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

Lagrangian particle addition slowing down solver to halt

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 28, 2016, 11:27
Default Lagrangian particle addition slowing down solver to halt
  #1
Member
 
Ali
Join Date: Oct 2013
Location: Scotland
Posts: 62
Rep Power: 9
ali.m.1 is on a distinguished road
Hello

I'm making a combined Euler-Euler Euler-Lagrange two phase model. I've combined reactingTwoPhaseEulerFoam and DPMFoam, which can be seen in the attached .C file.

The code runs well, and performs faster than standard DPMFoam when used on a coarse mesh with <1% particle concentration. However, when I increase the particle numbers, or increase the mesh density, the solver starts off fine, but then grinds to a halt. I can run DPMFoam alongside it, with the same mesh, same particle injection method (kinematicLookupTableInjection), same concentration of particles: but my solver almost stops injecting. It never crashes, or the memory doesn't go higher than the DPMFoam solver (by checking the terminal 'top'), it just slows down a lot. I've can run the program in a debugger (nemiver), and I've also run it using valgrind. I can attach the output from 'callgrind', in case anyone can spot something suspicious.

I've tried commenting out the lookupTable code, and that doesn't speed things up. The solver also runs ok when there are no particles, it's just after a few injections that things start to slow down.

If anyone could point me in the right direction that would be great!

Ali

Edit: It turns out the callgrind file is pretty big, so I'll leave it out. If anyone would like to see it I can email it or put it on dropbox or something.
Attached Files
File Type: c myReactingTwoPhaseEulerFoamParticles.C (14.9 KB, 33 views)
ali.m.1 is offline   Reply With Quote

Old   November 29, 2016, 19:00
Default Similar behavior with interFoam and particle cloud
  #2
New Member
 
Joseph Prince
Join Date: Apr 2014
Posts: 4
Rep Power: 9
jfp6 is on a distinguished road
I experienced the same problem when I added a particle cloud to interFoam. I was unable to track down the problem. When I had injected a certain # of particles, the time to evolve the cloud increased dramatically (see attached plot). I spent a lot of time adjusting the mesh to see if this affected it, but was not able to see any correlation.

Please post if you find a solution.

Cheers,

jfp6
Attached Images
File Type: jpeg Particle Slow Down.jpeg (45.2 KB, 84 views)
jfp6 is offline   Reply With Quote

Old   December 9, 2016, 11:35
Default
  #3
PK1
New Member
 
Paul K
Join Date: Aug 2015
Posts: 5
Rep Power: 7
PK1 is on a distinguished road
Same Problem here using a custom sprayFoam-derivative and using the patchInjector.

Takes about 0.35 s at an injection rate of 1M / s (stationary holdup approx 120k parcels) to bring the simulation to nearly a halt. Decreasing the injection rate does not seem to help.

EDIT 2:

My bad, I had patchInteraction set to none, which resulted in trouble when parcels hit the outlet patch without being removed. I figured this out by flipping the cloud debug switch on - which yielded a lot of tracking rescues. ParaView showed the slowdown to happen just as parcels hit the walls.

Last edited by PK1; December 10, 2016 at 13:31. Reason: More info.
PK1 is offline   Reply With Quote

Old   December 12, 2016, 09:42
Default
  #4
Member
 
Ali
Join Date: Oct 2013
Location: Scotland
Posts: 62
Rep Power: 9
ali.m.1 is on a distinguished road
Quote:
Originally Posted by PK1 View Post
Same Problem here using a custom sprayFoam-derivative and using the patchInjector.

Takes about 0.35 s at an injection rate of 1M / s (stationary holdup approx 120k parcels) to bring the simulation to nearly a halt. Decreasing the injection rate does not seem to help.

EDIT 2:

My bad, I had patchInteraction set to none, which resulted in trouble when parcels hit the outlet patch without being removed. I figured this out by flipping the cloud debug switch on - which yielded a lot of tracking rescues. ParaView showed the slowdown to happen just as parcels hit the walls.
Hi Paul

Thanks a lot for the advice. I had my patchInteraction set to 'standardWallInteraction'. This setting seemed to work with DPMFoam, but didn't work with my solver. I changed the settings to 'localInteraction', and defined types for each patch and now the solver doesn't crash! I'll need to look into what the standardWallInteraction does.

Cheers

Ali
ali.m.1 is offline   Reply With Quote

Old   January 11, 2017, 10:43
Default
  #5
Member
 
Ali
Join Date: Oct 2013
Location: Scotland
Posts: 62
Rep Power: 9
ali.m.1 is on a distinguished road
Hi Joseph

How did you create that plot? I'm interested in doing the same, as my solver still isn't running as it should.

Cheers
ali.m.1 is offline   Reply With Quote

Old   February 7, 2017, 15:23
Default Code for the plot
  #6
New Member
 
Joseph Prince
Join Date: Apr 2014
Posts: 4
Rep Power: 9
jfp6 is on a distinguished road
Attached is the python code for the plot. There are probably better ways to do this with pyFoam, but this worked. You may have to add you current directory to your path.

Cheers,

Joseph
Attached Files
File Type: txt logReader.txt (1.2 KB, 22 views)
jfp6 is offline   Reply With Quote

Reply

Tags
dpmfoam, lagrangian, particles, slow

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
Evaporation in an Incompressible Lagrangian (LPT) solver? jheide OpenFOAM Programming & Development 4 December 15, 2020 23:39
Particle tracking error alchem OpenFOAM Bugs 5 May 6, 2017 16:30
Request for Lagrangian Particle Tracking Validation or Verification Paper Mojtaba.a OpenFOAM Verification & Validation 6 May 23, 2016 01:47
steady state lagrangian solver kalyan OpenFOAM Running, Solving & CFD 0 March 6, 2015 05:26
which solver for particle tracking through a fluid for lagrangian based method? ranasa OpenFOAM Running, Solving & CFD 0 August 9, 2014 03:09


All times are GMT -4. The time now is 12:20.