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

Parallel using icoLagrangianFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 24, 2009, 05:51
Default Parallel using icoLagrangianFoam
  #1
Senior Member
 
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 9
flying is on a distinguished road
Hey Foamers:

It is very my pleasure to discuss the parallel running of icoLagrangianFoam.

When I use icoLagrangianFoam, at first I use the command' decomposePar' and there are two folders of 'processor0' and 'processor1' to be created. And then I used the command of ''mpriun -np icoLagrangianFoam'.

The case is run, but there is no result to be saved in the folder of 'processor1'and'processor0', and the result is saved under the folder of case.

I feel a little confused whether the icoLangrangianFoam could be run paralleled or the result is saved under the folder of case other in the 'processor*`. Would anyone like to help me for the question?

Thanks and best wishes!
flying is offline   Reply With Quote

Old   August 24, 2009, 07:58
Default
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by flying View Post
Hey Foamers:

It is very my pleasure to discuss the parallel running of icoLagrangianFoam.

When I use icoLagrangianFoam, at first I use the command' decomposePar' and there are two folders of 'processor0' and 'processor1' to be created. And then I used the command of ''mpriun -np icoLagrangianFoam'.

The case is run, but there is no result to be saved in the folder of 'processor1'and'processor0', and the result is saved under the folder of case.

I feel a little confused whether the icoLangrangianFoam could be run paralleled or the result is saved under the folder of case other in the 'processor*`. Would anyone like to help me for the question?

Thanks and best wishes!
Try again with
mpriun -np 2 icoLagrangianFoam -parallel
(what you did was run two serial runs in parallel

Bernhard
gschaider is offline   Reply With Quote

Old   August 24, 2009, 09:48
Default
  #3
Senior Member
 
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 9
flying is on a distinguished road
Sincerely thanks! And it is work now. But for running paralleled with two processors is even slower than one processor.
flying is offline   Reply With Quote

Old   August 24, 2009, 10:00
Default
  #4
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by flying View Post
Sincerely thanks! And it is work now. But for running paralleled with two processors is even slower than one processor.
For small cases that is not surprising, because the communication needs more time than the actual calculation
gschaider is offline   Reply With Quote

Old   August 24, 2009, 12:06
Default
  #5
Senior Member
 
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 9
flying is on a distinguished road
Thanks a lot
flying is offline   Reply With Quote

Old   November 9, 2009, 03:37
Default
  #6
Senior Member
 
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 9
flying is on a distinguished road
Long time no see. And wish all foamers are fine.

There are big bugs on "icoLagrangianFoam" in the case of paralleling computing. There is no problem for the case are computed using one process. If the mesh is decomposed in the z direction for cavity, the particle could be moved, but the result is different with case of using one process, it is the same situation for the y direction. The worst thing is that the particles can not be moved if it is decomposed in x direction after the computation starts some steps. It is absolutely there is some problem for the particle transfered between processors.

Does anyone also find the bug?
It is very sad I know few about the part of transfer field of particles. Who would like to give me some advice on it?

Thanks and best wishes!
flying is offline   Reply With Quote

Old   November 9, 2009, 06:50
Default
  #7
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by flying View Post
Long time no see. And wish all foamers are fine.

There are big bugs on "icoLagrangianFoam" in the case of paralleling computing. There is no problem for the case are computed using one process. If the mesh is decomposed in the z direction for cavity, the particle could be moved, but the result is different with case of using one process, it is the same situation for the y direction. The worst thing is that the particles can not be moved if it is decomposed in x direction after the computation starts some steps. It is absolutely there is some problem for the particle transfered between processors.

Does anyone also find the bug?
It is very sad I know few about the part of transfer field of particles. Who would like to give me some advice on it?

Thanks and best wishes!
Before we start talking: which version? (OpenFOAM and icoLagrangianFoam)

I just had a quick look at the latest version and noticed that in method HardBallParticle::hitProcessorPatch it reads
td.switchProcessor=false;
where in my opinion it should be
td.switchProcessor=true;
but I'm not 100% sure whether this will fix it and I havn't got the time to test it

Bernhard
gschaider is offline   Reply With Quote

Old   November 9, 2009, 11:57
Default
  #8
Senior Member
 
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 9
flying is on a distinguished road
It is icoLangrangianFoam for OpenFoam 1.5.

In the HardBallParticle.C, there is no lines in the member function of HardBallParticle::hitProcessorPatch. Maybe I should add these lines. I will try it. Thanks a lot.
flying is offline   Reply With Quote

Old   November 9, 2009, 17:45
Default
  #9
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by flying View Post
It is icoLangrangianFoam for OpenFoam 1.5.

In the HardBallParticle.C, there is no lines in the member function of HardBallParticle::hitProcessorPatch. Maybe I should add these lines. I will try it. Thanks a lot.
There are two such methods. One is empty. The other not.
gschaider is offline   Reply With Quote

Old   May 31, 2010, 02:42
Unhappy
  #10
Member
 
foamWang's Avatar
 
Roro Wang
Join Date: Mar 2010
Location: Cambridge, MA, USA
Posts: 30
Rep Power: 8
foamWang is on a distinguished road
Hi Bernhard,

Yes, this solves the problem.
However, if I set useMomentumSource to 1, i.e. two-way coupling of solid and fluid phase, a extremely high value of Co will be achieved. This obviously not physical. This may be dedicated to the suddenly appearance of particles in a new processor.

Any idea to solve this?

Thanks.

Roro

Quote:
Originally Posted by gschaider View Post
Before we start talking: which version? (OpenFOAM and icoLagrangianFoam)

I just had a quick look at the latest version and noticed that in method HardBallParticle::hitProcessorPatch it reads
td.switchProcessor=false;
where in my opinion it should be
td.switchProcessor=true;
but I'm not 100% sure whether this will fix it and I havn't got the time to test it

Bernhard
foamWang is offline   Reply With Quote

Old   June 1, 2010, 07:42
Default
  #11
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by foamWang View Post
Yes, this solves the problem.
However, if I set useMomentumSource to 1, i.e. two-way coupling of solid and fluid phase, a extremely high value of Co will be achieved. This obviously not physical. This may be dedicated to the suddenly appearance of particles in a new processor.

Any idea to solve this?
Does this happen only in parallel runs? (I doubt it)

I think it IS physical: particles with a momentum appear out of nowhere (OK. THAT is unphysical). What should the fluid do? Suffer silently (that would be unphysical) or try to incorporate the additional momentum (that is what you're seeing)

Solutions all have to do with the injector:
- inject less (volume fraction of the particles should be well below 10% for the solver to be valid)
- inject slower
- write a different injector (on the patch, one that injects with no relative velocity to the fluid)

Bernhard
gschaider is offline   Reply With Quote

Old   June 3, 2010, 21:46
Default
  #12
Member
 
foamWang's Avatar
 
Roro Wang
Join Date: Mar 2010
Location: Cambridge, MA, USA
Posts: 30
Rep Power: 8
foamWang is on a distinguished road
Hi, Bernard,

Yes, it's not the parallel problem. Particles can smoothly pass the processorPatch.

Thanks.

Roro

Quote:
Originally Posted by gschaider View Post
Does this happen only in parallel runs? (I doubt it)

I think it IS physical: particles with a momentum appear out of nowhere (OK. THAT is unphysical). What should the fluid do? Suffer silently (that would be unphysical) or try to incorporate the additional momentum (that is what you're seeing)

Solutions all have to do with the injector:
- inject less (volume fraction of the particles should be well below 10% for the solver to be valid)
- inject slower
- write a different injector (on the patch, one that injects with no relative velocity to the fluid)

Bernhard
foamWang is offline   Reply With Quote

Old   October 22, 2010, 16:20
Default problems in parallel
  #13
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 565
Rep Power: 20
chegdan will become famous soon enoughchegdan will become famous soon enough
Hi All,

I downloaded the icoLagrangianFoam from (http://openfoam-extend.svn.sourcefor...agrangianFoam/) and everything compiled fine in OF-1.5-dev

I tried to run icoLagrangianFoam in parallel and it failed, giving the following error messages:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.5-dev                               |
|   \\  /    A nd           | Revision: 1664                                  |
|    \\/     M anipulation  | Web:      http://www.OpenFOAM.org               |
\*---------------------------------------------------------------------------*/
Exec   : /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam -parallel
Date   : Oct 22 2010
Time   : 15:17:32
Host   : aris
PID    : 5532
Case   : /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/icoLagrangianFoam/channelParticles
nProcs : 2
Slaves : 
1
(
aris.5533
)

Pstream initialized with:
    floatTransfer     : 0
    nProcsSimpleSum   : 0
    commsType         : nonBlocking

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

Create mesh for time = 0

Reading transportProperties

Reading field p

Reading field U

Reading/calculating face flux field phi


Reading environmentalProperties
Constructing kinematicCloud
--> FOAM Warning : 
    From function Cloud<ParticleType>::initCloud(const bool checkClass)
    in file /home/dcombest/OpenFOAM/OpenFOAM-1.5-dev/src/lagrangian/basic/lnInclude/CloudIO.C at line 51
    Cannot read particle positions file 
    "/home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/icoLagrangianFoam/channelParticles/processor0/0/lagrangian/kinematicCloud"
    assuming the initial cloud contains 0 particles.
Selecting DispersionModel NoDispersion
Selecting DragModel SphereDrag
Selecting InjectionModel ConeInjection
Selecting pdfType RosinRammler
Selecting WallInteractionModel StandardWallInteraction
Selecting U IntegrationScheme Euler

Starting time loop

Time = 0.001

Courant Number mean: 0 max: 0.2 velocity magnitude: 1
Evolving kinematicCloud
[aris:05532] *** Process received signal ***
[aris:05532] Signal: Segmentation fault (11)
[aris:05532] Signal code:  (-6)
[aris:05532] Failing at address: 0x3e80000159c
[aris:05532] [ 0] /lib/libc.so.6 [0x7f24fce05530]
[aris:05532] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7f24fce054b5]
[aris:05532] [ 2] /lib/libc.so.6 [0x7f24fce05530]
[aris:05532] [ 3] /lib/libc.so.6 [0x7f24fce4afc2]
[aris:05532] [ 4] /lib/libc.so.6(__libc_malloc+0x6e) [0x7f24fce4cd4e]
[aris:05532] [ 5] /usr/lib/libstdc++.so.6(_Znwm+0x1d) [0x7f24fd6a464d]
[aris:05532] [ 6] /usr/lib/libstdc++.so.6(_Znam+0x9) [0x7f24fd6a4769]
[aris:05532] [ 7] /home/dcombest/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4ListIcE7setSizeEi+0x33) [0x7f24fdcb48a3]
[aris:05532] [ 8] /home/dcombest/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam8OPstreamC1ENS_7Pstream10commsTypesEiiNS_8IOstream12streamFormatENS3_13versionNumberE+0xce) [0x7f24fdcb3b7e]
[aris:05532] [ 9] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x43a220]
[aris:05532] [10] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x448ede]
[aris:05532] [11] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x449cde]
[aris:05532] [12] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x419353]
[aris:05532] [13] /lib/libc.so.6(__libc_start_main+0xfd) [0x7f24fcdf0abd]
[aris:05532] [14] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x416b29]
[aris:05532] *** End of error message ***
mpirun noticed that job rank 0 with PID 5532 on node aris exited on signal 11 (Segmentation fault). 
1 additional process aborted (not shown)
I thought it might be a recent update of my kernel, but a quick parallel run of interFoam on the damBreak case finished without any problems.

I ran a parallel run using
Code:
mpirun -np 2 `which icoLagrangianFoam` -parallel < /dev/null >& log.icoLagrangianFoam &
Im sure its something I'm doing wrong. Any help?

Dan
chegdan is offline   Reply With Quote

Old   October 24, 2010, 06:47
Default
  #14
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by chegdan View Post
Hi All,

I downloaded the icoLagrangianFoam from (http://openfoam-extend.svn.sourcefor...agrangianFoam/) and everything compiled fine in OF-1.5-dev

I tried to run icoLagrangianFoam in parallel and it failed, giving the following error messages:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.5-dev                               |
|   \\  /    A nd           | Revision: 1664                                  |
|    \\/     M anipulation  | Web:      http://www.OpenFOAM.org               |
\*---------------------------------------------------------------------------*/
Exec   : /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam -parallel
Date   : Oct 22 2010
Time   : 15:17:32
Host   : aris
PID    : 5532
Case   : /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/icoLagrangianFoam/channelParticles
nProcs : 2
Slaves : 
1
(
aris.5533
)

Pstream initialized with:
    floatTransfer     : 0
    nProcsSimpleSum   : 0
    commsType         : nonBlocking

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

Create mesh for time = 0

Reading transportProperties

Reading field p

Reading field U

Reading/calculating face flux field phi


Reading environmentalProperties
Constructing kinematicCloud
--> FOAM Warning : 
    From function Cloud<ParticleType>::initCloud(const bool checkClass)
    in file /home/dcombest/OpenFOAM/OpenFOAM-1.5-dev/src/lagrangian/basic/lnInclude/CloudIO.C at line 51
    Cannot read particle positions file 
    "/home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/icoLagrangianFoam/channelParticles/processor0/0/lagrangian/kinematicCloud"
    assuming the initial cloud contains 0 particles.
Selecting DispersionModel NoDispersion
Selecting DragModel SphereDrag
Selecting InjectionModel ConeInjection
Selecting pdfType RosinRammler
Selecting WallInteractionModel StandardWallInteraction
Selecting U IntegrationScheme Euler

Starting time loop

Time = 0.001

Courant Number mean: 0 max: 0.2 velocity magnitude: 1
Evolving kinematicCloud
[aris:05532] *** Process received signal ***
[aris:05532] Signal: Segmentation fault (11)
[aris:05532] Signal code:  (-6)
[aris:05532] Failing at address: 0x3e80000159c
[aris:05532] [ 0] /lib/libc.so.6 [0x7f24fce05530]
[aris:05532] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7f24fce054b5]
[aris:05532] [ 2] /lib/libc.so.6 [0x7f24fce05530]
[aris:05532] [ 3] /lib/libc.so.6 [0x7f24fce4afc2]
[aris:05532] [ 4] /lib/libc.so.6(__libc_malloc+0x6e) [0x7f24fce4cd4e]
[aris:05532] [ 5] /usr/lib/libstdc++.so.6(_Znwm+0x1d) [0x7f24fd6a464d]
[aris:05532] [ 6] /usr/lib/libstdc++.so.6(_Znam+0x9) [0x7f24fd6a4769]
[aris:05532] [ 7] /home/dcombest/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam4ListIcE7setSizeEi+0x33) [0x7f24fdcb48a3]
[aris:05532] [ 8] /home/dcombest/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam8OPstreamC1ENS_7Pstream10commsTypesEiiNS_8IOstream12streamFormatENS3_13versionNumberE+0xce) [0x7f24fdcb3b7e]
[aris:05532] [ 9] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x43a220]
[aris:05532] [10] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x448ede]
[aris:05532] [11] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x449cde]
[aris:05532] [12] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x419353]
[aris:05532] [13] /lib/libc.so.6(__libc_start_main+0xfd) [0x7f24fcdf0abd]
[aris:05532] [14] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/icoLagrangianFoam [0x416b29]
[aris:05532] *** End of error message ***
mpirun noticed that job rank 0 with PID 5532 on node aris exited on signal 11 (Segmentation fault). 
1 additional process aborted (not shown)
I thought it might be a recent update of my kernel, but a quick parallel run of interFoam on the damBreak case finished without any problems.

I ran a parallel run using
Code:
mpirun -np 2 `which icoLagrangianFoam` -parallel < /dev/null >& log.icoLagrangianFoam &
Im sure its something I'm doing wrong. Any help?

Dan
Hi Dan!

Could you try the same with the rhoTurbTwinParcelFoam? Just to make sure whether the problem is with the solver or with the library?

Bernhard
gschaider is offline   Reply With Quote

Old   October 24, 2010, 16:39
Default same error...
  #15
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 565
Rep Power: 20
chegdan will become famous soon enoughchegdan will become famous soon enough
Thanks for the reply, I tried the rhoTurbTwinParcelFoam solver and it compiled fine. When i ran the test case received the error:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.5-dev                               |
|   \\  /    A nd           | Revision: 1664                                  |
|    \\/     M anipulation  | Web:      http://www.OpenFOAM.org               |
\*---------------------------------------------------------------------------*/
Exec   : /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/rhoTurbTwinParcelFoam -parallel
Date   : Oct 24 2010
Time   : 15:32:19
Host   : aris
PID    : 3572
Case   : /home/dcombest/OpenFOAM/dcombest-1.5-dev/run/tutorials/rhoTurbTwinParcelFoam/simplifiedSiwek
nProcs : 2
Slaves : 
1
(
aris.3573
)

Pstream initialized with:
    floatTransfer     : 0
    nProcsSimpleSum   : 0
    commsType         : nonBlocking

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

Create mesh for time = 0


Reading environmentalProperties
Reading thermophysical properties

Selecting thermodynamics package hThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>

Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    alphah          1;
    alphak          1;
    alphaEps        0.76923;
}

Creating field DpDt

Constructing thermoCloud1
--> FOAM Warning : 
    From function Cloud<ParticleType>::initCloud(const bool checkClass)
    in file /home/dcombest/OpenFOAM/OpenFOAM-1.5-dev/src/lagrangian/basic/lnInclude/CloudIO.C at line 51
    Cannot read particle positions file 
    "/home/dcombest/OpenFOAM/dcombest-1.5-dev/run/tutorials/rhoTurbTwinParcelFoam/simplifiedSiwek/processor0/0/lagrangian/thermoCloud1"
    assuming the initial cloud contains 0 particles.
Selecting DispersionModel StochasticDispersionRAS
Selecting DragModel SphereDrag
Selecting InjectionModel ManualInjection
Selecting pdfType RosinRammler
Selecting WallInteractionModel StandardWallInteraction
Selecting U IntegrationScheme Euler
Selecting HeatTransferModel RanzMarshall
Selecting T IntegrationScheme Analytical
Constructing kinematicCloud1
--> FOAM Warning : 
    From function Cloud<ParticleType>::initCloud(const bool checkClass)
    in file /home/dcombest/OpenFOAM/OpenFOAM-1.5-dev/src/lagrangian/basic/lnInclude/CloudIO.C at line 51
    Cannot read particle positions file 
    "/home/dcombest/OpenFOAM/dcombest-1.5-dev/run/tutorials/rhoTurbTwinParcelFoam/simplifiedSiwek/processor0/0/lagrangian/kinematicCloud1"
    assuming the initial cloud contains 0 particles.
Selecting DispersionModel StochasticDispersionRAS
Selecting DragModel SphereDrag
Selecting InjectionModel ManualInjection
Selecting pdfType RosinRammler
Selecting WallInteractionModel StandardWallInteraction
Selecting U IntegrationScheme Euler
Courant Number mean: 0 max: 0

Starting time loop

Courant Number mean: 0 max: 0
deltaT = 0.000119047619
Time = 0.000119048

Evolving thermoCloud1
[aris:03572] *** Process received signal ***
[aris:03572] Signal: Segmentation fault (11)
[aris:03572] Signal code:  (-6)
[aris:03572] Failing at address: 0x3e800000df4
[aris:03572] [ 0] /lib/libc.so.6 [0x7fdde01b9530]
[aris:03572] [ 1] /lib/libc.so.6(gsignal+0x35) [0x7fdde01b94b5]
[aris:03572] [ 2] /lib/libc.so.6 [0x7fdde01b9530]
[aris:03572] [ 3] /lib/libc.so.6 [0x7fdde01feaf0]
[aris:03572] [ 4] /lib/libc.so.6(__libc_malloc+0x6e) [0x7fdde0200d4e]
[aris:03572] [ 5] /usr/lib/libstdc++.so.6(_Znwm+0x1d) [0x7fdde0a5864d]
[aris:03572] [ 6] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/rhoTurbTwinParcelFoam [0x465b9c]
[aris:03572] [ 7] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/rhoTurbTwinParcelFoam [0x46650f]
[aris:03572] [ 8] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/rhoTurbTwinParcelFoam [0x41b8e7]
[aris:03572] [ 9] /lib/libc.so.6(__libc_start_main+0xfd) [0x7fdde01a4abd]
[aris:03572] [10] /home/dcombest/OpenFOAM/dcombest-1.5-dev/applications/bin/linux64GccDPOpt/rhoTurbTwinParcelFoam [0x418eb9]
[aris:03572] *** End of error message ***
mpirun noticed that job rank 0 with PID 3572 on node aris exited on signal 11 (Segmentation fault). 
1 additional process aborted (not shown)
the code works fine in serial.

I then went to the lagrangian folder in the $FOAM_SRC and performed and "svn update" and then recompiled the lagrangian files with the ./Allwmake script. Still the same error. Is there another folder I should update? Should I do a complete update of 1.5-dev?

Dan
chegdan is offline   Reply With Quote

Old   October 24, 2010, 20:10
Default update and recompile did not help
  #16
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 565
Rep Power: 20
chegdan will become famous soon enoughchegdan will become famous soon enough
I just wanted to make sure it wasn't something else that was out of date and needed to be updated. I updated all of of-1.5-dev through svn and recompiled the changes, tried to run parallel again with icoLagrangianFoam and same error messages.

I'm working on 64bit ubuntu 9.10

Dan
chegdan is offline   Reply With Quote

Old   October 27, 2010, 05:32
Default
  #17
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by chegdan View Post
I just wanted to make sure it wasn't something else that was out of date and needed to be updated. I updated all of of-1.5-dev through svn and recompiled the changes, tried to run parallel again with icoLagrangianFoam and same error messages.

I'm working on 64bit ubuntu 9.10

Dan
This seems to be a general problem with the 1.5-dev (I'm getting it too). The nature of the stack-trace indicates that somewhere memory is freed twice somewhere

Bernhard
gschaider is offline   Reply With Quote

Old   December 6, 2010, 23:46
Default
  #18
Member
 
Paul Reichl
Join Date: Feb 2010
Location: Melbourne, Victoria, Australia
Posts: 33
Rep Power: 8
preichl is on a distinguished road
Hi All,

Does anyone know how to get around the failure with resulting stack trace problem when running icoLagrangianFoam in parallel?.
I am also getting this with OF 1.5-dev. It works fine on one processor, but as soon as I try to run it in parallel I also get this error.

I also noted that icoLagrangianFoam is not included in OF 1.6-ext. I tried to move it across but when I tried to compile it with (wmake icoLagrangianFoam ) it complains about a missing CintDefs.H file.

Thanks in advance (again),

Paul.
preichl is offline   Reply With Quote

Old   December 7, 2010, 15:05
Default
  #19
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by preichl View Post
Hi All,

Does anyone know how to get around the failure with resulting stack trace problem when running icoLagrangianFoam in parallel?.
I am also getting this with OF 1.5-dev. It works fine on one processor, but as soon as I try to run it in parallel I also get this error.

I also noted that icoLagrangianFoam is not included in OF 1.6-ext. I tried to move it across but when I tried to compile it with (wmake icoLagrangianFoam ) it complains about a missing CintDefs.H file.

Thanks in advance (again),

Paul.
Hi Paul!

icoLagrangianFoam should be in 1.6-ext, but not in the solver directory but in $FOAM_TUTORIALS/lagrangian

Bernhard
gschaider is offline   Reply With Quote

Old   December 7, 2010, 20:03
Default
  #20
Member
 
Paul Reichl
Join Date: Feb 2010
Location: Melbourne, Victoria, Australia
Posts: 33
Rep Power: 8
preichl is on a distinguished road
Hi Bernhard,

I compiled the icoLagrangianFoam files in $FOAM_TUTORIALS/lagrangian of OF 1.6-ext and everything now works.

Thanks again,

Paul.
preichl 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
HP MPI warning...Distributed parallel processing Peter CFX 10 May 14, 2011 06:17
Parallel Moving Mesh Bug for Multi-patch Case albcem OpenFOAM 0 May 21, 2009 00:23
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 23:54.