CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)
-   -   [Gmsh] gmshToFoam unhandled element (https://www.cfd-online.com/Forums/openfoam-meshing/78163-gmshtofoam-unhandled-element.html)

flowris July 14, 2010 09:48
gmshToFoam unhandled element
 
Hello,

1. I am trying to convert a gmsh using gmshtoFoam. The .msh-file I use is good, because I see a nice mesh in the gmsh GUI. When I type
gmshToFoam blok01.msh

the console answers (only the lower lines)

Code:
...
Unhandled element 1 at line 430
Unhandled element 1 at line 431
Unhandled element 1 at line 432
Unhandled element 1 at line 433
Unhandled element 1 at line 434
Unhandled element 1 at line 435
Unhandled element 1 at line 436
Unhandled element 1 at line 437
Unhandled element 1 at line 438
Mapping region 0 to Foam patch 0
Cells:
    total:0
    hex  :0
    prism:0
    pyr  :0
    tet  :0



No cells read from file "blok01.msh"
Does your file specify any 3D elements (hex=5, prism=6, pyramid=7, tet=4)?
Perhaps you have not exported the 3D elements?

    From function readCells(..)
    in file gmshToFoam.C at line 662.

FOAM exiting

My blok.msh file is attached.



2. How do I define the patches? I assume I have to make physical surfaces in the .geo file, but this has not been succesfull so far.

KateEisenhower June 25, 2015 09:35
Quote:
Originally Posted by flowris (Post 267250)
Hello,

1. I am trying to convert a gmsh using gmshtoFoam. The .msh-file I use is good, because I see a nice mesh in the gmsh GUI. When I type
gmshToFoam blok01.msh

the console answers (only the lower lines)

Code:
...
Unhandled element 1 at line 430
Unhandled element 1 at line 431
Unhandled element 1 at line 432
Unhandled element 1 at line 433
Unhandled element 1 at line 434
Unhandled element 1 at line 435
Unhandled element 1 at line 436
Unhandled element 1 at line 437
Unhandled element 1 at line 438
Mapping region 0 to Foam patch 0
Cells:
    total:0
    hex  :0
    prism:0
    pyr  :0
    tet  :0



No cells read from file "blok01.msh"
Does your file specify any 3D elements (hex=5, prism=6, pyramid=7, tet=4)?
Perhaps you have not exported the 3D elements?

    From function readCells(..)
    in file gmshToFoam.C at line 662.

FOAM exiting

My blok.msh file is attached.



2. How do I define the patches? I assume I have to make physical surfaces in the .geo file, but this has not been succesfull so far.
Hello,

how did you solve this problem?

Best regards,

Kate

jcharbonneau August 6, 2018 09:13
I fell upon this thread when looking up the error.

I got the same error because I had forgotten to define physical surfaces in the .geo file.

I did not look at your .geo file (can't find it/not attached anymore, new guy on the forum here), but I assume that all surfaces must have a physical name.

This is for someone in the future like me who might get the same error.

wa$$im February 20, 2023 17:31
It's not mandatory to assign a physical surface to each geometrical surface. Non assigned surfaces are converted into "defaultFaces" patch in OpenFoam.

Whereas, you should always take care of creating a physical volume.

Also, surfaces that belong to more than one physical surface ususally generate errors.

wa$$im February 20, 2023 17:50
The error about unhandled elements : 'Unhandled element 1 at line 430 ... ' comes out because gmshToFoam does not support geometrical entities (geometrical points, lines, surfaces, ...). So the error has nothing to do with the quality of the mesh that you see in the GUI, but with how you write the mesh in the .msh-file.

When writing your msh, do not just 'Save Mesh'. Instead, go to Export and pick .msh file format. Then in 'MSH Option' uncheck 'Save all Elements'. And finally Save the mesh.

Preferably, also select the 'Version 2 ASCII' file format.


All times are GMT -4. The time now is 08:00.