In this tutorial you will learn how to perform a two dimensional simulation of a wing section with a double-slotted flap.
Before you begin download the geometry file.
- Click Load Geometry button
- Select geometry file
- Click Open
After the geometry is loaded it will appear in the 3D window. The geometry was prepared for the simulation and it was scaled so that all the dimensions are in meters. Additionally the geometry was located in a way that the XY plane is the symmetry plane of the model.
Geometry Meshing Properties
Now you need to define meshing parameters for the wing geometry.
- Go to Hex Meshing panel
- Enable meshing of the
- Enable boundary layer
wingmeshing parameters by clicking on the name
- Set minimum refinement to 4
- Set maximum refinement to 7
For the 2D simulation, you can use a dedicated Plate mesh type.
- Go to Base tab
- Select Plate mesh type
- Define minimum of the base mesh bounds
- Define maximum of the base mesh bounds
- Set the division of the base mesh
Material Point Location
Location of the material point indicates to the meshing algorithm on which side of the geometry the mesh is to be retained.
- Go to Point tab
- Specify location inside base mesh but outside the wing geometry
Define Mesh Size Transition
To make cell size vary slower throughout the domain increase the number of buffer cells between each cell refinement level.
- Go to Controls tab
- Select Castellated Mesh tab
- Increase Cells Between Levels to 5
Start the Meshing Process
When everything is set up you can start the meshing process. In this particular case, it usually takes a few minutes.
- Go to Mesh tab
- Click Mesh button to start meshing process
After meshing is finished the new mesh will be displayed in the 3D window.
You want to analyze incompressible turbulent flow around the wing. For this purpose you should use the
- Go to Setup panel
- Pick the
- Submit selected solver with Select button
You can use standard
k-ω SST model to handle turbulence. This model gives very good agreement with experimental data and is commonly used for aerodynamics problems.
- Go to Turbulence panel
- Expand the Model drop-down menu
You need to define free-stream boundary conditions on the external boundary.
- Go to Boundary Conditions panel
Free Streamcharacter for the
- Define free-stream velocity
In order to set low turbulence level in the free-stream:
- Go to Turbulence tab
- Set turbulence intensity to
Enable Force Monitors
You may want to monitor simulation process by observing plots of the force coefficients.
- Go to Monitors panel
- Go to Forces tab
wingboundary to monitor
- Select Monitor Coefficients
- Define Lift Direction to be along
- Define Pitch Axis to be along
- Set reference velocity equal to free-stream velocity
- Go to Run panel
- Set number of iterations to 250
- Click Run Calculation
End time in steady state simulation (such as this one) represents the number of iterations.
End time in transient simulation is expressed in seconds.
Start Postprocessing with ParaView
- Go to Postprocessing panel
- Start ParaView
- In ParaView click Apply to load results
- Load latest results
- Select velocity U from the drop-down menu
- Re-scale color map to fit result range
You can drag right mouse button to zoom in and out the view.
- Create Stream Tracer
- Select seed from
High Resolution Line Source
- Define start point of the line
- Define end point of the line
- Click Apply to display streamlines
Now you want to display geometry file located in the
- Click Open
- Find and select geometry file
- Click OK to load geometry
- Click Apply to display geometry
Streamlines with Geometry
Streamlines flowing around the geometry can now be observed in the 3D window.
Second Order Discretization
Return to simFlow and change velocity discretization to second order to increase accuracy.
- Go to Discretization panel
- Go to Convection tab
- Expand velocity scheme
Linear Upwinddiscretization scheme
vectorvariant of the scheme
- Return to Run panel
- Increase the number of iterations to at least 500
- Click Run Calculation
You can observe in the Force Coefficient plot that after switching to second order the coefficients started to oscillate.
To observe the cause for this oscillation load the latest results into ParaView.
- Click Refresh load all newly created result files
- Click Last Frame to display the latest results
In the 3D window you can now observe that there is a flow separation on the second flap airfoil. This separation is the cause of the flow instability that results in oscillating values of the force coefficients.
This concludes this tutorial.