Hello, I am a student researcher and am trying to implement a volume of fluid (vof) interface tracking algorithm into an existing fluid dynamics code based on the simpler algorithm. I have done an extensive literature review, and find that mostly the vof papers are using the simple algorithm, or other solution schemes. I was wondering if anyone might know of a piece of work using both simpler and vof together, or if these two methods are imcompatible for another reason? Any help anybody can is greatly appreciated.

common implemwentation of VOF is quite separate from NS solver, in fact after having a correct velosity filed u advect fluid by VOF, of course there may be several copuling but common one is using one VOF time step after one NS time step in which time step is restricted by CFL

in S. zaleski page there r some codes useful for start. further in book by CP Hong (Computer Modelling of Heat and Fluid Flow in Materials Processing) he present VOF and simple methods. He has several papers ISIJ Internationals if u do not have access to this book.

hope this helps

My question is different from the previous post. I am trying to determine the position of free-surface by using the interface-tracking method. As we know this free surface must satisfy the dynamic boundary condition and kinematic boundary condition.

As the viscous and surface tension are neglected here, the free surface is solved as in the case of prescribed pressure boundary. The kinematic boundary condition is satisfied by correcting the non-zero mass flux at the free surface, leading to correction on swept volume. This needs iteration to find the new position of free surface.

My question is that when we do this iteration : 1. The iteration is within one outer iteration;i.e. solving the momentum eq and pressure-correction, then correct the free-surface position,

2. or after several outer iterations;i.e.get the mass and momentum conservation satisfied first, then do the iteration before proceding to the next time step ?

Any comments would be greatly appreciated. Thank you.

actually interface tracking should be coupled with momentum eq., but in practice peoples do not do this, i.e. ignor inner/outer iterations

regarding to bc on free surface there r several method, some based on physically consistence interpolation, i.e., zero shear stress and balanced normal stress by pressure grad and surface tension force, some of them use velosity extrapolation (extension), refere to the following papers for more:

(very excellent 3D) A numerical method for three-dimensional gasâ€"liquid flow computations, Journal of Computational Physics 196 (2004) 126â€"144

(very excellent 2D) Bubble collapse near a solid boundary: a numerical study of the influence of viscosity, J. Fluid Mech. (2002), vol. 464, pp. 137-163

Discontinuous fluids, ACM Transactions on Graphics (TOG) archive, Volume 24 , Issue 3 (2005)

On the simulation of flows with violent free surface motion, Comput. Methods Appl. Mech. Engrg. 195 (2006) 5597â€"5620

On Boundary Condition Capturing for Multiphase Interfaces, Journal of Scientific Computing, Vol. 31, Nos. 1/2, 2007

A partial differential equation approach to multidimensional extrapolation, Journal of Computational Physics 193 (2003) 349â€"355

The Fast Construction of Extension Velocities in Level Set Methods, Journal of Computational Physics 148, 2â€"22 (1999)

Hi, I have no experience with VOF method, and i am supposed to implement vof for a polymer flow in a SIMPLE based solver. I hope you could comment on method i am thinking of using.

I read about explicit implementation that says

fr_n+1 = fr_n - delta_t * [div( U_n.fr_n)]

This is explicit method. I wish to change this and couple this with sub iterations of SIMPLE, so at each iteration i have values of velocity. So i use the best values of fr_best, available at each time step.

So

fr_best_new = fr_n - delta_t * [div( U_subiter . fr_best)]

end of sub iterations fr_n+1 = fr_best_new

What do you think, would this work.

hi,

not that interface advection is sensitive to numerical diffusion (smearing interface), and so to cope this, peoples usually use geometrical flux computation, like PLIC VOF, so algebraic computation of div operator may not be a good idea.

btw, your meth can work, there are some works on this, e.g., see paper by V. Voller: A time-implicit filling algorithm, Applied Mathematical Modelling, Volume 18, Issue 2, February 1994, Pages 101-108

but it has its known limitation.

in brief (i have 7 years back in this field), i should say that implicit VOF is not a good idea.

also. there are sme explicit time step free methods too (of course not accepted well, has their limitation, consider rule of physical time-scale too), e.g. works by Yabe Xiao under context of CIP, or semi lagrangian LS of John Strain (check in JCP), or semi lag particle level set of Fedkiw ...

PS: a nice vof code: Gerris Flow Solver

First a big thanks.

I tried to implement both versions, and so far it seems that though implicit method is more stable, its damn diffusive. And the explicit method that i mentioned seems to be less stable than the version that only uses previous time step velocity field.

BUT, I just have found out that in my solver, the single processor version is working flawless but openmp based version has some stability issue. (I messed up somewhere).

SO i would be running these test cases on single processor version again.

Out of things you mentioned, CIP looked very promising. I am trying to read about it. I got some phd thesis to guide me through.

But for me, i guess, my problem is not going to be solved easily because, i have a polymer - air system to solve and poly has very very high viscosity.

This high viscosity ratio makes solution very unstable. I am not sure about any cure for this, other than pray to God.

Thanks again for time you gave. It was valuable for me.