*3.1. Preprocessing*

The overview of the considered geometry is visible in Figure 2. Two domains were distinguished in order to represent the fluid flow: rotor domain, in the form of a flat cylinder in which blade and hub are modelled, and stationary domain, which encompasses the former. In between the two domains, an interface is placed to permit the exchange of data. There is no relative movement between domains since the problem is considered as steady state. Instead, the frozen rotor model is employed, where the relative orientation of the components across the interface remains fixed along with the calculations and the flow from one component to the next changes the frame of reference [23]. The steady-state approach was chosen, as the simulation is performed under uniform, time-independent inflow conditions and one-way FSI. The transient analysis would require numerical and time resources prohibitively large for this—initial—phase of computations. The rotational velocity ω is imposed on the particles flowing through the rotor domain—analyzed cases are seen in Figure 4. The values of ω mimic those set in the benchmark experiment, performed independently by team GUST at TU Delft Open Jet Facility wind tunnel [24]. The experimental investigations were not a part of this study, and their results were made available as reference values at the courtesy of the GUST team. The authors estimate that the relative error of the experimental results is in range of 5%.

**Figure 2.** Side and front view of the analyzed problem geometry (elements are in scale).

Both domains were discretized together using tetrahedral, unstructured mesh (Figure 3) in ANSYS Mesher software. Refinement was performed in the rotor vicinity in order to better model the expected high gradients within the flow. The inflation layer was created around blades and hub surfaces to ensure a full resolution of boundary layer flow. The resulting mesh size is 10.8 <sup>×</sup> 106 nodes and 22.8 <sup>×</sup> <sup>10</sup><sup>6</sup> elements.

**Figure 3.** Mesh cross-section views: global (top) and around blade and hub (bottom).

Boundary conditions (see Figure 2 and Table 2) were set in order to mimic the outdoor wind turbine operation. The reference pressure was set to 1 atm (101,325 Pa). Chosen turbulence closure was k-ω SST with a standard set of coefficients, as this model proved trustworthy in previous wind turbine applications [22,23]. The considered flow medium (air) density <sup>ρ</sup> <sup>=</sup> 1.185 kg·m−<sup>3</sup> and dynamic viscosity is 1.831 <sup>×</sup> 10−<sup>5</sup> kg·m−1·s<sup>−</sup>1. The fluid is considered to be an incompressible (*Ma* < 0.3) ideal gas. Double precision, the fully coupled pressure-based solver was used, and the resolved equations involved flow continuity, momentum, and total energy conservation.

**Table 2.** Flow simulation boundary conditions.

