[samiam1000]

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]

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]

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]

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

[samiam1000]

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]

Originally Posted by samiam1000

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

Originally Posted by samiam1000

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"