## 2 Computational Analysis  
Three-dimensional (3D) CFD analysis was performed for a mixed flow dual entry turbocharger turbine. The turbine was constructed by ABB turbo systems. The geometry map of the turbine and experimental data was taken from [PERSON] et al. (2010) [7]. For equal and unequal admission modeling, a whole turbine, which includes the double entry volute, a stator with 24 blades, a rotor with 12 blades, and a diffuser were used. The rotor and stator were modeled with Ansys BladeGen software and modified in Ansys DesignModeler. The volute model was constructed in SolidWorks 2016. All of the turbine components were assembled in DesignModeler. Table 1 records some of the geometry characteristics of the rotor and the stator. The computational analysis was performed using the ANSYS CFX 17 CFD package. CFX is a commercial CFD code and it's pre- and post-processors include many functions for the turbomachinary analysis. In a dual volute turbine, the flow around the rotor is introduced non-uniformly, so an acceptable result can only be obtained by taking all of the circumference into account. A frozen rotor interface was implemented between the rotor and the stator. A structured mesh was generated for the rotor and stator mesh using TurboGrid-11. In the tip clearance gap, at least 10 nodes were assumed. Different cell numbers were used to find the most proper mesh density; specifications of the trials for rotor and stator are depicted in Table 2. Between the applied grid resolutions, rows 4 and 5 show the least variation in the efficiency and mass flow. However, there is a significant difference in their CPU time. Therefore, as a balance between the precision, computational expenditure, and grid independence, mesh size in the fourth row of Table 3 was selected. Furthermore, to ensure that all of the flow features were simulated, contour plots at different streamwise locations were produced and compared with raising the mesh size, until the flow features remained without any changes. Figure 1 shows the structured mesh of the rotor and nozzle passages with detailed enlargements of the areas of interest. \begin{table}
\begin{tabular}{c c} Root mean radius at trailing edge of rotor [mm] & 52 \\ Length of axial chord of rotor [mm] & 40 \\ Tip gap height of rotor (\% of blade span) & 3 \\ Inlet cone angle of rotor & 55.1\({}^{\circ}\) \\ Exit cone angle of rotor & 7.2\({}^{\circ}\) \\ Nozzle vane angle & 70\({}^{\circ}\) \\ Total pressure ratio (Design point) & 2.1 \\ Design shaft speed 20,000 rpm & 53,344 \\ Hub-to-tip-ratio rotor blade & 0.84 \\ Nozzle throat diameter [mm] & 4.405 \\ Blade width of nozzle [mm] & 12.963 \\ \end{tabular}
\end{table} 
Table 1: Turbine geometry parameters. \begin{table}
\begin{tabular}{c c c c c} \hline \hline \multirow{2}{*}{**Trial**} & \multirow{2}{*}{**Number of Elements**} & \multicolumn{2}{c}{**Stage Total-to-Static**} & \multirow{2}{*}{**Mass Flow**} & \multirow{2}{*}{**CPU Time (h)**} \\  & & & **Efficiency (\%)** & & \\ \hline \multirow{3}{*}{1} & Nozzle & Rotor & & \\  & 153,545 & 254,354 & 58.354985 & 0.495454 & 12 \\
2 & 436,565 & 625,873 & 60.865447 & 0.502279 & 23 \\
3 & 835,463 & 1,135,512 & 62.096835 & 0.506682 & 46 \\
4 & 1,465,436 & 1,825,434 & 61.5592978 & 0.505397 & 75 \\
5 & 1,980,345 & 2,538,034 & 61.453565 & 0.505322 & 105 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Mesh intensity study. Figure 1: (**a**) Rotor blade mesh (**b**) Stator blade mesh. The finite volume method was used to discretize and solve the governing flow equations. The high-resolution scheme was used for the calculation of the advection term. The Reynolds number was \(6\times 10^{5}\) at the stator inlet, so the flow was assumed to be fully turbulent. The standard k-\(\epsilon\) was implemented for turbulence modeling. The root mean square (RMS) residual level was set as \(1\times 10^{-5}\), this is a good convergence by CFX [22] code from Ansys. Y+ values were obtained that were lower than two in most places. In the other areas, the maximum Y+ was 6.