[Dan709]

Hi all,

I am working on a simulation of a vertical axis wind turbine operating at low TSR and thus in the dynamic stall regime. I am using an overset region around each blade and polygonal elements everywhere.

I am having issues with getting the residuals of momentum in particular to drop in an expected manner - i.e. in the range of a 3 order of magnitude drop in a reasonable number of inner iterations. So far I've been primarily using the segregated flow solver, but the residual trend for both momentum quantities is often very irregular and oscillatory (continuity is fine and behaves as expected).

To try and solve the problem I've been doing some testing whereby I use the same model setup but look at a static airfoil case with an angle of attack of 15 degrees (see attached mesh image) and Reynolds of approximately 1.1E5. I am using 960 nodes on the airfoil with a thick boundary layer and my time-step should be sufficiently small, being the equivalent of 2000 steps/cycle under the turbine's operating conditions.

Under the exact same static setup, I've done a comparison between using the segregated flow solver and coupled implicit one. I've attached an example output of residuals from both of these (turbulent quantities are not displayed because they are always orders of magnitude smaller). Basically, the segregated solver can reach a low residual (say 1E-4), but this takes almost 100 inner iterations to accomplish. Conversely, the residuals of the coupled solver completely bottom out and flat-line after approximately 50 inner iterations (I set a maximum number of inner iterations of 200 here just to investigate).

As my mesh and time-step size should be sufficiently refined for this static airfoil case, I am trying to find the reason for this bizarre residual behaviour and am thinking that it may have something to do with the overset interpolation? But I am really not sure and very much welcome all suggestions.

As I imagine someone may propose, I do also monitor the instantaneous forces on the blades as a means of convergence during my actual full turbine simulations. However, having the residuals not converging within time-steps is unsettling and is definitely something I'd like to address.

Thanks for any help!

Cheers,
Dan

[me3840]

Why do you need to use overset for this? There's no way to do a sliding mesh?

Do the forces converge before the residuals drop that far?

I don't really see any issues with those residual curves, they're just slow. Have you turned the URFs up? If your mesh is good quality you should be able to increase them a lot over the default values.

[Dan709]

Originally Posted by me3840

Why do you need to use overset for this? There's no way to do a sliding mesh?

Do the forces converge before the residuals drop that far?

I don't really see any issues with those residual curves, they're just slow. Have you turned the URFs up? If your mesh is good quality you should be able to increase them a lot over the default values.

Hi me3840,

Thanks for the reply, I appreciate it.

You are indeed correct in that I could just use a sliding mesh for this. I should have explained further: the traditional VAWT here is only the validation case for my project, the actual turbine I will be modelling uses a unique blade path trajectory and thus the overset meshing greatly simplifies the motion definition.

Since posting this I have managed to more or less fix the problem I believe (with the help of my post-doc friend ). Still using the Implicit Coupled model, we added in the Coupled Energy model option and changed the fluid model from Constant Density to Ideal Gas. Despite the fact that at this low of a Mach number compressibility effects are of course negligible, this change in model/solver formulation had a huge effect on the residuals trend (see attached plot). Now the residuals fall smoothly below to 1E-4 in 40-60 inner iterations, at which point the forces are also converged sufficiently.

I think the URFs are only applicable to the Segregated solver for pressure and velocity, and after this new discovery with the Coupled solver I'll be sticking with it for now. But thanks for the suggestion!

Cheers,
Dan

[me3840]

Still, 40-60 iterations per timestep is very slow. Turning on compressibility making the coupled solver easier to converge isn't much of a surprise, it lets the system be a little less stiff.

What CFL are you using for the solver?

[Dan709]

Originally Posted by me3840

What CFL are you using for the solver?

If you're referring to using CFL to control the time-step of the transient run, I set my time-step directly as 7.7E-5 s, which is the time-step I use in my actual turbine simulations to provide me with 2000 steps per rotor cycle, or equivalently 0.18 degrees of rotor rotation per step.

I see in the Solvers->Coupled Implicit node within the STAR simulation tree there is a Courant Number field, and I have simply left this at the default of 50. Since I specify my time-step manually, I am not sure what this Courant Number specification actually does to be honest. Do you have an explanation?

Also, I should mention that the bottleneck on the number of inner iterations now seems to be the force convergence criteria, which I have set quite high for the time being at essentially 0.01% difference between successive inner iteration values. The continuity and momentum residual criteria of 1E-4 are usually satisfied 10-20 iterations before this.

Thanks for the help and discussion.

Cheers,
Dan