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

Repeating boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 6, 2010, 17:06
Default Repeating boundary condition
  #1
New Member
 
Join Date: Jan 2010
Posts: 3
Rep Power: 6
Marco83 is on a distinguished road
Hi all,

I would like to know how to set up a repeating boundary condition in CFX. To understand my problem, you can imagine to have a geometry with one inlet and one outlet. This geometry is an elementary cell that gets repeated an ungodly large number of times in reality.

My goal is to set inlet and outlet pressures and require the velocity profiles at the inlet and outlet to be identical.

The tedious way of doing it is to set an arbitrary inlet, solve, take the outlet and use it as the inlet over and over again. Since I have to run 100+ simulations varying a few parameters, doing it manually is not exactly an option.

Any suggestion?
Marco83 is offline   Reply With Quote

Old   January 6, 2010, 18:27
Default
  #2
Member
 
Tristan Burton
Join Date: Mar 2009
Posts: 43
Rep Power: 7
Tristan is on a distinguished road
So you want a periodic boundary condition, right?

Tristan
Tristan is offline   Reply With Quote

Old   January 7, 2010, 08:14
Default
  #3
New Member
 
Join Date: Jan 2010
Posts: 3
Rep Power: 6
Marco83 is on a distinguished road
I am not sure if a repeating boundary condition is exactly what I am looking for (I mean it; I am not too familiar with this type of BC and I may be missing the right way to use it).

I still want a pressure gradient between inlet and outlet, but the velocity profile has to be the same.

How would you implement this condition in CFX?
Marco83 is offline   Reply With Quote

Old   January 7, 2010, 08:19
Default
  #4
Senior Member
 
Join Date: Jul 2009
Posts: 206
Rep Power: 8
kingjewel1 is on a distinguished road
If you're wanting the same profiles, set your inlet in CEL or otherwise... and then set your outlet by CEL to be the same as your inlet:
eg you want your inlet profile to be x^2-3/2x+9, then you can make this a CEL function and attatch it to the outlet too.
or in my experience i set inlet to be velocity and then do outlet:=ave(Velocity)@Inlet
kingjewel1 is offline   Reply With Quote

Old   January 7, 2010, 08:33
Default
  #5
New Member
 
Join Date: Jan 2010
Posts: 3
Rep Power: 6
Marco83 is on a distinguished road
The point is that I don't know the shape of the velocity profile. If I were to code this problem, I would use an iterative approach, setting an arbitrary inlet profile, getting an outlet profile and feeding it back at the inlet over and over, until the difference between the two becomes small enough.
Marco83 is offline   Reply With Quote

Old   January 7, 2010, 16:58
Default
  #6
Member
 
Tristan Burton
Join Date: Mar 2009
Posts: 43
Rep Power: 7
Tristan is on a distinguished road
For fully developed turbulent channel flow simulations, they use periodic boundary conditions at the inlet and outlet. Since the pressure can't be periodic (it drops along the channel) they add a source term to the streamwise momentum equation to include the non-periodic part of the pressure and the solver is therefore only finding the periodic part of the pressure. So your source term is something like -(Pout-Pin)/L and the inlet/outlet velocity profiles will adjust together since you have a periodic boundary condition. Your "true" pressure is the solver computed perdiodic part plus a linearly decaying (Pin at inlet, Pout at outlet) non-periodic part.

Tristan
Tristan 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
Boundary Conditions Thomas P. Abraham Main CFD Forum 20 July 7, 2013 05:05
Transient outlet boundary condition problem jwillie2000 CFX 1 December 7, 2009 17:07
Axis Boundary Condition..what is it? CFDtoy FLUENT 6 February 13, 2007 05:51
How to set boundary condition in Fluent for the fo Peiyong FLUENT 1 November 10, 2006 11:44
How to resolve boundary condition problem? sam FLUENT 2 July 20, 2003 02:19


All times are GMT -4. The time now is 00:02.