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

error in fvsolutions file in interDyMFOAM sloshingTank2d

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 28, 2013, 00:05
Default error in fvsolutions file in interDyMFOAM sloshingTank2d
  #1
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Dear all:

I recently started getting this strange error when trying to run sloshingTank2D in interDyMFoam while trying to do a parallel processing run:

[0]
[0]
[0] --> FOAM FATAL IO ERROR:
[0] Unable to set reference cell for field p
Reference point pRefPoint (0 0 0.15) found on 2 domains (should be one)
[0]
[0]
[0] file: /home/cfsengineers/OpenFOAM/cfsengineers-2.2.1/run/tutorials/multiphase/interDyMFoam/ras/sloshingTank2D/processor0/../system/fvSolution.PIMPLE from line 94 to line 103.
[0]
[0] From function void Foam::setRefCell
(
const volScalarField&,
const volScalarField&,
const dictionary&,
label& scalar&,
bool
)
[0] in file cfdTools/general/findRefCell/findRefCell.C at line 105.[1]
[1]
[1] --> FOAM FATAL IO ERROR:
[1] Unable to set reference cell for field p
Reference point pRefPoint (0 0 0.15) found on 2 domains (should be one)

The lines referenced in fvsolution are as follows:

PIMPLE
{
momentumPredictor no;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
nAlphaCorr 1;
nAlphaSubCycles 3;
cAlpha 1.5;
correctPhi no;

pRefPoint (0 0 0.15);
pRefValue 1e5;
}

Any help would be greatly appreciated
musahossein is offline   Reply With Quote

Old   July 28, 2013, 03:06
Default
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Good morning Musaddeque,

I have just tried running the tutorial as is, and I do not get that error. Have you change the decomposition method/number of processors compared to the original tutorial?

I suspect that the reason is the location of the point relative to the computational mesh. It is placed exactly on one of the faces, so if you are unlucky, the decomposition is along this face, and both processorN and processorM find the point.

You could try to displace the point a little bit, or give a reference cell rather than a reference point. The latter should be robust on moving meshes.

Kind regards

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   July 28, 2013, 16:22
Default error in fvsolutions file in interDyMFOAM sloshingTank2d
  #3
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Quote:
Originally Posted by ngj View Post
Good morning Musaddeque,

I have just tried running the tutorial as is, and I do not get that error. Have you change the decomposition method/number of processors compared to the original tutorial?

I suspect that the reason is the location of the point relative to the computational mesh. It is placed exactly on one of the faces, so if you are unlucky, the decomposition is along this face, and both processorN and processorM find the point.

You could try to displace the point a little bit, or give a reference cell rather than a reference point. The latter should be robust on moving meshes.

Kind regards

Niels
Niels:

Thankyou very much for your response. I did not have any problems until I changed the mesh size. In all cases I am using 12 processors. However in my first run, my mesh size was 271X271 and domain decomposition for parallel processing was (1 4 3). I kept the domain decomposition same but changed the mesh to 100X600. That is when I started getting the error messages. I tried something like (1 2 6), but still got the error. The final option is (1 1 12). Is there a rule of thumb that can be applied in such circumstances?

Thanks
Musa
musahossein is offline   Reply With Quote

Old   July 28, 2013, 19:16
Default error in fvsolutions file in interDyMFOAM sloshingTank2d
  #4
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Niels:

Since the mesh size is 100X600 I changed the decomposition to (1 1 12) and interDyMFoam ran w/o complaints. Thanks for your suggestion.
musahossein is offline   Reply With Quote

Reply

Tags
field for p, fvsolutions, interdymfoam, sloshingtank2d

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 in openFOAM-2.0 for parabolic velocity bc ofslcm OpenFOAM 24 August 23, 2015 22:41
Error installing swak4Foam Hisham OpenFOAM Installation 123 July 25, 2015 14:34
"parabolicVelocity" in OpenFoam 2.1.0 ? sawyer86 OpenFOAM Running, Solving & CFD 21 February 7, 2012 12:44
pisoFoam compiling error with OF 1.7.1 on MAC OSX Greg Givogue OpenFOAM Programming & Development 3 March 4, 2011 18:18
error while compiling the USER Sub routine CFD user CFX 3 November 25, 2002 16:16


All times are GMT -4. The time now is 01:19.