CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

Mapping of pointFields with topology changes

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

Like Tree7Likes
  • 1 Post By deepsterblue
  • 1 Post By mturcios777
  • 1 Post By deepsterblue
  • 1 Post By deepsterblue
  • 1 Post By mturcios777
  • 1 Post By mturcios777
  • 1 Post By mm.abdollahzadeh

Reply
 
LinkBack Thread Tools Display Modes
Old   August 29, 2012, 15:17
Default Mapping of pointFields with topology changes
  #1
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
Hello all,

This question is related to the thread Mesh Motion and Refinement in 2.1.x, but since this is more general it might not be found later on by interested parties.

When a mesh undergoes a topology change, the updateFields() function is called for the mesh classes in a way that should map all fields in the object registry. In testing combinations of mesh topology/movement operations, I've found that only volume and surface fields are mapped by default. The following code calls the functions that should do the mapping:

Code:
pointMesh motionUpdate(*this);
motionUpdate.updateMesh(map);
, where *this is a mesh class pointer. However, executing this gives a message such as the following for all pointFields

Code:
Not mapping point<Type>Field <fieldName> since originating mesh differs from that of mapper.
Does anyone know how to properly do this mapping, or if it is even possible in the current 2.1.x release?

Thanks!
mturcios777 is offline   Reply With Quote

Old   August 29, 2012, 16:55
Default
  #2
Senior Member
 
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 386
Rep Power: 15
deepsterblue will become famous soon enough
You shouldn't have to worry about this. Point fields should be mapped automatically in the polyMesh::updateMesh(const mapPolyMesh& mpm) member function. Take a look at polyMeshUpdate.C. The pointMesh should automatically map all related pointFields (see pointMesh.C and the pointMeshMapper for details).
mm.abdollahzadeh likes this.
__________________
Sandeep Menon
University of Massachusetts Amherst
https://github.com/smenon
deepsterblue is offline   Reply With Quote

Old   August 29, 2012, 17:07
Default
  #3
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
Thanks for the reply Sandeep; I assume you are referring to this code snippet:

Code:
// pointMesh
if (thisDb().foundObject<pointMesh>(pointMesh::typeName))
{
     const_cast<pointMesh&>
     (
         thisDb().lookupObject<pointMesh>
         (
             pointMesh::typeName
         )
     ).updateMesh(mpm);
}
which definitely looks like it should do the mapping for pointfields. That is why the message that the pointField isn't being updated so puzzling. Besides not registering the pointField with the objectRegistry (which doesn't make sense as a volScalarField created inside the motionSolver IS mapped automatically), can you think of a reason why the pointMesh wouldn't get mapped? The message says that the mapping is refused as the originating mesh differs from the mapper; I tried placing the pointMesh update after the updateMesh for refinement and it still fails.

I've added the files required to run the case I've been testing it against (I hadn't included a solver; my bad), as well as commented the lines in dynamicMotionSolverRefineFvMesh::refine and unrefine that try to do the mapping. Thanks for the help!
Attached Files
File Type: gz aachenBombMoveRefine.tar.gz (6.1 KB, 13 views)
File Type: gz dynamicMotionSolverRefineFvMesh.tar.gz (9.0 KB, 12 views)
File Type: gz sprayDyMFoam.tar.gz (4.0 KB, 13 views)
hua1015 likes this.
mturcios777 is offline   Reply With Quote

Old   August 29, 2012, 17:20
Default
  #4
Senior Member
 
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 386
Rep Power: 15
deepsterblue will become famous soon enough
It appears that MapGeometricFields does a pointer comparison of the mesh returned by the mapper and the mesh defined for the field. Perhaps you could check through gdb to see which one of the two is inconsistent?

Print out the addresses of both the polyMesh and pointMesh objects, and it should become clear. If there's an inconsistency somewhere, then this is surely a bug - possibly due to a polyMesh reference being returned instead of a pointMesh, or something similar.
hua1015 likes this.
__________________
Sandeep Menon
University of Massachusetts Amherst
https://github.com/smenon
deepsterblue is offline   Reply With Quote

Old   August 29, 2012, 17:30
Default
  #5
Senior Member
 
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 386
Rep Power: 15
deepsterblue will become famous soon enough
Ah.. I get what might be wrong.. You're instantiating a pointMesh within the updateMesh member function within dynamicRefineFvMesh, which destroys itself when the function goes out of scope.

Obviously, any pointField instantiated prior to this call is using a pointMesh registered elsewhere, which is why it doesn't get mapped. You _have_ to use the polyMesh update functionality - there's simple no other way.

Hope this helps.
mm.abdollahzadeh likes this.
__________________
Sandeep Menon
University of Massachusetts Amherst
https://github.com/smenon
deepsterblue is offline   Reply With Quote

Old   August 29, 2012, 17:59
Default
  #6
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
That makes sense; I was attempting the manual method to provide what is seemingly missing from the code. What is odd is that right after the refinement there is a call to updateMesh(map), which following the chain up should end up in the pointField mapping and execute, even if it only returns that "unable to map" message. I think this may be a bug: will post a report with the relevant files and see what happens.

EDIT: Here is the bug report, if anyone finds anything relevant be sure to share it with the developers: http://www.openfoam.org/mantisbt/view.php?id=638
mturcios777 is offline   Reply With Quote

Old   October 26, 2012, 10:02
Default
  #7
Senior Member
 
mahdi abdollahzadeh
Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 149
Rep Power: 6
mm.abdollahzadeh is on a distinguished road
Dear Marco and Sandeep

I am trying to add Mesh refinment to my code using multiDirRefinement.
The code is doing the refinment on newMesh which is at the begining the same as mesh .
then with changemesh the mesh is changed according to newMesh.

Code:
multiDirRefinement multiRef(newMesh, refCells, refineDict);
        polyTopoChange meshMod(newMesh);
       autoPtr<mapPolyMesh> morphMapPtr = meshMod.changeMesh(mesh, false, true);
       const mapPolyMesh& morphMap = morphMapPtr();
But I dont know how to map the feilds which have been calculated on the mesh ( not the newMesh) to the mesh which is changed.

Best
Mahdi
mm.abdollahzadeh is offline   Reply With Quote

Old   October 26, 2012, 12:34
Default
  #8
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
Hello Mahdi,

After calling changemesh, you are returned a mapPolyMesh that needs to be applied to the fields. There should be a member function for your mesh called "updateMesh" that takes as its argument the mapPolyMesh. Have a look at the post earlier up where there is a code snippet for updating the pointmesh. Most meshes that hold data have this member function.
mm.abdollahzadeh likes this.
mturcios777 is offline   Reply With Quote

Old   November 5, 2012, 06:41
Default
  #9
Senior Member
 
mahdi abdollahzadeh
Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 149
Rep Power: 6
mm.abdollahzadeh is on a distinguished road
Dear Marco

Thanks for your answer. I have tried your suggestion.

Code:
multiDirRefinement multiRef(newMesh, refCells, refineDict);
 newMesh.write();
 newMesh.readUpdate();
 polyTopoChange meshMod(newMesh);
 autoPtr<mapPolyMesh> morphMapPtr = meshMod.changeMesh(mesh, false);
 mesh.write();
 const mapPolyMesh& morphMap = morphMapPtr();
//mesh.readUpdate();
mesh.updateMesh(morphMap);
But it gives me a following error :

Code:
#0  Foam::error::printStack(Foam::Ostream&) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::sigFpe::sigFpeHandler(int) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2   in "/lib/libc.so.6"
#3  Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#4  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#5  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#6  __libc_start_main in "/lib/libc.so.6"
#7  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
Floating point exception
Best
Mahdi
mm.abdollahzadeh is offline   Reply With Quote

Old   November 6, 2012, 14:42
Default
  #10
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
Does this happen at the solver step? Check to make sure the fields were actually mapped and then we can see what the problem may be.
mturcios777 is offline   Reply With Quote

Old   November 6, 2012, 18:42
Default
  #11
Senior Member
 
mahdi abdollahzadeh
Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 149
Rep Power: 6
mm.abdollahzadeh is on a distinguished road
Dear Marco

Thanks for the reply.

Yes its exactly happening at the solver step . field are not mapped as you guessed. but the mesh is refined.

Best
Mahdi
mm.abdollahzadeh is offline   Reply With Quote

Old   November 7, 2012, 11:37
Default
  #12
Senior Member
 
mahdi abdollahzadeh
Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 149
Rep Power: 6
mm.abdollahzadeh is on a distinguished road
Quote:
Originally Posted by mturcios777 View Post
Does this happen at the solver step? Check to make sure the fields were actually mapped and then we can see what the problem may be.

Dear Marco

I have changed the position of the refinement and mapping to after the solution of equations.
The data are now mapped. but still there is a problem. I have checked the values for p. some of them are almost NAN and some of them zero. the mapping of the data has problem. and because of that I am receiving the following error.

Code:
#0  Foam::error::printStack(Foam::Ostream&) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::sigFpe::sigFpeHandler(int) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2   in "/lib/libc.so.6"
#3  Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#4  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#5  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#6  __libc_start_main in "/lib/libc.so.6"
#7  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
Floating point exception
Best
Mahdi
mm.abdollahzadeh is offline   Reply With Quote

Old   November 7, 2012, 13:51
Default
  #13
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
If p is nan/0 in locations then there is something wrong with the mapPolyMesh that was created. I seem to recall that when using refinement that some of the fields are reconstructed (like flux and such). Have a look at dynamicRefineFvMesh.C (particularly the refine/unrefine functions) to see what else needs to be done to properly map all the fields.

On that subject, is it only p that is mapped improperly, or are other fields still problematic?

Good luck,
Marco

UPDATE: Its been a while, but the bug reported above has been fixed. Coupled with some changes to the pEqn in the engine solvers, layerAdditionRemoval can now be used! You will need to make a new engineMesh class that has the polyTopoChangers included. This is truly awesome! Still trying to get it to work with dynamicFvMeshes, but there appears to be an issue with the thermophysical properties coupling. More updates on other threads as we go.
wyldckat likes this.

Last edited by mturcios777; November 7, 2012 at 15:04.
mturcios777 is offline   Reply With Quote

Old   November 9, 2012, 08:09
Default
  #14
Senior Member
 
mahdi abdollahzadeh
Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 149
Rep Power: 6
mm.abdollahzadeh is on a distinguished road
Dear Marco

I have checked that the problem is somehow both at p and U. I have doubt as you mention that my map maybe wrong. the mesh modifer that i am using is multiDirRefinment which is using the undoablemeshcutter when doing the refinment on specified direction. the thing is that when doing the refinment with dynamicRefineFvMesh it is using the hexRef8 meshcutter. the diffrence is that the hexRef8 meshcutter will use the poloytopochange (meshmod) as input for mesh refinment. but in the multiDirRefinment it uses the mesh.
because of that i use to equal mesh at the beginging to generate the map. doing the refinment on one and the changing the the other according to poloytopochange of the other and creating the map.

Code:
    multiDirRefinement multiRef(newMesh, refCells, refineDict);
     newMesh.write();
    multiDirRefinement multiRef(newMesh, refCells, refineDict);
     newMesh.write();
     polyTopoChange meshMod(newMesh);
     autoPtr<mapPolyMesh> morphMapPtr = meshMod.changeMesh(mesh,false);
     const mapPolyMesh& morphMap = morphMapPtr();
     mesh.updateMesh(morphMap);  
    mesh.write();
the second point is that I also uses the meshtomesh interpolation between my two different meshes. doing the refinement just on newMesh, interpolate the data to the newMesh from Mesh for storing the values. then doing the refinement on mesh and interpolating the data to mesh using mesh to mesh interpolation. untill here p and U are mapped correctly . but the problem is interpolating the surfacescaler as meshtomesh interpolation cannot handle that. so i try to do construct the phi by interpolating velocities. but it gives a error . infact no data is created for phi !!!

/////////////////
MyIcoFoam

Code:
#include "fvCFD.H"
#include "multiDirRefinement.H" 
#include "undoableMeshCutter.H" 
#include "polyTopoChange.H"
#include "errorEstimate.H"
#include "resError.H"
#include "evaluateError.H"
#include "errorDrivenRefinement.H"
#include "meshToMesh.H"
#include "GeometricField.H"
#include "IOobjectList.H"
#include "mapPolyMesh.H"
#include "polyMesh.H"
#include "dynamicRefineFvMesh.H"
#include "addToRunTimeSelectionTable.H"
#include "surfaceFields.H"
#include "pointFields.H"

static const scalar errTol = 1E-5;
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argc, char *argv[])
{
    #include "setRootCase.H"
    #include "createTime.H"
    #include "createmainMesh.H"
   #include "createNewMesh.H"
 //   #include "createDynamicFvMesh.H"
    #include "createFields.H"
   #include "createFieldsn.H"
    #include "initContinuityErrs.H"
    Info<< "\nStarting time loop\n" << endl;
    
while (runTime.run())
    {

        scalar  realTime=0.0;
        Info<< "Time = " << runTime.timeName() << nl << endl;

        #include "readPISOControls.H"
        #include "CourantNo.H"

if(runTime.write()) 
{
//////////////////////////////////////////////////////////////////////////
///  Error Calculation 

   #include "IcoFoamErrorCalc.H"

/////////////////////////////////////////////////////////////////////////
//////////////////////////////////////////////////////////////////////////
/// Mark Cells For refinment

   #include "Markcellforref.H"

/////////////////////////////////////////////////////////////////////////
//////////////////////////////////////////////////////////////////////////
///  Refinment

 #include "RefinmentwithoutMap.H"
/////////////////////////////////////////////////////////////////////////
//////////////////////////////////////////////////////////////////////////
///  Mapping 
  #include "MaptomeshNew.H"
  #include "MapfromMeshnew.H"
} 

runTime++;

    fvVectorMatrix UEqn
        (
            fvm::ddt(U)
          + fvm::div(phi, U)
          - fvm::laplacian(nu, U)
        );

        solve(UEqn == -fvc::grad(p));

        // --- PISO loop

        for (int corr=0; corr<nCorr; corr++)
        {
            volScalarField rUA = 1.0/UEqn.A();

            U = rUA*UEqn.H();
            phi = (fvc::interpolate(U) & mesh.Sf());
               + fvc::ddtPhiCorr(rUA, U, phi);

            adjustPhi(phi, U, p);

            for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++)
            {
                fvScalarMatrix pEqn
                (
                    fvm::laplacian(rUA, p) == fvc::div(phi)
                );

                pEqn.setReference(pRefCell, pRefValue);
                pEqn.solve();

                if (nonOrth == nNonOrthCorr)
                {
                    phi -= pEqn.flux();
                }
            }
            #include "continuityErrs.H"

            U -= rUA*fvc::grad(p);
            U.correctBoundaryConditions();
        }
runTime.write();

        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
            << nl << endl;
    }

    Info<< "End\n" << endl;

    return 0;
}
////////////////
interpolating from mesh to meshNew
Code:
         

meshToMesh  meshToMeshInterp(mesh, newMesh);
        const fvMesh& meshSource = meshToMeshInterp.fromMesh();
        const fvMesh& meshTarget = meshToMeshInterp.toMesh();
       
        volScalarField pnn
        (
        IOobject
        (
            "pnn",
            runTime.timeName(),
            meshTarget,
            IOobject::READ_IF_PRESENT,
            IOobject::AUTO_WRITE
        ),
        meshTarget,
        dimensionedScalar("zero", dimensionSet(0,2,-2,0,0,0,0), scalar(0.0))
        );


        volVectorField Unn
        (
        IOobject
        (
            "Unn",
            runTime.timeName(),
            meshTarget,
            IOobject::READ_IF_PRESENT,
            IOobject::AUTO_WRITE
        ),
        meshTarget,
        dimensionedVector("zero", dimensionSet(0,1,-1,0,0,0,0), vector::zero)
        );

  // Interpolate field

Info << "***************interpolate from mesh to meshNEw ***********************" << endl;
Info << "***********  interpolate p to pnn ***************" << endl;
       meshToMeshInterp.interpolate(pnn,p,meshToMesh::MAP);

         pnn.write();
Info << "***********  interpolate U to Unn ***************" << endl;
       meshToMeshInterp.interpolate(Unn,U,meshToMesh::MAP);

         Unn.write();
Info << "***********  interpolation Finish***************" << endl;
Info << "***********  mesh change according to meshmod of newMesh***************" << endl;
     polyTopoChange meshMod(newMesh);
     autoPtr<mapPolyMesh> morphMapPtr = meshMod.changeMesh(mesh, false);
     mesh.write();
//////////////////////////
interpolating from meshNew to mesh
Code:
   meshToMesh  meshToMeshInterpb(newMesh, mesh);
    const fvMesh& meshSourceb = meshToMeshInterpb.fromMesh();
    const fvMesh& meshTargetb = meshToMeshInterpb.toMesh();

      GeometricField<scalar, fvPatchField, volMesh> pfieldSourceb
        (
            pnn,
            meshSourceb
        );

    p=dimensionedScalar("zero", dimensionSet(0,2,-2,0,0,0,0), scalar(0.0));
    p.write();

 IOobject fieldTargetIOobjectb
        (
            "p",
            meshTargetb.time().timeName(),
            mesh,
            IOobject::READ_IF_PRESENT,
            IOobject::AUTO_WRITE
        );
            // Read fieldTarget
            GeometricField<scalar, fvPatchField, volMesh> fieldTargetb
            (
                fieldTargetIOobjectb,
                meshTargetb
            ); 

      GeometricField<vector, fvPatchField, volMesh> ufieldSourceb
        (
            Unn,
            meshSourceb
        );

    U=dimensionedVector("zero", dimensionSet(0,1,-1,0,0,0,0), vector::zero);
    U.write();

       IOobject fieldTargetIOobjectub
        (
            "U",
            meshTargetb.time().timeName(),
            meshTargetb,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        );

            // Read fieldTarget
            GeometricField<vector, fvPatchField, volMesh> fieldTargetub
            (
                fieldTargetIOobjectub,
                meshTargetb
            ); 
 Info << "***************interpolate from meshNEw to mesh ***********************" << endl;

// Interpolate field
Info << "***********  interpolate pnn to p ***************" << endl;
           meshToMeshInterpb.interpolate(fieldTargetb,pnn,meshToMesh::MAP);
            fieldTargetb.write();
Info << "***********  interpolate Unn to U ***************" << endl;
           meshToMeshInterpb.interpolate(fieldTargetub,Unn,meshToMesh::MAP);
            fieldTargetub.write();

Info << "***********  interpolate phi on surface ***************" << endl;

       phi=dimensionedScalar("zero", dimensionSet(0,3,-1,0,0,0,0), scalar(0.0));
       phi.write();
       phi=(dimensionedVector("zero", dimensionSet(0,1,-1,0,0,0,0), vector::zero) & mesh.Sf());
       phi.write();
       phi=(fvc::interpolate(U) & mesh.Sf());
       phi.write();

Info << "***********" << endl;
///////////////////////////////
Error
Code:
#0  Foam::error::printStack(Foam::Ostream&) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::sigSegv::sigSegvHandler(int) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2   in "/lib/libc.so.6"
#3  Foam::surfaceInterpolationScheme<Foam::Vector<double> >::interpolate(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > const&) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#4  Foam::surfaceInterpolationScheme<Foam::Vector<double> >::interpolate(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libfiniteVolume.so"
#5  
 at myicoFoam.C:0
#6  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#7  __libc_start_main in "/lib/libc.so.6"
#8  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
Segmentation fault
if i move this part of code (refinment and mapping ) to the end of code after runTime.write() , some value are mapped for phi . the values are wrong and even there is some value for boundaries. the error that this time is occurring is

Code:
Foam::error::printStack(Foam::Ostream&) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::sigFpe::sigFpeHandler(int) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2   in "/lib/libc.so.6"
#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#4  void Foam::divide<Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#5  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#6  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
#7  __libc_start_main in "/lib/libc.so.6"
#8  
 in "/home/mahdi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/myicoFoam"
Floating point exception



I will be thankful if i have your help.

Best
Mahdi
hua1015 likes this.

Last edited by mm.abdollahzadeh; November 9, 2012 at 08:33.
mm.abdollahzadeh is offline   Reply With Quote

Old   November 9, 2012, 11:34
Default
  #15
Senior Member
 
mahdi abdollahzadeh
Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 149
Rep Power: 6
mm.abdollahzadeh is on a distinguished road
Dear Marco

I have also added #include "CorrectFluxinterpolated.H" to my code according to dynamicRefineFvMesh.C . this code is supposed to check and correct the phi while it is mapped.!!!!?
But now just it is correcting the boundary condition and make the value of phi zero. moreover there is still a NAN in one cell surface in phi.

Best
Mahdi
Attached Files
File Type: h CorrectFluxinterpolated.H (3.9 KB, 9 views)
mm.abdollahzadeh is offline   Reply With Quote

Old   May 28, 2015, 21:29
Default
  #16
New Member
 
Su Xiaohui
Join Date: Mar 2009
Location: Singapore
Posts: 29
Rep Power: 8
sxhdhi is on a distinguished road
Send a message via Skype™ to sxhdhi
Dear Mahdi

I've got the same error info as you said when foam does flux update if my guess is correct after UpdateMesh(map).

May I know whether you have fixed the problem or not and how? thanks in advance!

Best Regards

sxh
sxhdhi 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
Cht tutorial in 15 braennstroem OpenFOAM Running, Solving & CFD 197 June 10, 2015 03:02
solid to fluid heattransfer with chtMultiRegionFoam nakor OpenFOAM 11 March 21, 2011 09:28
[ICEM] Building topology command script files Anorky ANSYS Meshing & Geometry 8 January 11, 2010 08:25
ICEM topology Igor-a CFX 0 July 24, 2008 07:05
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19


All times are GMT -4. The time now is 10:49.