1. Download SimFlow
SimFlow is a general purpose CFD Software
To follow this tutorial, you will need SimFlow free version, you may download it via the following link:
Download SimFlow
2. Create Case
Open SimFlow and create a new case named car
Go to New panel
Provide name car
Click Create Case

3. Import Geometry
Firstly we need to Download GeometryCar_body
Click Import Geometry
Select geometry file car_body.stl
Click Open

4. 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, what should help to choose the correct unit. In ours case, the default unit meter is correct.
To confirm default unit meter, press OK

5. Geometry - Car Body
After importing geometry, it will appear in the 3D window
Click Fit View to zoom in on the geometry

6. Meshing Properties - Car Body
After geometry is loaded, we can proceed to define meshing properties. To better resolve the flow around the car body, we want to refine mesh near the car geometry by specifying minimum and maximum refinement levels.
Go to Hex Meshing panel
Select car_body geometry
Enable Meshing Geometry
Refine mesh near the surface of the car_body
Refinement Min 3 Max 5

7. 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.
Go to Base tab
Define base mesh parameters accordingly
Min \({\sf [m]}\)-600
Max \({\sf [m]}\)1468Set the division of the base mesh
Division501520

8. 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.
Define boundary names accordingly
X- inlet
X+ outlet
Y- bottom
Y+ top
Z- symmetry
Z+ right3 Define boundary types accordingly
Y- wall
Z- symmetry

9. 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.
Go to Point tab
Specify location inside base mesh but outside car geometry
Material Point032

10. Start Meshing
Everything is now set up for meshing
Go to Mesh tab
Press Mesh button to start meshing process

11. 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.
Click Graphics Object List icon
Select Mesh to show meshes list

12. Mesh - Toggle Visibility
You can hide domain boundaries to inspect the mesh on the car body.
2 Hide the following objects
bottom
inlet
outlet
right
symmetry
top

13. Select Solver - SIMPLE
We want to analyze incompressible turbulent flow around the car body. For this purpose, we will use the SIMPLE (simpleFoam) solver.
Go to Setup panel
Enable Steady State filter
Enable Incompressible filter
Select SIMPLE (simpleFoam) solver
Select solver

14. 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.
Go to Turbulence panel
Select turbulence model
Turbulence Modelling RANSChange default turbulence model
Model \(k{-}\omega \; SST\)

15. 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 fixed velocity boundary condition on the bottom of the domain.
Go to Boundary Conditions panel
Select bottom boundary
4 Set velocity
UTypeFixed Value
UValue \({\sf [m/s]}\)2000

16. Boundary Conditions - Inlet (Flow)
On the inlet, we are going to apply constant velocity, similarly to the bottom .
Select inlet boundary
Change boundary character
inlet Velocity InletDefine inlet velocity
UReference Value \({\sf [m/s]}\)20

17. Boundary Conditions - Inlet (Turbulence)
We are simulating a car moving in otherwise stationary air. Therefore, we specify low turbulence intensity on the inlet.
Go to Turbulence boundary conditions tab
3 Set the following parameters accordingly
kIntensity \({\sf [-]}\)5e-03
\(\omega\)Mixing Length \({\sf [m]}\)1e-03

18. Boundary Conditions - Right (Flow)
On the right and top boundary, we are going to force velocity to be tangent to the boundary.
Select right boundary condition
Go to Flow tab
4 Define slip wall condition
TypepZero Gradient
TypeUSlip

19. Boundary Conditions - Right (Turbulence)
Go to Turbulence tab
3 Change turbulent kinetic energy and frequency types to
TypekZero Gradient
Type\(\omega\)Zero Gradient

20. Boundary Conditions - Top (Flow)
We need to repeat the same steps to the top boundary condition
Select top boundary condition
Go to Flow tab
4 Define slip wall condition
TypepZero Gradient
TypeUSlip

21. Boundary Conditions - Top (Turbulence)
Go to Turbulence tab
3 Change turbulent kinetic energy and frequency types
TypekZero Gradient
Type\(\omega\)Zero Gradient

22. Monitors - Forces
We want to monitor the simulation process by observing plots of the aerodynamic forces on the car
Go to Monitors panel
Go to Forces tab
Enable observing forces on the car_body boundary
Monitored Boundaries car_body

23. Run Simulation
Go to Run panel
Set maximal number of iteration that solver can perform before stopping
Number of Iterations200Click Run Simulation button
Estimated computation time: 2 minutes

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

25. Postprocessing - ParaView
After the simulation is finished, we can proceed to post-processing
Go to Postprocessing panel
Start ParaView

26. ParaView - Load Results
Make sure you have your case selected car.foam
Click Apply to load results

27. ParaView - Set View Direction
After loading results, we have to rotate the domain or change view direction to see the car.
Click Set view direction to +Z

28. ParaView - Display Velocity
We will now display velocity (U) contours.
Load latest results by clicking Last Frame icon
Select U (velocity) from the dropdown menu
Click Rescale to data range

29. ParaView - Coloring (I)
We can change the coloring scheme in ParaView to have nicer colors.
Click Edit Color Map from the menu placed on the left side, if the panel is not already shown.
Select Choose Preset from the Color Map Editor placed by default on the right side of the ParaView

30. ParaView - Coloring (II)
We can now select a new Color Preset.
Select jet preset
Apply changes
Close the window

31. 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.
Decrease color scale resolution to make velocity regions more distinguishable (non-smooth color transition)
Number of Table Values 20

32. ParaView - Import Geometry
To display results on the original geometry, we can import the geometry directly into ParaView.
Click Open and select the original car_body.stl geometry to import it into ParaView.
Click on the Visibility icon to show the geometry.

33. ParaView - Final Results
Now we can see the final results with the original geometry.
