[isaacOF]

Hi all,

I'm new to OpenFoam and I would like to learn it because I think it is a "must have" knowledge for an engineer.
I started with a simple geometry in order to understand the flow path inside a rectangular duct with two honeycomb filters inside it.
The mesh of the fluid domain was made with SALOME (v 7.8.0) and imported the .unv file in OpenFoam with the ideasUnvToFoam.
To prepare the simulation I started from the incompressible/pitzDaily tutorial, and applide it to a 3D domain.
However, an error occurred, but I really don't know what it belongs to and how to debug it. You can find attached the log of error.

I really hope in your help!!
many thanks in advantage,
isaacOF

[alexeym]

Hi,

Since the error happens during solution of pressure equation, could you post checkMesh command output?

[isaacOF]

Hi alexeym,

thank you for the answer. Here it is the checkMesh output.

[alexeym]

Does your domain really consist of 63 disjoint parts? I think there is a problem with mesh conversion. Is UNV the only option for mesh export?

[isaacOF]

I guess disjoint parts are mesh parts that are not connected together: how can I avoid them during the mesh creation?
UNV is not the only format, SALOME allows the following ones: DAT, MED, UNV, STL, CGNF, SAUV, GMF.

[alexeym]

Since amount of information about mesh and geometry is rather limited, I guess, the problem happens not during mesh creation but during mesh export/import.

There is https://github.com/nicolasedh/salomeToOpenFOAM, it can help to avoid UNV as intermediate format.

[isaacOF]

It worked fine and the simulation started.
You were right, it was an export/import issue!
However, after a few time steps, the simulation crashes and the following error:

Time = 17

smoothSolver: Solving for Ux, Initial residual = 0.999619, Final residual = 0.0772869, No Iterations 10
smoothSolver: Solving for Uy, Initial residual = 0.999906, Final residual = 0.0994966, No Iterations 9
smoothSolver: Solving for Uz, Initial residual = 0.999473, Final residual = 0.0911458, No Iterations 9
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#5 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<d ouble>&, Foam::Field<double> const&) const at ??:?
#6 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const at ??:?
#7 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#8 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) at ??:?
#9 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#10 Foam::fvMatrix<double>::solve() in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#11 ? in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#12 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#13 ? in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
Floating point exception (core dumped)

How can i manage this?

[alexeym]

Since your mesh has changed, let's start again with checkMesh output.

[isaacOF]

Here it is!

[alexeym]

Here is main points of the output:

Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    300225
    polyhedra:     0

and

    Mesh non-orthogonality Max: 84.9448 average: 19.4851
   *Number of severely non-orthogonal (> 70 degrees) faces: 620.
    Non-orthogonality check OK.
  <<Writing 620 non-orthogonal faces to set nonOrthoFaces

pitzDaily has hexagonal mesh with 5 degree of maximum non-orthogonality, so fvSchemes and fvSolution from this tutorial is not quite applicable to your situation.

So, you have several choices:

0. Go to tutorials folder and search to cases, where nNonOrthogonalCorrectors in SIMPLE sub-dictionary is non-zero (heatTransfer/buoyantBoussinesqSimpleFoam/iglooWithFridges for example).
1. Get yourself new mesh
2. Set nNonOrthogonalCorrectors in fvSolution to, let's say, 2.
3. Change gradSchemes to leastSquares. Or even to cellLimited leastSquares.
4. Use "limited corrected" schemes.
5. Google "OpenFOAM highly non-orthogonal meshes"

[isaacOF]

Thank you Alexey for all these hints. I've tried some of them, but without any success. Surely it depends on my limited knowledge of OpenFOAM
So I decided to strongly simplify the geometrical model by mantaining the main characteristics (shapes, discontinuities, ecc.). Then I made a better mesh and got the incompressible/pitzDaily tutorial settings again: however, the only way I found to carry out the full simulation without any errors is by modifying the following fvSchemes setting:

divSchemes
{
default none;
div(phi,U) bounded Gauss upwind;
div(phi,k) bounded Gauss upwind;
div(phi,epsilon) bounded Gauss upwind;
div(phi,omega) bounded Gauss upwind;
div(phi,v2) bounded Gauss upwind;
div((nuEff*dev2(T(grad(U))))) Gauss linear;
div(nonlinearStress) Gauss linear;
}

I'd like to improve my knowledge of the solver settings, do you know a good documentation (in addition to the official one) where I can find useful information about the relationship between settings and simulation solutions?

Thanks again for your help

[kera]

Originally Posted by isaacOF

I'd like to improve my knowledge of the solver settings, do you know a good documentation (in addition to the official one) where I can find useful information about the relationship between settings and simulation solutions?

have a look at this one Tips and triks in OF

Regards,
Ricky

[isaacOF]

Thank you very much Ricky, it's a very useful document: by following the tricks that it suggests, I could run the whole simulation.
Howeveer, I'm still interested in improving my knowledge of the theory that is behind these settings, do you have any other documentation to suggest?

Thanks in advance!