[zaynah04]

stil same things command not found.

[Rophys]

Hi all,

Did anyone solved the problem with the mesh conversion from fluent to OpenFOAM ?

I am getting the same error cited earlier in this thread but seems that nobody solved it, right ? Below follow the error that I got when I tried to convert the mesh:

Any solution for it ?

Thanks

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

Dimension of grid: 3
Number of points: 5643542
Reading points
Number of cells: 5546832
Other readCellGroupData: c 1 54a350 1 0
Reading mixed cells
number of faces: 16736999
Reading mixed faces
Reading mixed faces
Reading uniform faces
Reading mixed faces
Reading mixed faces
Read zone1:12 name:FLUID patchTypeID:fluid
Reading zone data
Read zone1:13 name:int_FLUID patchTypeID:interior
Reading zone data
Read zone1:14 name:INLET:243.254.177 patchTypeID:velocity-inlet
Reading zone data
Read zone1:15 name:SYM:243.254.177 patchTypeID:wall
Reading zone data
Read zone1:16 name:WALL:243.254.177 patchTypeID:wall
Reading zone data
Read zone1:17 name:OUTLET patchTypeIDutlet-vent
Reading zone data


FINISHED LEXING


dimension of grid: 3
Creating shapes for 3-D cells


--> FOAM FATAL ERROR:
Cannot find match for face 1.
Model: hex model face: 4(0 1 5 4) Mesh faces:
6
(
4(5144554 5144555 5144557 5144556)
4(5160836 5160837 5144557 5144556)
4(5144557 5160837 5160835 5144555)
4(5160834 5160836 5144556 5144554)
4(5160835 5160837 5160836 5160834)
4(5144555 5160835 5160834 5144554)
)
Matched points: 8(5144554 -1 -1 5144556 5144555 -1 -1 5144557)

From function create3DCellShape(const label cellIndex, const labelList& faceLabels, const labelListList& faces, const labelList& owner, const labelList& neighbour, const label fluentCellModelID)
in file create3DCellShape.C at line 280.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2
in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
#3
in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
#4 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#5
in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
Aborted (core dumped)

[wyldckat]

Quick answer: This looks to me to have already been answered on this thread. Use fluent3DMeshToFoam for converting meshes that have more than 6 vertices. You can find more details here:

• https://openfoamwiki.net/index.php/F...nt3DMeshToFoam
• https://openfoamwiki.net/index.php/F...am#Limitations

[Rophys]

Thanks Bruno for your response.

I manage to export from fluent to OpenFoam; however, when I check the mesh (command checkMesh), I have 5 failures (see below). In addition, when I initialized the case I received a warning (see below). Anybody knows how to solve this problem?

Thanks.

CheckMesh

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           1463379
    faces:            4298112
    internal faces:   4207320
    cells:            1417572
    faces per cell:   6
    boundary patches: 5
    point zones:      0
    face zones:       1
    cell zones:       1

Overall number of cells of each type:
    hexahedra:     1417572
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
 ****Problem with boundary patch 0 named Inlet of type patch. The patch should start on face no 4207320 and the patch specifies 4229394.
Possibly consecutive patches have this same problem. Suppressing future warnings.
 ***Boundary definition is in error.
    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                  
    Inlet               9945     10132    ok (non-closed singly connected)  
    Sym                 39780    40512    ok (non-closed singly connected)  
    Outlet              7527     7683     ok (non-closed singly connected)  
    Inlet2              11466    11692    ok (non-closed singly connected)  
    Wall                22074    22397    ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-0.3000000142 -3.024070027e-14 -3.241690292e-09) (0.6500000309 0.800000038 0.800000038)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
 ***Boundary openness (1.281722558e-05 0.01952710315 0.01952386798) possible hole in boundary description.
 ***Open cells found, max cell openness: 0.9711407906, number of open cells 4602
  <<Writing 4602 non closed cells to set nonClosedCells
  <<Writing 89739 cells with high aspect ratio to set highAspectRatioCells
    Minimum face area = 3.116805768e-07. Maximum face area = 0.0001277530998.  Face area magnitudes OK.
 ***Zero or negative cell volume detected.  Minimum negative volume: -2.707374999e-08, Number of negative volume cells: 89739
  <<Writing 89739 zero volume cells to set zeroVolumeCells
    Mesh non-orthogonality Max: 179.8440355 average: 35.79636703
 ***Number of non-orthogonality errors: 265395.
  <<Writing 265395 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 538434 faces are incorrectly oriented.
  <<Writing 273039 faces with incorrect orientation to set wrongOrientedFaces
    Max skewness = 1.793962489 OK.
    Coupled point location match (average 0) OK.

Failed 5 mesh checks.

End

Problem during the initialization

--> FOAM Warning : 
    From function List<tetIndices> polyMeshTetDecomposition::faceTetIndices(const polyMesh&, label, label)
    in file meshes/polyMesh/polyMeshTetDecomposition/polyMeshTetDecomposition.C at line 570
    No base point for face 544557, 4(4 192002 192003 6), produces a valid tet decomposition.

[wyldckat]

Greetings Rophys,

It looks like OpenFOAM's converter is not prepared to handle the way that mesh is structured. Even though the mesh is identified as composed only with hexahedral cells, it looks like they were incorrectly identified, since everything seems to be out of order, starting with the patch faces and ending with the way the cells are structured, which result in the "tet decomposition" problems.

Any chance you can provide a small example mesh that demonstrates this exact problem?
And is there any meshing options that you have on your mesher that affects the face/cell orientation? Because it looks like it's inverted somehow...

Best regards,
Bruno

[Rophys]

Hi Bruno,

I am using ICEM to produce the mesh. I guess, it is possible to give a certain orientation to the cells, as you mentioned earlier. I will save the mesh with different orientation and after that i will use the fluent3DToFoam again.

Have you used ICEM ?

Below, I am posting the begging and the ending of the mesh file. If you have any idea in how to fix it, just let me know.

Thanks.

(0 " Created by : Fluent_V6 Interface Vers. 14.0.3")
(2 3)
(0 "Node Section")
(10 (0 1 165453 0 3))
(10 (c 1 165453 1 3)
(
-0.2966559747 0.0898771548 0
-0.2961757546 0.09700568627 0
-0.296520199 0.08987585485 0.002303220235
-0.2960393028 0.09699380518 0.002439532348
-0.2915548178 0.08987218627 0
-0.2910773979 0.09693254987 0
-0.2914210849 0.08987106613 0.002303270841
-0.2909429803 0.0969209887 0.00243821977
-0.286453661 0.08986721774 0
.
.
.
.
.
16252a 162e27 162e62 162565 157840 0
162565 162e62 162e9d 1625a0 15787b 0
1625a0 162e9d 162ed8 1625db 1578b6 0
1625db 162ed8 162f13 162616 1578f1 0
162616 162f13 162f4e 162651 15792c 0
162651 162f4e 162f89 16268c 157967 0
)
)
(0 "Zone Sections")
(39 (13 fluid FLUID)())
(39 (14 interior int_FLUID)())
(39 (15 wall Wall)())
(39 (16 velocity-inlet Inlet)())
(39 (17 wall Sym)())
(39 (18 outlet-vent Outlet)())
(39 (19 velocity-inlet Inlet2)())

[wyldckat]

Hi Rophys,

Originally Posted by Rophys

Have you used ICEM ?

Nope, never used it and I don't have access to it, which is why I'm asking for a small example mesh file that demonstrates the same error.

Originally Posted by Rophys

Below, I am posting the begging and the ending of the mesh file. If you have any idea in how to fix it, just let me know.

Uh... the beginning of the file would only be useful if fluent3DMeshToFoam crashed right at the start. There is nothing else I can do without a complete (preferably small) file I can test with to try and diagnose the problem.

Best regards,
Bruno

[wyldckat]

Hi Rophys,

Since you've sent me the mesh via PM, it made it a lot easier to diagnose what's wrong.
After you import the mesh and run checkMesh, run the following commands:

foamToVTK -cellSet nonClosedCells -poly
foamToVTK -cellSet highAspectRatioCells -poly
foamToVTK -cellSet zeroVolumeCells -poly
foamToVTK -faceSet nonOrthoFaces -poly
foamToVTK -faceSet wrongOrientedFaces -poly

Then open the following files in ParaView:

VTK/highAspectRatioCells_0.vtk
VTK/nonClosedCells_0.vtk
VTK/zeroVolumeCells_0.vtk
VTK/nonOrthoFaces/nonOrthoFaces_0.vtk
VTK/wrongOrientedFaces/wrongOrientedFaces_0.vtk

All of these show us that there is a particular mesh block that was configured completely in reverse, i.e. it's interpreted as negative volume because it's not designed in the same order as all of the other blocks.

Attached is the image that shows the problem block (in grey), which is at the bottom-centre of the mesh. The mesh is the white wire-frame.

As a reminder, the correct way of visual diagnosing meshes in ParaView is explained here: http://openfoamwiki.net/index.php/FA...is_in_ParaView

Best regards,
Bruno

[Rophys]

Hi wyldckat,

Sorry for my later response.

You were right! I fixed the problem and now the mesh looks fine. I didn't have any other problem with negative volumes

Thanks again for your help.

Cheers.