The CFD process begins with a CAD model, which is given by softwares like Catia, PTC Creo and Solidworks. They supply the CAD model that will be discretized. This is a process in which the CAD file is converted into a surface mesh. In this step occurs the inclusion of the RANS equations, which are the ones from the turbulence models. In some applications, the Navier-Stokes Equations (NSE) are applied on the mesh elements. The setup of the model is defined by several split NSE. The objective is to simplify the calculations. This article is a summarization of lecture notes taken during the Industrial Aerodynamics lectures attended at Dallara Academy.

Boundary conditions setup

The main boundary conditions are the incompressible Newtonian fluid and the steady flow. The air is a simple model. The incompressible fluid is applied, because it is used to relate the velocities developed during the cycles. The assumption of Newtonian fluid is used, because it avoids errors in the fluid. The steady flow is adopted to consider a simpler model. These assumptions are applied in order to reduce NSE to simpler forms of it, instead of the complete one. Although this makes the calculation easier, there are two equations with complex partial derivatives and non-linear parts:

∇∙(u) = 0

ρu∙∇u = -∇P + ∇∙τ

It is not possible to solve it in a closed way, thus it is required a mathematical model to discretize it and solve it in a computational model. This is the finite volume method (FVM), which requires the equation to be re-written in the integral form with the greenhouse theorem. For the finite volume method these equations become:

∮ρΦv∙dA = ∮Γ_Φ∇Φ∙dA + ∮_vS_ΦdV

Where Φ is an unknown parameter, ρ is the air density, v is the velocity vector, A is the surface area vector, Γ_Φ is the diffusion coefficient for Φ, ∇Φ is the gradient of Φ and S_Φ is the source of Φ per unit volume. Hence, it is possible to simplify the gradients, the fluxes and then discretize the integral forms into the co-location of the mesh elements. In this way, all the variables solved have a single value in the centroid of the cells of the simulation mesh. Therefore, the volume mesh has a discretized set of equations and variables ready to be solved:

[(∂ρΦ/∂t)V] + ∑_ƒ^N_ƒfaces(ρ_ƒv_ƒΦ_ƒ∙A_ƒ ) = ∑_ƒ^N_ƒaces(Γ_Φ∇Φ_ƒ∙A_ƒ + S_ΦV)

The equation above is the discretized equation when applied to each element of the mesh, which is the reason why it is discretized in each face.

The boundaries of a race car cfd simulation

At this step, all the equations were defined, in order to characterize the racing car aerodynamics problem, additional information are according to the case. These are the boundary and the initial conditions, but for all boundaries of the car volume. The first boundary is also called free stream box, which is where the car surface is positioned. This is the watertight model derived from the CAD one, it is cut in halves to reduce the computational effort and the simulation results are replicated to the other side.

The free stream simulation box of the simulation domain has a properly defined box. This is designed to subject all boundaries in the free stream to be trivial. The measure of the box is biased in the vehicle wheelbase. If this is between 3 and 5 m, the box is 50x40x20 m. The x-coordinate has 50 m and the car is positioned 20 m from the wall of the box. More precisely, the front axle of the model is positioned 20 m from the wall. This leaves 30 m from the rest of the vehicle wheelbase and the free stream. The reason for this is to leave enough space for the vehicle wake to dissipate. The y-direction has 40 m and the z-direction has 50 m. In these cases, the greater dimension relative to the vehicle length is to avoid any flow interference due to the box walls. For this reason, the walls are sufficiently far from the car model, in order to not have any interference.

Types of boundary conditions

The boundary conditions assigned are the Dirichlet and the Neumann ones.

Φ(x|_bound,t) = a → Dirichlet

The Dirichlet boundary condition is described above, it is based in the assigning of a value for one of the boundaries. This can be pressure or velocity field itself.

∂Φ(x|_bound,t)/∂n = b → Neumann

The Neumann boundary condition (equation above) specifies the value of the normal derivative of these fields. It imposes how faster the variable is changing across the boundary, the rate of change of the pressure or the velocity fields.

For instance, if it is imposed a zero gradient ∂P/∂n = 0 (Figure 2) in one of the boundaries, it means that after this face, the variable P is not changing. Therefore, after the face that the derivative is set as zero, the field will not change.

Domain boundary conditions

There are some specific boundary conditions applied at each face of the box as illustrated in Figure 3.

First, the principle of Galilean relativity is applied, because different from the real situation is not the car that is moving, instead the air is moving and the car is stationary. The principle of the Galilean relativity states the same laws of motion for all inertial frames. Hence, the boundary conditions imposed are the inlet, the outlet, the ground, the top and the sidewall ones.

Car boundary conditions

The car boundary conditions can vary along its body. It is imposed a fixed velocity equal to zero. Hence all the patches have a fixed boundary condition of u = 0. There are some specific parts of the car that require different boundary conditions. For example, wheels have a rotating wall boundary condition that follows the displacement of the ground. Since the simulations are about vehicle aerodynamics, there is no reason to simulate combustion. Hence, there are some batches created for the airbox and the exhausts. Hence, it is imposed a fixed velocity at the inlet and outlet of the airbox and the exhausts, respectively. In addition, there is the porous media, which is not a proper boundary condition, it is a special treatment.

The interesting point about wheel rotation is that the imposed velocity does not mean that the tire geometry will rotate. Actually, it is fixed, the mesh is static, but the centroid experiments the linear and angular velocity. Hence, the velocity is just imposed similar to the boundaries of the domain. It is imposed on the axis of the rotation of the tire plus the angular speed ω of the wheel. Hence, the boundary condition of the cell centroid is specified according to the distance from the centroid. In this way, ω∙r is defined as the velocity of that domain region.

Symmetry plane

The symmetry plane, or rather, symmetry boundary conditions are applied, because the simulation of a full size car requires a big computational effort. Hence, it is common to cut one half of the car. Establishing a symmetry plane is done and the simulation is performed with a zero normal component of the velocity and a zero gradient of the other variables. This is used whenever is possible, because neither in all situations the flow behaves in a way that allows a symmetry boundary conditions. For instance, when simulating a cornering condition, the air reaches the car at a certain angle, where the two halves of the car face different conditions.

Boundary condition compatibility

Sometimes boundary conditions are not compatible. This occurs mainly when Dirichlet boundary conditions are set. For instance, in the array, there are some boundaries which are imposed different values for pressure. The problem occurs when a cell has a different boundary condition of the faces of the array. This problem is common when setting the boundary condition of the inlet and the ground. For the inlet, there is a free stream velocity, while on the ground there is the same boundary condition, but considering the boundary condition of the tires. In other words, the ground velocity must match, the free stream and the wheel velocities. In addition, it has adopted a slip wall, which means zero shear stress.

For the plinth, the configuration requires more attention. This is a critical zone due to the tire contact patch. At this region an extrusion is created over this area, because due to the tire deformation, the mesh generated at the flat zone has a very low quality. This is called plinth, which is an extrusion of the area to generate good quality mesh to narrow cells. The plinth has no physical impact, it is just to improve the quality of the discretization. Consequently, it helps in compatibility since there are rotating elements at that region. The boundary conditions applied are really sensitive for the results. This occurs because the plinth is close to the ground, which is connected to the free stream velocity while in contact with the wheel. This has its own boundary conditions already defined, all of these should match.

Radiator and intercoolers boundary conditions

Radiators, intercoolers or any other heat exchangers do not have boundary conditions. Actually, they are modeled as a porous media. Considering a radiator, because it is the most common heat exchanger analyzed in CFD simulations, it has a complex geometry, its simulation would be very time consuming. Hence, it is assumed that the radiator is a simple box which is modeled with a pressure jump across the body of the radiator and the introduction of the air at the inlet (Figure 8).

The incompressibility of the flow results in a pressure jump across the radiator. If the pressure and the velocity is plotted together, it is possible to visualize the pressure jump. Actually, this curve is used to be sent by the radiator supplier. Hence, it is possible to use this data to feed the CFD software. The most of it offer some radiator models which the second order interpolation is easy to be performed. This can also be done with data sheet given by the supplier. The porous media requires a proper method to model it, which is the Darcy’s model, which is give by:

ΔP = ΔP(v) ≃ a₁∙v + a₂∙v² = (μu_i/α + C₂ρuu_i/2)Δn ; a₁ = μΔn/α ; a₂ = C₂ρΔn/2

This method uses constants to impose the pressure jump based on the velocity into the radiator. This is done by two parameters, 1/α and C₂, which are the viscous and the inertial resistance. From these a₁ and a₂ are computed, then it is possible to find the velocity according to the pressure. It is a different way to apply linear and quadratic coefficients in the quadratic interpolation. This method has the advantage of using two coefficients which are dependent by on the flow characteristics. For instance, density, kinematic viscosity and the thickness of the radiator. These parameters are not related with the velocity field of the flow. Hence, the pressure jump is more related to the radiator thickness. Darcy’s law is a proper theory to assign porosity in a model. A radiator is simplified to a box with a known geometry, then a pressure drop is imposed with Darcy’s law, thus 1/α and C₂ are proportional to the radiator thickness. Finally, when the velocity field is applied, it is possible to find the pressure drop across the radiator. A typical data is the sheet with the velocity and the pressure drop. The procedure is to plot velocity against the pressure delta (ΔP), thus apply a second order interpolation of the delta and get the parameters a₁ and a₂. Hence, these are the correlations between the fluid characteristics and the radiator thickness.

References

• This is article is based on the lecture notes taken by the author during the Industrial Aerodynamics lectures hold by Muner at Dallara Accademy.