CFD Online Discussion Forums - [snappyHexMesh] Parallel sHM error

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)

- - [snappyHexMesh] Parallel sHM error (https://www.cfd-online.com/Forums/openfoam-meshing/97115-parallel-shm-error.html)

Parallel sHM error

Hi folks,

i'm trying to run snappyHexMesh (OF 2.1.x) in parallel mode using following commands:

Code:

blockmesh

decomposePar (using scotch in decomposeParDict)

mpirun -np 6 snappyHexMesh -parallel -overwrite (using ptscotch in decomposeParDict)

reconstructParMesh -constant -mergeTol 1E-6

Unfortunately, I get following error message, probably caused by snappyHexMesh:

Quote:

stss3@itlrstud041:~/OpenFOAM/stss3-2.1.x/run/mappedCase2D/mappedCase102> ./parallelSHM
[2]
[2]
[2] --> FOAM FATAL ERROR:
[2] face 7 area does not match neighbour by 0.276304% -- possible face ordering problem.
patch:procBoundary2to1 my area:9.14844e-07 neighbour area:9.17375e-07 matching tolerance:9.08608e-11
Mesh face:25882 vertices:4((0.372 0.0709347 0) (0.372 0.0691 0) (0.372 0.0691 0.0005) (0.372 0.0709246 0.0005))
If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.
Rerun with processor debug flag set for more information.
[2]
[2] From function processorPolyPatch::calcGeometry()
[2] in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 239.
[2]
FOAM parallel run exiting
[2]
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 2 in communicator MPI_COMM_WORLD
with errorcode 1.

NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
You may or may not see output from other processes, depending on
exactly when Open MPI kills them.
--------------------------------------------------------------------------
[1]
[1]
[1] --> FOAM FATAL ERROR:
[1] face 7 area does not match neighbour by 0.276304% -- possible face ordering problem.
patch:procBoundary1to2 my area:9.17375e-07 neighbour area:9.14844e-07 matching tolerance:9.04077e-11
Mesh face:25839 vertices:4((0.372 0.0709347 0) (0.372 0.0709347 0.0005) (0.372 0.0691 0.0005) (0.372 0.0691 0))
If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.
Rerun with processor debug flag set for more information.
[1]
[1] From function processorPolyPatch::calcGeometry()
[1] in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 239.
[1]
FOAM parallel run exiting
[1]
--------------------------------------------------------------------------
mpirun has exited due to process rank 2 with PID 5675 on
node itlrstud041 exiting improperly. There are two reasons this could occur:

1. this process did not call "init" before exiting, but others in
the job did. This can cause a job to hang indefinitely while it waits
for all processes to call "init". By rule, if one process calls "init",
then ALL processes must call "init" prior to termination.

2. this process called "init", but exited without calling "finalize".
By rule, all processes that call "init" MUST call "finalize" prior to
exiting or it will be considered an "abnormal termination"

This may have caused other processes in the application to be
terminated by signals sent by mpirun (as reported here).
--------------------------------------------------------------------------
[itlrstud041:05672] 1 more process has sent help message help-mpi-api.txt / mpi-abort
[itlrstud041:05672] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages

At the end of my sHM-Logfile there is following statement:

Quote:

Scaling iteration 0
Moving mesh using diplacement scaling : min:1 max:1
Correcting 2-D mesh motion--> FOAM Warning :
From function motionSmoother::movePoints(pointField& newPoints)
in file motionSmoother/motionSmoother.C at line 809
2D mesh-motion probably not correct in parallel
--> FOAM Warning :
From function twoDPointCorrector::twoDPointCorrector(const polyMesh& mesh, const vector& n)
in file twoDPointCorrector/twoDPointCorrector.C at line 164
The number of points in the mesh is not equal to twice the number of edges normal to the plane - this may be OK only for wedge geometries.
Please check the geometry or adjust the orthogonality tolerance.

Number of normal edges: 8676 number of points: 10872
...done
[1] processorPolyPatch::calcGeometry : Writing my 172 faces to OBJ file "/home/stss3/OpenFOAM/stss3-2.1.x/run/mappedCase2D/mappedCase102/processor1/procBoundary1to2_faces.obj"
[2] processorPolyPatch::calcGeometry : Writing my 172 faces to OBJ file "/home/stss3/OpenFOAM/stss3-2.1.x/run/mappedCase2D/mappedCase102/processor2/procBoundary2to1_faces.obj"
[2] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/home/stss3/OpenFOAM/stss3-2.1.x/run/mappedCase2D/mappedCase102/processor2/procBoundary2to1_faceCentresConnections.obj"
[1] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/home/stss3/OpenFOAM/stss3-2.1.x/run/mappedCase2D/mappedCase102/processor1/procBoundary1to2_faceCentresConnections.obj"

Do you have an idea how to fix this?
Thanks in advance!

I'm having the same issue… did you manage to solve sort it out eventually?

Sorry, I haven't got any solution.
I gave up after trying an entire weekend :confused:

Have you solve your problem ? What command line did you executed before reconstructPartMesh ?

Maybe I have a solution to solve your problem

Ive a similar problem when running my solver. I had a closer look in the C++documentation and somehow figured out the reason.

The problem is caused by the decomposition of the domain. There a default_matchTolerance for the faces which is automatically applied (the value is 1e-4).
You can see this setting in your processor*/constant/polyMesh/boundary file at the processor-patches.

"
[2] face 7 area does not match neighbour by 0.276304% -- possible face ordering problem.
patch:procBoundary2to1 my area:9.14844e-07 neighbour area:9.17375e-07 matching tolerance:9.08608e-11
"
The matching tolerance 9.08608e-11 is calculated as followed: matchTol*length^2
The length is the maximal distance from the face center to a vertice ( in this case: ~ 9.532e-4 Squared this corresponds to a kind of equivalent face area. This value is compared with the difference between "my area" and "neighbour area".

I could not figure out how to change this matchTolerance so I just changed the entry in the boundary-files after the decomposition with this command:
"
sed 's/0.0001/0.05/g' processor*/constant/polyMesh/boundary -i
"
-> the matchTolerance is 0.05 now

I think it is very difficult to match this very small default tolerance for a refined mesh. I also use SHM and therefore have the same problem. I dont know yet if the calculation is stable.

Do you know any better solution (e.g. where to set the matchTolerance - entry, e.g. in the decomposeParDict)??

Could you copy your files here ? (decomposePar, snappyHexMesh, controlDict)

I decomposed with "method hierarchical"
This error just occured when running my solver; I had no problems with snappyhexmesh.

Did you try my solution?
Do you use cyclic boundary conditions?

Quote:

Originally Posted by MacGyver (Post 358436)

I decomposed with "method hierarchical"
This error just occured when running my solver; I had no problems with snappyhexmesh.

I didn't said that you have problem with sHM.

Quote:

Originally Posted by MacGyver (Post 358436)

Did you try my solution?
Do you use cyclic boundary conditions?

No, but it's difficult to help you, if we don't see what parameters you used

exit with error when parallelized

I just run sHM in serial and it finished correctly, without snapped and layered mesh.
it seems that the problem in sHM

Hi guys,
I know, that this thread is pretty old, but I'm having the same issues.
I am using OpenFOAM 6 and snappyHexMesh.

Here is how I get the same matching Error:
1. blockMesh
2. decomposePar
3. runParallel snappyHexMesh -overwrite

SnappyHexMesh is running until it is snapping and displacing the mesh to fit to my surfaceFeatureExtract-Object (or in some cases until layerAddition).

Here is the last bit of my log.snappyHexMesh file:

Code:



Morph iteration 3

-----------------

Calculating patchDisplacement as distance to nearest surface point ...

Wanted displacement : average:0.000594714 min:5.62277e-07 max:0.00214618

Calculated surface displacement in = 0.11 s





Detecting near surfaces ...

Overriding nearest with intersection of close gaps at 0 out of 27372 points.

Overriding displacement on features :

   implicit features    : false

   explicit features    : true

   multi-patch features : false

Morph iteration 3

-----------------

Calculating patchDisplacement as distance to nearest surface point ...

Wanted displacement : average:0.000594714 min:5.62277e-07 max:0.00214618

Calculated surface displacement in = 0.11 s





Detecting near surfaces ...

Overriding nearest with intersection of close gaps at 0 out of 27372 points.

Overriding displacement on features :

   implicit features    : false

   explicit features    : true

   multi-patch features : false



Detected 0 baffle edges out of 54250 edges.

--> FOAM Warning : 

    From function Foam::treeBoundBox::treeBoundBox(const Foam::UList<Foam::Vector<double> >&)

    in file meshes/treeBoundBox/treeBoundBox.C at line 136

    cannot find bounding box for zero-sized pointField, returning zero

Initially selected 0 points out of 27372 for reverse attraction.

Selected 0 points out of 27372 for reverse attraction.

Stringing feature edges : changed 0 points

Attraction:

     linear   : max:(0.00183956 -0.00110546 -7.51662e-06) avg:(4.50171e-05 -2.00879e-05 -2.80543e-09)

     feature  : max:(0 0 0) avg:(0 0 0)

Feature analysis : total master points:27048 attraction to :

    feature point   : 0

    feature edge    : 0

    nearest surface : 0

    rest            : 27048



Smoothing displacement ...

Iteration 0

Iteration 10

Iteration 20

Displacement smoothed in = 6.6 s





Moving mesh ...



Iteration 0

Moving mesh using displacement scaling : min:1  max:1

Correcting 2-D mesh motion--> FOAM Warning : 

    From function void Foam::motionSmootherAlgo::modifyMotionPoints(Foam::pointField&) const

    in file motionSmoother/motionSmootherAlgo.C at line 657

    2D mesh-motion probably not correct in parallel

 ...done

[1] processorPolyPatch::calcGeometry : Writing my 14323 faces to OBJ file "/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor1/procBoundary1to2_faces.obj"

[2] processorPolyPatch::calcGeometry : Writing my 14323 faces to OBJ file "/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor2/procBoundary2to1_faces.obj"

[2] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor2/procBoundary2to1_faceCentresConnections.obj"

[1] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor1/procBoundary1to2_faceCentresConnections.obj"

[2] 

[2] 

[2] --> FOAM FATAL ERROR: 

[2] face 5738 area does not match neighbour by 0.0267405% -- possible face ordering problem.

patch:procBoundary2to1 my area:3.99941e-06 neighbour area:3.99835e-06 matching tolerance:1.03479e-09

Mesh face:1177078 vertices:4((-0.0929725 0.00598575 0.04625) (-0.0993708 0.00603835 0.04625) (-0.0993676 0.00603726 0.045625) (-0.0929683 0.00598432 0.045625))

If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.

Rerun with processor debug flag set for more information.

[2] 

[2]     From function virtual void Foam::processorPolyPatch::calcGeometry(Foam::PstreamBuffers&)

[2]     in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 284.

[2] 

FOAM parallel run exiting

[2] 

--------------------------------------------------------------------------

MPI_ABORT was invoked on rank 2 in communicator MPI COMMUNICATOR 3 SPLIT FROM 0

with errorcode 1.



NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.

You may or may not see output from other processes, depending on

exactly when Open MPI kills them.

--------------------------------------------------------------------------

[1] 

[1] 

[1] --> FOAM FATAL ERROR: 

[1] face 5738 area does not match neighbour by 0.0267405% -- possible face ordering problem.

patch:procBoundary1to2 my area:3.99835e-06 neighbour area:3.99941e-06 matching tolerance:1.03424e-09

Mesh face:1187038 vertices:4((-0.0929725 0.00598575 0.04625) (-0.0929683 0.00598432 0.045625) (-0.0993664 0.00603686 0.045625) (-0.0993686 0.00603759 0.04625))

If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.

Rerun with processor debug flag set for more information.

[1] 

[1]     From function virtual void Foam::processorPolyPatch::calcGeometry(Foam::PstreamBuffers&)

[1]     in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 284.

[1] 

FOAM parallel run exiting

[1] 



Detected 0 baffle edges out of 54250 edges.

--> FOAM Warning : 

    From function Foam::treeBoundBox::treeBoundBox(const Foam::UList<Foam::Vector<double> >&)

    in file meshes/treeBoundBox/treeBoundBox.C at line 136

    cannot find bounding box for zero-sized pointField, returning zero

Initially selected 0 points out of 27372 for reverse attraction.

Selected 0 points out of 27372 for reverse attraction.

Stringing feature edges : changed 0 points

Attraction:

     linear   : max:(0.00183956 -0.00110546 -7.51662e-06) avg:(4.50171e-05 -2.00879e-05 -2.80543e-09)

     feature  : max:(0 0 0) avg:(0 0 0)

Feature analysis : total master points:27048 attraction to :

    feature point   : 0

    feature edge    : 0

    nearest surface : 0

    rest            : 27048



Smoothing displacement ...

Iteration 0

Iteration 10

Iteration 20

Displacement smoothed in = 6.6 s





Moving mesh ...



Iteration 0

Moving mesh using displacement scaling : min:1  max:1

Correcting 2-D mesh motion--> FOAM Warning : 

    From function void Foam::motionSmootherAlgo::modifyMotionPoints(Foam::pointField&) const

    in file motionSmoother/motionSmootherAlgo.C at line 657

    2D mesh-motion probably not correct in parallel

 ...done

[1] processorPolyPatch::calcGeometry : Writing my 14323 faces to OBJ file "/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor1/procBoundary1to2_faces.obj"

[2] processorPolyPatch::calcGeometry : Writing my 14323 faces to OBJ file "/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor2/procBoundary2to1_faces.obj"

[2] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor2/procBoundary2to1_faceCentresConnections.obj"

[1] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor1/procBoundary1to2_faceCentresConnections.obj"

[2] 

[2] 

[2] --> FOAM FATAL ERROR: 

[2] face 5738 area does not match neighbour by 0.0267405% -- possible face ordering problem.

patch:procBoundary2to1 my area:3.99941e-06 neighbour area:3.99835e-06 matching tolerance:1.03479e-09

Mesh face:1177078 vertices:4((-0.0929725 0.00598575 0.04625) (-0.0993708 0.00603835 0.04625) (-0.0993676 0.00603726 0.045625) (-0.0929683 0.00598432 0.045625))

If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.

Rerun with processor debug flag set for more information.

[2] 

[2]     From function virtual void Foam::processorPolyPatch::calcGeometry(Foam::PstreamBuffers&)

[2]     in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 284.

[2] 

FOAM parallel run exiting

[2] 

--------------------------------------------------------------------------

MPI_ABORT was invoked on rank 2 in communicator MPI COMMUNICATOR 3 SPLIT FROM 0

with errorcode 1.



NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.

You may or may not see output from other processes, depending on

exactly when Open MPI kills them.

--------------------------------------------------------------------------

[1] 

[1] 

[1] --> FOAM FATAL ERROR: 

[1] face 5738 area does not match neighbour by 0.0267405% -- possible face ordering problem.

patch:procBoundary1to2 my area:3.99835e-06 neighbour area:3.99941e-06 matching tolerance:1.03424e-09

Mesh face:1187038 vertices:4((-0.0929725 0.00598575 0.04625) (-0.0929683 0.00598432 0.045625) (-0.0993664 0.00603686 0.045625) (-0.0993686 0.00603759 0.04625))

If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.

Rerun with processor debug flag set for more information.

[1] 

[1]     From function virtual void Foam::processorPolyPatch::calcGeometry(Foam::PstreamBuffers&)

[1]     in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 284.

[1] 

FOAM parallel run exiting

[1]

I have tried to use different type of decomposition (simple, scotch), but still the same problem. I have also tried to reduce the mergeTolerance to 1e-04 instead of using the recommendet value of 1e-06.

Would someone be so kind and enlighten me, please? Since I want to make a parameter study, I need to run the meshing in parallel, otherwise it would take too long for me...

I have compressed my blockMeshDict, decomposeParDict and my snappyHexMeshDict to system.zip:

Quote:

Originally Posted by Agit (Post 716630)

Code:



Morph iteration 3

-----------------

Calculating patchDisplacement as distance to nearest surface point ...

Wanted displacement : average:0.000594714 min:5.62277e-07 max:0.00214618

Calculated surface displacement in = 0.11 s





Detecting near surfaces ...

Overriding nearest with intersection of close gaps at 0 out of 27372 points.

Overriding displacement on features :

   implicit features    : false

   explicit features    : true

   multi-patch features : false

Morph iteration 3

-----------------

Calculating patchDisplacement as distance to nearest surface point ...

Wanted displacement : average:0.000594714 min:5.62277e-07 max:0.00214618

Calculated surface displacement in = 0.11 s





Detecting near surfaces ...

Overriding nearest with intersection of close gaps at 0 out of 27372 points.

Overriding displacement on features :

   implicit features    : false

   explicit features    : true

   multi-patch features : false



Detected 0 baffle edges out of 54250 edges.

--> FOAM Warning : 

    From function Foam::treeBoundBox::treeBoundBox(const Foam::UList<Foam::Vector<double> >&)

    in file meshes/treeBoundBox/treeBoundBox.C at line 136

    cannot find bounding box for zero-sized pointField, returning zero

Initially selected 0 points out of 27372 for reverse attraction.

Selected 0 points out of 27372 for reverse attraction.

Stringing feature edges : changed 0 points

Attraction:

     linear   : max:(0.00183956 -0.00110546 -7.51662e-06) avg:(4.50171e-05 -2.00879e-05 -2.80543e-09)

     feature  : max:(0 0 0) avg:(0 0 0)

Feature analysis : total master points:27048 attraction to :

    feature point   : 0

    feature edge    : 0

    nearest surface : 0

    rest            : 27048



Smoothing displacement ...

Iteration 0

Iteration 10

Iteration 20

Displacement smoothed in = 6.6 s





Moving mesh ...



Iteration 0

Moving mesh using displacement scaling : min:1  max:1

Correcting 2-D mesh motion--> FOAM Warning : 

    From function void Foam::motionSmootherAlgo::modifyMotionPoints(Foam::pointField&) const

    in file motionSmoother/motionSmootherAlgo.C at line 657

    2D mesh-motion probably not correct in parallel

 ...done

[1] processorPolyPatch::calcGeometry : Writing my 14323 faces to OBJ file "/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor1/procBoundary1to2_faces.obj"

[2] processorPolyPatch::calcGeometry : Writing my 14323 faces to OBJ file "/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor2/procBoundary2to1_faces.obj"

[2] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor2/procBoundary2to1_faceCentresConnections.obj"

[1] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor1/procBoundary1to2_faceCentresConnections.obj"

[2] 

[2] 

[2] --> FOAM FATAL ERROR: 

[2] face 5738 area does not match neighbour by 0.0267405% -- possible face ordering problem.

patch:procBoundary2to1 my area:3.99941e-06 neighbour area:3.99835e-06 matching tolerance:1.03479e-09

Mesh face:1177078 vertices:4((-0.0929725 0.00598575 0.04625) (-0.0993708 0.00603835 0.04625) (-0.0993676 0.00603726 0.045625) (-0.0929683 0.00598432 0.045625))

If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.

Rerun with processor debug flag set for more information.

[2] 

[2]     From function virtual void Foam::processorPolyPatch::calcGeometry(Foam::PstreamBuffers&)

[2]     in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 284.

[2] 

FOAM parallel run exiting

[2] 

--------------------------------------------------------------------------

MPI_ABORT was invoked on rank 2 in communicator MPI COMMUNICATOR 3 SPLIT FROM 0

with errorcode 1.



NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.

You may or may not see output from other processes, depending on

exactly when Open MPI kills them.

--------------------------------------------------------------------------

[1] 

[1] 

[1] --> FOAM FATAL ERROR: 

[1] face 5738 area does not match neighbour by 0.0267405% -- possible face ordering problem.

patch:procBoundary1to2 my area:3.99835e-06 neighbour area:3.99941e-06 matching tolerance:1.03424e-09

Mesh face:1187038 vertices:4((-0.0929725 0.00598575 0.04625) (-0.0929683 0.00598432 0.045625) (-0.0993664 0.00603686 0.045625) (-0.0993686 0.00603759 0.04625))

If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.

Rerun with processor debug flag set for more information.

[1] 

[1]     From function virtual void Foam::processorPolyPatch::calcGeometry(Foam::PstreamBuffers&)

[1]     in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 284.

[1] 

FOAM parallel run exiting

[1] 



Detected 0 baffle edges out of 54250 edges.

--> FOAM Warning : 

    From function Foam::treeBoundBox::treeBoundBox(const Foam::UList<Foam::Vector<double> >&)

    in file meshes/treeBoundBox/treeBoundBox.C at line 136

    cannot find bounding box for zero-sized pointField, returning zero

Initially selected 0 points out of 27372 for reverse attraction.

Selected 0 points out of 27372 for reverse attraction.

Stringing feature edges : changed 0 points

Attraction:

     linear   : max:(0.00183956 -0.00110546 -7.51662e-06) avg:(4.50171e-05 -2.00879e-05 -2.80543e-09)

     feature  : max:(0 0 0) avg:(0 0 0)

Feature analysis : total master points:27048 attraction to :

    feature point   : 0

    feature edge    : 0

    nearest surface : 0

    rest            : 27048



Smoothing displacement ...

Iteration 0

Iteration 10

Iteration 20

Displacement smoothed in = 6.6 s





Moving mesh ...



Iteration 0

Moving mesh using displacement scaling : min:1  max:1

Correcting 2-D mesh motion--> FOAM Warning : 

    From function void Foam::motionSmootherAlgo::modifyMotionPoints(Foam::pointField&) const

    in file motionSmoother/motionSmootherAlgo.C at line 657

    2D mesh-motion probably not correct in parallel

 ...done

[1] processorPolyPatch::calcGeometry : Writing my 14323 faces to OBJ file "/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor1/procBoundary1to2_faces.obj"

[2] processorPolyPatch::calcGeometry : Writing my 14323 faces to OBJ file "/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor2/procBoundary2to1_faces.obj"

[2] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor2/procBoundary2to1_faceCentresConnections.obj"

[1] processorPolyPatch::calcGeometry : Dumping cell centre lines between corresponding face centres to OBJ file"/media/agit/Volume/OpenFOAM/_baseCaseTest01/1_cases/0.507/5E-02/processor1/procBoundary1to2_faceCentresConnections.obj"

[2] 

[2] 

[2] --> FOAM FATAL ERROR: 

[2] face 5738 area does not match neighbour by 0.0267405% -- possible face ordering problem.

patch:procBoundary2to1 my area:3.99941e-06 neighbour area:3.99835e-06 matching tolerance:1.03479e-09

Mesh face:1177078 vertices:4((-0.0929725 0.00598575 0.04625) (-0.0993708 0.00603835 0.04625) (-0.0993676 0.00603726 0.045625) (-0.0929683 0.00598432 0.045625))

If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.

Rerun with processor debug flag set for more information.

[2] 

[2]     From function virtual void Foam::processorPolyPatch::calcGeometry(Foam::PstreamBuffers&)

[2]     in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 284.

[2] 

FOAM parallel run exiting

[2] 

--------------------------------------------------------------------------

MPI_ABORT was invoked on rank 2 in communicator MPI COMMUNICATOR 3 SPLIT FROM 0

with errorcode 1.



NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.

You may or may not see output from other processes, depending on

exactly when Open MPI kills them.

--------------------------------------------------------------------------

[1] 

[1] 

[1] --> FOAM FATAL ERROR: 

[1] face 5738 area does not match neighbour by 0.0267405% -- possible face ordering problem.

patch:procBoundary1to2 my area:3.99835e-06 neighbour area:3.99941e-06 matching tolerance:1.03424e-09

Mesh face:1187038 vertices:4((-0.0929725 0.00598575 0.04625) (-0.0929683 0.00598432 0.045625) (-0.0993664 0.00603686 0.045625) (-0.0993686 0.00603759 0.04625))

If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.

Rerun with processor debug flag set for more information.

[1] 

[1]     From function virtual void Foam::processorPolyPatch::calcGeometry(Foam::PstreamBuffers&)

[1]     in file meshes/polyMesh/polyPatches/constraint/processor/processorPolyPatch.C at line 284.

[1] 

FOAM parallel run exiting

[1]

hello agit,
did you find any solutions? i have the same problem...
best regards.

I've had the same error, when using SHM and I found this thread, in which the 3rd post suggests that you must not have the boundary type empty in your model.

I just tried it out by switching each empty boundary to type patch and it worked!

The same thing applies to type cyclic as far as I know.

Best regards
Finn

Quote:

Originally Posted by finn_amann (Post 836329)

Hello Finn,
Yes snappy does not support defining boundaries with, empty cyclic, cyclicAMi, symmetry, symmetry plane. This type of boundaries should be created after the meshing with createPatch utility
F.