VOF

 Register Blogs Members List Search Today's Posts Mark Forums Read

 December 16, 2003, 09:56 VOF #1 özgür Guest   Posts: n/a 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.

 December 16, 2003, 10:31 Re: VOF #2 Johan W Guest   Posts: n/a 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?

 December 16, 2003, 10:36 Re: VOF #3 özgür Guest   Posts: n/a 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?

 December 16, 2003, 11:01 Re: VOF #4 özgür Guest   Posts: n/a 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?

 December 16, 2003, 14:41 Re: VOF #5 thomas Guest   Posts: n/a 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 !!!!

 December 17, 2003, 04:57 Re: VOF #6 Özgür Guest   Posts: n/a 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.

 December 22, 2003, 07:08 Re: VOF #8 Özgür Guest   Posts: n/a 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

 January 6, 2004, 09:23 Re: VOF #9 Frank Meissen Guest   Posts: n/a 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post ariorus FLUENT 0 August 7, 2009 10:57 Garima Chaudhary FLUENT 0 July 13, 2007 02:20 ozgur Main CFD Forum 3 February 18, 2004 19:19 ozgur FLUENT 1 February 18, 2004 12:59 Yongguang Cheng FLUENT 0 September 19, 2003 07:39

All times are GMT -4. The time now is 09:34.