Forward facing step simulaiton

ghoshi1983 · June 9, 2010, 06:02

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.

June 9, 2010, 06:02	Forward facing step simulaiton	#1
ghoshi1983 New Member Join Date: Jun 2009 Posts: 21 Rep Power: 16	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

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[swak4Foam] GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh	gschaider	OpenFOAM Community Contributions	300	October 29, 2014 18:00
How to write k and epsilon before the abnormal end	xiuying	OpenFOAM Running, Solving & CFD	8	August 27, 2013 15:33
IcoFoam parallel woes	msrinath80	OpenFOAM Running, Solving & CFD	9	July 22, 2007 02:58
Could anybody help me see this error and give help	liugx212	OpenFOAM Running, Solving & CFD	3	January 4, 2006 18:07
Supersonic flow over a forward facing step	Chan K I	Main CFD Forum	1	October 19, 2000 16:43

June 9, 2010, 06:23		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	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?

June 9, 2010, 07:46		#3
ghoshi1983 New Member Join Date: Jun 2009 Posts: 21 Rep Power: 16	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.

June 9, 2010, 07:52		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	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.

June 9, 2010, 08:43		#5
ghoshi1983 New Member Join Date: Jun 2009 Posts: 21 Rep Power: 16	Actually i running steady simulations. I have tried what you suggested but still its giving error (now after 1st iteration).

June 9, 2010, 18:35		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	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.

June 10, 2010, 08:02		#7
ghoshi1983 New Member Join Date: Jun 2009 Posts: 21 Rep Power: 16	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.