## 3 Calculation Model and Reliability Verification  
This paper uses the size of Joukowsky airfoil studied by [PERSON] [25] as the original size for research. The LES Smagorinsky SGS (sub-grid-scale) model approach was adopted to resolve time-wise and space-wise variation in the flow due to large-scale eddies. The finite volume method was applied to discretize the differential equation, and the SIMPLE algorithm was used to solve the discrete equation. The accuracy of spatial discretization was second-order. The Green-Gauss node-based method was used to calculate the gradient and derivative of variables at the center of the element cell through Ansys Fluent numerical simulation, and heat transfer was not considered. As two-dimensional calculations can also obtain results that are relatively close to experimental ones [26; 27], the airfoil was calculated using a two-dimensional model. The model uses the Integrated Computer Engineering and Manufacturing code for Computational Fluid Dynamics (ICEM-CFD) for grid division, and the airfoil outer flow field radius is 20 chord. The fluid domain and fluid mesh is shown in Figure 3a. In order to ensure that the number of elements in the mesh has no impact on the results, a mesh independence verification was carried out, as shown in Figure 3b; when the number of meshes reached a certain value, further increases in the number of meshes had no significant effect on the calculation results but increased the calculation time. Considering the balance between solution accuracy and calculation time, the number of meshes selected for this study was approximately 0.4 million. In order to ensure the accuracy of the simulation calculation, the Y+ value of each airfoil was less than 1 [28], as shown in Figure 4b. Additionally, in the LES, the Taylor length scale (\(\lambda\)) was examined to verify the sufficiency of the mesh resolution. According to [PERSON] [29], the mesh resolution (\(\Delta=\sqrt[3]{V_{cell}}\)) should at least be in the order of \(\lambda\) to completely solve the Taylor length scale. This method was applied to the wake of an airfoil, at \(Y/\delta=\pm 1\), since this is expected to be the area where the effects of the turbulence are most noticeable and, therefore, where the best resolution is required [30]; for data extraction, 11 spanwise planes normal to the streamwise direction located on the wake behind the airfoil were considered. These planes were located from 226 from the TE (trailing edge), separated 2\(\delta\) between each other, as shown in Figure 4a. Figure 4c shows that the criteria proposed by [PERSON] are fulfilled along the whole wake behind the airfoil, which means that the mesh is suitable for LES simulations. The details of the Computational Fluid Dynamics (CFD) model are presented in Table 1.  
Figure 2: Airfoil tail optimization. (**a**) Step I. (**b**) Step II. Figure 4: (**a**) Data extraction. (**b**) Y+ distribution of airfoil and (**c**) Taylor length scale on the wake behind the airfoil. Figure 3: (**a**) Fluid domain and fluid mesh. (**b**) Mesh independence. In order to verify the reliability of this simulation, experimental data obtained from references were used [31; 32]. The experimental data included the pressure coefficient distribution of the original Joukowsky airfoil at different Reynolds numbers and different angles of attack. The expression of the pressure coefficient is as follows:  
\[C_{P}=\frac{p-p_{inlet}}{(0.5\rho U^{2})_{inlet}} \tag{6}\]  
where \(p\) is the point static pressure on the airfoil; \(p_{inlet}\) is the inlet static pressure; \(\rho U^{2}\) is the dynamic pressure. Comparing the simulation data with the experimental data, we found that the simulation data at different Reynolds numbers and different elevation angles are relatively close to the experimental data, which shows that the simulation has high reliability in analyzing the influence of different elevation angles and different Reynolds numbers on an airfoil, as shown in Figure 5.