2. Create Case
Open SimFlow and create a new case named wing
Go to New panel
Provide name wing
Click Create Case
3. Import Geometry
Firstly, we need to Download GeometryWing
Click Import Geometry
Select geometry file wing.stl
Click Open
4. Imported Geometry Units
The STL format does not contain the unit information which are defined during the geometry export. If we do not know the exported unit, we can estimate it based on the total size of the model. It is displayed next to Geometry size label. In our case, the default unit meter is correct.
To confirm default unit meter, press OK
5. Geometry - Wing
After importing geometry, it will appear in the 3D window.
Set the XY orientation View XY
Click Fit View to fit geometry in the view
6. Meshing Parameters - Wing
In order to create the mesh, we need to specify geometry options for the meshing process. We will increase mesh resolution near the wing surface.
Go to Hex Meshing panel
Select wing
Enable Mesh Geometry
Enable Create Boundary Layer Mesh
Set Refinement to Min 4 Max 7
7. Base Mesh - Domain
Our simulation will be limited to a 2D flow. This can be accomplished by choosing the Plate type as the background mesh.
Go to Base tab
Select Plate as a Base Mesh Type
Define minimum and maximum extend
Min \({\sf [m]}\)-15-15
Max \({\sf [m]}\)2015Set the division of the base mesh
Division10590
8. Material Point
Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. Since we are considering flow around the wing we need to place the material point outside the geometry.
Go to Point tab
Specify location inside base mesh but outside wing geometry
Material Point-200
You can specify the point location from the 3D view. Hold the CTRL key and drag the arrows to the destination.
9. Start Meshing
We can define the count of the buffer cells between refinement levels. This parameter determines the width of the transition zone between refined and background mesh. A higher value of this parameter will increase the overall cells count.
Switch to Mesh tab
Go to Settings
Change Cells Between Levels to 5
Start the meshing process with Mesh button
10. Mesh
After the meshing process is finished the mesh should appear in the graphics window.
Click Fit View to fit mesh in the view
11. Examine Mesh
For further examination, we should zoom in to see the refinement mesh. Additionally, we can switch projection view from perspective to parallel as the parallel view is more appropriate for visualizing 2D objects.
Zoom in the mesh - use the Scroll Wheel or drag mouse with RMB (right mouse button) pressed
Click on Change View Projection
Select Parallel view
12. Select Solver - SIMPLE
We want to compute the steady-state solution of the incompressible turbulent flow around the airfoil. For this purpose, we will use the SIMPLE (simpleFoam) solver.
Go to SETUP panel
Select Steady State filter
Check Incompressible flow
Pick SIMPLE (simpleFoam) solver
Select solver
13. Turbulence
For the purpose of this tutorial, we will simulate the turbulence phenomenon using the \(k{-}\omega \; SST\) model.
Go to Turbulence panel
Select RANS turbulence formulation
Select \(k{-}\omega \; SST\) model
14. Boundary Conditions - Boundaries (Flow)
The domain has only one external boundary. We will use the Free Stream character type to model the far field conditions. The flow will be aligned with the x-axis.
Go to Boundary Conditions panel
Select boundaries
Set the Free Stream character
5 Change the velocity type and value accordingly
U TypeFree Stream
U Freestream Value \({\sf [m/s]}\)4000
15. Boundary Conditions - Boundaries (Turbulence)
Additionally, to flow conditions, we will modify default free stream turbulence properties.
Switch to Turbulence tab
Set the k Intensity [-] to 1e-02
16. Monitors - Forces
In order to measure aerodynamic forces, we will use the force monitor. We will observe drag and lift force coefficients on the aerofoil boundary.
Go to Monitors panel
Switch to Forces tab
Expand Monitored Boundaries list and check wing
Check Monitor Coefficients option
Set lift direction vector along Y axis
Lift Direction010Set pitch axis vector along Z axis
Pitch Axis001Set the reference velocity
\(U_{\infty}\) \({\sf [m/s]}\)40
17. Run - Time Control
Go to RUN panel
Set the maximal Number of Iterations to 250
Click Run Simulation button
18. Results - Force Coefficient
During the simulation, we can observe whether forces on the wing stabilize which will mean that our simulation converges
Go to Force Coefficient tab
19. Postprocessing - ParaView
After the computation is finished we can do a comprehensive visualization of our results with ParaView.
Go to POSTPROCESSING panel
Click on Run ParaView
20. ParaView - Load Results
After opening the ParaView, we need to load the simulation results from SimFlow.
Select your case wing.foam
Click Apply to load results into ParaView
Click Load a color palette and choose White Background
Select the velocity U from the list
Load the latest results by clicking Last Frame icon
Click Rescale to data range
After loading results they will be shown in the 3D graphic window. Your default color map may be different than the one below. Go to the next slide and choose an appropriate preset.
21. ParaView - Choose Preset
Click Edit Color Map from the menu placed on the left side
Select Choose Preset from the Color Map Editor placed by default on the right side of the ParaView
Search rainbow
Choose Blue to Red Rainbow preset
Apply changes
Close Choose Preset window
Set Number of Table Values to 20
Click Save current color map settings values as default for all arrays
22. ParaView - Streamlines
We can visualize the flow by displaying the streamlines.
Select your case wing.foam
Select Stream Tracer from top menu
Set the start point and end point of the streamline source
Point1-5-30.5
Point2-530.5Set the number of streamlines
Resolution300Click Apply
Select StreamTracer1
Select the velocity U from the list
Zoom in to the wing profile
23. ParaView - Import Wing Geometry (I)
To display the wing geometry with the streamlines, we need to read the geometry file to the ParaView.
Select Open from top menu
From the bottom left menu select wing folder
From the right menu open constant and than triSurface folder
Select wing.stl
Press OK
24. ParaView - Import Wing Geometry (II)
Confirm default properties and display geometries with streamlines.
Click Apply to load geometry
After loading geometry, it will be shown in the 3D graphic window
25. Discretization - Convection
After preliminary calculation, we will continue with a more accurate algorithm. Go back to the Simflow but do not close the ParaView yet. Change velocity discretization to the Linear Upwind scheme. This will decrease numerical diffusion affecting the results.
Go to Discretization panel
Switch to Convection tab
Click on Upwind to extend the list
Select Linear Upwind
26. Run - Continue Simulation
Go to RUN panel
Increase the Number of Iterations to 500
Click Continue Simulation button
Estimated computation time: 1 minute
27. Force Coefficient
You can observe in the Force Coefficient plot that after switching to second-order the coefficients started to oscillate.
Switch tab to Force Coefficient
28. ParaView - Reload the results
Switch window to ParaView once again. To read newly calculated steps we need to reload the results.
Click Refresh
Click Last Frame to display the latest results
29. ParaView - Streamlines Results
Finally, we can see the results in the 3D window. We observe the flow separation on the second flap. This separation is the cause of the flow instability that we have observed as oscillating values of the force coefficients.
