# Wing - CFD Simulation

Source: https://help.sim-flow.com/tutorials/wing
Last updated: 2026-10-14

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

## 1. Introduction

In this tutorial, we are examining the airflow around the wing’s profile. We will focus on the two-dimensional flow around the wing’s airfoil. To enhance precision, we will implement the second-order velocity discretization method following the initial run. The presentation of results will be done in ParaView, utilizing streamlines.

## 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 *wing*.

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

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

## 4. Import Geometry

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

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

![Wing 02 Import Geometry](https://help.sim-flow.com/tutorials/images/wing/Wing_02_Import_Geometry.png)

## 5. Imported Geometry Units

The STL format does not contain the unit information, which is 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 the *Geometry size* label. In our case, the default unit meter is correct.

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

![Wing 02 unit](https://help.sim-flow.com/tutorials/images/wing/Wing_02_unit.png)

## 6. Geometry - Wing

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

1. Set the XY orientation **View XY**
2. Click **Fit View** to fit geometry in the view

![Wing 03 Geometry](https://help.sim-flow.com/tutorials/images/wing/Wing_03_Geometry.png)

## 7. 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.

1. Go to *Hex Meshing* panel
2. Select *wing*
3. Enable *Mesh Geometry*
4. Enable *Create Boundary Layer Mesh*
5. Set *Refinement* to *Min 4* *Max 7*

![Wing 04 Hex meshing](https://help.sim-flow.com/tutorials/images/wing/Wing_04_Hex_meshing.png)

## 8. 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.

1. Go to *Base* tab
2. Select *Plate* as a *Base Mesh Type*
3. Define minimum and maximum extent
   *Min \({\sf [m]}\)*`-15``-15`
   *Max \({\sf [m]}\)*`20``15`
4. Set the division of the base mesh
   *Division*`105``90`

![Wing 05 Base](https://help.sim-flow.com/tutorials/images/wing/Wing_05_Base.png)

## 9. 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.

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

You can specify the point location from the 3D view. Hold the `CTRL` key and drag the arrows to the destination.

![Wing 06 Mat point](https://help.sim-flow.com/tutorials/images/wing/Wing_06_Mat_point.png)

## 10. 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 cell count.

1. Switch to *Mesh* tab
2. Go to *Settings*
3. Change *Cells Between Levels* to `5`
4. Start the meshing process with **Mesh** button

![Wing 07 Meshing](https://help.sim-flow.com/tutorials/images/wing/Wing_07_Meshing.png)

## 11. Mesh

After the meshing process is finished, the mesh should appear in the graphics window.

1. Click **Fit View** to fit mesh in the view

![Wing 08 Mesh](https://help.sim-flow.com/tutorials/images/wing/Wing_08_Mesh.png)

## 12. Examine Mesh

For further examination, we should zoom in to see the refinement mesh. Additionally, we can switch the projection view from perspective to parallel as the parallel view is more appropriate for visualizing 2D objects.

1. Zoom in the mesh - use the *Scroll Wheel* or drag mouse with `RMB` (right mouse button) pressed
2. Click on *Change View Projection*
3. Select *Parallel* view

![Wing 09 Mesh 2](https://help.sim-flow.com/tutorials/images/wing/Wing_09_Mesh_2.png)

## 13. Simulation Type

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

![Simulation Panel](https://help.sim-flow.com/assets/images/go-to-simulation-panel@2x.png)

![Step 1](https://help.sim-flow.com/assets/images/solvers-selection/simpleFoam/01_single_phase@2x.png)

![Step 2](https://help.sim-flow.com/assets/images/solvers-selection/simpleFoam/02_low_speed@2x.png)

![Step 3](https://help.sim-flow.com/assets/images/solvers-selection/simpleFoam/03_steady-state@2x.png)

![Step 4](https://help.sim-flow.com/assets/images/solvers-selection/simpleFoam/04_apply@2x.png)

## 14. Turbulence

For the purpose of this tutorial, we will simulate the turbulence phenomenon using the *\(k{-}\omega \; SST\)* model.

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

![Wing 11 Turbulence](https://help.sim-flow.com/tutorials/images/wing/Wing_11_Turbulence.png)

## 15. 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.

1. Go to *Boundary Conditions* panel
2. Select *boundaries*
3. Set the *Free Stream* character
4. 5 Change the velocity type and value accordingly
   *U Type*`Free Stream`
   *U Freestream Value \({\sf [m/s]}\)*`40``0``0`

![Wing 12 BC inlet](https://help.sim-flow.com/tutorials/images/wing/Wing_12_BC_inlet.png)

## 16. Boundary Conditions - Boundaries (Turbulence)

In addition to flow conditions, we will modify the default free stream turbulence properties.

1. Switch to *Turbulence* tab
2. Set the *k* *Intensity [-]* to `1e-02`

![Wing 13 BC turbulece](https://help.sim-flow.com/tutorials/images/wing/Wing_13_BC_turbulece.png)

## 17. Monitors - Forces

In order to measure aerodynamic forces, we will use the force monitor. We will observe drag and lift force coefficients on the airfoil boundary.

1. Go to *Monitors* panel
2. Switch to *Forces* tab
3. Expand *Monitored Boundaries* list and check *wing*
4. Check *Monitor Coefficients* option
5. Set lift direction vector along Y axis
   *Lift Direction*`0``1``0`
6. Set pitch axis vector along Z axis
   *Pitch Axis*`0``0``1`
7. Set the reference velocity
   *\(U_{\infty}\) \({\sf [m/s]}\)*`40`

![Wing 14 Monitor Force](https://help.sim-flow.com/tutorials/images/wing/Wing_14_Monitor_Force.png)

## 18. Run - Time Control

1. Go to *RUN* panel
2. Set the maximal *Number of Iterations* to `250`
3. Click **Run Simulation** button

![Wing 15 RUN](https://help.sim-flow.com/tutorials/images/wing/Wing_15_RUN.png)

## 19. Results - Force Coefficient

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

1. Go to *Force Coefficient* tab

![Wing 15 1 Residuals](https://help.sim-flow.com/tutorials/images/wing/Wing_15_1_Residuals.png)

## 20. Postprocessing - ParaView

After the computation is finished, we can do a comprehensive visualization of our results with ParaView.

1. Go to *POSTPROCESSING* panel
2. Click on **Run ParaView**

![Wing 16 PV postprocessing](https://help.sim-flow.com/tutorials/images/wing/Wing_16_PV_postprocessing.png)

## 21. ParaView - Load Results

After opening ParaView, we need to load the simulation results from SimFlow.

1. Select your case *wing.foam*
2. Click **Apply** to load results into ParaView
3. Click *Load a color palette* and choose *White Background*
4. Select the velocity *U* from the list
5. Load the latest results by clicking the *Last Frame* icon
6. Click *Rescale to data range*
7. 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.

![Wing 17 PV import results](https://help.sim-flow.com/tutorials/images/wing/Wing_17_PV_import_results.png)

## 22. ParaView - Choose Preset

1. Click *Edit Color Map* from the menu placed on the left side
2. Select *Choose Preset* from the *Color Map Editor* placed by default on the right side of ParaView
3. Search `rainbow`
4. Choose *Blue to Red Rainbow* preset
5. **Apply** changes
6. **Close** Choose Preset window
7. Set *Number of Table Values* to `20`
8. Click *Save current color map settings values as default for all arrays*

![Wing 18 PV preset](https://help.sim-flow.com/tutorials/images/wing/Wing_18_PV_preset.png)

## 23. ParaView - Streamlines

We can visualize the flow by displaying the streamlines.

1. Select your case *wing.foam*
2. Select *Stream Tracer* from top menu
3. Set the start point and end point of the streamline source
   *Point1*`-5``-3``0.5`
   *Point2*`-5``3``0.5`
4. Set the number of streamlines
   *Resolution*`300`
5. Click **Apply**
6. Select *StreamTracer1*
7. Select the velocity *U* from the list
8. Zoom in to the wing profile

![Wing 18 PV Streamlines settings](https://help.sim-flow.com/tutorials/images/wing/Wing_18_PV_Streamlines_settings.png)

## 24. ParaView - Import Wing Geometry (I)

To display the wing geometry with the streamlines, we need to read the geometry file into ParaView.

1. Select *Open* from top menu
2. From the bottom left menu select *wing* folder
3. From the right menu open *constant* and then *triSurface* folder
4. Select *wing.stl*
5. Press **OK**

![Wing 19 PV Import geometry](https://help.sim-flow.com/tutorials/images/wing/Wing_19_PV_Import_geometry.png)

## 25. ParaView - Import Wing Geometry (II)

Confirm default properties and display geometries with streamlines.

1. Click **Apply** to load geometry
2. After loading geometry, it will be shown in the 3D graphic window

![Wing 20 PV Import geometry 2](https://help.sim-flow.com/tutorials/images/wing/Wing_20_PV_Import_geometry_2.png)

## 26. Discretization - Convection

After the preliminary calculation, we will continue with a more accurate algorithm. Go back to SimFlow but do not close ParaView yet. Change the velocity discretization to the *Linear Upwind* scheme. This will decrease numerical diffusion affecting the results.

1. Go to *Discretization* panel
2. Switch to *Convection* tab
3. Click on *Upwind* to expand the list
4. Select *Linear Upwind*

![Wing 21 Discretization](https://help.sim-flow.com/tutorials/images/wing/Wing_21_Discretization.png)

## 27. Run - Continue Simulation

1. Go to *RUN* panel
2. Increase the *Number of Iterations* to `500`
3. Click **Continue Simulation** button

Estimated computation time: 1 minute

![Wing 22 RUN 2](https://help.sim-flow.com/tutorials/images/wing/Wing_22_RUN_2.png)

## 28. Force Coefficient

You can observe in the *Force Coefficient* plot that after switching to second order, the coefficients started to oscillate.

1. Switch tab to *Force Coefficient*

![Wing 23 Force coeff](https://help.sim-flow.com/tutorials/images/wing/Wing_23_Force_coeff.png)

## 29. ParaView - Reload the results

Switch window to ParaView once again. To read newly calculated steps, we need to reload the results.

1. Click **Refresh**
2. Click *Last Frame* to display the latest results

![Wing 24 PV Streamlines update](https://help.sim-flow.com/tutorials/images/wing/Wing_24_PV_Streamlines_update.png)

## 30. 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.

![Wing 25 PV Streamlines](https://help.sim-flow.com/tutorials/images/wing/Wing_25_PV_Streamlines.png)

## 31. 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)