CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Cyclic B.C -interDyMFOAM-Gambit Mesh-Parallel (http://www.cfd-online.com/Forums/openfoam/86019-cyclic-b-c-interdymfoam-gambit-mesh-parallel.html)

farhagim March 11, 2011 19:03

Cyclic B.C -interDyMFOAM-Gambit Mesh-Parallel
 
Hello

I have problem With Cyclic B.C . I searched all the forum and followed step by step the procedure but still have problem.
I create a 3D mesh(ex. cube) in Gambit, I linked the MEsh of front and Back face and make it periodic in Gambit) then I named it ex. periodic.1 and export as cube.msh.
Then I imported by fluent3DMeshToFoam to OF 1.7.1. it created two boundary in boundary file. periodic.1 &periodic.1_shadow. I changed the periodic.1_shadow to periodic.2 and use createPatch Dict. to create cyclic B.c. here is my createPatch Dict.

matchTolerance 1e-3;

// Do a synchronisation of coupled points.
pointSync true;


// Patches to create.
// If no patches does a coupled point and face synchronisation anyway.
patches
(
{
// Name of new patch
name periodic.2;

// Type of new patch
type cyclic;

// How to construct: either 'patches' or 'set'
constructFrom patches;

// If constructFrom = patches : names of patches
patches ("periodic.*");

// If constructFrom = set : name of faceSet
//set f0;
}
);

everythings was fine and I copied the new polyMesh file which was created after running createPatch in to my constant directory. I can run it in serial and works fine. But when I want to run it in Parallel I got this error. I have to mention that I use interDyMFoam for my case.
Selecting turbulence model type laminar

....
Reading g
Calculating field g.h


time step continuity errors : sum local = 8.951529e-06, global = -8.951529e-06, cumulative = -8.951529e-06
DICPCG: Solving for pcorr, Initial residual = 1, Final residual = 9.610304e-11, No Iterations 492
time step continuity errors : sum local = 1.227278e-15, global = -3.512952e-18, cumulative = -8.951529e-06
Courant Number mean: 0.0008794369 max: 0.009276953


Starting time loop


Interface Courant Number mean: 3.106989e-06 max: 0.2330362
Courant Number mean: 0.04397184 max: 0.4638476
deltaT = 5e-05
Time = 5e-05


Selected 704 cells for refinement out of 405600.
--> FOAM Warning :
From function syncTools<class T, class CombineOp>::syncEdgeList(const polyMesh&, UList<T>&, const CombineOp&, const T&, const bool)
in file /home/farhangi/OpenFOAM/OpenFOAM-1.7.1/src/OpenFOAM/lnInclude/syncToolsTemplates.C at line 1311
There are decomposed cyclics in this mesh with transformations.
This is not supported. The result will be incorrect

Any help ??

Thanks,

Mehran

cnsidero March 11, 2011 23:05

Mehran,

I'm not 100% this is the solution but based on the error it doesn't look like periodic (cyclic) patches should be decomposed. To prevent this from happening trying adding one/both of these to your decomposeParDict:

globalFaceZones ( periodic.1 periodic.2 );
preservePatches ( periodic.1 periodic.2);

The first option ensures the specified face zones are on all processors. The second option ensures all the cells that use the faces on the specified patches are on the same processor.

I use the ggi patches a lot and the first one is necessary to use the ggi in parallel.

Let me know if this works.

farhagim March 12, 2011 12:22

Hello Chris,

Thanks for your help. Now its working. I have to wait for the results and I will get back to you if everything is ok;)!!!

Thanks,

Mehran


Quote:

Originally Posted by cnsidero (Post 299065)
Mehran,

I'm not 100% this is the solution but based on the error it doesn't look like periodic (cyclic) patches should be decomposed. To prevent this from happening trying adding one/both of these to your decomposeParDict:

globalFaceZones ( periodic.1 periodic.2 );
preservePatches ( periodic.1 periodic.2);

The first option ensures the specified face zones are on all processors. The second option ensures all the cells that use the faces on the specified patches are on the same processor.

I use the ggi patches a lot and the first one is necessary to use the ggi in parallel.

Let me know if this works.


farhagim March 13, 2011 00:29

Chris,

I got the results but the problem is now with reconstructing the Meshes. Since I am using interDyMFoam, First, I have to run reconstructMesh(because the mesh has been changed) and then reconstruct it. Here is the error that I got by running the reconstructMesh:

Merge tolerance : 1e-07
Write tolerance : 1e-07
Doing geometric matching on correct procBoundaries only.
This assumes a correct decomposition.
Found 8 processor directories

Reading database "testparallelcyclic/processor0"
Reading database "testparallelcyclic/processor1"
Reading database "testparallelcyclic/processor2"
Reading database "testparallelcyclic/processor3"
Reading database "testparallelcyclic/processor4"
Reading database "testparallelcyclic/processor5"
Reading database "testparallelcyclic/processor6"
Reading database "testparallelcyclic/processor7"
Setting master time to 0.239

Reading points from "testparallelcyclic/processor0" for time = 0.239

Reading points from "testparallelcyclic/processor1" for time = 0.239

Reading points from "testparallelcyclic/processor2" for time = 0.239

Reading points from "testparallelcyclic/processor3" for time = 0.239

Reading points from "testparallelcyclic/processor4" for time = 0.239

Reading points from "testparallelcyclic/processor5" for time = 0.239

Reading points from "testparallelcyclic/processor6" for time = 0.239

Reading points from "testparallelcyclic/processor7" for time = 0.239

Overall mesh bounding box : (-1.401849e-10 0 0) (0.23858 0.235 0.04)
Relative tolerance : 1e-07
Absolute matching distance : 3.372616e-08

Constructing empty mesh to add to.

Reading mesh to add from "testparallelcyclic/processor0" for time = 0.239

Adding to master mesh


Reading mesh to add from "testparallelcyclic/processor1" for time = 0.239

Adding to master mesh



--> FOAM FATAL ERROR:
face 0 area does not match neighbour 2337 by 186.979% -- possible face ordering problem.
patch:periodic.2 my area:4.58316e-06 neighbour area:1.54214e-07 matching tolerance:0.001
Mesh face:423717 vertices:4((0.02625 0.079155 0.04) (0.02625 0.0864881 0.04) (0.025625 0.0864881 0.04) (0.025625 0.079155 0.04))
Neighbour face:426054 vertices:4((0.0529859 0.0342575 0.04) (0.053981 0.0342322 0.04) (0.0539878 0.0343869 0.04) (0.052991 0.0344122 0.04))
Rerun with cyclic debug flag set for more information.

From function cyclicPolyPatch::calcTransforms()
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 179.

FOAM exiting

Any idea why I got this message??
looking forward to hearing back from you,

Thanks,

MEhran


Quote:

Originally Posted by farhagim (Post 299107)
Hello Chris,

Thanks for your help. Now its working. I have to wait for the results and I will get back to you if everything is ok;)!!!

Thanks,

Mehran



All times are GMT -4. The time now is 04:35.