## 2 Materials and Methods
### Numerical Methods of Steady Simulations  
Setting up a simulation model is the first significant step for the accurate study of the flow field inside the compressor. For this purpose, the Computational Fluid Dynamic (CFD) simulation was conducted based on a three-dimensional, steady-state, compressible and finite volume layout. EURANUS (NUMECA FINE/Turbo) [27] solver was used to solve the Reynolds-averaged Navier-Stokes equations. The central scheme and fourth-order Runge-Kutta scheme were utilized for spatial discretization and temporal discretization, respectively. We compared four various turbulence models (Spalart-Allamaras (SA) [28], SARC [29], k-\(\varepsilon\) with extended wall function [30] and SST [31]) for analyzing the same compressor prototype with the same numerical setup (Figure 2 and Table 2). We confirmed the reliability of the Spalart-Allamaras (SA) model in terms of performance as well as computational time and cost. Therefore, the one-equation model, Spalart-Allamaras (SA) is applied as the turbulence model in this investigation. A real gas is utilized for representing the air characteristics as the working fluid in all simulations. The boundary conditions used in this research are summarized in Table 3. The absolute total \begin{table}
\begin{tabular}{c c c c c} \hline \hline
**Models** & **Equation Numbers** & **Time (10,000 Iterations Per Core)** & \(\mathbf{\eta_{1-4}}\) & \(\mathbf{\pi_{1-4}}\) \\ \hline SST & 2 & 23.3 h & 0.8042 & 8.03 \\ k-\(\varepsilon\) & 2 & 19.5 h & 0.7871 & 7.83 \\ SA & 1 & 17.4 h & 0.7989 & 8.05 \\ SARC & 1 & 27.0 h & 0.7924 & 7.89 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Turbulence model overview. Figure 2: Performance at design speed predicted by different turbulence models. temperature and absolute total pressure were imposed as the inlet boundary conditions. Depending on the operating condition, two types of outlet boundary condition are set. At the near surge condition, the averaged mass flow rate is imposed at the diffuser exit while an averaged static pressure with backflow control is set for other operating points. The impeller of the compressor is rotating and the vaned diffuser is set as stationary. The impeller hub wall is rotating with the impeller blade, while the diffuser hub stands stationary with the diffuser blade. The shroud of both the impeller and diffuser remains stationary. The thermal condition for the simulation is set as adiabatic. A non-slip condition is adjusted for the solid walls. A periodic matching boundary condition is applied between the adjacent compressor passages. For choosing an appropriate interface model in this investigation, we compared the effects of different interface model on the compressor performance and flow field (Figure 3). We also compared the absolute Mach number in different interface model with unsteady simulation (Figure 4). Finally, in this study, the rotor/stator interface is achieved with the non-reflecting 2D model, which is a subset of the mixing-plane method because it has better performance and is consistent with unsteady simulation and can predict the flow behavior inside the compressor accurately. A significant issue in this study is studying the effects of even small radial gap ratios (e.g., radial gap ratio of 1.04) on the high-pressure ratio centrifugal compressor performance. Thus, the physical model (except the radial gap ratio) for all cases should be kept constant. Therefore, the interface radius ratio, which is defined as \(\mathrm{r}_{\mathrm{Interface}}/\mathrm{r}_{2}\), is set as small value of 1.02. To confirm that the small interface radius ratio does not have a substantial influence on the compressor performance, the performance of a compressor with interface radius ratio of 1.02 and 1.05 are compared in Figure 5. The compressor prototype, physical model, turbulence model, boundary condition, and the simulation settings are all the same for this comparison.