CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLOW-3D

Time-step setting

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

Like Tree1Likes
  • 1 Post By JBurnham

Reply
 
LinkBack Thread Tools Display Modes
Old   December 18, 2013, 06:25
Default Time-step setting
  #1
New Member
 
tsung han yang
Join Date: Dec 2013
Posts: 12
Rep Power: 3
robin781105 is on a distinguished road
Dear all

I have a quick equation to ask.

How to set the "delta t" in the Flow-3D or if the model will automatically set during the simulation ?

Thanks all

by Robin
robin781105 is offline   Reply With Quote

Old   December 18, 2013, 21:34
Default
  #2
Senior Member
 
Jeff Burnham
Join Date: Apr 2010
Posts: 204
Rep Power: 8
JBurnham is on a distinguished road
It will automatically set delta t (dt), and dt can change throughout the simulation. The setting of dt depends on what physics models you have active, the velocity of the flow, and the cell size. You can also limit dt to a maximum value from the Model Setup > Numerics tab, but usually I just let FLOW-3D pick dt for me.
JBurnham is offline   Reply With Quote

Old   December 19, 2013, 07:45
Default
  #3
New Member
 
tsung han yang
Join Date: Dec 2013
Posts: 12
Rep Power: 3
robin781105 is on a distinguished road
Learn a new lesson, thank you Jeff.

Can I ask another question?
So, If we let the model automatically setting dt then we just need to change the cells size for simulation?
robin781105 is offline   Reply With Quote

Old   December 22, 2013, 03:01
Default
  #4
Senior Member
 
Jeff Burnham
Join Date: Apr 2010
Posts: 204
Rep Power: 8
JBurnham is on a distinguished road
Yes. The time step size will change when you change the cell size. Other things that affect the time step size are:

1) too many pressure iteration failures (check boundary conditions, initial conditions, mesh resolution and aspect ratio.stl files for correctness, and that gridlines match at mesh block interfaces).

2) sudden changes in flow direction, which may give a 'convective volume flux' error, which is harmless (the time step is just reduced and the cycle is run again).

3) splashing or droplets may reduce the time step because they have high velocity. You can remove flying droplets by setting FCLEAN = 0.01 to 0.05 in the Numerics tab, or set initial conditions so that fluid is not splashing on solid surfaces.
zhouyu3092070 likes this.
JBurnham is offline   Reply With Quote

Old   December 27, 2013, 01:21
Default
  #5
New Member
 
tsung han yang
Join Date: Dec 2013
Posts: 12
Rep Power: 3
robin781105 is on a distinguished road
Thanks Burnham

Can I ask a new question about time step?

I set my model's finish time at 100s and the simulation process is all fine, but when I change the finish time to 4500s then I got the "time step size < dtmin" problem at 400s(The time step setting is automatically), how does it mean? If I need to change the time-step size artificially?
robin781105 is offline   Reply With Quote

Old   December 31, 2013, 12:41
Default
  #6
Senior Member
 
Jeff Burnham
Join Date: Apr 2010
Posts: 204
Rep Power: 8
JBurnham is on a distinguished road
DTMIN is based on the finish time TWFIN. It's different in different versions, but for example it might be DTMIN = TWFIN/1000. You can check DTMIN value in Diagnostics > Preprocessor Summary (or file prpout.xxx). If DTMIN > 1E-6, I would set DTMIN = 1E-6 or 1E-7 for most hydraulics problems (and smaller for microfluidics).
JBurnham 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
Time step size and max iterations per time step pUl| FLUENT 31 August 21, 2015 04:46
Sudden jump in Courant number NJG OpenFOAM Running, Solving & CFD 7 May 15, 2014 13:52
Orifice Plate with a fully developed flow - Problems with convergence jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24
directMapped problem panda60 OpenFOAM Bugs 4 July 8, 2010 10:23
A Problem with setting the time step in VOF model Le FLUENT 2 July 20, 2006 22:00


All times are GMT -4. The time now is 19:13.