Error, rhosimplefoam solver
 

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::printStack(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::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::calculate() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::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

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

Richard

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

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.

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

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.

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 :-)

good to know :)