CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Post-Processing

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

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By gschaider

Reply
 
LinkBack Thread Tools Display Modes
Old   March 21, 2013, 04:33
Default Lack of RAM to visualize a big mesh. How can I do?
  #1
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
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
samiam1000 is offline   Reply With Quote

Old   March 21, 2013, 04:42
Default
  #2
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   March 21, 2013, 04:51
Default
  #3
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
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
samiam1000 is offline   Reply With Quote

Old   March 21, 2013, 05:06
Default
  #4
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
You could indeed make a coarser mesh, and then use mapFields to project your solution on the coarse mesh.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology

Last edited by akidess; March 21, 2013 at 05:07. Reason: Language, spelling
akidess is offline   Reply With Quote

Old   March 21, 2013, 05:09
Default
  #5
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 490
Rep Power: 9
samiam1000 is on a distinguished road
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
samiam1000 is offline   Reply With Quote

Old   March 24, 2013, 07:39
Default
  #6
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by samiam1000 View Post
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 View Post
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"
akidess likes this.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
Add Mesh Layers doesnt work on the whole surface Kryo OpenFOAM Native Meshers: snappyHexMesh and Others 8 September 13, 2012 09:28
Layers:problem with curvature giulio.topazio OpenFOAM Native Meshers: snappyHexMesh and Others 10 August 22, 2012 09:03
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 19:58.