Verification & Validation

Verification

Adapt the Mesh

In order to test our simulation for convergence, we will refine the mesh. However, instead of refining the mesh everywhere (which would be wasteful, as most of the area of the domain far away from the shock has constant values), we will use our results to refine our mesh. Specifically, we are going to use the gradient of the pressure to determine where to refine the mesh. First, let's take a look at our mesh. In the Outline window, select Graphics and Animations, under _Graphics, select Mesh, then press Setup. Select all of the surfaces (except y=0.35) and press Display. This will display the current mesh.

You may now close the Mesh Display window. In the menu bar, go to Adapt > Gradient. Under Options uncheck Coarsen. Ensure that Gradients of > Pressure... Static Pressure are selected. Then press Compute.

This will compute the maximum and minimum gradients of static pressure. Next, we need to pick a threshold. For every element that has a pressure above that threshold, that element will be refined. Let's make our threshold 10000. Enter 10000 into Refine Threshold. Then press Adapt. You will be asked if you want to change the mesh. Press Yes.

It will seem like nothing has changed, but that is because we need to re-display the mesh in order to see the adaption. The new mesh should look something like this.

Notice that the area surrounding the shock was refined. Now, re-initialize the solution, (Solution Initialization > Compute From Farfield > Initialize), and rerun the solution (you will also need to increase the number of iterations – I recommend 3000).

Now, once again, plot the contours of the mach number. Below is a comparison of the mach number results from the original mesh and the refined mesh.

Original Mesh

Refined Mesh

The most striking difference between the two results is the thickness of the shock. Notice that for the refined mesh, the shock is less thick that for the original mesh. This shows that the refined mesh is converging towards the real case.

Separated Shock

Next, we will alter the geometry to achieve a separated shock. Close FLUENT and open the Design Modeler. We want to increase the angle of the wedge above its critical angle. We will increase the angle to 35 degrees. Change the geometry's dimensions to match that of the diagram below.

Once the geometry has changed, close the design modeler. We will have to re-calculate the solution, but we will want to change some factors affecting the solution. Usually, when you make an upstream change in ANSYS, the program will update all of the downstream data. We want to break this connection, so right click and select
Reset. We will have to input the boundary conditions again, but that shouldn't take long – and will end up saving us time when we calculate the solution inside of the FLUENT environment.

Next, open up the mesher by double clicking . Update the mesh by clicking . Close the mesher, click , then once again double click . Re-enter all of the data from Step 5 (here is link for reference). This time, set the Courant Number to 1.0. This will make the solution a little more unstable, but it will solve much, much faster. Run the solution again, this time with 5000 iterations.