hi can anybody provide me with any tutorial about cyclone. for working in fluent and pre processor gambit. thanks Anjum

hello,

sorry, but everything i have (no tutorials) about cyclones and cfd is written in german. i think you are not very familiar with german, aren´t you? the only thing i can tell you, is that you might better use the RNG (k-e) turbulence model. the standart k-e model gives not very good results according to the radial velocity profile in a cyclone flow. use standard k-e just for initialization or any test runs.

I very fine grid might be a good idea, too.

good luck

hi you can send me i wil it apreciate this and also if you can guide me how to creat geomtry and mesh in better way. if u have any solved problem with u u can also send it to me. i will apreciate any thing. my email is anjumnaveed76@yahoo.com thanks in advance Amjum

I'v done a cyclone simulation for the last 3 year. It quite easy and straightforward some guide for CFD simulations are as follow:

1)RNG k-e or RSM or LES 2)2nd order discretization, SIMPLE, PRESTO! 3)DPM can be used with considerable accurate grade efficiency calculation 4)standard wall is just fine

Better set the bottom outlet as wall but in DPM particle must be trapped or collected, not reflacted. Some of my published paper are available online via www.sciencedirect.com or search in www.scopus.com.

Good luck.

Hello, Gimbun: I guess I read your paper in CEP(2005). what is your time step when you do the transient computation? and how about your velocity-time series profile? My result is that the magnitude of velocity attenuates with time, why is this? Thank you.

LCW

transient computation dt=.025s, after your residuals almost or near converged, please change to steady solver. LCW, don't think too much about time function or unsteady iteration, it just a matter of how to get your simulation converged. I've experienced that there is no convergence until 20000 iterations using a steady solver for cyclone, therefore Dr. Fraser give me this hint. I guess tiny dt will allowed the numerical flow in cyclone to be steady. Hope it useful.

Gimbun:Thank you for advice! I know Fraser' work is also good. I have done as you mentioned. When I change unsteady iteration to steady solver, after some iterations, the oscillation of the velocity at a point appears again, the magnitude of oscillation of the velocity is not small, approximate 2~3m/s. the residuals still exhibit cyclic tendencies, but keep horizontal as a whole, anyway I can not get the steady solution.

The dt=0.025s in my previous work cannot be applied in your problem. If you're working with sampling cyclone and low inlet velocity it does not need a transient solver at all. Similarly if you are working with industrial scale cyclone (>0.7m diameter) or/and higher inlet velocity or/and extreme temperature, the dt=0.025 cannot be applied, you must try what dt is suitable for your problem, but I'm very sure that this method will give you a convergence. To reach a convergence in CFD is a skill to be developed along with your work. Good luck.

respeced sir, i have been also working in modeling of cyclones ,i have been using RSm trurbulence model.The simulations predict the expected pressure drop & velocity profiles well ,but i am not able to predict the staic pressure at the gas outlet (which has to normally negative )the simulations predict it to be in possitive range .But iam geting the expected pressure drop.May i know why its happening like this. Also iam facing reverse flow problem occuring in my outlets how to face this problem.

Hi Ganesh, where did you put your measurement point in your simulation? It must be at the same point of your exeriment. In my case, I just create a point at the centre outlet of the cyclone. Sometimes, the static pressure at outlet is -ve but not in all case. I do find them to be +ve sometimes too, by the way why your are intetested in this parameter? since this doesn't contribute anything tho the cyclone operation.

Thanku sir, i was actually intersted in modelling of industrial calciner-cyclones.so i was intersted in knowing what will be the negative pressure effect on Calcination kinetics ,coz under high pressures reversible reaction can take place.

I faced one problem while simulating a cyclone with a high inlet temperature of 1200 k and with a gas inlet velocity of 37 m/s ,where the cyclone is of diameter of 6 m its an industrial calciner.I was getting the maximum velocity in the cyclone of 150 m/s and pressure drop of 5000 Pa. which was a little contradictory to the lab scale cyclone where the maximum velocity is twice the inlet velocity and pressure drop is will be around of 1200 Pa for a same inlet velocity.I refered your paper also"The influence of temperature and inlet velocity on cyclone pressure drop: a CFD study".Iam using RSm only.Can i know why is this discrepency? Regards Ganesh kumar.v

The first thing, is your simulation converged? if so then maybe you have to validate your simulation with experimental measurement. To be honest, I never did any simulation on very big cyclone and therefore not very sure why your velocity can be very high. I suggest this explaination, in the small cyclone the wall friction have a significant effect but in the big cyclone it is insignificant and therefore you get a very high velocity. Anyway, it just my assumption and only an experimental measurement can tell you the truth. Good luck.

Thanku for your kind reply sir, I dont have experimental industrial data to validate the simulations. is there is any method to make RSM converge fast ,what normally i do is i start with K-E model ,once the ke model gets converged ,i switch it on to RSM model and run it at low URL for momentum equation. after some stage i change it to unsteady state with a time scale less than 1E-03 .almost it takes 1,50,000 iterations to reach the convergence.My mesh size is 50,000 ,also i do fine mesh at the axis to catch the unsteady state behavior of innex forced vortex core.It will be of great help if u give me some tips to make the run converge faster. Regards Ganesh kumar.v

[EYITAYOAFOLABI]

can you kindly send me tutorial on cyclone simulation to this e mail id.

e.a.afolabi@ncl.ac.uk

[esicia]

hello
I have got the good counters of the static pressure and velocity in a tangential cyclone. but a question how to calculate the pressure drop in cyclone. I have the ststic pressure of 280000 pa in velocity inlet and the 50000 pa in outflow. the difference is too large. is there any recommendation

best wishes

[arjun3020]

Hello Mr. J.Gimbun,

I have gone through Paper,
I found two plots of pressure drop with respect to inlet velocity. please see attached plots.

In all other literature fig. 5 holds good.
but i am not able to draw conclusions from fig.3.
i am also doing cyclone analysis and as you say in your paper i am also getting cyclic fluctuations of residuals.
so i need to run transient case. cyclone diameter is 0.650 m. and flow rate is 3119 m3/Hr, with inlet velocity is 12 m/s.

could you please help me to decide parameters of transient run.

Great work. in paper.

Please help me.

[arjun3020]

Hello Mr. J.Gimbun,

I have gone through Paper,
I found two plots of pressure drop with respect to inlet velocity. please see attached plots.

In all other literature fig. 5 holds good.
but i am not able to draw conclusions from fig.3.
i am also doing cyclone analysis and as you say in your paper i am also getting cyclic fluctuations of residuals.
so i need to run transient case. cyclone diameter is 0.650 m. and flow rate is 3119 m3/Hr, with inlet velocity is 12 m/s.

could you please help me to decide parameters of transient run.

Great work. in paper.

Please help me.