Sign-up for free online course on ANSYS simulations!Unable to render {include} The included page could not be found.
Problem Specification
1. Pre-Analysis & Start-Up
2. Geometry
3. Mesh
4. Setup (Physics)
5. Solution
6. Results
7. Verification & Validation
Problem 1
Site Under Construction
We are working on updating this part of the tutorial. Please come back soon.
Step 7: Verification & Validation
In order to assess the numerical accuracy of the results obtained, it is necessary to compare results on different meshes. We'll re-do the calculation on a 100x60 mesh which has twice the number of nodes in the radial direction as the 100x30 mesh.
In Workbench, under Turbulent Flow project, right click on Fluid Flow (FLUENT) and click duplicate. Rename the duplicate project to Turbulent Flow Refined Mesh. You should have three project cells in workbench.
Double click on Mesh for Forced Convection Refined Mesh. The ANSYS Mesher window will open. Under Outline, expand mesh tree and click on Edge Sizing 2.
Highlight "Edge Sizing 2". Under Details of "Edge Sizing 2", increase Number of Divisions to 60. This will refine the mesh in the radial direction at the inlet.
Highlight "Edge Sizing 3". Under Details of "Edge Sizing 3", increase Number of Divisions to 60. This will refine the mesh in the radial direction at the outlet.
Click Update to generate the new mesh.
Close the ANSYS Mesher and go back to Workbench windows. Under Turbulent Flow Refined Mesh, right click on Fluid Flow (FLUENT) and click Update. Wait for a few minutes for FLUENT to obtain a solution and update all the results.
We would want to compare the solution on the two meshes. To do that, drag the Solution cell of Turbulent Flow Refined Mesh to Results cell of Turbulent Flow.
Double click the Results cell of Turbulent Flow, and after CFD Post opens, we can compare our results by simply selecting the desired chart!
Finer Mesh Analysis
Repeat steps 4, 5, and 6 of this tutorial with the finer mesh.
When you get to step 6 of the tutorial, plot each of the graphs as described. However, for each of the plots, overlay the corresponding result for the coarser mesh so that we may compare them. To do this, after the plotting the finer mesh result, in the Solution XY Plot Window, click on Load File.... Navigate to your working folder, click on the appropriate filename for the previous result, eg. vel.xy for centerline velocity, and click OK. Click Plot. You'll see both results plotted in the same the graphics window.
In the centerline velocity plot above, the white line represents the centerline velocity of the finer mesh, while the red line represents the velocity of the coarser mesh from before. As we can see, there isn't too much of a difference between the two plots. Save this plot as vel2.xy.
Now, let's take a look at the coefficient of skin friction. This time, load the cf.xy file to compare against the plot. This is the coefficient of skin friction plot:
Once again, we can see that due to the fine degree of each mesh, there isn't much difference between the two plots. Save this plot as cf2.xy. Now, study the velocity of the outlet by plotting and comparing to the graph in profile.xy.
Once again, the finer mesh in this case doesn't offer much more precision than the coarser mesh. Save this plot as profile2.xy. Now let's take a look at the YPlus plot.
As we can see, there is a significant increase in the accuracy of the plot from the finer mesh. Save this plot as yplus2.xy.
You may want to experiment with meshes of other granularities and compare their plots with the plots saved from the 100x30 and 100x60 meshes.
In Problem 1, we will be looking at the effect of coarse meshes with uniform granularity.
Go to Problem 1