
[Sponsors] 
February 6, 2018, 14:30 
Cyclone analysis

#1 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
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 . 

February 6, 2018, 15:28 

#2 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27 
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....... 

February 6, 2018, 16:25 

#3 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
Thank you for your reply. I get about %1520 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?


February 6, 2018, 16:35 

#4 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27 
What formula? Your own? A CFXfomula? 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)@inletmassFlowAve(Total Pressure)@outle. 

February 6, 2018, 17:18 

#5 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
I calculate from the formula (velocity=flow/area) . CFX is calculating more than this formula.


February 6, 2018, 17:26 

#6 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27 
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? 

February 7, 2018, 10:41 

#7 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
Mr. GertJan, 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.


February 7, 2018, 16:10 

#8 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
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 ?


February 7, 2018, 17:03 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143 
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

February 8, 2018, 10:39 

#10 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
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? 

February 8, 2018, 10:56 

#11 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27 
what turbulence model are your using?


February 8, 2018, 11:36 

#12 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
I am using RNG kEpsilon 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.


February 8, 2018, 11:54 

#13 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27 
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, GertJan 

February 8, 2018, 12:56 

#14 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
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.


February 8, 2018, 13:10 

#15 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27 
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. 

February 8, 2018, 14:35 

#16 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
thank you . are there any experimental data books you can recommend?


February 28, 2018, 16:34 

#17 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
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 .


February 28, 2018, 17:25 

#18 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143 
Please define cyclone efficiency and what you mean by "trap".
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

March 1, 2018, 13:25 

#19 
Member
Join Date: Oct 2016
Posts: 31
Rep Power: 9 
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).


March 1, 2018, 16:40 

#20 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143 
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).
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ANSYS WORKBENCH Transfer result of one analysis to a new analysis as preload  ingjuanm90  ANSYS  0  July 26, 2016 14:04 
cyclone analysis error  arjun3020  FLUENT  4  May 15, 2014 01:05 
Convergence of Cyclone Analysis  arjun3020  FLUENT  5  April 25, 2012 01:50 
Cyclone analysis  subramaniam.CR  CFX  1  March 5, 2005 10:22 
Modelling Industrial cyclone behaviour  Günther Hasse  Main CFD Forum  3  October 12, 1999 19:34 