[sega]

Hello World.

I was not able to decompose a case which used the timeVaryingMappedFixedValue boundary condition!

Does anybody know if it's possible to use this boundary condition in parallel?

sega

[henrik]

Dear Sebastian,

it should work out of the box. There will be triangulated surfaces on every processor. But that's not something to worry about.

Henrik

[sega]

Thank you Henrik.

But I was not able to do so.
I got a segmentation fault when running the decomposer.
Is there some trick involved?

[sega]

I want to get back to my problem with decomposing a case with timeVaryingMappedFixedValue boundary conditions.

I got this message when running decomposePar

sega@deepblue:~/OpenFOAM/sega-1.5/run/arcSmall0$ decomposePar 
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.5                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Exec   : decomposePar
Date   : Aug 25 2009
Time   : 16:22:49
Host   : deepblue
PID    : 4859
Case   : /home/sega/OpenFOAM/sega-1.5/run/arcSmall0
nProcs : 1

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

Time = 0
Create mesh

Calculating distribution of cells
Selecting decompositionMethod simple

Finished decomposition in 0.03 s

Calculating original mesh data

Distributing cells to processors

Distributing faces to processors

Calculating processor boundary addressing

Distributing points to processors

Constructing processor meshes

Processor 0
    Number of cells = 4000
    Number of faces shared with processor 1 = 200
    Number of processor patches = 1
    Number of processor faces = 200
    Number of boundary faces = 1400

Processor 1
    Number of cells = 4000
    Number of faces shared with processor 0 = 200
    Number of processor patches = 1
    Number of processor faces = 200
    Number of boundary faces = 1400

Number of processor faces = 200
Max number of processor patches = 1
Max number of faces between processors = 200
#0  Foam::error::printStack(Foam::Ostream&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::sigSegv::sigSegvHandler(int) in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  ?? in "/lib/libc.so.6"
#3  vbedg(double, double, int, double*, int, int*, int*, int*, int*, int*, int*) in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libmeshTools.so"
#4  dtris2(int, double*, int*, int*, int*) in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libmeshTools.so"
#5  Foam::triSurfaceTools::delaunay2D(Foam::List<Foam::Vector2D<double> > const&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libmeshTools.so"
#6  Foam::timeVaryingMappedFixedValueFvPatchField<double>::readSamplePoints() in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
#7  Foam::timeVaryingMappedFixedValueFvPatchField<double>::checkTable() in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
#8  Foam::timeVaryingMappedFixedValueFvPatchField<double>::updateCoeffs() in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
#9  Foam::timeVaryingMappedFixedValueFvPatchField<double>::timeVaryingMappedFixedValueFvPatchField(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
#10  Foam::fvPatchField<double>::adddictionaryConstructorToTable<Foam::timeVaryingMappedFixedValueFvPatchField<double> >::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
#11  Foam::fvPatchField<double>::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/decomposePar"
#12  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::GeometricBoundaryField(Foam::fvBoundaryMesh const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/decomposePar"
#13  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readField(Foam::Istream&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/decomposePar"
#14  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/decomposePar"
#15  void Foam::readFields<domainDecomposition, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(domainDecomposition const&, Foam::IOobjectList const&, Foam::PtrList<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >&) in "/home/sega/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/decomposePar"
#16  main in "/home/sega/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/decomposePar"
#17  __libc_start_main in "/lib/libc.so.6"
#18  Foam::fvMesh::readUpdate() in "/home/sega/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/decomposePar"
Segmentation fault

I can't tell whats wrong in this case.
Please feel free to have a look at the case itself: http://therealsega.th.funpic.de/open...cSmall0.tar.gz

If you are talking about triangulation ... Do I have to switch one anything for it to work?!
All I was doing was collecting the necessary data for the boundary condition and setting them like this:

    f0      
    {
        type            timeVaryingMappedFixedValue;
        setAverage    off;
    }

So, where may be the fault?!

[mattijs]

icoFoam does not run with your point set either. Seems your pointset makes the triangulation routine fall over. Set the debug flag timeVaryingMappedFixedValue to 1 in the etc/controlDict. It will output a triangulation.stl which you can load into paraview for checking.

[sega]

Originally Posted by mattijs

icoFoam does not run with your point set either. Seems your pointset makes the triangulation routine fall over. Set the debug flag timeVaryingMappedFixedValue to 1 in the etc/controlDict. It will output a triangulation.stl which you can load into paraview for checking.

I could narrow the problem down and have taken my questions concerning it to an other thread. Have a look:
http://www.cfd-online.com/Forums/ope...ixedvalue.html

(or maybe http://www.cfd-online.com/Forums/ope...tal-error.html)

[Hisham]

Hello Sebastian

I have a Seg Fault (fp) error in running a case in parallel that has a timeVarryingMapped BC that is divided. So I think it may be the cause of the error ... so how is your status on the topic???

Best regards
Hisham

[abhishekgoyal1111]

To anyone who is struggling with this error in decomposePar while using timeVaryingMappedFixedValue, try to make sure that your first three points in the points file do not lie on a straight line because an infinite number of planes can pass through a straight line, so the plane (if) found using these three points will unlikely contain the other points.

I tried this after reading mattijs's comment here: What is DTRIS2 - Fatal error?, and it worked without any other issues.

I think this information might be useful for someone because you don't get this idea directly from the error messages (unless you are an expert in openfoam, of course!).