Hi,

I am simulating a single free falling liquid drop in gas in 2D. I use VOF, Geo-Reconst. Scheme with implicit body force, Laminar (turbulent requires extremely small time steps) with periodic BC's at the x and y boundaries. I have the following problems:

- Drop deforms while it should stay spherical according to the experiments (Surface tension is switched on!!)

- The wakes inside the drop are not satisfying (there should be inner circulation inside drops, as well as outside the drop)

- The time step of 0.0002 results oscillations on the surface of the drop, but a time step of 0.0001 does not, while they both are converging!!

Does anyone has an idea? Moreover, does any one has an experience of using UDF's for defining interphase boundary conditions on the drop surface? May I simply skip VOF and try to simulate this by defining a wall BC at the surface where I define the actual 2 phase interphase BC's on it by UDF's(the wall stays there to prevent penetration btw. phases and to ensure spherical interphase)

Thanks in advance.

Hi

As a rule of thumb I have learn to set the time step to a 1/10 of the time it takes for the interface/particle to pass over a cell, it use to work.

Have you controlled for grid independenece?

A bit more about what I mean by 2 phase interphase BC's for the drop to be defined by UDF's, if possibble:

- Same tangential velocities & stresses at the both sides of the interphase

- normal velocities at both sides are zero

-tangential stress at the gas side + surface tension = tangential shear st. at the liquid side

Can I define those BC's to the cells at the interphase of my drop by using UDF so that I do not have to use VOF which unnecessarily tracks the interphase of the drop?

So far, I have mainly used 25 micron grid for 1 mm drop. For such case, it means for a drop falling with 2 m/s near terminal velocity, I need to have a time step of 1.25x10^(-6) sec. This means I have to wait quite long for my simulation. Moreover since adaptive time stepping should not be used with VOF, do I have to change the time step manually throughout my unsteady calculations then since the drop velocity changes?

Do you mean by grid independency that, to adapt the grid and calculate again if something changes?

Hi, here are some thoughts. 1 - Considering a courant number = 1, I have following your mesh size (25 microns) and Terminal droplet velocity (2m/s) a time step of 1.25 10 ^-5 and not 1.25 10^-6. Also you have turned on the surface tension option. The thickness of your mesh will allow to take into account the capillar effect at the droplet interface. Therefore you should make sure your time step fits to the capilarity characteristic time to make sure the surface tension option has an effect on your simulation.

2 - I agree on the idea to set an underformable surface to simulate a constant shape bubble. Some people might complete what I am gonna say but here is what I would suggest you to try. A - Define 2 fluid zones in gambit separted by a simple circle (d=diameter of your bubble, or Radius if you use a symmetry) B - In fluent use the Euler-euler model, set 2 phases materials: water and air. Then when you initialize, set the outter domain as Volume fraction of air = 1. At contrario set volume fraction of water(droplet) inside the circle = 1. C - For your UDF ? I First think you could use a define_profile macro hooking in fluent by a velocity inlet boundary condition. But for coding facilies, I would suggest to forget imposing effect of the inner fluid at the face. Why? At the interface the cell faces are linked by 2 cells (inner one and a outter one). At a boundary condition you can only access one cell by the macro F_C0. The other macro F_C1 accessing the other cell data does not exist or is equivalent to F_C0 in the case of a boundary condition. That is why I think you can only take into account one effect.

My Second sugestion is you can define a source term at this interface modelling the exchange of momemtum at the face. You need to find the the mometum value and the momemtum direction. This solution seems to be the best one cause it allows you to catch both inner and outter fluid effects.

Go on www.fluentusers.com -> User Group Meeting USA 2003, there is a presentation an excellent presentation about UDF you will find a lot of simple and practical infos !!!.

I hope I have been clear and you'll find some stuff you need. Thomas

PS: Definition -> Qu'est ce qu'un accident ? Le PSG 2em du championnat !!!!

Hi, I really appreciated your valuable suggestions. Here are some thoughts from me.

- The time step as you calculated as 1.25x10(-5) is the internal time step the solver used only for the volume fraction equation(Fluent Manual 22.6.14). The value as I calculate as 1.25x10(-6) is based on the rule of thumb as suggested by Johan W in the previous reply, and to be used by the solver for the rest of the transport equations.

- Can you explain a bit more what you mean by the time step to be fitted to the capilarity characteristic time to make sure the surface tension option has an effect on my simulation. Isn't it so that, as far as my calculations converge, the solution should not depend on the time step I've used??

- I have tried smilarly as you've said, to define 2 fluid zones seperated by the solid circle. I did not used multiphase models, since the two phases were seperated by a solid wall (a circele, or a sphere in 3D). What interesting was, I got somehow!! an interaction (a kind of coupling) btw. 2 phases even they were seperated completely by this solid wall (i.e. I got some wakes inside the drop). How this could happen? But since the circle does not behaves like the real interphase (which is a moving boundary indeed) I switched to multiphase models. I have the same question in my mind for your suggestion to use Euler-Euler model, i.e. is it possible to use multiphase models when the 2 phases are seperated completely by a third phase (a solid circle) ?

-May I have some possibility to set my interphase BC's on the wall at the interphase (which will be defied by fluent as two-sided wall, since there are fluid at the both sides) so that, I will have the coupling of the two phases?

- I also do not understand your footnote

Thanks a lot.

Hi, I have read the fluent doc about time dependent simulation usinf VOF model. As far I understand what is in it, The VOF model calculates its own time step to solve continuity and momemtum equation NEARBY the interface. This time step (= free surface time step) is different from the time step used for the momemtum/transport equations far from the interface. Fluent computes automatically this time step based on 2 things: 1 - The characteristic time which is equivalent to the time step of the faster phase based on courant number =1. I guess This is the time step expected in the 'ITERATIVE' panel. 2 - Second parameter, The maximum current number allowed (Default 0.25).

From this, I would like to make 2 comments:

1 - I do not understand why you set a time step of 10^-6 when the 10^-5 correspond to the characteristic time (Courant number=1). There is a factor 10 which is no neglectable from my hand. I do not understand the interest in using such a small 10^-6 time step knowing fluent reduce it nearby the interface.

2 - From the time step strategy above you can see that the interphase phenomena and the inside phase phenomena are different. Very roughly let say that the 'informations' are not transport are the same velocity depending if you are inside a phase or at the interphase -> Therefore you need different time step for each domain, this is what fluent does by computing a free surface time step. The capillarity is one of these interphase phenomena. Turn it on gives a more cohesive phase interface (means better sharpness -> see fluent doc). To understand what I meant with capillarity characteristic time let me take an example totally out of the context. Take a cloud in the sky. In this cloud you have the big structure with a characteristic length of sevral kilometers ( low frequency, big characteristic time ) and you have small structures with a characteristic length counted in meters (hight frequency, small characteristic time) . The big structures correspond to the advective term of the transport equation when the small structures depend on turbulent agitation or turbulent diffusivity if you prefer. So if you want to see the effect the tuburlent diffusivity you have to set an enought small mesh to the characteristic lenght and adapt the time step to the low characteristic time. So if you do not satisfy both of those conditions, the turbulent diffusivity is still include in the equation but won't appear on the results. Following that it is the same thing with capillary. By analogy, your Bubble speed represents advection and capillarity represents turbulent diffusivity effect. According to me you have an enought small mesh I just wondered if your time step was adapted. HOWEVER the fisrt time I said that I have not read the docmentation about the time step reduction near the interphase, so I guess it is no big deal. But I would be interested to know if your results change when surface tension is not turn on.

Finally, I would like to know how you interpreted the fact is appeared some wake inside your bubble define by a wall. How informations can come acroos a wall boundary condition. Does the 2D sphere descrive by a wall BC can generate inner wake by some inside frictions ???

Sorry if I made it too long, but I am learning at the same time . Greeting thomas.

Hi,

Thanks for your reply. I would like to ask if my grid is enough fine and time step is enough small (either 10^-5 or 10^-6), then what else may be wrong, so that my drop is deforming, and I could not get the velocity fields showing the coupling between the phases.

What I know about capillar number is that it is a nondimensional number indicating if the surface tension effects are negligible or not under the laminar flow conditions (for turbulent flow, Weber number is used). Then, what do you mean by turning on the capillarity? Is there such an option in the VOF menus so that I have to activate it?

By the way, deactivating surface tension does not change much things, just the drop is deforming less smooth.(surface tension: 0.024 N/m)

Regards

Hi,

not to use adaptive time stepping in VOF-simulations is not quite correct. There are two possibilities:

1) Use an UDF, which looks how fast your solution converges (w/o adaptive time steps). if it converges fast, it increases the timestep, otherwise it decreases the timestep.

2) Fluent has written an udf, which can be used in the adaptive time steps. It ensures that the VOF-sub-timesteps is about 8 by variation of the global timestep.

Frank