 |
 |
 |
|
|
|
[Sponsors] | ||||
February 9, 2012, 04:43
|
Parallel sHM error
|
#1 | ||
|
Member
Join Date: Oct 2011
Posts: 36
Rep Power: 14  |
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 Quote:
Quote:
Thanks in advance! Last edited by vigges; February 9, 2012 at 05:26. Reason: Provide version of used sofware |
|||
|
|
|||
|
April 4, 2012, 09:18
|
|
#2 |
|
Senior Member
lore
Join Date: Mar 2010
Location: Italy
Posts: 460
Rep Power: 18  |
I'm having the same issue… did you manage to solve sort it out eventually?
|
|
|
|
|
|
|
April 4, 2012, 09:42
|
|
#3 |
|
Member
Join Date: Oct 2011
Posts: 36
Rep Power: 14 |
Sorry, I haven't got any solution.
I gave up after trying an entire weekend 
|
|
|
|
|
|
|
April 18, 2012, 11:17
|
|
#4 |
|
Member
Join Date: Apr 2012
Location: France
Posts: 72
Rep Power: 14 |
Have you solve your problem ? What command line did you executed before reconstructPartMesh ?
Maybe I have a solution to solve your problem |
|
|
|
|
|
|
April 24, 2012, 03:37
|
|
#5 |
|
New Member
Join Date: Apr 2012
Posts: 4
Rep Power: 14 |
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  rocBoundary2to1 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)?? |
|
|
|
|
|
|
April 24, 2012, 03:43
|
|
#6 |
|
Member
Join Date: Apr 2012
Location: France
Posts: 72
Rep Power: 14 |
Could you copy your files here ? (decomposePar, snappyHexMesh, controlDict)
|
|
|
|
|
|
|
April 30, 2012, 04:59
|
|
#7 |
|
New Member
Join Date: Apr 2012
Posts: 4
Rep Power: 14 |
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? |
|
|
|
|
|
|
May 2, 2012, 06:44
|
|
#8 | ||
|
Member
Join Date: Apr 2012
Location: France
Posts: 72
Rep Power: 14 |
Quote:
Quote:
|
|||
|
|
|
|||
|
March 18, 2013, 06:27
|
exit with error when parallelized
|
#9 |
|
Member
|
I just run sHM in serial and it finished correctly, without snapped and layered mesh.
it seems that the problem in sHM
__________________
practice makes perfect |
|
|
|
|
|
|
November 23, 2018, 08:45
|
|
#10 |
|
New Member
Join Date: Oct 2018
Posts: 5
Rep Power: 7 |
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]
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: |
|
|
|
|
|
|
June 3, 2020, 08:34
|
|
#11 | |
|
Senior Member
Franco
Join Date: Nov 2019
Location: Compiègne, France
Posts: 129
Rep Power: 6 |
Quote:
did you find any solutions? i have the same problem... best regards. |
||
|
|
|
||
|
September 22, 2022, 15:41
|
|
#12 |
|
New Member
Join Date: Dec 2021
Posts: 27
Rep Power: 4 |
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 |
|
|
|
|
|
|
September 23, 2022, 01:23
|
|
#13 | |
|
Senior Member
Franco
Join Date: Nov 2019
Location: Compiègne, France
Posts: 129
Rep Power: 6 |
Quote:
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. |
||
|
|
|
||
 |
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| Mesquite - Adaptive mesh refinement / coarsening? | philippose | OpenFOAM Running, Solving & CFD | 94 | January 27, 2016 09:40 |
| Undeclared Identifier Errof UDF | SteveGoat | Fluent UDF and Scheme Programming | 7 | October 15, 2014 07:11 |
| Errors in UDF | shashank312 | Fluent UDF and Scheme Programming | 6 | May 30, 2013 20:30 |
| Ansys Fluent 13.0 UDF compilation problem in Window XP (32 bit) | Yogini | Fluent UDF and Scheme Programming | 7 | October 3, 2012 07:24 |
| Installation OF1.5-dev | ttdtud | OpenFOAM Installation | 46 | May 5, 2009 02:32 |
3Likes
Linear Mode
