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

Particle tracking

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

Like Tree10Likes
  • 1 Post By lasherwc
  • 5 Post By lasherwc
  • 1 Post By lasherwc
  • 2 Post By lasherwc
  • 1 Post By veeturi

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 1, 2018, 10:15
Default Particle tracking
  #1
Member
 
Bill Lasher
Join Date: Jun 2009
Posts: 36
Rep Power: 15
lasherwc is on a distinguished road
Hi:

I'm trying to do a simple particle tracking using one-way coupling (only the effect of the liquid on the particle). I've read conflicting things about whether icoUncoupledKinematicParcelFoam will do this. I've been able to model a single particle with buoyancy in a still fluid and get accurate results. When I specify a uniform velocity nothing changes - as though the solver doesn't recognize it. My eventual goal is to use another solver to get the flow field, then use a particle tracker to get the track. Am I going down the right path or do I need to use a different solver?

Thanks,

Bill
sourav90 likes this.
lasherwc is offline   Reply With Quote

Old   February 1, 2018, 14:28
Default Answer to question
  #2
Member
 
Bill Lasher
Join Date: Jun 2009
Posts: 36
Rep Power: 15
lasherwc is on a distinguished road
Ok, so I solved my own problem and thought I might put it here for others, since I've seen a lot of posts about this.

First, I had an error in my kinematicCloudProperties dictionary where the patch names didn't match what was in blockMesh. I fixed that and everything worked as expected.

To use icoUncoupledKinematicParcelFoam on an already-solved flow field, this is all I had to do:

1. Solve the original flow problem (I did the pitzDaily tutorial from the simpleFoam tutorials).
2. To the constant directory add/edit the following files, which you can get from the hopper tutorial:
-g, kinematicCloudProperties, kinematicCloudPositions
-add rhoinf to the transport properties dictionary
3. Replace the controlDict file with the one from the hopper tutorial and make the appropriate changes
4. Run icoUncoupledKinematicParcelFoam, then visualize using the instructions that can be found on the OpenFOAM wiki.

Voila!
lasherwc is offline   Reply With Quote

Old   July 10, 2019, 12:41
Default
  #3
New Member
 
Join Date: Jun 2017
Posts: 10
Rep Power: 7
Simone81 is on a distinguished road
Hi,


I follow your instructions but the solver get stock forever on the first time step! perhaps do you have a working example?
Thank you!
Simone81 is offline   Reply With Quote

Old   July 11, 2019, 15:04
Default Example
  #4
Member
 
Bill Lasher
Join Date: Jun 2009
Posts: 36
Rep Power: 15
lasherwc is on a distinguished road
Hi:

I do not still have the files but I can try to re-create the case. Give me a few days and I'll get back to you.
Simone81 likes this.
lasherwc is offline   Reply With Quote

Old   July 11, 2019, 16:28
Default
  #5
New Member
 
Join Date: Jun 2017
Posts: 10
Rep Power: 7
Simone81 is on a distinguished road
Hi,
Thank you very much for your help! I really appreciate it.
Simone81 is offline   Reply With Quote

Old   July 14, 2019, 15:05
Default Example
  #6
Member
 
Bill Lasher
Join Date: Jun 2009
Posts: 36
Rep Power: 15
lasherwc is on a distinguished road
Here is an example. Run the pitzDaily tutorial using simpleFoam, rename the last directory (288) to 0 and remove the other time directories.

Copy the attached controlDict, fvSchemes and fvSolution files to the system directory, and the remaining files to the constant directory, and run icoUncoupledKinematicParcelFoam (I used OpenFoam v. 6).

You should be able to view the results in paraFoam.

Good luck, and let me know if you have any problems!
Attached Files
File Type: zip particle_tracking.zip (4.1 KB, 186 views)
Jaxon18 and sourav90 like this.
lasherwc is offline   Reply With Quote

Old   June 14, 2020, 05:25
Default
  #7
New Member
 
Join Date: May 2020
Posts: 27
Blog Entries: 1
Rep Power: 4
Mars409 is on a distinguished road
I ran the pitzDaily case with simpleFoam and then overwrote the system/ directory and constant/ directory files with those from your zip file, and ran icoUncoupledKinematicParcelFoam. Finally, where I ran paraFoam, selecting kinematicCloud - Lagrangian under Mesh Parts and selecting all under Lagrangian fields, ParaView showed nothing.

Can you show what ParaView is supposed to show?

I ran mine on Raspberry Pi-4 (Buster 32 bits), with ParaView built to 64-bit architecture and 32-bit IDs.

=====
I see I missed out the steps in OpenFoamWiki: https://openfoamwiki.net/index.php/H...er_in_paraFoam (but isn't this said to be for massless particles tracking, whereas we are interesting in tracing Lagrangian particles?).

Following that instruction, ParaView through errors complaining "The input dataset did not have a valid DATA_TIME_STEPS information key.

I have seen this error message before when running ParticleTracks and trying to display the filter Temporal Particles to Pathlines.

Last edited by Mars409; June 14, 2020 at 05:51. Reason: newer info.
Mars409 is offline   Reply With Quote

Old   June 15, 2020, 11:09
Default Postprocessing
  #8
Member
 
Bill Lasher
Join Date: Jun 2009
Posts: 36
Rep Power: 15
lasherwc is on a distinguished road
Hi:

The wiki link you noted is different than the one I used and I believe it's for showing the flowfield rather than Lagrangian particle tracking (thus the massless particles).

The link I was referring to is here:

http://openfoamwiki.net/index.php/FA...gian_particles

Note that you need to unselect everything in Volume Fields.

Let me know if this solves the problem - if not perhaps zip your case and post it, I will take a look.
lasherwc is offline   Reply With Quote

Old   June 15, 2020, 12:07
Default
  #9
New Member
 
Join Date: May 2020
Posts: 27
Blog Entries: 1
Rep Power: 4
Mars409 is on a distinguished road
Thanks. It works now using the Glyph filter.

Indeed after posting the last remark yesterday I looked through the time directories and inspected the Lagrangian VTK files (they are in ASCII) and came away wondering why ParaView wasn't showing the ball since the Lagrangian Fields list a whole bunch of them.

So it's the Glyph filter that needs to get applied.

Now I see the ball moving from left the the right when I tripled the end time.

Strangely, though, in a separate cyclone simulation case prepared through the SimFlow GUI and viewed separately using ParaFoam invoked from the command line I did not have to apply the Glyph filter to see the particles. With that experience, I was expecting the same in this pitzDaily tutorial case that it caught my blindsided.

On top of that--it maybe just me--somehow I am unable to display the Lagrangian field at the mesh at the same time. It's not just this case but that cyclone simulation as well.
Mars409 is offline   Reply With Quote

Old   June 15, 2020, 12:47
Default
  #10
Member
 
Bill Lasher
Join Date: Jun 2009
Posts: 36
Rep Power: 15
lasherwc is on a distinguished road
Glad you got it to work! I'm not an expert on Paraview, I just figured this particular thing out and thought I'd share it.

Good luck!
lasherwc is offline   Reply With Quote

Old   July 2, 2020, 19:13
Default
  #11
New Member
 
Sricharan S Veeturi
Join Date: Jun 2016
Posts: 5
Rep Power: 8
veeturi is on a distinguished road
Quote:
Originally Posted by lasherwc View Post
Ok, so I solved my own problem and thought I might put it here for others, since I've seen a lot of posts about this.

First, I had an error in my kinematicCloudProperties dictionary where the patch names didn't match what was in blockMesh. I fixed that and everything worked as expected.

To use icoUncoupledKinematicParcelFoam on an already-solved flow field, this is all I had to do:

1. Solve the original flow problem (I did the pitzDaily tutorial from the simpleFoam tutorials).
2. To the constant directory add/edit the following files, which you can get from the hopper tutorial:
-g, kinematicCloudProperties, kinematicCloudPositions
-add rhoinf to the transport properties dictionary
3. Replace the controlDict file with the one from the hopper tutorial and make the appropriate changes
4. Run icoUncoupledKinematicParcelFoam, then visualize using the instructions that can be found on the OpenFOAM wiki.

Voila!
An alternative I found was to use the "particle tracer" filter in ParaView. The downside is that you have to reconstruct all the time steps of interest, at least on a coarse temporal resolution. i.e. if you're simulating for 10 sec, get results for each second and then use the temporal interpolation in ParaView.

This may not be completely accurate but its a technique to get quick results.
sourav90 likes this.
veeturi is offline   Reply With Quote

Reply

Tags
particle tracking

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Particle tracking error alchem OpenFOAM Bugs 5 May 6, 2017 16:30
Lagrangian Particle Tracking in Eulerian-Eulerian Multiphase Flow DarrenC CFX 5 April 7, 2016 14:50
Ubuntu 12.10 + openfoam2.2.0 ==> paraview error message peteryuan OpenFOAM Installation 6 August 18, 2013 18:00
[OpenFOAM] ParaView ErrOr soheil nazmdeh ParaView 1 August 17, 2013 07:40
injection problem Mark New FLUENT 0 August 4, 2013 01:30


All times are GMT -4. The time now is 18:46.