|
[Sponsors] |
December 19, 2007, 10:46 |
Dears,
I've a problem with Fo
|
#1 |
New Member
Stefano Dalla Costa
Join Date: Mar 2009
Posts: 4
Rep Power: 17 |
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:stream&) 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. |
|
December 19, 2007, 10:54 |
I bet you initialised k or eps
|
#2 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
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 Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
December 19, 2007, 11:13 |
Thanks
While I'm punishing m
|
#3 |
New Member
Stefano Dalla Costa
Join Date: Mar 2009
Posts: 4
Rep Power: 17 |
Thanks
While I'm punishing myself, could you to explain me something about this initialization values? Stefano. |
|
December 19, 2007, 14:35 |
Yes, have a look at the k-epsi
|
#4 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
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
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
December 20, 2007, 03:11 |
Yes, thanks.
If we consider
|
#5 |
New Member
Stefano Dalla Costa
Join Date: Mar 2009
Posts: 4
Rep Power: 17 |
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. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Compiling MRFSimple foam error | mrangitschdowcom | OpenFOAM Installation | 0 | September 15, 2008 15:09 |
FOAM FATAL IO ERROR | msrinath80 | OpenFOAM Running, Solving & CFD | 4 | July 30, 2008 10:06 |
FOAM FATAL ERROR | derath | OpenFOAM Pre-Processing | 1 | June 10, 2006 14:20 |
FOAM installation error gcc amp g | hanks | OpenFOAM Installation | 9 | January 26, 2006 14:14 |
FOAM FATAL IO ERROR | sita | OpenFOAM Running, Solving & CFD | 2 | August 23, 2005 04:37 |