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

Problems with interFoam usage

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 4, 2008, 08:51
Default Hi all, I am trying to calcul
  #1
New Member
 
Damjan
Join Date: Mar 2009
Location: Velenje, Slovenia
Posts: 3
Rep Power: 7
vrecha is on a distinguished road
Hi all,
I am trying to calculate a free surface flow around fixed body using interFoam solver. But I didn't came far ...
What can be seen from the log is that time step keeps decreasing trying to keep the Courant number under specified value. When time step reaches values around 10^(-10) the solver crashes (segmentation fault ...).

What I have already done:
- checked mesh : It reports 131 severely non-orthogonal faces out of 3000000. All other tests are OK, and the checker concludes that mesh is OK.

- played with MaxCo and allowed it even to reach maximum of 0.5 . Made no significiant difference, a solver took a little more time to crash.

- played a little with PISO settings: increased nCorrectors, nNonOrthogonalCorrectors, nGammaCorr, nGammaSubCycles. -> no difference.

Any idea of what to try/do will be appreciated.

Regards,
Damjan.
vrecha is offline   Reply With Quote

Old   January 4, 2008, 09:06
Default Well, it is likely that someth
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,747
Rep Power: 20
hjasak will become famous soon enough
Well, it is likely that something is badly and obviously wrong with the case set-up. Dump the results in every time-step and see where the velocity increases without bounds: what you are seeing is the automatic time-step control trying to "save you" from increasing velocity.

Incidentally, if you're interested, I will be delivering a lecture on my work and OpenFOAM in general at the University of Ljubljana next Thursday (10/Jan/2008) - not too far from you.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 4, 2008, 09:12
Default I would suspect your interFoam
  #3
caw
Member
 
Christian Winkler
Join Date: Mar 2009
Location: Mannheim, Germany
Posts: 63
Rep Power: 7
caw is on a distinguished road
I would suspect your interFoam-chrash is caused by a bad mesh. I have observed the same thing on a mesh with big changes in cell size. After remeshing everthing went fine.

Regards
Christian
caw is offline   Reply With Quote

Old   January 4, 2008, 17:44
Default Thank you, both suggestions
  #4
New Member
 
Damjan
Join Date: Mar 2009
Location: Velenje, Slovenia
Posts: 3
Rep Power: 7
vrecha is on a distinguished road
Thank you,

both suggestions were extremely useful. Some pictures of what is going on:

http://lmmri.fri.uni-lj.si/damjan/beforeCrash.png
http://lmmri.fri.uni-lj.si/damjan/beforeCrash_1.png
http://lmmri.fri.uni-lj.si/damjan/beforeCrash_2.png

The problems with velocity arise exactly at mesh seam. So remeshing is inevitable ...

Any othr suggestions/remarks/comments etc are welcome. As you can see I am at a very early stage of learning the art of CFD.


---
PS (to Hrvoje): I will try my best to attend your talk in Ljubljana, tnx for invitation.
vrecha is offline   Reply With Quote

Old   January 5, 2008, 04:34
Default Yes, i see.... First of all
  #5
caw
Member
 
Christian Winkler
Join Date: Mar 2009
Location: Mannheim, Germany
Posts: 63
Rep Power: 7
caw is on a distinguished road
Yes, i see....

First of all, from my experience free surface codes usually do not like tetrahedral meshes. Also size jumps from cell to cell are to be avoided. So for you there are same ways to follow:

1) if you have to stick to tetrahedrons, use reasonable size functions with growth rates of about 1.2
2) Try to use a polyhedra mesh, this can be made out of a tet mesh using polydualmesh in FOAM
3) Best mesh for interFoam (goes for CFD in general) is still a hex mesh, you might want to give this a try. Your geometry is not that complex, so at least a hex dominant mesh shold be possible without to much effort. I heard some rumors about a hexdominant auto-mesher being available in the next release of OF, but there are others available right now as well (harpoon for example, but: commercial)

Suggestion: Use a good tet mesh and convert it to polyhedrons then you should be fine....

Regards
Christian
caw 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
Problems calculating field gh with interFoam cricke OpenFOAM Running, Solving & CFD 0 December 10, 2007 08:17
Problems with foamLog and interFoam OF 14 sinusmontis OpenFOAM Bugs 2 June 1, 2007 09:57
Problems involving interFoam and GCC 410 gschaider OpenFOAM Installation 1 July 30, 2006 20:58
Problems starting new case interFoam billy OpenFOAM Running, Solving & CFD 3 June 21, 2006 11:18
CFX-5.7.1 RAM usage Sandeep CFX 1 January 30, 2005 18:14


All times are GMT -4. The time now is 20:24.