[sebonator]

Hi everybody,

I got a problem with reconstructing my fields after running "interDyMFoam" with "dynamicRefineFvMesh" in parallel.

A first thing to say is that I am sure the simulation completed successfully, because I can postprocess the results for each processor alone.

The reconstruction of the mesh using "reconstructParMesh" still works fine, although I think I did not use the easiest way, as I have to use "reconstructParMesh -time x.xx" for every single timestep.

My problem occurs when doing "reconstructPar" to reconstruct the fields. When I am trying it from inside a case directory, the function aborts already during the first timestep. I found a tip in another thread that it might help to use it like "reconstructPar -case xxxxx" from outside the case directory. I was kind of surprised that it almost worked this way. But still, after about the half of the timesteps, the function aborts, always showing the same error:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5.x |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : reconstructPar -time 0.56
Date : Aug 25 2009
Time : 16:09:30
Host : ttdws69
PID : 25049
Case : /home/lang/OpenFOAM/lang-1.5.x/run/SebLangBachelorArbeit/03-DuharColin-3DStroemung-Vorarbeiten/06-AdaptiveGitterverfeinerung/03-BrokenDamMit2
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0.8

Time = 0.56

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam:bjectRegistry::checkOut(Foam::regIOobject&) const in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::regIOobject::checkOut() in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 Foam::regIOobject::~regIOobject() in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#6 Foam::IOList<int>::~IOList() in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/applications/bin/linuxGccDPOpt/reconstructPar"
#7 Foam:rocessorMeshes::read() in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/applications/bin/linuxGccDPOpt/reconstructPar"
#8 Foam:rocessorMeshes::readUpdate() in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/applications/bin/linuxGccDPOpt/reconstructPar"
#9 main in "/home/lang/OpenFOAM/OpenFOAM-1.5.x/applications/bin/linuxGccDPOpt/reconstructPar"
#10 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#11 __gxx_personality_v0 at ../sysdeps/i386/elf/start.S:122
Speicherzugriffsfehler

I do not know why the last line is written in german, but I think it can be translated as memory access error (Do not know if its exactly called like this in english).

Has anybody got an idea how to solve this problem? I also tried running the case on a single processor and this worked absolutely fine, but for those cases I want to use it a single processor will work for weeks, so that is no option.

Thanks a lot for your help!

Greetings Sebastian

[sega]

Dear Sebastian.

I used a small bash-script for such cases:

#!/bin/bash
timeList=$(ls processor0/ | awk '$1!="constant"');

for line in $timeList
do
    echo "Recontructing mesh for t = "$line" s";
    reconstructParMesh -time $line > logTmp;

    echo "Reconstructing fields for t = "$line" s";
    reconstructPar -time $line > logTmp;

    echo "";
done

rm logTmp;

Basically it's doing reconstructParMesh and reconstructPar alternating.
Maybe you can try this, but if there is a problem with the single commands it will be of no help ...

[sebonator]

Danke Sebastian!

Ich schreibe übrigens die Nachfolgearbeit zu deiner Studienarbeit am TTD!

Gruß Sebastian

[sebonator]

Dear Sebastian,

Thanks for your help with this script. Seems to be working fine, although I do not think that I tried anything else than reconstructParMesh and reconstructPar before.

Well, after using computers for more than eight years I got comfortable with solving problems without knowing how

Thanks again,
Greetings Sebastian

[mattijs]

Did you checkMesh the mesh resulting from reconstructParMesh? It uses a geometric tolerance so might get things wrong for large refinement levels. If the problem persists in 1.6.x. can you report a bug+testcase in OpenFOAM-bugs?

[sebonator]

Hi mattijs,

no, I did not checkMesh the reconstructed Mesh, but I used a refinement level of only 1! This would mean there is a general problem, I think.

But as I replied to Sebastian above, the Script that alternates reconstructParMesh and reconstructPar works fine. I only tried to reconstructParMesh for all time and after that reconstructPar for all time. Maybe this was the Problem, I will check that up on Monday.

Bye, Sebastian

[sebonator]

Hi,

I just tried to manually alternate reconstructParMesh and reconstructPar. It worked fine, without any problem.

The reason for my problems must have been that I tried to do reconstructParMesh fol all time and after that reconstructPar for all time.

As I can not check it up with 1.6.x, I will not report a bug+testcase.
But it does not seem to be a general problem anyway, I think.

Thanks for your help!

Greets Sebastian

[openfoam_user]

Hi,

the script works fine with OpenFOAM-1.6.x.

Manually it works (for example):
reconstructParMesh -time 0.002
reconstructPar -time 0.002

Regards,

Stephane.

[liping_he]

Hi sega

I am a newcomer. I have the same problem when I do reconstruction. So I hope you can tell me how to use your code mentioned in the thread detailedly. Step by step is the best. Thank you very much.

Good luck

Liping He

[jiahui_93]

Originally Posted by sega

Dear Sebastian.

I used a small bash-script for such cases:

#!/bin/bash
timeList=$(ls processor0/ | awk '$1!="constant"');

for line in $timeList
do
    echo "Recontructing mesh for t = "$line" s";
    reconstructParMesh -time $line > logTmp;

    echo "Reconstructing fields for t = "$line" s";
    reconstructPar -time $line > logTmp;

    echo "";
done

rm logTmp;

Basically it's doing reconstructParMesh and reconstructPar alternating.
Maybe you can try this, but if there is a problem with the single commands it will be of no help ...

hi, I built my mesh using blockMesh and refineMesh, then solve my moving mesh using dynamic movingConeTopoFvMesh and command "pimpleDyMFoam -parallel". After that, I reconstruct my mesh by running the given script. But it outputs the following error. May I get some help here? Thanks for your time for looking through my case

ang@atmosfera3:~/OpenFOAM/JH/PARALLEL_linear_smallBlock_U2_TS0.015_refined$ ./reconstruct
Recontructing mesh for t = 0 s
Reconstructing fields for t = 0 s

Recontructing mesh for t = 0.01 s
Reconstructing fields for t = 0.01 s
                                                                                          
Reconstructing mesh for t = 0.02 s


--> FOAM FATAL ERROR:
Did not match all of the master faces to the slave faces
This usually means that the slave patch and master patch do not align to within 7.269285e-07 metre.

    From function void Foam::faceCoupleInfo::perfectPointMatch(Foam::scalar, bool)
    in file polyMeshAdder/faceCoupleInfo.C at line 1503.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::faceCoupleInfo::perfectPointMatch(double, bool) at ??:?
#3  Foam::faceCoupleInfo::faceCoupleInfo(Foam::polyMesh const&, Foam::List<int> const&, Foam::polyMesh const&, Foam::List<int> const&, double, bool, bool, bool) at ??:?
#4  ? at ??:?
#5  ? at ??:?
#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  ? at ??:?
./reconstruct: line 4:   420 Aborted                 (core dumped) reconstructParMesh -time $line > logTmp
Reconstructing fields for t = 0.02 s


--> FOAM FATAL ERROR:
cannot find file "/home/ang/OpenFOAM/JH/PARALLEL_linear_smallBlock_U2_TS0.015_refined/processor0/0.02/polyMesh/pointProcAddressing"

    From function virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 505.

FOAM exiting


Recontructing mesh for t = 0.03 s


--> FOAM FATAL ERROR:
Did not match all of the master faces to the slave faces
This usually means that the slave patch and master patch do not align to within 7.269285e-07 metre.

    From function void Foam::faceCoupleInfo::perfectPointMatch(Foam::scalar, bool)
    in file polyMeshAdder/faceCoupleInfo.C at line 1503.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::faceCoupleInfo::perfectPointMatch(double, bool) at ??:?
#3  Foam::faceCoupleInfo::faceCoupleInfo(Foam::polyMesh const&, Foam::List<int> const&, Foam::polyMesh const&, Foam::List<int> const&, double, bool, bool, bool) at ??:?
#4  ? at ??:?
#5  ? at ??:?
#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  ? at ??:?
./reconstruct: line 4:   447 Aborted                 (core dumped) reconstructParMesh -time $line > logTmp
Reconstructing fields for t = 0.03 s


--> FOAM FATAL ERROR:
cannot find file "/home/ang/OpenFOAM/JH/PARALLEL_linear_smallBlock_U2_TS0.015_refined/processor0/0.03/polyMesh/pointProcAddressing"

    From function virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 505.

FOAM exiting


Recontructing mesh for t = 0.04 s


--> FOAM FATAL ERROR:
Did not match all of the master faces to the slave faces
This usually means that the slave patch and master patch do not align to within 7.269285e-07 metre.

    From function void Foam::faceCoupleInfo::perfectPointMatch(Foam::scalar, bool)
    in file polyMeshAdder/faceCoupleInfo.C at line 1503.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::faceCoupleInfo::perfectPointMatch(double, bool) at ??:?
#3  Foam::faceCoupleInfo::faceCoupleInfo(Foam::polyMesh const&, Foam::List<int> const&, Foam::polyMesh const&, Foam::List<int> const&, double, bool, bool, bool) at ??:?
#4  ? at ??:?
#5  ? at ??:?
#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  ? at ??:?
./reconstruct: line 4:   474 Aborted                 (core dumped) reconstructParMesh -time $line > logTmp
Reconstructing fields for t = 0.04 s


--> FOAM FATAL ERROR:
cannot find file "/home/ang/OpenFOAM/JH/PARALLEL_linear_smallBlock_U2_TS0.015_refined/processor0/0.04/polyMesh/pointProcAddressing"

    From function virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 505.

FOAM exiting
Error of reconstruct script

Recontructing mesh for t = 0.05 s


--> FOAM FATAL ERROR:
Did not match all of the master faces to the slave faces
This usually means that the slave patch and master patch do not align to within 7.269285e-07 metre.

    From function void Foam::faceCoupleInfo::perfectPointMatch(Foam::scalar, bool)
    in file polyMeshAdder/faceCoupleInfo.C at line 1503.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::faceCoupleInfo::perfectPointMatch(double, bool) at ??:?
#3  Foam::faceCoupleInfo::faceCoupleInfo(Foam::polyMesh const&, Foam::List<int> const&, Foam::polyMesh const&, Foam::List<int> const&, double, bool, bool, bool) at ??:?
#4  ? at ??:?
#5  ? at ??:?
#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  ? at ??:?
./reconstruct: line 4:   503 Aborted                 (core dumped) reconstructParMesh -time $line > logTmp
Reconstructing fields for t = 0.05 s


--> FOAM FATAL ERROR:
cannot find file "/home/ang/OpenFOAM/JH/PARALLEL_linear_smallBlock_U2_TS0.015_refined/processor0/0.05/polyMesh/pointProcAddressing"

    From function virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 505.

FOAM exiting