CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Coalescence and breakup in twoPhaseEulerFoam (http://www.cfd-online.com/Forums/openfoam-solving/59446-coalescence-breakup-twophaseeulerfoam.html)

m9819348 September 13, 2007 08:03

Dear all, I am trying to si
 
Dear all,

I am trying to simulate a two phase flow which contains two liquids with similar densities (ratio ~ 1.1).

These liquids might mix, but most of the time they should exist as seperate liquids (with a clear interface).

I can not use interFoam (or any variation of it), since one of the fluids might be blocked by a filter while the other fluid flows past the filter. I see no way of dealing with this situation using interFoam (which is based on a uniform velocity field).

I believe that the twoPhaseEulerFoam solver can be applied since it calculates the motion equations for each phase.

However, I have run the tutorials and some simple tests (a bubble of liquid 2 that rises in liquid 1). But liquid 2 always seems to mix completely with liquid 1. The interface is not clearly kept.

I also read the PhD of Mr Krusche and Mr Hill where it says that droplets (and even coalescence and break-up of these droplets) can be simulated with the twoPhaseEulerFoam solver. However, no clear example (benchmark, tutorial, ...) is given.

Since I can not set a surface tension or any other parameter to make the interface more rigid, I wonder how I could make the two liquids immiscable.

To make a long story short:
Can anybody give me a hint on how I can simulate clearly defined droplets of a slightly denser liquid in another liquid with the possibility of the droplets to move at a different speed than the main liquid and that can show effects like coalescence and break-up?

Ries

msrinath80 September 13, 2007 13:27

interFoam can do that. Coalesc
 
interFoam can do that. Coalescence and breakup are handled inherently by interFoam. They are resolved. If you need to use twoPhaseEulerFoam, then you will need to implement additional population-balance equations to account for breakup and coalescence. Plus, you can forget about the interface in twoPhaseEulerFoam as it does not resolve it at all. twoPhaseEulerFoam involves a lot of modeling as opposed to VOF which relies on direct simulation.

alberto September 13, 2007 13:27

Hello Ries, the twoPhaseEuler
 
Hello Ries,
the twoPhaseEulerFoam solver is based on the Eulerian-Eulerian two-fluid model, whose basic assumption is that the phases are continua which exchange properties (momentum, in the case of this solver, because it's isothermal and no mass transfer is considered) and interpenetrates each other.

Each phase is identified by its volume fraction, so if you consider a gas-liquid flow, where you have bubbles in a liquid, you won't see bubbles, but a field of the volume fraction of the gas inside the liquid (see H. Rusche thesis for some contour plot).

About coalescence or breakage, you need to implement additional models to keep these phenomena into account because the current code doesn't provide these functionalities.

If you need to simulate a filtration process, you don't need to consider well defined droplets. You can do it with the Eulerian approach, modifying the code so that the secondary phase velocity (flux) is set to zero when it hits the filter.

Something like this was already done when the twoPhaseEulerFoam was written by Niklas Nordin.

With kind regards,
Alberto

sradl September 14, 2007 01:12

Dear Srinath, I must disagr
 
Dear Srinath,

I must disagree regarding:

"interFoam can do that. Coalescence and breakup are handled inherently by interFoam"

Of course, if two droplets in interFoam will collide they will merge to a single droplet and vice versa.

However, if two liquid particles (especially bubbles) collide, they NOT necessarily must merge (depending on the Weber number) - the very small film (we are speaking of [nm] scale) between the two colliding partners has to be trained - you cannot resolve this with VOF or other convential CFD method.

However, you get a result for the case where every liquid particle will merge and overpredict coalescence. The only change you have is to use a Euler-Lagrange approach and incorporate a "coalescence efficiency" based on the collision Weber number (closure information can be obtained exp. or via mathematical models).

Just a comment to start in the moring :-)

br
Stefan Radl

msrinath80 September 14, 2007 02:08

Stefan, I must totally agree w
 
Stefan, I must totally agree with your answer :-) Here is a more verbose interpretation of the situation. Perhaps other experts like Henry, Hrv et al. can comment on this too!

If I follow the assumptions of continuum mechanics (which is imperative if we are to use the N-S equations), then the continuum hypothesis dictates that if the length scale of the problem in question should ever become comparable to the mean free path, then the continuum hypothesis breaks down and Newton's laws don't hold good anymore (Remember the N-S equations are merely a restatement of Newton's laws written for a fluid particle). The dimensionless quantity of interest for this case is the Knudsen number (ratio of mean free path to length scale of the problem). As the mean free path of water is of the order of nanometres, the problem of the thin film that needs to be drained for coalescence to occur cannot ever be resolved using Newton's laws. Up to the smallest possible length scale within the continuum hypothesis limits, I can use the N-S equations. After that point, I will need to get into quantum mechanics in conjunction with statistical mechanics to resolve the problem. This is why most continuum-based research in this area will resort to a phenomenological model (i.e. one that is based on empirical data). So one can handle collision/coalescence of drops/bubbles/rigid particles through these models. Of course, the situation becomes more exasperated when surfactants are present at the fluid interface!

m9819348 September 14, 2007 04:42

Dear Srinath, Dear Alberto,
 
Dear Srinath,
Dear Alberto,
Dear Stefan,

thank you all for your quick responses!

@Srinath: I agree that interFoam can show coalescence and break-up, but it can not simulate how the second fluid is blocked (stopped) at a filter, while the other fluid flows by. In my opinion it is not possible to get a zero velocity for one fluid and a non-zero for the second phase with interFoam (or VoF for all that matters).

Concerning your remarks on the continuum hypothesis: I agree. However, at this point I only have some rough experimental (phenomenological) data to compare with. So I am not interested in an exact solution of the physics (yet), but more in a reproduction of the experiments. As a start. But even the "simple" case of a bubble being stopped at the wall, while the main fluid flows by, I can not resolve (yet).

@Alberto: Is it possible to build in some code that might force the volume fraction of the second phase to stay close to one? This would create a more clear boundary between the two phases. At this point, the code immediately dissolves the second phase, which is not always correct in my opinion.

I am trying to simulate how the second phase (slightly denser) is being stopped at a filter and at that time, blocks the filter partially. To visualise this, interFoam would be very usefull, however, in my opinion, it is not possible to simulate blocking processes in interFoam. Do you think this might be possible with an Euler code?

@Stefan: I agree with you. The bubbles I am working with are in the scale of 100micrometer up to 1 mm. So a film the size of nm is a good assupmtion. I am aware that this process is depending on the Weber number, but at this point, I can't even simulate one bubble that is being blocked, let alone two bubbles that might merge.

In my opinion, interFoam is not the solution. twoPhaseEulerFoam might be, if I can slow down (or even stop) the mixing of the two fluids. Any suggestions?

Ries

sradl September 14, 2007 05:27

Dear Ries, you cannot use t
 
Dear Ries,

you cannot use twoPhaseEulerFoam for your purposes, because you cannot "Stop mixing" in this kind of simulation, as Euler-Euler a prioriy assumes two interpenetrating phases!

The best way is to use a Euler-Lagrange approach where every particle is tracked.

br
Stefan Radl

m9819348 September 14, 2007 05:44

Dear Stefan, I believe you
 
Dear Stefan,

I believe you are right. I was already thinking of assuming that the small bubbles (< 100 micron) might behave like solid particles. An Euler-Lagrange approach is the best then.

alberto September 14, 2007 09:54

Hello Ries, Stefan is right.
 
Hello Ries,
Stefan is right. You can't fix the volume fraction at a value close to one a priori in a Eulerian model.

A Euler-Lagrange approach is ok if you have a reasonable number of particles, and if you really need to consider particles as separate entities. If this is not the case (the concentration of particles is high), the Euler-Euler approach with a population balance is the most viable solution. You will lose information about the single bubble, but you can consider coalescence and filtration quite easily.

About the implementation of a filter in a Euler-Euler code, I know it has already been done with twoPhaseEulerFoam (you can see a filter dictionary file in the tutorials, to set a filtering plane), but the code was not released. The basic idea is to set the phase flux to zero, or to adapt it according to the filter efficiency.

With kind regards,
Alberto

sharonyue November 5, 2012 04:34

sorry to hijack this thread.



Quote:

Originally Posted by alberto (Post 205986)
About coalescence or breakage, you need to implement additional models to keep these phenomena into account because the current code doesn't provide these functionalities.

@alberto

If I want to simulate bubble coalescence and breakup in a stireed tank which has been done in Hill Phd thesis using STAR-CD,page 295-318 . Should I implement the PDF(probability density function) approach?
btw, does that mean STARCD has been implemented this model?

Im going to simulate air injected in a stirred tank filled with high viscosity (about 2000cp)non-Newtonian fluid(xanthan gum), in experiment, I find there are numerous small air bubble (1mm) cause of the high viscosity,and many big bubbles breakup like boiling in the free water level.seems like I have to implement non-Newtonian fluid power law model and the PDF approach mentioned above? thats maybe tough.

I would be very grateful if u give me some hints.

Best,

prithvi yesudas February 12, 2013 13:07

Particle impregnated bubble coalescence
 
Hello Friends,

I am new to this forum and also to CFD platform , I want to know which software to use to model coalescence of two bubbles with particle/s impregnated to them. the size of the particle is 100 microns approx and bubble 3 mm size . Also the particles are the same density as the water medium could someone please tell me which software allows this , because fluent cant solve this problem

thanks & regards

Prithvi:)


All times are GMT -4. The time now is 15:36.