[stootoon]

Hi folks,

I'm running OpenFoam-6 and gmsh 4.0.4 on macOS High Sierra.

My question: Is there a version of gmshToFoam that supports the latest .msh format generated by the latest version of gmsh?

Background:
I've just started learning to mesh with gmsh with the aim of doing some simple simulations in OpenFoam. I followed some simple gmsh tutorials such as https://www.youtube.com/watch?v=C_sCHpLaz3Y and generated some very simple meshes. However whenever I tried to run gmshToFoam, I'd get the following fatal IOError:

--> FOAM FATAL IO ERROR:
wrong token type - expected word, found on line 0 the label 18

I managed to track this down to the format of the .msh file generated by gmsh. The latest version of gmsh (4.0.4) uses a format in which e.g. the size of the $Nodes block is set with two numbers, such as

$Nodes
27 1331
...

whereas the .msh files generated by older versions of gmsh (such as 2.9.3 used in the youtube tutorial above) specify $Nodes as

$Nodes
1331
...

This older .msh format seems to be what the latest version of gmshToFoam is expecting, as I was able to run it successfully on the .msh file generated by the old gmsh version.

Is there a version of gmshToFoam that supports the latest .msh formats?

Thanks for your help,

Sina

[stootoon]

SOLVED: There doesn't appear to be a version of gmshToFoam that supports the new .msh format, but there is an option in the latest gmsh to export to the old .msh format: File > Export > *.msh > Version 2 ASCII.

[openfoamtutorials]

Hi, author of the linked tutorial video here. Thanks for making a post about this! You can also specify the old format (until gmshToFoam is updated) in the command line via "gmsh ... -format msh2". I will be using this in all of my future videos!

[Talder]

Thanks Stootoon,


I ran in exactly the same 'gmshToFoam' FATAL ERROR issue, with a recently build mesh with gmsh 4.0.7. When I regenerated the mesh with an older gmsh 2.10 version, the problem disappeared.



Many thanks for locating this issue !!

[Talder]

In my cases, I found out by just editing the .msh files obtained and adding a line with '$End' just to give it a word it was expecting, made it perfectly happy !!
I could convert any .msh file with this added '$end' line with gmshToFoam into Foam, ParaFoam didn't seem to have any issue.


Hope this helps,
Tom.

[dokeun]

Originally Posted by stootoon

SOLVED: There doesn't appear to be a version of gmshToFoam that supports the new .msh format, but there is an option in the latest gmsh to export to the old .msh format: File > Export > *.msh > Version 2 ASCII.

It's awesome !! Thank you for solving my nettlesome problem.
I converted Gmsh ver2 file successfully and ran the icoFoam from cavity.
But I got an error message from paraview when I load the result.
It tells some problem about discordance of face number and I and stuck there.

The error is as below.

ERROR: In /Users/kitware/dashboards/buildbot-slave/8275bd07/build/superbuild/paraview/src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6876
vtkOpenFOAMReaderPrivate (0x7f9f900ad050): The end face number 309 of patch top is not consistent with the start face number 280 of patch bottom

ERROR: In /Users/kitware/dashboards/buildbot-slave/8275bd07/build/superbuild/paraview/src/VTK/Common/ExecutionModel/vtkExecutive.cxx, line 782
vtkPVCompositeDataPipeline (0x600001d097a0): Algorithm vtkPOpenFOAMReader(0x7f9f90097060) returned failure for request: vtkInformation (0x600027bdbac0)
Debug: Off
Modified Time: 4803293
Reference Count: 1
Registered Events: (none)
Request: REQUEST_DATA
FROM_OUTPUT_PORT: 0
ALGORITHM_AFTER_FORWARD: 1
FORWARD_DIRECTION: 0
----------
and here is my case set.
Does it have relevance to converting stuff?





It was because boundary file
I changed physicalType as below

back
{
type empty;
physicalType empty;
nFaces 100;
startFace 180;
}
bottom
{
type wall;
physicalType wall;
nFaces 10;
startFace 280;
}
right
{
type wall;
physicalType wall;
nFaces 10;
startFace 290;
}
top
{
type zeroGradient;
physicalType zeroGradient;
nFaces 10;
startFace 300;
}
left
{
type wall;
physicalType wall;
nFaces 10;
startFace 310;
}
front
{
type empty;
physicalType empty;
nFaces 100;
startFace 320;
}

from zipped file.

[Abbasi_Maaz]

Originally Posted by Talder

In my cases, I found out by just editing the .msh files obtained and adding a line with '$End' just to give it a word it was expecting, made it perfectly happy !!
I could convert any .msh file with this added '$end' line with gmshToFoam into Foam, ParaFoam didn't seem to have any issue.


Hope this helps,
Tom.

Thank you. It worked for me.

[sourav90]

I dunno why but this is what's happening with two versions of OpenFOAM in macOS Monterey, arm64 M1Pro:

• OpenFOAMv-2106
  
  PHP Code:

  /*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2106                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : _c15bfde3cb-20210624 OPENFOAM=2106
Arch   : "LSB;label=32;scalar=64"
Exec   : gmshToFoam NeighborhoodConnected_MedianRadius5_ROI300_OctreeDepth7Original.msh
Date   : Feb 14 2022
Time   : 14:57:33
Host   : coldandwhite.local
PID    : 41390
I/O    : uncollated
Case   : /Users/massisenergy/OpenFOAM/massisenergy-9/run/TestingGmshToFoam
nProcs : 1
trapFpe: Floating point exception trapping - not supported on this platform
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

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



--> FOAM FATAL IO ERROR: (openfoam-2106)
Wrong token type - expected word, found on line 0: variable "$Entities"

file: input at line 0.

    From Foam::Istream &Foam::operator>>(Foam::Istream &, Foam::word &)
    in file primitives/strings/word/wordIO.C at line 70.

FOAM exiting 

• OpenFOAM-9
  
  PHP Code:

  /*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : 9
Exec   : gmshToFoam NeighborhoodConnected_MedianRadius5_ROI300_OctreeDepth7Original.msh
Date   : Feb 14 2022
Time   : 14:57:44
Host   : "coldandwhite.local"
PID    : 41623
I/O    : uncollated
Case   : /Users/massisenergy/OpenFOAM/massisenergy-9/run/TestingGmshToFoam
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

Skipping tag $end at line 2
Starting to read points at line 6
Vertices to be read:789686
Vertices read:789686

Starting to read cells at line 789695
Cells to be read:4697264

Mapping region 2 to Foam patch 0
Mapping region 2 to Foam cellZone 0
Cells:
    total:4247972
    hex  :0
    prism:0
    pyr  :0
    tet  :4247972

CellZones:
Zone    Size
    0    4247972

Skipping tag $End at line 5486962
Patch 0 gets name patch0

--> FOAM Warning :
    From function Foam::polyMesh::polyMesh(const Foam::IOobject &, Foam::pointField &&, const Foam::cellShapeList &, const Foam::faceListList &, const Foam::wordList &, const Foam::wordList &, const Foam::word &, const Foam::word &, const Foam::wordList &, const bool)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 595
    Found 449292 undefined faces in mesh; adding to default patch.
Finding faces of patch 0

FaceZones:
Zone    Size

Writing zone 0 to cellZone cellZone_0 and cellSet
End 


I could visualise it with paraFoam. So, with version 2 ascii .msh exported from Gmsh, gmshToFoam command is working in OpenFOAM-9 but not with v-2106. Haven't figured out how to specify the boundary conditions yet, but that's the topic of another post!

gmshToFoam.jpg