## 3 Methodology
### Validation of Computational Method  
In CFD simulation, the conservation equation of mass, energy and momentum are solved by Reynolds-Averaged Navier-Stokes (RANS) method. In this investigation, a compressible and steady turbulent flow is simulated. The equations can be expressed as below:  
\[\frac{\partial(\rho u_{i})}{\partial x_{j}}=0 \tag{5}\]  
\[\frac{\partial\Big{(}\rho u_{i}u_{j}\Big{)}}{\partial x_{j}}=-\frac{\partial p }{\partial x_{i}}+\frac{\partial\Big{(}\mu\frac{\partial x_{i}}{\partial x_{j} }-\rho\overline{u_{i}^{\prime}u_{j}^{\prime}}\Big{)}}{\partial x_{j}}+S_{i} \tag{6}\]  
\[\frac{\partial(\rho u_{i}T)}{\partial x_{j}}=-\frac{\partial\Big{(}\Gamma\frac {\partial T}{\partial x_{j}}-\rho\overline{u_{i}^{\prime}T^{\prime}}\Big{)}} {\partial x_{j}}+S \tag{7}\]  
where \(u\) stands for velocity components, \(x\) is displacement term, \(S_{i}\) and \(S\) are, respectively, the source term of momentum and inner heat. To handle the governing equations of turbulent flow, the RANS method is adopted. Hence, a turbulence model is needed for the calculation of Reynolds stress. To discretize the governing equations, an element-based finite volume method is adopted. TurboGrid 18.2 is employed to generate the hexahedral meshes in all fluid domains, which correspond to lower truncation error. To obtain the best accuracy and the influence of the wake flow, a full cycle of the impeller and the nozzle is adopted in the investigation. Figure 5 shows the mesh of the fluid domain including the partially enlarged view of the leading edge of the nozzle, the rotor-stator interface and the trailing edge of the rotor. O-type mesh is applied around the rotor blades and nozzle blades. The mesh of the boundary layers has been densely generated to adapt the turbulence model. Concretely, the discretization in the boundary layer area ensures the averaged solver \(y^{+}\) is set around 1 as recommended in the CFX User Guide. Figure 4: Splitter structures for the lowest solidity case: (**a**) normal; (**b**) ps offset; (**c**) ss offset. For the determination of near-wall velocities, the automatic wall function is chosen. Total energy equation including the viscous work term is used for energy conservation. A high-resolution advection scheme of CFX is used. The boundary conditions employed in this research are listed in Table 2. We use total pressure and temperature as inlet boundary conditions. To simulate the inlet solute, the flow angle at the nozzle inlet is set as 45\({}^{\circ}\). The static pressure is used for outlet boundary condition while the rotation speed is set as 50,000 rpm for the rotor. A frozen-rotor method is adopted to handle the interface between stator and rotor. An automatic domain initialization method is used. The computation is considered converged when RMS residuals are below 10\({}^{-5}\). In the meantime, we evaluate the mass flow rate of the turbine inlet and outlet. If they are equal and slightly fluctuate with each iteration step, the case reaches convergence. In order to validate the method of CFD simulation, we choose a similar radial-inflow turbine working with air from [PERSON] et al. [29], which possesses experimental results. A CFD simulation with [PERSON]'s model and boundary conditions under design point is conducted. Four common turbulence models for turbomachinery simulation including k-\(\varepsilon\), RNG k-\(\varepsilon\), k-\(\omega\), and SST k-\(\omega\) are adopted and the validation results are given in Figure 6. It can be seen from Figure 6 that compared with the results in [29], the mass flow rate and efficiency calculated by k-\(\varepsilon\) models are higher. Compared with the experiment, we adopt a shrouded impeller in the design. The leakage flow derived from tip clearance is not taken into account. Besides, due to the simplification of the research model, the leakage flow between the nozzle and impeller is not considered in the numerical simulation. These cause the simulated mass flow rate higher than [PERSON]'s experiment.