Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field


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:

flow behavior shown by streamlines around a car
Figure 1: Post-processing of the CFD simulation results with streamlines

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.

The following picture demonstrates what should be visible after importing the tutorial project:

import cad model simscale workbench to study the flow behavior
Figure 2: The imported CAD model of the vehicle.

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.

car symmetry plane cfd
Figure 3: Half of the car geometry, with the XZ symmetry plane highlighted in red

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

1.2. CAD Mode

The first step for this simulation is the creation of a bounding box. 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 for the simulation, so it is important that the SimScale features are used to generate this unique flow part around the geometry that was imported. Eventually, this geometry will be discarded, so only the flow volume remains. To enter the CAD mode click on the following icon:

entering the CAD mode environment
Figure 4: Clicking on this icon will redirect you to the CAD mode interface.

Select ‘Flow volume’ under, at the top left of the interface.

top menu of CAD mode containing all the operation options
Figure 5: All of the available features in the CAD mode are located at the top of the interface.

The External option that is listed in the drop down menu is used to create the flow domain around the model:

flow volume options on the CAD Mode external and internal
Figure 6: External aerodynamics typically use the ‘External’ option for the flow volume creation.

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.
enclosure size to analyze the external flow behavior around a car
Figure 7: The recommended sizing of the domain for a car aerodynamics case

For this simulation project, we are going to use only half of the car, due to symmetry. Set up the enclosure dimensions in meters as shown below:

enclosure external flow domain for cfd analysis of vehicle
Figure 8: While creating the sizing of the enclosure in CAD mode, you can visualize the result.
  • X min: ‘-17.5’ \(m\)
  • Y min: ‘-15’ \(m\)
  • Z min: ‘-0.005’ \(m\)
  • X max: ‘37.5’ \(m\)
  • Y max: ‘0’ \(m\)
  • Z max: ‘15.005’ \(m\)

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

deleting the solid body from the model so the flow region is the only part used for the incompressible analysis
Figure 9: The car must also be removed from the model, so only the flow region remains.

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

deleting the car after selecting it from the geometry tree.
Figure 10: The necessary removal of the solid body using the geometry tree in the CAD mode

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

finishing with the CAD mode operations and exiting the interface to proceed with the set up
Figure 11: Go back to the Workbench when only the flow region is present, and the space where the solid part was located is now hollow.

When the Workbench loads, another geometry appears which is the copy created from the original model, after the CAD mode operations. You can delete the initial version as follows:

delete original CAD model after CAD mode edit
Figure 12: Deleting the CAD model can help avoiding confusion between different versions.

Rename the new version as ‘Car’ as well:

rename the new CAD model after CAD Mode
Figure 13: To rename the new version, place your cursor next to the checkmark, until the edit icon appears. Then click on it to enter a new name.

1.3 Create the Simulation

Figure 14 shows the resulting enclosure. Proceed by clicking on the ‘Create Simulation’ button.

create new simulation after the CAD mode
Figure 14: The CAD model is now ready to be used for the simulation set up.

Doing so opens the analysis type choice widget:

incompressible cfd analysis
Figure 15: 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:

turbulence incompressible cfd analysis
Figure 16: Incompressible analysis properties

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.

1.4 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. To begin with, you will have to hide the walls of the enclosure. In order 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.

hiding the walls of the domain on the workbench by selecting them first
Figure 17: To manually select the faces of the wheel, the walls of the enclosure must be hidden using the workbench.

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

  • 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.
assigning topological entity set front wheel car
Figure 18: Adding a topological entity set for the front wheel faces

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

topological entity vehicle body assignment workbench
Figure 19: Creating a topological entity set for the vehicle’s body
  • 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 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’ from the material library that pops up.

material option list
Figure 20: List of presaved fluid materials available in SimScale

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

air assignment and properties to flow region
Figure 21: Air properties

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 21 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:

boundary condition overview domain to analyze the flow behavior around a car
Figure 22: Overview of the boundary conditions applied to the walls of the enclosure

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

boundary condition overview car to study the flow behavior
Figure 23: An overview of the boundary conditions as applied on the topological entity sets of the car

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

boundary conditions new simulation tree
Figure 24: Adding a new boundary condition

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 24.

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’ \(m/s\).

velocity inlet airflow domain face assignment to analyze flow behavior
Figure 25: Velocity inlet for the airflow.

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:

pressure outlet cfd domain fixed value gauge
Figure 26: Pressure outlet on 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 for the top and side faces of the enclosure, 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:

assigning slip wall boundary condition external aerodynamics
Figure 27: Slip wall boundary condition assignment

d. Symmetry

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

symmetry face assignment external aerodynamics domain
Figure 28: Symmetry face of the domain

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:

moving road ground simulation with velocity
Figure 29: The moving road assignment on the bottom face

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.

no-slip wall assignment on vehicle's body
Figure 30: No-slip wall boundary condition for the faces of the vehicle’s body

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 31, we are using Onshape to determine the coordinates of a point on the rotation axis for the front wheel.
point on axis coordinates cad software
Figure 31: Obtaining the coordinates for a point on the front wheel’s axis of rotation
  • 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 32:
rotating walls axis of rotation right-hand rule
Figure 32: Rotation axis in the negative y-direction (red) and the resulting direction of rotation (blue), due to the right-hand rule.
  • (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 31). 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:

rotating wall set up wheel
Figure 33: Setting the rotating wall properties for the front wheel
  • 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:

rotating wall set up wheel
Figure 34: Setting the rotating wall properties for the rear wheel
  • 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:

simulation control settings
Figure 35: Simulation control properties
  • 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.

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.

For more notes on the simulation control settings, please visit the following page: Simulation control for fluid flow simulations.

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:

forces and moments coefficients result control creation
Figure 36: Adding a set of coefficients calculation

Please set up the result control as below:

forces and moments coefficients drag lift pitch center of rotation projected area reference length
Figure 37: Settings for the force and moment coefficients result control
  • 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 axes receive a value of ‘0’;
  • Set the positive x-axis as the Drag direction by applying ‘1’. The other axes receive a value of ‘0’;
  • Set the positive y-axis as the Pitch direction by applying ‘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.
car reference projected area
Figure 38: Using Onshape to determine the projected frontal area of half of the car
  • 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.


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:

How to analyze the pitch, lift, and drag coefficients?
Why are my lift and drag coefficients too big/small?

3. Mesh

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, including a ‘Small feature suppression‘ of 0.001 \(m\) under the Advanced settings:

standard mesher default settings external aerodynamic flow car simulation
Figure 39: The settings for the standard mesher.

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 number of 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.

flow behavior around car wake region
Figure 40: Velocity profile around the car. Notice sudden changes around the car body and also the wake region downstream.

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.

creating mesh refinements standard mesher
Figure 41: Adding a new mesh refinement

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.

geometry primitive creation
Figure 42: Adding a new geometry primitive

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

cartesian box geometry primitive creation
Figure 43: Cartesian box geometry primitive creation

The dimensions of the first box are the following:

region refinement wake region car cfd to capture the flow behavior for aerodynamic analysis
Figure 44: First cartesian box created for region refinements.
  • 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 40.

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

region refinement wake region car cfd to capture the flow behavior for aerodynamic analysis
Figure 45: Small cartesian box created for a region refinement. The smaller box also extends further downstream.
  • 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 41 as a reference, create a ‘Region refinement’. Set the Maximum edge length to ‘0.1’ \(m\) and toggle on the ‘Large Box‘ selection:

large cartesian box region refinement for aerodynamic analysis
Figure 46: Setting the region refinement properties for the large Cartesian box

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’ \(m\):

small cartesian box region refinement
Figure 47: Setting the region refinement properties for the small Cartesian box.

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.

local element size maximum edge length front and rear wheel for aerodynamic flow
Figure 48: Local element size settings for the wheels.

3.2 Meshing Results

Now you can go back to the main meshing settings and click on ‘Generate’, as in Figure 39. 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:

meshing result for aerodynamic tutorial to analyze the flow behavior
Figure 49: Mesh result; take a look what each refinement is doing.

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.

new simulation run simulation tree for aerodynamic flow
Figure 50: Creating a new simulation run

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.


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’:

creating a new simulation run warning
Figure 51: Creating a new run. You can proceed by clicking on ‘Start’

The simulation run takes about 2 hours to finish. At this point, you can access the post-processing environment by clicking on ‘Solution Fields’ or ‘Post-process results’:

accessing the post-processing environment simulation aerodynamic flow
Figure 52: Accessing the post-processing environment for a finished simulation run.

5. Post-Processing

5.1 Force and Moment Coefficients

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

forces and moments coefficients results of the aerodynamics flow behavior
Figure 53: Forces and moments result control, showing how the coefficients are changing over the iterations.

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’. 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.

first look at the post-processor
Figure 54: Pressure distribution in the fluid domain is automatically displayed when entering the post-processor. Changing the Coloring in the Filters panel will change the quantity visualized.

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

hide selection tutorial simscale
Figure 55: Hiding the enclosure of the car to better visualize pressure distribution on the vehicle.

In Figure 56, 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. In order to add a smooth distribution of the colors on the vehicle, right-click on the legend at the bottom, and select the ‘Use continuous scale” :

pressure results on car stepped scale
Figure 56: The pressure distribution on the vehicle with a stepped scale.

The upgrade in the visualization quality is evident:

Pressure-Distribution around a vehicle simscale
Figure 57: Visualization of pressure distribution on the vehicle. Visualize other quantities by changing the Coloring in the Filters panel.

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’:

steps to create a cutting plane
Figure 58: Selecting ‘Cutting Plane’ from the Filters ribbon

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 ‘Turbulent Kinetic Energy’;
  • Set the maximum value of the range to ’10’ \(\frac{m^2} {s^2}\) and use the continuous scale feature.

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;
  • Modify the number of particles under # Seeds horizontally and # Seeds vertically. Use ’20’ points horizontally and ’30’ 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]’ \(m \over s \).
air flow around a vehicle streamlines
Figure 59: Setting particle traces around a vehicle with position at the inlet and 20 points horizontally and 30 points vertically.

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.

animation filter for particle traces
Figure 60: Creating an animation filter for particle traces

The result is shown in the animation below:

aerodynamic animation of particle traces around a vehicle
Animation 1: Velocity streamlines around a vehicle with aerodynamic flow separation at the trailing edge of the car combined with pressure contours on the body.

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!


If you have questions or suggestions, please reach out either via the forum or contact us directly.

Last updated: March 15th, 2022