trying to simulate the splashing phenomenon with multiphaseInterFoam
 

Hi to evrybody,

I'm working with droplets impingement on a thin liquid film, and I'm trying to simulate the splashing phenomenon with corolla rising and instability. So I succesfully use interFoam, but now I want to distinguish the drop liquid from the film liquid, and so i decided to use multiphaseInterFoam with the same boundary condition (that besides are the test case BC) .
This kind of simulation is not able to reproduce the splaching phenomenon.
Can anyone help me?
Thanks

is anyone familiar with multiphaseInterFoam?

When you say it does not reproduce the splashing phenomenon do you mean that you see different results between your interFoam case and the one with multiphaseInterFoam on the same mesh? Which version are you using? Perhaps a few side-by-side comparisons of what you are seeing would be helpful. What about interfacial tension for your two liquids? Have you set this to zero to mimick interFoam behavior and match what you want to see?

Also, the newest version (2.1.1) should have much improved phase conservation in multiphaseInterFoam over older versions.
-Kent

First of all thanks for answering my post.
My intent is to use multiphaseinterFoam to distinguish different liquid (from drop anf film) in the corona formation.
I use the same mesh, the same initial and boundary condition in the interFoam and multiphase case. Moreover i set to zero the surface tension value for the drop and film mixture and to 1 the contactangle (however I've done different case in witch I've changed sigma and the contact angle).
I use the 2.0 OpenFoam version.


Recently I improved my results changing the solution scheme(now i can see the splash), but they are still different from interFoam.

Yeah, I think I understand what you are trying to do. Does the version of multiphaseEulerFoam print out a line like, "Phase-sum volume fraction, min, max = 1 0.999909 1.00003"? The version with improved phase conservation should do this.

The other thing to consider (and it sounds like maybe you have) is that as part of the sharp interface tracking it uses interface compression along with an appropriate discretization scheme to keep the interface sharp. Have you change the divSchemes for alpha in fvScheme? The problem is that you cannot in multiphaseInterFoam change them independently for each phase pair. So, even if you are using the same fluid props, etc., it will keep a sharp interface between the two which might alter the results a little from the interFoam case. I wonder if you would get better results by using vanLeer/interfaceCompression only for the liquid-air part? Incidentally, you can do this in multiphaseEulerFoam, but I don't think that is what you need here.

What value for cAlpha are you using in fvSolution? The tutorials use 2, but I would not go more than 1 or 1.5 to avoid spurious interfacial currents. And 1 is sufficient in any case I have tried.

Hi Every Foamers:
 

I want to add surfacetension in one solver(my solver is interPhsaeChangeFoam),for this reason I added :

#include ''fvCFD.H''




please help me,and tell me ,How to correct this problem???

The interface become fuzzy with multiphaseinterFoam
 

Hi, Kent!

I work with the Multiphaseinterfoam which is added energy equation and a viscosity model. Firstly, this solver have finished the two phase flow like the picture 1, and the interface between red and blue is good. secondly, I set the third phases with funkysetfields in a circle(to be a bubble) like the picture 2. Lastly, I run the Multiphaseinterfoam again to get the deformation of the bubble.

Unfortunately, the interface of the bubble become more and more fuzzy with the time going as shown as the picture 3. what's more, the interface between the early two phases is still good.

why the interface of bubble become fuzzy? Any answer is welcome! Thanks in advance!

Just looks to me like your mesh resolution is too coarse. That is unless you have set cAlpha=0 for some reason in your setup.

Thank you so much!

After correct the cAlpha as you told me, I got a quite sharp interface.

About the mesh resolution, I want to change the mesh tool,because the piontwise can not deal with the small size area(0.003m*0.01m*0.0001m) very well.

On the other hand, I find the sharp interface(cAlpha=1) will become unstable when the difference of physical properties of the two phase is large. About the "unstable", in my case, the interface become asymmetric as shown in the picture. Do you have any good way to deal with this "asymmetric" problem?
thanks in advance!

What you are seeing is a well-known issue with interface compression schemes such as used by interFoam. This has been discussed elsewhere--search for 'spurious currents' and have a look at this thread:
http://www.cfd-online.com/Forums/ope...tml#post349907
I mention there a paper by Gopala et al that compares the accuracy of various methods.

thanks for your reply, I know a little about the 'spurious currents' and I found the greater the viscosity ratio, the greater the 'spurious currents' in my case