Tutorial: Aerodynamics Simulation of Flow Around a Vehicle

This tutorial shows how the aerodynamics of a vehicle can be analyzed by setting up an incompressible turbulent airflow around a moving vehicle. Figure 1 shows an example of the resulting flow behavior:

This tutorial teaches how to:

• Set up and run an incompressible simulation;
• Assign topological entity sets;
• Assign boundary conditions, material, and other properties to the simulation;
• Mesh with the SimScale standard meshing algorithm.

We are following the typical SimScale workflow:

1. Prepare the CAD model for the simulation;
2. Set up the simulation;
3. Create the mesh;
4. Run the simulation and analyze the results.

1. Prepare the CAD Model and Select the Analysis Type

1.1. Import the CAD into Your Workbench

The first step is to click on the button below. It will copy the tutorial project containing the geometry into your Workbench.

Figure 2 demonstrates what should be visible after importing the tutorial project:

Note that the car geometry is not too detailed. Small and detailed features that don’t greatly affect aerodynamics, such as bolts and windshield wipers, should be removed or simplified.

With this approach, the computation effort necessary throughout the entire simulation process can be reduced, while still obtaining meaningful results. Find more information about CAD preparation on this documentation page.

1.2. CAD Mode

The first step for this simulation is the creation of the fluid region. This will be the flow domain that will be used for the external aerodynamic analysis. For the incompressible analysis type, only the fluid region is used. The SimScale ‘Edit in CAD mode’ is used to generate the flow region around the geometry that was imported. Eventually, the geometry of the car will be discarded, so only the flow region remains. To enter the CAD mode click on the following icon:

The External option is used to create the flow region around the model. Select ‘External’ next to Create, at the top left of the interface.

The dimensions of the flow region are chosen according to the length (L) of the vehicle. As a rule of thumb, the following values can be used:

• Downstream: ‘8-10’ times the length of the vehicle;
• Upstream: ‘3-5’ times the length of the vehicle;
• As much as necessary to the minimum z-direction, so that the ground can be tangent to the wheels;
• Other directions: ‘3’ times the length of the vehicle.

To further simplify the simulation the symmetric shape of the car is used to reduce the size of the flow domain. Set up the flow region dimensions in meters as shown below:

• X min: ‘-17.5’ \(m\)
• Y min: ‘-15’ \(m\)
• Z min: ‘0.0’ \(m\)
• X max: ‘37.5’ \(m\)
• Y max: ‘0’ \(m\)
• Z max: ’15’ \(m\)

After you are done, click ‘Apply’. Then select the ‘Delete’ feature next to the BODY section, to remove the ‘Car’ solid part:

Select ‘Car’ from the Geometry tree at the top right and click ‘Apply’.

When the operation is finished and the car body is removed successfully, click on ‘Export’ at the top right of the interface to get redirected to the Workbench:

After the export two geometries are now in the geometry section, Car and Copy of Car. For better clarity rename Copy of Car as ‘Car Flow Region’:

1.3 Create the Simulation

To start the simulation setup process, select the CAD ‘Car Flow Region’ and click on the ‘Create Simulation’ button.

Doing so opens the analysis type choice widget. Choose ‘Incompressible’ as the analysis type. It can be used for cases where the Mach number remains lower than 0.3 in the entire domain, which will be the case for this tutorial. Proceed by clicking on the ‘Create Simulation’ button.

The simulation tree will be visible on the left-hand side of the interface. We have to set up all entries to be able to run the simulation. The global settings of the simulation remain as default:

In this tutorial, we want to calculate the steady-state solution, which is independent of time. SimScale also supports transient analysis, which allows the calculation of time-dependent results.

1.4 Create Topological Entity Sets

Topological entity sets are groups of faces. They are particularly helpful when the same group of faces is used several times during the simulation setup. The user can quickly select a given group of topological entities at once whenever they need to be assigned to a condition.

Let’s create three topological entity sets for this tutorial. To begin with, hide the walls of the flow region. To do this, select all six faces of the domain by rotating the model (they should turn to red). Then right-click in the viewer, and pick the ‘Hide selection‘ option, so they turn invisible.

After the walls of the domain are hidden, follow the steps below:

• Pick the 9 faces of the front wheel;
• Create a new set by clicking the ‘+ button ‘ next to the Topological Entity Sets;
• Name the set appropriately (e.g., ‘Front Wheel’) and click on ‘Create New Set‘ after you are done.
• Repeat the same process for the 9 faces of the rear wheel.

Now, let’s create one topological entity set for the remaining faces of the vehicle. Follow the steps below:

• Hide the front wheel and rear wheel topological entity sets by clicking on the eye icon next to them;
• Right-click in the viewer and click on ‘Select all ‘;
• Click on the ‘+ button ‘ next to Topological Entity Sets;
• Name the newly created set appropriately (e.g., ‘Body’).

After creating the Body topological entity set, you can make the walls reappear by right-clicking in the viewer and selecting ‘Show all’. The walls of the flow region will be necessary to assign boundary conditions later on in the tutorial.

2. Assigning the Material and Boundary Conditions

Now we are ready to set up the physics of the simulation.

2.1 Define a Material

In the simulation tree, click on the ‘+ button’ next to Materials.

After opening the materials section, select ‘Air’ from the SimScale materials library. Click on ‘Apply’ to confirm your selection.

The flow region that was created at the beginning of the simulation setup is automatically assigned to the material:

2.2 Assign the Boundary Conditions

The physical situation simulated is a car moving with 20 \(m/s\). Now it is rather difficult to directly model the car’s velocity in a CFD simulation. We get the same result if we turn the situation around. Instead of a moving car and the still-standing street, we make the car stand still and let the air around the car and the street move with 20 \(m/s\).

An overview of the boundary conditions for the domain can be seen below:

Similarly, for the car walls, the following boundary conditions are applied:

To create a boundary condition, click on the ‘+ button’ next to Boundary conditions, and select the desired type from the drop-down menu.

a. Velocity Inlet

Let’s define the air velocity at the inlet face. To do so, create a new boundary condition, selecting ‘Velocity Inlet’ from the drop-down menu, as seen in Figure 22.

With a Fixed value velocity inlet boundary condition, the velocity that we define is a vector. You can use the orientation cube in the bottom-right corner of the viewer for reference. In this tutorial, set the velocity in the x-direction to ’20’ \(m/s\). Last assign the front face of the flow region to the boundary condition.

b. Pressure Outlet

We want to specify the outlet of the flow region as normal atmosphere, zero gauge pressure. Create a second boundary condition, this time a ‘Pressure Outlet’ and specify a fixed gauge pressure. The gauge pressure is relative to a reference value (ambient pressure, for example). Therefore, a pressure outlet condition with ‘0’ \(Pa\) gauge pressure is applied to the outlet face of the domain. Assign the back face of the flow region to this boundary condition.

c. Walls: Slip Condition

For the third boundary condition, select ‘Wall’ from the drop-down menu. Set (U) Velocity to ‘Slip’.

The slip condition allows flow tangent to the face without the creation of a boundary layer, but won’t allow flow in a normal direction. This is a good approximation for the top and side faces of the flow region, which are far away from the car. Therefore, assign the slip wall condition to the top (XY-plane) and the right side (XZ-plane) of the domain, as seen below. Assign both, the right and the top face of the flow region to this boundary condition.

d. Symmetry

As previously discussed, a ‘Symmetry’ boundary condition will be applied to the symmetry plane, since we expect mirrored aerodynamic flow patterns on the two sides of the car. Assign the symmetry face to the boundary condition.

e. Wall: Moving Wall

Now, assign a boundary condition to the ground face which is the street. Create another ‘Wall’ boundary condition. For better clarity rename the boundary condition to ‘Street’. This time, set (U) Velocity to ‘Moving wall’. In this configuration, specify the tangential component for the fluid velocity on the assigned face.

Define a velocity of ’20’ \(m/s\) in the x-direction, which is the same vector that was defined for the velocity inlet boundary condition.

h. Wall: Rotating Wall – Front Wheel

We can model the rotating car wheels with a ‘Wall’ boundary condition. This time, select ‘Rotating wall’ for (U) Velocity. The following information is necessary to set up a rotating wall condition:

• Point on axis: The user should define a point on the axis of rotation. In our case, the center of the wheel should be used as a reference. In Figure 28, this can be done by selecting the center face of the wheel and selecting the ‘Pick center from current selection’ icon. This will automatically enter the center point of the face as the Point on axis.

• Rotation axis: This is the axis about which the faces will rotate. The direction of the rotation is given by the right-hand rule. In the right-hand rule, the thumb represents the rotation axis and the movement of the other fingers represents the direction of rotation. See Figure 29:

• (ω) Rotational velocity: The last parameter to define is the rotational velocity \(\omega\) (\(rad/s\)) for the wheels. It can be calculated using formula (1) below:

$$\omega = \frac {U} {r} \tag{1}$$

Where \(U \ [m/s]\) is the linear velocity of the car and \(r\ [m]\) is the radius of the wheel.

In our case, the car velocity is 20 \(m/s\) and the wheel radius is 0.3495 \(m\). Therefore, our rotational velocity \(\omega\) is ‘57.22’ \(rad/s\).

Now we have the necessary information to set up the rotating wall condition for the front wheel, as seen in Figure 30 below:

• Rename the boundary condition to ‘Front Wheel’
• Define (U) Velocity as a ‘Rotating wall’;
• Specify ‘-1’ in the y-direction for the Rotation axis. The Rotational velocity is ‘57.22’ \(rad/s\).
• Lastly, clear the list of assigned faces and assign this boundary condition to the previously defined ‘Front Wheel’ topological entity set.

g. Wall: Rotating Wall – Rear Wheel

The same procedure is also followed for the rear wheel. The only difference between the front wheel and the rear wheel boundary conditions will be the Point on axis coordinates.

Please set up the final wall boundary condition as shown below:

• Rename the boundary condition to ‘Rear Wheel’
• Define (U) Velocity as a ‘Rotating wall’;
• Select the Point on axis using the same method as for the Front Wheel boundary condition.
• Specify ‘-1’ in the y-direction for the Rotation axis. The Rotational velocity is ‘57.22’ \(rad/s\).
• Lastly, assign this boundary condition to the previously defined ‘Rear Wheel’ topological entity set.

Find in this article relevant information about wall functions and other wall treatments.

How to Choose Between Wall Resolution and Wall Modelling?

2.3. Simulation Control

In the simulation tree, click on the ‘Simulation control’ tab, and configure it as shown:

• Change the Maximum runtime for the simulation to ‘30000’ seconds;
• ‘Enable’ Potential flow initialization. This setting initializes the velocity field and enhances stability in the early iterations.

2.4 Results Control

Lift and drag coefficients are some of the most important parameters when evaluating the performance of the flow aerodynamics of a vehicle. Therefore, let’s create a ‘Force and moment coefficients’ result control, as shown below:

Please set up the result control as below:

• The Center of rotation coordinates of our car is determined as follows:
  • Use the center of the Rear Wheel for Center of rotation. The coordinates can be obtained using the same pick center from current selection option as used for the rear wheel boundary condition.
• Set the positive z-axis as the Lift direction by entering ‘1’. The other axes receive a value of ‘0’;
• Set the positive x-axis as the Drag direction by entering ‘1’. The other axes receive a value of ‘0’;
• Apply ’20’ \(m/s\) as (|U<∞>|) Freestream velocity magnitude, which is the same magnitude that was defined for the velocity inlet boundary condition;
• The Reference length is the car’s length along the x-axis. Our car’s length is ‘4.65’ \(m\);
• The Reference area value is a projection of the frontal car area onto a plane. It’s important to note that, as we’re using half of the car geometry, the area projection must account only for half of the model.

• Clear the list of assigned faces and assign the result control to all of the car faces. The easiest way to do that is by assigning the three previously created topological entity sets.

3. Mesh

For the meshing operation, we recommend using the standard algorithm. The standard meshing algorithm is a good choice in general, as it is quite automated and delivers good results for most geometries, with the following default properties, including a Small feature suppression of ‘0.001’ \(m\) under the Advanced settings:

3.1 Adding Refinements

Use region refinements to more accurately capture the wake and the aerodynamic flow around the car. A region refinement is used to refine the volume mesh for one or more user-specified geometry primitives.

To add a refinement region to your mesh, first, create two geometry primitive boxes. On the right-hand panel click the ‘+ button’ next to the geometry primitives and select the cartesian box.

a. Region Refinements

Set the values for the first region refinement as seen below. This region refinement is used for the first refinement region of the far field around the car.

Rename the first box ‘Far Field’ and add the dimensions as follows:

• Minimum (x) value: ‘-5’ \(m\)
• Minimum (y) value: ‘-5’ \(m\)
• Minimum (z) value: ‘-0.2’ \(m\)
• Maximum (x) value: ’15’ \(m\)
• Maximum (y) value: ‘1’ \(m\)
• Maximum (z) value: ‘5’ \(m\)

Repeat the process to create the second smaller box. This box is used to even further refine the mesh directly around the car.

Rename the box to ‘Close Field’ and the dimensions of the box are as follows:

• Minimum (x) value: ‘-1’ \(m\)
• Minimum (y) value: ‘-2’ \(m\)
• Minimum (z) value: ‘-0.2’ \(m\)
• Maximum (x) value: ‘7’ \(m\)
• Maximum (y) value: ‘1’ \(m\)
• Maximum (z) value: ‘2’ \(m\)

Notice how the boxes extend further downstream from the car. The objective is to capture the high gradients from the wake, which is pictured in Figure 37.

Next, create a new Region refinement by clicking on the ‘+ button’ and selecting ‘Region refinement’.

Rename the region refinement as ‘Region refinement Far Field’ and set the Maximum edge length to ‘0.1’ \(m\) and toggle on the Far Field selection:

Repeat the process for the Close Field. As the smaller box is closer to the surface, a finer discretization will be enforced. Please set the Maximum edge length to ‘0.07’ \(m\):

b. Local Element Size

To refine the cells directly at the wheel faces a local element refinement is used. This refinement is applied to faces and limits the cell edge lengths based on the input.

Create a ‘Local element size Wheels’ refinement and set the Maximum edge length to ‘0.005’ \(m\). Assign it to both ‘Front Wheel’ and ‘Rear Wheel’ topological entity sets, to capture the region next to the rotating walls accurately.

3.2 Meshing Results

Now you can go back to the main meshing settings and click on ‘Generate’, as in Figure 36. Note that this is not a mandatory step: You can also just start the aerodynamic flow simulation and the mesh will be created automatically. However, let’s have a look at the finished mesh in this simulation before starting the simulation.

This mesh will take around 30 minutes to complete and this is what it will look like:

4. Start the Simulation

The simulation setup is now ready. We can proceed to create a new simulation run. To do so, click on the ‘+ button’ next to Simulation Runs.

This way, if not generated in advance, the mesh will be generated, and, afterward, the simulation run will start automatically. While the simulation results are being calculated, you can already have a look at the intermediate aerodynamic flow results in the post-processor. They are being updated in real-time!

You will also find a link to the finished project at the end of the tutorial.

The simulation run takes about 70 minutes to finish. At this point, you can access the post-processing environment by clicking on ‘Solution Fields’ or ‘Post-process results’:

5. Post-Processing

5.1 Force and Moment Coefficients

The drag and lift coefficients are available in the ‘Force and moment coefficients’ tab:

The plot shows you how the coefficients are changing throughout the simulation process, as the iterations go on. In a converged simulation, the coefficients will stabilize around a value.

Therefore, in a steady-state simulation, the intermediate results are important to assess convergence. The final, converged solution is the one that should be analyzed to obtain the aerodynamic flow parameters.

Calculating the Aerodynamic Balance

From the force and moment coefficient report it can be seen that a moment coefficient of -0.18 and a lift coefficient of -0.27 is calculated. As the force and moment coefficient report was defined at the center of the rear wheel the aerodynamic balance of the car can be calculated using the formula \(1\) below.

$$\%_{Front} = \frac{Coef.Moment_{Rear}*Reference Length}{Wheelbase *Coef.Lift}\tag{1}$$

The wheelbase of the car is 2.665 \(m\) and the reference length was set to 4.6 \(m\). Using these values an aerodynamic balance of 115% front is calculated. This means that most of the aerodynamic force is on the front axle of the car.

5.2 Surface Visualization

After accessing the post-processor, you can use several post-processing filters to further analyze the results. If the pressure distribution is not yet visualized, go to Parts color and change the Coloring to ‘Pressure’. The legend at the bottom of the page includes a default range set by the lowest and highest values inside the domain. By clicking on the upper and lower limits and editing their values, you can control the quality of visualization, making sure that the color map on the surface is insightful.

To better visualize the aerodynamic flow around the car you can hide the flow region by selecting all faces of the flow region, right-clicking your mouse, and choosing ‘Hide selection’.

In Figure 52, we have the pressure contours on the car body. As previously discussed, these are gauge pressures. In the areas where aerodynamic flow stagnation occurs (e.g., on the bumper), pressure exhibits larger values. To add a smooth distribution of the colors on the vehicle, right-click on the legend at the bottom, and select ‘Use continuous scale’ :

The upgrade in the visualization quality is evident:

5.3 Cutting Planes

If you want to observe the aerodynamic flow characteristics around the car, then you can obtain some insights with a ‘Cutting Plane’:

Configure the cutting plane by following the steps below:

• Change the Position by changing the Y coordinate to: ‘-0.5’;
• Make sure the Orientation is on the ‘Y’ axis;
• Change the Coloring to ‘Turbulent Kinetic Energy’;
• Set the maximum value of the range to ’10’ \(\frac{m^2} {s^2}\).

From the figure above, we can see that the car creates a disturbance in the aerodynamic flow which produces high turbulent kinetic energy, especially behind the trunk, closer to the ground.

5.4 Streamlines and Animation

Streamlines are useful to visualize the aerodynamic flow path around the car. To do this, select ‘Particle Trace’ from the Filters panel and its settings will be shown.

Next, pick the start position of the particles by clicking the button beside Position.

• Place this at the inlet of the flow region and the streamlines will be shown from the start point;
• Modify the number of particles under # Seeds horizontally and # Seeds vertically. Use ’20’ points horizontally and ’20’ points vertically.
• Change the Spacing of the streamlines to ‘5e-2’ and the size to ‘1e-2’;
• The Trace both directions option is not necessary here, you can disable it;
• Set the range of the velocity magnitude scale to ‘[0, 25]’ \(m \over s \).

Animations can be started by choosing ‘Animation’ from the Filters panel. After changing the Animation type to ‘Particle Trace’, click the play button to start the animation.

The result is shown in the animation below, for better visualization the traces has been changed from cylinders to comets:

When combining the pressure distribution on the surfaces of the car with the velocity streamlines around the car, we can see that high pressure is created at the front when the velocity is at the lowest. Aerodynamic flow seems to be accelerating as it travels over the roof and beyond. A Suction region with very low velocities can be analyzed with blue streamlines.

You can analyze the aerodynamic flow results further with the SimScale post-processor. Have a look at our post-processing guide to learn how to use it.

Congratulations! You finished the aerodynamic flow behavior tutorial!

Last updated: September 7th, 2023