Sign-up for free online course on ANSYS simulations!...
In order to test our simulation for convergence, we will refine the mesh. Refining the mesh will allow us to make sure that the results we are calculating are independent of 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. Under Method click the radio box next to Gradient. 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. In order to do this, click on Contours.... This will open the familiar Contours window. In the Contours window, select Contours of Adaption... Existing Value, then press Compute. This will populate the Contours menu with the values were were viewing for adaption, in this case, gradient of the static pressure. Also, make sure to uncheck Node Values (by first checking filled).
Finally, press Display to display the contours of static pressure gradient.
Our goal is to discover the areas of high gradient, and mark those areas for adaption. Using the contour graph we can then find the areas of high pressure gradient that we want to refine. In the Contours window, uncheck Auto Range. This will allow us to specify the range of gradients we can see in the graph. Change the Min value to 10000. Then press Display. You will see that the pressure gradients above 10000 generally mark the area of high pressure gradient quite well. We will use 10000 as our threshold for refinement.
Return to the Gradient Adaption window, and enter 10000 into Refine Threshold. Then press Mark. The print window will inform us we have marked 70 elements for refinement. Next, 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 150).
| HTML |
|---|
<iframe width="560" height="315" src="https://www.youtube.com/embed/49U2YxZ9JsA?rel=0" frameborder="0" allowfullscreen></iframe> |
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.
...
In order to verify our simulation, we need to compare our results to either an analytical solution or an experiment. Below is a table comparing the values from the simulation with the calculations from the pre-analysis.
Mach Number | Static Pressure (atm) | Shock Angle (degrees) | |
|---|---|---|---|
Theory Value | 2.254 | 2.824 | 32.22 |
FLUENT Solution | 2.243 | 2.803 | 34.99 |
Percent Difference | 0.8% | 0.7% | 8.2% |
As we can see from the table, we are getting fairly good matching match between the computation and analytical approaches. From this we can build our trust in our simulation. Note that in this case, adaptive mesh refinement doesn't have a significant effect on the values behind the shock but makes the shock less smeared.
Save Project
Save the project using File > Save. Copy wedge.wbpj and the associated wedge_files folder to a flash drive. You will need both entities to resume the project.
Alternately, you can select File > Archive and save the project as one file called wegewedge.wbpz. When prompted, select the option to save Result/Solution also. You will then need to save only this file. This is also convenient to e-mail the project. Double-clicking on the wedge.wbpz file will resume the project. Note on some computers, double-clicking the wbpz file will open it in ANSYS AIM (a different application) rather than ANSYS Workbench. This is not right. The workaround is to start Workbench and then select File > Open.