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

Time-step for Implicit Unsteady solver in STARCCM+ and maximum number of steps?

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 24, 2020, 07:12
Default Time-step for Implicit Unsteady solver in STARCCM+ and maximum number of steps?
  #1
Senior Member
 
MA
Join Date: Mar 2020
Posts: 162
Rep Power: 3
mazhar16823 is on a distinguished road
Hi,


I am working on the CFD simulation for a wind turbine blade. I chose Implicit Unsteady Solver for this purpose. I want to associate the time step with rotational speed of the blade I am unable to figure out how should I do this and what should be the max. physical time and maximum steps for the stopping criteria? Any comments please.
mazhar16823 is offline   Reply With Quote

Old   April 24, 2020, 12:42
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,389
Rep Power: 52
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Check the Courant number field. Make your physical time small enough to keep that Courant number in the single digits (e.g. <10) but large enough that you don't have enough time to forget about your CFD.


Max steps is however many you need for your solution to converge at each time-step. This you get by creating monitors and checking for convergence at every time-step.
LuckyTran is offline   Reply With Quote

Old   April 24, 2020, 12:50
Default
  #3
Senior Member
 
MA
Join Date: Mar 2020
Posts: 162
Rep Power: 3
mazhar16823 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
Check the Courant number field. Make your physical time small enough to keep that Courant number in the single digits (e.g. <10) but large enough that you don't have enough time to forget about your CFD.


Max steps is however many you need for your solution to converge at each time-step. This you get by creating monitors and checking for convergence at every time-step.



How would I know that that Courant is below 10 if I choose a physical time?
Also, I want to relate the time step with the rotational speed of the blade so that steadiness of the results is obtained.
mazhar16823 is offline   Reply With Quote

Old   April 24, 2020, 13:10
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,389
Rep Power: 52
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Well you can guess it. Either way, you pick a time. Run it for a few time-steps. Check the Courant number field. And then adjust it.


I don't know what time has to do with rotational speed. Velocity and time are different concepts.
LuckyTran is offline   Reply With Quote

Old   April 24, 2020, 13:16
Default
  #5
Senior Member
 
MA
Join Date: Mar 2020
Posts: 162
Rep Power: 3
mazhar16823 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
Well you can guess it. Either way, you pick a time. Run it for a few time-steps. Check the Courant number field. And then adjust it.


I don't know what time has to do with rotational speed. Velocity and time are different concepts.

I am talking about "Time Step'' for the Implicit Unsteady solver not the physical time. However, I am not clear about their difference.
mazhar16823 is offline   Reply With Quote

Old   April 24, 2020, 13:22
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,389
Rep Power: 52
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Sorry, there was a typo. I meant physical time-step size.

Physical time starts at 0s and accumulates time according to how long you have run your simulation, the time-step size and number of time-steps that have been run.

You set a time-step size according to Courant number.

The max physical time is a stop criterion for when the simulation ends. You pick this based on how long you want the CFD to run. If you want to simulate a wind turbine spinning for 1s, set it to 1s. If you want to see it spin for a year, set it to 31,536,000 seconds.
LuckyTran is offline   Reply With Quote

Old   April 24, 2020, 13:28
Default
  #7
Senior Member
 
MA
Join Date: Mar 2020
Posts: 162
Rep Power: 3
mazhar16823 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
Sorry, there was a typo. I meant physical time-step size.

Physical time starts at 0s and accumulates time according to how long you have run your simulation, the time-step size and number of time-steps that have been run.

You set a time-step size according to Courant number.

The max physical time is a stop criterion for when the simulation ends. You pick this based on how long you want the CFD to run. If you want to simulate a wind turbine spinning for 1s, set it to 1s. If you want to see it spin for a year, set it to 31,536,000 seconds.

But what if I choose a time step size based on each degree in full turbine blade rotation i.e. 360. For instance I choose time-step based on 2, 4, and 6 degree and see in which rotating position the solution is converged. Isn't that a good way?
mazhar16823 is offline   Reply With Quote

Old   April 24, 2020, 14:54
Default
  #8
agd
Senior Member
 
Join Date: Jul 2009
Posts: 311
Rep Power: 16
agd is on a distinguished road
In the turbine simulations that I have done, typically you want the time step to represent one degree or less of rotation to capture the physics. It can also depend the passage size - for example, rotor67 has 22 blades on a rotor so the passage between the blades is approximately 17 degrees. At a bare minimum you want 5 timesteps for the passage, or a max of about 3 degrees per timestep as an upper bound.
agd is offline   Reply With Quote

Old   April 24, 2020, 15:09
Default
  #9
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,389
Rep Power: 52
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
I mean you certainly can just put in any time-step size that you want. But good luck getting it to converge. The Courant number check just helps with the numerics.
LuckyTran is offline   Reply With Quote

Old   April 24, 2020, 15:21
Default
  #10
Senior Member
 
MA
Join Date: Mar 2020
Posts: 162
Rep Power: 3
mazhar16823 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
I mean you certainly can just put in any time-step size that you want. But good luck getting it to converge. The Courant number check just helps with the numerics.



Where can I see the Courant number changing in simulation once I set the time-step?
mazhar16823 is offline   Reply With Quote

Old   April 24, 2020, 15:22
Default
  #11
Senior Member
 
MA
Join Date: Mar 2020
Posts: 162
Rep Power: 3
mazhar16823 is on a distinguished road
Quote:
Originally Posted by agd View Post
In the turbine simulations that I have done, typically you want the time step to represent one degree or less of rotation to capture the physics. It can also depend the passage size - for example, rotor67 has 22 blades on a rotor so the passage between the blades is approximately 17 degrees. At a bare minimum you want 5 timesteps for the passage, or a max of about 3 degrees per timestep as an upper bound.



I am talking about three bladed horizontal axis wind turbine.
mazhar16823 is offline   Reply With Quote

Old   April 24, 2020, 15:27
Default
  #12
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,389
Rep Power: 52
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
It's a field function. Just make a plot like you would for pressure or anything. Or you can make a report or whatever is your preference for looking at data.
LuckyTran is offline   Reply With Quote

Old   April 24, 2020, 15:37
Default
  #13
Senior Member
 
MA
Join Date: Mar 2020
Posts: 162
Rep Power: 3
mazhar16823 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
It's a field function. Just make a plot like you would for pressure or anything. Or you can make a report or whatever is your preference for looking at data.

Thanks. One more thing:


- The reference area for the blade to create the Reports for any parameter such as drag (STARCCM) is the frontal area calculated via Report or it would be 1/3 of swept area as I have one wind turbine blade?


- In STARCCM+, Stream Edge Function for SST Transition Model is defined as $WallDistance>0.005?1:0 which means that BL is 5 mm thin but in my case maximum BL is 0.1 m. If I replace 0.005 with 0.1 won't it create a problem in the simulation?
mazhar16823 is offline   Reply With Quote

Old   April 24, 2020, 18:11
Default
  #14
New Member
 
Paul Hancock
Join Date: Mar 2009
Location: Bellingham, WA
Posts: 28
Rep Power: 14
Paulh is on a distinguished road
In the CCM+ help, look up the key phrase 'Cyclic Time Unit'. I think that's the functionality that gives you a link between rotational rate and time step.
Paulh is offline   Reply With Quote

Reply

Tags
implicit unsteady, starccm+, time-step

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On



All times are GMT -4. The time now is 12:49.