CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Forward facing step simulaiton (http://www.cfd-online.com/Forums/cfx/76950-forward-facing-step-simulaiton.html)

ghoshi1983 June 9, 2010 06:02

Forward facing step simulaiton
 
Hi everybody,

I am trying to do mesh study for FFS. Following are the BC'S:

Inlet velocity profile (1/7th power law)
Outlet Avg static Press 0 Pa
Translational periodicity instead of symmetry for sides

I have started from coarse mesh (500k) and then a bit finer (800k) both had no problems. but when i have made the mesh more finer (1 Million) then i got the floating point exception overflow error (After 2 iterations). But with same mesh (1 Million) with symmetry bc's it seems to have no such problems.

I have tried the following to solve the problem but no success:

1- Increased timescale factor to 2
2- Checked double precision
3- Run Check on mesh (no problems found) in ICEM
4- Tried mesh smoothing globally

Any suggestions/feedback will be highly appreciated. Thanks in advance

Regards,
Atif

ghorrocks June 9, 2010 06:23

You should be able to make a very high quality hex grid for this simulation. Not only will that improve accuracy, speed the simulation and use less memory, but it will also make obtaining convergence much easier. Are you using a hex grid?

ghoshi1983 June 9, 2010 07:46

Hi Glenn,

Thanks for the reply. Yes i am using hex grid. You are right basically i am getting convergence in much easier passion. But somehow its not the case when i make it finer.

ghorrocks June 9, 2010 07:52

OK, thanks. Here's some suggestions:
- don't smooth the grid in ICEM. for a forward facing step you should get a perfectly orthogonal grid with no smoothing.
- If it blows up in the first time step or two try reducing the time step size. Once convergence is proceeding nicely then increase the time step size.
- Convergence is harder to achieve with finer grids. But the difference between your grids is not too much, I suspect something else is wrong.

ghoshi1983 June 9, 2010 08:43

Actually i running steady simulations. I have tried what you suggested but still its giving error (now after 1st iteration).

ghorrocks June 9, 2010 18:35

Try a smaller physical time step to start things off. Or you may need Local Timescale factor to start it going.

Also try using the previous simulations as initial guesses. That will help a lot.

ghoshi1983 June 10, 2010 08:02

I have tried with physical timescale (1e-1 since my fluid timescale is 1e-2) instead of automatic timescale .and it worked and it seems converged (40 iterations) too. But still i had to check whether this physical timescale value has an effect on my results. for that i have tried to reduce (1e-2) and increase (1e-0)it of the order of one. and then i compared the results and it seems ok.
Thank you very much Glenn for your help and suggestions.


All times are GMT -4. The time now is 10:34.