CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   error in fvsolutions file in interDyMFOAM sloshingTank2d (http://www.cfd-online.com/Forums/openfoam-solving/121405-error-fvsolutions-file-interdymfoam-sloshingtank2d.html)

musahossein July 28, 2013 00:05

error in fvsolutions file in interDyMFOAM sloshingTank2d
 
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

ngj July 28, 2013 03:06

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

musahossein July 28, 2013 16:22

error in fvsolutions file in interDyMFOAM sloshingTank2d
 
Quote:

Originally Posted by ngj (Post 442393)
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 July 28, 2013 19:16

error in fvsolutions file in interDyMFOAM sloshingTank2d
 
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.


All times are GMT -4. The time now is 13:10.