# Wind Turbine Enhancement via Active Flow Control Implementation
## 2 Numerical Method
### Numerical Domain and Boundary Conditions  
For computational domains relatively small in respect to the bluff-body characteristic length, the flow around the bluff-body is affected by the boundary conditions defined at the boundaries. Conversely, if the domain is chosen to be too large, there may be excessive mesh cells, resulting in longer computational times and poor simulation efficiency. Therefore, it is crucial to choose an appropriate domain size that balances the need for accurate results with computational efficiency. Based on the previous research undertaken by [22; 24; 50], the computational domain employed in the present research has the following dimensions: 10C from the domain inlet to the airfoil leading edge, 15C from the trailing edge to the domain outlet, and 10C from the body surface to both the upper and lower limits of the domain, \(C\) being the airfoil chord; see Figure 1.  
Two points, \(P\) and \(Q\), delimiting the inlet and outlet boundaries, have been implemented in Figure 1. The outlet boundary extends from \(P\) to \(Q\) in a clockwise direction, and from \(P\) to \(Q\) in a counterclockwise direction is to be found the inlet boundary. The curvilinear shape of the domain at the inlet has been selected to facilitate the simulation of various angles of attack without altering the mesh geometry. It should be noted that the airfoil has been horizontally positioned, and by adjusting the inlet velocity components, any required angle of attack can be obtained. This approach not only allows flexibility in the simulation but also ensures that the mesh remains consistent throughout the analysis. The present research focuses on simulating external aerodynamics with transient turbulent flow (aerodynamic forces change over time) and at large Reynolds numbers of the order of \(\mathcal{O}(10^{7})\). Additionally, the angle of attack is relatively high for the two baseline case sections studied, which, particularly for the section placed nearest the blade root (Section 54 of the DTU-10 MW-HAWT), is expected to produce the separation of the boundary layer at some point along the chord, generating the corresponding vortical structures and vortex shedding. Moreover, since the relative velocity in both sections studied does not exceed the incompressible flow limit, which is commonly accepted as \(M<0.3\), the flow will be considered as incompressible across the entire study. The flow solver contained in the OpenFOAM package, which fulfills the needs for the present research, is _PisoFoam_ (Pressure implicit with splitting operator). This solver is particularly well suited for simulating unsteady turbulent flow and is widely used in aerodynamic simulations due to its accuracy and efficiency. Section 54 with a wind speed of 10 m/s was chosen to perform the mesh independence study. Notice that the Reynolds number is almost the same in both sections, and the angle of attack is much larger in this particular one. The main data relative to the two sections studied, Sections 54 and 81, are presented in Table 1, which includes the airfoil type, the radius versus the turbine main axis, the section number, the chord length, the Reynolds number, the angle of attack, and the relative velocity, which is the vectorial magnitude  
Figure 1: Schematic view of the meshing domain within its general dimensions. obtained from the combination of the wind and turning speeds and when considering the axial (a) and angular (a') induction factors. Figure 2 introduces the approximate location of the two sections under study as well as their respective profile. The different boundary conditions employed to simulate section 54, regardless of the mesh density considered, are outlined in Table 2. It's worth noting that these specific values are based on the \(k\)-\(\omega\) SST turbulence model, aligned with the corresponding chord length and a turbulence intensity at the inlet of 0.1 % and according to [48; 49]. In this paper, all simulations were performed using air at sea level based on the International Standard Atmosphere (ISA).