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

Error during Foam simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 19, 2007, 11:46
Default Dears, I've a problem with Fo
  #1
New Member
 
Stefano Dalla Costa
Join Date: Mar 2009
Posts: 4
Rep Power: 8
stefano is on a distinguished road
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.
stefano is offline   Reply With Quote

Old   December 19, 2007, 11:54
Default I bet you initialised k or eps
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
hjasak is offline   Reply With Quote

Old   December 19, 2007, 12:13
Default Thanks While I'm punishing m
  #3
New Member
 
Stefano Dalla Costa
Join Date: Mar 2009
Posts: 4
Rep Power: 8
stefano is on a distinguished road
Thanks
While I'm punishing myself, could you to explain me something about this initialization values?
Stefano.
stefano is offline   Reply With Quote

Old   December 19, 2007, 15:35
Default Yes, have a look at the k-epsi
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
hjasak is offline   Reply With Quote

Old   December 20, 2007, 04:11
Default Yes, thanks. If we consider
  #5
New Member
 
Stefano Dalla Costa
Join Date: Mar 2009
Posts: 4
Rep Power: 8
stefano is on a distinguished road
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.
stefano 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
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 15:14
FOAM FATAL IO ERROR sita OpenFOAM Running, Solving & CFD 2 August 23, 2005 04:37


All times are GMT -4. The time now is 15:41.