*4.1. Numerical Setup and Validation*

The numerical simulations presented in this paper were performed using the commercial CFD software ANSYS® FLUENT® [38]. The solver-setting process for the numerical solutions involved the use of a two-dimensional unsteady Reynolds-averaged Navier–Stokes (U-RANS) approach with a pressure-based formulation of the solver and a *Coupled* algorithm for the pressure-velocity coupling. The second order upwind discretization scheme was used for momentum, energy, and turbulence parameters, and the pressure interpolation was second order. As far as the turbulence settings are concerned, the Transitional κ-ω SST (Shear Stress Transport) model was adopted for predicting the transition between laminar to turbulent flow of the boundary layer. The choice was related to three different requirements:


It has to be noted that in case of a three-equation U-RANS simulation characterized by an elevated level of turbulence intensity, the dominant turbulent parameter is the turbulence intensity itself. Therefore, the length scale ultimately affects the rate of decay of the turbulence intensity, while having a negligible impact on the turbulent shear stress [7].

The computational domain is an open-field type having an overall extent of 60 chords and a width of 40 chords to avoid any blockage effect on the blade profile. A Dirichlet boundary condition was employed to prescribe a uniform velocity profile at the inlet boundary. The operating pressure input is set at the outlet boundary as the static pressure of the environment. The blade surface is modeled using the standard smooth no-slip wall. To replicate the conditions of the experiments, the turbulent intensity was specified at the inlet boundary in order to obtain a turbulence level (after the intrinsic decay along the domain) of roughly 9.5% at the blade location. Among the different levels tested for the turbine (Figure 6), the selection of the highest one was motivated by the fact that effects are expected to be more visible and less affected by the possible uncertainty of the CFD approach. The application of the transitional turbulence model used in the URANS approach is in fact critical in case of very low turbulence levels and Reynolds numbers.

A grid independence test was carried out for different mesh sizes in order to define the optimum mesh for the best tradeoff between accuracy and fast computation. The convergence study was performed considering three different grids. Due to the *Low-Re* number wall treatment, the size of the wall-adjacent cell for all meshes was defined such as to satisfy the requirement of the dimensionless wall distance (*y*+) lower than ~1. The baseline coarse mesh was defined by adopting a discretization of the airfoil surface with 750 nodes, thus obtaining a size of 1.6 <sup>×</sup> 105 cells in the whole domain. The medium and fine meshes were defined by progressively doubling the overall elements count. In particular, the fine mesh was featuring 1500 nodes on the blade and 6.8 <sup>×</sup> <sup>10</sup><sup>5</sup> domain cells. The error in the estimation of lift and drag coefficients at *Re* = 80 k between the medium and fine mesh was lower than 0.2%. Therefore, the medium mesh featuring 1100 nodes on the blade and 3.3 <sup>×</sup> <sup>10</sup><sup>5</sup> domain cells, whose details are shown in Figure 8, was adopted for all of the computations presented in the paper. The core region of the flow is discretized by means of an unstructured triangular mesh, with a clustering of the mesh elements in airfoil walls. An O-grid of quadrilateral elements was used around the blade, with an extrusion of 40 layers off the wall to guarantee a sufficient boundary layer resolution.

**Figure 8.** Computational grid used for the airfoil polars calculations.

As a result, Figure 9 shows the comparison between the experimental polars for the airfoil tested at *Re* = 80 k with a high turbulence flow and those resulting from the CFD simulations of the current study in the same flow conditions. The validity of the CFD approach is clearly confirmed, since measurements and numerical results are in good agreement. The CFD model is able to properly capture the trends of lift and drag coefficients as well as the maximum values, although a 1 degree shift of the static stall location between the experimental and the simulated curves can be observed.

**Figure 9.** Comparison between CFD and experimental polars with a high turbulence flow.
