[foamiste]

Hello foamers,

Does anyone work on multiphase cases, especially with solvers: twoPahseEulerFoam and multiphaseEulerFoam?

[avila.vc]

Hi. I do. I work with twoPhaseEulerFoam.

[foamiste]

Did you ever get this error message?? because at first everything was ok from time=0 to time=0.0410 with timeStep=0.0002

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

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::rhoConst<Foam::specie> >; Type = Foam::sensibleInternalEnergy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::rho Const<Foam::specie> >, Foam::sensibleInternalEnergy>]
in file /opt/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.

FOAM aborting

[mnikku]

From my limited experience this error could be due (but not limited) to
a) problems in defining the boundary conditions
b) too large time step

Temperature of one the phases is probably showing negative temperatures in Kelvins? I had this several times, but managed to fix with checking the boundary conditions.

[avila.vc]

Please, post the log from the last timesteps, so we can have a better idea about what is happening. Also, your checkMesh log and explain your case

[foamiste]

Thank you for your fast reply

I am simulating a mixing tank with MRF zone and two phases (fluid+particles) . I have 5 walls and 1 symmetry plane. I am not interested about heat transfer in my case ( but I don't know how to desactivate it)

For the boundary conditions:
alpha.particles: zerogradient in the walls
alpha.water: zerogradient in the walls

alphat.particles: calculated $InternalField
alphat.water: calculated $InternalField

epsilon.water: epsilonWallFunction $InternalField
k.water: kqRWallFunction $InternalField
nut.water: nutkWallFunction $internalFields
nut.particles:calculated $InternalField

p: calculated $InternalField
p_rgh: fixedFluxPressure $internalField

T.particles: fixedValue $internalField
T.water: fixedValue $internalField
Theta.particles: fixedValue $internalField

U.particles & U.water: fixedValue (0 0 0) in 4 walls and rotatingWallVelocity in 1 wall


NB: for the symmetry plane all the boundary conditions are defined as symmetryPlane

Please find attached my checkMEsh and the last timesteps in my log

[mnikku]

Courant number is also increasing before the crash but already at the beginning of log of the last timesteps T.particles is ~100 K and T.water ~230 K. Do you have maxCo set on your controlDict? It should be below 1, I use 0.5 and still get less with the maxDeltaT used.

Does your solution converge to the criterion you have set? The log-file doesn't report that solution would have converged, though it doesn't report it not having converged either...

[foamiste]

This is my controlDict for maxCo is set on 0.9.. Please find attached my file controlDict

How can I desactivate heat transfer? because as i mentionned i don't need it, also it can be the problem that block convergence.

[mnikku]

I think you should have the adjustTimeStep as yes for the maxCo and maxDeltaT to work.
As for the heat transfer, probably there is no way to deactivate it without modifying the solver. In my isothermal cases I set all the phases to the same temperature, so there is no heat transfer. However, as you can see from the twoPhaseEulerFoam/EEqns.H, there are other things affecting to the energy equation than just temperature and this is causing the problems to appear in the temperature. From my experience, the problems in the temperature field are symptoms from problems elsewhere, so the deactivation of heat transfer won't be a solution.

[avila.vc]

What value did you set the temperatures at initial conditions?
what are your other internalFields? your boundaries were incomplete when you posted. Post them complete, please.

Follow mnikku advice and set adjustTimeStep on controlDict
Put maxDeltaT = 1 on controlDict

Now, I am assuming you are using the tutorials configuration for my tips below:

You may need to correct orthogonality, it seems a bit high (58), try using 1 or 2 non-ortho correctors on fvSolution and maybe test snGrad and laplacian with limited 0.777 at fvSchemes (change the word uncorrected to limited 0.777)

You have big mesh, half million cells, so try increasing nCellsonCoarsestLevel to 500 (at GAMG solver at fvSolution)

Post your fvSchemes and fvSolution for us to check if there is anything else.

Edit: I use this solver to simulate liquid-gas flows, so if there is any specific problems with particles configuration I am not sure I will notice it. Also, I dont have experiente with boundary condition as simmetryPlane neither with movingWalls, so you may re-check those aspects independently.

Edit2: also post yous constant files (phaseProp, turbulences, thermo..prop.)

Edit3: re-checking your logfile, it really seems you got something not well-configurated for temperature low values to appear, post your logfile since a bit before the temperatures get below 273.

[foamiste]

please find attachef 0 files of alpha and alphat aloso epsilon

[foamiste]

Find attached k, nut, and p

[foamiste]

Find attached T, Theta and U

[foamiste]

These are my constant files

[foamiste]

This is my log with fvschemes and fvsolution

[avila.vc]

Hi, on the logfile you sent, T.particles starts below 200, show us from the beginning.

Remove the word bounded from divSchemes. As far as I know, limitedLinear and vanLeer dont need it.

turbulence and thermo.prop. particles are the same as the tutorial, right? if not, try running with the same parameters for those.

What is liquid level on your geometry? show us your mesh. If there is a region with just one phase, you should use setFieldsDict

Try following also the previous tips I gave you, but it is really important to look at the logfile when the temperature falls below 300K and the geometry.

As I said, I dont know much about moving wall nor particles simulations, if the error is related about those aspects, I probably wouldnt notice.

[foamiste]

Hi, thank you for all your clarifications, well I tested moving wall previously with one phase and it works perfectly so I am pretty sure that it isn't the problem. And for particles it's my first time to work with so it can probably the source of the problem.
For now, please find attached my log file divided on 5 files because it is heavy to be uploaded for once, if you can pick which is the problem about the temperature especially for particles

[mnikku]

Looking at your fvSolution I'd suggest adding some more iterations to the nOuterCorrectors and testing how that affects your solution. You might want to add also the residualControl for PIMPLE.
Based on the log files, the temperature "leak" begins from the start. I had similar issues (either that or "leak" in alpha.particles) and this was due to solution not converging.

[foamiste]

Thank you for all your advice, I don't have temperature problem anymore. It seems that the solution converges.

Now I am interested at simulating the same thing but in steady state. Is it possible with twoPhaseEulerFoam or should I try to construct my own solver?

Best regards

[foamiste]

Hello foamers,

While I am running me case using the solver twoPhaseEulerFoam, at first everything seems to be OK but after 4 second and in just one step the temperaure goes from 299K to -117K so openfoam exit!! I don't know what could be the source of this crush.
Please find attached my log.
Any answer or remark will be appreciated.

Thanks in advance