responsible for the consequences of any errors or omissions that may appear in this documentation.
The Abaqus Software is available only under license from Dassault Systèmes or its subsidiary and may be used or reproduced only in accordance with the
terms of such license. This documentation is subject to the terms and conditions of either the software license agreement signed by the parties, or, absent
such an agreement, the then current software license agreement to which the documentation relates.
This documentation and the software described in this documentation are subject to change without prior notice.
No part of this documentation may be reproduced or distributed in any form without prior written permission of Dassault Systèmes or its subsidiary.
The Abaqus Software is a product of Dassault Systèmes Simulia Corp., Providence, RI, USA.
© Dassault Systèmes, 2012
Abaqus, the 3DS logo, SIMULIA, CATIA, and Unified FEA are trademarks or registered trademarks of Dassault Systèmes or its subsidiaries in the United
States and/or other countries.
Other company, product, and service names may be trademarks or service marks of their respective owners. For additional information concerning
trademarks, copyrights, and licenses, see the Legal Notices in the Abaqus 6.12 Installation and Licensing Guide.
Abaqus Version 6.12 ID:
Printed on:
Locations
SIMULIA Worldwide Headquarters
SIMULIA European Headquarters
Rising Sun Mills, 166 Valley Street, Providence, RI 02909–2499, Tel: +1 401 276 4400,
Fax: +1 401 276 4408, simulia.support@3ds.com, http://www.simulia.com
Stationsplein 8-K, 6221 BT Maastricht, The Netherlands, Tel: +31 43 7999 084,
Fax: +31 43 7999 306, simulia.europe.info@3ds.com
Dassault Systèmes’ Centers of Simulation Excellence
United States
Australia
Austria
Benelux
Canada
China
Finland
France
Germany
India
Italy
Japan
Korea
Latin America
Scandinavia
United Kingdom
Fremont, CA, Tel: +1 510 794 5891, simulia.west.support@3ds.com
West Lafayette, IN, Tel: +1 765 497 1373, simulia.central.support@3ds.com
Northville, MI, Tel: +1 248 349 4669, simulia.greatlakes.info@3ds.com
Woodbury, MN, Tel: +1 612 424 9044, simulia.central.support@3ds.com
Mayfield Heights, OH, Tel: +1 216 378 1070, simulia.erie.info@3ds.com
Mason, OH, Tel: +1 513 275 1430, simulia.central.support@3ds.com
Warwick, RI, Tel: +1 401 739 3637, simulia.east.support@3ds.com
Lewisville, TX, Tel: +1 972 221 6500, simulia.south.info@3ds.com
Richmond VIC, Tel: +61 3 9421 2900, simulia.au.support@3ds.com
Vienna, Tel: +43 1 22 707 200, simulia.at.info@3ds.com
Maarssen, The Netherlands, Tel: +31 346 585 710, simulia.benelux.support@3ds.com
Toronto, ON, Tel: +1 416 402 2219, simulia.greatlakes.info@3ds.com
Beijing, P. R. China, Tel: +8610 6536 2288, simulia.cn.support@3ds.com
Shanghai, P. R. China, Tel: +8621 3856 8000, simulia.cn.support@3ds.com
Espoo, Tel: +358 40 902 2973, simulia.nordic.info@3ds.com
Velizy Villacoublay Cedex, Tel: +33 1 61 62 72 72, simulia.fr.support@3ds.com
Aachen, Tel: +49 241 474 01 0, simulia.de.info@3ds.com
Munich, Tel: +49 89 543 48 77 0, simulia.de.info@3ds.com
Chennai, Tamil Nadu, Tel: +91 44 43443000, simulia.in.info@3ds.com
Lainate MI, Tel: +39 02 3343061, simulia.ity.info@3ds.com
Tokyo, Tel: +81 3 5442 6302, simulia.jp.support@3ds.com
Osaka, Tel: +81 6 7730 2703, simulia.jp.support@3ds.com
Mapo-Gu, Seoul, Tel: +82 2 785 6707/8, simulia.kr.info@3ds.com
Puerto Madero, Buenos Aires, Tel: +54 11 4312 8700, Horacio.Burbridge@3ds.com
Stockholm, Sweden, Tel: +46 8 68430450, simulia.nordic.info@3ds.com
Warrington, Tel: +44 1925 830900, simulia.uk.info@3ds.com
Authorized Support Centers
Argentina
Brazil
Czech & Slovak Republics
Greece
Israel
Malaysia
Mexico
New Zealand
Poland
Russia, Belarus & Ukraine
Singapore
South Africa
Spain & Portugal
Abaqus Version 6.12 ID:
Printed on:
SMARTtech Sudamerica SRL, Buenos Aires, Tel: +54 11 4717 2717
KB Engineering, Buenos Aires, Tel: +54 11 4326 7542
Solaer Ingeniería, Buenos Aires, Tel: +54 221 489 1738
SMARTtech Mecânica, Sao Paulo-SP, Tel: +55 11 3168 3388
Synerma s. r. o., Psáry, Prague-West, Tel: +420 603 145 769, abaqus@synerma.cz
3 Dimensional Data Systems, Crete, Tel: +30 2821040012, support@3dds.gr
ADCOM, Givataim, Tel: +972 3 7325311, shmulik.keidar@adcomsim.co.il
WorleyParsons Services Sdn. Bhd., Kuala Lumpur, Tel: +603 2039 9000, abaqus.my@worleyparsons.com
Kimeca.NET SA de CV, Mexico, Tel: +52 55 2459 2635
Matrix Applied Computing Ltd., Auckland, Tel: +64 9 623 1223, abaqus-tech@matrix.co.nz
BudSoft Sp. z o.o., Poznań, Tel: +48 61 8508 466, info@budsoft.com.pl
TESIS Ltd., Moscow, Tel: +7 495 612 44 22, info@tesis.com.ru
WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com
Finite Element Analysis Services (Pty) Ltd., Parklands, Tel: +27 21 556 6462, feas@feas.co.za
Principia Ingenieros Consultores, S.A., Madrid, Tel: +34 91 209 1482, simulia@principia.es
Taiwan
Thailand
Turkey
Simutech Solution Corporation, Taipei, R.O.C., Tel: +886 2 2507 9550, camilla@simutech.com.tw
WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com
A-Ztech Ltd., Istanbul, Tel: +90 216 361 8850, info@a-ztech.com.tr
Complete contact information is available at http://www.simulia.com/locations/locations.html.
Abaqus Version 6.12 ID:
Printed on:
Preface
This section lists various resources that are available for help with using Abaqus Unified FEA software.
Support
Both technical engineering support (for problems with creating a model or performing an analysis) and
systems support (for installation, licensing, and hardware-related problems) for Abaqus are offered through
a network of local support offices. Regional contact information is listed in the front of each Abaqus manual
and is accessible from the Locations page at www.simulia.com.
Support for SIMULIA products
SIMULIA provides a knowledge database of answers and solutions to questions that we have answered,
as well as guidelines on how to use Abaqus, SIMULIA Scenario Definition, Isight, and other SIMULIA
products. You can also submit new requests for support. All support incidents are tracked. If you contact
us by means outside the system to discuss an existing support problem and you know the incident or support
request number, please mention it so that we can query the database to see what the latest action has been.
Many questions about Abaqus can also be answered by visiting the Products page and the Support
page at www.simulia.com.
Anonymous ftp site
To facilitate data transfer with SIMULIA, an anonymous ftp account is available at ftp.simulia.com.
Login as user anonymous, and type your e-mail address as your password. Contact support before placing
files on the site.
Training
All offices and representatives offer regularly scheduled public training classes. The courses are offered in
a traditional classroom form and via the Web. We also provide training seminars at customer sites. All
training classes and seminars include workshops to provide as much practical experience with Abaqus as
possible. For a schedule and descriptions of available classes, see www.simulia.com or call your local office
or representative.
Feedback
We welcome any suggestions for improvements to Abaqus software, the support program, or documentation.
We will ensure that any enhancement requests you make are considered for future releases. If you wish to
make a suggestion about the service or products, refer to www.simulia.com. Complaints should be made by
contacting your local office or through www.simulia.com by visiting the Quality Assurance section of the
Support page.
Abaqus Version 6.12 ID:
Printed on:
CONTENTS
Contents
Volume I
1.
Static Stress/Displacement Analyses
Static and quasi-static stress analyses
Axisymmetric analysis of bolted pipe flange connections
Elastic-plastic collapse of a thin-walled elbow under in-plane bending and internal
pressure
Parametric study of a linear elastic pipeline under in-plane bending
Indentation of an elastomeric foam specimen with a hemispherical punch
Collapse of a concrete slab
Jointed rock slope stability
Notched beam under cyclic loading
Uniaxial ratchetting under tension and compression
Hydrostatic fluid elements: modeling an airspring
Shell-to-solid submodeling and shell-to-solid coupling of a pipe joint
Stress-free element reactivation
Transient loading of a viscoelastic bushing
Indentation of a thick plate
Damage and failure of a laminated composite plate
Analysis of an automotive boot seal
Pressure penetration analysis of an air duct kiss seal
Self-contact in rubber/foam components: jounce bumper
Self-contact in rubber/foam components: rubber gasket
Submodeling of a stacked sheet metal assembly
Axisymmetric analysis of a threaded connection
Direct cyclic analysis of a cylinder head under cyclic thermal-mechanical loadings
Erosion of material (sand production) in an oil wellbore
Submodel stress analysis of pressure vessel closure hardware
Using a composite layup to model a yacht hull
1.1.1
1.1.2
1.1.3
1.1.4
1.1.5
1.1.6
1.1.7
1.1.8
1.1.9
1.1.10
1.1.11
1.1.12
1.1.13
1.1.14
1.1.15
1.1.16
1.1.17
1.1.18
1.1.19
1.1.20
1.1.21
1.1.22
1.1.23
1.1.24
Buckling and collapse analyses
Snap-through buckling analysis of circular arches
Laminated composite shells: buckling of a cylindrical panel with a circular hole
Buckling of a column with spot welds
Elastic-plastic K-frame structure
Unstable static problem: reinforced plate under compressive loads
Buckling of an imperfection-sensitive cylindrical shell
i
Abaqus ID:exa-toc
Printed on: Fri February 3 -- 17:59:59 2012
1.2.1
1.2.2
1.2.3
1.2.4
1.2.5
1.2.6
CONTENTS
Forming analyses
Upsetting of a cylindrical billet: quasi-static analysis with mesh-to-mesh solution
mapping (Abaqus/Standard) and adaptive meshing (Abaqus/Explicit)
Superplastic forming of a rectangular box
Stretching of a thin sheet with a hemispherical punch
Deep drawing of a cylindrical cup
Extrusion of a cylindrical metal bar with frictional heat generation
Rolling of thick plates
Axisymmetric forming of a circular cup
Cup/trough forming
Forging with sinusoidal dies
Forging with multiple complex dies
Flat rolling: transient and steady-state
Section rolling
Ring rolling
Axisymmetric extrusion: transient and steady-state
Two-step forming simulation
Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic
analysis
Unstable static problem: thermal forming of a metal sheet
Inertia welding simulation using Abaqus/Standard and Abaqus/CAE
1.3.1
1.3.2
1.3.3
1.3.4
1.3.5
1.3.6
1.3.7
1.3.8
1.3.9
1.3.10
1.3.11
1.3.12
1.3.13
1.3.14
1.3.15
1.3.16
1.3.17
1.3.18
Fracture and damage
A plate with a part-through crack: elastic line spring modeling
Contour integrals for a conical crack in a linear elastic infinite half space
Elastic-plastic line spring modeling of a finite length cylinder with a part-through axial
flaw
Crack growth in a three-point bend specimen
Analysis of skin-stiffener debonding under tension
Failure of blunt notched fiber metal laminates
Debonding behavior of a double cantilever beam
Debonding behavior of a single leg bending specimen
Postbuckling and growth of delaminations in composite panels
1.4.1
1.4.2
1.4.3
1.4.4
1.4.5
1.4.6
1.4.7
1.4.8
1.4.9
Import analyses
Springback of two-dimensional draw bending
Deep drawing of a square box
2.
1.5.1
1.5.2
Dynamic Stress/Displacement Analyses
Dynamic stress analyses
Nonlinear dynamic analysis of a structure with local inelastic collapse
Detroit Edison pipe whip experiment
ii
Abaqus ID:exa-toc
Printed on: Fri February 3 -- 17:59:59 2012
2.1.1
2.1.2
CONTENTS
Rigid projectile impacting eroding plate
Eroding projectile impacting eroding plate
Tennis racket and ball
Pressurized fuel tank with variable shell thickness
Modeling of an automobile suspension
Explosive pipe closure
Knee bolster impact with general contact
Crimp forming with general contact
Collapse of a stack of blocks with general contact
Cask drop with foam impact limiter
Oblique impact of a copper rod
Water sloshing in a baffled tank
Seismic analysis of a concrete gravity dam
Progressive failure analysis of thin-wall aluminum extrusion under quasi-static and
dynamic loads
Impact analysis of a pawl-ratchet device
High-velocity impact of a ceramic target
2.1.3
2.1.4
2.1.5
2.1.6
2.1.7
2.1.8
2.1.9
2.1.10
2.1.11
2.1.12
2.1.13
2.1.14
2.1.15
2.1.16
2.1.17
2.1.18
Mode-based dynamic analyses
Analysis of a rotating fan using substructures and cyclic symmetry
Linear analysis of the Indian Point reactor feedwater line
Response spectra of a three-dimensional frame building
Brake squeal analysis
Dynamic analysis of antenna structure utilizing residual modes
Steady-state dynamic analysis of a vehicle body-in-white model
2.2.1
2.2.2
2.2.3
2.2.4
2.2.5
2.2.6
Eulerian analyses
Rivet forming
Impact of a water-filled bottle
2.3.1
2.3.2
Co-simulation analyses
Dynamic impact of a scooter with a bump
2.4.1
iii
Abaqus ID:exa-toc
Printed on: Fri February 3 -- 17:59:59 2012
CONTENTS
Volume II
3.
Tire and Vehicle Analyses
Tire analyses
Symmetric results transfer for a static tire analysis
Steady-state rolling analysis of a tire
Subspace-based steady-state dynamic tire analysis
Steady-state dynamic analysis of a tire substructure
Coupled acoustic-structural analysis of a tire filled with air
Import of a steady-state rolling tire
Analysis of a solid disc with Mullins effect and permanent set
Tread wear simulation using adaptive meshing in Abaqus/Standard
Dynamic analysis of an air-filled tire with rolling transport effects
Acoustics in a circular duct with flow
3.1.1
3.1.2
3.1.3
3.1.4
3.1.5
3.1.6
3.1.7
3.1.8
3.1.9
3.1.10
Vehicle analyses
Inertia relief in a pick-up truck
Substructure analysis of a pick-up truck model
Display body analysis of a pick-up truck model
Continuum modeling of automotive spot welds
3.2.1
3.2.2
3.2.3
3.2.4
Occupant safety analyses
Seat belt analysis of a simplified crash dummy
Side curtain airbag impactor test
4.
Mechanism Analyses
Resolving overconstraints in a multi-body mechanism model
Crank mechanism
Snubber-arm mechanism
Flap mechanism
Tail-skid mechanism
Cylinder-cam mechanism
Driveshaft mechanism
Geneva mechanism
Trailing edge flap mechanism
Substructure analysis of a one-piston engine model
Application of bushing connectors in the analysis of a three-point linkage
Gear assemblies
5.
3.3.1
3.3.2
4.1.1
4.1.2
4.1.3
4.1.4
4.1.5
4.1.6
4.1.7
4.1.8
4.1.9
4.1.10
4.1.11
4.1.12
Heat Transfer and Thermal-Stress Analyses
Thermal-stress analysis of a disc brake
5.1.1
iv
Abaqus ID:exa-toc
Printed on: Fri February 3 -- 17:59:59 2012
CONTENTS
A sequentially coupled thermal-mechanical analysis of a disc brake with an Eulerian
approach
Exhaust manifold assemblage
Coolant manifold cover gasketed joint
Conductive, convective, and radiative heat transfer in an exhaust manifold
Thermal-stress analysis of a reactor pressure vessel bolted closure
6.
Fluid Dynamics and Fluid-Structure Interaction
Conjugate heat transfer analysis of a component-mounted electronic circuit board
7.
5.1.2
5.1.3
5.1.4
5.1.5
5.1.6
6.1.1
Electromagnetic Analyses
Piezoelectric analyses
Eigenvalue analysis of a piezoelectric transducer
Transient dynamic nonlinear response of a piezoelectric transducer
7.1.1
7.1.2
Joule heating analyses
Thermal-electrical modeling of an automotive fuse
8.
Mass Diffusion Analyses
Hydrogen diffusion in a vessel wall section
Diffusion toward an elastic crack tip
9.
8.1.1
8.1.2
Acoustic and Shock Analyses
Fully and sequentially coupled acoustic-structural analysis of a muffler
Coupled acoustic-structural analysis of a speaker
Response of a submerged cylinder to an underwater explosion shock wave
Convergence studies for shock analyses using shell elements
UNDEX analysis of a detailed submarine model
Coupled acoustic-structural analysis of a pick-up truck
Long-duration response of a submerged cylinder to an underwater explosion
Deformation of a sandwich plate under CONWEP blast loading
10.
7.2.1
9.1.1
9.1.2
9.1.3
9.1.4
9.1.5
9.1.6
9.1.7
9.1.8
Soils Analyses
Plane strain consolidation
Calculation of phreatic surface in an earth dam
Axisymmetric simulation of an oil well
Analysis of a pipeline buried in soil
Hydraulically induced fracture in a well bore
Permafrost thawing–pipeline interaction
v
Abaqus ID:exa-toc
Printed on: Fri February 3 -- 17:59:59 2012
10.1.1
10.1.2
10.1.3
10.1.4
10.1.5
10.1.6
CONTENTS
11.
Structural Optimization Analyses
Topology optimization analyses
Shape optimization analyses
12.
Abaqus/Aqua Analyses
Jack-up foundation analyses
Riser dynamics
13.
12.1.1
12.1.2
Design Sensitivity Analyses
Overview
Design sensitivity analysis: overview
13.1.1
Examples
Design sensitivity analysis of a composite centrifuge
Design sensitivities for tire inflation, footprint, and natural frequency analysis
Design sensitivity analysis of a windshield wiper
Design sensitivity analysis of a rubber bushing
14.
13.2.1
13.2.2
13.2.3
13.2.4
Postprocessing of Abaqus Results Files
User postprocessing of Abaqus results files: overview
Joining data from multiple results files and converting file format: FJOIN
Calculation of principal stresses and strains and their directions: FPRIN
vi
Abaqus ID:exa-toc
Printed on: Fri February 3 -- 17:59:59 2012
14.1.1
14.1.2
14.1.3
CONTENTS
Creation of a perturbed mesh from original coordinate data and eigenvectors: FPERT
Output radiation viewfactors and facet areas: FRAD
Creation of a data file to facilitate the postprocessing of elbow element results:
FELBOW
vii
Abaqus ID:exa-toc
Printed on: Fri February 3 -- 17:59:59 2012
14.1.4
14.1.5
14.1.6
Abaqus Version 6.12 ID:
Printed on:
INTRODUCTION
1.0
INTRODUCTION
This is the Example Problems Manual for Abaqus. It contains many solved examples that illustrate the use of
the program for common types of problems. Some of the problems are quite difficult and require combinations
of the capabilities in the code.
The problems have been chosen to serve two purposes: to verify the capabilities in Abaqus by exercising
the code on nontrivial cases and to provide guidance to users who must work on a class of problems with which
they are relatively unfamiliar. In each worked example the discussion in the manual states why the example
is included and leads the reader through the standard approach to an analysis: element and mesh selection,
material model, and a discussion of the results. Many of these problems are worked with different element
types, mesh densities, and other variations.
Input data files for all of the analyses are included with the Abaqus release in compressed archive
files. The abaqus fetch utility is used to extract these input files for use. For example, to fetch input file
boltpipeflange_3d_cyclsym.inp, type
abaqus fetch job=boltpipeflange_3d_cyclsym.inp
Parametric study script (.psf) and user subroutine (.f) files can be fetched in the same manner. All files for
a particular problem can be obtained by leaving off the file extension. The abaqus fetch utility is explained
in detail in “Fetching sample input files,” Section 3.2.14 of the Abaqus Analysis User’s Manual.
It is sometimes useful to search the input files. The findkeyword utility is used to locate input files
that contain user-specified input. This utility is defined in “Querying the keyword/problem database,”
Section 3.2.13 of the Abaqus Analysis User’s Manual.
To reproduce the graphical representation of the solution reported in some of the examples, the output
frequency used in the input files may need to be increased. For example, in “Linear analysis of the Indian
Point reactor feedwater line,” Section 2.2.2, the figures that appear in the manual can be obtained only if the
solution is written to the results file every increment; that is, if the input files are changed to read
*NODE FILE, ..., FREQUENCY=1
instead of FREQUENCY=100 as appears now.
In addition to the Example Problems Manual, there are two other manuals that contain worked
problems. The Abaqus Benchmarks Manual contains benchmark problems (including the NAFEMS suite
of test problems) and standard analyses used to evaluate the performance of Abaqus. The tests in this
manual are multiple element tests of simple geometries or simplified versions of real problems. The Abaqus
Verification Manual contains a large number of examples that are intended as elementary verification of the
basic modeling capabilities.
The qualification process for new Abaqus releases includes running and verifying results for all problems
in the Abaqus Example Problems Manual, the Abaqus Benchmarks Manual, and the Abaqus Verification
Manual.
1.0–1
Abaqus Version 6.12 ID:
Printed on:
STATIC STRESS/DISPLACEMENT ANALYSES
1.
Static Stress/Displacement Analyses
•
•
•
•
•
“Static and quasi-static stress analyses,” Section 1.1
“Buckling and collapse analyses,” Section 1.2
“Forming analyses,” Section 1.3
“Fracture and damage,” Section 1.4
“Import analyses,” Section 1.5
Abaqus Version 6.12 ID:
Printed on:
STATIC AND QUASI-STATIC STRESS ANALYSES
1.1
Static and quasi-static stress analyses
•
•
“Axisymmetric analysis of bolted pipe flange connections,” Section 1.1.1
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
“Parametric study of a linear elastic pipeline under in-plane bending,” Section 1.1.3
“Elastic-plastic collapse of a thin-walled elbow under in-plane bending and internal pressure,”
Section 1.1.2
“Indentation of an elastomeric foam specimen with a hemispherical punch,” Section 1.1.4
“Collapse of a concrete slab,” Section 1.1.5
“Jointed rock slope stability,” Section 1.1.6
“Notched beam under cyclic loading,” Section 1.1.7
“Uniaxial ratchetting under tension and compression,” Section 1.1.8
“Hydrostatic fluid elements: modeling an airspring,” Section 1.1.9
“Shell-to-solid submodeling and shell-to-solid coupling of a pipe joint,” Section 1.1.10
“Stress-free element reactivation,” Section 1.1.11
“Transient loading of a viscoelastic bushing,” Section 1.1.12
“Indentation of a thick plate,” Section 1.1.13
“Damage and failure of a laminated composite plate,” Section 1.1.14
“Analysis of an automotive boot seal,” Section 1.1.15
“Pressure penetration analysis of an air duct kiss seal,” Section 1.1.16
“Self-contact in rubber/foam components: jounce bumper,” Section 1.1.17
“Self-contact in rubber/foam components: rubber gasket,” Section 1.1.18
“Submodeling of a stacked sheet metal assembly,” Section 1.1.19
“Axisymmetric analysis of a threaded connection,” Section 1.1.20
“Direct cyclic analysis of a cylinder head under cyclic thermal-mechanical loadings,” Section 1.1.21
“Erosion of material (sand production) in an oil wellbore,” Section 1.1.22
“Submodel stress analysis of pressure vessel closure hardware,” Section 1.1.23
“Using a composite layup to model a yacht hull,” Section 1.1.24
1.1–1
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
1.1.1
AXISYMMETRIC ANALYSIS OF BOLTED PIPE FLANGE CONNECTIONS
Product: Abaqus/Standard
A bolted pipe flange connection is a common and important part of many piping systems. Such connections
are typically composed of hubs of pipes, pipe flanges with bolt holes, sets of bolts and nuts, and a gasket.
These components interact with each other in the tightening process and when operation loads such as internal
pressure and temperature are applied. Experimental and numerical studies on different types of interaction
among these components are frequently reported. The studies include analysis of the bolt-up procedure
that yields uniform bolt stress (Bibel and Ezell, 1992), contact analysis of screw threads (Fukuoka, 1992;
Chaaban and Muzzo, 1991), and full stress analysis of the entire pipe joint assembly (Sawa et al., 1991). To
establish an optimal design, a full stress analysis determines factors such as the contact stresses that govern
the sealing performance, the relationship between bolt force and internal pressure, the effective gasket seating
width, and the bending moment produced in the bolts. This example shows how to perform such a design
analysis by using an economical axisymmetric model and how to assess the accuracy of the axisymmetric
solution by comparing the results to those obtained from a simulation using a three-dimensional segment
model. In addition, several three-dimensional models that use multiple levels of substructures are analyzed
to demonstrate the use of substructures with a large number of retained degrees of freedom. Finally, a
three-dimensional model containing stiffness matrices is analyzed to demonstrate the use of the matrix input
functionality.
Geometry and model
The bolted joint assembly being analyzed is depicted in Figure 1.1.1–1. The geometry and dimensions
of the various parts are taken from Sawa et al. (1991), modified slightly to simplify the modeling. The
inner wall radius of both the hub and the gasket is 25 mm. The outer wall radii of the pipe flange and the
gasket are 82.5 mm and 52.5 mm, respectively. The thickness of the gasket is 2.5 mm. The pipe flange
has eight bolt holes that are equally spaced in the pitch circle of radius 65 mm. The radius of the bolt
hole is modified in this analysis to be the same as that of the bolt: 8 mm. The bolt head (bearing surface)
is assumed to be circular, and its radius is 12 mm.
The Young’s modulus is 206 GPa and the Poisson’s ratio is 0.3 for both the bolt and the pipe
hub/flange. The gasket is modeled with either solid continuum or gasket elements. When continuum
elements are used, the gasket’s Young’s modulus, E, equals 68.7 GPa and its Poisson’s ratio, , equals
0.3.
When gasket elements are used, a linear gasket pressure/closure relationship is used with the
effective “normal stiffness,”
, equal to the material Young’s modulus divided by the thickness so
that
27.48 GPa/mm. Similarly a linear shear stress/shear motion relationship is used with an
effective shear stiffness, , equal to the material shear modulus divided by the thickness so that
10.57 GPa/mm. The membrane behavior is specified with a Young’s modulus of 68.7 GPa and a
Poisson’s ratio of 0.3. Sticking contact conditions are assumed in all contact areas: between the bearing
surface and the flange and between the gasket and the hub. Contact between the bolt shank and the bolt
hole is ignored.
1.1.1–1
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
The finite element idealizations of the symmetric half of the pipe joint are shown in Figure 1.1.1–2
and Figure 1.1.1–3, corresponding to the axisymmetric and three-dimensional analyses, respectively.
The mesh used for the axisymmetric analysis consists of a mesh for the pipe hub/flange and gasket and a
separate mesh for the bolts. In Figure 1.1.1–2 the top figure shows the mesh of the pipe hub and flange,
with the bolt hole area shown in a lighter shade; and the bottom figure shows the overall mesh with the
gasket and the bolt in place.
For the axisymmetric model second-order elements with reduced integration, CAX8R, are used
throughout the mesh of the pipe hub/flange. The gasket is modeled with either CAX8R solid continuum
elements or GKAX6 gasket elements. Contact between the gasket and the pipe hub/flange is modeled
with contact pairs between surfaces defined on the faces of elements in the contact region or between such
element-based surfaces and node-based surfaces. In an axisymmetric analysis the bolts and the perforated
flange must be modeled properly. The bolts are modeled as plane stress elements since they do not carry
hoop stress. Second-order plane stress elements with reduced integration, CPS8R, are employed for this
purpose. The contact surface definitions, which are associated with the faces of the elements, account
for the plane stress condition automatically. To account for all eight bolts used in the joint, the combined
cross-sectional areas of the shank and the head of the bolts must be calculated and redistributed to the
bolt mesh appropriately using the area attributes for the solid elements. The contact area is adjusted
automatically.
Figure 1.1.1–4 illustrates the cross-sectional views of the bolt head and the shank. Each plane stress
element represents a volume that extends out of the x–y plane. For example, element A represents a
volume calculated as ( ) × (
). Likewise, element B represents a volume calculated as (
)×
(
). The sectional area in the x–z plane pertaining to a given element can be calculated as
where R is the bolt head radius,
, or the shank radius,
(depending on the element
location), and
and
are x-coordinates of the left and right side of the given element, respectively.
If the sectional areas are divided by the respective element widths,
and
, we obtain
representative element thicknesses. Multiplying each element thickness by eight (the number of bolts
in the model) produces the thickness values that are found in the solid section definition.
Sectional areas that are associated with bolt head elements located on the model’s contact surfaces
are used to calculate the surface areas of the nodes used in defining the node-based surfaces of the model.
Referring again to Figure 1.1.1–4, nodal contact areas for a single bolt are calculated as follows:
1.1.1–2
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
where
through
are contact areas that are associated with contact nodes 1–9 and
through
are
sectional areas that are associated with bolt head elements C–F. Multiplying the above areas by eight (the
number of bolts in the model) provides the nodal contact areas found in the contact property definitions.
A common way of handling the presence of the bolt holes in the pipe flange in axisymmetric
analyses is to smear the material properties used in the bolt hole area of the mesh and to use
inhomogeneous material properties that correspond to a weaker material in this region. General
guidelines for determining the effective material properties for perforated flat plates are found in
ASME Section VIII Div 2 Article 4–9. For the type of structure under study, which is not a flat
plate, a common approach to determining the effective material properties is to calculate the elasticity
moduli reduction factor, which is the ratio of the ligament area in the pitch circle to the annular area
of the pitch circle. In this model the annular area of the pitch circle is given by
6534.51 mm2 ,
2
and the total area of the bolt holes is given by
1608.5 mm . Hence, the reduction
factor is simply
0.754. The effective in-plane moduli of elasticity,
and
,
are obtained by multiplying the respective moduli,
and
, by this factor. We assume material
isotropy in the r–z plane; thus,
The modulus in the hoop direction,
, should
be very small and is chosen such that
106 . The in-plane shear modulus is then calculated
based on the effective elasticity modulus:
The shear moduli in the hoop
direction are also calculated similarly but with set to zero (they are not used in an axisymmetric
model). Hence, we have
155292 MPa,
0.155292 MPa,
59728 MPa,
and
0.07765 MPa. These orthotropic elasticity moduli are specified using engineering
constants for the bolt hole part of the mesh.
The mesh for the three-dimensional analysis without substructures, shown in Figure 1.1.1–3,
represents a 22.5° segment of the pipe joint and employs second-order brick elements with reduced
integration, C3D20R, for the pipe hub/flange and bolts. The gasket is modeled with C3D20R elements
or GK3D18 elements. The top figure shows the mesh of the pipe hub and flange, and the bottom
figure shows both the gasket and bolt (in the lighter color). Contact is modeled by the interaction of
contact surfaces defined by grouping specific faces of the elements in the contacting regions. For
three-dimensional contact where both the master and slave surfaces are deformable, the small-sliding
contact pair formulation must be used to indicate that small relative sliding occurs between contacting
surfaces. No special adjustments need be made for the material properties used in the three-dimensional
model because all parts are modeled appropriately.
Four different meshes that use substructures to model the flange are tested. A first-level substructure
is created for the entire 22.5° segment of the flange shown in Figure 1.1.1–3, while the gasket and the bolt
are meshed as before. The nodes on the flange in contact with the bolt cap form a node-based surface,
while the nodes on the flange in contact with the gasket form another node-based surface. These nodebased surfaces will form contact pairs with the master surfaces on the bolt cap and on the gasket, which
are defined using the surface definition options. The retained degrees of freedom on the substructure
include all three degrees of freedom for the nodes in these node-based surfaces as well as for the nodes
on the 0° and 22.5° faces of the flange. Appropriate boundary conditions are specified at the substructure
usage level.
A second-level substructure of 45° is created by reflecting the first-level substructure with respect
to the 22.5° plane. The nodes on the 22.5° face belonging to the reflected substructure are constrained
1.1.1–3
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
in all three degrees of freedom to the corresponding nodes on the 22.5° face belonging to the original
first-level substructure. The half-bolt and the gasket sector corresponding to the reflected substructure
are also constructed by reflection. The retained degrees of freedom include all three degrees of freedom
of all contact node sets and of the nodes on the 0° and 45° faces of the flange. MPC-type CYCLSYM is
used to impose cyclic symmetric boundary conditions on these two faces.
A third-level substructure of 90° is created by reflecting the original 45° second-level substructure
with respect to the 45° plane and by connecting it to the original 45° substructure. The remaining part
of the gasket and the bolts corresponding to the 45°–90° sector of the model is created by reflection and
appropriate constraints. In this case it is not necessary to retain any degrees of freedom on the 0° and
90° faces of the flange because this 90° substructure will not be connected to other substructures and
appropriate boundary conditions can be specified at the substructure creation level.
The final substructure model is set up by mirroring the 90° mesh with respect to the symmetry
plane of the gasket perpendicular to the y-axis. Thus, an otherwise large analysis ( 750,000 unknowns)
when no substructures are used can be solved conveniently ( 80,000 unknowns) by using the third-level
substructure twice. The sparse solver is used because it significantly reduces the run time for this model.
Finally, a three-dimensional matrix-based model is created by replacing elements for the entire 22.5°
segment of the flange shown in Figure 1.1.1–3 with stiffness matrices, while the gasket and the bolt
are meshed as before. Contact between the flange and gasket and the flange and bolt cap is modeled
using node-based slave surfaces just as for the substructure models. Appropriate boundary conditions
are applied as in the three-dimensional model without substructures.
Loading and boundary conditions
The only boundary conditions are symmetry boundary conditions. In the axisymmetric model
0
is applied to the symmetry plane of the gasket and to the bottom of the bolts. In the three-dimensional
model
0 is applied to the symmetry plane of the gasket as well as to the bottom of the bolt. The
0° and
22.5° planes are also symmetry planes. On the
22.5° plane, symmetry boundary
conditions are enforced by invoking suitable nodal transformations and applying boundary conditions to
local directions in this symmetry plane. These transformations are implemented using a local coordinate
system definition. On both the symmetry planes, the symmetry boundary conditions
0 are imposed
everywhere except for the dependent nodes associated with the C BIQUAD MPC and nodes on one side
of the contact surface. The second exception is made to avoid overconstraining problems, which arise if
there is a boundary condition in the same direction as a Lagrange multiplier constraint associated with
the rough friction specification.
In the models where substructures are used, the boundary conditions are specified depending on
what substructure is used. For the first-level 22.5° substructure the boundary conditions and constraint
equations are the same as for the three-dimensional model shown in Figure 1.1.1–3. For the 45° secondlevel substructure the symmetry boundary conditions are enforced on the
45° plane with the constraint
equation
0. A transform could have been used as well. For the 90° third-level substructure
the face
90° is constrained with the boundary condition
0.
For the three-dimensional model containing matrices, nodal transformations are applied for
symmetric boundary conditions. Entries in the stiffness matrices for these nodes are also in local
coordinates.
1.1.1–4
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
A clamping force of 15 kN is applied to each bolt by associating the pre-tension node with a pretension section. The pre-tension section is identified by means of a surface definition. The pre-tension
is then prescribed by applying a concentrated load to the pre-tension node. In the axisymmetric analysis
the actual load applied is 120 kN since there are eight bolts. In the three-dimensional model with no
substructures the actual load applied is 7.5 kN since only half of a bolt is modeled. In the models using
substructures all half-bolts are loaded with a 7.5 kN force. For all of the models the pre-tension section
is specified about halfway down the bolt shank.
Sticking contact conditions are assumed in all surface interactions in all analyses and are simulated
with rough friction and no-separation contact.
Results and discussion
All analyses are performed as small-displacement analyses.
Figure 1.1.1–5 shows a top view of the normal stress distributions in the gasket at the
interface between the gasket and the pipe hub/flange predicted by the axisymmetric (bottom) and
three-dimensional (top) analyses when solid continuum elements are used to model the gasket. The
figure shows that the compressive normal stress is highest at the outer edge of the gasket, decreases
radially inward, and changes from compression to tension at a radius of about 35 mm, which is consistent
with findings reported by Sawa et al. (1991). The close agreement in the overall solution between
axisymmetric and three-dimensional analyses is quite apparent, indicating that, for such problems,
axisymmetric analysis offers a simple yet reasonably accurate alternative to three-dimensional analysis.
Figure 1.1.1–6 shows a top view of the normal stress distributions in the gasket at the
interface between the gasket and the pipe hub/flange predicted by the axisymmetric (bottom) and
three-dimensional (top) analyses when gasket elements are used to model the gasket. Close agreement
in the overall solution between the axisymmetric and three-dimensional analyses is also seen in this case.
The gasket starts carrying compressive load at a radius of about 40 mm, a difference of 5 mm with the
previous result. This difference is the result of the gasket elements being unable to carry tensile loads in
their thickness direction. This solution is physically more realistic since, in most cases, gaskets separate
from their neighboring parts when subjected to tensile loading. Removing the no-separation contact
from the gasket/flange contact surface definition in the input files that model the gasket with continuum
elements yields good agreement with the results obtained in Figure 1.1.1–6 (since, in that case, the solid
continuum elements in the gasket cannot carry tensile loading in the gasket thickness direction).
The models in this example can be modified to study other factors, such as the effective seating width
of the gasket or the sealing performance of the gasket under operating loads. The gasket elements offer
the advantage of allowing very complex behavior to be defined in the gasket thickness direction. Gasket
elements can also use any of the small-strain material models provided in Abaqus including user-defined
material models. Figure 1.1.1–7 shows a comparison of the normal stress distributions in the gasket at
the interface between the gasket and the pipe hub/flange predicted by the axisymmetric (bottom) and
three-dimensional (top) analyses when isotropic material properties are prescribed for gasket elements.
The results in Figure 1.1.1–7 compare well with the results in Figure 1.1.1–5 from analyses in which
solid and axisymmetric elements are used to simulate the gasket.
Figure 1.1.1–8 shows the distribution of the normal stresses in the gasket at the interface in the plane
0. The results are plotted for the three-dimensional model containing only solid continuum elements
1.1.1–5
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
and no substructures, for the three-dimensional model with matrices, and for the four models containing
the substructures described above.
An execution procedure is available to combine model and results data from two substructure
output databases into a single output database. For more information, see “Combining output from
substructures,” Section 3.2.19 of the Abaqus Analysis User’s Manual.
This example can also be used to demonstrate the effectiveness of the quasi-Newton nonlinear
solver. This solver utilizes an inexpensive, approximate stiffness matrix update for several consecutive
equilibrium iterations, rather than a complete stiffness matrix factorization each iteration as used in the
default full Newton method. The quasi-Newton method results in an increased number of less expensive
iterations, and a net savings in computing cost.
Input files
boltpipeflange_axi_solidgask.inp
boltpipeflange_axi_node.inp
boltpipeflange_axi_element.inp
boltpipeflange_3d_solidgask.inp
boltpipeflange_axi_gkax6.inp
boltpipeflange_3d_gk3d18.inp
boltpipeflange_3d_substr1.inp
boltpipeflange_3d_substr2.inp
boltpipeflange_3d_substr3_1.inp
boltpipeflange_3d_substr3_2.inp
boltpipeflange_3d_gen1.inp
boltpipeflange_3d_gen2.inp
boltpipeflange_3d_gen3.inp
Axisymmetric analysis containing a gasket modeled with
solid continuum elements.
Node definitions for boltpipeflange_axi_solidgask.inp
and boltpipeflange_axi_gkax6.inp.
Element definitions for
boltpipeflange_axi_solidgask.inp.
Three-dimensional analysis containing a gasket modeled
with solid continuum elements.
Axisymmetric analysis containing a gasket modeled with
gasket elements.
Three-dimensional analysis containing a gasket modeled
with gasket elements.
Three-dimensional analysis using the first-level
substructure (22.5° model).
Three-dimensional analysis using the second-level
substructure (45° model).
Three-dimensional analysis using the third-level
substructure once (90° model).
Three-dimensional analysis using the third-level
substructure twice (90° mirrored model).
First-level substructure generation data referenced by
boltpipeflange_3d_substr1.inp and
boltpipeflange_3d_gen2.inp.
Second-level substructure generation data referenced by
boltpipeflange_3d_substr2.inp and
boltpipeflange_3d_gen3.inp.
Third-level substructure generation data referenced by
boltpipeflange_3d_substr3_1.inp and
boltpipeflange_3d_substr3_2.inp.
1.1.1–6
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
boltpipeflange_3d_node.inp
boltpipeflange_3d_cyclsym.inp
boltpipeflange_3d_missnode.inp
boltpipeflange_3d_isomat.inp
boltpipeflange_3d_ortho.inp
boltpipeflange_axi_isomat.inp
boltpipeflange_3d_usr_umat.inp
boltpipeflange_3d_usr_umat.f
boltpipeflange_3d_solidnum.inp
boltpipeflange_3d_matrix.inp
boltpipeflange_3d_stiffPID4.inp
boltpipeflange_3d_stiffPID5.inp
boltpipeflange_3d_qn.inp
Nodal coordinates used in
boltpipeflange_3d_substr1.inp,
boltpipeflange_3d_substr2.inp,
boltpipeflange_3d_substr3_1.inp,
boltpipeflange_3d_substr3_2.inp,
boltpipeflange_3d_cyclsym.inp,
boltpipeflange_3d_gen1.inp,
boltpipeflange_3d_gen2.inp, and
boltpipeflange_3d_gen3.inp.
Same as file boltpipeflange_3d_substr2.inp except that
CYCLSYM type MPCs are used.
Same as file boltpipeflange_3d_gk3d18.inp except that
the option to generate missing nodes is used for gasket
elements.
Same as file boltpipeflange_3d_gk3d18.inp except that
gasket elements are modeled as isotropic using the
*MATERIAL option.
Same as file boltpipeflange_3d_gk3d18.inp except that
gasket elements are modeled as orthotropic and the
*ORIENTATION option is used.
Same as file boltpipeflange_axi_gkax6.inp except that
gasket elements are modeled as isotropic using the
*MATERIAL option.
Same as file boltpipeflange_3d_gk3d18.inp except that
gasket elements are modeled as isotropic with user
subroutine UMAT.
User subroutine UMAT used in
boltpipeflange_3d_usr_umat.inp.
Same as file boltpipeflange_3d_gk3d18.inp except that
solid element numbering is used for gasket elements.
Three-dimensional analysis containing matrices and a
gasket modeled with solid continuum elements.
Matrix representing stiffness of a part of the flange
segment for three-dimensional analysis containing
matrices.
Matrix representing stiffness of the remaining part of the
flange segment for three-dimensional analysis containing
matrices.
Same as file boltpipeflange_3d_gk3d18.inp except that
the quasi-Newton nonlinear solver is used.
1.1.1–7
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
References
•
Bibel, G. D., and R. M. Ezell, “An Improved Flange Bolt-Up Procedure Using Experimentally
Determined Elastic Interaction Coefficients,” Journal of Pressure Vessel Technology, vol. 114,
pp. 439–443, 1992.
•
Chaaban, A., and U. Muzzo, “Finite Element Analysis of Residual Stresses in Threaded End
Closures,” Transactions of ASME, vol. 113, pp. 398–401, 1991.
•
Fukuoka, T., “Finite Element Simulation of Tightening Process of Bolted Joint with a Tensioner,”
Journal of Pressure Vessel Technology, vol. 114, pp. 433–438, 1992.
•
Sawa, T., N. Higurashi, and H. Akagawa, “A Stress Analysis of Pipe Flange Connections,” Journal
of Pressure Vessel Technology, vol. 113, pp. 497–503, 1991.
1.1.1–8
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
Top View
π
θ= 4
centerline
Side View
15
47
r=8
20
26
d = 50
d = 105
d = 130
d = 165
2.5
Gasket
d = 50
d = 105
Bolt
24
16
10
Figure 1.1.1–1
80
Schematic of the bolted joint. All dimensions in mm.
1.1.1–9
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
2
3
1
2
3
1
Figure 1.1.1–2
Axisymmetric model of the bolted joint.
1.1.1–10
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
2
1
3
2
3
Figure 1.1.1–3
1
22.5° segment three-dimensional model of the bolted joint.
1.1.1–11
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
TOP VIEW
area B
area A
Rbolthead
Rshank
x
y
WB
WA
z
C
D
E
F
12 3 4 5 6 7 8 9
contact nodes
HA
element A
FRONT VIEW
HB
element B
Figure 1.1.1–4
Cross-sectional views of the bolt head and the shank.
1.1.1–12
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
S22
VALUE
1
2
3
4
5
6
7
8
9
10
11
12
-1.00E+02
-8.90E+01
-7.81E+01
-6.72E+01
-5.63E+01
-4.54E+01
-3.45E+01
-2.36E+01
-1.27E+01
-1.81E+00
+9.09E+00
+2.00E+01
6
5
4
6
7
5
4
3
8
9
10
1
1
2 2
1
3
8
3
9
10
11
4
5
6
7
2
5
7
9
10
11
1
23
1
6
8
1212
11
12
10
4
7
8
11
12
12
3
22
3
5
6
9
10
11
12
7
8
9
11
2
3
4
5
2
6
10
12
2
8
9
11
7
4
3
1
3
S22
VALUE
1
2
3
4
5
6
7
8
9
10
11
12
-1.00E+02
-8.90E+01
-7.81E+01
-6.72E+01
-5.63E+01
-4.54E+01
-3.45E+01
-2.36E+01
-1.27E+01
-1.81E+00
+9.09E+00
+2.00E+01
5
6
7
5
6
7
4
3
8
9
10
6
7
5
2
4
2
3
8
10
11
9
11
5
4
9
12
6
7
8
10
12
6
7
8
10
5
3
4
2
9
11
12
10
11
12
12
12
7
8
9
5
6
10
11
11
10
11
10
12
5
2
3
4
3
4
2
32
9
8
7
6
9
8
7
2
4 3
6 5
9
8
12
11
2
2
4 3
1
3
Figure 1.1.1–5 Normal stress distribution in the gasket contact surface when solid elements are
used to model the gasket: three-dimensional versus axisymmetric results.
1.1.1–13
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
S11
VALUE
1
-2.00E+01
2
-9.09E+00
3
+1.82E+00
4
+1.27E+01
5
+2.36E+01
6
+3.45E+01
7
+4.55E+01
8
+5.64E+01
9
+6.73E+01
10
+7.82E+01
11
+8.91E+01
12
+1.00E+02
7
4
3
3
3
3
3
3
3
77 8
6
4
3
5
5
6
6
10
9
7 8 10
7
5
6
89
3
2
8
11
11
10
910
11
11
10
5
910
78
4
4
6 7
11
10
5
11
9
4
4
6 77 8
5
4
11
10
9 11
89
6 78
7
5
4
5
10
1
3
S11
VALUE
1
-2.00E+01
2
-9.09E+00
3
+1.82E+00
4
+1.27E+01
5
+2.36E+01
6
+3.45E+01
7
+4.55E+01
8
+5.64E+01
9
+6.73E+01
10
+7.82E+01
11
+8.91E+01
12
91011
6
7 8 910
11
4
6
5
7 8 91011
4
5
3
+1.00E+02
6
4
3
5
7 8 910
11
6
4
3
5
3
3
5
5
3
4
3
4
5
4
5
3
2
4
7 8 9 10
11
6
4
6
7 89
10
11
6
7 8
9 10
11
6
7 8
9 10
11
7 8
1
3
Figure 1.1.1–6 Normal stress distribution in the gasket contact surface when gasket elements are used
with direct specification of the gasket behavior: three-dimensional versus axisymmetric results.
1.1.1–14
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
S11
VALUE
1
-1.00E+02
2
-8.91E+01
3
-7.82E+01
4
-6.73E+01
5
-5.64E+01
6
-4.55E+01
7
-3.45E+01
8
-2.36E+01
9
-1.27E+01
10
-1.82E+00
11
+9.09E+00
12
+2.00E+01
8
9
10
10
8
8
7
8
8
10
10
2
3 2
4 3
2
3 2
4 3
6 55
6
2
3
4 3 2
6 55
6
7
99
10
10
11
11
5
6 5
6
7
8
8
99
2
4 3
5
6 5
6
7
9
9
2
3
2
4
5 4 3
5
2
12
12
10
10
11
12
12
11
12
12
8
8
9
9
12
12
6
7
6
2
10
10
3
4
4 3
5
5
11
12
12
9
9
12
12
2
12
1
8
8
11
10
10
11
10
6
7
6
8
8
9
9
7
6
5
3
4
4 3
3
S11
VALUE
1
-1.00E+02
2
-8.91E+01
3
-7.82E+01
4
-6.73E+01
5
-5.64E+01
6
-4.55E+01
7
-3.45E+01
8
-2.36E+01
9
-1.27E+01
10
-1.82E+00
11
+9.09E+00
12
+2.00E+01
88
4 3 2
8
10
7
10
4 3 2
6
8
5
9
7
5
9
7
10
11
4 3 2
6
8
11
12
5
9
11
12
4 3 2
6
8
9
12
11
5
10
7
12
12
10
9
5
7
11
12
10
12
11
12
11
12
12
11
4 3
2
6
8
11
1
5
6
7
99
10
2
2
44 33 2
5
6
6
7
9
6
8
10
9
8
10
10
9
8
5
7
6
7
6
5
5
4 3
2
4 3
2
4 3 2
3
Figure 1.1.1–7 Normal stress distribution in the gasket contact surface when gasket elements are
used with isotropic material properties: three-dimensional versus axisymmetric results.
1.1.1–15
Abaqus Version 6.12 ID:
Printed on:
BOLTED PIPE JOINT
22.5_matrix
22.5_no_sup
22.5_sup
45_sup
90_sup
90r_sup
Figure 1.1.1–8
Normal stress distribution in the gasket contact surface along the line
0 for the models with and without substructures.
1.1.1–16
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
1.1.2
ELASTIC-PLASTIC COLLAPSE OF A THIN-WALLED ELBOW UNDER IN-PLANE
BENDING AND INTERNAL PRESSURE
Product: Abaqus/Standard
Elbows are used in piping systems because they ovalize more readily than straight pipes and, thus, provide
flexibility in response to thermal expansion and other loadings that impose significant displacements on the
system. Ovalization is the bending of the pipe wall into an oval—i.e., noncircular—configuration. The elbow
is, thus, behaving as a shell rather than as a beam. Straight pipe runs do not ovalize easily, so they behave
essentially as beams. Thus, even under pure bending, complex interaction occurs between an elbow and the
adjacent straight pipe segments; the elbow causes some ovalization in the straight pipe runs, which in turn
tend to stiffen the elbow. This interaction can create significant axial gradients of bending strain in the elbow,
especially in cases where the elbow is very flexible. This example provides verification of shell and elbow
element modeling of such effects, through an analysis of a test elbow for which experimental results have
been reported by Sobel and Newman (1979). An analysis is also included with elements of type ELBOW31B
(which includes ovalization but neglects axial gradients of strain) for the elbow itself and beam elements for
the straight pipe segments. This provides a comparative solution in which the interaction between the elbow
and the adjacent straight pipes is neglected. The analyses predict the response up to quite large rotations across
the elbow, so as to investigate possible collapse of the pipe and, particularly, the effect of internal pressure on
that collapse.
Geometry and model
The elbow configuration used in the study is shown in Figure 1.1.2–1. It is a thin-walled elbow with
elbow factor
and radius ratio
3.07, so the flexibility factor from Dodge and Moore (1972) is 10.3. (The
flexibility factor for an elbow is the ratio of the bending flexibility of an elbow segment to that of a
straight pipe of the same dimensions, for small displacements and elastic response.) This is an extremely
flexible case because the pipe wall is so thin.
To demonstrate convergence of the overall moment-rotation behavior with respect to meshing, the
two shell element meshes shown in Figure 1.1.2–2 are analyzed. Since the loading concerns in-plane
bending only, it is assumed that the response is symmetric about the midplane of the system so that in
the shell element model only one-half of the system need be modeled. Element type S8R5 is used, since
tests have shown this to be the most cost-effective shell element in Abaqus (input files using element
types S9R5, STRI65, and S8R for this example are included with the Abaqus release). The elbow
element meshes replace each axial division in the coarser shell element model with one ELBOW32
or two ELBOW31 elements and use 4 or 6 Fourier modes to model the deformation around the pipe.
Seven integration points are used through the pipe wall in all the analyses. This is usually adequate to
1.1.2–1
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
provide accurate modeling of the progress of yielding through the section in such cases as these, where
essentially monotonic straining is expected.
The ends of the system are rigidly attached to stiff plates in the experiments. These boundary
conditions are easily modeled for the ELBOW elements and for the fixed end in the shell element model.
For the rotating end of the shell element model the shell nodes must be constrained to a beam node that
represents the motion of the end plate using a kinematic coupling constraint as described below.
The material is assumed to be isotropic and elastic-plastic, following the measured response of type
304 stainless steel at room temperature, as reported by Sobel and Newman (1979). Since all the analyses
give results that are stiffer than the experimentally measured response, and the mesh convergence tests
(results are discussed below) demonstrate that the meshes are convergent with respect to the overall
response of the system, it seems that this stress-strain model may overestimate the material’s actual
strength.
Loading
The load on the pipe has two components: a “dead” load, consisting of internal pressure (with a closed
end condition), and a “live” in-plane bending moment applied to the end of the system. The pressure
is applied to the model in an initial step and then held constant in the second analysis step while the
bending moment is increased. The pressure values range from 0.0 to 3.45 MPa (500 lb/in2 ), which is the
range of interest for design purposes. The equivalent end force associated with the closed-end condition
is applied as a follower force because it rotates with the motion of the end plane.
Kinematic boundary conditions
The fixed end of the system is assumed to be fully built-in. The loaded end is fixed into a very stiff plate.
For the ELBOW element models this condition is represented by the NODEFORM boundary condition
applied at this node. In the shell element model this rigid plate is represented by a single node, and the
shell nodes at the end of the pipe are attached to it by using a kinematic coupling constraint and specifying
that all degrees of freedom at the shell nodes are constrained to the motion of the single node.
Results and discussion
The moment-rotation responses predicted by the various analysis models and measured in the experiment,
all taken at zero internal pressure, are compared in Figure 1.1.2–3. The figure shows that the two shell
models give very similar results, overestimating the experimentally measured collapse moment by about
15%. The 6-mode ELBOW element models are somewhat stiffer than the shell models, and those with
4 Fourier modes are much too stiff. This clearly shows that, for this very flexible system, the ovalization
of the elbow is too localized for even the 6-mode ELBOW representation to provide accurate results.
Since we know that the shell models are convergent with respect to discretization, the most likely
explanation for the excessive stiffness in comparison to the experimentally measured response is that
the material model used in the analyses is too strong. Sobel and Newman (1979) point out that the
stress-strain curve measured and used in this analysis, shown in Figure 1.1.2–1, has a 0.2% offset
yield that is 20% higher than the Nuclear Systems Materials Handbook value for type 304 stainless
steel at room temperature, which suggests the possibility that the billets used for the stress-strain curve
1.1.2–2
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
measurement may have been taken from stronger parts of the fabrication. If this is the case, it points
out the likelihood that the elbow tested is rather nonuniform in strength properties in spite of the care
taken in its manufacture. We are left with the conclusion that discrepancies of this magnitude cannot be
eliminated in practical cases, and the design use of such analysis results must allow for them.
Figure 1.1.2–4 compares the moment-rotation response for opening and closing moments under
0 and 3.45 MPa (500 lb/in2 ) internal pressure and shows the strong influence of large-displacement
effects. If large-displacement effects were not important, the opening and closing moments would
produce the same response. However, even with a 1° relative rotation across the elbow assembly, the
opening and closing moments differ by about 12%; with a 2° relative rotation, the difference is about
17%. Such magnitudes of relative rotation would not normally be considered large; in this case it is the
coupling into ovalization that makes geometric nonlinearity significant. As the rotation increases, the
cases with closing moment loading show collapse, while the opening moment curves do not. In both
cases internal pressure shows a strong effect on the results, which is to be expected in such a thin-walled
pipeline. The level of interaction between the straight pipe and the elbows is well illustrated by the strain
distribution on the outside wall, shown in Figure 1.1.2–5. The strain contours are slightly discontinuous
at the ends of the curved elbow section because the shell thickness changes at those sections.
Figure 1.1.2–6 shows a summary of the results from this example and “Uniform collapse of straight
and curved pipe segments,” Section 1.1.5 of the Abaqus Benchmarks Manual. The plot shows the
collapse value of the closing moment under in-plane bending as a function of internal pressure. The
strong influence of pressure on collapse is apparent. In addition, the effect of analyzing the elbow
by neglecting interaction between the straight and curved segments is shown: the “uniform bending”
results are obtained by using elements of type ELBOW31B in the bend and beams (element type B31)
for the straight segments. The importance of the straight/elbow interaction is apparent. In this case the
simpler analysis neglecting the interaction is conservative (in that it gives consistently lower values for
the collapse moment), but this conservatism cannot be taken for granted. The analysis of Sobel and
Newman (1979) also neglects interaction and agrees quite well with the results obtained here.
For comparison the small-displacement limit analysis results of Goodall (1978), as well as his largedisplacement, elastic-plastic lower bound (Goodall, 1978a), are also shown in this figure. Again, the
importance of large-displacement effects is apparent from that comparison.
Detailed results obtained with the model that uses ELBOW31 elements are shown in Figure 1.1.2–7
through Figure 1.1.2–9. Figure 1.1.2–7 shows the variation of the Mises stress along the length of the
piping system. The length is measured along the centerline of the pipe starting at the loaded end. The
figure compares the stress distribution at the intrados (integration point 1) on the inner and outer surfaces
of the elements (section points 1 and 7, respectively). Figure 1.1.2–8 shows the variation of the Mises
stress around the circumference of two elements (451 and 751) that are located in the bend section of
the model; the results are for the inner surface of the elements (section point 1). Figure 1.1.2–9 shows
the ovalization of elements 451 and 751. A nonovalized, circular cross-section is included in the figure
for comparison. From the figure it is seen that element 751, located at the center of the bend section,
experiences the most severe ovalization. These three figures were produced with the aid of the elbow
element postprocessing program felbow.f (“Creation of a data file to facilitate the postprocessing of
elbow element results: FELBOW,” Section 14.1.6), written in FORTRAN. The postprocessing programs
felbow.C (“A C++ version of FELBOW,” Section 10.15.6 of the Abaqus Scripting User’s Manual)
1.1.2–3
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
and felbow.py (“An Abaqus Scripting Interface version of FELBOW,” Section 9.10.12 of the Abaqus
Scripting User’s Manual), written in C++ and Python, respectively, are also available for generating the
data for figures such as Figure 1.1.2–8 and Figure 1.1.2–9. The user must ensure that the output variables
are written to the output database to use these two programs.
Shell-to-solid submodeling
One particular case is analyzed using the shell-to-solid submodeling technique. This problem verifies the
interpolation scheme in the case of double curved surfaces. A solid submodel using C3D27R elements is
created around the elbow part of the pipe, spanning an angle of 40°. The finer submodel mesh has three
elements through the thickness, 10 elements around half of the circumference of the cylinder, and 10
elements along the length of the elbow. Both ends are driven from the global shell model made of S8R
elements. The time scale of the static submodel analysis corresponds to the arc length in the global Riks
analysis. The submodel results agree closely with the shell model. The total force and the total moment
in a cross-section through the submodel are written to the results (.fil) file.
Shell-to-solid coupling
A model using the shell-to-solid coupling capability in Abaqus is included. Such a model can be used
for a careful study of the stress and strain fields in the elbow. The entire elbow is meshed with C3D20R
elements, and the straight pipe sections are meshed with S8R elements (see Figure 1.1.2–10). At each
shell-to-solid interface illustrated in Figure 1.1.2–10, an element-based surface is defined on the edge
of the solid mesh and an edge-based surface is defined on the edge of the shell mesh. A shell-to-solid
coupling constraint is used in conjunction with these surfaces to couple the shell and solid meshes.
Edge-based surfaces are defined at the end of each pipe segment. These surfaces are coupled to
reference nodes that are defined at the center of the pipes using a distributing coupling constraint. The
loading and fixed boundary conditions are applied to the reference points. The advantage of using this
method is that the pipe cross-sectional areas are free to deform; thus, ovalization at the ends is not
constrained. The moment-rotation response of the shell-to-solid coupling model agrees very well with
the results shown in Figure 1.1.2–4.
Input files
In all the following input files (with the exception of elbowcollapse_elbow31b_b31.inp,
elbowcollapse_s8r5_fine.inp, and elbowcolpse_shl2sld_s8r_c3d20r.inp) the step concerning the
application of the pressure load is commented out. To include the effects of the internal pressure in any
given analysis, uncomment the step definition in the appropriate input file.
elbowcollapse_elbow31b_b31.inp
elbowcollapse_elbow31_6four.inp
elbowcollapse_elbow32_6four.inp
elbowcollapse_s8r.inp
elbowcollapse_s8r5.inp
elbowcollapse_s8r5_fine.inp
ELBOW31B and B31 element model.
ELBOW31 model with 6 Fourier modes.
ELBOW32 model with 6 Fourier modes.
S8R element model.
S8R5 element model.
Finer S8R5 element model.
1.1.2–4
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
elbowcollapse_s9r5.inp
elbowcollapse_stri65.inp
elbowcollapse_submod.inp
elbowcolpse_shl2sld_s8r_c3d20r.inp
S9R5 element model.
STRI65 element model.
Submodel using C3D27R elements.
Shell-to-solid coupling model using S8R and C3D20R
elements.
References
•
Dodge, W. G., and S. E. Moore, “Stress Indices and Flexibility Factors for Moment Loadings on
Elbows and Curved Pipes,” Welding Research Council Bulletin, no. 179, 1972.
•
Goodall, I. W., “Lower Bound Limit Analysis of Curved Tubes Loaded by Combined Internal
Pressure and In-Plane Bending Moment,” Research Division Report RD/B/N4360, Central
Electricity Generating Board, England, 1978.
•
Goodall, I. W., “Large Deformations in Plastically Deforming Curved Tubes Subjected to In-Plane
Bending,” Research Division Report RD/B/N4312, Central Electricity Generating Board, England,
1978a.
•
Sobel, L. H., and S. Z. Newman, “Elastic-Plastic In-Plane Bending and Buckling of an Elbow:
Comparison of Experimental and Simplified Analysis Results,” Westinghouse Advanced Reactors
Division, Report WARD–HT–94000–2, 1979.
1.1.2–5
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
407 mm
(16.02 in)
1.83 m
(72.0 in)
10.4 mm (0.41 in)
thickness
Moment applied here
610 mm
(24.0 in)
70
60
400
Stress, MPa
300
Young's modulus:
193 GPa
(28 x 106 lb/in2 )
Poisson's ratio:
0.2642
40
30
200
20
100
10
0
0
0
Figure 1.1.2–1
1
2
3
Strain, %
4
5
MLTF elbow: geometry and measured material response.
1.1.2–6
Abaqus Version 6.12 ID:
Printed on:
Stress, 103 lb/in2
50
ELASTIC-PLASTIC COLLAPSE
Figure 1.1.2–2
Models for elbow/pipe interaction study.
1.1.2–7
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
Line variable
9
200
1 Experiment
2 S8R5
3 S8R5-finer mesh
4 ELBOW32 - 6 mode
5 ELBOW32 - 4 mode
6 ELBOW31 - 6 mode
7 ELBOW31 - 4 mode
8 ELBOW31 - Coarse 6
9 ELBOW31 - Coarse 4
10 ELBOW31B - 6 mode
11 ELBOW31B - 4 mode
6 8
Moment, kN-m
13.0
11
2
3
4
150
1
10
1.0
100
50
0
0.04
Figure 1.1.2–3
2.0
5,7
Moment, 106 lb-in
End rotation, deg
4.0
7.0
10.0
1.0
0.08 0.12 0.16
End rotation, rad
0.20
0
0.24
Moment-rotation response: mesh convergence studies.
ELBOW31closing/0
ELBOW31closing/500
ELBOW31opening/0
ELBOW31opening/500
S8R5closing/0
S8R5closing/500
S8R5opening/0
S8R5opening/500
6
[x10 ]
4.0
3.5
Moment, lb-in
3.0
2.5
2.0
1.5
1.0
0.5
0.0
0.00
0.04
0.08
0.12
0.16
0.20
0.24
End Rotation, rad
Figure 1.1.2–4
Moment-rotation response: pressure dependence.
1.1.2–8
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
E22
VALUE
-1.56E-02
-1.35E-02
-1.14E-02
-9.40E-03
-7.33E-03
-5.26E-03
-3.19E-03
-1.12E-03
+9.47E-04
+3.01E-03
+5.08E-03
+7.15E-03
+9.22E-03
+1.12E-02
E11
Hoop strain
VALUE
-1.36E-02
-1.02E-02
-6.82E-03
-3.43E-03
-4.61E-05
+3.34E-03
+6.73E-03
+1.01E-02
+1.35E-02
+1.69E-02
+2.02E-02
+2.36E-02
+2.70E-02
+3.04E-02
Axial strain
Figure 1.1.2–5
Strain distribution on the outside surface: closing moment case.
1.1.2–9
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
Internal pressure, lb/in2
0
250
500
750
1000
275
2.4
Goodall (1978a), large
displacement
31
W
O
elastic-plastic
B
EL R5
lower bound
S8
225
2.2
2.0
1.8
200
Goodall(1978), small–
displacement limit analysis
175
1.6
1.4
150
ELBOW31B
125
Sobel and Newman (1979),
uniform bending analysis
Collapse moment, 106 lb-in
Collapse moment, kN-m
250
1.2
1.0
1
2
3
4
5
6
Internal pressure, MPa
Figure 1.1.2–6
In-plane bending of an elbow, elastic-plastic collapse moment results.
50.
[ x10 3 ]
Mises stress, psi
MISES_I
MISES_O
40.
30.
20.
XMIN
XMAX
YMIN
YMAX
1.500E+00
1.322E+02
4.451E+03
5.123E+04
10.
0.
50.
100.
Length along pipe, in
Figure 1.1.2–7
Mises stress distribution along the length of the piping system.
1.1.2–10
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC COLLAPSE
60.
[ x10 3 ]
MISES451
MISES751
55.
Mises stress, psi
50.
45.
40.
35.
XMIN
XMAX
YMIN
YMAX
30.
0.000E+00
4.892E+01
2.635E+04
5.778E+04
25.
0.
5.
10.
15.
20.
25.
30.
35.
40.
45.
50.
Length around element circumference, in
Figure 1.1.2–8
Mises stress distribution around the circumference of elements 451 and 751.
10.
CIRCLE
OVAL_451
OVAL_751
Local y-axis
5.
0.
-5.
XMIN -7.805E+00
XMAX 7.805E+00
YMIN -8.732E+00
YMAX 8.733E+00
-10.
-10.
-5.
0.
5.
Local x-axis
Figure 1.1.2–9
Ovalization of elements 451 and 751.
1.1.2–11
Abaqus Version 6.12 ID:
Printed on:
10.
ELASTIC-PLASTIC COLLAPSE
solid elements
shell elements
shell-to-solid
interface
3
1
2
Figure 1.1.2–10
Shell-to-solid coupling model study.
1.1.2–12
Abaqus Version 6.12 ID:
Printed on:
LINEAR ELASTIC PIPELINE
1.1.3
PARAMETRIC STUDY OF A LINEAR ELASTIC PIPELINE UNDER IN-PLANE
BENDING
Products: Abaqus/Standard
Abaqus/Explicit
Elbows are used in piping systems because they ovalize more readily than straight pipes and, thus, provide
flexibility in response to thermal expansion and other loadings that impose significant displacements on the
system. Ovalization is the bending of the pipe wall into an oval—i.e., noncircular—configuration. The elbow
is, thus, behaving as a shell rather than as a beam. This example demonstrates the ability of elbow elements
(“Pipes and pipebends with deforming cross-sections: elbow elements,” Section 29.5.1 of the Abaqus
Analysis User’s Manual) to model the nonlinear response of initially circular pipes and pipebends accurately
when the distortion of the cross-section by ovalization is significant. It also provides some guidelines on
the importance of including a sufficient number of Fourier modes in the elbow elements to capture the
ovalization accurately. In addition, this example illustrates the shortcomings of using “flexibility knockdown
factors” with simple beam elements in an attempt to capture the effects of ovalization in an ad hoc manner
for large-displacement analyses. Similar analyses involving pipe elements in Abaqus/Explicit are included.
Geometry and model
The pipeline configuration used in the study is shown in Figure 1.1.3–1. It is a simple model with two
straight pipe sections connected by a 90° elbow. The straight pipes are 25.4 cm (10.0 inches) in length,
the radius of the curved section is 10.16 cm (4.0 inches), and the outer radius of the pipe section is 1.27
cm (0.5 inches). The wall thickness of the pipe is varied from 0.03175 cm to 0.2032 cm (0.0125 inches to
0.08 inches) in a parametric study, as discussed below. The pipe material is assumed to be isotropic linear
elastic with a Young’s modulus of 194 GPa (28.1 × 106 psi) and a Poisson’s ratio of 0.0. The straight
portions of the pipeline are assumed to be long enough so that warping at the ends of the structure is
negligible.
Two loading conditions are analyzed. The first case is shown in Figure 1.1.3–1 with unit inward
displacements imposed on both ends of the structure. This loading condition has the effect of closing the
pipeline in on itself. In the second case the sense of the applied unit displacements is outward, opening
the pipeline. Both cases are considered to be large-displacement/small-strain analyses.
A parametric study comparing the results obtained with different element types (shells, elbows, and
pipes) over a range of flexibility factors, k, is performed. As defined in Dodge and Moore (1972), the
flexibility factor for an elbow is the ratio of the bending flexibility of the elbow segment to that of a
straight pipe of the same dimensions, assuming small displacements and an elastic response. When the
internal (gauge) pressure is zero, as is assumed in this study, k can be approximated as
where
1.1.3–1
Abaqus Version 6.12 ID:
Printed on:
LINEAR ELASTIC PIPELINE
R is the bend radius of the curved section, r is the mean radius of the pipe, t is the wall thickness of
the pipe, and is Poisson’s ratio. Changes in the flexibility factor are introduced by varying the wall
thickness of the pipe.
The pipeline is modeled with three different element types: S4 shell elements, ELBOW31 elbow
elements, and PIPE31 pipe elements. The S4 shell element model consists of a relatively fine mesh
of 40 elements about the circumference and 75 elements along the length. This mesh is deemed fine
enough to capture the true response of the pipeline accurately, although no mesh convergence studies are
performed. Two analyses are conducted with the shell mesh: one with automatic stabilization using a
constant damping factor (see “Automatic stabilization of static problems with a constant damping factor”
in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User’s Manual), and one with
adaptive automatic stabilization (see “Adaptive automatic stabilization scheme” in “Solving nonlinear
problems,” Section 7.1.1 of the Abaqus Analysis User’s Manual). The pipe and elbow element meshes
consist of 75 elements along the length; the analyses with these element types do not use automatic
stabilization.
The results of the shell element model with automatic stabilization using a constant damping factor
are taken as the reference solution. The reaction force at the tip of the pipeline is used to evaluate the
effectiveness of the pipe and elbow elements. In addition, the ovalization values of the pipeline crosssection predicted by the elbow element models are compared.
The elbow elements are tested with 0, 3, and 6 Fourier modes, respectively. In general, elbow
element accuracy improves as more modes are used, although the computational cost increases
accordingly. In addition to standard pipe elements, tests are performed on pipe elements with a special
flexibility knockdown factor. Flexibility knockdown factors (Dodge and Moore, 1972) are corrections to
the bending stiffness based upon linear semianalytical results. They are applied to simple beam elements
in an attempt to capture the global effects of ovalization. The knockdown factor is implemented in the
PIPE31 elements by scaling the true thickness by the flexibility factor; this is equivalent to scaling the
moment of inertia of the pipe element by
.
Results and discussion
The results obtained with the shell element model with automatic stabilization using a constant damping
factor are taken as the reference solution. Very similar results are obtained with the same mesh using the
adaptive automatic stabilization scheme.
The tip reaction forces due to the inward prescribed displacements for the various analysis models
are shown in Figure 1.1.3–2. The results are normalized with respect to those obtained with the shell
model. The results obtained with the ELBOW31 element model with 6 Fourier modes show excellent
agreement with the reference solution over the entire range of flexibility factors considered in this study.
The remaining four models generally exhibit excessively stiff response for all values of k. The PIPE31
element model, which uses the flexibility knockdown factor, shows a relatively constant error of about
1.1.3–2
Abaqus Version 6.12 ID:
Printed on:
LINEAR ELASTIC PIPELINE
20% over the entire range of flexibility factors. The 0-mode ELBOW31 element model and the PIPE31
element model without the knockdown factor produce very similar results for all values of k.
The normalized tip reaction forces due to the outward unit displacement for the various analysis
models are shown in Figure 1.1.3–3. Again, the results obtained with the 6-mode ELBOW31 element
model compare well with the reference shell solution. The 0-mode and 3-mode ELBOW31 and the
PIPE31 (without the flexibility knockdown factor) element models exhibit overly stiff response. The
PIPE31 element model with the knockdown factor has a transition region near k = 1.5, where the response
changes from being too stiff to being too soft. The results in Abaqus/Explicit for pipe elements are
consistent with those obtained in Abaqus/Standard.
Figure 1.1.3–4 and Figure 1.1.3–5 illustrate the effect of the number of included Fourier modes (0,
3, and 6) on the ability of the elbow elements to model the ovalization in the pipebend accurately in both
load cases considered in this study. By definition, the 0-mode model cannot ovalize, which accounts for
its stiff response. The 3-mode and the 6-mode models show significant ovalization in both loading cases.
Figure 1.1.3–6 compares the ovalization of the 6-mode model in the opened and closed deformation
states. It clearly illustrates that when the ends of the pipe are displaced inward (closing mode), the
height of the pipe’s cross-section gets smaller, thereby reducing the overall stiffness of the pipe; the
reverse is true when the pipe ends are displaced outward: the height of the pipe’s cross-section gets
larger, thereby increasing the pipe stiffness. These three figures were produced with the aid of the elbow
element postprocessing program felbow.f (“Creation of a data file to facilitate the postprocessing of
elbow element results: FELBOW,” Section 14.1.6), written in FORTRAN. The postprocessing programs
felbow.C (“A C++ version of FELBOW,” Section 10.15.6 of the Abaqus Scripting User’s Manual)
and felbow.py (“An Abaqus Scripting Interface version of FELBOW,” Section 9.10.12 of the Abaqus
Scripting User’s Manual), written in C++ and Python, respectively, are also available for generating the
data for these figures. The user must ensure that the output variables are written to the output database
to use these two programs.
Parametric study
The performance of the pipe and elbow elements investigated in this example is analyzed conveniently
in a parametric study using the Python scripting capabilities of Abaqus (“Scripting parametric studies,”
Section 20.1.1 of the Abaqus Analysis User’s Manual). We perform a parametric study in which eight
analyses are executed automatically for each of the three element types (S4, ELBOW31, and PIPE31)
discussed above; these parametric studies correspond to wall thickness values ranging from 0.03175 cm
to 0.2032 cm (0.0125 inches to 0.08 inches).
The Python script file elbowtest.psf is used to perform the parametric study. The function
customTable (shown below) is an example of advanced Python scripting (Lutz and Ascher,
1999), which is used in elbowtest.psf. Such advanced scripting is not routinely needed, but in this
case a dependent variable such as k cannot be included as a column of data in an XYPLOT file.
customTable is designed to overcome this limitation by taking an XYPLOT file from the parametric
study and converting it into a new file of reaction forces versus flexibility factors (k).
###############################################################
#
def customTable(file1, file2):
1.1.3–3
Abaqus Version 6.12 ID:
Printed on:
LINEAR ELASTIC PIPELINE
for line in file1.readlines():
print line
nl = string.split(line,',')
disp = float(nl[0])
bend_radius = float(nl[1])
wall_thick = float(nl[2])
outer_pipe_radius = float(nl[3])
poisson = float(nl[4])
rf = float(nl[6])
mean_rad = outer_pipe_radius - wall_thick/2.0
k = bend_radius*wall_thick/mean_rad**2
k = k/sqrt(1.e0 - poisson**2)
k = 1.66e0/k
outputstring = str(k) + ', ' + str(rf) + '\n'
file2.write(outputstring)
#
#############################################################
Input files
elbowtest_shell.inp
elbowtest_shell_stabil_adap.inp
elbowtest_elbow0.inp
elbowtest_elbow3.inp
elbowtest_elbow6.inp
elbowtest_pipek.inp
elbowtest_pipek_xpl.inp
elbowtest_pipe.inp
elbowtest_pipe_xpl.inp
elbowtest.psf
S4 model.
S4 model with adaptive stabilization.
ELBOW31 model with 0 Fourier modes.
ELBOW31 model with 3 Fourier modes.
ELBOW31 model with 6 Fourier modes.
PIPE31 model with the flexibility knockdown factor.
PIPE31 model with the flexibility knockdown factor in
Abaqus/Explicit.
PIPE31 model without the flexibility knockdown factor.
PIPE31 model without the flexibility knockdown factor
in Abaqus/Explicit.
Python script file for the parametric study.
References
•
Dodge, W. G., and S. E. Moore, “Stress Indices and Flexibility Factors for Moment Loadings on
Elbows and Curved Pipes,” Welding Research Council Bulletin, no. 179, 1972.
•
Lutz, M., and D. Ascher, Learning Python, O’Reilly, 1999.
1.1.3–4
Abaqus Version 6.12 ID:
Printed on:
LINEAR ELASTIC PIPELINE
a
R
u
a
r
t
pipe cross-section
Figure 1.1.3–1
u
Pipeline geometry with inward prescribed tip displacements.
ELBOW31 0 modes
ELBOW31 3 modes
ELBOW31 6 modes
PIPE31
PIPE31 with knockdown
Shell S4
Figure 1.1.3–2
Normalized tip reaction force: closing displacement case.
1.1.3–5
Abaqus Version 6.12 ID:
Printed on:
LINEAR ELASTIC PIPELINE
ELBOW31 0 modes
ELBOW31 3 modes
ELBOW31 6 modes
PIPE31
PIPE31 with knockdown
Shell S4
Figure 1.1.3–3
Normalized tip reaction force: opening displacement case.
close-0
close-3
close-6
Figure 1.1.3–4 Ovalization of the ELBOW31 cross-sections for
0, 3, and 6 Fourier modes: closing displacement case.
1.1.3–6
Abaqus Version 6.12 ID:
Printed on:
LINEAR ELASTIC PIPELINE
open-0
open-3
open-6
Figure 1.1.3–5 Ovalization of the ELBOW31 cross-sections for
0, 3, and 6 Fourier modes: opening displacement case.
close-6
open-6
Figure 1.1.3–6 Ovalization of the ELBOW31 cross-sections for
6 Fourier modes: opening and closing displacement cases.
1.1.3–7
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
1.1.4
INDENTATION OF AN ELASTOMERIC FOAM SPECIMEN WITH A HEMISPHERICAL
PUNCH
Products: Abaqus/Standard
Abaqus/Explicit
Abaqus/Design
In this example we consider a cylindrical specimen of an elastomeric foam, indented by a rough, rigid,
hemispherical punch. Examples of elastomeric foam materials are cellular polymers such as cushions,
padding, and packaging materials. This problem illustrates a typical application of elastomeric foam
materials when used in energy absorption devices. The same geometry as the crushable foam model of
“Simple tests on a crushable foam specimen,” Section 3.2.7 of the Abaqus Benchmarks Manual, is used but
with a slightly different mesh. Design sensitivity analysis is carried out for a shape design parameter and
a material design parameter to illustrate the usage of design sensitivity analysis for a problem involving
contact.
Geometry and model
The axisymmetric model (135 linear 4-node elements) analyzed is shown in Figure 1.1.4–1. The mesh
refinement is biased toward the center of the foam specimen where the largest deformation is expected.
The foam specimen has a radius of 600 mm and a thickness of 300 mm. The punch has a radius of
200 mm. The bottom nodes of the mesh are fixed, while the outer boundary is free to move.
A contact pair is defined between the punch, which is modeled by a rough spherical rigid surface,
and a slave surface composed of the faces of the axisymmetric elements in the contact region. The friction
coefficient between the punch and the foam is 0.8. A point mass of 200 kg representing the weight of
the punch is attached to the rigid body reference node. The model is analyzed in both Abaqus/Standard
and Abaqus/Explicit.
Material
The elastomeric foam material is defined using experimental test data. The uniaxial compression and
simple shear data stress-strain curves are shown in Figure 1.1.4–2. Other available test data options
are biaxial test data, planar test data, and volumetric test data. The test data are defined in terms of
nominal stress and nominal strain values. Abaqus performs a nonlinear least-squares fit of the test data
to determine the hyperfoam coefficients
and .
Details of the formulation and usage of the hyperfoam model are given in “Hyperelastic behavior
in elastomeric foams,” Section 22.5.2 of the Abaqus Analysis User’s Manual; “Hyperelastic material
behavior,” Section 4.6.1 of the Abaqus Theory Manual; and “Fitting of hyperelastic and hyperfoam
constants,” Section 4.6.2 of the Abaqus Theory Manual. “Fitting of elastomeric foam test data,”
Section 3.1.5 of the Abaqus Benchmarks Manual, illustrates the fitting of elastomeric foam test data to
derive the hyperfoam coefficients.
For the material used in this example,
is zero, since the effective Poisson’s ratio, , is zero as
specified by the POISSON parameter. The order of the series expansion is chosen to be
2 since this
fits the test data with sufficient accuracy. It also provides a more stable model than the
3 case.
1.1.4–1
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
The viscoelastic properties in Abaqus are specified in terms of a relaxation curve (shown in
Figure 1.1.4–3) of the normalized modulus
, where
is the shear or bulk modulus as a
function of time and
is the instantaneous modulus as determined from the hyperfoam model. This
requires Abaqus to calculate the Prony series parameters from data taken from shear and volumetric
relaxation tests. The relaxation data are specified as part of the definition of shear test data but
actually apply to both shear and bulk moduli when used in conjunction with the hyperfoam model.
Abaqus performs a nonlinear least-squares fit of the relaxation data to a Prony series to determine the
coefficients,
, and the relaxation periods, . A maximum order of 2 is used for fitting the Prony
series. If creep data are available, you can specify normalized creep compliance data to compute the
Prony series parameters.
A rectangular material orientation is defined for the foam specimen, so stress and strain are reported
in material axes that rotate with the element deformation. This is especially useful when looking at the
stress and strain values in the region of the foam in contact with the punch in the direction normal to the
punch (direction “22”).
The rough surface of the punch is modeled by specifying a friction coefficient of 0.8 for the contact
surface interaction.
Procedure and loading definitions
Two cases are analyzed. In the first case the punch is displaced statically downward to indent the foam,
and the reaction force-displacement relation is measured for both the purely elastic and viscoelastic cases.
In the second case the punch statically indents the foam through gravity loading and is then subjected
to impulsive loading. The dynamic response of the punch is sought as it interacts with the viscoelastic
foam.
Case 1
In Abaqus/Standard the punch is displaced downward by a prescribed displacement boundary condition
in the first step, indenting the foam specimen by a distance of 250 mm. Geometric nonlinearity should be
accounted for in this step, since the response involves large deformation. In the second step the punch is
displaced back to its original position. Two analyses are performed—one using the static procedure for
both steps and the other using the quasi-static procedure for both steps. During a static step the material
behaves purely elastically, using the properties specified with the hyperfoam model. The quasi-static,
direct-integration implicit dynamic, or fully coupled thermal-stress procedure must be used to activate
the viscoelastic behavior. In this case the punch is pushed down in a period of one second and then
moved back up again in one second. The accuracy of the creep integration in the quasi-static procedure
can be controlled and is typically calculated by dividing an acceptable stress error tolerance by a typical
elastic modulus. In this problem we estimate a stress error tolerance of about 0.005 MPa and use the
initial elastic modulus, E
2
0.34, to determine an accuracy tolerance of 0.01.
In Abaqus/Explicit the punch is also displaced downward by a prescribed displacement boundary
condition, indenting the foam by a depth of 250 mm. The punch is then lifted back to its original position.
In this case the punch is modeled as either an analytical rigid surface or a discrete rigid surface defined
with RAX2 elements. The entire analysis runs for 2 seconds. The actual time period of the analysis
1.1.4–2
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
is large by explicit dynamic standards. Hence, to reduce the computational time, the mass density of
the elements is increased artificially to increase the stable time increment without losing the accuracy of
the solution. The mass scaling factor is set to 10, which corresponds to a speedup factor of
. The
reaction force-displacement relation is measured for both the elastic and viscoelastic cases.
Case 2
The Abaqus/Standard analysis is composed of three steps. The first step is a quasi-static step, where
gravity loading is applied to the point mass of the punch. The gravity loading is ramped up in two seconds,
and the step is run for a total of five seconds to allow the foam to relax fully. In the second step, which is
a direct-integration implicit dynamic step, an impulsive load in the form of a half sine wave amplitude
with a peak magnitude of 5000 N is applied to the punch over a period of one second. In the third step,
also a direct-integration implicit dynamic step, the punch is allowed to move freely until the vibration
is damped out by the viscoelastic foam. For a dynamic analysis with automatic time incrementation,
the value of the half-increment residual tolerance for the direct-integration implicit dynamic procedure
controls the accuracy of the time integration. For systems that have significant energy dissipation, such
as this heavily damped model, a relatively high value of this tolerance can be chosen. We choose the
tolerance to be 100 times a typical average force that we estimate (and later confirm from the analysis
results) to be on the order of 50 N. Thus, the half-increment residual tolerance is 5000 N. For the second
direct-integration implicit dynamic step we bypass calculation of initial accelerations at the beginning of
the step, since there is no sudden change in load to create a discontinuity in the accelerations.
In the Abaqus/Explicit analysis the punch indents the foam quasi-statically through gravity loading
and is then subjected to an impulsive loading. In the first step gravity loading is applied to the point mass
of the punch, and the foam is allowed to relax fully. The mass scaling factor in this step is set to 10. In
the second step a force in the form of a half sine wave is applied to the punch, and the dynamic response
of the punch is obtained as it interacts with the viscoelastic foam. In the third step the load is removed,
and the punch is allowed to move freely. Mass scaling is not used in Steps 2 and 3 since the true dynamic
response is sought.
Design sensitivity analysis
For the design sensitivity analysis (DSA) carried out with static steps in Abaqus/Standard, the hyperfoam
material properties are given using direct input of coefficients based on the test data given above. For
2, the coefficients are
0.16245,
3.59734E−05,
8.89239,
–4.52156, and
0.0. Since the quasi-static procedure is not supported for DSA, it is replaced with the static
procedure and the viscoelastic material behavior is removed. In addition, since a more accurate tangent
stiffness leads to improved sensitivity results, the solution controls are used to tighten the residual
tolerance.
The material parameter
is chosen as one of the design parameters. The other (shape) design
parameter used for design sensitivity analysis, L, represents the thickness of the foam at the free end (see
Figure 1.1.4–1). The z-coordinates of the nodes on the top surface are assumed to depend on L via the
equation
. The r-coordinates are considered to be independent of L. To define
this dependency in Abaqus, the gradients of the coordinates with respect to
1.1.4–3
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
are given as part of the specification of parameter shape variation.
Results and discussion
This problem tests the hyperfoam material model in Abaqus but does not provide independent verification
of the model. The results for all analyses are discussed in the following paragraphs.
Case 1
Deformation and contour plots for oriented S22 stress and LE22 strain are shown for the viscoelastic foam
in Figure 1.1.4–4 through Figure 1.1.4–6 for the Abaqus/Standard analysis and Figure 1.1.4–7 through
Figure 1.1.4–9 for the Abaqus/Explicit analysis. Even though the foam has been subjected to large strains,
only moderate distortions occur because of the zero Poisson’s ratio. The maximum logarithmic strain is
on the order of −1.85, which is equivalent to a stretch of
0.16 or a nominal compressive
strain of 84%, indicating severe compression of the foam.
Figure 1.1.4–10 shows a comparison of the punch reaction force histories obtained with
Abaqus/Standard and Abaqus/Explicit. In the viscoelastic case the stresses relax during loading
and, consequently, lead to a softer response than in the purely elastic case. A comparison of the
force-displacement responses obtained with Abaqus/Standard and Abaqus/Explicit is shown in
Figure 1.1.4–11. The purely elastic material is reversible, while the viscoelastic material shows
hysteresis.
Case 2
Figure 1.1.4–12 shows various displaced configurations during the Case 2 analysis for Abaqus/Standard
and Abaqus/Explicit. Displacement, velocity, and acceleration histories for the punch are shown in
Figure 1.1.4–13, Figure 1.1.4–14, and Figure 1.1.4–15, respectively. The displacement is shown to reach
a steady value at the stress relaxation stage, followed by a severe drop due to the impulsive dynamic load.
This is followed by a rebound and then finally by a rapid decay of the subsequent oscillations due to the
strong damping provided by the viscoelasticity of the foam.
Abaqus/Design
Figure 1.1.4–16 and Figure 1.1.4–17 show the contours of sensitivity of the displacement in the
z-direction to the design parameters
and , respectively. Figure 1.1.4–18 and Figure 1.1.4–19
show the contours of sensitivity of S22 to the design parameters L and , respectively. To provide
an independent assessment of the results provided by Abaqus, sensitivities were computed using the
overall finite difference (OFD) technique. The central difference method with a perturbation size of
1.1.4–4
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
0.1% of the value of the design parameter was used to obtain the OFD results. Table 1.1.4–1 shows that
the sensitivities computed using Abaqus compare well with the overall finite difference results.
Input files
indentfoam_std_elast_1.inp
indentfoam_std_elast_1_st.inp
indentfoam_std_elast_1_eh.inp
indentfoam_std_visco_1.inp
indentfoam_std_visco_1_st.inp
indentfoam_std_visco_1_eh.inp
indentfoam_std_visco_2.inp
indentfoam_std_visco_2_surf.inp
indentfoam_xpl_elast_1.inp
indentfoam_xpl_elast_1_subcyc.inp
indentfoam_xpl_elast_fac_1.inp
Case 1 of the Abaqus/Standard example using elastic
properties of the foam, which is statically deformed in
two *STATIC steps.
Case 1 of the Abaqus/Standard example (CAX4R
elements with hourglass control based on total stiffness)
using elastic properties of the foam, which is statically
deformed in two *STATIC steps.
Case 1 of the Abaqus/Standard example (CAX4R
elements with enhanced hourglass control) using elastic
properties of the foam, which is statically deformed in
two *STATIC steps.
Case 1 of the Abaqus/Standard example using
viscoelastic properties of the foam, which is statically
deformed in two *VISCO steps.
Case 1 of the Abaqus/Standard example (CAX4R
elements with hourglass control based on total stiffness)
using viscoelastic properties of the foam, which is
statically deformed in two *VISCO steps.
Case 1 of the Abaqus/Standard example (CAX4R
elements with enhanced hourglass control) using
viscoelastic properties of the foam, which is statically
deformed in two *VISCO steps.
Case 2 of the Abaqus/Standard example using
viscoelastic properties of the foam.
Case 2 of the Abaqus/Standard example using
viscoelastic properties of the foam. Surface-to-surface
contact is utilized.
Case 1 of the Abaqus/Explicit example using elastic
properties of the foam with the punch modeled as an
analytical rigid surface.
Case 1 of the Abaqus/Explicit example using elastic
properties of the foam with the punch modeled as an
analytical rigid surface using the subcycling feature.
Case 1 of the Abaqus/Explicit example using elastic
properties of the foam with the punch modeled as a
faceted rigid surface.
1.1.4–5
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
indentfoam_xpl_visco_1.inp
indentfoam_xpl_visco_2.inp
indentfoamhemipunch_dsa.inp
Table 1.1.4–1
Case 1 of the Abaqus/Explicit example using viscoelastic
properties of the foam with the punch modeled as an
analytical rigid surface.
Case 2 of the Abaqus/Explicit example using viscoelastic
properties of the foam with the punch modeled as an
analytical rigid surface.
Design sensitivity analysis.
Comparison of normalized sensitivities at the end of the analysis computed
using Abaqus and the overall finite difference (OFD) method.
Normalized sensitivity
Abaqus
OFD
0.4921
0.4922
1.085
1.104
0.006925
0.006927
0.4059
0.4120
0.5084
0.5085
0.3252
0.3207
1.1.4–6
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
L
300
2
3
1
600
Figure 1.1.4–1
Model for foam indentation by a spherical punch.
1.1.4–7
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
Nominal Shear
Transv. Shear
Uniaxial Compr.
Figure 1.1.4–2
Elastomeric foam stress-strain curves.
Norm. modulus
Figure 1.1.4–3
Elastic modulus relaxation curve.
1.1.4–8
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
2
3
Figure 1.1.4–4
1
Maximum deformation of viscoelastic foam: Case 1, Abaqus/Standard.
Figure 1.1.4–5
S22 contour plot of viscoelastic foam: Case 1, Abaqus/Standard.
1.1.4–9
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
Figure 1.1.4–6
LE22 contour plot of viscoelastic foam: Case 1, Abaqus/Standard.
2
3
1
Figure 1.1.4–7
Deformed plot at 1.0 s: Case 1, Abaqus/Explicit.
1.1.4–10
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
Figure 1.1.4–8
Figure 1.1.4–9
S22 contour plot of viscoelastic foam at 1.0 s: Case 1, Abaqus/Explicit.
LE22 contour plot of viscoelastic foam at 1.0 s: Case 1, Abaqus/Explicit.
1.1.4–11
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
ABAQUS/Standard:
ABAQUS/Standard:
ABAQUS/Explicit:
ABAQUS/Explicit:
Elastic
Visco
Elastic
Visco
Figure 1.1.4–10
ABAQUS/Standard:
ABAQUS/Standard:
ABAQUS/Explicit:
ABAQUS/Explicit:
Punch reaction force history: Case 1.
Elastic
Visco
Elastic
Visco
Figure 1.1.4–11 Punch reaction force versus displacement
response (loading-unloading curves): Case 1.
1.1.4–12
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
2
2
3
3
Step 1: ABAQUS/Standard, Time = 5.00 sec.
Step 1: ABAQUS/Explicit, Time = 5.00 sec.
2
2
3
3
1
Step 2: ABAQUS/Standard, Time = 6.00 sec.
1
Step 2: ABAQUS/Explicit, Time = 6.00 sec.
2
2
3
1
1
3
1
Step 3: ABAQUS/Standard, Time = 16.00 sec.
Figure 1.1.4–12
1
Step 3: ABAQUS/Explicit, Time = 16.00 sec.
Deformed shape plots at the end of visco and dynamic steps:
Case 2, Abaqus/Standard (left) and Abaqus/Explicit (right).
1.1.4–13
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
ABAQUS/Standard
ABAQUS/Explicit
Figure 1.1.4–13 Displacement histories of the punch: Case 2,
Abaqus/Standard and Abaqus/Explicit.
ABAQUS/Standard
ABAQUS/Explicit
Figure 1.1.4–14 Velocity histories of the punch: Case 2,
Abaqus/Standard and Abaqus/Explicit.
1.1.4–14
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
ABAQUS/Standard
ABAQUS/Explicit
Figure 1.1.4–15 Acceleration histories of the punch: Case 2,
Abaqus/Standard and Abaqus/Explicit.
1.1.4–15
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
Figure 1.1.4–16 Sensitivities at the end of the analysis for
displacement in the z-direction with respect to L.
Figure 1.1.4–17 Sensitivities at the end of the analysis for
displacement in the z-direction with respect to .
1.1.4–16
Abaqus Version 6.12 ID:
Printed on:
ELASTOMERIC FOAM INDENTATION
Figure 1.1.4–18
Sensitivities at the end of the analysis for stress S22 with respect to L.
Figure 1.1.4–19
Sensitivities at the end of the analysis for stress S22 with respect to
1.1.4–17
Abaqus Version 6.12 ID:
Printed on:
.
COLLAPSE OF A CONCRETE SLAB
1.1.5
COLLAPSE OF A CONCRETE SLAB
Products: Abaqus/Standard
Abaqus/Explicit
This problem examines the use of the smeared crack model (“Concrete smeared cracking,” Section 23.6.1
of the Abaqus Analysis User’s Manual) and the brittle cracking model (“Cracking model for concrete,”
Section 23.6.2 of the Abaqus Analysis User’s Manual) for the analysis of reinforced concrete structures. The
geometry of the problem is defined in Figure 1.1.5–1. A square slab is supported in the transverse direction
at its four corners and loaded by a point load at its center. The slab is reinforced in two directions at 75%
of its depth. The reinforcement ratio (volume of steel/volume of concrete) is 8.5 × 10−3 in each direction.
The slab was tested experimentally by McNeice (1967) and has been analyzed by a number of workers,
including Hand et al. (1973), Lin and Scordelis (1975), Gilbert and Warner (1978), Hinton et al. (1981), and
Crisfield (1982).
Geometric modeling
Symmetry conditions allow us to model one-quarter of the slab. A 3 × 3 mesh of 8-node shell elements
is used for the Abaqus/Standard analysis. No mesh convergence studies have been performed, but the
reasonable agreement between the analysis results and the experimental data suggests that the mesh is
adequate to predict overall response parameters with usable accuracy. Three different meshes are used
in Abaqus/Explicit to assess the sensitivity of the results to mesh refinement: a coarse 6 × 6 mesh, a
medium 12 × 12 mesh, and a fine 24 × 24 mesh of S4R elements. Nine integration points are used
through the thickness of the concrete to ensure that the development of plasticity and failure is modeled
adequately. The two-way reinforcement is modeled using layers of uniaxial reinforcement (rebars).
Symmetry boundary conditions are applied on the two edges of the mesh, and the corner point is
restrained in the transverse direction.
Material properties
The material data are given in Table 1.1.5–1. The material properties of concrete are taken from Gilbert
and Warner (1978). Some of these data are assumed values, because they are not available for the concrete
used in the experiment. The assumed values are taken from typical concrete data. The compressive
behavior of concrete in the cracking model in Abaqus/Explicit is assumed to be linear elastic. This is a
reasonable assumption for a case such as this problem, where the behavior of the structure is dominated
by cracking resulting from tension in the slab under bending.
The modeling of the concrete-reinforcement interaction and the energy release at cracking is of
critical importance to the response of a structure such as this once the concrete starts to crack. These
effects are modeled in an indirect way by adding “tension stiffening” to the plain concrete model. This
approach is described in “A cracking model for concrete and other brittle materials,” Section 4.5.3 of the
Abaqus Theory Manual; “Concrete smeared cracking,” Section 23.6.1 of the Abaqus Analysis User’s
Manual; and “Cracking model for concrete,” Section 23.6.2 of the Abaqus Analysis User’s Manual.
The simplest tension stiffening model defines a linear loss of strength beyond the cracking failure of the
1.1.5–1
Abaqus Version 6.12 ID:
Printed on:
COLLAPSE OF A CONCRETE SLAB
concrete. In this example three different values for the strain beyond failure at which all strength is lost
(5 × 10−4 , 1 × 10−3 , and 2 × 10−3 ) are used to illustrate the effect of the tension stiffening parameters on
the response.
Since the response is dominated by bending, it is controlled by the material behavior normal to the
crack planes. The material’s shear behavior in the plane of the cracks is not important. Consequently, the
choice of shear retention has no significant influence on the results. In Abaqus/Explicit the shear retention
chosen is exhausted at the same value of the crack opening at which tension stiffening is exhausted. In
Abaqus/Standard full shear retention is used because it provides a more efficient numerical solution.
Solution control
Since considerable nonlinearity is expected in the response, including the possibility of unstable
regimes as the concrete cracks, the modified Riks method is used with automatic incrementation in the
Abaqus/Standard analysis. With the Riks method the load data and solution parameters serve only to
give an estimate of the initial increment of load. In this case it seems reasonable to apply an initial load
of 1112 N (250 lb) to the quarter-model for a total initial load on the structure of 4448 N (1000 lb).
This can be accomplished by specifying a load of 22241 N (5000 lb) and an initial time increment of
0.05 out of a total time period of 1.0. The analysis is terminated when the central displacement reaches
25.4 mm (1 in).
Since Abaqus/Explicit is a dynamic analysis program and in this case we are interested in static
solutions, the slab must be loaded slowly enough to eliminate any significant inertia effects. The slab is
loaded in its center by applying a velocity that increases linearly from 0 to 2.0 in/second such that the
center displaces a total of 1 inches in 1 second. This very slow loading rate ensures quasi-static solutions;
however, it is computationally expensive. The CPU time required for this analysis can be reduced in one
of two ways: the loading rate can be increased incrementally until it is judged that any further increase in
loading rate would no longer result in a quasi-static solution, or mass scaling can be used (see “Explicit
dynamic analysis,” Section 6.3.3 of the Abaqus Analysis User’s Manual). These two approaches are
equivalent. Mass scaling is used here to demonstrate the validity of such an approach when it is used in
conjunction with the brittle cracking model. Mass scaling is done by increasing the density of the concrete
and the reinforcement by a factor of 100, thereby increasing the stable time increment for the analysis by a
factor of 10 and reducing the computation time by the same amount while using the original slow loading
rate. Figure 1.1.5–4 shows the load-deflection response of the slab for analyses using the 12 × 12 mesh
with and without mass scaling. The mass scaling used does not affect the results significantly; therefore,
all subsequent analyses are performed using mass scaling.
Results and discussion
Results for each analysis are discussed in the following sections.
Abaqus/Standard results
The numerical and experimental results are compared in Figure 1.1.5–2 on the basis of load versus
deflection at the center of the slab. The strong effect of the tension stiffening assumption is very clear
in that plot. The analysis with tension stiffening, such that the tensile strength is lost at a strain of 10−3
1.1.5–2
Abaqus Version 6.12 ID:
Printed on:
COLLAPSE OF A CONCRETE SLAB
beyond failure, shows the best agreement with the experiment. This analysis provides useful information
from a design viewpoint. The failure pattern in the concrete is illustrated in Figure 1.1.5–3, which shows
the predicted crack pattern on the lower surface of the slab at a central deflection of 7.6 mm (0.3 in).
Abaqus/Explicit results
Figure 1.1.5–5 shows the load-deflection response of the slab for the three different mesh densities using
a tension stiffening value of 2 × 10−3 . Since the coarse mesh predicts a slightly higher limit load than the
medium and fine meshes do and the limit loads for the medium and fine mesh analyses are very close,
the tension stiffening study is performed using the medium mesh only.
The numerical (12 × 12 mesh) results are compared to the experimental results in Figure 1.1.5–6
for the three different values of tension stiffening. It is clear that the less tension stiffening used, the
softer the load-deflection response is. A value of tension stiffening somewhere between the highest and
middle values appears to match the experimental results best. The lowest tension stiffening value causes
more sudden cracking in the concrete and, as a result, the response tends to be more dynamic than that
obtained with the higher tension stiffening values.
Figure 1.1.5–7 shows the numerically predicted crack pattern on the lower surface of the slab for
the medium mesh.
Input files
Abaqus/Standard input files
collapseconcslab_s8r.inp
collapseconcslab_s9r5.inp
collapseconcslab_postoutput.inp
S8R elements.
S9R5 elements.
*POST OUTPUT analysis.
Abaqus/Explicit input files
mcneice_1.inp
mcneice_2.inp
mcneice_3.inp
mcneice_4.inp
mcneice_5.inp
mcneice_6.inp
Coarse (6 × 6) mesh; tension stiffening = 2 × 10−3 .
Medium (12 × 12) mesh; tension stiffening = 2 × 10−3 .
Fine (24 × 24) mesh; tension stiffening = 2 × 10−3 .
Medium (12 × 12) mesh; tension stiffening = 1 × 10−3 .
Medium (12 × 12) mesh; tension stiffening = 5 × 10−4 .
Medium (12 × 12) mesh; tension stiffening = 2 × 10−3 ; no
mass scaling.
References
•
Crisfield, M. A., “Variable Step-Length for Nonlinear Structural Analysis,” Report 1049, Transport
and Road Research Lab., Crowthorne, England, 1982.
•
Gilbert, R. I., and R. F. Warner, “Tension Stiffening in Reinforced Concrete Slabs,” Journal of the
Structural Division, American Society of Civil Engineers, vol. 104, ST12, pp. 1885–1900, 1978.
1.1.5–3
Abaqus Version 6.12 ID:
Printed on:
COLLAPSE OF A CONCRETE SLAB
•
Hand, F. D., D. A. Pecknold, and W. C. Schnobrich, “Nonlinear Analysis of Reinforced Concrete
Plates and Shells,” Journal of the Structural Division, American Society of Civil Engineers, vol. 99,
ST7, pp. 1491–1505, 1973.
•
Hinton, E., H. H. Abdel Rahman, and O. C. Zienkiewicz, “Computational Strategies for
Reinforced Concrete Slab Systems,” International Association of Bridge and Structural
Engineering Colloquium on Advanced Mechanics of Reinforced Concrete, pp. 303–313, 1981.
•
Lin, C. S., and A. C. Scordelis, “Nonlinear Analysis of Reinforced Concrete Shells of General
Form,” Journal of the Structural Division, American Society of Civil Engineers, vol. 101,
pp. 523–238, 1975.
•
McNeice, A. M., “Elastic-Plastic Bending of Plates and Slabs by the Finite Element Method,”
Ph. D. Thesis, London University, 1967.
1.1.5–4
Abaqus Version 6.12 ID:
Printed on:
COLLAPSE OF A CONCRETE SLAB
Table 1.1.5–1
Material properties for the McNeice slab.
Concrete properties:
Properties are taken from Gilbert and Warner (1978) if available in that paper.
Properties marked with a * are not available and are assumed values.
Young’s modulus
Poisson’s ratio
28.6 GPa (4.15 × 106 lb/in2 )
0.15
Uniaxial compression values:
Yield stress
20.68 MPa (3000 lb/in2 )*
Failure stress
37.92 MPa (5500 lb/in2 )
Plastic strain at failure
1.5 × 10−3 *
Ratio of uniaxial tension
to compression failure stress
8.36 × 10−2
Ratio of biaxial to uniaxial
compression failure stress
1.16*
Cracking failure stress
459.8 lb/in2 (3.17 MPa)
Density (before mass scaling)
2.246 × 10−4 lb s2 /in4 (2400 kg/m3 )
“Tension stiffening” is assumed as a linear decrease of the stress to zero stress, at a strain of 5 × 10−4 , at
a strain of 10 × 10−4 , or at a strain of 20 × 10−4 .
Steel (rebar) properties:
Young’s modulus
Yield stress
Density (before mass scaling)
200 GPa (29 × 106 lb/in2 )
345 MPa (50 × 103 lb/in2 )
7.3 × 10−4 lb s2 /in4 (7800 kg/m3 )
1.1.5–5
Abaqus Version 6.12 ID:
Printed on:
COLLAPSE OF A CONCRETE SLAB
CL
Corners supported in transverse
direction only
Point load
CL
457.2 mm
(18.0 in)
457.2 mm
(18.0 in)
33.3 mm
(1.31 in)
depth to reinforcement
44.45 mm
(1.75 in)
thickness
Figure 1.1.5–1
McNeice slab.
1.1.5–6
Abaqus Version 6.12 ID:
Printed on:
COLLAPSE OF A CONCRETE SLAB
0.2
Central deflection, in
0.4
0.6
0.8
1.0
1.2
5.0
Central load, kN
4.0
15.0
3.0
10.0
2.0
Experiment (McNeice, 1967)
Tension stiffening, ε0 = 5.0 x 10-4
Tension stiffening, ε0 = 1.0 x 10-3
Tension stiffening, ε0 = 2.0 x 10-3
5.0
10.0
20.0
Central load, 103 lb
20.0
1.0
30.0
Central deflection, mm
Figure 1.1.5–2
Figure 1.1.5–3
Load-deflection response of McNeice slab, Abaqus/Standard.
Crack pattern on lower surface of slab, Abaqus/Standard.
1.1.5–7
Abaqus Version 6.12 ID:
Printed on:
COLLAPSE OF A CONCRETE SLAB
4.0
3
[ x10 ]
3.5
Central load "lb"
3.0
2.5
2.0
1.5
Mass Scaling
No Mass Scaling
1.0
.5
.0
.0
.2
.4
.6
.8
1.0
Central Displacement "in"
Figure 1.1.5–4 Load-deflection response of McNeice slab,
Abaqus/Explicit; influence of mass scaling.
4.0
[ x10 3 ]
3.6
3.2
Central load "lb"
2.8
2.4
2.0
1.6
1.2
6x6 mesh
12x12 mesh
24x24 mesh
.8
.4
.0
.0
.2
.4
.6
.8
1.0
Central Displacement "in"
Figure 1.1.5–5 Load-deflection response of McNeice slab,
Abaqus/Explicit; influence of mesh refinement.
1.1.5–8
Abaqus Version 6.12 ID:
Printed on:
COLLAPSE OF A CONCRETE SLAB
4.0
3
[ x10 ]
3.6
3.2
Central load "lb"
2.8
2.4
2.0
1.6
1.2
MCNEICE
Tens_Stiff 5e-4
Tens_Stiff 1e-3
Tens_Stiff 2e-3
.8
.4
.0
.0
.2
.4
.6
.8
1.0
Central Displacement "in"
Figure 1.1.5–6 Load-deflection response of McNeice slab,
Abaqus/Explicit; influence of tension stiffening.
Figure 1.1.5–7
Crack pattern on lower surface of slab, Abaqus/Explicit.
1.1.5–9
Abaqus Version 6.12 ID:
Printed on:
JOINTED ROCK SLOPE
1.1.6
JOINTED ROCK SLOPE STABILITY
Product: Abaqus/Standard
This example illustrates the use of the jointed material model in the context of geotechnical applications. We
examine the stability of the excavation of part of a jointed rock mass, leaving a sloped embankment. This
problem is chosen mainly as a verification case because it has been studied previously by Barton (1971) and
Hoek (1970), who used limit equilibrium methods, and by Zienkiewicz and Pande (1977), who used a finite
element model. This example also has been extended to study the slope stability of excavated soil medium
with the same geometry, by using the Mohr-Coulomb plasticity model with and without the tension cutoff
feature.
Geometry and model
The plane strain model analyzed is shown in Figure 1.1.6–1 together with the excavation geometry
and material properties. The rock mass contains two sets of planes of weakness: one vertical set of
joints and one set of inclined joints. We begin from a nonzero state of stress. In this problem this
consists of a vertical stress that increases linearly with depth to equilibrate the weight of the rock and
horizontal stresses caused by tectonic effects: such stress is quite commonly encountered in geotechnical
engineering. The active “loading” consists of removal of material to represent the excavation. It is clear
that, with a different initial stress state, the response of the system would be different. This illustrates the
need of nonlinear analysis in geotechnical applications—the response of a system to external “loading”
depends on the state of the system when that loading sequence begins (and, by extension, to the sequence
of loading). We can no longer think of superposing load cases, as is done in a linear analysis.
Practical geotechnical excavations involve a sequence of steps, in each of which some part of
the material mass is removed. Liners or retaining walls can be inserted during this process. Thus,
geotechnical problems require generality in creating and using a finite element model: the model
itself, and not just its response, changes with time—parts of the original model disappear, while other
components that were not originally present are added. This example is somewhat academic, in that we
do not encounter this level of complexity. Instead, following the previous authors’ use of the example,
we assume that the entire excavation occurs simultaneously.
Solution controls
The jointed material model includes a joint opening/closing capability. When a joint opens, the material
is assumed to have no elastic stiffness with respect to direct strain across the joint system. Because of
this, and also as a result of the fact that different combinations of joints may be yielding at any one time,
the overall convergence of the solution is expected to be nonmonotonic. In such cases setting the time
incrementation parameters automatically is generally recommended to prevent premature termination of
the equilibrium iteration process because the solution may appear to be diverging.
1.1.6–1
Abaqus Version 6.12 ID:
Printed on:
JOINTED ROCK SLOPE
As the end of the excavation process is approached, the automatic incrementation algorithm reduces
the load increment significantly, indicating the onset of failure of the slope. In such analyses it is useful
to specify a minimum time step to avoid unproductive iteration.
For the nonassociated flow case the unsymmetric equation solver should be used. This is essential
for obtaining an acceptable rate of convergence since nonassociated flow plasticity has a nonsymmetric
stiffness matrix.
Results and discussion
In this problem we examine the effect of joint cohesion on slope collapse through a sequence of solutions
with different values of joint cohesion, with all other parameters kept fixed. Figure 1.1.6–2 shows
the variation of horizontal displacements as cohesion is reduced at the crest of the slope (point A in
Figure 1.1.6–1) and at a point one-third of the way up the slope (point B in Figure 1.1.6–1). This plot
suggests that the slope collapses if the cohesion is less than 24 kPa for the case of associated flow or
less than 26 kPa for the case of nonassociated flow. These compare well with the value calculated
by Barton (26 kPa) using a planar failure assumption in his limit equilibrium calculations. Barton’s
calculations also include “tension cracking” (akin to joint opening with no tension strength) as we do
in our calculation. Hoek calculates a cohesion value of 24 kPa for collapse of the slope. Although he
also makes the planar failure assumption, he does not include tension cracking. This is, presumably, the
reason why his calculated value is lower than Barton’s. Zienkiewicz and Pande assume the joints have a
tension strength of one-tenth of the cohesion and calculate the cohesion value necessary for collapse as
23 kPa for associated flow and 25 kPa for nondilatant flow.
Figure 1.1.6–3 shows the deformed configuration after excavation for the nonassociated flow case
and clearly illustrates the manner in which the collapse is expected to occur. Figure 1.1.6–4 shows the
magnitude of the frictional slip on each joint system for the nonassociated flow case. A few joints open
near the crest of the slope.
The study of soil slope stability using the Mohr-Coulomb plasticity model is performed for two
cases: one without tension cutoff and one including the tension cutoff feature. The tension cutoff feature
limits the stress carrying capacity of soil in tension. It can be seen that the maximum principal stress
without tension cutoff (see contour plot in Figure 1.1.6–5) is higher than the limiting maximum principal
stress (see Figure 1.1.6–6) with tension cutoff as expected. With tension cutoff, one also observes the
appearance of the equivalent plastic strain in tension, PEEQT in the region of maximum principal stress.
In this case it is also seen that the equivalent plastic strain, PEEQ on the cohesion failure surface is higher
compared to the case without tension cutoff. The contour plots for the equivalent plastic strains are not
shown.
Input files
jointrockstabil_nonassoc_30pka.inp
jointrockstabil_assoc_25kpa.inp
mc_slopestabil.inp
Nonassociated flow case problem; cohesion = 30 kPa.
Associated flow case; cohesion = 25 kPa.
Slope stability analysis, Mohr-Coulomb plasticity
without tension cutoff
1.1.6–2
Abaqus Version 6.12 ID:
Printed on:
JOINTED ROCK SLOPE
mctc_slopestabil.inp
Slope stability analysis, Mohr-Coulomb plasticity with
tension cutoff
References
•
Barton, N., “Progressive Failure of Excavated Rock Slopes,” Stability of Rock Slopes, Proceedings
of the 13th Symposium on Rock Mechanics, Illinois, pp. 139–170, 1971.
•
Hoek, E., “Estimating the Stability of Excavated Slopes in Open Cast Mines,” Trans. Inst. Min.
and Metal., vol. 79, pp. 109–132, 1970.
•
Zienkiewicz, O. C., and G. N. Pande, “Time-Dependent Multilaminate Model of Rocks – A
Numerical Study of Deformation and Failure of Rock Masses,” International Journal for Numerical
and Analytical Methods in Geomechanics, vol. 1, pp. 219–247, 1977.
1.1.6–3
Abaqus Version 6.12 ID:
Printed on:
JOINTED ROCK SLOPE
O
90 Joint set 1
70 m
60
O
O
52.5 Joint set 2
Joint sets : βa
da
Bulk rock : βb
db
E = 28 GPa
ν = 0.2
K0 = 1/3
ρ = 2500 kg/m3
removed in
single stage
g = 9.81 m/s2
A
B
Figure 1.1.6–1
Jointed rock slope problem.
1.1.6–4
Abaqus Version 6.12 ID:
Printed on:
O
= 45
= variable
= 45
= 5600 kPa
O
JOINTED ROCK SLOPE
+1
Horizontal displacement (mm)
x x
x o
o
0
20
-1
x
o
40
o o
o
x
o
x
o
x
o
60
80
100
o
o
o
x
x
o Point A
120 da (kPa)
o
x Point B
x
x
x
-2
x
x
Associated
o
Nonassociated
x
x
-3
-4
Figure 1.1.6–2
Horizontal displacements with varying cohesion.
2
DISPLACEMENT MAGNIFICATION FACTOR =
3
3.000E+03
1
Figure 1.1.6–3
Deformed configuration (nonassociated flow).
1.1.6–5
Abaqus Version 6.12 ID:
Printed on:
JOINTED ROCK SLOPE
PEQC1
VALUE
-6.03E-07
+2.30E-05
+4.66E-05
+7.02E-05
+9.38E-05
+1.17E-04
+1.41E-04
+1.64E-04
2
3
1
Joint set 1 (vertical joints).
PEQC2
VALUE
-3.74E-06
+6.47E-06
+1.66E-05
+2.69E-05
+3.71E-05
+4.73E-05
+5.75E-05
+6.78E-05
2
3
1
Joint set 2 (inclined joints).
Figure 1.1.6–4
Contours of frictional slip magnitudes (nonassociated flow).
1.1.6–6
Abaqus Version 6.12 ID:
Printed on:
JOINTED ROCK SLOPE
S, Max. In−Plane Principal
(Avg: 75%)
+2.790e+01
−8.444e+01
−1.968e+02
−3.091e+02
−4.215e+02
−5.338e+02
−6.462e+02
−7.585e+02
−8.709e+02
−9.832e+02
−1.096e+03
−1.208e+03
−1.320e+03
Figure 1.1.6–5
Maximum principal stress without tension cutoff.
S, Max. In−Plane Principal
(Avg: 75%)
+1.069e+01
−1.002e+02
−2.111e+02
−3.220e+02
−4.329e+02
−5.438e+02
−6.547e+02
−7.656e+02
−8.765e+02
−9.874e+02
−1.098e+03
−1.209e+03
−1.320e+03
Figure 1.1.6–6
Maximum principal stress with tension cutoff.
1.1.6–7
Abaqus Version 6.12 ID:
Printed on:
NOTCHED BEAM UNDER CYCLIC LOADING
1.1.7
NOTCHED BEAM UNDER CYCLIC LOADING
Product: Abaqus/Standard
This example illustrates the use of the nonlinear isotropic/kinematic hardening material model to simulate the
response of a notched beam under cyclic loading. The model has two features to simulate plastic hardening in
cyclic loading conditions: the center of the yield surface moves in stress space (kinematic hardening behavior),
and the size of the yield surface evolves with inelastic deformation (isotropic hardening behavior). This
combination of kinematic and isotropic hardening components is introduced to model the Bauschinger effect
and other phenomena such as plastic shakedown, ratchetting, and relaxation of the mean stress.
The component investigated in this example is a notched beam subjected to a cyclic 4-point bending load.
The results are compared with the finite element results published by Benallal et al. (1988) and Doghri (1993).
No experimental data are available.
Geometry and model
The geometry and mesh are shown in Figure 1.1.7–1. Figure 1.1.7–2 shows the discretization in the
vicinity of the notch, which is the region of interest in this analysis. Only one-half of the beam is modeled
since the geometry and loading are symmetric with respect to the x= 0 plane. All dimensions are given in
millimeters. The beam is 1 mm thick and is modeled with plane strain, second-order, reduced-integration
elements (type CPE8R). The mesh is chosen to be similar to the mesh used by Doghri (1993). No mesh
convergence studies have been performed.
Material
The material properties reported by Doghri (1993) for a low-carbon (AISI 1010), rolled steel are used in
this example.
A Young’s modulus of E= 210 GPa and a Poisson’s ratio of = 0.3 define the elastic response of
the material. The initial yield stress is
= 200 MPa.
The nonlinear evolution of the center of the yield surface is defined by the equation
where
is the backstress,
is the size of the yield surface (size of the elastic range),
is the
equivalent plastic strain, and C = 25.5 GPa and = 81 are the material parameters that define the
initial hardening modulus and the rate at which the hardening modulus decreases with increasing plastic
strain, respectively. The quantity
257 MPa defines the limiting value of the equivalent
backstress
; further hardening is possible only through the change in the size of the
yield surface (isotropic hardening).
The isotropic hardening behavior of this material is modeled with the exponential law
1.1.7–1
Abaqus Version 6.12 ID:
Printed on:
NOTCHED BEAM UNDER CYCLIC LOADING
where
is the size of the yield surface (size of the elastic range),
= 2000 MPa is the maximum
increase in the elastic range, and b = 0.26 defines the rate at which the maximum size is reached as plastic
straining develops.
The material used for this simulation is cold rolled. This work hardened state is represented by
specifying an initial equivalent plastic strain
= 0.43 (so that = 411 MPa) and an initial backstress
tensor
Loading and boundary conditions
The beam is subjected to a 4-point bending load. Since only half of the beam is modeled, the model
contains one concentrated load at a distance of 26 mm from the symmetry plane (see Figure 1.1.7–1).
The pivot point is 42 mm from the symmetry plane. The simulation runs 3 1/2 cycles over 7 time units.
In each cycle the load is ramped from zero to 675 N and back to zero. An amplitude curve is used to
describe the loading and unloading. The increment size is restricted to a maximum of 0.125 to force
Abaqus to follow the prescribed loading/unloading pattern closely.
Results and discussion
Figure 1.1.7–3 shows the final deformed shape of the beam after the 3 1/2 cycles of load; the final load
on the beam is 675 N.
The deformation is most severe near the root of the notch. The results reported in Figure 1.1.7–4
and Figure 1.1.7–5 are measured in this area (element 166, integration point 3). Figure 1.1.7–4 shows the
time evolution of stress versus strain. Several important effects are predicted using this material model.
First, the onset of yield occurs at a lower absolute stress level during the first unloading than during the
first loading, which is the Bauschinger effect. Second, the stress-strain cycles tend to shift and stabilize
so that the mean stress decreases from cycle to cycle, tending toward zero. This behavior is referred to
as the relaxation of the mean stress and is most pronounced in uniaxial cyclic tests in which the strain is
prescribed between unsymmetric strain values. Third, the yield surface shifts along the strain axis with
cycling, whereas the shape of the stress-strain curve tends to remain similar from one cycle to the next.
This behavior is known as ratchetting and is most pronounced in uniaxial cyclic tests in which the stress is
prescribed between unsymmetric stress values. Finally, the hardening behavior during the first half-cycle
is very flat relative to the hardening curves of the other cycles, which is typical of work hardened metals
whose initial hardened state is a result of a large monotonic plastic deformation caused by a forming
process such as rolling. The low hardening modulus is the result of the initial conditions on backstress,
which places the center of the yield surface at a distance of
228 MPa away from
the origin of stress space. Since this distance is close to the maximum possible distance (257 MPa), most
of the hardening during the first cycle is isotropic.
1.1.7–2
Abaqus Version 6.12 ID:
Printed on:
NOTCHED BEAM UNDER CYCLIC LOADING
These phenomena are modeled in this example primarily by the nonlinear evolution of the
backstress, since the rate of isotropic hardening is very small. This behavior can be verified by
conducting an analysis in which the elastic domain remains fixed throughout the analysis.
Figure 1.1.7–5 shows the evolution of the direct components of the deviatoric part of the backstress
tensor. The backstress components evolve most during the first cycle as the Bauschinger effect
overcomes the initial hardening configuration. Only the deviatoric components of the backstress are
shown so that the results obtained using Abaqus can be compared to those reported by Doghri (1993).
Since Abaqus uses an extension of the Ziegler evolution law, a backstress tensor with nonzero pressure
is produced, whereas the backstress tensor produced with the law used by Doghri (which is an extension
of the linear Prager law) is deviatoric. Since the plasticity model considers only the deviatoric part of
the backstress, this difference in law does not affect the other solution variables.
The results shown in Figure 1.1.7–4 and Figure 1.1.7–5 agree well with the results reported by
Doghri (1993).
Input files
cyclicnotchedbeam.inp
cyclicnotchedbeam_mesh.inp
Input data.
Element and node data.
References
•
Benallal, A., R. Billardon, and I. Doghri, “An Integration Algorithm and the Corresponding
Consistent Tangent Operator for Fully Coupled Elastoplastic and Damage Equations,”
Communications in Applied Numerical Methods, vol. 4, pp. 731–740, 1988.
•
Doghri, I., “Fully Implicit Integration and Consistent Tangent Modulus in Elasto-Plasticity,”
International Journal for Numerical Methods in Engineering, vol. 36, pp. 3915–3932, 1993.
1.1.7–3
Abaqus Version 6.12 ID:
Printed on:
NOTCHED BEAM UNDER CYCLIC LOADING
R60
;;
;;
;;
;;
0.33
2.48
9.85
2
y
z
3
8
P
10.2
6
26
1
10
52
x
Figure 1.1.7–1
Undeformed mesh (dimensions in mm).
1.64
30o
2.48
;
;
;
;
R0.4
2
y3
z
1
x
Figure 1.1.7–2
Magnified view of the root of the notch.
1.1.7–4
Abaqus Version 6.12 ID:
Printed on:
NOTCHED BEAM UNDER CYCLIC LOADING
2
3
1
Figure 1.1.7–3 Deformed mesh at the conclusion of the
simulation. Displacement magnification factor is 3.
ABAQUS
Doghri
Figure 1.1.7–4
Evolution of stress versus strain in the vicinity of the root of the notch.
1.1.7–5
Abaqus Version 6.12 ID:
Printed on:
NOTCHED BEAM UNDER CYCLIC LOADING
ABAQUS alpha11
alpha22
alpha33
Doghri alpha11
alpha22
alpha33
Figure 1.1.7–5 Evolution of the diagonal components of
the deviatoric part of the backstress tensor.
1.1.7–6
Abaqus Version 6.12 ID:
Printed on:
UNIAXIAL RATCHETTING UNDER TENSION AND COMPRESSION
1.1.8
UNIAXIAL RATCHETTING UNDER TENSION AND COMPRESSION
Product: Abaqus/Standard
Objectives
This example demonstrates the following Abaqus features and techniques:
•
using the nonlinear isotropic/kinematic hardening model to predict deformation in a specimen
subjected to monotonic and cyclic loading; and
•
modeling the effect of ratchetting (accumulation of plastic strain under a cyclic load).
Application description
Preventing ratchetting is very important in the design of components subject to cyclic loading in the
inelastic domain. The amount of plastic strain can accumulate continuously with an increasing number
of cycles and may eventually cause material failure. Therefore, many cyclic plastic models have been
developed with the goal of modeling ratchetting correctly. In this example we show that the combined
isotropic/kinematic hardening model available in Abaqus can predict ratchetting and that the results
obtained using this model correlate very well with experimental results.
This example considers two loading conditions: monotonic deformation and uniaxial cyclic tension
and compression.
Geometry
The specimen studied is shown in Figure 1.1.8–1. All dimensions are specified in the figure. For the
experiments (Portier et al., 2000) the specimens were obtained from a tube with an outer diameter of
130 mm and a wall thickness of 28 mm. The specimens were heat treated to ensure the initial isotropy
of the material.
Materials
The specimen is made of austenitic type 316 stainless steel. The material mechanical properties are listed
in Table 1.1.8–1. A detailed description of the calibration of parameters is given in “Material parameters
determination” below.
Boundary conditions and loading
The specimen is constrained at the bottom surface in the longitudinal direction, and a load is applied to
the top surface.
1.1.8–1
Abaqus Version 6.12 ID:
Printed on:
UNIAXIAL RATCHETTING UNDER TENSION AND COMPRESSION
Abaqus modeling approaches and simulation techniques
In this example deformations of a specimen subject to monotonic and cyclic loads are studied. In
both cases static analyses are performed. Taking advantage of the axial symmetry of the specimen,
axisymmetric elements are used.
Summary of analysis cases
Case 1
Static analysis of a specimen subject to a monotonic load.
Case 2
Static analysis of a specimen subject to an unsymmetric cyclic load.
Case 1 Monotonic load
The experimental monotonic load data are used to calibrate the kinematic hardening model. The purpose
of this case is to verify that the simulation results agree with the experimental results and to compare the
accuracy of the results obtained using a model with one backstress and a model with two backstresses.
Analysis types
A static stress analysis is performed.
Mesh design
The specimen is meshed with CAX4R and CAX3 elements. The mesh is shown in Figure 1.1.8–2.
Material model
The combined isotropic/kinematic hardening model is used to model the response of the material. This
material model requires that the elastic parameters (Young’s modulus and Poisson’s ratio), the initial
yield stress, the isotropic hardening parameters, and the kinematic hardening parameters are specified.
Material parameters determination
The elastic parameters, the initial yield stress, and the isotropic hardening parameters are assumed to be
equal to those reported in Portier et al. (2000) for the Ohno and Wang model. The kinematic hardening
component is defined by specifying half-cycle test data, where the data are obtained by digitizing the
results reported by Portier et al. The values of all the parameters, including the kinematic hardening
parameters obtained from the test data, are presented in Table 1.1.8–1.
Boundary conditions
The specimen is fixed in the longitudinal direction at the bottom surface.
Loading
A displacement of 0.45 mm is applied to the top surface.
1.1.8–2
Abaqus Version 6.12 ID:
Printed on:
UNIAXIAL RATCHETTING UNDER TENSION AND COMPRESSION
Results and discussion
The simulation and experimental results are presented graphically in Figure 1.1.8–3. The strains and
stresses are computed by averaging the values in the elements lying at the center of the specimen. The
experimental curve shows three distinct regions: a linear elastic region, an elastic-plastic transition zone,
and an almost linear response region at large strain values. The model with two backstresses captures
this response very well. One of the backstresses has a large value of the parameter , which captures
the shape of the transition zone correctly, while the second backstress with a relatively small value of
captures the nearly linear response at large strains correctly. The parameter in the model with one
backstress has a relatively large value, which results in large discrepancies between the experimental and
predicted responses at large strains.
Case 2 Uniaxial tension and compression cyclic analysis
The objective of this case is to show that the combined isotropic/kinematic hardening model can be used
to predict the response of a material subject to a cyclic load accurately and, in particular, to predict the
ratchetting effect. In addition, the results obtained using a model with one backstress are compared to
those obtained using a model with two backstresses.
Analysis types
A static stress analysis is performed.
Mesh design
The mesh is the same as in Case 1.
Material model
The material model is the same as in Case 1.
Boundary conditions
The specimen is fixed in the longitudinal direction at the bottom surface.
Loading
A cyclic load of
MPa and
This load produces an approximate cyclic load of
part of the specimen.
MPa is applied to the top surface of the specimen.
MPa and
MPa at the center
Results and discussion
The simulation results obtained for the model with one backstress and the model with two backstresses,
together with the experimental results, are depicted in Figure 1.1.8–4. The strains were computed by
averaging the strains in the elements lying at the center of the specimen. The figure shows that both
simulation models are capable of predicting ratchetting. It also shows that the results obtained using the
model with two backstresses correlate better with the experimental results.
1.1.8–3
Abaqus Version 6.12 ID:
Printed on:
UNIAXIAL RATCHETTING UNDER TENSION AND COMPRESSION
Discussion of results and comparison of cases
The results of the analyses show that the combined isotropic/kinematic hardening model can be used to
predict the ratchetting effect accurately. In addition, a substantial improvement in the agreement between
simulation and experimental results can be achieved by using a model with multiple backstresses instead
of a model with a single backstress. The former model predicts more accurately the shape of the stressstrain curve in the monotonic loading case and the ratchetting strain in a cyclic loading case. In this
example increasing the number of backstresses from one to two produced a substantial improvement in
the results. However, further increasing the number of backstresses does not significantly improve the
results.
Files
Case 1 Monotonic
ratch_axi_monotonic_1.inp
ratch_axi_monotonic_2.inp
Input file to analyze a specimen subjected to a monotonic
load using the model with one backstress.
Input file to analyze a specimen subjected to a monotonic
load using the model with two backstresses.
Case 2 Cyclic
ratch_axi_unsymcyclic_1.inp
ratch_axi_unsymcyclic_2.inp
Input file to analyze a specimen subjected to a cyclic load
using the model with one backstress.
Input file to analyze a specimen subjected to a cyclic load
using the model with two backstresses.
References
Abaqus Analysis User’s Manual
•
“Models for metals subjected to cyclic loading,” Section 23.2.2 of the Abaqus Analysis User’s
Manual
Abaqus Keywords Reference Manual
•
•
*CYCLIC HARDENING
*PLASTIC
•
Portier, L., S. Calloch, D. Marquis, and P. Geyer, “Ratchetting Under Tension-Torsion Loadings:
Experiments and Modelling,” International Journal of Plasticity, vol. 16, pp. 303–335, 2000.
Other
1.1.8–4
Abaqus Version 6.12 ID:
Printed on:
UNIAXIAL RATCHETTING UNDER TENSION AND COMPRESSION
Table 1.1.8–1
Mechanical properties for 316 steel.
Material properties:
Young’s modulus
192.0 GPa
Poisson’s ratio
0.3
Initial yield stress
120.0 MPa
Isotropic hardening parameters:
120.0 MPa
Q∞
b
13.2
Kinematic hardening parameters:
Model with one backstress
218.5 GPa
C
γ
1956.6
Model with two backstresses
2.067 GPa
C1
γ1
44.7
246.2 GPa
C2
γ2
2551.4
8 mm
8 mm
R 60 mm
15.4 mm
6 mm
12 mm
15.4 mm
10 mm
8 mm
8 mm
18 mm
Figure 1.1.8–1
Geometry and size of the specimen.
1.1.8–5
Abaqus Version 6.12 ID:
Printed on:
UNIAXIAL RATCHETTING UNDER TENSION AND COMPRESSION
Figure 1.1.8–2
Finite element mesh of the specimen.
1.1.8–6
Abaqus Version 6.12 ID:
Printed on:
UNIAXIAL RATCHETTING UNDER TENSION AND COMPRESSION
300.
axial stress, (MPa)
250.
200.
150.
experiment
simulation (one backstress)
simulation (two backstresses)
100.
50.
0.
0.0
0.5
1.0
1.5
2.0
axial strain, (%)
Figure 1.1.8–3
Stress-strain curves for monotonic tensile loading.
maximum axial strain, (%)
2.0
1.5
1.0
experiment
simulation (one backstress)
simulation (two backstresses)
0.5
0.0
0.
20.
40.
60.
80.
100.
cycle
Figure 1.1.8–4
Maximum axial strain versus number of cycles.
1.1.8–7
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
1.1.9
HYDROSTATIC FLUID ELEMENTS: MODELING AN AIRSPRING
Products: Abaqus/Standard
Abaqus/Explicit
Airsprings are rubber or fabric actuators that support and contain a column of compressed air. They are
used as pneumatic actuators and vibration isolators. Unlike conventional pneumatic cylinders, airsprings
have no pistons, rods, or dynamic seals. This makes them better suited to handle off-center loading and
shock. In addition, airsprings are considerably more flexible than other types of isolators: the airspring’s
inflation pressure can be changed to compensate for different loads or heights without compromising isolation
efficiency. Dils (1992) provides a brief discussion of various practical uses of airsprings.
In this section two examples of the analysis of a cord-reinforced rubber airspring are discussed. Static
analyses are performed in Abaqus/Standard, and quasi-static analyses are performed in Abaqus/Explicit. The
first example is a three-dimensional, half-symmetry model that uses finite-strain shell elements to model the
rubber spring and rebar to model the multi-ply steel reinforcements in the rubber membrane. In addition,
a three-dimensional, element-based rigid surface is used to define the contact between the airspring and the
lateral metal bead. The cord-reinforced rubber membrane is modeled using a hyperelastic material model
with steel rebar.
The second example is a two-dimensional, axisymmetric version of the first model that uses composite
axisymmetric, finite-strain shell elements to model the cord-reinforced rubber spring and an axisymmetric,
element-based rigid surface in the contact definition. This model uses a composite shell section consisting of
a thin orthotropic elastic layer sandwiched between two hyperelastic layers. The orthotropic layer captures
the mechanical properties of the rebar definition used in the three-dimensional model.
The orthotropic material constants have been obtained by performing simple tests on a typical element
of the three-dimensional model. The three-dimensional shell model uses rebar with material properties that
are initially identical to the properties of the composite shell section in the axisymmetric shell model.
For comparison, Abaqus/Standard input files that use finite-strain membrane elements instead of finitestrain shell elements to model the cord-reinforced rubber spring are also included for both the axisymmetric
and three-dimensional models.
In all analyses the airspring cavity is modeled using the surface-based fluid cavity capability (see
“Surface-based fluid cavities: overview,” Section 11.5.1 of the Abaqus Analysis User’s Manual) and air
inside the cavity is modeled as a compressible or “pneumatic” fluid satisfying the ideal gas law.
Geometry and model
The dimensions of the airspring have been inferred from the paper by Fursdon (1990). This airspring,
shown in Figure 1.1.9–1, is fairly large and is used in secondary suspension systems on railway bogies.
However, the shape of the airspring is typical of airsprings used in other applications. The airspring’s
cross-section is shown in Figure 1.1.9–2. The airspring is toroidal in shape, with an inner radius of
200 mm and an outer radius of 400 mm. The airspring has been idealized in the model as consisting of
two circular, metal disks connected to each other via a rubber component. The lower disk has a radius of
200 mm, and the upper disk has a radius of 362.11 mm. The disks are initially coaxial and are 100 mm
1.1.9–1
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
apart. The rubber component is doubly curved and toroidal in shape. The rubber is constrained in the
radial direction by a circular bead 55 mm in radius that goes around the circumference of the upper disk.
The rubber “hose” in the half-symmetry, three-dimensional model is modeled with 550 S4R finitestrain shell elements. The mesh in the upper hemisphere of the hose is more refined than that in the lower
hemisphere, because the rubber membrane undergoes a reversal in curvature in the upper region as it
contours the circular bead attached to the upper disk. The circular bead is modeled using an axisymmetric,
discrete rigid surface. Contact with the rubber is enforced by defining a contact pair between this rigid
surface and a surface defined on the (deformable) shell mesh in the contacting region. The metal disks are
assumed to be rigid relative to the rubber component of the airspring. The lower metal disk is modeled
using boundary conditions, while the upper disk is modeled as part of the rigid surface. The meshes of
the rubber membrane and the rigid surface are shown in Figure 1.1.9–3.
The fluid cavity is modeled using the surface-based fluid cavity capability (see “Surface-based
fluid cavities: overview,” Section 11.5.1 of the Abaqus Analysis User’s Manual). To define the
cavity completely and to ensure proper calculation of its volume, surface elements are defined in the
three-dimensional models along the bottom and top rigid disk boundaries of the cavity, even though
no displacement elements exist along those surfaces. Since Abaqus does not provide two-dimensional
surface elements, the rigid disk boundaries are modeled with structural elements instead of surface
elements in the axisymmetric models. The cavity reference node 50000 has a single degree of freedom
representing the pressure inside the cavity. Because of symmetry only half of the cavity boundary has
been modeled. The cavity reference node has been placed on the model’s symmetry plane, y = 0, to
assure proper calculation of the cavity volume. Figure 1.1.9–4 shows the mesh of the airspring’s cavity.
To facilitate comparisons, the two-dimensional axisymmetric model uses the same cross-sectional
mesh refinement as the 180° model. The rubber component is modeled with 25 SAX1 shell elements.
The circular bead is modeled with an element-based rigid surface constructed of RAX2 rigid elements.
Contact with the hose is enforced by defining a contact pair between this rigid surface and a surface
defined on the (deformable) shell mesh in the contacting region. Once again, the lower rigid metal disk
is modeled by boundary conditions, and the upper rigid metal disk is modeled as part of the rigid body.
The mesh of the rubber membrane and the contact master surface is shown in Figure 1.1.9–5, and the
mesh of the cavity is shown in Figure 1.1.9–6. For the membrane model the SAX1 elements are replaced
with either MAX1 elements or MGAX1 elements.
Symmetry boundary conditions and initial shell curvature
Symmetry has been exploited in the three-dimensional airspring model, and the plane y = 0 has been
made a plane of symmetry. Since S4R shell elements are true curved shell elements, accurate definition
of the initial curvature of the surface being modeled is required, especially on the plane of symmetry.
If the user does not provide this information by specifying the normal to the surface at the shell nodes,
Abaqus will estimate the normal direction based on the coordinates of the surrounding nodes on the shell.
Normals computed in this fashion will be inaccurate on the symmetry plane: they will have out-of-plane
components, which will lead to convergence difficulties in Abaqus/Standard and inaccurate results. To
avoid these difficulties, direction cosines have been specified for all shell nodes in the model.
1.1.9–2
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
Material properties
The walls of an airspring’s rubber component are made from plies of symmetrically placed, positively
and negatively oriented reinforcement cords. The walls of an actual component are made of several
such layers. However, for the purposes of the three-dimensional example problem being considered, the
airspring’s wall is taken to be a rubber matrix with a single 6-mm-thick symmetric layer of positively and
negatively oriented cords. The cords are modeled by uniformly spaced skew rebar in the shell elements.
The rebar are assumed to be made of steel. The rubber is modeled as an incompressible Mooney-Rivlin
(hyperelastic) material with
= 3.2 MPa and
= 0.8 MPa, and the steel is modeled as a linear elastic
material with E = 210.0 GPa and = 0.3.
Skew rebar orientations in shell elements are defined by giving the angle between the local 1-axis
and the rebar. The default local 1-direction is the projection of the global x-axis onto the shell surface
(see “Conventions,” Section 1.2.2 of the Abaqus Analysis User’s Manual). It is for this reason, and to
make the rebar definition uniform for all elements, that the axis of revolution of the airspring model has
been chosen to be the global x-axis. Two rebar layers, PLSBAR and MNSBAR, have been defined with
orientation angles of 18° and −18°, respectively. The cross-sectional area of the rebar is 1 mm2 , and they
are spaced every 3.5 mm in the shell surface.
The above rebar specification is simplified and somewhat unrealistic. The reinforced plies used in
the manufacture of the airspring are located in an initially cylindrical tube with uniform rebar angles.
However, the transformation of these layers from a cylindrical geometry to a toroidal one gives the
airspring a variable rebar angle and rebar spacing that is dependent on the radius from the axis of
revolution of the torus and on the initial rebar angle (see Fursdon, 1990). Hence, a more realistic
simulation would require different rebar definitions in each ring of elements in the airspring model.
In the axisymmetric shell model the airspring walls are modeled by a three-layer composite shell
section. The two outer layers are each 2.5 mm thick and made up of the same Mooney-Rivlin material
that is used in the 180° model. The middle “rebar” layer is 1 mm thick and is made up of an orthotropic
elastic material that captures the mechanical behavior of the positively and negatively oriented rebar
definition used in the three-dimensional airspring model.
The plane stress orthotropic engineering constants are obtained by looking at the response of a
typical element in the three-dimensional model (element 14) subjected to uniaxial extensions along the
local 1- and 2-directions. Using a shell thickness of 1 mm, the in-plane states of stress and strain resulting
from these two tests are
Test
1-direction
2-direction
−2
1.00 × 10
−1.05 × 10−3
−2
−8.75 × 10
1.00 × 10−2
(MPa)
2.48 × 101
−5.96 × 10−6
(MPa)
−2.41 × 10−5
2.86 × 10−1
For a plane-stress orthotropic material the in-plane stress and strain components are related to each
other as follows:
1.1.9–3
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
where , ,
, and
are engineering constants. Solving for these constants using the above stressstrain relation and the results of the two uniaxial tests yields
The remaining required engineering constants—
,
, and
—play no role in the rebar layer
definition. Consequently, they have been arbitrarily set to be equal to the shear modulus of the rubber,
which is given by
.
For the axisymmetric membrane model the bulk material is chosen to have the same material
properties (Mooney-Rivlin hyperelastic) as those used in the 180° model and the axisymmetric shell
model. The rebar parameters and material properties are chosen such that they capture the initial
material properties of the sandwiched steel layer in the axisymmetric shell model. The principal
material directions do not rotate in the axisymmetric shell model (they are the default element basis
directions—the meridional and the hoop directions, respectively). However, they do rotate with finite
strain in the axisymmetric membrane model as a result of the use of rebar. Initial stresses are applied
to the rebar in the axisymmetric membrane model.
In all analyses the air inside the airspring cavity has been modeled as an ideal gas with molecular
weight of 0.044 kg and molar heat capacity of 30 J/kg °K.
Loading
In the Abaqus/Standard model the airspring is first pressurized to 506.6 × 103 kPa (5 atms) while holding
the upper disk fixed. This pressure is applied by prescribing boundary degree of freedom 8 at the cavity
reference node. In this case the air volume is adjusted automatically to fill the cavity.
In the next step the prescribed boundary condition on the pressure degree of freedom is removed,
thus sealing the cavity with the current air volume. In addition, during this step the boundary condition
on the vertical displacement degree of freedom of the rigid body reference node is removed, and in its
place a downward load of 150 kN is applied.
The next step is a static linear perturbation procedure. In the axisymmetric model two load cases
are considered: one tests the axial stiffness of the airspring with the cavity pressure allowed to vary
(closed cavity conditions) and the other tests its axial stiffness with the cavity pressure fixed. The linear
perturbation step in the three-dimensional analysis contains three load cases, all under variable cavity
pressure (closed cavity) conditions: the first tests the axial stiffness of the airspring, the second tests its
lateral stiffness, and the third tests its rotational stiffness for rocking motion in the symmetry plane.
The axisymmetric analysis concludes with a general step in which the airspring is compressed by
increasing the downward load to 240.0 kN. The three-dimensional analysis concludes with a general step
in which the airspring is subjected to a lateral displacement of 20 mm.
1.1.9–4
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
The loading for the Abaqus/Explicit model is similar to that for the Abaqus/Standard model, except
for the linear perturbation steps. The airspring is first pressurized to 506.6 × 103 kPa (5 atms) while
holding the upper disk fixed. In the next step the boundary condition on the pressure degree of freedom
is removed, thereby sealing the cavity with the current air volume. In addition, for both the axisymmetric
and three-dimensional models, the boundary condition on the vertical displacement degree of freedom
of the rigid body reference node is modified, so that a downward displacement is applied. This is in
contrast to the Abaqus/Standard axisymmetric analysis, where a force was applied. Since the airspring
is pressurized, a sudden change in applied force would cause a sudden change in acceleration and induce
a low frequency transient response. As a result, the simulation time required for the transient effects to
diminish would be very long. Hence, we apply a displacement instead of a force. In the axisymmetric
analysis the downward displacement is chosen to be 75 mm, so that the increase in pressure is close to
the increase seen in Step 4 of the Abaqus/Standard axisymmetric analysis. The downward displacement
in the three-dimensional Abaqus/Explicit analysis is set to 20 mm so that the results from this step may
be compared with those from Step 4 of the Abaqus/Standard three-dimensional analysis.
Results and discussion
Figure 1.1.9–7 and Figure 1.1.9–8 show displaced shape plots of the axisymmetric shell model at the
end of the pressurization step. It is of interest to compare the results from this model with those from the
180° model to validate the material model that was used for the rebar reinforcements in the axisymmetric
model. A close look at the nodal displacements reveals that the deformation is practically identical
for the axisymmetric and three-dimensional models. The results are also virtually identical between
corresponding Abaqus/Standard and Abaqus/Explicit models. Moreover, the axial reaction force at the
rigid body reference node is 156 kN for the axisymmetric model and 155 kN for the 180° model (after
multiplication by a factor of 2). The cavity volume predicted by the axisymmetric model is 8.22 × 10−2 m3
versus 8.34 × 10−2 m3 for the 180° model (again, after multiplication by a factor of 2).
Linearized stiffnesses for the airspring are obtained from the Abaqus/Standard linear perturbation
load cases. The stiffness is computed by dividing the relevant reaction force at the rigid body reference
node by the appropriate displacement. For the axisymmetric model the airspring’s axial stiffness under
variable cavity pressure conditions is 826 kN/m; its axial stiffness under fixed cavity pressure conditions
is 134 kN/m. The difference in axial stiffness between these two cases (a factor of 6) is the result of
differences in cavity pressure experienced during axial compression. Under variable cavity pressure
conditions, a fixed mass of fluid (air) is contained in a cavity whose volume is decreasing; thus, the
cavity pressure increases. Under fixed cavity pressure conditions, the pressure is prescribed as a constant
value for the load case. For the 180° model the predicted stiffnesses under variable cavity pressure are
as follows: the axial stiffness is 821 kN/m, the lateral stiffness is 3.31 MN/m, and the rotational stiffness
is 273 kN/m.
Figure 1.1.9–9 shows a series of displaced shape plots associated with the compression of the
axisymmetric Abaqus/Standard airspring model during Step 4. For comparison, Figure 1.1.9–10 shows
a series of displaced shape plots associated with the compression of the axisymmetric Abaqus/Explicit
model during Step 2. Figure 1.1.9–11 shows the corresponding load-deflection curves. Although the
displacement of the rigid body in the Abaqus/Explicit analysis was applied over a short time period
(which caused significant inertial effects in the model), there is still good agreement between the
1.1.9–5
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
slope of the load-displacement curves from the two analyses. The response of the airspring is only
slightly nonlinear; consequently, there is good agreement between the axial stiffness obtained with
the linear perturbation load case and that obtained from the slope of the load-displacement curve.
Figure 1.1.9–12 shows a plot of cavity pressure versus the downward displacement of the rigid body in
Step 4 of the Abaqus/Standard analysis and Step 2 of the Abaqus/Explicit analysis. The gauge pressure
in the cavity increases by approximately 50% during this step. This pressure increase substantially
affects the deformation of the airspring structure and cannot be specified as an externally applied load
during the step since it is an unknown quantity. Figure 1.1.9–13 shows a plot of cavity volume versus
the downward displacement of the rigid body in Step 4 of the Abaqus/Standard analysis and Step 2
of the Abaqus/Explicit analysis. The cavity pressure and the cavity volume results from the static
Abaqus/Standard analysis and the quasi-static Abaqus/Explicit analysis are virtually identical. The
corresponding results from the axisymmetric membrane model (not shown) are also in good agreement
with the above results.
Figure 1.1.9–14 shows the displaced shape of the 180° Abaqus/Standard model at the end of
Step 4, in which a lateral displacement was applied to the airspring. Figure 1.1.9–15 shows the
corresponding displaced shape of the 180° model at the end of Step 2 of the Abaqus/Explicit analysis.
Figure 1.1.9–16 shows a plot of the load-displacement curves obtained from these steps. Although
there is a certain amount of noise that results from the contact conditions and the coarseness of the
mesh, the load-deflection curve shows good agreement between the analyses performed quasi-statically
in Abaqus/Explicit and statically in Abaqus/Standard. The Abaqus/Explicit analysis was run in double
precision to eliminate some of the noise in the load-displacement curve.
Input files
hydrofluidairspring_s4r.inp
hydrofluidairspring_s4r_surf.inp
hydrofluidairspring_sax1.inp
hydrofluidairspring_sax1_surf.inp
airspring_exp_s4r_surfcav.inp
airspring_exp_sax1_surfcav.inp
hydrofluidairspring_m3d4.inp
hydrofluidairspring_m3d4_surf.inp
hydrofluidairspring_max1.inp
Three-dimensional Abaqus/Standard model using shell
elements.
Three-dimensional Abaqus/Standard model using shell
elements with surface-to-surface contact.
Axisymmetric Abaqus/Standard model using shell
elements.
Axisymmetric Abaqus/Standard model using shell
elements with surface-to-surface contact.
Three-dimensional Abaqus/Explicit model using shell
elements.
Axisymmetric Abaqus/Explicit model using shell
elements.
Three-dimensional Abaqus/Standard model using
membrane elements.
Three-dimensional Abaqus/Standard model using
membrane elements with surface-to-surface contact.
Axisymmetric Abaqus/Standard analysis using rebar
reinforced membrane elements.
1.1.9–6
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
hydrofluidairspring_mgax1.inp
airspring_s4r_gcont_surfcav.inp
Axisymmetric Abaqus/Standard analysis using rebar
reinforced membrane elements with twist.
Three-dimensional Abaqus/Explicit analysis using shell
elements and general contact.
References
•
•
Dils, M., “Air Springs vs. Air Cylinders,” Machine Design, May 7, 1992.
Fursdon, P. M. T., “Modelling a Cord Reinforced Component with ABAQUS,” 6th UK ABAQUS
User Group Conference Proceedings, 1990.
1.1.9–7
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
Figure 1.1.9–1
A cord-reinforced airspring.
CL
55 mm
100 mm
Airspring
Cavity
Rubber
component
Lower disk
200 mm
Circular bead
100 mm
6 mm
Figure 1.1.9–2
The airspring model cross-section.
1.1.9–8
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
1
2
3
Figure 1.1.9–3 180° model: mesh of the rubber membrane
and the contact master surface.
1
2
3
Figure 1.1.9–4
180° model: mesh of the airspring cavity.
1.1.9–9
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
2
3
1
Figure 1.1.9–5 Axisymmetric model: mesh of the rubber
membrane and the contact master surface.
2
3
1
Figure 1.1.9–6
Axisymmetric model: mesh of the airspring cavity.
1.1.9–10
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
2
3
Figure 1.1.9–7
1
Axisymmetric Abaqus/Standard model: deformed configuration at the end of Step 1.
2
3
Figure 1.1.9–8
1
Axisymmetric Abaqus/Explicit model: deformed configuration at the end of Step 1.
1.1.9–11
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
2
3
1
Figure 1.1.9–9 Axisymmetric Abaqus/Standard model: progressive
deformed configurations during Step 4.
2
3
1
Figure 1.1.9–10 Axisymmetric Abaqus/Explicit model: progressive
deformed configurations during Step 2.
1.1.9–12
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
Explicit
Standard
Figure 1.1.9–11
Load-displacement curves (axisymmetric models).
PCAV-exp
PCAV-std
Figure 1.1.9–12 Cavity pressure versus downward
displacement (axisymmetric models).
1.1.9–13
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
CVOL-exp
CVOL-std
Figure 1.1.9–13 Cavity volume versus downward
displacement (axisymmetric models).
1
2
Figure 1.1.9–14
3
180° Abaqus/Standard model: deformed configuration at the end of Step 4.
1.1.9–14
Abaqus Version 6.12 ID:
Printed on:
MODELING AN AIRSPRING
1
2
Figure 1.1.9–15
3
180° Abaqus/Explicit model: deformed configuration at the end of Step 2.
ABAQUS/Explicit
ABAQUS/Standard
Figure 1.1.9–16
Load-displacement curves for the 180° analyses.
1.1.9–15
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
1.1.10
SHELL-TO-SOLID SUBMODELING AND SHELL-TO-SOLID COUPLING OF A PIPE
JOINT
Products: Abaqus/Standard
Abaqus/Explicit
Abaqus/CAE
Submodeling is the technique used in Abaqus for analyzing a local part of a model with a refined mesh, based
on interpolation of the solution from an initial global model (usually with a coarser mesh) onto the nodes on
the appropriate parts of the boundary of the submodel. Shell-to-solid submodeling models a region with solid
elements, when the global model is made up of shell elements. This example uses the scaling parameter in
the submodel boundary condition to scale the values of prescribed boundary conditions for driven variables
without requiring the global model to be rerun.
Shell-to-solid coupling is a feature in Abaqus by which three-dimensional shell meshes can be coupled
automatically to three-dimensional solid meshes. Unlike shell-to-solid submodeling, which first performs a
global analysis on a shell model followed by a submodel analysis with a continuum model, the shell-to-solid
coupling model uses a single analysis, with solid and shell elements used in different regions.
Both shell-to-solid submodeling and shell-to-solid coupling provide cost-effective approaches to
model enhancement. The purpose of this example is to demonstrate both capabilities in Abaqus. The
analysis is tested as a static process in Abaqus/Standard and as a dynamic process in both Abaqus/Standard
and Abaqus/Explicit. To demonstrate the shell-to-solid submodeling capability, the problem is solved
quasi-statically in Abaqus/Explicit. The overall displacements are small, and to avoid noise-induced dynamic
effects, the quasi-static Abaqus/Explicit analysis is run in double precision.
In addition, an Abaqus Scripting Interface script is included that creates a shell global model using
Abaqus/CAE. The script then uses data from the output database created by the analysis of the global model
to drive a solid submodel. The script ends by displaying an overlay plot of the global model and the submodel
in the Visualization module.
Geometry and model
In this problem the joint between a pipe and a plate is analyzed. A pipe of radius 10 mm and thickness
0.75 mm is attached to a plate that is 10 mm long, 5 mm wide, and 1 mm thick. The pipe-plate intersection
has a fillet radius of 1 mm. Taking advantage of the symmetry of the problem, only half the assembly
is modeled. Both the pipe and the plate are assumed to be made of aluminum with E = 69 × 103 MPa,
= 0.3, and = 2740 kg/m3 .
The global model for the submodeling analysis is meshed with S4R elements as shown in
Figure 1.1.10–1. The fillet radius is not taken into consideration in the shell model. The static submodel
is meshed using three-dimensional C3D20R continuum elements (see Figure 1.1.10–2). A coarser
mesh using C3D8R elements is chosen for the dynamic tests. The shell-to-solid coupling model is
meshed with S4R shell elements and C3D20R continuum elements as shown in Figure 1.1.10–3. The
continuum meshes used in the static submodeling and shell-to-solid coupling analyses are identical.
The continuum meshes extend 10 mm along the pipe length, have a radius of 25 mm in the plane of
the plate, and use four layers through the thickness. The continuum meshes accurately model the fillet
radius at the joint. Hence, it is possible to calculate the stress concentration in the fillet. The problem
1.1.10–1
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
could be expanded by adding a ring of welded material to simulate a welded joint (for this case the
submodel would have to be meshed with new element layers representing the welded material at the
joint). The example could also be expanded by including plastic material behavior in the submodel
while using an elastic global model solution.
A reference static solution consisting entirely of C3D20R continuum elements is also included (see
Figure 1.1.10–4). The mesh of the reference solution in the vicinity of the joint is very similar to that
used in the submodeling and shell-to-solid coupling analyses.
The geometry and material properties of the Abaqus/Explicit shell-to-solid coupling model are
identical to the Abaqus/Standard models. The Abaqus/Explicit shell model is meshed with S4R elements,
and the continuum model is meshed with C3D10M elements.
Loading
The pipe is subjected to a concentrated load acting in the x-direction applied at the free end, representing
a shear load on the pipe. An edge-based surface is defined at the free edge of the pipe. This surface
is coupled to a reference node that is defined at the center of the pipe using a distributing coupling
constraint. The concentrated load is applied to the reference point. For the submodeling approach the
load magnitude is 10 N for the global analysis and 10 N and 20 N, respectively, in the two steps of the
submodel analysis (a scale factor of 2.0 is applied to the displacements of the driven nodes in the second
step of the submodel analysis). For the shell-to-solid coupling approach the load magnitude is 10 N
and 20 N, respectively, in the two steps, as in the submodel analysis. For the dynamic cases the load is
applied gradually over the entire step time by using a smooth-step amplitude curve.
Kinematic boundary conditions
The plate is clamped along all edges. In the solid submodel, kinematic conditions are interpolated from
the global model at two surfaces of the submodel: one lying within the pipe and the other within the plate.
The default center zone size, equal to 10% of the maximum shell thickness, is used. Thus, only one layer
of driven nodes lies within the center zone, and only these nodes have all three displacement components
driven by the global solution. For the remaining driven nodes only the displacement components parallel
to the global model midsurface are driven from the global model. Thus, a single row of nodes transmits
the transverse shear forces from the shell solution to the solid model.
Results and discussion
The loading and boundary conditions are such that the pipe is subjected to bending. The end of the
pipe that is attached to the plate leads to deformation of the plate itself (see Figure 1.1.10–5 and
Figure 1.1.10–6). From a design viewpoint the area of interest is the pipe-plate joint where the pipe is
bending the plate. Hence, this area is modeled with continuum elements to gain a better understanding
of the deformation and stress state.
Figure 1.1.10–7 shows the contours of the out-of-plane displacement component in the plate for
both the static submodel and the shell-to-solid coupling analyses. The submodel is in good agreement
with the displacement of the global shell model around the joint. The out-of-plane displacement for the
1.1.10–2
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
shell-to-solid coupling is slightly less than that for the submodel analysis but is in good agreement with
the reference solution shown in Figure 1.1.10–8.
The stress concentration in the fillet radius is obtained for the solid models. The maximum Mises
stresses at the integration points and nodes for the reference solution, submodel, and shell-to-solid
coupling analyses are shown in Table 1.1.10–1. As illustrated in Table 1.1.10–1 and Figure 1.1.10–9,
the Mises stress computed in the shell-to-solid coupling analysis agrees very well with the reference
solution. The continuity of displacements and the minimal distortion of the stress field at the
shell-to-solid interface indicates that the shell-to-solid coupling has been modeled accurately. The
difference in the maximum Mises stress between the submodel analysis and the shell-to-solid coupling
solution (see Figure 1.1.10–10) can be partially attributed to the fact that the global shell model is
more flexible than the shell-to-solid coupling model. The x-displacement at the distributing coupling
reference node for the global shell model due to the 10 N load is .605 mm compared to .513 mm for the
shell-to-solid coupling analysis and .512 mm for the reference solution. Thus, the static submodel mesh
is subjected to slightly higher deformation. If the global shell analysis is run with an x-displacement
boundary condition of .513 mm on the reference node instead of a concentrated load of 10 N, the
subsequent maximum nodal Mises stress in the submodel analysis drops to 80.2 MPa, which is in better
agreement with the reference solution. Figure 1.1.10–11 and Figure 1.1.10–12 show, respectively,
the comparison of the out-of-plane displacement component in the continuum-mesh plate and the
comparison of the Mises stress for the submodel with scaled boundary condition and the shell-to-solid
coupling model with scaled load. The submodel results are in good agreement with the shell-to-solid
coupling results.
The relatively large difference between the maximum Mises stresses at the integration points and
the nodes in the region of the fillet (as illustrated in Table 1.1.10–1) indicates that the mesh in the fillet
region is probably too coarse and should be refined. No such refinement was performed in this example.
Overall, the Abaqus/Explicit shell-to-solid coupling analysis is in good agreement with the
Abaqus/Standard shell-to-solid coupling results. The continuity of displacements and the minimal
distortion of the stress field at the shell-to-solid interface indicate that the shell-to-solid coupling has
been modeled accurately. The out-of-plane displacements of the plate predicted by Abaqus/Explicit
are very close to the Abaqus/Standard values. The maximum nodal Mises stress in the fillet region is
56 MPa, and the x-displacement at the coupling constraint reference node for the global shell model
due to the 10 N load is .423 mm. The Abaqus/Explicit analysis is solved quasi-statically by assigning
a nominal density of 500 kg/m3 to the pipe-plate material and ramping up the load over 12,000
increments. Closer approximation to the static limit, achieved by reducing the density of the pipe-plate
material to 50 kg/m3 , results in a maximum Mises stress of 87 MPa in the fillet region, which is very
close to the Abaqus/Standard result.
The results for the submodel dynamic cases agree well with the global results.
Both
Abaqus/Standard and Abaqus/Explicit submodels read the results of the same global Abaqus/Explicit
analysis. Good agreement is also found between the Abaqus/Explicit and Abaqus/Standard submodel
analyses.
1.1.10–3
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
Input files
Static and quasi-static input files
pipe_submodel_s4r_global.inp
pipe_submodel_s4r_global_n.inp
pipe_submodel_s4r_global_e.inp
pipe_submodel_c3d20r_sub_s4r.inp
pipe_submodel_c3d20r_sub_s4r_n.inp
pipe_submodel_c3d20r_sub_s4r_e.inp
pipe_submodel_s4_global.inp
pipe_submodel_s4_global_n.inp
pipe_submodel_s4_global_e.inp
pipe_submodel_c3d20r_sub_s4.inp
pipe_submodel_c3d20r_sub_s4_n.inp
pipe_submodel_c3d20r_sub_s4_e.inp
pipe_cae_c3d20rsub_s4.py
pipe_shell2solid_c3d20r_s4r.inp
pipe_shell2solid_c3d20r_s4r_n1.inp
pipe_shell2solid_c3d20r_s4r_n2.inp
pipe_shell2solid_c3d20r_s4r_n3.inp
pipe_shell2solid_c3d20r_s4r_e1.inp
pipe_shell2solid_c3d20r_s4r_e2.inp
pipe_shell2solid_c3d20r_s4r_e3.inp
pipe_shell2solid_c3d10_s4r.inp
pipe_shell2solid_c3d10_s4r_n1.inp
S4R global model.
Node definitions for the S4R global model.
Element definitions for the S4R global model.
C3D20R submodel that uses the S4R global model. The
scaling parameter is used in the second step.
Node definitions for the C3D20R submodel that uses the
S4R global model.
Element definitions for the C3D20R submodel that uses
the S4R global model.
S4 global model.
Node definitions for the S4 global model.
Element definitions for the S4 global model.
C3D20R submodel that uses the S4 global model.
Node definitions for the C3D20R submodel that uses the
S4 global model.
Element definitions for the C3D20R submodel that uses
the S4 global model.
Python script that creates an S4 global model and a
C3D20R submodel using Abaqus/CAE.
Shell-to-solid coupling model with C3D20R and S4R
elements. The load is scaled in the second step.
Node definitions for the shell-to-solid coupling model
with C3D20R and S4R elements.
Node definitions for the shell-to-solid coupling model
with C3D20R and S4R elements.
Node definitions for the shell-to-solid coupling model
with C3D20R and S4R elements.
Element definitions for the shell-to-solid coupling model
with C3D20R and S4R elements.
Element definitions for the shell-to-solid coupling model
with C3D20R and S4R elements.
Element definitions for the shell-to-solid coupling model
with C3D20R and S4R elements.
Shell-to-solid coupling model with C3D10 and S4R
elements.
Node definitions for the shell-to-solid coupling model
with C3D10 and S4R elements.
1.1.10–4
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
pipe_shell2solid_c3d10_s4r_n2.inp
pipe_shell2solid_c3d10_s4r_n3.inp
pipe_shell2solid_c3d10_s4r_e1.inp
pipe_shell2solid_c3d10_s4r_e2.inp
pipe_shell2solid_c3d10_s4r_e3.inp
pipe_shell2solidx_c3d10m_s4r.inp
pipe_shell2solidx_c3d10m_s4r_n1.inp
pipe_shell2solidx_c3d10m_s4r_n2.inp
pipe_shell2solidx_c3d10m_s4r_n3.inp
pipe_shell2solidx_c3d10m_s4r_e1.inp
pipe_shell2solidx_c3d10m_s4r_e2.inp
pipe_shell2solidx_c3d10m_s4r_e3.inp
pipe_c3d20r.inp
pipe_c3d20r_n.inp
pipe_c3d20r_e.inp
Node definitions for the shell-to-solid coupling model
with C3D10 and S4R elements.
Node definitions for the shell-to-solid coupling model
with C3D10 and S4R elements.
Element definitions for the shell-to-solid coupling model
with C3D10 and S4R elements.
Element definitions for the shell-to-solid coupling model
with C3D10 and S4R elements.
Element definitions for the shell-to-solid coupling model
with C3D10 and S4R elements.
Abaqus/Explicit shell-to-solid coupling model with
C3D10M and S4R elements.
Node definitions for the Abaqus/Explicit shell-to-solid
coupling model with C3D10M and S4R elements.
Node definitions for the Abaqus/Explicit shell-to-solid
coupling model with C3D10M and S4R elements.
Node definitions for the Abaqus/Explicit shell-to-solid
coupling model with C3D10M and S4R elements.
Element definitions for the Abaqus/Explicit shell-to-solid
coupling model with C3D10M and S4R elements.
Element definitions for the Abaqus/Explicit shell-to-solid
coupling model with C3D10M and S4R elements.
Element definitions for the Abaqus/Explicit shell-to-solid
coupling model with C3D10M and S4R elements.
Reference model with C3D20R elements.
Node definitions for the reference model with C3D20R
elements.
Element definitions for the reference model with C3D20R
elements.
Dynamic input files
pipe_submodelx_s4r_global.inp
pipe_submodelx_s4r_global_n.inp
pipe_submodelx_s4r_global_e.inp
pipe_submodelx_c3d8r_sub_s4r.inp
pipe_submodelx_c3d8r_sub_s4r_n.inp
pipe_submodelx_c3d8r_sub_s4r_e.inp
pipe_submodel_c3d8r_sub_s4r.inp
Abaqus/Explicit S4R global model.
Node definitions for the Abaqus/Explicit S4R global
model.
Element definitions for the Abaqus/Explicit S4R global
model.
Abaqus/Explicit C3D8R submodel.
Node definitions for the Abaqus/Explicit C3D8R
submodel.
Element definitions for the Abaqus/Explicit C3D8R
submodel.
Abaqus/Standard C3D8R submodel.
1.1.10–5
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
pipe_submodel_c3d8r_sub_s4r_n.inp
pipe_submodel_c3d8r_sub_s4r_e.inp
Table 1.1.10–1
Node definitions for the Abaqus/Standard C3D8R
submodel.
Element definitions for the Abaqus/Standard C3D8R
submodel.
Mises stress comparison for static analyses.
Maximum integration
point Mises stress (MPa)
Maximum nodal
Mises stress (MPa)
Shell-to-solid submodeling
80.1
97.5
Shell-to-solid coupling
59.8
72.6
Reference
59.9
73.6
1.1.10–6
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
Figure 1.1.10–1
Figure 1.1.10–2
Global shell model of pipe-plate structure.
Magnified solid submodel of the pipe-plate joint.
1.1.10–7
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
3
2
1
Figure 1.1.10–3
Shell-to-solid coupling model of the pipe-plate joint.
Figure 1.1.10–4
Solid reference model of the pipe-plate joint.
1.1.10–8
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
Figure 1.1.10–5 Solid submodel overlaid on the shell model in
the deformed state, using a magnification factor of 20.
Figure 1.1.10–6 Shell-to-solid coupling model in the deformed
state, using a magnification factor of 20.
1.1.10–9
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
Figure 1.1.10–7 Comparison of out-of-plane displacement in the continuum mesh plate for
the submodel (top) and the shell-to-solid coupling analysis (bottom).
Figure 1.1.10–8 Comparison of out-of-plane displacement in the plate for the reference
solution (top) and the shell-to-solid coupling analysis (bottom).
1.1.10–10
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
Figure 1.1.10–9 Comparison of the Mises stress in the plate for the reference solution
(top) and the shell-to-solid coupling analysis (bottom).
Figure 1.1.10–10 Comparison of the Mises stress in the continuum mesh plate for the
submodel (top) and the shell-to-solid coupling analysis (bottom).
1.1.10–11
Abaqus Version 6.12 ID:
Printed on:
SHELL-TO-SOLID MODELING OF A PIPE JOINT
U, U3
+2.780e−04
+2.317e−04
+1.853e−04
+1.390e−04
+9.264e−05
+4.630e−05
−4.596e−08
−4.639e−05
−9.273e−05
−1.391e−04
−1.854e−04
−2.318e−04
−2.781e−04
Figure 1.1.10–11 Comparison of out-of-plane displacement in the continuum mesh plate for the
submodel with scaled boundary (top) and the shell-to-solid coupling analysis with scaled load (bottom).
S, Mises
(Avg: 75%)
+1.949e+08
+1.787e+08
+1.625e+08
+1.462e+08
+1.300e+08
+1.138e+08
+9.757e+07
+8.134e+07
+6.511e+07
+4.888e+07
+3.266e+07
+1.643e+07
+2.011e+05
Figure 1.1.10–12 Comparison of the Mises stress in the continuum mesh plate for the submodel with
scaled boundary condition (top) and the shell-to-solid coupling analysis with scaled load (bottom).
1.1.10–12
Abaqus Version 6.12 ID:
Printed on:
ELEMENT REACTIVATION
1.1.11
STRESS-FREE ELEMENT REACTIVATION
Product: Abaqus/Standard
This example demonstrates element reactivation for problems where new elements are to be added in a stressfree state. Typical examples include the construction of a gravity dam, in which unstressed layers of material
are added to a mesh that has already deformed under geostatic load, or a tunnel in which a concrete or steel
support liner is installed. Element pair reactivation during a step (“Element and contact pair removal and
reactivation,” Section 11.2.1 of the Abaqus Analysis User’s Manual) provides for this type of application
directly because the strain in newly added elements corresponds to the deformation of the mesh since the
reactivation.
Verification of the element pair reactivation capability is provided in “Model change,” Section 3.10 of
the Abaqus Verification Manual.
Problem description
The example considers the installation of a concrete liner to support a circular tunnel. Practical
geotechnical problems usually involve a complex sequence of construction steps. The construction
details determine the appropriate analysis method to represent these steps accurately. Such details have
been avoided here for the sake of simplifying the illustration.
The tunnel is assumed to be excavated in clay, with a Young’s modulus of 200 MPa and a Poisson’s
ratio of 0.2 (see Figure 1.1.11–1). The diameter of the tunnel is 8 m, and the tunnel is excavated 20 m
below ground surface. The material surrounding the excavation is discretized with first-order 4-node
plane strain elements (element type CPE4). The infinite extent of the soil is represented by a 30-m-wide
mesh that extends from the surface to a depth of 50 m below the surface. The left-hand boundary
represents a vertical symmetry axis. Far-field conditions on the bottom and right-hand-side boundaries
are modeled by infinite elements (element type CINPE4). No mesh convergence studies have been
performed to establish if these boundary conditions are placed far enough away from the excavation.
An initial stress field due to gravitational and tectonic forces exists through the depth of the soil. It
is assumed that this stress varies linearly with depth and that the ratio between the horizontal and vertical
stress components is 0.5. The self weight of the clay is 20.0 kN/m3 .
The excavation of the tunnel material is accomplished by applying the forces that are required to
maintain equilibrium with the initial stress state in the surrounding material as loads on the perimeter
of the tunnel. These loads are then reduced to zero to simulate the excavation. The three-dimensional
effect of face advancement during excavation is taken into account by relaxing the forces gradually over
several steps. The liner is installed after 40% relaxation of the loads. Further deformation continues to
occur as the face of the excavation advances. This ongoing deformation loads the liner.
In the first input file the 150-mm-thick liner is discretized with one layer of incompatible mode
elements (element type CPE4I). These elements are recommended in regions where bending response
must be modeled accurately. In the second input file beam elements are used to discretize the liner. The
liner is attached rigidly to the tunnel. The concrete is assumed to have cured to a strength represented by
1.1.11–1
Abaqus Version 6.12 ID:
Printed on:
ELEMENT REACTIVATION
the elastic properties shown in Figure 1.1.11–1 by the time the liner is loaded. The liner is not shown in
this diagram.
It is expected that an overburden load representing the weight of traffic and buildings exists after
the liner is installed.
Analysis method
The excavation and installation of the liner is modeled in four analysis steps. In the first step the initial
stress state is applied and the liner elements are removed. Concentrated loads that are in equilibrium
with the initial stress field are applied on the perimeter of the tunnel. These forces were obtained from
an independent analysis where the displacements on the tunnel perimeter were constrained. The reaction
forces at the constrained nodes are the loads applied here. The second step begins the tunnel excavation
by reducing the concentrated loads on the tunnel surface. The loads are reduced by 40% in this step
before the liner is installed in the third step. No deformation takes place in the soil or liner during the
third step. In the fourth step the surface load is applied, and the excavation is completed by removing
the remainder of the load on the tunnel perimeter.
In problems involving geometric nonlinearities with finite deformation, it is important to recognize
that element reactivation occurs in the configuration at the start of the reactivation step. If the NLGEOM
parameter were used in this problem, the thickness of the liner, when modeled with the continuum
elements, would have a value at reactivation that would be different from its original value. This result
would happen because the outside nodes (the nodes on the tunnel/liner interface) displace with the mesh,
whereas the inside nodes remain at their current locations since liner elements are inactive initially. This
effect is not relevant in this problem because geometric nonlinearities are not included. However, it may
be significant for problems involving finite deformation, and it may lead to convergence problems in cases
where elements are severely distorted upon reactivation. This problem would not occur in the model
with beam elements because they have only one node through the thickness. In the model where the
liner is modeled with continuum elements, the problem can be eliminated if the inner nodes are allowed
to follow the outer nodes prior to reactivation, which can be accomplished by applying displacement
boundary conditions on the inner nodes. Alternatively, the liner can be overlaid with (elastic) elements
of very low stiffness. These elements use the same nodes as the liner but are so compliant that their effect
on the analysis is negligible when the liner is present. They remain active throughout the analysis and
ensure that the inner nodes follow the outer nodes, thereby preserving the liner thickness.
Results and discussion
Figure 1.1.11–2 shows the stress state at a material point in the liner. The figure clearly indicates that the
liner remains unstressed until reactivated.
Figure 1.1.11–3 compares the axial stress obtained from the CPE4I and beam elements at the top
and bottom of the liner section. A local cylindrical coordinate system (“Orientations,” Section 2.2.5
of the Abaqus Analysis User’s Manual) is used to orient the liner stresses in the continuum element
model along the beam axis so that these stresses can be compared directly with the results of the beam
element model. The small difference between the results can be attributed to the element type used in
1.1.11–2
Abaqus Version 6.12 ID:
Printed on:
ELEMENT REACTIVATION
the discretization of the liner: the beam element model uses a plane stress condition, and the continuum
element model uses a plane strain condition.
Input files
modelchangedemo_continuum.inp
modelchangedemo_beam.inp
modelchangedemo_node.inp
modelchangedemo_element.inp
*MODEL CHANGE with continuum elements.
*MODEL CHANGE with beam elements.
Nodal coordinates for the soil.
Element definitions for the soil.
CL
50 kN/m
30 m
30 m
D=20m
H=50m
R=4m
26 m
Clay:
E = 200 MPa
ν = 0.2
3
γ = 20 kN/m
26 m
Concrete:
E = 19 GPa
ν = 0.2
L=30m
Figure 1.1.11–1
Geometry and finite element discretization.
1.1.11–3
Abaqus Version 6.12 ID:
Printed on:
ELEMENT REACTIVATION
0.5
S22 @ 4000
0.0
Axial Stress (MPa)
-0.5
-1.0
-1.5
-2.0
XMIN 1.000E+00
XMAX 4.000E+00
YMIN -2.441E+00
YMAX 8.269E-15
-2.5
1.0
1.5
2.0
2.5
3.0
3.5
4.0
Time (s)
Figure 1.1.11–2
Liner stress during analysis history.
-2.
CPE4I
B21
CPE4I
B21
Inside
Axial Stress (MPa)
-4.
XMIN 0.000E+00
XMAX 1.257E+01
YMIN -7.607E+00
YMAX -2.112E+00
Outside
-6.
-8.
0.
2.
4.
6.
8.
10.
Distance along beam axis (m)
Figure 1.1.11–3
Axial stress along beam inside and outside.
1.1.11–4
Abaqus Version 6.12 ID:
Printed on:
12.
VISCOELASTIC BUSHING
1.1.12
TRANSIENT LOADING OF A VISCOELASTIC BUSHING
Product: Abaqus/Standard
This example demonstrates the automatic incrementation capability provided for integration of
time-dependent material models and the use of the viscoelastic material model in conjunction with
large-strain hyperelasticity in a typical design application. The structure is a bushing, modeled as a hollow,
viscoelastic cylinder. The bushing is glued to a rigid, fixed body on the outside and to a rigid shaft on the
inside, to which the loading is applied. A static preload is applied to the shaft, which moves the inner shaft
off center. This load is held for sufficient time for steady-state response to be obtained. Then a torque
is applied instantaneously and held for a long enough period of time to reach steady-state response. We
compute the bushing’s transient response to these events.
Geometry and model
The viscoelastic bushing has an inner radius of 12.7 mm (0.5 in) and an outer radius of 25.4 mm
(1.0 in). We assume that the bushing is long enough for plane strain deformation to occur. The problem
is modeled with first-order reduced-integration elements (CPE4R). The mesh is regular, consisting of
6 elements radially, repeated 56 times to cover the 360° span in the hoop direction. The mesh is shown
in Figure 1.1.12–1. No mesh convergence studies have been performed.
The fixed outer body is modeled by fixing both displacement components at all the outside nodes.
The nodes in the inner boundary of the bushing are connected, using a kinematic coupling constraint, to
a node located in the center of the model. This node, thus, defines the inner shaft as a rigid body.
Material
The material model is not defined from any particular physical material.
The instantaneous behavior of the viscoelastic material is defined by hyperelastic properties.
A polynomial model with
1 (a Mooney-Rivlin model) is used for this, with the constants
27.56 MPa (4000 psi),
6.89 MPa (1000 psi), and
0.0029 MPa−1 (0.00002 psi−1 ).
The viscous behavior is modeled by a time-dependent shear modulus,
, and a time-dependent
bulk modulus,
, each of which is expanded in a Prony series in terms of the corresponding
instantaneous modulus,
1.1.12–1
Abaqus Version 6.12 ID:
Printed on:
VISCOELASTIC BUSHING
The relative moduli
and
and time constants
are
sec
i
1
0.2
0.5
0.1
2
0.1
0.2
0.2
This model results in an initial instantaneous Young’s modulus of 206.7 MPa (30000 psi) and Poisson’s
ratio of 0.45. It relaxes pressures faster than shear stresses.
Analysis
The analysis is done in four steps. The first step is a preload of 222.4 kN (50000 lbs) applied in the
x-direction to the node in the center of the model in 0.001 sec with a static procedure (“Static stress
analysis,” Section 6.2.2 of the Abaqus Analysis User’s Manual). The static procedure does not allow
viscous material behavior, so this response is purely elastic. During the second step the load stays
constant and the material is allowed to creep for 1 sec by using the quasi-static procedure (“Quasi-static
analysis,” Section 6.2.5 of the Abaqus Analysis User’s Manual). Since 1 sec is a long time compared
with the material time constants, the solution at that time should be close to steady state. The accuracy
of the automatic time incrementation during creep response can be controlled. This accuracy tolerance is
an upper bound on the allowable error in the creep strain increment in each time increment. It is chosen
as 5 × 10−4 , which is small compared to the elastic strains. The third step is another static step. Here
the loading is a torque of 1129.8 N-m (10000 lb-in) applied in 0.001 sec. The fourth step is another
quasi-static step with a time period of 1 sec.
Results and discussion
Figure 1.1.12–2 through Figure 1.1.12–5 depict the deformed shape of the bushing at the end of each
step. Each of the static loads produces finite amounts of deformation, which are considerably expanded
during the holding periods. Figure 1.1.12–6 shows the displacement of the center of the bushing in the
x-direction and its rotation as functions of time.
Input file
viscobushing.inp
Input data for the analysis.
1.1.12–2
Abaqus Version 6.12 ID:
Printed on:
VISCOELASTIC BUSHING
2
3
1
Figure 1.1.12–1
Finite element model of viscoelastic bushing.
2
3
1
Figure 1.1.12–2
Deformed model after horizontal static loading.
1.1.12–3
Abaqus Version 6.12 ID:
Printed on:
VISCOELASTIC BUSHING
2
3
1
Figure 1.1.12–3
Deformed model after first holding period.
2
3
1
Figure 1.1.12–4
Deformed model after static moment loading.
1.1.12–4
Abaqus Version 6.12 ID:
Printed on:
VISCOELASTIC BUSHING
2
3
1
Figure 1.1.12–5
Deformed model after second holding period.
DISPLACEMENT
ROTATION
Figure 1.1.12–6
Displacement and rotation of center of bushing.
1.1.12–5
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
1.1.13
INDENTATION OF A THICK PLATE
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing and distortion control in deep indentation problems.
Problem description
A deep indentation problem is solved for both axisymmetric and three-dimensional geometries, as shown
in Figure 1.1.13–1. Each model consists of a rigid punch and a deformable blank. The punch has a
semicircular nose section and a radius of 100 mm. The blank is modeled as a crushable foam with the
elastic response given as follows (see Schluppkotten, 1999):
7.5 MPa (Young’s modulus) and
0.0 (elastic Poisson’s ratio).
The material parameters for the isotropic hardening are given as
1.0 (yield strength ratio) and
0.0 (plastic Poisson’s ratio),
and the density is
60 kg/m3 .
In both cases the punch is fully constrained except in the vertical direction. A deep indentation is
made by moving the punch into the blank to a depth of 250 mm when adaptive meshing is used and to a
depth of 285 mm when distortion control is used. The displacement of the punch is prescribed using a
smooth-step amplitude so that a quasi-static response is generated.
Case 1: Axisymmetric model
The blank is meshed with CAX4R elements and measures 300 × 300 mm. The punch is modeled as
an analytical rigid surface using a planar analytical surface in conjunction with a rigid body constraint.
The bottom of the blank is constrained in the x- and z-directions, and symmetry boundary conditions are
prescribed at r=0.
Case 2: Three-dimensional models
Two models are analyzed. For one model the blank is meshed uniformly, while for the other a graded
mesh is used. For both models the blank is meshed with C3D8R elements and measures 600 × 300
× 600 mm. The punch is modeled as an analytical rigid surface using a three-dimensional surface of
revolution in conjunction with a rigid body constraint. The bottom of the blank is fully constrained.
1.1.13–1
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
Adaptive meshing
A single adaptive mesh domain that incorporates the entire blank is used for each model. A Lagrangian
boundary region type (the default) is used to define the constraints along the bottom of the plate for both
models and along the axis of symmetry in two dimensions. A sliding boundary region (the default) is
used to define the contact surface on the plate. To obtain a good mesh throughout the simulation, the
number of mesh sweeps is increased to 3 as part of the specification of the adaptive mesh domain. For
the graded three-dimensional model a graded smoothing objective is specified to preserve the gradation
of the mesh while adaptive meshing is performed.
Distortion control
In contrast to the adaptive meshing technique, distortion control does not attempt to maintain a highquality mesh throughout an analysis but instead tries to prevent negative element volumes or other
excessive distortion from occurring during an analysis. By using distortion control, it is possible to
prevent an analysis from failing prematurely when the mesh is coarse relative to the strain gradients
and the amount of compression. The distortion control capability is tested for axisymmetric and threedimensional models with a uniformly meshed blank.
Results and discussion
Figure 1.1.13–2 to Figure 1.1.13–4 show the initial configurations for the axisymmetric model, the
three-dimensional uniform mesh model, and the three-dimensional graded mesh model. Although the
punch is not shown in these figures, it is initially in contact with the plate. Figure 1.1.13–5 shows the
final deformed mesh for the axisymmetric indentation. The meshing algorithm attempts to minimize
element distortion both near and away from the contact surface with the punch. Figure 1.1.13–6 and
Figure 1.1.13–7 show the deformed mesh of the entire blank and a quarter-symmetry, cutaway view,
respectively, for the three-dimensional model with an initially uniform mesh. Even under this depth of
indentation, elements appear to be nicely shaped both on the surface and throughout the cross-section
of the plate.
Figure 1.1.13–8 and Figure 1.1.13–9 show the deformed mesh of the entire plate and a quartersymmetry, cutaway view, respectively, for the three-dimensional case with an initially graded mesh.
Adaptive meshing with the graded smoothing objective preserves the mesh gradation throughout the
indentation process while simultaneously minimizing element distortion. Preserving mesh gradation in
adaptivity problems is a powerful capability that allows mesh refinement to be concentrated in the areas
of highest strain gradients. A contour plot of equivalent plastic strain for the graded mesh case is shown
in Figure 1.1.13–10.
Figure 1.1.13–11 shows the final deformed mesh for the axisymmetric indentation using distortion
control without adaptive meshing. Figure 1.1.13–12 and Figure 1.1.13–13 show the deformed mesh of
the entire blank and a quarter-symmetry, cutaway view, respectively, for the three-dimensional model
with an initially uniform mesh using distortion control without adaptive meshing. The distortion control
simply prevents element distortion near the contact surface with the punch. Without distortion control
both of the analyses fail prematurely under this depth of indentation.
1.1.13–2
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
Input files
ale_indent_axi.inp
ale_indent_sph.inp
ale_indent_gradedsph.inp
ale_indent_sphelset.inp
dis_indent_axi.inp
dis_indent_sph.inp
Case 1 using adaptive meshing.
Case 2 with a uniform mesh using adaptive meshing.
Case 2 with a graded mesh using adaptive meshing.
External file referenced by Case 2.
Case 1 using distortion control.
Case 2 with a uniform mesh using distortion control.
Reference
•
Schluppkotten, J., Investigation of the ABAQUS Crushable Foam Plasticity Model, Internal report
of BMW AG, 1999.
1.1.13–3
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
r = 100mm
symmetry axis
punch
z
300 mm
r
300 mm
300 mm
punch
y
x
600 mm
z
600 mm
Figure 1.1.13–1
Axisymmetric and three-dimensional model geometries.
1.1.13–4
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
2
3
1
Figure 1.1.13–2
2
Initial configuration for the axisymmetric model.
1
3
Figure 1.1.13–3
Initial configuration for the three-dimensional model with a uniform mesh.
1.1.13–5
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
2
1
3
Figure 1.1.13–4
Initial configuration for the three-dimensional model with a graded mesh.
2
3
1
Figure 1.1.13–5
Deformed configuration for the axisymmetric model.
1.1.13–6
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
2
1
3
Figure 1.1.13–6 Deformed configuration for the three-dimensional
model with an initially uniform mesh.
2
3
1
Figure 1.1.13–7 Quarter-symmetry, cutaway view of the deformed configuration for the
three-dimensional model with an initially uniform mesh.
1.1.13–7
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
2
1
3
Figure 1.1.13–8 Deformed configuration for the three-dimensional
model with an initially graded mesh.
2
3
Figure 1.1.13–9
1
Quarter-symmetry, cutaway view of the deformed configuration for the
three-dimensional model with an initially graded mesh.
1.1.13–8
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
PEEQ
(Ave. Crit.: 75%)
+2.09e+00
+1.83e+00
+1.57e+00
+1.31e+00
+1.04e+00
+7.84e-01
+5.22e-01
+2.61e-01
+0.00e+00
2
3
1
Figure 1.1.13–10 Contours of equivalent plastic strain for the
three-dimensional model with an initially graded mesh.
2
3
1
Figure 1.1.13–11 Deformed configuration for the axisymmetric
model using distortion control.
1.1.13–9
Abaqus Version 6.12 ID:
Printed on:
INDENTATION OF A THICK PLATE
2
1
3
Figure 1.1.13–12 Deformed configuration for the three-dimensional
model with an initially uniform mesh using distortion control.
2
3
1
Figure 1.1.13–13 Quarter-symmetry, cutaway view of the
deformed configuration for the three-dimensional model with an
initially uniform mesh using distortion control.
1.1.13–10
Abaqus Version 6.12 ID:
Printed on:
LAMINATED COMPOSITE PLATE FAILURE
1.1.14
DAMAGE AND FAILURE OF A LAMINATED COMPOSITE PLATE
Products: Abaqus/Standard
Abaqus/Explicit
This example demonstrates how the nonlinear material behavior of a composite laminate can be specified as a
function of solution-dependent variables. The user subroutines USDFLD in Abaqus/Standard and VUSDFLD
in Abaqus/Explicit can be used to modify the standard linear elastic material behavior (for example, to include
the effects of damage) or to change the behavior of the nonlinear material models in Abaqus. The material
model in this example includes damage, resulting in nonlinear behavior. It also includes various modes of
failure, resulting in abrupt loss of stress carrying capacity (Chang and Lessard, 1989). The analysis results
are compared with experimental results.
Problem description and material behavior
A composite plate with a hole in the center is subjected to in-plane compression. The plate is made of
24 plies of T300/976 graphite-epoxy in a [(−45/+45) ] layup. Each ply has a thickness of 0.1429 mm
(0.005625 in); thus, the total plate thickness is 3.429 mm (0.135 in). The plate has a length of 101.6 mm
(4.0 in) and a width of 25.4 mm (1.0 in), and the diameter of the hole is 6.35 mm (0.25 in). The plate is
loaded in compression in the length direction. The thickness of the plate is sufficient that out-of-plane
displacements of the plate can be ignored. The compressive load is measured, as well as the length
change between two points, originally a distance of 25.4 mm (1.0 in) apart, above and below the hole.
The plate geometry is shown in Figure 1.1.14–1.
The material behavior of each ply is described in detail by Chang and Lessard. The initial
elastic ply properties are longitudinal modulus
=156512 MPa (22700 ksi), transverse modulus
=12962 MPa (1880 ksi), shear modulus
=6964 MPa (1010 ksi), and Poisson’s ratio
=0.23.
The material accumulates damage in shear, leading to a nonlinear stress-strain relation of the form
where
is the (initial) ply shear modulus and the nonlinearity is characterized by the factor
=2.44×10−8 MPa−3 (0.8×1−5 ksi−3 ).
Failure modes in laminated composites are strongly dependent on geometry, loading direction,
and ply orientation. Typically, one distinguishes in-plane failure modes and transverse failure modes
(associated with interlaminar shear or peel stress). Since this composite is loaded in-plane, only in-plane
failure modes need to be considered, which can be done for each ply individually. For a unidirectional
ply as used here, five failure modes can be considered: matrix tensile cracking, matrix compression,
fiber breakage, fiber matrix shearing, and fiber buckling. All the mechanisms, with the exception of fiber
breakage, can cause compression failure in laminated composites.
The failure strength in laminates also depends on the ply layup. The effective failure strength of
the layup is at a maximum if neighboring plies are orthogonal to each other. The effective strength
decreases as the angle between plies decreases and is at a minimum if plies have the same direction.
(This is called a ply cluster.) Chang and Lessard have obtained some empirical formulas for the effective
1.1.14–1
Abaqus Version 6.12 ID:
Printed on:
LAMINATED COMPOSITE PLATE FAILURE
transverse tensile strength; however, in this model we ignore such effects. Instead, we use the following
strength properties for the T300/976 laminate: transverse tensile strength =102.4 MPa (14.86 ksi),
ply shear strength =106.9 MPa (15.5 ksi), matrix compressive strength =253.0 MPa (36.7 ksi), and
fiber buckling strength
=2707.6 MPa (392.7 ksi).
The strength parameters can be combined into failure criteria for multiaxial loading. Four different
failure modes are considered in the model analyzed here.
•
Matrix tensile cracking can result from a combination of transverse tensile stress, , and shear
stress,
. The failure index,
, can be defined in terms of these stresses and the strength
parameters, and . When the index exceeds 1.0, failure is assumed to occur. Without nonlinear
material behavior, the failure index has the simple form,
With nonlinear shear behavior taken into consideration, the failure index takes the more complex
form,
•
•
•
Matrix compressive failure results from a combination of transverse compressive stress and shear
stress. The failure criterion has the same form as that for matrix tensile cracking:
The same failure index is used since the previous two failure mechanisms cannot occur
simultaneously at the same point. After the failure index exceeds 1.0, both the transverse stiffness
and Poisson’s ratio of the ply drop to zero.
Fiber-matrix shearing failure results from a combination of fiber compression and matrix shearing.
The failure criterion has essentially the same form as the other two criteria:
This mechanism can occur simultaneously with the other two criteria; hence, a separate failure index
is used. Shear stresses are no longer supported after the failure index exceeds 1.0, but direct stresses
in the fiber and transverse directions continue to be supported.
Fiber buckling failure occurs when the maximum compressive stress in the fiber direction (
)
exceeds the fiber buckling strength,
, independent of the other stress components:
1.1.14–2
Abaqus Version 6.12 ID:
Printed on:
LAMINATED COMPOSITE PLATE FAILURE
It is obvious that, unless the shear stress vanishes exactly, fiber-matrix shearing failure occurs prior
to fiber buckling. However, fiber buckling may follow subsequent to fiber shearing because only the
shear stiffness degrades after fiber-matrix shearing failure. Fiber buckling in a layer is a catastrophic
mode of failure. Hence, after this failure index exceeds 1.0, it is assumed that the material at this
point can no longer support any loads.
In this example the primary loading mode is shear. Therefore, failure of the plate occurs well before the
fiber stresses can develop to a level where fiber buckling takes place, and this failure mode need not be
taken into consideration.
Chang and Lessard assume that after failure occurs, the stresses in the failed directions drop to zero
immediately, which corresponds to brittle failure with no energy absorption. This kind of failure model
usually leads to immediate, unstable failure of the composite. This assumption is not very realistic: in
reality, the stress-carrying capacity degrades gradually with increasing strain after failure occurs. Hence,
the behavior of the composite after onset of failure is not likely to be captured well by this model.
Moreover, the instantaneous loss of stress-carrying capacity also makes the postfailure analysis results
strongly dependent on the refinement of the finite element mesh and the finite element type used.
Material model implementation
To simulate the shear nonlinearity and the failure modes (matrix failure in tension or compression and
fiber-matrix shear failure), the elastic properties are made linearly dependent on three field variables.
The first field variable represents the matrix failure index, the second represents the fiber-matrix shear
failure index, and the third represents the shear nonlinearity (damage) prior to failure. The dependence
of the elastic material properties on the field variables is shown in Table 1.1.14–1.
To account for the nonlinearity, the nonlinear stress-strain relation must be expressed in a different
form: the stress at the end of the increment must be given as a linear function of the strain. The most
obvious way to do this is to linearize the nonlinear term, leading to the relation
where i represents the increment number. This relation can be written in inverted form as
thus providing an algorithm to define the effective shear modulus.
However, this algorithm is not very suitable because it is unstable at higher strain levels, which
is readily demonstrated by stability analysis. Consider an increment where the strain does not change;
i.e.,
Let the stress at increment i have a small perturbation from
, the exact
. Similarly, at increment i+1,
solution at that increment:
. For the algorithm to be stable,
should not be larger than
. The perturbation in
in the effective shear modulus equation and linearizing
increment i+1 is calculated by substituting
it about
:
1.1.14–3
Abaqus Version 6.12 ID:
Printed on:
LAMINATED COMPOSITE PLATE FAILURE
where
The perturbation in increment i+1 is larger than the perturbation in increment i if
which, after elimination of
, reduces to the expression
Hence, instability occurs when the “nonlinear” part of the shear strain is larger than the “linear” part of
the shear strain.
To obtain a more stable algorithm, we write the nonlinear stress-strain law in the form
where
is an as yet unknown coefficient. In linearized form this leads to the update algorithm
or, in inverted form,
Following the same procedure as that for the original update algorithm, it is readily derived that a small
, in increment i reduces to zero in increment i+1 if
. Hence, the optimal
perturbation,
algorithm appears to be
Finally, this relation is written in terms of the damage parameter d:
where
1.1.14–4
Abaqus Version 6.12 ID:
Printed on:
LAMINATED COMPOSITE PLATE FAILURE
This relation is implemented in user subroutines USDFLD and VUSDFLD, and the value of the damage
parameter is assigned directly to the third field variable used for definition of the elastic properties.
The failure indices are calculated with the expressions discussed earlier, based on the stresses at the
start of the increment:
The values of the failure indices are not assigned directly to the field variables: instead, they are stored as
solution-dependent state variables. Only if the value of a failure index exceeds 1.0 is the corresponding
user-defined field variable set equal to 1.0. After the failure index has exceeded 1.0, the associated userdefined field variable continues to have the value 1.0 even though the stresses may reduce significantly,
which ensures that the material does not “heal” after it has become damaged.
Finite element model
The plate consists of 24 plies of T300/976 graphite-epoxy in a [(−45/+45) ] layup. Instead of modeling
each ply individually, we combine all plies in the −45° direction and all plies in the +45° direction.
Consequently, only two layers need to be modeled separately:
1. A layer in the −45° direction with a thickness of 1.715 mm (0.0675 in).
2. A layer in the +45° direction with a thickness of 1.715 mm (0.0675 in).
The corresponding finite element model consists of two layers of CPS4 plane stress elements, with
thicknesses and properties as previously discussed. The quarter-symmetry finite element model is shown
in Figure 1.1.14–1.
The implementation of nonlinear material behavior with user-defined field variables is explicit: the
nonlinearity is based on the state at the start of the increment. Hence, in Abaqus/Standard analyses the
user must ensure that the time increments are sufficiently small, which is particularly important because
the automatic time increment control in Abaqus/Standard is ineffective with the explicit nonlinearity
implemented in USDFLD. If automatic time incrementation is used, the maximum time increment can
be controlled from within subroutine USDFLD with the variable PNEWDT. This capability is useful
if there are other nonlinearities that require automatic time incrementation. In this example the only
significant nonlinearity is the result of the material behavior. Hence, fixed time incrementation can be
used effectively. In Abaqus/Explicit analyses the stable time increment is usually sufficiently small to
ensure good accuracy.
1.1.14–5
Abaqus Version 6.12 ID:
Printed on:
LAMINATED COMPOSITE PLATE FAILURE
Results and discussion
For this problem experimental load-displacement results were obtained by Chang and Lessard. The
experimental results, together with the numerical results obtained with Abaqus/Standard, are shown in
Figure 1.1.14–2. The agreement between the experimental and numerical results is excellent up to the
point where the load maximum is reached. After that, the numerical load-displacement curve drops off
sharply, whereas the experimental data indicate that the load remains more or less constant. Chang and
Lessard also show numerical results: their results agree with the results obtained by Abaqus but do not
extend to the region where the load drops off. The dominant failure mode in this plate is fiber/matrix
shear: failure occurs first at a load of approximately 12.15 kN (2700 lbs) and continues to grow in a
stable manner until a load of approximately 13.5 kN (3000 lbs) is reached. Figure 1.1.14–3 shows the
extent of the damage in the Abaqus/Standard finite element model at the point of maximum load. In this
figure an element is shaded if fiber/matrix shear failure has occurred at at least three integration points.
These results also show excellent agreement with the results obtained by Chang and Lessard.
As discussed earlier, the sharp load drop-off in the numerical results is the result of the lack of
residual stress carrying capacity after the failure criterion is exceeded. Better agreement could be reached
only if postfailure material data were available. Without postfailure data the results are very sensitive to
the mesh and element type, which is clearly demonstrated by changing the element type from CPS4 (full
integration) to CPS4R (reduced integration). The results are virtually identical up to the point where first
failure occurs. After that point the damage in the CPS4R model spreads more rapidly than in the CPS4
model until a maximum load of about 12.6 kN (2800 lbs) is reached. The load then drops off rapidly.
The problem is also analyzed with Abaqus/Standard models consisting of S4R and S4 elements.
The elements have a composite section with two layers, with each layer thickness equal to the thickness
of the plane stress elements in the CPS4 and CPS4R models. The results that were obtained with the
S4R and S4 element models are indistinguishable from those obtained with the CPS4R element model.
The numerical results obtained with Abaqus/Explicit using the CPS4R element model (not shown)
are consistent with those obtained with Abaqus/Standard.
Input files
Abaqus/Standard input files
damagefailcomplate_cps4.inp
damagefailcomplate_cps4.f
damagefailcomplate_node.inp
damagefailcomplate_element.inp
damagefailcomplate_cps4r.inp
damagefailcomplate_cps4r.f
damagefailcomplate_s4.inp
damagefailcomplate_s4.f
CPS4 elements.
User subroutine USDFLD used in
damagefailcomplate_cps4.inp.
Node definitions.
Element definitions.
CPS4R elements.
User subroutine USDFLD used in
damagefailcomplate_cps4r.inp.
S4 elements.
User subroutine USDFLD used in
damagefailcomplate_s4.inp.
1.1.14–6
Abaqus Version 6.12 ID:
Printed on:
LAMINATED COMPOSITE PLATE FAILURE
damagefailcomplate_s4r.inp
damagefailcomplate_s4r.f
S4R elements.
User subroutine USDFLD used in
damagefailcomplate_s4r.inp.
Abaqus/Explicit input files
damagefailcomplate_cps4r_xpl.inp
damagefailcomplate_cps4r_xpl.f
damagefailcomplate_node.inp
damagefailcomplate_element.inp
CPS4R elements.
User subroutine VUSDFLD used in
damagefailcomplate_cps4r_xpl.inp.
Node definitions.
Element definitions.
Reference
•
Chang, F-K., and L. B. Lessard, “Damage Tolerance of Laminated Composites Containing an Open
Hole and Subjected to Compressive Loadings: Part I—Analysis,” Journal of Composite Materials,
vol. 25, pp. 2–43, 1991.
Table 1.1.14–1
Dependence of the elastic material properties on the field variables.
Material State
Elastic Properties
FV1
FV2
FV3
0
0
0
1
0
0
0
0
1
0
0
0
0
1
No failure
Matrix failure
0
Fiber/matrix shear
0
0
Shear damage
Matrix failure and fiber/matrix shear
0
0
0
1
1
0
Matrix failure and shear damage
0
0
0
1
0
1
0
0
0
1
1
0
0
1
1
1
Fiber/matrix shear and shear damage
All failure modes
0
1.1.14–7
Abaqus Version 6.12 ID:
Printed on:
LAMINATED COMPOSITE PLATE FAILURE
E
4.0 0.25
0.135
2
1.0
3
E = 1.0
Figure 1.1.14–1
Plate geometry.
1.1.14–8
Abaqus Version 6.12 ID:
Printed on:
1
LAMINATED COMPOSITE PLATE FAILURE
4000
Experiment (Chang et al., 1989)
ABAQUS (CPS4)
ABAQUS (CPS4R)
Applied load P (lb)
3000
2000
1000
0
0.000
Figure 1.1.14–2
0.010
0.020
0.030
Experimental and numerical (Abaqus/Standard) load displacement curves.
fiber-matrix shear
failure
2
3
Figure 1.1.14–3
1
Distribution of material damage at maximum load obtained with Abaqus/Standard.
1.1.14–9
Abaqus Version 6.12 ID:
Printed on:
THE BOOT SEAL PROBLEM
1.1.15
ANALYSIS OF AN AUTOMOTIVE BOOT SEAL
Product: Abaqus/Standard
Boot seals are used to protect constant velocity joints and steering mechanisms in automobiles. These flexible
components must accommodate the motions associated with angulation of the steering mechanism. Some
regions of the boot seal are always in contact with an internal metal shaft, while other areas come into contact
with the metal shaft during angulation. In addition, the boot seal may also come into contact with itself, both
internally and externally. The contacting regions affect the performance and longevity of the boot seal.
In this example the deformation of the boot seal, caused by a typical angular movement of the shaft,
is studied. It provides a demonstration and verification of the finite-sliding capability in three-dimensional
deformable-to-deformable contact and self-contact in Abaqus. This problem also demonstrates how to model
a hyperelastic material using the UMAT user subroutine.
Geometry and model
The boot seal with the internal shaft is shown in Figure 1.1.15–1. The corrugated shape of the boot
seal tightly grips the steering shaft at one end, while the other end is fixed. The rubber seal is modeled
with first-order, hybrid brick elements with two elements through the thickness using symmetric model
generation. The seal has a nonuniform thickness varying from a minimum of 3.0 mm to a maximum of
4.75 mm at the fixed end. The internal shaft is considered to be rigid and is modeled as an analytical
rigid surface; the radius of the shaft is 14 mm. The rigid body reference node is located precisely in the
center of the constant velocity joint.
The rubber is modeled as a slightly compressible neo-Hookean (hyperelastic) material with
=0.752 MPa and
=0.026 MPa−1 . For illustrative purposes an input file using the Marlow model
is included; the model is defined using uniaxial test data generated by running a uniaxial test with the
neo-Hookean model.
Contact is specified between the rigid shaft and the inner surface of the seal. Self-contact is specified
on the inner and outer surfaces of the seal.
Loading
The mounting of the boot seal and the angulation of the shaft are carried out in a three-step analysis. The
inner radius at the neck of the boot seal is smaller than the radius of the shaft so as to provide a tight
fit between the seal and the shaft. In the first step the initial interference fit is resolved, corresponding
to the assembly process of mounting the boot seal onto the shaft. The automatic “shrink” fit method is
utilized. The second step simulates the angulation of the shaft by specifying a finite rotation of 20° at
the rigid body reference node of the shaft. During the third step the angulated shaft travels around the
entire circumference to demonstrate the robustness of the algorithm.
1.1.15–1
Abaqus Version 6.12 ID:
Printed on:
THE BOOT SEAL PROBLEM
User subroutine for neo-Hookean hyperelasticity
In Abaqus/Standard user subroutine UHYPER is used to define a hyperelastic material. However, in this
problem we illustrate the use of user subroutine UMAT as an alternative method of defining a hyperelastic
material. In particular, we consider the neo-Hookean hyperelastic material model. The form of the neoHookean strain energy density function is given by
Here, , , and are the strain invariants of the deviatoric left Cauchy-Green deformation tensor .
This tensor is defined as
, where
is the distortion gradient. “Hyperelastic
material behavior,” Section 4.6.1 of the Abaqus Theory Manual, contains detailed explanations of these
quantities.
The constitutive equation for a neo-Hookean material is
where
stress
where
is the Cauchy stress. The material Jacobian,
, is defined by the variation of the Kirchhoff
is the virtual rate of deformation and is defined as
For a neo-Hookean material the components of
are given by
Results and discussion
Figure 1.1.15–2 shows the deformed configuration of the model. The rotation of the shaft causes the
stretching of one side and compression on the other side of the boot seal. The surfaces have come into
self-contact on the compressed side. Figure 1.1.15–3 shows the contours of maximum principal stresses
in the boot seal.
Comparison of the analysis times when using fixed and automated contact patches shows that both
analyses complete in approximately the same amount of time. This can be expected for this type of
problem since the fixed contact patches are limited in size to a few elements. For the case with fixed
1.1.15–2
Abaqus Version 6.12 ID:
Printed on:
THE BOOT SEAL PROBLEM
contact patches the wavefront is somewhat larger, requiring more memory and solution time per iteration.
However, this is offset by the time required to form new contact patches and to reorder the equations for
the case with automatic contact patches. The results obtained with the model that uses user subroutine
UMAT are identical to those obtained using the built-in Abaqus material model.
Input files
bootseal.inp
bootseal_surf.inp
bootseal_2d.inp
bootseal_2d_surf.inp
bootseal_umat.inp
bootseal_2d_umat.inp
bootseal_umat.f
bootseal_marlow.inp
bootseal_2d_marlow.inp
Analysis with node-to-surface contact.
Analysis with surface-to-surface contact.
Two-dimensional model for symmetric model generation
in bootseal.inp.
Two-dimensional model for symmetric model generation
in bootseal.inp using surface-to-surface contact.
Analysis with user subroutine UMAT.
Two-dimensional model for symmetric model generation
in bootseal_umat.inp.
UMAT for the neo-Hookean hyperelasticity model.
Analysis with Marlow hyperelasticity model.
Two-dimensional model for symmetric model generation
in bootseal_marlow.inp.
Figure 1.1.15–1
Undeformed model.
1.1.15–3
Abaqus Version 6.12 ID:
Printed on:
THE BOOT SEAL PROBLEM
2
31
Figure 1.1.15–2
SP3
Deformed configuration of half the model.
VALUE
-7.63E-02
+5.83E-02
+1.93E-01
+3.27E-01
+4.62E-01
+5.96E-01
+7.31E-01
+8.65E-01
+1.00E+00
+1.31E+00
2
1
3
Figure 1.1.15–3
Contours of maximum principal stress in the seal.
1.1.15–4
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
1.1.16
PRESSURE PENETRATION ANALYSIS OF AN AIR DUCT KISS SEAL
Product: Abaqus/Standard
Seals are common structural components that often require design analyses. Abaqus can be used to perform
nonlinear finite element analyses of seals and provide information needed to determine the seal performance.
Information such as a load-deflection curve, seal deformation and stresses, and contact pressure distribution
is readily obtained in these analyses. Abaqus allows for pressure penetration effects between the seal and
the contacting surfaces to be considered in these analyses, making routine analyses of seals more realistic
and accurate. Analyses of clutch seals, threaded connectors, car door seals, and air duct kiss seals are some
applications where pressure penetration effects are important.
The surface-based pressure penetration capability is used to simulate pressure penetration between
contacting surfaces. It is invoked by using the pressure penetration option, which is described in “Pressure
penetration loading,” Section 36.1.7 of the Abaqus Analysis User’s Manual. This capability is provided
for simulating cases where a joint between two deforming bodies (for example, between two components
threaded onto each other) or between a deforming body and a rigid surface (such as a soft gasket used in a
joint) is exposed at one or multiple ends to a fluid or air pressure. This air pressure will penetrate into the
joint and load the surfaces forming the joint until some area of the surfaces is reached where the contact
pressure between the abutting surfaces exceeds the critical value specified on the pressure penetration option,
cutting off further penetration.
Geometry and model
The major consideration in an air duct kiss seal design is to provide sealing while avoiding excessive
closure force. A poorly designed air duct seal that minimizes the amount of effort to close the fan cowl
door may fail to prevent leakage and reduce wind noise. The model used in this example is a simplified
version of an air duct kiss seal. It illustrates how pressure penetration effects can be modeled using
Abaqus.
The seal modeled is a rolled shape seal. An axisymmetric model of the seal is developed first, as
shown in Figure 1.1.16–1. A three-dimensional model of the seal is also developed with only a 5-degree
fraction of the seal discretized, as shown in Figure 1.1.16–2. The top horizontal rigid surface represents
the air fan cowl door, and the bottom horizontal rigid surface represents the seal groove. The rolled seal is
2.54 mm (0.1 in) thick and 74.66 mm (2.9 in) high; and its inner diameters at the top and bottom surfaces
are 508.5 mm (20 in) and 528.3 mm (20.8 in), respectively. A folded metal clip is partially bonded to
the top surface of the seal. The thickness of the metal clip is 0.48 mm (0.019 in).
The material of the seal is taken to be an incompressible rubberlike material. To obtain the material
constants, the Ogden form of the strain energy function with
4 is used to fit the uniaxial test data.
The metal clip is made of steel, with a Young’s modulus of 206.8 GPa (3.0 × 107 lb/in2 ) and a Poisson’s
ratio of 0.3. CAX4H elements are used to model the seal and the metal clip in the axisymmetric model,
and C3D8H elements are used in the three-dimensional model. The contact pair approach is used to
model the contact between the top surface of the metal clip and the top rigid surface representing the
fan cowl door, where the pressure penetration is likely to occur. The contact pair approach is also used
1.1.16–1
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
to model the contact between the seal and the bottom rigid surface, the contact between the seal and
the unbonded portion of the metal clip, and the self-contact of the seal. The mechanical interaction
between the contact surfaces is assumed to be frictional contact. Therefore, the friction option is used
to specify friction coefficients. To increase computational efficiency, the slip tolerance (the ratio of
allowable maximum elastic slip to characteristic contact surface face dimension) on the friction option
is specified for the contact surfaces between the seal and the metal clip because the dimensions of these
elements vary greatly. Fixed boundary conditions are applied initially to the reference node of the top
rigid surface, 5001, and the reference node of the bottom rigid surface, 5002. The vertical edge at the
bottom of the seal is constrained such that it cannot be moved in the 1-direction. The bottom node of
the vertical edge, 1, touches the bottom rigid surface and is held fixed in the 2-direction. The top rigid
surface is located initially 1.27 mm (0.05 in) above the top surface of the metal clip.
The seal and the unbonded portion of the clip are loaded by air pressure on all of their inner surfaces
and by contact pressure generated by closing the air fan cowl door. Two nonlinear static steps, all of
which include large-displacement effects, are used to simulate these loading conditions.
In the first step the top rigid surface moves 35.56 mm (1.4 in) downward in the y-direction,
simulating the closing of the fan cowl door.
In the second step the inner surface of the seal is subjected to a uniform air pressure load of 206.8 KPa
(30.0 lb/in2 ) since some gaps between the seal and the top rigid surface have been closed. The pressure
penetration is simulated between the top surface of the metal clip (PPRES), which includes 31 elements,
and the top rigid surface (CFACE). Air pressure penetration does not need to be modeled between the
metal clip and the seal because they are well bonded.
The pressure penetration option is invoked to define the node exposed to the air pressure, the
magnitude of the air pressure, and the critical contact pressure. The surface PPRES is exposed to the air
pressure at node 597, with a pressure magnitude of 206.8 KPa (30.0 lb/in2 ). A default value of zero for
the critical contact pressure is used, indicating that the pressure penetration occurs only when contact
at a slave node is lost.
Results and discussion
The deformed configuration and the contours of the contact pressures on the seal at the end of Step 1 are
shown in Figure 1.1.16–3 and Figure 1.1.16–4 for the axisymmetric model and in Figure 1.1.16–5 for
the three-dimensional model. A nonuniform contact pressure is observed along the surface of the seal.
The contact pressure at the first five slave nodes is zero.
The penetrating pressure loads are applied during Step 2. The air pressure is applied immediately to
elements associated with the first five slave nodes since the contact pressure there is zero and the pressure
penetration criterion is satisfied. For the axisymmetric model, the spread of the penetration is captured in
Figure 1.1.16–6 through Figure 1.1.16–14, which show the deformed seal, the contact pressure profile,
and the air pressure profiles corresponding to load increments 2, 10, and 16 of Step 2. The pressures
applied to the surface corresponding to these three increments are 1.296 KPa (0.188 lb/in2 ), 13.96 KPa
(2.03 lb/in2 ), and 70.88 KPa (10.28 lb/in2 ), respectively. For the three-dimensional model, the spread
of the penetration is captured in Figure 1.1.16–15 through Figure 1.1.16–17, which show the contact
pressure profiles corresponding to load increments 2, 6, and 14 of Step 2.
1.1.16–2
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
Increased penetrating pressure loads applied in Step 2 further reduce the contact pressure, eventually
causing complete air penetration through the seal. The seal was lifted off from the air fan cowl door
except at the last slave node, 663, where the contact pressure is well maintained due to imposed boundary
conditions and the air pressures. For the axisymmetric model, the development of the weakening of the
sealing is captured in Figure 1.1.16–18 through Figure 1.1.16–21, which show the deformed seal and
the contact pressure profile corresponding to load increment 20 and at the end of Step 2. The pressures
applied to the surface corresponding to these two increments are 112.3 KPa (16.28 lb/in2 ) and 206.8 KPa
(30.0 lb/in2 ), respectively. For the three-dimensional model, the development of the weakening of the
sealing is captured in Figure 1.1.16–22 through Figure 1.1.16–23, which show the contact pressure profile
corresponding to load increment 19 and at the end of Step 2.
The behavior of the seal throughout the loading histories can be best described by plotting the air
penetration distance as a function of the air pressure, as shown in Figure 1.1.16–24 for both axisymmetric
and three-dimensional models. It is clear that air penetration into the seal accelerates only when the
pressure is on the order of 51.7 KPa (7.5 lb/in2 ). The air completely penetrates through the seal when
the pressure is 82.7 KPa (12.0 lb/in2 ), which is approximately equal to 80% of the sea level atmospheric
pressure.
In addition, the same model is analyzed with the adaptive automatic stabilization scheme, which
improves the robustness by automatically adjusting the damping factor based on the convergence history
while having very little effect on the results. The dissipated stabilization energy is found to be small
when the adaptive stabilization scheme is used.
Input files
presspenairductseal.inp
presspenairductseal_stabil_adap.inp
presspenairductseal_node.inp
presspenairductseal_elem_metal.inp
presspenairductseal_elem_rub.inp
presspenairductseal_c3d8h.inp
Pressure penetration simulation of an air duct kiss seal.
Same as presspenairductseal.inp with adaptive automatic
stabilization.
Node definitions for the seal model.
Element definitions for the metal part of the seal model.
Element definitions for the rubber part of the seal model.
Pressure penetration simulation of an air duct kiss seal in
three dimensions.
1.1.16–3
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
2
3
1
Figure 1.1.16–1
Axisymmetric model of air duct kiss seal.
1.1.16–4
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
Y
Z
X
Figure 1.1.16–2
Three-dimensional model of air duct kiss seal.
Figure 1.1.16–3 For the axisymmetric model, deformed
configuration of the seal at the end of Step 1.
1.1.16–5
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
CPRESS
1.967
1.803
1.639
1.475
1.311
1.147
0.983
0.819
0.656
0.492
0.328
0.164
0.000
Figure 1.1.16–4 For the axisymmetric model, contact stress
contours in the seal at the end of Step 1.
CPRESS
2.060
1.888
1.717
1.545
1.373
1.202
1.030
0.858
0.687
0.515
0.343
0.172
0.000
Y
Z
Figure 1.1.16–5
X
For the three-dimensional model, deformed configuration and contact
stress contours of the seal at the end of Step 1.
1.1.16–6
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
Figure 1.1.16–6 For the axisymmetric model, deformed
configuration of the seal at Step 2, increment 2.
CPRESS
2.264
2.076
1.887
1.698
1.510
1.321
1.132
0.944
0.755
0.566
0.377
0.189
0.000
Figure 1.1.16–7 For the axisymmetric model, contact stress
contours in the seal at Step 2, increment 2.
1.1.16–7
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
PPRESS
0.188
0.172
0.156
0.141
0.125
0.109
0.094
0.078
0.063
0.047
0.031
0.016
0.000
Figure 1.1.16–8 For the axisymmetric model, air pressure
contours in the seal at Step 2, increment 2.
Figure 1.1.16–9 For the axisymmetric model, deformed
configuration of the seal at Step 2, increment 10.
1.1.16–8
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
CPRESS
7.941
7.280
6.618
5.956
5.294
4.633
3.971
3.309
2.647
1.985
1.324
0.662
0.000
Figure 1.1.16–10 For the axisymmetric model, contact stress
contours in the seal at Step 2, increment 10.
PPRESS
2.025
1.856
1.687
1.519
1.350
1.181
1.012
0.844
0.675
0.506
0.337
0.169
0.000
Figure 1.1.16–11 For the axisymmetric model, air pressure
contours in the seal at Step 2, increment 10.
1.1.16–9
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
Figure 1.1.16–12 For the axisymmetric model, deformed
configuration of the seal at Step 2, increment 16.
CPRESS
88.650
81.263
73.875
66.488
59.100
51.713
44.325
36.938
29.550
22.163
14.775
7.388
0.000
Figure 1.1.16–13 For the axisymmetric model, contact stress
contours in the seal at Step 2, increment 16.
1.1.16–10
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
PPRESS
10.277
9.421
8.564
7.708
6.851
5.995
5.139
4.282
3.426
2.569
1.713
0.856
0.000
Figure 1.1.16–14 For the axisymmetric model, air pressure
contours in the seal at Step 2, increment 16.
CPRESS
2.705
2.479
2.254
2.029
1.803
1.578
1.352
1.127
0.902
0.676
0.451
0.225
0.000
Y
Z
Figure 1.1.16–15
X
For the three-dimensional model, deformed configuration and contact
stress contours of the seal at Step 2, increment 2.
1.1.16–11
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
CPRESS
6.913
6.337
5.760
5.184
4.608
4.032
3.456
2.880
2.304
1.728
1.152
0.576
0.000
Y
Z
X
Figure 1.1.16–16
For the three-dimensional model, deformed configuration and contact
stress contours of the seal at Step 2, increment 6.
CPRESS
133.458
122.337
111.215
100.094
88.972
77.851
66.729
55.608
44.486
33.365
22.243
11.122
0.000
Y
Z
Figure 1.1.16–17
X
For the three-dimensional model, deformed configuration and contact
stress contours of the seal at Step 2, increment 14.
1.1.16–12
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
Figure 1.1.16–18 For the axisymmetric model, deformed
configuration of the seal at Step 2, increment 20.
CPRESS
84.219
77.201
70.182
63.164
56.146
49.128
42.109
35.091
28.073
21.055
14.036
7.018
0.000
Figure 1.1.16–19 For the axisymmetric model, contact stress
contours in the seal at Step 2, increment 20.
1.1.16–13
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
Figure 1.1.16–20 For the axisymmetric model, deformed
configuration of the seal at the end of Step 2.
CPRESS
353.998
324.498
294.998
265.499
235.999
206.499
176.999
147.499
117.999
88.500
59.000
29.500
0.000
Figure 1.1.16–21 For the axisymmetric model, contact stress
contours in the seal at the end of Step 2.
1.1.16–14
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
CPRESS
95.244
87.307
79.370
71.433
63.496
55.559
47.622
39.685
31.748
23.811
15.874
7.937
0.000
Y
Z
X
Figure 1.1.16–22
For the three-dimensional model, deformed configuration and contact
stress contours of the seal at Step 2, increment 19.
CPRESS
355.826
326.174
296.522
266.870
237.217
207.565
177.913
148.261
118.609
88.957
59.304
29.652
0.000
Y
Z
Figure 1.1.16–23
X
For the three-dimensional model, deformed configuration and contact
stress contours of the seal at the end of Step 2.
1.1.16–15
Abaqus Version 6.12 ID:
Printed on:
PRESSURE PENETRATION
Air Penetration Distance
1.0
0.8
0.6
0.4
0.2
0.0
0.
5.
10.
15.
20.
25.
Air Pressure
Axisymmetric
Three−dimensional
Figure 1.1.16–24 Air penetration distance as a function
of air pressure in the seal
1.1.16–16
Abaqus Version 6.12 ID:
Printed on:
30.
JOUNCE BUMPER
1.1.17
SELF-CONTACT IN RUBBER/FOAM COMPONENTS: JOUNCE BUMPER
Products: Abaqus/Standard
Abaqus/Explicit
The self-contact capability in Abaqus is illustrated with two examples derived from the automotive component
industry: this problem and the following one, which discusses a rubber gasket. These examples demonstrate
the use of the single-surface contact capability available for large-sliding analysis in Abaqus. Components
that deform and change their shape substantially can fold and have different parts of the surface come into
contact with each other. In such cases it can be difficult to predict at the outset of the analysis where such
contact may occur and, therefore, it can be difficult to define two independent surfaces to make up a contact
pair.
A jounce bumper, sometimes referred to as a “helper spring,” is a highly compressible component that
is used as part of the shock isolation system in a vehicle. It is typically located above the coil spring that
connects the wheels to the frame. Microcellular material is used because of its high compressibility and low
Poisson’s ratio value at all but fully compressed configurations.
The bumper is mounted on a mandrel with a diameter larger than the bumper’s inner diameter
(Figure 1.1.17–1). The first step of the analysis solves this interference fit problem. The bumper initially sits
against a fixed flat rigid surface on one end; on the other end, another flat rigid surface is used to model the
compression of the bumper. The geometry of the bumper is such that it folds in three different locations.
Separate surfaces are defined at the locations where self-contact is expected. This modeling technique
produces an economical analysis because the scope of contact searches is limited.
Geometry and model
The bumper is 76.0 mm (3.0 in) long and has an inside diameter of 20.0 mm (.8 in). The mandrel,
which is modeled as a rigid surface, has a diameter of 22.0 mm (.9 in). The bumper is modeled with
the hyperfoam material model. The compressible, nonlinear elastic behavior is described by a strain
energy function. A mesh of either CAX3 or CAX4R elements is produced using an automatic mesh
generator. Figure 1.1.17–1 and Figure 1.1.17–2 show the initial mesh with CAX3 elements and CAX4R
elements, respectively. In addition to the portions of the bumper’s surface used to define self-contact,
additional regions are defined to model contact between the bumper and the fixed surface, the bumper
and the mandrel, and the bumper and the moving rigid surface. A small amount of friction (a Coulomb
coefficient of 0.05) is applied to all of the surfaces.
Results and discussion
The bumper analysis is a two-step process. In the first step the interference between the bumper’s inner
diameter and the mandrel is resolved. In the Abaqus/Standard analysis the automatic “shrink” fit method
(see “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2
of the Abaqus Analysis User’s Manual) is used: the calculated initial penetration is allowed at the
beginning of the step and scaled linearly to zero at the end of the step. In the Abaqus/Explicit analysis
the interference resolution step is performed in one of two ways. In the first approach the mandrel is
1.1.17–1
Abaqus Version 6.12 ID:
Printed on:
JOUNCE BUMPER
positioned so that no contact or overclosure exists between the bumper and the mandrel at the outset of
the analysis. The rigid surface representing the mandrel is then moved in the radial direction to simulate
the compression of the bumper due to the interference fit. In the second approach the shrink fit solution
from Abaqus/Standard is imported into Abaqus/Explicit. A comparison of the Mises stresses predicted
by Abaqus/Standard and Abaqus/Explicit at the end of the interference step shows that the results are
very similar (see Figure 1.1.17–3 and Figure 1.1.17–4).
In the second step the bottom surface compresses the bumper 42.0 mm (1.7 in) as a result of the
application of displacement boundary conditions to the reference node of the surface. Figure 1.1.17–5,
Figure 1.1.17–6, and Figure 1.1.17–7 show the final deformed shape of the bumper; the high
compressibility of the material is apparent, as well as the folding of the surface onto itself. Although a
general knowledge of where the folding would occur was used in the definition of the self-contacting
surfaces, it is not necessary to know exactly where the kinks in the surface will form.
The final deformed shapes predicted by Abaqus/Standard and Abaqus/Explicit for the CAX3
element mesh are the same (see Figure 1.1.17–5 and Figure 1.1.17–6, respectively). A similar shape
is predicted by Abaqus/Explicit when CAX4R elements are used (see Figure 1.1.17–7). However, the
solution obtained with CAX4R elements in Abaqus/Explicit reveals that local buckling occurs in the
upper-left folding radius. This makes a similar analysis using CAX4R elements in Abaqus/Standard
very difficult. The local buckling is not captured in the CAX3 analysis due to the stiffer nature of these
elements.
The load versus displacement curves of the bottom surface are shown in Figure 1.1.17–8. The
results obtained with CAX3 elements in Abaqus/Standard and with CAX3 and CAX4R elements in
Abaqus/Explicit are very similar. The energy absorption capacity of the bumper is seen through these
curves.
Input files
selfcontact_bump_std_cax3.inp
selfcontact_bump_surf.inp
selfcontact_bump_std_imp_surf.inp
selfcontact_bump_xpl_cax3.inp
selfcontact_bump_xpl_cax4r.inp
selfcontact_bump_std_resinter_cax4r.inp
selfcontact_bump_std_imp_cax3.inp
Jounce bumper model for Abaqus/Standard using CAX3
elements.
Jounce bumper model for Abaqus/Standard using CAX3
elements and surface-to-surface contact.
Jounce bumper model for Abaqus/Standard using CAX3
elements and surface-to-surface contact. This input file
depends on selfcontact_bump_surf.inp.
Jounce bumper model for Abaqus/Explicit using CAX3
elements.
Jounce bumper model for Abaqus/Explicit using CAX4R
elements.
Jounce bumper model for Abaqus/Standard using
CAX4R elements to resolve the interference fit.
Jounce bumper model for Abaqus/Standard using
CAX3 elements; interference fit solution imported
from Abaqus/Standard.
1.1.17–2
Abaqus Version 6.12 ID:
Printed on:
JOUNCE BUMPER
selfcontact_bump_xpl_imp_cax3.inp
selfcontact_bump_xpl_imp_cax4r.inp
selfcontact_bump_node_cax3.inp
selfcontact_bump_node_cax4r.inp
selfcontact_bump_element_cax3.inp
selfcontact_bump_element_cax4r.inp
selfcontact_bump_surfdef_cax3.inp
selfcontact_bump_surfdef_cax4r.inp
Jounce bumper model for Abaqus/Explicit using CAX3
elements; interference fit solution imported from
Abaqus/Standard.
Jounce bumper model for Abaqus/Explicit using
CAX4R elements; interference fit solution imported
from Abaqus/Standard.
Node definitions for the bumper model with CAX3
elements.
Node definitions for the bumper model with CAX4R
elements.
Element definitions for the bumper model with CAX3
elements.
Element definitions for the bumper model with CAX4R
elements.
Surface definitions for the bumper model with CAX3
elements.
Surface definitions for the bumper model with CAX4R
elements.
1.1.17–3
Abaqus Version 6.12 ID:
Printed on:
JOUNCE BUMPER
2
3
1
Figure 1.1.17–1
Jounce bumper initial mesh with CAX3 elements (Abaqus/Standard).
2
3
Figure 1.1.17–2
1
Jounce bumper initial mesh with CAX4R elements (Abaqus/Explicit).
1.1.17–4
Abaqus Version 6.12 ID:
Printed on:
JOUNCE BUMPER
Figure 1.1.17–3 Mises stresses in bumper after interference is
resolved with Abaqus/Standard automatic shrink fit option.
Figure 1.1.17–4 Mises stresses in bumper after interference
is resolved with Abaqus/Explicit.
1.1.17–5
Abaqus Version 6.12 ID:
Printed on:
JOUNCE BUMPER
2
3
1
Figure 1.1.17–5
Bumper mesh after crushing (Abaqus/Standard; CAX3 elements).
2
3
Figure 1.1.17–6
1
Bumper mesh after crushing (Abaqus/Explicit; CAX3 elements).
1.1.17–6
Abaqus Version 6.12 ID:
Printed on:
JOUNCE BUMPER
2
3
1
Figure 1.1.17–7
Bumper mesh after crushing (Abaqus/Explicit; CAX4R elements).
ABAQUS/Standard CAX3 Elements
ABAQUS/Explicit CAX3 Elements
ABAQUS/Explicit CAX4R Elements
Figure 1.1.17–8
Bumper load-displacement curve.
1.1.17–7
Abaqus Version 6.12 ID:
Printed on:
RUBBER GASKET
1.1.18
SELF-CONTACT IN RUBBER/FOAM COMPONENTS: RUBBER GASKET
Products: Abaqus/Standard
Abaqus/Explicit
The self-contact capability in Abaqus is illustrated with two examples derived from the automotive
component industry: this problem and the preceding one, which discusses a jounce bumper. These examples
demonstrate the use of the single-surface contact capability available for two-dimensional large-sliding
analysis. Components that deform and change their shape substantially can fold and have different parts of
the surface come into contact with each other. In such cases it can be difficult to predict at the outset of the
analysis where such contact may occur and, therefore, it can be difficult to define two independent surfaces
to make up a contact pair.
This model is used to analyze an oil pan gasket, which enhances the sealing of the oil pan against the
engine block. A primary objective of gasket designers is to reach or exceed a threshold value of contact
pressure at the gasket bead/cover/engine block interfaces. Experience shows that, above such a threshold,
oil will not leak. Another item of interest is the load-deflection curve obtained when compressing the gasket
cross-section since it is indicative of the bolt load required to attain a certain gap between the oil pan and the
engine block. Finally, the analysis provides details to ensure that stresses and strains are within acceptable
bounds.
The rubber gasket is embedded in a plastic backbone. It has two planes of symmetry and a bead that,
when compressed, provides the sealing effect (Figure 1.1.18–1). A flat rigid surface, parallel to one of the
symmetry planes, pushes the gasket into the backbone. The geometry of the gasket is such that it folds in
two different locations. In this model the entire free surface of the gasket and of the backbone is declared as
a single surface allowed to contact itself. This modeling technique, although very simple, is more expensive
because of the extensive contact searches required, as well as a larger wavefront of the equation system when
using Abaqus/Standard.
The analysis is performed using both Abaqus/Standard and Abaqus/Explicit.
Geometry and model
The rubber gasket is modeled as a quarter of a plane strain section, initially in contact with a flat rigid
surface. The clearance between the plastic backbone and the surface is 0.612 mm (.024 in). The height
of the bead in the gasket is 1.097 mm (.043 in). The backbone is modeled with a linear elastic material
with a Young’s modulus of 8000.0 MPa (1160 ksi) and a Poisson’s ratio of 0.4. In Abaqus/Standard
the gasket is modeled as a fully incompressible hyperelastic material, which is much softer than the
backbone material at all strain levels. In Abaqus/Explicit a small amount of compressibility is assumed
for the gasket material. The nonlinear elastic behavior of the gasket is described by a strain energy
function that is a first-order polynomial in the strain invariants. The model is discretized with first-order
quadrilaterals. Standard elements are used for the backbone. In Abaqus/Standard full-integration hybrid
elements are used for the gasket, while reduced-integration elements are used to model the gasket in
Abaqus/Explicit. The interface between the gasket and the backbone is assumed to be glued with no
special treatment required. A single surface definition covers all of the free surface of the gasket and the
backbone. Through the definition of contact pairs, this surface is allowed to contact both the rigid surface
1.1.18–1
Abaqus Version 6.12 ID:
Printed on:
RUBBER GASKET
and itself. A small amount of friction (Coulomb coefficient of 0.05) is applied to the interface with the
rigid surface, which is assumed to be lubricated. Sticking surface behavior, through the specification of
rough friction (“Frictional behavior,” Section 36.1.5 of the Abaqus Analysis User’s Manual), is applied
when the gasket contacts itself, denoting a clean surface.
Results and discussion
The gasket analysis is a single-step procedure in which the rigid surface moves down almost all of
the backbone clearance (0.61 mm or .024 in). The relative rigidity of the backbone forces the rubber
gasket to fit inside the cavity provided by the backbone, folding in two regions (Figure 1.1.18–2 and
Figure 1.1.18–3). Although the general vicinity of the location of the folds can be estimated from the
initial configuration, their exact locations are difficult to predict.
The deformed shape of the gasket and the locations of the folds predicted by Abaqus/Standard and
Abaqus/Explicit agree well. The rigid surface load-displacement curve is also in good agreement, as
shown in Figure 1.1.18–4.
Acknowledgments
SIMULIA would like to thank Mr. DeHerrera of Freudenberg-NOK General Partnership for providing
these examples.
Input files
selfcontact_gask.inp
selfcontact_gask_xpl.inp
selfcontact_gask_node.inp
selfcontact_gask_element1.inp
selfcontact_gask_element2.inp
selfcontact_gask_c3d8h.inp
Gasket model for Abaqus/Standard.
Gasket model for Abaqus/Explicit.
Node definitions for the gasket model.
Element definitions for the rubber part of the gasket
model.
Element definitions for the backbone part of the gasket
model.
Three-dimensional gasket model for Abaqus/Standard.
1.1.18–2
Abaqus Version 6.12 ID:
Printed on:
RUBBER GASKET
Figure 1.1.18–1
Figure 1.1.18–2
Gasket initial mesh.
Gasket mesh after loading as predicted by Abaqus/Standard.
1.1.18–3
Abaqus Version 6.12 ID:
Printed on:
RUBBER GASKET
Figure 1.1.18–3
Gasket mesh after loading as predicted by Abaqus/Explicit.
ABAQUS/Explicit
ABAQUS/Standard
Figure 1.1.18–4
Rigid surface load-displacement curve.
1.1.18–4
Abaqus Version 6.12 ID:
Printed on:
SUBMODELING OF A STACKED SHEET METAL ASSEMBLY
1.1.19
SUBMODELING OF A STACKED SHEET METAL ASSEMBLY
Product: Abaqus/Standard
Sheet metal stampings stacked and fitted on top of each other and secured together via mechanical fasteners
such as bolts or rivets are commonly used in the automotive industry. Examples include seat belt anchors
and seating track assemblies. The submodeling capability in Abaqus facilitates economical, yet detailed,
prediction of the ultimate strength and integrity of such jointed assemblies. A global model analysis of an
assembly is first performed to capture the overall deformation of the system. Subsequently, the displacement
results of this global analysis are used to drive the boundaries of a submodeled region of critical concern. The
submodeling methodology provides accurate modeling that is more economical than using a globally refined
mesh in a single analysis.
In a finite element analysis of such a structure, shell elements are commonly used to represent the sheet
metal stampings. The nodes of each shell typically lie along the mid-plane of the shell thickness. The thickness
of the shells is used in the structural calculations but is not taken into account in the contact calculations.
Hence, a structure composed of a stack-up of several sheet stampings may have the nodes of each sheet all
lying in the same spatial plane. This close proximity creates uncertainty in a submodel analysis since Abaqus
will not be able to determine the correct correspondence between the sheets in the submodel and the global
model. Therefore, Abaqus provides a capability that allows the user to specify particular elements of the
global model that are used to drive a particular set of nodes in a submodel, which eliminates the uncertainty.
This capability is demonstrated in this example problem.
Geometry and model
The global model consists of five separate metal stampings meshed with S4R and S3R shell elements.
An exploded view of the global finite element model is shown in Figure 1.1.19–1. The stampings are
stacked one upon the other by collapsing the configuration in the 3-direction. All the shell elements
are 0.5 mm thick, with all nodes positioned at the mid-surface of each shell. The separate meshes are
connected together with BEAM-type MPCs between corresponding perimeter nodes on the large bolt
holes through each layer. The nodes on the edges of the two small holes at the bottom of Layer 1 are
constrained in all six degrees of freedom, representing the attachment point to ground. The translational
degrees of freedom of the nodes around the perimeter of Layer 2 are also constrained, representing the
far-field boundary condition in that plate.
Several surface definitions are used to model the contact between the various adjacent layers. The
contact definitions prevent unwanted penetration between shell element layers. The small-sliding contact
formulation is employed. Most of the contact in this problem is between adjacent layers, but there is also
direct contact between Layer 2 and Layer 4. To avoid overconstraints, it is important that no point on
Layer 4 simultaneously contact Layer 3 and Layer 2; therefore, node-based surfaces are used for the
slave surfaces. This precludes accurate calculation of contact stresses, but that is not important in this
case since more accurate contact stresses are obtained in the submodel.
1.1.19–1
Abaqus Version 6.12 ID:
Printed on:
SUBMODELING OF A STACKED SHEET METAL ASSEMBLY
All five stampings are made of steel and are modeled as an elastic-plastic material. The elastic
modulus is 207,000 MPa, Poisson’s ratio is 0.3, and the yield stress is 250 MPa. The metal plasticity
definition includes moderate strain hardening.
The submodel stampings are truncated versions of the global model, located in the same physical
position as the global model. In this case these are the regions of concern for high stresses and potential
failure of the joint. The submodel is discretized with a finer mesh than the global model to provide
a higher level of accuracy. Figure 1.1.19–2 shows an exploded view of the submodel. Because the
stampings in the submodel contain the large bolt holes, the submodel contains BEAM-type MPCs in a
manner analogous to that in the global model.
The submodel has several surface definitions and contact pairs to avoid penetration of one stamping
into another. The submodel contains no node-based surfaces, however. The contact is modeled as
element-based surface-to-surface in each layer.
The material definition and shell thicknesses in the submodel are the same as those in the global
model.
Results and discussion
The global model is loaded by enforcing prescribed boundary conditions on the protruding edge of Layer
3. This edge is displaced −5.0 mm in the 1-direction and −12.5 mm in the 3-direction. Figure 1.1.19–3
shows the deformed shape of the global model. The displacements at the nodes are saved to the results
file for later use by the submodel analysis.
The submodel driven nodes are loaded using a submodel boundary condition. The perimeter nodes
of each layer of the submodel that correspond to a “cut” out of the global geometry are driven by the
interpolated nodal displacement results in the global results file. Each driven node set is in a separate shell
layer. Therefore, the submodel analysis contains multiple submodels, which designate the global model
element sets to be searched for the responses that drive the submodel driven node sets. For example, the
driven nodes in submodel Layer 1 (node set L1BC) are driven by the results for the global element set
which contains the elements of (global) Layer 1 (element set LAYER1). The driven nodes for Layers
2–4 are specified in a similar way. Because submodel Layer 5 has no driven nodes, only four submodels
are required.
Figure 1.1.19–4 shows the deformed shape of the submodel. Figure 1.1.19–5 and Figure 1.1.19–6
show contour plots of the out-of-plane displacements in Layer 2 for the global model and submodel,
respectively. In both cases the displacement patterns are similar; however, the maximum displacement
predicted by the global model is about 7.8% larger than that predicted by the submodel.
Input files
stackedassembly_s4r_global.inp
stackedassembly_s4r_global_mesh.inp
stackedassembly_s4r_sub.inp
stackedassembly_s4r_sub_mesh.inp
S4R global model.
Key input data for the S4R global model.
S4R submodel.
Key input data for the S4R submodel.
1.1.19–2
Abaqus Version 6.12 ID:
Printed on:
SUBMODELING OF A STACKED SHEET METAL ASSEMBLY
Layer 5
Layer 4
Layer 3
Layer 2
Layer 1
231
Figure 1.1.19–1
Exploded view of global model.
1.1.19–3
Abaqus Version 6.12 ID:
Printed on:
SUBMODELING OF A STACKED SHEET METAL ASSEMBLY
Layer 5
Layer 4
Layer 3
Layer 2
Layer 1
2
3
1
Figure 1.1.19–2
Exploded view of submodel.
1.1.19–4
Abaqus Version 6.12 ID:
Printed on:
SUBMODELING OF A STACKED SHEET METAL ASSEMBLY
2
1
3
Figure 1.1.19–3
2
Deformed shape of global model.
1
3
Figure 1.1.19–4
Deformed shape of submodel.
1.1.19–5
Abaqus Version 6.12 ID:
Printed on:
SUBMODELING OF A STACKED SHEET METAL ASSEMBLY
U, U3
+2.046e-01
-1.453e-01
-4.951e-01
-8.450e-01
-1.195e+00
-1.545e+00
-1.895e+00
-2.244e+00
-2.594e+00
-2.944e+00
-3.294e+00
-3.644e+00
-3.994e+00
2
3
1
Layer 2
Figure 1.1.19–5
Out-of-plane displacement in Layer 2, global model.
U, U3
-1.437e+00
-1.626e+00
-1.815e+00
-2.004e+00
-2.193e+00
-2.382e+00
-2.571e+00
-2.760e+00
-2.949e+00
-3.138e+00
-3.327e+00
-3.516e+00
-3.705e+00
2
3
1
Layer 2
Figure 1.1.19–6
Out-of-plane displacement in Layer 2, submodel.
1.1.19–6
Abaqus Version 6.12 ID:
Printed on:
THREADED CONNECTION
1.1.20
AXISYMMETRIC ANALYSIS OF A THREADED CONNECTION
Product: Abaqus/Standard
Threaded connectors are commonly used components in the piping and offshore industry. They must
withstand a variety of loading conditions: thread engagement, torque, bending, axial pullout, internal
pressure under operating and overload conditions, and potential fluid leakage through threaded connections.
Abaqus provides a wide range of modeling, analysis, and output capabilities that can be used to assess the
design of a connector under these and other loading conditions.
Two Abaqus methods that are particularly useful for analyzing threaded connectors are the specification
of an allowable contact interference and of pressure penetration loads.
•
The automatic “shrink” fit method can be used to automatically resolve the overclosure of two contacting
surfaces. This method is applicable only during the first step of an analysis, and it cannot be used with
self-contact. See “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4 of the Abaqus
Analysis User’s Manual, for details.
•
The surface-based pressure penetration capability described in “Pressure penetration loading,”
Section 36.1.7 of the Abaqus Analysis User’s Manual, is used to simulate pressure penetration between
contacting surfaces. This capability is provided for simulating cases where a joint between two
deforming bodies (for example, between two components threaded onto each other) or between a
deforming body and a rigid surface (such as a soft gasket used in a joint) is exposed at one or multiple
ends to a fluid pressure. This pressure will penetrate into the joint and load the surfaces forming the
joint until some area of the surfaces is reached where the contact pressure between the abutting surfaces
exceeds the critical value specified in the pressure penetration load, cutting off further penetration.
The contact output variables in Abaqus can provide the designer a wealth of information about the
performance of a connector during all steps of an analysis. When modeling surface-based contact with
axisymmetric elements (CAX- and CGAX-type elements) an output quantity of particular use is the
maximum torque that can be transmitted about the z-axis by a specified contact pair. The maximum torque,
T, is a scalar value defined as
where p is the pressure transmitted across the interface, r is the radius to a point on the interface, and s is the
current distance along the interface in the r–z plane. T is not a real torque; it is a computed limit of torque
that a contact pair may transmit about the z-axis assuming that all the slave nodes on the contact surface are
slipping and that the friction coefficient is set to 1. The actual maximum torque that can be transmitted about
the z-axis by a specified contact pair can be estimated by scaling T by the friction coefficient specified for the
contact pair. The value of T can be output by requesting the contact output variable CTRQ.
This example demonstrates the usefulness of the specification of allowable contact interference and of
pressure penetration loads as well as the Abaqus contact output variables in an axisymmetric analysis of a
particular threaded connector.
1.1.20–1
Abaqus Version 6.12 ID:
Printed on:
THREADED CONNECTION
Geometry and model
A three-dimensional cut-away view of the threaded connection assembly analyzed in this example
is shown in Figure 1.1.20–1. Although the actual threads are helical, they are represented with an
axisymmetric geometry. Previous experience has shown this simplification to be appropriate for these
types of problems. Both the “pin” and the “box” are made from steel with a Young’s modulus of
207 GPa (30 × 106 psi) and a Poisson’s ratio of 0.3, which is characterized by a von Mises plasticity
model. The unthreaded section of the pin has inner and outer radii of 48.6 mm (1.913 in) and 57.2 mm
(2.25 in), respectively. The major diameter of the threads on the pin (diameter measured at the crest of
the threads) is slightly larger than the major diameter of the threads on the box (diameter measured at the
roots of the threads); thus, there is an initial interference between the threads on the pin and on the box.
The deformed axisymmetric mesh (after the initial interference has been resolved) in the vicinity
of the threads is illustrated in Figure 1.1.20–2. Contact is modeled by the interaction of contact surfaces
defined by grouping specific faces of the elements in the contacting regions.
Loading and boundary conditions
Two analyses of the threaded connection are performed: an axisymmetric analysis using CAX4 elements
and an axisymmetric analysis with twist using CGAX4 elements. The first four steps for the two analyses
are identical. The CGAX4 model has an additional fifth step.
The initial interference fit of the threads on the pin and box is resolved in the first step using the
automatic “shrink” fit method with a friction coefficient of 0. In the second step the assembly is held fixed
while the friction coefficient is changed from 0 to 0.1 using changes to friction properties. An internal
gauge pressure of 0.689 MPa (100 psi) is applied to the connector in the third step. The pressure on the
contact surfaces is applied using pressure penetration loading. In the first three steps the displacements
in the 2-direction are constrained to be zero at both ends of the assembly. To simulate an axial load in the
fourth step, a displacement boundary condition of −0.254 cm (−0.1 in) is applied to the end of the box in
the 2-direction. In the fifth step for the CGAX4 model the end of the pin is held fixed while the end of
the box is rotated 0.1 radians about the 2-axis, simulating a torque being applied to the connector. The
actual torques generated about the 2-axis by the frictional stresses in the fifth step are given by the output
variable CMS2. This value is compared to the estimated value given by CTRQ for the fourth step.
Results and discussion
All analyses are performed as large-displacement analyses. The results from the first four steps for
both models are identical. Figure 1.1.20–3 and Figure 1.1.20–4, respectively, show the Mises stress
distributions in the threaded assembly after the overclosure has been resolved in Step 1 and after the
displacement boundary condition has been applied in Step 4. As is illustrated in Figure 1.1.20–4, some
of the threads on the pin are beginning to pull out at the end of Step 4. However, plots of the pressure
penetration on the contact surface of the box in Figure 1.1.20–5 and Figure 1.1.20–6 show that the seal
of the threads is maintained; thus, no leakage is indicated. If the seal had failed, the penetration pressure
on the box surface in contact with the pin would be 0.689 MPa (100 psi) instead of 0. Other contact
1.1.20–2
Abaqus Version 6.12 ID:
Printed on:
THREADED CONNECTION
output variables such as CPRESS and COPEN provide additional information about the contact state
throughout the analysis.
The scaled values of CTRQ (scaled by the friction coefficient of 0.1) and the values of CMS2 for
all five steps in the CGAX4 analysis are illustrated in Figure 1.1.20–7. The value of CTRQ at the end
of Step 4 is 1.22 × 106 lb-in, which translates into an estimated maximum torque of 1.22 × 105 lb-in
for a friction coefficient of 0.1. The value of CMS2 computed during Step 5 for the CGAX4 model is
1.18 × 105 lb-in. The 3.7% difference in this example between the predicted and actual torque values
can be attributed to a slight change in the normal pressure distribution between the contact surfaces that
occurs when the box is rotated. The value of CMS2 is zero for the first four steps since no frictional
stresses are generated between the contact surfaces until the fifth step. The value of CTRQ increases in
the first step as the overclosure is resolved and dips in the fourth step due to the change in the contact
pressure as the box is pulled away from the pin (see Figure 1.1.20–7).
Acknowledgments
SIMULIA gratefully acknowledges the ExxonMobil Upstream Research Corporation for their
cooperation in implementing the CTRQ output variable and for supplying the geometry, mesh, and
material properties used in this example.
Input files
threadedconnector_cax4.inp
threadedconnector_cax4_n.inp
threadedconnector_cax4_e.inp
threadedconnector_cgax4.inp
threadedconnector_cgax4_n.inp
threadedconnector_cgax4_e.inp
Axisymmetric analysis of the threaded connector using
CAX4 elements.
Node definitions for the axisymmetric analysis of the
threaded connector using CAX4 elements.
Element definitions for the axisymmetric analysis of the
threaded connector using CAX4 elements.
Axisymmetric analysis of the threaded connector using
CGAX4 elements.
Node definitions for the axisymmetric analysis of the
threaded connector using CGAX4 elements.
Element definitions for the axisymmetric analysis of the
threaded connector using CGAX4 elements.
1.1.20–3
Abaqus Version 6.12 ID:
Printed on:
THREADED CONNECTION
box
pin
1
2
3
Figure 1.1.20–1
Three-dimensional cut-away view of the threaded connection.
Figure 1.1.20–2 Axisymmetric mesh in the vicinity of the threads
after the initial interference has been resolved.
1.1.20–4
Abaqus Version 6.12 ID:
Printed on:
THREADED CONNECTION
S, Mises
(Ave. Crit.: 75%)
+1.867e+05
+1.714e+05
+1.561e+05
+1.408e+05
+1.254e+05
+1.101e+05
+9.483e+04
+7.952e+04
+6.421e+04
+4.890e+04
+3.359e+04
+1.828e+04
+2.974e+03
Figure 1.1.20–3 Stress distribution in the threads after the
initial overclosure has been resolved.
S, Mises
(Ave. Crit.: 75%)
+2.132e+05
+1.956e+05
+1.781e+05
+1.605e+05
+1.430e+05
+1.255e+05
+1.079e+05
+9.038e+04
+7.284e+04
+5.530e+04
+3.777e+04
+2.023e+04
+2.689e+03
Figure 1.1.20–4
Stress distribution in the threads after axial loading.
1.1.20–5
Abaqus Version 6.12 ID:
Printed on:
THREADED CONNECTION
PPRESS
SURFBOX/SURFPIN
+1.000e+02
+8.333e+01
+6.667e+01
+5.000e+01
+3.333e+01
+1.667e+01
-3.815e-06
-1.667e+01
-3.333e+01
-5.000e+01
-6.667e+01
-8.333e+01
-1.000e+02
Figure 1.1.20–5
Figure 1.1.20–6
Pressure penetration on box contact surface after axial loading.
Plot of pressure penetration on box contact surface after axial loading.
1.1.20–6
Abaqus Version 6.12 ID:
Printed on:
THREADED CONNECTION
CMS2
0.1*CTRQ
Figure 1.1.20–7
Comparison of 0.1*CTRQ to CMS2 for the CGAX4 model.
1.1.20–7
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
1.1.21
DIRECT CYCLIC ANALYSIS OF A CYLINDER HEAD UNDER CYCLIC THERMALMECHANICAL LOADINGS
Product: Abaqus/Standard
The prediction of fatigue and failure in structures is fundamental in assessing product performance. This
example demonstrates the use of the direct cyclic analysis procedure to obtain results that can be used for
fatigue life calculations.
It is well known that a highly loaded structure, such as a cylinder head in an engine subjected to large
temperature fluctuations and clamping loads, can undergo plastic deformations. After a number of repetitive
loading cycles there will be one of three possibilities: elastic shakedown, in which case there is no danger
of low-cycle fatigue; plastic shakedown, leading to a stabilized plastic strain cycle, in which case energy
dissipation criteria will be used to estimate the number of cycles to failure; and plastic ratchetting, in which
case the design is rejected. The classical approach to obtaining the response of such a structure is to apply the
periodic loading repetitively to the structure until a stabilized state is obtained or plastic ratchetting occurs.
This approach can be quite expensive, since it may require application of many loading cycles to obtain the
steady response. To avoid the considerable numerical expense associated with such a transient analysis, the
direct cyclic analysis procedure, described in “Direct cyclic analysis,” Section 6.2.6 of the Abaqus Analysis
User’s Manual, can be used to calculate the cyclic response of the structure directly.
Geometry and model
The cylinder head analyzed in this example is depicted in Figure 1.1.21–1. The cylinder head (which is
a single cylinder) has three valve ports, each with an embedded valve seat; two valve guides; and four
bolt holes used to secure the cylinder head to the engine block.
The body of the cylinder head is made from aluminum with a Young’s modulus of 70 GPa, a yield
stress of 62 MPa, a Poisson’s ratio of 0.33, and a coefficient of thermal expansion of 22.6 × 10–6 per °C
at room temperature. In this example the region in the vicinity of the valve ports, where the hot exhaust
gases converge, is subjected to cyclic temperature fluctuations ranging from a minimum value of 35°C
to a maximum value of 300°C. The temperature distribution when the cylinder head is heated to its
peak value is shown in Figure 1.1.21–2. Under such operating conditions plastic deformation, as well
as creep deformation, is observed. The two-layer viscoelastic-elastoplastic model, which is best suited
for modeling the response of materials with significant time-dependent behavior as well as plasticity at
elevated temperatures, is used to model the aluminum cylinder head (see “Two-layer viscoplasticity,”
Section 23.2.11 of the Abaqus Analysis User’s Manual). This material model consists of an elasticplastic network that is in parallel with an elastic-viscous network. The Mises metal plasticity model with
kinematic hardening is used in the elastic-plastic network, and the power-law creep model with strain
hardening is used in the elastic-viscous network. Since the elastic-viscoplastic response of aluminum
varies greatly over this range of temperatures, temperature-dependent material properties are specified.
The two valve guides are made of steel, with a Young’s modulus of 106 GPa and a Poisson’s ratio
of 0.35. The valve guides fit tightly into two of the cylinder head valve ports and are assumed to behave
1.1.21–1
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
elastically. The interface between the two components is modeled by using matched meshes that share
nodes along the interface.
The three valve seats are made of steel, with a Young’s modulus of 200 GPa and a Poisson’s ratio
of 0.3. The valve seats are press-fit into the cylinder head valve ports. This is accomplished by defining
radial constraint equations of the form
between the nodes on the valve seat surface and
the nodes on the valve port surface, where
is the radial displacement on the valve port,
is the
radial displacement on the valve seat, and
is a reference node. During the first step of the analysis
a prescribed displacement is applied to the reference node, resulting in normal pressures developing
between the two components. The valve seats are assumed to behave elastically.
All of the structural components (the cylinder head, the valve guides, and the valve seats) are
modeled with three-dimensional continuum elements. The model consists of 19394 first-order brick
elements (C3D8) and 1334 first-order prism elements (C3D6), resulting in a total of about 80,000 degrees
of freedom. The C3D6 elements are used only where the complex geometry precludes the use of C3D8
elements.
Loading and boundary constraints
The loads are applied to the assembly in two analysis steps. In the first step the three valve seats are
press-fit into the corresponding cylinder head valve port using linear multi-point equation constraints
and prescribed displacement loadings as described above. A static analysis procedure is used for this
purpose. The cyclic thermal loads are applied in the second analysis step. It is assumed that the cylinder
head is securely fixed to the engine block through the four bolt holes, so the nodes along the base of the
four bolt holes are secured in all directions during the entire simulation.
The cyclic thermal loads are obtained by performing an independent thermal analysis. In this
analysis three thermal cycles are applied to obtain a steady-state thermal cycle. Each thermal cycle
involves two steps: heating the cylinder head to the maximum operating temperature and cooling it to
the minimum operating temperature using concentrated flux and film conditions. The nodal temperatures
for the last two steps (one thermal cycle) are assumed to be a steady-state solution and are stored in
a results (.fil) file for use in the subsequent thermal-mechanical analysis. The maximum value of
the temperature occurs in the vicinity of the valve ports where the hot exhaust gases converge. The
temperature in this region (node 50417) is shown in Figure 1.1.21–3 as a function of time for a steadystate cycle.
In the second step of the mechanical analysis cyclic nodal temperatures generated from the previous
heat transfer analysis are applied. The direct cyclic procedure with a fixed time incrementation of 0.25
and a load cycle period of 30 is specified in this step, resulting in a total number of 120 increments for
one iteration. The number of terms in the Fourier series and the maximum number of iterations are 40
and 100, respectively.
For comparison purposes the same model is also analyzed using the classical transient analysis,
which requires 20 repetitive steps before the solution is stabilized. A cyclic temperature loading with a
constant time incrementation of 0.25 and a load cycle period of 30 is applied in each step.
1.1.21–2
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Results and discussion
One of the considerations in the design of a cylinder head is the stress distribution and deformation
in the vicinity of the valve ports. Figure 1.1.21–4 shows the Mises stress distribution in the cylinder
head at the end of a loading cycle (iteration 75, increment 120) in the direct cyclic analysis. The total
strain distribution at the same time in the direct cyclic analysis is shown in Figure 1.1.21–5. The
deformation and stress are most severe in the vicinity of the valve ports, making this region critical in
the design. The results shown in Figure 1.1.21–6 through Figure 1.1.21–16 are measured in this region
(element 50152, integration point 1). Figure 1.1.21–6, Figure 1.1.21–7, and Figure 1.1.21–8 show the
evolution of the stress component, plastic strain component, and viscous strain component, respectively,
in the global 1-direction throughout a complete load cycle during iterations 50, 75, and 100 in the direct
cyclic analysis. The time evolution of the stress versus the plastic strain, shown in Figure 1.1.21–9, is
obtained by combining Figure 1.1.21–6 with Figure 1.1.21–7. Similarly, the time evolution of the stress
versus the viscous strain, shown in Figure 1.1.21–10, is obtained by combining Figure 1.1.21–6 with
Figure 1.1.21–8. The shapes of the stress-strain curves remain unchanged after iteration 75, as do the
peak and mean values of the stress over a cycle. However, the mean value of the plastic strain and the
mean value of the viscous strain over a cycle continue to grow from one iteration to another iteration,
indicating that the plastic ratchetting occurs in the vicinity of the valve ports.
Similar results for the evolution of stress versus plastic strain and the evolution of stress versus
viscous strain during cycles 5, 10, and 20 obtained using the classical transient approach are shown in
Figure 1.1.21–11 and Figure 1.1.21–12, respectively. The plastic ratchetting is observed to be consistent
with that predicted using the direct cyclic approach. A comparison of the evolution of stress versus
plastic strain obtained during iteration 100 in the direct cyclic analysis with that obtained during cycle 20
in the transient approach is shown in Figure 1.1.21–13. A similar comparison of the evolution of stress
versus viscous strain obtained using both approaches is shown in Figure 1.1.21–14. The shapes of the
stress-strain curves are similar in both cases.
One advantage of using the direct cyclic procedure, in which the global stiffness matrix is inverted
only once, instead of the classical approach in Abaqus/Standard is the cost savings achieved. In this
example the total computational time leading to the first occurrence of plastic ratchetting in the direct
cyclic analysis (75 iterations) is approximately 70% of the computational time spent in the transient
analysis (20 steps). The savings will be more significant as the problem size increases.
Additional cost savings for the solution can often be obtained by using a smaller number of terms
in the Fourier series and/or a smaller number of increments in an iteration. In this example, if 20 rather
than 40 Fourier terms are chosen, the total computational time leading to the first occurrence of plastic
ratchetting in the direct cyclic analysis (75 iterations) is approximately 65% of the computational time
spent in the transient analysis (20 steps). Furthermore, if a fixed time incrementation of 0.735 rather than
0.25 is specified, leading to a total number of 41 increments for one iteration, the total computational
time in the direct cyclic analysis is reduced by a factor of three without compromising the accuracy of
the results. A comparison of the evolution of stress versus plastic strain obtained using fewer Fourier
terms during iteration 75 is shown in Figure 1.1.21–15. A similar comparison of the evolution of stress
versus viscous strain obtained using fewer Fourier terms is shown in Figure 1.1.21–16. The shapes of
1.1.21–3
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
the stress-strain curves and the amount of energy dissipated during the cycle are similar in both cases,
although the case with fewer Fourier terms provides less accurate stress results.
Another advantage of using the direct cyclic approach instead of the classical approach is that
the likelihood of plastic ratchetting or stabilized cyclic response can be predicted automatically by
comparing the displacement and residual coefficients with some internal control variables. There is no
need to visualize the detailed results for the whole model throughout the loading history, which leads to
a further reduction of the data storage and computational time associated with output. For this example
examination of the displacement and the residual coefficients written to the message (.msg) file makes
it clear that the constant term in the Fourier series does not stabilize and, thus, plastic ratchetting occurs.
Acknowledgments
SIMULIA gratefully acknowledges PSA Peugeot Citroën and the Laboratory of Solid Mechanics of the
Ecole Polytechnique (France) for their cooperation in developing the direct cyclic analysis capability and
for supplying the geometry and material properties used in this example.
Input files
dircyccylinderhead_heat.inp
dircyccylinderhead_heat_mesh.inp
dircyccylinderhead_heat_sets.inp
dircyccylinderhead_heat_load1.inp
dircyccylinderhead_heat_load2.inp
dircyccylinderhead_dcm.inp
dircyccylinderhead_dcm_mesh.inp
dircyccylinderhead_dcm_sets.inp
dircyccylinderhead_dcm_eqc.inp
dircyccylinderhead_dcm_ps.inp
Input data for the heat transfer analysis.
Node and element definitions for the heat transfer
analysis.
Node set, element set, and surface definitions for the heat
transfer analysis.
Loading definitions during the heating process for the heat
transfer analysis.
Loading definitions during the cooling process for the
heat transfer analysis.
Input data for the direct cyclic analysis.
Node and element definitions for the direct cyclic
analysis.
Node set and element set definitions for the direct cyclic
analysis.
Kinematic constraint definitions for the direct cyclic
analysis.
Post output for the direct cyclic analysis.
References
•
Maitournam, H., B. Pommier, and J. J. Thomas, “Détermination de la réponse asymptotique d’une
structure anélastique sous chargement thermomécanique cyclique,” C. R. Mécanique, vol. 330,
pp. 703–708, 2002.
•
Maouche, N., H. Maitournam, and K. Dang Van, “On a new method of evaluation of the inelastic
state due to moving contacts,” Wear, pp. 139–147, 1997.
1.1.21–4
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
•
Nguyen-Tajan, T. M. L., B. Pommier, H. Maitournam, M. Houari, L. Verger, Z. Z. Du,
and M. Snyman, “Determination of the stabilized response of a structure undergoing cyclic
thermal-mechanical loads by a direct cyclic method,” ABAQUS Users’ Conference Proceedings,
2003.
Valve seats
Valve guides
Figure 1.1.21–1
Figure 1.1.21–2
A cylinder head model.
Temperature distribution when the cylinder head is heated to its peak value.
1.1.21–5
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
280.00
Temperature
240.00
200.00
160.00
120.00
80.00
40.00
0.00
10.00
20.00
30.00
Time
Figure 1.1.21–3 Temperature at node 50417 as a function
of time for a steady-state cycle.
Figure 1.1.21–4
Mises stress distribution in the cylinder head at the end of a loading cycle
(iteration 75, increment 120) in the direct cyclic analysis.
1.1.21–6
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Figure 1.1.21–5 Total strain distribution in the cylinder head at the end of a loading cycle
(iteration 75, increment 120) in the direct cyclic analysis.
Iteration 50
Iteration 75
Iteration 100
Figure 1.1.21–6 Evolution of the stress component in the global 1-direction during
iterations 50, 75, and 100 in the direct cyclic analysis.
1.1.21–7
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Iteration 50
Iteration 75
Iteration 100
Figure 1.1.21–7
Evolution of the plastic strain component in the global 1-direction during
iterations 50, 75, and 100 in the direct cyclic analysis.
Iteration 50
Iteration 75
Iteration 100
Figure 1.1.21–8
Evolution of the viscous strain component in the global 1-direction during
iterations 50, 75, and 100 in the direct cyclic analysis.
1.1.21–8
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Iteration 50
Iteration 75
Iteration 100
Figure 1.1.21–9 Evolution of the stress versus plastic strain during
iterations 50, 75, and 100 in the direct cyclic analysis.
Iteration 50
Iteration 75
Iteration 100
Figure 1.1.21–10 Evolution of the stress versus viscous strain
during iterations 50, 75, and 100 in the direct cyclic analysis.
1.1.21–9
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Cycle 5
Cycle 10
Cycle 20
Figure 1.1.21–11 Evolution of the stress versus plastic strain
during steps 5, 10, and 20 in the transient analysis.
Cycle 5
Cycle 10
Cycle 20
Figure 1.1.21–12 Evolution of the stress versus viscous strain
during steps 5, 10, and 20 in the transient analysis.
1.1.21–10
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Classical approach (cycle=20)
Direct cyclic analysis (iteration=100)
Figure 1.1.21–13 Comparison of the evolution of stress versus plastic strain obtained with
the direct cyclic analysis and transient analysis approaches.
Classical approach (cycle=20)
Direct cyclic analysis (iteration=100)
Figure 1.1.21–14 Comparison of the evolution of stress versus viscous strain obtained with
the direct cyclic analysis and transient analysis approaches.
1.1.21–11
Abaqus Version 6.12 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Direct cyclic analysis (n=40)
Direct cyclic analysis (n=20)
Figure 1.1.21–15 Comparison of the evolution of stress versus plastic strain obtained using
different numbers of Fourier terms during iteration 75 in a direct cyclic analysis.
Direct cyclic analysis (n=40)
Direct cyclic analysis (n=20)
Figure 1.1.21–16 Comparison of the evolution of stress versus viscous strain obtained using
different numbers of Fourier terms during iteration 75 in a direct cyclic analysis.
1.1.21–12
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
1.1.22
EROSION OF MATERIAL (SAND PRODUCTION) IN AN OIL WELLBORE
Product: Abaqus/Standard
This example demonstrates the use of adaptive meshing and adaptive mesh constraints in Abaqus/Standard
to model the large-scale erosion of material such as sand production in an oil well as oil is extracted. In
Abaqus/Standard the erosion of material at the external surface is modeled by declaring the surface to be
part of an adaptive mesh domain and by prescribing surface mesh motions that recede into the material.
Abaqus/Standard will then remesh the adaptive mesh domain using the same mesh topology but accounting
for the new location of the surface. All the material point and node point quantities will be advected to their
new locations. This example also demonstrates the use of mesh-to-mesh solution mapping in a case where a
new mesh topology is desired to continue the analysis beyond a certain stage.
Problem description
The process of optimizing the production value of an oil well is complex but can be simplified as a
balance between the oil recovery rate (as measured by the volumetric flow rate of oil), the sustainability
of the recovery (as measured by the amount of oil ultimately recovered), and the cost of operating the
well. In practice, achieving this balance requires consideration of the erosion of rock in the wellbore, a
phenomenon that occurs when oil is extracted under a sufficiently high pressure gradient. This erosion
phenomenon is generally referred to as “sand production.” Depending on the flow velocities the sand
may accumulate in the well, affecting the sustainability of recovery, or it may get carried to the surface
along with the oil. The sand in the oil causes erosion in the piping system and its components such
as chokes and pipe bends, increasing the costs of operating the well. Excessive sand production is,
therefore, undesirable and will limit oil recovery rates. A typical measure of these limits on recovery
rates is the so-called “sandfree rate.” A sandfree rate might be based on direct damage caused by sand
production or might be based on the cost of sand management systems that limit the damage of the
sand. The former measure is called the maximum sandfree rate, or MSR. The latter measure is called the
acceptable sandfree rate, or ASR. The ASR concept has become possible with the availability of many
commercial sand management systems as well as new designs of piping components. The ASR concept
has also engendered a need for predicting the sand production rates to properly choose and size the sand
management systems and piping components. In this example we focus on measures that can be obtained
from Abaqus to predict these rates.
Geometry and model
The geometry of an oil well has two main components. The first is the wellbore drilled through the rock.
The second component is a series of perforation tunnels that project perpendicular to the wellbore axis.
These tunnels, which are formed by explosive shape charges, effectively increase the surface area of the
wellbore for oil extraction. The perforation tunnels are typically arranged to fan out in a helical fashion
around the wellbore, uniformly offset in both vertical spacing and azimuthal angle.
1.1.22–1
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
Three-dimensional model
The domain of the problem considered in the three-dimensional example is a 203 mm (8 in) thick circular
slice of oil-bearing rock with both the wellbore and perforation tunnels modeled. The domain has a
diameter of 10.2 m (400 in). The perforation tunnels emanate radially from the wellbore and are spaced
90° apart. Each perforation tunnel is 43.2 mm (1.7 in) diameter and 508 mm (20 in) long. The wellbore
has a radius of 158.8 mm (6.25 in). Due to symmetry only a quarter of the domain that contains one
perforation tunnel is modeled. Figure 1.1.22–1 shows the finite element model. The rock is modeled
with C3D8P elements, and the well’s casing is modeled with M3D4 elements.
Planar model
The planar model is a simplified version of the three-dimensional model, where the perforation tunnels
and wellbore casing are neglected. The rock is modeled with CPE4P elements. The model domain
consists of a quarter-symmetry square domain of length 10.2 m (400 in), with a single wellbore with a
radius of 158.8 mm (6.25 in). Figure 1.1.22–5 shows the finite element model. Figure 1.1.22–6 details
the region near the wellbore.
Material
A linear Drucker-Prager model with hardening is chosen for the rock, and the casing in the
three-dimensional model is linear elastic.
Loading
The loading sequence for a wellbore analysis generally includes
•
•
•
establishing geostatic equilibrium, based on the overburden loading;
simulation of material removal operations, including drilling the wellbore and forming the
perforation tunnel; and
applying a drawdown pressure in the wellbore to simulate pumping.
This sequence is modeled slightly differently in the three-dimensional and planar models.
Three-dimensional model
The analysis consists of five steps. First, a geostatic step is performed where equilibrium is achieved after
applying the initial pore pressure, the initial stress, and the distributed load representing the soil above
the perforation tunnel. The second step represents the drilling operation where the elements representing
the wellbore and the perforation tunnel are removed using the element removal capability in Abaqus
(see “Element and contact pair removal and reactivation,” Section 11.2.1 of the Abaqus Analysis User’s
Manual). In the third step the boundary conditions are changed to apply the pore pressure on the face
of the perforation tunnel. In the fourth step a steady-state soils analysis is carried out in which the pore
pressure on the perforation tunnel surface is reduced to the desired drawdown pressure of interest. The
fifth step consists of a soils consolidation analysis for four days during which the erosion occurs.
1.1.22–2
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
Planar model
The analysis consists of three steps. First, a geostatic step is performed where equilibrium is achieved
after applying the initial pore pressure and the initial stress, representing an underbalanced state on the
wellbore. The second step represents the drilling operation where the elements representing the wellbore
are removed using the element removal capability, and the boundary conditions are changed to apply the
pore pressure on the face of the perforation tunnel. The third step consists of a soils consolidation analysis
for 32 hours during which the erosion occurs. As discussed below in “Rezoning the planar model,” this
third step is interrupted in order to rezone the model.
Erosion criterion
There are two main sources of eroded material in a well bore. One of the sources is volumetric and is due
to the material that is broken up due to high stresses and transported by the fluid through the pores. The
other source is surface based and is due to the material that is broken up by the hydrodynamic action of
the flow on the surface. Depending on the properties of the oil-bearing strata and the flow velocities, one
or the other may be the dominant source of eroded material. Development of equations describing the
erosion in a well bore is an active research field. In this example we consider surface erosion only but
choose a form for the erosion equation that has dependencies that are similar to those used by Papamichos
and Stavropoulou for volumetric erosion. This approximation is reasonable because high stresses exist
only in a very thin layer surrounding the well bore. The erosion equation is
where
is the erosion velocity,
is the pore fluid velocity, c is the transport concentration, n is the
porosity, and is the so-called sand production coefficient. depends on the equivalent plastic strain
( ). It is zero below a cutoff equivalent plastic strain (
), is equal to
, and is
limited by a constant .
Both
and
must be determined experimentally. In this example
,
, and
. We choose
as recommended by Papamichos and Stavropoulo. These values are
chosen to show visible erosion in a reasonably short analysis time.
Adaptive mesh domain
Erosion is modeled during the final step of each analysis. The erosion equation describes the velocity
of material recession as a local function of solution quantities. Abaqus/Standard provides functionality
through adaptive meshing for imposing this surface velocity, maintaining its progression normal to the
surface as the surface moves, and adjusting subsurface nodes to account for large amounts of erosive
material loss.
Erosion itself is described through a spatial adaptive mesh constraint, which is applied to all the
nodes on the surface of the perforation tunnel. Adaptive mesh constraints can be applied only on
adaptive mesh domains; in this example a sufficiently large extent of the finite element mesh near the
wellbore and perforation tunnel surfaces is declared as the adaptive mesh domain. A cut section of the
1.1.22–3
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
adaptive mesh domain for the three-dimensional model, including the perforation tunnel, is shown in
Figure 1.1.22–2. The adaptive mesh domain for the planar model is the regular mesh near the wellbore
(refer to Figure 1.1.22–6 and Figure 1.1.22–8). Identification of the adaptive mesh domain will result in
smoothing of the near-surface mesh that is necessary to enable erosion to progress to arbitrary depths.
All the nodes on the boundary of the adaptive mesh domain where it meets the regular mesh must be
considered as Lagrangian to respect the adjacent nonadaptive elements.
A velocity adaptive mesh constraint is defined. The generality and solution dependence of the
erosion equation are handled by describing the erosion equation in user subroutine UMESHMOTION
(see “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6 of the Abaqus
Analysis User’s Manual). User subroutine UMESHMOTION is called at a given node for every mesh
smoothing sweep. Mesh velocities computed by the Abaqus/Standard meshing algorithm for that
node are passed into UMESHMOTION, which modifies them to account for the erosion velocities
computed at that node. The modified velocities are determined according to the equation for
,
where local results are needed for , n, and . To obtain these values, we request results for output
variables PEEQ, VOIDR, and FLVEL respectively, noting that void ratio is related to porosity by
. Since these output variables are all available at element material points,
the utility routine GETVRMAVGATNODE is used to obtain results extrapolated to the surface nodes
(see “Obtaining material point information averaged at a node,” Section 2.1.8 of the Abaqus User
Subroutines Reference Manual).
Rezoning the planar model
Rezoning, the process of creating a new mesh in the model’s deformed configuration, is a useful technique
in addressing element distortion in erosion problems.
The erosion model in this example is solution dependent in the sense that it defines an erosion
velocity as a function of local values of equivalent plastic strain, PEEQ, and fluid velocity, FLVEL. Since
these node-located results values are extrapolated from adjacent elements’ material point results, using
utility routine GETVRMAVGATNODE, the quality of the results used in the erosion model is dependent on
local element quality. In practice, as elements near the surface deform, there is a tendency for instability
in the erosion model.
This instability is mitigated by rezoning the model and providing a more regular mesh to continue
the analysis. The rezoned model is created in Abaqus/CAE, and transfer of state variables occurs using
mesh-to-mesh solution mapping in Abaqus/Standard. Rezoning occurs at 55,000 seconds (15.3 hours)
into the 32-hour erosion analysis of the planar model.
Extracting two-dimensional profiles and remeshing using Abaqus/CAE
The rezoned model is created by extracting the two-dimensional profile of the deformed rock region
from the output database for the original analysis. You perform this operation in Abaqus/CAE by
entering commands into the command line interface at the bottom of the Abaqus/CAE main window.
To extract the deformed geometry from the output database as an orphan mesh part, use the command
PartFromOdb, which takes the following arguments:
name
odb
The name of the orphan mesh part to be created.
The output database object returned from the command openOdb.
1.1.22–4
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
instance
The name of the part instance in the initial model in capital letters.
shape
Determines whether to import the part in its UNDEFORMED or DEFORMED
shape.
The command PartFromOdb returns a Part object that is passed to the command
Part2DGeomFrom2DMesh. This command creates a geometric Part object from the orphan
mesh imported earlier. It takes the following arguments:
name
The name of the part to be created.
part
The part object returned from the command PartFromOdb.
featureAngle
A float specifying the angle (in degrees) between line segments that triggers a break
in the geometry.
Once the profile of the deformed part has been created, you will prepare an input file for the
subsequent period in the erosion analysis as follows:
•
Reestablish all attributes that relate to the geometry of the deformed part. These attributes include
load and boundary condition definitions, and set and surface definitions.
•
•
•
Remesh the part.
Create a single consolidation step that completes the duration of your intended erosion period.
Write out the new input file.
Mesh-to-mesh solution mapping in Abaqus/Standard
The interpolation technique used in solution mapping is a two-step process. First, values of all solution
variables are obtained at the nodes of the old mesh by extrapolating the values from the integration points
to the nodes of each element and averaging those values over all elements abutting each node. The second
step is to locate each integration point in the new mesh with respect to the old mesh. The variables are
then interpolated from the nodes of the element in the old mesh to the location in the new mesh. All
solution variables are interpolated automatically in this way so that the solution can proceed on the new
mesh. Whenever a model is mapped, it can be expected that there will be some discontinuity in the
solution because of the change in the mesh. To address this discontinuity the rezone analysis includes a
geostatic step, which reestablishes equilibrium before the erosion process continues in a following step.
Results and discussion
The analysis scenarios and results differ between the three-dimensional and planar analyses.
Three-dimensional analysis
The consolidation analysis in which erosion takes place is run for a time period of four days to observe
the initiation of sand production and predict its initial rate. Figure 1.1.22–3 shows the perforation tunnel
at the end of four days where it is seen that the largest amount of material is eroded near the junction
of the wellbore and perforation tunnel. Further away from the wellbore boundary the amount of erosion
progressively decreases. This behavior is expected because there are high strains near the junction of
1.1.22–5
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
the wellbore and perforation tunnel, and the erosion criterion is active only for values of the equivalent
plastic strain above a threshold value.
The amount of the volume change due to erosion in an adaptive domain is available using the history
output variable VOLC. The actual amount of the solid material eroded depends on the porosity of the rock
and is obtained by multiplying VOLC by
. Figure 1.1.22–4 shows the volume change of the sand
produced in cubic inches over the time period of the consolidation step. As the material consolidates, the
erosion rate slows down. The stresses in the perforation hole reduce and stabilize over the time period.
From Figure 1.1.22–4 it can be concluded that the stresses generated by the drawdown pressure, the fluid
velocities, the wellbore and casing geometry, and the initial perforation tunnel geometry are such that
this perforation tunnel will produce sand at a more stable rate as oil recovery continues; however, this
rate could vary with further changes to the perforation tunnel caused by the erosion. At a design stage
any of these parameters could be modified to limit the sand production rate. Many perforation tunnels
emanate from a wellbore, and the total sand production from the wellbore will be the sum total of all the
perforation tunnels.
Planar analysis
The underbalanced consolidation analysis in which erosion takes place is run for a time period of 32 hours
to observe the initiation of sand production and predict its initial rate. Figure 1.1.22–7 shows the wellbore
at 15 hours, the end of the first analysis job. Based on this configuration a new mesh is created, as shown
in Figure 1.1.22–8. The final configuration of this model, representing 32 hours of erosion, is shown in
Figure 1.1.22–9. As expected, the results show that erosion continues outward from the location of the
maximum equivalent plastic straining. Figure 1.1.22–10 shows the total amount of sand produced, in
cubic inches per inch of depth, over the time period of the consolidation step.
Input files
exa_erosion.inp
exa_erosion_planar.inp
exa_erosion_planar_rezone.inp
exa_erosion.f
Three-dimensional model of the oil wellbore perforation
tunnel.
Planar model of the oil wellbore.
Rezone analysis of the planar model.
UMESHMOTION user subroutine.
Reference
•
Papamichos, E., and M. Stavropoulou, “An Erosion-Mechanical Model for Sand Production Rate
Prediction,” International Journal of Rock Mechanics and Mining Sciences, no. 35, pp. 4–5, Paper
No 090, 1998.
1.1.22–6
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
Figure 1.1.22–1
A cut section of the model showing the wellbore and perforation tunnel.
Figure 1.1.22–2 Half-section of the adaptive mesh domain
showing the wellbore face and the perforation tunnel.
1.1.22–7
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
PEEQ
(Avg: 75%)
+3.314e−02
+3.038e−02
+2.762e−02
+2.485e−02
+2.209e−02
+1.933e−02
+1.657e−02
+1.381e−02
+1.105e−02
+8.285e−03
+5.523e−03
+2.762e−03
+0.000e+00
Figure 1.1.22–3
Shape of the perforation tunnel after four days of erosion.
Figure 1.1.22–4 Total sand production volume change in a single perforation tunnel
indicating a stabilized rate as the consolidation continues.
1.1.22–8
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
Figure 1.1.22–5
Figure 1.1.22–6
Planar model mesh.
Planar model mesh: wellbore region detail.
1.1.22–9
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
PEEQ
(Avg: 75%)
+4.882e−02
+4.475e−02
+4.068e−02
+3.661e−02
+3.254e−02
+2.848e−02
+2.441e−02
+2.034e−02
+1.627e−02
+1.220e−02
+8.136e−03
+4.068e−03
+0.000e+00
Figure 1.1.22–7
Equivalent plastic strain distribution and eroded shape of the wellbore.
Figure 1.1.22–8
Planar model mesh: wellbore region detail: rezone analysis.
1.1.22–10
Abaqus Version 6.12 ID:
Printed on:
EROSION OF MATERIAL
PEEQ
(Avg: 75%)
+9.966e−02
+9.136e−02
+8.305e−02
+7.475e−02
+6.644e−02
+5.814e−02
+4.983e−02
+4.153e−02
+3.322e−02
+2.492e−02
+1.661e−02
+8.305e−03
+0.000e+00
Figure 1.1.22–9
Equivalent plastic strain distribution and eroded shape of the wellbore: rezone analysis.
exa_erosion_planar
exa_erosion_planar_rezone
[x1.E−3]
8.0
Sand loss (in^3 / in)
6.0
4.0
2.0
0.0
0.
5.
10.
15.
20.
25.
30.
Time (hours)
Figure 1.1.22–10
Total sand production volume per unit of depth.
1.1.22–11
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
1.1.23
SUBMODEL STRESS ANALYSIS OF PRESSURE VESSEL CLOSURE HARDWARE
Product: Abaqus/Standard
Objectives
This example demonstrates the use of surface-based submodeling as a technique to obtain solutions that
are more accurate than those obtained using node-based submodeling in cases where:
•
•
the submodel displacement field is expected to differ from the global model displacement field by
a rigid translation and
the geometry of the submodel differs from the global model in a region whose response is primarily
load controlled.
This section details scenarios for each of these cases.
Application description
This example examines the stress behavior of closure head standpipe structures in a nuclear reactor vessel
closure assembly. The vessel assembly forms the pressure boundary surrounding the fuel core. This
example considers the following loading conditions:
•
•
•
pre-tension load in the stud bolts,
constant internal pressure, and
loading due to the control rod drive mechanism (CDM) plug.
The loading conditions cover the most basic structural operation of a reactor vessel. The International
System of units (SI) is used in the following sections to describe the model. The analysis itself is
performed in English units. The model and analysis are derived from details of the Shippingport
pressurized water reactor (1958).
Geometry
The problem domain comprises a cylindrical vessel shell, a hemispherical bottom head, a dome-shaped
closure head, and the closure and seal assembly, as shown in Figure 1.1.23–1. The overall height of the
vessel shell including the bottom head is 7650 mm (301 in). The bottom head has an inner radius of
1410 mm (55.5 in) and a thickness of 157 mm (6.18 in). The inlet nozzles on the bottom head are not
considered in this example. The inner radius of the vessel shell is 1380 mm (54.5 in), and the thickness
is 213 mm (8.40 in). The closure head has a height of 2330 mm (91.8 in), an inner radius of 1310 mm
(51.5 in), and a thickness of 210 mm (8.25 in).
The closure head includes eight standpipes with CDM plugs inserted in each. The standpipes have
an inside diameter of 472 mm (12 in) and an outside diameter of 630 mm (16 in) and extend roughly
1000 mm (25 in) above the closure head. The CDM plugs have an outside diameter of 465 mm (11.8 in)
and a flange diameter of 630 mm (16 in) and are 748 mm (19 in) tall. Each CDM plug sits in a closure
head standpipe on a 404 mm (10.25 in) diameter ledge.
1.1.23–1
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
The closure head is attached to the vessel shell by a seal and closure assembly. The assembly
includes 40 stud bolts passing through the bolting flanges of the closure head and the vessel shell, each
of which is restrained by two cap nuts (one on each end). Each stud bolt is 2290 mm (90 in) in length
and has a diameter of 146 mm (5.75 in). The closure nuts are 304 mm (12 in) long with a thickness of
28.6 mm (1.13 in). To complete the closure assembly, an Omega seal is welded to the under surface of
the closure head and top surface of the vessel shell.
Materials
All components are constructed of high-strength steel.
Boundary conditions and loading
A pre-tension load of 2200 kN (5 × 106 lbf) is applied to each bolt. The inner surfaces of the head and
the vessel shell are subject to a constant pressure of 1.38 × 107 Pa (2000 psi) from the water.
Interactions
Contact occurs between
•
•
•
•
the reactor vessel and closure head,
the lower nuts and the reactor vessel bolting flange,
the upper nuts and the closure head bolting flange, and
the closure head standpipe and CDM plug.
Model terminology
This example illustrates the use of the submodeling technique in ways that are generalizations of the
Abaqus user interface concept of a global model driving the response of a submodel. Specifically, some
submodel analyses described in this section represent material domains that are adjacent to, rather than
lying within, the domain considered in the initial analysis. To more clearly describe the models in this
example, the term “source model” is used instead of “global model.” A source model is a model that
provides solution results to a subsequent submodel analysis.
Abaqus modeling approaches and simulation techniques
The objective of the analyses in this example is an understanding of stresses in the region of the closure
head standpipe.
Summary of analysis cases
Case 1
Reactor closure analysis:
reference solution
The stress distribution in the closure head is determined from a
single, finely meshed model that includes closure head standpipe and
CDM plug details.
1.1.23–2
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Case 2
Submodeling of the closure
head standpipe region
A defeatured source model of the vessel assembly is analyzed first.
Features excluded are the closure head standpipes and the CDM
plugs. This model then drives a submodel with a more detailed
representation of the closure head standpipe region.
Case 3
Submodel application of
CDM hardware loading
The CDM plug is analyzed separately as a source model. Boundary
conditions are introduced on the CDM plug where it interacts with
the closure head standpipe seating ledge to determine the surface
traction characteristics at this interface. This model is then used to
drive a submodel of the remaining vessel assembly.
In the two submodel analysis cases the node-based submodeling technique, in which the submodel
is driven with displacements, is compared to the surface-based submodeling technique, in which the
submodel is driven with stresses. The three cases are discussed in more detail below.
Case 1 Reactor closure analysis: reference solution
This reference case determines the stress response of the reactor vessel assembly when subjected to
boltup and pressure loading using a single analysis. By comparison, the other modeling cases make
use of submodeling. The reactor vessel assembly is cyclic-symmetric with respect to the axis of the
cylindrical vessel body and only one-quarter of the whole assembly is modeled. The global geometry is
shown in Figure 1.1.23–2.
Analysis types
A static stress analysis is performed.
Mesh design
The vessel is meshed with C3D20R elements, and the closure head is meshed with C3D10M elements.
All other parts including the head, bolts, and Omega seal are meshed with C3D8R elements. The mesh
is shown in Figure 1.1.23–3.
Material model
The elastic model is used in all models with a Young’s modulus of 2.07 × 1011 N/m2 (3.0 × 107 lbf/in2 )
and a Poisson’s ratio of 0.29.
Boundary conditions
Symmetric boundary conditions are applied to the two side surfaces of the vessel quarter. The nodes
on the centerline are constrained separately and are free to move only along the vessel central axis. The
node located at the center of the vessel bottom surface is pinned to give the model a statically determinant
condition.
1.1.23–3
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Loading
A pre-tension load of 2200 kN (5 × 106 lbf) is applied to each stud bolt in the model. The inner surfaces
of the head, the vessel body, and the nozzle are subject to a constant pressure of 1.38 × 107 Pa (2000 psi)
from the water.
Bolting of the CDM plug to the closure head standpipe, defined as the CDM assembly, is simulated
in this analysis by the application of a pair of concentrated loads acting through distributing coupling
constraints. Refer to Figure 1.1.23–4 for identification of the loaded regions of each CDM assembly.
For each CDM plug one coupling constraint acts on the top surface of the plug (region B). For each
standpipe one coupling constraint acts across the top surface (region C). The reference node for each
coupling constraint is positioned along the center axis of the CDM assembly so that vertical concentrated
loads can be applied without generating overturning moments. A bolting force of 106 kN (2.4 × 105 lbf)
for each CDM assembly is chosen as adequate to overcome the liftoff force due to the vessel internal
pressure. This force is applied vertically in the up direction to the standpipe coupling constraint. A
downward force is applied to the accompanying coupling constraint on the CDM plug, but this force is
lessened by the amount of the pressure-generating liftoff force due to the operating pressure acting on
region A (shown in Figure 1.1.23–4), since the capping of this region is not considered explicitly in the
model. Based on the diameter of region A, this pressure liftoff force equals 99 kN (2.26 × 105 lbf).
Constraints
The Omega seal is tied to the flange surfaces of the vessel head and the vessel body. As mentioned above,
distributing coupling constraints are applied to the CDM plugs and the closure head standpipes.
Interactions
Small-sliding contact definitions are prescribed between
•
•
•
•
the reactor vessel and closure head,
the lower nuts and the reactor vessel bolting flange,
the upper nuts and the closure head bolting flange, and
the CDM plug and the accompanying seating ledge in the closure head.
Analysis steps
The analysis is performed in a single static step with automatic stabilization to help establish the contact
between the stud bolts, head, seal, and vessel. Results show that the static dissipation energy is minimal
compared to the strain energy; therefore, its effect on the response can be neglected.
Output requests
Default field and history output requests are specified in the step.
1.1.23–4
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Results and discussion
This case is provided as a reference. Submodel analysis results are compared to these results in the
discussion of Case 2 and Case 3 below.
Case 2 Submodel analysis of the closure head standpipe region
This case is representative of the most common submodel analysis approach: a global analysis of a
coarse source model followed by a detailed submodel analysis representing a smaller region of the source
model. Here, the coarse source model excludes details of the CDM plug and closure head standpipe as
an illustration of a source model with significant defeaturing—a common motivation for subsequent
submodel analysis. The submodel comprises a portion of the closure head and two CDM plugs, using
a finer mesh and with feature details included. The relation between the source model and submodel is
shown in Figure 1.1.23–5.
Analysis types
A static stress analysis is performed.
Mesh design
In the source model the vessel and closure head are meshed with C3D20R elements; all the other parts
including the head, bolts, and Omega seal are meshed with C3D8R elements. The source model mesh is
shown in Figure 1.1.23–6.
For the submodel the CDM plug is meshed with C3D8R elements and the closure head is meshed
with C3D10M elements. The submodel mesh is shown in Figure 1.1.23–7.
Material model
The material model is the same as in Case 1.
Boundary conditions
The source model boundary conditions reflect those applied in Case 1. Similarly, the submodel has
symmetric boundary conditions applied to the two side surfaces of the closure head. In the node-based
submodel analysis, submodel boundary conditions are applied to the submodel boundary. In the surfacebased submodel analysis, a boundary condition is applied in the 2-direction on the coupling constraint
for each CDM plug in the closure head to suppress the rigid body mode.
Loading
The source model loads reflect those applied in Case 1 except for the bolting of the CDM plugs to the
closure head, which is introduced in the submodel.
In the surface-based submodel analysis, submodel distributed loads are applied to the submodel
boundary surface.
1.1.23–5
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Constraints
Distributing coupling constraints are applied to the CDM plugs and the closure head standpipes, as in
Case 1.
Interactions
Contact interactions are the same as in Case 1.
Analysis steps
The global analysis of the source model is performed in a single static step with automatic stabilization
to help establish the contact between the stud bolts, head, seal, and vessel. The submodel analysis is
performed in a single static step.
Output requests
Default field and history output requests are specified in the step.
Results and discussion
Mises stress results are compared along paths in two regions in the closure head:
•
•
the first comparison is made along a ligament through the closure head shell, as shown in
Figure 1.1.23–8; and
the second comparison is made along a circular path in the vicinity of the CDM hardware seating
ledge, as shown in Figure 1.1.23–9.
By reviewing the stress distribution comparisons (discussed below), you can see that in this case, surfacebased submodeling is superior to node-based submodeling for results lying within the main closure head
shell. In the upper region of the standpipe, neither method provides adequate results indicating that the
level of defeaturing in the source model is too great for an accurate submodel analysis of the standpipe
region.
Closure head shell ligament
Figure 1.1.23–10 compares the Mises stress distribution on the path shown in Figure 1.1.23–8 for the
reference model, the node-based submodel solution, and the surface-based submodel solution. These
results show that the surface-based submodel solution provides a more accurate stress distribution
than the node-based submodel technique in this region. This result is consistent with the guidelines
documented in “Surface-based submodeling” in “Submodeling: overview,” Section 10.2.1 of the
Abaqus Analysis User’s Manual, namely that a surface-based solution is more accurate in cases where
the environment is load controlled—the vessel pressurization dominates the closure head response in
the shell region—and the submodel geometry differs from the source model geometry—the source
model does not include the standpipe detail.
In practice, the classification of an analysis according to these guidelines, particularly the
classification of load-controlled vs. displacement-controlled, is often not obvious nor is the reference
solution available for comparison. Therefore, you should always compare measures of interest between
1.1.23–6
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
the source model and the submodel on or near the submodel driven boundary and confirm that they show
reasonable agreement. In this case the Mises stress is compared along a path, shown in Figure 1.1.23–7,
cutting across the submodel driven boundary. In Figure 1.1.23–11 the results comparison shows that
the surface-based submodel solution provides a stress distribution on the submodel boundary that more
closely matches that for the global solution of the source model. This plot also shows the reference
solution, which shows better agreement with the surface-based submodel solution at the outer edge of
the shell and better agreement with the node-based submodel solution at the inner edge of the shell.
Hence, the agreement between global model and submodel stress distributions, while necessary, is not
sufficient to confirm an adequate submodel solution at all locations. You must also use judgment as to
whether geometric differences are too great between the source model and submodel.
Standpipe seating ledge
Figure 1.1.23–12 compares the Mises stress distribution on the path shown in Figure 1.1.23–9 for the
reference model, the node-based submodel solution, and the surface-based submodel solution. The stress
results near the seating ledge show that neither submodeling technique is clearly superior or provides
adequate accuracy. This follows from the fact that the standpipe and seating ledge region did not appear
at all in the source model analysis; the defeaturing was too severe in this case for an adequate submodel
solution in this region.
This seating ledge stress comparison makes it clear that although a favorable comparison of results
on the submodel boundary, as was done in Figure 1.1.23–11, is necessary, it is not sufficient to ensure
adequate submodel results in all locations in the model. In this case the seating ledge region was absent
entirely from the defeatured source model, and you should not expect accurate results in this region.
Case 3 Submodel application of CDM plug loading
This case represents an atypical use of submodeling in which the source model is associated with a small
part of the structure and the submodel comprises most of the overall structure. Here, the source model
focuses on the CDM plugs to predict how each of the CDM plugs loads the closure head.
The subsequent submodel analysis uses results from the source analysis for loading the remainder of
the structure. The regions considered for the source model and submodel are shown in Figure 1.1.23–13.
Mesh design
In the source model the CDM plug hardware is meshed with C3D8R elements. The source model mesh
is shown in Figure 1.1.23–13. The geometry for the remaining structure is also shown in this figure to
illustrate the plug positioning relative to the overall reactor assembly.
The submodel mesh is nearly identical to that shown in Figure 1.1.23–3 for Case 1. The only
difference is that the CDM plugs are excluded from the model in Case 3.
Boundary conditions
The submodel analysis of the CDM plug source model simulates contact with the seating ledge with a
boundary condition constraint on the plug seating surface.
1.1.23–7
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Loading
The loading follows that for Case 1 with the application of the loads split between the source model and
submodel.
Source model analysis
The bolt load applied to the CDM plug is simulated through a downward concentrated force applied
to a distributing coupling constraint reference node in each of the CDM plugs. The magnitude of this
force is the bolting force of 106 kN (2.4 × 105 lbf) less the pressure generating liftoff force of 99 kN
(2.26 × 105 lbf), for the reasons detailed in the Case 1 description.
Submodel analysis
A pre-tension load of 2200 kN (5 × 106 lbf) is applied to each stud bolt in the model. The inner surfaces
of the head, the vessel body, and the nozzle are subject to a constant pressure of 1.38 × 107 Pa (2000 psi)
from the water.
The bolt load applied to the standpipe is simulated through an upward concentrated force applied
to a distributing coupling constraint reference node in each of the standpipes. The magnitude of this
force is the bolting force of 106 kN (2.4 × 105 lbf) less the pressure generating liftoff force of 99 kN
(2.26 × 105 lbf).
Constraints
All constraint definitions are the same as in Case 1.
Interactions
All interaction definitions are the same as in Case 1, except that the contact interaction between the CDM
plug and the standpipe seating ledge is effected through submodel loads and boundary conditions.
Run procedure
Run the analyses with the input files listed for Case 3 below.
Results and discussion
Stress results are considered on the same paths defined for comparison of reference and submodel
results in Case 2. The Mises stress distribution on these paths is compared in Figure 1.1.23–14 and
Figure 1.1.23–15 for the two forms of submodeling and the reference solution.
These results show that in both the high-stressed region, shown in the ligament stress plot, and
in the vicinity of the seating ledge, the surface-based submodeling approach provides a more accurate
solution. The poor results for node-based submodeling follow from the fact that the assembly model—the
submodel in this case—elongates along the vessel main axis. The CDM assembly region experiences
this elongation as a rigid body translation. The standpipe seating ledge, however, is constrained in its
movement by the submodel boundary conditions. These boundary conditions follow from the separate
1.1.23–8
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
analysis of the CDM plug source model that does not consider the solution-dependent elongation of the
vessel assembly.
Discussion of results and comparison of cases
Case 2 and Case 3 illustrate situations where you may see improved accuracy when using the surfacebased submodeling approach.
The effect of stiffness change on submodel analysis
In cases where the submodel stiffness matches that of the source model, you can expect, using
reasonable modeling practices, that the submodel analysis will provide adequate results. In cases where
the submodel stiffness differs, such as in Case 2, you must exercise caution in evaluating your submodel
solution. Comparison of stress contours on the common boundary of the source model and submodel
can aid you in determining if your solution is adequate. In the case of significant defeaturing, you
should not rely on the submodeling analysis technique in any form for detailed stress response in areas
absent from the source model, such as the closure head standpipe.
The effect of displacement discrepancies on submodel analysis
In cases where you expect that the submodel displacement solution will differ from the corresponding
source model solution by only a rigid body motion, such as in Case 3, you can expect that a node-based
submodeling approach will give incorrect results. In this case you can use the alternative surface-based
submodeling of stresses and obtain improved solution accuracy.
Files
Case 1 Reactor closure analysis: reference solution
ReactorHead_reference.inp
Input file to analyze the reactor vessel closure assembly.
Case 2 Submodeling of the closure head standpipe region
ReactorHead_global.inp
ReactorHead_submodel_node.inp
ReactorHead_submodel_surface.inp
Global analysis of the reactor vessel closure assembly
source model with a defeatured closure head.
Closure head submodel analysis using node-based
submodeling.
Closure head submodel analysis using surface-based
submodeling.
Case 3 Submodel application of CDM plug loading
ReactorHead_CDMdetail.inp
ReactorHead_assembly_node.inp
Global analysis of the CDM plug source model.
Reactor vessel closure assembly submodel analysis with
CDM loading effected through node-based submodeling.
1.1.23–9
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
ReactorHead_assembly_surface.inp
Reactor vessel closure assembly submodel analysis
with CDM loading effected through surface-based
submodeling.
References
Abaqus Analysis User’s Manual
•
•
•
“Submodeling: overview,” Section 10.2.1 of the Abaqus Analysis User’s Manual
“Node-based submodeling,” Section 10.2.2 of the Abaqus Analysis User’s Manual
“Surface-based submodeling,” Section 10.2.3 of the Abaqus Analysis User’s Manual
Abaqus Keywords Reference Manual
•
•
•
*BOUNDARY
*DSLOAD
•
Naval Reactors Branch, Division of Reactor Development, United States Atomic Energy
Commission, The Shippingport Pressurized Water Reactor, Reading, Massachusetts: Addison
Wesley Publishing Company, 1958.
*SUBMODEL
Other
1.1.23–10
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
CDM plug
Closure head
standpipe
Closure head
standpipes
Omega seal
Closure head
Closure nuts and
washers
Closure stud bolts
Outlet nozzles
Vessel shell
Inlet nozzles
Bottom head
Figure 1.1.23–1
Reactor vessel assembly.
1.1.23–11
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
CDM plug
Closure head
Closure hardware
Vessel shell
Bottom head
Figure 1.1.23–2
Reactor vessel assembly model.
1.1.23–12
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Figure 1.1.23–3
B
A
Reference analysis mesh.
B
C
CDM plug
C
Closure head standpipe
Seating ledge
Figure 1.1.23–4
Load application areas on the CDM plug and closure head standpipe.
1.1.23–13
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Defeatured closure head
Fully featured closure head
Source model
Submodel
Figure 1.1.23–5
Case 2 closure head submodel relation to the source model.
Figure 1.1.23–6
Case 2 global analysis mesh with defeatured closure head.
1.1.23–14
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
submodel boundary
Start
End
path for stress
comparison
submodel boundary
Figure 1.1.23–7
Case 2 submodel analysis showing the mesh (left) and the path definition
for stress comparison to the source model (right).
End
Stress comparison
path
Start
Figure 1.1.23–8
Through-ligament path definition.
1.1.23–15
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Stress comparison
path
Figure 1.1.23–9
Seating ledge path definition.
Surface−based submodel
Node−based submodel
Reference solution
[x1.E3]
16.
Mises stress (psi)
14.
12.
10.
8.
6.
0.0
2.0
4.0
6.0
8.0
10.0
Distance through cut (in)
Figure 1.1.23–10
Case 2 stress distribution comparison through the closure head ligament.
1.1.23–16
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Surface−based submodel
Node−based submodel
Global solution
Reference solution
[x1.E3]
Mises stress (psi)
12.
10.
8.
6.
0.0
2.0
4.0
6.0
8.0
Distance through cut (in)
Figure 1.1.23–11 Comparison of the closure head through-thickness
Mises stress distribution at the location of the submodel boundary.
Surface−based submodel
Node−based submodel
Reference solution
[x1.E3]
Mises stress (psi)
10.0
8.0
6.0
4.0
0.
5.
10.
15.
20.
25.
30.
35.
Distance around perimeter (in)
Figure 1.1.23–12
Case 2 stress distribution comparison around the seating ledge.
1.1.23–17
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
CDM plug mesh
Position relative
to reactor assembly
Figure 1.1.23–13
Case 3 CDM plug analysis mesh.
1.1.23–18
Abaqus Version 6.12 ID:
Printed on:
REACTOR STRUCTURE SUBMODEL STRESS ANALYSIS
Surface−based submodel
Node−based submodel
Reference solution
[x1.E3]
16.
Mises stress (psi)
14.
12.
10.
8.
0.0
2.0
4.0
6.0
8.0
10.0
Distance through cut (in)
Figure 1.1.23–14
Case 3 stress distribution comparison through the closure head ligament.
Surface−based submodel
Node−based submodel
Reference solution
[x1.E3]
60.
Mises stress (psi)
50.
40.
30.
20.
10.
0.
5.
10.
15.
20.
25.
30.
35.
Distance around perimeter (in)
Figure 1.1.23–15
Case 3 stress distribution comparison around the seating ledge.
1.1.23–19
Abaqus Version 6.12 ID:
Printed on:
COMPOSITE LAYUPS
1.1.24
USING A COMPOSITE LAYUP TO MODEL A YACHT HULL
Products: Abaqus/Standard
Abaqus/CAE
Abaqus/Viewer
Objectives
This example problem demonstrates the following Abaqus features and techniques:
•
•
•
•
•
•
importing the shell geometry of a yacht hull from an ACIS (.sat) file,
creating a composite layup using Abaqus/CAE,
applying plies in the layup to regions of the model,
viewing a ply stack plot from a region of the model,
viewing an envelope plot that shows the critical plies in each region of the model, and
viewing an X–Y plot through the thickness of an element.
Application description
Composite hulls are used routinely in the yacht industry. Composite materials allow manufacturers
to create high-performance marine vessels that incorporate the complex hull shapes that engineers
have derived from computational fluid dynamics analyses and from experimental testing. Composites
also provide the strength, rigidity, and low mass that high-performance yachts require. However,
incorporating many layers of material with varying orientations in a complex three-dimensional finite
element model can be time consuming. The addition of local reinforcements complicates the process.
These issues are described by Bosauder et al. (2006).
The composite layup capability in Abaqus/CAE simplifies the process of composites modeling
by mirroring the procedure that manufacturers follow on the shop floor—stacking sheets of composite
material in a region of a mold and aligning the material in a specified direction. The Abaqus/CAE
composite layup editor allows you to easily add a ply, choose the region to which it is applied, specify
its material properties, and define its orientation. You can also read the definition of the plies in a layup
from data in a text file, which is convenient when the data are stored in a spreadsheet or are generated
by a third-party tool.
Geometry
Figure 1.1.24–1 shows the hull, mast, rigging, and keel of the yacht model. The geometry of the model
is imported as a single part from an ACIS (.sat) file, as shown in Figure 1.1.24–2. The part models one
half of the hull, and symmetric boundary conditions are applied. The hull represents a high-performance
20-meter yacht with reinforced bulkheads that stiffen the structure. The infrastructure above the deck
does not play a role in modeling the performance of the hull and is not included in the model.
Sets are created that correspond to the regions of the composite layup to which plies are applied.
1.1.24–1
Abaqus Version 6.12 ID:
Printed on:
COMPOSITE LAYUPS
Materials
The model is partitioned into 27 regions. Each region contains plies of glass-epoxy cloth surrounding a
Nomex core. Most regions contain nine plies—four glass-epoxy plies on either side of the Nomex core.
However, additional plies are added to reinforce regions of high strain. Some bulkheads are reinforced
with stringers made of glass-epoxy cloth with an effective Young’s modulus of 128000 N/mm2 .
Table 1.1.24–1 shows the material properties of the glass-epoxy cloth, and Table 1.1.24–2 shows the
material properties of the Nomex core.
Figure 1.1.24–3 shows several rows of the composite layup table and illustrates how plies and
material orientations are assigned to a region of the model. Figure 1.1.24–4 shows a ply stack plot
of the same region.
Boundary conditions and loading
The center of the model is constrained to be symmetric about the y-axis, as shown in Figure 1.1.24–2.
The following loads are applied:
•
•
•
•
•
A hydrostatic pressure is applied to the hull. The pressure is modeled with an analytical field that
increases the pressure linearly along the z-axis.
Concentrated forces that model the tension from the sail rigging are applied to the front, rear, and
side of the deck. The forces are applied along the x-axis of a datum coordinate system. Each
coordinate system has an origin at the location of the load, and the x-axis orients the load toward
the location of the top of the mast. The concentrated forces are transferred to the deck through
distributing couplings.
The load from the mast is applied at the base of the hull in the z-direction.
The keel is modeled with a lumped mass attached to the hull through a kinematic coupling.
An inertia relief load is applied at the center of the hull to bring the model into equilibrium after the
loads are applied.
Abaqus modeling approaches and simulation techniques
A single loading case is considered that uses a static analysis to study the effect of the loading on the
composite layup.
Mesh design
The model is meshed by Abaqus/CAE using the free meshing technique and quadrilateral-dominated
elements.
Loading
•
•
•
The tension load from the sail rigging is 5500 N at the front of the hull, 4000 N at the rear of the
hull, and 7500 N at the side of the hull.
The load from the mast is 17500 N.
A lumped mass of 10 metric tons models the keel.
1.1.24–2
Abaqus Version 6.12 ID:
Printed on:
COMPOSITE LAYUPS
Constraints
A kinematic coupling transfers the weight of the keel to the base of the hull, and three distributing
couplings transfer the load from the rigging to the hull.
Analysis steps
A single static load step is defined for the analysis; nonlinear effects are not included.
Output requests
By default, Abaqus/CAE writes field output data from only the top and bottom section points of a
composite layup, and no data are generated from the other plies. In this model, output is requested
for all section points in all plies. This allows you to create an envelope plot of the entire model that
indicates which plies in each region are carrying the highest strain.
Results and discussion
Figure 1.1.24–5 shows an envelope plot of the in-plane shear strain (E12) in the middle of the hull.
Figure 1.1.24–6 shows the through-thickness variation of this strain component.
Files
You can use the Abaqus/CAE Python scripts to create the model and to run the analysis. You can also
use the Abaqus/Standard input file to run the analysis.
compositehull_model.py
compositehull_geometry.sat
compositehull_layup.txt
compositehull_job.py
compositehull_job.inp
Script to create the model using the geometry from
compositehull_geometry.sat and the composite layup
from compositehull_layup.txt.
ACIS file containing the geometry of the model.
A comma-separated text file defining the plies in the
composite layup.
Script to analyze the model.
Input file to analyze the model.
References
Abaqus Analysis User’s Manual
•
“Shell elements,” Section 29.6 of the Abaqus Analysis User’s Manual
Abaqus/CAE User’s Manual
•
•
“Creating composite layups,” Section 12.4.4 of the Abaqus/CAE User’s Manual
Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Manual
1.1.24–3
Abaqus Version 6.12 ID:
Printed on:
COMPOSITE LAYUPS
Other
•
Bosauder, P., D. Campbell, and B. Jones, “Improvements in the Commercial Viability of Finite
Element Analysis (FEA) for Accurate Engineering of Marine Structures,” JEC conference, Paris,
March 2006.
Table 1.1.24–1
Material properties of the glass-epoxy cloth.
Variable
Value
35000 N/mm2
7500 N/mm2
0.3
3600 N/mm2
3000 N/mm2
3000 N/mm2
1.5 × 10–9 metric tons/mm3
Table 1.1.24–2
Variable
Material properties of the Nomex core.
Value
10 N/mm2
10 N/mm2
0.3
1 N/mm2
30 N/mm2
30 N/mm2
8.0 × 10−11 metric tons/mm3
1.1.24–4
Abaqus Version 6.12 ID:
Printed on:
COMPOSITE LAYUPS
Y
X
Z
Figure 1.1.24–1
Y
The yacht model.
Symmetry boundary condition
X
Z
Figure 1.1.24–2
The symmetric model.
1.1.24–5
Abaqus Version 6.12 ID:
Printed on:
COMPOSITE LAYUPS
Figure 1.1.24–3
Assigning plies in the layup table to a region of the model.
1.1.24–6
Abaqus Version 6.12 ID:
Printed on:
COMPOSITE LAYUPS
COCKPIT_OS_4
COCKPIT_OS_3
COCKPIT_OS_2
t = 1.25
t = 0.5
t = 0.5
t = 0.5
COCKPIT_OS_1
Glass−Epoxy
Glass−Epoxy
Glass−Epoxy
t=8
COCKPIT_CORE
Glass−Epoxy
t = 0.5
t = 0.5
t = 0.5
t = 1.25
COCKPIT_IS_4
COCKPIT_IS_3
Core
COCKPIT_IS_2
COCKPIT_IS_1
Glass−Epoxy
Glass−Epoxy
Glass−Epoxy
3
2
1
Glass−Epoxy
Figure 1.1.24–4
A ply stack plot from the cockpit.
1.1.24–7
Abaqus Version 6.12 ID:
Printed on:
COMPOSITE LAYUPS
E, E12
Envelope (max abs)
(Avg: 75%)
+1.50e−02
+1.40e−02
+1.30e−02
+1.20e−02
+1.10e−02
+1.00e−02
+9.00e−03
+8.00e−03
+7.00e−03
+6.00e−03
+5.00e−03
+4.00e−03
+3.00e−03
+2.00e−03
+1.00e−03
+0.00e+00
Y
X
Z
Figure 1.1.24–5
Envelope plot of strain in the critical plies in the center of the hull.
20.
Thickness
15.
10.
5.
0.
−0.015
−0.010
−0.005
0.000
0.005
0.010
0.015
Strain
Figure 1.1.24–6
Strain (E12) across the thickness of an element.
1.1.24–8
Abaqus Version 6.12 ID:
Printed on:
BUCKLING AND COLLAPSE ANALYSES
1.2
Buckling and collapse analyses
•
•
•
•
•
•
“Snap-through buckling analysis of circular arches,” Section 1.2.1
“Laminated composite shells: buckling of a cylindrical panel with a circular hole,” Section 1.2.2
“Buckling of a column with spot welds,” Section 1.2.3
“Elastic-plastic K-frame structure,” Section 1.2.4
“Unstable static problem: reinforced plate under compressive loads,” Section 1.2.5
“Buckling of an imperfection-sensitive cylindrical shell,” Section 1.2.6
1.2–1
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
1.2.1
SNAP-THROUGH BUCKLING ANALYSIS OF CIRCULAR ARCHES
Product: Abaqus/Standard
It is often necessary to study the postbuckling behavior of a structure whose response is unstable during part
of its loading history. Two of the models in this example illustrate the use of the modified Riks method, which
is provided to handle such cases. The method is based on moving with fixed increments along the static
equilibrium path in a space defined by the displacements and a proportional loading parameter. The actual
load value may increase or decrease as the solution progresses. The modified Riks method implemented in
Abaqus is described in “Modified Riks algorithm,” Section 2.3.2 of the Abaqus Theory Manual.
The other two models illustrate the use of viscous damping. One example applies viscous damping
as a feature of surface contact, which allows for the definition of a “viscous” pressure that is proportional
to the relative velocity between the surfaces. The implementation of this option in Abaqus is described
in “Contact pressure definition,” Section 5.2.1 of the Abaqus Theory Manual. The other example applies
volume proportional damping to the model. The implementation of this option is described in the automatic
stabilization section of “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User’s Manual.
Three separate cases are considered here. The first is a clamped shallow arch subjected to a pressure
load. Reference solutions for this case are given by Ramm (1981) and Sharafi and Popov (1971). The second
case is the instability analysis of a clamped-hinged circular arch subjected to a point load. The exact analytical
solution for this problem is given by DaDeppo and Schmidt (1975). The third case is a modification of the
shallow arch problem in which the ends are pinned rather than clamped and the arch is depressed with a rigid
punch.
Model and solution control
The shallow circular arch is shown in Figure 1.2.1–1. Since the deformation is symmetric, one-half of
the arch is modeled. Ten elements of type B21 (linear interpolation beams) are used. A uniform pressure
is first applied to snap the arch through. The loading is then reversed so that the behavior is also found
as the pressure is removed.
The deep circular arch is shown in Figure 1.2.1–2. One end of the arch is clamped, and the other
is hinged. A concentrated load is applied at the apex of the arch. The arch undergoes extremely large
deflections but small strains. Because of the asymmetric boundary conditions, the arch will sway toward
the hinged end and then collapse. The arch is almost inextensible for most of the response history. Sixty
elements of type B31H are used. Hybrid elements are used because they are most suitable for problems
such as this.
Solution controls are used to set a very tight convergence tolerance because the problem contains
more than one equilibrium path. If tight tolerances are not used, the response might follow a path that is
different from the one shown.
In the Riks procedure actual values of load magnitudes cannot be specified. Instead, they are
computed as part of the solution, as the “load proportionality factor” multiplying the load magnitudes
given on the loading data lines. User-prescribed load magnitudes serve only to define the direction and
to estimate the magnitude of the initial increment of the load for a step. This initial load increment is
1.2.1–1
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
the product of the ratio of the initial time increment to the time period and the load magnitudes given
in the loading options. The user can terminate a Riks analysis by specifying either a maximum load
proportionality factor or a maximum displacement at a node, or both. When a solution point is computed
at which either of these limits is crossed, the analysis will stop. In any event, or if neither option is used,
the analysis ends when the maximum number of increments for the step is exceeded.
In snap-through studies such as these, the structure can carry increasing load after a complete snap.
Therefore, the analysis is terminated conveniently by specifying a maximum load proportionality factor.
For the clamped shallow arch the initial snap occurs at a pressure of about −1000 (force/length2
units). Thus, −250 (force/length2 units) seems to be a reasonable estimate for the first increment of
load to be applied. Accordingly, an initial time increment of 0.05 is specified for a time period of 1.0
and a pressure load of −5000 (force/length2 units). The solution will have been sufficiently developed
at a pressure of about −2000 (force/length2 units). Therefore, the analysis is terminated when the load
proportionality factor exceeds 0.4.
To illustrate the use of Riks in several steps, a second step is included in which the pressure is taken
off the arch so that it will snap back toward its initial configuration. At any point in a Riks analysis, the
actual load is given by
, where
is the load at the end of the previous step,
is the load magnitude prescribed in the current step, and is the load proportionality factor. The
arch is unloaded so that in the initial time increment, a pressure of approximately 0.15 is removed.
Using an initial time increment of 0.05 in a time period of 1.0, a load of
is prescribed for
this restarted step. Furthermore, we want the analysis to end when all the load is removed and the arch
has returned to its initial configuration. Therefore, a displacement threshold of 0.0 is set for the center
of the arch. The analysis terminates when this limit is crossed. Because Abaqus must pick up the load
magnitude at the end of the initial Riks step to start the next step, any step following a Riks step can be
done only as a restart job from the previous step.
For the deep clamped-hinged arch, the initial snap occurs at a load of about 900 (force units). The
load magnitude specified is 100 (force units), and the maximum load proportionality factor is specified
as 9.5.
The shallow arch depressed with a rigid punch is shown in Figure 1.2.1–3. The analysis uses
the same model of the arch as the first problem. However, the end is pinned rather than clamped,
and load is applied through the displacement of the punch. The pinned boundary condition makes
the problem more unstable than the clamped-end case. A preliminary analysis in which the arch is
depressed with a prescribed displacement of the midpoint of the arch shows that the force will become
negative during snap-through. Thus, if the arch is depressed with a rigid punch, the Riks method will
not help convergence because, at the moment of snap-through, the arch separates from the punch, and
the movement of the punch no longer controls the displacement of the arch. Therefore, contact damping
is introduced to aid in convergence. Viscous damping with surface contact adds a pressure that is
proportional to the relative velocity to slow down the separation of the arch from the punch.
The viscous damping clearance is set to 10.0, and the fraction of the clearance interval is set to
0.9; the damping is constant for a clearance of up to 9.0. Since the arch is 4.0 units high, the distance
traveled by the top of the arch from the initial position to the final snap-through position is 8.0 units. This
distance is clearly larger than the clearance between the middle of the arch and the tip of the punch at
1.2.1–2
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
any time during the analysis. Thus, the viscous damping is in effect for the whole period when the arch
has separated from the punch.
To choose the viscous damping coefficient, note that it is given as pressure per relative velocity. The
relevant pressure is obtained by dividing the approximate peak force (10000.0) by the contact area (1.0).
The relevant velocity is obtained by dividing the distance over which the top of the arch travels (8.0 from
initial to snapped position, which can be rounded to 10.0) by the time (approximately 1.0, the total time
of the step). A small percentage (0.1%) of this value is used for the viscous damping coefficient:
With
1.0, the analysis runs to completion. Another analysis was run with a smaller value of
0.1,
but the viscous damping was not sufficient to enable the analysis to pass the point of snap-through. Thus,
a damping coefficient of 1.0 was determined to be an appropriate value.
Automatic stabilization based on volume proportional damping is also considered for the shallow
arch compressed with a rigid punch, as an alternative to contact damping. Two forms of automatic
stabilization are considered: one with a constant damping factor that is chosen by default (see
“Automatic stabilization of static problems with a constant damping factor” in “Solving nonlinear
problems,” Section 7.1.1 of the Abaqus Analysis User’s Manual), and one with an adaptive damping
factor (see “Adaptive automatic stabilization scheme” in “Solving nonlinear problems,” Section 7.1.1
of the Abaqus Analysis User’s Manual).
Results and discussion
The results for the clamped shallow arch are shown in Figure 1.2.1–4, where the downward displacement
of the top of the arch is plotted as a function of the pressure. The algorithm obtains this solution in
12 increments, with a maximum of three iterations in an increment. At the end of 12 increments the
displacement of the top of the arch is about 7.5 length units. This represents a complete snap through,
as the original rise of the arch was 4 length units. Figure 1.2.1–5 and Figure 1.2.1–6 show a series of
deformed configuration plots for this problem. Several other authors have examined this same case and
have obtained essentially the same solution (see Ramm, 1981, and Sharafi and Popov, 1971).
The results for the deep clamped-hinged arch are shown in Figure 1.2.1–7, where the displacement
of the top of the arch is plotted as a function of the applied load. Figure 1.2.1–8 shows a series of
deformed configuration plots for this problem. The arch collapses unstably at the peak load. Following
this, the beam stiffens rapidly as the load increases. The ability of the Riks method to handle unstable
response is well-illustrated by this example.
The results of the preliminary analysis of the prescribed displacement of a pinned shallow arch
are shown in Figure 1.2.1–9, with the displacement of the top of the arch plotted as a function of the
reaction force at that point. This plot shows the negative force that develops during snap-through. A
series of deformed configuration plots for the pinned shallow arch depressed with a punch and with
viscous damping introduced is shown in Figure 1.2.1–10, with one plot showing the arch separated from
the punch. Figure 1.2.1–11 is a plot of the force between the punch and the top of the arch. The force
is positive until snap-through, when the arch separates from the punch and a negative viscous force
1.2.1–3
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
develops. Once the snap-through is complete, the force drops to zero as the punch continues to move
down while separated from the arch. When the punch contacts the arch, a positive force develops again.
Similar results are produced when the contact viscous damping is replaced by volume proportional
damping (with either constant or adaptive damping coefficients). A sequence of configurations like
Figure 1.2.1–10 is obtained, in which separation of the arch from the punch occurs during snap-through.
At the end of the analysis the amount of energy dissipated is similar to the amount dissipated with the
viscous damping option.
You can use the abaqus restartjoin execution procedure to extract data from the output database
created by a restart analysis and append the data to a second output database. For more information, see
“Joining output database (.odb) files from restarted analyses,” Section 3.2.18 of the Abaqus Analysis
User’s Manual.
Input files
snapbuckling_shallow_step1.inp
snapbuckling_shallow_unload.inp
snapbuckling_deep.inp
snapbuckling_shallow_midpoint.inp
snapbuckling_shallow_punch.inp
snapbuckling_b21h_deep.inp
snapbuckling_b32h_deep.inp
snapbuckling_restart1.inp
snapbuckling_restart2.inp
snapbuckling_shallow_stabilize.inp
snapbuckling_shallow_stabilize_adap.inp
Initial analysis step for the shallow arch.
Restart run to obtain the unloading response of the
shallow arch.
Deep arch.
Shallow arch loaded by a fixed displacement of the
midpoint.
Shallow arch loaded by the displacement of a rigid punch.
60 elements of type B21H used for the deep clampedhinged arch analysis.
30 elements of type B32H used for the deep clampedhinged arch analysis.
Restart analysis of snapbuckling_shallow_step1.inp
during the RIKS step.
Restart analysis of snapbuckling_restart1.inp during the
RIKS step. This illustrates restarting an existing RIKS
restart analysis.
Same as snapbuckling_shallow_punch.inp with the
surface contact viscous damping replaced by the volume
proportional damping of *STATIC, STABILIZE.
Same as snapbuckling_shallow_punch.inp with the
surface contact viscous damping replaced by adaptive
stabilization of *STATIC, STABILIZE, ALLSDTOL.
References
•
DaDeppo, D. A., and R. Schmidt, “Instability of Clamped-Hinged Circular Arches Subjected to a
Point Load,” Transactions of the American Society of Mechanical Engineers, Journal of Applied
Mechanics, pp. 894–896, Dec. 1975.
1.2.1–4
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
•
Ramm, E., “Strategies for Tracing the Nonlinear Response Near Limit Points,” in Nonlinear Finite
Element Analysis in Structural Mechanics, edited by W. Wunderlich, E. Stein and K. J. Bathe,
Springer Verlag, Berlin, 1981.
•
Sharifi, P., and E. P. Popov, “Nonlinear Buckling Analysis of Sandwich Arches,” Proc. ASCE,
Journal of the Engineering Mechanics Division, vol. 97, pp. 1397–1412, 1971.
R = 100
β 2 = 0.08
E = 10 7
υ = .25
P
2
β
1
R
Figure 1.2.1–1
Clamped shallow circular arch.
P
2.289
1
E = 10 6
υ = 0.
Figure 1.2.1–2
Deep clamped-hinged arch.
1.2.1–5
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
R = 100
β 2 = 0.08
E = 10 7
υ = .25
+
2
β
1
R
Figure 1.2.1–3
Pinned shallow arch with rigid punch.
3
(*10**3)
DISTRIBUTED LOAD
2
1
0
0
Figure 1.2.1–4
1
2
3
4
DISPLACEMENT
6
7
8
(*10**-2)
Load versus displacement curve for clamped shallow arch.
1.2.1–6
Abaqus Version 6.12 ID:
Printed on:
5
SNAP-THROUGH BUCKLING
2
3
1
Figure 1.2.1–5
Deformed configuration plots for clamped shallow arch–Step 1.
2
3
1
Figure 1.2.1–6
Deformed configuration plots for clamped shallow arch–Step 2.
1.2.1–7
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
12
(*10**2)
LINE
1
2
ABSCISSA
VARIABLE
ORDINATE
VARIABLE
Y DISP
LOAD
(*-1.0E+00)
(*-1.0E+00)
X DISP
LOAD
(*-1.0E+00)
(*-1.0E+00)
8
2
1
2
1
LOAD
2
1
4
21
2
2
1
0
1
2
1
2
0
Figure 1.2.1–7
4
1
8
12
DISPLACEMENT
16
20
(*10**1)
Load versus displacement curves for deep clamped-hinged arch.
2
3
Figure 1.2.1–8
1
Deformed configuration plots for deep clamped-hinged arch.
1.2.1–8
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
4
(*10**4)
LINE
1
ABSCISSA
VARIABLE
ORDINATE
VARIABLE
DISP OF TOP
FORCE
(*-1.0E+00)
(*-1.0E+00)
3
FORCE
2
1
0
-1
-2
0
Figure 1.2.1–9
2
4
6
DISPLACEMENT
8
10
Force versus displacement curve for fixed displacement of pinned shallow arch.
Figure 1.2.1–10
Deformed configuration plots for pinned arch depressed with rigid punch.
1.2.1–9
Abaqus Version 6.12 ID:
Printed on:
SNAP-THROUGH BUCKLING
LINE
1
VARIABLE
SCALE
FACTOR
RF2 Node 100
-1.00E+00
20
(*10**3)
15
FORCE
10
5
0
-5
-10
0
2
4
6
TIME
Figure 1.2.1–11
10
(*10**-1)
Force between the punch and the top of the pinned arch.
1.2.1–10
Abaqus Version 6.12 ID:
Printed on:
8
LAMINATED PANEL
1.2.2
LAMINATED COMPOSITE SHELLS: BUCKLING OF A CYLINDRICAL PANEL WITH
A CIRCULAR HOLE
Product: Abaqus/Standard
This example illustrates a type of analysis that is of interest in the aerospace industry. The objective is to
determine the strength of a thin, laminated composite shell, typical of shells used to form the outer surfaces
of aircraft fuselages and rocket motors. Such analyses are complicated by the fact that these shells typically
include local discontinuities—stiffeners and cutouts—which can induce substantial stress concentrations that
can delaminate the composite material. In the presence of buckling this delamination can propagate through
the structure to cause failure. In this example we study only the geometrically nonlinear behavior of the shell:
delamination or other section failures are not considered. Some estimate of the possibility of material failure
could presumably be made from the stresses predicted in the analyses reported here, but no such assessment
is included in this example.
The example makes extensive use of material orientation in a general shell section to define the
multilayered, anisotropic, laminated section. The various orientation options for shells are discussed in
“Analysis of an anisotropic layered plate,” Section 1.1.2 of the Abaqus Benchmarks Manual.
General shell sections offer two methods of defining laminated sections: defining the thickness,
material, and orientation of each layer or defining the equivalent section properties directly. The last
method is particularly useful if the laminate properties are obtained directly from experiments or a separate
preprocessor. This example uses both methods with a general shell section definition. Alternatively, you
could use a shell section to analyze the model; however, because the material behavior is linear, no difference
in solution would be obtained and the computational costs would be greater.
Geometry and model
The structure analyzed is shown in Figure 1.2.2–1 and was originally studied experimentally by Knight
and Starnes (1984). The test specimen is a cylindrical panel with a 355.6 mm (14 in) square platform
and a 381 mm (15 in) radius of curvature, so that the panel covers a 55.6° arc of the cylinder. The
panel contains a centrally located hole of 50.8 mm (2 in) diameter. The shell consists of 16 layers of
unidirectional graphite fibers in an epoxy resin. Each layer is 0.142 mm (.0056 in) thick. The layers
are arranged in the symmetric stacking sequence { 45/90/0/0/90/ 45} degrees repeated twice. The
nominal orthotropic elastic material properties as defined by Stanley (1985) are
= 135 kN/mm2
= 13 kN/mm2
= 6.4 kN/mm2
= 4.3 kN/mm2
= 0.38,
(19.6 × 106 lb/in2 ),
(1.89 × 106 lb/in2 ),
(.93 × 106 lb/in2 ),
(0.63 × 106 lb/in2 ),
where the 1-direction is along the fibers, the 2-direction is transverse to the fibers in the surface of the
lamina, and the 3-direction is normal to the lamina.
1.2.2–1
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
The panel is fully clamped on the bottom edge, clamped except for axial motion on the top edge
and simply supported along its vertical edges. Three analyses are considered. The first is a linear
(prebuckling) analysis in which the panel is subjected to a uniform end shortening of 0.8 mm (.0316 in).
The total axial force and the distribution of axial force along the midsection are used to compare
the results with those obtained by Stanley (1985). The second analysis consists of an eigenvalue
extraction of the first five buckling modes. The buckling loads and mode shapes are also compared with
those presented by Stanley (1985). Finally, a nonlinear load-deflection analysis is done to predict the
postbuckling behavior, using the modified Riks algorithm. For this analysis an initial imperfection is
introduced. The imperfection is based on the fourth buckling mode extracted during the second analysis.
These results are compared with those of Stanley (1985) and with the experimental measurements of
Knight and Starnes (1984).
The mesh used in Abaqus is shown in Figure 1.2.2–2. The anisotropic material behavior precludes
any symmetry assumptions, hence the entire panel is modeled. The same mesh is used with the 4-node
shell element (type S4R5) and also with the 9-node shell element (type S9R5); the 9-node element mesh,
thus, has about four times the number of degrees of freedom as the 4-node element mesh. The 6-node
triangular shell element STRI65 is also used; it employs two triangles for each quadrilateral element of the
second-order mesh. Mesh generation is facilitated by specifying node fill and node mapping, as shown
in the input data. In this model specification of the relative angle of orientation to define the material
orientation within each layer, along with orthotropic elasticity in plane stress, makes the definition of the
laminae properties straightforward.
The shell elements used in this example use an approximation to thin shell theory, based on a
numerical penalty applied to the transverse shear strain along the element edges. These elements are
not universally applicable to the analysis of composites since transverse shear effects can be significant
in such cases and these elements are not designed to model them accurately. Here, however, the geometry
of the panel is that of a thin shell; and the symmetrical lay-up, along with the relatively large number of
laminae, tends to diminish the importance of transverse shear deformation on the response.
Relation between stress resultants and generalized strains
The shell section is most easily defined by giving the layer thickness, material, and orientation, in which
case Abaqus preintegrates to obtain the section stiffness properties. However, the user can choose to
input the section stiffness properties directly instead, as follows.
In Abaqus a lamina is considered as an orthotropic sheet in plane stress. The principal material axes
of the lamina (see Figure 1.2.2–3) are longitudinal, denoted by L; transverse to the fiber direction in the
surface of the lamina, denoted by T; and normal to the lamina surface, denoted by
The constitutive
relations for a general orthotropic material in the principal directions (
) are
1.2.2–2
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
In terms of the data required to define orthotropic elasticity by specifying terms in the elastic stiffness
matrix in Abaqus these are
then
This matrix is symmetric and has nine independent constants. If we assume a state of plane stress,
is taken to be zero. This yields
where
The correspondence between these terms and the usual engineering constants that might be given
for a simple orthotropic layer in a laminate is
The parameters used on the right-hand side of the above equation are those that must be provided as part
of the definition of orthotropic elasticity in plane stress.
1.2.2–3
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
If the (
) system denotes the standard shell basis directions that Abaqus chooses by default,
the local stiffness components must be rotated to this system to construct the lamina’s contribution to the
general shell section stiffness. Since
represent fourth-order tensors, in the case of a lamina they are
oriented at an angle to the standard shell basis directions used in Abaqus. Hence, the transformation is
where
are the stiffness coefficients in the standard shell basis directions used by Abaqus.
Abaqus assumes that a laminate is a stack of laminae arranged with the principal directions of each
layer in different orientations. The various layers are assumed to be rigidly bonded together. The section
force and moment resultants per unit length in the normal basis directions in a given layer can be defined
on this basis as
where h is the thickness of the layer.
This leads to the relations
1.2.2–4
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
where the components of this section stiffness matrix are given by
and
Here m indicates a particular layer. Thus, the
depend on the material properties and fiber orientation
of the mth layer. The
1,2 parameters are the shear correction coefficients as defined by
Whitney (1973). If there are n layers in the lay-up, we can rewrite the above equations as a summation
of integrals over the n laminae. The material coefficients will then take the form
where the
and
in these equations indicate that the mth lamina is bounded by surfaces
and
See Figure 1.2.2–4 for the nomenclature.
These equations define the coefficients required for the direct input of the section stiffness matrix
method in the general shell section. Only the
,
, and
submatrices are needed for that option.
The three terms in
, if required, are defined as part of the transverse shear stiffness. The section forces
as defined above are in the normal shell basis directions.
Applying these equations to the laminate defined for this example leads to the following overall
section stiffness:
1.2.2–5
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
kN/mm
kN-mm
kN/mm,
or
lb/in
lb-in
lb/in
Results and discussion
The total axial force necessary to compress the panel 0.803 mm (0.0316 in) is 100.2 kN (22529 lb) for the
mesh of S9R5 elements, 99.5 kN (22359 lb) for the mesh of S4R5 elements, and 100.3 kN (22547 lb) for
the mesh of STRI65 elements. These values match closely with the result of 100 kN (22480 lb) reported
by Stanley (1985). Figure 1.2.2–5 shows the displaced configuration and a profile of axial force along
the midsection of the panel (at
). It is interesting to note that the axial load is distributed almost
evenly across the entire panel, with only a very localized area near the hole subjected to an amplified
stress level. This suggests that adequate results for this linear analysis could also be obtained with a
coarser mesh that has a bias toward the hole.
The second stage of the analysis is the eigenvalue buckling prediction. To obtain the buckling
predictions with Abaqus, an eigenvalue buckling prediction step is run. In this step nominal values
of load are applied. The magnitude that is used is not of any significance, since eigenvalue buckling
is a linear perturbation procedure: the stiffness matrix and the stress stiffening matrix are evaluated
at the beginning of the step without any of this load applied. The eigenvalue buckling prediction step
calculates the eigenvalues that, multiplied with the applied load and added to any “base state” loading, are
the predicted buckling loads. The eigenvectors associated with the eigenvalues are also obtained. This
procedure is described in more detail in “Eigenvalue buckling prediction,” Section 6.2.3 of the Abaqus
Analysis User’s Manual.
The buckling predictions are summarized in Table 1.2.2–1 and Figure 1.2.2–6. The buckling load
predictions from Abaqus are higher than those reported by Stanley. The eigenmode predictions given
by the mesh using element types S4R5, S9R5, and STRI65 are all the same and agree well with those
reported by Stanley. Stanley makes several important observations that remain valid for the Abaqus
results: (1) the eigenvalues are closely spaced; (2) nevertheless, the mode shapes vary significantly in
1.2.2–6
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
character; (3) the first buckling mode bears the most similarity to the linear prebuckling solution; (4)
there is no symmetry available that can be utilized for computational efficiency.
Following the eigenvalue buckling analyses, nonlinear postbuckling analysis is carried out by
imposing an imperfection based on the fourth buckling mode. The maximum initial perturbation is
10% of the thickness of the shell. The load versus normalized displacement plots for the S9R5 mesh,
the S4R5 mesh, and the STRI65 mesh are compared with the experimental results and those given by
Stanley in Figure 1.2.2–7. The overall response prediction is quite similar for the Abaqus elements,
although the general behavior predicted by Stanley is somewhat different. The Abaqus results show
a peak load slightly above the buckling load predicted by the eigenvalue extraction, while Stanley’s
results show a significantly lower peak load. In addition, the Abaqus results show rather less loss of
strength after the initial peak, followed quite soon by positive stiffness again. Neither the Abaqus results
nor Stanley’s results agree closely with the experimentally observed dramatic loss of strength after peak
load. Stanley ascribes this to material failure (presumably delamination), which is not modeled in his
analyses or in these.
Figure 1.2.2–8 shows the deformed configurations for the panel during its postbuckling response.
The plots show the results for S4R5, but the pattern is similar for S9R5 and STRI65. The response is
quite symmetric initially; but, as the critical load is approached, a nonsymmetric dimple develops and
grows, presumably accounting for the panel’s loss of strength. Later in the postbuckling response another
wrinkle can be seen to be developing.
Input files
laminpanel_s9r5_prebuckle.inp
laminpanel_s9r5_buckle.inp
laminpanel_s9r5_postbuckle.inp
laminpanel_s4r5_prebuckle.inp
laminpanel_s4r5_buckle.inp
laminpanel_s4r5_postbuckle.inp
laminpanel_s4r5_node.inp
laminpanel_s9r5_stri65_node.inp
laminpanel_stri65_prebuckle.inp
laminpanel_stri65_buckle.inp
laminpanel_stri65_postbuckle.inp
laminpanel_s4_prebuckle.inp
laminpanel_s4_buckle.inp
Prebuckling analysis for the 9-node (element type S9R5)
mesh.
Eigenvalue buckling prediction using element type S9R5.
Nonlinear postbuckling analysis using element type
S9R5.
Prebuckling analysis using element type S4R5.
Eigenvalue buckling prediction using element type S4R5.
Nonlinear postbuckling analysis using element type
S4R5.
Nodal coordinate data for the imperfection imposed for
the postbuckling analysis using element type S4R5.
Nodal coordinate data for the imperfection imposed for
the postbuckling analysis using element types S9R5 and
STRI65.
Prebuckling analysis using element type STRI65.
Eigenvalue buckling prediction using element type
STRI65.
Nonlinear postbuckling analysis using element type
STRI65.
Prebuckling analysis using element type S4.
Eigenvalue buckling prediction using element type S4.
1.2.2–7
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
laminpanel_s4_postbuckle.inp
Nonlinear postbuckling analysis using element type S4.
References
•
Knight, N. F., and J. H. Starnes, Jr., “Postbuckling Behavior of Axially Compressed GraphiteEpoxy Cylindrical Panels with Circular Holes,” presented at the 1984 ASME Joint Pressure Vessels
and Piping/Applied Mechanics Conference, San Antonio, Texas, 1984.
•
Stanley, G. M., Continuum-Based Shell Elements, Ph.D. Dissertation, Department of Mechanical
Engineering, Stanford University, 1985.
•
Whitney, J. M., “Shear Correction Factors for Orthotropic Laminates Under Static Loads,” Journal
of Applied Mechanics, Transactions of the ASME, vol. 40, pp. 302–304, 1973.
1.2.2–8
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
Table 1.2.2–1
Summary of buckling load predictions.
Mode 1
Stanley
S9R5
S4R5
S4
STRI65
107.0 kN (24054 lb)
113.4 kN (25501 lb)
115.5 kN (25964 lb)
114.3 kN (25696 lb)
113.8 kN (25579 lb)
Mode 2
Stanley
S9R5
S4R5
S4
STRI65
109.6 kN (24638 lb)
117.6 kN (26429 lb)
121.2 kN (27244 lb)
116.5 kN (26196 lb)
117.8 kN (26492 lb)
Mode 3
Stanley
S9R5
S4R5
S4
STRI65
116.2 kN (26122 lb)
120.3 kN (27049 lb)
124.7 kN (28042 lb)
124.1 kN (27889 lb)
121.1 kN (27217 lb)
Mode 4
Stanley
S9R5
S4R5
S4
STRI65
140.1 kN
147.5 kN
156.1 kN
152.3 kN
146.9 kN
(31494
(33161
(35092
(34247
(33015
lb)
lb)
lb)
lb)
lb)
Mode 5
Stanley
S9R5
S4R5
S4
STRI65
151.3 kN
171.3 kN
181.5 kN
184.2 kN
172.8 kN
(34012
(38512
(40800
(41413
(38843
lb)
lb)
lb)
lb)
lb)
1.2.2–9
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
z
R
δ
θ
R
d
L
C
GEOMETRIC PROPERTIES:
L = 355.6 mm (14 in)
C = 355.6 mm (14 in)
R = 381.0 mm (15 in)
d = 50.80 mm (2 in)
θ = 55.6°
hlayer = 0.142 mm (.0056 in)
LOADING:
Uniform axial compression δ = 0.803 mm (.0316 in)
Figure 1.2.2–1
Geometry for cylindrical panel with hole.
1.2.2–10
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
3
1
2
1
2
3
Figure 1.2.2–2
Mesh for cylindrical panel with hole.
1.2.2–11
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
N
δ2
T (Transverse)
θ
Fiber
z
θ
y
δ1
x
L (Longitudinal)
Matrix
Figure 1.2.2–3
Typical lamina.
1.2.2–12
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
(a) unbonded
3
L
2
θ3
m=1
(b) bonded
θ1
L
x
-θ2 x
L
x
m=n
hm
hm-1
h
z
3
y
2
1
x
Figure 1.2.2–4
Typical laminate.
1.2.2–13
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
z
S
P = 100.2 kN
(22530 lb)
(Axial)
5000.00
Stanley (1985)
4000.00
N (lb/in)
Stanley (1985)
ABAQUS
3000.00
ABAQUS
2000.00
1000.00
0.00
0.0
1.0
2.0
3.0
4.0
5.0
6.0
7.0
8.0
9.0 10.0 11.0 12.0 13.0 14.0
Arc position S, in
Figure 1.2.2–5
Displaced shape and axial force distribution.
1.2.2–14
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
Buckling Mode 1
Buckling Mode 2
Buckling Mode 3
Buckling Mode 4
Buckling Mode 5
Figure 1.2.2–6
Buckling modes, element types S4R5, S9R5, and STRI65.
1.2.2–15
Abaqus Version 6.12 ID:
Printed on:
LAMINATED PANEL
3.0
Linear Buckling Load
P/EA, 10-3
2.0
S 4R 5
S 9R 5
STRI65
F.E. (Stanley)
Experimental
1.0
0
0
1.0
2.0
3.0
4.0
Delta/L, 10-3
Figure 1.2.2–7
Load-displacement response.
1.2.2–16
Abaqus Version 6.12 ID:
Printed on:
5.0
LAMINATED PANEL
Figure 1.2.2–8
Postbuckling deformations: 10% h imperfection with S4R5.
1.2.2–17
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
1.2.3
BUCKLING OF A COLUMN WITH SPOT WELDS
Products: Abaqus/Standard
Abaqus/Explicit
Abaqus/CAE
This example illustrates both a static and dynamic collapse of a steel column constructed by spot welding
two channel sections. It is intended to illustrate the modeling of spot welds. “Mesh-independent fasteners,”
Section 34.3.4 of the Abaqus Analysis User’s Manual, discusses the mesh-independent spot weld modeling
capabilities provided in Abaqus; while “Breakable bonds,” Section 36.1.9 of the Abaqus Analysis User’s
Manual, discusses the use of bonds and bonding properties to model breakable spot welds in Abaqus/Explicit.
Problem description
The pillar is composed of two columns of different cross-sections, one box-shaped and the other
W-shaped, welded together with spot welds (Figure 1.2.3–1). The top end of the pillar is connected to
a rigid body, which makes the deformation of the pillar easy to control by manipulating the rigid body
reference node. The box-shaped column is welded to the W-shaped column with five spot welds on
either side of the box-shaped column.
The columns are both composed of aluminum-killed steel, which is assumed to satisfy the RambergOsgood relation between true stress and logarithmic strain,
where Young’s modulus (E) is 206.8 GPa, the reference stress value (K) is 0.510 GPa, and the
work-hardening exponent (n) is 4.76. In the present Abaqus analyses the Ramberg-Osgood relation
is approximated using elastic and plastic material properties. The material is assumed to be linear
elastic up to a yield stress of 170.0 MPa, and the stress-strain curve beyond the yield stress is defined in
piecewise linear segments using plastic material properties. Poisson’s ratio is 0.3.
The spot welds are modeled in both Abaqus/Standard and Abaqus/Explicit using the
mesh-independent fastener capability.
Connector elements with CARTESIAN and CARDAN
sections are used to define deformable fasteners. Alternatively, a BUSHING connection type could have
been used. The element set containing the connector elements is referenced in the mesh-independent
fastener. The spot welds at nodes 5203, 15203, 25203, 35203, and 45203 are all located on the positive
z-side of the box-shaped column, with node 5203 at the bottom end of the column and node 45203 at the
top end of the column (see Figure 1.2.3–2). Spot welds at nodes 5211, 15211, 25211, 35211, and 45211
are all located on the negative z-side of the box-shaped column, with node 5211 at the bottom end of
the column and node 45211 at the top end of the column. The surfaces of the box-shaped column and
the W-shaped column are specified in the mesh-independent fastener. The spot welds are defined with
a diameter of .002 m. The deformable behavior in the fastener is modeled using connector elasticity,
with an elastic spring stiffness of 2 × 1011 N/m in translational as well as rotational components.
For the Abaqus/Explicit analysis spot weld damage and failure are modeled using connector damage
behavior. A force-based coupled damage initiation criterion that uses a connector potential with both
connector force and connector moment ingredients is used. (For further description of the connector
1.2.3–1
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
potential used, see the spot weld example in “Connector functions for coupled behavior,” Section 31.2.4
of the Abaqus Analysis User’s Manual.) Damage initiates when the value of the potential exceeds
2 × 105 N. A post-damage-initiation equivalent displacement of 1 × 10−7 m is allowed. Once the
post-damage-initiation equivalent displacement in a spot weld reaches this value, the spot weld ceases to
carry any load. Both the continuum and structural coupling capabilities are used to define the fasteners.
To study spot weld failure and the post-yield behavior of the spot welds in detail, the problem is also
solved using the bond properties available in Abaqus/Explicit. The column with the box-shaped crosssection is defined to be the slave surface in contact with the column with the W-shaped cross-section.
The spot welds on the two sides of the box-shaped column are modeled with different yield forces and
post-yield behavior to illustrate the two failure models. For the spot-welded nodes 5203, 15203, 25203,
35203, and 45203, the force to cause failure for the spot welds is 3000 N in pure tension and 1800 N
in pure shear. Once the spot welds start to fail, the maximum force that they can bear is assumed to
decay linearly with time over the course of 2.0 msec, which illustrates the modeling of complete loss
of strength over a given time period. For the spot-welded nodes 5211, 15211, 25211, 35211, and 45211,
the force to cause failure for these spot welds is 4000 N in pure tension and 2300 N in pure shear. These
spot welds fail according to the damaged failure model, which assumes that the maximum forces that the
spot welds can carry decay linearly with relative displacement between the welded node and the master
surface. The welds are defined to fail completely once their total relative displacement reaches 0.3mm,
which illustrates the modeling of loss of strength in the spot welds based on energy absorption.
A Python script is included that reproduces the model using the Scripting Interface in Abaqus/CAE.
The script creates and assembles Abaqus/CAE parts and uses discrete fasteners to model the spot welds.
The script creates an Abaqus/Standard model that is ready to be submitted for analysis from the Job
module. The discrete fasteners created by the script result in the following differences compared with
the mesh-independent, or point-based, fasteners used by the example input files:
•
When you submit the Abaqus/CAE job for analysis, the discrete fasteners created by the Python
script generate coupling constraints and distributing coupling constraints in the input file, together
with connector elements. The example input files use mesh-independent fasteners to model pointbased fasteners using connector elements.
•
You must define the radius of influence when you create a discrete fastener using Abaqus/CAE. In
contrast, the example input files allow Abaqus to compute a default value of the radius of influence
based on the geometric properties of the fastener, the characteristic length of connected facets, and
the type of weighting function selected.
•
The input files share nodes between the pillar and the rigid body. To achieve similar behavior, the
Python script creates tie constraints between the pillar and the rigid body.
For a description of the differences between discrete fasteners and point-based fasteners in Abaqus/CAE,
see “About fasteners,” Section 29.1 of the Abaqus/CAE User’s Manual.
Loading
The bottom of the pillar is fully fixed. In the Abaqus/Standard analysis the reference node for the rigid
body at the top of the pillar moves 0.25 m in the y-direction, thus loading it in compression, together with
1.2.3–2
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
a displacement of .02 m in the z-direction that shears it slightly. At the same time the end of the pillar is
rotated about the negative z-axis by 0.785 rad and rotated about the negative x-axis by 0.07 rad.
In the Abaqus/Explicit analyses the reference node for the rigid body at the top of the pillar moves at
a constant velocity of 25 m/sec in the y-direction, thus loading it in compression, together with a velocity
of 2 m/sec in the z-direction that shears it slightly. At the same time the end of the pillar is rotated about
the negative z-axis at 78.5 rad/sec and rotated about the negative x-axis at 7 rad/sec. This loading is
applied by prescribing the velocities of the rigid body reference node that is attached to the top end of
the compound pillar.
The analysis is carried out over 10 milliseconds.
Results and discussion
The mesh-independent spot weld capability and the contact-based spot weld capability predict very
similar deformation patterns and deformed shapes for the pillar. Figure 1.2.3–3 shows the deformed
shape of the pillar after 5.0 msec in the Abaqus/Explicit analysis. Figure 1.2.3–4 shows the deformed
shape of the pillar after 10.0 msec. The spot welds in the mesh-independent Abaqus/Explicit analysis
undergo damage and fail. For the current choice of parameters for the connector damage model, it is
found that damage initiates in the spot welds at nodes 15203 through 45203 on the positive side of the
box-shaped column and at nodes 15211 through 45211 on the negative side of the box-shaped column.
However, the post-damage-initiation displacement is sufficient to cause ultimate failure of the spot welds
at nodes 15203, 25203, 15211, and 25211 only. Figure 1.2.3–9 illustrates the undamaged connector
force CTF3 in the spot welds associated with reference nodes 25203 and 25211 as computed in the
Abaqus/Standard analyses. Figure 1.2.3–10 illustrates the damaged connector force CTF3 in the spot
welds associated with reference nodes 25203 and 25211 as computed in the Abaqus/Explicit analyses.
Forces in both spot welds drop to zero when ultimate failure occurs in the Abaqus/Explicit analyses.
The failure and post-yield behaviors of the pillar are also studied using the contact-based spot weld
capability. Figure 1.2.3–5 and Figure 1.2.3–6 show the status of the spot welds on the positive z-side of
the column and the negative z-side of the column, respectively. In these figures a status of 1.0 means
that the weld is fully intact, and a status of 0.0 means that the weld has failed completely. Figure 1.2.3–7
shows the load on spot weld node 25203 relative to the failure load. This relative value is called the bond
load and is defined to be 1.0 when the spot weld starts to fail and 0.0 when the spot weld is broken. Figures
showing the bond status and bond load may not match the analysis results on a particular platform. This is
due to the fact that contact forces in this analysis show significant noise, which can vary across platforms.
When the time-to-failure model is used, spot weld behavior is very sensitive to any spike in the bond
force that reaches the bond strength. Spot weld behavior is less sensitive to individual spikes in the bond
force when the damaged failure model is used. Figure 1.2.3–8 shows the time history of the total kinetic
energy, the total work done on the model, the total energy dissipated by friction, the total internal energy,
and the total energy balance.
Input files
pillar_fastener_xpl.inp
Input data for the Abaqus/Explicit mesh-independent spot
weld analysis.
1.2.3–3
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
pillar_fastener_structcoup_xpl.inp
pillar_fastener_std.inp
pillar_fastener_structcoup_std.inp
pillar_fastener_smslide_std.inp
pillar.inp
pillar_gcont.inp
pillar_rest.inp
pillar_ds.inp
Input data for the Abaqus/Explicit mesh-independent spot
weld analysis using structural coupling in the fastener
definitions.
Input data for the Abaqus/Standard mesh-independent
spot weld analysis.
Input data for the Abaqus/Standard mesh-independent
spot weld analysis using structural coupling in the
fastener definitions.
Input data for the Abaqus/Standard mesh-independent
spot weld analysis using small-sliding contact with shell
thickness taken into account.
Input data for the contact-pair-based spot weld analysis.
Input data for the general-contact-based spot weld
analysis.
Input data used to test the restart capability with spot
welds.
Analysis using the double-sided surface capability.
Python script
pillar_fastener_std.py
Script that creates a model with discrete fasteners using
Abaqus/CAE.
1.2.3–4
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
2
1
3
Figure 1.2.3–1
Initial configuration of the compound pillar.
2
3
Figure 1.2.3–2
1
Initial configuration of the box-shaped column showing spot welds.
1.2.3–5
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
2
1
3
Figure 1.2.3–3
Deformed shape at 5.0 msec.
2
3
1
Figure 1.2.3–4
Deformed shape at 10.0 msec.
1.2.3–6
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
Figure 1.2.3–5
Time histories of the status of all spot welds on positive z-side of column.
node
node
node
node
node
Figure 1.2.3–6
5211
15211
25211
35211
45211
Time histories of the status of all spot welds on negative z-side of column.
1.2.3–7
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
Figure 1.2.3–7
Time histories of the load on spot weld node 25203 relative to the failure load.
Figure 1.2.3–8 Time histories of the total kinetic energy, energy dissipated by friction,
work done on the model, internal energy, and total energy.
1.2.3–8
Abaqus Version 6.12 ID:
Printed on:
BUCKLING OF A COLUMN WITH SPOT WELDS
Figure 1.2.3–9
Connector force CTF3 in spot welds at reference nodes 25203
and 25211 for Abaqus/Standard.
Figure 1.2.3–10
Connector force CTF3 in spot welds at reference nodes
25203 and 25211 for Abaqus/Explicit.
1.2.3–9
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC FRAME
1.2.4
ELASTIC-PLASTIC K-FRAME STRUCTURE
Product: Abaqus/Standard
This example illustrates the use of the frame element FRAME2D. Frame elements (“Frame elements,”
Section 29.4.1 of the Abaqus Analysis User’s Manual) can be used to model elastic, elastic-plastic, and
buckling strut responses of individual members of frame-like structures. The elastic response is defined by
Euler-Bernoulli beam theory. The elastic-plastic response is modeled with nonlinear kinematic hardening
plasticity concentrated at the element’s ends, simulating the development of plastic hinges. The buckling
strut response is a simplified, phenomenological representation of the highly nonlinear cross-section collapse
and material yielding that takes place when slender members are loaded in compression .Therefore, frame
elements can be elastic, elastic-plastic, behave as struts (with or without buckling), or switch during the
analysis to strut behavior followed by postbuckling behavior. Both the elastic-plastic and buckling strut
responses are simplifications of highly nonlinear responses. They are designed to approximate these complex
responses with a single finite element representing a structural member between connections. For parts of
the model where higher solution resolution is required, such as stress prediction, the model should be refined
with beam elements.
The geometry in this example is a typical K-frame construction used in applications such as offshore
structures (see Figure 1.2.4–1). A push-over analysis is performed to determine the maximum horizontal
load that the structure can support before collapse results from the development of plastic hinges or buckling
failure. During a push-over test, many structural members are loaded in compression. Slender members
loaded in compression often fail due to geometric buckling, cross-section collapse, and/or material yielding.
The buckling strut response, which models such compressive behavior, is added in separate simulations to
investigate the effect of the compressive failure of critical members in the structure. A dead load is applied to
the top of the structure representing the weight supported by the K-frame. Push-over analyses are either load
or displacement control tests.
Geometry and model
The structure consists of 19 members between structural connections. Each finite element models a
member of the frame. Hence, 19 frame elements are used: 17 elements with PIPE cross-sections of
varying properties and 2 elements (the top platform) with I cross-sections. The plastic response of the
elements is calculated from the yield stress of the material, using the plastic default values provided
by Abaqus. (The default values for the plastic response are based on experiments with slender steel
members. For details on the default values, see “Frame section behavior,” Section 29.4.2 of the Abaqus
Analysis User’s Manual.) The default plastic response includes mild hardening for axial forces and
strong hardening for bending moments. The default hardening responses for a typical element in the
model are shown in Figure 1.2.4–2 and Figure 1.2.4–3.
A dead load of 444.8 kN (100,000 lb) is applied to the top of the K-frame, representing the part of
the structure above the K-frame. Subsequently, the top platform is loaded or displaced horizontally. The
load level or applied displacement is chosen to be large enough so that the entire structure fails by the
formation of plastic hinges and, consequently, loses load carrying capacity.
1.2.4–1
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC FRAME
Three different models are investigated. A limit load is expected, since the goal of the analysis
is to determine when the structure loses overall stiffness. Large- and small-displacement analyses are
performed for all three models for comparison. Large-displacement analyses using frame elements are
valid for large overall rotations but small strains, since frame elements assume that the strains are small.
In the first model all elements use elastic-plastic material response. In the second model buckling is
checked for all elements with PIPE cross-sections. The ISO equation is used as a criteria for buckling,
and the default Marshall strut envelope is followed for the postbuckling behavior. The buckling strut
envelope is calculated from the yield stress of the material and the default Marshall Strut theory. (For
details on the default buckling strut envelope, see “Frame section behavior,” Section 29.4.2 of the Abaqus
Analysis User’s Manual.) All frame members that use the buckling strut response check the ISO criteria
for the switching-to-strut algorithm. In the third model the member that switches to strut behavior in the
second model (element 7) is replaced by a frame element with buckling strut response from the beginning
of the analysis. To proceed beyond the unstable phase of the response, the Riks static solution procedure
is used in the elastic-plastic problems. To decrease the number of solution iterations, the solution controls
are used in the elastic-plastic problem with large displacement, with the value of the ratio of the largest
solution correction to the largest incremental solution set to 1.0, since displacement increments are very
small after plasticity occurs.
Results and discussion
The structure is loaded or displaced to the point at which all load carrying capacity is lost. In the first
model with elastic-plastic frame elements, the results for the linear and nonlinear geometries compare
as expected. That is, the limit load for the large-displacement analysis is reached at a load of 1141 kN
(256,000 lb) as compared to a higher load of 1290 kN (291,000 lb) in the small-displacement analysis.
The plastic hinge pattern is the same in both cases.
The second model uses the switching algorithm. It shows that element 7 first violates the ISO
equation (buckles) at a prescribed displacement equal to 1.32 cm (0.52 in), before any elements form
plastic hinges. The critical compressive force in this element is –318 kN (–71,400 lb). Next, plasticity
develops at several elements, and the structure reaches its limit capacity. The frame elements with the
switching algorithm predict the structural behavior in the most accurate way, since the possibility of
buckling is checked for all elements in the model, and highly compressed members switch automatically
to postbuckling behavior (see the plastic and buckled frame elements in Figure 1.2.4–4). When the
structure can no longer support horizontal loading, the patterns of plastic hinges for linear and nonlinear
geometry are the same. The results differ more for loads close to the limit load.
To investigate the effect of buckling, the first and the third (element 7 defined with
buckling strut response from the beginning) models are compared (kframe_loadcntrl_nlgeom.inp
and kframe_dispcntrl_buckle_nlgeom.inp).
Load versus horizontal deflection curves for the
large-displacement analyses are shown in Figure 1.2.4–5. Similar to the model with switching
algorithm, first element 7 buckles. As the other members deform and absorb the load no longer carried
by the buckled member, the structure regains stiffness and plasticity develops in other members. When
seven members develop plastic hinges, the structure can no longer support additional horizontal loading.
The limit load in the third model is only about 28% of the limit load in the model without buckling.
1.2.4–2
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC FRAME
The load-displacement curves for the switching algorithm and for the example with element 7 using
buckling strut response compare well and are not shown.
Input files
kframe_loadcntrl_nlgeom.inp
kframe_loadcntrl.inp
kframe_dispcntrl_switch_nlgeom.inp
kframe_dispcntrl_switch.inp
kframe_dispcntrl_buckle_nlgeom.inp
kframe_dispcntrl_buckle.inp
Elastic-plastic analysis with load control;
large-displacement analysis.
Elastic-plastic analysis with load control;
small-displacement analysis.
Elastic-plastic frame element with the switching
algorithm and displacement control; large-displacement
analysis.
Elastic-plastic frame element with the switching
algorithm and displacement control; small-displacement
analysis.
Elastic-plastic and buckling strut response with load
control; large-displacement analysis.
Elastic-plastic and buckling strut response with
displacement control; small-displacement analysis.
I section
5.33 m
1.52 m
PIPE sections
8.05 m 4.08 m
2.44 m
;;;;;;;
;;;;;;;
;;;;;;;
;;;;;;;
;;;;;;;
;;;;;;;
7.11 m
Figure 1.2.4–1
Two-dimensional K-frame structure.
1.2.4–3
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC FRAME
1.0
[ x10 3 ]
axial force (kN)
0.8
0.6
0.4
fitted curve
default values
0.2
0.0
0.
5.
10.
15.
20.
plastic displacement / L
25.
30.
[ x10 -3 ]
Figure 1.2.4–2 Default hardening response for axial force in a
typical element with PIPE cross-section (element 7 in the model).
40.
36.
bending moment (kN-m)
32.
28.
24.
20.
16.
fitted curve
default values
12.
8.
4.
0.
0.00
0.02
0.04
0.06
0.08
plastic rotation / L (1/m)
Figure 1.2.4–3 Default hardening response for bending moments in
a typical element with PIPE cross-section (element 7 in the model).
1.2.4–4
Abaqus Version 6.12 ID:
Printed on:
ELASTIC-PLASTIC FRAME
12
10
10
18
buckled element
with postbuckling
behavior
13
11
12
11
19
9
9
7
16
7
8
5
4
plastic element
with lumped
plasticity
17
6
5
6
2
14
3
3
4
15
1
1
1
2
2
3
Figure 1.2.4–4 Results of analysis with switching algorithm:
K-frame model with plastic and buckled elements.
1.2
[ x10 3 ]
1.0
applied load (kN)
0.8
elastic-plastic
buckling strut
0.6
0.4
0.2
0.0
0.
10.
20.
30.
40.
50.
horizontal displacement (cm)
Figure 1.2.4–5 Applied force versus horizontal displacement of the load point for the
elastic-plastic model and the model including buckling strut response.
1.2.4–5
Abaqus Version 6.12 ID:
Printed on:
REINFORCED PLATE
1.2.5
UNSTABLE STATIC PROBLEM: REINFORCED PLATE UNDER COMPRESSIVE
LOADS
Product: Abaqus/Standard
This example demonstrates the use of automatic techniques to stabilize unstable static problems.
Geometrically nonlinear static problems can become unstable for a variety of reasons. Instability may occur
in contact problems, either because of chattering or because contact intended to prevent rigid body motions
is not established initially. Localized instabilities can also occur; they can be either geometrical, such as
local buckling, or material, such as material softening.
This problem models a reinforced plate structure subjected to in-plane compressive loading that produces
localized buckling. Structures are usually designed for service loads properly augmented by safety factors.
However, it is quite often of interest to explore their behavior under extreme accident loads. This example
looks into a submodel of a naval construction structure. It is a rectangular plate reinforced with beams in
its two principal directions (Figure 1.2.5–1). The plate has symmetry boundary conditions along the longer
edges and is pinned rigidly along the shorter sides. An in-plane load is applied to one of the pinned sides,
compressing the plate. Gravity loads are also applied. The plate buckles under the load. The buckling is
initially localized within each of the sections bounded by the reinforcements. At higher load levels the plate
experiences global buckling in a row of sections closest to the applied load.
Standard analysis procedures typically provide the load at which the structure starts to buckle. The
user may be interested in knowing the structure’s additional load carrying capacity. This information could
translate, for instance, into knowing when the onset of global buckling takes place or how far into the structure
damage propagates. In such situations more sophisticated analysis techniques are necessary. Arc length
methods such as the Riks method available in Abaqus are global load-control methods that are suitable for
global buckling and postbuckling analyses; they do not function well when buckling is localized. Alternatives
are to analyze the problem dynamically or to introduce damping. In the dynamic case the strain energy
released locally from buckling is transformed into kinetic energy; in the damping case this strain energy is
dissipated. To solve a quasi-static problem dynamically is typically an expensive proposition. In this example
the automatic stabilization capability in Abaqus, which applies volume proportional damping to the structure,
is used.
Geometry and model
The model consists of a rectangular plate 10.8 m (425.0 in) long, 6.75 m (265.75 in) wide, and 5.0 mm
(0.2 in) thick. This plate has several reinforcements in both the longitudinal and transverse directions
(Figure 1.2.5–1). The plate represents part of a larger structure: the two longitudinal sides have symmetry
boundary conditions, and the two transverse sides have pinned boundary conditions. In addition, springs
at two major reinforcement intersections represent flexible connections to the rest of the structure. The
mesh consists of S4 shell elements for both the plate and larger reinforcements and additional S3 shell
and B31 beam elements for the remaining reinforcements. The entire structure is made of the same
construction steel, with an initial flow stress of 235.0 MPa (34.0 ksi).
1.2.5–1
Abaqus Version 6.12 ID:
Printed on:
REINFORCED PLATE
To provide stability to the numerical solution upon the anticipated buckling, automatic stabilization
based on volume proportional damping is added to the model. Two forms of automatic stabilization are
considered: one with a constant damping factor that is chosen by default (see “Automatic stabilization
of static problems with a constant damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the
Abaqus Analysis User’s Manual), and one with an adaptive damping factor (see “Adaptive automatic
stabilization scheme” in “Solving nonlinear problems,” Section 7.1.1 of the Abaqus Analysis User’s
Manual).
Results and discussion
The analysis consists of two steps. In the first step a gravity load perpendicular to the plane of the plate
is applied. In the second step a longitudinal compressive load of 6.46 × 106 N (1.45 × 106 lbf) is applied
to one of the pinned sides of the plate. All the nodes on that side are forced to move equally by means
of multi-point constraints. The analysis is quasi-static, but buckling is expected.
Initially local out-of-plane buckling develops throughout the plate in an almost checkerboard
pattern inside each one of the sections delimited by the reinforcements (Figure 1.2.5–2). Later, global
buckling develops along a front of sections closer to the applied load (Figure 1.2.5–3). The evolution
of the displacements produced by the applied load is very smooth (Figure 1.2.5–4) and does not reflect
the early local instabilities in the structure. However, when the global instability develops, the curve
becomes almost flat, indicating the complete loss of load carrying capacity. An inspection of the
model’s energy content (Figure 1.2.5–5 and Figure 1.2.5–6) reveals that while the load is increasing, the
amount of dissipated energy is negligible. As soon as the load flattens out, the strain energy also flattens
out (indicating a more or less constant load carrying capacity), while the dissipated energy increases
dramatically to absorb the work done by the applied loads.
Figure 1.2.5–7 shows the ratio of the dissipated energy to the total strain energy obtained using a
constant damping factor versus using an adaptive damping factor.
Acknowledgments
SIMULIA would like to thank IRCN (France) for providing this example.
Input files
unstablestatic_plate.inp
unstablestatic_plate_stabil_adap.inp
unstablestatic_plate_node.inp
unstablestatic_plate_elem.inp
Plate model.
Plate model with adaptive stabilization.
Node definitions for the plate model.
Element definitions for the plate model.
1.2.5–2
Abaqus Version 6.12 ID:
Printed on:
REINFORCED PLATE
Figure 1.2.5–1
Reinforced plate initial mesh.
Figure 1.2.5–2
Plate localized buckling.
1.2.5–3
Abaqus Version 6.12 ID:
Printed on:
REINFORCED PLATE
Figure 1.2.5–3
Figure 1.2.5–4
Plate global buckling.
Plate load-displacement curve.
1.2.5–4
Abaqus Version 6.12 ID:
Printed on:
REINFORCED PLATE
SD_LOAD
SE_LOAD
Figure 1.2.5–5
Dissipated and strain energies as functions of load.
SD_DISP
SE_DISP
Figure 1.2.5–6
Dissipated and strain energies as functions of displacement.
1.2.5–5
Abaqus Version 6.12 ID:
Printed on:
REINFORCED PLATE
Ratio of dissipated energy to total energy
Stabilization with constant damping factor
Adaptive automatic stabilization
0.25
0.20
0.15
0.10
0.05
0.00
0.0
1.0
2.0
3.0
4.0
5.0
6.0
[x1.E6]
Concentrated Load − CF1
Figure 1.2.5–7
Ratio of dissipated energy to total strain energy using a constant
damping factor and adaptive stabilization.
1.2.5–6
Abaqus Version 6.12 ID:
Printed on:
IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
1.2.6
BUCKLING OF AN IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
Product: Abaqus/Standard
This example serves as a guide to performing a postbuckling analysis using Abaqus for an imperfectionsensitive structure. A structure is imperfection sensitive if small changes in an imperfection change the
buckling load significantly. Qualitatively, this behavior is characteristic of structures with closely spaced
eigenvalues. For such structures the first eigenmode may not characterize the deformation that leads to the
lowest buckling load. A cylindrical shell is chosen as an example of an imperfection-sensitive structure.
Geometry and model
The cylinder being analyzed is depicted in Figure 1.2.6–1. The cylinder is simply supported at its ends
and is loaded by a uniform, compressive axial load. A uniform internal pressure is also applied to the
cylinder. The material in the cylinder is assumed to be linear elastic. The thickness of the cylinder is
1/500 of its radius, so the structure can be considered to be a thin shell.
The finite element mesh uses the fully integrated S4 shell element. This element is based on a finite
membrane strain formulation and is chosen to avoid hourglassing. A full-length model is used to account
for both symmetric and antisymmetric buckling modes. A fine mesh, based on the results of a refinement
study of the linear eigenvalue problem, is used. The convergence of the mesh density is based on the
relative change of the eigenvalues as the mesh is refined. The mesh must have several elements along
each spatial deformation wave; therefore, the level of mesh refinement depends on the modes with the
highest wave number in the circumferential and axial directions.
Solution procedure
The solution strategy is based on introducing a geometric imperfection in the cylinder. In this study
the imperfections are linear combinations of the eigenvectors of the linear buckling problem. If details
of imperfections caused in a manufacturing process are known, it is normally more useful to use
this information as the imperfection. However, in many instances only the maximum magnitude of
an imperfection is known. In such cases assuming the imperfections are linear combinations of the
eigenmodes is a reasonable way to estimate the imperfect geometry (Arbocz, 1987).
Determining the most critical imperfection shape that leads to the lowest collapse load of an axially
compressed cylindrical shell is an open research issue. The procedure discussed in this example does
not, therefore, claim to compute the lowest collapse load. Rather, this example discusses one approach
that can be used to study the postbuckling response of an imperfection-sensitive structure.
The first stage in the simulation is a linear eigenvalue buckling analysis. To prevent rigid body
motion, a single node is fixed in the axial direction. This constraint is in addition to the simply supported
boundary conditions noted earlier and will not introduce an overconstraint into the problem since the
axial load is equilibrated on opposing edges. The reaction force in the axial direction should be zero at
this node.
1.2.6–1
Abaqus Version 6.12 ID:
Printed on:
IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
The second stage involves introducing the imperfection into the structure using geometric
imperfections. A single mode or a combination of modes is used to construct the imperfection. To
compare the results obtained with different imperfections, the imperfection size must be fixed. The
measure of the imperfection size used in this problem is the out-of-roundness of the cylinder, which is
computed as the radial distance from the axis of the cylinder to the perturbed node minus the radius of
the perfect structure. The scale factor associated with each eigenmode used to seed the imperfection is
computed with a FORTRAN program. The program reads the results file produced by the linear analysis
and determines the scale factors so that the out-of-roundness of the cylinder is equal to a specified value.
This value is taken as a fraction of the cylinder thickness.
The final stage of the analysis simulates the postbuckling response of the cylinder for a given
imperfection. The primary objective of the simulation is to determine the static buckling load. The
modified Riks method is used to obtain a solution since the problem under consideration is unstable. The
Riks method can also be used to trace the unstable and stable solution branches of a buckled structure.
However, with imperfection-sensitive structures the first buckling mode is usually catastrophic, so further
continuation of the analysis is usually not undertaken. When using a static Riks step, the tolerance used
for the force residual convergence criteria may need to be tightened to ensure that the solution algorithm
does not retrace its original loading path once the limit point is reached. Simply restricting the maximum
arc length allowed in an increment is normally not sufficient.
Parametric study
There are two factors that significantly alter the buckling behavior: the shape of the imperfection and
the size of the imperfection. A convenient way to investigate the effects of these factors on the buckling
response is to use the parametric study capabilities of Abaqus. A Python script file is used to perform
the study. The script executes the linear analysis, runs the FORTRAN routine to create an input file with
a specified imperfection size, and finally executes the postbuckling analysis.
Before executing the script, copy the FORTRAN routine cylsh_maximp.f to your work directory
using the Abaqus fetch command,
abaqus fetch job=cylsh_maximp.f
and compile it using the Abaqus make command,
abaqus make job=cylsh_maximp.f
Parametrized template input data are used to generate variations of the parametric study. The
script allows the analyst to vary the eigenmodes used to construct the imperfection, out-of-roundness
measure, cylindrical shell geometry (radius, length, thickness), mesh density, material properties
(Young’s modulus and Poisson’s ratio), etc. The results presented in the following section, however,
are based on an analysis performed with a single set of parameters.
Results and discussion
The results for both the linear eigenvalue buckling and postbuckling analyses are discussed below.
1.2.6–2
Abaqus Version 6.12 ID:
Printed on:
IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
Linear eigenvalue buckling
The Lanczos eigensolver is used to extract the linear buckling modes. This solver is chosen because
of its superior accuracy and convergence rate relative to wavefront solvers for problems with closely
spaced eigenvalues. Table 1.2.6–1 lists the first 19 eigenvalues of the cylindrical shell. The eigenvalues
are closely spaced with a maximum percentage difference of 1.3%.
The geometry, loading, and material properties of the cylindrical shell analyzed in this example are
characterized by their axisymmetry. As a consequence of this axisymmetry the eigenmodes associated
with the linear buckling problem will be either (1) axisymmetric modes associated with a single
eigenvalue, including the possibility of eigenmodes that are axially symmetric but are twisted about
the symmetry axis or (2) nonaxisymmetric modes associated with repeated eigenvalues (Wohlever,
1999). The nonaxisymmetric modes are characterized by sinusoidal variations (n-fold symmetry)
about the circumference of the cylinder. For most practical engineering problems and as illustrated
in Table 1.2.6–1, it is usually found that a majority of the buckling modes of the cylindrical shell are
nonaxisymmetric.
The two orthogonal eigenmodes associated with each repeated eigenvalue span a two-dimensional
space, and as a result any linear combination of these eigenmodes is also an eigenmode; i.e., there
is no preferred direction. Therefore, while the shapes of the orthogonal eigenmodes extracted by the
eigensolver will always be the same and span the same two-dimensional space, the phase of the modes is
not fixed and might vary from one analysis to another. The lack of preferred directions has consequences
with regard to any imperfection study based upon a linear combination of nonaxisymmetric eigenmodes
from two or more distinct eigenvalues. As the relative phases of eigenmodes change, the shape of
the resulting imperfection and, therefore, the postbuckling response, also changes. To avoid this
situation, postprocessing is performed after the linear buckling analysis on each of the nonaxisymmetric
eigenmode pairs to fix the phase of the eigenmodes before the imperfection studies are performed. The
basic procedure involves calculating a scaling factor for each of the eigenvectors corresponding to a
repeated eigenvalue so that their linear combination generates a maximum displacement of 1.0 along
the global X-axis. This procedure is completely arbitrary but ensures that the postbuckling response
calculations are repeatable.
For the sake of consistency the maximum radial displacement associated with a unique eigenmode
is also scaled to 1.0. These factors are further scaled to satisfy the out-of-roundness criterion mentioned
earlier.
Postbuckling response
The modes used to seed the imperfection are taken from the first 19 eigenmodes obtained in the linear
eigenvalue buckling analysis. Different combinations are considered: all modes, unique eigenmodes,
and pairs of repeated eigenmodes. An imperfection size (i.e., out-of-roundness) of 0.5 times the shell
thickness is used in all cases. The results indicate that the cylinder buckles at a much lower load than
the value predicted by the linear analysis (i.e., the value predicted using only the lowest eigenmode
of the system). An imperfection based on mode 1 (a unique eigenmode) results in a buckling load of
about 90% of the predicted value. When the imperfection was seeded with a combination of all modes
(1–19), a buckling load of 33% of the predicted value was obtained. Table 1.2.6–2 lists the buckling
1.2.6–3
Abaqus Version 6.12 ID:
Printed on:
IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
loads predicted by Abaqus (as a fraction of linear eigenvalue buckling load) when different modes are
used to seed the imperfection.
The smallest predicted buckling load in this study occurs when using modes 12 and 13 to seed
the imperfection, yet the results obtained when the imperfection is seeded using all 19 modes indicate
that a larger buckling load can be sustained. One possible explanation for this is that the solution
strategy used in this study (discussed earlier) involves using a fixed value for the out-of-roundness of
the cylinder as a measure of the imperfection size. Thus, when multiple modes are used to seed the
imperfection, the overall effect of any given mode is less than it would be if only that mode were used to
seed the imperfection. The large number of closely spaced eigenvalues and innumerable combinations
of eigenmodes clearly demonstrates the difficulty of determining the collapse load of structures such as
the cylindrical shell. In practice, designing imperfection-sensitive structures against catastrophic failure
usually requires a combination of numerical and experimental results as well as practical building
experience.
The final deformed configuration shown in Figure 1.2.6–2 uses a displacement magnification
factor of 5 and corresponds to using all the modes to seed the imperfection. Even though the cylinder
appears to be very short, it can in fact be classified as a moderately long cylinder using the parameters
presented in Chajes (1985). The cylinder exhibits thin wall wrinkling; the initial buckling shape can be
characterized as dimples appearing on the side of the cylinder. The compression of the cylinder causes a
radial expansion due to Poisson’s effect; the radial constraint at the ends of the cylinder causes localized
bending to occur at the ends. This would cause the shell to fold into an accordion shape. (Presumably
this would be seen if self-contact was specified and the analysis was allowed to run further. This is not
a trivial task, however, and modifications to the solution controls would probably be required. Such
a simulation would be easier to perform with Abaqus/Explicit.) This deformed configuration is in
accordance with the perturbed reference geometry, shown in Figure 1.2.6–3. To visualize the imperfect
geometry, an imperfection size of 5.0 times the shell thickness (i.e., 10 times the value actually used in
the analysis) was used to generate the perturbed mesh shown in this figure. The deformed configuration
in the postbuckling analysis depends on the shape of the imperfection introduced into the structure.
Seeding the structure with different combinations of modes and imperfection sizes produces different
deformed configurations and buckling loads. As the results vary with the size and shape of the
imperfection introduced into the structure, there is no solution to which the results from Abaqus can
be compared.
The load-displacement curve for the case when the first 19 modes are used to seed the imperfection
is shown in Figure 1.2.6–4. The figure shows the variation of the applied load (normalized with respect
to the linear eigenvalue buckling load) versus the axial displacement of an end node. The peak load that
the cylinder can sustain is clearly visible.
Input files
cylsh_buck.inp
cylsh_postbuck.inp
cylsh_maximp.f
cylsh_script.psf
Linear eigenvalue buckling problem.
Postbuckling problem.
FORTRAN program to compute the scaling factors for the
imperfection size.
Python script to generate the parametrized input files.
1.2.6–4
Abaqus Version 6.12 ID:
Printed on:
IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
References
•
Arbocz, J., “Post-Buckling Behaviour of Structures: Numerical Techniques for More Complicated
Structures,” in Lecture Notes in Physics, Ed. H. Araki et al., Springer-Verlag, Berlin, 1987,
pp. 84–142.
•
Chajes, A., “Stability and Collapse Analysis of Axially Compressed Cylindrical Shells,” in Shell
Structures: Stability and Strength, Ed. R. Narayanan, Elsevier, New York, 1985, pp. 1–17.
•
Wohlever, J. C., “Some Computational Aspects of a Group Theoretic Finite Element Approach to
the Buckling and Postbuckling Analyses of Plates and Shells-of-Revolution,” in Computer Methods
in Applied Mechanics and Engineering, vol. 170, pp. 373–406, 1999.
1.2.6–5
Abaqus Version 6.12 ID:
Printed on:
IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
Table 1.2.6–1
Eigenvalue estimates for the first 19 modes.
Mode number
Eigenvalue
1
11723
2, 3
11724
4, 5
11728
6, 7
11734
8, 9
11744
10, 11
11757
12, 13
11775
14, 15
11798
16, 17
11827
18, 19
11864
Table 1.2.6–2
Summary of predicted buckling loads.
Mode used to seed Normalized
the imperfection buckling load
1
0.902
2, 3
0.625
4, 5
0.480
6, 7
0.355
8, 9
0.351
10, 11
0.340
12, 13
0.306
14, 15
0.323
16, 17
0.411
18, 19
0.422
All modes (1–19)
0.325
1.2.6–6
Abaqus Version 6.12 ID:
Printed on:
IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
h
l
a
Uniform
axial pressure
Figure 1.2.6–1
Cylindrical shell with uniform axial loading.
2
1
3
Figure 1.2.6–2 Final deformed configuration of the cylindrical shell (first 19 eigenmodes used to seed
the imperfection; displacement magnification factor of 5.0; normalized end load = 0.29).
1.2.6–7
Abaqus Version 6.12 ID:
Printed on:
IMPERFECTION-SENSITIVE CYLINDRICAL SHELL
2
1
3
Figure 1.2.6–3 Perturbed geometry of the cylindrical shell (imperfection factor = 5 × thickness
for illustration only; actual imperfection factor used = .5 × thickness).
Figure 1.2.6–4 Normalized applied load versus axial displacement
at node 5040 (first 19 modes used to seed the imperfection).
1.2.6–8
Abaqus Version 6.12 ID:
Printed on:
FORMING ANALYSES
1.3
Forming analyses
•
“Upsetting of a cylindrical billet: quasi-static analysis with mesh-to-mesh solution mapping
(Abaqus/Standard) and adaptive meshing (Abaqus/Explicit),” Section 1.3.1
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
“Superplastic forming of a rectangular box,” Section 1.3.2
•
•
“Unstable static problem: thermal forming of a metal sheet,” Section 1.3.17
“Stretching of a thin sheet with a hemispherical punch,” Section 1.3.3
“Deep drawing of a cylindrical cup,” Section 1.3.4
“Extrusion of a cylindrical metal bar with frictional heat generation,” Section 1.3.5
“Rolling of thick plates,” Section 1.3.6
“Axisymmetric forming of a circular cup,” Section 1.3.7
“Cup/trough forming,” Section 1.3.8
“Forging with sinusoidal dies,” Section 1.3.9
“Forging with multiple complex dies,” Section 1.3.10
“Flat rolling: transient and steady-state,” Section 1.3.11
“Section rolling,” Section 1.3.12
“Ring rolling,” Section 1.3.13
“Axisymmetric extrusion: transient and steady-state,” Section 1.3.14
“Two-step forming simulation,” Section 1.3.15
“Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis,”
Section 1.3.16
“Inertia welding simulation using Abaqus/Standard and Abaqus/CAE,” Section 1.3.18
1.3–1
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
1.3.1
UPSETTING OF A CYLINDRICAL BILLET: QUASI-STATIC ANALYSIS WITH
MESH-TO-MESH SOLUTION MAPPING (Abaqus/Standard) AND ADAPTIVE
MESHING (Abaqus/Explicit)
Products: Abaqus/Standard
Abaqus/Explicit
This example illustrates the use of the solution mapping capabilities of Abaqus/Standard and the adaptive
meshing capabilities of Abaqus/Explicit in a metal forming application; the analysis results are compared with
the results of Taylor (1981). The same problem is also analyzed using the coupled temperature-displacement
elements in “Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis,”
Section 1.3.16. Coupled temperature-displacement elements are included in this example only for solution
mapping verification purposes; no heat generation occurs in these elements for this example.
When the strains become large in a geometrically nonlinear analysis, the elements often become so
severely distorted that they no longer provide a good discretization of the problem. When this occurs,
it is necessary to map the solution onto a new mesh that is better designed to continue the analysis. In
Abaqus/Standard the procedure is to monitor the distortion of the mesh—for example, by observing
deformed configuration plots—and decide when the mesh needs to be mapped. When mesh distortion is so
severe that a new mesh must be created, the new mesh can be generated using the mesh generation options
in Abaqus/CAE. The output database is useful in this context since the current geometry of the model can
be extracted from the data in the output database. Once a new mesh is defined, the analysis is continued by
beginning a new problem using the solution from the old mesh at the point of mapping as initial conditions
by specifying the step number and increment number at which the solution should be read from the previous
analysis. Abaqus/Standard interpolates the solution from the old mesh onto the new mesh to begin the new
problem. This technique provides considerable generality. For example, the new mesh might be more dense
in regions of high-strain gradients and have fewer elements in regions that are moving rigidly—there is no
restriction that the number of elements be the same or that element types agree between the old and new
meshes. In a typical practical analysis of a manufacturing process, mesh-to-mesh solution mapping may
have to be done several times because of the large shape changes associated with such a process.
Abaqus/Explicit has capabilities that allow automatic solution mapping using adaptive meshing.
Therefore, the mapping process is easier since it is contained within the analysis and the user only has to
decide how frequently remeshing should be done and what method to use to map the solution from the
old mesh to the new mesh as the solution progresses. Abaqus/Explicit offers default choices for adaptive
meshing that have been shown to work for a wide variety of problems. Finally, solution-dependent meshing
is used to concentrate mesh refinement areas of evolving boundary curvature. This counteracts the tendency
of the basic smoothing methods to reduce the mesh refinement near concave boundaries where solution
accuracy is important.
Geometry and model
The geometry is the standard test case of Lippmann (1979) and is defined in “Upsetting of a cylindrical
billet: coupled temperature-displacement and adiabatic analysis,” Section 1.3.16. It is a circular billet,
1.3.1–1
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
30 mm long, with a radius of 10 mm, compressed between two flat, rigid dies that are defined to be
perfectly rough.
The mesh used to begin the analysis is shown in Figure 1.3.1–1. The finite element model is
axisymmetric and includes the top half of the billet only since the middle surface of the billet is a plane of
symmetry. In both the Abaqus/Standard and Abaqus/Explicit simulations, element type CAX4R is used:
this is a 4-node quadrilateral with a single integration point and “hourglass control” to control spurious
mechanisms caused by the fully reduced integration. The element is chosen here because it is relatively
inexpensive for problems involving nonlinear constitutive behavior since the material calculations are
only done at one point in each element. In addition, in the Abaqus/Standard simulations element types
CGAX4R, CGAX4T, CAX4P, and CAX4I are also used to model the billet; in the Abaqus/Explicit
simulations element type CAX6M is also used to model the billet.
The contact between the top and lateral exterior surfaces of the billet and the rigid die is modeled
with a contact pair. The billet surface is specified as a surface definition in the model. The rigid die is
modeled in a variety of different ways as described in Table 1.3.1–1. The mechanical interaction between
the contact surfaces is assumed to be nonintermittent, rough frictional contact. Therefore, the contact
property includes two additional specifications: rough friction to enforce a no-slip constraint between
the two surfaces, and a no-separation contact pressure-overclosure relationship to ensure that separation
does not occur once contact has been established. All the contact simulations in Abaqus/Standard use
the node-to-surface formulation except one case where the surface-to-surface formulation is introduced.
Table 1.3.1–1 summarizes the different analysis cases that are studied. The column headings
indicate whether the problem was analyzed using Abaqus/Standard and/or Abaqus/Explicit.
For Case 1 several different analyses are performed to compare the different section control options
available in Abaqus/Explicit and to evaluate the effects of mesh refinement for the billet modeled with
CAX4R elements. A coarse mesh (analysis COARSE_SS) and a fine mesh (analysis FINE_SS) are
analyzed with the pure stiffness form of hourglass control. A coarse mesh (analysis COARSE_CS)
is analyzed with the combined hourglass control. A coarse mesh (analysis COARSE_ENHS) and a
fine mesh (analysis FINE_ENHS) are analyzed with the hourglass control based on the enhanced strain
method. The default section controls, using the integral viscoelastic form of hourglass control, are
tested on a coarse mesh (analysis COARSE) and a fine mesh (analysis FINE). Since this is a quasi-static
analysis, the viscous hourglass control option should not be used. All other cases use the default section
controls.
The Abaqus/Standard analyses for Case 1 compare the two hourglass control options and evaluate
the effect of mesh refinement for the billet modeled with CAX4R elements. A coarse mesh (analysis
COARSE_S) and a fine mesh (analysis FINE_S) are analyzed with the pure stiffness form of hourglass
control. A coarse mesh (analysis COARSE_EH) and a fine mesh (analysis FINE_EH) are analyzed with
hourglass control based on the enhanced strain method. A coarse mesh (analysis COARSE_EHG) with
CGAX4R elements is also analyzed with hourglass control based on the enhanced strain method for
comparison purposes.
No mesh convergence studies have been done, but the agreement with the results given in
Lippmann (1979) suggests that the meshes used here are good enough to provide reasonable predictions
of the overall force on the dies.
1.3.1–2
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
Material
The material model assumed for the billet is that given in Lippmann (1979). Young’s modulus is 200 GPa,
Poisson’s ratio is 0.3, and the density is 7833 kg/m3 . A rate-independent von Mises elastic-plastic
material model is used, with a yield stress of 700 MPa and a hardening slope of 0.3 GPa.
Boundary conditions and loading
The kinematic boundary conditions are symmetry on the axis (nodes at
0, in node set AXIS, have
0 prescribed) and symmetry about
0 (all nodes at
0, in node set MIDDLE, have
0
prescribed). The node on the top surface of the billet that lies on the symmetry axis is not part of the
node set AXIS to avoid overconstraint: the radial motion of this node is already constrained by a no slip
frictional constraint (see “Common difficulties associated with contact modeling in Abaqus/Standard,”
Section 38.1.2 of the Abaqus Analysis User’s Manual, and “Common difficulties associated with contact
modeling using contact pairs in Abaqus/Explicit,” Section 38.2.2 of the Abaqus Analysis User’s Manual).
In Abaqus/Standard the rigid die is displaced by −9 mm in the axial direction using a displacement
boundary condition. In Abaqus/Explicit the -displacement of the rigid die is prescribed using a
velocity boundary condition whose value is ramped up to a velocity of 20 m/s and then held constant
until the die has moved a total of 9 mm. The total simulation time of the Abaqus/Explicit analysis is
0.55 millisec, and the loading rate is slow enough to be considered quasi-static. In both Abaqus/Standard
and Abaqus/Explicit the radial and rotational degrees of freedom of the rigid die are constrained.
For all cases the analyses are done in two steps so that the first step can be stopped at a die
displacement corresponding to 44% upsetting; the second step carries the analysis to 60% upsetting. In
the Abaqus/Standard simulations the solution mapping analysis restarts from the end of the first step
with a new mesh and proceeds until 60% upsetting is achieved.
Mesh-to-mesh solution mapping in Abaqus/Standard
The interpolation technique used in solution mapping is a two-step process. First, values of all solution
variables are obtained at the nodes of the old mesh by extrapolating the values from the integration points
to the nodes of each element and averaging those values over all elements abutting each node. The second
step is to locate each integration point in the new mesh with respect to the old mesh (this assumes all
integration points in the new mesh lie within the bounds of the old mesh: warning messages are issued
if this is not so, and new model solution variables at the integration point are set to zero). The variables
are then interpolated from the nodes of the element in the old mesh to the location in the new mesh.
All solution variables are interpolated automatically in this way so that the solution can proceed on the
new mesh. Whenever a model is mapped, it can be expected that there will be some discontinuity in the
solution because of the change in the mesh. If the discontinuity is significant, it is an indication that the
meshes are too coarse or that the mapping should have been done at an earlier stage before too much
distortion occurred.
1.3.1–3
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
Extracting two-dimensional profiles and remeshing using Abaqus/CAE
The model is built and meshed using Abaqus/CAE. The solution mapping for the Abaqus/Standard
analysis is done by extracting the two-dimensional profile of the deformed billet from the output; the user
must enter commands into the command line interface at the bottom of the Abaqus/CAE main window.
To extract the deformed geometry from the output database as an orphan mesh part, use the command
PartFromOdb, which takes the following arguments:
name
odb
instance
shape
The name of the orphan mesh part to be created.
The output database object returned from the command openOdb.
The name of the part instance in the initial model in capital letters.
Determines whether to import the part in its UNDEFORMED or DEFORMED
shape.
The command PartFromOdb returns a Part object that is passed to the command
Part2DGeomFrom2DMesh. This command creates a geometric Part object from the orphan
mesh imported earlier. It takes the following arguments:
name
part
featureAngle
The name of the part to be created.
The part object returned from the command PartFromOdb.
A float specifying the angle (in degrees) between line segments that triggers a break
in the geometry.
Once the profile of the deformed part has been created, the user can switch to the Mesh module,
remesh the part, and write out the new node and element definitions to be used in the mapping analysis.
The Python script file billet_rezone.py is included to demonstrate the process described above.
Adaptive meshing in Abaqus/Explicit
Adaptive meshing consists of two fundamental tasks: creating a new mesh, and remapping the solution
variables from the old mesh to the new mesh with a process called advection. A new mesh is created at a
specified frequency for each adaptive mesh domain. The mesh is found by sweeping iteratively over the
adaptive mesh domain and moving nodes to smooth the mesh. The process of mapping solution variables
from an old mesh to a new mesh is referred to as an advection sweep. At least one advection sweep is
performed in every adaptive mesh increment. The methods used for advecting solution variables to
the new mesh are consistent; monotonic; (by default) accurate to the second order; and conserve mass,
momentum, and energy. This example problem uses the default settings for adaptive mesh domains.
Results and discussion
The following discussion focuses primarily on the results for Case 1, where the billet is modeled with
CAX4R elements, the rigid die is modeled using an analytical rigid surface, and the pure stiffness
hourglass control is used in Abaqus/Explicit. The deformed meshes at 44% billet upsetting (73.3%
of the total die displacement) are shown in Figure 1.3.1–2, Figure 1.3.1–3, and Figure 1.3.1–4. The
folding of the top outside surface of the billet onto the die is clearly visible. In Abaqus/Standard
1.3.1–4
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
(Figure 1.3.1–2) severe straining and element distortion can be seen through the center of the specimen.
At this point the Abaqus/Standard mesh is mapped. The new mesh for the mapped model is shown in
Figure 1.3.1–3. Figure 1.3.1–4 clearly indicates the benefits of adaptive meshing as the mesh used in
Abaqus/Explicit has very little distortion.
The final configurations at 60% billet upsetting are shown in Figure 1.3.1–5 and Figure 1.3.1–6.
Both the Abaqus/Standard and Abaqus/Explicit results compare well, and the meshes appear only
slightly distorted. Similarily, the equivalent plastic strain magnitudes compare well (Figure 1.3.1–7 and
Figure 1.3.1–8).
Figure 1.3.1–9 is a plot of upsetting force versus vertical displacement at the rigid surface reference
node. The results of both the Abaqus/Standard and the Abaqus/Explicit analyses show excellent
agreement with the rate-independent results obtained by Taylor (1981). Also worth noting is that the
mapping in Abaqus/Standard does not appear to have a significant effect on the total upsetting force.
Figure 1.3.1–10 is a plot of upsetting force versus vertical displacement at the rigid surface
reference node with the section control options identified in Table 1.3.1–2. The curves obtained using
CAX4R and CAX6M elements are very close and agree well with the rate-independent results obtained
by Taylor (1981). The results from the COARSE_SS analysis are virtually the same as the results from
the FINE analysis but at a much reduced cost; therefore, such analysis options are recommended for
this problem. The results for all the other cases (which use the default section controls but different
rigid surface models) are the same as the results for Case 1 using the default section controls.
Input files
Abaqus/Standard input files
billet_case1_std_coarse.inp
billet_coarse_nodes.inp
billet_coarse_elem.inp
billet_case1_std_coarse_rez.inp
billet_coarse_nodes_rez.inp
billet_coarse_elem_rez.inp
billet_case1_std_coarse_eh.inp
billet_case1_std_fine.inp
billet_case1_std_fine_rez.inp
billet_case1_std_fine_eh.inp
billet_case1_std_coarse_cax4i.inp
billet_case1_std_coarse_cax4i_surf.inp
billet_case1_std_coarse_cax4i_rez.inp
billet_case1_std_coarse_cgax4r.inp
Original COARSE CAX4R mesh using STIFFNESS
hourglass control.
Node definitions for original COARSE mesh.
Element definitions for original COARSE mesh.
Mapped COARSE CAX4R mesh.
Node definitions for mapped COARSE mesh.
Element definitions for mapped COARSE mesh.
Original COARSE CAX4R mesh using ENHANCED
hourglass control.
Original FINE CAX4R mesh using STIFFNESS
hourglass control.
Mapped FINE CAX4R mesh.
Original FINE CAX4R mesh using ENHANCED
hourglass control.
Original COARSE CAX4I mesh.
Original COARSE CAX4I mesh using surface-to-surface
contact formulation.
Mapped COARSE CAX4I mesh.
Original COARSE CGAX4R mesh.
1.3.1–5
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
billet_case1_std_coarse_cgax_eh.inp
billet_case1_std_coarse_cgax4r_rez.inp
billet_case1_std_coarse_cgax4t.inp
billet_case1_std_coarse_cgax4t_rez.inp
billet_case1_std_coarse_cax4p.inp
billet_case1_std_coarse_cax4p_rez.inp
billet_rezone.py
billet_case2_std.inp
billet_case2_std_rez.inp
billet_case3_std.inp
billet_case3_std_rez.inp
billet_case6_std.inp
billet_case6_std_rez.inp
Original COARSE CGAX4R mesh using ENHANCED
hourglass control.
Mapped COARSE CGAX4R mesh.
Original COARSE CGAX4T mesh.
Mapped COARSE CGAX4T mesh.
Original COARSE CAX4P mesh.
Mapped COARSE CAX4P mesh.
Python script showing an example of the command usage
to extract the geometric profile of the deformed mesh
from an output database.
Original COARSE CAX4R mesh.
Mapped COARSE CAX4R mesh.
Original COARSE CAX4R mesh.
Mapped COARSE CAX4R mesh.
Original COARSE CAX4R mesh.
Mapped COARSE CAX4R mesh.
Abaqus/Explicit input files
billet_case1_xpl_coarse.inp
billet_case1_xpl_coarse_ss.inp
billet_case1_xpl_coarse_cs.inp
billet_case1_xpl_coarse_enhs.inp
billet_case1_xpl_fine.inp
billet_case1_xpl_fine_ss.inp
billet_case1_xpl_fine_cs.inp
billet_case1_xpl_fine_enhs.inp
billet_case1_xpl_coarse_cax6m.inp
billet_case1_xpl_fine_cax6m.inp
billet_case2_xpl.inp
billet_case3_xpl.inp
COARSE CAX4R mesh using RELAX STIFFNESS
hourglass control.
COARSE CAX4R mesh using STIFFNESS hourglass
control.
COARSE CAX4R mesh using COMBINED hourglass
control.
COARSE CAX4R mesh using ENHANCED hourglass
control.
FINE CAX4R mesh using RELAX STIFFNESS
hourglass control.
FINE CAX4R mesh using STIFFNESS hourglass control.
FINE CAX4R mesh using COMBINED hourglass
control.
FINE CAX4R mesh using ENHANCED hourglass
control.
COARSE CAX6M mesh using RELAX STIFFNESS
hourglass control.
FINE CAX6M mesh using RELAX STIFFNESS
hourglass control.
COARSE CAX4R mesh using RELAX STIFFNESS
hourglass control.
COARSE CAX4R mesh using RELAX STIFFNESS
hourglass control.
1.3.1–6
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
billet_case4_xpl.inp
billet_case5_xpl.inp
billet_case6_xpl.inp
billet_case7_xpl.inp
COARSE CAX4R
hourglass control.
COARSE CAX4R
hourglass control.
COARSE CAX4R
hourglass control.
COARSE CAX4R
hourglass control.
mesh using RELAX STIFFNESS
mesh using RELAX STIFFNESS
mesh using RELAX STIFFNESS
mesh using RELAX STIFFNESS
References
•
•
Lippmann, H., Metal Forming Plasticity, Springer-Verlag, Berlin, 1979.
Taylor, L. M., “A Finite Element Analysis for Large Deformation Metal Forming Problems
Involving Contact and Friction,” Ph.D. Thesis, U. of Texas at Austin, 1981.
1.3.1–7
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
Table 1.3.1–1
Case
Cases describing the modeling of the rigid die.
Description
STD
XPL
1
The die is modeled as an analytical rigid surface using a planar analytical
surface and a rigid body constraint. The rigid surface is associated with a rigid
body by its specified reference node.
Yes
Yes
2
Axisymmetric rigid elements of type RAX2 are used to model the rigid die.
Yes
Yes
3
The die is modeled with RAX2 elements, as in Case 2. However, the die is
assigned a mass by specifying point masses at the nodes of the RAX2 elements.
Yes
Yes
4
The rigid die is modeled with RAX2 elements, as in Case 2. The rigid elements
are assigned a thickness and density values such that the mass of the die is
the same as in Case 3.
No
Yes
5
The die is modeled with RAX2 elements, as in Case 2. In this case the
thickness of the rigid elements is interpolated from the thickness specified at
the nodes. The same thickness value is prescribed as in Case 4.
No
Yes
6
Axisymmetric shell elements of type SAX1 are used to model the die, and they
are included in the rigid body definition.
Yes
Yes
7
The die is modeled with axisymmetric shell elements of type SAX1 and with
axisymmetric rigid elements of type RAX2. The deformable elements are
included in the rigid body definition. Both element types have the same
thickness and density as in Case 4.
No
Yes
1.3.1–8
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
Table 1.3.1–2
Analysis options for Case 1 using CAX4R elements.
Analysis Label
Mesh
Type
Hourglass
Control
Analysis Type
COARSE_SS
FINE_SS
COARSE_CS
COARSE
FINE
COARSE_ENHS
FINE_ENHS
COARSE_S
FINE_S
COARSE_EH
FINE_EH
COARSE_EHG
coarse
fine
coarse
coarse
fine
coarse
fine
coarse
fine
coarse
fine
coarse
stiffness
stiffness
combined
relax stiffness
relax stiffness
enhanced
enhanced
stiffness
stiffness
enhanced
enhanced
enhanced
XPL
XPL
XPL
XPL
XPL
XPL
XPL
STD
STD
STD
STD
STD
1.3.1–9
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
Figure 1.3.1–1
Figure 1.3.1–2
Axisymmetric upsetting example: initial mesh.
Abaqus/Standard: Deformed configuration at 44% upset (original mesh).
1.3.1–10
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
Figure 1.3.1–3
Figure 1.3.1–4
Abaqus/Standard: New mesh at 44% upset.
Abaqus/Explicit: Deformed configuration at 44% upset (CAX4R elements).
1.3.1–11
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
Figure 1.3.1–5
Figure 1.3.1–6
Abaqus/Standard: New mesh at 60% upset.
Abaqus/Explicit: Deformed mesh at 60% upset (CAX4R elements).
1.3.1–12
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
PEEQ
(Ave. Crit.: 75%)
+1.862e+00
+1.707e+00
+1.552e+00
+1.397e+00
+1.243e+00
+1.088e+00
+9.333e-01
+7.785e-01
+6.238e-01
+4.691e-01
+3.144e-01
+1.597e-01
+4.958e-03
Figure 1.3.1–7
Abaqus/Standard: Plastic strain of new mesh at 60% upset.
PEEQ
(Ave. Crit.: 75%)
+1.862e+00
+1.693e+00
+1.524e+00
+1.355e+00
+1.186e+00
+1.018e+00
+8.489e-01
+6.801e-01
+5.113e-01
+3.425e-01
+1.737e-01
+4.958e-03
+4.958e-03
Figure 1.3.1–8
Abaqus/Explicit: Plastic strain at 60% upset (CAX4R elements).
1.3.1–13
Abaqus Version 6.12 ID:
Printed on:
UPSETTING OF CYLINDRICAL BILLET
Explicit
Standard Original
Standard Rezoned
Taylor
ABAQUS/Standard rezoning
starts here.
Figure 1.3.1–9
Force-deflection response for cylinder upsetting.
COARSE
COARSE_CAX6M
COARSE_CS
COARSE_ENHS
COARSE_SS
Taylor
Figure 1.3.1–10 Force-deflection response for cylinder upsetting.
Comparison of Abaqus/Explicit hourglass controls.
1.3.1–14
Abaqus Version 6.12 ID:
Printed on:
SUPERPLASTIC BOX
1.3.2
SUPERPLASTIC FORMING OF A RECTANGULAR BOX
Product: Abaqus/Standard
In this example we consider the superplastic forming of a rectangular box. The example illustrates the use of
rigid elements to create a smooth three-dimensional rigid surface.
Superplastic metals exhibit high ductility and very low resistance to deformation and are, thus, suitable
for forming processes that require very large deformations. Superplastic forming has a number of advantages
over conventional forming methods. Forming is usually accomplished in one step rather than several, and
intermediate annealing steps are usually unnecessary. This process allows the production of relatively
complex, deep-shaped parts with quite uniform thickness. Moreover, tooling costs are lower since only a
single die is usually required. Drawbacks associated with this method include the need for tight control of
temperature and deformation rate. Very long forming times make this method impractical for high volume
production of parts.
A superplastic forming process usually consists of clamping a sheet against a die whose surface forms
a cavity of the shape required. Gas pressure is then applied to the opposite surface of the sheet, forcing it to
acquire the die shape.
Rigid surface
A rigid faceted surface can be created from an arbitrary mesh of three-dimensional rigid elements
(either triangular R3D3 or quadrilateral R3D4 elements). See “Analytical rigid surface definition,”
Section 2.3.4 of the Abaqus Analysis User’s Manual, for a discussion of smoothing of master surfaces.
Abaqus automatically smoothes any discontinuous surface normal transitions between the surface
facets.
Solution-dependent amplitude
One of the main difficulties in superplastically forming a part is the control of the processing parameters.
The temperature and the strain rates that the material experiences must remain within a certain range for
superplasticity to be maintained. The former is relatively easy to achieve. The latter is more difficult
because of the unknown distribution of strain rates in the part. The manufacturing process must be
designed to be as rapid as possible without exceeding a maximum allowable strain rate at any material
point. For this purpose Abaqus has a feature that allows the loading (usually the gas pressure) to be
controlled by means of a solution-dependent amplitude and a target maximum creep strain rate. In
the loading options the user specifies a reference value. The amplitude definition requires an initial,
a minimum, and a maximum load multiplier. During a quasi-static procedure Abaqus will then monitor
the maximum creep strain rate and compare it with the target value. The load amplitude is adjusted
based on this comparison. This controlling algorithm is simple and relatively crude. The purpose is not
to follow the target values exactly but to obtain a practical loading schedule.
1.3.2–1
Abaqus Version 6.12 ID:
Printed on:
SUPERPLASTIC BOX
Geometry and model
The example treated here corresponds to superplastic forming of a rectangular box whose final
dimensions are 1524 mm (60 in) long by 1016 mm (40 in) wide by 508 mm (20 in) deep with a 50.8 mm
(2 in) flange around it. All fillet radii are 101.6 mm (4 in). The box is formed by means of a uniform
fluid pressure.
A quarter of the blank is modeled using 704 membrane elements of type M3D4. These are fully
integrated bilinear membrane elements. The initial dimensions of the blank are 1625.6 mm (64 in) by
1117.6 mm (44 in), and the thickness is 3.175 mm (0.125 in). The blank is clamped at all its edges.
The flat initial configuration of the membrane model is entirely singular in the normal direction unless
it is stressed in biaxial tension. This difficulty is prevented by applying a small biaxial initial stress of
6.89 kPa (1 lb/in2 ) by means of the initial stress conditions.
The female die is modeled as a rigid body and is meshed with rigid R3D3 elements. The rigid
surface can be defined by grouping together those faces of the 231 R3D3 elements used to model the die
that face the contact direction. See Figure 1.3.2–1 for an illustration of the rigid element mesh.
To avoid having points “fall off” the rigid surface during the course of the analysis, more than a
quarter of the die has been modeled, as shown in Figure 1.3.2–2. It is always a good idea to extend the
rigid surface far enough so that contacting nodes will not slide off the master surface.
By default, Abaqus generates a unique normal to the rigid surface at each node point, based on
the average of the normals to the elements sharing each node. There are times, however, when the
normal to the surface should be specified directly. This is discussed in “Node definition,” Section 2.1.1
of the Abaqus Analysis User’s Manual. In this example the flange around the box must be flat to ensure
compatibility between the originally flat blank and the die. Therefore, an outer normal (0, 1, 0) has been
specified at the 10 nodes that make up the inner edge of the flange. This is done by entering the direction
cosines after the node coordinates. The labels of these 10 vertices are 9043, 9046, 9049, 9052, 9089,
9090, 9091, 9121, 9124, and 9127; and their definitions can be found in superplasticbox_node.inp.
Material
The material in the blank is assumed to be elastic-viscoplastic, and the properties roughly represent
the 2004 (Al-6Cu-0.4Zr)-based commercial superplastic aluminum alloy Supral 100 at 470°C. It has a
Young’s modulus of 71 GPa (10.3 × 106 lb/in2 ) and a Poisson’s ratio of 0.34. The flow stress is assumed
to depend on the plastic strain rate according to
where A is 179.2 MPa (26. × 103 lb/in2 ) and the time is in seconds.
Loading and controls
We perform two analyses to compare constant pressure loading and a pressure schedule automatically
adjusted to achieve a maximum strain rate of 0.02/sec. In the constant load case the prestressed blank is
subjected to a rapidly applied external pressure of 68.8 kPa (10 lb/in2 ), which is then held constant for
1.3.2–2
Abaqus Version 6.12 ID:
Printed on:
SUPERPLASTIC BOX
3000 sec until the box has been formed. In the second case the prestressed blank is subjected to a rapidly
applied external pressure of 1.38 kPa (0.2 lb/in2 ). The pressure schedule is then chosen by Abaqus.
The initial application of the pressures is assumed to occur so quickly that it involves purely elastic
response. This is achieved by using the static procedure. The creep response is developed in a second
step using a quasi-static procedure.
During the quasi-static step an accuracy tolerance controls the time increment and, hence, the
accuracy of the transient creep solution. Abaqus compares the equivalent creep strain rate at the
beginning and the end of an increment. The difference should be less than this tolerance divided by
the time increment. Otherwise, the increment is reattempted with a smaller time increment. The usual
guideline for setting this accuracy tolerance is to decide on an acceptable error in stress and convert
it to an error in strain by dividing by the elastic modulus. For this problem we assume that moderate
accuracy is required and choose this tolerance as 0.5%. In general, larger tolerance values allow Abaqus
to use larger time increments, resulting in a less accurate and less expensive analysis.
In the automatic scheduling analysis the pressure refers to an amplitude that allows for a maximum
pressure of 1.38 MPa (200 lb/in2 ) and a minimum pressure of 0.138 kPa (0.02 lb/in2 ). The target creep
strain rate is a constant entered using creep strain rate control. The node-to-surface (default) and surfaceto-surface contact formulations are considered for this case where the creep strain rate is used to control
the pressure amplitude. In the node-to-surface contact formulation the thickness of the blank is ignored
and the blank is positioned such that its midsurface is used in the contact calculations as an approximation.
However, the surface-to-surface contact formulation explicitly accounts for the blank thickness, as in
reality.
Results and discussion
Figure 1.3.2–3 through Figure 1.3.2–5 show a sequence of deformed configurations during the
automatically controlled forming process. The stages of deformation are very similar in the constant
load process. However, the time necessary to obtain the deformation is much shorter with automatic
loading—the maximum allowable pressure is reached after 83.3 seconds. The initial stages of the
deformation correspond to inflation of the blank because there is no contact except at the edges of the
box. Contact then occurs at the box’s bottom, with the bottom corners finally filling. Although there is
some localized thinning at the bottom corners, with strains on the order of 100%, these strains are not
too much larger than the 80% strains seen on the midsides.
Figure 1.3.2–6 and Figure 1.3.2–7 show the equivalent plastic strain at the end of the process using
the surface-to-surface and the node-to-surface contact formulations, respectively. The differences in the
results are primarily due to differences in the way that the blank thickness is handled. Consequently,
results from the surface-to-surface contact formulation are more reliable since the blank thickness is
considered.
Figure 1.3.2–8 shows the evolution in time of the ratio between the maximum creep strain rate found
in the model and the target creep strain rate for the two contact formulations. The load applied initially
produces a low maximum creep strain rate at the beginning of the analysis. At the end the maximum creep
strain rate falls substantially as the die cavity fills up. Although the curve appears very jagged, it indicates
that the maximum peak strain rate is always relatively close to the target value. This is quite acceptable
in practice. Figure 1.3.2–9 shows the pressure schedule that Abaqus calculates for this problem. For
1.3.2–3
Abaqus Version 6.12 ID:
Printed on:
SUPERPLASTIC BOX
most of the time, while the sheet does not contact the bottom of the die, the pressure is low. Once the
die starts restraining the deformation, the pressure can be increased substantially without producing high
strain rates. Again, the differences in the pressure schedule toward the end of the simulation are due
primarily to the differences in the handling of the blank thickness.
Input files
superplasticbox_constpress.inp
superplasticbox_autopress.inp
superplasticbox_autopress_surf.inp
Constant pressure main analysis.
Automatic pressurization main analysis.
Automatic pressurization main analysis using the surfaceto-surface contact formulation.
Node definitions for the rigid elements.
Element definitions for the rigid R3D3 elements.
superplasticbox_node.inp
superplasticbox_element.inp
2
1
3
Figure 1.3.2–1
Rigid surface for die.
2
1
3
Figure 1.3.2–2
Initial position of blank with respect to die.
1.3.2–4
Abaqus Version 6.12 ID:
Printed on:
SUPERPLASTIC BOX
2
1
3
Figure 1.3.2–3 Automatic loading: deformed configuration after
34 sec in Step 2 using the node-to-surface contact formulation.
2
1
3
Figure 1.3.2–4 Automatic loading: deformed configuration after
63 sec in Step 2 using the node-to-surface contact formulation.
1.3.2–5
Abaqus Version 6.12 ID:
Printed on:
SUPERPLASTIC BOX
2
1
3
Figure 1.3.2–5 Automatic loading: deformed configuration after
83 sec in Step 2 using the node-to-surface contact formulation.
CEEQ
(Avg: 75%)
+1.375e+00
+1.266e+00
+1.158e+00
+1.049e+00
+9.407e-01
+8.321e-01
+7.235e-01
+6.149e-01
+5.063e-01
+3.977e-01
+2.892e-01
+1.806e-01
+7.200e-02
2
1
3
Figure 1.3.2–6
Automatic loading: inelastic strain in the formed box using the
surface-to-surface contact formulation.
1.3.2–6
Abaqus Version 6.12 ID:
Printed on:
SUPERPLASTIC BOX
CEEQ
(Avg: 75%)
+1.375e+00
+1.266e+00
+1.158e+00
+1.049e+00
+9.407e-01
+8.321e-01
+7.235e-01
+6.149e-01
+5.063e-01
+3.977e-01
+2.892e-01
+1.806e-01
+7.200e-02
2
1
3
Figure 1.3.2–7
Automatic loading: inelastic strain in the formed box using the
node-to-surface contact formulation.
Node to Surface
Surface to Surface
2.00
c.s.r ratio
1.50
1.00
0.50
0.00
0.00
20.00
40.00
60.00
80.00
100.00
Time
Figure 1.3.2–8
History of ratio between maximum creep strain rate and target creep strain rate.
1.3.2–7
Abaqus Version 6.12 ID:
Printed on:
SUPERPLASTIC BOX
Node to Surface
Surface to Surface
3
[x10 ]
1.00
Pressure amplitude
0.80
0.60
0.40
0.20
0.00
0.00
20.00
40.00
60.00
80.00
100.00
Time
Figure 1.3.2–9
History of pressure amplitude.
1.3.2–8
Abaqus Version 6.12 ID:
Printed on:
HEMISPHERICAL PUNCH STRETCHING
1.3.3
STRETCHING OF A THIN SHEET WITH A HEMISPHERICAL PUNCH
Products: Abaqus/Standard
Abaqus/Explicit
Stamping of sheet metals by means of rigid punches and dies is a standard manufacturing process. In most bulk
forming processes the loads required for the forming operation are often the primary concern. However, in
sheet forming the prediction of strain distributions and limit strains (which define the onset of local necking)
are most important. Such analysis is complicated in that it requires consideration of large plastic strains
during deformation, an accurate description of material response including strain hardening, the treatment of
a moving boundary that separates the region in contact with the punch head from the unsupported one, and
the inclusion of friction between the sheet and the punch head.
The stretching of a thin circular sheet with a hemispherical punch is considered in this example.
Geometry and model
The geometry of this problem is shown in Figure 1.3.3–1. The sheet being stretched has a clamping
radius, , of 59.18 mm. The radius of the punch, , is 50.8 mm; the die radius, , is 6.35 mm;
and the initial thickness of the sheet, , is 0.85 mm. Such a sheet has been tested experimentally by
Ghosh and Hecker (1975) and has been analyzed by Wang and Budiansky (1978) using an axisymmetric
membrane shell finite element formulation. The analysis is conducted statically in Abaqus/Standard and
dynamically in Abaqus/Explicit such that inertial forces are relatively small. The initial configuration
for the analysis is shown in Figure 1.3.3–2.
The sheet, the punch, and the die are modeled as separate parts, each instanced once. As an
axisymmetric problem in Abaqus/Standard the sheet is modeled using 50 elements of type SAX1 (or
MAX1) or 25 elements of type SAX2 (or MAX2). The Abaqus/Explicit model uses 50 elements of
type SAX1. Mesh convergence studies (not reported here) have been done and indicate that these
meshes give acceptably accurate results for most of the values of interest. To test the three-dimensional
membrane and shell elements in Abaqus/Standard, a 10° sector is modeled using 100 elements of
type S4R, S4, SC8R, or M3D4R or 25 elements of type M3D9R. All these meshes are reasonably
fine; they are used to obtain good resolution of the moving contact between the sheet and the dies. In
the Abaqus/Standard shell models nine integration points are used through the thickness of the sheet
to ensure the development of yielding and elastic-plastic bending response; in Abaqus/Explicit five
integration points are used through the thickness of the sheet.
The rigid punch and die are modeled in Abaqus/Standard as analytical rigid surfaces with a surface
in conjunction with a rigid body constraint. The top and bottom surfaces of the sheet are defined with
surface definitions. In Abaqus/Explicit the punch and die are modeled as rigid bodies; the surface of the
punch and die are modeled either by analytical rigid surfaces or RAX2 elements. In the Abaqus/Explicit
analyses the rigid surfaces are offset from the blank by half the thickness of the blank because the contact
algorithm in Abaqus/Explicit takes the shell thickness into account. Similarly, when the surface-tosurface contact formulation in Abaqus/Standard is used, the blank thickness is considered by default and
the rigid surfaces are offset from the blank by half the blank thickness, consistent with the physical reality.
However, most of the input files presented in this section use the node-to-surface contact formulation in
1.3.3–1
Abaqus Version 6.12 ID:
Printed on:
HEMISPHERICAL PUNCH STRETCHING
Abaqus/Standard. In these cases the shell thickness is ignored, and the mid-surface of the shell is used
in the contact calculations as an approximation.
Material properties
The material (aluminum-killed steel) is assumed to satisfy the Ramberg-Osgood relation between true
stress and logarithmic strain,
where Young’s modulus, E, is 206.8 GPa; the reference stress value, K, is 0.510 GPa; and the
work-hardening exponent, n, is 4.76. In the present Abaqus analyses the Ramberg-Osgood relation is
approximated using an elastic-plastic material. The material is assumed to be linear elastic up to a yield
stress of 170.0 MPa, and the stress-strain curve beyond the yield stress is defined in piecewise linear
segments. Poisson’s ratio is 0.3.
The membrane element models in Abaqus/Standard are inherently unstable in a static analysis unless
some prestress is present in the elements prior to the application of external loading. Therefore, an
equibiaxial initial stress condition equal to 5% of the initial yield stress is prescribed for the membrane
elements in Abaqus/Standard.
Contact interactions
The contact between the sheet and the rigid punch and the rigid die is modeled with a contact pair. The
mechanical interaction between the contact surfaces is assumed to be frictional contact, with a coefficient
of friction of 0.275.
Loading
The Abaqus/Standard analysis is carried out in five steps; the Abaqus/Explicit analysis is carried out in
four steps. In Abaqus/Explicit the velocity of the punch head is prescribed using a velocity boundary
condition whose amplitude is ramped up to 30 m/s at 1.24 milliseconds during the first step and then kept
constant until time reaches 1.57 milliseconds at the end of the second step. It is then ramped down to zero
at a time of 1.97 milliseconds at the end of the third step. In the first three steps of the Abaqus/Standard
and Abaqus/Explicit analyses, the punch head is moved toward the sheet through total distances of
18.6 mm, 28.5 mm, and 34.5 mm, respectively. The purpose of these three steps is to compare the
results with those provided experimentally by Ghosh and Hecker for these punch displacements. More
typically the punch would be moved through its entire travel in one step.
Two final steps are included in the Abaqus/Standard analysis. In the first step the metal sheet is
held in place and the contact pairs are removed from the model. In the second step the original boundary
conditions for the metal sheet are reintroduced for springback analysis. However, this springback step is
not included for the analyses using membrane elements, since these elements do not have any bending
stiffness and residual bending stress is often a key determinant of springback.
In the final step of the Abaqus/Explicit analysis the punch head is moved away from the sheet for
springback analysis. A viscous pressure load is applied to the surface of the shell during this step to damp
1.3.3–2
Abaqus Version 6.12 ID:
Printed on:
HEMISPHERICAL PUNCH STRETCHING
out transient wave effects so that quasi-static equilibrium can be reached quickly. This effect happens
within approximately 2 milliseconds from the start of unloading. The coefficient of viscous pressure is
chosen to be 0.35 MPa sec/m, approximately 1% of the value of
, where is the material density
of the sheet and is the dilatational wave speed. A value of viscous pressure of
would absorb all
the energy in a pressure wave. For typical structural problems choosing a small percentage of this value
provides an effective way of minimizing ongoing dynamic effects. Static equilibrium is reached when
residual stresses in the sheet are reasonably constant over time.
Results and discussion
Figure 1.3.3–2 shows the initial, undeformed profile of the blank, the die, and the punch. Figure 1.3.3–3
illustrates the deformed sheet and the punch and the die. Figure 1.3.3–4 shows a plot of the same system
after the punch is lifted back, showing the springback of the sheet.
Figure 1.3.3–5 shows the distribution of nominal values of radial and circumferential membrane
strain in the sheet for an 18.6 mm punch head displacement. Figure 1.3.3–6 shows the strain distributions
at a punch head displacement of 28.5 mm, and Figure 1.3.3–7 shows the strain distributions at a punch
head displacement of 34.5 mm. The strain distributions for the SAX1 models compare well with those
obtained experimentally by Ghosh and Hecker (1975) and those obtained numerically by Wang and
Budiansky (1978), who used a membrane shell finite element formulation. The important phenomenon
of necking during stretching is reproduced at nearly the same location, although slightly different strain
values are obtained. Draw beads are used to hold the edge of the sheet in the experiment, but in this
analysis the sheet is simply clamped at its edge. Incorporation of the draw bead boundary conditions
may further improve the correlation with the experimental data.
A spike can be observed in the radial strain distribution toward the edge of the sheet in some of the
Abaqus/Standard shell models. This strain spike is the result of the sheet bending around the die. The
spike is not present in the membrane element models since they possess no bending stiffness. All of
the Abaqus/Standard results presented in Figure 1.3.3–5 through Figure 1.3.3–9 use the node-to-surface
contact formulation. Similar results are obtained when using the surface-to-surface contact formulation.
The results obtained with the axisymmetric membrane models are compared with those obtained
from the axisymmetric shell models and are found to be in good agreement.
These analyses assume a value of 0.275 for the coefficient of friction. Ghosh and Hecker do not
give a value for their experiments, but Wang and Budiansky assume a value of 0.17. The coefficient of
friction has a marked effect on the peak strain during necking and may be a factor contributing to the
discrepancy of peak strain results during necking. The values used in these analyses have been chosen
to provide good correlation with the experimental data.
The distributions of the residual stresses on springback of the sheet are shown in Figure 1.3.3–8 and
Figure 1.3.3–9.
Input files
Abaqus/Standard input files
thinsheetstretching_m3d4r.inp
Element type M3D4R.
1.3.3–3
Abaqus Version 6.12 ID:
Printed on:
HEMISPHERICAL PUNCH STRETCHING
thinsheetstretching_m3d4r_surf.inp
Element type M3D4R using surface-to-surface contact
while accounting for shell thickness.
Element type M3D9R.
Element type MAX1.
Element type MAX2.
Element type S4.
Element type S4R.
*POST OUTPUT analysis.
Element type SC8R.
Element type SAX1.
Element type SAX2.
Restart of thinsheetstretching_sax2.inp.
thinsheetstretching_m3d9r.inp
thinsheetstretching_max1.inp
thinsheetstretching_max2.inp
thinsheetstretching_s4.inp
thinsheetstretching_s4r.inp
thinsheetstretching_s4r_po.inp
thinsheetstretching_sc8r.inp
thinsheetstretching_sax1.inp
thinsheetstretching_sax2.inp
thinsheetstretching_restart.inp
Abaqus/Explicit input files
hemipunch_anl.inp
Model using analytical rigid surfaces to describe the rigid
surface.
Model using rigid elements to describe the rigid surface.
hemipunch.inp
References
•
Ghosh, A. K., and S. S. Hecker, “Failure in Thin Sheets Stretched Over Rigid Punches,”
Metallurgical Transactions, vol. 6A, pp. 1065–1074, 1975.
•
Wang, N. M., and B. Budiansky, “Analysis of Sheet Metal Stamping by a Finite Element Method,”
Journal of Applied Mechanics, vol. 45, pp. 73–82, 1978.
Punch
rp
Die
ro
rd
ro = 59.18 mm
rp = 50.8 mm
rd = 6.35 mm
Figure 1.3.3–1
Configuration and dimensions for hemispherical punch stretching.
1.3.3–4
Abaqus Version 6.12 ID:
Printed on:
HEMISPHERICAL PUNCH STRETCHING
Punch
Sheet
Die
2
3
1
Figure 1.3.3–2
Initial configuration.
2
3
Figure 1.3.3–3
1
Configuration for punch head displacement of 34.5 mm, Abaqus/Explicit.
1.3.3–5
Abaqus Version 6.12 ID:
Printed on:
HEMISPHERICAL PUNCH STRETCHING
2
3
1
Figure 1.3.3–4
Final configuration after springback, Abaqus/Explicit.
ABAQUS/Explicit
ABAQUS/Explicit
Ghosh et al.(1975)
Ghosh et al.(1975)
ABAQUS/Standard
ABAQUS/Standard
Wang et al.(1978)
Wang et al.(1978)
Radial
Circumferential
Figure 1.3.3–5
Strain distribution for punch head displacement of 18.6 mm.
1.3.3–6
Abaqus Version 6.12 ID:
Printed on:
HEMISPHERICAL PUNCH STRETCHING
ABAQUS/Explicit
ABAQUS/Explicit
Ghosh et al.(1975)
Ghosh et al.(1975)
ABAQUS/Standard
ABAQUS/Standard
Wang et al.(1978)
Wang et al.(1978)
Radial
Circumferential
Figure 1.3.3–6
Strain distribution for punch head displacement of 28.5 mm.
ABAQUS/Explicit
ABAQUS/Explicit
Ghosh et al.(1975)
Ghosh et al.(1975)
ABAQUS/Standard
ABAQUS/Standard
Wang et al.(1978)
Wang et al.(1978)
Radial
Circumferential
Figure 1.3.3–7
Strain distribution for punch head displacement of 34.5 mm.
1.3.3–7
Abaqus Version 6.12 ID:
Printed on:
HEMISPHERICAL PUNCH STRETCHING
ABAQUS/Explicit
ABAQUS/Explicit
ABAQUS/Standard
ABAQUS/Standard
Figure 1.3.3–8
Residual stress on top surface after springback.
ABAQUS/Explicit
ABAQUS/Explicit
ABAQUS/Standard
ABAQUS/Standard
Figure 1.3.3–9
Circumferential
Radial
Circumferential
Radial
Residual stress on bottom surface after springback.
1.3.3–8
Abaqus Version 6.12 ID:
Printed on:
Circumferential
Radial
Circumferential
Radial
CYLINDRICAL CUP DEEP DRAWING
1.3.4
DEEP DRAWING OF A CYLINDRICAL CUP
Product: Abaqus/Standard
Deep drawing of sheet metal is an important manufacturing technique. In the deep drawing process a “blank”
of sheet metal is clamped by a blank holder against a die. A punch is then moved against the blank, which is
drawn into the die. Unlike the operation described in the hemispherical punch stretching example (“Stretching
of a thin sheet with a hemispherical punch,” Section 1.3.3), the blank is not assumed to be fixed between the
die and the blank holder; rather, the blank is drawn from between these two tools. The ratio of drawing versus
stretching is controlled by the force on the blank holder and the friction conditions at the interface between the
blank and the blank holder and the die. Higher force or friction at the blank/die/blank holder interface limits
the slip at the interface and increases the radial stretching of the blank. In certain cases drawbeads, shown in
Figure 1.3.4–1, are used to restrain the slip at this interface even further.
To obtain a successful deep drawing process, it is essential to control the slip between the blank and its
holder and die. If the slip is restrained too much, the material will undergo severe stretching, thus potentially
causing necking and rupture. If the blank can slide too easily, the material will be drawn in completely and
high compressive circumferential stresses will develop, causing wrinkling in the product. For simple shapes
like the cylindrical cup here, a wide range of interface conditions will give satisfactory results. But for more
complex, three-dimensional shapes, the interface conditions need to be controlled within a narrow range to
obtain a good product.
During the drawing process the response is determined primarily by the membrane behavior of the sheet.
For axisymmetric problems in particular, the bending stiffness of the metal yields only a small correction to
the pure membrane solution, as discussed by Wang and Tang (1988). In contrast, the interaction between
the die, the blank, and the blank holder is critical. Thus, thickness changes in the sheet material must be
modeled accurately in a finite element simulation, since they will have a significant influence on the contact
and friction stresses at the interface. In these circumstances the most suitable elements in Abaqus are the
4-node reduced-integration axisymmetric quadrilateral, CAX4R; the first-order axisymmetric shell element,
SAX1; the first-order axisymmetric membrane element, MAX1; the first-order finite-strain quadrilateral shell
element, S4R; the fully integrated general-purpose finite-membrane-strain shell element, S4; and the 8-node
continuum shell element, SC8R.
Membrane effects and thickness changes are modeled properly with CAX4R. However, the bending
stiffness of the element is low. The element does not exhibit “locking” due to incompressibility or parasitic
shear. It is also very cost-effective. For shells and membranes the thickness change is calculated from the
assumption of incompressible deformation of the material.
Geometry and model
The geometry of the problem is shown in Figure 1.3.4–2. The circular blank being drawn has an initial
radius of 100 mm and an initial thickness of 0.82 mm. The punch has a radius of 50 mm and is rounded
off at the corner with a radius of 13 mm. The die has an internal radius of 51.25 mm and is rounded off
at the corner with a radius of 5 mm. The blank holder has an internal radius of 56.25 mm.
1.3.4–1
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
The blank is modeled using 40 elements of type CAX4R or 31 elements of type SAX1, MAX1,
S4R, S4, or SC8R. An 11.25° wedge of the circular blank is used in the three-dimensional S4R and S4
models. These meshes are rather coarse for this analysis. However, since the primary interest in this
problem is to study the membrane effects, the analysis will still give a fair indication of the stresses and
strains occurring in the process.
The contact between the blank and the rigid punch, the rigid die, and the rigid blank holder is
modeled with a contact pair. The top and bottom surfaces of the blank are defined as surfaces in the model.
The rigid punch, the die, and the blank holder are modeled as analytical rigid surfaces. The mechanical
interaction between the contact surfaces is assumed to be frictional contact. Therefore, friction is used
in conjunction with the various contact property definitions to specify coefficients of friction.
At the start of the analysis for the CAX4R model, the blank is positioned precisely on top of the
die and the blank holder is precisely in touch with the top surface of the blank. The punch is positioned
0.18 mm above the top surface of the blank.
In the case of shells and membranes, the positioning of the blank depends on the contact formulation
used. Node-to-surface and surface-to-surface contact formulations are available in Abaqus/Standard.
For the node-to-surface formulation, the shell/membrane thickness is modeled using an exponential
pressure-overclosure relationship (“Contact pressure-overclosure relationships,” Section 36.1.2 of the
Abaqus Analysis User’s Manual). The blank holder is positioned a fixed distance above the blank.
This fixed distance is the distance at which the contact pressure is set to zero using an exponential
pressure-overclosure relationship. However, the surface-to-surface contact formulation automatically
takes thickness into account, and the need for specifying pressure overclosure relations is eliminated.
Examples of the surface-to-surface contact formulation with S4 and S4R elements are provided in this
problem.
Material properties
The material (aluminum-killed steel) is assumed to satisfy the Ramberg-Osgood relation between true
stress and logarithmic strain:
The reference stress value, K, is 513 MPa; and the work-hardening exponent, n, is 0.223. The Young’s
modulus is 211 GPa, and the Poisson’s ratio is 0.3. An initial yield stress of 91.3 MPa is obtained
with these data. The stress-strain curve is defined in piecewise linear segments in the metal plasticity
specification, up to a total (logarithmic) strain level of 107%.
The coefficient of friction between the interface and the punch is taken to be 0.25; and that between
the die and the blank holder is taken as 0.1, the latter value simulating a certain degree of lubrication
between the surfaces. The stiffness method of sticking friction is used in these analyses. The numerics
of this method make it necessary to choose an acceptable measure of relative elastic slip between mating
surfaces when sticking should actually be occurring. The basis for the choice is as follows. Small
values of elastic slip best simulate the actual behavior but also result in a slower convergence of the
solution. Permission of large relative elastic displacements between the contacting surfaces can cause
higher strains at the center of the blank. In these runs we let Abaqus choose the allowable elastic
1.3.4–2
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
slip, which is done by determining a characteristic interface element length over the entire mesh and
multiplying by a small fraction to get an allowable elastic slip measure. This method typically gives a
fairly small amount of elastic slip.
Although the material in this process is fully isotropic, the local coordinate system is used with the
CAX4R elements to define a local orientation that is coincident initially with the global directions. The
reason for using this option is to obtain the stress and strain output in more natural coordinates: if the local
coordinate system is used in a geometrically nonlinear analysis, stress and strain components are given
in a corotational framework. Hence, in our case throughout the motion, S11 will be the stress in the r–z
plane in the direction of the middle surface of the cup. S22 will be the stress in the thickness direction,
S33 will be the hoop stress, and S12 will be the transverse shear stress, which makes interpreting the
results considerably easier. This orientation definition is not necessary with the SAX1 or MAX1 elements
since the output for shell and membrane elements is already given in the local shell system. For the
SAX1 and MAX1 model, S11 is the stress in the meridional direction and S22 is the circumferential
(hoop) stress. An orientation definition would normally be needed for the S4R and S4 models but can
be avoided by defining the wedge in such a manner that the single integration point of each element lies
along the global x-axis. Such a model definition, along with appropriate kinematic boundary conditions,
keeps the local stress output definitions for the shells as S11 being the stress in the meridional plane and
S22 the hoop stress. There should be no in-plane shear, S12, in this problem. A transformation is used
in the S4R and S4 models to impose boundary constraints in a cylindrical system.
Loading
The entire analysis is carried out in five steps. In the first step the blank holder is pushed onto the
blank with a prescribed displacement to establish contact. In the shell models this displacement roughly
corresponds to zero clearance across the interface.
In the second step the boundary condition is removed and replaced by the applied force of 100 kN
on the blank holder. This force is kept constant during Steps 2 and 3. This technique of simulating the
clamping process is used to avoid potential problems with rigid body modes of the blank holder, since
there is no firm contact between the blank holder, the blank, and the die at the start of the process. The
two-step procedure creates contact before the blank holder is allowed to move freely.
In the third step the punch is moved toward the blank through a total distance of 60 mm. This
step models the actual drawing process. During this step the time incrementation parameters are set to
improve efficiency for severely discontinuous behavior associated with frictional contact.
The last two steps are used to simulate springback. In the fourth step all the nodes in the model
are fixed in their current positions and the contact pairs are removed from the model. This is the most
reliable method for releasing contact conditions. In the fifth, and final, step the regular set of boundary
conditions is reinstated and the springback is allowed to take place. This part of the analysis with the
CAX4R elements is included to demonstrate the feasibility of the unloading procedure only and is not
expected to produce realistic results, since the reduced-integration elements have a purely elastic bending
behavior. The springback is modeled with more accuracy in the shell element models.
1.3.4–3
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
Results and discussion
Figure 1.3.4–3 shows deformed shapes that are predicted at various stages of the drawing process for the
CAX4R model. The profiles show that the metal initially bends and stretches and is then drawn in over the
surface of the die. The distributions of radial and circumferential strain for all three models and thickness
strain for the CAX4R model are shown in Figure 1.3.4–4. The thickness for the shell or membrane models
can be monitored with output variable STH (current shell or membrane thickness). The thickness does not
change very much: the change ranges from approximately −12% in the cylindrical part to approximately
+16% at the edge of the formed cup. Relatively small thickness changes are usually desired in deep
drawing processes and are achieved because the radial tensile strain and the circumferential compressive
strain balance each other.
The drawing force as a function of punch displacement for various element types is shown in
Figure 1.3.4–5, where the curves are seen to match closely. Similarly, the drawing force as a function
of punch displacement with S4R elements using the node-to-surface and surface-to-surface contact
formulations is shown in Figure 1.3.4–6. The differences in the reaction force history are due to
consideration of the blank thickness explicitly in the surface-to-surface contact formulation as compared
to the node-to-surface contact formulation where a pressure-overclosure relationship is specified. In all
of the cases, oscillations in the force history are seen. These oscillations are a result of the rather coarse
mesh—each oscillation represents an element being drawn over the corner of the die. Compared to
the shell models, the membrane model predicts a smaller punch force for a given punch displacement.
Thus, toward the end of the analysis the results for punch force versus displacement for the MAX1
model are closer to those for the CAX4R model.
The deformed shape after complete unloading is shown in Figure 1.3.4–7, superimposed on the
deformed shape under complete loading. The analysis shows the lip of the cup springing back strongly
after the blank holder is removed for the CAX4R model. No springback is evident in the shell models.
As was noted before, this springback in the CAX4R model is not physically realistic: in the first-order
reduced-integration elements an elastic “hourglass control” stiffness is associated with the “bending”
mode, since this mode is identical to the “hourglass” mode exhibited by this element in continuum
situations. In reality the bending of the element is an elastic-plastic process, so that the springback
is likely to be much less. A better simulation of this aspect would be achieved by using several elements
through the thickness of the blank, which would also increase the cost of the analysis. The springback
results for the shell models do not exhibit this problem and are clearly more representative of the actual
elastic-plastic process.
1.3.4–4
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
Input files
deepdrawcup_cax4r.inp
deepdrawcup_cax4r_surf.inp
deepdrawcup_cax4i.inp
deepdrawcup_s4.inp
deepdrawcup_s4_surf.inp
deepdrawcup_s4r.inp
deepdrawcup_s4r_surf.inp
deepdrawcup_sc8r.inp
deepdrawcup_sax1.inp
deepdrawcup_postoutput.inp
deepdrawcup_max1.inp
deepdrawcup_mgax1.inp
CAX4R model.
CAX4R model using surface-to-surface contact.
Model using the incompatible mode element, CAX4I,
as an alternative to the CAX4R element. In contrast to
the reduced-integration, linear isoparametric elements
such as the CAX4R element, the incompatible mode
elements have excellent bending properties even
with one layer of elements through the thickness (see
“Geometrically nonlinear analysis of a cantilever beam,”
Section 2.1.2 of the Abaqus Benchmarks Manual) and
have no hourglassing problems. However, they are
computationally more expensive.
S4 model.
S4 model using surface-to-surface contact.
S4R model.
S4R model using surface-to-surface contact.
SC8R model.
SAX1 model.
*POST OUTPUT analysis of deepdrawcup_sax1.inp.
MAX1 model.
MGAX1 model.
Reference
•
Wang, N. M., and S. C. Tang, “Analysis of Bending Effects in Sheet Forming Operations,”
International Journal for Numerical Methods in Engineering, vol. 25, pp. 253–267, January 1988.
1.3.4–5
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
Figure 1.3.4–1
A typical drawbead used to limit slip between the blank and die.
Rp = 50 mm
RH = 56.25 mm
R = 13 mm
t = 0.82 mm
r
R = 5 mm
RB = 100 mm
RD = 51.25 mm
Figure 1.3.4–2
Geometry and mesh for the deep drawing problem.
1.3.4–6
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
Figure 1.3.4–3
Deformed shapes at various stages of the analysis.
1.3.4–7
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
1.0
RADIAL STRAIN
HOOP STRAIN
THICK STRAIN
CAX4R MODEL
STRAIN
0.5
0.0
-0.5
-1.0
0.00
0.02
0.04
0.06
RADIAL POSITION (m)
0.08
0.10
0.08
0.10
0.08
0.10
1.0
RADIAL STRAIN
HOOP STRAIN
SAX1 MODEL
STRAIN
0.5
0.0
-0.5
-1.0
0.00
0.02
0.04
0.06
RADIAL POSITION (m)
1.0
RADIAL STRAIN
HOOP STRAIN
S4R MODEL
STRAIN
0.5
0.0
-0.5
-1.0
0.00
Figure 1.3.4–4
0.02
0.04
0.06
RADIAL POSITION (m)
Strain distribution at the end of the deep drawing step.
1.3.4–8
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
100.
scale
1.0
1.0
32.
1.0
80.
Punch Force (Pa)
CAX4R
SAX1
S4R
MAX1
[ x10 3 ]
60.
40.
20.
0.
0.00
0.01
0.02
0.03
0.04
0.05
0.06
Punch Displacement (m)
Figure 1.3.4–5
Punch force versus punch displacement using the node-to-surface contact formulation.
Node-to-surface
Surface-to-surface
3
[x10 ]
3.00
2.50
Punch Force (Pa)
2.00
1.50
1.00
0.50
0.00
0.00
0.01
0.02
0.03
0.04
0.05
0.06
Punch Displacement (m)
Figure 1.3.4–6
Comparison of punch force versus punch displacement with S4R
elements for different contact formulations.
1.3.4–9
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL CUP DEEP DRAWING
CAX4R MODEL
SAX1 MODEL
S4R MODEL
Figure 1.3.4–7
Deformed shape after unloading.
1.3.4–10
Abaqus Version 6.12 ID:
Printed on:
EXTRUSION OF A METAL BAR
1.3.5
EXTRUSION OF A CYLINDRICAL METAL BAR WITH FRICTIONAL HEAT
GENERATION
Products: Abaqus/Standard
Abaqus/Explicit
This analysis illustrates how extrusion problems can be simulated with Abaqus. In this particular problem
the radius of an aluminum cylindrical bar is reduced 33% by an extrusion process. The generation of heat
due to plastic dissipation inside the bar and the frictional heat generation at the workpiece/die interface are
considered.
Geometry and model
The bar has an initial radius of 100 mm and is 300 mm long. Figure 1.3.5–1 shows half of the crosssection of the bar, modeled with first-order axisymmetric elements (CAX4T and CAX4RT elements in
Abaqus/Standard and CAX4RT elements in Abaqus/Explicit).
In the primary analysis in both Abaqus/Standard and Abaqus/Explicit, heat transfer between the
deformable bar and the rigid die is not considered, although frictional heating is included. A fully
coupled temperature-displacement analysis is performed with the die kept at a constant temperature.
In addition, an adiabatic analysis is presented using Abaqus/Standard without accounting for frictional
heat generation. Both the node-to-surface (default) and the surface-to-surface contact formulations
in Abaqus/Standard are presented. In the case of Abaqus/Explicit, penalty and kinematic contact
formulations are used in the definition of contact interactions.
Various techniques are used to model the rigid die. In Abaqus/Standard the die is modeled with
CAX4T elements made into an isothermal rigid body using an isothermal rigid body and with an
analytical rigid surface. In Abaqus/Explicit the die is modeled with an analytical rigid surface and
discrete rigid elements (RAX2). The fillet radius is set to 0.075 for models using an analytical rigid
surface to smoothen the die surface.
The Abaqus/Explicit simulations are also performed with Arbitrary Lagrangian-Eulerian (ALE)
adaptive meshing and enhanced hourglass control.
Material model and interface behavior
The material model is chosen to reflect the response of a typical commercial purity aluminum alloy. The
material is assumed to harden isotropically. The dependence of the flow stress on the temperature is
included, but strain rate dependence is ignored. Instead, representative material data at a strain rate of
0.1 sec−1 are selected to characterize the flow strength.
The interface is assumed to have no conductive properties. Coulomb friction is assumed for the
mechanical behavior, with a friction coefficient of 0.1. Gap heat generation is used to specify the fraction,
, of total heat generated by frictional dissipation that is transferred to the two bodies in contact. Half
of this heat is conducted into the workpiece, and the other half is conducted into the die. Furthermore,
90% of the nonrecoverable work due to plasticity is assumed to heat the work material.
1.3.5–1
Abaqus Version 6.12 ID:
Printed on:
EXTRUSION OF A METAL BAR
Boundary conditions, loading, and solution control
In the first step the bar is moved to a position where contact is established and slipping of the workpiece
against the die begins. In the second step the bar is extruded through the die to realize the extrusion
process. This is accomplished by prescribing displacements to the nodes at the top of the bar. In the third
step the contact elements are removed in preparation for the cool down portion of the simulation. In
Abaqus/Standard this is performed in a single step: the bar is allowed to cool down using film conditions,
and deformation is driven by thermal contraction during the fourth step.
Volume proportional damping is applied to two of the analyses that are considered. In one case
the automatic stabilization scheme with a constant damping factor is used. A nondefault damping
density is chosen so that a converged and accurate solution is obtained. In another case the adaptive
automatic stabilization scheme with a default damping density is used. In this case the damping factor
is automatically adjusted based on the convergence history.
In Abaqus/Explicit the cool down simulation is broken into two steps: the first introduces viscous
pressure to damp out dynamic effects and, thus, allow the bar to reach static equilibrium quickly; the
balance of the cool down simulation is performed in a fifth step. The relief of residual stresses through
creep is not analyzed in this example.
In Abaqus/Explicit mass scaling is used to reduce the computational cost of the analysis; nondefault
hourglass control is used to control the hourglassing in the model. The default integral viscoelastic
approach to hourglass control generally works best for problems where sudden dynamic loading occurs;
a stiffness-based hourglass control is recommended for problems where the response is quasi-static. A
combination of stiffness and viscous hourglass control is used in this problem.
For purposes of comparison a second problem is also analyzed, in which the first two steps of the
previous analysis are repeated in a static analysis with the adiabatic heat generation capability. The
adiabatic analysis neglects heat conduction in the bar. Frictional heat generation must also be ignored in
this case. This problem is analyzed only in Abaqus/Standard.
Results and discussion
The following discussion centers around the results obtained with Abaqus/Standard. The results of the
Abaqus/Explicit simulation are in close agreement with those obtained with Abaqus/Standard for both
the node-to-surface and surface-to-surface contact formulations.
Figure 1.3.5–2 shows the deformed configuration after Step 2 of the analysis. Figure 1.3.5–3
and Figure 1.3.5–4 show contour plots of plastic strain and the Mises stress at the end of Step 2 for
the fully coupled analysis using CAX4RT elements. These plots show good agreement between the
results using the two contact formulations in Abaqus/Standard. The plastic deformation is most severe
near the surface of the workpiece, where plastic strains exceed 100%. The peak stresses occur in the
region where the diameter of the workpiece narrows down due to deformation and also along the
contact surface. Figure 1.3.5–5 compares nodal temperatures obtained at the end of Step 2 using the
surface-to-surface contact formulation in Abaqus/Standard with those obtained using kinematic contact
in Abaqus/Explicit. In both cases CAX4RT elements are used. The results from both of the analyses
match very well even though mass scaling is used in Abaqus/Explicit for computational savings. The
1.3.5–2
Abaqus Version 6.12 ID:
Printed on:
EXTRUSION OF A METAL BAR
peak temperature occurs at the surface of the workpiece because of plastic deformation and frictional
heating. The peak temperature occurs immediately after the radial reduction zone of the die. This is
expected for two reasons. First, the material that is heated by dissipative processes in the reduction zone
will cool by conduction as the material progresses through the postreduction zone. Second, frictional
heating is largest in the reduction zone because of the larger values of shear stress in that zone.
Similar results were obtained with the two types of stabilization considered. Adaptive automatic
stabilization is generally preferred because it is easier to use. It is often necessary to specify a nondefault
damping factor for the stabilization approach with a constant damping factor; whereas, with an adaptive
damping factor, the default settings are typically appropriate.
Figure 1.3.5–6 compares results of a thermally coupled analysis with an adiabatic analysis using the
surface-to-surface contact formulation in Abaqus/Standard. If we ignore the zone of extreme distortion at
the end of the bar, the temperature increase on the surface is not as large for the adiabatic analysis because
of the absence of frictional heating. As expected, the temperature field contours for the adiabatic heating
analysis, shown in Figure 1.3.5–6, are very similar to the contours for plastic strain from the thermally
coupled analysis, shown in Figure 1.3.5–3.
As noted earlier, excellent agreement is observed for the results obtained with Abaqus/Explicit
(using both the default and enhanced hourglass control) and Abaqus/Standard. Figure 1.3.5–7 compares
the effects of ALE adaptive meshing on the element quality. The results obtained with ALE adaptive
meshing show significantly reduced mesh distortion. The material point in the bar that experiences the
largest temperature rise during the course of the simulation is indicated (node 2029 in the model without
adaptivity). Figure 1.3.5–8 compares the results obtained for the temperature history of this material point
using Abaqus/Explicit with the results obtained using the two contact formulations in Abaqus/Standard.
Again, a very good match between the results is obtained.
Input files
Abaqus/Standard input files
metalbarextrusion_coupled_fric.inp
Thermally coupled extrusion using CAX4T elements
with frictional heat generation.
metalbarextrusion_stabil.inp
Thermally coupled extrusion using CAX4T elements
with frictional heat generation and automatic
stabilization, user-defined damping.
metalbarextrusion_stabil_adap.inp
Thermally coupled extrusion using CAX4T elements
with frictional heat generation and adaptive automatic
stabilization, default damping.
metalbarextrusion_coupled_fric_surf.inp
Thermally coupled extrusion using CAX4T elements
with frictional heat generation and the surface-to-surface
contact formulation.
metalbarextrusion_s_coupled_fric_cax4rt.inp Thermally coupled extrusion using CAX4RT elements
with frictional heat generation.
1.3.5–3
Abaqus Version 6.12 ID:
Printed on:
EXTRUSION OF A METAL BAR
metalbarextrusion_s_coupled_fric_cax4rt_surf.inp
Thermally coupled extrusion using CAX4RT elements
with frictional heat generation and the surface-to-surface
contact formulation.
metalbarextrusion_adiab.inp
Extrusion with adiabatic heat generation and without
frictional heat generation.
metalbarextrusion_adiab_surf.inp
Extrusion with adiabatic heat generation and without
frictional heat generation using the surface-to-surface
contact formulation.
Abaqus/Explicit input files
metalbarextrusion_x_cax4rt.inp
metalbarextrusion_x_cax4rt_enh.inp
metalbarextrusion_xad_cax4rt.inp
metalbarextrusion_xad_cax4rt_enh.inp
metalbarextrusion_xd_cax4rt.inp
metalbarextrusion_xd_cax4rt_enh.inp
metalbarextrusion_xp_cax4rt.inp
metalbarextrusion_xp_cax4rt_enh.inp
Thermally coupled extrusion with frictional heat
generation and without ALE adaptive meshing; die
modeled with an analytical rigid surface; kinematic
mechanical contact.
Thermally coupled extrusion with frictional heat
generation and without ALE adaptive meshing; die
modeled with an analytical rigid surface; kinematic
mechanical contact; enhanced hourglass control.
Thermally coupled extrusion with frictional heat
generation and ALE adaptive meshing; die modeled
with an analytical rigid surface; kinematic mechanical
contact.
Thermally coupled extrusion with frictional heat
generation and ALE adaptive meshing; die modeled
with an analytical rigid surface; kinematic mechanical
contact; enhanced hourglass control.
Thermally coupled extrusion with frictional heat
generation and without ALE adaptive meshing; die
modeled with RAX2 elements; kinematic mechanical
contact.
Thermally coupled extrusion with frictional heat
generation and without ALE adaptive meshing; die
modeled with RAX2 elements; kinematic mechanical
contact; enhanced hourglass control.
Thermally coupled extrusion with frictional heat
generation and without ALE adaptive meshing; die
modeled with an analytical rigid surface; penalty
mechanical contact.
Thermally coupled extrusion with frictional heat
generation and without ALE adaptive meshing; die
modeled with an analytical rigid surface; penalty
mechanical contact; enhanced hourglass control.
1.3.5–4
Abaqus Version 6.12 ID:
Printed on:
EXTRUSION OF A METAL BAR
2
3
1
Figure 1.3.5–1 Mesh and geometry: axisymmetric extrusion
with meshed rigid die, Abaqus/Standard.
2
3
Figure 1.3.5–2
1
Deformed configuration: Step 2, Abaqus/Standard.
1.3.5–5
Abaqus Version 6.12 ID:
Printed on:
EXTRUSION OF A METAL BAR
PEEQ
(Avg: 75%)
+1.107e+00
+1.015e+00
+9.227e-01
+8.305e-01
+7.383e-01
+6.462e-01
+5.540e-01
+4.618e-01
+3.696e-01
+2.775e-01
+1.853e-01
+9.313e-02
+9.640e-04
PEEQ
(Avg: 75%)
+1.107e+00
+1.015e+00
+9.226e-01
+8.304e-01
+7.383e-01
+6.461e-01
+5.539e-01
+4.618e-01
+3.696e-01
+2.774e-01
+1.853e-01
+9.313e-02
+9.650e-04
2
2
3
1
3
1
Figure 1.3.5–3 Plastic strain contours: Step 2, thermally coupled analysis (frictional heat generation),
Abaqus/Standard (surface-to-surface contact formulation, left; node-to-surface contact formulation, right).
S, Mises
(Avg: 75%)
+1.424e+08
+1.309e+08
+1.194e+08
+1.078e+08
+9.631e+07
+8.479e+07
+7.327e+07
+6.175e+07
+5.023e+07
+3.871e+07
+2.719e+07
+1.567e+07
+4.144e+06
2
2
3
S, Mises
(Avg: 75%)
+1.424e+08
+1.309e+08
+1.193e+08
+1.078e+08
+9.630e+07
+8.478e+07
+7.326e+07
+6.174e+07
+5.022e+07
+3.870e+07
+2.718e+07
+1.566e+07
+4.144e+06
1
3
1
Figure 1.3.5–4 Mises stress contours: Step 2, thermally coupled analysis (frictional heat generation),
Abaqus/Standard (surface-to-surface contact formulation, left; node-to-surface contact formulation, right).
1.3.5–6
Abaqus Version 6.12 ID:
Printed on:
EXTRUSION OF A METAL BAR
NT11
+1.125e+02
+1.048e+02
+9.708e+01
+8.938e+01
+8.167e+01
+7.396e+01
+6.625e+01
+5.854e+01
+5.083e+01
+4.313e+01
+3.542e+01
+2.771e+01
+2.000e+01
NT11
+1.125e+02
+1.048e+02
+9.708e+01
+8.937e+01
+8.166e+01
+7.396e+01
+6.625e+01
+5.854e+01
+5.083e+01
+4.312e+01
+3.542e+01
+2.771e+01
+2.000e+01
2
3
2
1
3
1
Figure 1.3.5–5 Temperature contours: Step 2, thermally coupled analysis (frictional heat generation);
surface-to-surface contact formulation in Abaqus/Standard, left; Abaqus/Explicit, right.
NT11
+1.125e+02
+1.048e+02
+9.708e+01
+8.938e+01
+8.167e+01
+7.396e+01
+6.625e+01
+5.854e+01
+5.083e+01
+4.313e+01
+3.542e+01
+2.771e+01
+2.000e+01
TEMP
(Avg: 75%)
+1.111e+02
+1.035e+02
+9.595e+01
+8.835e+01
+8.075e+01
+7.315e+01
+6.555e+01
+5.796e+01
+5.036e+01
+4.276e+01
+3.516e+01
+2.756e+01
+1.996e+01
2
3
2
1
3
1
Figure 1.3.5–6 Temperature contours: Step 2, Abaqus/Standard using surface-to-surface
contact formulation; thermally coupled analysis, left; adiabatic heat generation (without
heat generation due to friction), right.
1.3.5–7
Abaqus Version 6.12 ID:
Printed on:
EXTRUSION OF A METAL BAR
2029
Figure 1.3.5–7
Deformed shape of the workpiece: Abaqus/Explicit; without adaptive
remeshing, left; with ALE adaptive remeshing, right.
Explicit
Standard SurfacetoSurface
Standard NodetoSurface
NT at a Node on Contact Suface
100.00
80.00
60.00
40.00
20.00
0.00
2.00
4.00
6.00
8.00
3
10.00 [x10 ]
Time (Sec)
Figure 1.3.5–8 Temperature history of a node on the
contact surface (nonadaptive result).
1.3.5–8
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
1.3.6
ROLLING OF THICK PLATES
Product: Abaqus/Explicit
Hot rolling is a basic manufacturing technique used to transform preformed shapes into a form suitable for
further processing. Rolling processes can be divided into different categories, depending on the complexity
of metal flow and on the geometry of the rolled product. Finite element computations are used increasingly
to analyze the elongation and spread of the material during rolling (Kobayashi, 1989). Although the forming
process is often carried out at low roll speed, this example shows that a considerable amount of engineering
information can be obtained by using the explicit dynamics procedure in Abaqus/Explicit to model the process.
The rolling process is first investigated using plane strain computations. These results are used to choose
the modeling parameters associated with the more computationally expensive three-dimensional analysis.
Since rolling is normally performed at relatively low speeds, it is natural to assume that static analysis is
the proper modeling approach. Typical rolling speeds (surface speed of the roller) are on the order of 1 m/sec.
At these speeds inertia effects are not significant, so the response—except for rate effects in the material
behavior—is quasi-static. Representative rolling geometries generally require three-dimensional modeling,
resulting in very large models, and include nonlinear material behavior and discontinuous effects—contact
and friction. Because the problem size is large and the discontinuous effects dominate the solution, the explicit
dynamics approach is often less expensive computationally and more reliable than an implicit quasi-static
solution technique.
The computer time involved in running a simulation using explicit time integration with a given mesh is
directly proportional to the time period of the event. This is because numerical stability considerations restrict
the time increment to
where the minimum is taken over all elements in the mesh,
is a characteristic length associated with an
element, is the density of the material in the element, and and are the effective Lamé’s constants for
the material in the element. Since this condition effectively means that the time increment can be no larger
than the time required to propagate a stress wave across an element, the computer time involved in running
a quasi-static analysis can be very large. The cost of the simulation is directly proportional to the number of
time increments required,
if
remains constant, where T is the time period of the event being
simulated. (
will not remain constant in general, since element distortion will change
and nonlinear
material response will change the effective Lamé constants and density; but the assumption is acceptable for
the purposes of this discussion.) Thus,
To reduce n, we can speed up the simulation compared to the time of the actual process; that is, we can
artificially reduce the time period of the event, T. This will introduce two possible errors. If the simulation
1.3.6–1
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
speed is increased too much, the inertia forces will be larger and will change the predicted response (in an
extreme case the problem will exhibit wave propagation response). The only way to avoid this error is to
find a speedup that is not too large. The other error is that some aspects of the problem other than inertia
forces—for example, material behavior—may also be rate dependent. This implies that we cannot change the
actual time period of the event being modeled. But we can see a simple equivalent—artificially increasing the
material density, , by a factor
reduces n to
, just as decreasing T to
does. This concept, which is
called “mass scaling,” reduces the ratio of the event time to the time for wave propagation across an element
while leaving the event time fixed, thus allowing treatment of rate-dependent material and other behaviors
while having exactly the same effect on inertia forces as speeding up the time of simulation. Mass scaling is
attractive because it allows us to treat rate-dependent quasi-static problems efficiently. But we cannot take it
too far or we allow the inertia forces to dominate and, thus, change the solution. This example illustrates the
use of mass scaling and shows how far we can take it for a practical case.
The trial and error method works well for most generic quasi-static problems; however, for rolling
processes Abaqus/Explicit can set the mass scaling factor automatically based on the rolling geometry and
mesh properties. An acceptable value for the stable time increment is calculated, and the appropriate mass
scaling factor is applied on an element-by-element basis. The value of the stable time increment is based on
the average element length in the rolling direction, the average velocity of the product through the rollers, and
the number of nodes in the cross-section of the mesh.
Problem description
A steel plate of an original square cross-section of 40 mm by 40 mm and a length of 92 mm is reduced
to a 30 mm height by rolling through one roll stand. The radius of the rollers is 170 mm. The single
roller in the model (taking advantage of symmetry) is assumed to be rigid and is modeled as an analytical
rigid surface. The isotropic hardening yield curve of the steel is taken from Kopp and Dohmen (1990).
Isotropic elasticity is assumed, with Young’s modulus of 150 GPa and Poisson’s ratio of 0.3. The strain
hardening is described using 11 points on the yield stress versus plastic strain curve, with an initial yield
stress of 168.2 MPa and a maximum yield stress of 448.45 MPa. No rate dependence or temperature
dependence is taken into account.
Coulomb friction is assumed between the roller and the plate, with a friction coefficient of 0.3.
Friction plays an important role in this process, as it is the only mechanism by which the plate is pulled
through the roll stand. If the friction coefficient is too low, the plate cannot be drawn through the roll
stand. Initially, when a point on the surface of the plate has just made contact with the roller, the roller
surface is moving faster than the point on the surface of the plate and there is a relative slip between the
two surfaces. As the point on the plate is drawn into the process zone under the roller, it moves faster
and, after a certain distance, sticks to the roller. As the point on the surface of the plate is pushed out
of the process zone, it picks up speed and begins to move faster than the roller. This causes slip in the
opposite direction before the point on the surface of the sheet finally loses contact with the roller.
For plane strain computations a half-symmetry model with CPE4R elements is used. For the
three-dimensional computations a one-quarter symmetry model with C3D8R elements is used. The
roller is modeled with analytical rigid surfaces for both the two-dimensional and three-dimensional
cases. For quasi-static rolling problems perfectly round analytical surfaces can provide a more accurate
1.3.6–2
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
representation of the revolved roller geometry, improve computational efficiency, and reduce noise
when compared to element-based rigid surfaces.
The roller is rotated through 32° at a constant angular velocity of 1 revolution per second
(6.28 rad/sec), which corresponds to a roller surface speed of 1.07 m/sec. The plate is given an initial
velocity in the global x-direction. The initial velocity is chosen to match the x-component of velocity
of the roller at the point of first contact. This choice of initial velocity results in a net acceleration of
zero in the x-direction at the point of contact and minimizes the initial impact between the plate and the
roller. This minimizes the initial transient disturbance.
In all but one of the analyses performed in this example, the masses of all elements in the model
are scaled by factors of either 110, 2758, or 68962. These scaling factors translate into effective roller
surface speeds of 11.2 m/sec, 56.1 m/sec, and 280.5 m/sec. An alternative, but equivalent, means of mass
scaling could be achieved by scaling the material mass density by the aforementioned factors. In one
analysis, automatic mass scaling is used.
The element formulation for the two-dimensional (using CPE4R elements) and three-dimensional
(using C3D8R elements) analyses uses the pure stiffness form of hourglass control. The element
formulation is selected using section controls. In addition, the three-dimensional model (using C3D8R
elements) uses the centroidal kinematic formulation. These options are economical yet provide the
necessary level of accuracy for this class of problems. Two- and three-dimensional analyses using the
default hourglass control formulation, the combined hourglass control formulation, and the enhanced
hourglass control formulation are included for comparison. For the three-dimensional case, both the
orthogonal kinematic formulation and the centroidal kinematic formulation are considered.
For the sole purpose of testing the performances of the modified triangular and tetrahedral elements,
the problem is also analyzed in two dimensions using CPE6M elements and in three dimensions using
C3D10M elements.
Results and discussion
Table 1.3.6–1 shows the effective rolling speeds and the relative CPU cost of the cases using the element
formulations recommended for this problem. The relative costs are normalized with respect to the CPU
time for the two-dimensional model (using CPE4R elements) with the intermediate mass scaling value.
In addition, Table 1.3.6–2 compares the relative CPU cost and accuracy between the different element
formulations of the solid elements using the intermediate mass scaling value.
Plane strain rolling (CPE4R elements)
A plane strain calculation allows the user to resolve a number of modeling questions in two dimensions
before attempting a more expensive three-dimensional calculation. In particular, an acceptable effective
mass scaling factor for running the transient dynamics procedure can be determined.
Figure 1.3.6–1 through Figure 1.3.6–3 show contours of equivalent plastic strain for the three
mass scaling factors using the stiffness hourglass control. Figure 1.3.6–4 through Figure 1.3.6–6 show
contours of shear stress for the same cases. These results show that there is very little difference
between the lowest and the intermediate mass scaling cases. All the results are in good agreement
with the quasi-static analysis results obtained with Abaqus/Standard. The results of the largest mass
1.3.6–3
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
scaling case show pronounced dynamic effects. Table 1.3.6–1 shows the relative run time of the
quasi-static calculation, and Table 1.3.6–2 compares the different element formulations at the same
level of mass scaling. The intermediate mass scaling case gives essentially the same results as the
quasi-static calculation, using about one-thirteenth of the CPU time. In addition to the savings provided
by mass scaling, more computational savings are achieved using the stiffness hourglass control element
formulation; the results for this formulation compare well to the results for the computationally more
expensive element formulations.
Three-dimensional rolling (C3D8R elements)
We have ascertained with the two-dimensional calculations that mass scaling by a factor of 2758 gives
results that are essentially the same as a quasi-static solution. Figure 1.3.6–7 shows the distribution of
the equivalent plastic strain of the deformed sheet for the three-dimensional case using the centroidal
kinematic formulation and stiffness hourglass control. Figure 1.3.6–8 shows the distribution of the
equivalent plastic strain of the deformed sheet for the three-dimensional case using the default section
controls (average strain kinematic and relax stiffness hourglass). Table 1.3.6–1 compares this threedimensional case with the plane strain, quasi-static, and three-dimensional automatic mass scaling cases;
and Table 1.3.6–2 compares the five different three-dimensional element formulations included here
with the two-dimensional cases at the same level of mass scaling. The accuracy for all five element
formulations tested is very similar for this problem, but significant savings are realized in the threedimensional analyses when using more economical element formulations.
Analyses using CPE6M and C3D10M elements
The total number of nodes in the CPE6M model is identical to the number in the CPE4R model. The
number of nodes in the C3D10M model is 3440 (compared to 3808 in the C3D8R model). The analyses
using the CPE6M and C3D10M elements use a mass scaling factor of 2758. Figure 1.3.6–9 and
Figure 1.3.6–10 show the distribution of the equivalent plastic strain of the plate for the two-dimensional
and three-dimensional cases, respectively. The results are in reasonably good agreement with other
element formulations. However, the CPU costs are higher since the modified triangular and tetrahedral
elements use more than one integration point in each element and the stable time increment size is
somewhat smaller than in analyses that use reduced-integration elements with the same node count. For
the mesh refinements used in this problem, the CPE6M model takes about twice the CPU time as the
CPE4R model, while the C3D10M model takes about 5.75 times the CPU time as the C3D8R model.
Input files
roll2d330_anl_ss.inp
roll3d330_rev_anl_css.inp
Two-dimensional case (using CPE4R elements) with
a mass scaling factor of 2758 and the STIFFNESS
hourglass control.
Three-dimensional case (using C3D8R elements) with a
mass scaling factor of 2758, an analytical rigid surface of
TYPE=REVOLUTION, and the CENTROID kinematic
and STIFFNESS hourglass section control options.
1.3.6–4
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
roll2d66_anl_ss.inp
roll2d330_anl_cs.inp
roll2d330_anl_enhs.inp
roll2d330_cs.inp
roll3d330_css.inp
roll3d330_css_gcont.inp
roll3d330_ocs.inp
roll3d330_ocs_gcont.inp
roll2d1650_anl_ss.inp
roll3d330_rev_anl_ocs.inp
roll3d330_rev_anl_oenhs.inp
Two-dimensional case (using CPE4R elements) with
a mass scaling factor of 110 using the STIFFNESS
hourglass control.
Two-dimensional case (using CPE4R elements) with
a mass scaling factor of 2758 using the COMBINED
hourglass control.
Two-dimensional case (using CPE4R elements) with
a mass scaling factor of 2758 using the ENHANCED
hourglass control.
Two-dimensional case (using CPE4R elements) with
a mass scaling factor of 2758 using the COMBINED
hourglass control and rigid elements.
Three-dimensional case (using C3D8R elements) with
a mass scaling factor of 2758, rigid elements, and
the CENTROID kinematic and STIFFNESS hourglass
section control options.
Three-dimensional case (using C3D8R elements) with
a mass scaling factor of 2758, rigid elements, the
CENTROID kinematic and STIFFNESS hourglass
section control options, and the general contact capability.
Three-dimensional case (using C3D8R elements) with
a mass scaling factor of 2758, rigid elements, and the
ORTHOGONAL kinematic and COMBINED hourglass
section control options.
Three-dimensional case (using C3D8R elements) with
a mass scaling factor of 2758, rigid elements, the
ORTHOGONAL kinematic and COMBINED hourglass
section control options, and the general contact capability.
Two-dimensional case (using CPE4R elements) with a
mass scaling factor of 68962 using STIFFNESS hourglass
control.
Three-dimensional model (using C3D8R elements) with
a mass scaling factor of 2758, an analytical rigid surface
of TYPE=REVOLUTION, and the ORTHOGONAL
kinematic and COMBINED hourglass section control
options.
Three-dimensional model (using C3D8R elements) with
a mass scaling factor of 2758, an analytical rigid surface
of TYPE=REVOLUTION, and the ORTHOGONAL
kinematic and ENHANCED hourglass section control
options.
1.3.6–5
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
roll3d330_rev_anl_cenhs.inp
roll3d330_rev_anl.inp
roll3d_auto_rev_anl_css.inp
roll3d330_cyl_anl.inp
roll2d66.inp
roll2d330.inp
roll2d1650.inp
roll3d330.inp
roll3d330_gcont.inp
roll2d66_anl.inp
roll2d330_anl.inp
roll2d1650_anl.inp
roll2d_impl_qs.inp
roll2d330_anl_cpe6m.inp
Three-dimensional model (using C3D8R elements) with a
mass scaling factor of 2758, an analytical rigid surface of
TYPE=REVOLUTION, and the CENTROID kinematic
and ENHANCED hourglass section control options.
Three-dimensional model (using C3D8R elements) with
a mass scaling factor of 2758, an analytical rigid surface
of TYPE=REVOLUTION, and the default section control
options.
Three-dimensional case (using C3D8R elements) with
automatic mass scaling, an analytical rigid surface of
TYPE=REVOLUTION, and the CENTROID kinematic
and STIFFNESS hourglass section control options.
Three-dimensional model (using C3D8R elements) with
a mass scaling factor of 2758, an analytical rigid surface
of TYPE=CYLINDER, and the default section control
options.
Two-dimensional model (using CPE4R elements) with a
mass scaling factor of 110 and the default section controls.
Two-dimensional model (using CPE4R elements) with
a mass scaling factor of 2758 and the default section
controls.
Two-dimensional model (using CPE4R elements) with
a mass scaling factor of 68962 and the default section
controls.
Three-dimensional model using rigid elements and the
default section controls.
Three-dimensional model using rigid elements, the
default section controls, and the general contact
capability.
Two-dimensional model (using CPE4R elements) with a
mass scaling factor of 110, analytical rigid surfaces, and
the default section controls.
Two-dimensional model (using CPE4R elements) with a
mass scaling factor of 2758, analytical rigid surfaces, and
the default section controls.
Two-dimensional model (using CPE4R elements) with a
mass scaling factor of 68962, analytical rigid surfaces,
and the default section controls.
Implicit, quasi-static, two-dimensional model (using
CPE4R elements) with analytical rigid surfaces.
Two-dimensional case (using CPE6M elements) with a
mass scaling factor of 2758.
1.3.6–6
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
roll3d330_anl_c3d10m.inp
roll3d_medium.inp
roll3d_medium_gcont.inp
Three-dimensional case (using C3D10M elements) with
a mass scaling factor of 2758.
Additional mesh refinement case (using C3D8R
elements) included for the sole purpose of testing the
performance of the code.
Additional mesh refinement case (using C3D8R
elements) with the general contact capability.
References
•
Kobayashi, S., S. I. Oh, and T. Altan, Metal Forming and the Finite Element Method, Oxford
University Press, 1989.
•
Kopp, R., and P. M. Dohmen, “Simulation und Planung von Walzprozessen mit Hilfe der FiniteElemente-Methode (FEM),” Stahl U. Eisen, no. 7, pp. 131–136, 1990.
1.3.6–7
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
Table 1.3.6–1 Analysis cases and relative CPU costs. (The two-dimensional explicit analyses all use
CPE4R elements and stiffness hourglass control. The three-dimensional explicit analyses use C3D8R
elements and the centroidal kinematic and stiffness hourglass section controls.)
Analysis Type
Mass Scaling
Factor
Effective Roll Surface
Speed (m/sec)
Relative CPU
Time
Explicit, plane strain
Explicit, plane strain
Explicit, plane strain
Implicit, plane strain
Explicit, 3-D
Explicit, 3-D
110.3
2758.5
68961.8
11.2
56.1
280.5
quasi-static
56.1
~96
4.99
1.00
0.21
13.4
13.8
9.5
2758.5
automatic
Table 1.3.6–2 Explicit section controls tested (mass scaling factor=2758.5). CPE4R and
C3D8R elements are employed for the two-dimensional and three-dimensional cases, respectively.
Spread values are reported for the half-model at node 24015.
Analysis Type
Explicit, plane strain
Explicit, plane strain
Explicit, plane strain
Explicit, plane strain
Explicit, 3-D
Explicit, 3-D
Explicit, 3-D
Explicit, 3-D
Explicit, 3-D
Section Controls
Kinematic
Hourglass
n/a
n/a
n/a
n/a
average strain
orthogonal
centroidal
centroidal
orthogonal
stiffness
relax stiffness
combined
enhanced
relax stiffness
combined
stiffness
enhanced
enhanced
1.3.6–8
Abaqus Version 6.12 ID:
Printed on:
Relative
CPU Time
Spread
(mm)
1.00
1.11
1.04
1.02
20.8
17.1
13.8
14.8
17.3
n/a
n/a
n/a
n/a
2.06
2.07
2.10
2.10
2.10
ROLLING OF THICK PLATES
PEEQ
VALUE
+0.00E+00
+2.22E-16
+4.62E-02
+9.25E-02
+1.39E-01
+1.85E-01
+2.31E-01
+2.77E-01
2
3
+3.24E-01
1
Density Scale Factor 110.3
Two-dimensional Rolling
+3.70E-01
+4.65E-01
Figure 1.3.6–1 Equivalent plastic strain for the plane strain case (CPE4R) with
stiffness hourglass control (mass scaling factor=110.3).
PEEQ
VALUE
+0.00E+00
+2.22E-16
+4.62E-02
+9.25E-02
+1.39E-01
+1.85E-01
+2.31E-01
+2.77E-01
2
3
Figure 1.3.6–2
+3.24E-01
1
Density Scale Factor 2758.5
Two-dimensional Rolling
+4.43E-01
Equivalent plastic strain for the plane strain case (CPE4R) with stiffness
hourglass control (mass scaling factor=2758.5).
1.3.6–9
Abaqus Version 6.12 ID:
Printed on:
+3.70E-01
ROLLING OF THICK PLATES
PEEQ
VALUE
+0.00E+00
+2.22E-16
+4.62E-02
+9.25E-02
+1.39E-01
+1.85E-01
+2.31E-01
+2.77E-01
2
3
+3.24E-01
1
Figure 1.3.6–3
Density Scale Factor 68961.8
Two-dimensional Rolling
+3.70E-01
+4.64E-01
Equivalent plastic strain for the plane strain case (CPE4R) with stiffness
hourglass control (mass scaling factor=68961.8).
S12
VALUE
-1.05E+08
-8.00E+07
-6.38E+07
-4.75E+07
-3.13E+07
-1.50E+07
+1.25E+06
+1.75E+07
2
3
+3.37E+07
1
Figure 1.3.6–4
Density Scale Factor 110.3
Two-dimensional Rolling
+7.25E+07
Shear stress for the plane strain case (CPE4R) with stiffness hourglass
control (mass scaling factor=110.3).
1.3.6–10
Abaqus Version 6.12 ID:
Printed on:
+5.00E+07
ROLLING OF THICK PLATES
S12
VALUE
-9.75E+07
-8.00E+07
-6.38E+07
-4.75E+07
-3.13E+07
-1.50E+07
+1.25E+06
+1.75E+07
2
3
+3.37E+07
1
Figure 1.3.6–5
Density Scale Factor 2758.5
Two-dimensional Rolling
+5.00E+07
+6.91E+07
Shear stress for the plane strain case (CPE4R) with stiffness hourglass
control (mass scaling factor=2758.5).
S12
VALUE
-1.23E+08
-8.00E+07
-6.38E+07
-4.75E+07
-3.13E+07
-1.50E+07
+1.25E+06
+1.75E+07
2
3
+3.37E+07
1
Figure 1.3.6–6
Density Scale Factor 68961.8
Two-dimensional Rolling
+1.20E+08
Shear stress for the plane strain case (CPE4R) with stiffness hourglass
control (mass scaling factor=68961.8).
1.3.6–11
Abaqus Version 6.12 ID:
Printed on:
+5.00E+07
ROLLING OF THICK PLATES
Roller
Plate
PEEQ
Symmetry
Plane
VALUE
+0.00E+00
+2.22E-16
+4.62E-02
+9.25E-02
+1.39E-01
+1.85E-01
+2.31E-01
+2.77E-01
2
+3.24E-01
+3.70E-01
3
+4.35E-01
Density Scale Factor 2758.5
1
Figure 1.3.6–7 Equivalent plastic strain for the three-dimensional case (C3D8R) using the centroidal
kinematic and stiffness hourglass section controls (mass scaling factor=2758.5).
Roller
Plate
PEEQ
Symmetry
Plane
VALUE
+0.00E+00
+2.22E-16
+4.62E-02
+9.25E-02
+1.39E-01
+1.85E-01
+2.31E-01
+2.77E-01
2
+3.24E-01
+3.70E-01
3
1
Density Scale Factor 2758.5
+4.72E-01
Figure 1.3.6–8 Equivalent plastic strain for the three-dimensional case (C3D8R) using the average
strain kinematic and relax stiffness hourglass section controls (mass scaling factor=2758.5).
1.3.6–12
Abaqus Version 6.12 ID:
Printed on:
ROLLING OF THICK PLATES
PEEQ
VALUE
+0.00E+00
+2.22E-16
+4.62E-02
+9.25E-02
+1.39E-01
+1.85E-01
+2.31E-01
+2.77E-01
2
3
Figure 1.3.6–9
+3.24E-01
1
Density Scale Factor 2758.5
Two-dimensional Rolling
+3.70E-01
+4.55E-01
Equivalent plastic strain for the plane strain case (CPE6M) (mass scaling factor=2758.5).
Roller
Plate
PEEQ
Symmetry
Plane
VALUE
+0.00E+00
+2.22E-16
+4.62E-02
+9.25E-02
+1.39E-01
+1.85E-01
+2.31E-01
+2.77E-01
2
+3.24E-01
+3.70E-01
3
1
Density Scale Factor 2758.5
+5.23E-01
Figure 1.3.6–10 Equivalent plastic strain for the three-dimensional case
(C3D10M) (mass scaling factor=2758.5).
1.3.6–13
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC FORMING OF A CUP
1.3.7
AXISYMMETRIC FORMING OF A CIRCULAR CUP
Products: Abaqus/Standard
Abaqus/Explicit
This example illustrates the hydroforming of a circular cup using an axisymmetric model. In this case a
two-stage forming sequence is used, with annealing between the stages. Two analysis methods are used: in
one the entire process is analyzed using Abaqus/Explicit; in the other the forming sequences are analyzed
with Abaqus/Explicit, while the springback analyses are run in Abaqus/Standard. Here, the import capability
is used to transfer results between Abaqus/Explicit and Abaqus/Standard and vice versa.
Problem description
The model consists of a deformable blank and three rigid dies. The blank has a radius of 150.0 mm,
is 1.0 mm thick, and is modeled using axisymmetric shell elements, SAX1. The coefficient of friction
between the blank and the dies is taken to be 0.1. Dies 1 and 2 are offset from the blank by half of the
thickness of the blank, because the contact algorithm takes into account the shell thickness. To avoid
pinching of the blank while die 3 is put into position for the second forming stage, the radial gap between
dies 2 and 3 is set to be 20% bigger than the initial shell thickness. Figure 1.3.7–1 and Figure 1.3.7–2
show the initial geometry of the model.
The three dies are modeled with either two-dimensional analytical rigid surfaces or RAX2 rigid
elements. An analytical rigid surface can yield a more accurate representation of two-dimensional
curved punch geometries and result in computational savings. Contact pressure can be viewed on the
specimen surface, and the reaction force is available at the rigid body reference node. In addition, both
the kinematic (default) and penalty contact formulations are tested. Results for the kinematic contact
formulation using rigid elements are presented here.
The blank is made of aluminum-killed steel, which is assumed to satisfy the Ramberg-Osgood
relation between true stress and logarithmic strain,
with a reference stress value (K) of 513 MPa and work-hardening exponent (n) of 0.223. Isotropic
elasticity is assumed, with Young’s modulus of 211 GPa and Poisson’s ratio of 0.3. With these data an
initial yield stress of 91.3 MPa is obtained. The stress-strain behavior is defined by piecewise linear
segments matching the Ramberg-Osgood curve up to a total (logarithmic) strain level of 107%, with
Mises yield, isotropic hardening, and no rate dependence.
The analysis that is performed entirely within Abaqus/Explicit consists of six steps. In the first step
contact is defined between the blank and dies 1 and 2. Both dies remain fixed while a distributed load of
10 MPa in the negative z-direction is ramped onto the blank. This load is then ramped off in the second
step, allowing the blank to spring back to an equilibrium state.
The third step is an annealing step. The annealing procedure in Abaqus/Explicit sets all appropriate
state variables to zero. These variables include stresses, strains (excluding the thinning strain for shells,
1.3.7–1
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC FORMING OF A CUP
membranes, and plane stress elements), plastic strains, and velocities. There is no time associated with
an annealing step. The process occurs instantaneously.
In the fourth step contact is defined between the blank and die 3 and contact is removed between
the blank and die 1. Die 3 moves down vertically in preparation for the next pressure loading.
In the fifth step another distributed load is applied to the blank in the positive z-direction, forcing
the blank into die 3. This load is then ramped off in the sixth step to monitor the springback of the blank.
To obtain a quasi-static response, an investigation was conducted to determine the optimum rate
for applying the pressure loads and removing them. The optimum rate balances the computational time
against the accuracy of the results; increasing the loading rate will reduce the computer time but lead to
less accurate quasi-static results.
The analysis that uses the import capability consists of four runs. The first run is identical to Step 1
of the Abaqus/Explicit analysis described earlier. In the second run the Abaqus/Explicit results for the
first forming stage are imported into Abaqus/Standard without updating the reference configuration and
with an import of the material state for the first springback analysis. The third run imports the results of
the first springback analysis into Abaqus/Explicit for the subsequent annealing process and the second
forming stage. By updating the reference configuration and not importing the material state, this run
begins with no initial stresses or strains, effectively simulating the annealing process. The final run
imports the results of the second forming stage into Abaqus/Standard for the second springback analysis.
Results and discussion
Figure 1.3.7–3 to Figure 1.3.7–5 show the results of the analysis conducted entirely within
Abaqus/Explicit using the rigid element approach and the kinematic contact formulation. Figure 1.3.7–3
shows the deformed shape at the end of Step 2, after the elastic springback. Figure 1.3.7–4 shows the
deformed shape at the end of the analysis, after the second elastic springback. Although it is not shown
here, the amount of springback observed during the unloading steps is negligible. Figure 1.3.7–5 shows
a contour plot of the shell thickness (STH) at the end of the analysis. The thickness of the material at
the center of the cup has been reduced by about 20%, while the thickness at the edges of the cup has
been increased by about 10%.
The results obtained using the import capability to perform the springback analyses in
Abaqus/Standard are nearly identical, as are those obtained using analytical rigid surfaces and/or
penalty contact formulations.
You can use the abaqus restartjoin execution procedure to extract data from the output database
created by a restart analysis and append the data to a second output database. For more information, see
“Joining output database (.odb) files from restarted analyses,” Section 3.2.18 of the Abaqus Analysis
User’s Manual.
Input files
axiform.inp
Abaqus/Explicit analysis that uses rigid elements and
kinematic contact. This file is also used for the first step
of the analysis that uses the import capability.
1.3.7–2
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC FORMING OF A CUP
axiform_anl.inp
axiform_pen.inp
axiform_anl_pen.inp
axiform_sprbk1.inp
axiform_form2.inp
axiform_sprbk2.inp
axiform_restart.inp
axiform_rest_anl.inp
Model using analytical rigid surfaces and kinematic
contact.
Model using rigid elements and penalty contact.
Model using analytical rigid surfaces and penalty contact.
First springback analysis using the import capability.
Second forming analysis using the import capability.
Second springback analysis using the import capability.
Restart of axiform.inp included for the purpose of testing
the restart capability.
Restart of axiform_anl.inp included for the purpose of
testing the restart capability.
1.3.7–3
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC FORMING OF A CUP
blank
die2
die1
2
3
1
Figure 1.3.7–1
Configuration at the beginning of stage 1.
die2
die3
2
3
1
Figure 1.3.7–2 Configuration of dies in forming stage 2. (The
dotted line shows the initial position of die 3.)
1.3.7–4
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC FORMING OF A CUP
2
3
1
Figure 1.3.7–3
Deformed configuration after the first forming stage.
2
3
1
Figure 1.3.7–4
Final configuration.
1.3.7–5
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC FORMING OF A CUP
STH
VALUE
+8.63E-04
+8.83E-04
+9.02E-04
+9.22E-04
+9.41E-04
+9.61E-04
+9.80E-04
+1.00E-03
+1.11E-03
2
1
3
Figure 1.3.7–5
Contour plot of shell thickness.
1.3.7–6
Abaqus Version 6.12 ID:
Printed on:
CUP/TROUGH FORMING
1.3.8
CUP/TROUGH FORMING
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing in forging problems that include large amounts of shearing
at the tool-blank interface; a cup and a trough are formed.
Problem description
Three different geometric models are considered, as shown in Figure 1.3.8–1. Each model consists of
a rigid punch, a rigid die, and a deformable blank. The outer top and bottom edges of the blank are
cambered, which facilitates the flow of material against the tools. The punch and die have semicircular
cross-sections; the punch has a radius of 68.4 mm, and the die has a radius of 67.9 mm. The blank is
modeled as a von Mises elastic, perfectly plastic material with a Young’s modulus of 4000 MPa and a
yield stress of 5 MPa. The Poisson’s ratio is 0.21; the density is 1.E−4 tonne/mm3 .
In each case the punch is moved 61 mm, while the die is fully constrained. A smooth amplitude
curve is used to ramp the punch velocity to a maximum, at which it remains constant. The smoothing of
the velocity promotes a quasi-static response to the loading.
Case 1: Axisymmetric model for cup forming
The blank is meshed with CAX4R elements and measures 50 × 64.77 mm. The punch and the die are
modeled as analytical rigid surfaces using connected line segments. Symmetry boundary conditions are
prescribed at r=0. The finite element model is shown in Figure 1.3.8–2.
Case 2: Three-dimensional model for trough forming
The blank is meshed with C3D8R elements and measures 50 × 64.7 × 64.7 mm. The punch and the die
are modeled as three-dimensional cylindrical analytical rigid surfaces. Symmetry boundary conditions
are applied at the x=0 and z=0 planes. The finite element model of the blank is shown in Figure 1.3.8–3.
Case 3: Three-dimensional model for cup forming
The blank is meshed with C3D8R elements. A 90° wedge of the blank with a radius of 50 mm and
a height of 64.7 mm is analyzed. The punch and the die are modeled as three-dimensional revolved
analytical rigid surfaces. Symmetry boundary conditions are applied at the x=0 and y=0 planes. The
finite element model of the blank is shown in Figure 1.3.8–4.
Adaptive meshing
A single adaptive mesh domain that incorporates the entire blank is used for each model. Symmetry
planes are defined as Lagrangian boundary regions (the default), and contact surfaces are defined as
sliding boundary regions (the default). Since this problem is quasi-static with relatively small amounts
of deformation per increment, the default values for frequency, mesh sweeps, and other adaptive mesh
parameters and controls are sufficient.
1.3.8–1
Abaqus Version 6.12 ID:
Printed on:
CUP/TROUGH FORMING
Results and discussion
Figure 1.3.8–5 through Figure 1.3.8–7 show the mesh configuration at the end of the forging simulation
for Cases 1–3. In each case a quality mesh is maintained throughout the simulation. As the blank flattens
out, geometric edges and corners that exist at the beginning of the analysis are broken and adaptive
meshing is allowed across them. The eventual breaking of geometric edges and corners is essential for
this type of problem to minimize element distortion and optimize element aspect ratios.
For comparison purposes Figure 1.3.8–8 shows the deformed mesh for a pure Lagrangian simulation
of Case 1 (the axisymmetric model). The mesh is clearly better when continuous adaptive meshing
is used. Several diamond-shaped elements with extremely poor aspect ratios are formed in the pure
Lagrangian simulation. Adaptive meshing improves the element quality significantly, especially along
the top surface of the cup where solution gradients are highest. Figure 1.3.8–9 and Figure 1.3.8–10
show contours of equivalent plastic strain at the completion of the forging for the adaptive meshing and
pure Lagrangian analyses of Case 1, respectively. Overall plastic strains compare quite closely. Slight
differences exist only along the upper surface, where the pure Lagrangian mesh becomes very distorted
at the end of the simulation. The time histories of the vertical punch force for the adaptive and pure
Lagrangian analyses agree closely for the duration of the forging, as shown in Figure 1.3.8–11.
Input files
ale_cupforming_axi.inp
ale_cupforming_axinodes.inp
ale_cupforming_axielements.inp
ale_cupforming_cyl.inp
ale_cupforming_sph.inp
lag_cupforming_axi.inp
Case 1.
External file referenced by Case 1.
External file referenced by Case 1.
Case 2.
Case 3.
Lagrangian solution of Case 1.
1.3.8–2
Abaqus Version 6.12 ID:
Printed on:
CUP/TROUGH FORMING
case 2
case 1
case 3
punch
punch
punch
v
v
symmetry axis
v
blank
blank
64.7 mm
symmetry symmetry
plane
plane
symmetry
planes
fixed die
90°
fixed die
50 mm
Figure 1.3.8–1
Model geometries for each case.
2
3
1
Figure 1.3.8–2
Undeformed mesh for Case 1.
1.3.8–3
Abaqus Version 6.12 ID:
Printed on:
blank
fixed die
CUP/TROUGH FORMING
2
3
1
Figure 1.3.8–3
Undeformed mesh for Case 2.
Figure 1.3.8–4
Undeformed mesh for Case 3.
3
2
1
1.3.8–4
Abaqus Version 6.12 ID:
Printed on:
CUP/TROUGH FORMING
2
3
1
Figure 1.3.8–5
Deformed mesh for Case 1.
Figure 1.3.8–6
Deformed mesh for Case 2.
1.3.8–5
Abaqus Version 6.12 ID:
Printed on:
CUP/TROUGH FORMING
3
2
1
Figure 1.3.8–7
Deformed mesh for Case 3.
2
3
1
Figure 1.3.8–8
Deformed mesh for Case 1 using a pure Lagrangian formulation.
1.3.8–6
Abaqus Version 6.12 ID:
Printed on:
CUP/TROUGH FORMING
PEEQ
VALUE
+2.38E-01
+4.41E-01
+8.93E-01
+1.34E+00
+1.80E+00
+2.25E+00
+2.70E+00
+2.90E+00
2
3
Figure 1.3.8–9
1
Contours of equivalent plastic strain for Case 1 using adaptive meshing.
PEEQ
VALUE
+2.13E-01
+4.41E-01
+8.93E-01
+1.34E+00
+1.80E+00
+2.25E+00
+2.70E+00
+2.91E+00
2
3
Figure 1.3.8–10
1
Contours of equivalent plastic strain for Case 1 using a pure Lagrangian fomulation.
1.3.8–7
Abaqus Version 6.12 ID:
Printed on:
CUP/TROUGH FORMING
0.
3
[ x10 ]
LAG
ALE
VERTICAL REACTION FORCE (N)
-40.
XMIN 0.000E+00
XMAX 1.000E+00
YMIN -2.157E+05
YMAX 0.000E+00
-80.
-120.
-160.
-200.
0.0
0.2
0.4
0.6
0.8
1.0
TOTAL TIME (seconds)
Figure 1.3.8–11
Comparison of time histories for the vertical punch force for Case 1.
1.3.8–8
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH SINUSOIDAL DIES
1.3.9
FORGING WITH SINUSOIDAL DIES
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing in forging problems that incorporate geometrically
complex dies and involve substantial material flow.
Problem description
Three different geometric models are considered, as shown in Figure 1.3.9–1. Each model consists of a
rigid die and a deformable blank. The cross-sectional shape of the die is sinusoidal with an amplitude and
a period of 5 and 10 mm, respectively. The blank is steel and is modeled as a von Mises elastic-plastic
material with a Young’s modulus of 200 GPa, an initial yield stress of 100 MPa, and a constant hardening
slope of 300 MPa. Poisson’s ratio is 0.3; the density is 7800 kg/m3 .
In all cases the die is moved downward vertically at a velocity of 2000 mm/sec and is constrained
in all other degrees of freedom. The total die displacement is 7.6 mm for Case 1, 6.7 mm for Case 2,
and 5.6 mm for Case 3. These displacements represent the maximum possible given the refinement
and topology of the initial mesh (if the quality of the mesh is retained for the duration of the analysis).
Although each analysis uses a sinusoidal die, the geometries and flow characteristics of the blank material
are quite different for each problem.
Case 1: Axisymmetric model
The blank is meshed with CAX4R elements and measures 20 × 10 mm. The dies are modeled as analytical
rigid surfaces comprised of connected line segments. The bottom of the blank is constrained in the
z-direction, and symmetry boundary conditions are prescribed at r=0. The initial configuration of the
blank and the die is shown in Figure 1.3.9–2.
Case 2: Three-dimensional model
The blank is meshed with C3D8R elements and measures 20 × 10 × 10 mm. The dies are modeled
as three-dimensional cylindrical analytical rigid surfaces. The bottom of the blank is constrained in the
y-direction, and symmetry boundary conditions are applied at the x=0 and z=10 planes. The finite element
model of the blank and the die is shown in Figure 1.3.9–3.
Case 3: Three-dimensional model
The blank is meshed with C3D8R elements and measures 20 × 10 × 20 mm. The dies are modeled
as three-dimensional revolved analytical rigid surfaces. The bottom of the blank is constrained in the
y-direction, and symmetry boundary conditions are applied at the x=0 and z=10 planes. The finite element
model of the blank and the die is shown in Figure 1.3.9–4. The revolved die is displaced upward in the
figure from its initial position for clarity.
1.3.9–1
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH SINUSOIDAL DIES
Adaptive meshing
A single adaptive mesh domain that incorporates the entire blank is used for each model. Symmetry
planes are defined as Lagrangian boundary regions (the default), and contact surfaces are defined as
sliding boundary regions (the default). Because the material flow for each of the geometries is substantial,
the frequency and the intensity of adaptive meshing must be increased to provide an accurate solution.
The frequency at which adaptive meshing is to be performed is reduced from the default of 10 to 5 for
all cases. The number of mesh sweeps is increased from the default of 1 to 3 for all cases.
Results and discussion
Figure 1.3.9–5 and Figure 1.3.9–6 show the deformed mesh and contours of equivalent plastic strain
at the completion of the forming step for Case 1. Adaptive meshing maintains reasonable element
shapes and aspect ratios. This type of forging problem cannot typically be solved using a pure
Lagrangian formulation. Figure 1.3.9–7 shows the deformed mesh for Case 2. A complex, doubly
curved deformation pattern is formed on the free surface as the material spreads under the die. Element
distortion appears to be reasonable. Figure 1.3.9–8 and Figure 1.3.9–9 show the deformed mesh
and contours of equivalent plastic strain for Case 3. Although the die is a revolved geometry, the
three-dimensional nature of the blank gives rise to fairly complex strain patterns that are symmetric
with respect to the planes of quarter symmetry.
Input files
ale_sinusoid_forgingaxi.inp
ale_sinusoid_forgingaxisurf.inp
ale_sinusoid_forgingcyl.inp
ale_sinusoid_forgingrev.inp
Case 1.
External file referenced by Case 1.
Case 2.
Case 3.
1.3.9–2
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH SINUSOIDAL DIES
v
symmetry axis
punch
z
10 mm
r
case 1
20 mm
v
y
punch
x
z
10 mm
sym
m
pla etry
ne
case 2
y
etr
mm e
sy plan
20 mm
10 mm
y
symmetry
planes
v
z
case 3
punch
x
10 mm
20 mm
20 mm
symmetry
plane
Figure 1.3.9–1
Model geometries for each of the three cases.
1.3.9–3
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH SINUSOIDAL DIES
2
3
1
Figure 1.3.9–2
Initial configuration for Case 1.
Figure 1.3.9–3
Initial configuration for Case 2.
2
1
3
1.3.9–4
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH SINUSOIDAL DIES
2
1
3
2
1
3
Figure 1.3.9–4
Initial configuration for Case 3.
1.3.9–5
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH SINUSOIDAL DIES
2
3
1
Figure 1.3.9–5
PEEQ
Deformed mesh for Case 1.
VALUE
+4.77E-01
+8.14E-01
+1.15E+00
+1.49E+00
+1.83E+00
+2.16E+00
+2.50E+00
+2.84E+00
2
3
1
Figure 1.3.9–6
Contours of equivalent plastic strain for Case 1.
1.3.9–6
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH SINUSOIDAL DIES
2
1
3
Figure 1.3.9–7
Deformed mesh for Case 2.
Figure 1.3.9–8
Deformed mesh for Case 3.
2
1
3
1.3.9–7
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH SINUSOIDAL DIES
PEEQ
VALUE
+1.34E-01
+4.16E-01
+6.98E-01
+9.79E-01
+1.26E+00
+1.54E+00
+1.82E+00
+2.11E+00
2
1
3
Figure 1.3.9–9
Contours of equivalent plastic strain for Case 3.
1.3.9–8
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH MULTIPLE COMPLEX DIES
1.3.10
FORGING WITH MULTIPLE COMPLEX DIES
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing in forging problems that use multiple geometrically
complex dies. The problem is based on a benchmark presented at the “FEM–Material Flow Simulation in the
Forging Industry” workshop.
Problem description
The benchmark problem is an axisymmetric forging, but in this example both axisymmetric and
three-dimensional geometric models are considered. For the axisymmetric models the default hourglass
formulation (HOURGLASS=RELAX STIFFNESS) and the enhanced strain hourglass formulation
(HOURGLASS=ENHANCED) are considered. For the three-dimensional geometric models the
pure stiffness hourglass formulation (HOURGLASS=STIFFNESS) and the enhanced strain hourglass
formulation with the orthogonal kinematic formulation (KINEMATIC SPLIT=ORTHOGONAL) are
considered. Each model is shown in Figure 1.3.10–1. Both models consist of two rigid dies and a
deformable blank. The blank’s maximum radial dimension is 895.2 mm, and its thickness is 211.4 mm.
The outer edge of the blank is rounded to facilitate the flow of material through the dies. The blank is
modeled as a von Mises elastic-plastic material with a Young’s modulus of 200 GPa, an initial yield
stress of 360 MPa, and a constant hardening slope of 30 MPa. The Poisson’s ratio is 0.3; the density is
7340 kg/m3 .
Both dies are fully constrained, with the exception of the top die, which is moved 183.4 mm
downward at a constant velocity of 166.65 mm/s.
Case 1: Axisymmetric model
The blank is meshed with CAX4R elements. A fine discretization is required in the radial direction
because of the geometric complexity of the dies and the large amount of material flow that occurs
in that direction. Symmetry boundary conditions are prescribed at r=0. The dies are modeled as
TYPE=SEGMENTS analytical rigid surfaces. The initial configuration is shown in Figure 1.3.10–2.
Case 2: Three-dimensional model
The blank is meshed with C3D8R elements. A 90° wedge of the blank is analyzed. The level of mesh
refinement is the same as that used in the axisymmetric model. Symmetry boundary conditions are
applied at the x=0 and z=0 planes. The dies are modeled as TYPE=REVOLUTION analytical rigid
surfaces. The initial configuration of the blank only is shown in Figure 1.3.10–3. Although the tools are
not shown in the figure, they are originally in contact with the blank.
Adaptive meshing
A single adaptive mesh domain that incorporates the entire blank is used for each model. Symmetry
planes are defined as Lagrangian boundary regions (the default), and contact surfaces are defined as
1.3.10–1
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH MULTIPLE COMPLEX DIES
sliding boundary regions (the default). Since this problem is quasi-static with relatively small amounts of
deformation per increment, the defaults for frequency, mesh sweeps, and other adaptive mesh parameters
and controls are sufficient.
Results and discussion
Figure 1.3.10–4 and Figure 1.3.10–5 show the deformed mesh for the axisymmetric case using the
default hourglass control formulation (HOURGLASS=RELAX STIFFNESS) at an intermediate stage
(
0.209 s) and in the final configuration (
0.35 s), respectively. The elements remain well
shaped throughout the entire simulation, with the exception of the elements at the extreme radius of
the blank, which become very coarse as material flows radially during the last 5% of the top die’s
travel. Figure 1.3.10–6 shows contours of equivalent plastic strain at the completion of forming.
Figure 1.3.10–7 and Figure 1.3.10–8 show the deformed mesh for the three-dimensional case using
the pure stiffness hourglass control (HOURGLASS=STIFFNESS) and the orthogonal kinematic
formulation (KINEMATIC SPLIT=ORTHOGONAL) at
0.209 and
0.35, respectively. Although
the axisymmetric and three-dimensional mesh smoothing algorithms are not identical, the elements
in the three-dimensional model also remain well shaped until the end of the analysis, when the same
behavior that is seen in the two-dimensional model occurs. Contours of equivalent plastic strain for the
three-dimensional model (not shown) are virtually identical to those shown in Figure 1.3.10–6.
Input files
ale_duckshape_forgingaxi.inp
ale_duckshape_forgingaxi_enhs.inp
ale_duckshape_forg_axind.inp
ale_duckshape_forg_axiel.inp
ale_duckshape_forg_axiset.inp
ale_duckshape_forg_axirs.inp
ale_duckshape_forgingrev.inp
ale_duckshape_forgingrev_oenhs.inp
Case 1 using the default hourglass formulation
(HOURGLASS=RELAX STIFFNESS).
Case 1 using the enhanced strain hourglass formulation
(HOURGLASS=ENHANCED).
External file referenced by the Case 1 analyses.
External file referenced by the Case 1 analyses.
External file referenced by the Case 1 analyses.
External file referenced by the Case 1 analyses.
Case 2 using the pure stiffness hourglass
formulation
(HOURGLASS=STIFFNESS)
and
the orthogonal kinematic formulation (KINEMATIC
SPLIT=ORTHOGONAL).
Case 2 using the enhanced strain hourglass
formulation
(HOURGLASS=ENHANCED)
and
the orthogonal kinematic formulation (KINEMATIC
SPLIT=ORTHOGONAL).
Reference
•
Industrieverband Deutscher Schmieden e.V. (IDS), “Forging of an Axisymmetric Disk,”
FEM–Material Flow Simulation in the Forging Industry, Hagen, Germany, October 1997.
1.3.10–2
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH MULTIPLE COMPLEX DIES
punch
symmetry axis
v
z
blank
fixed die
r
y
v
punch
x
fixed die
sym
me
try
pla
ne
Figure 1.3.10–1
ne
pla
y
r
t
me
sym
Axisymmetric and three-dimensional model geometries.
1.3.10–3
Abaqus Version 6.12 ID:
Printed on:
z
FORGING WITH MULTIPLE COMPLEX DIES
2
3
1
Figure 1.3.10–2
Initial configuration for the axisymmetric model.
2
1
3
Figure 1.3.10–3
Initial configuration mesh for the three-dimensional model.
1.3.10–4
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH MULTIPLE COMPLEX DIES
2
3
1
Figure 1.3.10–4 The deformed mesh for the axisymmetric model using the default hourglass
formulation (HOURGLASS=RELAX STIFFNESS) at an intermediate stage.
2
3
1
Figure 1.3.10–5 The deformed mesh for the axisymmetric model using the default hourglass
formulation (HOURGLASS=RELAX STIFFNESS) at the end of forming.
1.3.10–5
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH MULTIPLE COMPLEX DIES
PEEQ
(Ave. Crit.: 75%)
+2.481e+00
+2.296e+00
+2.110e+00
+1.925e+00
+1.739e+00
+1.553e+00
+1.368e+00
+1.182e+00
+9.966e-01
+8.110e-01
+6.254e-01
+4.398e-01
+2.542e-01
2
3
1
Figure 1.3.10–6 Contours of equivalent plastic strain for
the axisymmetric model using the default hourglass formulation
(HOURGLASS=RELAX STIFFNESS) at the end of forming.
1.3.10–6
Abaqus Version 6.12 ID:
Printed on:
FORGING WITH MULTIPLE COMPLEX DIES
2
3
1
Figure 1.3.10–7 The deformed mesh for the three-dimensional model using the pure stiffness
hourglass formulation (HOURGLASS=STIFFNESS) and the orthogonal kinematic formulation
(KINEMATIC SPLIT=ORTHOGONAL) at an intermediate stage.
2
1
3
Figure 1.3.10–8 The deformed mesh for the three-dimensional model using the pure stiffness
hourglass formulation (HOURGLASS=STIFFNESS) and the orthogonal kinematic formulation
(KINEMATIC SPLIT=ORTHOGONAL) at the end of forming.
1.3.10–7
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
1.3.11
FLAT ROLLING: TRANSIENT AND STEADY-STATE
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing to simulate a rolling process using both transient and
steady-state approaches, as shown in Figure 1.3.11–1. A transient flat rolling simulation is performed using
three different methods: a “pure” Lagrangian approach, an adaptive meshing approach using a Lagrangian
domain, and a mixed Eulerian-Lagrangian adaptive meshing approach in which material upstream from
the roller is drawn from an Eulerian inflow boundary but the downstream end of the blank is handled in a
Lagrangian manner. In addition, a steady-state flat rolling simulation is performed using an Eulerian adaptive
mesh domain as a control volume and defining inflow and outflow Eulerian boundaries. Solutions using
each approach are compared.
Problem description
For each analysis case quarter symmetry is assumed; the model consists of a rigid roller and a deformable
blank. The blank is meshed with C3D8R elements. The cylindrical roller is modeled as an analytical
rigid surface. The radius of the cylinder is 175 mm. Symmetry boundary conditions are prescribed on
the right (z=0 plane) and bottom (y=0 plane) faces of the blank.
Coulomb friction with a friction coefficient of 0.3 is assumed between the roller and the plate. All
degrees of freedom are constrained on the roller except rotation about the z-axis, where a constant angular
velocity of 6.28 rad/sec is defined. For each analysis case the blank is given an initial velocity of 0.3 m/s
in the x-direction to initiate contact.
The blank is steel and is modeled as a von Mises elastic-plastic material with isotropic hardening.
The Young’s modulus is 150 GPa, and the initial yield stress is 168.2 MPa. The Poisson’s ratio is 0.3; the
density is 7800 kg/m3 . The masses of all blank elements are scaled by a factor of 2750 at the beginning
of the step so that the analysis can be performed more economically. This scaling factor represents an
approximate upper bound on the mass scaling possible for this problem, above which significant inertial
effects would be generated.
The criteria for stopping the rolling analyses based on the achievement of a steady-state condition
is defined. The criteria used require the satisfaction of the steady-state detection norms of equivalent
plastic strain, spread, force, and torque within the default tolerances. The exit plane for each norm is
defined as the plane passing through the center of the roller with the normal to the plane coincident with
the rolling direction. For Case 1 through Case 3 the steady-state detection norms are evaluated as each
plane of elements passes the exit plane. Case 4 requires uniform sampling since the initial mesh is
roughly stationary due to the initial geometry and the inflow and outflow Eulerian boundaries.
The finite element models used for each analysis case are shown in Figure 1.3.11–2. A description
of each model and the adaptive meshing techniques used follows:
Case 1: Transient simulation—pure Lagrangian approach
The blank is initially rectangular and measures 224 × 20 × 50 mm. No adaptive meshing is performed.
The analysis is run until steady-state conditions are achieved.
1.3.11–1
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
Case 2: Transient simulation—Lagrangian adaptive mesh domain
The finite element model for this case is identical to that used for Case 1, with the exception that a single
adaptive mesh domain that incorporates the entire blank is defined to allow continuous adaptive meshing.
Symmetry planes are defined as Lagrangian surfaces (the default), and the contact surface on the blank is
defined as a sliding surface (the default). The analysis is run until steady-state conditions are achieved.
Case 3: Transient simulation—mixed Eulerian-Lagrangian approach
This analysis is performed on a relatively short initial blank measuring 65 × 20 × 50 mm. Material is
continuously drawn by the action of the roller on the blank through an inflow Eulerian boundary defined
on the upstream end. The blank is meshed with the same number of elements as in Cases 1 and 2 so that
similar aspect ratios are obtained as the blank lengthens and steady-state conditions are achieved.
An adaptive mesh domain is defined that incorporates the entire blank. Because it contains at least
one Eulerian surface, this domain is considered Eulerian for the purpose of setting parameter defaults.
However, the analysis model has both Lagrangian and Eulerian aspects. The amount of material flow
with respect to the mesh will be large at the inflow end and small at the downstream end of the domain.
To account for the Lagrangian motion of the downstream end, change the adaptive mesh controls for
this problem so that adaptive meshing is performed based on the positions of the nodes at the start of
the current adaptive mesh increment. To mesh the inflow end accurately and to perform the analysis
economically, the frequency is set to 5 and the number of mesh sweeps is set to 5.
As in Case 2, symmetry planes are defined as Lagrangian boundary regions (the default), and
the contact surface on the blank is defined as a sliding boundary region (the default). In addition, the
boundary on the upstream end is defined as an Eulerian surface. Adaptive mesh constraints are defined
on the Eulerian surface using adaptive mesh constraints to hold the inflow surface mesh completely
fixed while material is allowed to enter the domain normal to the surface. An equation constraint is used
to ensure that the velocity normal to the inflow boundary is uniform across the surface. The velocity of
nodes in the direction tangential to the inflow boundary surface is constrained.
Case 4: Steady-state simulation—Eulerian adaptive mesh domain
This analysis employs a control volume approach in which material is drawn from an inflow Eulerian
boundary and is pushed out through an outflow boundary by the action of the roller. The blank geometry
for this analysis case is defined such that it approximates the shape corresponding to the steady-state
solution: this geometry can be thought of as an “initial guess” to the solution. The blank initially measures
224 mm in length and 50 mm in width and has a variable thickness such that it conforms to the shape of
the roller. The surface of the blank transverse to the rolling direction is not adjusted to account for the
eventual spreading that will occur in the steady-state solution. Actually, any reasonable initial geometry
will reach a steady state, but geometries that are closer to the steady-state geometry often allow a solution
to be obtained in a shorter period of time.
As in the previous two cases an adaptive mesh domain is defined on the blank, symmetry planes
are defined as Lagrangian surfaces (the default), and the contact surface is defined as a sliding surface
(the default). Inflow and outflow Eulerian surfaces are defined on the ends of the blank using the same
1.3.11–2
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
techniques as in Case 3, except that for the outflow boundary adaptive mesh constraints are applied only
normal to the boundary surface and no material constraints are applied tangential to the boundary surface.
To improve the computational efficiency of the analysis, the frequency of adaptive meshing is
increased to every fifth increment because the Eulerian domain undergoes very little overall deformation
and the material flow speed is much less than the material wave speed. This frequency will cause the
mesh at Eulerian boundaries to drift slightly. However, the amount of drift is extremely small and does
not accumulate. There is no need to increase the mesh sweeps because this domain is relatively stationary
and, by default, adaptive meshing is performed based on the nodal positions of the original mesh. Very
little mesh smoothing is required.
Results and discussion
The final deformed configurations of the blank for each of the three transient cases are shown in
Figure 1.3.11–3. The transient cases have reached a steady-state solution and have been terminated
based on the criteria given in the steady-state detection definition. Steady-state conditions are
determined to have been reached when the reaction forces and moments on the roller have stabilized
and the cross-sectional shape and distribution of equivalent plastic strain under the roller become
constant over time. When using a steady-state detection definition, these conditions imply that the
force, moment, spread, and equivalent plastic strain norms have stabilized such that the changes in the
norms over three consecutive sampling intervals have fallen below the user-prescribed tolerances. See
“Steady-state detection,” Section 11.8.1 of the Abaqus Analysis User’s Manual, for a detailed discussion
on the definition of the norms. Contours of equivalent plastic strain for each of the three transient
cases are in good agreement and are shown in the final configuration of each blank in Figure 1.3.11–4.
Figure 1.3.11–5 shows the initial and final mesh configurations at steady state. With the exception of
Case 3 all analyses were terminated using the default steady-state norm tolerances. Case 3 required
that the force and torque norm tolerances be increased from .005 to .01 due to the force and torque at
the roller being rather noisy.
To compare the results from the transient and steady-state approaches, the steady-state detection
norms are summarized for each case in Table 1.3.11–1. The table shows a comparison of the values of
the steady-state detection norms after the analyses have been terminated. The only significant difference
is in the value of the spread norm for Case 4, which is higher than the others. The spread norm is defined
as the largest of the second principle moments of inertia of the workpiece’s cross-section. Since the
spread norm is a cubic function of the lateral deformation of the workpiece, rather small differences in
displacements between the test cases can lead to significant differences in the spread norms.
Time history plots of the steady-state detection norms are also shown. Figure 1.3.11–9 and
Figure 1.3.11–10 show time history plots of the steady-state force and torque norms, respectively, for
all cases. The force and torque norms are essentially running averages of the force and moment on the
roller and show good agreement for all four test cases. Figure 1.3.11–7 and Figure 1.3.11–8 show time
history plots of the steady-state equivalent plastic strain and spread norms, respectively, for all cases.
The equivalent plastic strains norms are in good agreement for all cases.
1.3.11–3
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
Input files
lag_flatrolling.inp
lag_flatrolling_gcont.inp
ale_flatrolling_noeuler.inp
ale_flatrolling_inlet.inp
ale_flatrolling_inletoutlet.inp
Table 1.3.11–1
Formulation
Case
Case
Case
Case
Spread norm
1
2
3
4
1.349
1.369
1.365
1.485
E−7
E−7
E−7
E−7
Case 1 with contact pairs.
Case 1 with general contact.
Case 2.
Case 3.
Case 4.
Comparison of steady-state detection norms.
Effective
plastic strain
norm
.8037
.8034
.8018
.8086
Force norm
−1.43
−1.43
−1.43
−1.40
E6
E6
E6
E6
Torque norm
3.59
3.55
3.61
3.65
E4
E4
E4
E4
Transient: Pure Lagrangian
(case 1)
Transient: Adaptive Meshing with
(case 3)
Eulerian Inflow
Transient: Adaptive Meshing
(case 2)
Steady State: Adaptive Meshing with
Eulerian Inflow and Outflow (case 4)
smoothed mesh
Figure 1.3.11–1
Diagram illustrating the four analysis approaches used in this problem.
1.3.11–4
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
2
3
1
Case 1 & Case 2
2
3
1
Case 3
2
3
1
Case 4
Figure 1.3.11–2
Initial configurations for each case.
1.3.11–5
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
2
Case 1
1
3
2
Case 2
1
3
2
Case 3
1
3
Figure 1.3.11–3
Deformed mesh for Cases 1–3.
1.3.11–6
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
PEEQ
VALUE
+.00E+00
+1.25E-01
+2.50E-01
+3.75E-01
+5.01E-01
Case 1
+6.26E-01
+7.51E-01
+8.74E-01
PEEQ
VALUE
+.00E+00
+1.25E-01
+2.50E-01
+3.75E-01
+5.01E-01
Case 2
+6.26E-01
+7.51E-01
+8.76E-01
PEEQ
VALUE
+.00E+00
+1.25E-01
+2.50E-01
+3.75E-01
+5.01E-01
Case 3
+6.26E-01
+7.51E-01
+8.75E-01
Figure 1.3.11–4
Contours of equivalent plastic strain for Cases 1–3.
1.3.11–7
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
Case 4
2
1
3
Initial Mesh
Deformed Mesh
Figure 1.3.11–5
PEEQ
Deformed mesh for Case 4 (shown with initial mesh for comparison).
VALUE
+.00E+00
+1.25E-01
+2.50E-01
+3.75E-01
+5.01E-01
Case 4
+6.26E-01
+7.51E-01
+8.52E-01
Figure 1.3.11–6
Contours of equivalent plastic strain for Case 4.
1.3.11–8
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
SSPEEQ1
SSPEEQ1
SSPEEQ1
SSPEEQ1
Figure 1.3.11–7
(Case
(Case
(Case
(Case
1)
2)
3)
4)
Comparison of equivalent plastic strain norm versus time for all cases.
SSSPRD1
SSSPRD1
SSSPRD1
SSSPRD1
(Case
(Case
(Case
(Case
Figure 1.3.11–8
1)
2)
3)
4)
Comparison of spread norm versus time for all cases.
1.3.11–9
Abaqus Version 6.12 ID:
Printed on:
FLAT ROLLING
SSFORC1
SSFORC1
SSFORC1
SSFORC1
(Case
(Case
(Case
(Case
Figure 1.3.11–9
SSTORQ1
SSTORQ1
SSTORQ1
SSTORQ1
(Case
(Case
(Case
(Case
Figure 1.3.11–10
1)
2)
3)
4)
Comparison of force norm versus time for all cases.
1)
2)
3)
4)
Comparison of torque norm versus time for all cases.
1.3.11–10
Abaqus Version 6.12 ID:
Printed on:
SECTION ROLLING
1.3.12
SECTION ROLLING
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing in a transient simulation of section rolling. Results are
compared to a pure Lagrangian simulation.
Problem description
This analysis shows a stage in the rolling of a symmetric I-section. Because of the cross-sectional shape
of the I-section, two planes of symmetry exist and only a quarter of the section needs to be modeled. The
quarter-symmetry model, shown in Figure 1.3.12–1, consists of two rigid rollers and a blank. Roller 1
has a radius of 747 mm, and roller 2 has a radius of 452 mm. The blank has a length of 850 mm, a web
half-width of 176.7 mm, a web half-thickness of 24 mm, and a variable flange thickness.
The finite element model is shown in Figure 1.3.12–2. The blank is meshed with C3D8R elements.
Symmetry boundary conditions are applied on the y and z symmetry planes of the blank. The rollers
are modeled as three-dimensional revolved analytical rigid surfaces. Roller 1 has all degrees of freedom
constrained except rotation about the z-axis, where a constant angular velocity of 5 rad/sec is specified.
Roller 2 has all degrees of freedom constrained except rotation about the y-axis. An initial velocity of
4187.0 mm/sec in the negative x-direction is applied to the blank to initiate contact between the blank
and the rollers. This velocity corresponds to the velocity of the rollers at the point of initial contact.
Variable mass scaling is used to scale the masses of all the blank elements so that a desired minimum
stable time increment is achieved initially and the stable time increment does not fall below this minimum
throughout the analysis. The loading rates and mass scaling definitions are such that a quasi-static
solution is generated.
The blank is steel and is modeled as a von Mises elastic-plastic material with a Young’s modulus of
212 GPa, an initial yield stress of 80 MPa, and a constant hardening slope of 258 MPa. Poisson’s ratio is
0.281; the density is 7833 kg/m3 . Coulomb friction with a friction coefficient of 0.3 is assumed between
the rollers and the blank.
Adaptive meshing
Adaptive meshing can improve the solution and mesh quality for section rolling problems that involve
large deformations. A single adaptive mesh domain that incorporates the entire blank is defined.
Symmetry planes are defined as Lagrangian boundary regions (the default), and the contact surface
on the blank is defined as a sliding boundary region (the default). The default values are used for all
adaptive mesh parameters and controls.
Results and discussion
Figure 1.3.12–3 shows the deformed configuration of the blank when continuous adaptive meshing is
used. For comparison purposes a pure Lagrangian simulation is performed. Figure 1.3.12–4 shows
the deformed configuration for a pure Lagrangian simulation. The mesh at the flange-web interface is
1.3.12–1
Abaqus Version 6.12 ID:
Printed on:
SECTION ROLLING
distorted in the Lagrangian simulation, but the mesh remains nicely proportioned in the adaptive mesh
analysis. A close-up view of the deformed configuration of the blank is shown for each analysis in
Figure 1.3.12–5 and Figure 1.3.12–6 to highlight the differences in mesh quality. Contours of equivalent
plastic strain for each analysis are shown in Figure 1.3.12–7 and Figure 1.3.12–8. The plastic strain
distributions are very similar.
Figure 1.3.12–9 and Figure 1.3.12–10 show time history plots for the y-component of reaction force
and the reaction moment about the z-axis, respectively, for roller 1. The results for the adaptive mesh
simulation compare closely to those for the pure Lagrangian simulation.
Input files
ale_rolling_section.inp
ale_rolling_sectionnode.inp
ale_rolling_sectionelem.inp
ale_rolling_sectionnelset.inp
ale_rolling_sectionsurf.inp
lag_rolling_section.inp
lag_rolling_section_gcont.inp
Analysis that uses adaptive meshing.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
Lagrangian analysis using contact pairs.
Lagrangian analysis using general contact.
1.3.12–2
Abaqus Version 6.12 ID:
Printed on:
SECTION ROLLING
747 mm
roller 1
blank
775 mm
y
x
z
roller 2
452 mm
workpiece with rigid tools
y
z
x
symmetry planes
24 mm
176.5 mm
cross-sectional view of blank
Figure 1.3.12–1
Geometry of the quarter-symmetry blank and the rollers.
1.3.12–3
Abaqus Version 6.12 ID:
Printed on:
SECTION ROLLING
Roller 1
Blank
2
1
3
Roller 2
Figure 1.3.12–2
Quarter-symmetry finite element model.
1.3.12–4
Abaqus Version 6.12 ID:
Printed on:
SECTION ROLLING
2
1
3
Figure 1.3.12–3
Deformed blank for the adaptive mesh simulation.
2
1
3
Figure 1.3.12–4
Deformed blank for the pure Lagrangian simulation.
1.3.12–5
Abaqus Version 6.12 ID:
Printed on:
SECTION ROLLING
2
1
3
Figure 1.3.12–5
Close-up of the deformed blank for the adaptive mesh simulation.
2
1
3
Figure 1.3.12–6
Close-up of the deformed blank for the pure Lagrangian simulation.
1.3.12–6
Abaqus Version 6.12 ID:
Printed on:
SECTION ROLLING
PEEQ
VALUE
+0.00E+00
+3.32E-01
+6.94E-01
+1.06E+00
+1.42E+00
+1.78E+00
+2.14E+00
+2.33E+00
2
1
3
Figure 1.3.12–7
PEEQ
Contours of equivalent plastic strain for the adaptive mesh simulation.
VALUE
+0.00E+00
+3.32E-01
+6.94E-01
+1.06E+00
+1.42E+00
+1.78E+00
+2.14E+00
+2.50E+00
2
1
Figure 1.3.12–8
3
Contours of equivalent plastic strain for the pure Lagrangian simulation.
1.3.12–7
Abaqus Version 6.12 ID:
Printed on:
SECTION ROLLING
-2.
Lagrangian
Adaptive Mesh
[ x10 6 ]
REACTION FORCE - RF2 (N)
-4.
-6.
-8.
-10.
XMIN 0.000E+00
XMAX 2.270E-01
YMIN -1.139E+07
YMAX -1.078E+06
0.00
0.04
0.08
0.12
0.16
0.20
TOTAL TIME (sec)
Figure 1.3.12–9 Time history of the reaction force in the
y-direction at the reference node of Roller 1.
1.6
[ x10 6 ]
Lagrangian
Adaptive Mesh
REACTION MOMENT - RM3 (N-m)
1.2
0.8
0.4
0.0
-0.4
XMIN 0.000E+00
XMAX 2.270E-01
YMIN -9.567E+05
YMAX 1.700E+06
-0.8
0.00
0.04
0.08
0.12
0.16
0.20
TOTAL TIME (sec)
Figure 1.3.12–10 Time history of the reaction moment about
the z-axis at the reference node of Roller 1.
1.3.12–8
Abaqus Version 6.12 ID:
Printed on:
RING ROLLING
1.3.13
RING ROLLING
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing in a two-dimensional rolling simulation. Results are
compared to those obtained using a pure Lagrangian approach.
Problem description
Ring rolling is a specialized process typically used to manufacture parts with revolved geometries such as
bearings. The three-dimensional rolling setup usually includes a freely mounted, idle roll; a continuously
rotating driver roll; and guide rolls in the rolling plane. Transverse to the rolling plane, conical rolls are
used to stabilize the ring and provide a forming surface in the out-of-plane direction. In this example a
two-dimensional, plane stress idealization is used that ignores the effect of the conical rolls. A schematic
diagram of the ring and the surrounding tools is shown in Figure 1.3.13–1.
The driver roll has a diameter of 680 mm, and the idle and guide rolls have diameters of 102 mm.
The ring has an initial inner diameter of 127.5 mm and a thickness of 178.5 mm. The idle and driver
rolls are arranged vertically and are in contact with the inner and outer surfaces of the ring, respectively.
The driver roll is rotated around its stationary axis, while the idle roll is moved vertically downward at
a specified feed rate. For this simulation the x–y motion of the guide rolls is determined a priori and
is prescribed so that the rolls remain in contact with the ring throughout the analysis but do not exert
appreciable force on it. In practice the guide rolls are usually connected through linkage systems, and
their motion is a function of both force and displacement.
The ring is meshed with CPS4R elements, as shown in Figure 1.3.13–2. The ring is steel and is
modeled as a von Mises elastic-plastic material with a Young’s modulus of 150 GPa, an initial yield
stress of 168.7 MPa, and a constant hardening slope of 884 MPa. The Poisson’s ratio is 0.3; the density
is 7800 kg/m3 .
The analysis is run so that the ring completes approximately 20 revolutions (16.5 seconds). The
rigid rolls are modeled as analytical rigid surfaces using connected line segments. The driver roll is
rotated at a constant angular velocity of 3.7888 rad/sec about the z-axis, while the idle roll has a constant
feed rate of 4.9334 mm/sec and is free to rotate about the z-axis. All other degrees of freedom for the
driver and idle rolls are constrained. A friction coefficient of 0.5 is defined at the blank-idle roll and
blank-drive roll interfaces. Frictionless contact is used between the ring and guide rolls, and the rotation
of the guide rolls is constrained since the actual guide rolls are free to rotate and exert negligible torque
on the ring.
To obtain an economical solution, the masses of all elements in the ring are scaled by a factor
of 2500. This scaling factor represents a reasonable upper limit on the mass scaling possible for
this problem, above which significant inertial effects would be generated. Furthermore, since the
two-dimensional model does not contain the conical rolls, the ring oscillates from side to side even
under the action of the guide rolls. An artificial viscous pressure of 300 MPa sec/m is applied on the
inner and outer surfaces of the ring to assist the guide rolls in preserving the circular shape of the ring.
The pressure value was chosen by trial and error.
1.3.13–1
Abaqus Version 6.12 ID:
Printed on:
RING ROLLING
Adaptive meshing
A single adaptive mesh domain that incorporates the ring is defined. Contact surfaces on the ring are
defined as sliding boundary regions (the default). Because of the large number of increments required
to simulate 20 revolutions, the deformation per increment is very small. Therefore, the frequency of
adaptive meshing is changed from the default of 10 to every 50 increments. The cost of adaptive meshing
at this frequency is negligible compared to the underlying analysis cost.
Results and discussion
Figure 1.3.13–3 shows the deformed configuration of the ring after completing 20 revolutions with
continuous adaptive meshing. High-quality element shapes and aspect ratios are maintained throughout
the simulation. Figure 1.3.13–4 shows the deformed configuration of the ring when a pure Lagrangian
simulation is performed. The pure Lagrangian mesh is distorted, especially at the inner radius where
elements become skewed and very small in the radial direction.
Figure 1.3.13–5 and Figure 1.3.13–6 show time history plots for the y-component of reaction force
on the idle roll and the reaction moment about the z-axis for the driver roll, respectively, for both the
adaptive mesh and pure Lagrangian approaches. Although the final meshes are substantially different,
the roll force and torque match reasonably well.
For both the adaptive and pure Lagrangian solutions the plane stress idealization used here results
in very localized through-thickness straining at the inner and outer radii of the ring. This specific type of
localized straining is unique to plane stress modeling and does not occur in ring rolling processes. It is
also not predicted by a three-dimensional finite element model. If adaptivity is used and refined meshing
is desired to capture strong gradients at the inner and outer extremities, the initially uniform mesh can be
replaced with a graded mesh. Although not shown here, a graded mesh concentrates element refinement
in areas of strong gradients. You can specify in the adaptive mesh controls that the initial mesh gradation
should be preserved while distortions are reduced as the analysis evolves.
Input files
ale_ringroll_2d.inp
ale_ringroll_2dnode.inp
ale_ringroll_2delem.inp
guideamp.inp
lag_ringroll_2d.inp
Analysis that uses adaptive meshing.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
Lagrangian analysis.
1.3.13–2
Abaqus Version 6.12 ID:
Printed on:
RING ROLLING
ring
306 mm
idle
roll
127 mm
guide roll
guide roll
102 mm
v(t)
102 mm
102 mm
680 mm
ω0
driver roll
Figure 1.3.13–1
Model geometry for the two-dimensional ring rolling analysis.
1.3.13–3
Abaqus Version 6.12 ID:
Printed on:
RING ROLLING
Figure 1.3.13–2
Figure 1.3.13–3
Initial mesh configuration.
Deformed configuration after 20 revolutions using adaptive meshing.
1.3.13–4
Abaqus Version 6.12 ID:
Printed on:
RING ROLLING
Figure 1.3.13–4
Deformed configuration after 20 revolutions using a pure Lagrangian approach.
1.3.13–5
Abaqus Version 6.12 ID:
Printed on:
RING ROLLING
-1.
ale_1648
6
[ x10 ]
lag_1648
REACTION FORCE - RF2 (N)
-2.
-3.
-4.
-5.
-6.
XMIN 0.000E+00
XMAX 1.650E+01
YMIN -6.899E+06
YMAX -5.424E+05
-7.
0.
4.
8.
12.
16.
TOTAL TIME (sec)
Figure 1.3.13–5
Time history of the reaction force in the y-direction for the idle roll.
[ x10 6 ]
ale_1648
-0.2
REACTION MOMENT - RM3 (N-m)
lag_1648
-0.4
-0.6
-0.8
XMIN 0.000E+00
XMAX 1.650E+01
YMIN -9.855E+05
YMAX -5.462E+04
-1.0
0.
4.
8.
12.
16.
TOTAL TIME (sec)
Figure 1.3.13–6
Time history of the reaction moment about the z-axis for the driver roll.
1.3.13–6
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
1.3.14
AXISYMMETRIC EXTRUSION: TRANSIENT AND STEADY-STATE
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing in simulations of extrusion processes with three
axisymmetric analysis cases. First, a transient simulation is performed for a backward, flat-nosed die,
extrusion geometry using adaptivity on a Lagrangian mesh domain. Second, a transient simulation is
performed on the analogous forward, square die, extrusion geometry, also using adaptivity on a Lagrangian
mesh domain. Finally, a steady-state simulation is performed for the forward extrusion geometry using
adaptivity on an Eulerian mesh domain.
Problem description
The model configurations for the three analysis cases are shown in Figure 1.3.14–1. Each of the models
is axisymmetric and consists of one or more rigid tools and a deformable blank. The rigid tools are
modeled as analytical rigid surfaces of connected line segments. All contact surfaces are assumed to be
well-lubricated and, thus, are treated as frictionless. The blank is made of aluminum and is modeled as
a von Mises elastic-plastic material with isotropic hardening. The Young’s modulus is 38 GPa, and the
initial yield stress is 27 MPa. The Poisson’s ratio is 0.33; the density is 2672 kg/m3 .
Case 1: Transient analysis of a backward extrusion
The model geometry consists of a rigid die, a rigid punch, and a blank. The blank is meshed with CAX4R
elements and measures 28 × 89 mm. The blank is constrained along its base in the z-direction and at the
axis of symmetry in the r-direction. Radial expansion is prevented by contact between the blank and the
die. The punch and the die are fully constrained, with the exception of the prescribed vertical motion of
the punch. The punch is moved downward 82 mm to form a tube with wall and endcap thicknesses of
7 mm each. The punch velocity is specified using a smooth amplitude so that the response is essentially
quasi-static.
The deformation that occurs in extrusion problems, especially in those that involve flat-nosed die
geometries, is extreme and requires adaptive meshing. Since adaptive meshing in Abaqus/Explicit works
with the same mesh topology throughout the step, the initial mesh must be chosen such that the mesh
topology will be suitable for the duration of the simulation. A simple meshing technique has been
developed for extrusion problems such as this. In two dimensions it uses a four-sided, mapped mesh
domain that can be created with nearly all finite element mesh preprocessors. The vertices for the
four-sided, mapped mesh are shown in Figure 1.3.14–1 and are denoted A, B, C, and D. Two vertices
are located on either side of the extrusion opening, the third is in the corner of the dead material zone
(the upper left corner of the blank), and the fourth vertex is located in the diagonally opposite corner.
A 10 × 60 element mesh using this meshing technique is created for this analysis case and is shown in
Figure 1.3.14–2. The mesh refinement is oriented such that the fine mesh along sides AB and DC will
move up along the extruded walls as the punch is moved downward.
An adaptive mesh domain is defined that incorporates the entire blank. Because of the extremely
large distortions expected in the backward extrusion simulation, three mesh sweeps, instead of the default
1.3.14–1
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
value of one, are specified for each adaptive mesh increment. The default adaptive meshing frequency
of 10 is used. Alternatively, a higher frequency could be specified to perform one mesh sweep per
adaptive mesh increment. However, this method would result in a higher computational cost because of
the increased number of advection sweeps it would require.
A substantial amount of initial mesh smoothing is performed by increasing the number of mesh
sweeps to be performed at the beginning of the step to 100. The initially smoothed mesh is shown in
Figure 1.3.14–2. Initial smoothing reduces the distortion of the mapped mesh by rounding out corners
and easing sharp transitions before the analysis is performed; therefore, it allows the best mesh to be
used throughout the analysis.
Case 2: Transient analysis of a forward extrusion
The model geometry consists of a rigid die and a blank. The blank geometry and the mesh are identical
to those described for Case 1, except that the mapped mesh is reversed with respect to the vertical plane
so that the mesh lines are oriented toward the forward extrusion opening. The blank is constrained at the
axis of symmetry in the r-direction. Radial expansion is prevented by contact between the blank and the
die. The die is fully constrained. The blank is pushed up 19 mm by prescribing a constant velocity of
5 m/sec for the nodes along the bottom of the blank. As the blank is pushed up, material flows through
the die opening to form a solid rod with a 7 mm radius.
Adaptive meshing for Case 2 is defined in a similar manner as for Case 1. The undeformed mesh
configurations, before and after initial mesh smoothing, are shown in Figure 1.3.14–3.
Case 3: Steady-state analysis of a forward extrusion
The model geometry consists of a rigid die, identical to the die used for Case 2, and a blank. The blank
geometry is defined such that it closely approximates the shape corresponding to the steady-state solution:
this geometry can be thought of as an “initial guess” to the solution. As shown in Figure 1.3.14–4, the
blank is discretized with a simple graded pattern that is most refined near the die fillet. No special mesh
is required for the steady-state case since minimal mesh motion is expected during the simulation. The
blank is constrained at the axis of symmetry in the r-direction. Radial expansion of the blank is prevented
by contact between it and the die.
An adaptive mesh domain is defined that incorporates the entire blank. Because the Eulerian domain
undergoes very little overall deformation and the material flow speed is much less than the material wave
speed, the frequency of adaptive meshing is changed to 5 from the default value of 1 to improve the
computational efficiency of the analysis.
The outflow boundary is assumed to be traction-free and is located far enough downstream to ensure
that a steady-state solution can be obtained. This boundary is cast as an Eulerian boundary region. A
multi-point constraint is defined on the outflow boundary to keep the velocity normal to the boundary
uniform. The inflow boundary is defined using an Eulerian boundary condition to prescribe a velocity of
5 m/sec in the vertical direction. Adaptive mesh constraints are defined on both the inflow and outflow
boundaries to fix the mesh in the vertical direction. This effectively creates a stationary control volume
with respect to the inflow and outflow boundaries through which material can pass.
1.3.14–2
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Results and discussion
The results for each analysis case are described below.
Case 1
The use of the mapped meshing technique along with adaptive meshing allows the backward extrusion
analysis to run to completion, creating the long tube with an endcap. Three plots of the deformed mesh
at various times are shown in Figure 1.3.14–5. These plots clearly show how the quality of the mesh is
preserved for the majority of the simulation. Despite the large amount of deformation involved, the mesh
remains smooth and concentrated in the areas of high strain gradients. Extreme deformation and thinning
at the punch fillet occurs near the end of the analysis. This thinning can be reduced by increasing the fillet
radius of the punch. Corresponding contours of equivalent plastic strain are plotted in Figure 1.3.14–6.
The plastic strains are highest along the inner surface of the tube.
Case 2
Adaptive meshing enables the transient forward extrusion simulation to proceed much further than would
be possible using a pure Lagrangian approach. After pushing the billet 19 mm through the die, the
analysis cannot be continued because the elements become too distorted. Since the billet material is
essentially incompressible and the cross-sectional area of the die opening at the top is 1/16 of the original
cross-sectional area of the billet, a rod measuring approximately 304 mm (three times the length of the
original billet) is formed.
Three plots of the deformed mesh at various times in the transient forward extrusion are shown
in Figure 1.3.14–7. As in the backward extrusion case, the plots show that the quality of the mesh is
preserved for a majority of the simulation. The last deformed shape has been truncated for clarity because
the extruded column becomes very long and thin. Contours of equivalent plastic strain at similar times
are shown in Figure 1.3.14–8. The plastic strain distribution developing in the vertical column does
not reach a steady-state value, even at a height of 304 mm. The steady-state results reported in the
discussion for Case 3 show that a steady-state solution based on the equivalent plastic strain distribution
is not reached until much later. An absolute steady-state solution cannot be reached until the material
on the upstream side of the dead material zone first passes along that zone and through the die opening.
The dead material zone is roughly the shape of a triangle and is located in the upper right-hand corner
of the die.
Case 3
The steady-state solution to the forward extrusion analysis is obtained at an extruded column height of
800 mm, which corresponds to pushing the billet 50 mm through the die. Thus, this analysis runs 2.5
times longer than Case 2.
Contours of equivalent plastic strain in the middle and at the end of the simulation are shown in
Figure 1.3.14–9. Time histories of the equivalent plastic strains on the outer edge of the extruded column
at the outflow boundary and 27.5 mm below the outflow boundary are shown in Figure 1.3.14–10. The
plastic strains at both locations converge to the same value by the end of the simulation, which indicates
1.3.14–3
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
that the solution has reached a steady state. The final mesh configuration is shown in Figure 1.3.14–11.
The mesh undergoes very little change from the beginning to the end of the analysis because of the
accurate initial guess made for the steady-state domain shape and the ability of the adaptive meshing
capability in Abaqus/Explicit to retain the original mesh gradation.
As a further check on the accuracy of the steady-state simulation and the conservation properties of
adaptive meshing, a time history of the velocity at the outflow boundary is shown in Figure 1.3.14–12.
The velocity reaches a steady value of approximately 80 m/s, which is consistent with the incompressible
material assumption and the 1/16 ratio of the die opening to the billet size.
Input files
ale_extrusion_back.inp
ale_extrusion_backnode.inp
ale_extrusion_backelem.inp
ale_extrusion_forward.inp
ale_extrusion_forwardnode.inp
ale_extrusion_forwardelem.inp
ale_extrusion_eulerian.inp
ale_extrusion_euleriannode.inp
ale_extrusion_eulerianelem.inp
Case 1.
Node data for Case 1.
Element data for Case 1.
Case 2.
Node data for Case 2.
Element data for Case 2.
Case 3.
Node data for Case 3.
Element data for Case 3.
1.3.14–4
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Transient:
Backward Extrusion
(case 1)
Transient:
Forward Extrusion
(case 2)
Steady State:
Forward Extrusion
(case 3)
punch
Eulerian
outflow
7 mm
21 mm
69 mm
v
C
flow
fixed die
symmetry axis
symmetry axis
flow
fixed die
flow
symmetry axis
B
fixed die
A
89 mm
Eulerian
inflow
D
simple
support
v = 5000 mm/s
Figure 1.3.14–1
Axisymmetric model geometries used in the extrusion analysis.
1.3.14–5
Abaqus Version 6.12 ID:
Printed on:
v = 5000 mm/s
AXISYMMETRIC EXTRUSION
Figure 1.3.14–2
Undeformed configuration for Case 1, before and after initial smoothing.
1.3.14–6
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Figure 1.3.14–3
Undeformed configuration for Case 2, before and after initial smoothing.
1.3.14–7
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Figure 1.3.14–4
Undeformed configuration for Case 3.
1.3.14–8
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Figure 1.3.14–5
Deformed mesh at various times for Case 1.
1.3.14–9
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Figure 1.3.14–6
Contours of equivalent plastic strain at various times for Case 1.
1.3.14–10
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Figure 1.3.14–7
Deformed mesh at various times for Case 2.
1.3.14–11
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Figure 1.3.14–8
Contours of equivalent plastic strain at various times for Case 2.
1.3.14–12
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Figure 1.3.14–9 Contours of equivalent plastic strain at an
intermediate stage and at the end of the analysis for Case 3.
Figure 1.3.14–10 Time history of equivalent plastic strain along
the outer edge of the extruded column for Case 3.
1.3.14–13
Abaqus Version 6.12 ID:
Printed on:
AXISYMMETRIC EXTRUSION
Figure 1.3.14–11
Figure 1.3.14–12
Final deformed mesh for Case 3.
Time history of material velocity at the outflow boundary for Case 3.
1.3.14–14
Abaqus Version 6.12 ID:
Printed on:
TWO-STEP FORMING SIMULATION
1.3.15
TWO-STEP FORMING SIMULATION
Product: Abaqus/Explicit
This example illustrates the use of adaptive meshing in simulations of a two-step, bulk metal forming process.
The problem is based on a benchmark problem presented at the Metal Forming Process Simulation in Industry
conference.
Problem description
The model consists of two sets of rigid forming tools (one set for each forming step) and a deformable
blank. The blank and forming die geometries used in the simulation are shown in Figure 1.3.15–1.
The initial configurations of the blank and the tools for each step are shown in Figure 1.3.15–2 and
Figure 1.3.15–4. All forming tools are modeled as discrete rigid bodies and meshed with R3D4 and R3D3
elements. The blank, which is meshed with C3D8R elements, is cylindrical and measures 14.5 × 21 mm.
A half model is constructed, so symmetry boundary conditions are prescribed at the y=0 plane.
The blank is made of a steel alloy that is assumed to satisfy the Ramberg-Osgood relation for true
stress and logarithmic strain,
with a reference stress value (K) of 763 MPa and a work-hardening exponent (n) of 0.245. Isotropic
elasticity is assumed, with a Young’s modulus of 211 GPa and a Poisson’s ratio of 0.3. An initial yield
stress of 200 MPa is obtained with these data. The stress-strain behavior is defined by piecewise linear
segments matching the Ramberg-Osgood curve up to a total (logarithmic) strain level of 140%, with von
Mises yield and isotropic hardening.
The analysis is conducted in two steps. For the first step the rigid tools consist of a planar punch,
a planar base, and a forming die. The initial configuration for this step is shown in Figure 1.3.15–2.
The base, which is not shown, is placed at the opening of the forming die to prevent material from
passing through the die. The motion of the tools is fully constrained, with the exception of the prescribed
displacement in the z-direction for the punch, which is moved 12.69 mm toward the blank at a constant
velocity of 30 m/sec consistent with a quasi-static response. The deformed configuration of the blank at
the completion of the first step is shown in Figure 1.3.15–3.
In the second step the original punch and die are removed from the model and replaced with a new
punch and die, as shown in Figure 1.3.15–4. The removal of the tools is accomplished by deleting the
contact pairs between them and the blank. Although not shown in the figure, the base is retained; both
it and the new die are fully constrained. The punch is moved 10.5 mm toward the blank at a constant
velocity of 30 m/sec consistent with a quasi-static response. The deformed configuration of the blank at
the completion of the second step is shown in Figure 1.3.15–5.
1.3.15–1
Abaqus Version 6.12 ID:
Printed on:
TWO-STEP FORMING SIMULATION
Adaptive meshing
A single adaptive mesh domain that incorporates the entire blank is used for both steps. A Lagrangian
boundary region type (the default) is used to define the constraints on the symmetry plane, and a sliding
boundary region type (the default) is used to define all contact surfaces. The frequency of adaptive
meshing is increased to 5 for this problem since material flows quickly near the end of the step.
Results and discussion
Figure 1.3.15–6 shows the deformed mesh at the completion of forming for an analysis in which a pure
Lagrangian mesh is used. Comparing Figure 1.3.15–5 and Figure 1.3.15–6, the resultant mesh for the
simulation in which adaptive meshing is used is clearly better than that obtained with a pure Lagrangian
mesh.
In Figure 1.3.15–7 through Figure 1.3.15–9 path plots of equivalent plastic strain in the blank are
shown using the pure Lagrangian and adaptive mesh domains for locations in the y=0 symmetry plane
at an elevation of z=10 mm. The paths are defined in the positive x-direction (from left to right in
Figure 1.3.15–4 to Figure 1.3.15–6). As shown in Figure 1.3.15–7, the results are in good agreement
at the end of the first step. At the end of the second step the path is discontinuous. Two paths are
considered: one that spans the left-hand side and another that spans the right-hand side of the U-shaped
cross-section along the symmetry plane. The left- and right-hand paths are shown in Figure 1.3.15–8
and Figure 1.3.15–9, respectively. The solutions from the second step compare qualitatively. Small
differences can be attributed to the increased mesh resolution and reduced mesh distortion for the adaptive
mesh domain.
Input files
ale_forging_steelpart.inp
ale_forging_steelpartnode1.inp
ale_forging_steelpartnode2.inp
ale_forging_steelpartnode3.inp
ale_forging_steelpartnode4.inp
ale_forging_steelpartelem1.inp
ale_forging_steelpartelem2.inp
ale_forging_steelpartelem3.inp
ale_forging_steelpartelem4.inp
ale_forging_steelpartelem5.inp
ale_forging_steelpartsets.inp
lag_forging_steelpart.inp
lag_forging_steelpart_gcont.inp
Analysis with adaptive meshing.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
External file referenced by the adaptive mesh analysis.
Pure Lagrangian analysis.
Pure Lagrangian general contact analysis.
1.3.15–2
Abaqus Version 6.12 ID:
Printed on:
TWO-STEP FORMING SIMULATION
Reference
•
Hermann, M., and A. Ruf, “Forming of a Steel Part,” Metal Forming Process Simulation in Industry,
Stuttgart, Germany, September 1994.
punch
⇒
2
1
die
2
3
1
3
symmetry plane
initial configuration for the first step
blank
⇓
punch
⇐
die
2
1
symmetry
plane
3
2
3
deformed blank at the end of first step
1
⇓
configuration at the
beginning of second step
3
2
1
deformed blank at the end of second step
Figure 1.3.15–1
Two-step forging process.
1.3.15–3
Abaqus Version 6.12 ID:
Printed on:
TWO-STEP FORMING SIMULATION
punch
2
1
3
die
Figure 1.3.15–2
Initial configuration for the first step.
2
1
3
Figure 1.3.15–3
Deformed blank at the end of the first step.
1.3.15–4
Abaqus Version 6.12 ID:
Printed on:
TWO-STEP FORMING SIMULATION
punch
die
3
2
1
Figure 1.3.15–4
Configuration at the beginning of the second step.
1.3.15–5
Abaqus Version 6.12 ID:
Printed on:
TWO-STEP FORMING SIMULATION
Figure 1.3.15–5
Figure 1.3.15–6
Deformed blank at the end of the second step for the adaptive mesh analysis.
Deformed blank at the end of the second step for the pure Lagrangian analysis.
1.3.15–6
Abaqus Version 6.12 ID:
Printed on:
TWO-STEP FORMING SIMULATION
0.5
ALE
LAG
PLASTIC STRAIN - PEEQ
0.4
0.3
0.2
0.1
XMIN
XMAX
YMIN
YMAX
0.000E+00
3.910E+01
0.000E+00
5.082E-01
0.0
0.
5.
10.
15.
20.
25.
30.
35.
40.
Distance along X-axis at Y(0) and Z(10) (mm)
Figure 1.3.15–7
Path plot of equivalent plastic strain at the end of the first step.
3.5
ALE
3.0
LAG
PLASTIC STRAIN - PEEQ
2.5
2.0
1.5
1.0
0.5
XMIN
XMAX
YMIN
YMAX
0.000E+00
5.000E+00
0.000E+00
3.412E+00
0.0
0.0
0.5
1.0
1.5
2.0
2.5
3.0
3.5
4.0
4.5
Distance along X-axis at Y(0) and Z(10) (mm)
Figure 1.3.15–8 Path plot of equivalent plastic strain along
the left side at the end of the second step.
1.3.15–7
Abaqus Version 6.12 ID:
Printed on:
5.0
TWO-STEP FORMING SIMULATION
ALE
2.0
PLASTIC STRAIN - PEEQ
LAG
1.5
1.0
XMIN
XMAX
YMIN
YMAX
0.000E+00
5.500E+00
7.967E-01
2.216E+00
0.
1.
2.
3.
4.
Distance along X-axis at Y(0) and Z(10) (mm)
Figure 1.3.15–9 Path plot of equivalent plastic strain along
the right side at the end of the second step.
1.3.15–8
Abaqus Version 6.12 ID:
Printed on:
5.
CYLINDRICAL BILLET
1.3.16
UPSETTING OF A CYLINDRICAL BILLET: COUPLED TEMPERATUREDISPLACEMENT AND ADIABATIC ANALYSIS
Products: Abaqus/Standard
Abaqus/Explicit
This example illustrates coupled temperature-displacement analysis in a metal forming application. The
case studied is an extension of the standard test case that is defined in Lippmann (1979); thus, some
verification of the results is available by comparison with the numerical results presented in that reference.
The example is that of a small, circular billet of metal that is reduced in length by 60%. Here the problem
is analyzed as a viscoplastic case, including heating of the billet by plastic work. Such analysis is often
important in manufacturing processes, especially when significant temperature rises degrade the material.
The problem is also analyzed in Abaqus/Standard using a porous metal material model. The same problem
is used in “Upsetting of a cylindrical billet: quasi-static analysis with mesh-to-mesh solution mapping
(Abaqus/Standard) and adaptive meshing (Abaqus/Explicit),” Section 1.3.1, to illustrate mesh rezoning in
Abaqus/Standard and adaptive meshing in Abaqus/Explicit.
Geometry and model
The specimen is shown in Figure 1.3.16–1: a circular billet, 30 mm long, with a radius of 10 mm,
compressed between flat, rough, rigid dies. All surfaces of the billet are assumed to be fully insulated:
this thermal boundary condition is chosen to maximize the temperature rise.
The finite element model is axisymmetric and includes the top half of the billet only since the middle
surface of the billet is a plane of symmetry. In Abaqus/Standard elements of type CAX8RT, 8-node
quadrilaterals with reduced integration that allow for fully coupled temperature-displacement analysis,
are used. A regular mesh with six elements in each direction is used, as shown in Figure 1.3.16–1. In
addition, the billet is modeled with CAX4RT elements in a 12 × 12 mesh for both Abaqus/Standard and
Abaqus/Explicit analyses.
The contact between the top and the lateral exterior surfaces of the billet and the rigid die is modeled
with a contact pair. The billet surface is defined by means of an element-based surface. The rigid
die is modeled as an analytical rigid surface or as an element-based rigid surface. The mechanical
interaction between the contact surfaces is assumed to be nonintermittent, rough frictional contact in
Abaqus/Standard. Therefore, the contact property includes two additional specifications: a no-separation
contact pressure-overclosure relationship to ensure that separation does not occur once contact has been
established and rough friction to enforce a no-slip constraint once contact has been established. In
Abaqus/Explicit the friction coefficient between the billet and the rigid die is 1.0.
The problem is also solved in Abaqus/Standard with the first-order fully coupled temperaturedisplacement CAX4T elements in a 12 × 12 mesh. Similarly, the problem is solved using CAX8RT
elements and user subroutines UMAT and UMATHT to illustrate the use of these subroutines.
No mesh convergence studies have been performed, but the comparison with results given in
Lippmann (1979) suggests that these meshes provide accuracy similar to the best of those analyses.
The Abaqus/Explicit simulations are performed both with and without adaptive meshing.
1.3.16–1
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
Material
The material definition is basically that given in Lippmann (1979), except that the metal is assumed to
be rate dependent. The thermal properties are added, with values that correspond to a typical steel, as
well as the data for the porous metal plasticity model. The material properties are then as follows:
Young’s modulus:
Poisson’s ratio:
Thermal expansion coefficient:
Initial static yield stress:
Work hardening rate:
Strain rate dependence:
Specific heat:
Density:
Conductivity:
Porous material parameters:
Initial relative density:
200 GPa
0.3
1.2×10−5 per °C
700 MPa
300 MPa
;
/s,
586 J/(kg°C)
7833 kg/m3
52 J/(m-s-°C)
0.95 (
0.05)
Since the problem definition in Abaqus/Standard assumes that the dies are completely rough, no
tangential slipping is allowed wherever the metal contacts the die.
Boundary conditions and loading
The kinematic boundary conditions are symmetry on the axis (nodes at
0, in node set AXIS, have
0 prescribed) and symmetry about
0 (all nodes at
0, in node set MIDDLE, have
0
prescribed). To avoid overconstraint, the node on the top surface of the billet that lies on the symmetry
axis is not part of the node set AXIS: the radial motion of this node is already constrained by a no-slip
frictional constraint (see “Common difficulties associated with contact modeling in Abaqus/Standard,”
Section 38.1.2 of the Abaqus Analysis User’s Manual, and “Common difficulties associated with contact
modeling using contact pairs in Abaqus/Explicit,” Section 38.2.2 of the Abaqus Analysis User’s Manual).
The rigid body reference node for the rigid surface that defines the die is constrained to have no rotation or
-displacement, and its -displacement is prescribed to move 9 mm down the axis at constant velocity.
The reaction force at the rigid reference node corresponds to the total force applied by the die.
The thermal boundary conditions are that all external surfaces are insulated (no heat flux allowed).
This condition is chosen because it is the most extreme case: it must provide the largest temperature rises
possible, since no heat can be removed from the specimen.
One of the controls for the automatic time incrementation scheme in Abaqus/Standard is the limit on
the maximum temperature change allowed to occur in any increment. It is set to 100°C, which is a large
value and indicates that we are not restricting the time increments because of accuracy considerations in
integrating the heat transfer equations. In fact, the automatic time incrementation scheme will choose
fairly small increments because of the severe nonlinearity present in the problem and the resultant need
for several iterations per increment even with a relatively large number of increments. The maximum
1.3.16–2
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
allowable temperature change in an increment is set to a large value to obtain a reasonable solution at
low cost.
In Abaqus/Explicit the automatic time incrementation scheme is used to ensure numerical stability
and to advance the solution in time. Mass scaling is used to reduce the computational cost of the analysis.
The amplitude is applied linearly over the step because the default amplitude variation for a transient,
coupled temperature-displacement analysis is a step function, but here we want the die to move down at
a constant velocity.
Two versions of the analysis are run: a slow upsetting, where the upsetting occurs in 100 seconds,
and a fast upsetting, where the event takes 0.1 second. Both versions are analyzed with the coupled
temperature-displacement procedure. The fast upsetting is also run in Abaqus/Standard as an adiabatic
static stress analysis. The time period values are specified with the respective procedure options. The
adiabatic stress analysis is performed in the same time frame as the fast upsetting case. In all cases
analyzed with Abaqus/Standard an initial time increment of 1.5% of the time period is used; that is,
1.5 seconds in the slow case and 0.0015 second in the fast case. This value is chosen because it will
result in a nominal axial strain of about 1% per increment, and experience suggests that such increment
sizes are generally suitable for cases like this.
Results and discussion
The results of the Abaqus/Standard simulations are discussed first, beginning with the results for the
viscoplastic fully dense material. The results of the slow upsetting are illustrated in Figure 1.3.16–2
to Figure 1.3.16–4. The results for the fast upsetting coupled temperature-displacement analysis are
illustrated in Figure 1.3.16–5 to Figure 1.3.16–7; those for the adiabatic static stress analysis are shown
in Figure 1.3.16–8 and Figure 1.3.16–9. Figure 1.3.16–2 and Figure 1.3.16–5 show the configuration
that is predicted at 60% upsetting. The configuration for the adiabatic analysis is not shown since it is
almost identical to the fast upsetting coupled case. Both the slow and the fast upsetting cases show the
folding of the top outside surface of the billet onto the die, as well as the severe straining of the middle
of the specimen. The second figure in each series (Figure 1.3.16–3 for the slow case, Figure 1.3.16–6
for the fast case, and Figure 1.3.16–8 for the adiabatic case) shows the equivalent plastic strain in the
billet. Peak strains of around 180% occur in the center of the specimen. The third figure in each series
(Figure 1.3.16–4 for the slow case, Figure 1.3.16–7 for the fast case, and Figure 1.3.16–9 for the adiabatic
case) shows the temperature distributions, which are noticeably different between the slow and fast
upsetting cases. In the slow case there is time for the heat to diffuse (the 60% upsetting takes place
in 100 sec, on a specimen where a typical length is 10 mm), so the temperature distribution at 100 sec is
quite uniform, varying only between 180°C and 185°C through the billet. In contrast, the fast upsetting
occurs too quickly for the heat to diffuse. In this case the middle of the top surface of the specimen
remains at 0°C at the end of the event, while the center of the specimen heats up to almost 600°C. There
is no significant difference in temperatures between the fast coupled case and the adiabatic case. In
the outer top section of the billet there are differences that are a result of the severe distortion of the
elements in that region and the lack of dissipation of generated heat. The temperature in the rest of
the billet compares well. This example illustrates the advantage of an adiabatic analysis, since a good
representation of the results is obtained in about 60% of the computer time required for the fully coupled
analysis.
1.3.16–3
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
The results of the slow and fast upsetting of the billet modeled with the porous metal plasticity
model are shown in Figure 1.3.16–10 to Figure 1.3.16–15. The deformed configuration is identical to
that of Figure 1.3.16–2 and Figure 1.3.16–5. The extent of growth/closure of the voids in the specimen at
the end of the analysis is shown in Figure 1.3.16–10 and Figure 1.3.16–13. The porous material is almost
fully compacted near the center of the billet because of the compressive nature of the stress field in that
region; on the other hand, the corner element is folded up and stretched out near the outer top portion
of the billet, increasing the void volume fraction to almost 0.1 (or 10%) and indicating that tearing of
the material is likely. The equivalent plastic strain is shown in Figure 1.3.16–11 (slow upsetting) and
Figure 1.3.16–14 (fast upsetting) for the porous material; Figure 1.3.16–12 and Figure 1.3.16–15 show
the temperature distribution for the slow and the fast upsetting of the porous metal. The porous metal
needs less external work to achieve the same deformation compared to a fully dense metal. Consequently,
there is less plastic work being dissipated as heat; hence, the temperature increase is not as much as that
of fully dense metal. This effect is more pronounced in the fast upsetting problem, where the specimen
heats up to only 510°C, compared to about 600°C for fully dense metal.
Figure 1.3.16–16 to Figure 1.3.16–18 show predictions of total upsetting force versus displacement
of the die. In Figure 1.3.16–16 the slow upsetting viscoplastic and porous plasticity results are
compared with several elastic-plastic and rigid-plastic results that were collected by Lippmann (1979)
and slow viscoplastic results obtained by Taylor (1981). There is general agreement between all the
rate-independent results, and these correspond to the slow viscoplastic results of the present example
and of those found by Taylor (1981). In Figure 1.3.16–17 rate dependence of the yield stress is
investigated. The fast viscoplastic and porous plasticity results show significantly higher force values
throughout the event than the slow results. This effect can be estimated easily. A nominal strain
rate of 6 sec is maintained throughout the event. With the viscoplastic model that is used, this effect
increases the yield stress by 68%. This factor is very close to the load amplification factor that appears
in Figure 1.3.16–17. Figure 1.3.16–18 shows that the force versus displacement prediction of the fast
viscoplastic adiabatic analysis agrees well with the fully coupled results.
Two cases using an element-based rigid surface to model the die are also considered in
Abaqus/Standard. To define the element-based rigid surface, the elements are assigned to rigid bodies
using an isothermal rigid body constraint. The results agree very well with the case when the analytical
rigid surface is used.
The automatic load incrementation results suggest that overall nominal strain increments of about
2% per increment were obtained, which is slightly better than what was anticipated in the initial time
increment suggestion. These values are typical for problems of this class and are useful guidelines for
estimating the computational effort required for such cases.
The results obtained with Abaqus/Explicit compare well with those obtained with Abaqus/Standard,
as illustrated in Figure 1.3.16–19, which compares the results obtained with Abaqus/Explicit (without
adaptive meshing) for the total upsetting force versus the displacement of the die against the same
results obtained with Abaqus/Standard. The agreement between the two solutions is excellent. Similar
agreement is obtained with the results obtained from the Abaqus/Explicit simulation using adaptive
meshing. The mesh distortion is significantly reduced in this case, as illustrated in Figure 1.3.16–20.
1.3.16–4
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
Input files
Abaqus/Standard input files
cylbillet_cax4t_slow_dense.inp
cylbillet_cax4t_fast_dense.inp
cylbillet_cax4rt_slow_dense.inp
cylbillet_cax4rt_fast_dense.inp
cylbillet_cax8rt_slow_dense.inp
cylbillet_cax8rt_rb_s_dense.inp
cylbillet_cax8rt_fast_dense.inp
cylbillet_cax8rt_slow_por.inp
cylbillet_cax8rt_fast_por.inp
cylbillet_cgax4t_slow_dense.inp
cylbillet_cgax4t_fast_dense.inp
cylbillet_cgax4t_rb_f_dense.inp
cylbillet_cgax4t_rb_f_dense_surf.inp
cylbillet_cgax8rt_slow_dense.inp
cylbillet_cgax8rt_fast_dense.inp
cylbillet_c3d10m_adiab_dense.inp
cylbillet_c3d10m_adiab_dense_surf.inp
Slow upsetting case with 144 CAX4T elements, using the
fully dense material.
Fast upsetting case with 144 CAX4T elements, using the
fully dense material.
Slow upsetting case with 144 CAX4RT elements, using
the fully dense material.
Fast upsetting case with 144 CAX4RT elements, using the
fully dense material.
Slow upsetting case with CAX8RT elements, using the
fully dense material.
Slow upsetting case with CAX8RT elements, using the
fully dense material and an element-based rigid surface
for the die.
Fast upsetting case with CAX8RT elements, using the
fully dense material.
Slow upsetting case with CAX8RT elements, using the
porous material.
Fast upsetting case with CAX8RT elements, using the
porous material.
Slow upsetting case with 144 CGAX4T elements, using
the fully dense material.
Fast upsetting case with 144 CGAX4T elements, using
the fully dense material.
Fast upsetting case with 144 CGAX4T elements, using
the fully dense material and an element-based rigid
surface for the die.
Fast upsetting case with 144 CGAX4T elements, using
the fully dense material and an element-based rigid
surface for the die with surface-to-surface contact.
Slow upsetting case with CGAX8RT elements, using the
fully dense material.
Fast upsetting case with CGAX8RT elements, using the
fully dense material.
Adiabatic static analysis with fully dense material
modeled with C3D10M elements.
Adiabatic static analysis with fully dense material
modeled with C3D10M elements using surface-tosurface contact.
1.3.16–5
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
cylbillet_c3d10m_adiab_dense_po.inp
cylbillet_cax6m_adiab_dense.inp
cylbillet_cax8r_adiab_dense.inp
cylbillet_postoutput.inp
cylbillet_slow_usr_umat_umatht.inp
cylbillet_slow_usr_umat_umatht.f
*POST OUTPUT analysis of
cylbillet_c3d10m_adiab_dense.inp.
Adiabatic static analysis with fully dense material
modeled with CAX6M elements.
Adiabatic static analysis with fully dense material
modeled with CAX8R elements.
*POST OUTPUT analysis using the fully dense material.
Slow upsetting case with the material behavior defined in
user subroutines UMAT and UMATHT.
User subroutines UMAT and UMATHT used in
cylbillet_slow_usr_umat_umatht.inp.
Abaqus/Explicit input files
cylbillet_x_cax4rt_slow.inp
cylbillet_x_cax4rt_fast.inp
cylbillet_x_cax4rt_slow_adap.inp
cylbillet_x_cax4rt_fast_adap.inp
cylbillet_xp_cax4rt_fast.inp
Slow upsetting case with fully dense material modeled
with CAX4RT elements and without adaptive meshing;
kinematic mechanical contact.
Fast upsetting case with fully dense material modeled
with CAX4RT elements and without adaptive meshing;
kinematic mechanical contact.
Slow upsetting case with fully dense material modeled
with CAX4RT elements and with adaptive meshing;
kinematic mechanical contact.
Fast upsetting case with fully dense material modeled
with CAX4RT elements and with adaptive meshing;
kinematic mechanical contact.
Fast upsetting case with fully dense material modeled
with CAX4RT elements and without adaptive meshing;
penalty mechanical contact.
References
•
•
Lippmann, H., Metal Forming Plasticity, Springer-Verlag, Berlin, 1979.
Taylor, L. M., “A Finite Element Analysis for Large Deformation Metal Forming Problems
Involving Contact and Friction,” Ph.D. Thesis, U. of Texas at Austin, 1981.
1.3.16–6
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
Portion modeled
30 mm
20 mm
Figure 1.3.16–1
Axisymmetric upsetting example: geometry and mesh (element type CAX8RT).
1.3.16–7
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
U
MAG. FACTOR = +1.0E+00
SOLID LINES - DISPLACED MESH
DASHED LINES - ORIGINAL MESH
2
1
Figure 1.3.16–2 Deformed configuration at 60% upsetting: slow
case, coupled temperature-displacement analysis, Abaqus/Standard.
PEEQ
VALUE
+9.55E-03
+2.33E-01
+4.56E-01
+6.80E-01
+9.04E-01
+1.12E+00
+1.35E+00
+1.57E+00
+1.79E+00
+2.02E+00
+2.24E+00
Figure 1.3.16–3 Plastic strain at 60% upsetting: slow case, coupled
temperature-displacement analysis, Abaqus/Standard.
NT11
VALUE
+0.00E-00
+1.80E+02
+1.80E+02
+1.80E+02
+1.81E+02
+1.81E+02
+1.82E+02
+1.82E+02
+1.82E+02
+1.83E+02
+1.83E+02
Figure 1.3.16–4 Temperature at 60% upsetting: slow case, coupled
temperature-displacement analysis, Abaqus/Standard.
1.3.16–8
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
U
MAG. FACTOR = +1.0E+00
SOLID LINES - DISPLACED MESH
DASHED LINES - ORIGINAL MESH
2
1
Figure 1.3.16–5 Deformed configuration at 60% upsetting: fast
case, coupled temperature-displacement analysis, Abaqus/Standard.
PEEQ
VALUE
+3.56E-02
+2.43E-01
+4.50E-01
+6.58E-01
+8.66E-01
+1.07E+00
+1.28E+00
+1.48E+00
+1.69E+00
+1.90E+00
+2.11E+00
Figure 1.3.16–6 Plastic strain at 60% upsetting: fast case, coupled
temperature-displacement analysis, Abaqus/Standard.
NT11
VALUE
-1.58E+01
+4.48E+01
+1.05E+02
+1.66E+02
+2.26E+02
+2.87E+02
+3.48E+02
+4.08E+02
+4.69E+02
+5.30E+02
+5.90E+02
Figure 1.3.16–7 Temperature at 60% upsetting: fast case, coupled
temperature-displacement analysis, Abaqus/Standard.
1.3.16–9
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
PEEQ
VALUE
+1.38E-03
+2.16E-01
+4.32E-01
+6.47E-01
+8.62E-01
+1.07E+00
+1.29E+00
+1.50E+00
+1.72E+00
+1.93E+00
+2.15E+00
2
3
1
Figure 1.3.16–8 Plastic strain at 60% upsetting: fast case,
adiabatic stress analysis, Abaqus/Standard.
TEMP
VALUE
-2.09E+01
+5.66E+01
+1.34E+02
+2.11E+02
+2.89E+02
+3.66E+02
+4.44E+02
+5.21E+02
+5.99E+02
+6.76E+02
+7.54E+02
2
3
1
Figure 1.3.16–9 Temperature at 60% upsetting: fast case,
adiabatic stress analysis, Abaqus/Standard.
1.3.16–10
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
VVF
VALUE
-7.50E-02
+2.22E-16
+1.47E-02
+2.94E-02
+4.42E-02
+5.89E-02
+7.37E-02
+8.84E-02
+1.03E-01
+1.17E-01
Figure 1.3.16–10
Void volume fraction at 60% upsetting: porous material, slow coupled
temperature-displacement analysis, Abaqus/Standard.
PEEQ
VALUE
+2.38E-03
+1.94E-01
+3.87E-01
+5.79E-01
+7.72E-01
+9.64E-01
+1.15E+00
+1.34E+00
+1.54E+00
+1.73E+00
Figure 1.3.16–11 Plastic strain at 60% upsetting: porous material,
slow coupled temperature-displacement analysis, Abaqus/Standard.
NT11
VALUE
+1.74E+02
+1.74E+02
+1.75E+02
+1.75E+02
+1.76E+02
+1.76E+02
+1.76E+02
+1.77E+02
+1.77E+02
+1.77E+02
Figure 1.3.16–12 Temperature at 60% upsetting: porous material,
slow coupled temperature-displacement analysis, Abaqus/Standard.
1.3.16–11
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
VVF
VALUE
-6.66E-02
+2.22E-16
+1.26E-02
+2.52E-02
+3.79E-02
+5.05E-02
+6.32E-02
+7.58E-02
+8.84E-02
+1.01E-01
Figure 1.3.16–13 Void volume fraction at 60% upsetting: porous material, fast coupled
temperature-displacement analysis, Abaqus/Standard.
PEEQ
VALUE
+3.85E-04
+1.95E-01
+3.90E-01
+5.85E-01
+7.79E-01
+9.74E-01
+1.16E+00
+1.36E+00
+1.55E+00
+1.75E+00
Figure 1.3.16–14 Plastic strain at 60% upsetting: porous material,
fast coupled temperature-displacement analysis, Abaqus/Standard.
NT11
VALUE
-2.73E+00
+5.46E+01
+1.12E+02
+1.69E+02
+2.26E+02
+2.84E+02
+3.41E+02
+3.98E+02
+4.56E+02
+5.13E+02
Figure 1.3.16–15 Temperature at 60% upsetting: porous material,
fast coupled temperature-displacement analysis, Abaqus/Standard.
1.3.16–12
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
1600
Slow case, viscoplastic
Slow case, porous plasticity
Taylor (1981), viscoplastic
upper, viscoplastic
lower, viscoplastic
Lippmann (1979)
upper, rigid-plastic
1400
1200
lower, rigid-plastic
⎫
⎬
⎭
Total force, kN
1000
800
600
400
200
0
Figure 1.3.16–16
1
2
3
4
5
6
Deflection, mm
8
9
10
Force-deflection response for slow cylinder upsetting, Abaqus/Standard.
1.3.16–13
Abaqus Version 6.12 ID:
Printed on:
7
CYLINDRICAL BILLET
1600
1400
Fast case ⎫
⎬ viscoplastic
Slow case ⎭
1200
Fast case ⎫
⎬ porous plasticity
Slow case ⎭
Total force, kN
1000
800
600
400
200
0
Figure 1.3.16–17
1
2
3
4
5
6
Deflection, mm
8
9
10
Rate dependence of the force-deflection response, Abaqus/Standard.
1.3.16–14
Abaqus Version 6.12 ID:
Printed on:
7
CYLINDRICAL BILLET
1600
1400
⎫
Fast case
⎬ viscoplastic
Adiabatic fast case ⎭
1200
Total force, kN
1000
800
600
400
200
0
1
2
3
4
5
6
Deflection, mm
7
8
9
10
Figure 1.3.16–18 Force-deflection response: adiabatic versus
fully coupled analysis, Abaqus/Standard.
1.3.16–15
Abaqus Version 6.12 ID:
Printed on:
CYLINDRICAL BILLET
Explicit
Explicit
Standard
Standard
Figure 1.3.16–19
(fast)
(slow)
(fast)
(slow)
Force-deflection response: Abaqus/Explicit versus Abaqus/Standard.
Figure 1.3.16–20 Deformed configuration at 60% upsetting: slow case, Abaqus/Explicit
(without adaptive meshing, left; with adaptive meshing, right).
1.3.16–16
Abaqus Version 6.12 ID:
Printed on:
METAL SHEET
1.3.17
UNSTABLE STATIC PROBLEM: THERMAL FORMING OF A METAL SHEET
Product: Abaqus/Standard
This example demonstrates the use of automatic contact stabilization to avoid unstable static problems.
Geometrically nonlinear static problems can become unstable for a variety of reasons. Instability may occur
in contact problems, either because of chattering or because contact intended to prevent rigid body motions
is not established initially. Localized instabilities can also occur; they can be either geometrical, such as
local buckling, or material, such as material softening.
This problem models the thermal forming of a metal sheet; the shape of the die may make it difficult to
place the undeformed sheet exactly in initial contact, in which case the initial rigid body motion prevention
algorithm is useful. Metal forming problems are characterized by relatively simply shaped parts being
deformed by relatively complex-shaped dies. The initial placement of the workpiece on a die or the initial
placement of a second die may not be a trivial geometrical exercise for an engineer modeling the forming
process. Abaqus accepts initial penetrations in contact pairs and instantaneously tries to resolve them; as
long as the geometry allows for this to happen without excessive deformation, the misplacement of the
workpiece usually does not cause problems. On the other hand, if the workpiece is initially placed away
from the dies, serious convergence problems may arise. Unless there are enough boundary conditions
applied or a stabilization method is used, singular finite element systems of equations result because one
or more of the bodies has free rigid body motions. This typically arises when the deformation is applied
through loads instead of boundary conditions. Contact stabilization can be helpful for avoiding convergence
problems while contact is established without significantly influencing the results of interest (see “Automatic
stabilization of rigid body motions in contact problems” in “Adjusting contact controls in Abaqus/Standard,”
Section 35.3.6 of the Abaqus Analysis User’s Manual).
This example looks at the thermal forming of an aluminum sheet. The deformation is produced by
applying pressure and gravity loads to push the sheet against a sculptured die. The deformation is initially
elastic. Through heating, the yield stress of the material is lowered until permanent plastic deformations are
produced. Subsequently, the assembly is cooled and the pressure loads are removed, leaving a formed part
with some springback. Although the sheet is initially flat, the geometrical nature of the die makes it difficult
to determine the exact location of the sheet when it is placed on the die. Therefore, an initial gap between the
two bodies is modeled, as shown in Figure 1.3.17–1.
Geometry and model
The model consists of a trapezoidal sheet 10.0 m (394.0 in) long, tapering from 2.0 m (78.75 in) to 3.0 m
(118.0 in) wide, and 10.0 mm (0.4 in) thick. The die is a ruled surface controlled by two circles of
radii 13.0 m (517.0 in) and 6.0 m (242.0 in) and dimensions slightly larger than the sheet. The sheet is
initially placed over 0.2 m (7.9 in) apart from the die. The sheet has a longitudinal symmetry boundary
condition, and one node prevents the remaining nodes from experiencing in-plane rigid body motion.
The die is fixed throughout the analysis. The sheet mesh consists of 640 S4R shell elements, while the
die is represented by 640 R3D4 rigid elements. The material is an aluminum alloy with a flow stress of
1.0 × 108 Pa (14.5 ksi) at room temperature. A flow stress of 1.0 × 103 Pa (0.15 psi) at 400°C is also
1.3.17–1
Abaqus Version 6.12 ID:
Printed on:
METAL SHEET
provided, essentially declaring that at the higher temperature the material will flow plastically at any
stress. A Coulomb friction coefficient of 0.1 is used to model the interaction between the sheet and die.
Results and discussion
The analysis consists of three steps. In the first step a gravity load and a pressure load of 1.0 × 105 Pa
(14.5 psi) are applied, both pushing the sheet against the die. This step is aided by contact stabilization
to prevent unrestrained motion of the sheet prior to establishing contact with the die. In this case,
contact stabilization normal to the nearby contact surfaces provides adequate stabilization. Avoiding
tangential contact stabilization is recommended, if possible, because tangential contact stabilization
is more likely to influence solution variables. The clearance distance range over which the contact
stabilization is effective has been specified in this example such that contact stabilization is active for
the initial separation distance between the sheet and die. Abaqus ramps down the contact stabilization
such that no contact stabilization remains at the end of the first step. This guarantees that the viscous
forces decrease to zero, thus avoiding any discontinuity in the forces at the start of the next step. The
shape and relatively low curvatures of the die are such that the deformation at the end of the step is
elastic (Figure 1.3.17–2). In the second step a two-hour heating (from room temperature to 360°C)
and cooling (back to 50°C) cycle is applied to the loaded assembly. As a result of the decrease in flow
stress permanent (plastic) deformation develops, as shown in Figure 1.3.17–3. Finally, in the third step
the pressure load is removed and the springback of the deformed sheet is calculated, as depicted in
Figure 1.3.17–4.
Acknowledgments
SIMULIA would like to thank British Aerospace Airbus, Ltd. for providing the basic data from which
this example was derived.
Input files
unstablestatic_forming.inp
unstablestatic_forming_surf.inp
Thermal forming model.
Thermal forming model with surface-to-surface contact.
1.3.17–2
Abaqus Version 6.12 ID:
Printed on:
METAL SHEET
Figure 1.3.17–1
Figure 1.3.17–2
Initial placement of the sheet apart from the die.
Elastic deformation after gravity and pressure loading.
1.3.17–3
Abaqus Version 6.12 ID:
Printed on:
METAL SHEET
PEEQ
SNEG, (fraction = -1.0)
(Ave. Crit.: 75%)
+6.757e-02
+5.000e-03
+4.286e-03
+3.571e-03
+2.857e-03
+2.143e-03
+1.429e-03
+7.143e-04
+0.000e+00
Figure 1.3.17–3
Permanent deformation produced by heating.
U, U3
-2.097e-01
-2.186e-01
-2.275e-01
-2.364e-01
-2.454e-01
-2.543e-01
-2.632e-01
-2.721e-01
-2.810e-01
-2.899e-01
-2.988e-01
Figure 1.3.17–4
Springback.
1.3.17–4
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
1.3.18
INERTIA WELDING SIMULATION USING Abaqus/Standard AND Abaqus/CAE
Products: Abaqus/Standard
Abaqus/CAE
Objectives
This example demonstrates the following Abaqus features:
•
•
thermal-mechanical coupling for inertia welding simulation,
•
•
•
defining a complex friction law in a user subroutine,
semi-automatic remeshing using Python scripting and output database scripting methods for
extracting deformed configurations,
flywheel loading through user subroutine definitions, and
combining and presenting results from a sequence of output database (.odb) files.
Application description
This example examines the inertia friction welding process of the pipes shown in Figure 1.3.18–1. The
specific arrangement considered is the resulting as-welded configuration shown in Figure 1.3.18–2. In
this weld process kinetic energy is converted rapidly to thermal energy at a frictional interface. The
resulting rapid rise in interface temperature is exploited to produce high-quality welds. In this example
the weld process is simulated, and the initial temperature rise and material plastic flow are observed. An
important factor in the process design is control of the initial speed of the flywheel so that, when the
flywheel stops, the temperature rises to just below the melting point, which in turn results in significant
flow of material in the region of the weld joint. Understanding the friction, material properties, and
heat transfer environment are important design aspects in an effective inertia welding process; therefore,
simulation is a helpful tool in the process design.
Geometry
The weld process in this example is shown in Figure 1.3.18–1, where two pipes are positioned for girthweld joining. The two pipes are identical, each with a length of 21.0 mm, an inside radius of 42.0 mm,
and an outside radius of 48.0 mm. The pipes are adjacent, touching each other initially at the intended
weld interface.
Materials
The pipes are made of Astroloy, a high-strength alloy used in gas turbine components. Figure 1.3.18–3
shows flow stress curves as a function of temperature and plastic strain rate. At temperatures relevant to
the welding process, the material is highly sensitive to plastic strain rate and temperature. Specific heat
is a function of temperature, as shown in Figure 1.3.18–4.
1.3.18–1
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
Other material properties are defined as follows:
Young’s modulus:
Poisson’s ratio:
Density:
Conductivity:
180,000 MPa
0.3
7.8 × 10−9 Mg/mm3
14.7 W/m/°C at 20°C
28 W/m/°C at 1200°C
Initial conditions
The pipes are initially set at 20°C, representing room temperature.
Boundary conditions and loading
A pressure of 360 MPa is applied to the top surface of the upper pipe. The initial rotational velocity
of the flywheel is set at 48.17 rad/s, or 7.7 revolutions per second. The mass moment of inertia of the
flywheel is 102,000 Mg mm2 .
Interactions
The principal interaction occurs at the weld interface between the pipes; however, a secondary concern
is the possibility of contact of weld flash with the side of the pipes. The weld-interface friction behavior
is assumed to follow that described by Moal and Massoni (1995), where the ratio of shear stress to the
prescribed pressure is observed to be a complex function of interface slip rate. The heat generation from
the frictional sliding, combined with plastic deformation, contributes to the temperature rise in the pipes.
Abaqus modeling approaches and simulation techniques
Abaqus/CAE and Abaqus/Standard are used together to affect the weld simulation in a way that permits
extreme deformation of the pipes in the weld region. This process is automated through the use of Python
scripts. Three cases are studied in this example.
Summary of analysis cases
Case 1
Initial flywheel velocity = 48.17 rad/s. This case produces a successful weld.
Case 2
Initial flywheel velocity = 20.0 rad/s. This case illustrates an unsuccessful weld
scenario; the flywheel has insufficient energy to begin the weld process.
Case 3
Initial flywheel velocity = 70.0 rad/s. This case illustrates an unsuccessful weld
scenario; the flywheel has excessive energy, resulting in a temperature rise into the
liquidus regime of the pipe material.
The following sections discuss analysis considerations that are applicable to all the cases. Python
scripts that generate the model databases and Abaqus/Standard input files are provided for Case 1, with
instructions in the scripts for executing the Case 2 and Case 3 simulations.
1.3.18–2
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
Analysis types
The analysis is nonlinear, quasi-static with thermal-mechanical coupling. A fully coupled temperaturedisplacement procedure is used.
Analysis techniques
The key feature required for successful simulation of this process is remeshing. In this example,
because of the large deformation near the weld region, multiple analyses are employed to limit element
distortion. These analyses are executed in sequence, with remeshing performed between executions,
and are automated through the use of Python scripts.
At each remesh point the current model configuration represents a significant change in the pipes’
shape and in the current analysis mesh. Abaqus/CAE is used to extract the outer surface of the pipes,
reseed the surface, and remesh the pipe regions. This process employs the Abaqus Scripting Interface
PartFromOdb command, which is used to extract orphan mesh parts representing the deformed pipes.
These parts are then passed to the Part2DGeomFrom2DMesh command. This command creates a
geometric Part object from the orphan mesh imported earlier. Once the profile of the deformed part
has been created, options in the Mesh module are used to remesh the part. The new mesh results in a
new Abaqus/Standard analysis, and the map solution procedure maps state variables from the previous
analysis (see “Mesh-to-mesh solution mapping,” Section 12.4.1 of the Abaqus Analysis User’s Manual).
Mesh design
The pipes are modeled as axisymmetric. The element formulation used is the fully coupled
temperature-displacement axisymmetric elements with twist degrees of freedom (element types
CGAX4HT and CGAX3HT), where the twist degree of freedom enables modeling of rotation and
shear deformation in the out-of-plane direction. The hybrid formulation is required to handle the
incompressible nature of the material during the plastic flow. The mesh is divided into two regions for
each pipe. In the region near the weld interface, smaller elements are created (see Figure 1.3.18–5).
During the remeshing process, the region near the weld surface is recalculated so that the new flash
region is also meshed with smaller elements (see Figure 1.3.18–6).
Material model
The material model defined for this example approximates the high-temperature behavior of Astroloy,
where it is reported by Soucail et al. (1992) using a Norton-Hoff constitutive law to describe
the temperature and strain-rate viscoplastic behavior. A similar model is defined in Abaqus as a
rate-dependent perfectly plastic material model. For the loading in this model, these material parameters
result in the onset of local plastic flow only after the interface temperature has exceeded roughly
1200°C, near the material solidus temperature of 1250°C. Above this temperature the Mises flow stress
is highly sensitive to variations in temperature and strain rate. A special adjustment in the flow stress
at high strain rates is necessary to avoid divergence during the iteration procedure of the nonlinear
solution. In the material model definition an extreme case of stress data is defined when the strain rate
is 1.0 × 106 s−1 . Stress data when the strain rate equals zero are also defined to be the same as the stress
1.3.18–3
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
data at strain rate 1.0 × 10−5 s−1 . As a result of large deformation, thermal expansion is not considered
in the material model.
It is assumed that 90% of the inelastic deformation energy contributes to the internal heat generation,
which is the Abaqus default for inelastic heat fraction.
Initial conditions
An initial temperature of 20°C is specified for the entire model. The flywheel initial velocity is specified
as a solution-dependent variable initial condition for the user element (see inertiaweld_sub.f).
Boundary conditions
The bottom pipe is fixed completely. The top pipe is free of boundary conditions.
Loading
A pressure of 360 MPa is applied as a distributed load on the top surface of the upper pipe.
The heat flux resulting from frictional heat generation is considered to be many times greater than
any heat lost due to convection. Thus, all boundaries are assumed to be adiabatic.
Interactions
Five interactions are defined: four contact interactions and one actuator-sensor interaction.
The contact interactions include a pair of interactions that define the weld interface between the
pipes, which is identified in Figure 1.3.18–1. This pair of interactions is symmetrical: one interaction
defines the top pipe as the master surface with the bottom pipe as the slave surface, and the second
interaction reverses the master-slave pairing. This “balanced master-slave” arrangement is important for
the analysis to obtain more uniform contact pressure in the weld interface and to avoid hourglass effects,
and it is combined with a softened contact interaction property to promote a sharing of the local contact
pressure among nodes on both sides of the interface.
To simulate the Moal and Massoni (1995) friction definition, the weld interface friction model is
defined in user subroutine FRIC (see inertiaweld_sub.f). This model is nonlocal in the sense that the
interface pressure for all contact nodes is the applied pressure of 360 MPa, and the sliding velocity is
computed based on the rotational angular velocity of the flywheel. This treatment of the friction force
helps stabilize the solution. Frictional heat generation is calculated based on the frictional traction and
the sliding velocity. Nondefault contact controls definitions are used to improve convergence. These
definitions include delaying the friction computation upon contact and automatic tolerance control to
avoid contact chattering.
The two remaining contact interactions address the possibility of self-contact near the weld
area in the pipes. Self-contact in the flash area can cause problems during remeshing: the
Part2DGeomFrom2DMesh command that was used to generate the new, current configuration
geometry performs curve-fit operations that can result in self intersections of the boundary, which lead
to invalid part topology and a meshing failure. To avoid this problem, a softened contact model that
introduces a normal pressure with a small separation distance (−0.01 mm) is used. It is important to
keep this separation distance as small as practical to avoid causing any nonphysical contact behavior.
1.3.18–4
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
The actuator-sensor interaction, which acts through user subroutine UEL, enables the simulation of
a flywheel attached to the top pipe. The user element also has a sensor role in the analysis, measuring
the weld upset, or axial shortening, of the weld assembly. When a critical user-defined upset distance
is exceeded, the user element subroutine calls XIT to terminate the analysis and signal a remesh point.
This parameter, the allowed “upset distance,” correlates well with the extent of mesh deformation in the
weld region.
Analysis steps
Each of the analyses run in the simulation sequence uses a single fully coupled temperature-displacement
step. Since the duration of the step is controlled by the user element, as described above, it is not known
a priori for each analysis. Therefore, the step duration is set in each analysis to be the total remaining
time for the simulation, a time that is reached only in the final analysis in the simulation sequence.
Solution controls
Full Newton iteration is used for the nonlinear solution. Automatic time stepping is based on the
maximum temperature change in each increment. Results from the previous increment are used as the
initial guess in the current increment, with the parabolic extrapolation technique adopted to transfer the
previous state to the current state.
Heat fluxes due to frictional heat generation can cause contact chattering. To overcome this
difficulty, contact controls with the automatic tolerances parameter are used.
Output requests
Field output of temperature, stress, and equivalent plastic strain is requested. Various energy measures
are requested for history output, allowing you to record the flywheel energy change during the simulation.
Convergence
In general, convergence is difficult in the initial increments, especially after remeshing. More iterations
are also observed near the end of the analysis-run sequence when deformation increases and the mesh
distortion becomes severe.
Run procedure
This example is run using the Abaqus/CAE Python scripts provided. Use the following command to run
the example:
abaqus cae –script inertiaweld.py
The simulation results in a sequence of separate output database (.odb) files, each corresponding to one
of the analyses.
For postprocessing convenience a number of scripts are provided for evaluating
simulation results across the sequence of files.
Use the following command to create the
inertia_weld_animation.avi animation file:
abaqus cae –script inertiaweld_movie.py
1.3.18–5
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
Run the following Python scripts to create X–Y plots:
•
•
•
inertiaweld_xy.py, for a history plot of energy results.
inertiaweld_upset.py, for a history plot of assembly upset.
inertiaweld_maxtemp.py, for a history plot of the maximum temperature.
Discussion of results and comparison of cases
This example focuses mainly on the successful weld case, Case 1. Case 2 and Case 3 are provided to
show the precarious nature of the inertia weld process, where it is essential to select the flywheel size
correctly, measured by the mass moment of inertia, and the initial velocity of the flywheel. Case 2 and
Case 3 illustrate why simulation is a valuable tool in the weld process design as each case clearly shows
that the selected process parameters do not result in a successful weld.
Welding success: Case 1
The example simulation creates multiple output database (.odb) files, requiring 22 remeshings to reach
the simulation time of 5.0 seconds. The results in the first analysis before the first remeshing show that the
temperature rises very fast near the weld interface. At about 1.6 seconds the temperature reaches 1172°C
and the material starts to flow, squeezing out to form flash (see Figure 1.3.18–7). After 2.31 seconds
and 5 remeshings the flash extends enough to fold back and contact the pipe (see Figure 1.3.18–8). At
3.51 seconds the flywheel velocity slows down to 3.51 rad/s, the temperature starts to drop, and the
material flow slows down. At this point a considerable amount of flash build-up can be observed (see
Figure 1.3.18–9). After 5.0 seconds the flywheel stops, the temperature drops below 1000°C, and the
pipes are welded (see Figure 1.3.18–10).
The flash prediction in Figure 1.3.18–11 is in good agreement with those shown by Moal and
Massoni (1995). Figure 1.3.18–12 plots the kinetic energy history (created with inertiaweld_xy.py)
and shows how the flywheel slows down and stops. The “RemeshPoints” marks indicate the time at
which the remeshing procedure occurred. The upset distance during the welding process is shown in
Figure 1.3.18–13 (created with inertiaweld_upset.py). The curve of the maximum temperature for Case
1 is plotted in Figure 1.3.18–14 (created with inertiaweld_maxtemp.py).
Insufficient flywheel energy: Case 2
If a lower initial flywheel velocity is selected, the temperature may not reach a level high enough for
the material to flow. For this case the initial velocity is reduced to 20 rad/s. Figure 1.3.18–15 shows
the configuration at 5.0 seconds, where not much deformation is observed and the temperature near the
interface is about 250°C. The history plot of the maximum temperature for Case 2 in Figure 1.3.18–14
shows the pipe temperature reaches only 700°C about 1.1 seconds before it cools down. In this case the
material is not hot enough to initiate the material flow, and welding will not be successful.
Excessive flywheel energy: Case 3
If a higher initial velocity of the flywheel is selected, the material becomes so hot that it starts to melt. For
this case the initial velocity of the flywheel is set at 70 rad/s. Figure 1.3.18–16 shows that the temperature
rapidly reaches 1360°C (at about 0.9 seconds), which is well beyond the melting temperature at 1250°C,
1.3.18–6
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
before convergence failures stop the analysis. Figure 1.3.18–14 shows the history plot of the maximum
temperature in the pipes for Case 3. In this case the excessive energy results in melting and a failed weld.
Python scripts
inertiaweld.py
Main Python script to control model building, remeshing,
and the analyses.
Script to initialize base options for an Abaqus/Standard
analysis.
Script to define utility functions, such as applying seeds
and replacing the part after deformation.
Script to create the initial model.
Script to provide control parameters and input data, such
as mesh size and simulation time.
Script to create a remeshed model and provide input files
for restart.
Script to create an animation of this welding simulation.
Script to create an X–Y plot of flywheel kinetic energy
history.
Script to create an X–Y plot of the upset history.
Script to create an X–Y plot of the maximum temperature
history during the welding process.
inertiaweld_solver_param.py
inertiaweld_utils.py
inertiaweld_original_build.py
inertiaweld_job_param.py
inertiaweld_remesh_build.py
inertiaweld_movie.py
inertiaweld_xy.py
inertiaweld_upset.py
inertiaweld_maxtemp.py
Input files
inertiaweld_sub.f
FORTRAN file containing user subroutines UEL and
FRIC.
References
Abaqus Analysis User’s Manual
•
“Mesh-to-mesh solution mapping,” Section 12.4.1 of the Abaqus Analysis User’s Manual
Abaqus Keywords Reference Manual
•
*MAP SOLUTION
Abaqus User Subroutines Reference Manual
•
•
•
“FRIC,” Section 1.1.8 of the Abaqus User Subroutines Reference Manual
“UEL,” Section 1.1.27 of the Abaqus User Subroutines Reference Manual
“Terminating an analysis,” Section 2.1.15 of the Abaqus User Subroutines Reference Manual
1.3.18–7
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
Abaqus Scripting Reference Manual
•
•
“PartFromOdb,” Section 37.1.11 of the Abaqus Scripting Reference Manual
•
Moal, A., and E. Massoni, “Finite Element Simulation of the Inertia Welding of Two Similar Parts,”
Engineering Computations, vol. 12, pp. 497–512, 1995.
•
Soucail, M., A. Moal, L. Naze, E. Massoni, C. Levaillant, and Y. Bienvenu, “Microstructural Study
and Numerical Simulation of Inertia Friction Welding of Astroloy,” 7th International Symposium
on Superalloys, Seven Springs, USA, 1992.
“Part2DGeomFrom2DMesh,” Section 37.1.14 of the Abaqus Scripting Reference Manual
Other
1.3.18–8
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
axis of rotation
top surface
rotation
direction
weld
interface
top pipe
bottom pipe
Figure 1.3.18–1
Inertia weld configuration for two pipes.
Figure 1.3.18–2 Half-section view of the inertia welding final as-welded configuration
showing the temperature fields at 5 seconds after welding begins.
1.3.18–9
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
[x1.E3]
5.0
Stress (MPa)
4.0
3.0
2.0
1.0
0.0
0.0
0.4
0.8
1.2
[x1.E3]
Temperature (C)
strain rate=1e−5
strain rate=50
strain rate=100
Figure 1.3.18–3
Flow stress curves.
Specific Heat Coefficient (Nmm/kg/C)
[x1.E9]
1.2
1.0
0.8
0.6
0.4
0.0
0.4
0.8
1.2 [x1.E3]
Temperature (C)
Specific heat coefficient
Figure 1.3.18–4
Specific heat curve (N mm/kg/°C).
1.3.18–10
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
Figure 1.3.18–5
Figure 1.3.18–6
Initial mesh.
Typical mesh design on a deformed configuration pair of parts.
1.3.18–11
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
NT11
+1.400e+03
+1.283e+03
+1.167e+03
+1.050e+03
+9.333e+02
+8.167e+02
+7.000e+02
+5.833e+02
+4.667e+02
+3.500e+02
+2.333e+02
+1.167e+02
+0.000e+00
Figure 1.3.18–7
Temperature at 1.78 sec.
NT11
+1.400e+03
+1.283e+03
+1.167e+03
+1.050e+03
+9.333e+02
+8.167e+02
+7.000e+02
+5.833e+02
+4.667e+02
+3.500e+02
+2.333e+02
+1.167e+02
+0.000e+00
Figure 1.3.18–8
Temperature at 2.31 sec.
1.3.18–12
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
NT11
+1.400e+03
+1.283e+03
+1.167e+03
+1.050e+03
+9.333e+02
+8.167e+02
+7.000e+02
+5.833e+02
+4.667e+02
+3.500e+02
+2.333e+02
+1.167e+02
+0.000e+00
Figure 1.3.18–9
Temperature at 3.51 sec.
NT11
+1.400e+03
+1.283e+03
+1.167e+03
+1.050e+03
+9.333e+02
+8.167e+02
+7.000e+02
+5.833e+02
+4.667e+02
+3.500e+02
+2.333e+02
+1.167e+02
+0.000e+00
Figure 1.3.18–10
Temperature at 5.0 sec.
1.3.18–13
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
Time = 2.0 s
Time = 2.5 s
Time = 2.9 s
Time = 3.4 s
Time = 3.5 s
Time = 5.0 s
Figure 1.3.18–11
Flash prediction in current analysis.
1.3.18–14
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
Energy/Work (Newton−mm)
[x1.E9]
0.12
0.10
0.08
0.06
0.04
0.02
0.00
0.0
1.0
2.0
3.0
4.0
5.0
Time (s)
External work: ALLWK for Whole Model
Kinetic energy: ALLKE for Whole Model
RemeshPoints
Figure 1.3.18–12
Kinetic energy history showing the flywheel slowdown.
5.0
Axial shortening (mm)
4.0
3.0
2.0
1.0
0.0
0.0
1.0
2.0
3.0
4.0
5.0
Time (s)
Upset
RemeshPoints
Figure 1.3.18–13
Assembly upset (shortening) history.
1.3.18–15
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
1400.
Maximum Temperature (C)
1200.
1000.
800.
600.
400.
200.
0.
0.0
1.0
2.0
3.0
4.0
5.0
Time (s)
maxTemp − Case 1
maxTemp − Case 2
maxTemp − Case 3
RemeshPoints
Figure 1.3.18–14 Maximum temperature history comparisons of the three cases. Case 1: Successful weld;
Case 2: Failed weld with insufficient flywheel energy; Case 3: Failed weld with excessive flywheel energy.
NT11
+1.400e+03
+1.283e+03
+1.167e+03
+1.050e+03
+9.333e+02
+8.167e+02
+7.000e+02
+5.833e+02
+4.667e+02
+3.500e+02
+2.333e+02
+1.167e+02
+0.000e+00
Figure 1.3.18–15
Temperature distribution at 5.0 sec for Case 2 (insufficient flywheel energy for welding).
1.3.18–16
Abaqus Version 6.12 ID:
Printed on:
INERTIA WELDING
NT11
+1.400e+03
+1.283e+03
+1.167e+03
+1.050e+03
+9.333e+02
+8.167e+02
+7.000e+02
+5.833e+02
+4.667e+02
+3.500e+02
+2.333e+02
+1.167e+02
+0.000e+00
Figure 1.3.18–16 Temperature distribution at 0.9 sec for Case 3 (excessive initial flywheel
energy results in a rapid temperature rise into the melting regime).
1.3.18–17
Abaqus Version 6.12 ID:
Printed on:
FRACTURE AND DAMAGE
1.4
Fracture and damage
•
•
•
“A plate with a part-through crack: elastic line spring modeling,” Section 1.4.1
•
•
•
•
•
•
“Crack growth in a three-point bend specimen,” Section 1.4.4
“Contour integrals for a conical crack in a linear elastic infinite half space,” Section 1.4.2
“Elastic-plastic line spring modeling of a finite length cylinder with a part-through axial flaw,”
Section 1.4.3
“Analysis of skin-stiffener debonding under tension,” Section 1.4.5
“Failure of blunt notched fiber metal laminates,” Section 1.4.6
“Debonding behavior of a double cantilever beam,” Section 1.4.7
“Debonding behavior of a single leg bending specimen,” Section 1.4.8
“Postbuckling and growth of delaminations in composite panels,” Section 1.4.9
1.4–1
Abaqus Version 6.12 ID:
Printed on:
CRACKED PLATE
1.4.1
A PLATE WITH A PART-THROUGH CRACK: ELASTIC LINE SPRING MODELING
Product: Abaqus/Standard
The line spring elements in Abaqus allow inexpensive evaluation of the effects of surface flaws in shell
structures, with sufficient accuracy for use in design studies. The basic concept of these elements is that they
introduce the local solution, dominated by the singularity at the crack tip, into a shell model of the uncracked
geometry. The relative displacements and rotations across the cracked section, calculated in the line spring
elements, are then used to determine the magnitude of the local strain field and hence the J-integral and stress
intensity factor values, as functions of position along the crack front. This example illustrates the use of these
elements and provides some verification of the results they provide by comparison with a published solution
and also by making use of the shell-to-solid submodeling technique.
Problem description
A large plate with a symmetric, centrally located, semi-elliptic, part-through crack is subjected to edge
tension and bending. The objective is to estimate the Mode I stress intensity factor,
, as a function
of position along the crack front. Symmetry allows one quarter of the plate to be modeled, as shown
in Figure 1.4.1–1. The 8-node shell element, S8R, and the corresponding 3-node (symmetry plane) line
spring element LS3S are used in the model.
A mesh using LS6 elements is also included. Only half-symmetry is used in this case. When LS6
elements are used, the shell elements on either side of an LS6 element must be numbered such that the
normals to these shell elements point in approximately the same direction.
Geometry and model
For each load case (tension and bending) two plate thicknesses are studied: a “thick” case, for which the
plate thickness is 76.2 mm (3.0 in); and a “thin” case, for which the plate thickness is 19.05 mm (0.75 in).
For both thicknesses the semi-elliptic crack has a maximum depth ( in Figure 1.4.1–2) of 15.24 mm
(0.6 in) and a half-length, c, of 76.2 mm (3.0 in). The plate is assumed to be square, with dimensions
609.6 × 609.6 mm (24 × 24 in).
The material is assumed to be linear elastic, with Young’s modulus 207 GPa (30 × 106 lb/in2 ) and
Poisson’s ratio 0.3.
A quarter of the plate is modeled, with symmetry along the edges of the quarter-model at
0 and
0. On the edge containing the flaw (
0), the symmetry boundary conditions are imposed only on
the unflawed segment of the edge, since they are built into the symmetry plane of the line spring element
being used (LS3S).
The loading consists of a uniform edge tension (per unit length) of 52.44 kN/m (300 lb/in) or a
uniform edge moment (per unit length) of 1335 N-m/m (300 lb-in/in).
1.4.1–1
Abaqus Version 6.12 ID:
Printed on:
CRACKED PLATE
Results and discussion
The stress intensity factors for the thick and thin plates are compared with the detailed solutions of Raju
and Newman (1979) and Newman and Raju (1979) in Figure 1.4.1–3 (tension load) and Figure 1.4.1–4
(bending load). These plots show that the present results agree reasonably well with those of Raju and
Newman over the middle portion of the flaw (
30°), with better correlation being provided for the
thick case, possibly because the crack is shallower in that geometry. The accuracy is probably adequate
for basic assessment of the criticality of the flaw for design purposes. For values of less than about 30°
(that is, at the ends of the flaw), the stress intensity values predicted by the line spring model lose accuracy.
This accuracy loss arises from a combination of the relative coarseness of the mesh, (especially in this
end region where the crack depth varies rapidly), as well as from theoretical considerations regarding
the appropriateness of line spring modeling at the ends of the crack. These points are discussed in detail
by Parks (1981) and Parks et al. (1981).
Shell-to-solid submodeling around the crack tip
An input file for the case
= 0.2, which uses the shell-to-solid submodeling capability, is included.
This C3D20R element mesh allows the user to study the local crack area using the energy domain integral
formulation for the J-integral. The submodel uses a focused mesh with four rows of elements around
the crack tip. A
singularity is utilized at the crack tip, the correct singularity for a linear elastic
solution. Symmetry boundary conditions are imposed on two edges of the submodel mesh, while results
from the global shell analysis are interpolated to two edges by using the submodeling technique. The
global shell mesh gives satisfactory J-integral results; hence, we assume that the displacements at the
submodel boundary are sufficiently accurate to drive the deformation in the submodel. No attempt has
been made to study the effect of making the submodel region larger or smaller. The submodel is shown
superimposed on the global shell model in Figure 1.4.1–5.
The variations of the J-integral values along the crack in the submodeled analysis are compared
to the line spring element analysis in Figure 1.4.1–3 (tension load) and Figure 1.4.1–4 (bending load).
Excellent correlation is seen between the three solutions. A more refined mesh in the shell-to-solid
submodel near the plate surface would be required to obtain J-integral values that more closely match
the reference solution.
Input files
crackplate_ls3s.inp
crackplate_surfaceflaw.f
crackplate_ls6_nosym.inp
crackplate_postoutput.inp
crackplate_submodel.inp
LS3S elements.
A small program used to create a data file containing the
surface flaw depths.
LS6 elements without symmetry about
0.
*POST OUTPUT analysis.
Shell-to-solid submodel.
1.4.1–2
Abaqus Version 6.12 ID:
Printed on:
CRACKED PLATE
References
•
Newman, J. C., Jr., and I. S. Raju, “Analysis of Surface Cracks in Finite Plates Under Tension or
Bending Loads,” NASA Technical Paper 1578, National Aeronautics and Space Administration,
December 1979.
•
Parks, D. M., “The Inelastic Line Spring: Estimates of Elastic-Plastic Fracture Mechanics
Parameters for Surface-Cracked Plates and Shells,” Journal of Pressure Vessel Technology,
vol. 13, pp. 246–254, 1981.
•
Parks, D. M., R. R. Lockett, and J. R. Brockenbrough, “Stress Intensity Factors for SurfaceCracked Plates and Cylindrical Shells Using Line Spring Finite Elements,” Advances in Aerospace
Structures and Materials, Edited by S. S. Wang and W. J. Renton, ASME, AD–01, pp. 279–286,
1981.
•
Raju, I. S., and J. C. Newman, Jr., “Stress Intensity Factors for a Wide Range of Semi-Elliptic
Surface Cracks in Finite Thickness Plates,” Journal of Engineering Fracture Mechanics, vol. 11,
pp. 817–829, 1979.
y
Line spring elements
x
Figure 1.4.1–1
Quarter model of large plate with center surface crack.
1.4.1–3
Abaqus Version 6.12 ID:
Printed on:
CRACKED PLATE
t
a0
φ
c
a0 = maximum flaw depth
2c = surface length of crack
t = shell thickness
φ = angle on an inscribed circle for locating a
point on the crack
Figure 1.4.1–2
Schematic surface crack geometry for a semi-elliptical crack.
1.4.1–4
Abaqus Version 6.12 ID:
Printed on:
CRACKED PLATE
KI
πa0 1/2
)
Q
σ(
t
2.0
a0
= 0.8
t
1.6
1.2
a0
= 0.2
t
0.8
a0
c = 0.2
Q = 1.1
σt = P/t
0.4
0
0.2
Figure 1.4.1–3
Raju & Newman (1979)
ABAQUS line spring (a0/t = 0.8)
ABAQUS line spring (a0/t = 0.2)
ABAQUS shell-to-solid submodel (a0/t = 0.2)
φ
π/2
0.4
0.6
0.8
1.0
Stress intensity factor dependence on crack front position: tension loading.
σ(
b
KI
πa0 1/2
)
Q
1.0
a0
= 0.2
t
0.8
0.6
a0
= 0.8
t
0.4
Figure 1.4.1–4
0.2
a0
c = 0.2
Q = 1.1
σb = 6M/t2
0
0.2
Raju & Newman (1979)
ABAQUS line spring (a0/t = 0.8)
ABAQUS line spring (a0/t = 0.2)
ABAQUS shell-to-solid submodel (a0/t = 0.2)
0.4
0.6
0.8
1.0
φ
π/2
Stress intensity factor dependence on crack front position: moment loading.
1.4.1–5
Abaqus Version 6.12 ID:
Printed on:
CRACKED PLATE
2
3
1
Figure 1.4.1–5
Solid submodel superimposed on shell global model.
1.4.1–6
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
1.4.2
CONTOUR INTEGRALS FOR A CONICAL CRACK IN A LINEAR ELASTIC INFINITE
HALF SPACE
Products: Abaqus/Standard
Abaqus/CAE
Objectives
This example demonstrates the following Abaqus features and techniques for linear elastic fracture
mechanics:
•
evaluating contour integrals for axisymmetric and three-dimensional fracture mechanics based on
linear static stress analysis;
•
partitioning steps required to generate a mesh suitable for evaluating contour integrals in two- and
three-dimensional analyses;
•
evaluating three-dimensional contour integrals when the crack extension direction varies along the
crack front;
•
node-based submodeling in fracture problems (comparing results for a single refined analysis with
the submodeling approach);
•
surface-based submodeling based on global model stresses, with guidelines for obtaining adequate
accuracy; and
•
applying continuum infinite elements simulating an infinite domain.
Application description
This example examines the fracture behavior of a conical crack, which may result from a small hard
object impacting a large brittle body. It shows how to evaluate the propensity of the crack to propagate
under static loading but does not cover the event that formed the crack.
The J-integral is a widely applied fracture mechanics parameter that relates to energy release
associated with crack growth and is a measure of the deformation intensity at a crack tip. In practice,
the calculated J-integral can be compared with a critical value for the material under consideration to
predict fracture. The T-stress represents stress parallel to the crack face. Together, the T-stress and the
J-integral provide a two-parameter fracture model describing Mode I elastic-plastic crack-tip stresses
and deformation in plane strain or three dimensions over a wide range of crack configurations and
loadings. The stress intensity factors,
, relate to the energy release rate and measure the propensity
for crack propagation.
This example uses axisymmetric and three-dimensional models to demonstrate the Abaqus fracture
mechanics capability, where the crack extension direction varies along a curved crack front. Submodeling
and the use of infinite elements to simulate far-field boundaries are also demonstrated.
1.4.2–1
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Geometry
The problem domain contains a conical crack in an infinite solid half-space, as shown in Figure 1.4.2–1.
The crack extension direction changes as the crack is swept around a circle. The units for this example
are nonphysical; therefore, dimensions, loads, and material properties are described in terms of length
and force units. The crack circumscribes a circle with a radius of 10 length units on the free surface. The
crack intersects the free surface at 45° and extends 15 length units into the solid domain.
Materials
The material is a linear elastic solid.
Boundary conditions and loading
The semi-infinite domain is constrained from rigid body motion. The applied load is a static pressure
with a magnitude of 10 force/length2 applied on the circular free surface of the block circumscribed by
the crack. The loading is illustrated in Figure 1.4.2–1.
Abaqus modeling approaches and simulation techniques
This example includes six cases demonstrating different modeling approaches using Abaqus/Standard.
The crack is modeled as a seam since the crack surfaces in the unloaded state lie next to one another with
no gap.
The geometry is axisymmetric and can be modeled as such. However, the three-dimensional cases
demonstrate the Abaqus fracture mechanics capability, where the crack extension direction varies along
a curved crack front. The infinite half-space is treated using multiple techniques. In Case 1 through Case
4, the domain is extended well beyond the region of interest. Far-field boundary conditions applied
a significant distance from the region of interest have negligible influence on the response near the
crack. Cases 5 and Case 6 demonstrate the use of continuum infinite elements. Axisymmetric and
three-dimensional cases are provided with and without submodeling. “Fracture mechanics,” Section 7.10
of the Abaqus Analysis User’s Manual, provides detailed information on fracture mechanics procedures.
Summary of analysis cases
Case 1
Full axisymmetric model using Abaqus/CAE.
Case 2
Full three-dimensional model using Abaqus/CAE.
Case 3
Axisymmetric approach with submodeling using Abaqus/CAE.
Case 4
Three-dimensional approach with submodeling using Abaqus/CAE.
Case 5
Axisymmetric approach with submodeling and infinite elements using input files.
Case 6
Three-dimensional approach with submodeling and infinite elements using input files.
The following sections discuss analysis considerations that are applicable to several or all the cases. More
detailed descriptions are provided later including discussions of results and listings of files provided. The
1.4.2–2
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
models for Case 1 through Case 4 were generated using Abaqus/CAE. In addition to the Python scripts
that generate the model databases, Abaqus/Standard input files are also provided for those cases.
Mesh design
The mesh includes a seam along the crack with duplicate nodes, which allow the crack to open when
loaded. The geometry is partitioned to map rings of elements around the crack tip for the contour
integral calculations. The models use either quadrilateral or brick elements with a collapsed side to
create triangular elements for two-dimensional cases or wedge-shaped elements for three-dimensional
cases, which introduce a singularity at the crack tip. To be used for the evaluation of contour integrals,
the mesh around the crack tip must be modeled as described in “Using contour integrals to model fracture
mechanics,” Section 31.2 of the Abaqus/CAE User’s Manual. In the axisymmetric cases a circular
partition is created to mesh around the crack tip. In the three-dimensional cases the corresponding
partition is a curved tubular volume enclosing the crack tip.
A refined mesh at the crack tip is required to obtain contour-independent results; i.e., there is no
significant variation in the contour integral values calculated for successive rings of elements around
the crack tip. In the circular partitioned region surrounding the crack tip where the contour integrals
are calculated, the mesh should be biased moderately toward the crack tip. The accuracy of the contour
integrals is not very sensitive to the biasing. Engineering judgment is required to establish adequate mesh
refinement to produce contour-independent results while avoiding the possibility of creating elements at
the crack tip that are so small in relation to other elements that they introduce numerical conditioning
issues and associated round-off errors.
When the deformation and the material are linear as in this example, the diameter of the circular
partition used to map the crack-tip mesh for contour integral calculations is not critical. (If the material
is elastic-plastic, the size of the circular partition should generally contain the plastic zone and allow
a number of the contours for the contour integrals to enclose the plastic zone while still remaining in
the elastic region.) The remaining partitions are created so that the element shapes satisfy the element
quality criteria in the regions away from the crack tip.
To understand the types of singularities created by collapsing the side of an element in two or three
dimensions, see “Constructing a fracture mechanics mesh for small-strain analysis” in “Contour integral
evaluation,” Section 11.4.2 of the Abaqus Analysis User’s Manual. In this application we want to have
a square root singularity in strain at the crack since the material is linear elastic and we will perform a
small-strain analysis.
The stress intensity factors and the T-stresses are calculated using the interaction integral
method, in which auxiliary plane strain crack-tip fields are employed. The crack front radius of
curvature is significant for this problem. Therefore, to calculate the contour integrals accurately for
the three-dimensional cases, a very refined mesh is used to approach the plane strain condition locally
around the crack front. This refined mesh makes the contour integral domain sufficiently small to
minimize the influence of curvature on the results.
Additional details of the meshing procedures for the axisymmetric and three-dimensional cases are
discussed below within the descriptions of the individual cases.
1.4.2–3
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Material model
The linear static structural analysis requires specification of Young’s modulus, which is 30,000,000 units
of force/length2, and Poisson’s ratio, which is 0.3. One solid, homogenous section is used to assign
material properties to the elements.
Loading
A uniform pressure load of 10 units of force/length2 is applied along the free top surface of the crack. In
the axisymmetric models the load region, where the pressure is applied is represented by a line segment.
For the three-dimensional cases the load region where the pressure is applied an area.
Analysis steps
Each analysis is performed using a single linear static step.
Output requests
Output requests are used to specify calculation of contour integrals, stress intensity factors, and Tstress. See “Requesting contour integral output,” Section 31.2.11 of the Abaqus/CAE User’s Manual,
for more information regarding fracture mechanics output. The global models used in the submodeling
cases include output requests necessary to write displacement and stress results to the output database
(.odb) file; in the case where node-based submodeling is used, displacement results are used to establish
boundary conditions on the corresponding submodels. In the case where surface-based submodeling is
used, stress results are used to establish boundary tractions on the corresponding submodel.
Submodeling
Realistic fracture analyses tend to require significant computer resources. To obtain accurate results when
analyzing the stress field around a crack tip, a refined mesh must be used to capture the strong gradients
near the tip. The required mesh refinement can make fracture mechanics models large since a crack
is normally a very small feature compared with the model dimensions. An alternative technique that
reduces computational resources is to use submodeling to obtain accurate results by running two smaller
models sequentially instead of performing a single global analysis with a refined mesh around the crack.
The first step is to solve a less refined global model to obtain a solution that is accurate away from the
crack tip but is not sufficiently refined to capture strong gradients near the region of interest. A refined
submodel of the crack-tip region is then used to obtain a more accurate solution and, hence, more accurate
contour integrals. The boundaries of the submodel must be far enough from the region of interest that
the less refined global model is able to provide accurate results at the submodel boundaries, particularly
important when surface-based submodeling is used. This condition is verified during postprocessing by
confirming that the stress contours at the boundaries of the submodel are similar to the stress contours at
the same location in the global model.
Although the submodeling approach is not required for this example because the refined models
for the entire domain analyzed in Case 1 and Case 2 are small enough to run on commonly available
computing platforms, this application provides an opportunity to demonstrate submodeling techniques
1.4.2–4
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
for both axisymmetric and three-dimensional fracture mechanics cases, as well as showing the
differences between node-based submodeling based on displacements and surface-based submodeling
based on stresses. Submodeling procedures are described in detail in “Node-based submodeling,”
Section 10.2.2 of the Abaqus Analysis User’s Manual, “Surface-based submodeling,” Section 10.2.3
of the Abaqus Analysis User’s Manual, and Chapter 38, “Submodeling,” of the Abaqus/CAE User’s
Manual.
Modeling an infinite domain
Case 1 through Case 4 simulate the infinite extent of the domain with a continuum mesh that is large
compared to the crack dimensions with appropriate far-field boundary conditions. In those cases the
domain extends 20 times the crack length. Case 5 and Case 6 demonstrate the use of continuum infinite
elements and represent the region of interest with reduced-integration continuum elements to a distance
approximately 10 times the crack dimensions surrounded by a layer of continuum infinite elements. Farfield boundary conditions are not required in these cases.
Case 1 Full axisymmetric model with Abaqus/CAE
The axisymmetric domain is a solid with a radius equal to the height of 300 length units (see
Figure 1.4.2–2). The top edge of the model represents the free surface containing the crack. The
semi-infinite domain is simulated by extending the continuum model to a distance 20 times the length
of the crack and applying appropriate far-field boundary conditions. This model uses continuum
axisymmetric quadratic reduced-integration (CAX8R) elements.
Mesh design
When calculating contour integrals in two-dimensional problems, quadrilateral elements must be used
around the crack tip where the contour integral calculations will be performed with triangular elements
adjacent to the crack tip. These triangular elements are actually collapsed quadrilaterals, which introduce
a singularity. The axisymmetric model must be partitioned as shown in Figure 1.4.2–2 to define the crack,
introduce a singularity by collapsing elements at the crack tip, and create rings of quadrilateral elements
for contour integral calculations. A straight line partition is created where the seam crack is defined
along with a circular partition, which enables mapping rings of elements around the crack tip. When
structured meshing is used for this partition, triangular elements are created adjacent to the crack tip with
quadrilaterals surrounding them (see “Using contour integrals to model fracture mechanics,” Section 31.2
of the Abaqus/CAE User’s Manual). Abaqus/CAE automatically converts triangular elements at the
crack tip to quadrilaterals with one side collapsed to introduce a singularity.
“Creating a seam,” Section 31.1.2 of the Abaqus/CAE User’s Manual, describes how to pick
partition segments to define the seam (crack). Procedures to create a square root singularity in strain
at the crack tip are described in “Controlling the singularity at the crack tip,” Section 31.2.8 of the
Abaqus/CAE User’s Manual. After defining the seam, pick the crack tip to specify the region defining
the first contour integral and define the q vector to specify the crack extension direction as described in
“Creating a contour integral crack,” Section 31.2.9 of the Abaqus/CAE User’s Manual.
1.4.2–5
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Boundary conditions
The right edge of the model shown in Figure 1.4.2–3 is unconstrained to represent the far-field boundary.
The bottom edge of the model is constrained to zero displacement (U2) to eliminate rigid body motion
while simulating the far-field boundary. These edges are far enough away from the area of interest around
the crack to represent an infinite domain with negligible influence on the area of interest.
Run procedure
The Case 1 model is generated using Abaqus/CAE to create and to mesh native geometry. Python scripts
are provided to automate building the model and running the solution. The scripts can be run interactively
or from the command line.
To create the model interactively, start Abaqus/CAE and select Run Script from the Start
Session dialog box that appears. Select the first file for the case, AxisymmConeCrack_model.py.
When the script completes, you can use Abaqus/CAE commands to display and to query the model.
When you are ready to analyze the model, select Run Script from the File menu and choose the next
script, AxisymmConeCrack_job.py. The Python scripts provided allow you to modify the model
interactively with Abaqus/CAE to explore additional variations on the cases provided here.
Alternatively, the Python scripts can be run from the command line with the Abaqus/CAE noGUI
option in the order listed:
abaqus cae noGUI=filename.py
where abaqus is the system command to run the program and filename is the name of the script
to be run.
As an alternative to the Python scripts, an Abaqus/Standard input file AxisymmConeCrack.inp
is also provided to run this case. You can submit the analysis using the input file with the following
command:
abaqus input=AxisymmConeCrack.inp
Case 2 Full three-dimensional model with Abaqus/CAE
The three-dimensional domain is a cube with an edge length of 300 units, as shown in Figure 1.4.2–4. The
mesh represents a quarter-symmetric segment of the problem domain. The top of the model represents the
free surface containing the crack. The semi-infinite domain is represented by extending the continuum
mesh to a distance 20 times the length of the crack with appropriate symmetry and far-field boundary
conditions.
Mesh design
When calculating three-dimensional contour integrals, rings of brick elements must be used around the
crack tip where the contour integral calculations will be performed with wedge elements adjacent to
the crack tip (these wedges are actually collapsed bricks). Concentric tubular partitions are created to
map the mesh around the crack tip. The three-dimensional domain and partitioning of the geometry
are illustrated in Figure 1.4.2–5 and Figure 1.4.2–6. The seam crack is shown in Figure 1.4.2–7. When
1.4.2–6
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
structured meshing is used for the inner tubular partition, wedge elements are created adjacent to the crack
tip with rings of bricks surrounding them (see “Using contour integrals to model fracture mechanics,”
Section 31.2 of the Abaqus/CAE User’s Manual, for details). A swept mesh used in the inner ring creates
wedge elements at the crack tip. The outer ring is meshed with hexahedral elements using the structured
meshing technique.
For details on how to define the crack propagation direction where the direction of the vectors
varies along the crack front (referred to as the q vector), see “Defining the crack extension direction,”
Section 31.2.4 of the Abaqus/CAE User’s Manual. Figure 1.4.2–8 illustrates the q vectors.
Boundary conditions
Symmetric displacement boundary conditions are applied normal to the symmetry planes. The far-field
faces on the sides of the model, which are not symmetry planes, are unconstrained. The bottom face of
the model is constrained from displacement in the direction of the pressure load (U2=0) to prevent rigid
body motion while simulating a far-field boundary condition.
Run procedure
The Python scripts provided to generate the Abaqus/CAE model and to analyze the model are run
following the same procedures as those described for Case 1.
As an alternative to the Python scripts,
an Abaqus/Standard input file
SymmConeCrackOrphan.inp is also provided to run this case. You can submit the analysis
using the input file with the following command:
abaqus input= SymmConeCrackOrphan.inp
The files defining nodes and elements for this case, SymmConeCrackOrphan_node.inp and
SymmConeCrackOrphan_elem.inp, must be available when the input file is submitted.
Figure 1.4.2–9 shows a deformed shape plot for the three-dimensional model of the crack from
the full three-dimensional analysis of Case 2. The displacement is exaggerated using a scaling factor to
visualize the crack opening.
Case 3 Axisymmetric approach with submodeling using Abaqus/CAE
Case 3 uses the submodeling approach and, hence, requires two sequential analyses, which are referred
to as the global model and the submodel. First, a less refined global model is solved to obtain the
displacement solution with sufficient accuracy away from the crack tip. A refined submodel of the area
of interest driven by the displacement solution from the global model is then used to obtain an accurate
solution in the crack-tip region. Each of these models is much smaller than the fully refined axisymmetric
global model used in Case 1.
Mesh design
The axisymmetric global model has a relatively less refined mesh in the crack region. The global model
used for Case 3 has two rings of elements where the mesh focuses on the crack tip, compared to 13 rings
of elements around the crack tip in the full model used in Case 1.
1.4.2–7
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
The axisymmetric global model and the submodel meshes for Case 3 are shown in Figure 1.4.2–10.
The axisymmetric submodel has a refined mesh around the crack tip with 12 rings of elements
surrounding the crack tip. It is assumed that the global model’s coarse mesh is sufficiently accurate
to drive the submodel: the submodel can obtain accurate contour integral results if the global model’s
displacement field is accurate at the boundaries of the submodel, which lie far from the crack tip.
You can verify this at the postprocessing stage by comparing stress contours at the boundaries of the
submodel to the corresponding contours of the global model.
Boundary conditions
The boundary conditions applied to the axisymmetric global model are the same as those used in
Case 1. The displacement solution from the global model is applied to the submodel boundaries when
the submodeling technique is used.
Run procedure
The models used for Case 3 are generated using Abaqus/CAE to create and to mesh native geometry.
The same procedures used to run the Python scripts for Cases 1 and 2 are used to create and to analyze
the global model. The script that builds the submodel refers to the global model output database (.odb)
file, which must be available when the submodel is analyzed. After analyzing the global model, run the
scripts to build and to analyze the submodel using the same procedure used for the global model.
Abaqus/Standard input files are also provided to run this case. First, run the job to create and to
analyze the global model; then run the submodel job. The results from the global model must be available
to run the submodel. A typical execution procedure is as follows:
abaqus job=globalModelJobName input=globalModelInputfile.inp
abaqus job=submodelJobname, input=subModelInputfile.inp,
globalmodel=globalModelJobNameOutputDatabase
Case 4 Three-dimensional approach with submodeling using Abaqus/CAE
Case 4 uses a three-dimensional submodeling approach and requires two sequential analyses, a global
model and a submodel. First, a global model is solved with sufficient refinement to provide an accurate
displacement and stress solution away from the crack tip.
Two versions of refined submodels of the area of interest are then used to obtain an accurate solution
in the crack-tip region. In one submodel analysis the area of interest is driven by the displacement solution
from the global model. In the other submodel analysis the area of interest is driven by the stress solution
from the global model.
Each of the models used in this case is much smaller than the fully refined three-dimensional global
model used in Case 2.
Mesh design
The three-dimensional global model, with a less refined mesh in the crack region, is first analyzed and
then used to drive the submodel. For the three-dimensional global model only 18 elements are used
1.4.2–8
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
along the crack line, whereas 38 elements are used along the crack line in the submodel. Figure 1.4.2–11
shows the meshes for the three-dimensional global model and the submodel.
Boundary conditions
The boundary conditions applied to the global model in Case 4 are the same as those used in the full
three-dimensional Case 2. The submodeling approach uses either the displacement or stress solution
from the global model to drive the submodel boundaries.
Run procedure
The models used for Case 4 are generated using Abaqus/CAE to create and to mesh native geometry.
The same procedures used to run Case 3 can be used with Case 4. The script that builds the submodel
refers to the global model output database (.odb) file, which must be available when the submodel is
analyzed.
As an alternative to the Python scripts, Abaqus/Standard input files are also provided to run this
case. These are submitted using the same procedure described for the input files under Case 3.
Case 5 Axisymmetric submodeling approach with infinite elements using Abaqus/Standard
input files
Case 5 uses the submodeling approach with an axisymmetric mesh utilizing continuum infinite elements
to simulate the far-field boundary condition. The submodeling technique requires two sequential
analyses, a less refined global model and a refined submodel at the crack tip.
The global model in Case 5 comprises an axisymmetric representation of the hemispherical
domain with continuum elements to a radius of 170 length units. Eight-node biquadratic axisymmetric
quadrilateral, reduced-integration elements (CAX8R) are used to model the solid domain in the region
adjacent to the crack. The domain is further extended using a layer of continuum infinite elements to
a radius of 340 length units. Five-node quadratic axisymmetric one-way infinite elements (CINAX5R)
are used to simulate the far-field region of the solid. The submodel used in Case 5 does not encompass
the complete crack face but extends to a distance far enough from the crack tip that strong variations
in the stress field are captured within the submodel. This result can be verified by comparing stress
contours of the submodel with the corresponding stress contours in the global model.
Mesh design
The axisymmetric global model, with a relatively less refined mesh in the crack region, is first analyzed
and then used to drive the submodel. The axisymmetric global model and the submodel meshes for
Case 5 are shown in Figure 1.4.2–12.
Boundary conditions
The continuum infinite elements eliminate the need for far-field constraints, which were required in
Case 1 through Case 4.
1.4.2–9
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Run procedure
The models used for Case 5 are generated using Abaqus/Standard input files. First, run the job to create
and to analyze the global model; then run the submodel job. The results from the global model must be
available to run the submodel. A typical execution procedure is as follows:
abaqus job=globalModelJobName input=globalModelInputfile.inp
abaqus job=submodelJobname, input=subModelInputfile.inp,
globalmodel=globalModalJobNameOutputDatabase
Case 6 Three-dimensional approach with infinite elements using submodeling with
Abaqus/Standard input files
Case 6 uses the submodeling approach with a three-dimensional mesh utilizing continuum infinite
elements to simulate the far-field boundary condition. The domain modeled for Case 6 encompasses an
eighth of a sphere, representing one-quarter of the semi-infinite problem domain. Continuum elements
are used to a radius of 170 length units. The domain is extended using a layer of infinite continuum
elements to a radius of 340 length units.
The submodeling technique requires two separate analyses, a less refined global model and a refined
submodel at the crack tip. Case 6 uses Abaqus/Standard input files to generate the models rather than
Abaqus/CAE Python scripts. Twenty-node quadratic, reduced-integration solid elements (C3D20R) are
used to model the solid domain in the region adjacent to the crack. The domain is further extended using
a layer of 12-node quadratic one-way infinite brick elements (CIN3D12R) to a radius of 340 length units.
The submodel used in Case 6 does not encompass the complete crack face but extends to a distance
far enough from the crack tip that strong variations in the stress field are captured within the submodel.
Mesh design
The three-dimensional global model, with a relatively less refined mesh in the crack region, is first
analyzed and then used to drive the submodel. The three-dimensional global model and the submodel
meshes for Case 6 are shown in Figure 1.4.2–13.
Boundary conditions
The continuum infinite elements eliminate the need for far-field constraints, which were required in Case
1 through Case 4.
Run procedure
The models of Case 6 are generated using Abaqus/Standard input files. The same procedure used in Case
5 is also used in Case 6. The files containing the node and element definitions for the three-dimensional
global model must be available when the input file is run to create the global model . The output database
(.odb) file from the global model must be available to run the submodel.
1.4.2–10
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Discussion of results and comparison of cases
Contour integral results obtained from the data (.dat) file for each case are summarized in Table 1.4.2–1
through Table 1.4.2–4. These results are also available from the output database (.odb) file by displaying
history output in the Visualization module of Abaqus/CAE. While there is no analytical solution available
for comparison, an additional axisymmetric analysis with extreme mesh refinement is used as the basis
for a reference solution. Each table includes the reference solution value in the table title.
Abaqus calculates the J-integral using two methods. Values of the J-integral are based on the stress
intensity factors, JK, and by evaluating the contour integral directly, JA. The stress intensity factors
and
, and the T-stresses are given in Table 1.4.2–2, Table 1.4.2–3, and Table 1.4.2–4, respectively.
When the stress intensity factors are requested, Abaqus automatically outputs the J-integrals based on
the stress intensity factors, JK. Values of
are not tabulated because these values should equal zero
based on the loading and are negligibly small relative to
and
.
The tables list values for contour 1 through contour 5. Each contour corresponds to a successive
ring of elements progressing outward radially from the crack tip. For the axisymmetric cases one set of
results is available for each contour. For the three-dimensional cases Abaqus/Standard provides contour
integral values at each crack-tip node. The values listed in Table 1.4.2–1 through Table 1.4.2–4 for the
three-dimensional cases correspond to the location halfway along the circumference of the crack, which
lies midway between the symmetry faces of the three-dimensional models. A detailed examination of the
results for the three-dimensional cases confirms that the contour integral values are essentially constant at
each node along the circumference of the crack tip. The exception is the value calculated for
; which
fluctuates but remains small relative to
and
over almost the full length of the crack; however
increases at the open end faces of the crack corresponding to the symmetry planes. A loss of
accuracy occurring at the node corresponding to the open end of a three-dimensional crack is a known
limitation that can be expected when applying this method.
Results from the first contour are generally not used when evaluating fracture problems because the
first contour is influenced by the singularity associated with the crack tip. The average quantities reported
in the tabular results exclude the first contour. Comparisons refer only to contour 2 through contour 5.
The axisymmetric and the three-dimensional modeling approaches are in close agreement, with and
without submodeling. For each case, values of the tabulated quantities for J calculated by evaluating
the contour integrals directly, (JA),
,
, and T-stresses deviate by less than 2% of the average of
the corresponding values for contour 2 through contour 5. The J-integral for each case, calculated from
the stress intensity factors (JK) deviate by less than 3.5% of the average of corresponding values. The
larger deviation for JK versus JA is expected because the method of calculating contour integrals from
the stress intensity factors (JK) is more sensitive to numerical precision than calculating the contour
integrals directly (JA).
is analytically equal to zero due to the geometry and loading symmetry in
this example; the numerical results for
are negligibly small relative to
and
.
Submodeling results
The global models used to calculate the deformation and stress fields that drive the submodels use cracktip meshes that are too coarse to give accurate results for the contour integrals; therefore, the results
for the global models are not tabulated. Results are tabulated for the submodels that refer to this global
1.4.2–11
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
analysis. Generally these results verify that the submodeling approach provides adequate accuracy in
fracture problems where it may not be practical to use a sufficiently refined mesh in the crack-tip region of
a global model. The node-based submodeling approach provides greater accuracy than the surface-based
approach.
Node-based submodeling results
The J-integral values for the node-based submodel analyses match those for the full model analyses
(analyses with adequate mesh refinement around the crack tip) to within less than 1%.
Surface-based submodeling results
The three-dimensional submodeling case also considers surface-based submodeling, where the
submodel is driven by the global model stress field. Two different pairs of global models and
surface-based submodels are considered: one that matches the mesh design used in the node-based
analysis, and one where adjustments are made to improve accuracy. The J-integral values for the first
analysis pair, with the same meshes as in node-based submodeling, match those for the full model only
to within 6%. These inaccurate results arise from a modeling arrangement that violates guidelines
established in “Surface-based submodeling,” Section 10.2.3 of the Abaqus Analysis User’s Manual,
namely that
•
•
the submodel surface should intersect the global model in regions of relatively low stress gradients,
and
the submodel surface should intersect the global model in regions of uniform element size.
Adjusted global and submodel analyses that adhere to these guidelines are run. In this case the
submodel driven surface is farther from the crack region and the high stress gradient, and the global model
mesh is refined so that elements are more uniform in the region of the submodel surface. Figure 1.4.2–14
shows a comparison of the submodel/global model pairs. The modeling arrangement on the left places
the lower submodel boundary too near to the crack and high stress gradients and cuts through high aspect
ratio elements. The arrangement on the right provides lower aspect ratio elements in the global model
and positions the lower submodel boundary further from the crack. The adjusted analysis with the further
boundary now matches the J-integral values for the full model to within 2%. This accuracy difference
illustrates the importance of adhering to the guidelines for surface-based submodel design. In practice,
in the absence of a reference global solution, you should use the following guidelines to ensure your
surface-based solution is adequate:
•
•
As with any submodel analysis, compare solution results between the global model and submodel on
the submodel boundary. In this case a stress comparison is appropriate. Figure 1.4.2–15 compares
the 2-component of stress for the two surface-based submodel analyses and their corresponding
global model. Results are plotted on a path lying in the lower submodel boundary and extending
from the center radially outward. The near-boundary submodel has a significantly greater stress
discrepancy with the global model.
In cases where inertia relief is employed to address rigid body modes in surface-based submodeling,
if the inertia relief force output variable (IRF) is small compared to the prevailing force level in the
model, the surface-based stress distribution is equilibrated. In this model the prevailing force is the
1.4.2–12
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
10 units of pressure acting on the surface circumscribed on the crack (a radius of 6), or 786 units of
force for the three-dimensional quarter symmetry model.
In this analysis the inertia relief force in the 2-direction is similar in both cases (33 for the
near-boundary model and 32 for the far-boundary model) and relatively small; hence, in this case,
the inertia relief force would not suggest poorer results with the near-boundary submodel, and its
small value is not a sufficient measure of the adequacy of the submodel design.
Files
You can use the Python scripts for Abaqus/CAE and input files for Abaqus/Standard to create and to run
the cases.
Case 1 Full axisymmetric analysis
AxisymmConeCrack_model.py
AxisymmConeCrack_job.py
AxisymmConeCrack.inp
Script to create the model, including instructions for
creating the mesh used for the reference solution.
Script to analyze the model.
Input file to create and to analyze the model.
Case 2 Full three-dimensional model
SymmConeCrack_model.py
SymmConeCrack_job.py
SymmConeCrackOrphan.inp
SymmConeCrackOrphan_node.inp
SymmConeCrackOrphan_elem.inp
Script to create the model.
Script to analyze the model.
Input file to create and to analyze the model.
Nodes for SymmConeCrackOrphan.inp.
Elements for SymmConeCrackOrphan.inp.
Case 3 Axisymmetric submodel analysis
AxisymmConeCrackGl_model.py
AxisymmConeCrackGl_job.py
AxisymmConeCrackSub_model.py
AxisymmConeCrackSub_job.py
AxisymmConeCrackGl.inp
AxisymmConeCrackSub.inp
Script to create the model.
Script to analyze the model and to create the output
database file that drives the submodel.
Script to create the submodel.
Script to analyze the submodel using the results from the
global model output database file to drive it.
Input file to create and to analyze the global model.
Input file to create and to analyze the submodel.
Case 4 Three-dimensional submodel analysis
SymmConeCrackGl_model.py
SymmConeCrackGl_job.py
SymmConeCrackSub_model.py
Script to create the global model.
Script to analyze the global model and to create the output
database file that drives the submodel. Refer to parameter
definitions in the script to create the adjusted global model
referred to in “Submodeling results.”
Script to create the node-based submodel.
1.4.2–13
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
SymmConeCrackSub_job.py
SymmConeCrackSubSb_near_model.py
SymmConeCrackSubSb_near_job.py
SymmConeCrackSubSb_far_model.py
SymmConeCrackSubSb_far_job.py
SymmConeCrackGlOrphan.inp
SymmConeCrackGlOrphan_node.inp
SymmConeCrackGlOrphan_elem.inp
SymmConeCrackGlOrphanAdj.inp
SymmConeCrackGlOrphanAdj_node.inp
SymmConeCrackGlOrphanAdj_elem.inp
SymmConeCrackSubOr.inp
SymmConeCrackSubOr_node.inp
SymmConeCrackSubOr_elem.inp
SymmConeCrackSubOrSb_near.inp
SymmConeCrackSubOrSb_near_node.inp
SymmConeCrackSubOrSb_near_elem.inp
SymmConeCrackSubOrSb_far.inp
SymmConeCrackSubOrSb_far_node.inp
SymmConeCrackSubOrSb_far_elem.inp
Script to analyze the node-based submodel using the
results from the global model output database file to drive
it.
Script to create the surface-based submodel.
Script to analyze the surface-based submodel using the
stress results from the global model output database file
to drive it.
Script to create the surface-based submodel with a farboundary submodel.
Script to analyze the surface-based submodel with the
far-boundary submodel using the stress results from the
global model output database file to drive it.
Input file to create and to analyze the global model.
Nodes for SymmConeCrackGlOrphan.inp.
Elements for SymmConeCrackGlOrphan.inp.
Input file to create and to analyze the global model that is
adjusted for improved surface-based submodel accuracy.
Nodes for SymmConeCrackGlOrphanAdj.inp.
Elements for SymmConeCrackGlOrphanAdj.inp.
Input file to create and to analyze the node-based
submodel.
Nodes for SymmConeCrackSubOr.inp.
Elements for SymmConeCrackSubOr.inp.
Input file to create and to analyze the submodel using the
surface-based submodel technique to drive the submodel
stresses.
Nodes for SymmConeCrackSubOrSb_near.inp.
Elements for SymmConeCrackSubOrSb_near.inp.
Input file to create and to analyze the submodel with the
far-boundary submodel using the surface-based submodel
technique to drive the submodel stresses.
Nodes for SymmConeCrackSubOrSb_far.inp.
Elements for SymmConeCrackSubOrSb_far.inp.
Case 5 Axisymmetric submodel analysis using infinite continuum elements
conicalcrack_axiglobal.inp
conicalcrack_axisubmodel_rms.inp
Input file to analyze the axisymmetric global model and
to create the output database file that drives the submodel.
Input file to analyze the axisymmetric submodel using the
results from the global model output database file to drive
it.
1.4.2–14
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Case 6 Three-dimensional submodeling analysis using infinite continuum elements
conicalcrack_3dglobal.inp
conicalcrack_3dsubmodel_rms.inp
Input file to analyze the three-dimensional global model
and to create the output database file that drives the
submodel.
Input file to analyze the three-dimensional submodel
using the results from the global model output database
file to drive it.
Reference
Other
•
Shih, C. F., B. Moran, and T. Nakamura, “Energy Release Rate Along a Three-Dimensional Crack
Front in a Thermally Stressed Body,” International Journal of Fracture, vol. 30, pp.79–102, 1986.
1.4.2–15
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Table 1.4.2–1 J-integral estimates (×10−7 ) for conical crack using Abaqus. JK denotes the
J values estimated from stress intensity factors; JA denotes the J values estimated directly
by Abaqus. The reference solution J-integral value is 1.33.
Contour
Solution
J
estimate
method
1
2
3
4
5
Average
Value,
Contours
2–5
Case 1: Full
axisymmetric
JK
1.326
1.308
1.288
1.262
1.228
1.272
JA
1.334
1.333
1.334
1.334
1.334
1.334
Case 2:
Full threedimensional
JK
1.303
1.325
1.312
1.295
1.274
1.302
JA
1.308
1.334
1.336
1.337
1.337
1.336
Case 3:
Submodel
axisymmetric
JK
1.327
1.319
1.311
1.300
1.287
1.304
JA
1.330
1.329
1.330
1.330
1.330
1.330
Case 4:
Node-based
submodel
threedimensional
JK
1.314
1.316
1.303
1.285
1.264
1.292
JA
1.318
1.326
1.328
1.328
1.328
1.328
Case 4:
Surface-based
submodel
threedimensional
JK
1.396
1.398
1.385
1.367
1.345
1.374
JA
1.400
1.408
1.409
1.408
1.407
1.408
Case 4:
Surface-based
submodel with
far boundary,
threedimensional
JK
1.345
1.347
1.335
1.317
1.296
1.324
JA
1.349
1.357
1.359
1.358
1.358
1.358
Case 5:
Submodel
axisymmetric
with infinite
elements
JK
1.413
1.359
1.363
1.363
1.361
1.362
JA
1.407
1.360
1.365
1.365
1.365
1.364
1.4.2–16
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Solution
Contour
J
estimate
method
1
2
3
4
5
Average
Value,
Contours
2–5
JK
1.329
1.363
1.367
1.368
1.368
1.367
JA
1.336
1.361
1.366
1.366
1.366
1.365
Case 6:
Submodel
threedimensional
with infinite
elements
Table 1.4.2–2 Stress intensity factor
estimates for conical
crack using Abaqus. Contour 1 is omitted from the average value
calculations. The reference solution
value is 0.491.
Solution
1
2
3
4
5
Average
Value,
Contours
2–5
Case 1: Full
axisymmetric
0.495
0.497
0.499
0.500
0.499
0.499
Case 2:
Full threedimensional
0.492
0.501
0.503
0.502
0.500
0.502
Case 3:
Submodel
axisymmetric
0.491
0.493
0.494
0.495
0.496
0.494
Case 4:
Node-based
submodel threedimensional
0.491
0.496
0.498
0.497
0.494
0.497
Case 4:
Surface-based
submodel threedimensional
0.426
0.431
0.433
0.431
0.427
0.430
Contour
1.4.2–17
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Solution
Contour
1
2
3
4
5
Average
Value,
Contours
2–5
Case 4:
Surface-based
submodel
with far
boundary, threedimensional
0.436
0.441
0.443
0.442
0.439
0.441
Case 5:
Submodel
axisymmetric
with infinite
elements
0.537
0.527
0.528
0.528
0.529
0.528
Case 6:
Submodel three
dimensional
with infinite
elements
0.522
0.528
0.529
0.530
0.530
0.528
Table 1.4.2–3 Stress intensity factor
estimates for conical crack using Abaqus. Contour 1 is
value is −2.03.
omitted from the average value calculations. The reference solution
Solution
1
2
3
4
5
Average
Value,
Contours
2–5
Case 1: Full
axisymmetric
–2.032
–2.016
–2.000
–1.978
–1.949
–1.986
Case 2:
Full threedimensional
–2.013
–2.029
–2.018
–2.004
–1.987
–2.010
Case 3:
Submodel
axisymmetric
–2.033
–2.026
–2.019
–2.010
–1.999
–2.014
Contour
1.4.2–18
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Solution
Contour
1
2
3
4
5
Average
Value,
Contours
2–5
Case 4:
Node-based
submodel threedimensional
–2.023
–2.023
–2.012
–1.997
–1.980
–2.003
Case 4:
Surface-based
submodel threedimensional
–2.102
–2.103
–2.092
–2.078
–2.061
–2.084
Case 4:
Surface-based
submodel
with far
boundary, threedimensional
–2.060
–2.060
–2.050
–2.036
–2.019
–2.041
Case 5:
Submodel
axisymmetric
with infinite
elements
–2.090
–2.050
–2.053
–2.052
–2.051
–2.051
Case 6:
Submodel three
dimensional
with infinite
elements
2.027
2.053
2.057
2.057
2.057
2.056
1.4.2–19
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Table 1.4.2–4 T-stress estimates for conical crack using Abaqus. Contour 1 is omitted from the
average value calculations. The reference solution T-stress value is 0.979.
Solution
1
2
3
4
5
Average
Value,
Contours
2–5
Case 1:
Full axisymmetric
–0.982
–0.979
–0.976
–0.972
–0.967
–0.973
Case 2: Full
three-dimensional
–0.942
–0.972
–0.966
–0.960
–0.954
–0.963
Case 3:
Submodel
Axisymmetric
–0.980
–0.978
–0.977
–0.975
–0.973
–0.976
Case 4: Nodebased submodel
three-dimensional
–0.947
–0.966
–0.959
–0.953
–0.947
–0.956
Case 4: Surfacebased submodel
three-dimensional
–0.981
–0.996
–0.989
–0.983
–0.976
–0.986
Case 4: Surfacebased submodel
with far boundary,
three-dimensional
–0.958
–0.973
–0.966
–0.960
–0.954
–0.963
Case 5:
Submodel
axisymmetric with
infinite elements
–1.182
–0.983
–0.985
–0.984
–0.984
–0.984
Case 6:
Submodel
three-dimensional
with infinite
elements
–0.599
–0.982
–0.984
–0.983
–0.982
–0.982
Contour
1.4.2–20
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
conical crack
P
r
θ
infinite half-space
a
2
3
1
r = 10
a = 15
θ = 45 o
P = 10
Elastic material: E = 30E6
υ = 0.3
Figure 1.4.2–1
Conical crack in a half-space.
1.4.2–21
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Figure 1.4.2–2
Case 1: Partitioning axisymmetric geometry.
P
Figure 1.4.2–3
Case 1: Full axisymmetric mesh.
1.4.2–22
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
symmetry about
the 1-2 plane
symmetry about
the 2-3 plane
Figure 1.4.2–4
Figure 1.4.2–5
Case 2: Full three-dimensional mesh.
Case 2: Partitioned full three-dimensional model.
1.4.2–23
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
cone crack edges
outer ring
inner ring
Figure 1.4.2–6 Case 2: Partitions around the crack line. The
smaller inner ring is swept meshed using wedge elements. The
outer ring is meshed using hexahedral elements and the structured
meshing technique. The cone partitions are also visible.
crack line
Figure 1.4.2–7
seam crack face
Case 2: Seam crack faces for the cone.
1.4.2–24
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Figure 1.4.2–8
Case 2: q vectors defined along the entire crack line on an orphan mesh.
Figure 1.4.2–9
Case 2: Results three-dimensional displaced shape.
1.4.2–25
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Figure 1.4.2–10
Figure 1.4.2–11
Case 3: Axisymmetric global and submodel meshes around the crack line.
Case 4: Full three-dimensional global model and submodel meshes around the crack line.
1.4.2–26
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Figure 1.4.2–12
Figure 1.4.2–13
Case 5: Axisymmetric global model using infinite elements and submodel meshes.
Case 6: Three-dimensional global model with infinite elements and submodel meshes.
1.4.2–27
Abaqus Version 6.12 ID:
Printed on:
CONTOUR INTEGRALS FOR A CONICAL CRACK
Figure 1.4.2–14 Case 4: Comparison of inadequate (left) and adequate (right) global and
submodel designs for a surface-based submodel stress solution.
Far boundary −− global model
Far boundary −− submodel
Near boundary −− global model
Near boundary −− submodel
0.0
−0.5
Syy
−1.0
−1.5
−2.0
0.0
2.0
4.0
6.0
8.0
10.0
Distance from center
Figure 1.4.2–15
Case 4: Confirmation of stress agreement between the global model and submodel.
1.4.2–28
Abaqus Version 6.12 ID:
Printed on:
INELASTIC LINE SPRING
1.4.3
ELASTIC-PLASTIC LINE SPRING MODELING OF A FINITE LENGTH CYLINDER
WITH A PART-THROUGH AXIAL FLAW
Product: Abaqus/Standard
The elastic-plastic line spring elements in Abaqus are intended to provide inexpensive solutions for problems
involving part-through surface cracks in shell structures loaded predominantly in Mode I by combined
membrane and bending action in cases where it is important to include the effects of inelastic deformation.
This example illustrates the use of these elements. The case considered is a long cylinder with an axial flaw
in its inside surface, subjected to internal pressure. It is taken from the paper by Parks and White (1982).
When the line spring element model reaches theoretical limitations, the shell-to-solid submodeling
technique is utilized to provide accurate -integral results. The energy domain integral is used to evaluate
the J-integral for this case.
Geometry and model
The cylinder has an inside radius of 254 mm (10 in), wall thickness of 25.4 mm (1 in), and is assumed
to be very long. The mesh is shown in Figure 1.4.3–1. It is refined around the crack by using multipoint constraints (MPCs). There are 70 shell elements of type S8R in the symmetric quarter-model and
eight symmetric line spring elements (type LS3S) along the crack. The mesh is taken from Parks and
White, who suggest that this mesh is adequately convergent with respect to the fracture parameters (Jintegral values) that are the primary objective of the analysis. No independent mesh studies have been
done. The use of MPCs to refine a mesh of reduced integration shell elements (such as S8R) is generally
satisfactory in relatively thick shells as in this case. However, it is not recommended for thin shells
because it introduces constraints that “lock” the response in the finer mesh regions. In a thin shell case
the finer mesh would have to be carried out well away from the region of high strain gradients.
Three different flaws are studied. All have the semi-elliptic geometry shown in Figure 1.4.3–2,
with, in all cases,
The three flaws have
ratios of 0.25 (a shallow crack), 0.5, and 0.8 (a
deep crack). In all cases the axial length of the cylinder is taken as 14 times the crack half-length, : this
is assumed to be sufficient to approximate the infinite length.
An input data file for the case
.5 without making the symmetry assumption about
0
is also included. This mesh uses the LS6 line spring elements and serves to check the elastic-plastic
capability of the LS6 elements. The results are the same as for the corresponding mesh using LS3S
elements and symmetry about
0. The formulation of the LS6 elements assumes that the plasticity
is predominately due to Mode I deformation around the flaw and neglects the effect of the Mode II
and Mode III deformation around the flaw. In the global mesh the displacement in the -direction is
constrained to be zero at the node at the end of the flaw where the flaw depth goes to zero. To duplicate
this constraint in the mesh using LS6 elements, the two nodes at the end of the flaw (flaw depth = 0) are
constrained to have the same displacements.
1.4.3–1
Abaqus Version 6.12 ID:
Printed on:
INELASTIC LINE SPRING
Material
The cylinder is assumed to be made of an elastic-plastic metal, with a Young’s modulus of 206.8 GPa
(30 × 106 lb/in2 ), a Poisson’s ratio of 0.3, an initial yield stress of 482.5 MPa (70000 lb/in2 , and constant
work hardening to an ultimate stress of 689.4 MPa (105 lb/in2 ) at 10% plastic strain, with perfectly plastic
behavior at higher strains.
Loading
The loading consists of uniform internal pressure applied to all of the shell elements, with edge loads
applied to the far end of the cylinder to provide the axial stress corresponding to a closed-end condition.
Even though the flaw is on the inside surface of the cylinder, the pressure is not applied on the exposed
crack face. Since pressure loads on the flaw surface of line spring elements are implemented using linear
superposition in Abaqus, there is no theoretical basis for applying these loads when nonlinearities are
present. We assume that this is not a large effect in this problem. For consistency with the line spring
element models, pressure loading of the crack face is not applied to the shell-to-solid submodel.
Results and discussion
The line spring elements provide J-integral values directly. Figure 1.4.3–3 shows the -integral values at
the center of the crack as functions of applied pressure for the three flaws. In the input data the maximum
time increment size has been limited so that adequately smooth graphs can be obtained. Figure 1.4.3–4
shows the variations of the -integral values along the crack for the half-thickness crack (
0.5), at
several different pressure levels (a normalized pressure,
, is used, where is the mean radius
of the cylinder). These results all agree closely with those reported by Parks and White (1982), where
the authors state that these results are also confirmed by other work. In the region
30° the results
are inaccurate for two reasons. First, the depth of the flaw is changing very rapidly in this region, which
makes the line spring approximation quite inaccurate. Second,
is of the same order of magnitude as
, but the line spring plasticity model is only valid when
The results toward the center
of the crack (
30°) are more accurate than those at the ends of the crack since the flaw depth changes
less rapidly with position in this region and
is much larger than
For this reason only J values for
30° are shown in Figure 1.4.3–4.
Shell-to-solid submodeling around the crack tip
An input file for the case
0.25, which uses the shell-to-solid submodeling capability, is included.
This C3D20R element mesh allows the user to study the local crack area using the energy domain integral
formulation for the -integral. The submodel uses a focused mesh with four rows of elements around the
crack tip. A 1/r singularity is utilized at the crack tip, the correct singularity for a fully developed perfectly
plastic solution. Symmetry boundary conditions are imposed on two edges of the submodel mesh, while
results from the global shell analysis are interpolated to two surfaces via the submodeling technique. The
global shell mesh gives satisfactory J-integral results; hence, we assume that the displacements at the
submodel boundary are sufficiently accurate to drive the deformation in the submodel. No attempt has
1.4.3–2
Abaqus Version 6.12 ID:
Printed on:
INELASTIC LINE SPRING
been made to study the effect of making the submodel region larger or smaller. The submodel is shown
superimposed on the global shell model in Figure 1.4.3–5.
In addition, an input file for the case
0.25, which consists of a full three-dimensional C3D20R
solid element model, is included for use as a reference solution. This model has the same general
characteristics as the submodel mesh. See inelasticlinespring_c3d20r_ful.inp for further details about
this mesh. One important difference exists in performing this analysis with shell elements as opposed to
continuum elements. The pressure loading is applied to the midsurface of the shell elements as opposed to
the continuum elements, where the pressure is accurately applied along the inside surface of the cylinder.
For this analysis this discrepancy results in about 10% higher J-integral values for the line spring shell
element analysis as compared to the full three-dimensional solid element model.
Results from the submodeled analyses are compared to the LS3S line spring element analysis and
full solid element mesh for variations of the J-integral values along the crack at the a normalized pressure
loading of
0.898, where is the mean radius of the cylinder. As seen in Figure 1.4.3–6, the
line spring elements underestimate the -integral values for
50° for reasons described previously.
Note that at
0° the J-integral should be zero due to the lack of crack-tip constraint at the cylinder
surface. A more refined mesh would be required to model this phenomenon properly. It is quite obvious
that the use of shell-to-solid submodeling is required to augment a line spring element model analysis to
obtain accurate -integral values near the surface of the cylinder.
Input files
inelasticlinespring_05.inp
inelasticlinespring_05_nosym.inp
inelasticlinespring_progcrack.f
inelasticlinespring_025.inp
inelasticlinespring_08.inp
inelasticlinespring_c3d20r_sub.inp
inelasticlinespring_c3d20r_ful.inp
0.5.
0.5 without the symmetry assumption across
0, using line spring element type LS6.
A program used to create a data file giving the flaw depths
as a function of position along the crack.
Shallow crack case,
0.25.
Deep crack case,
0.8.
C3D20R (
0.25) submodel.
C3D20R (
0.25) full model.
Reference
•
Parks, D. M., and C. S. White, “Elastic-Plastic Line-Spring Finite Elements for Surface-Cracked
Plates and Shells,” Transactions of the ASME, Journal of Pressure Vessel Technology, vol. 104,
pp. 287–292, November 1982.
1.4.3–3
Abaqus Version 6.12 ID:
Printed on:
INELASTIC LINE SPRING
z
y
x
Figure 1.4.3–1
Finite element model for an axial flaw in a pressurized cylinder.
1.4.3–4
Abaqus Version 6.12 ID:
Printed on:
INELASTIC LINE SPRING
t
a0
φ
c
a0 = maximum flaw depth
2c = surface length of crack
t = shell thickness
φ = angle on an inscribed circle for locating a
point on the crack
Figure 1.4.3–2
Schematic of a semi-elliptical surface crack.
1.4.3–5
Abaqus Version 6.12 ID:
Printed on:
INELASTIC LINE SPRING
20
LINE
1
2
3
ABSCISSA
VARIABLE
Load
(*+1.5E-04)
Load
(*+1.5E-04)
Load
(*+1.5E-04)
ORDINATE
VARIABLE
J for a=.5
(*+6.1E-03)
J for a=.25
(*+6.1E-03)
J for a=.8
(*+6.1E-03)
15
Normalized J
3
10
2
3
5
1
3
1
3
1
2
3
1
0
0
Figure 1.4.3–3
4
1
2
1
8
Normalized Load
2
12
(*10**-1)
Normalized J-integral values
versus normalized applied pressure
, where is the mean radius of the cylinder.
5
(*10**1)
LINE
1
2
3
3
ABSCISSA
ORDINATE
VARIABLE
VARIABLE
Norm. Angle
J
for Normalized Load = .574
Norm. Angle
J
for Normalized Load = 1.097
Norm. Angle
J
for Normalized Load = 1.172
3
4
3
Normaized J
3
2
1
2
2
2
1
0
0
Figure 1.4.3–4
surface given by
2
1
4
6
Position along Flaw
1
8
10
(*10**-1)
Normalized J-integral values
versus position along the flaw
, for
0.5, and normalized applied pressures
= .574,
is the mean radius of the cylinder.
1.097, and 1.172.
1.4.3–6
Abaqus Version 6.12 ID:
Printed on:
INELASTIC LINE SPRING
3
2
1
3
1
2
Figure 1.4.3–5
Solid submodel superimposed on shell global model.
1.4.3–7
Abaqus Version 6.12 ID:
Printed on:
INELASTIC LINE SPRING
Line Springs
Full 3D Solid
Solid Submodel
Normalized J
0.6
XMIN
XMAX
YMIN
YMAX
0.4
0.2
0.000E+00
1.000E+00
1.086E-01
7.317E-01
0.0
0.2
0.4
0.6
0.8
Normalized Flaw Position
Figure 1.4.3–6 Normalized J-integral values
versus position along the flaw surface given by
0.25 and at the normalized pressure.
is the mean radius of the cylinder.
1.4.3–8
Abaqus Version 6.12 ID:
Printed on:
for
0.898.
1.0
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
1.4.4
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
Product: Abaqus/Standard
This example illustrates the modeling of crack length versus time to simulate crack propagation and the use
of crack opening displacement as a crack propagation criterion. For stable crack growth in ductile materials,
experimental evidence indicates that the value of the crack opening displacement (COD) at a specified distance
behind the crack tip associated with ongoing crack extension is usually a constant. Abaqus provides the critical
crack opening displacement, at a specified distance behind the crack tip, as a crack propagation criterion. The
other crack propagation model used in this example—prescribed crack length versus time—is usually used
to verify the results obtained from experiments. Abaqus also provides the critical stress criterion for crack
propagation in brittle materials.
In this example an edge crack in a three-point bend specimen is allowed to grow based on the crack
opening displacement criterion. Crack propagation is first modeled by giving the crack length as a function
of time. The data for the crack length are taken from Kunecke, Klingbeil, and Schicker (1993). The data
for the crack propagation analysis using the COD criterion are taken from the first analysis. This example
demonstrates how the COD criterion can be used in stable crack growth analysis.
Problem description
An edge crack in a three-point bend specimen in plane strain, subjected to Mode I loading, is considered
(see Figure 1.4.4–1). The crack length to specimen width ratio is 0.2. The length of the specimen is
55 mm, and its width is 10 mm. The specimen is subjected to bending loads such that initially a wellcontained plastic zone develops for the stationary crack. Subsequently, the crack is allowed to grow.
Geometry and model
Due to symmetry only one-half of the specimen is analyzed. The crack tip is modeled as initially blunted
so that finite deformation effects near the crack tip can be taken into account (geometric nonlinearities
considered in the step). The mesh is composed of 1737 CPE4 elements (Figure 1.4.4–2). A reasonably
fine mesh, necessary to obtain a smooth load versus crack length relation, is used to model the area in
which the plastic zone grows and crack propagation occurs. The loading point and the support points for
the specimen are simulated by analytical rigid surfaces, as shown in Figure 1.4.4–2.
Material
The material is assumed to be elastic-plastic, with a Young’s modulus of
ratio of 0.3. The plastic work hardening data are given in Table 1.4.4–1.
200 GPa and Poisson’s
Loading and solution control
The analysis is carried out in two stages. The first stage consists of pushing the rigid surface 1.0 mm into
the specimen. No crack growth is specified during this stage.
1.4.4–1
Abaqus Version 6.12 ID:
Printed on:
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
In the second stage the crack is allowed to propagate while the rigid surface is moved an additional
1.951 mm.
Once a crack-tip node debonds, the traction at the tip is initially carried as a reaction force at
that node. This force is ramped down to zero according to the amplitude curve specified in the crack
propagation analysis. The manner in which the forces at the debonded nodes are ramped down greatly
influences the convergence of the solution. The convergence of the solution is also affected by reversals
in plastic flow due to crack propagation. In such circumstances, very small time increments are required
to continue the analysis. In the present analysis solution controls are defined on the displacement field
and on the warping degree of freedom equilibrium equations to relax the tolerances so that more rapid
convergence is achieved. Because of the localized nature of the nonlinearity in this problem, the resulting
loss of accuracy is not significant. The definition of solution controls is generally not recommended.
Crack length versus time
In the case when the crack length is given as a function of time, the second step in the analysis consists
of letting the crack grow according to a prescribed crack length versus time relationship, using the data
taken from Kunecke, Klingbeil, and Schicker.
COD criterion
The loading of the specimen and the specification of the COD criterion for crack growth demonstrates
the flexibility of the critical crack opening displacement criterion. Frequently, the crack opening
displacement is measured at the mouth of the crack tip: this is called the crack mouth opening
displacement (CMOD). The crack opening displacement can also be measured at the position where
the initial crack tip was located. Alternatively, the crack-tip opening angle (CTOA), defined as the
angle between the two surfaces at the tip of the crack, is measured. The crack-tip opening angle can be
easily reinterpreted as the crack opening at a distance behind the crack tip. In this example the COD
specification required to use both the CMOD and the CTOA criteria is demonstrated.
For the purposes of demonstration the crack opening displacement at the mouth of the crack is used
as the initial debond criterion. The first three nodes along the crack propagation surface are allowed
to debond when the crack opening displacement at the mouth of the crack reaches a critical value. To
achieve this, the following loading sequence is adopted: in Step 1, the specimen is loaded to a particular
value (crack propagation analysis is not used), and in Step 2 the first crack-tip node is allowed to debond
(crack propagation analysis is used). Steps 3 and 4 and Steps 5 and 6 follow the same sequence as Steps 1
and 2 so that the two successive nodes can debond. Since, the crack opening displacement is measured at
the mouth of the crack, the value of the distance behind the crack tip along the slave surface is different
in Steps 2, 4, and 6.
The loading sequence adopted above outlines a way in which the CMOD measurements can be
simulated without encountering the situation in which the COD is measured beyond the bound of the
specimen, which would lead to an error message. In this example, the loads at which the crack-tip
nodes debonded were known a priori. In general, such information may not be available, and the restart
capabilities in Abaqus can be used to determine the load at which the fracture criterion is satisfied.
The remaining bonded nodes along the crack propagation surface are allowed to debond based
on averaged values of the crack-tip opening angles for different accumulated crack lengths. The data
1.4.4–2
Abaqus Version 6.12 ID:
Printed on:
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
prescribed under the crack propagation criteria in Step 7 are the crack opening displacement values
that were computed from the crack-tip opening angles observed in the analysis that uses the prescribed
crack length versus time criterion. These crack-tip opening angles are converted to critical crack opening
displacements at a fixed distance of 0.04 mm behind the crack tip. Hence, the crack opening displacement
is measured very close to the current crack tip.
Results and discussion
Figure 1.4.4–3 shows a plot of the accumulated incremental crack length versus time. The user-specified
data, as well as the results obtained from the finite element analysis based on the two criteria, are plotted.
Good agreement is observed between the user input values and the results from the analysis. The curve
based on the COD criterion does not correspond with the user-specified data toward the end of the analysis
because an average crack opening displacement was assumed.
Figure 1.4.4–4 shows the reaction force at the node where the displacements are applied as a function
of the accumulated incremental crack length, obtained from the analysis in which the crack length was
specified as a function of time. The curve obtained when the COD criterion is used is almost identical
and is not shown in this figure.
Figure 1.4.4–5 depicts the variation of the reaction force as a function of the displacement at the
rigid body reference node.
The contours of equivalent plastic strain in the near crack-tip region for two different crack advance
positions are shown in Figure 1.4.4–6 and Figure 1.4.4–7. Contours of the Mises equivalent stress at the
final stage of the analysis are shown in Figure 1.4.4–8.
Input files
crackgrowth_lengthvtime.inp
crackgrowth_cod.inp
crackgrowth_model.inp
Analysis with the crack length versus time criterion.
Analysis with the COD criterion.
Model data for the two analysis files.
Reference
•
G. Kunecke, D. Klingbeil, and J. Schicker, “Rißfortschrittssimulation mit der ABAQUS-option
DEBOND am Beispiel einer statisch belasteten Kerbschlagbiegeprobe,” presented at the ABAQUS
German Fracture Mechanics group meeting in Stuttgart, November 1993.
1.4.4–3
Abaqus Version 6.12 ID:
Printed on:
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
Table 1.4.4–1
Stress-strain data for isotropic plastic behavior.
True Stress
(MPa)
True Strain
461.000
472.810
521.390
628.960
736.306
837.413
905.831
1208.000
0.0
0.0187
0.0280
0.0590
0.1245
0.2970
0.5756
1.9942
1.4.4–4
Abaqus Version 6.12 ID:
Printed on:
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
55 mm
w = 10 mm
a0 = 2 mm
43 mm
Figure 1.4.4–1
Schematic of the three-point bend specimen.
2
3
1
Figure 1.4.4–2
Finite element mesh for the three-point bend specimen.
1.4.4–5
Abaqus Version 6.12 ID:
Printed on:
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
2.0
User data
CRACK LENGTH
COD
crack length in mm
1.6
1.2
0.8
0.4
XMIN
XMAX
YMIN
YMAX
1.000E+00
2.951E+00
1.000E-09
2.188E+00
0.0
1.0
1.5
2.0
2.5
3.0
total time
Figure 1.4.4–3
Accumulated incremental crack length versus time.
18.
[ x10 3 ]
rf1@9997_vs_dbdela
reaction force in N
16.
14.
12.
XMIN
XMAX
YMIN
YMAX
2.829E-02
2.188E+00
1.100E+04
1.606E+04
10.
0.0
0.4
0.8
1.2
1.6
2.0
cumulative crack length in mm
Figure 1.4.4–4
Variation of the reaction force as a function of the cumulative crack length.
1.4.4–6
Abaqus Version 6.12 ID:
Printed on:
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
[ x10 3 ]
15.
reaction force in N
rf1_vs_u1 @9997
XMIN
XMAX
YMIN
YMAX
1.000E-03
2.951E+00
6.931E+01
1.606E+04
10.
5.
0.
0.0
0.5
1.0
1.5
2.0
2.5
3.0
displacement in mm
Figure 1.4.4–5
PEEQ
Variation of the reaction force as a function of displacement.
VALUE
+0.00E-00
+5.30E-02
+1.06E-01
+1.59E-01
+2.12E-01
+2.65E-01
+3.18E-01
+3.71E-01
+4.24E-01
+4.77E-01
+5.30E-01
+5.84E-01
+6.37E-01
+6.90E-01
2
3
1
Figure 1.4.4–6
Plastic zone for an accumulated crack length of 1.03 mm.
1.4.4–7
Abaqus Version 6.12 ID:
Printed on:
CRACK GROWTH IN A THREE-POINT BEND SPECIMEN
PEEQ
VALUE
+0.00E-00
+5.30E-02
+1.06E-01
+1.59E-01
+2.12E-01
+2.65E-01
+3.18E-01
+3.71E-01
+4.24E-01
+4.77E-01
+5.30E-01
+5.84E-01
+6.37E-01
+6.90E-01
2
3
1
Figure 1.4.4–7
MISES
Plastic zone for an accumulated crack length of 2.18 mm.
VALUE
+9.24E+00
+9.20E+01
+1.74E+02
+2.57E+02
+3.40E+02
+4.23E+02
+5.06E+02
+5.89E+02
+6.71E+02
+7.54E+02
+8.37E+02
+9.20E+02
+1.00E+03
+1.08E+03
2
3
Figure 1.4.4–8
1
Contours of Mises stress for an accumulated crack length of 2.18 mm.
1.4.4–8
Abaqus Version 6.12 ID:
Printed on:
SKIN-STIFFENER DEBONDING
1.4.5
ANALYSIS OF SKIN-STIFFENER DEBONDING UNDER TENSION
Product: Abaqus/Standard
This example illustrates the application of cohesive elements in Abaqus to predict the initiation and
progression of debonding at the skin-stiffener interface in stiffened panels, which is a common failure mode
for this type of structure. The particular problem considered here is described in Davila (2003); it consists
of a stringer flange bonded onto a skin, originally developed by Krueger (2000). The results presented
are compared against the experimental results presented in Davila (2003). The problem is analyzed in
Abaqus/Standard using a damaged, linear elastic constitutive model for the skin/stiffener interface.
Geometry and model
The problem geometry and loading are depicted in Figure 1.4.5–1: a 203-mm-long and 12.7-mm-wide
specimen with a total skin thickness of 2.632 mm and maximum flange thickness of 1.88 mm, loaded in
tension along the length direction. For the model in which the loading is simulated through prescribed
displacements, the free gauge length is 127 mm. The skin thickness direction is comprised of 14
composite plies; while the flange is made up of 10 plies, each having a uniform thickness of 0.188 mm.
The finite element mesh for the three-dimensional model of the debonding problem is identical to
that used in Davila (2003) except that the “decohesion” elements utilized in that reference to represent
the skin/flange interface are replaced with Abaqus cohesive elements. Both the skin and the flange are
modeled by two layers each of C3D8I elements. The interface between them is represented by COH