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

Turbulent flow in duct

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 12, 2014, 00:51
Default Turbulent flow in duct
  #1
Member
 
Anonymous
Join Date: Mar 2014
Posts: 73
Rep Power: 4
marauder is on a distinguished road
I'm trying to simulate turbulent flow in a straight rectangular duct and calculate the pressure loss. I've created a wall biased mesh and I'm setting up all properties, default k-epsilon model and the relevant boundary conditions. For wall roughness I'm using the same mentioned in the experiment. But pressure loss I'm getting from fluent is much higher than the experimental values.

Can anybody explain what is it that is wrong with my approach or should I change any values so as to match my experimental values??

Thanks.
marauder is offline   Reply With Quote

Old   September 12, 2014, 10:17
Default
  #2
Member
 
Sangwoo Kim
Join Date: Jul 2014
Location: Seoul, South Korea
Posts: 98
Rep Power: 4
swtbkim is on a distinguished road
Did you check the quality of grid? the number of grids(mesh independence test), inflation layer, y+ issue, and so on

Did you consider flow development?

What is the fluid? air or water or else?
If air, did you consider Mach number?
swtbkim is offline   Reply With Quote

Old   September 12, 2014, 11:51
Default
  #3
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,305
Rep Power: 22
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Just guessing here because there isnt really much information, but usually people asking this question ignored that the experimental values were obtained for fully developed flows.
So the first thing you need to check is if the boundary conditions you used in your simulation represent the experimental setup accurately.
flotus1 is offline   Reply With Quote

Old   September 12, 2014, 16:45
Default
  #4
Member
 
Virendrasingh Pawar
Join Date: Jun 2013
Posts: 47
Rep Power: 5
virendra_p is on a distinguished road
Bc's can be accurately matched in this case so won't affect results much (unless input incorrect)..choice of turbulence model and mesh resolution will play an imp. role...use integral model (kw-sst) over wall function ke model. This way you will capture both near wall viscous effects and core turbulence further. If possible use structured o- grid for better control and quality. Grid y+~1 with 10 nodes upto y+~30 will resolve the near wall viscous region and relatively coarser mesh in core is sufficient...hopefully this improve your results...good luck!
virendra_p is offline   Reply With Quote

Old   October 1, 2014, 11:05
Default
  #5
Member
 
Anonymous
Join Date: Mar 2014
Posts: 73
Rep Power: 4
marauder is on a distinguished road
Sorry guys for coming back after these many days as I was busy with my course work. I was doing this simulation to study more into turbulence modelling in Fluent. Unfortunately my theoretical knowledge in CFD is very limited as I still have to take a course on that. Mostly I learn from internet.

Coming to the problem, yes I've considered flow development, grid dependence, and I'm using structured O grid, I've calculated the y+ value but I was unable to get the minimum height of cell near the wall to the value I desired as I was unable to get that thickness in Ansys mesh (showing some error! ). So I generated the mesh with minimum possible height it could generate near the wall. But anyways I'm guessing even if I end up with the required cell height at wall my pressure drop will further increase as this will allow fluent to consider the wall rougness. Is this right?

Also, I've seen some people who would generate a simple tet mesh and calculate the pressure drops in turbulent flows without considering y+ value. Is this correct??
Is there any turbulence model which would consider wall roughness with normal mesh without the need for finer mesh near wall?
marauder is offline   Reply With Quote

Old   October 1, 2014, 11:45
Default
  #6
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,305
Rep Power: 22
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Here is the thing with turbulence modeling and wall roughness:

As long as you use a wall-function approach and have y+ values in the range of 30-100 you can model the influence of a wall roughness with some empirical model.

But if you use a wall-resolving approach with y+ values in the order of 1 or below, things chance...
An y+ value of 1 means that the first cell is within the viscous sublayer which extends to about y+=5. But as you learned in fluid mechanics, a wall can be considered hydrodynamically smooth if the roughness height is within the viscous sublayer.
So if there was any influence from a wall roughness, the roughness height would have to be larger than the cell sizes, which basically means that you would have to simulate the roughness directly, using a geometrically rough wall.
flotus1 is offline   Reply With Quote

Old   October 2, 2014, 10:35
Default
  #7
Senior Member
 
Join Date: Mar 2014
Posts: 367
Rep Power: 5
hwet is on a distinguished road
regarding the meshing, tet mesh at the wall will be no good, having an inflation layer is compulsory (quoting a cfd expert with 30+ years exp), y+ you can check after the simulation from the contours generated and see if they fall in the desired limit. for the wall losses you will have to give more inputs at the wall boundaries depending on your setup's physics
hwet is offline   Reply With Quote

Old   October 2, 2014, 14:10
Default
  #8
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 613
Blog Entries: 17
Rep Power: 20
sbaffini will become famous soon enough
My guess is that the whole point is in:

"I've created a wall biased mesh "

Could you explain it further? What did you mean with it?
sbaffini is offline   Reply With Quote

Old   October 3, 2014, 01:07
Default
  #9
Member
 
Anonymous
Join Date: Mar 2014
Posts: 73
Rep Power: 4
marauder is on a distinguished road
Quote:
Originally Posted by sbaffini View Post
My guess is that the whole point is in:

"I've created a wall biased mesh "

Could you explain it further? What did you mean with it?
Sorry I just tried to explain it in ansys mesh terms where you use biasing to stack more cells near the edge or at the centre.
marauder is offline   Reply With Quote

Old   October 3, 2014, 04:56
Default
  #10
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 613
Blog Entries: 17
Rep Power: 20
sbaffini will become famous soon enough
Ok, my bad.
sbaffini is offline   Reply With Quote

Old   October 3, 2014, 15:36
Default
  #11
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 312
Rep Power: 7
JuPa is on a distinguished road
Quote:
Originally Posted by marauder View Post
I'm trying to simulate turbulent flow in a straight rectangular duct and calculate the pressure loss. I've created a wall biased mesh and I'm setting up all properties, default k-epsilon model and the relevant boundary conditions. For wall roughness I'm using the same mentioned in the experiment. But pressure loss I'm getting from fluent is much higher than the experimental values.

Can anybody explain what is it that is wrong with my approach or should I change any values so as to match my experimental values??

Thanks.

K Epsilon is notoriously bad at predicting anisotropic flows in rectangular ducts. Try an explicit algebraic Reynolds stress model.
JuPa is offline   Reply With Quote

Old   December 11, 2015, 08:18
Post
  #12
New Member
 
wangzhijun
Join Date: Aug 2013
Posts: 5
Rep Power: 5
QIAN06 is on a distinguished road
???could not understand
QIAN06 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Laminar Isothermal Flow in a duct HectorRedal Main CFD Forum 29 June 2, 2012 07:04
Turbulent Flow in a Square Duct using LES Hock Ming FLUENT 0 February 7, 2009 21:25
Turbulent flow in a rectangular duct foam vs fluent atzaru OpenFOAM Pre-Processing 7 February 13, 2007 15:42
Reynolds and Turbulent flow Frederic Dubinski CFX 5 October 21, 2004 04:12
Duct Flow omar Main CFD Forum 4 December 9, 1999 13:43


All times are GMT -4. The time now is 00:45.