[mou_mi]

Hi

I ran a case with kEpsilon model and set the wall for "k" and "epsilon" as a fixedValue for B.C. and OF gave me this error for "k" and "epsilon",


Create mesh for time = 70

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model kEpsilon

Starting time loop

Time = 70.001

Courant Number mean: 0.00103968 max: 0.0494671
DILUPBiCG: Solving for Ux, Initial residual = 5.85686e-05, Final residual = 4.6585e-10, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.000515567, Final residual = 3.09483e-09, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.00109401, Final residual = 7.4057e-09, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.942377, Final residual = 9.56964e-07, No Iterations 273
time step continuity errors : sum local = 2.11503e-12, global = 2.74312e-14, cumulative = 2.74312e-14
DICPCG: Solving for p, Initial residual = 0.000860842, Final residual = 9.75e-07, No Iterations 164
time step continuity errors : sum local = 4.12992e-12, global = -7.69118e-14, cumulative = -4.94806e-14


--> FOAM FATAL ERROR : fixedValue is the wrong epsilon patchField type for wall-functions on patch wall
should be zeroGradient

From function wall-function evaluation
in file /home/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/checkPatchFieldTypes.H at line 13.

FOAM exiting


I changed them to "zeroGradient" for wall boundary, after some calculation in the first time step it gave this error.

Create mesh for time = 70

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model kEpsilon

Starting time loop

Time = 70.001

Courant Number mean: 0.00103968 max: 0.0494671
DILUPBiCG: Solving for Ux, Initial residual = 5.85686e-05, Final residual = 4.6585e-10, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.000515567, Final residual = 3.09483e-09, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.00109401, Final residual = 7.4057e-09, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.942377, Final residual = 9.56964e-07, No Iterations 273
time step continuity errors : sum local = 2.11503e-12, global = 2.74312e-14, cumulative = 2.74312e-14
DICPCG: Solving for p, Initial residual = 0.000860842, Final residual = 9.75e-07, No Iterations 164
time step continuity errors : sum local = 4.12992e-12, global = -7.69118e-14, cumulative = -4.94806e-14
#0 Foam::error::printStack(Foam:stream&) in "/usr/local/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/usr/local/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt in "/lib64/tls/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/usr/local/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 void Foam::divide<foam::fvpatchfield,>(Foam::GeometricF ield<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&) in "/usr/local/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libincompressibleTurbule nceModels.so"
#5 Foam::tmp<foam::geometricfield<double,> > Foam::operator/<foam::fvpatchfield,>(Foam::tmp<foam::geometricfie ld<double,> > const&, Foam::GeometricField<double,> const&) in "/usr/local/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libincompressibleTurbule nceModels.so"
#6 Foam::turbulenceModels::kEpsilon::correct() in "/usr/local/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libincompressibleTurbule nceModels.so"
#7 main in "/usr/local/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/turbFoam"
#8 __libc_start_main in "/lib64/tls/libc.so.6"
#9 Foam::regIOobject::readIfModified() in "/usr/local/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/turbFoam"
Floating exception




would you help me what happened here?

Thank you
mou

[andersking]

Hi,

Floating Point Exception means that some of you numbers are unbounded - Inf (infinity) or NaN (not a number). Sometimes this can be overcome by executing
unset FOAM_SIGFPE
and running your simulation again (this basically stops checking for out of bounds errors).
Most of the time this won't fix the problem, however, it is more likely to be a problem with boundary conditions or the mesh.

Cheers
Andrew

[ngj]

Hi Mou

From your error-messages, especially #3 and #6, tells me that you are dividing by 0 in your turbulence model. Do you on any of your boundaries, inlet, outlet, etc, set either k or epsilon to 0 in stead of 1e-11?
My experience is that these properties cannot be zero, as you are dividing with them. I also believe that it would be necessary to put k!=0 in the interior, but you probably already have that.

Best regards,

Niels

[mou_mi]

hi Niels

as you mentioned, I set 0 for the k and it was the problem.

Thank you
mou