Can CFD analysis techniques be used for multiphase flow systems (i.e. dispersed gas bubbles in a liquid continuous phase)? It seems that in such cases the basic continuum assumption does not apply for the system as a whole. If CFD can handle this, it seems to me it would be of great use in chemical engineering reactor design (for which I have not seen it applied, though I am something of a novice in this field).

In 3-D computer graphic animation, people can simulate rain, snow, spray etc. on the screen by tracking each particle. The same concept can be applied to the bubbles in fluid flow. If you don't want to handle each individual particle, then you have to develop a model to describe the whole system. CFD can be interpreted as "computer-assisted fluid dynamics". The computer can not help you if you don't know how to solve the problem. The answer to your question is : it depends on your ability to solve the multiphase flow problem. If you do, the computer sure will help you a great deal in terms of speed.

Thanks for your response John. Perhaps I should have phrased my question as: Can commercial CFD codes simulate multiphase flows in reactor vessels? It seems any numerical analysis technique using a mesh (for the whole vessel) won't be able to handle bubbles or droplets of one fluid dispersed within another.

Well, people have been modeling two-phase flow of spray problem in two steps, first, compute the gas phase first, then, compute the particle trajectory and dynamics based on the initial particle size and conditions, over a group of sizes with the gas phase as the background flow field. Since there is a mutual interaction between the gas phase and the particle phase, the gas phase computation must be updated with this interaction (in terms of mass, momentum,and energy transfer between two phases.). At the particle level, people have been studying single particle dynamics in the gas phase, particle internal liquid motion, multi-particle interaction in gas phase, and even the formation of liquid spray processes. For cold flow alone, the limitation seems to be the capacity of the computer. For reacting flows, the chemical reactions and the turbulent nature of the flow will be the biggest uncertainty. With the high speed PC becomes more readily available at low prices, more people will be able to study these problems. The real problem can then be solved using a group of PC in a networked parallel environment. You are always limited by the computer capability, especially in the multi-phase reacting flows computation. In the combustor design case, most of the time, people are interested in knowing just the flow field behavior so that they can create the desirable environment. Running directly the reacting flow without detail knowledge of the flow field will simply make the design and analysis of reacting flow very complicated ( it's hard to extract reliable and useful information from "rough" calculation). I would say, the multi-phase reacting flow CFD will be a very good subject in the next century (based on the PC development). Some commercial code companies have more qualified engineers in computing reacting flow problems, but this does not mean that the code they use can handle every reacting flow cases. Codes are partial listing of engineer's idea in solving flow problems. Since it is impossible to put everything into a code, the most important factor in CFD is the engineer himself.

I definitely think that tracking each and every bubble in a multiphase mixture is more time consuming than the average engineer would like (though I'm working on something like this right now). On the other hand the most widely accepted method for computing flows with dispersed bubbles is using a modified equation of state: as a matter of fact at the last Cavitation and Multiphase Flows Symposium in Grenoble, one of the most interesting computational papers was the one by Merkle, who is using a N-S solver with an arbitrary eqn. of state (he published something on the AIAA J. too). CIRA and Centrospazio-CPR in Italy are working in the same direction and results look quite promising (well, maybe I'm not a reliable sorce of information cause I'm working on this project at Centrospazio-CPR !! ). Anyway, in this respect any commercial code which allows for the implementation of an arbitrary eqn. of state can be used for NON-REACTING dispersed bubbly flows. Unfortunately the reacting case is a completely different world: I've seen some papers about droplets, in which the methods of statistical mechanics are used to a certain extent (collision integrals etc.) but I've no experience on this. Maybe the particle/bubble-tracking method is the right way to go but it's going to be VERY computationally intensive.

Well, people in PC games business seem to be making a lot of progress to bring the 3-D real time games on the market. It requires a faster CPU design, a faster 3-D graphic board, and a faster API. Maybe someday, these individual bubbles and particles will be each processed on the hardware board. A brand new computer probably will be created for multi-phase flow calculation. By the way, particle tracking method was the method I used back in 1981. At that time I was working on dump combustor flow with swirl ( cold flow case only).

Take a look at the 'process' section under http://www.aeat.com/cfx/cfxapp.html and read about the EU ADMIRE project.

David, I think the simple answer to your question is YES, commercial CFD software can model multi-phase flows in reactor vessels. As I said that is the simple answer, and the extent to which you want the reaction itself modelled, the geometric complexity of the vessel, the number of phase etc, will all be a factor in whether CFD is the right tool in the circumstances. As a consultant working for Fluent, I have had some experience of both Lagrangian and Eulerian multi-phase modelling, and if you want to email me with a few more details on your particular problem, I'm sure I could give you some more details.

Hi David,

Yes, some multi-phase flows can be solved by current commercial codes. The first issue is what level of modelling is acceptable for the real problem.

1. An Eulerian-Eulerian approach which wiews both the continuous and dispersed phases as continuua. The averaging of the motions of the dispersed phase is done over length and time scales significantly larger than the dispersed phase length and time scales much like the approach in derriving the RANS (Reynolds Averaged Navier Stokes) equations or a porous media volume averaging approach. Therefore a closure model is required for these "sub-grid" processes.

2. The Eluerian fluid, Lagrangian particle approach may be used in which discrete Lagriangian ODE's equations of motion are solved for each particle. The continuous fluid is still solved with the Eulerian approach. The coupling can be added to the Eulerian fluid momentum equations as a source term or neglected in which the Lagrangian particles may be done as a post-process.

The second apprach looses validity as large volume fractions of particles are introduces since no particle-particle interactions are calculated. TASCflow or now called CFX-TASCflow 2.73 can only do the second approach. CFX 4 can do both.

You should ask Dave Straddioto about this .... I gave him a demo on TASCflow a few weeks ago!

Good luck, Duane Baker

If I want to deal with a pump with water and air, what kind of code suggested? The pressure up to 7 bar.

Is this a positive displacement pump or a turbomachine? If this is a turbomachine and the volume fraction or air is small (the order or 1%), then CFXTASCflow 2.74 is a good choice because of its capabilities for rotating frame analysis and the air bubbles can be treated with lagrangian tracking, including the mass transfer which occurs from/to the bubbles to/from the liquid. Similarly, if this is a compressor with a small volume fraction of entrained water dropplets a lagrangian analysis on the water dropplets may be performed.

If this is a positive displacement device then you need a moving boundary code...no knowledge of these.

good luck, Duane .................................................. .. Duane Baker P.Eng., B.Sc.(Mec E), M.A.Sc.(Chem E), M.A.Sc.(Mech E) CFD Research Engineer Alberta Research Council Email: baker@arc.ab.ca .................................................. ...

Rotating frames of reference is a very good thing but you have to be sure that it works for your pump reasonable well. All major codes have this capability now.

If it does not work for some reason, e.g. strong transient phenomena, you have to do a moving mesh (sliding mesh) calculation. This may be very painfull as you compute time jumps from 1 day to approx. 1 month You also have to save much more data (some GB).

In a first step I'd try a simulation without air .

If you find that a rotating frames calculation fits your needs and you can use a lagrangian approach for the air you are a lucky person.

If you have to do a sliding mesh calculation also with the lagrangian model for the air you have to look very carefully for a code which can handle this (e.g. StarCD). Some codes are not able to handle both features together (Fluent 2 years ago).

If there is a lot of air in your water and you have to use an euler-euler model then I can't help you.

Your partickle path in a rotating frames calculation looks a bit strange when the partickle is moving from the fixed frame into the rotating frame. Either it hits the wall or it looks as it would go through the wall or there is a crack in the path ... This results from the transformation of relativ and absolute velocities. So try to stay in one frame when you look at the trajectories.

Joern

( http://www.beilke-cfd.de )

Just a little remark.

It is true that 2 years ago Fluent software could not handle both, sliding mesh & particle tracking at the same time. Two years is a long time in the CFD business and in the meantime in its latest version Fluent now can handle both sliding mesh + time dependent particle tracking.