CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Main CFD Forum (https://www.cfd-online.com/Forums/main/)
-   -   Time-step for Implicit Unsteady solver in STARCCM+ and maximum number of steps? (https://www.cfd-online.com/Forums/main/226344-time-step-implicit-unsteady-solver-starccm-maximum-number-steps.html)

mazhar16823 April 24, 2020 08:12

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

LuckyTran April 24, 2020 13:42

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.

mazhar16823 April 24, 2020 13:50

Quote:

Originally Posted by LuckyTran (Post 767246)
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.

LuckyTran April 24, 2020 14:10

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.

mazhar16823 April 24, 2020 14:16

Quote:

Originally Posted by LuckyTran (Post 767258)
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.

LuckyTran April 24, 2020 14:22

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.

mazhar16823 April 24, 2020 14:28

Quote:

Originally Posted by LuckyTran (Post 767263)
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?

agd April 24, 2020 15:54

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.

LuckyTran April 24, 2020 16:09

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.

mazhar16823 April 24, 2020 16:21

Quote:

Originally Posted by LuckyTran (Post 767282)
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 April 24, 2020 16:22

Quote:

Originally Posted by agd (Post 767279)
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.

LuckyTran April 24, 2020 16:27

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.

mazhar16823 April 24, 2020 16:37

Quote:

Originally Posted by LuckyTran (Post 767287)
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?

Paulh April 24, 2020 19:11

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.


All times are GMT -4. The time now is 22:21.