[Zinedine]

Hi everybody

I have using reconstrucPar and it has been workiong fine until I had the following error:

[menzk@node16 oven3]$ reconstructPar -latestTime
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.1 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.7.1-03e7e056c215
Exec : reconstructPar -latestTime
Date : Nov 16 2011
Time : 16:51:53
Host : node16.beowulf.cluster
PID : 30586
Case : /home/abax2_a/menzk/OpenFOAM/menzk-1.7.1/run/oven3
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
word::stripInvalid() called for word pvsm
For debug level (= 2) > 1 this is considered fatal
Aborted


Has anybody encontered such error ?

Any help is kindly appreciated

Thanks

Z.

[mturcios777]

The stripInvalid function is called when there are invalid characters in a string that need to be removed. Sounds like the word pvsm somehow has an invalid character, and that at the debug level you are running at (2) this is crashing the program. I looked at reconstructPar for OF 2.0.x and can't find the word variable pvsm. Or perhaps pvsm is the word that stripInvalid is being called on, in which case it doesn't make sense why stripInvalid would be called. Can you identify what PVSM is?

[wyldckat]

Greetings to all!

I believe I know what the problem is:

• PVSM is usually a ParaView state file.
• reconstructPar does not know which files were generated by the executed solvers, so it tries to reconstruct whatever is in each "processor*" folder.
• Therefore, one or more ParaView files are contaminating one or more processor folders, simply because OpenFOAM does not use the same file format as ParaView!

Best regards,
Bruno

[Zinedine]

Hi Bruno
What do you suggest then ?
Is there anything I can do to make the utility work or not?
Regards

Z.

[wyldckat]

Hi Zinedine,

Originally Posted by wyldckat

• Therefore, one or more ParaView files are contaminating one or more processor folders, simply because OpenFOAM does not use the same file format as ParaView!

I implied that all you had to do is remove (or move) files created by ParaView that are located in the processor folders!

Best regards,
Bruno

[Zinedine]

Hi Bruno

thanks for your assitance - you were right.
there was some paraview psvm file in the case root directory,.
I moved them and here we go the reconstrcuPar worked fine !

I was wondering if you would know anything about mesh refinement.
I converted a mesh file from ANSYS Fluent to OpenFoam.

The application is for high speed jets applications - it seems that when I
increase the jet velocity (i.e. I am using simpleFoma with k-e turbulence model currently) I do not get any convergence.
Initially Im thought that my settings were not set properly.
Howeever when I undertake the same simjulation by loweirng the kjet velocity to 1m/s - Alleluya ! It works really fine.

I believe that the issue is the mesh is not fione enough to capture the
turbulent scales as higher speeds (i.e. velocity could reached 40m/s !).

I have tried to look into how the refine mesh works but it is not clear.

Would you have any idea of how to refine portion of a mesh please?
Any concrete example and the various to undergo in order to apply it
to my case ?

Thanks for your help.

Regards

Z.

[wyldckat]

Hi Zinedine,

In the tutorials folder run these commands:

find . -name Allrun | xargs grep 'refine' -sl
find . -name refineMeshDict

You can also run the last one on OpenFOAM's folder for more examples.

Those two command lines will tell you which tutorials and example dictionaries are available in OpenFOAM.

Best regards,
Bruno

[Hanzo]

Originally Posted by wyldckat

Hi Zinedine,


I implied that all you had to do is remove (or move) files created by ParaView that are located in the processor folders!

Best regards,
Bruno

Today I encountered the same and I think i figured the reason:

Yesterday, I ran paraFoam and created a pvsm statefile calles state01.pvsm. After I continued to work with paraFoam a file called state01.pvsm; (note the ; ) was created. I only needed to remove this somewhat strange state01.pvsm; file and then it worked fine again. The file was not located in any of my processor* folders but directly in my case directory. So I guess these strange files should not be located anywhere among the folders.

Best,
Hanzo

[ziad]

This happened to me too with decomposePar and OF2.2.x. The *.pvsm; files are created by Paraview by mistake when you save pvsm files with similar file names. As you're creating the new pvsm file with a similar name Paraview lists them in the saving window under a higher hierarchical listing with a ";" character appended to the file extension (pvsm in this case). In my case these are the offending file names:
Slice_withGlyphs_.10s.pvsm
Slice_withGlyphs_.25s.pvsm
Slice_withGlyphs_.50s.pvsm
They were listed under Paraview as Slice_withGlyphs_...s.pvsm. See attached screen capture.

Funny it should happen with decompose/reconstructPar, definitely a bug.

[wyldckat]

Greetings Ziad,

I've tested this with OpenFOAM 2.2.2, 2.2.x, 2.3.0 and 2.3.x and it seems that this bug has already been fixed as of OpenFOAM 2.3.0.

Best regards,
Bruno

[ziad]

Good to know, thanks Bruno

It's also a bug with Paraview since the pvsm; file is created by Paraview not OF. Happens with a local install of Paraview 4.1.0 and its native foam reader, as well as the OF ThirdParty 3.12.0 version and paraFoam.