[emjay]

Hello Community,

I have created a simple tetrahedral mesh and for me it is not possible to convert it to polyhedral mesh. I studied the documentation but I could not find the true configuration.

or, how could I merge the hexahedral elements to a polyhedral element?

fluent3DMeshToFoam test.msh
polyDualMesh 135
combinePatchFaces 75

checkMesh gives me for the imported grid:

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  dev
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : dev-1bbbd40a0d4e
Exec   : checkMesh -time 0
Date   : Mar 09 2022
Time   : 20:44:06
Host   : "ee4e6c8cc759"
PID    : 264
I/O    : uncollated
Case   : /home/openfoam/test
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

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

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           1274
    faces:            12390
    internal faces:   11502
    cells:            5973
    faces per cell:   4
    boundary patches: 1
    point zones:      0
    face zones:       1
    cell zones:       1

Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    5973
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    wall_0              888      446      ok (closed singly connected)      

Checking geometry...
    Overall domain bounding box (-1 -0.866025 -0.5) (1 0.866025 0.5)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (-2.58749e-17 1.42544e-17 3.74953e-17) OK.
    Max cell openness = 2.17769e-16 OK.
    Max aspect ratio = 4.48391 OK.
    Minimum face area = 0.00171147. Maximum face area = 0.0426597.  Face area magnitudes OK.
    Min volume = 4.1545e-05. Max volume = 0.0026691.  Total volume = 2.59808.  Cell volumes OK.
    Mesh non-orthogonality Max: 51.3143 average: 20.0735
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.467139 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

and for the "polyhedral mesh":

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  dev
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : dev-1bbbd40a0d4e
Exec   : checkMesh -time 1
Date   : Mar 09 2022
Time   : 20:44:48
Host   : "ee4e6c8cc759"
PID    : 265
I/O    : uncollated
Case   : /home/openfoam/test
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

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

Create polyMesh for time = 1

Time = 1

Mesh stats
    points:           27327
    faces:            73008
    internal faces:   70344
    cells:            23892
    faces per cell:   6
    boundary patches: 1
    point zones:      0
    face zones:       1
    cell zones:       1

Overall number of cells of each type:
    hexahedra:     23892
    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.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    wall_0              2664     2666     ok (closed singly connected)      

Checking geometry...
    Overall domain bounding box (-1 -0.866025 -0.5) (1 0.866025 0.5)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (8.34735e-17 1.58929e-16 1.57263e-17) OK.
    Max cell openness = 2.42594e-16 OK.
    Max aspect ratio = 4.69317 OK.
    Minimum face area = 0.00020238. Maximum face area = 0.0142199.  Face area magnitudes OK.
    Min volume = 1.03862e-05. Max volume = 0.000667274.  Total volume = 2.59808.  Cell volumes OK.
    Mesh non-orthogonality Max: 59.5439 average: 24.966
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.692838 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

thank you
for your help

[Nikoonz]

Marko, I add to your cause for a little help to solve this problem.
I try polyDualMesh with another basics geometries like cubes and cylinders without good visual results.

About your problem, I used your mesh and the problem is the same as yours: OpenFOAM turns tetrahedral to hexahedral elements.
So, I do the same geometry and mesh in Salome-Meca-2019-0.1, then apply your same steps and the result is different (see attached files)

With different mesher software the results are quite different. Obviously, that is a problem but I'm sure (and I hope) some another user can help us with this issue.

My initial geometry with tetrahedral elements:

Time = 0

Mesh stats
    points:           2431
    faces:            21706
    internal faces:   19058
    cells:            10191
    faces per cell:   4
    boundary patches: 1
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    10191
     polyhedra:     0

My final geometry with polyhedral elements:

Time = 0.005

Mesh stats
    points:           12839
    internal points:  10191
    faces:            15271
    internal faces:   13945
    cells:            2431
    faces per cell:   12.0181
    boundary patches: 1
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     5
    prisms:        6
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     2420

[Nikoonz]

Hey! I found a solution for the polyhedral visualization.
Paraview/Properties/"toogle advanced properties"/(unclick) Decompose polyhedra, "apply" and ready!


Credits: https://discourse.paraview.org/t/dec...in-v5-8-0/4327


Until now I don't have any answer for the unexpected transformation from tetra to hexa doing polyDualMesh with Fluent mesh.

[vinguva]

Originally Posted by Nikoonz

Hey! I found a solution for the polyhedral visualization.
Paraview/Properties/"toogle advanced properties"/(unclick) Decompose polyhedra, "apply" and ready!


Credits: https://discourse.paraview.org/t/dec...in-v5-8-0/4327


Until now I don't have any answer for the unexpected transformation from tetra to hexa doing polyDualMesh with Fluent mesh.

Seems like when using fluent3DMeshToFoam, polyDualMesh converts Tets to Hexas. Use fluentMeshToFoam instead, this seems to convert them from Tets to Polyhedrals.