## 2 Description of Compressor and Computational Considerations
### Computational Considerations  
All the numerical simulations were performed by CFX software (Pittsburgh, PA, USA) in this study. Based on the compressor model, the radial inlet, the first stage, the vaneless diffuser, and the return channel were selected as the simulation domain, which ensured the computing efficiency of the CFD. However, this study focused on the effect of the radial inlet on the flow field and the aerodynamic load, with the seal area ignored in this simulation. The heat transfer method adopts the total energy equation, and the turbulence model is the \(k\)-\(\omega\) model based on the shear-stress transport (SST). The SST model depends on the turbulence energy and the turbulence diffusion rate equations [33], and it is widely adopted in turbomachinery [34; 35; 36]. Under the adverse pressure gradients, the SST model could provide highly accurate predictions for onset and flow separation. The high-resolution advection was used in the simulation, and the target of the root mean square (RMS) residual was \(10^{-5}\) for variable components. The difference value between the inlet and outlet mass flow should be less than 0.2%, and the calculation of variables that should be stable are the two conditions for the standard of convergence. The RSI effect should be caught by the unsteady simulation. The steady simulation result is used as the initial value for the unsteady simulation. During the unsteady simulation, the total computing time is set to 10 circles of the impeller rotation for the compressor to record stable and precise aerodynamic data on the impeller. The time step size is related to the compressor operation condition [37]. Based on the verification of time step independence, one rotation cycle of the impeller contains 180 time steps, i.e., the length of the time step is 4.176 \(\times\)\(10^{-5}\) s. The time step coefficient loops are set from 3 to 10 to ensure simulation convergence. As the radial inlet is an upstream component of the impeller, the leading edge of the impeller is a primary region affected by the RSI. Therefore, from the hub to the shroud, the monitoring points are kept along a single impeller blade leading edge at an equal distance to record the data during the unsteady simulation. Figure 2 shows the location of the monitoring points where 12 points (P1 to P12) are on the pressure side, and 12 points (S1 to S12) are on the suction side. The monitoring points are associated with the rotating coordinate system related to the impeller operation and record the data on the impeller. The boundary conditions in this investigation were defined as follows. The \(P_{\text{in}}\) and \(T_{\text{in}}\) were set at the inlet with medium turbulence, i.e., 5% turbulence intensity, and the \(Q_{d}\) at the outlet was defined. The general grid interface (GGI) was used to connect each component. The frozen rotor and transient rotor-stator interfaces were selected for the \begin{table}
\begin{tabular}{c c c} \hline \hline
**Variable** & **Symbol** & **Value** \\ \hline Mass flow rate (kg/s) & \(Q_{d}\) & 60.95 \\ Rotate speed (rpm) & \(n\) & 7982 \\ Intake total pressure (MPa) & \(P_{in}\) & 6.53 \\ Intake total temperature (\({}^{\circ}\)C) & \(T_{in}\) & 45 \\ Pressure ratio & \(\varepsilon\) & 1.045 \\ Efficiency (\%) & \(\eta\) & 89.3 \\ \hline \hline \end{tabular}
\end{table} 
Table 3: Compressor performance at design condition. steady and the unsteady simulations, respectively, to ensure accurate transmission of the flow field between the rotor and stator. For the wall and impeller surface, the non-slip condition was used. In this article, the impeller passage structured meshes were generated by Turbo-grid. After that, this periodic passage was copied to the whole wheel model meshes. The commercial mesh generator ICEM generates structured and unstructured meshes in the radial inlet, as shown in Figure 3.  
Figure 3: _Cont._  
Figure 2: The monitoring points’ location.