CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Foam::error::PrintStack (http://www.cfd-online.com/Forums/openfoam-solving/89644-foam-error-printstack.html)

almir June 18, 2011 10:00

Foam::error::PrintStack
 
hi,
i have following errormessage in OpenFoam, as solver I use BuoyantSimpleFoam. I don´t understand that error.

Maybe someone can help me?


almir@ubuntu:~/OpenFOAM/zylinder$ buoyantSimpleFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.x |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.7.x-3776603e4c6c
Exec : buoyantSimpleFoam
Date : Jun 15 2011
Time : 12:26:48
Host : ubuntu
PID : 5430
Case : /home/almir/OpenFOAM/zylinder
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0


Reading g
Reading thermophysical properties

Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85034;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.85616;
Prt 1;
gamma1 0.5532;
gamma2 0.4403;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
c1 10;
}

Calculating field g.h

Reading field p_rgh


Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.00987294, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0157, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.00987846, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.0105804, No Iterations 1
GAMG: Solving for p_rgh, Initial residual = 0.899378, Final residual = 0.00305647, No Iterations 4
time step continuity errors : sum local = 18.9686, global = -1.40909e-15, cumulative = -1.40909e-15
rho max/min : 1.22108 1.13449
DILUPBiCG: Solving for omega, Initial residual = 0.999913, Final residual = 0.0105502, No Iterations 2
bounding omega, min: -902.694 max: 24331.5 average: 741.476
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.0973743, No Iterations 1
bounding k, min: -0.000335494 max: 0.0031317 average: 0.000848312
ExecutionTime = 0.11 s ClockTime = 0 s

Time = 2

DILUPBiCG: Solving for Ux, Initial residual = 0.11425, Final residual = 0.00308422, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.0715711, Final residual = 2.95363e-05, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.109402, Final residual = 0.00196119, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.177633, Final residual = 0.00377685, No Iterations 1
GAMG: Solving for p_rgh, Initial residual = 0.997056, Final residual = 0.00735437, No Iterations 4
time step continuity errors : sum local = 11.1294, global = 4.01181e-15, cumulative = 2.60272e-15
rho max/min : 309747 -321318
DILUPBiCG: Solving for omega, Initial residual = 0.594095, Final residual = 0.0340323, No Iterations 1
bounding omega, min: -7.04999e+17 max: 1.99134e+09 average: -1.78979e+14
DILUPBiCG: Solving for k, Initial residual = 0.999984, Final residual = 0.0558935, No Iterations 2
bounding k, min: -7.30668e+08 max: 1.51545e+08 average: -1.226e+06
ExecutionTime = 0.15 s ClockTime = 0 s

Time = 3

DILUPBiCG: Solving for Ux, Initial residual = 0.125933, Final residual = 0.0012217, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.097672, Final residual = 0.000856571, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.130559, Final residual = 0.00122656, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.467341, Final residual = 0.00933279, No Iterations 1
#0 Foam::error::PrintStack(Foam::Ostream&) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 in "/lib/libc.so.6"
#3 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
#5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
#6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam171/lib/linux64GccDPOpt/libfiniteVolume.so"
#8
in "/opt/openfoam171/applications/bin/linux64GccDPOpt/buoyantSimpleFoam"
#9 __libc_start_main in "/lib/libc.so.6"
#10
in "/opt/openfoam171/applications/bin/linux64GccDPOpt/buoyantSimpleFoam"
Gleitkomma-Ausnahme
almir@ubuntu:~/OpenFOAM/zylinder$


greets

almir

wyldckat June 18, 2011 16:53

Greetings Almir,

At the risk of sending you off in the wrong direction, you can try this answer: My program stops with an output that starts with #0 Foam::error:: PrintStack(Foam::Ostream&)

But in an attempt to send you in the right direction:
  1. You should pay closer attention to the output. For example:
    Code:

    Build  : 1.7.x-3776603e4c6c
    Exec  : buoyantSimpleFoam
    Date  : Jun 15 2011
    Time  : 12:26:48
    Host  : ubuntu
    PID    : 5430
    Case  : /home/almir/OpenFOAM/zylinder
    nProcs : 1
    SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

    The line in bold tells you what SigFpe is: Floating point exception @wikipedia
  2. The second line in the print stack says this:
    Code:

    #1  Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
    Which means that some bad math went about doing something wrong... in other words, division by infinite or by zero or something like that.
  3. Examining the iteration outputs, you will see the following breadcrumbs about the impeding doom that looms in the solver's horizon:
    Code:

    Time = 1

    DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.00987294, No Iterations 1
    DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.0157, No Iterations 1
    DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.00987846, No Iterations 1
    DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.0105804, No Iterations 1
    GAMG:  Solving for p_rgh, Initial residual = 0.899378, Final residual = 0.00305647, No Iterations 4
    time step continuity errors : sum local = 18.9686, global = -1.40909e-15, cumulative = -1.40909e-15
    rho max/min : 1.22108 1.13449
    DILUPBiCG:  Solving for omega, Initial residual = 0.999913, Final residual = 0.0105502, No Iterations 2
    bounding omega, min: -902.694 max: 24331.5 average: 741.476
    DILUPBiCG:  Solving for k, Initial residual = 1, Final residual = 0.0973743, No Iterations 1
    bounding k, min: -0.000335494 max: 0.0031317 average: 0.000848312
    ExecutionTime = 0.11 s  ClockTime = 0 s

    Time = 2

    DILUPBiCG:  Solving for Ux, Initial residual = 0.11425, Final residual = 0.00308422, No Iterations 1
    DILUPBiCG:  Solving for Uy, Initial residual = 0.0715711, Final residual = 2.95363e-05, No Iterations 2
    DILUPBiCG:  Solving for Uz, Initial residual = 0.109402, Final residual = 0.00196119, No Iterations 1
    DILUPBiCG:  Solving for h, Initial residual = 0.177633, Final residual = 0.00377685, No Iterations 1
    GAMG:  Solving for p_rgh, Initial residual = 0.997056, Final residual = 0.00735437, No Iterations 4
    time step continuity errors : sum local = 11.1294, global = 4.01181e-15, cumulative = 2.60272e-15
    rho max/min : 309747 -321318
    DILUPBiCG:  Solving for omega, Initial residual = 0.594095, Final residual = 0.0340323, No Iterations 1
    bounding omega, min: -7.04999e+17 max: 1.99134e+09 average: -1.78979e+14
    DILUPBiCG:  Solving for k, Initial residual = 0.999984, Final residual = 0.0558935, No Iterations 2
    bounding k, min: -7.30668e+08 max: 1.51545e+08 average: -1.226e+06
    ExecutionTime = 0.15 s  ClockTime = 0 s

    As I've noted in bold+underline: rho, omega, k and continuity errors indicate that something very not physical is happening!! Expressions like über compression and super turbulence come to mind! ;)
So, to sum up: you are giving very bad boundary conditions to your case!

Best regards,
Bruno

tfuwa August 3, 2011 11:00

Awesome analysis. Also solved my problem. Thanks.

Kanarya February 9, 2012 08:22

Hi Foamers,

I am running twoPhaseEulerFoam and i have increased the mesh size 6000(which was in tutorial bed2) to 24000 and I am getting following error. I tried for 12000 again same.in blockMeshDict it was (30 200 1) first I have changed it to (30 400 1) then (60 400 2) an so on.Another problem is that I have to change the file 0/alpha everytime.is there any other practical solution for that?


Courant Number mean: 0.263255 max: 12.2832
Max Ur Courant Number = 3.77181e+06
Time = 0.071

DILUPBiCG: Solving for alpha, Initial residual = 1.1014e-05, Final residual = 6.17658e-11, No Iterations 33
Dispersed phase volume fraction = 0.3 Min(alpha) = -1.92847 Max(alpha) = 2.81043
DILUPBiCG: Solving for alpha, Initial residual = 0.00010103, Final residual = 5.2889e-11, No Iterations 8
Dispersed phase volume fraction = 0.3 Min(alpha) = -0.247369 Max(alpha) = 1.92082
kinTheory: max(Theta) = 1000
kinTheory: min(nua) = 1.3774e-12, max(nua) = 0.0231854
kinTheory: min(pa) = -9295.94, max(pa) = 1.14803e+09
GAMG: Solving for p, Initial residual = 0.996287, Final residual = 0.0429939, No Iterations 1
time step continuity errors : sum local = 201567, global = 28.235, cumulative = 28.235
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8
in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/twoPhaseEulerFoam"
#9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10
in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/twoPhaseEulerFoam"
Floating point exception

Please help me...sorry for stupid questions

thanksss a lot!!!

Kanarya February 9, 2012 10:17

Hi all,

thanks I did it alone...

Thanks...

ebah6 February 17, 2012 22:33

Hello all,

I am having a similar error in using pimpleDyMFoam.
Below is the error output:

------------------------------------
Courant Number mean: 0.00997899 max: 0.807965
deltaT = 1.32295e-104
--> FOAM Warning :
From function Time::operator++()
in file db/Time/Time.C at line 982
Increased the timePrecision from 267 to 268 to distinguish between timeNames at time 1.97982e-05
Time = 1.979823486337861903608045799352055382769322022795 67718505859375e-05

solidBodyMotionFunctions::rotatingMotion::transfor mation(): Time = 1.97982e-05 transformation: ((0 0 0) (1 (0 0 0.000103663)))
AMI: Creating addressing and weights between 16 source faces and 16 target faces
AMI: Patch source weights min/max/average = 1, 1.0007, 1.00035
AMI: Patch target weights min/max/average = 0.986951, 0.987248, 0.987099
smoothSolver: Solving for Ux, Initial residual = 0.140328, Final residual = 5.75579e-08, No Iterations 3
smoothSolver: Solving for Uy, Initial residual = 0.140962, Final residual = 5.70666e-08, No Iterations 3
GAMG: Solving for p, Initial residual = 0.814891, Final residual = 0.00591061, No Iterations 3
time step continuity errors : sum local = 0.00031744, global = 5.68686e-06, cumulative = 0.00082973
#0 Foam::error::printStack(Foam::Ostream&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8
in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
#9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10
in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
--------------------------

Can you tell how you went along in solving the issue?

Thank you for your help.

wyldckat February 18, 2012 06:56

Greetings ebah6,

Quote:

Originally Posted by ebah6 (Post 345031)
Courant Number mean: 0.00997899 max: 0.807965
deltaT = 1.32295e-104
--> FOAM Warning :
From function Time::operator++()
in file db/Time/Time.C at line 982
Increased the timePrecision from 267 to 268 to distinguish between timeNames at time 1.97982e-05
Time = 1.979823486337861903608045799352055382769322022795 67718505859375e-05


solidBodyMotionFunctions::rotatingMotion::transfor mation(): Time = 1.97982e-05 transformation: ((0 0 0) (1 (0 0 0.000103663)))
AMI: Creating addressing and weights between 16 source faces and 16 target faces
AMI: Patch source weights min/max/average = 1, 1.0007, 1.00035
AMI: Patch target weights min/max/average = 0.986951, 0.987248, 0.987099
smoothSolver: Solving for Ux, Initial residual = 0.140328, Final residual = 5.75579e-08, No Iterations 3
smoothSolver: Solving for Uy, Initial residual = 0.140962, Final residual = 5.70666e-08, No Iterations 3
GAMG: Solving for p, Initial residual = 0.814891, Final residual = 0.00591061, No Iterations 3
time step continuity errors : sum local = 0.00031744, global = 5.68686e-06, cumulative = 0.00082973
#0 Foam::error::printStack(Foam::Ostream&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8
in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
#9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10
in "/home/alpha/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
--------------------------

Can you tell how you went along in solving the issue?

You've got a whole other set of problems on your case. In bold and underlined are the major indicators of what might be wrong:
  • Courant number seems just fine, or at least isn't going overboard...
  • ... at the cost of having a deltaT at a magnitude of 1e-104!? I don't even know what kind of level of simulation interaction this might be, but possibly at the quark level (http://en.wikipedia.org/wiki/Quark)?
  • Time precision at 268 digits... 64bit floating point can't go beyond... I can't remember right, but isn't the limit 14 or 19?
  • AMI... and using 2.1.0... mmm... you're trying to use a new feature that was released on OpenFOAM 2.1.0, so bugs are bound to pop up anywhere!
So, the diagnosis is this:
  1. Using an adaptive deltaT based on Courant, the solver was forced to virtually go into sub-atomic simulations, which isn't its natural operational zone. The "adaptive deltaT based on Courant" feature is usually based on the smallest cell your mesh has got. Did you run checkMesh to verify the quality of the mesh? Do you see the "minimum volume" value? Is it something like 1e-40?
  2. Also, go see the first tutorial on the user guide: Increasing the mesh resolution - read that section and you will see how the cell size relates to the deltaT needed for a stable Courant number.
  3. AMI, that's a new feature. If you are going to use new features, you better be ready to use the bleeding edge ... pardon, the bug fix version of OpenFOAM, namely 2.1.x, not 2.1.0 ;)
  4. If it's something new to you, Always start small!!
    You didn't specify anything about the case you are trying to simulate, so I'm assuming from the results that you are trying to simulate something that is really fast moving and has really a lot of refined zones in the mesh.
    Therefore, to avoid these kinds of issues, you should always start with something more simple. For example, if you want to simulate a fast moving F-16 going at Mach 2.1 (probably doing a full afterburner free fall? :rolleyes:), you first have to start simulating a simple trapezoid that barely resembles an airplane (ahmed body?), using a very coarse mesh and going at 1m/s. Then gradually work to a more complex mesh and geometry, so you can see the gradual needs for smaller deltaT and stuff...
Best regards and good luck!
Bruno

ebah6 February 18, 2012 17:54

Thank you Bruno.

I appreciate. Let me go through this and to see how I can correct my mistakes.
I will probably get back to you for more help.

My best regards.

ebah6 April 3, 2012 00:20

1 Attachment(s)
Hello Bruno and everyone else,

Allow that I follow up on this thread for I am experience similar issues as those for which the thread was initiated.
My log file is as follows:
PHP Code:

Courant Number mean0.00401268 max0.141369
deltaT 
1e-05
Time 
6e-05

solidBodyMotionFunctions
::rotatingMotion::transformation(): Time 6e-05 transformation: ((0 0 -8.67362e-19) ((0 0 0.0006111)))
AMICreating addressing and weights between 152 source faces and 152 target faces
AMI
Patch source weights min/max/average 1.000461.000591.00051
AMI
Patch target weights min/max/average 1.000271.000411.00034
PIMPLE
iteration 1
smoothSolver
:  Solving for UxInitial residual 0.556334, Final residual 0.0528731No Iterations 2
smoothSolver
:  Solving for UyInitial residual 0.548617, Final residual 0.0461752No Iterations 2
smoothSolver
:  Solving for UzInitial residual 0.815939, Final residual 0.0320452No Iterations 3
GAMG
:  Solving for pInitial residual 0.921675, Final residual 0.00854805No Iterations 2
time step continuity errors 
sum local 0.000398218, global = -2.4468e-06cumulative = -4.27843e-06
PIMPLE
iteration 2
smoothSolver
:  Solving for UxInitial residual 0.355747, Final residual 0.0276016No Iterations 3
smoothSolver
:  Solving for UyInitial residual 0.383216, Final residual 0.034923No Iterations 2
smoothSolver
:  Solving for UzInitial residual 0.532627, Final residual 0.0249993No Iterations 3
GAMG
:  Solving for pInitial residual 0.873111, Final residual 0.00495616No Iterations 3
time step continuity errors 
sum local 0.000579107, global = 3.73469e-05cumulative 3.30685e-05
PIMPLE
iteration 3
DILUPBiCG
:  Solving for UxInitial residual 0.464469, Final residual 7.77744e-07No Iterations 24
DILUPBiCG
:  Solving for UyInitial residual 0.5108, Final residual 5.63977e-07No Iterations 23
DILUPBiCG
:  Solving for UzInitial residual 0.472435, Final residual 1.84551e-07No Iterations 7
GAMG
:  Solving for pInitial residual 0.960559, Final residual 6.37384e-07No Iterations 22
time step continuity errors 
sum local 1.31687e-07, global = -1.43223e-08cumulative 3.30542e-05
DILUPBiCG
:  Solving for epsilonInitial residual 0.984696, Final residual 7.74724e-07No Iterations 25
DILUPBiCG
:  Solving for kInitial residual 0.971516, Final residual 7.10152e-07No Iterations 25
ExecutionTime 
5.57 s  ClockTime 6 s

Courant Number mean
0.0553216 max1.49585
deltaT 
1e-05
Time 
7e-05

solidBodyMotionFunctions
::rotatingMotion::transformation(): Time 7e-05 transformation: ((0 0 0) ((0 0 0.00071295)))
AMICreating addressing and weights between 152 source faces and 152 target faces
AMI
Patch source weights min/max/average 1.000451.000591.00051
AMI
Patch target weights min/max/average 1.000271.000411.00034
PIMPLE
iteration 1
smoothSolver
:  Solving for UxInitial residual 0.821499, Final residual 0.0529954No Iterations 2
smoothSolver
:  Solving for UyInitial residual 0.772528, Final residual 0.0435714No Iterations 2
smoothSolver
:  Solving for UzInitial residual 0.889394, Final residual 0.0573016No Iterations 3
GAMG
:  Solving for pInitial residual 0.927555, Final residual 0.00793319No Iterations 3
time step continuity errors 
sum local 0.00232858, global = 1.09112e-05cumulative 4.39653e-05
PIMPLE
iteration 2
smoothSolver
:  Solving for UxInitial residual 0.624835, Final residual 0.0579445No Iterations 8
smoothSolver
:  Solving for UyInitial residual 0.528869, Final residual 0.0500303No Iterations 7
smoothSolver
:  Solving for UzInitial residual 0.667562, Final residual 0.0371676No Iterations 4
GAMG
:  Solving for pInitial residual 0.921425, Final residual 0.00829498No Iterations 2
time step continuity errors 
sum local 0.0183302, global = 0.000417751cumulative 0.000461716
PIMPLE
iteration 3
DILUPBiCG
:  Solving for UxInitial residual 0.469402, Final residual 0.00155559No Iterations 1001
DILUPBiCG
:  Solving for UyInitial residual 0.456055, Final residual 0.00192389No Iterations 1001
DILUPBiCG
:  Solving for UzInitial residual 0.657918, Final residual 7.2394e-07No Iterations 26
GAMG
:  Solving for pInitial residual 0.940662, Final residual 9.79822e-07No Iterations 23
time step continuity errors 
sum local 5.83896e-06, global = -5.30525e-07cumulative 0.000461185
DILUPBiCG
:  Solving for epsilonInitial residual 0.989478, Final residual 10537.6No Iterations 1001
bounding epsilon
min: -1.28949e+18 max9.22403e+17 average: -3.22331e+14
DILUPBiCG
:  Solving for kInitial residual 1.42853e-05, Final residual 6.87541e-07No Iterations 30
bounding k
min: -1.84393e+10 max2.85172e+12 average1.06974e+10
ExecutionTime 
12.22 s  ClockTime 13 s

Courant Number mean
4.69634 max8810.84
deltaT 
2.26963e-09
Time 
7.00023e-05

solidBodyMotionFunctions
::rotatingMotion::transformation(): Time 7.00023e-05 transformation: ((0 0 -8.67362e-19) ((0 0 0.000712973)))
AMICreating addressing and weights between 152 source faces and 152 target faces
AMI
Patch source weights min/max/average 1.000451.000591.00051
AMI
Patch target weights min/max/average 1.000271.000411.00034
PIMPLE
iteration 1
smoothSolver
:  Solving for UxInitial residual 0.924264, Final residual 0.0530127No Iterations 2
smoothSolver
:  Solving for UyInitial residual 0.641598, Final residual 0.0386788No Iterations 2
smoothSolver
:  Solving for UzInitial residual 0.921792, Final residual 0.0461483No Iterations 2
GAMG
:  Solving for pInitial residual 1, Final residual 5705.13No Iterations 50
time step continuity errors 
sum local 9.40062e+08, global = 3.78949e+07cumulative 3.78949e+07
PIMPLE
iteration 2
smoothSolver
:  Solving for UxInitial residual 1, Final residual 0.0224152No Iterations 1
smoothSolver
:  Solving for UyInitial residual 1, Final residual 0.0293676No Iterations 1
smoothSolver
:  Solving for UzInitial residual 0.00299007, Final residual 6.31039e-05No Iterations 1
GAMG
:  Solving for pInitial residual 0.595319, Final residual 9.86458e-05No Iterations 1
time step continuity errors 
sum local 3.27194e+16, global = 4.33629e+15cumulative 4.33629e+15
PIMPLE
iteration 3
DILUPBiCG
:  Solving for UxInitial residual 0.999996, Final residual 5.86893e-07No Iterations 28
DILUPBiCG
:  Solving for UyInitial residual 0.999998, Final residual 7.80082e-07No Iterations 20
DILUPBiCG
:  Solving for UzInitial residual 0.000201204, Final residual 9.98882e-07No Iterations 5
GAMG
:  Solving for pInitial residual 0.879029, Final residual 7.05858e-07No Iterations 47
time step continuity errors 
sum local 4.76118e+19, global = -8.01772e+18cumulative = -8.01339e+18
DILUPBiCG
:  Solving for epsilonInitial residual 1, Final residual 48876.6No Iterations 1001
bounding epsilon
min: -1.7324e+51 max2.47572e+51 average5.46302e+48
DILUPBiCG
:  Solving for kInitial residual 1, Final residual 6.79817e-07No Iterations 96
bounding k
min: -1.36796e+48 max7.09554e+59 average6.62561e+56
ExecutionTime 
15.82 s  ClockTime 16 s

Courant Number mean
2.99449e+25 max3.21959e+28
deltaT 
1.40989e-37
--> FOAM Warning :
    
From function Time::operator++()
    
in file db/Time/Time.C at line 1010
    Increased the timePrecision from 6 to 7 to distinguish between timeNames at time 7.00023e-05
Time 
7.000227e-05

solidBodyMotionFunctions
::rotatingMotion::transformation(): Time 7.00023e-05 transformation: ((0 0 -8.67362e-19) ((0 0 0.000712973)))
AMICreating addressing and weights between 152 source faces and 152 target faces
AMI
Patch source weights min/max/average 1.000451.000591.00051
AMI
Patch target weights min/max/average 1.000271.000411.00034
PIMPLE
iteration 1
smoothSolver
:  Solving for UxInitial residual 0.904795, Final residual 0.0198399No Iterations 2
smoothSolver
:  Solving for UyInitial residual 0.920089, Final residual 0.00357272No Iterations 1
smoothSolver
:  Solving for UzInitial residual 0.770617, Final residual 0.0112283No Iterations 1
GAMG
:  Solving for pInitial residual 1, Final residual 3.34459e+74No Iterations 50
time step continuity errors 
sum local 2.15853e+83, global = 2.27242e+82cumulative 2.27242e+82
PIMPLE
iteration 2
smoothSolver
:  Solving for UxInitial residual 0.998805, Final residual 1.80506No Iterations 1000
smoothSolver
:  Solving for UyInitial residual 1, Final residual 1.93583e-05No Iterations 1
smoothSolver
:  Solving for UzInitial residual 0.000531627, Final residual 1.42642e-07No Iterations 1
#0  Foam::error::printStack(Foam::Ostream&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::DICSmoother::DICSmoother(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::DICGaussSeidelSmoother::DICGaussSeidelSmoother(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::lduMatrix::smoother::addsymMatrixConstructorToTable<Foam::DICGaussSeidelSmoother>::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
 #7  Foam::lduMatrix::smoother::New(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/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  Foam::GAMGSolver::initVcycle(Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::lduMatrix::smoother>&) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#11
 
in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/bin/pimpleDyMFoam"
#12  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#13
 
in "/home/alpha/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/bin/pimpleDyMFoam" 

I also attached my initial condition files in 0.zip.

Could you please have a look at this issue.

Thanks in advance.

samiam1000 April 3, 2012 03:32

Look at the courant number: it's increasing a lot. I think you should reduce the `maxCo' value in the system/controlDict file.

The solution will be slower, but I think it'll works,

wyldckat April 3, 2012 05:45

Greetings to all!

To add to samiam1000's answer:
edit: I based my answer on Samuele's answer... but apparently the problem is something else, simply because the time step is being automatically adjusted! So, if the time step is automatically adjusted and the solver still crashes, then it's either: a very bad mesh; or boundary conditions; or wrong fvSchemes... Either way, please create a small example case that reproduces your problem and post it here. Otherwise, it'll just be a long and tedious guessing game :(

Best regards,
Bruno

samiam1000 April 3, 2012 05:55

Dear Bruno, Dear All,

thanks for the links that you added.

I think they are very useful.

Also, I do have a problem with buoyantPimpleFoam.

I am trying to impose either temerature or velocity in some cells.

I did the same with buoyanSimpleFoam, but I have problems with the steady state. Could you check the folder I modified, please?

I am attaching the latest version of my solver, here.

Thanks a lot,

Samuele

ebah6 April 4, 2012 19:14

4 Attachment(s)
Quote:

Originally Posted by wyldckat (Post 352865)
Greetings to all!

To add to samiam1000's answer:
edit: I based my answer on Samuele's answer... but apparently the problem is something else, simply because the time step is being automatically adjusted! So, if the time step is automatically adjusted and the solver still crashes, then it's either: a very bad mesh; or boundary conditions; or wrong fvSchemes... Either way, please create a small example case that reproduces your problem and post it here. Otherwise, it'll just be a long and tedious guessing game :(

Best regards,
Bruno

Hello Bruno,

I did some dummy test cases:
1) a square box that rotates with the AMI; structured mesh
2) same thing with unstructured mesh.
Both these cases don't seem to give any error.
3) I did my learning case with unstructured mesh; it consists on two cylindrical rotors (Darrieus). But here I run into trouble with the problem described above.
Attached are some pictures to see how the meshes look like.
For the latter case, you can see the velocity field is messing in the outer domain where no rotation is happening.

Another question I had is how to export hybrid mesh from pointwise to openfoam?
By hybrid I mean unstructured in x-y place and we extrude in the z-direction which will then be structured.
I tried that but only the structured boundary faces are exported not the unstructured ones.

Thank you for your and my best regards.

wyldckat April 5, 2012 09:03

Hi ebah6,

Mmm... I'm not an expert on this subject, but this is what I can see that might be the source of the problems:
  • The cylindrical paddles are very thin, which usually leads to the requirement of additional resolution.
  • The sliding interface seems to be also lacking resolution, but again I'm no expert on this.
  • Still associated to this previous points, why doesn't your Darrieus structure have more cells from the tips of the cylindrical surfaces to the sliding interface, just like you have in the square-box experiments?
  • Replace the square version with a single thin linear paddle (basically a squished square :)), with the same space you've got on the square experiments. If it works well, then there are two kinds of tests to be done:
    1. Try making the paddle thinner, to see how thickness might affect the solver.
    2. Make the paddle longer, so the number of cells reduces between the tips of the paddle and the sliding interface.
My bet is that as soon as the paddle is too close to the sliding interface, in regards to cell count, the solver will start having serious problems.
The other theory is that the thickness of the paddles is having a very big effect on the development of vortexes... and if these are not properly solved, it's only natural that some seriously crazy "fluid pressure shocks" (not a very technical term) will occur.

Another issue might be the speed at which the rotor is running. Proper field initialization might be required to induce the solver to start with good starting values; otherwise, you probably will have to simulate starting with the rotation speed at 0 RPM.

I'm not very familiar with these solvers, but my guess is that if you only want to have an "averaging" result, then one of the LTS solvers might come in handy... although you would have to create one that would LTS with AMI...

Best regards,
Bruno

ebah6 April 10, 2012 18:02

Hello,

Yes Bruno, some of the possible issues are as you mentioned; thanks for your insight.
In particular, as the body becomes thinner, I run into problems.
However, I am only encountering problems when using a turbulence model: the laminar case runs fine.
For the cases with a turbulent flow, I refined the mesh again and again but it still crashes with a skyrocketing Courant Number.
My pressing issue is that I need to deal with thin bodies, so I need to a work-around.

Also, you suggested the STL snappyHexMesh. I did that in a recent past but the sliding interfaces show step like shape dispite the refinement.

Thanks for your help.

wyldckat April 11, 2012 04:38

Hi ebah6,

Mmm, if it's not the mesh, then you've got to start tuning the "fvSchemes" file and possibly the "fvSolution" one as well. Unfortunately I don't know much how to configure them properly for each scenario, so I suggest that you check all of the relevant tutorials in OpenFOAM, as well as the User Guide.

Good luck!
Bruno

iamed18 May 31, 2012 12:11

Similar Quandary
 
Good Afternoon, Everyone!

I come to this place with a similar issue, and upon reading the above comments and filtering through the User Guide for more information about initial conditions for k-epsilon and about the Courant number, I'm still having a heck of a time performing a run.

Let me explain the situation to you (I can't post the 0/ files for various reasons):

A 7m long blunt object is situated in a 10m/s wind-tunnel, with the floor of the tunnel moving with it (so we're in the blunt object's reference frame). The "ground" is of species 1 (alpha1), the wind-tunnel (or atmosphere) is of species 2 (alpha2) and the blunt object is spewing species 3 out of its' side at 40m/s (alpha3).

So, in my back-of-the-envelope calculations (inspired by the User Guide), I set my initial value of k=2.5 and epsilon=0.25. I also set the initial time-step to 0.005sec, and for the sake of early testing I turned off "adjustTimeStep." With all of that said and done, it only completes one iteration of calculation, the output for which is here:

Code:

Courant Number mean: 0.256274 max: 3.73333

PIMPLE: Operating solver in PISO mode

time step continuity errors : sum local = 0.000307692, global = -1.74165e-05, cumulative = -1.74165e-05
DICPCG:  Solving for pcorr, Initial residual = 1, Final residual = 9.01496e-11, No Iterations 589
time step continuity errors : sum local = 4.60233e-10, global = -4.49286e-16, cumulative = -1.74165e-05

Starting time loop

Courant Number mean: 0.27796 max: 9.09506
Interface Courant Number mean: 0 max: 0
Time = 0.005

diagonal:  Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for alpha2, Initial residual = 1, Final residual = 4.83778e-07, No Iterations 1
Air phase volume fraction = 0  Min(alpha1) = 0  Max(alpha1) = 1
Liquid phase volume fraction = 1  Min(alpha2) = 1  Max(alpha2) = 1
diagonal:  Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for alpha2, Initial residual = 0.354522, Final residual = 1.43335e-07, No Iterations 1
Air phase volume fraction = 0  Min(alpha1) = 0  Max(alpha1) = 1
Liquid phase volume fraction = 1  Min(alpha2) = 1  Max(alpha2) = 1
DICPCG:  Solving for p_rgh, Initial residual = 1, Final residual = 0.0479761, No Iterations 305
time step continuity errors : sum local = 2.33578, global = 2.22882, cumulative = 2.2288
[kaleva:14255] 5 more processes have sent help message help-mpi-common-sm.txt / mmap on nfs
[kaleva:14255] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages
DICPCG:  Solving for p_rgh, Initial residual = 0.683683, Final residual = 0.0337928, No Iterations 320
time step continuity errors : sum local = 3.34528, global = 2.22882, cumulative = 4.45762
DICPCG:  Solving for p_rgh, Initial residual = 0.473874, Final residual = 9.50935e-08, No Iterations 467
time step continuity errors : sum local = 2.35844, global = 2.22882, cumulative = 6.68644
DILUPBiCG:  Solving for epsilon, Initial residual = 0.999999, Final residual = 25.758, No Iterations 1001
bounding epsilon, min: -7.75298e+11 max: 1.02524e+12 average: -256836
DILUPBiCG:  Solving for k, Initial residual = 1, Final residual = 89.7085, No Iterations 1001
bounding k, min: -7.39749e+11 max: 6.80932e+11 average: -9.18358e+06
time step continuity errors : sum local = 2.35844, global = 2.22882, cumulative = 8.91526
ExecutionTime = 22.39 s  ClockTime = 23 s

Courant Number mean: 611.356 max: 4.60701e+06
Interface Courant Number mean: 0 max: 0
Time = 0.01

diagonal:  Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for alpha2, Initial residual = 1, Final residual = 1.1291e-10, No Iterations 1
Air phase volume fraction = -1.11442  Min(alpha1) = -339.921  Max(alpha1) = 1
Liquid phase volume fraction = -0.114296  Min(alpha2) = -4.60701e+06  Max(alpha2) = 614.595
[0] #0  Foam::error::printStack(Foam::Ostream&) in "/home/leonard/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #1  Foam::sigFpe::sigHandler(int) in "/home/leonard/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #2  __restore_rt at sigaction.c:0
[0] #3  void Foam::MULES::limiter<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::Field<double>&, Foam::geometricOneField const&, Foam::GeometricField<double,Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/home/leonard/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/interMixingFoam"

I can see where it blows up, I just don't know how to fix it!

I would much appreciate any input anyone has on this matter.
Thanks!

wyldckat May 31, 2012 14:32

Greetings Edward,

OK, if you've read about the Courant number, then you should know that you should check the smallest cell size you've got:
  1. Run:
    Code:

    checkMesh
  2. Search for the "Minimum volume" value.
That smallest cell is the one limiting everything!

Oh, and if checkMesh tells you that you've got bad cells or faces, then that's another source of your problems ;)

Best regards,
Bruno

iamed18 June 1, 2012 09:40

Quote:

Originally Posted by wyldckat (Post 364133)
...check the smallest cell size you've got:

...That smallest cell is the one limiting everything!

I had forgotten about a set of cells I had that were two orders smaller than the rest!

However, I've since decided to go a different route because this takes a painful amount of time to process. I had interFoam running on this large mesh (see checkMesh output below) on 8 CPUs, left it over-night and it had only gotten to 0.08sec by the following morning. Since my goal is a steady-state solution, I think what I want to try is to add the phase mixing of interFoam to the SIMPLE solver of simpleFoam. I took a quick look at it yesterday, and it seems like it will be a formidable task.

Any insight on the matter before I hit the ground running?
Thanks!
~Ed

wyldckat June 1, 2012 09:50

Hi Edward,

Mmm, you forgot to attach your checkMesh log. ;)

Anyway, if you want the steady state solution with interFoam, then probably this is what you want: http://www.openfoam.org/version2.0.0/steady-vof.php

Best regards,
Bruno


All times are GMT -4. The time now is 12:38.