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

Transient boundary condition with Fluent ANSYS12

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 30, 2011, 12:10
Default Transient boundary condition with Fluent ANSYS12
  #1
New Member
 
djan
Join Date: Jun 2011
Posts: 10
Rep Power: 6
jetboo is on a distinguished road
hi everyone, i need to set a transient boundary condition for a pressure outlet.

I want it to decrease linearly from 160000 Pa to 60000 in 0.2 secs

With StarCCM+ i use this field function
Quote:
($Time >= 0.2) ? -40000 : (60000-500000*$Time)
(the values are relatives to atmospheric pressure)

With fluent, i tried the profiles like stated in the manual (chapter7.1.9) but it doesnt seem to work. How can i do this either way ??

thx
Djan
jetboo is offline   Reply With Quote

Old   June 30, 2011, 12:23
Default
  #2
Member
 
Micael Boulet
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 95
Rep Power: 9
Micael is on a distinguished road
I think the best way to do this is with an UDF. Something like that:
Code:
 
DEFINE_PROFILE(outlet_pressure,t,i)
{
 real pressure;
 face_t f;
 pressure = (CURRENT_TIME >= 0.2) ? -40000 : (60000-500000*CURRENT_TIME);
 
 begin_f_loop(f,t)
   {
   F_PROFILE(f,t,i) = pressure;
   }
 end_f_loop(f,t)
}
Also, keep in mind that FLUENT solver normally expect that outlet pressure is gauge pressure.
Micael is offline   Reply With Quote

Old   June 30, 2011, 12:40
Default
  #3
New Member
 
djan
Join Date: Jun 2011
Posts: 10
Rep Power: 6
jetboo is on a distinguished road
wow thank you,i didnt expect an answer so quickly i am really a novice in C so i dont get all of

what you wrote there but it seems to work so it's GREAT !

Can you explain the
Code:
face_t f;
line plz?
jetboo is offline   Reply With Quote

Old   June 30, 2011, 13:02
Default
  #4
Member
 
Micael Boulet
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 95
Rep Power: 9
Micael is on a distinguished road
face_t is a data type specific to FLUENT. It is used to store an integer that identifies a particular face within a face thread (a boundary is a face thread). The macro begin_f_loop need it to work. Actually, begin_f_loop will give a value to the variable "f" that represents the current face under calculation. This value change at each loop. There is a lot of macro that use this value to give useful information about the given face, like its area or its temperature, as examples.
Micael 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
icem fluent mesh with cyclic boundary condition jiejie OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 1 April 5, 2011 03:36
problem about periodic boundary condition in Fluent winnawinna FLUENT 0 December 29, 2010 00:32
vorticity boundary condition bearcharge Main CFD Forum 0 May 14, 2010 11:32
How to use a solution as an inlet boundary condition in another problem in fluent geryes FLUENT 0 February 25, 2010 17:32
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 06:06.