CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Post-Processing (http://www.cfd-online.com/Forums/openfoam-post-processing/)
-   -   Lack of RAM to visualize a big mesh. How can I do? (http://www.cfd-online.com/Forums/openfoam-post-processing/114984-lack-ram-visualize-big-mesh-how-can-i-do.html)

samiam1000 March 21, 2013 04:33

Lack of RAM to visualize a big mesh. How can I do?
 
Dear All,

I have a big mesh 12.5M cells and I have performed a simulation (using simpleFoam first and then adjointShapeOptimizationFoam).

Everything seems to be ok, until when I try to visualize my data. Because of a lack of memory, paraview crashes.

Is there a way to visualize such a big field of results?

Thanks a lot,
Samuele

akidess March 21, 2013 04:42

Do you really need to see the whole domain? Either just look at a subset without reconstructing, or create some slices beforehand using the sample utility.

samiam1000 March 21, 2013 04:51

Actually, visualizing the whole domain would be the best way. Isn't there a way to see the domain in low-definition?

If this is not possible, I'll use a workaround with sets.

Thanks a lot,
Samuelel

akidess March 21, 2013 05:06

You could indeed make a coarser mesh, and then use mapFields to project your solution on the coarse mesh.

samiam1000 March 21, 2013 05:09

This is a great idea, but just for visualization, at the end.

But I need some calculations, first (e.g. I have to evaluate a certain function on a surface and I can not use a coarse mesh).

Anyway, this is a great advice I'll use for the final visualizations.

Thanks a lot

gschaider March 24, 2013 07:39

Quote:

Originally Posted by samiam1000 (Post 415427)
I have a big mesh 12.5M cells and I have performed a simulation (using simpleFoam first and then adjointShapeOptimizationFoam).

Everything seems to be ok, until when I try to visualize my data. Because of a lack of memory, paraview crashes.

Is there a way to visualize such a big field of results?

Several hints:
- have you tried both readers (the built-in one as well)
- Before clicking the button that actually loads the case have you tried deselecting all fields except one (or even deseleceting all to see if at least the mesh fits into memory)
- the "para" in Paraview stands for "parallel". It's a long time since I done it, but if I remember it correctly you've got to start pvserver (not paraview) in parallel and then start paraview regularly and "Connect" to the pvserver. Google around there are presentations about this

Quote:

Originally Posted by samiam1000 (Post 415437)
This is a great idea, but just for visualization, at the end.

But I need some calculations, first (e.g. I have to evaluate a certain function on a surface and I can not use a coarse mesh).

If the case fits into memory in parallel during solving than the postprocessing-utilities that come with OF can do it. Whether there is a ready-made util depends on your definition of "a surface". Also there is the possibility to do evaluations with funkyDoCalc from the swak-suite (with that "a surface" can be a faceSet, faceZone or a sampled surface)

Anyway: for quantitative analysis I'd prefer an option that is built only on OF to Paraview. Not because paraView is bad, but because it does its own interpolation, triangulation etc. With OF-native solutions (that includes swak) you use the values "as the OpenFOAM-solver saw them"


All times are GMT -4. The time now is 06:53.