CFD Online Discussion Forums - sonicFoam "prism" tutorial not working when inlet velocity is increased

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - sonicFoam "prism" tutorial not working when inlet velocity is increased (https://www.cfd-online.com/Forums/openfoam-solving/219112-sonicfoam-prism-tutorial-not-working-when-inlet-velocity-increased.html)

sonicFoam "prism" tutorial not working when inlet velocity is increased

hello foamDudes

I took up a tutorial case $FOAM_TUTORIALS/compressible/sonicFoam/RAS/prism

the default inlet velocity boundary condition in the tutorial was 650(which is M =1.89)

In 0 folder i have changed velocity from (650 0 0) to (1030 0 0) at inlet, top and bottom wall boundaries to get to Mach 3 over the prism, i havent changed anything else and then this error shows up while i try to run it:

HTML Code:

Time = 3.25e-05



Courant Number mean: 0.056095 max: 0.45764

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

PIMPLE: iteration 1

smoothSolver:  Solving for Ux, Initial residual = 0.00361405, Final residual = 1.25973e-07, No Iterations 2

smoothSolver:  Solving for Uy, Initial residual = 0.0121551, Final residual = 5.68609e-07, No Iterations 2

smoothSolver:  Solving for e, Initial residual = 0.00566519, Final residual = 3.57166e-07, No Iterations 2





--> FOAM FATAL ERROR:

Negative initial temperature T0: -32.7705



    From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hConstThermo<Foam::perfectGas<Foam::specie> >; Type = Foam::sensibleInternalEnergy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy>]

    in file /home/pawan/OpenFOAM/OpenFOAM-v1812/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 54.



FOAM aborting



#0  Foam::error::printStack(Foam::Ostream&)sh: 1: addr2line: not found

 addr2line failed

#1  Foam::error::abort()sh: 1: addr2line: not found

 addr2line failed

#2  Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy>::TEs(double, double, double) constsh: 1: addr2line: not found

 addr2line failed

#3  Foam::hePsiThermo<Foam::psiThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, bool)sh: 1: addr2line: not found

 addr2line failed

#4  Foam::hePsiThermo<Foam::psiThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct()sh: 1: addr2line: not found

 addr2line failed

#5  ?sh: 1: addr2line: not found

 addr2line failed

#6  __libc_start_mainsh: 1: addr2line: not found

 addr2line failed

#7  ?sh: 1: addr2line: not found

 addr2line failed

Aborted (core dumped)

please help me out in fixing this error to run the simulation at high mach numbers.
(i have later changed k and epsilon values in 0 folder but still the same story)

Apparently you reach nonphysical temperatures, this several different reasons may lead to this behavior.
In order to assess it several infos are missing from your post:

0 folder
checkMesh output,
fvSchemes used
fvSolution used
controlDict

If everything above is setup properly (BC, high quality mesh, low order schemes, properly set up of PIMPLE and relaxations, appropriate timestep... ), and still the computation explode, I suggest you to use fvOptions and add some limiters, in particular limiting temperature, so as to avoid nonphysical issues.

During the first part of the computation, the flow develops and hence it may reach very strong gradients (in particular near the object of interest). Hence by introducing temperature limiters, a decrease convergence / flow development rate can be expected, but overall computation stability shall be stiffer.

Seeing as how your timestep is good in this case, my bet is that you're using a scheme for temperature which can oscillate in the presence of sharp gradients, leading to zero temperatures. You can check if this is the issue by changing the temperature scheme to upwind.

I have resolved this issue successfully, by replacing the mesh, i just made a bad mesh! reducing the time step also dint work.

I suggest everyone to use ICEMCFD instead of doing blind meshing inside Mesh button of Ansys workbench. make sure aspect ratio is less than 20 in the regions away from the wall, there is no issue with cells with aspect ratio of even 200 closer to the walls.

a greatman once said:
"One who owns the Mesh, owns the solution"

Openfoam is not like fluent, it does not have robust automated adjustments which can manage divergence issues. In OF we need to tweak the schemes and paramaters a bit but the end result that OF gives you is more reliable is what i feel. cheers!

thanks a lot for the replies