In this example we shall study an airflow over a car. Such a kind of simulations are used in automotive industry to modelize the shape of cars. In this example we shall assume the flow to be steady turbulent.
We want to study the motion of air circulating over a car. The experimental set up for studying this problem is a wind tunnel. Instead of considering the full spatial domain the simulation can be carried out over a smaller domain by observing that the problem admits a symmetry, as shown in Fig.1 where is outlined the geometry. The air enters perpendicularly to the inlet at a velocity U = 27.8 m/s. The operating pressure is p = 1 atm = 101325 Pa.

As the case is steadystate and the fluid is supposed viscous and incompressible, the governing equations to be solved are:

We choose the standard k  ε turbulence model with coefficients C_{μ} = 0.09, C_{1} = 1.44, C_{2} = 1.92, α_{ k} = 1, α_{ ε} = 7.69. In this model the velocity of the turbulent flow is estimated as a fluctuation around an average value: U = ‹ U › + U^{'}; k = (1/2) U^{'}^{2} represents the turbulent kinetic energy per unit of mass and ε the energy dissipation rate. We set the a value of k = 0.02898 m^{2}/s^{2} at the inlet, the same value has been set at the outlet for modeling the turbulence in case of backflow. The value of ε is set to ε = 1.8239 m^{2}/s^{3}.
The mesh (about 3600000 cells) was generated by converting a .msh
GAMBIT file according to the procedure described in the section Mesh conversion.




The case requires initial and boundary conditions settings for all the involved fields: velocity U, pressure P, turbulent kinetic energy k and energy dissipation rate ε. The initial values for the fields are specified in the casename/0/fieldname
files. The reader may consult the boundary conditions documentation section (in Italian) for more details. We report the rilevant sections of the fieldname
files.
The initial velocity U has been set equal to 27.8 m/s in the y direction at the inlet:

We used the simpleFoam
solver, implemented for steady incompressible flow. The numerical schemes for terms such as derivatives, interpolation procedures etc. are set in the casename/system/fvSchemes
file. In this file we specify that the case is steadystate by giving the SteadyState
value to the keyword timeScheme
. The terms ∇ and ∇^{ 2} controlled respectively by the keywords gradSchemes
and laplacianSchemes
have been set to the value Gauss
because we adopted the standard finite volume discretization of Gaussian integration which requires the interpolation of values from cell centres to face centres. The divergence term ∇ ⋅, controlled by the keyword divSchemes
has been set to UD
to ensure boundedness.
In Fig. 3 are shown the residuals of the involved fields after 10000 iterations. The case has been run in parallel using 32 cores.

The same simulation has been run with Fluent. In order to make a comparison we shall analyse the shape of the fields on the central symmetry plane.


In Fig. 4 we observe that the magnitude of the velocity fields is of the same order. The velocity field around the car has a similar shape in both the two simulations. In particular, we observe a similar behaviour in the region at the rear of the car where turbulence effects are present. In Fig.5 is shown in more detail the vector velocity flow near the surface of the car.


In Fig. 6 is shown the pressure contour plot for Fluent and OpenFOAM on the central symmetry plane. The Fluent picture reports the pressure values (in Pa) referred to 1 atm, thus negative values indicate a pressure lower than 1 atm. On the other hand the OpenFOAM picture reports the absolute pressure values as displayed in the scale. Thus in this case an overall agreement is observed, too.

