|
[Sponsors] |
May 31, 2012, 08:15 |
transient profile-time step
|
#1 |
Senior Member
Join Date: Feb 2011
Posts: 140
Rep Power: 15 |
Dear all,
I have got a question concerning the time of my transient boundary profile. I want the velocity of my simulation to vary in time and wrote a profile that looks like this: ((profile transient 3 0) (time 0 1 2 ) (velocity 2 6 3) ) When I import this profile to FLUENT I can pick the velocity as b.c. at the inlet. But what is about the time? Can I pick it somewhere else too? Or is the selected time step size used for the velocity variation? I couldn't find this at the FLUENT manual. Does somebody know, where I can find it? Thank you for all your help! Lilly |
|
May 31, 2012, 09:06 |
|
#2 |
Senior Member
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26 |
The profile you wrote is represented in the attached picture.
If you use a profile you are performing a transient simulation, so choose an appropriate time step in the "Run" window, considering your profile. In other words "Or is the selected time step size used for the velocity variation?" this is true. If you want to change the profile other than linear you have to interpret/compile an udf. Daniele |
|
May 31, 2012, 09:51 |
|
#3 |
Senior Member
Join Date: Feb 2011
Posts: 140
Rep Power: 15 |
Thank you, ghost82,
the values of my velocity profile were just picked as an example . But that means (in case of that example), if I would use a time step size of 0.1 s,the new time axis of my velocity profile would be 0,0.1,0.2,...Have I got that right? Thank you for your help! Lilly |
|
May 31, 2012, 11:46 |
|
#4 |
Senior Member
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26 |
Lilly, take this as an example:
you want a profile as velocity=time This means at t=0 s, v=0 m/s; t=1 s, v=1 m/s and so on.. You want to study the system from t=0 till t=10 s. Your profile will be of 2 points: 0;0 and 10;10 (time;velocity) Fluent interprets this profile as a linear profile. Your time step will be for example of 1 s. So at t=0 fluent calculates v=0, at t=1 it calculates v=1 and so on (because profile are always linear between 2 points). This 2 points profile is EQUAL for example to this 4 points profile: 0;0 2;2 6;6 10;10 (time;velocity): this is the same as the 2 points profile. Your profile file has to include points when the slope of your profile changes: for example if your velocity is 0 m/s at t=0s, increases linearly till 10 s, reaching a velocity of 3 m/s, it maintains at 3 m/s till 15 s and then it decreases to 0 m/s at t=20 s your profile will be: 0;0 10;3 15;3 20;0 (time;velocity) You can see I include only points where slope of profile changes. Then you can choose the time step you want; fluent will calculate velocity value assuming a linear profile between 2 points. Hope now it's more clear. Daniele |
|
June 4, 2012, 06:33 |
|
#5 |
Senior Member
Join Date: Feb 2011
Posts: 140
Rep Power: 15 |
Hi Daniele,
thanks a million for your detailed explanation! I got it now! Lilly |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Problem with FloatingObject | Leech | OpenFOAM Running, Solving & CFD | 10 | March 29, 2012 15:24 |
Full pipe 3D using icoFoam | cyberbrain | OpenFOAM | 4 | March 16, 2011 09:20 |
time step changes with velocity in transient simulations | sandisk | FLUENT | 1 | February 6, 2011 10:56 |
DPM UDF particle position using the macro P_POS(p)[i] | dm2747 | FLUENT | 0 | April 17, 2009 01:29 |
Could anybody help me see this error and give help | liugx212 | OpenFOAM Running, Solving & CFD | 3 | January 4, 2006 18:07 |