# Surrogate-Based Optimization of a Centrifugal Pump with
## 4 CFD Setup  
The mesh generation and the flow-field have been computed using the 2020 R2 release of ANSYS [14]. The ANSYS CFX solver is used to solve the incompressible RANS (Reynolds Average Navier Stokes) equations coupled with the SST (Shear Stress Tensor) turbulence model [15]. The impeller inlet section has been extruded along the axial direction to avoid possible disturbance at the inflow due to the blade leading edge. The length of the inlet pipe is \(L=3D_{1}\), where \(D_{1}\) is the impeller inlet diameter. Only one blade passage is considered with periodic conditions. The mesh of the impeller is generated using the software ANSYS TurboGrid, while the mesh of the volute is generated using ANSYS FLUENT Meshing. The size of the elements  
Figure 8: Baffle tongue angle controlled by the design variable \(\alpha_{i}\). \begin{table}
\begin{tabular}{c c c c} \hline \hline
**Variable** & **Baseline** & **Min Value** & **Max Value** \\ \hline \(D_{2}\) & 70.1 mm & 97\% & 103\% \\ \(D_{0}/D_{2}\) & 0.589 & 95\% & 105\% \\ \(b_{2}\) & 8.1 mm & 90\% & 110\% \\ \(\frac{D_{2}-D_{1,k}}{D_{2}-b_{0}}\) & 0.739 & 90\% & 110\% \\ \(\frac{D_{2}-D_{1,k}}{D_{2}-D_{0}}\) & 1.00 & 90\% & 100\% \\ \(\hat{\beta}_{b1,k}\) & 29.5 \({}^{\circ}\) & 92\% & 108\% \\ \(\hat{\beta}_{b1,s}-\hat{\beta}_{b1,h}\) & 0 \({}^{\circ}\) & -5.0\({}^{\circ}\) & 0.0\({}^{\circ}\) \\ \(\hat{\beta}_{b2,h}\) & 40 \({}^{\circ}\) & 94\% & 106\% \\ \(\hat{\beta}_{b2,s}\) & 40 \({}^{\circ}\) & 94\% & 106\% \\ \(\gamma_{h}\) & 85 \({}^{\circ}\) & 88\% & 112\% \\ \(\gamma_{s}-\gamma_{h}\) & 0 \({}^{\circ}\) & -2.5\({}^{\circ}\) & 2.5\({}^{\circ}\) \\ \(\delta_{s}\) & 0 \({}^{\circ}\) & -2.5\({}^{\circ}\) & 2.5\({}^{\circ}\) \\ \(\frac{z_{1}}{b_{2}}\) & 0.5 & 0\% & 150\% \\ \(\frac{4(z_{2})}{z_{1}}\) & 1.0 & 0\% & 200\% \\ \(\frac{z_{5}-b_{2}}{b_{2}}\) & 0.742 & 34\% & 101\% \\ \(\frac{4(z_{2}-b_{2})}{z_{6}-b_{2}}\) & 1.0 & 0\% & 200\% \\ \(n_{b}\) & 6 & 5 & 7 \\ \hline \multirow{2}{*}{\(\Delta\)F} & \(R_{3}-D_{2}/2\) & 1.00 mm & 0.00 mm & 6.65 mm \\  & \(b_{3}/b_{2}\) & 1.00 & 1.00 & 1.925 \\ \hline \multirow{2}{*}{\(\Delta\)F} & \(A_{4}\) & 907 mm\({}^{2}\) & 80\% & 120\% \\  & \(\alpha_{i}\) & 30 \({}^{\circ}\) & 100\% & 133\% \\ \hline \hline \end{tabular}
\end{table} 
Table 3: List of the design variables (DVs) with the baseline values, the minimum/maximum values during the surrogate-based optimization (the percentage is computed with respect to the baseline value). adjacent to the solid walls is equal to an averaged non-dimensional distance \(y^{+}\approx 20\) and \(y^{+}\approx 4\) for the impeller and solute, respectively. CFX automatic wall treatment is applied to the blade wall, hub and shroud, i.e., CFX automatically switches from a wall function approach to a low Re approach, depending on the grid spacing near the wall. At the domain inlet the volumetric flow rate \(\dot{Q}=7.33\times 10^{-3}/\text{m}^{3}/\text{s}\), the turbulence intensity \(Tu_{0}=4\%\), and the ratio \(\left(v_{t}/v\right)_{0}=10\) are prescribed. The corresponding turbulent kinetic energy, \(k_{0}\), and the specific dissipation rate, \(\omega_{0}\), are computed as  
\[k_{0}=\frac{3}{2}U_{0}^{2}Tu_{0}^{2},\]  
\[\omega_{0}=\frac{k_{0}}{\
u}\Big{(}\frac{v_{t}}{\
u}\Big{)}^{-1},\]  
where \(U_{0}=4\dot{Q}/(\pi D_{0}^{2})\) is the inlet velocity. At the outflow a static pressure \(p_{4}=0\)\(Pa\) is set. The no-slip adiabatic condition is applied to the blade walls, hub and shroud. Steady-state simulations are performed using the multiple reference frame (MRF) approach, which implies no relative mesh motion between the rotating and stationary parts. In the rotating reference frame, where the relative velocity is computed, the momentum equation is modified, adding Coriolis and centrifugal terms. The interface between moving and fixed domain is treated using the mixing plane approach.