# Transient boundary condition with Fluent ANSYS12

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

June 30, 2011, 12:10
Transient boundary condition with Fluent ANSYS12
#1
New Member

djan
Join Date: Jun 2011
Posts: 10
Rep Power: 7
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

 June 30, 2011, 12:23 #2 Senior Member   Micael Boulet Join Date: Mar 2009 Location: Quebec, Canada Posts: 112 Rep Power: 11 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.

 June 30, 2011, 12:40 #3 New Member   djan Join Date: Jun 2011 Posts: 10 Rep Power: 7 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?

 June 30, 2011, 13:02 #4 Senior Member   Micael Boulet Join Date: Mar 2009 Location: Quebec, Canada Posts: 112 Rep Power: 11 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post jiejie OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 1 April 5, 2011 03:36 winnawinna FLUENT 0 December 29, 2010 00:32 bearcharge Main CFD Forum 0 May 14, 2010 11:32 geryes FLUENT 0 February 25, 2010 17:32 Mark CFX 6 November 15, 2004 16:55

All times are GMT -4. The time now is 02:31.