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

Cyclone Pressure Drop Too low

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 20, 2020, 16:16
Default Cyclone Pressure Drop Too low
  #1
New Member
 
CFDSim72
Join Date: Apr 2020
Posts: 17
Rep Power: 6
sirsammie72 is on a distinguished road
Hello,
I am simulating a cyclone separator and trying to match theoretical pressure drop values and achieve mesh independence - using Ansys Fluent.

I am using the static pressure value under volume integral to compute pressure drop in CFD.

The theoretical pressure drop for this cyclone is calculated to be 100 Pa. However, the CFD pressure drop is consistently around 10 Pa with any mesh size. I have double-checked units.

I have checked air flow properties, gravity, etc. The outlet velocity of the cyclone matches the theoretical predictions. It is just pressure drop that is off. Any thoughts on why this could be?

Thanks
sirsammie72 is offline   Reply With Quote

Old   August 20, 2020, 16:49
Default
  #2
Senior Member
 
karachun's Avatar
 
Join Date: Nov 2015
Posts: 244
Rep Power: 11
karachun is on a distinguished road
Pressure Drop is difference in Total Pressures, not Static Pressure.
karachun is offline   Reply With Quote

Old   August 20, 2020, 17:14
Default
  #3
New Member
 
CFDSim72
Join Date: Apr 2020
Posts: 17
Rep Power: 6
sirsammie72 is on a distinguished road
I have revised my method and am now taking the difference in pressure at surface of inlet and outlet, using total pressure. However, the value is still quite low.
sirsammie72 is offline   Reply With Quote

Old   August 20, 2020, 19:47
Default
  #4
Senior Member
 
karachun's Avatar
 
Join Date: Nov 2015
Posts: 244
Rep Power: 11
karachun is on a distinguished road
Do you perform mesh independence study?
karachun is offline   Reply With Quote

Old   August 21, 2020, 04:35
Default
  #5
jsm
Senior Member
 
JSM
Join Date: Mar 2009
Location: India
Posts: 192
Rep Power: 20
jsm is on a distinguished road
Hello,

Cyclone separator is somewhat unique to solve and get the accurate results.

Can you answer following questions.

Is your mesh is hexa or tetra?
How much have you refined your mesh nearer to wall & inner core of cyclone separator?
Which turbulence model are you using?
Have you extended the pressure inlet & outlet sufficient length to avoid back flow effect?

Please let me know your answer for these questions and post geometry image if possible for better understanding.
__________________
With regards,
JSM
jsm is offline   Reply With Quote

Old   August 21, 2020, 17:39
Default
  #6
New Member
 
CFDSim72
Join Date: Apr 2020
Posts: 17
Rep Power: 6
sirsammie72 is on a distinguished road
Hello, thank you for your response.

Mesh is tetra. We have not refined the mesh more near the wall and inner core, just mostly around the inlet. We are using RSM, and have enabled prevention of back-flow at the inlet.

Any tips for convergence with a finer mesh? We cannot reach convergence with fine mesh even with very small time step
sirsammie72 is offline   Reply With Quote

Old   August 22, 2020, 07:56
Default
  #7
jsm
Senior Member
 
JSM
Join Date: Mar 2009
Location: India
Posts: 192
Rep Power: 20
jsm is on a distinguished road
Tetra mesh is NOT good choice for RSM model. It will give very poor convergence.
Remember that RSM model solves six Reynolds's stress equation for each stress tensor. As tetra mesh is not single direction oriented, it will create unnecessary artificial diffusion and mislead the solution.

I would recommend to do hexa mesh with highly refined boundary layers nearer to wall and refined core region of cyclone separator. Y+ should be close to one. As RSM turbulence model doesn't like variation in mesh size, keep very less mesh growth rate for better convergence.
__________________
With regards,
JSM
jsm is offline   Reply With Quote

Reply

Tags
cyclone, cyclone separator, fluent, pressure drop, static pressure

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
Total pressure drop & static pressure drop Aarthar Main CFD Forum 3 April 11, 2018 03:32
Fluent cyclone pressure drop mkal FLUENT 4 February 5, 2018 13:05
How to study pressure drop of continous phase in VOF model sajeesh FLUENT 4 February 5, 2014 22:01
Pressure drop in cyclone separators. arjun3020 FLUENT 2 February 25, 2012 09:25
Pipe Flow - Pressure Drop Daniel L FLOW-3D 2 December 10, 2010 04:23


All times are GMT -4. The time now is 23:26.