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

Error in particle mapping using AMR in DPMDyMFoam

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 30, 2020, 18:38
Default Error in particle mapping using AMR in DPMDyMFoam
  #1
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 35
Rep Power: 8
jairoandres is on a distinguished road
Dear all

I am using a velocity gradient-based AMR criteria under the DPMDyMFoam solver (OpenFOAM V1912). The simulation consists of solid particles introduced into a confinement through a coaxial jet. It works fine and postprocessing shows good results. However, after several iterations (+10000) (long enough for some particles to exit the domain), the simulation crashes with the following error:

ExecutionTime = 12298.74 s ClockTime = 12308 s

Courant Number mean: 0.0093041779 max: 0.96458841
deltaT = 5e-05
Time = 1.6232

Selected 94 split points out of a possible 43041.
Unrefined from 441930 to 441272 cells.
[1]
[1]
[1] --> FOAM FATAL ERROR:
[1] "Particle mapped to a location outside of the mesh" when tracking from centre (0.028415721 -0.44624185 0.090168445) of cell 54248 to position (0.027997367 -0.44822535 0.091582116)
[1]
[1] From function void Foam:article::locate(const vector&, const vector*, Foam::label, bool, const Foam::string&)
[1] in file particle/particle.C at line 450.
[1]
FOAM parallel run exiting
[1]
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 1 in communicator MPI_COMM_WORLD
with errorcode 1.

NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
You may or may not see output from other processes, depending on
exactly when Open MPI kills them.


It is clear the error is produced after the refining/unrefining process is done. Because the mesh keeps changing, I am not sure about the exact location of that cell, but I am almost positive it represents an internal cell located near (downstream) the particle injector.

This zone is subjected to a lot of refinement / unrefinement. My best guess is that after the unrefinement, the particle mapping algorithm does not know the cell was refined. However, I am not sure if the particle locations can be corrected in the same way fluxes are in the dynamicMeshDict.

Have you got any ideas to fix this error?
jairoandres is offline   Reply With Quote

Old   August 8, 2020, 15:48
Default
  #2
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 35
Rep Power: 8
jairoandres is on a distinguished road
new update on this, the cell is a wall-boundary cell and the error occurs when openFoam maps the particle after the cell is unrefined. It might be related with the mapping of the particle position in the new cell. The cell is a hexahedral and is an elongated box (2:1) relation. In order to keep running the case I had to decrease the threshold for unrefinement. After some iterations, I increased the unrefining threshold again and the case kept working well. If the threshold is increased again, the same error reappears. Is more evident if more parcels are atomized.

Last edited by jairoandres; August 19, 2020 at 11:07.
jairoandres is offline   Reply With Quote

Old   January 5, 2021, 22:42
Default
  #3
ljj
New Member
 
liuJJ
Join Date: Sep 2020
Posts: 4
Rep Power: 2
ljj is on a distinguished road
Dear jairoandres,

I meet the same question,but I couldn't understand ''decrease the threshold for unrefinement''.Cloud you please tell me how to keep running the case.Thanks a lot.
ljj is offline   Reply With Quote

Old   January 6, 2021, 15:00
Default
  #4
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 35
Rep Power: 8
jairoandres is on a distinguished road
Hello, I meant to decrease the target value for refinement, so refined cells are not unrefined as often. The error appears to be related to a weakness in the Baryocentric particle tracking in OpenFOAM, retracking the particles outside of the domain when the unrefined element shape is a bit rough. I've read the release notes of OpenFOAM V2012 and they mention the following on the fixes:

Lagrangian: Improved particle tracking on moving meshes
This release includes several improvements to particle tracking on moving mesh cases. These cases would often fail in earlier versions due to:

particles crossing AMI patches;
particle-wall interactions; and
fragility of the barycentric tracking (ported from openfoam.org)


I will be checking that version soon enough. Let me know if you do it first and you are able to fix the error.

You can check it out in https://www.openfoam.com/releases/op...an-moving-mesh.
jairoandres is offline   Reply With Quote

Old   February 7, 2021, 02:44
Default
  #5
ljj
New Member
 
liuJJ
Join Date: Sep 2020
Posts: 4
Rep Power: 2
ljj is on a distinguished road
Hello,

Thanks for your reply. I tried to decrease the target value for refinement, the error still appear.But when I didn't use dynamic refinement, my case would keep running.
ljj is offline   Reply With Quote

Old   February 8, 2021, 09:12
Default
  #6
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 35
Rep Power: 8
jairoandres is on a distinguished road
I can now confirm you is a bug in OpenFOAM. I've posted the issue present in the previous OF version, with the solution I found (basically reverting to OF V8 code). According to Mattijs, " the code was indeed checking the old cell label instead of the found one". Therefore you have to modify particle.C and recompile to make it work (or use OpenFOAM v8).

This is the bug report with fix:
https://develop.openfoam.com/Develop.../-/issues/1992
jairoandres is offline   Reply With Quote

Old   February 8, 2021, 09:13
Default
  #7
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 35
Rep Power: 8
jairoandres is on a distinguished road
As particle is a global class, I suppose this issue was present in all Lagrangian solvers with DyM capability
jairoandres is offline   Reply With Quote

Old   February 16, 2021, 11:34
Default
  #8
ljj
New Member
 
liuJJ
Join Date: Sep 2020
Posts: 4
Rep Power: 2
ljj is on a distinguished road
It seems a random error,because only some cases reported the error.Thank you very much for your approach to fix it,Iwill try.
ljj is offline   Reply With Quote

Old   February 16, 2021, 11:36
Default
  #9
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 35
Rep Power: 8
jairoandres is on a distinguished road
Quote:
Originally Posted by ljj View Post
It seems a random error,because only some cases reported the error.Thank you very much for your approach to fix it,Iwill try.
It is not a random error. It shows itself when the cell containing the particle is unrefined.
jairoandres is offline   Reply With Quote

Old   February 20, 2021, 07:44
Default
  #10
ljj
New Member
 
liuJJ
Join Date: Sep 2020
Posts: 4
Rep Power: 2
ljj is on a distinguished road
Quote:
Originally Posted by jairoandres View Post
It is not a random error. It shows itself when the cell containing the particle is unrefined.
I modified the particle.C according to your method, but the error also occured.
ljj is offline   Reply With Quote

Old   March 16, 2021, 14:43
Default
  #11
Member
 
Jairo A. Gutiérrez S
Join Date: Nov 2014
Posts: 35
Rep Power: 8
jairoandres is on a distinguished road
What error msg are you getting? The same one than me? "Particle mapped to a location outside of the mesh"?

I fixed the error doing these things:

1) Recompiling according to the instructions above
2) Applying the modifications suggested here: strange stuck particles on the rebound wall in MPPICFoam

I tracked the mapping error in particle.C and concluded it only applied to very small particles getting stuck in a cell that was getting refined (or near one).
jairoandres is offline   Reply With Quote

Reply

Tags
dpmdymfoam, lagrangian, openfoam, particle mapping

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
[Other] dynamicTopoFVMesh and pointDisplacement RandomUser OpenFOAM Meshing & Mesh Conversion 6 April 26, 2018 07:30
Particle tracking error alchem OpenFOAM Bugs 5 May 6, 2017 16:30
[mesh manipulation] Importing Multiple Meshes thomasnwalshiii OpenFOAM Meshing & Mesh Conversion 18 December 19, 2015 18:57
injection problem Mark New FLUENT 0 August 4, 2013 01:30
[Gmsh] Import gmsh msh to Foam adorean OpenFOAM Meshing & Mesh Conversion 24 April 27, 2005 08:19


All times are GMT -4. The time now is 14:45.