## 2 Influences of the Size of Flow Field  
The computational efficiency and accuracy always need to be compromised in CFD calculations, particularly when simulating a large complex structure like a megawatt wind turbine. If the flow field is defined too small, computational accuracy cannot be guaranteed. However, if the flow field is defined too large, excessive computation will be caused. The research conducted below is to investigate how to define the size of the flow field properly in CFD calculations. To facilitate the study, a turbine model, whose prototype comes from a GE 1.5 MW wind turbine, is considered. Its parameters are listed in Table 1. The blade used in this wind turbine was designed using three types of airfoils, i.e., S818, S825, and S826. The 3D models of the turbine, the blade, and the corresponding three-bladed rotor in the flow field are shown in Figure 1. In Figure 1a, the yaw angle is defined as the angle difference between the wind direction and the axis of the wind rotor. Since the wind power theory has suggested that airflow will expand after passing through the wind rotor, the outlet diameter of the flow field in Figure 1b is defined larger than the inlet diameter of the flow field. There is no doubt that the flow field should be large enough to guarantee the computational accuracy. However, too large a size of the flow filed can cause excessive computation and thus make it difficult to obtain calculation results in a reasonable time. What is the optimal size of the flow field? To find a compromised solution for this issue, the influences of the flow field size on the simulation results were investigated within ANSYS Fluent, which is a popular commercial software for performing fluid dynamics simulation. When performing simulation calculations in ANSYS Fluent, the Reynolds number in each simulated scenario was defined indirectly by defining the values of the relative velocity \(v\), the air density \(\rho\), the dynamic viscosity of the fluid \(\eta\), and the characterized size \(r\). For example, the air density \(\rho\) is set to be 1.225 kg/m\({}^{3}\), the viscosity \(\eta\) is set to be \begin{table}
\begin{tabular}{c c c} \hline \hline
**Parameters** & **Values** & **Unit** \\ \hline Rated power & 1.5 & MW \\ Number of blades & 3 & - \\ Rotor diameter & 82.5 & m \\ Cut-in wind speed & 3.5 & m/s \\ Hub height & 80 & m \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Wind turbine parameters. \(1.7894\times 10^{-5}\) kg/m-s, \(r\) is determined by the data listed in Table 1, \(v\) is set to be different values in different simulation scenarios. The mesh size is 0.3 m and the meshing of the CFD model is performed using the default model in the software for simplicity. In the calculations, the k-omega viscous model is selected as a solver. In the software ANSYS Fluent 15.0, the item of the Pressure-Velocity Coupling is set to be \"Coupled\", the item of the Gradient is set to be \"Least Squares Cell Based\", the item of the Pressure is set to be \"Second Order\", the item of the Momentum is set to be \"Second Order Upwind\", and the item of the Turbulent Kinetic Energy is set to be \"Second Order Upwind\". Both edgewise and flapwise moments of the blade are employed as the indicators of the blade load. The calculation results obtained at different outlet-diameter-to-inlet-diameter ratios, when the inlet diameter is respectively 90, 144, 198, and 252 m, are shown in Figure 2. In the calculations, different wind speeds and rotor speeds are also considered in order to understand the influences of the flow field under different environmental and turbine control conditions. Herein, it is necessary to note that wind shear is temporarily not considered in this section in order to concentrate the research on investigating the effect of the flow field on the calculation results. Figure 1: The 3D models of the wind turbine. (**a**) Model of the wind turbine. (**b**) Model of the blade. (**c**) Model of the rotor in computational fluid dynamics (CFD).