CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

cyclone

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By J.Gimbun
  • 1 Post By J.Gimbun

Reply
 
LinkBack Thread Tools Display Modes
Old   February 17, 2006, 10:29
Default cyclone
  #1
ANJUM NAVEED
Guest
 
Posts: n/a
hi can anybody provide me with any tutorial about cyclone. for working in fluent and pre processor gambit. thanks Anjum
  Reply With Quote

Old   February 17, 2006, 16:24
Default Re: cyclone
  #2
tilman
Guest
 
Posts: n/a
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
  Reply With Quote

Old   February 18, 2006, 00:19
Default Re: cyclone
  #3
ANJUM NAVEED
Guest
 
Posts: n/a
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
  Reply With Quote

Old   February 20, 2006, 11:52
Default Re: cyclone
  #4
J.Gimbun
Guest
 
Posts: n/a
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.

ch3coohminh likes this.
  Reply With Quote

Old   February 21, 2006, 09:07
Default Re: cyclone
  #5
lcw
Guest
 
Posts: n/a
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
  Reply With Quote

Old   February 21, 2006, 13:02
Default Re: cyclone
  #6
J.Gimbun
Guest
 
Posts: n/a
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.
ch3coohminh likes this.
  Reply With Quote

Old   February 22, 2006, 04:58
Default Re: cyclone
  #7
lcw
Guest
 
Posts: n/a
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.

  Reply With Quote

Old   February 22, 2006, 13:40
Default Re: cyclone
  #8
J.Gimbun
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   February 23, 2006, 00:29
Default Re: cyclone
  #9
GANESH
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   February 23, 2006, 10:04
Default Re: cyclone
  #10
J.Gimbun
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   February 23, 2006, 11:27
Default Re: cyclone
  #11
GANESH
Guest
 
Posts: n/a
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

  Reply With Quote

Old   February 23, 2006, 14:33
Default Re: cyclone
  #12
J.Gimbun
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   February 23, 2006, 15:57
Default Re: cyclone
  #13
GANESH
Guest
 
Posts: n/a
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
  Reply With Quote

Old   October 26, 2009, 08:49
Default assistance
  #14
New Member
 
EYITAYO AFOLABI
Join Date: Apr 2009
Posts: 10
Rep Power: 8
EYITAYOAFOLABI is on a distinguished road
can you kindly send me tutorial on cyclone simulation to this e mail id.

e.a.afolabi@ncl.ac.uk
EYITAYOAFOLABI is offline   Reply With Quote

Old   December 8, 2009, 09:06
Default wrong pressure drop
  #15
New Member
 
Esmail
Join Date: May 2009
Posts: 11
Rep Power: 8
esicia is on a distinguished road
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
esicia is offline   Reply With Quote

Old   April 25, 2012, 01:43
Default
  #16
Member
 
arjun
Join Date: Oct 2011
Location: Tokyo, JAPAN
Posts: 66
Rep Power: 5
arjun3020 is on a distinguished road
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 is offline   Reply With Quote

Old   April 25, 2012, 01:47
Default
  #17
Member
 
arjun
Join Date: Oct 2011
Location: Tokyo, JAPAN
Posts: 66
Rep Power: 5
arjun3020 is on a distinguished road
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.
Attached Images
File Type: jpg Pressure plot.jpg (34.6 KB, 54 views)
arjun3020 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
pulverized coal cyclone burner Manuel Acosta FLUENT 9 May 24, 2007 05:04
Cyclone Design Sanjib FLUENT 0 August 1, 2005 20:00
How to mesh the worm-inlet cyclone Fuping Qian FLUENT 0 July 7, 2005 03:59
cyclone meshing Tom Robin FLUENT 1 September 16, 2004 06:58
Modelling Industrial cyclone behaviour Günther Hasse Main CFD Forum 3 October 12, 1999 19:34


All times are GMT -4. The time now is 21:00.