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

Cyclone separator Simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 10, 2013, 12:48
Default Cyclone separator Simulation
  #1
New Member
 
Arun Vasudevan
Join Date: Feb 2013
Posts: 6
Rep Power: 4
prohackrav is on a distinguished road
Hi I am a 3rd year BTech student trying to do a simulation on a Cyclone separator. I have tried using RNG K-e model standard values for convergence. My mesh has around 560000 cells but orthogonal quality is shown as 0.0096. I have set velocity inlet and one outlet at top. Should I enable DPM before or after calculation of flow field is done? I have used surface injection from inlet with a rosin rammler logarithmic distribution between 1-300micrmeter. I have used step length factor 5, and no. of steps 10000. But most of the particles are still incomplete......

Can you advice me on what to do?? I just need to show the collection effeciency.
prohackrav is offline   Reply With Quote

Old   April 11, 2013, 02:14
Default
  #2
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
Hi
I had already a 3D cyclone simulation. Let me tell you some tips to have a good performance in simulation:
1- try to generate a structured mesh, it's very important and requires some skills and work.
2- Apply RSM if you don't use LES. But, reaching a converged solution in RSM is somehow cumbersome. First start with k-e and after a few iterations e.g 200 go into RSM.Selecting RSM is due to high swirling flow inside cyclone.
3- If you need to obtain collection efficiency, then you should use DPM to track particles. Before injecting the particles, you must reach a converged fluid flow, and then perform your DPM. Regarding to lack of particles tracks visibility, there are some hints in fluent user guide, you can refer to. For instance increase the number of steps. Have a deep look at DPM modeling in fluent.
Good luck
__________________
Regard yours
A CFD free user is offline   Reply With Quote

Old   April 11, 2013, 04:21
Default
  #3
New Member
 
Arun Vasudevan
Join Date: Feb 2013
Posts: 6
Rep Power: 4
prohackrav is on a distinguished road
I read that LES and DPM are incompatible in ANSYS. I have tried increasing the no. of steps in tracking particles, but still the no incomplete is more than 50%. I think there is a recirculation zone inside the cyclone at a particular level. What should I do??
prohackrav is offline   Reply With Quote

Old   April 11, 2013, 04:27
Default
  #4
New Member
 
Arun Vasudevan
Join Date: Feb 2013
Posts: 6
Rep Power: 4
prohackrav is on a distinguished road
I have first got convergence using k-e model with first order discretisation then switched to RSM and got convergence with that too. I think i got the fluid flow more or less accurate with the swirl regions. But tracking particles still shows incomplete even after raising the no of steps for tracking to 10^5. The particle tracks show that the particles are recirculating in a particular horizontal zone.
prohackrav is offline   Reply With Quote

Old   April 11, 2013, 11:31
Default
  #5
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
Well, maybe it's a deficiency of your geometry. Who knows? nevertheless, get a contour of velocity ( magnitude, y and x direction) and see what exactly taking place inside cyclone. Use some larger or heavier particles and increase mass rate and see what comes up.
__________________
Regard yours
A CFD free user is offline   Reply With Quote

Old   April 12, 2013, 02:31
Default
  #6
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 899
Rep Power: 15
ghost82 will become famous soon enough
Quote:
Originally Posted by prohackrav View Post
I have first got convergence using k-e model with first order discretisation then switched to RSM and got convergence with that too. I think i got the fluid flow more or less accurate with the swirl regions. But tracking particles still shows incomplete even after raising the no of steps for tracking to 10^5. The particle tracks show that the particles are recirculating in a particular horizontal zone.

Hi, I had the same problem, particle tracks incomplete, if particles >critical diameter; this is ok, since I found that:

"The particles with diameters of 2x10-6 m and 7x10-6 m can spin down to the conical section of cyclone and then should be collected while the bigger particles with diameter of 3x10-5 m and 1x10-4 m spin downward first and then keep spinning near the wall at a certain horizontal level. There is therefore a critical value to distinguish the flow pattern of particles of different diameters. If the particle diameter is larger than the critical value, the particle will keep a circular motion in the cone of cyclone. In contrast, if the particle diameter is less than this critical value, the particles will be collected directly or escape from the cyclone. […] In the real industry, these bigger particles will be eventually collected due to their interactions with other particles."


From: NUMERICAL STUDY OF GAS-SOLID FLOW IN A CYCLONE SEPARATOR (Wang et al.)

So, when you calculate efficiency collection treat as collected incomplete particles track (make sure residence time is long enough to consider them as trapped in your volume)
Daniele

Last edited by ghost82; April 12, 2013 at 03:02.
ghost82 is offline   Reply With Quote

Old   April 12, 2013, 03:11
Default
  #7
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
Hi daniele
I just simulated the cyclone model you mentioned (Wang et al.) and I had the same problem, I just forgot to tell. Thank you for your recall.
__________________
Regard yours
A CFD free user is offline   Reply With Quote

Reply

Tags
ansys, cyclone separator, fluent, fluent 14, meshing

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
Steam-Water Vertical Cyclone Separator Munggang FLUENT 3 April 29, 2014 13:38
requiring solution for heat transfer from gas to solid particle in cyclone suvai79 FLUENT 0 September 1, 2012 05:48
[DPM problem] infinite particles loop in domain (twin cyclone - double cyclone)) ghost82 FLUENT 1 November 14, 2011 08:48
How to mesh the worm-inlet cyclone Fuping Qian FLUENT 0 July 7, 2005 03:59
Modelling Industrial cyclone behaviour GŁnther Hasse Main CFD Forum 3 October 12, 1999 19:34


All times are GMT -4. The time now is 18:55.