search

FloSewn / TQMesh

A simple two-dimensional mesh generator with triangular and quadrilateral elements in C++
MIT License
57 stars 16 forks source link

[Feature request] Exporting to OpenFOAM format #19

Closed OpenFoam-User closed 5 months ago

OpenFoam-User commented 9 months ago

Hello, This is a very nice project.

I wonder if there are plans to support OpenFOAM mesh format? That would be very useful for the OpenFOAM community.

Best regards

FloSewn commented 9 months ago

Hey,

this is definitely something I would like to implement in the near future.

In order to use the current state of the code, you could try exporting the meshes as VTU files and then convert them to the OpenFOAM format using auxiliary tools, such as for example meshio.

Do you think this could work?

Greetings Flo

OpenFoam-User commented 9 months ago

Hi, Thank you for your reply.

Unfortunately, accoding to my experience with meshio (using it for some time), it is unreliable at best. In particular the VTK/VTU et al. formats are very buggy, and in most cases it is not possible to get them to convert to OpenFOAM format properly.

Supporting OpenFOAM in TQMesh, in my opinion, is the right way to achieve this.

Best regards.

FloSewn commented 6 months ago

Hey,

I guess you're right!

Is there any way to test such a grid file if it fits the OpenFOAM format without installing OpenFOAM? This would make things a lot easier... ;-)

Regards, Flo

OpenFoam-User commented 6 months ago

Hey,

I guess you're right!

Is there any way to test such a grid file if it fits the OpenFOAM format without installing OpenFOAM? This would make things a lot easier... ;-)

Regards, Flo

Hi, thank you for your reply.

The easiest way I can think of is to use Paraview to open OpenFOAM meshes. You can download Paraview from the official website: https://www.paraview.org/download/

To open the Mesh, you need the following minimal setup (it doesn't require the 0 and system folders that are typically used by all OpenFOAM simulations):

$ tree .
.
├── constant
│   └── polyMesh
│       ├── boundary
│       ├── cells
│       ├── faces
│       ├── neighbour
│       ├── owner
│       └── points
└── test.foam

You need a folder named constant which contains a subfolder named polyMesh. The later contains the mesh files (boundary, points, faces, ... etc.).

To open the mesh in Paraview, you need to create an empty file with the extension .foam. For example touch test.foam. from Paraview, select File > Open ... to select the .foam file.

FloSewn commented 6 months ago

Hey,

thanks - this helped me a lot!

So I added a small python script which converts a TQMesh text file into the mentioned openFOAM directory structure including the different mesh files.

You can find it here in the "develop" branch.

However, I am not sure if I got the face-orientation and the resulting direction between owner- and neighbor-elements correctly. Would you mind to test the script and check if its output files can be read into openFOAM? At least Paraview seems to be fine with it...

Thank you very much for your help!

Regards, Flo

OpenFoam-User commented 6 months ago

Many thanks for your work.

Here is a link to the documenation about OpenFOAM meshes: https://www.openfoam.com/documentation/user-guide/4-mesh-generation-and-conversion/4.1-mesh-description

Meanwhile, could you please provide some meshes to play with? I am right now on Windows and I don't have TQMesh installed.

Regards

FloSewn commented 6 months ago

Hey there,

here is a sample file, that stems from example 1 (a simple triangular mesh): simple_triangular_mesh.txt

The python script to convert this file as an OpenFOAM mesh should also work on a Windows machine.

In case that it is not possible for you to run the script, here are the respective output-files of that script in a zip-file: simple_triangular_mesh.zip

Thank you very much for your help!

Regards, Flo

FloSewn commented 6 months ago

I just figured that the simple_triangular_mesh example only features triangular elements. For the testing purpose, it would be probably better to check if quad-elements do also work. Here is another converted mesh, which features both element types: fixed_vertices.zip

Greetings Flo

OpenFoam-User commented 5 months ago

Hi. I have played with fixed_vertices.zip. It opens in Paraview but unfortunately has some issues when checked with OpenFOAM. To check the mesh, I have run the OpenFOAM command checkMesh and here are the results:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2312                                  |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : _c39a0f64-20231220 OPENFOAM=2312 version=2312
Arch   : "LSB;label=32;scalar=64"
Exec   : checkMesh
Date   : Mar 18 2024
Time   : 13:36:17
Host   : PC1053
PID    : 2490
I/O    : uncollated
Case   : /mnt/c/Users/user/Desktop/test/tests/fixed_vertices
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = constant

Check mesh...

Time = constant

Mesh stats
    points:           2352
    internal points:  0
    faces:            7430
    internal faces:   3176
    cells:            2085
    faces per cell:   5.08681
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     181
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     1904
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            5   1904

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
 ***Faces not in upper triangular order.
  <<Writing 3176 unordered faces to set upperTriangularFace
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
                   Patch    Faces   Points  Surface topology
              boundary_1       84      168  ok (non-closed singly connected)
              boundary_2     2085     1176  ok (non-closed singly connected)
              boundary_3     2085     1176  ok (non-closed singly connected)
                    ".*"     4254     2352      ok (closed singly connected)

Checking faceZone topology for multiply connected surfaces...
    No faceZones found.

Checking basic cellZone addressing...
    No cellZones found.

Checking basic pointZone addressing...
    No pointZones found.

Checking geometry...
    Overall domain bounding box (0 0 0) (3 3 1)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (-2.13504e-18 0 -5.81691e-16) OK.
    Max cell openness = 1.73184e-16 OK.
    Max aspect ratio = 594.128 OK.
    Minimum face area = 1.06401e-05. Maximum face area = 0.320113.  Face area magnitudes OK.
    Min volume = 3.54668e-06. Max volume = 0.0119652.  Total volume = 2.  Cell volumes OK.
    Mesh non-orthogonality Max: 31.9636 average: 11.8505
    Non-orthogonality check OK.
 ***Error in face pyramids: 4170 faces are incorrectly oriented.
  <<Writing 4170 faces with incorrect orientation to set wrongOrientedFaces
    Max skewness = 2.4877 OK.
    Coupled point location match (average 0) OK.

Failed 2 mesh checks.

End

The command checkMesh will created two files for the two errors under constant/polyMesh/sets which are:

upperTriangularFace
wrongOrientedFaces
FloSewn commented 5 months ago

Hey,

thanks a lot! I guess the faces are not yet oriented correctly. I adjusted the script a little, such that the orientation should now be in accordance to the mesh format you showed me in the link above (at least I hope so...).

Maybe you could try if checkMesh will accept this updated mesh: fixed_vertices.zip

Otherwise, I will probably need to install openFOAM to debug this... ;-)

Anyway, thank you very much for helping!

Greetings Flo

OpenFoam-User commented 5 months ago

Thanks for the update.

Unfortunately, the number of errors now increased to 5 as you can see below:

Check mesh...

Time = constant

Mesh stats
    points:           2352
    internal points:  0
    faces:            7430
    internal faces:   3176
    cells:            2085
    faces per cell:   5.08681
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     181
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     1904
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            5   1904

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
 ***Faces not in upper triangular order.
  <<Writing 3176 unordered faces to set upperTriangularFace
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
                   Patch    Faces   Points  Surface topology
              boundary_1       84      168  ok (non-closed singly connected)
              boundary_2     2085     1176  ok (non-closed singly connected)
              boundary_3     2085     1176  ok (non-closed singly connected)
                    ".*"     4254     2352      ok (closed singly connected)

Checking faceZone topology for multiply connected surfaces...
    No faceZones found.

Checking basic cellZone addressing...
    No cellZones found.

Checking basic pointZone addressing...
    No pointZones found.

Checking geometry...
    Overall domain bounding box (0 0 0) (3 3 1)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (2.13504e-18 0 5.81687e-16) OK.
 ***High aspect ratio cells found, Max aspect ratio: 2.02375e+99, number of cells 2085
  <<Writing 2085 cells with high aspect ratio to set highAspectRatioCells
    Minimum face area = 1.06401e-05. Maximum face area = 0.320113.  Face area magnitudes OK.
 ***Zero or negative cell volume detected.  Minimum negative volume: -0.0119652, Number of negative volume cells: 2085
  <<Writing 2085 zero volume cells to set zeroVolumeCells
    Mesh non-orthogonality Max: 180 average: 168.15
 ***Number of non-orthogonality errors: 3176.
  <<Writing 3176 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 6436 faces are incorrectly oriented.
  <<Writing 3260 faces with incorrect orientation to set wrongOrientedFaces
    Max skewness = 2.4877 OK.
    Coupled point location match (average 0) OK.

Failed 5 mesh checks.

End
FloSewn commented 5 months ago

Thanks! I had to do some minor changes but finally got it working - does checkMesh also proceed for you?

fixed_vertices.zip

It seems to work with most of the meshes from the examples. However, for some examples checkMesh still has some problems. But this could also be related to the meshes...

Anyway, I hope for now the script should work.

Thanks for sharing your idea and for your help! :-)

Cheers Flo

OpenFoam-User commented 5 months ago

Thank you for the update! Indeed the new script fixes the issues with the first mesh. I have also tried it with the second example 02_square_in_channel but got a failing mesh due to some non-closed cells.

Check mesh...

Time = constant

Mesh stats
    points:           6616
    internal points:  0
    faces:            12777
    internal faces:   6161
    cells:            3159
    faces per cell:   5.99494
    boundary patches: 6
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     3147
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     12
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            4   4
            5   8

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
              boundary_1       38       84  ok (non-closed singly connected)
              boundary_2      184      376  ok (non-closed singly connected)
              boundary_3       28       62  ok (non-closed singly connected)
              boundary_4       48      106  ok (non-closed singly connected)
              boundary_5     3159     3308  ok (non-closed singly connected)
              boundary_6     3159     3308  ok (non-closed singly connected)
                    ".*"     6616     6616      ok (closed singly connected)

Checking faceZone topology for multiply connected surfaces...
    No faceZones found.

Checking basic cellZone addressing...
    No cellZones found.

Checking basic pointZone addressing...
    No pointZones found.

Checking geometry...
    Overall domain bounding box (0 0 0) (4 1 1)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (0 -2.91857e-17 -7.47199e-16) OK.
 ***Open cells found, max cell openness: 1, number of open cells 12
  <<Writing 12 non closed cells to set nonClosedCells
    Minimum face area = 1.59115e-05. Maximum face area = 0.0995267.  Face area magnitudes OK.
    Min volume = 2.15574e-05. Max volume = 0.00562089.  Total volume = 3.90993.  Cell volumes OK.
    Mesh non-orthogonality Max: 47.6795 average: 12.1584
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.46892 OK.
    Coupled point location match (average 0) OK.

Failed 1 mesh checks.
FloSewn commented 5 months ago

Thanks! I figured out that these errors are actually attributed to the meshes and not to the conversion script. This will be fixed in the coming release.

Greetings Flo