## 2 Numerical Simulation
### Boundary Conditions and Solver Settings  
The commercial software ANSYS Fluent 2023R2 is employed to solve the unsteady flow field inside the centrifugal pump under five different flow conditions, i.e., 0.8\(Q_{d}\), 0.9 \(Q_{d}\), 1.0 \(Q_{d}\), 1.1 \(Q_{d}\), and 1.2 \(Q_{d}\), while \(Q_{d}\) is the rated flow listed in Table 1. The rotational speed of the impeller remains constant at 2900 r/min for each flow condition. For each flow condition, a steady-state calculation is first conducted to provide the initial flow field for the unsteady calculation. In the steady-state calculation, the fluid medium is set as water at room temperature, with a density of 998.2 kg/m\({}^{3}\) and a dynamic viscosity of 1.006 \(\times\) 10\({}^{-3}\) Pa\(\cdot\)s. A velocity inlet condition is applied at the pump inlet, and the velocity magnitude is calculated based on the flow rate under the corresponding condition and the pump inlet area. The outflow boundary condition is imposed at the outlet pipe termination to emulate hydrodynamically developed free-stream conditions. This configuration is physically justified by the extended discharge section (see Figure 1), which provides sufficient flow development length to dampen flow asymmetries induced by the impeller's rotational effects. The \"outflow\" boundary condition optimizes centrifugal pump simulations by focusing computation on critical regions (impeller/volute), preventing artificial outlet constraints from distorting upstream flow. The Multiple Reference Frame (MRF) model is used to handle the flow in the impeller region. The mesh of the impeller itself is treated as a stationary grid region, and the \begin{table}
\begin{tabular}{c c c} \hline \hline
**Fluid Domain** & **Element Number** & **Node Number** \\ \hline Inlet pipe & 1,093,640 & 2,806,035 \\ Suction region & 423,445 & 1,089,239 \\ Impeller region & 2,349,537 & 6,029,682 \\ Discharge chamber & 4,224,759 & 10,842,508 \\ Outlet pipe & 447,719 & 1,157,567 \\ Total & 8,539,100 & 21,925,031 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Number of elements and nodes in each fluid domain. Figure 4: Calculated head and hydraulic efficiency results with different grid number. centrifugal effect due to its high-speed rotation is considered through an inertial coordinate system. A stage average condition is applied at the interface between the impeller region and the stator regions (such as the suction chamber and volute) to exchange flow field information, including velocity and pressure distribution. All wall surfaces are set with a \"no-slip\" condition. Referring to the manufacturer's process standards, the inner wall surfaces of the suction chamber and volute are given a roughness of 100 \(\upmu\)m, while the rest wall surfaces are set to a roughness of 50 \(\upmu\)m. Meanwhile, a standard wall function with semi-empirical formulas is used in the near wall region. This function simplifies the calculation and effectively connects the flow field in the near wall viscous sub-layer and the turbulent flow in the main flow region. The Semi-Implicit Method for Pressure Linked Equations (SIMPLE) algorithm is used for the solution. It is a semi-implicit pressure-velocity coupling algorithm that corrects the velocity and pressure fields by constructing a pressure correction equation, ensuring that the calculated velocity field satisfies the continuity equation. For each governing equation, a root mean square (RMS) convergence accuracy of \(10^{-4}\) is specified for computational convergence. The results of the steady-state calculation are used as the initial conditions for the unsteady calculation. Meanwhile, on the basis of the steady-state calculation settings, the MRF model is disabled, and the dynamic mesh technology is adopted. The impeller region is set as \"Mesh motion\" to accurately simulate the real flow in the impeller region.