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

How to choose hydraulic diameter for Flow through expansion pipe in Ansys Fluent

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

Like Tree1Likes
  • 1 Post By vinerm

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 26, 2020, 01:42
Default How to choose hydraulic diameter for Flow through expansion pipe in Ansys Fluent
  #1
New Member
 
Naveen
Join Date: Mar 2020
Posts: 2
Rep Power: 0
Naveenjanj is on a distinguished road
I am trying to solve Ansys Verification Manual number 28 using
Fluent 2D Axisymmetric option.

The title is “Flow and Heat Transfer Over Expansion Pipe”

In this manual I am having doubt as how to choose Hydraulic diameter for inlet and outlet boundary condition.

What should be the inlet boundary condition?
Outlet boundary condition??

Could anyone tell me the correct b/c ?
Attached Images
File Type: jpg Flow Domain.JPG (17.6 KB, 6 views)
File Type: jpg Material prop & BC.JPG (48.3 KB, 5 views)
File Type: jpg Result.JPG (37.5 KB, 4 views)

Last edited by Naveenjanj; March 26, 2020 at 02:46.
Naveenjanj is offline   Reply With Quote

Old   March 26, 2020, 03:58
Default Hydraulic Diameter
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
Since the problem is axisymmetric, actual diameter at the inlet is the hydraulic diameter; same is true for the outlet.

As far as outlet is concerned, pressure outlet is alright. However, for the inlet, you have to develop a profile and use that. You need to run a case with only inlet duct (no expanded portion) and then extract a fully-developed velocity profile from there. Then apply that profile in this simulation.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared on the Forum
vinerm is offline   Reply With Quote

Old   March 26, 2020, 04:31
Default
  #3
New Member
 
Naveen
Join Date: Mar 2020
Posts: 2
Rep Power: 0
Naveenjanj is on a distinguished road
Quote:
Originally Posted by vinerm View Post
Since the problem is axisymmetric, actual diameter at the inlet is the hydraulic diameter; same is true for the outlet.



As far as outlet is concerned, pressure outlet is alright. However, for the inlet, you have to develop a profile and use that. You need to run a case with only inlet duct (no expanded portion) and then extract a fully-developed velocity profile from there. Then apply that profile in this simulation.


Hi,

May I know how to extract a fully-developed velocity profile. Could you please elaborate.
Naveenjanj is offline   Reply With Quote

Old   March 26, 2020, 04:53
Default Profile
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
There are two options. One is to create a pipe with diameter of your first pipe. Ensure that it is long enough so that the profile gets developed. Run the case with the specified velocity inlet and pressure outlet. After the simulation has converged, write profile using File > Write > Profile > Define New Profile at the outlet for all three velocity components.

Another option is to create a pipe with the diameter of the first pipe, however, the length can be just a few mm or cm. Ensure that there are at least 5-6 cells across length. Then setup inlet and outlet as translational periodic boundaries. Apply periodic settings and assign either flow rate or pressure drop. Run the simulation. Once done, extract profile at either of the boundaries. This option is more sophisticated but you need to know Fluent little more than you may know at this stage. So, you may use first option.
Naveenjanj likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared on the Forum
vinerm is offline   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
looking for a smart interface matlab fluent chary FLUENT 20 November 6, 2017 09:12
Running UDF with Supercomputer roi247 FLUENT 4 October 15, 2015 13:41
Help me to choose between Ansys Meshing, Fluent Meshing or ICEM ? pipolaki ANSYS 0 December 6, 2013 08:12
The fluent stopped and errors with "Emergency: received SIGHUP signal" yuyuxuan FLUENT 0 December 3, 2013 22:56
[GAMBIT] hydraulic diameter? Zweeper ANSYS Meshing & Geometry 6 January 4, 2010 00:44


All times are GMT -4. The time now is 01:18.