Harpoon to Foam
 

Hi,

we have been testing Harpoon mesh generator to use it with openfoam. It produces a variaty of formats included fluent, gambit, ansys/ideas, etc. but so far we haven't been able to make the conversion. The main problem seems to be that Harpoon producess the binary version of the formats and OpenFoam converters use the Ascii version. Although gambit is ascii but gambitToFoam dies with a segmentation fault. HAs anyone have been able to convert meshes from Harpoon?

On the other hand I read in the forum that someone wrote a translator from netgen to openFoam. Is possible to have access to it?

thanks

manuel

Hi Manuel, Sorry to say th
 

Hi Manuel,

Sorry to say this here, but did you manage to build openFOAM from source for SGI IRIX. If so, a number of members (including me) would appreciate if we can access those binary files or instructions on how to build it for SGI IRIX.

Hi Manuel, I can send you
 

Hi Manuel,

I can send you the netgenNeutralToFoam converter. Just contact me directly at opencfd.co.uk as m.janssens.

Did you have a look at that segmentation fault in a debugger? Can you tell where it goes wrong? Do you have a simple testfile?

Mattijs

My understanding is that Harp
 

My understanding is that Harpoon is a cut-hex mesh generator which can produce arbitrary shaped cells. However, Gambit/Fluent cannot handle arbitrary shaped cells so what happens to the cut cells on the boundary when they are converted into Gambit format? Are they split into prisms and tets? If so that isn't ideal and OpenFOAM can handle the native polyhedra. What formats can Harpoon export?

1) Yes, I did finish compiling
 

1) Yes, I did finish compiling Openfoam on the SGI. That was like a two months task. I wonder how much time took to write the whole thing. I should do a cleaner build from zero to check everything is ok. I was procrastinating this one because I was so anxious of using it after all this time. What shall I do to provide the binary?

Also I did a small test of the parallel performance.
I used icoFoam on a cylinder geometry.
http://www.cs.ualberta.ca/~mgarcia/O...der-vortex.png
The grid has 88000 cells. The computer was a SGI Onix with 24 processors. Openfoam was compiled in 32 bit.
http://www.cs.ualberta.ca/~mgarcia/O...rallelPerf.png
This test is not by any way definitive. It was made to have an idea of OpenFoam parallel performance. If anyone knows about a good test? I can go up to 256 processors in another SGI machine.


2) Thevinitial reason of the thread. I put the gambit file produced by harpoon in
http://www.cs.ualberta.ca/~mgarcia/O...phin.gambit.gz
It is a 782 kBytes file. I tried to get a smaller one but the person who provide it to me wasn't here. I didn't go far with the debugger:


Exec : /compsci/foisy2/cshome/mgarcia/OpenFOAM/OpenFOAM-1.0.2/applications/bin/linuxOpt/gambitToFoam . dolphin Dolphin.gambit
Date : Mar 06 2005
Time : 14:10:27
Host : usona3
PID : 18421
Root : /compsci/foisy2/cshome/mgarcia/OpenFOAM/mgarcia-1.0.2/run/tutorials/icoFoam
Case : wing
Nprocs : 1
Create database


Written by Harpoon v1.4.0(a)Title:
Written by Harpoon v version 1.4.0
(a)
Date Time
NUMNP NELEM NGRPS NBSETS NDCFD NDFVL
30683 32764 1 0 3 3
Reading nodal coordinates

Program received signal SIGSEGV, Segmentation fault.
0x0804d23b in yyFlexLexer::yylex() ()
(gdb) where
#0 0x0804d23b in yyFlexLexer::yylex() ()
#1 0x0804e02d in main ()
#2 0x4097a62d in __libc_start_main () from /lib/libc.so.6
(gdb)

Manuel, if you have the binar
 

Manuel, if you have the binaries I think Mattijs can put up the binaries into the website.

thanks in advance to you and Mattijs.

Hi Manuel, I get a permissi
 

Hi Manuel,

I get a permission denied on all the files in
http://www.cs.ualberta.ca/~mgarcia/OpenFoam/

Mattijs

Harpoon does not create polyh
 

Harpoon does not create polyhedral cells but only hex, tet, pyramd and prism cells, either with or without hanging nodes (there is an option to choose) . As far as I know they do not save the mesh in an own format, but export it to the different formats (star, fluent , cfx, ...). So it is probably the best way to ask the developers of Harpoon for the implementation of the FOAM export.

Given that OpenFOAM supports
 

Given that OpenFOAM supports "hanging-nodes" in the form of correctly connected polyhedra it is probably best to choose this option in Harpoon. However, does Gambit support "hanging-nodes"? If not it would probably be better to use a file-format which does.

I agree it would probbably be best if the developers of Harpoon implement an OpenFOAM export option.

I just fixed the permision of
 

I just fixed the permision of the files. They can now be reached at http://www.cs.ualberta.ca/~mgarcia/OpenFoam/

The format files that harpoon support are:
Ensight, start-CD, CobaltAVVS STL, NAstran, Fluent, CFD++, Gambit, LS-Dyna, Abacus.. however most of them in the binary version. They do mention in the web page support for the FOAM format. However, when we got the evaluation copy, they say that it will be avalilable in future releases

manuel

Hi Manuel, we managed to g
 

Hi Manuel,

we managed to get a bit further with converting your gambit file. The problem is that the header written by Harpoon is not correct or at least not the same as that written by Gambit.

We changed on line 6 the NDCFD to NDFCD and then we get a message about some pointer dereference since there are 0 patches (NBSETS) in your file. Can you try putting all outside faces in patches in Harpoon before writing?

Mattijs

Hi, Manuel, I am also in t
 

Hi, Manuel,

I am also in the same boat as you. I got an evaluation verion last Friday and ran into the same problem you have.

Also, I built a simple part (a cube) using SoildWorks. Name all 6 faces indivisually, such as inlet, outlet, front, back, right, left. And saved it as stl format. It looked like Harpoon did not import the face information. After generating the mesh, I still have not face information for setting up boundary conditions.

Also, Harpoon told me the same thing - it is not clear when they will have the direct export for OpenFOAM.

I like netgen a lot, but, my concern with netgen is that it only meshes with tet elements and not enough control over cell density. I will have to keep looking for a decent mesher with reasonable price.

Please let me know if you solve this Harpoon problem. Thanks!

Pei

Hi Pei, after loading your
 

Hi Pei,

after loading your stl file into Harpoon do a Surface->Separate->by Region to get the surface splitted and then regroup and rename the surfaces as you want.

Do not expect too much from using harpoon. It is fine for some geometries and for a quick shot. But I would not consider using it for serious scientific work.

Jörn

thanks Mattijs for the convers
 

thanks Mattijs for the conversion program. These are the steps I followed:

0. export the file from netgen as neutral file

1. create a new case with foamX: Case Browser -> right click -> Create Case


2. Convert the mesh file to openFoam:

$ netgenNeutralToFoam


For some reason it creates the file in a subdirectory: case/0.005

3. copy the files from case/0.005/polyMesh to case/constant/polyMesh

4. Edit the boundary file and set proper names. That is, change patch by
wall, inlet, etc

5. In FoamX: Edit the field dictionary and save.


I was able to run icoFoam in a very simple case (fichera.geo from the netgen tutorial). However, when I visualize the mesh with paraFoam I notice that there were some elements missing. Although the number of elements is the same as in the neutral file... I put the files at http://www.cs.ualberta.ca/~mgarcia/OpenFoam/fichera.tgz
It may be a netgen related problem.

I also tried to mesh several stl files in netgen but it dies... I wonder how usefull netgen is with stl files...

I will try again with harpoon tonight...

thanks

manuel

Hi Manuel, the problem was
 

Hi Manuel,

the problem was in the converter. Some boundary faces were inside out. I think I fixed the problem in the converter - at least it works for your case.

My experience with netgen is that it requires a perfect stl, so fully closed (all edges connected to two triangles), not self intersecting. Usually if surfaceCheck does not complain it will mesh ok if your mesh resolution is fine enough.

Mattijs

Here is the new netgenNeutralT
 

Here is the new netgenNeutralToFoam.

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif netgenNeutralToFoam.tgz

Hi, manuel, I tried meshing
 

Hi, manuel,

I tried meshing a medium complex geometry (step format) using netgen without any problem. For the same problem with stl format that failed using netgen, can you convert it into step and try netgen again?

pei

Hi Manuel, netgen seems to
 

Hi Manuel,

netgen seems to need perfect surfaces as input: non self-intersecting, every edge connected to two faces. Also you need enough mesh resolution compared to the surface features.

Don't know how good or bad you surface files were. Does surfaceCheck throw up any problem with them?

Mattijs

Hi, Mattijss The netgenNeut
 

Hi, Mattijss

The netgenNeutralToFoam converter seems to be working fine now.

Is there a way to tell the converter to put the files at the constant/polyMesh directory?

manuel

Hi Manuel, glad to hear.
 

Hi Manuel,

glad to hear.

The 1.1 version should put them in the constant directory.

Mattijs