## 2 Aerodynamic Load and Deformation Analysis of Multi-Stage Telescopic Wings
### Aerodynamic Analysis of Flight Environmental Loads
#### 2.1.1 Flow Field Model Establishment  
The intended operational environment for the multi-stage telescopic wing corresponds to a maximum flight speed of Ma = 5 and a maximum flight altitude of 20 km. The aerodynamic analysis is conducted based on its maximum flight capability as the design condition. First, the standard atmospheric parameters under the specified design condition are determined, as listed in Table 2.  
For flow field modeling, a rectangular computational domain is selected to minimize the influence of fluid domain inlets and outlets on the results and ensure an adequate fluid region around the telescopic wing. The telescopic wing is positioned at the center of the domain, with the front designated as the inflow inlet and the rear as the outflow outlet. The other four sides are set as flow field boundaries to avoid undesired interference. One of these boundary surfaces is defined as the connection interface between the telescopic wing and the fuselage. The spatial arrangement is shown in Figure 3. \begin{table}
\begin{tabular}{c c c c c c} \hline \hline
**Temperature** & **Density** & **Thermal** & **Coefficient of** & **Elastic Modulus** & **Specific Heat** \\
**(\({}^{\circ}\)C)** & **(kg/m\({}^{3}\))** & **Conductivity** & **Linear Expansion** & **(GPa)** & **Capacity** \\
**(\({}^{\circ}\)C)** & **(W/(m\(\cdot\)K))** & **(10\({}^{-6}\)/K)** & **(10\({}^{-6}\)/K)** & **(J/(kg\(\cdot\)K))** \\ \hline
20 & & - & - & 205 & 385.97 \\
100 & & 14.56 & 13.2 & 201 & 420.35 \\
200 & & 15.91 & 13.3 & 196 & 470.68 \\
300 & & 17.59 & 13.8 & 189 & 481.4 \\
400 & & 18.84 & 14 & 183 & 493.9 \\
500 & & 20.1 & 14.6 & 176 & 514.8 \\
600 & & 21.77 & 15 & 169 & 539.0 \\
700 & & 23.03 & 15.8 & 164 & 573.4 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Physical and thermal properties of GH4169. Figure 3: Flow field of the telescoping wing. The aerodynamic simulations employ a locally refined polyhedral mesh to enhance computational accuracy and optimize boundary layer resolution. The mesh resolution is adjusted to ensure that the dimensionless wall parameter y+ remains below 1, and a low-Reynolds-number wall treatment is adopted to enable full resolution of the viscous sublayer. The total number of mesh elements is approximately \(1\times 10^{6}\), with the wing mesh element size set to \(10^{-2}\) m. The height of the first-layer boundary layer mesh on the wing surface is set to \(9\times 10^{-6}\) m, with a growth rate of 1.2 to ensure smooth mesh transitions. In hypersonic flow conditions, the temperature distribution on the wing surface is influenced by viscous dissipation heating of the surrounding gas. Therefore, as illustrated in Figure 4, local mesh refinement is applied near the fluid-solid interface in the aerodynamic model to enhance computational accuracy and ensure high-quality boundary layer resolution. After completing the flow field mesh division, the aerodynamic simulation solver and boundary conditions are configured. The most commonly used turbulence models in CFD analysis include the Spalart-Allmaras, k-\(\varepsilon\), and k-\(\omega\) models. Among these, the SST k-\(\omega\) two-equation model combines the strengths of the k-\(\varepsilon\) model for free-stream flow and the k-\(\omega\) model for near-wall flow by utilizing a blending function. This capability makes it particularly suitable for simulating large flow separations. The SST k-\(\omega\) turbulence model is selected for solving the flow field. Regarding boundary conditions, the inlet is set as a pressure far-field boundary with a static pressure of 5.5293 kPa, a temperature of 216.85 K, and an angle of attack of \(5^{\circ}\). The outlet static pressure is set identical to the inlet. The wall boundary condition is modeled as an adiabatic no-slip wall. Given the influence of compressibility and thermal effects in the hypersonic flight environment of the multi-stage telescopic wing, the energy equation and compressible flow solver are activated in the simulation to ensure the accuracy of the computational results.