When I run a bubble rising in stagnant water transient simulation and set Surface Tension Force Model = Continuum Surface Force, the solution didn't get convergence and I get a blurred air-water interface, but when I set Surface Tension Model = None, the solution get convergence.

My question:

If I don't take in consideration Surface Tension Force Model (=None), is surface tension effect equal to zero? otherwise, how is included this effect?

Regards

If I don't take in consideration Surface Tension Force Model (=None), is surface tension effect equal to zero? yes

Thanks for your reply.

I have run two times same simulation, first one with Surface Tension Force Model=None and Surface Tension Coefficient=0.0718 N/m, second one with Surface Tension Force Model=None and Surface Tension Coefficient=0.000718 N/m, but results were different.

I think although Surface Tension Model=None, surface tension effect is taken in consideration, but I don't know how.

Hi Miguel, I am simulating the same thing. I didnt understand what blurreed interface means? Have you noticed small vf of air in water while your bubble moves upwards?

theo

Hi Theo,

In my simulation I have noticed excessive smearing of the liquid-gas interface and separation of small air vf from the bubble. Do you have same problem?

Miguel

Gentlemen, you are always going to get some surface smearing with a finite volume method. This is due mainly to your using a mechanical sized cell to capture a molecular level phenomena, although I'm sure numerical diffusion will also have an effect. CFX has historically had some problems with the surface tension model (allegedly) so that at higher Weber numbers the solution becomes unstable and short-peroid numerical "waves" are seen at the interface. I do not know if CFX have solved this problem yet, but it was certainly evident as recently as 3 years ago. The practical upshot of this is that you are limited in the level of grid refinement you can apply (since reducing cell sizes has the effect of increasing the Weber number). If, as you have described above, you are getting separation of small air volume fractions, then this sounds like "Flotsam & Jetsam", a common numerical error associated with the VOF method. I don't want to sound like I'm teaching you to the very basics, but make sure your grid is as orthogonal as you can make it. If this does not help, try reducing your timestep size. You should contact CFX support, and ask explicilty about the Weber number problem associated with the surface tension model.

To end on a bit of a downer, I ended up not using CFX and switching to CFD-ACE instead since its surface tension model was much more robust (allegedly). Best of luck.

Hi Miguel, I have recently done a similar simulation (CFX 10). It works fine with "Surface Tension Force Model = Continuum Surface Force". If you make sure that Pe is around 1 (yes, this means small timesteps) you will most probably get what you expect with no smearing at the interface. Good luck. Ulian

Hi,

why is the Weber number increased when reducing cell sizes, as Jim says? Isn't We=rho*u^2*(cell size)/sigma?

Please give me some hint!