Effect of Courant number of grid independence study
 

Lets say I have a mesh of 130,000 cells which works fine with courant number of 200. Next we have a 180,000 cells which shows wave like pattern in Cl and residuals vs iteration plot with courant number 200 however works fine with courant number of 20.

So for grid independence study, is it necessary for us to simulate the mesh with 130,000 cells again with courant number 20 since we got a stable result with this courant number for 180,000 mesh.

Basically I want to know that does Courant number affect the flow result or is it just used to see faster convergence? Also, can we do grid independence study on different meshes with different courant number or courant number should be same for all the meshes to perform grid independence study?



P.S. I am simulating an external air flow over windsor model in Ansys Fluent using k-omega sst model in 2d.

I'm going to make a sarcastic response to illustrate a socratic point.

Let's say you have several meshes. Let's say you ran your original grid with 130k cells yesterday on Wednesday. Today is Thursday and you ran your new grid with 180k cells. Do you need to run your 130k cell grid today on a Thursday? Does day of the week have anything to do with grid convergence?

If you're sure that the day of the week will not affect the solution, then you wouldn't run the 130k grid on a Thursday. But if you're not.... well the answer is yes, you should run the 130k grid on Thursday in order to show day of the week convergence, but that is a separate matter than grid convergence.

The Courant number captures something that is slightly different about the grid than grid convergence.

hahahahahaha...i like the you explained. Thanks a ton. I got the point.

The key is that the CFL number is just one of the non-dimensional parameters in a simulation. It relies on the convective part and it can be shown for a wave equation that you need to work at constant CFL number to check the convergence of the solution.

But you are working with a viscus fluid and using further a turbulence model so that you have to consider that a numerical instability (wiggles appearing first) is due to the computation of the viscous terms. You have to consider the whole time-space discretization, the CFL being only one parameter of the global method.
Note that it has a physical meaning representing the ratio between the physical velocity and the numerical velocity h/dt. But you can read also as a ratio between two characteristic times. That is the reason why to simulate unsteady flow one has to work with CFL lesser than 1.

A lot of information is lacking from your question but, under the plausible assumption that you are using a steady solver (so that CFL really is an implicit URF), then the answer is that it doesn't matter what CFL you used in the different computations, provided that they all converged