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

mapFields taking too long

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

Like Tree4Likes
  • 4 Post By Carlen

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 29, 2015, 12:18
Default mapFields taking too long
  #1
Member
 
Join Date: Jul 2012
Posts: 67
Rep Power: 9
Carlen is on a distinguished road
Hi foamers,

I am facing a problem of mapFields taking too long to map fields from a fine mesh to a coarser mesh. I am running simulation using sprayFoam, and want to coarse the mesh to achieve faster solution. So I executed:

Code:
mpirun -n 4 mapFields ../aachenBomb-fine -sourceTime latestTime  -consistent -parallel
in the aacheBomb-coarse directory and it is running without errors. However, it gets stuck at here for four hours:
Code:
 Create meshes

Source mesh size: 42025    Target mesh size: 42025


Consistently creating and mapping fields for time 0.0004

Creating mesh-to-mesh addressing for region0 and region0 regions using cellVolumeWeight
    Overlap volume: 4e-05
Creating AMI between source patch walls and target patch walls using faceAreaWeightAMI
    AMI: Creating addressing and weights between 19762 source faces and 19762 target faces
    AMI: Patch source sum(weights) min/max/average = 1, 1, 1
    AMI: Patch target sum(weights) min/max/average = 1, 1, 1
    interpolating mut
    interpolating rho
    interpolating PaSR:kappa
    interpolating k
    interpolating H2O
    interpolating PaSR:dQ
    interpolating alphat
    interpolating N2
    interpolating O2
    interpolating dQ
    interpolating p
    interpolating T
    interpolating epsilon
    interpolating U

    processing cloud "sprayCloud"
Anybody knows what is wrong?

kind regards,
carlen

PS: I am using OF2.3.1

Last edited by wyldckat; March 29, 2015 at 13:02. Reason: merged posts that were 2 minutes apart and added [CODE][/CODE]
Carlen is offline   Reply With Quote

Old   March 29, 2015, 13:04
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,955
Blog Entries: 43
Rep Power: 121
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer: http://www.openfoam.org/mantisbt/view.php?id=1326#c3694
Quote:
Originally Posted by mattijs
The parallel mapFields uses conservative mapping ('cellVolumeWeight') by default which is slow since it has to do full tet-tet overlap calculations. The old behaviour is like the 'direct' method. Does using this method help?
wyldckat is offline   Reply With Quote

Old   March 29, 2015, 21:50
Default
  #3
Member
 
Join Date: Jul 2012
Posts: 67
Rep Power: 9
Carlen is on a distinguished road
Hi Bruno,
Thank you for kindly moving my thread to an appropriate section. I will try the direct method and let you know if the execution time is reduced.

Best regards,
carlen
Carlen is offline   Reply With Quote

Old   March 29, 2015, 22:38
Default
  #4
Member
 
Join Date: Jul 2012
Posts: 67
Rep Power: 9
Carlen is on a distinguished road
Hi bruno,

I have tried using direct mapMethod and now it gets to this state much faster (2s):

Code:
Source time: 0.0004
Target time: 0

Create meshes

Source mesh size: 42025	Target mesh size: 42025


Consistently creating and mapping fields for time 0.0004

Creating mesh-to-mesh addressing for region0 and region0 regions using direct
    Overlap volume: 4e-05
Creating AMI between source patch walls and target patch walls using directAMI
    AMI: Creating addressing and weights between 19762 source faces and 19762 target faces
    AMI: Patch source sum(weights) min/max/average = 1, 1, 1
    AMI: Patch target sum(weights) min/max/average = 1, 2, 1.0022
    interpolating mut
    interpolating rho
    interpolating PaSR:kappa
    interpolating k
    interpolating H2O
    interpolating PaSR:dQ
    interpolating alphat
    interpolating N2
    interpolating O2
    interpolating dQ
    interpolating p
    interpolating T
    interpolating epsilon
    interpolating U

    processing cloud "sprayCloud"
However, it still remains at such a state for way too long. More strangely, if I change the executing line from:

Code:
mpirun -n 4 mapFields ../aachenBomb-twoparcels -mapMethod direct -sourceTime latestTime -consistent -parallel
to

Code:
mpirun -n 4 mapFields ../aachenBomb-twoparcels -mapMethod direct  -consistent -parallel
and I modify the startTime in the controlDict of the source case to 0.0004. it finishes almost immediately but without showing
Code:
processing cloud "sprayCloud"
in the terminal window.I guess the sprayCloud properties are not mapped.

How can I solve this problem?
Carlen is offline   Reply With Quote

Old   March 30, 2015, 00:47
Default
  #5
Member
 
Join Date: Jul 2012
Posts: 67
Rep Power: 9
Carlen is on a distinguished road
Hi everyone,

I think I found a solution for this problem, I now type in
Code:
mpirun -n 4 mapFields ../aachenBomb-twoparcels -mapMethod direct -sourceTime latestTime -consistent -noLagrangian -parallel
Code:
Source time: 0.0004
Target time: 0

Create meshes

Source mesh size: 42025	Target mesh size: 42025


Consistently creating and mapping fields for time 0.0004

Creating mesh-to-mesh addressing for region0 and region0 regions using direct
    Overlap volume: 4e-05
Creating AMI between source patch walls and target patch walls using directAMI
    AMI: Creating addressing and weights between 19762 source faces and 19762 target faces
    AMI: Patch source sum(weights) min/max/average = 1, 1, 1
    AMI: Patch target sum(weights) min/max/average = 1, 2, 1.0022
    interpolating mut
    interpolating rho
    interpolating PaSR:kappa
    interpolating k
    interpolating H2O
    interpolating PaSR:dQ
    interpolating alphat
    interpolating N2
    interpolating O2
    interpolating dQ
    interpolating p
    interpolating T
    interpolating epsilon
    interpolating U

End

Finalising parallel run
It runs without mapping the lagrangian fields which is actually what I wanted in the first place (not allowing sprayParcels to be mapped)

Cheers,
Carlen is offline   Reply With Quote

Old   March 30, 2015, 01:18
Default
  #6
Member
 
Join Date: Jul 2012
Posts: 67
Rep Power: 9
Carlen is on a distinguished road
Carlen again,
I found that it is problematic to run simulation for the mapped case without mapping the lagrangian fields. it gives so many errors that I cannot find a solution for.
Code:
[[A[carlen@localhost aachenBomb-mapFields]$ mpirun -carlenSprayFoam -parallel
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.1-262087cdf8db
Exec   : carlenSprayFoam -parallel
Date   : Mar 30 2015
Time   : 15:14:11
Host   : "localhost.localdomain"
PID    : 13054
Case   : /home/carlen/OpenFOAM/carlen-2.3.1/carlenVOFLPT/run/aachenBomb-mapFields
nProcs : 4
Slaves : 
3
(
"localhost.localdomain.13055"
"localhost.localdomain.13056"
"localhost.localdomain.13057"
)

Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


Reading g
Creating combustion model

Selecting combustion model PaSR<psiChemistryCombustion>
Selecting chemistry type 
{
    chemistrySolver ode;
    chemistryThermo psi;
}

Selecting thermodynamics package 
{
    type            hePsiThermo;
    mixture         reactingMixture;
    transport       sutherland;
    thermo          janaf;
    energy          sensibleEnthalpy;
    equationOfState perfectGas;
    specie          specie;
}

Selecting chemistryReader chemkinReader
Reading CHEMKIN thermo data in new file format
[2] #0  Foam::error::printStack(Foam::Ostream&)[0] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[2] #1  Foam::sigFpe::sigHandler(int) at ??:?
[0] #1  Foam::sigFpe::sigHandler(int) at ??:?
[2] #2  
 at ??:?
[0] #2  
[2]  at sigaction.c:?
[2] #3  double Foam::max<Foam::fvPatchField, double>(Foam::FieldField<Foam::fvPatchField, double> const&)[0]  at sigaction.c:?
[0] #3   at ??:?
[2] #4  double Foam::max<Foam::fvPatchField, double>(Foam::FieldField<Foam::fvPatchField, double> const&)Foam::dimensioned<double> Foam::max<double, Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
[0] #4   at ??:?
[2] #5  Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::correctMassFractions()Foam::dimensioned<double> Foam::max<double, Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
[2] #6  Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::multiComponentMixture(Foam::dictionary const&, Foam::List<Foam::word> const&, Foam::HashPtrTable<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> >, Foam::word, Foam::string::hash> const&, Foam::fvMesh const&) at ??:?
[0] #5  Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::correctMassFractions() at ??:?
[2] #7  Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::reactingMixture(Foam::dictionary const&, Foam::fvMesh const&) at ??:?
[0] #6  Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::multiComponentMixture(Foam::dictionary const&, Foam::List<Foam::word> const&, Foam::HashPtrTable<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> >, Foam::word, Foam::string::hash> const&, Foam::fvMesh const&) at ??:?
[2] #8  Foam::heThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::heThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
[0] #7  Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::reactingMixture(Foam::dictionary const&, Foam::fvMesh const&) at ??:?
[2] #9  Foam::psiReactionThermo::addfvMeshConstructorToTable<Foam::hePsiThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > > >::New(Foam::fvMesh const&, Foam::word const&) at ??:?
[0] #8  Foam::heThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::heThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
[2] #10  Foam::autoPtr<Foam::psiReactionThermo> Foam::basicThermo::New<Foam::psiReactionThermo>(Foam::fvMesh const&, Foam::word const&) at ??:?
[0] #9  Foam::psiReactionThermo::addfvMeshConstructorToTable<Foam::hePsiThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > > >::New(Foam::fvMesh const&, Foam::word const&) at ??:?
[2] #11  Foam::psiReactionThermo::New(Foam::fvMesh const&, Foam::word const&) at ??:?
[0] #10  Foam::autoPtr<Foam::psiReactionThermo> Foam::basicThermo::New<Foam::psiReactionThermo>(Foam::fvMesh const&, Foam::word const&) at ??:?
[2] #12  Foam::psiChemistryModel::psiChemistryModel(Foam::fvMesh const&) at ??:?
[0] #11  Foam::psiReactionThermo::New(Foam::fvMesh const&, Foam::word const&) at ??:?
[2] #13  Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::chemistryModel(Foam::fvMesh const&) at ??:?
[2] #14  Foam::ode<Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::ode(Foam::fvMesh const&) at ??:?
[0] #12  Foam::psiChemistryModel::psiChemistryModel(Foam::fvMesh const&) at ??:?
[2] #15  Foam::psiChemistryModel::addfvMeshConstructorToTable<Foam::ode<Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&) at ??:?
[0] #13  Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::chemistryModel(Foam::fvMesh const&) at ??:?
[2] #16  Foam::autoPtr<Foam::psiChemistryModel> Foam::basicChemistryModel::New<Foam::psiChemistryModel>(Foam::fvMesh const&) at ??:?
[0] #14  Foam::ode<Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::ode(Foam::fvMesh const&) at ??:?
[2] #17  Foam::psiChemistryModel::New(Foam::fvMesh const&) at ??:?
[0] #15  Foam::psiChemistryModel::addfvMeshConstructorToTable<Foam::ode<Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&) at ??:?
[2] #18  Foam::combustionModels::psiChemistryCombustion::psiChemistryCombustion(Foam::word const&, Foam::fvMesh const&) at ??:?
[0] #16  Foam::autoPtr<Foam::psiChemistryModel> Foam::basicChemistryModel::New<Foam::psiChemistryModel>(Foam::fvMesh const&) at ??:?
[2] #19  Foam::combustionModels::laminar<Foam::combustionModels::psiChemistryCombustion>::laminar(Foam::word const&, Foam::fvMesh const&) at ??:?
[0] #17  Foam::psiChemistryModel::New(Foam::fvMesh const&) at ??:?
[2] #20  Foam::combustionModels::PaSR<Foam::combustionModels::psiChemistryCombustion>::PaSR(Foam::word const&, Foam::fvMesh const&) at ??:?
[2] #21  Foam::combustionModels::psiCombustionModel::adddictionaryConstructorToTable<Foam::combustionModels::PaSR<Foam::combustionModels::psiChemistryCombustion> >::New(Foam::word const&, Foam::fvMesh const&) at ??:?
[0] #18  Foam::combustionModels::psiChemistryCombustion::psiChemistryCombustion(Foam::word const&, Foam::fvMesh const&) at ??:?
[2] #22  Foam::combustionModels::psiCombustionModel::New(Foam::fvMesh const&) at ??:?
[0] #19  Foam::combustionModels::laminar<Foam::combustionModels::psiChemistryCombustion>::laminar(Foam::word const&, Foam::fvMesh const&) at ??:?
[2] #23   at ??:?
[0] #20  Foam::combustionModels::PaSR<Foam::combustionModels::psiChemistryCombustion>::PaSR(Foam::word const&, Foam::fvMesh const&)
 at ??:?
[0] #21  Foam::combustionModels::psiCombustionModel::adddictionaryConstructorToTable<Foam::combustionModels::PaSR<Foam::combustionModels::psiChemistryCombustion> >::New(Foam::word const&, Foam::fvMesh const&) at ??:?
[0] #22  Foam::combustionModels::psiCombustionModel::New(Foam::fvMesh const&)[2]  at ??:?
[2] #24  __libc_start_main at ??:?
[2] #25   at ??:?
[0] #23  

[2]  at ??:?
[localhost:13056] *** Process received signal ***
[localhost:13056] Signal: Floating point exception (8)
[localhost:13056] Signal code:  (-6)
[localhost:13056] Failing at address: 0x1f400003300
[localhost:13056] [ 0] /lib64/libc.so.6[0x3621c326a0]
[localhost:13056] [ 1] /lib64/libc.so.6(gsignal+0x35)[0x3621c32625]
[localhost:13056] [ 2] /lib64/libc.so.6[0x3621c326a0]
[localhost:13056] [ 3] carlenSprayFoam(_ZN4Foam3maxINS_12fvPatchFieldEdEET0_RKNS_10FieldFieldIT_S2_EE+0xdc)[0x449b5c]
[localhost:13056] [ 4] 
[localhost:13054] [23] carlenSprayFoam[0x42dffa]
[localhost:13054] [24] /lib64/libc.so.6(__libc_start_main+0xfd)[0x3621c1ed5d]
[localhost:13054] [25] carlenSprayFoam[0x4338e5]
[localhost:13054] *** End of error message ***
[localhost:13057] *** An error occurred in MPI_Pack
[localhost:13057] *** reported by process [140187236761601,140733193388035]
[localhost:13057] *** on a NULL communicator
[localhost:13057] *** Unknown error
[localhost:13057] *** MPI_ERRORS_ARE_FATAL (processes in this communicator will now abort,
[localhost:13057] ***    and potentially your MPI job)
--------------------------------------------------------------------------
mpirun noticed that process rank 0 with PID 13054 on node localhost exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------
How can I solve this problem?
Carlen is offline   Reply With Quote

Old   March 30, 2015, 01:30
Default
  #7
Member
 
Join Date: Jul 2012
Posts: 67
Rep Power: 9
Carlen is on a distinguished road
Hi everyone,
its carlen again. It is hilarious I have been talking to myself and get the solution by myself . Anyway, I figured out how to solve the problem. By looking into the 0 folder, I realise that only T, p, U fields are needed for such a simulation. So I type in:
Code:
mpirun -n 4 mapFields ../aachenBomb-twoparcels -mapMethod direct -sourceTime latestTime -fields '(U T p)' -consistent -noLagrangian -parallel
and it only maps the required fields for sprayFoam. Then simulation the runs perfectly fine. Hope this is helpful to those who have the same problem.

Cheers,
Carlen
Carlen is offline   Reply With Quote

Old   March 30, 2015, 01:53
Default
  #8
Member
 
Join Date: Jul 2012
Posts: 67
Rep Power: 9
Carlen is on a distinguished road
Now you can see the pressure field is identical for both the source and target case!
Attached Images
File Type: png 12.png (10.2 KB, 91 views)
Carlen is offline   Reply With Quote

Old   March 30, 2015, 06:19
Default
  #9
Member
 
Join Date: Jul 2012
Posts: 67
Rep Power: 9
Carlen is on a distinguished road
it turns out that I have to use
Code:
-mapMethod cellVolumeWeight
because "direct" method requires both the source and target to be identical. It is still time consuming for large cases. I wonder if OpenFoam has a faster implementation of such a process.

carlen
Carlen is offline   Reply With Quote

Old   April 4, 2015, 14:44
Default
  #10
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,955
Blog Entries: 43
Rep Power: 121
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Hi Carlen,

Many thanks for sharing each step you've done!

As for a faster method, have you tried using "-mapMethod mapNearest"? It should be faster, although it will strongly depend on how related the fine mesh is to the coarse mesh, i.e. if the fine mesh is simply the coarse refined for some or all cells in a 2x2x2 division for each cell.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Reply

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
Problem with pow and volScalarField _Stefan_ OpenFOAM Programming & Development 15 April 14, 2019 23:20
Transient Simulation Taking Very Long TIME!!!! Help 88phil88 CFX 17 November 3, 2017 05:07
Transient run taking too long time Alexander Tham Keat Fu CFX 3 June 20, 2012 07:53
OpenFOAM-1.5-dev svn revision 1438: libOpenFOAM does not compile in SP 4xF OpenFOAM Bugs 3 October 16, 2009 06:35
Missing math.h header Travis FLUENT 4 January 15, 2009 12:48


All times are GMT -4. The time now is 12:10.