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

Documentation

# Tutorial: Incompressible Flow around a Formula Student Car

This tutorial shows how an incompressible turbulent airflow around a Formula Student car moving in a straight line can be simulated. Figure 1 shows an example of the resulting flow behavior: Figure 1: The generated streamlines, colored with the velocity magnitude values

This tutorial teaches how to:

• Set up and run an incompressible simulation;
• Use SimScale’s CAD mode features;
• Assign topological entity sets;
• Assign boundary conditions, material, and other properties to the simulation;
• Mesh with SimScale’s 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

Note, if you are not using the tutorial CAD model

Prepare the geometry for the simulation (only if you are not using the tutorial’s CAD model):

• If the CAD model contains small features, fillets or round faces, which are unlikely to have an impact on the result, it is recommended to remove those details before importing the model into SimScale.
• Small and detailed features that don’t greatly affect the aerodynamics, such as bolts etc, should be removed or simplified.
• The solid volumes should be non-overlapping and should all be touching each other.

With this approach, you 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.

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

The following picture demonstrates what should be visible after importing the tutorial project: Figure 2: The imported CAD model of the Formula Student vehicle cut in half to leverage symmetry and reduce computational cost

At the right of the Workbench, the parts of the model can be seen. This is a watertight assembly of the P19 model, provided by the Prom Racing FSAE Team, with an aerodynamic package of a rear wing, a front wing, a configuration of elements at the sides of the car, an undertray, and finally sidepods that enclose radiators. The suspension system can be included, as long as it is simplified.

## 1.1. Edit in CAD Mode

For an incompressible analysis, only one part is allowed, which is the flow region. In case we want to add a cell zone too, we will have to include this part too. For the specific case, the car also includes a radiator, that will be modeled as a porous medium, so it is important that both the flow region and radiator remain as the only, and separate, parts. This is possible with the CAD mode features that allow performing a variety of operations, such as flow volume extractions, parts deletion, etc.

Note

In case that the model does not include parts to be modeled as cell zones, you can create an Enclosure, as described in this documentation page.

To enter the CAD mode, click on the CAD model and choose the option as shown below: Figure 3: Entering the CAD mode so that flow volume extractions and other geometry operations can be performed

Create an External flow volume extraction first. Figure 4: The external flow volume extraction is used to generate the domain of the simulation, which represents the surrounding air.

The size of the domain is chosen according to the reference length (L) of the model. Here, the reference length is the horizontal distance from the tip of the nose, to the back of the rear wing. 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 in the negative z-direction, so that the ground can be tangent to the wheels;
• Other directions: 3 times the length of the vehicle. Figure 5: The recommended sizing of the domain for a car aerodynamics case
• Enter the following dimensions that appear in the figure below, according to the recommended sizing that was introduced before;
• Enable the Seed face assignment;
• Choose a face of the car as a seed to indicate the flow region;
• Enable the Excluded parts assignment;
• Choose the Radiator from the scene tree at the right, so it is excluded. This will be later used as a cell zone;
• Create the domain by clicking ‘Apply’. Figure 6: Setting a new external flow volume extraction that represents the domain

We will use the Delete body feature afterward, to make sure only the flow region and the cell zone remain in the final version. Figure 7: The Delete feature removes all the unwanted parts, and keeps the flow region and the parts intended to be used as cell zones.

Remove everything except the Radiator and the Flow region.

Click on the ‘Export’ option to be redirected to the Workbench.

The final version will appear as ‘Copy of Formula Student car’. Before the setup, feel free to rename the new geometry as ‘Formula Student car’, and delete the one that is no longer necessary.

Did you know?

It is possible to rename a CAD model by clicking on it’s name and adding the name title:

Also, a geometry can be deleted by clicking on the trash icon, as you can see below:

### 1.1 Create the Simulation

To get started, click on ‘Create a Simulation’:

Doing so, the analysis type choice widget opens. 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 panel. We have to set up all entries, to be able to run the simulation. 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.

The global settings of the simulation remain as default: Figure 14: Incompressible analysis properties including the turbulence model and time dependency

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.

### 1.2 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.
For this tutorial, three topological entity sets will be used, one which will include all the faces of the Formula Student car, and one for each wheel.
First, hide the walls of the domain by selecting all of them (the face color must turn red), then right-clicking in the Workbench, and choosing the ‘Hide selection‘ option: Figure 15: Hiding the walls of the domain after manually selecting them

Activate the box selection and drag the cursor across the screen until all the remaining faces turn red. Then click on the ‘+’ icon under Topological entities. Name it as ‘Full car’. Figure 16: The faces of the whole Formula Student car that were selected with the box assignment.

Proceed to create a set for the wheels too. Each wheel consists of 9 faces, and we will need to rotate and adjust the model in order to click on all of them before the set creation. The following photo shows how the topological set of the front wheel should appear afterward, when everything else is hidden. See how the faces on the inside were included too: Figure 17: The topological entity of the front wheel, consisting of 11 faces

## 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 ‘+’ icon next to Materials:

Choose ‘Air‘ in the panel that pops up and click ‘Apply’: Figure 19: List of pre-saved fluid materials available in SimScale

To assign the flow region as air, click on ‘Flow region’ under the scene tree as shown below. Leave the properties as default: Figure 20: The air properties that are used to model the fluid medium

### 2.2 Assign the Boundary Conditions

The physical situation simulated is a straight line movement with 15 $$m \over s$$. An overview of the boundary conditions for the domain can be seen below: Figure 21: Overview of the boundary conditions applied on the domain faces

Similarly, for the car walls, the following boundary conditions are applied: Figure 22: Overview of the types of wall boundary conditions applied on the faces of the Formula Student car

Except for the wheels, all other faces of the car will receive a no-slip wall boundary condition.

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

a. Velocity Inlet

The straight-line simulation of a breeze-less environment can be achieved by setting a velocity inlet boundary condition at the frontal face of the domain. First, add a ‘Velocity inlet’ boundary condition from the menu:

The velocity value is 15 $$m \over s$$, and it represents the speed of the vehicle. It must be set according to the orientation cube, that is placed at the bottom right of the Workbench. Here, the air travels towards the negative x-direction, so $$U_x$$ should be set to -15 $$m \over s$$, and the remaining components are set to 0 $$m \over s$$: Figure 25: Assigning the fixed velocity value on the inlet of the domain

b. Pressure Outlet

As seen in the rest of the incompressible fluid dynamics tutorials, the most common boundary condition for the outlet of an external aerodynamics case is a zero Dirichlet condition for the gauge pressure. Proceed by selecting the ‘Pressure outlet‘ on the menu.

Rotate the CAD model and assign the condition on the outlet: Figure 27: Setting a 0 $$Pa$$ gauge pressure condition on the outlet of the domain

c. Walls: Slip Condition

There are many types of wall conditions to use and all of them can be checked here. The top and right faces of the domain represent the open-air environment, and by setting the wall velocity to ‘Slip‘, its normal component is erased, and the tangential components remain untouched. Select the ‘Wall‘ category from the menu first: Figure 28: To add any type of wall conditions, select the general category from the menu. Later we can select the specific usage.

Change the type of the wall by setting the (U) Velocity option, to ‘Slip‘. Figure 29: As the project simulates open-air conditions, the top and right sides should be set to slip walls.

d. Wall: Moving Wall

Another use of the wall category is to model a moving surface, like the ground.

• For this set, switch the (U) Velocity to ‘Moving wall‘;
• The components of the velocity are treated exactly like the flow inlet. Figure 30: The ground under the still faces of the car is modeled as a moving wall, to simulate the movement.

e. Symmetry

We are using half the Formula Student car model to save resources. Set the plane that is coincident with the cut surface as symmetry to indicate that the domain is mirrored. Select ‘Symmetry‘ from the Boundary conditions menu:

Then click on the respective side of the domain to set it as the mirroring plane: Figure 32: The face of the domain that “cuts” the model in half is picked as the symmetry plane.

f. Wall: Rotating Wall – Front Wheel

For each one of the two wheels, we will create a new wall set, but this time, it will be modeled as a rotating wall.

For the setting of the rotation axis, we will be using the right-hand rule. Use the following figure as reference: Figure 33: According to the right-hand rule, for a body that rolls towards the positive X direction, the positive Y direction should be selected as the rotation axis.

• Change the (U) Velocity to ‘Rotating wall‘;
• Set the coordinates of the wheel’s center of rotation. This can be measured in a CAD software. For this case, enter the following values:
• $$x$$: -0.91567 $$m$$
• $$y$$: 0.5983 $$m$$
• $$z$$: 0.20574 $$m$$
• Once again, the orientation cube indicates the correct direction of the rotation. Here, the car travels parallel to the positive $$x$$ direction, so according to the right-hand rule, the rotation axis is the $$y$$ direction;
• The rotational velocity is calculated with the formula: $$ω$$ = $$U \over r$$, where:
• $$U$$: the linear velocity
• $$r$$: the radius of the wheel
• Select the ‘Front wheel‘ topological entity set from the geometry tree. Figure 34: Setting the rotating wall boundary condition for the front wheel

g. Wall: Rotating Wall – Rear Wheel

The same procedure as before is followed for the rear wheel set. This time, the center of rotation coordinates are:

• $$x$$: -2.44567 $$m$$
• $$y$$: 0.5583 $$m$$
• $$z$$: 0.20574 $$m$$

Select the ‘Rear wheel’ topological entity set at the end: Figure 35: Setting the rotating wall boundary condition for the rear wheel

### 2.3. Advanced Concepts

Note

If you are using your own model, that does not include a radiator, you can skip this section.

A radiator can be modeled as a porous media. There are different types, and each approach is described in this knowledge base article. Figure 36: Choosing the Darcy-Forchheimer medium over the other available porous media practices

We will set four sections of settings for the porous medium, based on the Radiator’s placement and experimental data. The advanced concept can be either assigned to a volume, as in this project, or to user-created geometry primitive, like a cartesian box.

Have a look at this guide to learn more on how to set up unit vectors for the porous media.

• The first section, $$d$$, that stands for Darcy, is a linear resistance coefficient which has three entries, one for each direction. Apply the following values:
• $$d_x$$: 98008228.5 $$1 \over m^2$$
• $$d_y$$: 980082284.8 $$1 \over m^2$$
• $$d_z$$: 980082284.8 $$1 \over m^2$$
• The second section, $$f$$, includes three more entries, the Forchheimer resistance coefficients.
• $$f_x$$: 1050.8 $$1 \over m$$
• $$f_y$$: 10508.4 $$1 \over m$$
• $$f_z$$: 10508.4 $$1 \over m$$
• For a radiator that is angled, the Orientation should be set to ‘Custom‘;
• The appropriate coordinates of the Unit vector x are:
• $$x$$: -0.93256 $$m$$
• $$y$$: 0.09751 $$m$$
• $$z$$: 0.3476 $$m$$
• And for the Unit vector y:
• $$x$$: 0.33942 $$m$$
• $$y$$: 0.09119 $$m$$
• $$z$$: 0.9362 $$m$$ Figure 37: The resistance coefficients and the unit vectors of the porous media.

After the setup is complete, click on the ‘Radiator’ in the scene tree to assign the concept to it.

### 2.4. Set the Numerics & Simulation Control

The Numerics settings can be left as default, except from the absolute tolerance of $$omega$$, as it was observed to reach values smaller than 1e-6.

• Go to the Solvers section;
• Expand the $$ω$$ Specific dissipation rate;
• Set the absolute tolerance to ‘1e-8’. Figure 39: In order to avoid the oscillation of omega’s residual, reduce the absolute tolerance on the Numerics control.

In the simulation tree, click on ‘Simulation control’  and configure it like this:

• In order to create an animation with the simulation results, set the Write interval to 100, then the results will be written every 100 iterations, resulting in a simulation with 10 frames (without including the initial condition at 0 $$sec$$;
• Change the Maximum runtime for the simulation to ‘30000’ $$sec$$;
• Enable ‘Potential foam initialization‘. This setting initializes the velocity field and enhances stability in the early iterations. Figure 40: Increasing the maximum runtime, so the simulation will not be automatically canceled after 10000 sec.

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 Analysis.

### 2.5. Results Control

This section is important for the post-processing of the simulation run. There are many different features under the Result Control that we can use to evaluate the vehicle’s performance.

#### Forces and Moments

With the Forces and moments, we can extract the pressure, viscous and porous forces, and moments of various parts of the model. Figure 41: Under the Result control section, all of the available sets are listed, including the Forces and moments that will be use.

Lift and drag coefficients are some of the most important parameters when evaluating the performance of a vehicle. The center of rotation can be calculated externally using the CAD software, and for this specific geometry it has the following coordinates:

• $$x$$: -0.57895 $$m$$
• $$y$$: 0.23262 $$m$$
• $$z$$: 0.31138 $$m$$ Figure 42: Assigning the forces and moments set to the whole car apart from the faces of the radiator.

#### Force and Moment Coefficients

We can also create a Force and moment coefficients set, to monitor the drag and lift coefficients, $$C_d$$ and $$C_l$$ respectively.

• For this set, the coordinates of the center of rotation remain as in Table 1.
• The direction of lift, drag and pitch are set according to the coordinate cube:
• Set the positive z-axis as the Lift direction by assigning ‘1’. The other axis receive a value of ‘0’;
• Set the positive x-axis as the Drag direction by assigning ‘1’. The other axis receive a value of ‘0’;
• Set the positive y-axis as the Pitch direction by assigning ‘1’. The other axis receive a value of ‘0’;
• Apart from these, some new inputs must be also added, according to the boundary conditions and the characteristics of the Formula Student car:
• (|U<∞>|) Freestream velocity magnitude: 15 $$m \over \ s$$
• Reference length: 2.891 $$m$$, calculated with the CAD software
• Reference Area value: 0.59 $$m^2$$

The Reference area value is a projection of the frontal vehicle area onto a plane. When using half the Formula Student car geometry, the area projection must account only for half of the model. One way to do it is to create a sketch and project the faces on the plane. Then check the designed area. Figure 43: By projecting the faces on a new sketch, the reference area can be calculated.

The final Forces and moment coefficients panel should appear like this: Figure 44: We can calculate the appropriate inputs for the force coefficients in the CAD software, and then apply them on this tab.

Assign the result control to all of the car faces except the Radiator, like we did for the previous Result control set.

#### Field Calculations

Include more parameters in the results by clicking on the ‘+‘ icon and selecting each one of the entries. With the turbulence, for example, we will be able to check the $$y^+$$ value and make sure it is below 1. Figure 45: By adding field calculation we will be provided more parameters to be evaluated after the simulation run.

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:

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

## 3. Mesh

When the simulation is created with the standard mesher, the mesh set up is placed right before the end, as the boundary conditions were previously set on the faces of the enclosure. This means that even if the mesh is changed and re-generated, we will not have to re-assign the boundary conditions. Click on ‘Mesh‘ so we it starts. Figure 46: Accessing the mesh settings from the simulation tree

### 3.1. Create Geometry Primitives

Initially, we will create two cartesian boxes and region refinements will be assigned to each one of them later.
Click on the ‘+‘ button next to Geometry primitives, and choose the ‘Cartesian Box‘ option like below: Figure 47: After entering the Mesh section, create a cartesian box by adding a new geometry primitive on the geometry tree.

The first cartesian box is the biggest of the two and has the following dimensions, that are set in the same way as the background mesh box, which is by having a maximum and minimum value for each direction:

• Minimum x value: ‘-15’ $$m$$
• Minimum y value: ‘0’ $$m$$
• Minimum z value: ‘-0.001’ $$m$$
• Maximum x value: ‘3’ $$m$$
• Maximum y value: ‘3’ $$m$$
• Maximum z value: ‘3’ $$m$$ Figure 48: The dimensions of the big cartesian box

Then create the small box, with the following dimensions:

• Minimum x value: ‘-6’ $$m$$
• Minimum y value: ‘0’ $$m$$
• Minimum z value: ‘-0.001’ $$m$$
• Maximum x value: ‘1’ $$m$$
• Maximum y value: ‘1’ $$m$$
• Maximum z value: ‘1.5’ $$m$$ Figure 49: The dimensions of the small cartesian box

### 3.2. Apply the Main Mesh Settings

Go back to the Mesh panel, and make the following changes:

• Expand the ‘Automatic boundary layers’ section to prepare the boundary layer mesh creation. For this case, the full resolution wall treatment will be implemented instead of the wall functions, so the desired $$y+$$ value range is (0,1). So switch the Overall relative thickness to ‘0.1’, the Layer gradation control to ‘Specify first layer thickness’, and the First layer size to ‘4e-5’ $$m$$. This will be applied to all of the no-slip walls of the case;

Resolving the boundary layer

If you are using your own model, you can use this page to manually calculate the first layer thickness according to your case, or even try this online calculator. Keep in mind that if you choose the latter, you should double the result of the calculator, as your input should concern the whole thickness, not just the distance from the wall to the cell center that the calculator provides.

• De-activate the ‘Physics-based meaning’, so we can later introduce the radiator as a cell zone. If the model does not need to get assigned advanced concepts, keep this activated;
• Expand the ‘Advanced settings’ section to control the meshing. Set the Small feature suppression to ‘4e-5’ $$m$$, exactly like the first layer thickness. This will be the smallest edge resolved, which means that the fineness of the mesh will be reduced, reserving computational resources. Figure 50: The main settings for the standard mesher include the fineness of the global mesh, automatic boundary layer generation, and advanced options.

### 3.3. Add Refinements

For the standard mesher, several refinement options can be selected by the user to get the required mesh. These are all specified under the Refinements mesh sub-tree.

#### Region Refinements

The region refinement is used to refine the volume mesh for one or more user-specified volume regions under Geometry primitives. Add a Region Refinement by clicking on the ‘+’ icon next to Refinements, and then choosing the ‘Region Refinement’ option.

The first region refinement that we will create is matched to the big cartesian box. The Refinement mode will be automatically set to Inside. This refines all volume mesh cells inside the surface up to specified maximum edge length. The surface needs to be closed for this to be possible.

• Set the Maximum edge length to ‘0.15′;
• Toggle on the ‘Big box‘ for the assignment. Figure 52: Assigning a region refinement to the big cartesian box

Then add a second region refinement for the small cartesian box. This time:

• Set the Maximum edge length to ‘0.1’;
• Toggle on the ‘Small box’ for the assignment. Figure 53: Assigning a region refinement to the small cartesian box

#### Local Element Size

Add this type of surface refinement by clicking on the ‘+’ icon next to the Refinements, and then choosing the ‘Local Element Size’ option.
We will set a maximum edge length for the cells on the assigned surfaces.

• Set the Minimum edge length to ‘0.01’ $$m$$;
• Assign the refinement to the whole vehicle by clicking on the ‘Full car’ topological set as shown below. Figure 54: Assigning a local element size refinement to the surfaces of the whole vehicle

### 3.4. Add the Cell Zone

During the mesh setup, all the parts used for advanced concepts should be added as cell zones.

• Click on the ‘+’ icon next to Cell zones;
• Select the ‘Radiator‘ from the scene tree.

### 3.5. Generate Mesh

Go back to the main mesh tab. An estimation of the duration of the meshing procedure, the core hours that will be spent, as well as the size of the mesh, will appear. Click on the ‘Generate‘ option to get started. Figure 56: Before the mesh is generated, the tab introduces a variety of estimations.

### 3.6. Meshing Results

After approximately 30 minutes, the mesh is ready, and the icon next to the Mesh section on the simulation tree will have a green checkmark.

It is possible to zoom in to check the generated boundary layer or even create a mesh clip to inspect the interior of the mesh. Figure 58: The generated boundary layer for full resolution treatment is very thin, and can only be observed if we zoom in.

## 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 ‘+’ icon 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, we can already have a look at the intermediate results in the post-processor. They are being updated in real-time!

There is also a link to the finished project at the end of the tutorial.

Warning

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’: Figure 60: Creating a new run. Proceed by clicking on ‘Start’.

The simulation run takes a few hours to finish, depending on the model that is used, and its complexity. This case finished after 218 minutes. During the simulation, we can access the post-processing environment by clicking on ‘Solution Fields’ after expanding ‘Run 1‘: Figure 61: We can post-process the current state of the run by clicking on the ‘Solution Fields‘.

## 5. Post-Processing

After the simulation is finished, we can extend Run 1 to check the results.

### 5.1. Convergence Plot

Make sure to check whether the simulation converged or not, by expanding the Convergence plots section, and then clicking on ‘Residuals‘. Figure 62: During the simulation, the residual values should constantly reduce until they stabilize around a low value.

### 5.2 Forces and Moments

The drag and lift are available in the ‘Forces and moments’ graph that appears after expanding Force plot: Figure 63: All the forces and moments that were calculated can be retrieved from this graph.

The plot shows us how the values 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 flow parameters.

It is also possible to download the results in .csv format and analyze them with an external program, and get the average value from the final iterations. This can be done for all the plots by clicking on the icon at the top right of the plot, and selecting the format you want to export: Figure 64: All the available formats we can export the results to

The same steps can be applied to the Force coefficients plots section too.

### 5.3 Post-Processing Interface

In order to enter the post-processor, click on the ‘Post-process results’ option:

The first thing we might see is the whole domain, colored with pressure values. We can change the coloring, as shown in the next section, or use other features, in the Filters toolbar, and select one of the available choices. Figure 66: All the filters that are included in the new integrated post-processor

#### Surface visualization (Parts Color)

Initially, click on the walls of the flow domain, right-click on the screen, and choose ‘Hide selection’, so only the Formula Student car is visible:

When the walls are hidden, we will see the pressure distribution on the car:

The warm-colored contours showcase the areas with the highest pressure values. As expected, these are the upper sides of the downforce-generating airfoils, as well as surfaces that are the first to come in contact with the freestream air, such as the nosecone, the driver’s body, etc.

Pressure is not the only parameter that can be visualized on the model’s faces. We can switch to another parameter by changing the Coloring option. Figure 69: All the available parameters that are available for visualization are listed in this Coloring menu.

#### Cutting Planes

We can check different slices of the flow region, by creating cutting planes. For example, we can visualize the velocity on a plane that cuts across the front wing.

• Position: Extend this section, so that the coordinates of the seed face can be selected.
• Orientation: We can either choose the axis that the plane will be normal to or extend the section to customize the direction;
• Coloring: By clicking on this, we can select the parameter we want to visualize. The following figure uses the magnitude of the velocity.

Hide the ‘Parts Color‘ and activate the ‘Clip model‘ option, so the only feature that appears is the slice we created: Figure 70: Adding a cutting plane to visualize velocity on a slice normal to the y axis

Suction regions with very low velocities can be analyzed with blue contours, as well as the acceleration of the flow below the front wing, which is a clear indication of downforce generation.

#### Particle Trace

One more useful feature is the streamlines. To create this, select ‘Particle Trace’ from the Filters toolbar. The whole domain will appear at first, and we will choose the position of the seed face, by clicking on the inlet, in front of the car. This will be the starting point of the streamlines: Figure 71: The seed face indicates the source of the streamlines.

Only the streamlines and the radiator will be visible. Close the ‘Particle Trace 1’ tab, right-click on the workbench, and choose the ‘Show all’ option: Figure 72: Bring back to visibility all of the faces.

Proceed to select all six faces of the domain and hide them, like in Figure 67. Go back to the Particle Trace tab, and modify the number of particles under # Seeds horizontally and # Seeds vertically. For this tutorial, we can use ‘5’ points horizontally and ‘100’ points vertically. Change the Spacing of the streamlines to ‘5e-2’ and the size to ‘4e-3’.

With streamlines, the flow around the complex structures can be better analyzed. Other than the velocity magnitude, the visualization of the vorticity on the streamlines can help with the recognition of the areas that need smarter design and optimization.

We can customize the streamlines and other features as we wish, by changing the inputs on each tab. Have a look at our post-processing guide to learn how to use it.

Congratulations! You finished the aerodynamic flow behavior of an FSAE car tutorial!

Note

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

Last updated: March 15th, 2022