[Kostas_K]

Hi everyone,

I have been using OpenFoam for a while now so i have a little experience. So i was trying to simulate the flow over a 10% bump located inside a duct using rhoSimpleFoam. i have already solved it using turbulence model kEpsilon. the resulted y+ was between 1~3. So now i am trying to solve it using kOmegaSTT turbulence model. Since y+ is small, for the near wall treatment i am not using wall functions. Instead i define the values of k and omega as shown:
for k i use fixedValue with value 1e-10
for omega i use fixedValue with value 1e-10
To avoid potential erroneous arithmetic operations

I also tried solving using wall functions and in both situations (wall functions or not) i always end up with the same kind of error after the second timestep.

Error:

Time = 0.02

smoothSolver: Solving for Ux, Initial residual = 0.993471, Final residual = 0.598954, No Iterations 1000
smoothSolver: Solving for Uy, Initial residual = 0.906122, Final residual = 0.0897325, No Iterations 103
smoothSolver: Solving for Uz, Initial residual = 0.994686, Final residual = 0.239216, No Iterations 1000
smoothSolver: Solving for h, Initial residual = 0.998906, Final residual = 0.105037, No Iterations 1000
DICPCG: Solving for p, Initial residual = 0.991894, Final residual = 0.00967679, No Iterations 162
time step continuity errors : sum local = 1.73028, global = -0.117048, cumulative = -0.117048
rho max/min : 2 0.5
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::symGaussSeidelSmoother::smooth(Foam::word const&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::Field<double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, unsigned char, int) at ??:?
#4 Foam::symGaussSeidelSmoother::smooth(Foam::Field<d ouble>&, Foam::Field<double> const&, unsigned char, int) const at ??:?
#5 Foam::smoothSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#6 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) at ??:?
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#8 Foam::SolverPerformance<double> Foam::solve<double>(Foam::tmp<Foam::fvMatrix<doubl e> > const&) at ??:?
#9 Foam::compressible::RASModels::kOmegaSST::correct( ) at ??:?
#10
at ??:?
#11 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#12
at ??:?
Floating point exception (core dumped)


Does anyone have any idea why this is happening ?
And what do i have to do to fix it ??

Thanks in advance !!

[teuk]

Hi Kostas,


check your omega wall boundary condition.

What is your inital U-field? If it's zero: How is your U inlet condition?
(omega is not close to 0 at walls if an inital U-field is present, try zeroGradient)

Regards,
Teuk

[RodriguezFatz]

I just had a look at an old case and here I used omega=1000 and k=2 as initial condition.
Also, please post your b.c. of k and omega.

[Kostas_K]

Since i made the question i 've changed the files quite a bit but i will post them.
Also if anybody has a similar case and is happy to share it, that would be great so i can use it (or anybody else who has the same problem) as a tutorial.

thanks in advance.

[RodriguezFatz]

Kostas, you are using wrong boundary conditions.
I guess "upstream", "Bump" and "Downstream" are walls?
1) For "k" you use a wall function, but you wrote that you have y+ = 1..3, so set it to 1e-12.
2) For omega you also use a wall function, but this time it is correct, since it is for high and low-Re. So keep it. But "value" is used for the very first iteration as initialization as far as I know. Your simulations seems to crash here, so set it to some realistic value, such as 1e7. "teuk" already wrote that 0 is no realistic value for omega at the walls in his post.