|
[Sponsors] |
February 18, 2015, 08:36 |
Error running simpleFoam in parallel
|
#1 |
Member
Rubén
Join Date: Oct 2014
Location: Munich
Posts: 47
Rep Power: 12 |
Hi FOAMers!
I have recently posted one theard, but I have had another issue and I would like to know if you can help me. I have searched in the forums but I don't have found anything about this error. I have done decomposePar in order to do my snappy, and after then I write mpirun -np 8 simpleFoam -parallel in order to run simpleFoam in parallel but I receive this error. Can you help me to find the reason? Thank you very much indeed in advance! Code:
usuario@usuario-SATELLITE-P50-A-14G:~/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon$ mpirun -np 8 simpleFoam -parallel /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.3.0-f5222ca19ce6 Exec : simpleFoam -parallel Date : Feb 18 2015 Time : 13:25:03 Host : "usuario-SATELLITE-P50-A-14G" PID : 7464 Case : /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon nProcs : 8 Slaves : 7 ( "usuario-SATELLITE-P50-A-14G.7465" "usuario-SATELLITE-P50-A-14G.7466" "usuario-SATELLITE-P50-A-14G.7467" "usuario-SATELLITE-P50-A-14G.7468" "usuario-SATELLITE-P50-A-14G.7469" "usuario-SATELLITE-P50-A-14G.7470" "usuario-SATELLITE-P50-A-14G.7471" ) Pstream initialized with: floatTransfer : 0 nProcsSimpleSum : 0 commsType : nonBlocking polling iterations : 0 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading field p [4] [4] [4] --> FOAM FATAL IO ERROR: [4] Cannot find patchField entry for procBoundary4to5 [4] [4] file: /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon/processor4/0/p.boundaryField from line 28 to line 21. [4] [4] From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) [4] in file /home/usuario/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209. [4] FOAM parallel run exiting [4] [5] [5] [6] [6] [6] --> FOAM FATAL IO ERROR: [6] Cannot find patchField entry for procBoundary6to5 [6] [6] file: /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon/processor6/0/p.boundaryField from line 28 to line 21. [6] [7] [7] [7] --> FOAM FATAL IO ERROR: [7] Cannot find patchField entry for procBoundary7to4 [7] [7] file: [6] From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) [6] in file /home/usuario/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209. [6] FOAM parallel run exiting [6] [1] [1] [1] --> FOAM FATAL IO ERROR: [1] Cannot find patchField entry for procBoundary1to0 [1] [1] file: /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon/processor1/0/p.boundaryField from line 28 to line 21. [1] [1] From function /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon/processor7/0/p.boundaryField from line 28 to line 21. [7] [7] From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) [7] in file /home/usuario/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209. [7] FOAM parallel run exiting [7] [0] [0] [0] --> FOAM FATAL IO ERROR: [0] Cannot find patchField entry for procBoundary0to2 [0] [0] file: /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon/processor0/0/p.boundaryField from line 28 to line 21. [0] [0] From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) [0] in file /home/usuario/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209. [0] FOAM parallel run exiting [0] GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) [1] in file /home/usuario/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209. [1] FOAM parallel run exiting [1] [2] [2] [2] --> FOAM FATAL IO ERROR: [2] Cannot find patchField entry for procBoundary2to0 [2] [2] file: /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon/processor2/0/p.boundaryField from line 28 to line 21. [2] [2] From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) [2] in file /home/usuario/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209. [2] FOAM parallel run exiting [2] [3] [3] [3] --> FOAM FATAL IO ERROR: [3] Cannot find patchField entry for procBoundary3to0 [3] [3] file: /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon/processor3/0/p.boundaryField from line 28 to line 21. [3] [3] From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) [3] in file /home/usuario/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209. [3] FOAM parallel run exiting [3] [5] --> FOAM FATAL IO ERROR: [5] Cannot find patchField entry for procBoundary5to4 [5] [5] file: /home/usuario/OpenFOAM/usuario-2.3.0/run/Frisbee_KEpsilon/processor5/0/p.boundaryField from line 28 to line 21. [5] [5] From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) [5] in file /home/usuario/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209. [5] FOAM parallel run exiting [5] -------------------------------------------------------------------------- MPI_ABORT was invoked on rank 6 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. -------------------------------------------------------------------------- -------------------------------------------------------------------------- mpirun has exited due to process rank 5 with PID 7469 on node usuario-SATELLITE-P50-A-14G 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). -------------------------------------------------------------------------- [usuario-SATELLITE-P50-A-14G:07463] 7 more processes have sent help message help-mpi-api.txt / mpi-abort [usuario-SATELLITE-P50-A-14G:07463] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages |
|
February 20, 2015, 04:46 |
|
#2 |
Senior Member
Join Date: Jan 2015
Posts: 150
Rep Power: 11 |
It seems that you simple not define your boundary condition. It is not a problem of parallel execution. Try to execute program in serial and you will get the same error.
|
|
February 24, 2015, 12:15 |
|
#3 |
Member
Rubén
Join Date: Oct 2014
Location: Munich
Posts: 47
Rep Power: 12 |
No, I doesn't work even in serial.
Anyone can help me? I would be very pleased indeed |
|
February 24, 2015, 12:26 |
|
#4 |
Senior Member
Join Date: Jan 2015
Posts: 150
Rep Power: 11 |
I've told to you that the problem is not in the parallel execution. You incorrectly defined the boundary conditions.
If you can, post you U and p files here and I will help you. |
|
February 24, 2015, 12:26 |
|
#5 | |
Member
Thiago Parente Lima
Join Date: Sep 2011
Location: Diamantina, Brazil.
Posts: 65
Rep Power: 15 |
That's what Svensen said. There is nothing to do with parallel running, somethng is wrong with your boundary conditions:
Quote:
__________________
Fields of interest: buoyantFoam, chtMultRegionFoam. |
||
February 24, 2015, 12:32 |
|
#6 |
Senior Member
|
Hi,
Can you, please, post sequence of actions you've preformed to get this error? In particular how did you run snappyHexMesh? According to the message something happened to the decomposition, simpleFoam can find patches corresponding to processor boundaries. |
|
February 24, 2015, 12:43 |
|
#7 |
Member
Rubén
Join Date: Oct 2014
Location: Munich
Posts: 47
Rep Power: 12 |
Sorry!
I mean, it works in serial! Sorry for not explaining well. My run file is: Code:
#!/bin/sh cd constant/triSurface; surfaceOrient frisbee.stl "(1e10 1e10 1e10)" frisbee.stl; surfaceCheck frisbee.stl >surfaceCheck.log; cd ../../; cd ${0%/*} || exit 1 # run from this directory # Source tutorial run functions . $WM_PROJECT_DIR/bin/tools/RunFunctions runApplication surfaceFeatureExtract runApplication blockMesh runApplication decomposePar runParallel snappyHexMesh 8 -overwrite #- For non-parallel runningii #cp -r 0.org 0 > /dev/null 2>&1 #- For parallel running ls -d processor* | xargs -i rm -rf ./{}/0 $1 ls -d processor* | xargs -i cp -r 0.org ./{}/0 $1 cp -r 0.org 0 runApplication reconstructParMesh -constant |
|
February 24, 2015, 12:47 |
|
#8 |
Member
Rubén
Join Date: Oct 2014
Location: Munich
Posts: 47
Rep Power: 12 |
Sorry!
I mean, it works in serial! Sorry for not explaining well. My run file is: Code:
#!/bin/sh cd constant/triSurface; surfaceOrient frisbee.stl "(1e10 1e10 1e10)" frisbee.stl; surfaceCheck frisbee.stl >surfaceCheck.log; cd ../../; cd ${0%/*} || exit 1 # run from this directory # Source tutorial run functions . $WM_PROJECT_DIR/bin/tools/RunFunctions runApplication surfaceFeatureExtract runApplication blockMesh runApplication decomposePar runParallel snappyHexMesh 8 -overwrite #- For non-parallel runningii #cp -r 0.org 0 > /dev/null 2>&1 #- For parallel running ls -d processor* | xargs -i rm -rf ./{}/0 $1 ls -d processor* | xargs -i cp -r 0.org ./{}/0 $1 cp -r 0.org 0 runApplication reconstructParMesh -constant Code:
mpirun -np 8 simpleFoam -parallel Last edited by Yuby; February 24, 2015 at 14:17. |
|
February 24, 2015, 12:48 |
|
#9 |
Member
Rubén
Join Date: Oct 2014
Location: Munich
Posts: 47
Rep Power: 12 |
Do you think that it has to be with the type of decomposition?
I tried with both hierarchical and scotch decompositions and I get the same error Thank you very much for your replies! |
|
February 24, 2015, 12:52 |
|
#10 |
Senior Member
|
Hi,
This is fatal for the decomposed case: Code:
#- For parallel running ls -d processor* | xargs -i rm -rf ./{}/0 $1 ls -d processor* | xargs -i cp -r 0.org ./{}/0 $1 You see, fields in 0 folder are also decomposed, here is an example of modified file: Code:
boundaryField { ... procBoundary0to1 { type processor; value uniform 0; } procBoundary0to2 { type processor; value uniform 0; } } So you either, run reconstructParMesh, delete processor* folders, and decomposePar again. Or you can try to keep 0 folders in processor* folders. |
|
February 25, 2015, 18:57 |
|
#11 |
Member
Rubén
Join Date: Oct 2014
Location: Munich
Posts: 47
Rep Power: 12 |
Thank you very much indeed, Alexey!!!
That is the solution to this problem. Completely pleased! |
|
May 21, 2016, 23:20 |
Have spend roughly 6 hours on this file. No luck.
|
#12 |
New Member
LD
Join Date: May 2016
Location: Savannah, GA
Posts: 7
Rep Power: 10 |
This is my Allrun file. Is this what you meant when you said the two lines were fatal?
Code:
#!/bin/sh cd ${0%/*} || exit 1 # Run from this directory # Source tutorial run functions . $WM_PROJECT_DIR/bin/tools/RunFunctions runApplication surfaceFeatureExtract runApplication blockMesh runApplication decomposePar runParallel snappyHexMesh 4 -overwrite #mpirun -np 4 snappyHexMesh -overwrite -parallel >log.snappyHexMesh #- For non-parallel running #cp -r 0.org 0 > /dev/null 2>&1 #- For parallel running #ls -d processor* | xargs -I {} rm -rf ./{}/0 #ls -d processor* | xargs -I {} cp -r 0.org ./{}/0 reconstructPar -latestTime runParallel patchSummary 4 runParallel potentialFoam 4 runParallel $(getApplication) 4 runApplication reconstructParMesh -constant runApplication reconstructPar -latestTime # ----------------------------------------------------------------- end-of-file I have used simple, hierarchical; but still no luck. I have also tried the mpirun directly without using RunParallel, but still no luck. Also, the two lines are being used in MotorBike and the AllRun file works just fine. |
|
October 18, 2016, 05:53 |
|
#13 | |
Member
Rudolf Hellmuth
Join Date: Sep 2012
Location: Dundee, Scotland
Posts: 40
Rep Power: 14 |
Quote:
In 0/* dictionaries you have to have that #includeEtc below: Code:
boundaryField { //- Set patchGroups for constraint patches #includeEtc "caseDicts/setConstraintTypes" ... } I had deleted that #includeEtc line because my Paraview on Windows was not reading my case.foam because of the hashtag (#). Best regards, Rudolf |
||
April 17, 2017, 17:27 |
|
#14 | |
New Member
Join Date: Dec 2016
Posts: 6
Rep Power: 9 |
Quote:
|
||
October 7, 2021, 05:38 |
|
#15 | |
New Member
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 10 |
Quote:
Thanks! I was becoming crazy not understanding why serial was working but not parallel. But does someone know why? According to #includeEtc "caseDicts/setConstraintTypes" it seems it sets the same BC when using cyclic or empty. However, in my case I am setting a domain with only patches ( inlet / outlet ) and I still had that problem.
__________________
Enjoy the flow |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
simpleFoam parallel | AndrewMortimer | OpenFOAM Running, Solving & CFD | 12 | August 7, 2015 19:45 |
simpleFoam parallel solver & Fluent polyhedral mesh | Zlatko | OpenFOAM Running, Solving & CFD | 3 | September 26, 2014 07:53 |
simpleFoam in parallel issue | plucas | OpenFOAM Running, Solving & CFD | 3 | July 17, 2013 12:30 |
parallel Grief: BoundaryFields ok in single CPU but NOT in Parallel | JR22 | OpenFOAM Running, Solving & CFD | 2 | April 19, 2013 17:49 |
parallel simpleFoam freezes the whole system | vangelis | OpenFOAM Running, Solving & CFD | 14 | May 16, 2012 06:12 |