Hi to everybody,

I carried out a liquid sloshing CFD study with Fluent 6.2 VOF model, and I have a few questions about the model implemented in the solver.

Well, I know that the VOF model in Fluent is actually a variable-density approximation of the "real" VOF model by Hirt and Nichols and I also know that Flow Science (Hirt is one of the founders, if I'm not wrong) claims Flow 3D to be one of the few codes (the only one?) with all the three essential features needed to properly model free surfaces (-a scheme to describe the shape and location of a surface, -an algorithm is required to evolve the shape and location with time, -free surface boundary conditions at the surface).

I'm actually going into details of the problem these days and trying to understand whenever and however this approximation will affect the results of the simulations. So my questions are:

1) Has anyone ever faced such a situation? I would really appreciate if someone would share his own experience and deal it with mine...

2) I think that Fluent's VOF model lacking feature is the ability to apply a boundary condition at the interface between the phases (velocity gradients, etc...), I'm right?

3) A fine mesh can improve the model and make the lack neglectable?

4) When body forces' effects decrease and surface tensions, wall adhesion become pre-eminent is the variable-density model even worse?

5) What codes (both commercial and freeware) have the best multiphase models implemented (VOF or even other techniques)?

Thank you in advance for any contribution,

Edi.

Fluent refer to the paper of Hirt and Nichols when explaining the VOF scheme so apparently they use their scheme in the Donor-Acceptor scheme. However the scheme is a bit different when Geometry-Reconstruction is used. Work of Young is used in the latter. The density and viscosity treatment at the interface is through the volume fraction of the phases as follows :

rho = f1*rho1 + f2*rho2

where rho is density and f is volume fraction The three essential features in VOF modeling can be all employed when surface tension is used becasue you have a scheme to describe the shape and location of a surface, an algorithm to evolve the shape and location with time specially in Geometry-Reconstruction, free surface boundary conditions at the surface when surface tension is activated. Getting back to your questions

1. yes I have a little bit of experience in that!

2. I think it's right, I haven't used surface tension models but I guess that's the only way you can specify the boundary condition at the interface. Although I have read some posting here that it's possible to apply some kind of boundary conditions there through UDF. it's also possible to describe mass transfer at the interface in ver 6.2

3. In my case it helped to have more accurate result. I didn't look at that with that perspective

4. No idea

5. I compared free surface modeling of FLUENT and CFX and got better result from FLUENT but CFX has better abilities in other multiphase schemse as it offers high flexibilty in coupling between phases.

First of all, thank you very much for your posting. Definitely interesting.

I thought that the VOF model taking into account surface tension effects should be the solution to specify some kind of boundary condition at the interface too, but it seems to be not the right way. Fluent uses the CSF model by Brackbill and the whole thing is basically an addition of a source term in the momentum equation...via the UDFs you can specify mass transfers or heterogeneous reaction rates, but one limitation in solving the momentum equation stands still: "One limitation of the shared-fields approximation is that in cases where large velocity differences exist between the phases, the accuracy of the velocities computed near the interface can be adversely affected" (copy & paste from page 24-8 Fluent 6.2 user's guide...)

So now the point is: when this affect take place? And how the hell other codes take into account this difference if exists?

Eulerian model is the most accurate available in Fluent but using it for a liquid slosh problem it sounds a bit like a suicide...

thanks for all,

Edi.

Hai fluent users

can any one give idea for my laser cutting problem.

wheather it is possible to remove the material(vaporization) by applying heat.

Actually beyond certain temperature all the materials will start to vaporize.Can this vaporization be modelled in fluent.

Thanks in advance

M.Sundar

Your welcome!

Not sure about the answer of your question. As far as I know, one velocity field is shared between two phases and the only contribution of the phases are through their properties. That's what they claim as the advantage of the VOF as there's no need to solve for extra momentum equations relative to the other multiphase flow schemes.

for flow sloshing problem, you definitely and solely need to use VOF. There're some recommendations given by FLUENT about how to treat such problems. such as proper Courant number, discretization method and so on. you may check that out on their site. I guess the title of that is "best practices for modeling multiphase flows in automotive industry"

cheers

Dear Fluent users, I am Research Scholar in the Dept of Ocean Engg, IIT Madras, India. I am just about to venture into the use of Fluent for my thesis problem. Have any one experience on the simulation of water waves using Fluent. Looking forward for suggestions. Many people suggest me to use Fluent for the above problem than CFX. But they didnot give me clear reason, why so. If anyone has idea, pl, let me know.

Thanks in advance... Balaji

Balaji,

I would recommend CFX over Fluent for any analysis of this type. CFX solves an Eularian-Eularian form of the momentum equations for multiphase in either a homogeneous (shared velocity field) or inhomogeneous (multiple velocity fields) form. The phase interface is captured by an implicit compressive advection scheme, rather than through interface tracking and therefore allows much larger timesteps and faster convergence.

Also, if you have waves crashing (or sloshing in a tank), the inhomogeneous formulation allows the separation of the liquid and air phases. In inhomogeneous simulations, all (n-)phases are also solved simultaneously in a single, coupled matrix, which is critical for stability in such simulations where interphase drag is significant.

-Guy

Guy, Thanks for the suggestion. Please mention few examples, if you have, of earlier work done in both CFX and Fluent on the water wave problem. Infact i am in dark about both CFX and Fluent. Few people doubt about the accuracy of the surface following characteristics of CFX. Is that true. If you have any papers/reports/publications regarding the water wave simulation on CFX & Fluent, pl, let me or pass over to me.

Thanks in advance... Balaji.