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

Cyclic B.C -interDyMFOAM-Gambit Mesh-Parallel

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 11, 2011, 19:03
Default Cyclic B.C -interDyMFOAM-Gambit Mesh-Parallel
  #1
Member
 
Join Date: Nov 2009
Posts: 48
Rep Power: 8
farhagim is on a distinguished road
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
farhagim is offline   Reply With Quote

Old   March 11, 2011, 23:05
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 386
Rep Power: 13
cnsidero is on a distinguished road
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.
cnsidero is offline   Reply With Quote

Old   March 12, 2011, 12:22
Default
  #3
Member
 
Join Date: Nov 2009
Posts: 48
Rep Power: 8
farhagim is on a distinguished road
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 View Post
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 is offline   Reply With Quote

Old   March 13, 2011, 00:29
Default
  #4
Member
 
Join Date: Nov 2009
Posts: 48
Rep Power: 8
farhagim is on a distinguished road
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.
patcheriodic.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 View Post
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
farhagim 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
Moving mesh still crashes in parallel in 1.6-ext paul b OpenFOAM Running, Solving & CFD 36 February 17, 2014 09:35
problem when I import mesh with cyclic graduated BC Cyp OpenFOAM 0 March 3, 2011 11:38
Cyclic patches and parallel postprocessing problems askjak OpenFOAM Bugs 18 October 27, 2010 03:35
InterDyMFoam dynamic messing in parallel fails under nonquiescent conditions adona058 OpenFOAM Running, Solving & CFD 5 August 19, 2010 11:47
Adaptive Mesh Refinement and Cyclic Boundary Conditions adona058 OpenFOAM Running, Solving & CFD 6 October 23, 2009 09:17


All times are GMT -4. The time now is 20:50.