CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Paraview & paraFoam

Cannot track LAgrangian particles

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

Like Tree2Likes
  • 2 Post By Eranho

Reply
 
LinkBack Thread Tools Display Modes
Old   September 26, 2014, 06:19
Default Cannot track LAgrangian particles
  #1
New Member
 
Na
Join Date: Sep 2014
Posts: 5
Rep Power: 2
Eranho is on a distinguished road
Hello

I have a problem to visualize Lagrangian particles at aachenBomb tutorial. The case executes correctly and I can see temperature and pressure field etc. When I run the 'foamToVTK' it makes the VTK directory.

But when I open the Paraview and open the files at VTK directory according this tutorial (page 8):
http://www.tfd.chalmers.se/~hani/kur...ered_NL_HN.pdf

and when I try to create glyphs for claud and press 'apply', the Paraview crashes down every time. Is this a known problem or do I do something wrong?

I'm using OpenFOAM 2.1.1 and Paraview 3.12.0

Thanks, Eranho
Eranho is offline   Reply With Quote

Old   September 28, 2014, 14:40
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Eranho,

I've done a really quick test just now and I had no problems by following these steps:
  1. Used Ubuntu 12.04 and OpenFOAM 2.1.1.
  2. Used a clean copy of the original tutorial "lagrangian/sprayFoam/aachenBomb".
  3. Ran:
    Code:
    blockMesh
    sprayFoam
    
    foamToVTK
    paraview
    Honestly I only allows the solver to only run up to the time 5e-05.
  4. When ParaView finally opened up, I opened the file "VTK/lagrangian/sprayCloud/sprayCloud_24.vtk" in it.
  5. Then applied the Glyph filter, but with these settings:
    • Glyph type: Sphere
    • Scale Mode: Off
    • Mask Points: unchecked
    • Random mode: unchecked
You might also want to check the values that were read from the VTK file, namely by using the "Spreadsheet View" in ParaView: http://www.itk.org/Wiki/ParaView/Use...readsheet_View - it's possible that some values are of type NaN (Not-a-Number). Which would explain why it crashes.


Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   September 28, 2014, 23:53
Default
  #3
New Member
 
Na
Join Date: Sep 2014
Posts: 5
Rep Power: 2
Eranho is on a distinguished road
Thanks Bruno,

I got the post-processing to work by doing following procedure (found from the forum):

I do the following tasks after the solver has finished:
"1) rm -r 0
2) paraFoam
3) in ParaView press apply
4) in mesh parts select kinematicCloud - lagrangian
5) in lagrangian fields U and others > apply
6) menu filters > alphabetical > extractBlock
7) select lagrangian (black cross) > apply
8) glyph > glyph type sphere > radius 0.? > theta resolution 24 > scale mode off > apply
9) choose display color"

I will try with the VTK as you described later. Thank you very much , Erkki
wyldckat and JuanRodriguez like this.
Eranho 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
Accessing the position and diameter of lagrangian particles ahcai007 OpenFOAM Programming & Development 3 March 31, 2014 19:22
Lagrangian material particles bramv101 STAR-CCM+ 3 October 24, 2011 08:31
Multiphase Lagrangian Particles moritzhoefert OpenFOAM 1 December 8, 2010 09:48
How to set correct mass flow rate for lagrangian particles ? sankarv OpenFOAM 0 April 19, 2010 11:40
Mapping Lagrangian particles gschaider OpenFOAM Bugs 1 April 1, 2009 05:05


All times are GMT -4. The time now is 20:50.