CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   How to visualize spray (http://www.cfd-online.com/Forums/openfoam-solving/60224-how-visualize-spray.html)

hsieh March 21, 2006 16:57

Hi, I downloaded the solver
 
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

hjasak March 21, 2006 17:10

I use dxFoam - that has got th
 
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

gschaider March 21, 2006 17:20

paraFoam can't do it, but para
 
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)

hemph March 22, 2006 03:59

paraFoam is just paraview, but
 
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.

hsieh March 22, 2006 08:52

Thanks guys! This is helpful.
 
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 March 22, 2006 08:53

Thanks guys! This is helpful.
 
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 March 22, 2006 08:56

Sorry that I accidently hit th
 
Sorry that I accidently hit the "post message" before I finished revising the message.

gschaider March 22, 2006 10:59

Hello Pei! Yes, I did it (a
 
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)

tsencic May 9, 2006 03:43

How can I visualize the spray?
 
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 May 9, 2006 05:49

After running foamToVTK, in th
 
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


All times are GMT -4. The time now is 11:58.