Aerodynamic Numerical Simulation of a Race Car

Filipe Miguel Gaspar Correiafilipe.g.correia@ist.utl.pt

Instituto Superior Tecnico, Universidade de Lisboa, Portugal

November 2018

Abstract

The main goal of this work is the simulation of the three-dimensional flow around a racingcar. OpenFOAM was used to solved the RANS equations complemented with the k-ω SST twoequation eddy-viscosity model. First, a two-dimensional flow simulation around a NACA 23012 airfoilwas conducted in order to implement OpenFOAM. Code to Code comparison was performed usingReFRESCO and ANSYS Fluent R©. The influence of different parameters on the simulation wereaddressed: computational domain size; boundary conditions; structured versus unstructured gridsand discretization of the turbulence quantities transport equations. Numerical uncertainty estimatesare performed for the selected quantities of interest: lift and drag coefficients. Results obtained inthis exercise show consistency between the three flow solvers. In the second part of this work, thethree-dimensional flow simulation around the car was performed assuming steady state flow. Anunstructured full hexahedral mesh was generated using NUMECA OMNIS R©, followed by the numericalsimulation. Besides the use of wall functions on the surface of the car, moving floor and rotating wheelswere applied as boundary conditions. The simulation convergence is discussed and a flow patternanalysis is conducted, where the car performance is evaluated and the steady state flow assumption iscalled into question.Keywords: Race Car, OpenFOAM, RANS, Three-dimensional Simulation, Moving Floor, RotatingWheels

1. Introduction

Aerodynamics has been a subject of growing inter-est in the automotive industry for both road vehi-cles and racing cars. The addition of aerodynamicelements and appendices, mainly for downforce gen-eration but also for drag reduction, has seen an in-crease in development and research especially due tothe great interest in the racing community. Compu-tational Fluid Dynamics (CFD) is a very useful tooldespite the flow over most race cars not being easyto predict, because of phenomena as flow separationor laminar to turbulent transition. However, the in-creased availability of commercial CFD codes andsignificant developments in computational resourcesduring the last decade allowed smaller companiesand racing teams to explore its use. The goal of thepresent work is to simulate and analyse the aerody-namic behaviour of a prototype Gran Turismo (GT)race car by numerically solving the Reynolds Av-eraged Navier-Stokes (RANS) equations. The carin study is the Pininfarina H2 Speed, presented inthe Geneva International Motorshow 2018, built byPininfarina as a proof of concept for an hydrogenpowered race car. The objectives of this work in-clude obtaining the car forces acting on the body-

work with its baseline setup evaluating the perfor-mance of each aero appendix in order to understandhow the flow generates force in the bodywork, un-derstanding the impact of several radiators and itslocation, and finally analysing critical areas withflow separation and how to improve them. A fullCFD simulation procedure will be followed, includ-ing pre-processing (CAD preparation, mesh setupand generation, selection of physics and fluid prop-erties and specification of boundary conditions), nu-merical solution with initialization, solution controland convergence monitoring, and post-processingcontaining data report, flow visualization and anal-ysis.

An extensive amount of CFD simulations havealready been conducted in the racing industry, in-cluding steady and unsteady flows and consideringseveral different turbulence models. Previously atADESS AG [1], a LMP2 (Lotus T128) was studiedand several configurations were analysed recurringto the resolution of RANS equations combined withthe realizable k-ε turbulence model. Preliminarystudies were conducted in a NACA 23012 wherethree turbulence models were considered: realiz-able k-ε, Spalart-Allmaras and k-ω SST. The main

1

objective of this work was to obtain forces actingon the bodywork, which were monitored during thesimulation and considered converged when the os-cillations were smaller than +/- 1N. The residu-als were also monitored and were between 1E-03and 1E-04. In this case, the use of wall functionswas mandatory due to computational resources lim-itations. Formula Society Automotive Engineering(SAE) teams also commonly use the standard orrealizable k-ε model, with wall functions and verycoarse meshes, for the design process of aerody-namic packages, based on the same referred reason[2, 3]. In the work performed by Doddegowda etal. [3], a wing in two dimensions was study in or-der to verify the solver and assess which turbulencemodel was the most suitable, with options betweenthe k-ε, RSM and Spalart-Allmaras. A comparisonwith experimental data was also done and the k-ε model was chosen due to its stability. Althoughit is not the most accurate option it provides a fastand stable solution that allows a qualitative analysisthat was further investigated on track with a sim-ple data acquisition system. Another widely provenoption is the SST variant of the k-ω model whichbrings major improvements when compared to thek-ε, as shown by Menter [4]. It combines the best ofboth the k-ω and the k-ε by using the first in innerparts of the boundary layer and switching to a k-εbehaviour in the freestream where the k-ω is verysensitive to the inlet freestream turbulence proper-ties. Several two dimension airfoil studies were alsoconducted by by Grabis and Agarwal [5], includingmesh refinement studies to determine the accuracyof various mesh densities, solution monitoring to as-sure all residuals were below 1E-05. Wall functionswere not used and instead the no slip condition wasapplied with a y+ of 1 for the first cell. In morecomplex, three dimensional simulations [6, 7] wallfunctions were again adopted, with y+ between 30-100 and monitoring residuals only until 1E-04. Dueto time and computational constraints the statis-tically steady flow assumption was not questionedin any of these studies. Unsteady flow simulationis often considered due to the limitations of RANSsolvers on resolving separated flows [8, 9, 10]. Itprovides a better characterization of separated tur-bulent flows, such as the front wheels wakes, sep-aration at the nose in a formula type car in caseswith side wind [9] or significant wakes behind thecar diffuser, which have a substantial impact in racecars performance. The trade-off is a major increasein computational resources and time.

In order to obtain a reliable and trustworthy sim-ulation it is necessary to take several steps, namelyregarding the solver, CAD preparation and meshrequirements, and to considerer the challenges toovercome. First, it is necessary to implement Open-

FOAM and conduct a solver verification. It wouldbe unrealistic to use an extremely complex geome-try, as the Pininfarina H2 SPEED, for an initialtest, therefore a two-dimensional study was con-ducted on a NACA 23012 airfoil. Structured andunstructured grids were generated for result com-parison in order to evaluate the quality of the lat-ter for further use in the three dimensional case.As convergence proved difficult to reach, an ex-tended control of solution procedure was requiredby adding explicit sub-relaxation. Through the as-sessment of numerical errors, using increasingly re-fined grids, an uncertainty estimation was made.Simulations made in parallel with ANSYS FLU-ENT R© and ReFRESCO were available for compari-son. Afterwards, in order to generate grids for aero-dynamic analysis several criteria should be met, in-cluding a proper CAD geometry, whose preparationinvolves several time-consuming steps, especially incomplex geometries. It was necessary to ensure thecar was a single closed surface, as any gaps largerthan the minimum element size could compromisethe entire mesh generation process. Overlappingsurfaces are another issue that needs to be ad-dressed since the applied algorithms can have prob-lems which result in zero or negative volume cells,resulting in an unusable mesh. With time beinga resource of significant importance, several geom-etry simplifications were taken into considerationfor the purpose of cell count reduction which leadsto lower mesh generation time, especially with theexisting software/hardware limitations. Regardingmesh generation, refinement regions needed to bedefined to guarantee a correct geometry acquisitionand wake capturing without wasting elements onunnecessary areas while obtaining sufficient detailon zones where the flow becomes more complex.Most refinement was done around the wheels andafter the diffuser as separation is expected down-stream of these areas. The rear wing also neededsome adjustments to obtain the necessary refine-ment and correctly capture the wake. Although aninitial estimate was made, viscous layers setup re-quired several attempts to obtain the desired y+for the first cell near the wall. Local adverse pres-sure gradients and unexpected flow separation zonesdemanded a considerable amount of modifications.Proximity refinements were another concern, as ex-cessively close parts of the bodywork resulted indeformed geometries that needed further correc-tions. In a complex geometry such as a racing car,flow separation is a possibility that could make thestatistically steady flow a questionable assumption,namely when it does not reattach to the car or floor.Solution convergence should be a concern, with par-ticular attention to fluctuating forces.

2

2. Background

2.1. Mathematical model

Both test cases in this work are wall bounded flowsat a high Reynolds number, which means that theboundary-layers developing on surface will exhibittransition to the turbulent regime. Therefore, theflow will be unsteady, exhibiting a wide range oflength and time scales that make the direct solutionof the mass conservation and momentum equationsimpossible. The standard practice in engineering isto apply Reynolds-Averaging, which means that allinstantaneous flow variables Φ are decomposed ina mean value Φ and a fluctuation value φ (turbu-lence). The type of averaging applied to determineΦ depends on the physics of the flow. In the absenceof significant regions of flow separation, the logicalchoice is time-averaging leading to the Reynolds-Averaged Navier-Stokes (RANS) equations. Thisresults in a statistically steady flow. As a conse-quence of the averaging process, the Reynolds stresstensor −ρvivj is generated. With the addition ofthis unknown a turbulence model is required toclose the system of equations.

Turbulence models for RANS equations focus onthe mean flow and the effects of turbulence onits properties and can be classified by the numberof additional transport equations that need to besolved. This work will focus on using a two equationturbulence model since they have been widely usedand proven in CFD simulations for the racing indus-try. In the present study, the k-ω SST (Shear StressTransport) suggested by Menter [4] was preferred.This model uses the standard k-ε in the turbulentregion far from the wall but switches to k-ω in thenear-wall region. It is based on the original Wilcox’smodel [11] but the ε equation is transformed into aω equation by substitution of variables ε = kω. Thisway, it combines the good behaviour of the k-ω in-side the boundary layer and in adverse pressure gra-dients while avoiding the high sensitivity of the ω inthe freestream. As adverse pressure gradients andseparating flows are expected, namely in the racecar simulation, it is the selected turbulence modelto complete the RANS equations in this work.

2.2. OpenFOAM

OpenFOAM is an open source CFD software withan extensive range of features to conduct a widerange of complex fluids flows simulations includingheat transfer, chemical reactions and turbulence. Itincludes several pre-processing tools, solvers, phys-ical models and also post-processing capabilitiesthrough the inclusion of ParaView software. Onedistinctive feature is its syntax that resembles theequations being solved, which allows user to eas-ily create customs solver. The result is a softwarewith excellent extensibility qualities. It is based on

a large base library that includes all the core capa-bilities of the code, such as tensor and field opera-tions, discretization of partial differential equations,general physical models, turbulence models, amongothers. This library is then used to develop appli-cations, each with specific capabilities, that can bedivided into solvers and utilities. Solvers performthe calculations to solve a given problem while util-ities are used to pre and post-processing, such asmesh preparation, case setup or result processing.Finally, several third-party packages are usually in-cluded to provide additional functions as parallelfunctionality, with OpenMPI, and graphical post-processing, with ParaView. The main advantagesare the fully documented source code with a widerange applications and models to use without any li-cense costs. However, the development communityis severely fragmented due to the fact that the codeis open source and the absence of a graphical inter-face requires adaptation. Since OpenFOAM doesnot contain an embedded graphical user interface(GUI), all the pre-processing, setups and runs wereperformed through the Ubuntu v16.04 LTS termi-nal environment. This includes mesh import andconversion, boundary and initial conditions defi-nition, solver and discretization schemes parame-ters setup and live simulation monitoring, namelyforces and residuals convergence. Complete post-processing was made through ParaView, where itwas possible to import the case and analyse every-thing from mesh quality to flow patterns, includingpressure and velocity fields, flow streamlines andisolines.

Two modifications were required since the avail-able version of OpenFOAM had some significantdifferences when compared to the other softwaresused, where one would not allow for direct codecomparison and the other could lead to problems initerative convergence. The implemented k-ω SSTmodel version was not in compliance with NASA’sTurbulence Modelling Resource [12], ANSYS FluentR© and ReFRESCO, where all use the latest revisionfrom 2003 [13]. The code was modified as suggestedelsewhere [14] and all simulations were conductedusing this version. After several convergence prob-lems in structured grids, explicit under-relaxationwas added, in addition to the already implementedimplicit. This modification was more coherent withother codes, especially ReFRESCO, and revealedfundamental during the three-dimensional simula-tion.

3. 2D Airfoil Preliminary CaseThe main purpose of the study of the two-dimensional flow of an incompressible fluid aroundthe NACA 23012 airfoil was to check the correct im-plementation of OpenFOAM by performing a Codeto Code comparison of the three previously referred

3

codes. Furthermore, the influence of several condi-tions that are required by the simulation of rac-ing cars were also analysed, such as the size of thecomputational domain and its connection with thespecified boundary conditions, the use of unstruc-tured versus structured grids and the impact on thenumerical accuracy of discretization techniques ap-plied to the turbulence model equations. Grid re-finement studies were also performed to enable theestimation of the numerical uncertainty of CL andCD.

3.1. Domain, flow and boundary conditionsThe computational domain is a rectangle with theincoming flow V∞ aligned with the horizontal sides.The leading edge of the foil is located at the ori-gin of the (x, y) Cartesian coordinate system withx aligned with V∞. The chord c makes an an-gle of attack α = 12o with the incoming flow,which means that the trailing edge is located atx = cos(α)c, y = − sin(α)c. The length of domainis 36cλ with the inlet located at −15cλ and theoutlet at 21cλ, whereas the top and bottom bound-aries are placed at ±12.5cλ. The selected domainmatches calculations performed with STAR-CCM+in [1], available at ADESS AG. The reference do-main corresponds to λ = 1, but values of λ equal to1.25, 1.5, 1.75 and 2 were tested to assess the influ-ence of the size of the computational domain. TheReynolds number Re based on the undisturbed in-coming velocity V∞, chord of the airfoil c and kine-matic viscosity of the fluid ν is Re = V∞c

ν = 3×106.At the inlet boundary the velocity is set equal

to undisturbed flow conditions, i.e. Vx = V∞ andVy = 0 and the pressure is extrapolated from theinterior assuming zero streamwise derivative. Theturbulence kinetic energy k was approximated byκ = 3

2 (IV∞)2 with a turbulence intensity I of 1%.The value of ω is derived from k and a kinematiceddy-viscosity

(νtν

)inlet

= 10−8Re and ω = κνt

. Atthe outlet, two different types of boundary condi-tions are tested:

1. Fixed pressure (P = 0) with zero streamwisederivatives applied to all remaining flow vari-ables that we will designate by Pout.

2. Zero streamwise derivative applied to all de-pendent variables, that will be designated asP1.

In the second option, the pressure level is not fixedbecause momentum equations and its boundaryconditions include only pressure derivatives. There-fore, the pressure is fixed at the top left corner of thecomputational domain. At the top and bottom, inthe airfoil case, and top and side boundaries, in therace car, the normal velocity component is assumedto be zero (Vy = 0) and the normal derivatives ofall the remaining dependent variables is set equal

to zero. At the surface of the airfoil the no-slipcondition is applied. As mean velocity profiles inthe near-wall region only remain linear for approxi-

mately y+n < 5, with y+n = uτynν and uτ =

√τwρ the

accurate determination of τw using the definitionrequires near-wall cells sizes with (y+n )2 < 1. Tur-bulence kinetic energy is equal to k = 0, but ω goesto infinity at the wall. In order to avoid the singularbehaviour of ω at the wall, the near-wall analyticsolution of the ω transport equation [11] is used tospecify ω at the near-wall cell centre ω2 = 6ν

β(yn)22.

As suggested in [4], the value of ω at the boundaryface can be set equal to 10 times the value obtainedfrom ω2. At the top and bottom the normal velocitycomponent is assumed to be zero (Vy = 0) and thenormal derivatives of all the remaining dependentvariables is set equal to zero.

3.2. Numerical settingsSeveral structured geometrically similar and un-structured nearly geometrically similar grid setshave been generated to discretize the selected com-putational domain. The grids were generated withtwo completely different tools:

1. Multi-block structured grids have been gener-ated using algebraic and elliptic grid generatorsdescribed in [15].

2. Unstructured grids have been generated withNUMECA HEXPRESS R© [16].

Figure 1 illustrates the topology of the grids forthe reference computational domain (λ = 1). Eachset contains five grids and the number of volumesNv, number of cell faces on the airfoil Nf , grid re-finement ratio hi/h1 and ((y+n )2)max of the two ref-erence sets, S1 and U1, are presented in table 1.The number of cells of the finest grid is very similarin both sets, but the U1 grids exhibit a significantlarger values of faces on the surface of the airfoilthan the S1 grids. On the other hand, the near-wall cell height is smaller for the S1 than for the U1grids.

x/c

y/c

­15 ­10 ­5 0 5 10 15 20

­10

­5

0

5

10

x/c

y/c

­15 ­10 ­5 0 5 10 15 20

­10

­5

0

5

10

Figure 1: Illustration of the topology of the multi-block structured and unstructured grids used in thecalculation of the flow around the NACA 23012 air-foil at 12o angle of attack and Reynolds number of3 × 106.

4

Multi-block structured, S1Nv Nf hi/h1 ((y+n )2)max

929280 960 1.00 0.12711480 840 1.14 0.14522720 720 1.33 0.16363000 600 1.60 0.19232320 480 2.00 0.24

Unstructured, U1Nv Nf hi/h1 ((y+n )2)max

929450 2644 1.00 0.20608581 2116 1.25 0.25353360 1590 1.66 0.33251132 1326 1.99 0.40167628 1062 2.49 0.50

Table 1: Number of volumes Nv, number of cellfaces on the airfoil Nf , grid refinement ratio hi/h1and ((y+n )2)max of the reference grid sets for thecalculation of the flow around the NACA 23012 air-foil at 12o angle of attack and Reynolds number of3 × 106.

Besides the two reference grid sets, ten other setswere generated using the two alternative topologies:

• Sets S2 and U2 have the same finest grid ofthe reference sets, but instead of having thenear-wall cell size changing with grid refine-ment they exhibit a nearly constant near-wallcell height.

• Eight additional sets were generated to dis-cretize domains with λ = 1.25 (S3 and U3),λ = 1.5 (S4 and U4), λ = 1.75 (S5 and U5)and λ = 2. (S6 and U6).

The purpose of the S2 and U2 sets is to illustratethe effect of the wrong refinement strategy on theestimation of the numerical uncertainty of the quan-tities of interest. In fact, two extra sets (S1a andS2a) were also generated for the multi-block gridsexhibiting the same number of cells but an increasedvalue of ((y+n )2)max when compared to S1 and S2.((y+n )2)max varies between 0.6 and 1.2 for S1a andremains approximately equal to 0.6 for all the gridsof set S2a. The remaining grid sets (S3 to S6 andU3 to U6) remain similar (for U) or identical (for S)to the reference grid sets in the common part of thecomputational domain. The goal of these extra setsis to quantify the influence of the computational do-main size and of the outlet boundary conditions onthe selected quantities of interest, the lift and dragcoefficients of the airfoil.

3.3. ResultsThe two quantities of interest are the lift and dragcoefficients, CL and CD respectively, which are ob-tained from the integration of the pressure andshear-stress distributions at the wall.

The first check performed with ReFRESCO andOpenFOAM was the ability to iteratively convergethe solutions to negligible residuals. Figure 2 illus-trates the iterative convergence of CD and CL ob-tained in the finest grids of the S1 and U1 sets. Inthe case, the Pout boundary conditions were used atthe outlet and first-order upwind is applied to theconvective terms of the turbulence quantities trans-port equations. The ratio between the iterativeconvergence criteria applied and its lowest value,ε, is equal to 10−6 for the OpenFOAM calculationsand 10−11 for the ReFRESCO simulations. As ex-pected, the data show that iterative errors are sig-nificantly larger than the order of the residuals usedas iterative convergence criteria. Nonetheless, it ispossible to obtain negligible levels of iterative er-rors with both codes in the two grids. However, thetrends obtained for the two flow solvers are exactlythe opposite. The S1 grid leads to a faster conver-gence for OpenFOAM and to a slower convergencefor ReFRESCO. In the remaining calculations per-formed in this study at least 10−6 was adopted asiterative convergence criteria for the OpenFOAMsimulations and 10−8 was used in the ReFRESCOcalculations. Therefore, iterative errors can be ne-glected when compared to discretization errors. Inthe remaining calculations performed in this studyat least 10−6 was adopted as iterative convergencecriteria for the OpenFOAM simulations and 10−8

was used in the ReFRESCO calculations. There-fore, iterative errors can be neglected when com-pared to discretization errors.

ε

∆φ

%

101

102

103

104

105

106

107

10­6

10­5

10­4

10­3

10­2

10­1

100

101

102

φ=CD, S1

φ=CL, S1

φ=CD, U1

φ=CL, U1

ReFRESCO

ε

∆φ

%

101

102

103

104

105

106

107

10­6

10­5

10­4

10­3

10­2

10­1

100

101

102

φ=CD, S1

φ=CL, S1

φ=CD, U1

φ=CL, U1

OpenFoam

Figure 2: Iterative convergence of drag CD and liftCL coefficients in the finest grids of the S1 and

U1 sets. ∆φ = φ(ε)−φ(1)φ(1) × 100 where ∆φ is the

percentual difference to the results of the most de-manding iterative convergence criteria and φ(1) des-ignates the values obtained with the most demand-ing iterative convergence criteria.

Estimating numerical uncertainties based on apower series expansion requires the generation ofa family of (nearly) geometrically similar grids toallow the definition of a typical cell size hi. One ofthe most important features of a grid for the calcu-lation of a viscous flow without wall functions is the

5

size of the near-wall cell size. It is not unusual tosee families of grids where the size of near-wall cellsize is kept constant1. However, such option maylead to misleading results because the discretizationerror would not vanish when hi tends to zero.

Results obtained with two types of grids sets arecompared:

1. Grid sets with a near-wall cell that decreaseswith grid refinement (S1, S1a and U1).

2. Grid sets with a nearly constant near-wall cellsize (S2, S2a and U2).

Calculations were performed with ReFRESCOfor all sets and with OpenFOAM for S1,U1,S2 andU2. The results obtained with ReFRESCO in theS1, S1a, S2 and S2a grid sets are illustrated in Fig-ure 3. As expected, there is a significant influenceof ((y+n )2)max on CD and CL. The extrapolations tocell size zero performed for the S1 and S1a sets (con-sistent refinement) are in agreement. However, theextrapolated solutions obtained from the grid setswith near-wall cells of fixed size (S2 and S2a) do notmatch. The most troublesome result is obtained forCL in the S2a set, which exhibits an error bar forthe finest grid solution that does not included theestimate of the exact solution obtained with S1 andS2.

hi/h

1

CD

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 20.014

0.016

0.018

0.02

0.022S1

ah+bh2

S2

p= 1.2

hi/h

1

CD

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 20.014

0.016

0.018

0.02

0.022S1a

ah+bh2

S2a

ah+bh2

hi/h

1

CL

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 21.335

1.34

1.345

1.35

1.355

1.36

1.365S1

ah+bh2

S2

p= 0.9

hi/h

1

CL

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 21.335

1.34

1.345

1.35

1.355

1.36

1.365S1a

ah+bh2

S2a

ah+bh2

Figure 3: Convergence of the drag CD and lift CLcoefficients with grid refinement. Results obtainedwith ReFRESCO in multi-block structured grid setsusing consistent (S1 and S1a) and inconsistent (S2and S2a) refinement strategies.

The first Code to Code comparison is presented inFigure 4 that depicts the convergence of CD and CLwith grid refinement obtained with ReFRESCO andOpenFOAM for grid sets using consistent (S1 andU1) and inconsistent (S2 and U2) refinement strate-gies. In general, there is more scatter in the dataobtained with OpenFOAM than in the ReFRESCOresults. Although the trend is not as clear as theprevious, results from the HEXPRESS R© grids (U1and U2) tend to have more scatter than the dataobtained in the S1 and S2. As a consequence ofthe noisy data, estimation of observed orders ofgrid convergence is troublesome and so uncertaintyestimations are most likely too conservative. Al-though the level of estimated numerical uncertainty

1Usually with the argument that (yn)2 ' 1.

is larger than desirable, all discrepancies betweenthe two flow solvers are significantly smaller thanthe estimated numerical uncertainties. The mostsimilar results of the two solvers are obtained forCL is the multi-block structured grids. These re-sults suggest that Code to Code comparisons re-quire grid densities larger than those used in thisstudy to obtain smallest levels of numerical uncer-tainty.

hi/h

1

CD

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 20.014

0.016

0.018

0.02

0.022

S1

ah+bh2

S2

p= 1.2

ReFRESCO

hi/h

1

CD

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 20.014

0.016

0.018

0.02

0.022

S1

ah+bh2

S2

p=2

OpenFoam

hi/h

1

CL

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 21.2

1.25

1.3

1.35

1.4

S1

ah+bh2

S2

p= 0.9

ReFRESCO

hi/h

1

CL

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 21.2

1.25

1.3

1.35

1.4

S1

ah+bh2

S2

ah+bh2

OpenFoam

hi/h

1

CD

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 20.014

0.016

0.018

0.02

0.022

U1

p=2

U2

p=2

ReFRESCO

hi/h

1

CD

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 20.014

0.016

0.018

0.02

0.022

U1

p=2

U2

p=2

OpenFoam

hi/h

1

CL

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 21.2

1.25

1.3

1.35

1.4

U1

ah+bh2

U2

p=2

ReFRESCO

hi/h

1

CL

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 21.2

1.25

1.3

1.35

1.4

U1

ah+bh2

U2

ah+bh2

OpenFoam

Figure 4: Convergence of the drag CD and lift CLcoefficients with grid refinement. Results obtainedin grid sets using consistent (S1 and U1) and incon-sistent (S2 and U2) refinement strategies.

4. Car Simulation

In the second part of this work the Pininfarina H2Speed aerodynamics will be studied in three dimen-sions with the main focus placed on the flow patternanalysis, the assumptions made and its correspond-ing consequences on the results and force conver-gence analysis.

4.1. Domain, flow and boundary conditions

The computational domain is a parallelepiped withthe incoming flow V∞ aligned with the horizon-tal, top and bottom sides. The front centre of thecar is located at the origin of the (x, y) Cartesiancoordinate system with x aligned with V∞. Thereference length was defined as the car’s length,Lref = 5m. The length of domain is 9Lref withthe inlet located at −3Lref and the outlet at 6Lref ,whereas the top and side boundaries are placed at1Lref . The selected domain matches calculationsperformed with STAR-CCM+ in [1], available atADESS AG. The Reynolds number Re based on theundisturbed incoming velocity V∞ = 70m/s, lengthof the car Lref and kinematic viscosity of the fluid νis Re = V∞c

ν = 2.4× 107. The model was simulatedwith ground movement with the same velocity asthe freestream and with wheels rotation calculatedfor the same speed.

At the floor and surface of the car wall functionswere used which requires y+n > 30 − 50. The tar-get was set for ((y+n )2)avg > 50. Turbulence kineticenergy is equal to k = 0 and ω was defined identi-

6

cal to the airfoil simulation. At the outlet the Poutboundary conditions were used, with fixed pressure(P = 0) with zero streamwise derivatives applied toall remaining flow variables. In the radiators andducts, a fixed pressure value was specified based onprevious studies made at ADESS AG. Zero stream-wise derivatives were applied for the patch outflow.For the inflow, the velocity was obtained from theflow with a specified inlet direction. At the top andside boundaries, in the race car, the normal velocitycomponent is assumed to be zero (Vy = 0) and thenormal derivatives of all the remaining dependentvariables is set equal to zero.

4.2. Geometry and Mesh Generation

The car has approximately 5 meters length, by 1.2meters of height, by 2 meters of width and is illus-trated in figure 5. The main aerodynamic appen-dices are the rear wing, front splitter, underfloorand diffuser whose main objective are downforcegeneration.

Figure 5: Pininfarina H2 Speed.

The CAD geometry was provided by ADESS AGin CATIA V5 format. This geometry was not readyfor meshing and CAD cleaning was required. Sev-eral corrections were necessary in order to obtainan accurate geometry of the car. The first step wasupdating the CAD model by assembling all the nec-essary bodywork components and removing partswith negligible impact on aerodynamics but signif-icant effect in the mesh complexity. This includedremoving the rear wing support and all the suspen-sion components as shown in Figure 6. Internalparts were not included, as our objective is the ex-ternal flow analysis, which decreased the complexityand size of the model, improving the import timein NUMECA OMNIS R©. After the CAD had all thenecessary components, focus shifted to the require-ments for mesh generation including the need for asealed volume and elimination of any overlappingor intersecting surfaces. Sealing the bodywork asa unique volume required a number simplificationsand included covering all the open areas.

The computational model was discretized on afull hexahedral unstructured mesh using a beta de-

(a) Original (b) Simplified

(c) Original (d) Simplified

Figure 6: Rear wing support and suspension sim-plification.

velopment version of NUMECA OMNIS R©, whichbase code and algorithms are the same to those inNUMECA HEXPRESS R© used in Section 3. Sim-ilarly to the 2D case, parallelepipedic refinementregions were created around the geometry: threeprogressively more refined enveloping the entire car,one around each wheel, one for the rear wing andits wake and the last one for the diffuser and carwake. A general surface refinement was defined tocapture an accurate representation of the geome-try, with an element size of 10 mm. However, un-like the 2D case, the complexity of the geometryrequires refinements on specific surfaces not onlyto capture relevant small edges and curvatures, inorder to keep the geometry details as close to re-ality as possible, but also to avoid mesh problemssuch as negative cells. The distance between dis-tinct surfaces is, sometimes, smaller than the tar-get element size in that refinement region which canlead to problems, mainly negative cells and surfacemerging, resulting in poor geometry definition. Inthose cases, further refinement is required by us-ing the ”Proximity Refinement” option available atNUMECA OMNIS R© which allows to reduce thetarget element size between the defined surfaces.Viscous Layers were inserted in order to obtain anadequate resolution near the wall. Since the meshsize was in the order of the 40 million cells and dueto time an resources limitations, it was not possi-ble to calculate the shear stress at the wall by its

definition, τw = µ∆U

∆y, which requires (y+n )2 < 1.

Instead, wall functions were used and the (y+n )2 wastargeted to be above 30-50.

4.3. Numerical Settings

Based on the results obtained from Section 3, thepreferred option was to apply a second-order up-wind scheme to the convective terms of the momen-tum equations and first-order upwind to the convec-

7

tive terms of the turbulence quantities transportequations. Approximation of diffusive fluxes wasperformed with second-order central-differences inthe three flow solvers and gradients of dependentvariables are calculated with the Gauss theorem.

4.4. Result AnalysisFigure 7 shows a significant separation zone at thecar’s rear and at the wing. Although the firsthas a significant recirculation zone it reattaches tothe ground, while the latter has a massive separa-tion that extends for approximately 4 chords lengthwithout reattachment. It immediately raises con-cern towards the statistically steady approximationmade previously as inevitably there will exist forcesfluctuation. As expected, the solution did not fullyconverged as shown in figure 8(a) by the stagna-tion in the pressure around 1E-03 and, most impor-tantly, as shown by the periodic fluctuation in theforces plot, figure 8(b). These convergence difficul-ties can be related to regions of poor grid quality.However, the flow separation region obtained be-hind the rear wing suggests that the problems mightbe originated by the use of time-averaged RANSequations.

Figure 7: Velocity distribution with streamlines onthe rear. Cross section at y = 0.25 m.

(a) Residuals. (b) Forces.

Figure 8: Convergence plots.

Although convergence was not optimal, many ofthe main flow features can be discussed with thefinal solution obtained, namely surface pressure andvelocity distributions.

4.4.1. Surface Pressure DistributionThe pressure distribution on the car’s surface isshown in Figure 9, in dimensionless form as pres-sure coefficient Cp. On (1) it is possible to see thatthe flow stagnation zone (maximum pressure, dis-played in red) is small due to the shape of the front

structure (bonnet and front bumper), with a smallleading edge and a smooth curvature throughoutthe bonnet, resulting in low drag force. It is also im-portant to note the front radiators and brake duct,displayed in light blue, are positioned in order toreceive an undisturbed flow.

Figure 9: Surface pressure coefficient.

The splitter and front bumper junction createsa concave shape generating a high pressure zoneclose to a small radius corner, indicated by (2),leading to the front radiator duct entrance. Thesteep curvature and the pressure gradient results inflow separation, displayed in dark blue, which reat-taches before the front radiator entrance. On theother hand, the large blue zones indicated by (3)represents high velocity regions near the car’s sur-face. These are related to the car’s shape, wherethe cockpit and the wheel arch are the highest sec-tions, relative to the ground and transversal to theflow, therefore the streamlines curvature are moreintense and the velocity is, by definition, higher.

Figure 10 shows that the splitter’s leading edgecreates a high velocity and low pressure zone (4)with the objective of generating downforce at thefront of the car. However, the rest of the splitterhas higher pressure than expected. The reason forthis pressure loss is the flat shape of the bottomof the splitter and, more importantly, the huge gapbetween the latter and the underfloor. This gapdoes not allow for a gradual pressure recovery, re-sulting in an abrupt flow expansion, which leads toa velocity decrease, pressure increase and downforceloss on the entire splitter and underfloor. A moredetailed analysis of the flow and velocity distribu-tion is made posteriorly.

Figure 10: Underfloor pressure coefficient.

As expected, the imposed rotation on the wheels

8

and floor movement result in a very high pressureon the front section of the front wheel (5), especiallynear the ground. Adding this to the closed wheelarches results in a high turbulence zone around thewheel envelops. As referred above, the underfloor’sdownforce is seriously compromised as most of theflow escapes through the gap between the under-floor and the splitter. Therefore it was expectedthat the diffuser effect would be very poor sincethere is no gradual acceleration of the flow through-out the underfloor and so there is no low pressureareas. The upstream flow pressure coefficient wasalmost zero and so the diffuser does not have anypressure to recover. The side channel has almost noeffect while the one in the centre still generates asmall zone of low pressure at the beginning (6). Inconclusion, the underfloor and diffuser combinationdoes not generate any significant downforce.

4.4.2. Velocity Fields by Sections

In (7), Figure 11, it is possible to see the flow accel-erating after the leading edge for a short distance toreach a maximum across the longitudinal directionof the splitter. Note that the velocity near split-ter’s surface is lower than the freestream due to theground effect. In zone (8) it is possible to noticea small recirculation bubble due to the fast accel-eration after the splitter’s leading edge, where theflow detaches from the wall and reattaches a fewcentimetres further, similar to what is described in(2). Between the splitter and underfloor there isa significant gap (9) which creates a low velocityregion with recirculation due to the abrupt expan-sion of the flow. The sudden transition from theflat bottom surface of the splitter and the gap tothe underfloor does not allow any pressure recov-ery, resulting in a flow behaviour similar to a freejet and consequently all the downforce in the split-ter is lost. The radiators location (10) is a goodperformance decision. The intake section presentsa uniform velocity profile.

Figure 11: Velocity stream lines on the front. Sec-tion y = 0.25 m.

Figure 12 shows the proximity between the wingand bodywork increases the velocity in the suctionside of the wing (11) resulting, not only, in stalland flow separation, due to the increase of the ad-

verse pressure gradient, but also in lift generationon the bodywork’s surface. Therefore, the sharkfin and the endplate height should be modified sothat undisturbed flow reaches the wing. A transla-tion in the X direction, downstream, would also bebeneficial. The stalled wing creates a freestream re-circulation (12) zone which reduces downforce andcontributes to drag force increase.

Figure 12: Velocity distribution on the rear. Sec-tion y = 0.25 m.

After conducting a complete flow pattern analy-sis, the steady state assumption becomes question-able due to the massive flow separation caused bythe rear wing. Unlike the recirculation zone be-hind the diffuser that reattaches to the floor, theone in the wing does not, which causes fluctuatingforces and so the real flow will exhibit vortex shed-ding, preventing the solution convergence. For thisreason, an unsteady flow simulation was attemptedwith the existing mesh. The Courant number wastargeted for C < 1 as suggested by Ferziger andPeric [17]. Two options regarding this parameterwere tested. The first was to set the time step fora fixed value while the second, was to allow thesolver to automatically adjust the time step. How-ever, both efforts revealed the same problem: thedifference between the smallest and largest cells onthe mesh was several orders of magnitude apart,which resulted in an unrealistic small time steps,rendering the simulation unfeasible. For a success-ful attempt, the mesh would require improvementsas the smallest cells had 5e-14 m3 while largest werearound the 0.02 m3. These cells were located in theon the tip of the rear wing, near the connectionwith the endplate. This could suggest the existenceof a gap and/or overlapping surfaces, therefore, athorough check of the CAD should be made.

5. ConclusionsThe main goal of the present work was to simu-late the flow around the Pininfarina H2 SPEED us-ing OpenFOAM and evaluate its performance. Toachieve this, an initial two-dimensional study on anairfoil was conducted to access the correct imple-mentation of the solver. Afterwards, the car sim-ulation was conducted. A statistically steady flowsimulation was performed using RANS equationscomplemented by the k− ωSST turbulence model.

9

The important findings and results of this work aresummarized and listed below:

• Correct implementation of OpenFOAM, veri-fied by a Code to Code comparison whose re-sults allowed to confidently define the outletboundary condition, domain size and approxi-mation of the convective terms of the transportequations.

• A convergence criteria for OpenFOAM forwhich the iterative error is neglected whencompared to the discretization errors was de-fined.

• Structured and unstructured grids were com-pared in order to confirm that the latter obtainadequate results.

• Proper cell quality across the entire meshproved troublesome to accomplish as achievingthe target (y+n )2 on the entire surface of the carproved troublesome. Obtaining cells within thesame order of magnitude size also revealed tobe a difficulty.

• It was found that a significant stall in the rearwing which reduces the generated downforce.It also raised the question whether or not thesteady flow approximation was adequate.

• The underfloor and diffuser proved to be inef-ficient. This was mainly due to a large gap be-tween the underfloor and the splitter which re-duce the flow speed below the bodywork. Thediffuser also revealed stall.

• The front ducts and radiators were a good de-sign decision. The high pressure area in thefront of the car was reduced and the receivedflow was undisturbed. However, the rear radi-ators were not operating in the best conditionsbecause there was a low velocity region thatsuggested flow separation in a part of the duct.

References[1] Y. Pichon. CFD analysis of a Le Mans pro-

totype race car. Master’s thesis, School ofApplied Sciences, Motorsport Engineering andManagement MSc, 2011.

[2] S. Rehnberg, L. Borjesson, R. Svensson, andJ. Rice. Race car aerodynamics-the design pro-cess of an aerodynamic package for the 2012chalmers formula sae car. Technical report,SAE Technical Paper, 2013.

[3] P. Doddegowda, A. L. Bychkovsky, and A. R.George. Use of computational fluid dynamicsfor the design of formula SAE race car aerody-namics. Technical report, SAE Technical Pa-per, 2006.

[4] F. R. Menter. Two-equation eddy-viscosityturbulence models for engineering applications.AIAA journal, 32(8):1598–1605, 1994.

[5] M. Grabis and R. K. Agarwal. Computationalfluid dynamics analysis of high lift, single ele-ment, inverted airfoils in ground effect for anfsae car front wing. 2017.

[6] A. Huminic and G. Huminic. On the aerody-namics of the racing cars. Technical report,SAE Technical Paper, 2008.

[7] S. Desai, E. Leylek, C. B. Lo, P. Doddegowda,A. Bychkovsky, and A. R. George. Experimen-tal and CFD comparative case studies of aero-dynamics of race car wings, underbodies withwheels, and motorcycle flows. Technical report,SAE Technical Paper, 2008.

[8] R. Lewis, A. Mosedale, and I. Annetts. Usingopenfoam and ansa for road and race car cfd.In Proceedings of the 3rd ANSA and µETA In-ternational Conference. September, 2009.

[9] C. Albukrek, P. Doddegowda, A. Ivaldi,J. Amodeo, and E. Bardoscia. Unsteady flowanalysis of a formula type open wheel race carin cornering. Technical report, SAE TechnicalPaper, 2006.

[10] B. D. Duncan and K. Golsch. Characteriza-tion of separated turbulent flow regions in cfdresults for a pontiac nascar race car. Technicalreport, SAE Technical Paper, 2004.

[11] David C Wilcox. Formulation of the kωturbulence model revisited. AIAA journal,46(11):2823–2838, 2008.

[12] American Institute of Aeronautics and Astro-nautics. Nasa turbulence modelling resource.https://turbmodels.larc.nasa.gov/.

[13] F. R. Menter, M. Kuntz, and R. Langtry. TenYears of Industrial Experience with the SSTTurbulence Model, volume 4. Begell House,Inc., 2003.

[14] American Institute of Aeronautics and Astro-nautics. Nasa turbulence modelling resource,changes to openfoam. https://turbmodels.

larc.nasa.gov/ChangesToOpenFOAM.pdf.

[15] L Eca, M Hoekstra, and J Windt. Practi-cal grid generation tools with applications toship hydrodynamics. In 8th International Con-ference in Grid Generation in ComputationalField Simulations, 2002.

[16] NUMECA. Hexpress description. https://

www.numeca.com/product/hexpress.

[17] J. H. Ferziger and M. Peric. Computationalmethods for fluid dynamics. Springer Science& Business Media, 2012.

10