CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Transient boundary condition with Fluent ANSYS12 (http://www.cfd-online.com/Forums/fluent/90103-transient-boundary-condition-fluent-ansys12.html)

 jetboo June 30, 2011 12:10

Transient boundary condition with Fluent ANSYS12

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

 Micael June 30, 2011 12:23

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.

 jetboo June 30, 2011 12:40

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 ! :D

Can you explain the
Code:

`face_t f;`
line plz?

 Micael June 30, 2011 13:02

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.

 All times are GMT -4. The time now is 18:48.