Tutorial: Aerodynamics Simulation of Flow Around a Vehicle

This tutorial shows how an incompressible turbulent airflow around a moving vehicle can be simulated. 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:

Prepare the CAD model for the simulation;

Set up the simulation;

Create the mesh;

Run the simulation and analyze the results.

1. Prepare the CAD Model and Select the Analysis Type

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

The following picture 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 the aerodynamics, such as bolts and windshield wipers, should be removed or simplified.

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

Did you know?

We can use the car’s symmetrical shape in our favor. As we expect the flow field to be mirrored along the symmetry plane of the car, we only need to use one half of the geometry.

As a result, it’s possible to run the simulations faster.

1.1. Create an Enclosure

The first step for this simulation is the creation of an enclosure. This will create the flow domain that will be used for the external aerodynamics analysis.

Select a new ‘Geometry Operation’, then pick the ‘Enclosure‘ operation.

The enclosure dimensions 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.

For this simulation project, we are going to use only half of the car, due to symmetry. Please set up the enclosure dimensions as seen below:

Minimum (x) value: -15 m

Minimum (y) value: -15 m

Minimum (z) value: -0.01 m

Maximum (x) value: 40 m

Maximum (y) value: 0 m

Maximum (z) value: 15 m

After you are done, click ‘Start‘.

1.2 Create the Simulation

Figure 7 shows the resulting enclosure. Proceed by clicking on the ‘Create a 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 in the left-hand side panel. 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.

Did you know?

The k-omega SST turbulence model is recommended for external aerodynamics cases. It works as a blend between the k-omega and k-epsilon models. The k-omega model is predominant in the near-wall, switching to the k-epsilon model in the free-stream.

Find more information about the k-omega SST model in this documentation page.

1.3 Create Topological Entity Sets

Topological entity sets are groups of faces. They’re 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. Please follow the steps below:

Hide the walls of the domain and pick the 5 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 5 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 finishing to create the Body topological entity set, you can make the enclosure walls reappear by right-clicking in the viewer and selecting ‘Show all’. The enclosure walls 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. Choose ‘Air‘ in the panel that pops up.

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

Did you know?

For this tutorial, we will use the default values for the air properties. It’s possible, however, to edit each one of the values from Figure 13 by clicking on them.

2.2 Assign the Boundary Conditions

The physical situation simulated is a car moving with 20 \(m/s\) through a breezeless environment. 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, breezeless air, 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 patch. To do so, create a new boundary condition, selecting ‘Velocity Inlet‘ from the drop-down menu, as seen in Figure 16.

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, let’s set the velocity in the x-direction to 20 \(m/s\).

b. Pressure Outlet

Create a second boundary condition, this time a ‘Pressure Outlet’. In incompressible analysis, the user has to specify a 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:

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, but won’t allow flow in a normal direction. This is a good approximation to the top and side faces of the enclosure, which are far away from the car.

Therefore, assign the slip wall condition to the top and the right side of the domain, as seen below:

d. Symmetry

As previously discussed, a ‘Symmetry’ boundary condition will be applied to the symmetry plane, since we expect mirrored aerodynamic flow patterns along this plane:

e. Wall: Moving Wall

Now, we are going to assign a boundary condition to the road. Create yet another ‘Wall’ boundary condition. This time, set (U) Velocity to ‘Moving wall’. In this configuration, the user can specify the tangential component for the fluid velocity on the assigned faces.

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:

f. Wall: No-Slip

The next ‘Wall’ boundary condition will have a no-slip condition for (U) Velocity. This defines a velocity equal to zero on the assigned entities.

Furthermore, we will use ‘Wall functions’ to model the near-wall velocity profiles. Assign this boundary condition to the previously created ‘Body’ topological entity set.

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

g. 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 23, we are using Onshape to determine the coordinates of a point on the rotation axis for the front wheel.

Rotation axis: this is the axis around 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 24:

(ω) Rotational velocity: the last parameter to define is the rotational velocity ω (\(rad/s\) for the wheels. It can be calculated using the 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 \(m\) (see Figure 23). 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 the figure below:

Define (U) Velocity as ‘Rotating wall’;

Input (0.916, -0.97, 0.349) for the Point on axis coordinates;

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 ‘Front Wheel’ topological entity set.

h. Wall: Rotating Wall – Rear Wheel

Finally, 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 last ‘Wall’ boundary condition as shown below:

Define (U) Velocity as ‘Rotating wall’;

Input (3.584, -1, 0.349) for the Point on axis coordinates;

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.

2.3. Set the Numerics & Simulation Control

The Numerics settings can be left as default.

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;

EnablePotential foam initialization. This setting initializes the velocity field and enhances stability in the early iterations.

Did you know?

In a steady-state simulation, the End time and Delta t parameters control the number of iterations to be performed. With the default settings, a simulation consists of a total of 1000 iterations, which is enough for most simulations to converge.

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 are determined as follows:

x coordinate: halfway between the center of the front and rear wheel;

y coordinate: on the symmetry plane;

z coordinate: on the ground level;

Using Onshape to determine the exact coordinates, our Center of rotation is located on (2.246, 0, 0).

Set the positive z-axis as the Lift direction by applying 1. The other axis receive a value of 0;

Set the positive x-axis as the Drag direction by applying 1. The other axis receive a value of 0;

Set the positive y-axis as the Pitch direction by applying 1. The other axis 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 across 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.

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.

Important

Be careful when setting up the result control parameters, as they are used by the algorithm to calculate the drag and lift coefficients.

For the drag and lift formulas, and more examples on how to set up the forces and moment coefficients result control, please refer to the following articles:

For the meshing operation, we recommend using the standard algorithm. The standard mesher is a good choice in general, as it is quite automated and delivers good results for most geometries, with the following default properties:

Did you know?

Often, large changes in the mesh’s cell sizes only occur in a few regions. Increasing the global mesh refinements rises the cells drastically.

When using the standard mesher, SimScale offers a physics-based meshing option, which automatically refines the regions around the inlets and outlets.

You can also do this manually, by using one of the local refinement options, foremost being local element size and region refinements.

If you want to learn more about the Standard meshing algorithm, please have a look at the relevant documentation page.

3.1 Adding Refinements

Why do we need mesh refinements?

In external aerodynamic simulations, as air flows around the body, two regions have important physical effects: the regions close to the car body and the wake region, which develops downstream from the object.

Since the gradients in velocity and pressure are large in those areas, they require finer cells to be resolved accurately. Therefore, further refinements will be necessary.

To add a refinement to your mesh, click on the ‘+ button’ next to Refinements.

a. Region Refinements

First, let’s create region refinements downstream from the car to capture the wake of the aerodynamic flow. A region refinement is used to refine the volume mesh for one or more user-specified geometry primitives.

First, create two new cartesian boxes, which will be assigned to the region refinements later on. Click on the ‘+ button’ next to the Geometry primitives in the right-hand side panel.

Then choose a ‘Cartesian Box’ from the drop-down menu.

The dimensions of the first box are the following:

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

Notice how the box extends further downstream from the car. The objective is to capture the high gradients from the wake, which is pictured in Figure 32.

Repeat the process for a second Cartesian box, now with the given dimensions:

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

We are now ready to create the region refinements. Using Figure 33 as a reference, create a ‘Region refinement’. Set the Maximum edge length to 0.1 \(m\) and toggle on the ‘Large Box‘ selection:

Repeat the process for the Small Box. 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

This refinement is applied to faces, and limits the cell edge lengths based on the input.

Create a ‘Local element size’ 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 31. 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 25 minutes to complete and this is what it will look like:

Be Aware

This tutorial presents how the simulation is set up for a successful CFD run. The setup for this tutorial is simplified. To ensure the reliability of the results, a series of studies have to be performed.

Further tests with finer meshes, improved layering control, extended enclosures, etc., should be performed. Naturally, it’s important to make sure that each of the simulation runs are also converging. For bigger meshes, it might be necessary to prescribe more iterations.

For more insights on how to assess convergence in a CFD simulation, please refer to this documentation page.

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, 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.

Note

A red warning message may appear, stating that the duration of the simulation exceeds the maximum runtime. The defined maximum runtime of 30000 seconds will be enough for this simulation, therefore, please proceed by clicking on ‘Start’:

The simulation run takes from 2 to 3 hours 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.

5.2 Surface Visualization

After accessing the post-processor by clicking on ‘Solution Fields‘, 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’.

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

In Figure 48, 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.

5.3 Cutting Planes

If you want to observe the aerodynamic flow characteristics around the car click the ‘Add filters’ button and create a ‘Cutting Plane’:

Configure the cutting plane by following the steps below:

Change the Position by changing the coordinates to: 12.5, -0.5, 7.495.

Make sure the Orientation is on the ‘Y’ axis.

Change the Coloring to ‘k’.

For example, the figure below is a cutting plane that is placed around the vehicle showing the turbulent kinetic energy (k) around the car.

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 where aerodynamic flow separation occurs. 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 enclosure and the streamlines will be shown from the start point. You can also modify the number of particles under # Seeds horizontally and # Seeds vertically. We will use ’20’ points horizontally and ’30’ points vertically. Change the Spacing of the streamlines to ‘5e-2’ and the size to ‘1e-2’.

Animations can be started by choosing ‘Animation’ from the Filters panel. Click the play button to start the animation.

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 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!

This website uses cookies so that we can provide you with the best user experience possible. Cookie information is stored in your browser and performs functions such as recognising you when you return to our website and helping our team to understand which sections of the website you find most interesting and useful.

Strictly Necessary Cookies

Strictly Necessary Cookie should be enabled at all times so that we can save your preferences for cookie settings.

If you disable this cookie, we will not be able to save your preferences. This means that every time you visit this website you will need to enable or disable cookies again.