CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Forward facing step simulaiton

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 9, 2010, 06:02
Default Forward facing step simulaiton
  #1
New Member
 
Join Date: Jun 2009
Posts: 16
Rep Power: 8
ghoshi1983 is on a distinguished road
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
ghoshi1983 is offline   Reply With Quote

Old   June 9, 2010, 06:23
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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?
ghorrocks is offline   Reply With Quote

Old   June 9, 2010, 07:46
Default
  #3
New Member
 
Join Date: Jun 2009
Posts: 16
Rep Power: 8
ghoshi1983 is on a distinguished road
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.
ghoshi1983 is offline   Reply With Quote

Old   June 9, 2010, 07:52
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   June 9, 2010, 08:43
Default
  #5
New Member
 
Join Date: Jun 2009
Posts: 16
Rep Power: 8
ghoshi1983 is on a distinguished road
Actually i running steady simulations. I have tried what you suggested but still its giving error (now after 1st iteration).
ghoshi1983 is offline   Reply With Quote

Old   June 9, 2010, 18:35
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   June 10, 2010, 08:02
Default
  #7
New Member
 
Join Date: Jun 2009
Posts: 16
Rep Power: 8
ghoshi1983 is on a distinguished road
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.
ghoshi1983 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM 300 October 29, 2014 19:00
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 19:07
Supersonic flow over a forward facing step Chan K I Main CFD Forum 1 October 19, 2000 16:43


All times are GMT -4. The time now is 02:22.