[jmf]

Hi forum

UNV mesh converter succeeds in converting nodes and cells of .unv from SALOME, but fails while building patches of some meshes.

The message is :

Build  : 1.6-53b7f692aa41
Exec   : ideasUnvToFoam mesh.unv
Date   : Sep 09 2009
Time   : 22:26:38
Host   : linux-a6ws
PID    : 5383
Case   : /home/nous/OpenFOAM/nous-1.6/run/run/case
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
 Create time
 Processing tag:2411
Starting reading points at line 3.
Read 4156 points.
 Processing tag:2412
Starting reading cells at line 8318.
First occurrence of element type 11 for cell 1 at line 8319
First occurrence of element type 41 for cell 378 at line 9450
First occurrence of element type 111 for cell 2584 at line 13862
Read 21238 cells and 2206 boundary faces.
 Processing tag:2467
Starting reading patches at line 56340.
For facegroup 0 named outer trying to read 76 patch face indices.
 When reading patches expect Entity Type Code 8
At line 56343
     From function readPatches
    in file ideasUnvToFoam.C at line 464.
 FOAM exiting

Hereafter is an extract of the .unv file. "outer" is the patch name. The failure line 56343 is the last one:

      2052      1936      1962      2063
     23821       111         2         1         7         4
      2236      2220      2461      1745
    -1
    -1
  2467
         0         0         0         0         0         0         0        76
outer
         7       317         0         0         7       318         0         0
         7       319         0         0         7       320         0         0

Any help would be appreciated

Thanks in advance

Jean-Michel

[mattijs]

What is the difference between files that work and those that don't? In the source directory ($FOAM_UTILITIES/mesh/conversion/ideasUnvToFoam/) there is a unv/ subdirectory with some sample files.

[jmf]

Dear Mattijs

Thanks for your advise : I compared sample .unv files with mine and found out that ideasUnvToFoam failure was caused by useless groups of nodes (Entity code = 7 instead of 8)

Everything runs fine now

Best wishes

J-Michel

[druckgott]

How do you have changed this.

In the Unv file or is it posible to change this in salome?

thx

PS because have same problem.
Also starts at 7

[jmf]

Hi Michael

I just deleted all nodes groups in SALOME before exporting to .unv

Best wishes

J-Michel

[druckgott]

How can I do this?
Could you give me a short explanation?

I have just start working with salome
thx

[jmf]

Dear Michael

- activate Mesh module (scroll list or mesh icon)
- develop your mesh tree completely
--> you should find "Group of Nodes" and "Goup of Faces"
- right mouse button on each group of nodes names and delete them

SALOME in line help is quite nice, have a look inside

Otherwise you might try removing in your .unv file all the lines with entity code 7. It may work, I did not try

Best wishes

J-Michel

[druckgott]

ok thx I get it

[mattijs]

Hi,

do you have a sample file that fails? I'll fix it in the converter itself.

[druckgott]

Originally Posted by druckgott

ok thx I get it

Ah thank you it works with the solution of jmf

[jmf]

Hi Mattijs

Please find here enclosed a small .unv file

Jean-Michel

[mattijs]

Thanks. I pushed a fix to 1.6.x so it can read your file and I've added your file as an example to the unv/ subdirectory.

[jonmec]

Hello ...

I tried to convert a .unv mesh using ideasUnvToFoam utility, but I have always the same problem:

" Cannot open file ...

From function ideasUnvToFoam in file ideasUnvToFoam.C at line 585

FOAM exiting"

Please ... I need help!!

Thanks

[mattijs]

You need to supply the complete filename as an argument. This does not sound like a bug so please move this discussion off this OpenFOAM-bugs forum and into e.g. the preprocessing forum.

[jonmec]

Mattijs ... how could I delete my message?

[fede32]

Originally Posted by jmf

Dear Michael

- activate Mesh module (scroll list or mesh icon)
- develop your mesh tree completely
--> you should find "Group of Nodes" and "Goup of Faces"
- right mouse button on each group of nodes names and delete them

SALOME in line help is quite nice, have a look inside

Otherwise you might try removing in your .unv file all the lines with entity code 7. It may work, I did not try

Best wishes

J-Michel

Hi, I'm having the same error. I have not group of nodes. I dont know how to fix it.

[Saleh Abuhanieh]

Hi,


It seems there is a problem in ideasUnvToFoam with foam-Extended fork.


The foam can read the polyMesh folder (it works for me for many cases but not 100% sure) which has been generated using OpenFoam forks.
So, you may use ideasUnvToFoam with OpenFoam then copy the folder.


Saleh