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/)
-   -   How big is your mesh? (http://www.cfd-online.com/Forums/openfoam-paraview/123660-how-big-your-mesh.html)

Tobi September 18, 2013 06:02

How big is your mesh?
 
Hi all,

I have a question to you and that is about the mesh size.
How many cells does the mesh have you load into paraview and is the Performance good?

Maybe you make volume-rendering - how fast is that?

I have a mesh with 1,3 Million cells and the volume Rendering is soooo extrem slow. I tried several things Bruno mentioned but non of them are working.

To be sure if it is a compilation / System Setup mistake that I do or some Settings are wrong, I want to know if someone is doing big analysies with paraview?


Notice: I am always creating a file "paraview.foam" and load that file with paraview.

Thanks in advance
Tobi

wyldckat October 5, 2013 05:11

Hi Tobi,

Quoting MartinB, from this thread http://www.cfd-online.com/Forums/ope...paraview.html:
Quote:

Originally Posted by MartinB (Post 389245)
the attached image is rendered on a NVIDIA Geforce GTX 460 card (several years old by now) and it takes less then 2 seconds for a mesh with 2600000 cells.

But it seems to depend on how good the drivers really are...

Best regards,
Bruno

Tobi October 6, 2013 09:41

Hi Bruno,

thanks for your link.
This thread is making me sad. When I read the "2 seconds" I got very sad :D

My Linux is new installed and the actual driver is on my platform (331).
If I try to render, the GPU utilization is round about 0-5% and it take about 30 seconds to render my geometry (4million cells). I think my GPU is not used for that.

I am using PV binaries 3.12 on ubuntu 12.04.

Its annoying that this will not work on my computer.
Do you know what I can do?

Building PV from Source ? Latest version ?

wyldckat October 6, 2013 10:46

Hi Tobi,

Quote:

Originally Posted by Tobi (Post 455292)
Building PV from Source ? Latest version ?

I honestly don't know :( I've tried the latest ParaView on my machine, as well as building ParaView 3.12 from source code on my machine and neither resulted in having an unstructured mesh with fast volume rendering.

As I've written on another thread for you: http://www.cfd-online.com/Forums/par...tml#post455168 - I was only able to do really fast volume renders when the mesh is structured or comes from an image based representation, which I haven't been able to recreate myself :(

As I also wrote on that thread, try the examples on those structured ParaView data files, to confirm if they are blazing fast as well.


By the way, what graphics card are you using? And have you tried using ParaView on Windows, with the dedicated drivers installed as well? The ".foam" file extension can be used for opening OpenFOAM cases.

Best regards,
Bruno

Tobi October 6, 2013 10:52

Quote:

Originally Posted by wyldckat (Post 455307)
Hi Tobi,


I honestly don't know :( I've tried the latest ParaView on my machine, as well as building ParaView 3.12 from source code on my machine and neither resulted in having an unstructured mesh with fast volume rendering.

As I've written on another thread for you: http://www.cfd-online.com/Forums/par...tml#post455168 - I was only able to do really fast volume renders when the mesh is structured or comes from an image based representation, which I haven't been able to recreate myself :(

As I also wrote on that thread, try the examples on those structured ParaView data files, to confirm if they are blazing fast as well.


By the way, what graphics card are you using? And have you tried using ParaView on Windows, with the dedicated drivers installed as well? The ".foam" file extension can be used for opening OpenFOAM cases.

Best regards,
Bruno

Hi Bruno,

hmm ... okay so its possible that MarinB just had a hexaeder mesh.
Hmmm ... :/ thats not good.

Well but my meshes always build on sHM - so its hexadominant ... okay but I know what you mean.

My card is: Nvidia GeForce 560 GTX

As I told, my gpu utilization is just round about 0-5%....

Not tested paraview on my windows OS - i will do that - thanks for that hint.

To use the attribute --date=... is like paraview paraview.foam. With MPI on 8 cores pv will close and give the same error as above.

Tobi October 7, 2013 10:51

Dear Bruno,

I mailed with MartinB and he give the following information:
Quote:

Hallo Tobias,

das Netz war ein unstrukturiertes, hybrides Netz aus Tetraedern und Boundary-Layern (Prismen), sowie ca. 10% extrudierte Hexaeder-Zellen.

Die ParaView-Version war (bzw. ist, das System ist immer noch im Einsatz) die Standard-Paraview-Version 3.12 aus dem ThirdParty-Verzeichnis, wobei ich Python aktiviert, sonst aber keine Modifikationen vorgenommen habe.
Die OpenFOAM-Versionen sind mit "-O3" und "-march=native" Flags kompiliert, aber ich vermute, dass diese Flags nicht für die ParaView-Kompilierung verwendet werden.
1. He uses the PV in the ThirdPartys
2. His mesh is hybrid with tets and prisma (boundary layer) + 10 percent hex cells
3. He uses OpenSUSE - is that the reason why it do not work?
4. He uses the NVIDIA driver on the nvidia website.
5. he compiled PV with python enable

After all he mentioned that MPI is not good for a single machine.

wyldckat October 7, 2013 16:44

Hi Tobi,

Thanks for sharing this information!

Well, using openSUSE might help a bit. It's a bit of a known fact that Ubuntu can pick a fight with ParaView, if it has got the 3D animations turned on as well. And I haven't heard/read any problems like that on openSUSE, at least not lately.

I've got a machine with openSUSE 12.1 at the office, with a good NVidia card. I'll try to find some time this week to try it out.

Best regards,
Bruno

Tobi October 8, 2013 09:13

Hi Bruno,


well I switched to OpenSUSE to check this phenomena too.

Nothing changed:

- Rendering 26s
- Rotation 17s

:(

PV-3.12.0 with ThirdPartys (without python)
Gcc 4.7.2

Tobi October 8, 2013 11:46

Hi all (especially Bruno):

I had a talk to Mr. MartinB and he mentioned that my mesh (~5.000.000 cells) could be the problem (-> polyedras ~ 500.000). He said that it could be that I have to render a mesh with round about 15.000.000 cells caused by the splitting of polycells into tets.

He will test my case now and give me a feedback.
After that I give you a feedback.

Regards
Tobi

Tobi October 8, 2013 17:53

Hi all,

MartinB tested my test case and he got the following result:

- first volume rendering: 56s (compared with mine 26s)

He give me some good information due to the problem.
My mesh has the following cells included:

Code:

> Overall number of cells of each type:
 >    hexahedra:    4427938
 >    prisms:        424356
 >    wedges:        0
 >    pyramids:      0
 >    tet wedges:    274
 >    tetrahedra:    0
 >    polyhedra:    432535


Round about 5.000.000 cells. If you render PV triangulates your polyhedra cells and that is the reason why my rendering speed is so low. Its not caused by wrong or bad graphic card drivers. Its caused by the fact, that all polyhedra cells have to be triangulated (maybe the other cell types too).

At least he gave me the following hint:


Code:


dein  Netz ist nach der Triangulierung in ParaView 10380568 Tetraeder-Zellen  groß (Information Tab im Object Inspector von paraFoam).


This means that after triangulation my mesh has 10.380.568 tet cells :)
Thats the reason why my CPU is always used 100%.

Now I will try to set up pvserver with 4 cores to speed up the triangulation.

Thanks to MartinB for the clearification :)


Regards Tobi


All times are GMT -4. The time now is 11:13.