sHM cannot find file
 

Hey all,
I'm trying to run snappy in parallel and keep getting the error:

The case works on a single core, but barfs on a multicore job. Hoping that someone has seen this before!!
Thanks,
Dustin

Hi Dustin,

after you run decomposePar. You have copy the triSurface folder into every constant folder of every processor folder (processor0, processor1...)
Snappy should run afterwards.

Patrick

Thanks Patrick, that got it to run, but it's now failing on reconstructPar, again complaining about a missing file:

Looked at each of the processors with paraFoam and each looked as expected.
Thanks,
Dustin

Hey,

I've never had that problem when I worked with decomposePar so I have no idea what the problem might be. It's best if you search the forum.

Sorry that I couldn't be of more help.

I have managed to get SHM working in parallel and can offer a couple of comments.
i. You can just make soft links to your stl file in the processor directories rather than copying it lots of times.
ii. When doing the reconstruction after running SHM I found it necessary to use the -constant option to rebuild the mesh. I also found it necessary to increase the write tolerance to 10^-8 when using reconstructParMesh.

hello,

I am trying to run sHM in parallel.

When I run :

snappyHexMesh -parallel

I get the following error message

[250]cfs10-sanchi /shared/sanchi/OpenFOAM/sanchi-1.7.x/pippo % snappyHexMesh -parallel 12


--> FOAM FATAL ERROR:
bool Pstream::init(int& argc, char**& argv) : attempt to run parallel on 1 processor

From function Pstream::init(int& argc, char**& argv)
in file Pstream.C at line 73.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) in "/shared/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/shared/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::Pstream::init(int&, char**&) in "/shared/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/openmpi-1.4.1/libPstream.so"
#3 Foam::argList::argList(int&, char**&, bool, bool) in "/shared/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 main in "/shared/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/snappyHexMesh"
#5 __libc_start_main in "/lib64/libc.so.6"
#6 _start at /usr/src/packages/BUILD/glibc-2.10.1/csu/../sysdeps/x86_64/elf/start.S:116
[cfs10:09124] *** Process received signal ***
[cfs10:09124] Signal: Aborted (6)
[cfs10:09124] Signal code: (-6)
[cfs10:09124] [ 0] /lib64/libc.so.6 [0x2af77d069560]
[cfs10:09124] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x2af77d0694e5]
[cfs10:09124] [ 2] /lib64/libc.so.6(abort+0x180) [0x2af77d06a9b0]
[cfs10:09124] [ 3] /shared/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam5error5abortEv+0x241) [0x2af77c16f7f1]
[cfs10:09124] [ 4] /shared/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/openmpi-1.4.1/libPstream.so(_ZN4Foam7Pstream4initERiRPPc+0x2a6) [0x2af77d398b96]
[cfs10:09124] [ 5] /shared/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam7argListC1ERiRPPcbb+0x2869) [0x2af77c17ec49]
[cfs10:09124] [ 6] snappyHexMesh [0x40515a]
[cfs10:09124] [ 7] /lib64/libc.so.6(__libc_start_main+0xfd) [0x2af77d055a7d]
[cfs10:09124] [ 8] snappyHexMesh [0x404639]
[cfs10:09124] *** End of error message ***
Abort

Any idea ?

Stephane.

I have found the solution reading the advices of W. Heydlauff. You don't need to copy the stl file into each processor* folder.

Hereafter isthe procedure.

- run "blockMesh" a usual
- decomposeMethode in decomposeParDict must be hirarcial
- run "decomposePar"
- run "foamJob -p -s snappyHexMesh"
- afterwards run "reconstructParMesh -mergeTol 1e-06 -latestTime"
(or -time 1; -time 2; ...)

Works perfect for the 3 steps of sHM:
castellatedMesh true;
snap true;
addLayers true;


Stephane.

Actually it is not necessary to copy triSurface folder into every processor folder since it will read from the main constant folder anyway. I met a similar "cannot find file" problem. In my case, it was .eMesh file missing. So it was solved by just run "surfaceFeatureExtract"