[LutGoe]

Hello guys.

This morning i noticed some weird 'errors' while using ParaView. The same mesh that has been displayed without any Errors the last weeks now looks awfully distorted. After running foamToVTK i am able to look at the results and my mesh.

Any ideas why this happens?

CheckMesh looks fine as well and my Simulations do work properly on the mesh.

I added some Screenshots from paraView, the properly displayed mesh is the VTK Data Set.

I am using ParaView 3.8.0

CheckMesh.txt

Mesh1.jpg

Geo1.jpg

Geo2.jpg

Geo3.jpg

[wyldckat]

Greetings Lutz and welcome to the forum!

I suspect I know what the problem is and I'll quote myself from a bug report I commented on sometime ago: http://www.openfoam.org/mantisbt/view.php?id=746#c1922

In conclusion, this is an end-user situation, because ParaView also has issues with very small objects being represented too far away from the origin of the world referential.

In other words: your geometries from sometime ago were located near the origin, but now they are located somewhere far away from the origin.



... although, I've only now looked at the checkMesh output file and the sizes don't seem to be all that bad or far away from the origin.
On ParaView, in the "Information" tab, what does the "Bounds" group box say about the limits of the mesh? Are they the same as in the checkMesh output?

Overall domain bounding box (-4.541 -10 -1.47447e-14) (5.541 1.78674 1)

Best regards,
Bruno

[LutGoe]

Hi Bruno, thanks a lot for the kind words and even more for your answer.
I have been a long time lurker non-poster until now as i usually found what i needed to improve but didn't feel like i could contribute much by now.

paraView -> Information -> Bounds:

X Range: -4 to 5 (Delta: 9)
Y Range: -10 to 1 (Delta: 11)
Z Range: -9 to 9 (Delta: 18)

These are the outlines of the distorted Mesh displayed in paraView.
The Mesh itself seems to be fine, as OpenFOAM works fine and the results that can be viewed in VTK form are as expected.

The one thing that baffles me the most is that there has no changes been made neither at the Linux i am using nor with any of the Lib.-Files or paraView and still something changed.

So the problem is based on paraView and as it seems that it only affects my user specific installation. There seem to be no errors on another account using the same Data from my case.

I hope that i can solve this, as i am fairly new to both Linux and OpenFoam/paraView and have no ideas how to track down the specific reasons for this.


Best Regards, Lutz.

[wyldckat]

Hi Lutz,

Originally Posted by LutGoe

So the problem is based on paraView and as it seems that it only affects my user specific installation. There seem to be no errors on another account using the same Data from my case.

Ah, OK, then the problem should be ParaView's configuration file that got damaged somehow, possibly in the default camera settings.
The quick fix is to remove the file "ParaView*.ini" at the folder "$HOME/.config/ParaView/", where the "*" relates to the version of the ParaView you've been using.
For example, the following command should delete the configuration file for ParaView 3.12.0:

rm $HOME/.config/ParaView/ParaView3.12.0.ini

Keep in mind to not have ParaView open while performing this command, otherwise the file will simply be saved again upon closure.

Then start ParaView once again and everything should be OK once again.

Best regards,
Bruno

[LutGoe]

Originally Posted by wyldckat

Hi Lutz,


Ah, OK, then the problem should be ParaView's configuration file that got damaged somehow, possibly in the default camera settings.
The quick fix is to remove the file "ParaView*.ini" at the folder "$HOME/.config/ParaView/", [...]

Hi Bruno, thanks for your efforts.

Removing the ParaView.ini did not help fixing the problem. I know somethin has been resetted because the colour schemes i used are the default ones again but the display error still appear.

I am using the VTK data format right now because i can not invest a lot of time in tracking down the error as it is client based and therefore not important for other people working with the data i provide.

Still i am open to try any new ideas on how to fix this.

Thanks a lot for your input so far.

Regards, Lutz.

[wyldckat]

Hi Lutz,

I think now I know what it is. It's possibly a conflict of "." vs ",", namely "1.0" vs "1,0".

Try these commands from within your case folder:

export LC_ALL=C
paraFoam

It's not the first time this has happened: http://www.cfd-online.com/Forums/ope...tml#post433085 - check posts #4 and #5

Best regards,
Bruno

[LutGoe]

Awesome, this works.

Do you have any ideas what the origin of this error is? I don't mind to run the EXPORT command every time, though i wonder why this error actually appears, as nothing has been updated or changed on the computer i use (at least as far as i know).

Thanks for your help so far, i appreciate that a lot.

If you have any further ideas how to track down the error, let me know and i will try to fix it for future questions about this topic.

Regards, Lutz.

[wyldckat]

Hi Lutz,

I guess you didn't read the thread I told you about:

Originally Posted by wyldckat

It's not the first time this has happened: http://www.cfd-online.com/Forums/ope...tml#post433085 - check posts #4 and #5

As Tobi indicated in the thread above, the problem occurred after an update was made to Ubuntu.
My guess is that there was a specific fix for Germany in Ubuntu 13.04, that switched your system language's decimal separator from "." to "," ... apparently because the correct decimal separator in Germany is the comma and not the dot?

Anyway, there are a few ways you can make this permanent and you only need one :

• You can edit the paraFoam script and add the export line right after the big comment header. You can find out where the script is by running:
  

  which paraFoam

• Or you can edit the file "~/.bashrc" and either before or after the source command line for OpenFOAM, you can add the export line.
• Or you can edit the file "~/.bashrc" and add this line:
  

  alias paraFoam='export LC_ALL=C; paraFoam'

Best regards,
Bruno

[LutGoe]

Originally Posted by wyldckat

Hi Lutz,

I guess you didn't read the thread I told you about:

• Or you can edit the file "~/.bashrc" and add this line:
  

  alias paraFoam='export LC_ALL=C; paraFoam'

I guess you are right, i somehow missed that line

Adding the line you posted works fine for the global installation.

Thank you again for the help. I am still learning a lot as i am still very unfamiliar with Ubuntu.

Regards, Lutz.