[nileshjrane]

Hi folks,

I am trying to solve mixing of air and fuel jets in a combustor. PFA the case dict.

When i solve the case with rhoPisoFoam, the case diverges after some time. but till that time, when opened in paraview, i noticed that pressure wave is stating from inlet and it goes on reflection from walls and the inlets and outlets. The wave keeps moving in the domain. I searched on the forum for such problem. i couldn't find the solution for this. I have never done much of subsonic compressible simulations and i never saw such issue before.

I tried changing numerical schemes and relax. factors. but all in vein.

Anyone has any solution any info for this??

[nileshjrane]

some more info:

The solution always end with same error:

--> FOAM FATAL ERROR:
Maximum number of iterations exceeded

From function specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const
in file /home/opencfd/OpenFOAM/OpenFOAM-1.7.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 67.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam170/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam170/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::hPsiThermo<Foam:ureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > >::calculate() in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#3 Foam::hPsiThermo<Foam:ureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > >::correct() in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#4
in "/opt/openfoam170/applications/bin/linux64GccDPOpt/rhoPisoFoam"
#5 __libc_start_main in "/lib/libc.so.6"
#6
in "/opt/openfoam170/applications/bin/linux64GccDPOpt/rhoPisoFoam"
Aborted

This happens sooner or later depending on the change in BC. I think i might get correct solution if i can make it to run for long enough. But i just can't.

[alberto]

Mach number?

[nileshjrane]

Hi Alberto,

The mach number is 0.3 at air inlet (the pipe attaching from side) and 1 at fuel stream (chocked nozzle).

I suspect the pressures are not appropriate. (the values i have got are from my counter parts who r designing other components. Its a ducted rocket basically). As after doing some runs i saw that the air stream actually goes supersonic and a normal shock is forming. But as the shock tries to go out of the air inlet pipe the solution blows. PFA the pic of the last time step where it diverges.

Somewhere on the forum someone suggested that one can modify the max number of iterations for the solver in "/home/opencfd/OpenFOAM/OpenFOAM-1.7.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H", but i didn't like the idea as i suppose the physics need some check. I tried many things but numerics seem fine as it does make much difference. So i am currently trying with pressure BC.

[nileshjrane]

updates:

I figured out that the pressure BC are unrealistic. There is huge pressure jump at inlets and thus flow goes supersonic. And a normal shock is the ultimate fate.

So i reduced the pressure jump to zero with many intermediate permutations. Now i am using these pressure BCs:

Air inlet : 2358000Pa
Fuel inlet: 2400000Pa
Outlet: 2358000Pa
Initialisation of P: 2358000Pa

Now this is very much physical situation. But still i am getting tha pressure wave moving back and forth like a shock in a shock tube. and my solution meets same fate as i said in earlier posts sooner or later.

I think zeroGradient BC is prone to pressure wave relections ,please correct me if m wrong. So i tried with fixedValue or waveTransmissive BC as well but all in vein..


My problem is similar to this one: http://www.cfd-online.com/Forums/ope...implefoam.html

[Chris Lucas]

Hi,

at this high velocities, you should modify the solver a little bit. First of all, are you using the transonic setting for the pressure equation? Otherwise, the pressure equation is (more or less) for an incompressible flow (at least this is what I think). Secondly, a might want to implement a total energy equation instead of the thermal energy equation used in rhoPisoFoam.

http://www.cfd-online.com/Forums/ope...-equation.html

About the reflection outlet BC, there is no simple solution so far. You could program a new non reflection BC (would be great ). The Other possibility might be to place the outlet BC far away from the area of interest. This away, the dissipation might dissipate all pressure waves in the system (at least it helped me).

Regards,
Christian

[nileshjrane]

Thanx for reply Chris,

I am surprized to know that rhoPisoFoam does not solve energy equation. I never thought about it.

I have got only 3weeks to finish the simulations and its not possible to modify anything in the solver for me now. I have never used c++ before, neither i have enough knowledge of numerical schemes i feel.

I am thinking of writing a density based solver after this task is over.

[Chris Lucas]

Hi,

either I misunderstand you or you misunderstood me. rhoPisoFoam solves the thermal energy equation, which is fine for low speed flows. The total energy equation is more correct for high speed flows (link above).

About the transonic setting. Add "transonic true" in the fvSolution file under Piso.

Use low Co numbers. The BC should be far away from the area of interest.
Use limitedLinear Schemes for div. at least this works for me.


Regards,
Christian

[nileshjrane]

I made a boo boo..Sorry..i missed "total" word before energy equation. it should have been total energy equation rather than just energy equation. Sorry, my bad.

[alberto]

Have you ever considered rhoCentralFoam?

[nileshjrane]

Hello Alberto,

I did have a look at all the available solvers. rhoCentralFoam isn't meant for turbulent flows thats the problem. But it does solve total energy (rhoE) i suppose rather than enthalpy (h).

[alberto]

Well, if that's the solver that works in your case, adding turbulence means coding a bit... Probably better than trying to make a solver work at the limit of its capabilities.