[piyusharas]

Just consider I am modelling a flow in which water comes from a inlet on top an it splashes on the bottom wall of tank kept 40 mm down the inlet and then distributes in 6 symmetric outlets in the plate.
I am using a VOF model with primary phase as air and secondary phase as water.
Can someone please tell me what else should I consider . Is there some special model to consider the splash effect of water.
Please try to elaborate a little .

[mido66]

I think you will need the following parameters :

- general : transcient
- models VOF, implicit, with 'implicit body force' and 'zonal discretization'
- primary phase : air, secondary phase water-liquid
- phase's interactions : - surface tension (wall adhesion + constant surface tension = 0.072 N/m) - phase localized compressive scheme (constant = 2)
- 1 for water volume fraction inlet et 0 for outlets
- operating conditions with gravity et operating density
- initialization from inlet except water volume ration = 0 (i'm not sur about this point)
- if there are divergence problemes, halve default solution controls
- for the beginning, put onl first order upwind except gradient (put LSCB), pressure (put BFW) and volume fraction (put Compressive)

Try with that and see ...

Sorry for my english, and good luck !

[piyusharas]

One more thing do I have to keep my tank in which the tank is flowing or can I just apply or this to the fluid domain suppressing the tank after I fill it will fluid domain.???

[piyusharas]

You said
"1 for water volume fraction inlet 0 for outlets "

Here setting volume fraction for water 1 at inlet is fine but in case of outlet there is option of backflow volume fraction. Shoould I set it 0 for water.

[mido66]

Yep ! You don't have water at outlet at the beginning, so put 0 for backflow volume fraction.

aaand, i'm so sorry but I didn't understand you first question ...

[abhanja]

Hi,

i am also trying to analyze splashing in a 2 phase system where high speed jet of air comes through the inlet and impinges on a liquid pool which is nearly 1 m below the inlet.

Problem statement is to find/observe amount of splashing of liquid phase after 'n' seconds on the walls.

In design modeller, i have made 2 separate bodies (air and liquid) and combined them into 1 part body.
VOF multi-phase solver is used. Primary phase is air and secondary phase - liquid.
Meshing has been done.
In fluent, how do i proceed in providing boundary conditions (vel_inlet, pressure_outlet, walls)and initializing volume fraction of each phase.

[mido66]

yop,

You don't need to do two separate bodies.
initialize with air volume fraction =1
then click adapt -> region -> and click adapt for the region you want water.
after click patch (in initialize menu) select water volume fraction, put the value equal to 1 and select the region you just created and click patch.

you can search on google "patch fluent" or adapting region fluent", or in the fluent user's guide to have more details.

I don't understand, where is your outlet ?

Don't forget to put density of air as "ideal gaz", operating density equal to 0, activate energy model, and put phase interaction : wall adhesion, surface tension equal to 72 dyn/cm and discretization value equal to 2 (after activate it in VoF model.

hope it help you,
good luck.

[abhanja]

Hi,

Thank you. Pressure outlet is a air (Fume) suction duct.
Tried to run the model but their was divergence with message like courant number 250.
Will try again.

[mido66]

hello,

Try to go in advanced parameters of solution control.

Then put all cycle type on "flexible" and change the AMG method from aggregative to selective.

You can also divide by 2 all under-relaxation factors in solution control.

remember to not put a too big time step. (0.01s min)

good luck

edit : you can also put the VoF model in implicit mode to handle courant number issues.

[abhanja]

Hi,
Thanks.
Is there any criteria for selection of primary/secondary/tertiary phases in VOF model or any phase can be randomly selected?

In actual problem, vel_inlet has got six nozzles (circular pattern - 3D). Since, i am formulating in 2D with 2 nozzles, should i take the flow rate as it is or calculate flow rate and velocity for each nozzle?

[mido66]

Hello,

You need to let air as primary phase (because of its compressibility).

If your 3D model is a circular geometry, I don't think you can use a 2D model...

Anyway, you need to put boundarie conditions to have the correct flow through one nozzle. But once again, I think use a 2D model is not a good choice...

Good luck

[abhanja]

Thanks
Is it possible to use a mass source term in 2D so as to replicate conditions of 3D?
As mass of liquid is required in 3D

[mido66]

Hello,

I have never done that, I can't help you sorry ^^'