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

[OpenFOAM 3.0.1] DPMFoam domain decomposition bug

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

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   April 8, 2016, 12:45
Default [OpenFOAM 3.0.1] DPMFoam domain decomposition bug
  #1
C-L
New Member
 
Charlie Lloyd
Join Date: Feb 2016
Posts: 13
Rep Power: 2
C-L is on a distinguished road
Hi All,

I am currently experiencing a weird bug whereby my case is freezing after attempting to update the kinematic cloud, but only when decomposing my mesh in a certain way.

My case study models a particulate flow down a pipe, with cyclic boundary conditions placed at the ends and the LES-WALE turbulence model. When running in serial there are no errors and the solution seems reasonable. However, when decomposing the mesh (scotch or simple) in the z-direction the output file freezes at 'evolving kinematic cloud'. When decomposing the mesh in the (r,theta) directions the solver works again, but this seems like a very inefficient way to parallelise my pipe, especially when I start splitting it into 64 processors.

My case directory can be found on this dropbox link:

https://www.dropbox.com/s/qz9wpb5wt7...PM.tar.gz?dl=0

and I have attached the output file below.

I have changed the case file slightly so that it runs (with the same issues) on the standard DPMFoam solver rather than my altered one.

If someone could take a look at this I would be very grateful!

Thanks,
Charlie
Attached Files
File Type: txt log.txt (2.3 KB, 9 views)
C-L is offline   Reply With Quote

Old   April 16, 2016, 17:35
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,748
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Greetings Charlie,

The solution is simple, you need to use preservePatches in "system/decomposeParDict":
Code:
preservePatches (C1 C2);

numberOfSubdomains 4;
method          simple;

simpleCoeffs
{
    n    (4 1 1);
    delta    0.0001;
}
This way the two patches are in the same processor sub-domain, which allows for the algorithm to work properly.

For more details/examples, check the main example dictionary file, whose path is given by the following command:
Code:
echo $FOAM_UTILITIES/parallelProcessing/decomposePar/decomposeParDict
Best regards,
Bruno
vikramaditya91 likes this.
__________________
wyldckat is offline   Reply With Quote

Old   April 18, 2016, 06:40
Default
  #3
C-L
New Member
 
Charlie Lloyd
Join Date: Feb 2016
Posts: 13
Rep Power: 2
C-L is on a distinguished road
Hi Bruno,

I had tried the preservePatch feature before but clearly I got the notation wrong because your fix worked straight away! Thanks for the help,
Charlie
C-L 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
Domain decomposition method Bram OpenFOAM 4 August 19, 2010 18:14
Domain Decomposition ertan Main CFD Forum 2 September 1, 2009 12:22
CFX - domain decomposition. Urgent!!!! Elena Saldaeva CFX 4 June 30, 2008 07:18
CFX Solver Memory Error mike CFX 1 March 19, 2008 08:22
Domain decomposition rajesh Main CFD Forum 2 August 31, 1999 04:22


All times are GMT -4. The time now is 17:27.