Personal tools
You are here: Home Forum Extension of the platform Exporting a salome mesh to OpenFOAM

Exporting a salome mesh to OpenFOAM

Up to Extension of the platform

Exporting a salome mesh to OpenFOAM

Posted by Nicolas Edh at November 02. 2013

Hi all,

I've made little python script that exports a mesh to OpenFOAM.

It's available here: https://github.com/nicolasedh/salomeToOpenFOAM

I know there already are ways to export a mesh, like the unv-format but that format doesn't support pyramids. This script should handle any type of cell, I've tested pyramids, "wedges", tetrahedrons and hexahedrons. The script doesn't require any additional installation. It runs from inside salome as it is. 

The way to use the script would be to select the mesh you wish to export and the "load script" (ctrl-T) and selection salomeToOpenFOAM.py. I've included a couple of sample scripts in the above link as well. 

Anyways, since I've put some time into the script my hope is that others won't have to. I hope you find it useful.

Best

Nicolas

Re: Exporting a salome mesh to OpenFOAM

Posted by William Tougeron at November 03. 2013

Hello Nicolas, :)

Thank you very much ! :) Very nice initiative :)

Your code looks very nice :)

All the best :)

William

Re: Exporting a salome mesh to OpenFOAM

Posted by Nicolas Edh at November 11. 2013

Hi William,

Thanks for the nice feedback!

Best

Nicolas

 

Re: Exporting a salome mesh to OpenFOAM

Posted by Bernhard Linseisen at January 01. 2014

By now I am using the same script also for batch-mode meshing for testing different meshes for OpenFOAM.

It does run nicely and I will provide you with a full example script as soon as I have solved one or two issues which still exist.

Thanks a lot again, Nicolas, for your script! It arrived just at the right time for my work! :)

Re: Exporting a salome mesh to OpenFOAM

Posted by Bernhard Linseisen at February 10. 2014

Sorry Nicolas, this time I am quicker! ;)

 

A short information for all who want to use the script for MED-meshes: It is possible as well! But at least in my case it required some additional steps:

- Import the MED-file into SMESH

- "Compute" the imported mesh. You will receive some error message(s) about missing hypotheses or algorithm definitions. Just ignore these.

- Remove all groups but the ones for faces

- Within the "Groups of Faces", remove "Group of all Faces"

- Run Nicolas' script and be happy about your new OpenFoam-mesh!

 

Cheers,

Bernhard

 

PS: At some point you might receive errors about a list assignment out of range. In my case that was due to a non-conformal mesh which would have failed in OF anyway...

Re: Exporting a salome mesh to OpenFOAM

Posted by Naveed Saber at November 22. 2014

 I will provide you with a full example script as soon as I have solved one

 

 

Get

Re: Exporting a salome mesh to OpenFOAM

Posted by salvatore at December 20. 2014

Hi Nicolas,

I would like to use your script for my mesh, but when i run it i geti this error:

 

>>> execfile(r"/home/salvo/salomeToOpenFOAM-master/salomeToOpenFOAM.py")

Traceback (most recent call last):

File "<input>", line 1, in <module>

File "/home/salvo/salomeToOpenFOAM-master/salomeToOpenFOAM.py", line 46, in <module>

from salome.smesh import smeshBuilder

ImportError: cannot import name smeshBuilder

>>>

I guess coz i use salome 6.6.0, could u suggest me please how can i solve this problem?

Thank you very much,

salvo

Re: Exporting a salome mesh to OpenFOAM

Posted by Saint Michael at December 21. 2014

Hi Salvo

Reading http://docs.salome-platform.org/latest/gui/SMESH/smesh_migration_page.html lets you know what API changes were made after 6.6.0 and how to convert old scripts.

St.Michael

Re: Exporting a salome mesh to OpenFOAM

Posted by salvatore at January 05. 2015

Hi St.Michael,

thank you very much for your reply. I tried and it works perfectly!

best regards

Salvo

Re: Exporting a salome mesh to OpenFOAM

Posted by Bernhard Linseisen at January 27. 2015

Dear All,

 

While several of us have come to like Nicolas' script, I would like to continue working with OpenFOAM's snappyHexMesh as well. This program requires a list of points and lines contained on the different edges of the geometry within an eMesh-file.

I wonder, if it was possible to modify Nicolas' script in a way as to write this eMesh-file? Unfortunately I do not have the capabilities wrt python programming, so I have to ask: Has anyone of you done such a thing already?
And would that person be kind enough to upload the script somewhere accessible?

Thank you already in advance!

 

Cheers,

Bernhard

Re: Exporting a salome mesh to OpenFOAM

Posted by sheaker at October 24. 2015

Previously salvatore wrote:

Hi St.Michael,

thank you very much for your reply. I tried and it works perfectly!

best regards

Salvo

 

 

Hello Salvo.
Could You share Your modified salomeToOpenFOAM.py script? I can't get through def findSelectedMeshes()


 

Re: Exporting a salome mesh to OpenFOAM

Posted by John Handel Kennedy at February 04. 2016

Hi Nicolas,

 

I tried Meshing a cylinder using Radial Quadrangle 1D2D. However when I exported using the UNV format and later the script you provided,  unused Points error was displayed when checking the Mesh.

 

How do I solve this?

 

Thanks in Advance.

 

 

Re: Exporting a salome mesh to OpenFOAM

Posted by William Tougeron at February 04. 2016

Hello,

If you met the same error using the UNV format and the Nicolas' script, so the mistake should not be during export.

Possible sources of error:

- Only a part of the geometry associated to the mesh was meshed (and standalone nodes stand on vertexes of non-meshed parts of the geometry).

- The mesh was not extruded before export (since OpenFOAM needs 3D meshes even for 2D computations).

- ...

For more specific support, please, share here your study / study dump / geometry, or at least some screenshot(s).

Best regards,

William

Re: Exporting a salome mesh to OpenFOAM

Posted by John Handel Kennedy at February 05. 2016

Hello,

Thank you William, attached is the hdf file for my cylinder. Please look at it and let me know the errors. Thanks again.

 

Regards,

John

Attachments

Re: Exporting a salome mesh to OpenFOAM

Posted by William Tougeron at February 08. 2016

Hello,

Using Salome 7.7.1 on Linux and OpenFOAM 2.3.0, everything works fine for me.

 

 

Here, the output after exporting the mesh in UNV and imported it into OpenFOAM:

user@machine $ ideasUnvToFoam *.unv

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0-f5222ca19ce6
Exec   : ideasUnvToFoam Mesh_1.unv
Date   : Feb 08 2016
Time   : 10:06:23
Host   : "tougeron-prace"
PID    : 13341
Case   : /home/tougeron/documents/home/Desktop/of_test
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Processing tag:164
Starting reading units at line 3.
l:1
units:"  SI: Meter (newton)"
unitType:2
Unit factors:
    Length scale       : 1
    Force scale        : 1
    Temperature scale  : 1
    Temperature offset : 273.15


Processing tag:2420
Skipping tag 2420 on line 9
Skipping section at line 9.

Processing tag:2411
Starting reading points at line 20.
Read 2821 points.

Processing tag:2412
Starting reading cells at line 5665.
First occurrence of element type 11 for cell 1 at line 5666
First occurrence of element type 44 for cell 31 at line 5936
First occurrence of element type 41 for cell 33 at line 5940
First occurrence of element type 115 for cell 1171 at line 8096
First occurrence of element type 112 for cell 1231 at line 8216
Read 2700 cells and 1080 boundary faces.

Processing tag:2467
Starting reading patches at line 13498.
For group 1 named inlet trying to read 90 patch face indices.
For group 2 named outlet trying to read 90 patch face indices.
For group 3 named wall trying to read 900 patch face indices.

Sorting boundary faces according to group (patch)
0: inlet is patch
1: outlet is patch
2: wall is patch

Constructing mesh with non-default patches of size:
    inlet    90
    outlet    90
    wall    900

End


user@machine $ checkMesh 

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0-f5222ca19ce6
Exec   : checkMesh
Date   : Feb 08 2016
Time   : 10:09:20
Host   : "tougeron-prace"
PID    : 14056
Case   : /home/tougeron/documents/home/Desktop/of_test
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           2821
    faces:            8190
    internal faces:   7110
    cells:            2700
    faces per cell:   5.66667
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     1800
    prisms:        900
    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                 
    inlet               90       91       ok (non-closed singly connected) 
    outlet              90       91       ok (non-closed singly connected) 
    wall                900      930      ok (non-closed singly connected) 

Checking geometry...
    Overall domain bounding box (-5 -4.97261 0) (5 4.97261 100)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (2.56326e-18 -2.33391e-17 -3.20007e-17) OK.
    Max cell openness = 5.30175e-16 OK.
    Max aspect ratio = 20.3071 OK.
    Minimum face area = 0.257635. Maximum face area = 5.93849.  Face area magnitudes OK.
    Min volume = 0.860464. Max volume = 5.07388.  Total volume = 7796.69.  Cell volumes OK.
    Mesh non-orthogonality Max: 0.059133 average: 0.0308002
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.31696 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

 

 

 

Here, the output after using the Nicolas' script:

user@machine $ checkMesh

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0-f5222ca19ce6
Exec   : checkMesh
Date   : Feb 08 2016
Time   : 10:09:05
Host   : "tougeron-prace"
PID    : 14027
Case   : /home/tougeron/Mesh_1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           2821
    faces:            8190
    internal faces:   7110
    cells:            2700
    faces per cell:   5.66667
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     1800
    prisms:        900
    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                 
    inlet               90       91       ok (non-closed singly connected) 
    outlet              90       91       ok (non-closed singly connected) 
    wall                900      930      ok (non-closed singly connected) 

Checking geometry...
    Overall domain bounding box (-5 -4.97261 0) (5 4.97261 100)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-2.29344e-18 -1.24284e-17 7.15119e-18) OK.
    Max cell openness = 6.31392e-16 OK.
    Max aspect ratio = 20.3068 OK.
    Minimum face area = 0.257634. Maximum face area = 5.93844.  Face area magnitudes OK.
    Min volume = 0.860452. Max volume = 5.07384.  Total volume = 7796.69.  Cell volumes OK.
    Mesh non-orthogonality Max: 0.0591394 average: 0.0308026
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.316962 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

Best regards,

William

Re: Exporting a salome mesh to OpenFOAM

Posted by John Handel Kennedy at February 09. 2016

Hello William

Thank You for replying.I am getting the unused point error when I use a more refined Mesh. this is the result I get. Please let me know if I can rectify this.

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.4.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.4.0-f0842aea0e77
Exec   : checkMesh
Date   : Feb 08 2016
Time   : 15:48:46
Host   : "Kakas"
PID    : 5628
Case   : /home/student/Desktop/cylinderrefined
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

Time = 0

Mesh stats
    points:           142135
    faces:            162900
    internal faces:   159300
    cells:            54000
    faces per cell:   5.96667
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     52200
    prisms:        1800
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
 ***Unused points found in the mesh, number unused by faces: 87174 number unused by cells: 87174
  <<Writing 87174 unused points to set unusedPoints
    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               900      901      ok (non-closed singly connected) 
    outlet              900      901      ok (non-closed singly connected) 
    wall                1800     1830     ok (non-closed singly connected) 

Checking geometry...
    Overall domain bounding box (-5 -4.97261 0) (5 4.97261 100)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (5.26142e-18 -1.30861e-17 -1.56472e-17) OK.
    Max cell openness = 6.75814e-16 OK.
    Max aspect ratio = 96.1967 OK.
    Minimum face area = 0.00288761. Maximum face area = 1.74219.  Face area magnitudes OK.
    Min volume = 0.00481249. Max volume = 0.283967.  Total volume = 7796.69.  Cell volumes OK.
    Mesh non-orthogonality Max: 0.00380046 average: 0.000741252
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.318768 OK.
    Coupled point location match (average 0) OK.

Failed 1 mesh checks.

End


Regards

John

Attachments

Re: Exporting a salome mesh to OpenFOAM

Posted by William Tougeron at February 09. 2016

Hello,

On my computer, after exporting manually your mesh through UNV or the Nicolas' script, everything is OK.

Overall number of cells of each type:
    hexahedra:     52200
    prisms:        1800
    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).


I have however met this situation recently that Salome works fine on a computer and makes strange things on another, while using the same script, at the step of mesh generation/export.

So far, I have used Salome on several Ubuntu-based distributions (but also on OpenSUSE, a while ago) without problem. I know someone having today troubles to generate meshes for OpenFOAM with Salome on OpenSUSE. What works fine for me does not work for him.

So, please, give your complete configuration and let's wish the developer team to have a look at this issue.

Mine is: Salome 7.7.1 (universal binaries), Linux Mint 13 64bits (with Mate), OpenFOAM 2.3.0

Sorry for not being able to help more...

Best regards,

William

Re: Exporting a salome mesh to OpenFOAM

Posted by John Handel Kennedy at February 09. 2016

Hello William,

Thank you for your prompt response. My configuration is: Salome 7.6.0(universal binaries), Linux Ubuntu 14.04 LTS, OpenFOAM 2.4.0. Do you think my Salome version could be a problem?? Thanks again and hope this will help.

Regards,

John

Re: Exporting a salome mesh to OpenFOAM

Posted by William Tougeron at February 10. 2016

Hello,

I tested now your script with Salome 7.6.0 and the result was the same (checkMesh OK), so the Salome version is not the problem.

Best regards,

Willam

Re: Exporting a salome mesh to OpenFOAM

Posted by John Handel Kennedy at February 10. 2016

Hello,

Then, do you think the Problem is with openFoam or openFoam not installed properly?

 

Regards

John

Re: Exporting a salome mesh to OpenFOAM

Posted by Lucio Gomez at February 12. 2016

Hi all,

First of all, thanks for your script  Nicolas Edh

.

 

I made modification of "SalomeToOpenFoam" script to add a simple graphical interface.  I am an amateur programmer, so I apologize for the thoroughness of the code.
The modificated script is called salomeToOpenFOAM_GUI.py

 

The code it's available here: https://github.com/psicofil/salomeToOpenFOAM

 

 

A YouTube video demonstration: https://www.youtube.com/watch?v=JQbkhz984lM

 

 

Sorry for my bad English.

 

Regards.

 

Re: Exporting a salome mesh to OpenFOAM

Posted by William Tougeron at February 12. 2016

Hi, Lucio,

Very nice!

I didn't know it was possible to launch graphical interfaces from the "Load Script" option!

Very inspiring... :)

(I would have said, nevertheless, that for a better visibility, it would have been maybe better to start a new thread with a link to this one...)

All the best :)

William

Re: Exporting a salome mesh to OpenFOAM

Posted by Kasra Karimi at February 29. 2016

Dear Friends

i have had the same error " Foam::error::printStack(Foam::Ostream&;) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" when i was trying to convert my mesh from Salome to OpenFOAM. i tired many theories and finally i found out the reason was in mesh generating option when you have to select a 3D algorithm. all of those algorithms like (Hexahedron and ...) lead to that error for me but the only one worked OK was 3D Extrusion!

so for others who has the same problem and can change their algorithm, changing it to 3D Extrusion may work for you.

Best

Kasra

Re: Exporting a salome mesh to OpenFOAM

Posted by Ali Ibrahim at July 01. 2017

Dear Nicolas :-

Thank you for your valuable code. When I loaded the script, it run successfully and gives me the following:-

p, li { white-space: pre-wrap; }

Number of nodes: 20770

Number of cells: 31200

Counting number of faces:

total number of faces: 82312, internal: 73688, external 8624

Converting mesh to OpenFOAM

Warning, some elements don't have a group (BC). Adding to a new group called defaultPatches

Finished processing boundary faces

. . . . . . . . . : . . . . . . . . . : . . . . . . . . . : . . . . . . . . . : . . . . Finished processing volumes.

Sorting faces in upper triangular order

Writing the file points

Writing the file faces

Writing the file owner

Writing the file neighbour

Writing the file boundary

Finished writing to /home/ali//home/ali/Mesh_1/constant/polyMesh

Converted mesh in 2s

Wrote mesh in 1s

Total time: 3s

finished exporting

 

 

now, what is the next step to produce polymesh file ?

my best

Hi all,

I've made little python script that exports a mesh to OpenFOAM.

It's available here: https://github.com/nicolasedh/salomeToOpenFOAM

I know there already are ways to export a mesh, like the unv-format but that format doesn't support pyramids. This script should handle any type of cell, I've tested pyramids, "wedges", tetrahedrons and hexahedrons. The script doesn't require any additional installation. It runs from inside salome as it is. 

The way to use the script would be to select the mesh you wish to export and the "load script" (ctrl-T) and selection salomeToOpenFOAM.py. I've included a couple of sample scripts in the above link as well. 

Anyways, since I've put some time into the script my hope is that others won't have to. I hope you find it useful.

Best

Nicolas

 

Re: Exporting a salome mesh to OpenFOAM

Posted by Ali Ibrahim at July 01. 2017

I know the next step is to export the file as .UNV  then executing :-

 ideasUnvToFoam Mesh_1.unv

 

but unfortunately I got:-

Create polyMesh for time = 0

 

Time = 0

 

Mesh stats

    points:           20770

    faces:            82312

    internal faces:   73688

    cells:            31200

    faces per cell:   5

    boundary patches: 1

    point zones:      0

    face zones:       0

    cell zones:       0

 

Overall number of cells of each type:

    hexahedra:     0

    prisms:        31200

    wedges:        0

    pyramids:      0

    tet wedges:    0

    tetrahedra:    0

    polyhedra:     0

 

Checking topology...

    Boundary definition OK.

    Cell to face addressing OK.

 ***Unused points found in the mesh, number unused by faces: 570 number unused by cells: 570

  <<Writing 570 unused points to set unusedPoints

    Upper triangular ordering OK.

    Face vertices OK.

   *Number of regions: 4

    The mesh has multiple regions which are not connected by any face.

  <<Writing region information to "0/cellToRegion"

  <<Writing region 0 with 7800 cells to cellSet region0

  <<Writing region 1 with 7800 cells to cellSet region1

  <<Writing region 2 with 7800 cells to cellSet region2

  <<Writing region 3 with 7800 cells to cellSet region3

 

Checking patch topology for multiply connected surfaces...

    Patch               Faces    Points   Surface topology                 

    defaultPatches      8624     8320     ok (closed singly connected)     

 

Checking geometry...

    Overall domain bounding box (-5.4 -1.45 0) (5.4 41.4 160)

    Mesh (non-empty, non-wedge) directions (1 1 1)

    Mesh (non-empty) directions (1 1 1)

    Boundary openness (-2.02532e-18 -7.59056e-18 -3.0062e-18) OK.

    Max cell openness = 3.2864e-16 OK.

    Max aspect ratio = 15.6609 OK.

    Minimum face area = 0.0457798. Maximum face area = 3.22331.  Face area magnitudes OK.

    Min volume = 0.0732477. Max volume = 2.48227.  Total volume = 23472.9.  Cell volumes OK.

    Mesh non-orthogonality Max: 14.9383 average: 3.34947

    Non-orthogonality check OK.

    Face pyramids OK.

    Max skewness = 0.347155 OK.

    Coupled point location match (average 0) OK.

 

Failed 1 mesh checks.

 

End

 

 

So, may be that is because SALOME has different attitude for different computers as one member highlighted !

I am using SALOME  V8_2_0

Regards

 

Re: Exporting a salome mesh to OpenFOAM

Posted by Ali Ibrahim at July 01. 2017

I think you have messed the original python file of Nicolas. Try to download it again and run it. It should work fine.

 

Re: Exporting a salome mesh to OpenFOAM

Posted by Ali Ibrahim at July 01. 2017

I think you have messed the original python file of Nicolas. Try to download it again and run it. It should work fine.

 

Previously suneel wrote:

Hello everyone,

I am using SALOME version 8.2.0 and the script provided in the above link is not working, please suggest me what modifications I need to do to make this script working. Please see the error message in the attachment.


Thank you in advance

 

Re: Exporting a salome mesh to OpenFOAM

Posted by Ali Ibrahim at July 17. 2017

Previously Nicolas Edh wrote:

Hi all,

I've made little python script that exports a mesh to OpenFOAM.

It's available here: https://github.com/nicolasedh/salomeToOpenFOAM

I know there already are ways to export a mesh, like the unv-format but that format doesn't support pyramids. This script should handle any type of cell, I've tested pyramids, "wedges", tetrahedrons and hexahedrons. The script doesn't require any additional installation. It runs from inside salome as it is. 

The way to use the script would be to select the mesh you wish to export and the "load script" (ctrl-T) and selection salomeToOpenFOAM.py. I've included a couple of sample scripts in the above link as well. 

Anyways, since I've put some time into the script my hope is that others won't have to. I hope you find it useful.

Best

Nicolas

Dear Nicolas:-

Thank you so much for your valuable code. I have NETGEN2D-3D mesh created in Salome 8.2.0 to be exported to openFoam 2.4.0. I export it as .Unv file. When I load your script, Salome shows me the following:-

p, li { white-space: pre-wrap; }

found selected mesh exporting to /home/ali/Mesh_1/constant/polyMesh.

Number of nodes: 3873594

Number of cells: 2816410

Counting number of faces:

total number of faces: 5682885, internal: 5582755, external 100130

Converting mesh to OpenFOAM

Finished processing boundary faces

. . . . . . . . . : . . . . . . . . . : . . . . . . . . . : . . . . . . . . . : . . . . . . . . . Finished processing volumes.

Sorting faces in upper triangular order

Writing the file points

Writing the file faces

Writing the file owner

Writing the file neighbour

Writing the file boundary

Finished writing to /home/ali//home/ali/Mesh_1/constant/polyMesh

Converted mesh in 290s

Wrote mesh in 77s

Total time: 367s

finished exporting

 

 

What is the next step to get the file in its OpenFoam format ? If you tell me export it as .unv file, I would tell you that there is no difference wether or not I run your script!

Thank you again with my best.

 

Re: Exporting a salome mesh to OpenFOAM

Posted by Robert Castilla at July 25. 2017

Hi, I am trying to use this useful script, with Salome-Meca 2016 (Salome 7.8.0) and I get the message that I have to have selected a mesh, even when the mesh is selected.

Best regards

Robert

Powered by Ploneboard
Document Actions