Sign-up for free online course on ANSYS simulations!UNDER CONSTRUCTION
Author: Daniel Kantor and Andrew Einstein, Cornell University
Problem Specification
1. Create Geometry in GAMBIT
2. Mesh Geometry in GAMBIT
3. Specify Boundary Types in GAMBIT
4. Set Up Problem in FLUENT
5. Solve!
6. Analyze Results
7. Refine Mesh
Problem 1
Step 7: Refine Mesh
It our mesh refine enough? Will the current mesh give us an accurate representation of the physical flow? Mesh density determine the truncation error of our simulation. With too little mesh density, the result we obtain will be inaccurate. With too many mesh elements, we will be wasting unnecessary computational power (long computational time!). We will see what an optimal mesh will look like.
We'll re-do the calculation on a 570,000 element mesh. IMPORTANT NOTE: Running a mesh this size with our element type will take at least week to run on a single PC. You can try running smaller size meshes on your own but the results will not be as good as these. You can download the mesh HERE. If you want to create it, follow Step 1 through Step 5. At step 2, you can simply change the cell size from 0.8 to 0.4 .
After that, you should have three meshes with following mesh elements.
|
Coarse |
Medium |
Fine |
No. of cells |
6240 |
14040 |
31590 |
Drag Coefficient Comparison
For each mesh, take note of the drag coefficient and compare with each other.
|
Coarse |
Medium |
Fine |
Cd |
2.4981 |
2.4941 |
2.4927 |
% dif |
0.160378 |
0 |
0.056132 |
Taking medium as benchmark, we compare coarse and fine mesh. Note that the difference in drag coefficient between three meshes is negligibly small. For analysis of drag coefficient, it seems that coarse mesh provides enough resolution.
Pressure Coefficient Comparison
Let's analyze pressure coefficient plot around cylinder for three different mesh before we conclude which mesh to use. Let's start with a coarse mesh.
Plot > XY Plot...
Change the Y Axis Function to Pressure..., followed by Pressure Coefficient. Then, select cylinder under Surfaces. Check the option Write to File.
Click Write...
Enter the file name and directory to save.
Do the same for medium and fine meshes by opening different case and data files.
After that, open the files that you have written with excel spreadsheet. Compile and plot the data accordingly.
A quick and dirty way plotting three different mesh is to use FLUENT directly. Plot > XY Plot... You can Load File... that you have saved previously. However, using this way, you have less control of how you can present the data and is not recommended for report presentation.