CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Suitability of interface compression scheme for interface rupture simulations

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

Like Tree1Likes
  • 1 Post By kwardle

Reply
 
LinkBack Thread Tools Display Modes
Old   March 16, 2012, 11:06
Default Suitability of interface compression scheme for interface rupture simulations
  #1
New Member
 
Kishore, A.
Join Date: May 2010
Location: Cincinnati
Posts: 7
Rep Power: 7
Ak_cfd is on a distinguished road
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
Ak_cfd is offline   Reply With Quote

Old   March 16, 2012, 15:34
Default
  #2
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
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.
roenby likes this.
kwardle is offline   Reply With Quote

Old   March 19, 2012, 16:44
Default
  #3
New Member
 
Kishore, A.
Join Date: May 2010
Location: Cincinnati
Posts: 7
Rep Power: 7
Ak_cfd is on a distinguished road
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!
Ak_cfd is offline   Reply With Quote

Old   March 19, 2012, 17:43
Default
  #4
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
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.
kwardle is offline   Reply With Quote

Reply

Tags
interface compression, interface rupture, interfoam

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 34 October 16, 2014 05:27
CFX13 Post Periodic interface EtaEta CFX 7 December 8, 2011 18:15
Godunov scheme Peter Main CFD Forum 6 November 27, 2009 11:51
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 14:24.