## 2 Numerical Methods
### Compressor Geometry
\[\frac{\partial\rho h_{tot}}{\partial t}-\frac{\partial p}{\partial t}+\frac{ \partial}{\partial x_{j}}\big{(}\rho Uj_{ttot}\big{)}=\frac{\partial}{\partial x _{j}}\left(\lambda\frac{\partial T}{\partial x_{j}}-\rho\overline{u_{j}h} \right)+\frac{\partial}{\partial x_{j}}\big{[}(Ui_{j}\big{(}\tau_{ij}-\rho \overline{u_{i}u_{j}}\big{)}\big{]} \tag{3}\]  
where \(\rho\) presents the density, \(U\) the vector of velocity \(U_{x,y,z}\), \(p\) the pressure, \(\tau_{ij}\) the molecular stress tensor, \(T\) the temperature, \(\lambda\) the thermal conductivity, \(u\) the velocity fluctuation component, and the mean total enthalpy is given by:  
\[h_{tot}=h+\frac{1}{2}U_{l}U_{l}+k \tag{4}\]  
where, \(k\) is the turbulent kinetic energy. The selected turbulence closure model is the \(k-\omega\) shear stress transport model (SST). The \(k-\omega\) SST turbulence model is widely used in the numerical simulations of the aerodynamic performance in the turbomachinery research area, due to its accuracy and efficiency in prediction of the flow separations [31; 32; 33]. Figure 4: Contour of \(y^{*}\) at the impeller surfaces. Figure 3: Numerical mesh: (**a**) total view, (**b**) main and splitter blades of the impeller, (**c**) diffuser throat and diffuser vanes. In order to reduce the diffusion errors in the computational procedure [35], for discretizing the convection terms in the governing equations, a hybrid first-order and second-order upwind numerical schemes, which is known as high-resolution scheme was applied. The total pressure (101,325 Pa) and the total temperature (288 K) were the inlet boundary conditions, and the outlet boundary condition was the constant non-reflective static pressure boundary condition. To simulate the rotational effects of the impeller, a moving reference frame (MRF) for compressible flows was used. Rotational speed of the MRF was set to 21,789 rpm which is the speed of the compressor impeller at the design point condition. The adiabatic no slip boundary condition was chosen for all the walls. In order to preserve the stationary effects of the impeller shroud, a wall velocity boundary condition using the counter rotating option was applied. As the pitch ratio between the impeller and diffuser passages was 1, the frozen rotor interface was selected for the steady simulation. Although, this type of the interface model transfers the flow from one side of the interface to another side by changing the reference frame, but the relative position of the variables through the interface surfaces is unchanged. For unsteady simulations, the interface between the impeller and diffuser was treated by the transient rotor-stator interface, which includes all of the unsteady behaviors of the flow-field. Table 2 summarizes the solver setting used in the current study. For time discretization in the unsteady simulations, the backward Euler scheme was conducted, which is a second-order scheme. In order to take into account the effects of the relative positions of the impeller blades and diffuser vanes, a small time step of one-degree angular rotation was used with respect to the rotational speed of the impeller. The numerical simulations were carried out on a cluster including 256 CPU (3.3 GHz), and the unsteady simulation was performed until the flow-field fluctuations at various locations in the computational domain were time-periodic.