Hi All! I am using VOF model for simulating flow of liquid in vessel, solver is steady, segregated. Mixture of liquid and gas flow into the vessel from top (pressure inlet) and there two exits (pressure outlets) for gas and liquid (shortly it is a separator vessel). Solution converges in approx. 170 iteration BUT the result is not real. There is no phase separation taking place, the whole volume is filled up with mixture. Gravity option is enabled.

What could be the problem?

I need your help very much, since there is noone ask.

Hi,

steady : are you sure ?

For 90 % of the cases :

unsteady / Geo-reconstruct / small time step.

phase 1 : the lightest

Discretisation : Pressure : if gravity => Body force weighted / Pressure-velocity coupling : Piso.

Under-relaxation factor : 1 for volume fraction

And : skewness < 0,85

steph

As I remember, a VOF calculation must be done in transient.

You speak about phase separation: for VOF method, the 2 fluids must be non-miscible. So they are already separated.

I think you make a confusion between VOF method and euler-euler method.

Hi, If you use VOF model, it is recommended to use unsteady solver because the interface is unsteady and the liquid phase and the gas phase should be set separatly.

Hi All! Thanks for the response! Well I'm not sure about the steady/unsteady, so I tried as Steph offered, but in order to keep it running I had to set very small time step (1e-5 or even 5e-6). If i increase time step then Fluent reports "divergence detected in AMG solver: epsilon". Is it the way it should be? On the other hand according to results i have so far in unsteady (5000 time steps) it seems like the separation works.

So again I ask for your help, how can i decrease time step value? Or may be there is some other point to be considered?

Thanks All again!

Well, I don't know anything in particular about the reason of the divergence detected in the Algebraic MultiGrid solver, but I can suggest you a practice to find out a good TS (not too small) for a stable run:

-Start the simulation with a very small TS, allowing good convergence within 20 it. per time step. -After a number of TS save the data. -Specify a very large TS (at least 6 orders of magnitude larger than before). -Fluent should pass an error detailing the number N of VOF sub-time steps needed to cover the specified deltaT. -Thus, the VOF sub-time step is tau=deltaT/N. -They suggest to continue the simulation with a time step within the limit of 10-20 sub-time steps.

Hope it helps, Edi.

Thanks for response, presently I am doing almost the same, start with 1e-5 time step, after a few steps gradually increase it so that it takes 10-20 iteration per time step as you mentioned. On the other hand I'm wondering whether it is possible to increase time step without letting it diverge, may be by changing URF or something else.

Thanks for any idea and response!

And I am wondering whether it is possible this problem in steady mode. Short description is as follows: liquid with gas enter horizontal vessel and fall on an inclined shelf (sorry, not sure if this the wright word for it). Then gas separates from liq, liquid flows down the shelf as a film. Degassed liq goes to the bottom of vessel and leaves through preassure outlet, gas does the same from the top. As to me it seems like it could solved in steady mode, what you say?

Thanks again for any assistance!

I think you better change your model (VOF is preferred for stratified or free-surface flows, phases immiscibles), try eulerian or mixture.

By the way, I set these URFs for my liquid sloshing problem:

-pressure: 0.6 -momentum: 0.8 -others: 1

(discretization: BFW for pressure, PISO for pressure-velocity coupling)

Edi.

Ok I'll try to change the model, hope it will work

Your system is not steady, so you have to simulate it as unsteady. When you choose the time step, remember that you need to respect both numerical conditions (none for implicit schemes) and physical contraints. So your time step has to be smaller than the characteristic time of the phenomena you want to model.

The Eulerian model seems more appropriate to your case. You'd better to use a velocity inlet however, if possible.

Regards, ap

Well thanks, now it is clear that it should be unsteady (at least it works). As for the time step, seems like it is also clear. And the pressure inlet seems to be not the best choise, anyway to start up i have to init with velocity, otherwise fluent reports divergence in amg: pressure correction.

Well, thanks to All for the assistance again!

I'd like to add something on the choice of the boundary condition.

You have to choose pressure inlet when you have a compressible flow, while if you have an uncompressible one, velocity inlet should be the choice.

Regards, ap

Thanks for the assistance! Solution seems to work now, all equations converge but continuity. Its scaled residual is usually increasing as more time steps are proceeded (it goes up to 10e-1 or even more). Should i worry about it? May be i can use normalaized residual instead? Any advises are welcome

Thanks in advance!

Try to under-relax the momentum equation. Usually a good choice is to reduce momentum under-relaxation factor and to slightly increace the pressure URF.

Regards, ap