PLIC in InterFOAM???
 

Hi,

Does InterFOAM like Fluent also uses PLIC. also which part of the solver code can confirm this. Need urgent help.

Thanks

No interFOAM does not use PLIC like Fluent. OpenFOAM uses a scheme called interFAce compression scheme. You can look into

~/OpenFOAM/OpenFOAM-1.6.x/applications/solvers/multiphase/interFoam for the details and then for further details of compression scheme look into MULES . Search for it in the OpenFOAM directories. It will give you the details.

regards
K.Suresh kumar

Im also interested in the implementation of PLIC in interFoam. Is there any work done in this direction? The interface compression procedure gives bad results form small domains.

Regards

Robert

I am also interested in some algorithm that makes the interface sharp. From what i known PLIC algorithm is normally used on very simple mesh (all hexas) and may be difficult to adapt to a completely tet mesh. Would be interisting if some "expert" tell us if it is possible or not the implementation in openFoam.
In particular what i found from my experience using interFoam are very high spurious velocities at the interface when the domain size becomes smaller and this tends to affect the results. For this type of problem, considerable progress has been made in recent times but, in order to implement one of these techniques are necessary geometrical information about the interface, which are not available in interFoam.
So would be really helpful knowing in which direction would be better to move.

Best

andrea

Hi everyone,

I'm currently working on the "Geometric" Volume of Fluid solver in OpenFOAM (PLIC reconstruction + unsplit geometrical advection) as a part of my PhD topic. It's going quite well so far and the code will be released into the public domain as soon as it is possible (when it runs, validated, in parallel).

T.

The problem with the true interface capturing method, if it is based on purely geometrical solution to the volume fraction equation, is the fact that all of the developments so far have been done on Carthesian equidistant meshes. I'm trying my best to develop the method using OpenFOAM with support for arbitrary unstructured mesh. It is, well, difficulut, for various reasons.

Adaptive Mesh Refinement has been coupled with the geometrical VoF method in an open source flow solver called Gerris which has remarkable results in this area, but cannot deal with complex geometries because of the nature of the mesh it is built upon. If you need an outstanding DNS solutions for jet breakup, wave breaking, various kinds of interface breakup and coalescence dealt with on very low spatial scales, but for simple geometries, this is the way to go right now. If I manage to implement a true geometrical VoF on top of the polyhedral mesh in OF, then, of course, please do use my code in stead. :D

If you are interested in killing spurious currents, check out the articles on balanced force algorithm from Francois et al, Renardy and Rendardy and, the best one in my view, Popinet et al. Popinet shows how the combination of the height functions, octree based local AMR, and properly numerically balanced contributions of the pressure gradient and the curvature balanced force), reduce spurious currents to machine tolerance. All of the advancements rely, of course, on the true geometrical captured interface (not numerically compressed + iso-surface).

T.

Hi, Tomislav,

do you know this paper?

X. Yang and James, A.J. "Analytic relations for reconstructing piecewise linear interfaces in triangular and tetrahedral grids" Journal of Comp. Physics, 214 (2006) 41-54

If not, I hope you will find it useful.

regards

Robert

Hi Robert,

yep, I know that, and I did find it useful! :D Thanks a lot, anyway! :) Are you working on Geometrical VoF method as well?

T.

This is exactly the point!. As i said in my previous post, in my opinion all these techniques work well only with a sharp interface formulation. Im very familiar with the papers you mentioned and i've already tried to adapt the balance force algorithm to OpenFoam but without success in reducing spurious current, due to the fact that my interface is diffused over some cells.
I'm familiar with Gerris as well, but as you said it works only for very simple geometry and mesh, which is not my case (you cannot include obstacle and treat the contact angle as usual for example and you can not use polyhedral mesh). Currently i'm trying to "live" with the problem of spurious velocities and i would like to test how much they affect the results when the dimension of the domain decreases (for simple case and compared to other codes). The major problem is related to the time step, which is controlled by the CFL number and so by the highest velocity in the domain.
It would be great if you want to share your results in case you will be successful!!

Best

andrea

Right now I'm concentrated on coding the steps for the volume fraction equation solution, and as soon as the code runs (both interface steps), I'll need to validate it. I'll share the first results that show the code working properly when the time comes for it: there shall be debugging. ;)

Best regards,
Tomislav

Hi Tomislav

Congratulations on obtaining your master and also congratulations with obtaining a PhD scholarship. I am glad to see that you will continue to pursuit for a general method for interface tracking.

I need to begin this week to make a hexahedral approach similar to the one we talked about in Gothenburg last year, however, I did in my initial exercises last year experience problems with stability of the momentum equation at the interface. Hence, I would appreciate if you could either elaborate a little more on the references (full author list and title) or potentially send a copy to me.

All of my best wishes,

Niels

Hi Niels,

thanks for the congrats! The master degree I will remember for as long as I live: the acknowledgement process and all that surrounded it was very.... special. :)

Just send me an e-mail at the CSI email.

Best,
Tomislav

Hi Andrea et al,

I just stumbled upon this interesting discussion by chance.

I don't really agree with this. Gerris can be used with complex geometries. With "complex" ranging from relatively simple such as this example:

http://gerris.dalembert.upmc.fr/gerr...ples/ship.html

to multiphase flows in actual injector geometries. For example Figure 22 of the recent paper by Dos Santos and Le Moyne:

http://ogst.ifpenergiesnouvelles.fr/...ogst100079.pdf

It is correct that at the moment contact angle conditions are not treated accurately at the "triple points" between interfaces and complex solid boundaries. On the other hand I would be cautious about methods claiming to solve this accurately while still having substantial problems with spurious currents around stationary droplets.

If what you meant is that Gerris does not (and cannot) use an unstructured polyhedral mesh, this is entirely correct, however this does not mean that problems in complex geometries cannot be solved (or that the mesh itself is necessarily simple).

That said, I think that implementing a geometric VOF model within OpenFOAM is a very interesting project.

cheers

Stephane

Hi Stephane,

there must have been a misunderstanding, please accept my apologies for that. I was under the impression that dealing with complex geometries is a work in progress in Gerris. :)

Next time, I'll double check what I think I know (sorry again):

"Entirely automatic mesh generation in complex geometries"

http://gfs.sourceforge.net/wiki/inde...&printable=yes


Best regards,
Tomislav

Hi Stephan,
I apologize too for that, what i was saying was related to the particular case i want to simulate, for which i'm quite sure i cannot use Gerris (at least at the moment). I did not mean any kind of complex geometry or complex mesh, but it was more related to what I'm trying to do. So i'm sorry again to have explained myself bad.


Best


Andrea

Any progress with your Ph.D., Tomislav?

I am interested in interface reconstruction in Cartesian, structured grids and some cylindrical grids, all using hex cells.

I would like to accurately calculate the interface normal in a manner similar to that described by Kunkelmann: http://tuprints.ulb.tu-darmstadt.de/...Kunkelmann.pdf (pg.25).

James

Hi everyone,

I would like to revoke this thread. I am presently facing problems with badly smeared out interface using interfoam.

I tried to refine the domain fine but the smearing seems to reduce but not really satisfactory. Is this caused only due to spurious currents? {else in other words if I try to reduce spurious currents, would the smearing reduce?}

Any new updates over this issue Foamers.

Thanks and happy weekend,
-Saideep

In general the OpenFOAM VOF solver just needs lots and lots of mesh to stay resolved. In general if you turn up the interface compression coeffecient you'll get less smearing, however, you end up increasing the magnitude of spurious currents (from what I've seen).

One effective way (I've tested it its awesome) to mitigate spurious currents is to implement this laplacian smoothing sweep:
http://scitation.aip.org/content/aip...1063/1.4756069

http://www.cfd-online.com/Forums/ope...bill-work.html

Cheers!
Kyle

Sharp interface
 

Hello! Increasing cAlpha and refining the mesh are the only ways to get a sharper interface then, is it? Is there any other way to get a sharp interface? As I am simulating droplet evaporation, I require a sharp interface for my purpose.

Also, thank you for suggesting the laplacian smoother. I implemented it and it really sped up my simulation.