|
[Sponsors] |
September 18, 2013, 06:02 |
How big is your mesh?
|
#1 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
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 |
|
October 5, 2013, 05:11 |
|
#2 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
Hi Tobi,
Quoting MartinB, from this thread http://www.cfd-online.com/Forums/ope...paraview.html: Quote:
Best regards, Bruno
__________________
|
||
October 6, 2013, 09:41 |
|
#3 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Hi Bruno,
thanks for your link. This thread is making me sad. When I read the "2 seconds" I got very sad 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 ? |
|
October 6, 2013, 10:46 |
|
#4 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
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
__________________
|
|
October 6, 2013, 10:52 |
|
#5 | |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Quote:
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. |
||
October 7, 2013, 10:51 |
|
#6 | |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Dear Bruno,
I mailed with MartinB and he give the following information: Quote:
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. |
||
October 7, 2013, 16:44 |
|
#7 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
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
__________________
|
|
October 8, 2013, 09:13 |
|
#8 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
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 |
|
October 8, 2013, 11:46 |
|
#9 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
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 |
|
October 8, 2013, 17:53 |
|
#10 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
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 |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
sliding mesh problem in CFX | Saima | CFX | 46 | September 11, 2021 07:38 |
[snappyHexMesh] problems generating clean mesh | Christian_tt | OpenFOAM Meshing & Mesh Conversion | 2 | June 20, 2019 05:39 |
[snappyHexMesh] Snappyhex mesh: poor inlet mesh | Swagga5aur | OpenFOAM Meshing & Mesh Conversion | 1 | December 3, 2016 16:59 |
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation | tommymoose | ANSYS Meshing & Geometry | 48 | April 15, 2013 04:24 |
Icemcfd 11: Loss of mesh from surface mesh option? | Joe | CFX | 2 | March 26, 2007 18:10 |