Hy, I'm trying to analize the flow around a ship hull. Until now I used the VOF model, but the code has the moving mesh too.

What is better in this kind of analisys, what are its own advantages and drawbacks?

Thank you Giovanni

Since you have both capabilities, wouldn't you be the best person to find out the pros and cons of the two approach? I would have jumped on the opportunity and run another case with moving mesh, just to learn a new approach (at least)

Good luck

Adrin Gharakhani

With moving mesh you have to make sure you can represent the shape of the hull properly as the mesh moves (since part of the hull is always outside the domain in this case). Techniques I know assume a vertical deformation by default; but when the hull shape isn't perpendicular to the "grid surface" or when the hul shape is non-linear and complex this is probably going to be more difficult... I think industry uses multiphase with VOF.

Thank you for your suggestion. I would like to know more also about differences in acuracy, cpu time ecc.

Best Regards

Giovanni

I would say deformable grid is faster esp. on a large domain.

But here again you would probably need to do some mesh adaption or re-meshhing, say when the water level increases along a concave part of the hull (which was outside the domain at prior time steps), which would not allow a simple vertical "stretching" of your original grid.

You might look at a combination of VOF and FAVOR (fractional area volume obstacle representation). VOF handles the motion of the fluid surface, FAVOR represents the hull of the ship.

These features are combined in the NASA-sponsored codes developed at Los Alamos, NASA-VOF/2D and 3D. The latest wrinkles are included in FLOW-3D, a commercial code developed, maintained, and marketed by Flow Science Inc. a commercial firm also located in Los Alamos. Flow Science is one of the sponsors of cfd-online, so you can get info about them on this web site.

I believe that Flow3d doesn't deal well with entrapped or entrained air pockets within the free-surface calculation.

Is this true?

First, let me say I don't know the answer to that question!

Second, let me ask what you mean by 'doesn't deal well'?

What follows relates to VOF, which I have used in SOLA-VOF, not NASA-VOF. However the codes are similar in layout (much of the fortran in NASA-VOF can be recognized from SOLA-VOF), so perhaps my experience is of some value.

I have used VOF for sloshing (wave-breaking in a tank) problems. The code always slowed down (number of pressure iterations increased, time step was cut) whenever a wave collided with another wave or a wall or top of the tank. Sometimes, the code had to be stopped just before the collision, and some tinkering was required to get the simulation through the event. This was pretty common in dealing with codes from the 70's - I'll bet John Chien would second that thought.

I had similar experiences with simulations of mold filling; pouring molten metal into a crucible.

If this is what you mean by 'doesn't deal well', I agree. If it has to do with accuracy of the solution obtained, perhaps the folks at T-3 at LANL can comment. You might try to contact Doug Kothe (dbk@lanl.gov), who seems to be the current guru for these kinds of problems.

Good Luck!

A little clarification on my previous answer to your question:

"I believe that Flow3d doesn't deal well with entrapped or entrained air pockets within the free-surface calculation.

Is this true?"

My answer in the previous post presumes a one-fluid model; air over water (for example) is ignored. This is only an assumption, so I really didn't answer the question!

I checked the documentation for the 3 VOF codes developed by LANL in the late 70's, early 80's; sola-vof, nasa-vof2d, and nasa-vof3d. All define a fortran input variable nmat, which indicates the number of materials (ie, fluids) in the simulation.

However, the nasa-vof2d report labels nmat as "a fossil". It's not mentioned in the nasa-vof3d report, but the variable still appears in the fortran!

Clearly anyone doing two-fluid simulations with these VOF codes should proceed with caution.

About 10 years ago, I asked Tony Hirt (inventor of VOF) about using VOF to simulate the wind-driven generation of surface waves, with moving air (the first fluid) driving the motion of the liquid (the second fluid). His response was that there is an "impedence mismatch" between the two fluids that makes the calculation inappropriate. This answer might be useful in considering your question.

Yes, Jim. I agree with you. The NMAT varibale still appear in NASA code. But another strange thing happened is I cann't find the convergent test when choosing conjugate residual method. Did you notice about this? But the convergent test appeared in the pressure iteration method. If you find out any answer, please inform me. TQ.

Thank you all!!

I would like to know more about:

"About 10 years ago, I asked Tony Hirt (inventor of VOF) about using VOF to simulate the wind-driven generation of surface waves, with moving air (the first fluid) driving the motion of the liquid (the second fluid). His response was that there is an "impedence mismatch" between the two fluids that makes the calculation inappropriate. "

Are there new versions of VOF that overcome this "impedence" mismatch?

I Don't Know. But your technical library should be able to do a keywork search on "VOF" to see who's publishing in the field these days.

Try Hirt at FlowScience. FlowScience is one of the sponsors of this web site. (www.flow3d.com I think). But he IS selling a product, (flow3d) so may not want to get into details. All you can do is ask ...

Also, try the Los Alamos National Lab (T3 group).

(1). I think, we should encourage these masters in CFD to answer questions related to their work or invention, especially they are sponsors of this forum. (2). Selling products here without making any comments is going to be hard to convince our readers. What do you think? (3). This is not the forum about blind persons talking about big white elephant.

In Giovanni's original message request it was unclear whether his interest was in moving ships, free liquid surfaces, or both. Subsequent comments have all, but one, been directed to the free surface issue and whether or not the VOF method is a suitable modeling approach.

The following comments are directed to the issue of VOF free surface modeling.

First, a search of the literature will reveal that the VOF method has been widely used for a great variety of free-surface applications (with good results!). Numerous researchers have also reported a host of extensions and improvements in the original work performed for NASA and at Los Alamos.

With this in mind, one should not draw conclusions based only on model developments done more than 20 years ago. Nevertheless, those old methods have been responsible for many excellent simulations.

The original VOF method assumed that gas regions (also referred to as void regions) were treated as regions of constant pressure. No gas dynamics was computed because it was assumed that the inertia of the gas was negligible, which is a good approximation for most cases. Instead of modeling the gas, free-surface boundary conditions were applied at all liquid surfaces.

The normal stress condition included gas pressure and, in some programs, an equivalent surface tension pressure. A vanishing tangential stress is the appropriate tangential condition when the gas has no inertia.

If a wave folds over, trapping air, this original VOF model would simply treat it as though the trapping wasn't complete and that air venting could occur. In other words, the gas region would remain at a constant pressure no matter what happened.

Once a trapped region collapsed to the point where there were no empty grid cells it would disappear and the fluid in that region would then be considered continuous, even though the fluid fraction might not be unity everywhere in that region. A improvement was later introduced in the method to encourage the fluid fraction to pack up to unity in interior regions. This was typically done by adding a compression-like term (i.e., negative velocity divergence) to the equation that governs the fluid fraction. Of course, it's necessary to be careful with this sort of "un-physical" addition so that it doesn't affect the overall reliability of a simulation.

Further developments in the VOF method over the past 20 some years have given users the capability to model trapped air using an "adiabatic bubble" approximation. In this case, an isolated gas region has a pressure that is computed from a pressure-volume relation (usually pV**gamma=constant). This model has been used extensively, for example, in metal casting simulations with FLOW-3D(R) to model trapped air.

Recently, we further extended the adiabatic bubble model to account for heat transfer and phase changes with the surrounding liquid. In other words, the adiabatic restriction has been removed. This new model is called the "homogeneous, thermal bubble" model and is finding a number of interesting uses.

We allow both adiabatic and homogeneour bubbles to exchange gas with external sources through modeled valves.

It should be further noted that bubble models, when applicable, are preferred over a direct treatment of gas regions. This is so because inclusion of gas dynamics requires a considerable increase in computational effort, not only because of the additional elements to be solved for but also because gas velocities can be much larger requiring a smaller time-step size and because gas regions have nearly uniform pressures that make it difficult to get pressure convergence.

All of the more recent VOF developments mentioned above, along with many other improvements in the basic treatment of free surfaces using a VOF type of approach are contained in our commercial program, FLOW-3D(R), developed, sold, and supported by Flow Science, Inc.

On the issue of using a "moving mesh or VOF" for modeling the behavor of free boundaries: For ships with breaking bow waves and/or large wake cavities the VOF method should have a decided advantage because it does not require repeated grid reconstruction and the associated interpolations and smoothing necessary with such methods.

For a recent application of VOF to the "Green Water" problem, which is the crashing of very large waves into the superstructure of large ships, see MarineNews, April 30, 2001, page 22.

Finally, it has been held by some that moving grids, in particular, finite-element methods must be more accurate then VOF for small surface deformations because they always have nodes on the surface, while the VOF method must reconstruct a surface every time step. This is false. For a discussion of this point see the article "Connecting the Dots" in the FLOW-3D(R) Newsletter for Fall 1999 (Vol.4.4) that can be found at www.flow3d.com. Also, there are additional articles on VOF and FAVOR(tm) at the same web site under the section CFD101. In particular, see "VOF- What's in a Name."

My apologies if this response is a little too long, but previous respondents have raised many issues as well as suggested that those of us who "advertize" on this website should be willing to provide some useful information.

Tony Hirt/Chief Technologist/Flow Science, Inc.

Well John,

I guess Tony gave us the answer [see his post of Mon, 17 Sep 2001, 12:39 p.m, above]!

(1). I have asked a friend interested in ink-jet modeling to visit the websites of Flow Science and CFD research. (2). I think, the direct message from the experts should give some indications whether business is just business. (3). Computer code is not forever, and I am having difficulty in loading my old codes I developed ten years ago from 5" floppy disk. None of my PC has 5" disk drive. (4). CFD is to encourage the thinking process, to use different ways, to solve real problems. A bad code or a bad process can only create more damages once it gets into the hands (or brain) of a non-professional user.

Thank you very much.

Giovanni