CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

How to visualize spray

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 21, 2006, 16:57
Default Hi, I downloaded the solver
  #1
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 317
Rep Power: 9
hsieh is on a distinguished road
Hi,

I downloaded the solver and case from:
http://openfoamwiki.net/index.php/Contrib_icoLagr angianFoam.

I implemented the fix and re-compiled OpenFOAM and the solver. Ran the case. I got some files in lagrange directory (something like positions.gz). After I started paraFoam, I only saw p and U. It will be appreciated if someone can point to me how to visualize the particles.

Pei
hsieh is offline   Reply With Quote

Old   March 21, 2006, 17:10
Default I use dxFoam - that has got th
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
I use dxFoam - that has got the support for spray visualisation. You can also try Ensight, that has got support for spray stuff as well.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 21, 2006, 17:20
Default paraFoam can't do it, but para
  #3
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,914
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
paraFoam can't do it, but paraview can. Look at
http://openfoamwiki.net/index.php/Main_FAQ#Postpr ocessing_of_Lagrangian_particles
(which references http://www.cfd-online.com/cgi-bin/Op...show.cgi?1/853)
__________________
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

Old   March 22, 2006, 03:59
Default paraFoam is just paraview, but
  #4
Senior Member
 
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 8
hemph is on a distinguished road
paraFoam is just paraview, but with added support for reading OpenFOAM output format (except for lagrangian particles!). That means that you can run foamToVTK on the case, open it as usual in paraFoam and then use
File->Open Data
to open the files in the lagrangian-subdir. You then have to put a glyph (Filter->Glyph) on the position of the particle to see something.
hemph is offline   Reply With Quote

Old   March 22, 2006, 08:52
Default Thanks guys! This is helpful.
  #5
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 317
Rep Power: 9
hsieh is on a distinguished road
Thanks guys! This is helpful.

Bernhard, are you the person who built the solver and the case on the wiki? I am very impressed by it. Actually, spray/deselEngine are not my field, but, I cannot help myself but to play with this solver/case. I actually have few more questions for this:

1. in the time folders/lagrange, I saw d.gz/m.gz/U.gz/positions.gz. When I exported the results to VTK and started paraview, I only saw d/m/U not positions. Is this critical?
2. when I did glyph, I saw vectors. The pictures on the wiki, you have a big dot (looked like a solid particle) attached to the each vector. How was it done?
3. what are d and m (I apologize for the stupid question, but, I am not in the field of spray/deselEngine)?
4. On the wiki, there is another case called Ejector, but, it points to the main the page, not a download link.
5. I am wondering how difficult it is to modify the solver to handle solid particels in liquid.

I have been playing with OpenFOAM for about a year now. I am constantly amazed by how powerful it is and the wide range of problem it can solve. Great stuffs!

Pei
hsieh is offline   Reply With Quote

Old   March 22, 2006, 08:53
Default Thanks guys! This is helpful.
  #6
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 317
Rep Power: 9
hsieh is on a distinguished road
Thanks guys! This is helpful.

Bernhard, are you the person who built the solver and the case on the wiki? I am very impressed by it. Actually, spray/deselEngine are not my field, but, I cannot help myself but to play with this solver/case. I actually have few more questions for this:

1. in the time folders/lagrange, I saw d.gz/m.gz/U.gz/positions.gz. When I exported the results to VTK and started paraview, I only saw d/m/U not positions. Is this critical?
2. when I did glyph, I saw vectors. The pictures on the wiki, you have a big dot (looked like a solid particle) attached to the each vector. How was it done?
3. what are d and m (I apologize for the stupid question, but, I am not in the field of spray/deselEngine)?
4. On the wiki, there is another case called Ejector, but, it points to the main page, not a download link.
5. I am wondering how difficult it is to modify the solver to handle solid particels in liquid.

I have been playing with OpenFOAM for about a year now. I am constantly amazed by how powerful it is and the wide range of problem it can solve. Great stuffs!

Pei
hsieh is offline   Reply With Quote

Old   March 22, 2006, 08:56
Default Sorry that I accidently hit th
  #7
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 317
Rep Power: 9
hsieh is on a distinguished road
Sorry that I accidently hit the "post message" before I finished revising the message.
hsieh is offline   Reply With Quote

Old   March 22, 2006, 10:59
Default Hello Pei! Yes, I did it (a
  #8
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,914
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hello Pei!

Yes, I did it (although the majority of the stuff was copy/pasted from different parts of the original OF-sources). Glad you like it (It's not overdocumented, is it? ;) )

@1: position is the place of the particle. There's no use in displaying that separatly
@2: at the glyph-dialog there is a drop-down list of Glyphs. Choose sphere.
@3: d is particle diameter and m is mass (it really isn't overdocumented).
@4: Ups. Typo. Fixed that. Should be downloadable now.
@5: With "solid" particles you mean particles that collide (particle/particle-interaction). Not a big problem (depending on how accurate you want the collisions to be). Take one of the collision-Models in the dieselFoam-Hierarchy as a template. (I have done such a solver, and I will post it on the Wiki once I found time to check it)
__________________
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

Old   May 9, 2006, 03:43
Default How can I visualize the spray?
  #9
Member
 
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 8
tsencic is on a distinguished road
How can I visualize the spray?
When I open a case with paraFoam (previously treated with foamToVTK), open a time directory/lagrangian/positions I obtain a message: Could not find an appropriate reader for file...Would you like to manually select the reader for this file? Then I choose from a list but I can't visualize lagrangian particles, whatever I select.

When I try dxFoam I obtain:
Checking path to dx...Can't find dx executable. Please check your path.
Where should I check it? dxFoam is in OpenFOAM/OpenFOAM-1.2/bin
tsencic is offline   Reply With Quote

Old   May 9, 2006, 05:49
Default After running foamToVTK, in th
  #10
Member
 
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 8
tsencic is on a distinguished road
After running foamToVTK, in the case directory there appears a directory neamed VTK. Open the case as usual with paraFoam and then File->Open Data - open the case/VTK/lagrangian/position

I didn't notice the case/VTK
tsencic 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
visualize turbulence lee Main CFD Forum 1 September 27, 2007 06:00
Visualize nonOrthoFaces set r2d2 OpenFOAM Meshing & Mesh Conversion 1 November 28, 2006 11:43
How to visualize the components raintung FLUENT 3 May 20, 2003 09:47
How to Visualize Peter Main CFD Forum 2 May 3, 2002 23:44
how to visualize the result luo Phoenics 5 October 10, 2001 20:37


All times are GMT -4. The time now is 07:03.