CFD-Based Hydrodynamic Analysis of High Performance Racing Yachts

3rd High Performance Yacht Design Conference Auckland, 2-4 December, 2008 CFD-BASED HYDRODYNAMIC ANALYSIS OF HIGH PERFORMANCE RACING YACHTS Len Imas 1 , Len.Imas@stevens.edu Gregory Buley 2 , Greg.Buley@cdicorp.com Bryan Baker 3 , bryan@farrdesign.com Britton Ward 4 , britton@farrdesign.com Abstract. Advances in Navier-Stokes solver technology have enabled naval architects and hydrodynamicists to implement high fidelity CFD models as a means of analyzing complex flows around high performance racing yachts. As a consequence, recent research activity in this area has increased and the associated results have contributed to enlarging the boundaries of the design spaces being explored. This paper will present selected examples from a research study based around tow tank tests and CFD simulations of a canonical high-performance racing yacht. The geometry configuration studied was fully appended with rudders, keel/bulb and a dagger-board. Simulations were performed under a multitude of sailing conditions covering both lifting and non-lifting flow regimes. Topics covered will address (i) validation against tow tank measurements; (ii) efficient performance of large-scale computations; and (iii) numerical issues related to (a) mesh generation, (b) solution, discretization, and free surface capturing algorithms, (c) turbulence modelling, (d) rigid body dynamics and sail force models. 1. INTRODUCTION Simulation of free-surface hydrodynamics of a fullyappended sailing yacht has been undertaken in various studies utilizing Navier-Stokes based CFD solvers with varying degree of quantitative success. A number of factors related to the formulation of the transport equations in the solver, numerical solution algorithm, and computational mesh type and quality, contribute to the accuracy and validity of the solution. To fully assess the importance of multiple free variables in the set-up of a numerical solution requires systematic studies which themselves may be time and cost-prohibitive and require large computational resources. In this paper, we present an assessment and a discussion of factors that we believe are relevant to a successful cfd-based hydrodynamic analysis of a sailing yacht in a context of several examples. In our study, we simulate the hydrodynamics of a canonical ocean-going fully-appended racing yacht geometrically similar to that depicted in Figure 1 and make comparisons to tow tank measurements [2, 3]. In the simulations, which are performed over a range of upwind and downwind sailing conditions, the yacht is free to sink and trim, and the appendage angles of attack are adjusted according to the yacht’s heel and leeway angles relative to the boat track. In addition to validating our results against experimental data, we also study the accuracy with which both resistance (drag) and side force (lift) may be predicted on a fully-appended boat configuration and whether computations may be carried out utilizing an 1 2 3 4 unstructured mesh topology rather than a more traditional simulation approach, which makes of use of curvilinear or fully-hexahedral block-structured meshes. Figure 1. An Open 60 racing yacht [1] Lastly, we discuss several details hydrodynamic phenomena observed in simulation results, the relevance of the numerical solution scheme, and hydrodynamic load predictions. 2. PROBLEM DEFINITION AND APPROACH 2.1 Geometry At full-scale, our canonical racing yacht has a lengthoverall of approximately 21 meters and a maximum beam of approximately 5.5 meters, with a flotation weight of approximately 14000 kg. The yacht geometry consists of a transom-stern hull with a dual rudder system, a canting keel, and port and starboard canards. During the study, multiple appendage configurations were considered. Associate Professor Davidson Laboratory, Stevens Institute of Technology Senior Engineer, CDI Marine Company, Band Lavis Division Naval Architect, Farr Yacht Design Senior Naval Architect, Farr Yacht Design 130 of modelled the presented corresponding accuracy of 2.4 Grid The simulations were performed on unstructured hybrid meshes consisting of tetrahedral and prismatic elements in the mesh volume, including both the yacht’s boundary layer and the far-field. The surface mesh on the hull and appendages comprised triangular elements. The grid generation was performed using Pointwise Gridgen [4]. Figure 2. Canonical yacht geometry with starboard canard deployed and keel canted to port The yacht top-sides in the hydrodynamic model were represented by a sealed deck. The overall configuration is depicted in a CAD schematic shown in Figure 2. 2.2 Sailing Conditions Simulations are performed over a range of upwind and downwind sailing conditions where boat speeds vary from 5 knots to 30+ knots; heel angles range from 0 degrees to 20+ degrees; and yaw angles range from 0 degrees to 3+ degrees. Corresponding keel cant angles vary between 0 and 40 degrees while rudder angles range between 0 and 3+ degrees. Results presented here are for calm water conditions, i.e., no incident wave field is present. 2.3 Computational Domain For the simulation results presented, the computational domain is a rectangular bounding box, analogous to that shown in Figure 3. The extents of the domain are set so as to minimize reflections of waves generated by the advancing hull and to position the yacht sufficiently far from the inlet / outlet planes in order to minimize the effect of far-field boundary conditions on the near-field flow around the hull. While it is common practice to pay more attention to the former rather than the latter in freesurface computation, if solution accuracies on the O(1%) are required, care should also be taken with far-field boundary condition positioning relative to the yacht model. Figure 3. Canonical computational domain around a halfship body [5] In parametric studies involving large numbers of geometric configurations, the hybrid mesh approach is more attractive because it lends itself more readily to automation. Namely, the grid generation process may be scripted to the extent where the procedures of importing the CAD geometry into the meshing tool and preparing the surface and volume meshes is executed with minimal human intervention. Furthermore, and more importantly, the unstructured mesh approach is attractive when one considers the meshing requirements for appendages / lifting surfaces. Namely, to adequately predict the side (or lift) and drag forces acting on appendages or the hull, the representative length scale of the surface mesh resolution at and near the leading and trailing edges of the geometry in question must be at least an order of magnitude finer compared to the maximum allowable on that surface. While such meshing requirements can be achieved with structured mesh topologies, they will lead to an appreciably larger element count driving up the computational cost. As one consequence of this, what is often observed in structured mesh computations, are under-resolved solutions, leading to incorrect load predictions. A near wall boundary-layer grid with between 20 - 30 cells was formed around the entire yacht body, with a y+ value of the first grid point being O(10). For resolution of the boundary-layer then, wall-functions are deployed with the turbulence model. In simulated cases where investigating boundary layer transition was of interest, y+ value of the first grid point was reduced to O(1). The later was driven by the transitional turbulence model requirements. The surface mesh length scales at and near leading and trailing edges of appendages were further constrained by mesh element aspect ratios in the boundary layer. Namely, in the computations performed, maximum aspect ratios in the grid were constrained to O(1000) or less. To properly resolve the free-surface flow field, additional attention must be given to designing the mesh around the free-surface region. There are two aspects to this problem, one dealing with resolution normal to the mean water line, the other being the resolution parallel to and in the mean water line plane itself. The result is a pancake-type mesh layer, shown in Figure 3, which wraps around the mean water-line and yacht. The normal spacing requirement is dictated by anticipated crest and trough heights of waves generated 131 by the yacht in the near field and wake. Typically, 20 – 30 unequally-spaced points were used in the normal direction, with the minimum spacing based on Froude and Weber number considerations. The in-line spacing is dictated by the wavelength of the yacht-generated waves, hence the speed of the yacht. In the simulations performed, the yacht was permitted to dynamically sink and trim, therefore the computational grid has to be developed in a manner so as to allow for body motion. The approach taken in this regard is determined by the solver and mesh motion algorithm being used. This aspect of the simulation model is discussed in the following section. The mesh topology used to generate the presented results consisted of a two part grid; a rigid part which undergoes the same rigid body motions as the yacht and a moving part, which undergoes motions relative to the yacht. Grid quality was controlled by not permitting the mesh to deform near the body while far away from the body, mesh deformation was permitted. In dealing with grid deformation, grid quality was insured by appropriately designing the grid to fit the problem being simulated. The simulation grids for which results are shown typically consisted of about 6 - 8 million elements. This resolution was arrived upon in part based on mesh specifications outlined above and in part based on the computational resources that were being deployed in this study. 2.5 Solution method Computations were performed using Ansys CFX, a general finite-volume Navier-Stokes solver [6, 7]. Turbulence treatment was uRANS-based using a two transport equation kω SST (shear stress transport) type model with automatic wall functions. The automatic wall function formulation dynamically switches between the low Reynolds number formulation and a wall function formulation depending on the locally computer y+. When transitional turbulence physics were considered, additional transport equations for transitional flow transport were solved. No wall functions were employed in transitional flow computations. The selection of the turbulence model was based on physical considerations related to the flow around the yacht and results of a turbulence model sensitivity study performed by the authors. For the two-phase (air/water) flow with a free-surface, a homogeneous multiphase model based on a compressive volume of fluid type scheme was used. High order spatial discretization was employed in all equations. The turbulence and volume fractions equations are solved together with the momentum equations in a coupled (vs. segregated) manner. The coupled solution algorithm significantly improved convergence rates while reducing overall computational time. Unstructured meshes have in the past been employed in free-surface RANS finite volume computations using both interface tracking and 132 interface capturing methods. However, results obtained with tracking schemes have typically been of limited value since mesh deformation prevented simulation of flow fields with wave breaking and limited analysis to relatively low Froude numbers and/or simple hull topologies. Results previously obtained with capturing schemes have demonstrated that volume of fluid methods, when employed on unstructured grids, yielded mixed results because of numerical free surface wave diffusion and body surface smearing. In this work, we have revisited the technical problems previously observed in interface capturing methods on unstructured grids, within the framework of the tools we employed. To simulate yacht motions, two approaches were considered: a fully unsteady time-accurate pitch and heave motion solution using a 6dof rigid body motion solver and a quasi-steady force/moment balance iteration for sink and trim. In the results presented, since only the steady-state boat position was of interest, the latter approach was employed. The quasi-steady iterative solution was determined to be computationally less expensive in comparison to the former and for the iterative procedure itself, an algorithm was developed that optimized convergence rates based on Froude number, thereby further decreasing the run-time. The corresponding mesh-motion solution made use of a mesh deformation scheme based on a spring-type deformation approach. The rigid mesh motion was coupled to the deforming mesh though sliding and joined interfaces. While this approach was chosen in part based on solver capabilities available in CFX, the authors believe that in comparison to mesh motion treatments involving rigidly moving the entire computational domain, the presently-employed method allows for computations to be performed at larger time-steps (or fewer iterations) and reduces numerical stiffness issues associated with boundary conditions where the freesurface may not be near-normal to the inflow/outflow planes. Mesh domain partitioning was performed using a directionally-dominant partitioning method. The partitioning direction was chosen relative to the orientation of the free-surface. The simulations were performed as distributed-parallel using HPMPI. The computing cluster CPU and O/S are 64bit based. A gigabit backbone for inter-node communications was used. Anywhere from 8 to 24 processors were employed per calculation. In addition to the decay in transport equations’ residuals, the convergence of the calculations was judged based upon the convergence of the hydrodynamic loads. A typical convergence history is illustrated in Figure 4. Figure 4. Convergence of the differential in the vertical hydrodynamic force (left) and convergence of the pitching moments, showing the convergence of the pressure and viscous components of pitching moment Figure 4 shows the convergence of the differential between the vertical hydrodynamic force and weight as a measure of sink convergence and the convergence of the hydrodynamic pitch moment as a measure of trim convergence 3. DISCUSSION OF RESULTS The hydrodynamic complexity of the flow field around a modern ocean-going racing yacht is evident from the flow visualization shown in Figure 5. a boundary layer solver), Navier-Stokes (NS) based interface capturing solutions lend themselves more readily to simulation of the necessary physics. The result illustrated in Figure 5 shows the free-surface near-field around one of the configurations analyzed. The dynamic Cp contours on the surface of the hull are also shown. Some of the salient features that can be seen in the visualization are a semi-planning hull with bow wave breaking near the bow, separated stern flow, and appendages that are either surface-piercing or operating in very close proximity to the free-surface. While such phenomena have been resolved with non-NS based methods, numerical stiffness of the resulting solution scheme, variable solution accuracy, and limited ability to adequately represent viscous and multiphase effects, and free surface nonlinearities do not justify the lower computational overheads associated with such methods. Instead, NS solutions, while more computationally expensive and geometrically-complex in terms of mesh development, lend themselves more directly to simulation of such phenomena. Furthermore, increase in computational hardware performance, decrease in its cost, and advances in solver technology now permit for large-scale NS-based simulations to be performed efficiently. From our study, we present two sets of results; the first addressing resistance of an appended yacht sailing upright without any side force generation. This part of study is therefore concerned primarily with resolving the boundary layer and wave systems, including the bow and stern flows, generated by the hull. We simulate the model-scale canonical yacht at full Froude scale and make comparisons of the resulting resistance with tow tank measurements [2] made at same scale. 0.22 0.20 Drag (N) / Displacement (N) Oceanic TT Immersion Deep Figure 5a. Canonical yacht sailing upwind at high speed; bow view. 0.18 Oceanic TT Immersion Deeper 0.16 Oceanic TT Immersion Deepest CFX Immersion Deep 0.14 CFX Immersion Deeper 0.12 CFX Immersion Deepest 0.10 0.08 0.06 0.04 0.02 0.00 0 5 10 15 20 25 30 Vs Full Scale (knots) Figure 6. Upright resistance; comparison of CFD model vs. tow-tank data taken at 1/3 scale. Figure 5b. Canonical yacht sailing upwind at high speed; stern view. In comparison to more traditional analysis methods (e.g. potential flow panel method solution, possibly coupled to Results given in Figure 6 show a comparison between results obtained with our CFD model and those measured in the tank. In relative terms, the agreement between the two sets of results is on O(1%). In the plotted comparison, results are presented for three different transom immersions and the resistance is normalized by the yacht displacement. 133 The second part of the study addresses hydrodynamic loads acting on a sailing yacht sailing with heel and leeway. Hence, both drag and lift are present. We simulate the full-scale canonical yacht and make comparisons of the resulting loads to tow tank measurements [3] adjusted to full-scale. Figures 7 and 8 show flow visualizations of the results from one of the canonical yachts simulated. In the configuration shown in Figure 7, the daggerboard is deployed while in the configurations shown in Figure 8, no daggerboard is deployed. Differences in heel, yaw, sink, and trim between the two conditions are also evident. The corresponding free-surface is coloured by wave elevation amplitude with red indicating higher than static water line and blue indicating lower than the static water line. Figure 9 shows the computed variation in side force and resistance as a function of yaw angle for a given boat speed heel. Comparisons to tank measurements are also shown. Like in the upright results, the agreement shown is again of O(1%). In our model, the increase in error at large negative leeway may be attributed due to asymmetry in mesh resolution between port and starboard and relative to the oncoming flow as a consequence of appendage orientation. Consequently, the volumetric mesh distribution was redesigned to address this shortcoming. While boundary layer stimulation is employed in modeltests to generate fully turbulent boundary layers and minimize flow laminarization (even though the model is not Reynolds number scaled), it has also been observed to modify both drag and measured side force in a manner that is both scale-dependent and dependent on the type of stimulation used. To reduce uncertainty in comparisons of numerical and experimental data, the stimulation effect should be accounted for. In the context of the results and comparisons presented, the current study also considered the role of boundary layer stimulation at tow-tank model-scale and how it is accounted for in CFD vs. experiment comparisons. From the standpoint of CFD simulations, one can either simulate the flow at full-scale; at model-scale without including the effect of stimulation in the CFD model; or with the inclusion of stimulation in the CFD model. The latter can be done implicitly or explicitly depending on the numerical algorithm capabilities of the solver used. Consequently, depending on whether full-scale or modelscale simulations are performed, CFD results can be compared to measurements made at model-scale or comparisons can be made to model-scale data scaled to full-scale. Either way, if the contribution to the hydrodynamic loads due to presence of stimulation is not accounted for, it is unrealistic to expect quantitativelyacceptable agreement or even agreement in trends. Lack of including such a correction in the comparison, can 134 lead to observations of erroneous trends in measured data or conclusions indicating poor CFD solutions. One example where attention to this detail is important is analysis of attachment / separation streamlines. Surface streamlines for one particular configuration are shown in Figure 10. Figure 7. Flow visualization of yacht sailing with heel and yaw, no canard deployed. Figure 8. Flow visualization of yacht sailing with heel and yaw, with canard deployed. 135 • side force vs. yaw angle 20 deg heel and 14 knots • side force (N) 80000 70000 60000 50000 40000 30000 20000 CFD TANK 10000 0 -3 -2 -1 0 1 2 3 4 5 yaw (deg) Figure 9a. Side force vs. yaw; comparison of CFD results vs. tow-tank data taken at 1/9th scale. drag vs. side force 20 deg heel and 14 knots 20000 sink and trim convergence criteria were based on Froude number existing procedures for comparisons of simulation and measured data were extended to account for additional physics It is anticipated that future directions in this research area will focus in the following: • continue to expand on the fidelity of physics being resolved in the simulation models: ƒ unsteady and highly nonlinear flow effects ƒ nonhomogeneous multiphase effects ƒ multi-dof rigid and elastic body dynamics • further exploration and extension of the existing mesh generation and solver strategies total drag (N) 18000 16000 CFD TANK 14000 12000 10000 8000 0 10000 20000 30000 40000 50000 60000 70000 80000 side force (N) Figure 9b. Drag force vs. side force; comparison of CFD results vs. tow-tank data taken at 1/9th scale. Figure 10. Separation and attachment surface streamlines on yacht hull. 4. CONCLUSIONS Based on the results obtained in this study, we observe the following about our solution methodology: • • utilizing an unstructured mesh topology in our simulations, rather than a more traditional grid generation approach, permits us to achieve the necessary free-surface resolution and volume fraction fidelity while allowing for a much more direct manner in which: ƒ mesh resolution requirement for both resistance and drag may be met ƒ meshing procedures, for parametrically varying the geometric topology of the sailing configurations being analyzed, may be established use of a coupled solver improves convergence performance across all Froude numbers 136 CFD modelling methodologies are not unique. Among CFD practitioners experienced in engineering analysis simulations, it is well known that given a particular problem (statement), different results may be obtained depending purely on the grid generation and flow solution algorithms employed. While numerical fluid flow analysis theory provides us with guidelines by which to perform CFD analysis, namely mesh and algorithm selection, sensitivity, validation, and verification, application of these guidelines systematically and consistently is to a certain extent driven by problem complexity. While modelling of simple canonical problems may serve as a good academic example to illustrate these factors, simulation of more complex flow problems requires combining such guidelines with experience and developed best practices. Furthermore, the later item has to be considered in the context of the tools being employed to discretize and simulate the problem as well as the tools’ end user. As pointed out by one of the reviewers, others have done work in the subject area described here. All studies, past and present, add value to further developing best practices for a particular class of problems. In this paper, we have described one particular procedure with which we were able to simulate free-surface hydrodynamics around a sailing yacht using a particular set of tools. In the presented discussion, our objective was to describe various technical and scientific factors that we considered in the process of setting-up and executing the simulations as well as assessing the results. Acknowledgements The authors wish to thank Ansys Technical Support and Developer Staff for their guidance. References 1. http://www.farrdesign.com/602.htm 2. Oceanic Report BFA006 – Farr Yacht Design Transom Immersion Testing – October 2005. 3. Davidson Laboratory Report for Farr Yacht Design – April 2007 4. http://www.pointwise.com 5. Courtesy of Dr. J.M.T. Penrose, ANSYS-CFX, UK. 6. http://www.ansys.com/Products/cfx.asp 7. Penrose, J.M.T., Jones, I.P., Zwart, P.J., Imas, L. (2008), “Application of CFD to Flows Around Marine Vessels”, Proceedings of RINA Marine CFD Conference, Southampton, UK, 26th–27th March 2008 8. Menter F. R. and Egorov, Y., "Re-visiting the turbulent scale equation", Proc. IUTAM Symposium; One hundred years of boundary layer research, Göttingen, 2004. 137