[benru]

to Maintainers : ideasUnvToFoam utility has a serious bug - it couldn't correctly read complicated tet mesh, saved as unv-files, generated with Cubit (dont know about used mesh generator), SALOME (Netgen-4.5) and, perhaps, other CAD+meshing programs, and coudn't read grouped surfaces for BC patch from it. Topic was discussed here : http://www.cfd-online.com/OpenFOAM_D...tml?1186384437

Stefan Radl fixed problem of tet mesh reading, we fixed problem of correct reading generated patch for BC, now ideasUnvToFoam can read these big complicated mesh files. What is the way of posting source of new ideasUnvToFoam ?

with a best regards
ruben

[henry]

The best way is to post it hear using the attach command.

[henry]

Take a look at the formatting section of the documentation of the forum software which you will see on the left hand side of your browser window. In there you will see a description of how to attach files.

[benru]

Many Big Thanks, Henry - i was too harried, sorry 8-).

So, archieve with short test is placed here :
ideasUnvCSToFoam.tar.gz
To try and use :
1. It should be unpacked to OF/OF-1.4/applications/utilities/mesh/conversion
2. cd OF/OF-1.4/applications/utilities/mesh/conversion/ideasUnvCSToFoam
and wmake
FoamX will find it, or it would be used from command line.

[benru]

I've checked it on as simple box with groups inlet, outlet & walls, as tet mesh, created with SALOME-3.2.6 & their NETGEN-4.5 plugin, grouped faces for patching.

with a best regards
Ruben

[miwesse]

I have tried ideasUnvCSToFoam for a simple box with ~ 3000 hexaelements a two groups for inlet and outlet. The grid was generated with salome-3.2.6 .I got the following error
...............
................
reading face (faceI==)286;
reading face (faceI==)288;
reading face (faceI==)290;
reading face (faceI==)292;
reading face (faceI==)294;
reading face (faceI==)296;
reading face (faceI==)298;

Sorting boundary faces according to group (patch)


--> FOAM FATAL ERROR : 223 not found in table. Valid entries are 0()

From function HashTable<t,>::operator[](const Key&)
in file /home/miwesse/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/HashTableI.H at line 74.
FOAM exiting

What is the problem?

Michael

[mattijs]

Hi Michael,

does the 1.4.1 ideasUnvToFoam work? It contains some of the fixes from Ruben's version.

If not, can you attach (50K limit) or mail me the file that gives problems?

Mattijs

[miwesse]

Hi Mattijs,

the 1.4.1 ideasUnvToFoam also doesn't work. Therefore I attach .Thank you for your help.

Michael

[miwesse]

Hi Mattijs,

the 1.4.1 ideasUnvToFoam also doesn't work. Therefore I will send you the file(< 50 k) by mail .Thank you for your help.

Michael

[mattijs]

Added cell type 44. Works on your file. Compile under 1.4.1

ideasUnvToFoam.C

[benru]

Thank you, Mattijs. Stefan & i didn't serve problem for hex geom. It would be great to combine advantages both convertors into one.

ruben

[mattijs]

Hi Ruben,

I put in your fix for patch face reading. Can you test this one?

ideasUnvToFoam.C

[miwesse]

Hi Mattijs,

I have tested ideasUnvToFoam and it works wll till now.

Thanks

Michael

[benru]

Thank You, Mattijs, my tet mesh (46M) with BC converted correctly !

With Best Regards,
ruben

[miwesse]

Hi Mattijs,

I have again a problem with ideasUnvToFoam. I ahve now a grid with pentaeders and got the following error:
........
Processing tag:2411
Starting reading points at line 3.
Read 28104 points.

Processing tag:2412
Starting reading cells at line 56214.
--> FOAM Warning :
From function readCells(IFstream&, label&)
in file ideasUnvToFoam.C at line 335
Reading "Pent_Mesh_1.unv" at line 75163
Cell type 112 not supported
Read 0 cells and 19384 boundary faces.

Can you again correct ideasUnvToFoam for this celltype 112 ?

I will send you the example by e-mail.


Thanks
Michael

Hi

I have tried ideasUnvCSToFoam but got error for patchs

v
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : ideasUnvToFoam /home/gui/ test /home/gui/test/simple&wall.unv
Date : Oct 18 2007
Time : 14:21:49
Host : gui-desktop
PID : 19079
Root : /home/gui/
Case : test
Nprocs : 1
Create time

Processing tag:2411
Starting reading points at line 3.
Read 892 points.

Processing tag:2412
Starting reading cells at line 1790.
Read 2746 cells and 1654 boundary faces.

Processing tag:2467
Starting reading patches at line 10971.
For facegroup 0 named stator trying to read 1027 patch face indices.


--> FOAM FATAL IO ERROR : Attempt to get back from bad stream

file: IStringStream.sourceFile at line 0.

From function void Istream::getBack(token& t)
in file db/IOstreams/IOstreams/Istream.C at line 44.

FOAM exiting

someone can help me ?
thanks guillaume

[mattijs]

Does the standard 1.4.1 ideasUnvToFoam work?

[benru]

May be problem with your mesh. Yesterday I got the same error, and it was concerned with non-correct building of complicated mesh with SALOME-NETGEN. I'd generated new mesh (with more number of nodes) - and solved problem.

[benru]

It should be noted, that you need to use ideasUnvToFoam, posted at this topic 21.08.2007 - some problems of standard version (including 1.4.1) were patched there.

thanks
i have changed my mesh,generated new (with less number of nodes) and it work.
i think, like Rubben said ,it was concerned with non-correct building of complicated mesh with SALOME-NETGEN.

best regards
guillaume