# Mechanisms of Sweep on the Performance of Transonic Centrifugal Compressor Impellers
## Numerical Method and Validation  
### Numerical Method  
The simulation by computational fluid dynamics (CFD) is done with the solver EURANUS based on a three-dimensional steady, compressible, finite volume scheme to solve the Reynolds-averaged Navier-Stokes equations in the conservative formulation. To receive a credible viscosity resolution, spatial discretization is achieved with a modified Jameson central difference scheme. The fourth-order Runge-Kutta scheme is applied for temporal discretization. The convergence of the solver is accelerated by the multigrid procedure.  
Several turbulence models have been successfully applied to compressors. Near peak efficiency conditions, because the major flow phenomena (tip leakage flows, secondary flows and shock waves) are not essentially driven by viscosity, the basic physics can be well represented by simple turbulence models or even by the inviscid Euler equations [30]. Near surge conditions, significant differences between turbulence models occur because the predicted fully separated flow in blade passages is highly depended on the modeled turbulent viscosity, but there seems to be no universal turbulence model that is always superior to others [31]. Assessment of turbulence models in centrifugal compressors were carried out in the SRV2-O case [32] and the Radiver case [33]. It is generally found that the Spalart-Allamaras model, the k-\(\omega\) shear stress transport model, the v\({}^{2}\)-f-k-\(\varepsilon\) Durbin model and the Reynolds stress model can predict very similar flow features at the impeller peak efficiency condition, but the Spalart-Allamaras model has limitations in vaned diffuser flow fields where the fully separated flow is dominate. Considering both the accuracy for the impeller peak-efficiency flows and the calculation time, the Spalart-Allamaras one-equation model [34] is adopted.  
A multi-block structured grid is built to mesh the impeller. For the O4H topology of the impeller, it consists of 153, 69, and 43 nodes in the streamwise, spanwise, and pitchwise direction, respectively. The tip clearances of all blades are set constant to 4.4% of exit blade height. To predict a boundary layer resolution sufficiently fine for the Spalart-Allamaras model, a value of 0.001 mm is found appropriate for the first layer wall distance of the near-wall grid. The resulting local normalized wall distance y+ varies from 0 to 3. All fluid domains are calculated in the rotating reference frame, and thus no rotor-stator interfaces are needed. The final grid of the datum impeller has 2.3 million volume cells for single pitch, including around 0.2 million volume cells in tip gap regions. The final grid is shown in detail in Figure 4.  
Figure 4: Created computational mesh in detail.  
Total pressure, total temperature, and axial velocity direction are imposed at the inlet, and an average static pressure is imposed at the exit. The blades and casing surface are defined as rotational non-slip solid boundary and static non-slip solid boundary, respectively. For each rotation speed, the initial solution of the first simulation case is defined by estimation of velocity components, static pressure and static temperature for the whole domain. The former converged result is then used as the initial solution for the next case with higher backpressure. The step rise in backpressure at the near-surge condition is kept as 1 kPa. If no signs of numerical instabilities occur after 10,000 iterations, the solution is considered to have reached convergence.