# DPM in cyclone separator!!

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 4, 2008, 17:46 DPM in cyclone separator!! #1 Ines M Guest   Posts: n/a I'm working on cyclone separators gaz-solide (CFD simulation, Fluent), I found an article published in Elsevier and I considered it useful to validate my model, basing myself on its results, but now I have two big problems which prevent me from continuing my work: •The first problem: Distribution of particles: ROSIN-RAMMLER distribution with a min diameter 2e-07 (m), max diameter 0.0001 (m), mean diameter 2.99e-05 (m), spread parameter 0.806 and number of diameters 5 (type of injection: surface). Results: when I did particle tracks, I carried out that diameters chosen by Fluent are 2e-07, 2.5e-05, 5e-05, 7.5e-05, 1e-04 => in comparison with results of the article, I found a great difference; diameters schematized in the article are about 1e-06 (the diameters selected influence the performances of the cyclone and separation efficiency since particles having diameters about 1e-05 keep spinning near the wall at a certain horizontal level. •The second problem: I do not manage to have convergence with steady RSM. I will be grateful if you agree to help me to conclude my work.

 February 5, 2008, 14:03 Re: DPM in cyclone separator!! #2 Allan Walsh Guest   Posts: n/a For the first problem: I would not have Fluent generate the R-R distribution. I don't think the particle flow should have a big effect on the fluid flow, so your first job is to solve the fluid flow. Once you have that, set-up half-a-dozen particles of the size in the distribution you are intested in - each with a single diameter. Say 0.5, 1, 5, 10, 50 and 100 microns. Then for each particle size, find the separation efficiency and then look back at the distribution to find out what fraction of the particles have a certain diameter. For example, the 0.5 micron might represent 7% by mass of the distribution, the 1 micron 12% etc. This will give you the overall collection efficiency for that size distribution. Other variables will be important too, of course, like the coefficient of restitution, the step size for particle calculation, the initial particle velocity and position at the inlet,etc. For the second problem: what do you mean by lack of convergence? Do you get different collection efficiencies as you run the simulation longer? Divergence? Pressure difference keeps changing? I don't have a lot of experience with cyclones, but for one project we worked on recently, we went with the hexagonal cell option in Fluent 6.3 and had pretty good luck with the steady RSM model (second order), but couldn't get good results with LES model. Good luck. arjun3020 likes this.

 February 21, 2012, 05:17 #3 Member   arjun Join Date: Oct 2011 Location: Tokyo, JAPAN Posts: 66 Rep Power: 8 Hi, Allan Walsh. I have particle details, e.g. 10 particles of range 1 to 10 micron. 50 particals of 20 micron and so on. then how should i have to proceed to find out collection efficiency.? please help me in detail..

 February 21, 2012, 06:08 #4 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 1,003 Rep Power: 19 Inject your particles, then save or print to console escaped and trapped particles and mass flows and calculate from these data collection efficiencies. Daniele

 March 27, 2012, 04:57 #5 Member   arjun Join Date: Oct 2011 Location: Tokyo, JAPAN Posts: 66 Rep Power: 8 Hi, you said inject single diameter particle is it mean single injection? or surface injections of uniform diameter distribution? and what about flow rate of particle. if i inject particles of 20 (20% of total mass) micron then 30 micron (50% of total mass) and and 60 micron (30% of total mass). then what about mass flow rate? if my total mass flow rate is 0.01 kg/sec. then while running for first 20 micron particles 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.

 November 30, 2015, 05:14 #6 New Member   senthur rajasekar Join Date: Nov 2014 Posts: 16 Rep Power: 5 yes, same problem im facing in cyclone separator. i have to inject 10 different dia. size of particles in a single simulation. at first, i will simulate each and every particle dia. with corresponding mass flow rate(x percentage from total mass flow rate). i will calculate the collection efficiency. Now i calculated each and every particle dia. collection efficiency. now i going to analyze by injecting all particles dia. by rosin rammler. it will ask for only total mass flow rate of the particles. How it will take( that this particle dia. is x mass flow rate) .(i.e. fluent is asking only total mass flow rate not individual particle mass flow rate.) How to specify individual mass flow rate in rosin rammler model. And one more thing. how to post process the particle fate on the particular surface with particle dia. in that. Kindly help me please. im facing for long time.

 November 30, 2015, 05:23 #7 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 1,003 Rep Power: 19 It's ok; you specify the total mass flow rate, because when you specify the Rosin Rammler distribution you are specifying for every particles diameter also its fraction, so you don't need to specify the flowrates for each injection. __________________ Google is your friend and the same for the search button!

 November 30, 2015, 12:09 #8 New Member   senthur rajasekar Join Date: Nov 2014 Posts: 16 Rep Power: 5 okay.but how to post process the particle fate on the surface. 1. i need particle fate(escape, trap) on the surface along with particle diameter. 2. iam getting only total particle fate when i use summary not in particular surface( it is showing for full domain), how to get for particular surface. 3.And also how to find the particle fate for particular diameter on the surface. Thanks for replying.

 November 30, 2015, 12:45 #9 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 1,003 Rep Power: 19 Try to activate "sample" at reports-->discrete phase-->sample. Select the boundary(ies) and the release from injections. Then click on start and go on with calculation. In the working folder new .dpm files will be created. Let us know if this solves your problem. __________________ Google is your friend and the same for the search button!

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Lcw FLUENT 5 February 22, 2012 02:40 nagi FLUENT 6 March 6, 2011 20:59 jason FLUENT 4 November 12, 2007 04:15 fpingqian FLUENT 3 September 27, 2004 04:35 Vikky Main CFD Forum 1 June 29, 2003 06:05

All times are GMT -4. The time now is 19:03.

 Contact Us - CFD Online - Privacy Statement - Top