[gu1]

Anyone can help me to understand this erro:

ERRO LOG:
https://paste.ubuntu.com/24462211/

I used fluent3DMeshToFoam to convert the mesh. I did not get this error.

[Moderator note: added the content of the link below]

@ checkMesh -allTopology -allGeometry


/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 4.1
Exec   : checkMesh -allTopology -allGeometry
Date   : Apr 26 2017
Time   : 15:45:34
Host   : "user"
PID    : xxxx
Case   : /home/user/OpenFOAM/user-4.1/run/Cylinder_3D_RANS
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create polyMesh for time = 0

Enabling all (cell, face, edge, point) topology checks.

Enabling all geometry checks.

Time = 0

Mesh stats
    points:           3292200
    faces:            9690264
    internal faces:   9505584
    cells:            3199308
    faces per cell:   6
    boundary patches: 7
    point zones:      0
    face zones:       1
    cell zones:       1

Overall number of cells of each type:
    hexahedra:     3199308
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Topological cell zip-up check OK.
    Face-face connectivity OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                   Bounding box
    inlet               6713     6900     ok (non-closed singly connected)   (-10 -5 0) (-10 5 5)
    front               65292    65844    ok (non-closed singly connected)   (-10 -5 0) (10 5 0)
    outlet              6713     6900     ok (non-closed singly connected)   (10 -5 0) (10 5 5)
    cylinder            11564    11800    ok (non-closed singly connected)   (-0.499911 -0.499911 0) (0.499911 0.499911 5)
    top                 14553    14900    ok (non-closed singly connected)   (-10 5 0) (10 5 5)
    bottom              14553    14900    ok (non-closed singly connected)   (-10 -5 0) (10 -5 5)
    back                65292    65844    ok (non-closed singly connected)   (-10 -5 5) (10 5 5)

Checking geometry...
    Overall domain bounding box (-10 -5 0) (10 5 5)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (9.94425e-16 9.90732e-15 -6.95517e-15) OK.
    Max cell openness = 5.72257e-16 OK.
    Max aspect ratio = 102.472 OK.
    Minimum face area = 1.33069e-05. Maximum face area = 0.0706106.  Face area magnitudes OK.
    Min volume = 1.35784e-06. Max volume = 0.00720516.  Total volume = 996.074.  Cell volumes OK.
    Mesh non-orthogonality Max: 43.9434 average: 7.50068
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.714944 OK.
    Coupled point location match (average 0) OK.
    Face tets OK.
    Min/max edge length = 0.000998794 0.4362 OK.
    All angles in faces OK.
    Face flatness (1 = flat, 0 = butterfly) : min = 0.999996  average = 1
    All face flatness OK.
    Cell determinant (wellposedness) : minimum: 0.000123873 average: 1.55057
 ***Cells with small determinant (< 0.001) found, number of cells: 1122
  <<Writing 1122 under-determined cells to set underdeterminedCells
    Concave cell check OK.
    Face interpolation weight : minimum: 0.211939 average: 0.494961
    Face interpolation weight check OK.
    Face volume ratio : minimum: 0.269326 average: 0.981702
    Face volume ratio check OK.

Failed 1 mesh checks.

End

[gu1]

Hi,

Anyone can help me to understand this erro?
https://paste.ubuntu.com/24466273/

The checkMesh are 'OK'.

Thanks

[Moderator note: added the content of the link below]

USER@USER:~/OpenFOAM/USER-4.1/run/Cylinder_3D_RANS$ pisoFoam

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 4.1
Exec   : pisoFoam
Date   : Apr 27 2017
Time   : 08:49:13
Host   : "USER"
PID    : 4953
Case   : /home/USER/OpenFOAM/USER-4.1/run/Cylinder_3D_RANS
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0


PISO: Operating solver in PISO mode

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
bounding k, min: 0 max: 9.228e-08 average: 0
bounding omega, min: 0 max: 0.6 average: 0
kOmegaSSTCoeffs
{
    alphaK1         0.85;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.856;
    gamma1          0.555556;
    gamma2          0.44;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    b1              1;
    c1              10;
    F3              false;
}

No MRF models present

No finite volume options present

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:?
#5  Foam::kOmegaSST<Foam::eddyViscosity<Foam::RASModel<Foam::IncompressibleTurbulenceModel<Foam::transportModel> > >, Foam::IncompressibleTurbulenceModel<Foam::transportModel> >::F2() const at ??:?
#6  Foam::kOmegaSST<Foam::eddyViscosity<Foam::RASModel<Foam::IncompressibleTurbulenceModel<Foam::transportModel> > >, Foam::IncompressibleTurbulenceModel<Foam::transportModel> >::F23() const at ??:?
#7  Foam::kOmegaSST<Foam::eddyViscosity<Foam::RASModel<Foam::IncompressibleTurbulenceModel<Foam::transportModel> > >, Foam::IncompressibleTurbulenceModel<Foam::transportModel> >::correctNut() at ??:?
#8  ? at ??:?
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  ? at ??:?

[piu58]

Originally Posted by gu1

Hi,

Anyone can help me to understand this erro?
https://paste.ubuntu.com/24466273/

The checkMesh are 'OK'.

Thanks

The mesh is not the only thing what has to be ok. The boundary conditions are another important point.

[Joshua14]

gu1,

Please post what your boundary conditions are in your 0 folder.

Joshua

[gu1]

Hi,
I solved the problem, did a troubleshoting and understood that thanks to "sigFpe", some of the variables were being divided by zero. It concludes that the internalField for omega was set to zero, so I modified it, solved the problem and started the simulation.

[khedar]

Originally Posted by gu1

Anyone can help me to understand this erro:

ERRO LOG:
https://paste.ubuntu.com/24462211/

I used fluent3DMeshToFoam to convert the mesh. I did not get this error.

Why don't you visualise the cells with low Determinant .. checkMesh created a faceSet out of these faces. Use foamToVTK using faceSet Option and then open the created VTK Files in paraview.

[gu1]

Originally Posted by khedar

Why don't you visualise the cells with low Determinant .. checkMesh created a faceSet out of these faces. Use foamToVTK using faceSet Option and then open the created VTK Files in paraview.

I'm new in OpenFOAM. What are the benefits of doing this?

[khedar]

This allows you to have a look(visually in paraview) at the cells/faces for which checkMesh is reporting an error. With this knowledge, you can proceed further in tracking the problem, which most probably might have come during the mesh creation.

Regards,

khedar