VALIDITY OF COMMERCIAL CFD CODES IN LOW‐BUDGET RACE CAR DEVELOPMENT João Ginete, University of Bristol, Bristol, United Kingdom Jeron Moore, University of Washington, Seattle, WA Gianmarco Tartaglione, University of Washington, Seattle, WA ABSTRACT Computational Fluid Dynamics codes have been used in motorsports for decades, but have only recently become available to private and Formula Student teams. The use of “out of the box” codes by non-specialist personnel in the development of aerodynamic packages can produce poor results and lead to low quality designs. By comparing numerical results obtained using different basic settings with experimental tests of the same set-up, this project aims to determine whether commercial CFD packages can be used as a tool for race car aerodynamic design in a low-budget environment by relatively inexperienced engineers or students. The results show a good agreement between the experimental measurements and the calculations performed with the finer grids in all the studies, with the coarser meshes only producing good results when estimating the pressure distribution around the sidepod aerofoil sections. Among the turbulence models used, the SST formulation provided the most accurate representation of the flow field. It is therefore determined that CFD packages can be a powerful tool for race car development, so long as large enough meshes are used and a careful selection of the basic settings is performed. Validity of Commercial CFD Codes in Low-budget Race Car Development Table of Contents Introduction ...................................................................................................................... 1 Methodology ..................................................................................................................... 2 Results and Discussion ....................................................................................................... 3 Conclusion ......................................................................................................................... 7 References ......................................................................................................................... 8 Acknowledgements ........................................................................................................... 8 Appendix 1 ‐ Figures ...........................................................................................................i Validity of Commercial CFD Codes in Low-budget Race Car Development Introduction Aerodynamic development of race vehicles has taken place, in one way or another, since the early years of motorsports. However, its true potential was not unlocked until the advantages of the production of downforce became evident, first through the use of inverted wings and later through the shaping of the car’s underbody, turning the chassis into a very large wing in ground effect. The development of these features has historically been done using experimental methods, with purpose-build wind tunnels with rotating belts being part of any top-level motorsports organisation. According to reference [1], it was not until the early 1990’s that commercial Computational Fluid Dynamics (CFD) codes started to be regarded as a tool for aerodynamic design and it took another decade for these to be used as a benchmark to evaluate the effect of geometry changes. Simultaneously, the increased availability of open-source and commercial CFD packages have provided private and student teams with a very cost-efficient tool for the aerodynamic design of their cars, particularly when the use of wind tunnel facilities is deemed impossible due to the lack of resources. Moreover, real-life conditions are easier to simulate in CFD than in a wind tunnel, as for a flow solver they are simply boundary conditions rather than an expensive rotating belt mechanism Unfortunately, these tools are more often than not used by inexperienced or student engineers, with little understanding of the different settings necessary to set up a simulation properly. Incorrect boundary conditions, poor meshes and inadequate turbulence models can all lead to poor results when CFD codes are used as a black box, leading designers into making wrong decisions and expecting values of downforce and drag which are not verified on the track. Page 1 Validity of Commercial CFD Codes in Low-budget Race Car Development Since the vast majority of the experimental and numerical data is kept secret due to the competitive nature of the motorsports industry, little information is available on the comparison of the two categories of design tools, a void this project seeks to reduce. Methodology The aim of this project is to assess whether commercial CFD codes can in fact be used for aerodynamic design and, if so, what basic parameters provide the best results. This is done by comparing results obtained by an experiment in the wind tunnel with a set of simulations of the equivalent geometry, modelled using the industry-standard Star CCM+ code. The experimental side of this work seeks to simulate to an extent the aerodynamic development of a Formula Student single seater, with a 5/16 scale model assembled in the department’s 7x5 wind tunnel on an elevated ground plane, as rolling road or suction systems are not available. The experimental model was designed to incorporate a high degree of adjustability, with variable diffuser angles and sidepod height and incidence. Furthermore, the model’s ride height, pitch and roll can be adjusted through a set of turnbuckles, which connect the model to the six-degree of freedom load cell that measures the downforce and drag generated by the model. A set of 10 pressure tappings on the surface of the aerofoilshaped sidepods completes the set up, providing an idea of the pressure distribution around the part. This set-up was modelled in CAD with a high degree of accuracy and attention to detail. The geometry was then imported into Star CCM+ and the different model changes represented in a hybrid mesh with a structured component around the walls, ensuring a y+ value under one around the regions of interest in order to capture the boundary layer build-up on the walls; and an unstructured grid away from the walls, featuring regions of increased cell count around the diffuser, sidepods and vehicle body. These features were obtained with the use of Star’s automatic polyhedral and prism layer mesh generators and volumetric controls, where Page 2 Validity of Commercial CFD Codes in Low-budget Race Car Development three base sizes were used in order to obtain different meshes with different cell counts – coarse, with around 1.5 million cells; medium, between 4 and 5 million cells; and fine, between 12 and 13 million cells. The physics of the problem were modelled with a velocity inlet/pressure outlet arrangement, assuming compressible isothermal conditions in an attempt to reduce computational time. Although this will, in all likelihood, produce an unsteady flow field, steady calculations were performed since the increase in turnaround time inherent to unsteady solutions was not practical within the constraints of this project. The oscillating convergence was averaged to produce the final values, as suggested in reference [2]. Finally, as this kind of flow field features large regions of separated flow, three distinct turbulence models – SST, k-ω and Spalart-Allmaras – were tested with the medium meshes in order to investigate which option produced the best results. The use of a transition model was opted against as the only viable option available in Star CCM+ (the γ-Reθ formulation) could only be applied together with the SST model, introducing an extra variable to the comparison of the different representations of turbulence. All the different geometries were computed using these three meshes and three turbulence models, providing a wide array of levels of complexity in order to determine the simplest and least expensive configuration that provides accurate results. Downforce, drag and pressure coefficient data was extracted from the simulations for comparison with the experimental benchmark. Results and Discussion The first investigation evaluated the software’s ability to predict the evolution of the aerodynamic forces as the diffuser setting was increased. The results of the angle sweep indicate that an agreement with the experimental values can only be obtained with a reasonably large number of cells. The behaviour of the medium and coarse meshes seems to Page 3 Validity of Commercial CFD Codes in Low-budget Race Car Development suggest that two mechanisms for the production of downforce are happening simultaneously. The curvature of the diffuser induces circulation to the flow, increasing its velocity and subsequently reducing the pressure through the underside of the model until the stall angle, when separation from the wall causes a drop in downforce. At the same time, as the angle is raised, the pressure on the top of the diffuser will rise, since the plate is lifted away from the vehicle’s wake and its incidence relative to the airflow increased. Further evidence of this joint effect can be found in the experimental data, presented in figure 1, between points 8 and 10, which exhibit a reduction on the downforce growth followed by a sharp recovery all the way until setting 12. One of the key differences observed between the fine and medium meshes was the strength of an inward vortex, produced as the high-pressure flow on the outside of the diffuser negotiates the sharp edges of the diffuser side wall. The vortex captured by the larger grids is considerably stronger, potentially extending the region of attached flow on the outside of the diffuser surface. This effect may be one of the main reasons for the disparity in the results observed in figure 1: an extended range of angles with attached flow would lead to the two mechanisms of downforce generation to “blend in”, yielding the smoother lift coefficient curve verified in the fine mesh simulations and experimental values. Since the different turbulence models were tested in the medium mesh, which produced poor results, it is hard to define which formulation performs better through the numbers alone. However, through the visualization of the velocity profile near the diffuser wall (figure 3), it can be observed that the SST turbulence model is predicting the separation point more accurately than the remaining models. While these simulations show separation occurring near the beginning of the diffuser at setting 8, a behaviour verified by the random movement of the tufts placed on the wind tunnel model, the calculations performed using the SpalartAllmaras model suggest that the flow stays attached until it approaches the supporting bar. Page 4 Validity of Commercial CFD Codes in Low-budget Race Car Development This hypothesis is supported by the widely recognised advantage of the SST model when dealing with large regions of separated flow, a characteristic shown experimentally in reference [3]. The standard k-ω formulation provides erratic results at different angles, a behaviour probably connected to its reputation of being very sensitive to the freestream turbulence settings. A significant offset between the experimental and numerical values was verified and can be attributed to two different sources – the experimental set up, which in itself inevitably produced a certain amount of downforce and drag; and the inaccurate estimation of the height of the ground plane boundary layer, discussed later in this section. However, this paper evaluates the suitability of the code as an aid in the design stages, where the evolution of the performance with the geometry changes is more important than the absolute values. For this reason, the values presented in figures 1 and 2 are of the variation in the lift and drag coefficients, setting the values of the lowest diffuser setting to zero. A second study concerned the effect of the sidepod height on the downforce and drag produced by these sections, as well as the evolution of the pressure distribution around the aerofoil surfaces. While all the numerical simulations suggested a peak at the middle height of 25mm, the experimental results showed an improvement in performance all the way until the highest setting, 37.5mm above the ground. This evolution is backed by the pressure distribution measured by the tappings placed on the surface of the sidepods (visible in figure 4), which shows evidence of flow separation towards the rear of the bottom surface at the lower height (figure 4a) in the form of a flattening of the pressure curve in the recovery stage, a feature that is not matched by the CFD simulations. A better agreement is obtained at the highest ground clearance, where the flow remains attached in both experimental and numerical distributions (figure 4b), suggesting the effects of the ground plane boundary layer are diminished at that height. Page 5 Validity of Commercial CFD Codes in Low-budget Race Car Development More importantly, the prediction of the pressure coefficients around the sidepods was relatively consistent throughout the three meshes used. This provides an opportunity for a more extensive development of these sections, as a much larger number of simulations can be performed to achieve the desired pressure distribution before assessing the magnitude of the forces produced using the fine meshes. The surface roughness of the ground plane is likely to be one of the main sources of the discrepancies between the experimental and numerical values. The plywood board used to simulate the ground plane in the wind tunnel exhibited an unexpectedly rough surface, a feature that could not be replicated in the calculations as a significant number had already been performed before the experimental set-up was assembled. The thicker boundary layer produced by this surface compared with that of the CFD simulations (which assumed smooth walls) is likely to be one of the reasons for the offset in the experimental data and for the inaccurate evolution of the aerodynamic forces produced by the sidepods at different heights. A confirmation of the effect of the ground plane boundary layer in the results was obtained by varying the model’s ride height from 10mm to 20mm, which led to a reduction of 0.177 in the lift coefficient and an increase of 0.093 in the drag coefficient. This issue can be corrected by adjusting the surface roughness in the calculations or by polishing the physical plane. The ideal solution (not achievable within the time constraints of this project) would be the installation of a rotating belt in the tunnel, which would eliminate the ground plane boundary layer altogether, providing a closer representation of a real-life race vehicle. This addition would naturally be complemented by the inclusion of a slip condition in the ground plane wall on the CFD calculations. Page 6 Validity of Commercial CFD Codes in Low-budget Race Car Development Conclusion The set of results and observations included in this report suggests that CFD can be a very useful tool to support the aerodynamic design of race cars in the absence of dedicated experimental facilities. The most important requirement for the production of accurate results is the mesh resolution, with a minimum of 12 million cells advised for any calculations looking to determine the aerodynamic forces produced by the vehicle. If optimisation of selected components based on pressure distributions is performed, coarser meshes can be used but the best candidate configurations should still be evaluated using the larger grids. The choice of the appropriate turbulence model needs further investigation, as the different available formulations were not applied to the large meshes. However, the predicted flow patterns suggest that the SST model performs better when predicting the separation point on the aerodynamic surfaces and when dealing with transition and separation effects in general. With the evolution of computational power and mesh generation algorithms, larger and better quality grids will be available to private and student teams in the future, naturally increasing the quality of the simulations. It is then left to the designers to find the balance between the number of simulations they are able to run and the accuracy of these calculations. Whereas advances in turbulence modelling are likely to occur in the near future, the addition of a transition model to these calculations could greatly improve the results. Unfortunately, the only true model available in Star CCM+ (the γ-Reθ, developed by Menter et al.) has an incomplete formulation, with the calibration of a set of constants essential to produce accurate results for a given flow field. If this is performed, a much better agreement with the real-world flow patterns can be expected. This paper shows that current CFD codes and processing technology can be powerful tools for low-budget aerodynamic development, so long as a simple set of requirements is fulfilled. As the technology evolves, the importance of numerical methods in race car design is likely Page 7 Validity of Commercial CFD Codes in Low-budget Race Car Development to increase, although experimental methods are unlikely to be discarded by the top-level motorsports organisations in the near future. For teams operating with fewer resources, however, switching to a full-CFD approach may be a suitable way to reduce costs and shift resources to other areas of development, improving the competitiveness of the complete package. References [1] B. Agathangelou, M. Gascoyne, Aerodynamic Design Considerations of a Formula 1 Racing Car, SAE Technical Paper Series, Michigan, 1998; [2] S. Sebben, Numerical Flow Simulations of a Detailed Car Underbody, SAE Technical Paper Series, Michigan, 2001; [3] P. Godin, Turbulence modelling for high-lift multi-element airfoil configurations, University of Toronto, Canada, 2004 [4] P. Wright, Formula 1 Technology, SAE, 2001; Acknowledgements First and foremost, we would like to express our gratitude to CD-Adapco for supporting the aforementioned student team, providing the Star CCM+ licenses without which this project would have been very difficult to execute. Moreover, we cannot thank ATS and Todd Leighton enough for all the theoretical and technical support and for permitting the use of their facilities, without which this project would have been impossible to execute altogether. We must also thank the University of Bristol technicians Lee Winter, Neil Pearce and Russ Eyre for their invaluable help with the experimental part of this project. Page 8 Appendix 1 - Figures $'1%#2+34'+/5%67,'782/%!%&'(+,+/5%9+*:%-';+*% !#&$" !#&" !#%$" !"#$% -./012" 324567" !#%" 8592" :;<205729=/>" !#!$" !" %" &" '" (" $" )" *" +" ," %!" %%" %&" %'" %(" &'()*+,%-+./0% Figure 1 – Lift coefficient variation with diffuser angle for different mesh sizes &,10%#2+34'+/5%61,'172/%!%&'(+,+/5%8+*9%-':+*% "#$%& "#$& !"#$% "#"%& ./0123& "& $& '& (& )& %& *& +& ,& -& $"& $$& $'& $(& $)& 435678& 96:3& ;<=31683:>0?& !"#"%& !"#$& !"#$%& &'()*+,%-+./0% Figure 2 – Drag coefficient variation with diffuser angle for different mesh sixes SST S-A Figure 3 – Velocity distribution on the diffuser wall as predicted by the SST and Spalart-Allmaras turbulence models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igure 4 – Pressure distributions on the surface of the sidepods as predicted by different grid sizes at the medium (25mm) and maximum (37.5mm) heights. The distances on the titles refer to the equivalent full-scale dimensions i