CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Native Meshers: snappyHexMesh and Others

sHM cannot find file

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 4, 2010, 02:40
Default sHM cannot find file
  #1
New Member
 
Dustin
Join Date: Mar 2009
Posts: 6
Rep Power: 8
nitsud is on a distinguished road
Hey all,
I'm trying to run snappy in parallel and keep getting the error:

Code:
[0] 
[0] 
[0] Cannot find file "" in directory "constant/triSurface"
[0] 
[0]     From function Time::findInstance(const fileName&, const word&, const IOobject::readOption)
[0]     in file db/Time/findInstance.C at line 148.
[0]
The case works on a single core, but barfs on a multicore job. Hoping that someone has seen this before!!
Thanks,
Dustin
nitsud is offline   Reply With Quote

Old   March 8, 2010, 08:08
Default
  #2
New Member
 
Patrick Wang
Join Date: Dec 2009
Location: Stuttgart, Germany
Posts: 26
Rep Power: 7
foam_noob is on a distinguished road
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
foam_noob is offline   Reply With Quote

Old   March 14, 2010, 02:01
Default
  #3
New Member
 
Dustin
Join Date: Mar 2009
Posts: 6
Rep Power: 8
nitsud is on a distinguished road
Thanks Patrick, that got it to run, but it's now failing on reconstructPar, again complaining about a missing file:

Code:
cannot open file

file: caseRoot/processor0/1/polyMesh/pointProcAddressing at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 62.

FOAM exiting
Looked at each of the processors with paraFoam and each looked as expected.
Thanks,
Dustin
nitsud is offline   Reply With Quote

Old   March 15, 2010, 03:08
Default
  #4
New Member
 
Patrick Wang
Join Date: Dec 2009
Location: Stuttgart, Germany
Posts: 26
Rep Power: 7
foam_noob is on a distinguished road
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.
foam_noob is offline   Reply With Quote

Old   March 15, 2010, 05:09
Default
  #5
New Member
 
Simon Rees
Join Date: Mar 2009
Posts: 12
Rep Power: 8
sjrees is on a distinguished road
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.
sjrees is offline   Reply With Quote

Old   July 14, 2010, 04:08
Default
  #6
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
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:rintStack(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.
openfoam_user is offline   Reply With Quote

Old   July 20, 2010, 09:04
Default
  #7
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
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.
openfoam_user is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Compiling gmshFoam with OpenFOAM-1.5 BlGene Open Source Meshers: Gmsh, Netgen, CGNS, ... 10 August 6, 2009 04:26
ParaView Compilation jakaranda OpenFOAM Installation 3 October 27, 2008 12:46
Compiling OpenFOAM13 on AMD64 with Redhat Enterprise mbeaudoin OpenFOAM Installation 20 June 17, 2008 06:43
Axisymmetrical mesh Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00
error while compiling the USER Sub routine CFD user CFX 3 November 25, 2002 16:16


All times are GMT -4. The time now is 11:07.