*4.2. Meshes*

ANSYS-ICEM-CFD 14.5 software [28] was used to build the structured meshes associated with the block topology of Y-type and O-type. The mesh growth rate of boundary layer were considered to ensure the overall mesh thickness and density. The appropriate mesh density was decided according to the gird independence test [29,30]. Table 1 summarizes five schemes of different mesh numbers. By comparing the pump performance predicted by the same numerical methods we found that with the increase of mesh number, the numerical value of single-stage head, single-stage power, and efficiency show a stable trend. Between the schemes No. 4 and No. 5, increasing mesh has no influence on the simulation results, which means that the scheme No. 4 has enough accuracy with enough mesh density. Therefore, by considering the grid independence test and the computer capability, scheme No. 4 was selected as the optimal scheme of mesh for the numerical investigation. For the whole single-stage computational domain, the total of mesh elements is almost 4.9 million. Meanwhile, it was ensured that the entire computational domain 30 < y<sup>+</sup> < 60, which indicates that the near-wall mesh nodes are in a log-law layer. Figure 4 is the final mesh used for the impeller and the diffuser.


**Table 1.** Grid independence test.

**Figure 4.** Structured mesh of the impeller and diffuser.

## *4.3. Numerical Settings*

ANSYS-Fluent 14.5 software [31] was used to run the numerical simulation for this study, in which the SST *k*-ω turbulence model, and the SIMPLEC algorithm was used to solve the discrete difference equations of the second-order upwind scheme. As shown in Figure 5, no-slip boundary conditions were used on the wall surface, inlet boundary conditions of mass flow were used on the pump inlet, and outlet boundary conditions of pressure were used on the outlet of the pump. For instance, the mass flow rate for inlet was set as 10 kg/s at the design flow rate, and the total pressure for the outlet was set as 10,135 Pa. Using sliding grid technology, the impeller region in the flow channel was set to be a rotating grid coordinate system provided by ANSYS-Fluent, while the diffuser and other hydraulic components were set to be a stationary coordinate system. After reaching convergence of steady calculation based on the fixed rotor coordinate system (Frozen Rotor), the flowfield was used as the initial value to start the unsteady calculation. The Principle of a Frozen Rotor is to set the impeller part to be a rotating reference coordinate system, and the static and dynamic interface is coupled by combing with sliding mesh technology [32,33].

**Figure 5.** Boundary conditions.

#### *4.4. Time Step*

In general, in the periodic numerical simulation, the time step needs to satisfy the Courant number criterion [34], which is expressed as:

$$\mathcal{C}\_o = \frac{|\overline{v}|\Delta t}{l} \le 100. \tag{12}$$

In the above formula, \$ \$ \$*v* \$ \$ \$ is the absolute value of the estimated mean velocity, *<sup>l</sup>* is the smallest size of the grid, and *Co* is required to be no more than 100. When the numerical convergence is not good, it is appropriate to take smaller values.

According to the requirement of sampling theorem, 2.56–4 times of the signal maximum frequency is selected generally for the time step. In this study, the impeller has five blades, the rotational speed is 2850 r/min, so the blade passing frequency (BPF) is 332.5 Hz. If there are at least seven points in a BPF cycle, and the desirable maximum value of the time step is 4.2966 <sup>×</sup> <sup>10</sup>−<sup>4</sup> s accordingly.

If the time step size is too large, some minor changes of the pressure will not be captured, but time steps that are too small will also lead to a significant increase in computing time [35,36]. Therefore, considering the computer configuration, the time step *t* was chosen as 5.8478 <sup>×</sup> 10−<sup>5</sup> s, the impeller rotated one degree for one time step, 360 time steps were required for each rotation of the impeller. For this model, after 3600 time steps, that is, after 10 cycles of impeller rotation, the pressure fluctuation was periodic and the convergence condition was determined [37,38]. Defining this time as *t* = 0, and selecting a whole circle of the impeller rotation (360 time steps) as the analysis period for unsteady flow.
