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

Parallel rasInterFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 29, 2008, 07:16
Default Dear users, I am trying to
  #1
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Dear users,

I am trying to run a case with the rasInterFoam solver.

A- When I run it in serial it works.
B- When I run it in parallel (the 2 processors of my computer) it works.
C- When I run it in parallel (the 10 processors of our 5 computer) it crashes after 3-4 iterations.

For C, I noticed that Courant number mean and Courant number max are different after the 3rd iteration.

Has somebody already experienced it ?

Regards,

Stephane.
openfoam_user is offline   Reply With Quote

Old   October 29, 2008, 14:37
Default Hi Stephane, just as a first
  #2
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 215
Rep Power: 9
fra76 is on a distinguished road
Hi Stephane,
just as a first attempt, try to run double precision and switching floatTransfer to 0 in etc/controlDict file in the OpenFOAM installation.

Have a look to this thread for a similar problem: http://www.cfd-online.com/cgi-bin/Op...how.cgi?1/9732

Hope this helps,
Francesco
fra76 is offline   Reply With Quote

Old   October 30, 2008, 05:08
Default Hi Francesco, I have switch
  #3
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi Francesco,

I have switched float Transfert to 0 in etc/controlDict file in the OpenFOAM installation.

And now it works !

It is strange that it is a default setting.

At the beginning I thought that it was a mesh problem (bad quality) and then a problem with the set-up of the case.

Thanks a lot Francesco.

Stephane.
openfoam_user is offline   Reply With Quote

Old   October 30, 2008, 06:31
Default Hi Francesco, As told into
  #4
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi Francesco,

As told into my previous message 1 case, now, is running.

But I have still problems with a second one (rasInterFoam solver). It crashes after 2 iterations.

Following is the message error. I hope it will help you to give me some advice.

Create time

Create mesh for time = 0


Reading environmentalProperties
Reading field pd

Reading field gamma

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Calculating field g.h

Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphaEps 0.76923;
}

time step continuity errors : sum local = 6.40427e-09, global = -9.71065e-15, cumulative = -9.71065e-15
DICPCG: Solving for pcorr, Initial residual = 1, Final residual = 9.8909e-11, No Iterations 613
DICPCG: Solving for pcorr, Initial residual = 0.320316, Final residual = 9.67054e-11, No Iterations 549
DICPCG: Solving for pcorr, Initial residual = 0.0921141, Final residual = 9.80646e-11, No Iterations 536
time step continuity errors : sum local = 7.15513e-18, global = 1.31447e-19, cumulative = -9.71052e-15
Courant Number mean: 3.07564e-05 max: 0.0460139

Starting time loop

Courant Number mean: 0.000133683 max: 0.2
deltaT = 0.000434651
Time = 0.000434651

MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = 0 Max(gamma) = 1
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -3.18278e-22 Max(gamma) = 1
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -1.22552e-23 Max(gamma) = 1
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -8.09169e-24 Max(gamma) = 1
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 4.42631e-07, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 1.02311e-07, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 8.83972e-08, No Iterations 2
DICPCG: Solving for pd, Initial residual = 1, Final residual = 0.0342529, No Iterations 1
DICPCG: Solving for pd, Initial residual = 0.0181907, Final residual = 0.000895349, No Iterations 9
DICPCG: Solving for pd, Initial residual = 0.00189246, Final residual = 9.43079e-05, No Iterations 48
DICPCG: Solving for pd, Initial residual = 0.000543004, Final residual = 2.58335e-05, No Iterations 35
DICPCG: Solving for pd, Initial residual = 0.000215671, Final residual = 1.04855e-05, No Iterations 54
DICPCG: Solving for pd, Initial residual = 0.000105296, Final residual = 5.24317e-06, No Iterations 26
DICPCG: Solving for pd, Initial residual = 6.7759e-05, Final residual = 3.24401e-06, No Iterations 28
DICPCG: Solving for pd, Initial residual = 4.86539e-05, Final residual = 2.32617e-06, No Iterations 32
DICPCG: Solving for pd, Initial residual = 4.37942e-05, Final residual = 9.64813e-08, No Iterations 104
time step continuity errors : sum local = 1.36281e-10, global = 3.36473e-11, cumulative = 3.36376e-11
DILUPBiCG: Solving for epsilon, Initial residual = 0.0205726, Final residual = 4.41084e-11, No Iterations 4
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 2.71515e-11, No Iterations 4
ExecutionTime = 40.52 s ClockTime = 50 s

Courant Number mean: 0.00013599 max: 0.901774
deltaT = 9.63991e-05
Time = 0.00053105

MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -6.37168e-22 Max(gamma) = 1
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -4.39269e-23 Max(gamma) = 1.00001
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -2.32369e-23 Max(gamma) = 1.00001
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -3.39485e-23 Max(gamma) = 1.00001
DILUPBiCG: Solving for Ux, Initial residual = 0.00197648, Final residual = 1.50039e-07, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 0.0159727, Final residual = 1.1123e-07, No Iterations 3
DILUPBiCG: Solving for Uz, Initial residual = 0.00270569, Final residual = 2.41027e-08, No Iterations 4
DICPCG: Solving for pd, Initial residual = 0.000493505, Final residual = 2.40357e-05, No Iterations 67
DICPCG: Solving for pd, Initial residual = 0.000299434, Final residual = 1.41585e-05, No Iterations 38
DICPCG: Solving for pd, Initial residual = 0.000185027, Final residual = 9.08419e-06, No Iterations 29
DICPCG: Solving for pd, Initial residual = 0.000140907, Final residual = 6.72783e-06, No Iterations 32
DICPCG: Solving for pd, Initial residual = 0.000124686, Final residual = 5.81343e-06, No Iterations 34
DICPCG: Solving for pd, Initial residual = 0.000121187, Final residual = 5.70692e-06, No Iterations 37
DICPCG: Solving for pd, Initial residual = 0.000138079, Final residual = 6.27804e-06, No Iterations 37
DICPCG: Solving for pd, Initial residual = 0.000148248, Final residual = 6.95128e-06, No Iterations 39
DICPCG: Solving for pd, Initial residual = 0.000171414, Final residual = 9.66108e-08, No Iterations 113
time step continuity errors : sum local = 6.91233e-12, global = -3.09376e-12, cumulative = 3.05438e-11
DILUPBiCG: Solving for epsilon, Initial residual = 0.0916063, Final residual = 4.9656e-10, No Iterations 5
DILUPBiCG: Solving for k, Initial residual = 0.0954911, Final residual = 1.94605e-09, No Iterations 6
ExecutionTime = 56 s ClockTime = 69 s

Courant Number mean: 3.0478e-05 max: 1.93885
deltaT = 9.94394e-06
Time = 0.000540994

MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -8.58078e-24 Max(gamma) = 1.00001
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -8.49984e-24 Max(gamma) = 1.00001
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -1.27573e-23 Max(gamma) = 1.00001
MULES: Solving for gamma
Liquid phase volume fraction = 0.808191 Min(gamma) = -2.2741e-23 Max(gamma) = 1.00001
DILUPBiCG: Solving for Ux, Initial residual = 0.598091, Final residual = 2.10026e-07, No Iterations 9
DILUPBiCG: Solving for Uy, Initial residual = 0.122759, Final residual = 1.71e-07, No Iterations 6
DILUPBiCG: Solving for Uz, Initial residual = 0.0678085, Final residual = 6.71437e-07, No Iterations 8
DICPCG: Solving for pd, Initial residual = 0.0716861, Final residual = 0.00355337, No Iterations 41
DICPCG: Solving for pd, Initial residual = 0.0298115, Final residual = 0.00115368, No Iterations 7
DICPCG: Solving for pd, Initial residual = 0.0902737, Final residual = 0.00380365, No Iterations 9
DICPCG: Solving for pd, Initial residual = 0.279904, Final residual = 0.0138083, No Iterations 4
DICPCG: Solving for pd, Initial residual = 0.451369, Final residual = 0.01378, No Iterations 4
DICPCG: Solving for pd, Initial residual = 0.521629, Final residual = 0.016842, No Iterations 3
DICPCG: Solving for pd, Initial residual = 0.61108, Final residual = 0.0233927, No Iterations 3
DICPCG: Solving for pd, Initial residual = 0.680218, Final residual = 0.0339791, No Iterations 2
DICPCG: Solving for pd, Initial residual = 0.682929, Final residual = 9.60524e-08, No Iterations 218
time step continuity errors : sum local = 8.79992e-10, global = 3.75986e-11, cumulative = 6.81424e-11
DILUPBiCG: Solving for epsilon, Initial residual = 1, Final residual = 2.42838e-09, No Iterations 24
[0] #0 Foam::error::printStack(Foam:stream&)[8] [5] [6] [2] [1] ####0000 Foam::error::printStack(Foam:stream&) Foam::error::printStack(Foam:stream&)#0 Foam::error::printStack(Foam:stream&) Foam::error::printStack(Foam:stream&)Foam::error::printStack(Foam:stream&)[4] #0 Foam::error::printStack(Foam:stream&) in "/shared/OpenFOAM/OpenFOAM-1.5 in /li"b//slhianruexd6/4OGpcecnDFPOOApMt//OlpiebnOFpOeAnMF-O1A.M5./sloi"b
/[6] l#i1n uFoam::sigFpe::sigFpeHandler(int)x64GccDPOpt/libOpenFOAM.so"
[2] #1 Foam::sigFpe::sigFpeHandler(int) in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[0] #1 Foam::sigFpe::sigFpeHandler(int) in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[1] #1 Foam::sigFpe::sigFpeHandler(int) in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64 in "/sharedG/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[4] #1 Foam::sigFpe::sigFpeHandler(int)ccDPOpt/libOpenFOAM.so"
[5] #1 Foam::sigFpe::sigFpeHandler(int) in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[6] #2 in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[2] #2 in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[0] #2 in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[1] #2 in "??/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[4] #2 ?? in "/shared/OpenFOAM/OpenFO in AM"/-l1i.b564//lliibb/cl.??is??nou.x66"4
G[6] c#c3D Pvoid Foam::MULES::limiter<foam::onefield,>(Foam::Field< double>&, Foam::oneField const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int)Opt/libOpenFOAM.so"
[5] #2 ?? in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[8] #1 Foam::sigFpe::sigFpeHandler(int) in "/lib64/libc.so.6"
[2] #3 void Foam::MULES::limiter<foam::onefield,>(Foam::Field< double>&, Foam::oneField const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/lib64/libc.so.6"
[0] #3 void Foam::MULES::limiter<foam::onefield,>(Foam::Field< double>&, Foam::oneField const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int)?? in in "/lib64/libc.so.6"
[1] #"3 void Foam::MULES::limiter<foam::onefield,>(Foam::Field< double>&, Foam::oneField const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int)/lib64/libc.so.6"
[4] #3 void Foam::MULES::limiter<foam::onefield,>(Foam::Field< double>&, Foam::oneField const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[6] #4 void Foam::MULES::explicitSolve<foam::onefield,>(Foam:: oneField const&, Foam::GeometricField<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, Foam::zeroField const&, Foam::zeroField const&, double, double) in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[2] #4 void Foam::MULES::explicitSolve<foam::onefield,>(Foam:: oneField const&, Foam::GeometricField<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, Foam::zeroField const&, Foam::zeroField const&, double, double) in "/lib64/libc.so.6"
[5] #3 void Foam::MULES::limiter<foam::onefield,>(Foam::Field< double>&, Foam::oneField const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/shared/OpenFOAM/Ope in n"F/OsAhMa-r1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[4] e#4 d in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[0] #4 void Foam::MULES::explicitSolve<foam::onefield,>(Foam:: oneField const&, Foam::GeometricField<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, Foam::zeroField const&, Foam::zeroField const&, double, double)void Foam::MULES::explicitSolve<foam::onefield,>(Foam:: oneField const&, Foam::GeometricField<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, Foam::zeroField const&, Foam::zeroField const&, double, double)/ in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[1] #4 void Foam::MULES::explicitSolve<foam::onefield,>(Foam:: oneField const&, Foam::GeometricField<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, Foam::zeroField const&, Foam::zeroField const&, double, double)OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[6] #5 Foam::MULES::explicitSolve(Foam::GeometricField<do uble,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, double, double) in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfin in "/shared/OpenFOAM/OpenF in O"A/Ms-h1a.r5e/dl/iObp/elniFnOuAxM6/4OGpcecnDFPOOApMt-/1l.i5b/fliinbi/tleiVnoulx u6m4eG.cscoD"P
O[5] p#t4/ lvoid Foam::MULES::explicitSolve<foam::onefield,>(Foam:: oneField const&, Foam::GeometricField<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, Foam::zeroField const&, Foam::zeroField const&, double, double)ibfiniteVolume.so"
[6] #6 in "/shared/OpenFOAM/OpenFOAM-1 in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[0] #5 Foam::MULES::explicitSolve(Foam::GeometricField<do uble,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, double, double). in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[1] #5 Foam::MULES::explicitSolve(Foam::GeometricField<do uble,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, double, double)5/lib/linux64GccDPOpt/libfiniteVolume.so"
[4] #5 Foam::MULES::explicitSolve(Foam::GeometricField<do uble,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, double, double)iteVolume.so"
[2] #5 Foam::MULES::explicitSolve(Foam::GeometricField<do uble,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, double, double)main in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[1] #6 in "/shared/OpenFO in AM"//sOhpaenrFOeAdM/-O1p.5/lib/linux64GccDPOpt/libfiniteVolume.so"
e[4] #6 nFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[2] #6 in "/shared in "/shared/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/rasInterFoam"
[6] #7 __libc_start_main in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
[8] #2 in "/shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[5] #5 Foam::MULES::explicitSolve(Foam::GeometricField<do uble,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, double, double)/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[0] #6 ?? in "/lib64/libc.so.6"main
main in "/sha[6] #8 red/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
[5] #6 Foam::regIOobject::readIfModified()main in "/lib64/libc.so.6"
[8] #3 void Foam::MULES::limiter<foam::onefield,>(Foam::Field< double>&, Foam::oneField const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in main in ""//sshhaarreedd//OOppeennFFOOAAMM//OOppeennFFOOAAMM--11..55 in //"aa/ppspphllaiircceaadtt/iiOpenFOAM/OpenFOAM-1.5/applooications/bin/linux64nnG ccDPOpt/rasInterFoam"
ss[4] #7 //__libc_start_mainbbiinn//lliinnuuxx6644GGccccDDPPOOpptt//rraassIInntteerrFFooa amm""

[cfs9:26785] *** Process received signal ***
[0] [cfs9:26785] Signal: Floating point exception (8)
[cfs9:26785] Signal code: (-6)
[cfs9:26785] Failing at address: 0x45f000068a1
#[cfs9:26785] [ 0] /lib64/libc.so.6 [0x7f25b58a5660]
7[cfs9:26785] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x7f25b58a55c5]
[cfs9:26785] [ 2] /lib64/libc.so.6 [0x7f25b58a5660]
__libc_start_main[cfs9:26785] [ 3] /shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so(_ZN4Foam5MU LES7limiterINS_8oneFieldENS_9zeroFieldES3_EEvRNS_5 FieldIdEERKT_RKNS_14GeometricF ieldIdNS_12fvPatchFieldENS_7volMeshEEERKNSA_IdNS_1 3fvsPatchFieldENS_11surfaceMes hEEESK_RKT0_RKT1_ddi+0xe6a) [0x7f25b70176fa]
[cfs9:26785] [ 4] /shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so(_ZN4Foam5MU LES13explicitSolveINS_8oneFieldENS_9zeroFieldES3_E EvRKT_RNS_14GeometricFieldIdNS _12fvPatchFieldENS_7volMeshEEERKNS7_IdNS_13fvsPatc hFieldENS_11surfaceMeshEEERSE_ RKT0_RKT1_dd+0x274) [0x7f25b701a4e4]
[cfs9:26785] [ 5] /shared/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so(_ZN4Foam5MU LES13explicitSolveERNS_14GeometricFieldIdNS_12fvPa tchFieldENS_7volMeshEEERKNS1_I dNS_13fvsPatchFieldENS_11surfaceMeshEEERS8_dd+0x24 ) [0x7f25b7003f34]
[cfs9:26785] [ 6] rasInterFoam [0x420bb6]
[cfs9:26785] [ 7] /lib64/libc.so.6(__libc_start_main+0xe6) [0x7f25b5891436]
[cfs9:26785] [ 8] rasInterFoam(_ZN4Foam11regIOobject14readIfModified Ev+0x1c9) [0x41d6c9]
[cfs9:26785] *** End of error message ***

Regards,

Stephane.
openfoam_user is offline   Reply With Quote

Old   November 1, 2008, 05:14
Default Hi Stephane, The default valu
  #5
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 215
Rep Power: 9
fra76 is on a distinguished road
Hi Stephane,
The default value for floatTransfer has been changed to 0 in the 1.5.x version, as far as I know.
About your running error, it looks like the solvers are suffering. Is the problem the same in serial and in parallel? How big is your mesh? You can notice that your deltaT is reduced by a factor of 10 at each iteration. In this cases I usually check:
1. boundary conditions
2. initial conditions
3. Cells where the courant number is much higher than on the rest of the domain (there should be a "Co" application, if I'm not wrong). Sometimes bad cells, especially at the boundaries, can create many stability problems.
4. Try other solvers/schemes

Hope this helps,
Francesco
fra76 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
Bounding epsilon and K with rasInterFoam openfoam_user OpenFOAM Running, Solving & CFD 0 October 23, 2008 08:48
RasInterFoam solver paka OpenFOAM Running, Solving & CFD 3 July 9, 2007 04:17
ERRORS in rasInterFoam Turbulence kumar2 OpenFOAM Running, Solving & CFD 0 June 9, 2006 15:06
RasInterFoam or lesInterFoam hsieh OpenFOAM Running, Solving & CFD 2 March 31, 2006 14:42
RasInterFoam cavitation maritozzo OpenFOAM Running, Solving & CFD 2 December 6, 2005 15:09


All times are GMT -4. The time now is 17:13.