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

interDyMFoam problem

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

Like Tree2Likes
  • 2 Post By MartinB

Reply
 
LinkBack Thread Tools Display Modes
Old   May 17, 2011, 15:50
Default interDyMFoam problem
  #1
New Member
 
huxiaoxia
Join Date: Oct 2010
Posts: 18
Rep Power: 6
huxiaoxia is on a distinguished road
Hi,

I run a case with interDyMFoam for liquild flim flow, but it always shows the error "field does not correspond to level 0 sizes" after running for a few minutes. Can anybody help me ?

huxiaoxia is offline   Reply With Quote

Old   June 28, 2011, 11:17
Default problem for interDyMFoam
  #2
New Member
 
huxiaoxia
Join Date: Oct 2010
Posts: 18
Rep Power: 6
huxiaoxia is on a distinguished road
When I run the case for water film flowing on the substrate with the interDyMFoam, it gives me the error" FOAM FATAL ERROR:
field does not correspond to level 0 sizes: field = 1228021 level = 1200000
From function void GAMGAgglomeration::restrictField(Field<Type>& cf, const Field<Type>& ff, const label fineLevelIndex) const
in file lnInclude/GAMGAgglomerationTemplates.C at line 47.
FOAM aborting
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 void Foam::GAMGAgglomeration::restrictField<double>(Foa m::Field<double>&, Foam::Field<double> const&, int) const in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#3 Foam::GAMGSolver::agglomerateMatrix(int) in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::GAMGSolver::GAMGSolver(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::dictionary const&) in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#5 Foam::GAMGPreconditioner::GAMGPreconditioner(Foam: :lduMatrix::solver const&, Foam::dictionary const&) in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#6 Foam::lduMatrix:reconditioner::addsymMatrixConst ructorToTable<Foam::GAMGPreconditioner>::New(Foam: :lduMatrix::solver const&, Foam::dictionary const&) in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#7 Foam::lduMatrix:reconditioner::New(Foam::lduMatr ix::solver const&, Foam::dictionary const&) in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#8 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#9 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libfiniteVolume.so"
#10 main in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/interDyMFoam"
#11 __libc_start_main in "/lib64/libc.so.6"
#12 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/huxiaoxi/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/interDyMFoam"
Aborted"
Is there anyone who knows what happens here?
huxiaoxia is offline   Reply With Quote

Old   June 28, 2011, 13:04
Default
  #3
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 11
MartinB is on a distinguished road
Hi,

try setting:

cacheAgglomeration true;

to

cacheAgglomeration false;

for all GAMG preconditioners and solvers in system/fvSolution.

Martin
MartinB is offline   Reply With Quote

Old   June 29, 2011, 11:30
Default interDyMFoam
  #4
New Member
 
huxiaoxia
Join Date: Oct 2010
Posts: 18
Rep Power: 6
huxiaoxia is on a distinguished road
Thanks a lot. I try it and it works.
huxiaoxia is offline   Reply With Quote

Old   August 10, 2011, 02:40
Default
  #5
Member
 
liping_he
Join Date: Feb 2011
Posts: 34
Rep Power: 5
liping_he is on a distinguished road
Hello martinB


I run a case with interDyMFoam for liquid jet flow. And I use LES as my turbulent model. But, OpenFOAM complains a error “field does not correspond to level 0 sizes……”. And I do a change on my case as you said above. It works well.

Now , I want to know why we need to do this change.



Thanks very much
liping_he is offline   Reply With Quote

Old   August 10, 2011, 03:59
Default
  #6
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 11
MartinB is on a distinguished road
Hi,

I did not search for the reason in the source code, but the general idea of caching is: store the result or intermediate results and reuse them later to speed up computation. In the case of a dynamic mesh the size and composition of data structures change, because new cells come in, some cells go out. The stored cache is no longer valid and has to be dropped. If the source code does not account for this situation automatically, you must disable the caching completely, as it is done by the "cacheAgglomeration false;" flag.

Martin
nimasam and m_mousavi88 like this.
MartinB is offline   Reply With Quote

Old   August 10, 2011, 05:09
Default
  #7
Member
 
liping_he
Join Date: Feb 2011
Posts: 34
Rep Power: 5
liping_he is on a distinguished road
Hello martinB

Thanks for your patient explaination. Thank you very much.

liping_he
liping_he is offline   Reply With Quote

Old   August 10, 2011, 22:15
Default
  #8
Member
 
liping_he
Join Date: Feb 2011
Posts: 34
Rep Power: 5
liping_he is on a distinguished road
Hi Martin

I run a case using interDyMFoam solver in parallel. It works well. But when I want to use the command 'reconstructPar' to reconstrct mesh and data the computer complain ' cannot find file: /home/he/mywork/damBreakWithObstacle/processor0/0.02/polyMesh/pointProcAddressing at line 0.'
I want to know what is wrong with it and how I should do to reconstruct the case.

Thanks very much

Liping
liping_he is offline   Reply With Quote

Old   August 11, 2011, 00:04
Default
  #9
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 11
MartinB is on a distinguished road
Hi liping,

you must reconstruct the mesh first with "reconstructParMesh", then you can reconstruct the data with "reconstructPar".

You can try the script from this thread, too:
Reconstruction after parallel run with dynamic mesh refinement

Martin
MartinB 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
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Partitioning problem with interDyMFoam DLC OpenFOAM 0 March 7, 2011 17:28
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52


All times are GMT -4. The time now is 10:22.