[schalinski]

hey guys.
At first, great work you're doing here.
I'm completely new to openfoam, but i try to do some simulation of a gas burner.
when i start the solver, the following error-message appears:

Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0290357, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0162366, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.014761, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.517934, Final residual = 0.00675935, No Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 9.90403e-05, No Iterations 598
DICPCG: Solving for p, Initial residual = 0.401541, Final residual = 3.90591e-05, No Iterations 214
DICPCG: Solving for p, Initial residual = 0.0953977, Final residual = 9.29665e-06, No Iterations 266
time step continuity errors : sum local = 13.4007, global = 0.347056, cumulative = 0.347056
rho max/min : 0.821852 0.001
DILUPBiCG: Solving for omega, Initial residual = 1, Final residual = 0.0530614, No Iterations 2
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.0229082, No Iterations 2
ExecutionTime = 712.65 s ClockTime = 724 s

Time = 2

DILUPBiCG: Solving for Ux, Initial residual = 0.400034, Final residual = 0.0251938, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.457358, Final residual = 0.0190353, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.421311, Final residual = 0.0167393, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.0557149, No Iterations 2
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/libc.so.6"
#3 Foam::hPsiThermo<Foam:ureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam:erfectGas> > > > >::calculate() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam:ureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam:erfectGas> > > > >::correct() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#5
in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/rhoSimpleFoam"
#6 __libc_start_main in "/lib/libc.so.6"
#7
in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/rhoSimpleFoam"
Floating point exception (core dumped)


Would be great if anyone could help me.
As i already mentioned, i'm completely new to openfoam, solvers,...

Thanks in advance for your help!

Johannes

[moser_r]

If you're still having this problem, can you post the content of your /constant/thermophysicalProperties dictionary file?

Richard

[kalyangoparaju]

Hi,

I had exactly the same problem. I am trying to simulate a flow through a simple catalytic converter and I am using rhoPorousMRFSimpleFoam and I get the same error during the second iteration. I decreased the relaxation factors for p and rho to 0.05 each and that seems to work. I have decent results but unfortunately my timestep continuity error is quite high. It oscillates between 60 and 25

Kalyan

[mihaipruna]

check your fvsolution equation relaxation factors, make them bigger than 0.9.
you should have p and rho for field and the rest for equation relaxation factors.
also checking the thermo is a good idea, post it here maybe.

[kalyangoparaju]

Mihai,

Thanks for the reply. I am sorry but i don't understand your suggestion.

Do you want me to assign pressure and density relaxation to be greater than 0.9? Is there a reason why this might work?

Also, I setup the case almost exactly like the tutorial case ( rhoporousMRFsimpleFOAM - angledductexplicit) and I really don't understand the reason for the problem. I tried removing the porous zone and checking how rhoSimpleFoam would work and I still have the same problem. On the other hand, I don't have any problems with the incompressible case. This surely points towards the boundary and the initial conditions of the case.

Here are my boundary conditions

pressure
Inlet - zeroGradient
Outlet - fixedValue
walls -zeroGradient

Velocity
Inlet - flowRateInletVelocity
outlet - inletOutlet
walls - fixedValue ( 0 for no-slip)

Temperature
Inlet - fixedValue
Outlet - fixedvalue
walls - zeroGradient

This case is supposed to be a heat transfer case and hence I have to specific temperatures on both the inlet and outlet . I am not really confident if this over does the boundary conditions.

I am really sorry but the files are in my office and I don't think I have the permissions to share them. I will try my best to properly represent my case though.

Thanks,
Kalyan Goparaju

[mihaipruna]

I was struggling with the same problem and I got one case to work by setting those values in fvsolution as follows.
Be advised I am using rhoSimplecFoam .

relaxationFactors
{
fields
{
p 0.810000;
rho 0.810000;
}
equations
{
U 0.900000;
h 0.900000;
k 0.900000;
omega 0.900000;
}
}


However, I am now finding out the mesh quality might play a role as well. I will keep you posted on my findings.

[kalyangoparaju]

Mihai, u

Thanks a lot for the reply.

I actually was able to solve my problem.

The problem with my setup was that, the porous resistance was quite large and I somehow overlooked that and used an explicit porosity formulation which the solver didn't like. I changed the fvSolution dictionary to use the implicit porosity formulation and BAZINGA !!

But, I will definitely remember your advice for future problems.

Kalyan

Note - I had to use a pressure under relaxation value of 0.2 and density under relaxation of 0.05. It might have worked for higher values, but I didn't want to lose my almost perfect results :-)

[mihaipruna]

good to know