CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Pre-Processing

decomposePar error

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

Like Tree1Likes
  • 1 Post By alexeym

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 27, 2017, 12:06
Default decomposePar error
  #1
Member
 
Chia
Join Date: Jan 2016
Location: Singapore
Posts: 30
Rep Power: 10
chia87 is on a distinguished road
Hi Foamers,

I could run waveFoam on my school HPC , however when I tried to run decomposePar

i had some error

Quote:
Reading g

Reading waveProperties

Reading waveProperties
Reading field p_rgh

--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 3 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.
Quote:
--> FOAM FATAL ERROR:

request for dictionary waveProperties from objectRegistry region0 failed
available objects of type dictionary are

4
(
decomposeParDict
fvSchemes
fvSolution
data
)


From function objectRegistry::lookupObject<Type>(const word&) const
in file /apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM-3.0.1/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so"
#2 Foam::IOdictionary const& Foam:bjectRegistry::lookupObject<Foam::IOdiction ary>(Foam::word const&) const in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#3 Foam::waveTheories::waveTheory::New(Foam::word const&, Foam::fvMesh const&) in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/lib/libwaves2Foam.so"
#4 Foam::waveAlphaFvPatchScalarField::waveAlphaFvPatc hScalarField(Foam::fvPatch const&, Foam:imensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/lib/libwaves2Foam.so"
#5 Foam::fvPatchField<double>::adddictionaryConstruct orToTable<Foam::waveAlphaFvPatchScalarField>::New( Foam::fvPatch const&, Foam:imensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/lib/libwaves2Foam.so"
#6 Foam::fvPatchField<double>::New(Foam::fvPatch const&, Foam:imensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/bin/decomposePar"
#7 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::readField( Foam:imensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/bin/decomposePar"
#8 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readFields(Foam::dictionary const&) in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/bin/decomposePar"
#9 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readFields() in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/bin/decomposePar"
#10 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/bin/decomposePar"
#11 ? in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/bin/decomposePar"
#12 ? in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/bin/decomposePar"
#13 __libc_start_main in "/lib64/libc.so.6"
#14 ? in "/apps/newcastle/OpenFOAM/3.0.1/1/default/OpenFOAM/OpenFOAM-3.0.1/platforms/linux64GccDPInt32Opt/bin/decomposePar"
/var/spool/sge_prod/g10s14n4/job_scripts/6025526: line 14: 97996 Aborted (core dumped) decomposePar
[0]
[0]
[0] [1]
[1]
[1] --> FOAM FATAL IO ERROR:
[1] cannot find file
[1]
[1] file: /home/polaris_ncl1/ncldwc/processor1/0/p_rgh at line 0.
[1]
[1] From function regIOobject::readStream()
[1] in file db/regIOobject/regIOobjectRead.C at line 73.
[1]
FOAM parallel run exiting
[1]
--> FOAM FATAL IO ERROR:
[0] cannot find file
[0]
[0] file: /home/polaris_ncl1/ncldwc/processor0/0/p_rgh at line 0.
[0]
[0] From function regIOobject::readStream()
[0] in file db/regIOobject/regIOobjectRead.C at line 73.
[0]
FOAM parallel run exiting
[0]
[2]
[2]
[2] --> FOAM FATAL IO ERROR:
[2] cannot find file
[2]
[2] file: /home/polaris_ncl1/ncldwc/processor2/0/p_rgh at line 0.
[2]
[2] From function regIOobject::readStream()
[2] in file db/regIOobject/regIOobjectRead.C at line 73.
[2]
FOAM parallel run exiting
[2]
[8]
[8]
[8] --> FOAM FATAL IO ERROR:
[8] cannot find file
[8]
[8] file: /home/polaris_ncl1/ncldwc/processor8/0/p_rgh at line 0.
[8]
[8] From function regIOobject::readStream()
[8] in file db/regIOobject/regIOobjectRead.C at line 73.
[8]
FOAM parallel run exiting
My command list is

Quote:
decomposePar
mpirun waveFoam -parallel
Is there any difference to using OF231 and OF301 , in terms of using the decomposePar ?
In my system half way across the earth, i could use decomposePar in OF231, however I couldnt use it in OF301 (when i import the exact same case and files over)

Any help would be tremendously appreciated

Last edited by chia87; May 27, 2017 at 13:11. Reason: of231 vs of301
chia87 is offline   Reply With Quote

Old   May 28, 2017, 15:23
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,938
Rep Power: 38
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi,

In fact the error is caused by waveAlpha boundary condition for p_rgh (and the root of the problem is design of waveTheory::New method). Currently it asks for waveProperties in object registry (waveFoam reads this dictionary and puts it into object registry, while decomposePar knows nothing about this dictionary).

So, you have several solutions

1. Remove waveAlpha BC from p_rgh.
2. Remove waveAlpha BC from p_rgh, decompose case, correct Bfs in decomposed case.
3. Correct waveTheory::New method (so it looks up dictionary in the registry first and if it fails, reads the dictionary) submit patch upstream. I.e. this piece of code

Code:
    {
        const dictionary coeffDict_
        (
            (mesh_.thisDb().lookupObject<IOdictionary>("waveProperties"))
           .subDict(subDictName + "Coeffs")
        );

        coeffDict_.lookup("waveType") >> waveTheoryTypeName;
    }
should become something like

Code:
    {
        if (mesh_.thisDb().foundObject<IOdictionary>("waveProperties")
        {
            const dictionary coeffDict
            (
                (mesh_.thisDb().lookupObject<IOdictionary>("waveProperties"))
               .subDict(subDictName + "Coeffs")
            );
            coeffDict.lookup("waveType") >> waveTheoryTypeName;
        }
        else
        {
            const IOdictionary waveDict(
                IOobject(
                    "waveProperties", mesh_.time().constant(), mesh_,
                    IOobject::MUST_READ, IOobject::NO_WRITE, false)
            );
            waveDict.subDict(subDictName + "Coeffs").lookup("waveType") >> waveTheoryTypeName;
        }        
    }
em17 likes this.
alexeym 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
[OpenFOAM.org] compile error in dynamicMesh and thermophysicalModels libraries NickG OpenFOAM Installation 3 December 30, 2019 00:21
[blockMesh] blockMesh with double grading. spwater OpenFOAM Meshing & Mesh Conversion 92 January 12, 2019 09:00
[swak4Foam] GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM Community Contributions 300 October 29, 2014 18:00
OpenFOAM without MPI kokizzu OpenFOAM Installation 4 May 26, 2014 09:17
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51


All times are GMT -4. The time now is 05:11.