|
[Sponsors] |
May 21, 2014, 08:01 |
interFoam printStack error
|
#1 |
Member
Reza
Join Date: Feb 2012
Posts: 67
Rep Power: 14 |
Hello Foam'ers
I am working on a simple geometry(attachment). I fill the first part of volume with setField and when I run interFoam, this error appears: [PHP]MULES: Solving for alpha1 Phase-1 volume fraction = 0.0566561 Min(alpha1) = 0 Max(alpha1) = 1 MULES: Solving for alpha1 Phase-1 volume fraction = 0.0549789 Min(alpha1) = 0 Max(alpha1) = 1 #0 Foam::error:rintStack(Foam::Ostream&) in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #2 Uninterpreted: #3 void Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::Field<Foam::Vector<double> >&, Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/lib/libfiniteVolume.so" #4 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::surfaceIntegrate<Foam::Vector<double> >(Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/lib/libfiniteVolume.so" #5 at gaussDivSchemes.C:0 #6 Foam::fv::gaussDivScheme<Foam::Tensor<double> >::fvcDiv(Foam::GeometricField<Foam::Tensor<double >, Foam::fvPatchField, Foam::volMesh> const&) in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/lib/libfiniteVolume.so" #7 Foam::tmp<Foam::GeometricField<Foam::innerProduct< Foam::Vector<double>, Foam::Tensor<double> >::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::div<Foam::Tensor<double> >(Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh> const&) in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/lib/libincompressibleTurbulenceModel.so" #8 Foam::incompressible::laminar::divDevRhoReff(Foam: :GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&) const in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/lib/libincompressibleTurbulenceModel.so" #9 in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/bin/interFoam" #10 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6" #11 in "/home/reza/OpenFOAM/OpenFOAM-2.2.x/platforms/linuxGccDPOpt/bin/interFoam" Floating point exception (core dumped) /PHP] I appreciate any help thanks |
|
May 23, 2014, 07:43 |
|
#2 |
Member
Reza
Join Date: Feb 2012
Posts: 67
Rep Power: 14 |
Hello again,
It works with a simple rectangular cube, but when I add the triangle shape to the geometry (with just changing the blockMeshDict), this error appears. something is wrong with geometry that I cannot understand. I attached the blockmeshDict, which might help. |
|
May 23, 2014, 08:02 |
|
#3 |
Senior Member
|
Hi,
surely it'll be easier for everybody if you show... 1. Your case files (as the error may be in mesh, schemes, solver, boundary conditions, initial conditions, elsewhere). 2. If 1 is not possible for some reason, your checkMesh output in CODE tag. |
|
May 23, 2014, 08:19 |
|
#4 |
Member
Reza
Join Date: Feb 2012
Posts: 67
Rep Power: 14 |
Thank you. I attached the case.
|
|
May 23, 2014, 09:12 |
|
#5 |
Senior Member
|
Well,
I'd say it's rather rude to ignore blockMesh warning Code:
Creating block mesh topology --> FOAM Warning : From function cellModel::mag(const labelList&, const pointField&) in file meshes/meshShapes/cellModel/cellModel.C at line 128 zero or negative pyramid volume: -66666.7 for face 0 --> FOAM Warning : From function cellModel::mag(const labelList&, const pointField&) in file meshes/meshShapes/cellModel/cellModel.C at line 128 zero or negative pyramid volume: -66666.7 for face 1 ... As a result you've got these parameters of the mesh: Code:
Mesh non-orthogonality Max: 180 average: 151.951 ***Number of non-orthogonality errors: 7050. <<Writing 7050 non-orthogonal faces to set nonOrthoFaces Face pyramids OK. ***Max skewness = 6.01549, 3510 highly skew faces detected which may impair the quality of the results <<Writing 3510 skew faces to set skewFaces Coupled point location match (average 0) OK. Failed 2 mesh checks. |
|
June 3, 2014, 07:54 |
|
#6 |
Member
Reza
Join Date: Feb 2012
Posts: 67
Rep Power: 14 |
Thank you. I tried to change the blockMeshDict to correct the mesh generation problem (geometry shape is in first post). I tried the
PHP Code:
last update of mesh is like this: PHP Code:
|
|
June 3, 2014, 08:14 |
|
#7 |
Senior Member
|
Hi,
the code, you've posted, doesn't work at all. So I've decided to look closer at the case you've posted previously. I've modified blocks section the following way: Code:
blocks ( hex (2 6 7 3 0 4 5 1) (30 30 1) simpleGrading (1 1 1) hex (6 10 11 7 4 8 9 5) (30 30 1) simpleGrading (1 1 1) hex (10 14 15 11 8 12 13 9) (30 30 1) simpleGrading (1 1 1) hex (14 18 19 15 12 16 17 13) (30 30 1) simpleGrading (1 1 1) ); Code:
Checking geometry... Overall domain bounding box (0 -7e-05 0) (0.00088 0.00027 5e-06) Mesh (non-empty, non-wedge) directions (1 1 0) Mesh (non-empty) directions (1 1 0) All edges aligned with or perpendicular to non-empty directions. Boundary openness (6.37937e-19 -2.34485e-18 3.95487e-16) OK. Max cell openness = 1.92162e-16 OK. Max aspect ratio = 10.1333 OK. Minimum face area = 6.66667e-12. Maximum face area = 8.88889e-11. Face area magnitudes OK. Min volume = 4.4963e-17. Max volume = 4.44444e-16. Total volume = 9.08e-13. Cell volumes OK. Mesh non-orthogonality Max: 59.4113 average: 28.0489 Non-orthogonality check OK. Face pyramids OK. Max skewness = 3.65102 OK. Coupled point location match (average 0) OK. Not quite sure about high difference in cell sizes between outer and central parts of the mesh but you can start with the mesh you've got and if results should be improved, you can make mesh cell sizes more uniform. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[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 |
c++ libraries and solver compiling | vaina74 | OpenFOAM Installation | 13 | February 3, 2012 17:43 |
OpenFOAM on MinGW crosscompiler hosted on Linux | allenzhao | OpenFOAM Installation | 127 | January 30, 2009 19:08 |
DecomposePar links against liblamso0 with OpenMPI | jens_klostermann | OpenFOAM Bugs | 11 | June 28, 2007 17:51 |