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

Getting faster convergence in simpleFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 4, 2010, 10:35
Default Getting faster convergence in simpleFoam
  #1
New Member
 
Bastian Nebenfuehr
Join Date: Feb 2010
Location: Sverige
Posts: 27
Rep Power: 7
basneb is on a distinguished road
Hello there,

I am currentliy running simpleFoam on my mesh, which contains half an automotive geometry (station wagon) in order to find out the drag coefficient Cd. The mesh has a total of about 12 million cells and with my settings now, I get convergence after about 2000 iterations. This actually is very time consuming and an entire simulation (up to 5000 iterations) takes about 14 hours. The same case can be run in Fluent, which converges already after about 500 iterations. Is it somehow possible, to speed up the simulation?
So for further information, I'm using simpleFoam and the realizable k-epsilon-model with the default values. In order to intialize the pressure field, I run potentialFoam first. I use the GAMG solver for the pressure and the DILUPBiCG solver for the rest. Usually I run in double precision.
Hope that somebody can help me.
basneb is offline   Reply With Quote

Old   February 5, 2010, 05:39
Default
  #2
New Member
 
Dirk Voglander
Join Date: Mar 2009
Posts: 5
Rep Power: 8
dVoglander is on a distinguished road
Hi,

if you don't have stability problems, you could maybe try to increase the relaxation factors in system/fvSolution.
dVoglander is offline   Reply With Quote

Old   February 5, 2010, 11:26
Default
  #3
New Member
 
Join Date: Apr 2009
Posts: 26
Rep Power: 8
askjak is on a distinguished road
Try smoothSolver instead of DILUPBiCG to improve performance.
askjak is offline   Reply With Quote

Old   February 5, 2010, 18:33
Default
  #4
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Quote:
Originally Posted by basneb View Post
Hello there,
The same case can be run in Fluent, which converges already after about 500 iterations. Is it somehow possible, to speed up the simulation
I guess it is the "coupled" solver in FLUENT? Simple will behave very similar to OpenFOAM. Regards.
bastil is offline   Reply With Quote

Old   February 8, 2010, 04:27
Default
  #5
New Member
 
Bastian Nebenfuehr
Join Date: Feb 2010
Location: Sverige
Posts: 27
Rep Power: 7
basneb is on a distinguished road
Quote:
Originally Posted by dVoglander View Post
Hi,

if you don't have stability problems, you could maybe try to increase the relaxation factors in system/fvSolution.
I tried this already, but unfortunately I get stability problems then, but thx anyway.

Quote:
Originally Posted by askjak View Post
Try smoothSolver instead of DILUPBiCG to improve performance.
I will definitely try this, thx.

Quote:
Originally Posted by bastil View Post
I guess it is the "coupled" solver in FLUENT? Simple will behave very similar to OpenFOAM. Regards.
Unfortunately, I did not do the Fluent simulations, so I don't know, which solver was used, but actually it should have been the same one. Will try to find it out, thx.
basneb is offline   Reply With Quote

Old   February 8, 2010, 12:40
Default
  #6
New Member
 
Join Date: Apr 2009
Posts: 26
Rep Power: 8
askjak is on a distinguished road
I don't know fluent but I know the definition of residuals differ among CFD packages. So don't base convergence on the absolute residual levels.

I have found simpleFoam to convergence in as many steps as StarCD on the same mesh.
askjak is offline   Reply With Quote

Old   February 8, 2010, 15:13
Default
  #7
New Member
 
Bastian Nebenfuehr
Join Date: Feb 2010
Location: Sverige
Posts: 27
Rep Power: 7
basneb is on a distinguished road
After trying some stuff today, I can state that playing with the URFs really helps a lot in getting faster convergence. Now I am almost at Fluent-level. For the rest the use of the "applyBoundaryLayer" function seems to help speeding up the simulation as well. Setting the nonOrthogonalCorrectors to 0 gives a significant change.
basneb is offline   Reply With Quote

Old   February 9, 2010, 03:56
Default
  #8
Member
 
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 8
Thomas Baumann is on a distinguished road
Hi basneb,

Quote:
After trying some stuff today, I can state that playing with the URFs really helps a lot in getting faster convergence. Now I am almost at Fluent-level. For the rest the use of the "applyBoundaryLayer" function seems to help speeding up the simulation as well. Setting the nonOrthogonalCorrectors to 0 gives a significant change.
But don't you need nonOrthogonalCorrectors? I think a mesh of a station wagon is complex and should have deformed mesh cells. Have you compared the results of your flow problem with different numerical models, especially with and without nonOrthogonalCorrectors?

Regards Thomas

Last edited by Thomas Baumann; February 9, 2010 at 04:11.
Thomas Baumann is offline   Reply With Quote

Old   February 9, 2010, 05:20
Default
  #9
New Member
 
Bastian Nebenfuehr
Join Date: Feb 2010
Location: Sverige
Posts: 27
Rep Power: 7
basneb is on a distinguished road
Quote:
Originally Posted by Thomas Baumann View Post
Hi basneb,

But don't you need nonOrthogonalCorrectors? I think a mesh of a station wagon is complex and should have deformed mesh cells. Have you compared the results of your flow problem with different numerical models, especially with and without nonOrthogonalCorrectors?

Regards Thomas
Hi Thomas,

I don't need the nonOrthogonalCorrectors, since the mesh is really really good. The max. nonOrthogonolaty is very low. However, you are right, you cannot run every mesh without the nonOrthogonalCorrectors. In my case, I compared the results (i.e. drag coefficient) for both simulations (with and without nonOrthogonalCorrectors) and they are really similar, so I conclude that there is no problem for me.

Best regards
basneb 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
SimpleFoam convergence problems brahim OpenFOAM Running, Solving & CFD 20 June 9, 2015 09:09
Convergence Problems SimpleFOAM Kutti OpenFOAM 16 June 14, 2010 08:12
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
SimpleFoam solution convergence pattern philippose OpenFOAM Running, Solving & CFD 0 June 26, 2008 14:18
Slow convergence in steadystate incompressible simpleFoam suggestions brooksmoses OpenFOAM Running, Solving & CFD 0 March 3, 2006 05:57


All times are GMT -4. The time now is 19:35.