CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Cyclone analysis

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 6, 2018, 14:30
Default Cyclone analysis
  #1
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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 .
mkal is offline   Reply With Quote

Old   February 6, 2018, 15:28
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27
Gert-Jan will become famous soon enough
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.......
Gert-Jan is offline   Reply With Quote

Old   February 6, 2018, 16:25
Default
  #3
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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?
mkal is offline   Reply With Quote

Old   February 6, 2018, 16:35
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27
Gert-Jan will become famous soon enough
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.
Gert-Jan is offline   Reply With Quote

Old   February 6, 2018, 17:18
Default
  #5
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
I calculate from the formula (velocity=flow/area) . CFX is calculating more than this formula.
mkal is offline   Reply With Quote

Old   February 6, 2018, 17:26
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27
Gert-Jan will become famous soon enough
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?
Gert-Jan is offline   Reply With Quote

Old   February 7, 2018, 10:41
Default
  #7
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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 is offline   Reply With Quote

Old   February 7, 2018, 16:10
Default
  #8
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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 ?
mkal is offline   Reply With Quote

Old   February 7, 2018, 17:03
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is online now   Reply With Quote

Old   February 8, 2018, 10:39
Default
  #10
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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?
mkal is offline   Reply With Quote

Old   February 8, 2018, 10:56
Default
  #11
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27
Gert-Jan will become famous soon enough
what turbulence model are your using?
Gert-Jan is offline   Reply With Quote

Old   February 8, 2018, 11:36
Default
  #12
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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.
mkal is offline   Reply With Quote

Old   February 8, 2018, 11:54
Default
  #13
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27
Gert-Jan will become famous soon enough
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
Gert-Jan is offline   Reply With Quote

Old   February 8, 2018, 12:56
Default
  #14
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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.
mkal is offline   Reply With Quote

Old   February 8, 2018, 13:10
Default
  #15
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,835
Rep Power: 27
Gert-Jan will become famous soon enough
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.
Gert-Jan is offline   Reply With Quote

Old   February 8, 2018, 14:35
Default
  #16
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
thank you . are there any experimental data books you can recommend?
mkal is offline   Reply With Quote

Old   February 28, 2018, 16:34
Default
  #17
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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 .
mkal is offline   Reply With Quote

Old   February 28, 2018, 17:25
Default
  #18
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is online now   Reply With Quote

Old   March 1, 2018, 13:25
Default
  #19
Member
 
Join Date: Oct 2016
Posts: 31
Rep Power: 9
mkal is on a distinguished road
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).
mkal is offline   Reply With Quote

Old   March 1, 2018, 16:40
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,729
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is online now   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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 GŁnther Hasse Main CFD Forum 3 October 12, 1999 19:34


All times are GMT -4. The time now is 05:02.