Dears, I've a problem with Fo
 

Dears,
I've a problem with Foam simulation. I've defined a 3d domain (simple cylinder with inlet, outlet and wall) using Salome and then I've correctly imported the .unv file in Foam. When I launch a simulation using "simpleFoam" the results are the following messages:

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0142031, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0570803, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0482498, No Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.008993, No Iterations 18
time step continuity errors : sum local = 0.492712, global = -0.0016149, cumulative = -0.0016149
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/home/matteo/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/matteo/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xffffe420]
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/matteo/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 void Foam::divide<foam::fvpatchfield,>(Foam::GeometricF ield<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&) in "/home/matteo/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/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 "/home/matteo/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTurbule nceModels.so"
#6 Foam::turbulenceModels::kEpsilon::correct() in "/home/matteo/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTurbule nceModels.so"
#7 main in "/home/matteo/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#9 Foam::regIOobject::readIfModified() in "/home/matteo/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/simpleFoam"
Floating point exception (core dumped)

Is there someone that could help me?
Thanks
Stefano.

I bet you initialised k or eps
 

I bet you initialised k or epsilon to zero, probably in the internal field: check your files 0/k and 0/epsilon.

If so, pick your own punishment http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Hrv

Thanks While I'm punishing m
 

Thanks
While I'm punishing myself, could you to explain me something about this initialization values?
Stefano.

Yes, have a look at the k-epsi
 

Yes, have a look at the k-epsilon equations:

mu_t = C_mu sqt(k)/epsilon

and the source terms in epsilon eqn (for example)

C1 G epsilon/k and
C2 sqr(epsilon)/k

Thus, while

k = epsilon = 0

formally satisfies the equation set, you will get floating point exception: division by zero.

Got it?

Hrv

Yes, thanks. If we consider
 

Yes, thanks.

If we consider two different variables, i.e. turbulence intensity I and turbulent viscosity ratio Rv = mu(t) / mu where:

I = u' / u(avg) = 0.16 * Re(Dh)^-1/8;
Rv = [1, 10];

it is correct to assume:

k = (3 / 2) * (u(avg) * I)^2;
eps = rho * C(mu) * (k^2 / mu) * Rv^-1;
C(mu) = 0.09 (only for k-eps model)

Ste.