[mkal]

Hello friends.
I'm doing cyclone analysis. If the mass flow rate equals both inlet and outlet, Cfx and Fluent calculate the outlet velocity and dynamic pressure too high. In the analysis I made on the conical pipe, while calculating the output velocity correctly, it incorrectly calculates the outlet velocity in the cyclone analysis. Am I doing something wrong? How does Cfx calculate cyclone outlet velocity ? Thank you .

[Gert-Jan]

What makes you think both CFX and Fluent (or Post) calculate a too high velocity? Do you compare it with experiments? is the maximum too high? Or the average? What is wrong exactly?
Because, if you have performed a succesfull CFX calculation, you will have an output file. There the mass imbalance after the calculation is given. If the imbalance is (almost) zero, then the velocities on the outlets will be correct. Period.

Also the velocity can be too high, if you have a recirculation in the outlet, or walls on the outlet, or density is not as constant as your think, or whatever.......

[mkal]

Thank you for your reply. I get about %15-20 more than the calculated value according to the formula . There is no wall on exit and the density is constant. what else could be wrong? The static pressure drop gives reasonable results, but how can I calculate the total pressure drop?

[Gert-Jan]

What formula? Your own? A CFX-fomula? Please be more specific.

As mentioned, if CFX has a mass imbalance of zero, and density is constant, then the velocity is as it is. If it is not what you expect, then your surface areas are incorrect, or your formula is incorrect.

Determining pressure drop is a matter of taste and definition. I always take massFlowAve(Total Pressure)@inlet-massFlowAve(Total Pressure)@outle.

[mkal]

I calculate from the formula (velocity=flow/area) . CFX is calculating more than this formula.

[Gert-Jan]

For these basic calculations CFX won't make a mistake. If everything is correct, I even trust CFX more than my own hand calculations.

So trust me, something is wrong in your setup, approach, mass imbalance, formula, whatsoever........

You mentioned cyclone. This has 1 inlet, and two outlets. Did you take both outlets into account?

[mkal]

Mr. Gert-Jan, thank you so much for your reply. I just calculate the pressure drop. So I set the cyclone as 1 input and 1 output. I set the boundary condition of dustbin outlet as wall.

[mkal]

I noticed something in my analysis today. As the number mesh decreases, the output velocity increases . the finer weave is approaching the calculated value according to the outlet velocity formula . is this normal ?

[ghorrocks]

If you are saying that as you refine the mesh the simulation result gets more accurate - yes, this is normal. In fact this is important to do so you can show you have an accurate simulation.

[mkal]

Thank you Glenn Horrocks.
I am analyzing the cyclone at https://www.sciencedirect.com/scienc...07904X10004178. the difference between the number of 490,000 cells and the number of 1,174,000 cells in the book is around 3%. In my analysis, the output velocity is 6.1 m / s at 250,000 cells, 5.5 m / s at 490,000 cells, and 4.9 m / s at 750,000 cells. The velocity that should be according to the formula is 4.4 m / s. I thought I should not be so different . Is there a reliable book you can recommend?

[Gert-Jan]

what turbulence model are your using?

[mkal]

I am using RNG k-Epsilon because I have RSM convergence problem. I do the same cyclone fluent and CFX. The outlet velocity is the same in both. Pressure drop in CFX is better for coarse mesh.

[Gert-Jan]

We can only help in general ways.
- if you say I have 250.000 elements, that doesn't help. It all depends on what mesh, boundary elements, etc.
- Cyclones need to be analysed using RSM. Period. (unless it is laminar).
- Fluent has more turbulence models. You could try that. Convert your tet mesh to a polyhedral mesh, use the coupled scheme with Pseudo Transient analyses.Then it is like CFX. But still not as stable (by far).
- Cyclones are standard and popular applications for CFD. But they have very difficult behaviour. It can be a real pain in the "....".
- The vortex core will become unstable (precessing). So a transient analysis will be needed with time averaging results.

Good luck. Keep fingers crossed.

Regs, Gert-Jan

[mkal]

Thank you for taking the time to write an answer. I use a hexahedral mesh from ICEM CFD. The mesh quality is bad due to the tangential coupling of the input to the cylinder. Now I am going to try and increase the quality by using a Quad dominant mesh at the entrance. I start with Steady with Fluent de RSM and then converge to transiet. But the convergence of the CFX RSM is very difficult.

[Gert-Jan]

In transient, RSM should converge, if time steps are not too large.
In steady state it is harder. Reduce time scale from 1 to below 0.3.

[mkal]

thank you . are there any experimental data books you can recommend?

[mkal]

I calculate cyclone pressure drop and efficiency with Fluent in accordance with the experimental data. I calculate the pressure drop of the same cyclone with CFX according to the experimental data. But I do not know how CFX will calculate cyclone efficiency. Should I use the track transport solid feature? How do I set the trap feature? I have not found a CFX trap feature anywhere. It works well when I set the Fluent wall trap. What could be the most suitable boundary for cfx trap? Where can I learn how many pieces fall into the trap and how many pieces are missing? I am using total pressure input and mass flow output. Thank you .

[ghorrocks]

Please define cyclone efficiency and what you mean by "trap".

[mkal]

I inject parts with the track transport solid model from the cyclone inlet. I want to calculate cyclone efficiency = trap / escape formula. But I do not know where boundary features are made (escape, trap , reflect).

[ghorrocks]

The normal way of looking at particle trap efficiency is number of trapped particles/total number of particles. Is this what you mean?

Regarding your second question on boundary features - this is basic CFX operations and is covered by the CFX tutorials. You can get them from the ANSYS Customer webpage (or the student portal if you are a student).