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

interDyMFoam, problems in mesh motion solutor run in parallel

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 21, 2009, 17:39
Exclamation interDyMFoam, problems in mesh motion solutor run in parallel
  #1
DLC
Member
 
Davide Lupo Conti
Join Date: Nov 2009
Posts: 34
Rep Power: 7
DLC is on a distinguished road
Hello,
I'm using OpenFOAM 1.5-dev. I'm using the interDyMFoam solutor to run a free surface flow test case (a cube floating in water). I've modified a bit the floatingBody classes, but nothing of major importance.

I don't have problems in running the simulation in serial (one processor), but when I try to run the same case in parallel (on four processors) the simulation gets stuck though I think I've done all things correctly, using decomposePar.

I've done a bit of debugging and found out that the coode gets stuck on the solutor of the laplacian for the mesh motion in sixDofMotion.C,
more precisely in fvMesh::movePoints(motionPtr_->newPoints()).
the problem seems to be in newPoints().

In the end I found out that the problem seems to be in laplaceTetDecompositionMotionSolver.C in the line solverPerf_ = motionEqn.solve(). Unfortunately I couldn't get any 'deeper' than that in the code.

Does anybody have an idea why the simulation runs in serial and not in parallel? I mean, isn't pretty wierd that running in parallel gives problems in the solutor for the mesh motion? Any idea can be very useful!

thanks to all

Davide
DLC is offline   Reply With Quote

Old   November 23, 2009, 05:44
Default Known issues related to mesh motion
  #2
Member
 
Jean-Peer Lorenz
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 33
Rep Power: 8
jploz is on a distinguished road
Hi,

there are known issues related to mesh motion. Please read through the following threads, probably this will solve your questions:

no parallel computing using "dynamicBodyFvMesh"

Moving mesh crashes in parallel (1.5-dev)

Good luck.
Jean-Peer
jploz is offline   Reply With Quote

Old   November 23, 2009, 09:57
Default
  #3
DLC
Member
 
Davide Lupo Conti
Join Date: Nov 2009
Posts: 34
Rep Power: 7
DLC is on a distinguished road
Thank you very much, I got a bit further changing the comm blocking , but now it is giving me the following error:

temporary dellocated
From function const T& tmp<T>:perator()() const

It seems like a matrix has been deallocated. Should I manually allocate it inside the code?




thanks again

Davide
DLC is offline   Reply With Quote

Old   November 23, 2009, 10:30
Default
  #4
DLC
Member
 
Davide Lupo Conti
Join Date: Nov 2009
Posts: 34
Rep Power: 7
DLC is on a distinguished road
Actually these are the full error lines:

Please click one of the Quick Reply icons in the posts above to activate Quick Reply.[2]
[2]
[2] temporary deallocated
[2]
[2] From function const T& tmp<T>:perator()() const
[2] in file /u/cmcs/dlconti/OpenFOAM/OpenFOAM-1.5-dev/src/OpenFOAM/lnInclude/tmpI.H at line 190.
[2]
FOAM parallel run aborting
[2]
[iacspc122:21725] MPI_ABORT invoked on rank 2 in communicator MPI_COMM_WORLD with errorcode 1
[3]
[3]
[3] temporary deallocated
[3]
[3] From function const T& tmp<T>:perator()() const
[3] in file /u/cmcs/dlconti/OpenFOAM/OpenFOAM-1.5-dev/src/OpenFOAM/lnInclude/tmpI.H at line 190.
[3]
FOAM parallel run aborting
[3]
[iacspc122:21726] MPI_ABORT invoked on rank 3 in communicator MPI_COMM_WORLD with errorcode 1
[0]
[0]
[0] temporary deallocated
[0]
[0] From function const T& tmp<T>:perator()() const
[0] in file /u/cmcs/dlconti/OpenFOAM/OpenFOAM-1.5-dev/src/OpenFOAM/lnInclude/tmpI.H at line 190.
[0]
FOAM parallel run aborting
[0]
[iacspc122:21723] MPI_ABORT invoked on rank 0 in communicator MPI_COMM_WORLD with errorcode 1
[1]
[1]
[1] temporary deallocated
[1]
[1] From function const T& tmp<T>:perator()() const
[1] in file /u/cmcs/dlconti/OpenFOAM/OpenFOAM-1.5-dev/src/OpenFOAM/lnInclude/tmpI.H at line 190.
[1]
FOAM parallel run aborting
[1]
[iacspc122:21724] MPI_ABORT invoked on rank 1 in communicator MPI_COMM_WORLD with errorcode 1

[1] Exit 1 mpirun -np 4 rasInterDyMFoam_BOAT -parallel > log66.out
DLC is offline   Reply With Quote

Old   November 24, 2009, 05:14
Default
  #5
Member
 
Jean-Peer Lorenz
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 33
Rep Power: 8
jploz is on a distinguished road
You need to re-check your source code. The error you are facing is not related to the actual mesh motion, I guess.
jploz is offline   Reply With Quote

Old   December 1, 2009, 11:29
Default
  #6
DLC
Member
 
Davide Lupo Conti
Join Date: Nov 2009
Posts: 34
Rep Power: 7
DLC is on a distinguished road
I'm sorry bothering you again, but I still have problems running interDyMFoam on OF 1.5-dev in parallel...

I even downloaded and compiled again the source, but the same error pops up when I try to run a case in parallel:
[3] [0]
[0]
[0] temporary deallocated
[0]
[0] From function const T& tmp<T>:perator()() const
[0] in file
/usr/scratch122/OpenFOAM/OpenFOAM-1.5-devSVN/src/OpenFOAM/lnInclude/tmpI.H at
line [2]
[2]
[2] temporary deallocated
[2]
[2] From function const T& tmp<T>:perator()() const
[2] in file
/usr/scratch122/OpenFOAM/OpenFOAM-1.5-devSVN/src/OpenFOAM/lnInclude/tmpI.H at
line 190.
[2]
FOAM parallel run aborting
[2]
[iacspc122:00723] MPI_ABORT invoked on rank 2 in communicator
MPI_COMM_WORLD with errorcode 1

[3]
[3] temporary deallocated
[3]
[3] From function const T& tmp<T>:perator()() const
[3] in file
/usr/scratch122/OpenFOAM/OpenFOAM-1.5-devSVN/src/OpenFOAM/lnInclude/tmpI.H at
line 190.
[3]
FOAM parallel run aborting
[3]
[iacspc122:00724] MPI_ABORT invoked on rank 3 in communicator
MPI_COMM_WORLD with errorcode 1
190.
[0]
FOAM parallel run aborting
[0]
[iacspc122:00721] MPI_ABORT invoked on rank 0 in communicator
MPI_COMM_WORLD with errorcode 1
[1]
[1]
[1] temporary deallocated
[1]
[1] From function const T& tmp<T>:perator()() const
[1] in file
/usr/scratch122/OpenFOAM/OpenFOAM-1.5-devSVN/src/OpenFOAM/lnInclude/tmpI.H at
line 190.
[1]
FOAM parallel run aborting
[1]
[iacspc122:00722] MPI_ABORT invoked on rank 1 in communicator
MPI_COMM_WORLD with errorcode 1


does anyone have an Idea?...

Thanks!

Davide
DLC is offline   Reply With Quote

Old   December 1, 2009, 11:31
Default
  #7
DLC
Member
 
Davide Lupo Conti
Join Date: Nov 2009
Posts: 34
Rep Power: 7
DLC is on a distinguished road
are you completely sure that you have OF 1.5-dev working in parallel?
DLC is offline   Reply With Quote

Old   January 7, 2010, 08:06
Default Mesh motion in parallel
  #8
Member
 
matteo lombardi
Join Date: Apr 2009
Posts: 61
Rep Power: 8
matteoL is on a distinguished road
Hello everyone,
I have found out how to solve the issue of the " temporary deallocated" problem in the mesh motion in parallel.

To solve the mesh motion problem we were using the amgSolver and it seems that in parallel that solver for the tetfem mesh motion has not been ported correctly.

If ,instead, we switch to the classical CG solver, the mesh motion works smoothly in parallel.

If you can, please Prof. jasak have a look at it in the new 1.6-dev...

best regards,
matteo
matteoL is offline   Reply With Quote

Old   June 30, 2010, 10:02
Post
  #9
New Member
 
yannH
Join Date: Feb 2010
Posts: 26
Rep Power: 7
yannH is on a distinguished road
Hi everyone,

I have a question about using interDymFoam and dynamicMotionSolverFvMesh :

Is it possible to use it in parallel? because when I launch parallel calculation, decomposePar says :

keyword global is undefined in dictionary "/home/yhh/OFrun/0/pointDisplacement::boundaryField"

file: /home/yhh/OFrun/0/pointDisplacement::boundaryField from line 27 to line 42.

From function dictionary::subDict(const word& keyword) const
in file db/dictionary/dictionary.C at line 449.

FOAM exiting

I don't get the "global" keyword, I assume it's for parallel computing, so when I write this 'global' in my point Displacement I can't find a consistent type

Does anyone know something about it?

I use OF 1.6 and my dynamicMeshDict file looks like :

dynamicFvMesh dynamicMotionSolverFvMesh;
motionSolverLibs ("libfvMotionSolvers.so");
solver displacementLaplacian;
diffusivity uniform ;
yannH is offline   Reply With Quote

Old   June 30, 2010, 11:38
Default
  #10
New Member
 
yannH
Join Date: Feb 2010
Posts: 26
Rep Power: 7
yannH is on a distinguished road
ok my problem comes from my two cyclic patch... For one cyclic patch it's ok, but for two, it gives the error message... I tried to change the decomposition method but with no success.
yannH is offline   Reply With Quote

Old   December 6, 2012, 16:31
Default
  #11
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 6
Ralph M is on a distinguished road
Adding "global" didn't worked for me either! I've got no cyclic patches but moving patches instead so I guess the source of the problem is the same...
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   December 11, 2012, 03:20
Default
  #12
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 6
Ralph M is on a distinguished road
Quote:
Originally Posted by Ralph M View Post
Adding "global" didn't worked for me either! I've got no cyclic patches but moving patches instead so I guess the source of the problem is the same...
The problem is with the decomposition method and doesn't occur with scotch or simple. Try to decompose your case with one of the two mentioned decomposers and check your files (pointDisplacement). You'll find after the processorPatches something like this:
Code:
global
{
type      global;
}
This should solve your problem (at least it solved mine )

Cheers,

Ralph
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Reply

Tags
interdymfoam, parallel

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
Problems in mesh motion solutor in parallel 4 interDyMFoam. DLC Main CFD Forum 0 November 21, 2009 17:17
Problems in mesh motion solutor in parallel 4 interDyMFoam. DLC OpenFOAM 0 November 21, 2009 09:54
mesh motion samad87 FLUENT 0 August 6, 2009 03:15
Mesh motion Hex cells vs tets kev4573 OpenFOAM Running, Solving & CFD 6 December 13, 2007 15:37
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 09:55.