Wind turbine farm wake modelling

[FilipeRA]

Hello,

I was wondering if anyone in the Autodesk community could help me resolve/ inform on how to perform a specific simulation in the CFD package. The problem revolves around simulating the performance of a wind turbine park in the open sea with respect to wake interactions.

The company I work for already commissioned such a study from a well-known company within the field. However, this was performed in ANSYS CFX. Considering that we have access to Simulation CFD through our CleanTech subscription, we decided to attempt at a similar simulation. However, we found some limitations in Simulation CFD which might due to our lack of knowledge in the software. As such, we would like to ask for suggestions on how to approach this problem.

The commissioned study was based on the actuator disc method, whereby the turbine was represented by a porous subdomain. A pressure drop per meter profile representing a momentum loss was imposed to provide a kinetic energy corresponding to the site specific target profile provided by wind velocity, i.e. the pressure drop across the disc was made a function of the inlet conditions. The equation to estimate the pressure drop (Pdrop) is based on the average wind velocity V on the face of the disc and the thrust coefficient, Ct, and is defined as follows:

 Equation 1 (attachment 1)

Where ρ is the density of air (assumed as 1.225kg/m3), V is the average wind velocity, and Ct is the thrust coefficient (a parameter given by the turbine manufacturer).

At the inlet of the domain, a log-law mean wind speed profile representing a neutral atmospheric boundary layer (ABL) is imposed to provide a turbulent boundary layer corresponding to the site specific target profile provided by the Deaves and Harris log-law. An aerodynamic roughness height of about 0.0013m represents a uniformly rough on ground as urban terrain. The equation to estimate the wind speed (u) at height z (meters) above the ground is:

Equation 2 (attachment 2)

where u* is the friction (or shear) velocity (m s-1), κ is von Karman's constant (~0.41), d is the zero plane displacement, z0 is the surface roughness (in meters), and ψ is a stability term where L is the Monin-Obukhov stability parameter. Under neutral stability conditions, z / L = 0 and ψ drops out. An expression was used for surface roughness in the computational simulations as follows: zo = [0.025 * (u*) ^2 / 9.81] where u* is the friction velocity.

The RNG k-epsilon turbulent model was used to solve the 3D steady RANS equations.

Having described pretty much the whole setup, apart from the time steps and convergence criteria, how would I go about creating such a simulation in Simulation CFD.

I'd like to thank you in advance for the help,

Best regards,

Filipe

[apolo_vanderberg]

From the sounds of your description, it would seem that they used resistances to represent the pressure drop of each turbine. You could then have the full farm modelled and see just how much flow some of the turbines get that are downstream in the farm.

(See our distributed resistance section for defining a loss coefficient - here)

You might also want to look at out HVAC example model (on your machine and in the Help) for step by step on using and assigning resistances.

At this time the only method of producing the velocity profile at the inlet that you desire would be to split the inlet face in to a number of different surfaces. For each of those surfaces you can specify a unique velocity that would contribute to building the full profile from top to bottom.

Apolo

[FilipeRA]

Thank you for the quick response!

I assume that the same (specifying a velocity to each split face) can be done with turbulence, and length scale, right? Is it also possible to assign different resistance to the Actuator disc if I split it like you proposed for the velocity? This as in a real world scenario the wind speed increases with height, and as such the resistance should be different depending on the actuator height.

Also with regards to the splitting of the inlet conditions, does Simulation CFD interpolate between the values assigned (to produce something similar to the red line in the new attachment) or each face has a constant value until next face (blue line)?

Filipe

[apolo_vanderberg]

Filipe,
The resistance is a function of the velocity coming in such that as the velocity varies coming in to a resistance the pressure drop of the resistance can change. So if you had a square resistance and a high velocity near the top and low velocity near the bottom you would see the appropriate pressure loss based on those velocities given the K fact used to define that material

We do not interpolate and would be the blue line such that the more splitting you do the less faceted the profile would appear.