CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Paraview & paraFoam (http://www.cfd-online.com/Forums/openfoam-paraview/)
-   -   PostProcessing of a tworegion mesh (http://www.cfd-online.com/Forums/openfoam-paraview/61103-postprocessing-tworegion-mesh.html)

cosimobianchini December 15, 2006 07:45

Hi all, I'm working with a
 
Hi all,

I'm working with a Conjugate solver that explicitly passes boundary conditions between solid and fluid interface.
The two meshes are stored in two different directories:

case/constant/region1/polyMesh
case/constant/region2/polyMesh

What I usually do to post-process is:
- convert my result to VTK format with:
foamToVTK . <casename> -mesh region1
foamToVTK . <casename> -mesh region2

- upload data in paraview for the two meshes separately

This method works fine but is a little bit too long.
In fact, as far as boundary data are not stored together with the internalField ones, it means that I have to load data for each boundary patch one by one (for each mesh) to obtain the complete field.
I was just wondering if there was a better (faster and smarter) way of doing it.
Thanks in advance for all your replies.
Cosimo

mattijs December 18, 2006 04:14

There is not really a faster w
 
There is not really a faster way (without changing foamToVTK). The only thing that might help you is the -allPatches option which puts all patches into one file.

Just type foamToVTK without any arguments to see all the options.

cosimobianchini December 18, 2006 04:59

Thank you Mattijs for your sug
 
Thank you Mattijs for your suggestion.
-allPatches option works fine and it helps saving some time but you loose the opportunity of accessing separately to the patches data. It would be interesting expecially for the solid-fluid interface patch.
Anyway thanks a lot again.
Cosimo

gschaider December 18, 2006 05:17

Hi cosimo! I think, there i
 
Hi cosimo!

I think, there is a way, but it would involve heavy symbolic linking (and I havn't tried it):

Basically what you do is create two cases that point to the real data.

Suppose you have your case in aTaleOfTwoMeshes. Create two directories meshCase1, meshCase2. For each directory create these links:

meshCaseX/system -> aTaleOfTwoMeshes/system
meshCaseX/constant/polyMesh -> aTaleOfTwoMeshes/constant/regionX/polyMesh
meshCaseX/0 -> aTaleOfTwoMeshes/0/regionX
(the last has to be done for every time-step)

Now create a stub in one case (touch meshCase2/meshCase2.foam), open the other case from the command line (paraFoam . meshCase1), in that paraFoam open the stub you created from the File->Open-dialog (I think that is possible).

As I said: havn't tried that yet, but from past experience I would say it might work. (If it works one might write a script to automatize all that linking)

Of course you'll have to adjust the time for both data-sources separatly.

gschaider December 18, 2006 16:39

I got around to verify it: It
 
I got around to verify it: It works the way I described it.
For my own entertainment I wrote a script (in Python) that does all the linking:
http://openfoamwiki.net/index.php/Ho...rocMultiregion
(you are welcome to rewrite it in the Scripting-language of your choice)

maría July 30, 2007 14:04

Hi everybody! I have ran a ca
 
Hi everybody!
I have ran a case with two meshes, which are located in:
-case/constant/region1/polyMesh and
-case/constant/region2/polyMesh

I tried to postprocess the results using foamToVTK but a FATAL ERROR apears.
According to cosimo, I did:

- foamToVTK . <casename> -mesh region1
- foamToVTK . <casename> -mesh region2

And the error tells that OpenFoam cannot find the file called "points" in "constant/polyMesh".
The point, is that the file "points" exist but in "constant/region1/polyMesh" and"constant/region2/polyMesh".

What can I do to solve this error??

Thanks in advance.
María.

sradl July 31, 2007 01:04

Dear Maria I know the troub
 
Dear Maria

I know the trouble you are heading in and you will not get lucky with the conversion to VTK files.

May I suggest to use the python script posted by Bernhard in Dec 2006 on the wiki page. You have to install the pyFoam package, but then it is just one more command before "paraFoam . <case>" I can definitely recommend this python-approach and it works without trouble.

br
Stefan Radl

mattijs July 31, 2007 04:04

Hi María, this seems like a
 
Hi María,

this seems like a bug. Can you please report it in the bug-reports section and we'll have a look at it.

maría September 7, 2007 06:53

Hi, Mattijs was right. It
 
Hi,

Mattijs was right. It was just a bug, which has already been checked and now it's working.

See the following section for more details:

OpenFOAM Message Board: OpenFOAM-Bugs: FoamToVTK for cases with two meshes.

Thanks guys!

mabinty October 10, 2008 05:52

dear all!! i run the multiR
 
dear all!!

i run the multiRegionHeater tutorial case in OF 1.5 and would like to display the
results with paraView 3.3.0 dev. the case has 5 regions: left/rightSolid, heater, top/bottomAir where for each a <regionname>_1.vtk file is produced and stored in a VTK folder. i ve no problem to import the region meshes in paraview (file->open) but cannot display any quantity.
the inspector/properties menu of the different regions is empty (blank) so that non of the field variables can be chosen in the inspector/display/color by menu.

i ve no idea whats going wrong here. could anybody give me a hint? i would greatly appreciate any comments!

thx in advance!
aram


All times are GMT -4. The time now is 04:17.