[prohackrav]

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.

[A CFD free user]

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

[prohackrav]

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]

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.

[A CFD free user]

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.

[ghost82]

Originally Posted by prohackrav

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

[A CFD free user]

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.