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

transient profile-time step

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 31, 2012, 08:15
Default transient profile-time step
  #1
Senior Member
 
Join Date: Feb 2011
Posts: 128
Rep Power: 6
Lilly is on a distinguished road
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
Lilly is offline   Reply With Quote

Old   May 31, 2012, 09:06
Default
  #2
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
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
Attached Images
File Type: png profile.png (10.3 KB, 16 views)
ghost82 is offline   Reply With Quote

Old   May 31, 2012, 09:51
Default
  #3
Senior Member
 
Join Date: Feb 2011
Posts: 128
Rep Power: 6
Lilly is on a distinguished road
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
Lilly is offline   Reply With Quote

Old   May 31, 2012, 11:46
Default
  #4
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
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
ghost82 is offline   Reply With Quote

Old   June 4, 2012, 06:33
Default
  #5
Senior Member
 
Join Date: Feb 2011
Posts: 128
Rep Power: 6
Lilly is on a distinguished road
Hi Daniele,

thanks a million for your detailed explanation!
I got it now!

Lilly
Lilly 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
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 10:20
time step changes with velocity in transient simulations sandisk FLUENT 1 February 6, 2011 11:56
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 19:07


All times are GMT -4. The time now is 09:46.