## 3 Experimental Facility and Numerical Validation
### Numerical Calculation Method  
Two-dimensional steady numerical simulations are performed on the supersonic compressor cascade with the commercial CFD software ANSYS FLUENT 2020 R1. The fluid is set as an ideal gas, and steady-state numerical simulations of the internal flow field of the supersonic compressor were carried out. The software employs the finite volume method to solve the compressible Reynolds-averaged Navier-Stokes (CRANS) equations. A fully implicit simulation solution strategy with an upwind difference scheme is adopted to set the solver, which can be accurately obtained through the boundary layer separation induced by the shock for transonic and supersonic flow [33; 34; 35]. Before the shockwave interacts with the boundary layer, it is believed that the boundary layer has transformed into a turbulent boundary layer. [PERSON] and [PERSON] [36; 37; 38] evaluated and verified different turbulence models in ANSYS FLUENT. The SST(k-\(\omega\)) turbulence model is more accurate in predicting the SWBLI flow field and is in good agreement with the experimental data. Hence, the SST(k-\(\omega\)) model is adopted here for numerical simulation investigations. In order to improve the accuracy of the calculation results, the inlet and outlet positions of the calculation domain are 1.5 times the chord length from the leading edge and trailing edge of the cascade, respectively. The cascaded computational domain model consists of multiple blocks. The computed grid nodes generated by the commercial software ANSYS ICEM are shown in Figure 8. The O-block mesh topology type is employed around the vane with 30 grid nodes in the boundary layer, and H-blocks are adopted at the cascade leading edge and cascade trailing edge to guarantee the best grid quality. The first cell width close to the solid wall is less than \(1\times 10^{-6}\) m to ensure that its value y\({}^{+}<1\). The size and topology have been verified in the grid resolution study and valued to be sufficient. The boundary conditions are set as shown in Table 3. Total pressure, total temperature, and flow vector are given at the inlet in boundary conditions, which are consistent with the cascade experiment conditions. Static pressure is specified at the outlet. Nonslip and adiabatic conditions are defined for all solid walls. Figure 6: Supersonic compressor cascade with 6 vanes. Figure 7: Test section of supersonic compressor cascade wind tunnel. The overall aerodynamic performance of supersonic compressor cascade is obtained by adjusting the back pressure at the exit plane. The convergence of the calculation result is judged by the residual of the control equation. Some residuals of key parameters such as the inlet and outlet flow, velocity, and pressure of the cascade are monitored. A convergent numerical calculation result can be considered to be obtained when the residual of these key parameters is less than \(10^{-6}\). A laboratory server was used for numerical calculation; each workstation had 32 nodes and a 32 G memory. The calculation time for each example was about 12 h, and a converged result was obtained. In agreement with the most common methods for predicting the stall boundary of compressor cascades in numerical calculation, the stalling point of the compressor cascade was taken as the divergence point under a certain higher back pressure. Calculation convergence, which may take thousands of time steps, becomes more difficult with an increase in static pressure at the exit. The pressure increase is only 0.1% of the inlet pressure, near to the stalling point. The verification of numerical methods is the key to evaluating the reliability and feasibility of numerical results. The validation of mesh independence is conducted via variations in the mesh nodes in the computational domain. According to [PERSON] [39], computational errors accumulate faster for coarse grids. Therefore, the reliability of numerical results increases with an increase in grid resolution.