## 2 Materials and Methods
### Numerical Simulation  
For the sake of this study, numerical simulations have been performed as a verification of the proposed methodology. CFD simulations have been realized for recreating the operation of the case study Pelton turbine and predicting the efficiency of the optimized model.  
CFD simulations have been carried out using the open-source CFD software OpenFOAM, which has been reported by [27; 28] to provide high-accuracy numerical results in Pelton turbine research. As shown in Figure 9, the computational domain is composed of two regions: rotating and stationary. To reduce the computational cost of the simulation, just a section comprised of only three half buckets has been taken into account according to the methodology proposed by [29].  
Figure 8: The 3D scan and resultant surface of the operating Pelton turbine.  
\begin{table}
\begin{tabular}{c c} \hline \hline
**Parameter** & **Value** \\ \hline B & 26 [cm] \\ L & 23 [cm] \\ D & 7.5 [cm] \\ F & 7 [cm] \\ M & 9.5 [cm] \\ E & 3.9 [cm] \\ \(\beta_{1}\) & 165.66\({}^{\circ}\) \\ \(\beta_{2}\) & 17.42\({}^{\circ}\) \\ \hline \hline \end{tabular}
\end{table}
Table 5: Geometric parameters of the 3D-scanned bucket.  
Figure 7: Resultant Pelton bucket 3D model.  
Two interconnected hexa-dominant meshes with refinements between the buckets and the jet walls were produced because of the discretization of both stationary and rotatory computational domains using the built-in OpenFOAM meshing program \"snap-pyHexMesh\" (Figure 10). The relative motion characteristic in the operation of the Pelton turbine has been replicated using the Arbitrary Coupled Motion Interface (ACMI) boundary condition provided in OpenFOAM version 8, taking into account the operational parameters of the \"Illuchi N\({}^{\circ}\)2\" hydro powerplant listed in Table 1.  
Using the OpenFOAM interFoam solver for incompressible, isothermal, and immiscible fluids, a two-phase approach in a transient state study was carried out to replicate the flow behavior across the bucket surface precisely. Based on earlier research [28]. the k-SST turbulence model was selected. Because the courant number plays a crucial role in numerical simulation, a time-adaptive system with an initial timestep of \(1\times 10^{-6}\) [s] and a maximum courant value of 1 has been established.  
The CFD simulation boundary conditions are based on the operating conditions of the \"Illuchi N2\" turbine detailed in Table 1. Because the domain has been split in half, \"symmetry\" boundary conditions have been set on the \"SymRot\" and \"SymStat\" patches. The \"JET_WALL\" and \"BUCKETS\" patches were set under the condition of non-slip wall boundary. The \"JET_INLET\" patch represents the region where water is introduced to the domain and has a \"flowRateInletVelocity\" boundary condition, while all other regions are considered open to the environment with a \"zeroGradient\" boundary  
Figure 10: Resulting mesh for the CFD simulation.  
Figure 9: Computational domains of the CFD simulation. (**A**) Rotatory domain and (**B**) stationary domain.  
condition. The interface between the rotating and stationary domains is achieved by using the \"cyclicACMI\" boundary condition. Detailed information about the boundary conditions of the simulation can be found in Tables A1 and A2.