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/)
-   -   Any example of manualCoeffs for decomposeParDict? (http://www.cfd-online.com/Forums/openfoam-solving/63241-any-example-manualcoeffs-decomposepardict.html)

yuhai April 1, 2009 17:22

Any example of manualCoeffs for decomposeParDict?
 
Hi, everybody,
Good Day.
I am now a little comfuse on decomposePar for turbDyMFoam, it always cut through the GGI interface.
So I want to decompose manually,
firstly, I tried to set the "procBoundaryXXtoYY" interfaces in Gambit, and convert them to Foam, problems are countered:
1, if fluentMeshToFoam converting 2D mesh, defaultFaces (frontandBackPlane in Gambit) are not set into groups.
2, if fluent3DMeshToFoam converting 2D mesh with z depth, "faceZones" and "pointZones" don't provide enough information for "cellProcAddressing" and "pointProcAddressing".

Then, I go to the "manualCoeffs" in decomposeParDict, but I can't find the example or explain of the grammar of the DataFile.

Can anybody give me any hints?

Thanks in advance.

Hai Yu

alexm April 19, 2009 18:48

decomposeParDict & manualCoeffs
 
Hi,
sorry, I have no answer, but the same question. I also would like to know more about the manualCoeffs data file in decomposeparDict. Its just about an old problem of getting a sharp interface of two phases with the snappyHexMesh tool.
I hope, someone can help us.
Greetings, Axel

Schag July 22, 2009 12:16

Hi all,

I'm actually looking for the same thing.
Does anyone found an example or explanation/tutorial to do it?

Or eventually someone knows how to define precise cutting planes to separate regions in order to run in parallel without using manual option?

Thx,

Julien

novyno May 11, 2010 03:51

Hi All,

here you can find an example of a ManualDecompositionFile of a simple cube splitted in 8 elements. This file contains the same number of the mesh elements and the entries refer to the processor number. So in the example in attached the first and second elements are assigned to the processor0, etc...

novyno May 11, 2010 03:53

Sorry... I can't attach the file... I put it here!

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class labelList;
location "constant";
object cellDecomposition;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


8
(
0
0
1
1
1
1
0
0
)


// ************************************************** *********************** //

AdrianoCT June 30, 2015 13:11

Hy guys,

is it possible do a CellDecomposition from cellSet? I have to manage 15 mln of cells, so isn't convenient split the domain manually.

Any suggestions? Thanks

louisgag July 21, 2015 10:51

Quote:

Originally Posted by AdrianoCT (Post 552731)
Hy guys,

is it possible do a CellDecomposition from cellSet? I have to manage 15 mln of cells, so isn't convenient split the domain manually.

Any suggestions? Thanks

Yes, it is not obvious but here's how I managed to do it:
run topoSet to create a faceSet from a cellSet using the faceSet cellToFace option.

Here's an example of the topoSetDict (where you should have created a cellSet):
Code:

  {
      name    myFaceSet;
      type    faceSet;
      action    new;
      source    cellToFace;
      sourceInfo
      {
      set myCellZone;
      option all;
      }
  }

you can then run a decomposePar with the singleProcessorFaceSets command. You may want to also include both your cyclic patches in the singleProcessorFaceSets command if you are doing this for an AMI simulation...

-Louis


All times are GMT -4. The time now is 08:54.