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

reactingParcelFilmFoam parallel

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 28, 2011, 02:49
Default reactingParcelFilmFoam parallel
  #1
Member
 
Antoine Devesa
Join Date: Mar 2010
Posts: 36
Rep Power: 7
A.Devesa is on a distinguished road
Hello everybody,

could anyone please tell me, if the new solver reactingParcelFilmFoam (OF 2.0) can run in parallel. If yes, what do I need to do while decomposing? I tried several things, but I can't get a parallel simulation running with a surface film.

Thank you in advance!
Antoine
A.Devesa is offline   Reply With Quote

Old   July 28, 2011, 03:45
Default
  #2
New Member
 
Dima Risch
Join Date: Jun 2011
Location: Cologne
Posts: 22
Rep Power: 6
dima is on a distinguished road
hi Antoine

the new solver reactingParcelFilmFoam can run in parallel

so take a look to the hotBoxes tutorial

there is a Allrun-parallel script using decomposePar for both, the wallFilmRegion and the primaryRegion

if necessary modify the decomposeParDicts and the Allrun-parallel script

hope this helps
dima is offline   Reply With Quote

Old   April 12, 2012, 09:08
Default
  #3
New Member
 
Roman Fuchs
Join Date: Apr 2012
Location: Rapperswil, Switzerland
Posts: 4
Rep Power: 5
HPC on the Lake is on a distinguished road
The provided tutorial also crashes on my computer, caused by a segmentation fault. (see below, end of log.reactingParcelFilmFoam)

Other tutorials running in parallel are fine.

I installed OpenFoam 2.1.0, on Linux.

Anyone an idea where to check? Thanks!


...
Selecting composition model singlePhaseMixture
Selecting phase change model none
Selecting radiationModel none
Constructing surface film model
Selecting surfaceFilmModel thermoSingleLayer
[0] #0 Foam::error:rintStack(Foam::Ostream&)[1] #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #1 Foam::sigSegv::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #1 Foam::sigSegv::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #2 in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #2 in "/lib/libc.so.6"
[1] #3 Foam::UOPstream::write(char) in "/lib/libc.so.6"
[0] #3 Foam::UOPstream::write(char) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #4 Foam::UOPstream::write(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #4 Foam::UOPstream::write(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #5 Foam:perator<<(Foam::Ostream&, int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #5 Foam:perator<<(Foam::Ostream&, int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #6 in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #6 Foam::Ostream& Foam:perator<< <int>(Foam::Ostream&, Foam::UList<int> const&)Foam::Ostream& Foam:perator<< <int>(Foam::Ostream&, Foam::UList<int> const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/reactingParcelFilmFoam"
[0] #7 Foam:rocessorPolyPatch::initUpdateMesh(Foam::Pst reamBuffers&) in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/reactingParcelFilmFoam"
[1] #7 Foam:rocessorPolyPatch::initUpdateMesh(Foam::Pst reamBuffers&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
...
[hnordbor-laptop:09290] *** Process received signal ***
[hnordbor-laptop:09290] Signal: Segmentation fault (11)
[hnordbor-laptop:09290] Signal code: (-6)
[hnordbor-laptop:09290] Failing at address: 0x3ea0000244a
[hnordbor-laptop:09290] [ 0] /lib/libc.so.6(+0x33af0) [0x7f08a166eaf0]
[hnordbor-laptop:09290] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7f08a166ea75]
[hnordbor-laptop:09290] [ 2] /lib/libc.so.6(+0x33af0) [0x7f08a166eaf0]
[hnordbor-laptop:09290] [ 3] /opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam9UOPstream5writeEc+0x91) [0x7f08a255c711]
...
HPC on the Lake is offline   Reply With Quote

Old   April 13, 2012, 04:06
Default
  #4
Senior Member
 
Markus Rehm
Join Date: Mar 2009
Location: Erlangen (Germany)
Posts: 177
Rep Power: 8
markusrehm is on a distinguished road
Hi,

I have similar issues but haven't investigated further. Does the error appear also with a tutorial?

Markus
markusrehm is offline   Reply With Quote

Old   April 13, 2012, 05:12
Default
  #5
New Member
 
Roman Fuchs
Join Date: Apr 2012
Location: Rapperswil, Switzerland
Posts: 4
Rep Power: 5
HPC on the Lake is on a distinguished road
It IS (!) a tutorial:
tutorials/lagrangian/reactingParcelFilmFoam/hotBoxes

I'm running OpenFOAM version 2.1.0.
HPC on the Lake is offline   Reply With Quote

Old   April 13, 2012, 05:29
Default
  #6
New Member
 
Dima Risch
Join Date: Jun 2011
Location: Cologne
Posts: 22
Rep Power: 6
dima is on a distinguished road
Hi Roman,

do you run the ./Allrun-parallel skript unchaneged?

how many cores/processors do u use?

i do this tutorial with OF2.0.0
and today i try it with OF2.1.x

dima
dima is offline   Reply With Quote

Old   April 13, 2012, 07:11
Default
  #7
New Member
 
Roman Fuchs
Join Date: Apr 2012
Location: Rapperswil, Switzerland
Posts: 4
Rep Power: 5
HPC on the Lake is on a distinguished road
Hi Dima,

Yes, I run the script unchanged. I run it on Linux/Ubuntu in a Virtual Machine on Windows 7 on a Laptop with 4 processors. I tried 2 and 4.

Roman
HPC on the Lake is offline   Reply With Quote

Old   April 13, 2012, 08:02
Default
  #8
New Member
 
Dima Risch
Join Date: Jun 2011
Location: Cologne
Posts: 22
Rep Power: 6
dima is on a distinguished road
i tried it right now with 2 processors on openSuse

settings are in:

the Allrun-parallel script: runParallel $application 2

the system/decomposeParDict: numberOfSubdomains 2;

aswell the system/wallFilmRegion/decomposeParDict: numberOfSubdomains 2;

and it runs fine

Code:
...
Selecting composition model singlePhaseMixture
Selecting phase change model none
Selecting radiationModel none

Constructing surface film model
Selecting surfaceFilmModel thermoSingleLayer
    Selecting film injection models
        curvatureSeparation
        drippingInjection
Selecting distribution model RosinRammler
    Selecting film force models
        surfaceShear
        thermocapillary
        contactAngle
Selecting distribution model normal
    Selecting heatTransferModel mappedConvectiveHeatTransfer
    Selecting heatTransferModel constant
    Selecting phaseChangeModel standardPhaseChange
    Selecting radiationModel none
Courant Number mean: 0 max: 0

PIMPLE: Operating solver in PISO mode


Starting time loop

Courant Number mean: 0 max: 0
Film max Courant number: 0
deltaT = 0.0001436781609
Time = 0.000143678


Solving cloud reactingCloud1
Cloud: reactingCloud1
    Current number of parcels       = 0
    Current mass in system          = 0
    Linear momentum                 = (0 0 0)
   |Linear momentum|                = 0
    Linear kinetic energy           = 0
    Rotational kinetic energy       = 0
    Total number of parcels added   = 0
    Total mass introduced           = 0
    Parcels absorbed into film      = 0
    New film detached parcels       = 0
    New film splash parcels         = 0
    Parcel fate (number, mass)
      - escape                      = 0, 0
      - stick                       = 0, 0
    Mass transfer phase change      = 0


Evolving thermoSingleLayer for region wallFilmRegion
diagonal:  Solving for deltaf*rhof, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ufx, Initial residual = 0.9912919068, Final residual = 1.494629846e-17, No Iterations 1
smoothSolver:  Solving for Ufy, Initial residual = 0.9904653317, Final residual = 1.351398412e-17, No Iterations 1
smoothSolver:  Solving for Ufz, Initial residual = 0.9973363737, Final residual = 1.047149797e-17, No Iterations 1
smoothSolver:  Solving for hsf, Initial residual = 1, Final residual = 2.147073609e-19, No Iterations 1
smoothSolver:  Solving for deltaf, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for deltaf*rhof, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for deltaf, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for deltaf*rhof, Initial residual = 0, Final residual = 0, No Iterations 0

Surface film: thermoSingleLayer
    added mass         = 0
    current mass       = 0
    min/max(mag(U))    = 0, 1.643271902e-21
    min/max(delta)     = 0, 0
    injected mass      = 0
    min/max(T)         = 350, 350
    mass phase change  = 0
    vapourisation rate = 0

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 0.999999712, Final residual = 1.919568944e-06, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.9999997108, Final residual = 1.865176847e-06, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 3.672946737e-06, No Iterations 1
DILUPBiCG:  Solving for O2, Initial residual = 3.316429488e-05, Final residual = 1.064336272e-10, No Iterations 1
DILUPBiCG:  Solving for H2O, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for hs, Initial residual = 0.9999998726, Final residual = 2.498188599e-08, No Iterations 1
min/max(T) = 300, 350
GAMG:  Solving for p_rgh, Initial residual = 0.004945224294, Final residual = 0.0002832043458, No Iterations 2
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 2.402975678e-08, global = -7.22322855e-11, cumulative = -7.22322855e-11
GAMG:  Solving for p_rgh, Initial residual = 0.0002832555659, Final residual = 5.552262167e-07, No Iterations 4
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 4.689062126e-11, global = -1.044844441e-13, cumulative = -7.233676995e-11
DILUPBiCG:  Solving for epsilon, Initial residual = 2.208707685e-05, Final residual = 4.212265024e-11, No Iterations 1
DILUPBiCG:  Solving for k, Initial residual = 0.9999964134, Final residual = 1.87348777e-06, No Iterations 1
ExecutionTime = 22.55 s  ClockTime = 24 s
...
so it seems to be a virtual machine or maybe a OF-version problem

Dima
dima is offline   Reply With Quote

Old   April 18, 2012, 02:22
Default
  #9
New Member
 
Roman Fuchs
Join Date: Apr 2012
Location: Rapperswil, Switzerland
Posts: 4
Rep Power: 5
HPC on the Lake is on a distinguished road
The problem is fixed in OpenFOAM version 2.1.x, i.e. when using the repository release. Simply download the repository release and build the code; it takes hours, unfortunately.

Thanks for working together!
HPC on the Lake 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
Script to Run Parallel Jobs in Rocks Cluster asaha OpenFOAM Running, Solving & CFD 12 July 4, 2012 22:51
parallel performance on BX900 uzawa OpenFOAM Installation on Windows, Mac and other Unsupported Platforms 3 September 5, 2011 15:52
HP MPI warning...Distributed parallel processing Peter CFX 10 May 14, 2011 06:17
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58
Parallel Computing Classes at San Diego Supercomputer Center Jan. 20-22 Amitava Majumdar Main CFD Forum 0 January 5, 1999 13:00


All times are GMT -4. The time now is 01:10.