CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

simpleFoam parallel solver & Fluent polyhedral mesh

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

Like Tree1Likes
  • 1 Post By tomf

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 18, 2014, 06:25
Default simpleFoam parallel solver & Fluent polyhedral mesh
  #1
New Member
 
Zlatko's Avatar
 
Join Date: Mar 2009
Posts: 10
Rep Power: 13
Zlatko is on a distinguished road
Hi,

I have a problem with simpleFOAM parallel sover using fluent polyhedral mesh.

A tetrahedral mesh was created in GAMBIT and imported into Fluent, where computational domain was converted to polyhedral cells and rotational periodic boundary conditions were defined for two faces. The case was run without any problems in Fluent.

I wanted to use the same mesh with OpenFOAM simpleFoam solver, so I:
  1. used fluent3DMeshToFoam utility to create OpenFOAM mesh,
  2. applied createPatch tool to define rotational cyclic boundary conditions following this thread,
  3. decomposed the domain into 4 partitions using decomposePar utility.
New mesh was checked with checkMesh utillity and everything was OK.
First, I started simpleFoam serial solver and it converged well with the expected results. Then, I wanted to use parallel solver, but it crashed with error:
Code:
$ mpirun -np 4 simpleFoam -parallel 2>&1 | tee run.log
      
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  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   : Sep 18 2014
Time   : 11:12:40
Host   : "lfdt"
PID    : 17682
Case   : /work/cyclic-1phase-laminar
nProcs : 4
Slaves : 
3
(
"lfdt.17683"
"lfdt.17684"
"lfdt.17685"
)

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

[3] #0  Foam::error::printStack(Foam::Ostream&)[2] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[3] #1  Foam::sigSegv::sigHandler(int) at ??:?
[2] #1  Foam::sigSegv::sigHandler(int) at ??:?
[3] #2   in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #3  Foam::processorPolyPatch::updateMesh(Foam::PstreamBuffers&) at ??:?
[2] #2   at ??:?
[3] #4  Foam::polyBoundaryMesh::updateMesh() in "/lib/x86_64-linux-gnu/libc.so.6"
[2] #3  Foam::processorPolyPatch::updateMesh(Foam::PstreamBuffers&)[1] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[3] #5  Foam::polyMesh::polyMesh(Foam::IOobject const&) at ??:?
[2] #4  Foam::polyBoundaryMesh::updateMesh() at ??:?
[1] #1  Foam::sigSegv::sigHandler(int) at ??:?
[3] #6  Foam::fvMesh::fvMesh(Foam::IOobject const&) at ??:?
[2] #5  Foam::polyMesh::polyMesh(Foam::IOobject const&) at ??:?
[1] #2   at ??:?
[3] #7   at ??:?
[2] #6  Foam::fvMesh::fvMesh(Foam::IOobject const&) in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #3  Foam::processorPolyPatch::updateMesh(Foam::PstreamBuffers&)
 at ??:?
[2] #7   at ??:?
[1] #4  Foam::polyBoundaryMesh::updateMesh()[3]  at ??:?
[3] #8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #9  
 at ??:?
[1] #5  Foam::polyMesh::polyMesh(Foam::IOobject const&)
[2]  at ??:?
[2] #8  __libc_start_main[3]  at ??:?
[lfdt:17685] *** Process received signal ***
[lfdt:17685] Signal: Segmentation fault (11)
[lfdt:17685] Signal code:  (-6)
[lfdt:17685] Failing at address: 0x3e800004515
 at ??:?
[1] #6  Foam::fvMesh::fvMesh(Foam::IOobject const&) in "/lib/x86_64-linux-gnu/libc.so.6"
[2] #9  [lfdt:17685] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x36c30) [0x7f061b6b0c30]
[lfdt:17685] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x39) [0x7f061b6b0bb9]
[lfdt:17685] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x36c30) [0x7f061b6b0c30]
[lfdt:17685] [ 3] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam18processorPolyPatch10updateMeshERNS_14PstreamBuffersE+0x223) [0x7f061c8be663]
[lfdt:17685] [ 4] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam16polyBoundaryMesh10updateMeshEv+0x176) [0x7f061c8c49b6]
[lfdt:17685] [ 5] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam8polyMeshC2ERKNS_8IOobjectE+0xc05) [0x7f061c90c325]
[lfdt:17685] [ 6] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZN4Foam6fvMeshC2ERKNS_8IOobjectE+0x19) [0x7f061e1a1e99]
[lfdt:17685] [ 7] simpleFoam() [0x41aaf7]
[lfdt:17685] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf5) [0x7f061b69bec5]
[lfdt:17685] [ 9] simpleFoam() [0x41c640]
[lfdt:17685] *** End of error message ***

 at ??:?
[1] #7  
[2]  at ??:?
[lfdt:17684] *** Process received signal ***
[lfdt:17684] Signal: Segmentation fault (11)
[lfdt:17684] Signal code:  (-6)
[lfdt:17684] Failing at address: 0x3e800004514
[lfdt:17684] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x36c30) [0x7f9d15520c30]
[lfdt:17684] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x39) [0x7f9d15520bb9]
[lfdt:17684] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x36c30) [0x7f9d15520c30]
[lfdt:17684] [ 3] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam18processorPolyPatch10updateMeshERNS_14PstreamBuffersE+0x21b) [0x7f9d1672e65b]
[lfdt:17684] [ 4] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam16polyBoundaryMesh10updateMeshEv+0x176) [0x7f9d167349b6]
[lfdt:17684] [ 5] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam8polyMeshC2ERKNS_8IOobjectE+0xc05) [0x7f9d1677c325]
[lfdt:17684] [ 6] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZN4Foam6fvMeshC2ERKNS_8IOobjectE+0x19) [0x7f9d18011e99]
[lfdt:17684] [ 7] simpleFoam() [0x41aaf7]
[lfdt:17684] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf5) [0x7f9d1550bec5]
[lfdt:17684] [ 9] simpleFoam() [0x41c640]
[lfdt:17684] *** End of error message ***
[1]  at ??:?
[1] #8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #9  
[1]  at ??:?
[lfdt:17683] *** Process received signal ***
[lfdt:17683] Signal: Segmentation fault (11)
[lfdt:17683] Signal code:  (-6)
[lfdt:17683] Failing at address: 0x3e800004513
[lfdt:17683] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x36c30) [0x7fa0073e2c30]
[lfdt:17683] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x39) [0x7fa0073e2bb9]
[lfdt:17683] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x36c30) [0x7fa0073e2c30]
[lfdt:17683] [ 3] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam18processorPolyPatch10updateMeshERNS_14PstreamBuffersE+0x21b) [0x7fa0085f065b]
[lfdt:17683] [ 4] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam16polyBoundaryMesh10updateMeshEv+0x176) [0x7fa0085f69b6]
[lfdt:17683] [ 5] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam8polyMeshC2ERKNS_8IOobjectE+0xc05) [0x7fa00863e325]
[lfdt:17683] [ 6] /home/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZN4Foam6fvMeshC2ERKNS_8IOobjectE+0x19) [0x7fa009ed3e99]
[lfdt:17683] [ 7] simpleFoam() [0x41aaf7]
[lfdt:17683] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf5) [0x7fa0073cdec5]
[lfdt:17683] [ 9] simpleFoam() [0x41c640]
[lfdt:17683] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 3 with PID 17685 on node lfdt exited on signal 11 (Segmentation fault).
--------------------------------------------------------------------------
$
Does anyone have an idea what could be wrong?

Best regards.

Zlatko
Zlatko is offline   Reply With Quote

Old   September 22, 2014, 04:36
Default
  #2
New Member
 
Zlatko's Avatar
 
Join Date: Mar 2009
Posts: 10
Rep Power: 13
Zlatko is on a distinguished road
Update: If boundary type cyclic is changed to type wall in files 0/{U,p} and constant/polyMesh/boundary, then parallel simpleFoam runs without problem.
Is it possible that decomposePar has a problem with cyclic boundaries?
Zlatko is offline   Reply With Quote

Old   September 26, 2014, 06:32
Default
  #3
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 557
Rep Power: 22
tomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi,

For coupled patches you should keep them on the same processor when decomposing using:

preservePatches (cyclic_1 cyclic_2);

in the decomposeParDict

Where cyclic_1 and cyclic_2 are the names of your cyclic patches.

Regards,
Tom
Zlatko likes this.
tomf is offline   Reply With Quote

Old   September 26, 2014, 07:53
Default
  #4
New Member
 
Zlatko's Avatar
 
Join Date: Mar 2009
Posts: 10
Rep Power: 13
Zlatko is on a distinguished road
Quote:
Originally Posted by tomf View Post
For coupled patches you should keep them on the same processor when decomposing using:

preservePatches (cyclic_1 cyclic_2);

in the decomposeParDict

Where cyclic_1 and cyclic_2 are the names of your cyclic patches.
Tom, thank you very much. Now it works.

Best regards,

Zlatko
Zlatko is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
how to set periodic boundary conditions Ganesh FLUENT 14 November 26, 2018 12:26
[snappyHexMesh] No layers in a small gap bobburnquist OpenFOAM Meshing & Mesh Conversion 6 August 26, 2015 10:38
[ICEM] Missing face error from FLUENT even after repairing mesh + other questions unknown159 ANSYS Meshing & Geometry 0 July 5, 2013 21:18
Transport mesh from ICEM CFD, to Fluent, to Sysnoise Wieland FLUENT 2 April 15, 2012 07:28
mesh missing after import in fluent morteza08 FLUENT 0 July 23, 2010 03:22


All times are GMT -4. The time now is 16:29.