CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Suitability of interface compression scheme for interface rupture simulations (http://www.cfd-online.com/Forums/openfoam/98698-suitability-interface-compression-scheme-interface-rupture-simulations.html)

Ak_cfd March 16, 2012 11:06

Suitability of interface compression scheme for interface rupture simulations
 
Hello All,

I was hoping someone would be able to shed light on how suitable the interface compression method in interFoam is for simulations that involve accurate capture of interface breaking/rupture.

If suitable, how well does it compare with other methods like the PLIC (geometric reconstruction of the interface) ?

Thanks
-Aravind

kwardle March 16, 2012 15:34

Perhaps take a look at:

Gopala and van Waachem, "Volume of fluid methods for immiscible-fluid and free-surface flows", Chemical Engineering Journal, 141:204 (2008).

PDF is available on google --- first link when I search "gopala sharp interface"

Of course, the paper looks primarily at relatively simple test cases. If you are specifically interested in more complex flows involving interface breakage and such your choice may depend a bit on what you are looking at. As I understand it PLIC tends to have slightly more accurate interface motion when compared to compressive schemes like the one in interFoam (which is not exactly like the one mentioned in the Gopala paper but very close) because the latter suffers from interfacial parasitic currents. That said, PLIC itself is not perfect as it is not fully volume conservative. For me, I am happy with the speed and simplicity of the interFoam method---that said, I never use a value for cAlpha greater than 1. Also, the types of problems I am looking at are large scale in terms of the amount of interface motion such that I don't think the wavy currents on the interface have much effect. As an example, take a look at the top video here.

Hope this is useful.

Ak_cfd March 19, 2012 16:44

Thanks, Dr. Wardle. That was indeed useful! And you are right, the test cases in the paper - "Volume of fluid methods for immiscible-fluid and free-surface flows", Chemical Engineering Journal, 141:204 (2008), are simple, elegant cases that show the differences between the different interface capturing techniques. I'll look into this further to make sure I can use it in solving my case.

The problem I am trying to solve is along the lines of being able to simulate the air bubbles entrained when a solid body falls into a liquid. The interface which is continuous initially, now breaks since the surface tension is not enough to keep the interface continuous. The range of length scales involved is quite large.

One question that has come up is the suitability of interFoam to accurately capture interfaces between two different liquids instead of a liquid/gas interface. My understanding is that numerics within interfoam should be able to simulate the interface between two different liquids just as well. Am I missing something?

Any ideas, suggestions would be great. Thanks!

kwardle March 19, 2012 17:43

Well, you are correct that numerically there is no problem with using interFoam for liquid-liquid flows. The problems will be the same---can only resolve structures several times larger than the grid spacing, parasitic currents, etc. Given that the interfacial tension and density ratio are smaller in the liquid-liquid case than the liquid-air one, you would expect to have smaller droplets. So for a given mesh, the liquid-liquid case will be worse than the liquid-air one in terms of physicality. Also keep in mind that one additional issue which is common to all VOF methods is overprediction of droplet coalescence.

So again, it goes back to the conditions you would expect for your plunging object case. The other solver that might be of use is twoPhaseEulerFoam, or the new multiphaseEulerFoam which allows you to have any number of phases (with sharp interfaces if you want). Note that both of these use a fixed dispersed phase droplet diameter (though at least for multiphaseEulerFoam other diameterModels can be implemented).

Good luck.


All times are GMT -4. The time now is 23:53.