Have someone experience in modeling cyclones?

I have to model a gas-solid cyclone for my M Eng. study. I have a problem in defining the vortex finder outlet S (in figure), may I define it as OUTLET VENT?. I define my inlet as INLET, the top outlet as PRESSURE OUTLET, Bottom outlet as a WALL.

Inlet (INLET) gas outlet on cyclone top (PRESSURE OUTLET) solid outlet (WALL) Vortex finder (?)

I have try the simulation using k-e model however the result is not satisfactory. I also experience a 'error: access: unbound variable' in INLET and Outlet.

Thanks in advance

I'm not sure if I fully understand what you are trying to say but I'll tell you what I feel you need to know.

Set the inlet to a Velocity Inlet, Set the outlets to Pressure Outlets, the walls are standard walls with no slip condition. The vortex finder is also a wall so set that to wall too.

k-e model will not be able to model a cyclone correectly. The flow field is extremely complecated and it will not be able to reproduce features such as a rankine vortex or reverse flow.

What you need to do is use the RSM model. You also need to use second order upwind for discretization. Use PRESTO for pressure and SIMPLE for pressure-velocity coupling. I would use a hex mesh and try to get a good mesh qaulity as this will save you a lot of time later trying to get convergence.

Use the DPM model for modelling the solids.

May I ask you why you have set the bottom outlet to a wall. If this is an outlet as you have defined it why use the wall boundary condition?

As for your error message, I feel you need to set up your boundary conditions correctly first and then address other problems.

Hope this helps

Tom

Hii, Thank you very much for your advice, actually I'm referring a work of Dr. Micheal Slack which is defining the bottom outlet as a wall because he assumes the zero underflow components. Dr. Slack also using RSM on his cyclone simulation. I think my boundary condition now is ok since there is no more error massage displayed during simulation. I chose the OUTFLOW for top and bottom outlet. The flow simulations seem to be ok now, however I still have some problem on defining DPM for solid. Is it possible to define a particle size in fluent? Can anyone suggest a good CFD references book for my cyclone simulation? Thanks again.

In the DPM injection pannel you should find you can set the particle size either as a single size (single injection) or following a size distribution (point/surface injection).

If you chose the OUTFLOW condition you will not be able to represent reverse flow through this boundary which may occur depending on your flow conditions. I owuld have gone for the Pressure Outlet and set the pressure to atmospheric.

Remmeber if you set your bottom outlet to wall then you will have to set the DPM boundary condition to escape to allow for particle removal.

If you find any good literature on the subject or books, can you please let me know what they are.

Thanks again Tom, now I define the bottom outlet as OUTFLOW. I'm now using a fine mesh but it still very hard to converge. I never get the convergence solution even after 20000 iterations. Is it any tips to get the convergence solution in cyclone simulation?

Regarding on a literature I just searching through www.sciendirect.com and found a few cyclone CFD article there like Ray et al. (1998) Int. J. Mineral Processing, Griffiths & Boysan (1995) J. Aerosol Sci., Youngmin Jo et al (2000) Pow. Tech., & W. Peng et al. (2002) Pow. Tech.

Other articles that downloadable through internet are Wanka et al (2001) Latin American Research, & Robert Harwood and Michael Slack (2002) QNET-CFD Network Newsletter. In addition I have a PhD thesis of Christian Fredriksson from Lulea University of Technology Sweeden which is working on the cyclone gasifier experiment & simulation. His works include a combustion reaction in cyclone. I also still look for the good literature/books in this area.

Convergence is difficult in this type of simulation. Fisrt Order discretization shouldn't give you too much of a problem but you will find that the results will not compare well to experimental results. You need to use second order and you will probably find it hard to get continuity to converge. I would suggest increasing the pressure URF and decreasing the momentum equation. You should find you'll get better convergence.

Thanks for the info on literature. I have a copy of Fredriksson thesis. Is this the cyclone you are working on.

No, I'm not working with a gasifier. I simply do a cyclone pressure drop & efficiency simulation for now. I also comparing the CFD result with a number of presented numerical model on cyclone like Iozia model, Koch Licht model & Barth model. I have finish the numerical part the only thing is the CFD part.

I'm not only working with cyclone but also doing a catalytic converter simulation with CFD. However the catalytic converter simulation is easier because it is only related to laminar reactive flow. Thank you very much for your help, its really solve my problem.

Just one more point that I think might help.

When you switch over to using second order upwind for discretization you may find trouble reaching convergence. In fact, what you will probably find is that if you observe the behaviour of the residuals, you may find that they exhibit cyclic tendancies. What this means is that a transient pattern is occuring. In this instance, what you need to do is change over to a transient solver and make the time step something in the region of 0.025 seconds (or a tiny fraction of the residence time of the cyclone). I have found that by doing this, convergence is reached with relative ease.

Best of Luck.

I have try the transient solver and its work fairly good. Thank you very much.

Which pressure is it related to cyclone pressure drop? is it the static pressure? at inlet, outlet or any boundary? Thanks in advance.

It's the differnce between the pressure at the inlet and the gas outlet. You can use either absolute pressure or static pressure (Absolute Pressure = Static Pressure + Operating Pressure).

Thanks again Tom.... Since the begining I guess that must be the way of calculating the cyclone pressure drop... however my predicted pressure drop more than 1e5 Pa.... the experimental value is only about 8e2 Pa.. the empirical pressure drop model predict around 8e2 to 1.4e2 Pa... I might make mistake in gambit since the "Error: access: unbound variable" and "Error Object: phase-domain?" appear when I open the mesh file for the first time. I have 2 volume in my cyclone, 1st is cyclone body and 2nd is vortex finder.. any suggestion on that?.. Thanks.

Yeah, how have you named your boundary types? I knoiw this may sound strange but FLuent is sensitive to these things. If you named it something like inlet 1, you may find you get that error, however, if you name it inlet_1 then the error should go. Try it and see.

Your pressure drop problem seems a little bit more difficult. What discretization scheme have you used for calculating pressure? Also what type cells are you using in the mesh?

Regards Tom

Tom, your are amazing.... my simulation work with your suggestion. I'm using a RSM turbulence model with Presto!, Simple, and 2nd order upwind for discretization as your suggest that setting to me... I just get the massage below from fluent to confirm the bug in Fluent 6. Good luck... Thank you very much..

From: "Dipankar Bandyopadhyay" <db@fluent.co.in> | To: "jolius gimbun" <jolius21@yahoo.co.uk> Subject: Re: Problem on cyclone simulation

Hi,

Please name the boundaries something like 'pressure-outlet' instead of 'pressure outlet' while exporting the mesh from Gambit. This was a bug and fixed in the latest version. It automatically adds an '_' in between now. I mean 6.1.22.

Hope this helps Regards Dipankar

I wouldn't say amazing - I just have six years experience using Fluent every day. I also just finshed a PhD modelling cyclones so I know a little a bit about them thats all. Glad I could be of assistance as I know the learning curve is sometimes very frustrating.

Best of Luck

[arjun3020]

Hi, i want to find out efficiency of cyclone,
if i inject particles of 20 micron (20% of total mass) then 30 micron (50% of total mass) and and 60 micron (30% of total mass).
then what about mass flow rate?
if my total particle mass flow rate is 0.01 kg/sec. then while running for first 20 micron particles(for single injection) what is mass flow rate i have to give to fluent. is it 0.01 kg/sec or 20 % of 0.01 kg/sec.?
please help.

what type of injections i have to use.