# Car - CFD Simulation

Source: https://help.sim-flow.com/tutorials/car
Last updated: 2026-10-01

![front-image](https://help.sim-flow.com/tutorials/images/car.png)

## 1. Introduction

This tutorial presents a typical approach to external aerodynamic analysis. It considers a steady-state analysis of car body aerodynamic performance. The simulation includes symmetry conditions to reduce the size of the domain, modeling of turbulence, boundary conditions, and baseline postprocessing features.

## 2. Download SimFlow

SimFlow is a general-purpose [CFD Software](https://sim-flow.com/download/cfd-simulation-software/)

To follow this tutorial, you will need the SimFlow free version. You may download it via the following link:
[Download SimFlow](https://sim-flow.com/download-simflow/)

## 3. Create Case

Open SimFlow and create a new case named *car*.

1. Click **New**
2. Provide name `car`
3. Click **Create** to open a new case

![simflow-launcher](https://help.sim-flow.com/tutorials/images/launcher-car.png)

## 4. Import Geometry

Firstly, we need to [Download GeometryCar_body](https://help.sim-flow.com/tutorials/downloads/car/car_body.stl)

1. Click **Import Geometry**
2. Select geometry file *car_body.stl*
3. Click **Open**

![car 2 import geometry](https://help.sim-flow.com/tutorials/images/car/car-2-import-geometry.png)

## 5. Imported Geometry Units

The STL geometry format does not store the unit in which the geometry was created. *Geometry size* shows the overall size of the model in each direction, which should help to choose the correct unit. In our case, the default unit meter is correct.

1. To confirm the default unit *meter*, press **OK**

![car 2 unit](https://help.sim-flow.com/tutorials/images/car/car-2-unit.png)

## 6. Geometry - Car Body

After importing the geometry, it will appear in the 3D window.

1. Click **Fit View** to zoom in on the geometry

![car 3 geometry car body](https://help.sim-flow.com/tutorials/images/car/car-3-geometry-car-body.png)

## 7. Meshing Properties - Car Body

After the geometry is loaded, we can proceed to define meshing properties. To better resolve the flow around the car body, we want to refine the mesh near the car geometry by specifying minimum and maximum refinement levels.

1. Go to **Hex Meshing** panel
2. Select **car_body** geometry
3. Enable *Meshing Geometry*
4. Refine mesh near the surface of the car_body
   *Refinement* *Min 3* *Max 5*

![car 4 hex meshing geometry](https://help.sim-flow.com/tutorials/images/car/car-4-hex-meshing-geometry.png)

## 8. Base Mesh

Base Mesh is a domain mesh of our simulation from which the final mesh will be created by carving out the geometry of the car.

1. Go to **Base** tab
2. Define base mesh parameters accordingly
   *Min \({\sf [m]}\)*`-6``0``0`
   *Max \({\sf [m]}\)*`14``6``8`
3. Set the division of the base mesh
   *Division*`50``15``20`

![car 5 hex meshing base](https://help.sim-flow.com/tutorials/images/car/car-5-hex-meshing-base.png)

## 9. Base Mesh Boundaries

We need to assign individual names to each side of the base mesh in order to be later able to define different conditions on each side.

1. Define boundary names accordingly
   *X-* *inlet*
   *X+* *outlet*
   *Y-* *bottom*
   *Y+* *top*
   *Z-* *symmetry*
   *Z+* *right*
2. 3 Define boundary types accordingly
   *Y-* *wall*
   *Z-* *symmetry*

![car 6 initial boundary conditions](https://help.sim-flow.com/tutorials/images/car/car-6-initial-boundary-conditions.png)

## 10. Material Point

Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. We are modeling car aerodynamics, so our material point needs to be located inside the Base Mesh but outside the car body.

1. Go to **Point** tab
2. Specify location inside base mesh but outside car geometry
   *Material Point*`0``3``2`

![car 7 material point](https://help.sim-flow.com/tutorials/images/car/car-7-material-point.png)

## 11. Start Meshing

Everything is now set up for meshing.

1. Go to **Mesh** tab
2. Press **Mesh** button to start the meshing process

![car 8 meshing](https://help.sim-flow.com/tutorials/images/car/car-8-meshing.png)

## 12. Mesh

After meshing is finished, the new mesh will be displayed in the graphics window. To show the mesh of the car body, we can use the Graphics Object List.

1. Click **Graphics Object List** icon
2. Select **Mesh** to show meshes list

![car 9 mesh](https://help.sim-flow.com/tutorials/images/car/car-9-mesh.png)

## 13. Mesh - Toggle Visibility

You can hide domain boundaries to inspect the mesh on the car body.

1. 2 Hide the following objects
   *bottom*
   *inlet*
   *outlet*
   *right*
   *symmetry*
   *top*

![car 10 toggle visibility](https://help.sim-flow.com/tutorials/images/car/car-10-toggle-visibility.png)

## 14. Simulation Type

We want to analyze the airflow around the car body. For this purpose, we will use a single-phase, steady-state simulation of incompressible turbulent flow.

## 15. Turbulence

We are going to use the standard \(k{-}\omega \; SST\) model to handle turbulence. This model gives very good agreement with experimental data and is commonly used for aerodynamics applications.

1. Go to **Turbulence** panel
2. Select turbulence model
   *Turbulence Modelling* *RANS*
3. Change default turbulence model
   *Model* *\(k{-}\omega \; SST\)*

![car 12 turbulence](https://help.sim-flow.com/tutorials/images/car/car-12-turbulence.png)

## 16. Boundary Conditions - Bottom (Flow)

We are simulating a car moving on a road. In this reference frame, the road has to move with respect to the car. We can achieve this by applying a fixed velocity boundary condition on the bottom of the domain.

1. Go to **Boundary Conditions** panel
2. Select **bottom** boundary
3. 4 Set velocity
   *U**Type*`Fixed Value`
   *U**Value \({\sf [m/s]}\)*`20``0``0`

![car 13 boundary conditions bottom flow](https://help.sim-flow.com/tutorials/images/car/car-13-boundary-conditions-bottom-flow.png)

## 17. Boundary Conditions - Inlet (Flow)

On the inlet, we are going to apply a constant velocity, similarly to the *bottom* .

1. Select **inlet** boundary
2. Change boundary character
   *inlet* *Velocity Inlet*
3. Define inlet velocity
   *U**Reference Value \({\sf [m/s]}\)*`20`

![car 14 boundary conditions inlet flow](https://help.sim-flow.com/tutorials/images/car/car-14-boundary-conditions-inlet-flow.png)

## 18. Boundary Conditions - Inlet (Turbulence)

We are simulating a car moving in otherwise stationary air. Therefore, we specify low turbulence intensity on the inlet.

1. Go to **Turbulence** boundary conditions tab
2. 3 Set the following parameters accordingly
   *k**Intensity \({\sf [-]}\)*`5e-03`
   *\(\omega\)**Mixing Length \({\sf [m]}\)*`1e-03`

![car 15 boundary conditions inlet turbulence](https://help.sim-flow.com/tutorials/images/car/car-15-boundary-conditions-inlet-turbulence.png)

## 19. Boundary Conditions - Right (Flow)

On the right and top boundaries, we are going to force velocity to be tangent to the boundary.

1. Select **right** boundary condition
2. Go to **Flow** tab
3. 4 Define slip wall condition
   *p**Type*`Zero Gradient`
   *U**Type*`Slip`

![car 16 boundary conditions right flow](https://help.sim-flow.com/tutorials/images/car/car-16-boundary-conditions-right-flow.png)

## 20. Boundary Conditions - Right (Turbulence)

1. Go to **Turbulence** tab
2. 3 Change turbulent kinetic energy and frequency types to
   *k**Type*`Zero Gradient`
   *\(\omega\)**Type*`Zero Gradient`

![car 17 boundary conditions right turbulence](https://help.sim-flow.com/tutorials/images/car/car-17-boundary-conditions-right-turbulence.png)

## 21. Boundary Conditions - Top (Flow)

We need to repeat the same steps for the top boundary condition.

1. Select **top** boundary condition
2. Go to **Flow** tab
3. 4 Define slip wall condition
   *p**Type*`Zero Gradient`
   *U**Type*`Slip`

![car 18 boundary conditions top flow](https://help.sim-flow.com/tutorials/images/car/car-18-boundary-conditions-top-flow.png)

## 22. Boundary Conditions - Top (Turbulence)

1. Go to **Turbulence** tab
2. 3 Change turbulent kinetic energy and frequency types
   *k**Type*`Zero Gradient`
   *\(\omega\)**Type*`Zero Gradient`

![car 19 boundary conditions top turbulence](https://help.sim-flow.com/tutorials/images/car/car-19-boundary-conditions-top-turbulence.png)

## 23. Monitors - Forces

We want to monitor the simulation process by observing plots of the aerodynamic forces on the car.

1. Go to **Monitors** panel
2. Go to **Forces** tab
3. Enable observing forces on the car_body boundary
   *Monitored Boundaries* *car_body*

![car 20 monitors forces](https://help.sim-flow.com/tutorials/images/car/car-20-monitors-forces.png)

## 24. Run Simulation

1. Go to **Run** panel
2. Set the maximal number of iterations that the solver can perform before stopping
   *Number of Iterations*`200`
3. Click **Run Simulation** button

Estimated computation time: 20 minutes

![car 21 run simulation](https://help.sim-flow.com/tutorials/images/car/car-21-run-simulation.png)

## 25. Monitor Forces

During the simulation, we can observe whether forces on the car body stabilize, which will mean that our simulation converges.

![car 22 monitor solution](https://help.sim-flow.com/tutorials/images/car/car-22-monitor-solution.png)

## 26. Postprocessing - ParaView

After the simulation is finished, we can proceed to postprocessing.

1. Go to **Postprocessing** panel
2. Start **ParaView**

![car 23 paraview postprocessing](https://help.sim-flow.com/tutorials/images/car/car-23-paraview-postprocessing.png)

## 27. ParaView - Load Results

1. Make sure you have your case selected *car.foam*
2. Click **Apply** to load results

![car 24 paraview load results](https://help.sim-flow.com/tutorials/images/car/car-24-paraview-load-results.png)

## 28. ParaView - Set View Direction

After loading results, we have to rotate the domain or change the view direction to see the car.

1. Click **Set view direction to +Z**

![car 25 paraview set view direction](https://help.sim-flow.com/tutorials/images/car/car-25-paraview-set-view-direction.png)

## 29. ParaView - Display Velocity

We will now display velocity (U) contours.

1. Load the latest results by clicking the **Last Frame** icon
2. Select *U* (velocity) from the dropdown menu
3. Click **Rescale to data range**

![car 26 paraview display velocity](https://help.sim-flow.com/tutorials/images/car/car-26-paraview-display-velocity.png)

## 30. ParaView - Coloring (I)

We can change the coloring scheme in ParaView to have nicer colors.

1. Click **Edit Color Map** from the menu placed on the left side, if the panel is not already shown.
2. Select **Choose Preset** from the Color Map Editor placed by default on the right side of ParaView

![car 27 paraview coloring 1](https://help.sim-flow.com/tutorials/images/car/car-27-paraview-coloring-1.png)

## 31. ParaView - Coloring (II)

We can now select a new Color Preset.

1. Select **jet** preset
2. **Apply** changes
3. **Close** the window

![car 28 paraview coloring 2](https://help.sim-flow.com/tutorials/images/car/car-28-paraview-coloring-2.png)

## 32. ParaView - Coloring (III)

Now we can see the results with the new preset applied. We can also modify the number of displayed colors to see the results better.

1. Decrease color scale resolution to make velocity regions more distinguishable (non-smooth color transition)
   *Number of Table Values* `20`

![car 29 paraview coloring 3](https://help.sim-flow.com/tutorials/images/car/car-29-paraview-coloring-3.png)

## 33. ParaView - Import Geometry

To display results on the original geometry, we can import the geometry directly into ParaView.

1. Click **Open** and select the original **car_body.stl** geometry to import it into ParaView.
2. Click on the **Visibility** icon to show the geometry.

![car 30 paraview import geometry](https://help.sim-flow.com/tutorials/images/car/car-30-paraview-import-geometry.png)

## 34. ParaView - Final Results

Now we can see the final results with the original geometry.

![car 31 final results](https://help.sim-flow.com/tutorials/images/car/car-31-final-results.png)

## 35. Advanced Postprocessing with ParaView

This concludes the tutorial, covering all the aspects we intended to showcase. For a finely tuned presentation of the results, you may take advantage of the more advanced features.

In ParaView, you can display streamlines, contour plots, vector fields, line or time plots, calculate volume or surface integrals and create animations.

To familiarize yourself with the ParaView capabilities, it’s worth checking out our video tutorial, *Paraview CFD Tutorial - Advanced Postprocessing in ParaView*, in which we demonstrate some of the most commonly used postprocessing techniques.

[Paraview CFD Tutorial - Advanced Postprocessing in ParaView](https://www.youtube.com/watch?v=5M6VgXyHB60&list=PLy7xPqn9xXckoD2gZgPpv8mrxillJ9PWU&index=21)