Supersonic Flow Past a Wedge

This 2D verification test case studies steady inviscid compressible flow past a wedge at an incident angle of 15 degrees. As the supersonic flow (Ma = 2.5) hits the wedge a sharp oblique shock wave is formed, resulting in a reduced downstream flow velocity. The simulation uses the inviscid compressible Euler equations to model the flow, adaptively refining the mesh, and using FEM-TVD upwinding to stabilize the solution and resolve shock discontinuities [1].

The angle of the shock wave and downstream Mach number can be determined using oblique shock theory, Ma = 1.873526 at an angle of 36.9449 degrees, and also comparing to results from the NASA/NPARC CFD Verification and Validation Database and from the Wind-US CFD code [2].

Tutorial

This model is available as an automated tutorial by selecting Model Examples and Tutorials... > Fluid Dynamics > Supersonic Flow Past a Wedge from the File menu. Or alternatively, follow the step-by-step instructions below. Note that the CFDTool interface differ slightly from the FEATool Multiphysics instructions described in the following.

1. To start a new model click the New Model toolbar button, or select New Model... from the File menu.
2. Select the Euler Equations physics mode from the Select Physics drop-down menu.
3. Press OK to finish the physics mode selection.

The geometry can be created by splitting a rectangle at the base of the wedge.

1. To create a rectangle, first click on the Create square/rectangle Toolbar button. Then left click in the main plot axes window, and hold down the mouse button. Move the mouse pointer to draw the outline of the shape, and release the button to finalize the shape.
2. Select R1 in the geometry object Selection list box.
3. To modify and edit the selected rectangle, click on the Inspect/edit selected geometry object Toolbar button to open the Edit Geometry Object dialog box.
4. Enter 0 into the x_min edit field.
5. Enter 2 into the x_max edit field.
6. Enter 0 into the y_min edit field.
7. Enter 1 into the y_max edit field.
8. Press OK to finish and close the dialog box.

First split the rectangle at the point (1, 0) at and angle of 15 degrees, and then split again at 15 + 36.9449 degrees (to create an internal edge where the shock will be), then delete the lower segment.

1. Select R1 in the geometry object Selection list box.
2. Press the Split selected geometry object(s) with cutline Toolbar button.
3. Enter 1 0 into the Cutline point edit field.
4. Enter 1 atan(pi*15/180) into the Cutline direction vector edit field.
5. Press OK to finish and close the dialog box.
6. Select SP1 in the geometry object Selection list box.
7. Press the Split selected geometry object(s) with cutline Toolbar button.
8. Enter 1 0 into the Cutline point edit field.
9. Enter 1 atan(pi*(15+36.9449)/180) into the Cutline direction vector edit field.
10. Press OK to finish and close the dialog box.
11. Select SP2 in the geometry object Selection list box.

12. Press the Delete selected geometry object(s) Toolbar button.

    
13. Switch to Grid mode by clicking on the corresponding Mode Toolbar button.
14. Press the Settings Toolbar button.

Open the Grid Settings dialog box and prescribe a smaller value to the inner boundary.

1. Enter 0.05 0.05 0.001 0.05 0.05 0.05 0.05 into the Boundary Grid Size edit field.
2. Press the Generate button to call the grid generation algorithm.

3. Press OK to finish and close the dialog box.

   
4. Switch to Equation mode by clicking on the corresponding Mode Toolbar button.

First select both subdomains, and enter placeholder names for the initial flow coefficients.

1. Select 1 and 2 in the Subdomains list box.
2. Enter 1.4 into the Ratio of specific heats edit field.
3. Enter rho0 into the Initial condition for rho edit field.
4. Enter u0 into the Initial condition for u edit field.
5. Enter v0 into the Initial condition for v edit field.

6. Enter p0 into the Initial condition for p edit field.

   

For this problem it is beneficial to use FEM-TVD stablilization (Shock Capturing - Low Order), which ensures that the shock can be captured sharply without unphysical over or under-shoots.

1. Press the Artificial Stabilization button.
2. Clear the Enable/disable isotropic artificial diffusion check box.
3. Clear the Enable/disable streamline diffusion check box.

4. Select the Enable/disable shock capturing check box.

   
5. Press OK to finish and close the Artificial Stabilization dialog box.
6. Press OK to finish the equation and subdomain settings specification.
7. Press the Constants Toolbar button, or select the corresponding entry from the Equation menu, to open the Model Constants and Expressions dialog box. Enter the following expressions for the fluid parameters, and inlet velocity.

Name	Expression
Ma	1.4
rho0	1
p0	1
u0	Ma*sqrt(1.4*p0/rho0)
v0	0

1. Switch to Boundary mode by clicking on the corresponding Mode Toolbar button.
2. Select 4 in the Boundaries list box.
3. Select Inlet/outlet from the Euler Equations drop-down menu.
4. Enter rho0 into the Density edit field.
5. Enter u0 into the Velocity in x-direction edit field.
6. Enter v0 into the Velocity in y-direction edit field.

7. Enter p0 into the Pressure edit field.

   
8. Select 2 and 6 in the Boundaries list box.
9. Select Neutral/no stress boundary/outlet from the Euler Equations drop-down menu.
10. Press OK to finish the boundary condition specification.
11. Switch to Solve mode by clicking on the corresponding Mode Toolbar button.
12. Press the Settings Toolbar button.
13. In the Non-Linear Solver Settings section of the Solver Settings dialog box increase the Maximum non-linear iterations to 50, and decrease the Non-linear relaxation parameter to 0.9, to allow for the non-linear problem to converge.
14. To start the solver with the chosen settings press the Solve button, or press OK and then the = Toolbar button.

After the problem has been solved FEATool will automatically switch to postprocessing mode and here display the magnitude of the computed velocity field where the shock pattern can easily be seen. Plot the Mach number and click on a point in the downstream region to verify that the lower Mach number is close to the reference value (1.873526).

1. Press the Plot Options Toolbar button.
2. Select Mach number from the Predefined surface plot expressions drop-down menu.
3. Select the Enable/disable contour plot check box.
4. Select Mach number from the Predefined contour plot expressions drop-down menu.

5. Press OK to plot and visualize the selected postprocessing options.

   

The supersonic flow past a wedge fluid dynamics model has now been completed and can be saved as a binary (.fea) model file, or exported as a programmable MATLAB m-script text file (available as the example ex_compressibleeuler6 script file), or GUI script (.fes) file.

References

[1] D. Kuzmin, High-resolution FEM-TVD schemes based on a fully multidimensional flux limiter, Journal of Computational Physics, vol. 198, pp. 131-158, 2004.

[2] NPARC Alliance, Computational Fluid Dynamics (CFD) Verification and Validation Web Site.