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.

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]

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..

[ghost82]

Inject your particles, then save or print to console escaped and trapped particles and mass flows and calculate from these data collection efficiencies.

Daniele

[arjun3020]

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.

[senthur]

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.

[ghost82]

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.

[senthur]

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.

[ghost82]

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.