*2.1. Simulation Method*

The pump was modeled using Creo 2.0 software. Figure 2 is the main water body model of its computational area, including the inlet section, impeller, volute shell, outlet extension section, etc. The leakage loss of seal ring and balance hole, friction loss of the disc at the front and rear cover plate of the impeller were taken into account when establishing the model. During the numerical simulation of turbulence flow in the low-specific-speed centrifugal pump, the Reynolds averaged Navier-Stokes (RANS) method was used, and the renormalization group (RNG) k-ε turbulence model considering the effects of separated flow and eddy flow was selected [14]. The turbulence model governing equations are as follows:

$$\frac{\partial}{\partial t}(\rho k) + \frac{\partial}{\partial \mathbf{x}\_i}(\rho k u\_i) = \frac{\partial}{\partial \mathbf{x}\_j}[(a\_t k \mu\_{eff} \frac{\mu\_t}{\sigma\_k}) \frac{\partial \mathbf{k}}{\partial \mathbf{x}\_j}] + \mathbf{G}\_k + \mathbf{G}\_b - \rho \varepsilon - \mathbf{Y}\_M + \mathbf{S}\_k \tag{1}$$

$$\frac{\partial}{\partial t}(\rho \varepsilon) + \frac{\partial}{\partial \mathbf{x}\_i}(\rho \varepsilon u\_i) = \frac{\partial}{\partial \mathbf{x}\_j}[(a\_t k \mu\_{eff} \frac{\mu\_t}{\sigma\_k}) \frac{\partial \varepsilon}{\partial \mathbf{x}\_j}] + \mathbf{C}\_{1\varepsilon} \frac{\varepsilon}{k} (\mathbf{G}\_k + \mathbf{C}\_{3\varepsilon} \mathbf{G}\_b) - \mathbf{C}\_{2\varepsilon} \rho \frac{\varepsilon^2}{k} + \mathbf{S}\_{\varepsilon} \tag{2}$$

**Figure 2.** Water body model.

Compared with standard k-ε turbulence model, the rotation effect on α*<sup>k</sup>* and αε has been considered in the above formula, and the other terms have the same meaning as the standard k-ε turbulence model.

The boundary condition at the outlet was chosen as the pump's flow rate, while the boundary condition at the inlet was chosen as the total pressure, and the reference pressure was set be 1.0 atm at the inlet. The walls formed by the impeller were defined as the rotating boundary and its rotating speed was 2880 r/min, the other walls were defined as the non-slip boundary, and the wall roughness was set to be 0.025 mm uniformly. Simulations were carried out using the commercial software ANSYS-CFX, the governing equations were discretized using the finite volume method, the pressure term was solved using the central difference scheme, the velocity term was solved using the second-order upwind difference scheme, the turbulent kinetic energy term and the turbulent energy dissipation rate term were solved using the second-order upwind difference scheme, and the near-wall flow was approximated using the standard wall function method. The convergence accuracy was set to 10<sup>−</sup>5. In this paper, unstructured tetrahedral meshes were used to divide the computational water domain. The grid independence of numerical simulation was studied under a design flow rate, and it was found that when the number of grids was more than 3.9 million, the fluctuation of the head and hydraulic efficiency was small, and the relative fluctuation range was less than 1%; therefore, it can be considered that the number of grids had no effect on the calculation results.

#### *2.2. Experimental Method and Result*

The test bench mainly included a turbine flow-meter, valve, pressure transmitter, speed sensor, data acquisition instrument, etc. The valve at the outlet was used to control the flow rate, the pressure sensor was used to measure the inlet and outlet pressure of the pump, and the power of the pump was also measured and calculated. The head (H) and efficiency (η) comparison between the simulation and experiment is shown in Figure 3. It can be found that the simulation value was slightly higher

than the experimental value, the maximum relative error of head was about 4%, and the maximum relative error of efficiency was about 2%. Because of the complexity of the internal flow in the low-specific-speed centrifugal pump, the existing turbulence models could not accurately adapt to simulate the complex effects of the surface curvature, Coriolis force, and centrifugal force. There were also some manufacturing errors in the model pump, and there were inevitable errors in the head and efficiency obtained from experiments and simulation; however, the trends under different flow rates was close.

**Figure 3.** Comparison of simulation and experimental results.

#### **3. Internal Flow Characteristic Analysis**

In order to study the near-wall flow characteristics of the centrifugal pump's impeller with a low specific speed, the blades were numbered I, II, III, IV, and V; also, the flow channels between the blades were numbered 1, 2, 3, 4, and 5, respectively, as shown in Figure 4. The profiles of impeller blade I in the middle section with the distance of 0.5 mm and 2 mm are marked as lpI-0.5 and lpI-2 on the pressure side, and lsI-0.5 and lsI-2 on the suction side, respectively. The profiles of the impeller blade 2 in middle section are marked as lpII-0.5, lpII-2, lsI-0.5, and lsII-2 in accordance with the distance of 0.5 mm and 2 mm, as appropriate. Similar marking methods were used for the near-wall profiles of blades III, IV, and V.

**Figure 4.** Near-wall profiles of blades.

## *3.1. Whole Static Pressure and Relative Velocity*

From the static pressure distribution shown in Figure 5, it can be seen that, the static pressure increased gradually from the impeller inlet to the volute outlet, and the pressure distribution characteristics in the flow channels of 1, 2, 3, 4, and 5 were generally similar. The static pressure in the flow channels of Q = 7 m3/h was almost the same as that of Q = 13 m3/h. When increasing the flow rate to 20 m3/h, the static pressure in the flow channels decreased obviously. The area of low pressure in channel 5 was the largest. The static pressure in the volute of Q = 7 m3/h was larger than that of Q = 13 m3/h and Q = 20 m3/h, and the relative pressure at the wall of the volute was larger than that at the outlet of the impeller.

**Figure 5.** Static pressure distributions under different flow rates.

From the relative velocity distributions shown in Figure 6, it can be seen that the relative velocity increased with the increasing of flow rate. For Q = 7 m3/h, the relative velocity in the impeller blade channels and diffusive sections of volute shell was small, and the relative velocity from the tongue to the throat of the volute shell was large. For Q = 13 m3/h, the relative velocity inside the impeller increased obviously and the relative velocity near the pressure sides of blades was obviously less

than that near the suction sides of blades. When the flow rate increased to Q = 20 m3/h, the relative velocity increased obviously, both inside the impeller and inside the volute; however, there was a local low-speed zone on the suction sides of blades.

**Figure 6.** Relative velocity distributions under different flow rates.

#### *3.2. Pressure Distribution Near the Wall Region in the Impeller*

Figure 7 shows the static pressure distributions of profiles at the distance of 0.5 mm from the blades with Q = 13 m3/h. The pressure of the profiles at the distance of 0.5 mm from blade I is shown with a black solid line on the pressure side and with a black dotted line on the suction side, and the other pressure of profiles from blades II, III, IV, and V are shown with their respective colorful lines. The pressure distributions of near-wall profiles on pressure sides, as well as on the suction sides of five blades, were almost the same, and the pressure on the pressure sides was greater than that on the suction sides. The pressure on the pressure side at the outlet of blade I was slightly higher than that of other blades due to the affection of the tongue separation.

**Figure 7.** Static pressure distributions of profiles at the distance of 0.5 mm from the blade with Q = 13 m3/h.

Figure 8 shows the static pressure distributions of the profiles near the wall under different flow rates on blade I, where the smaller the flow rate was, the greater the pressure on the pressure sides and the suction sides of the blades was. The pressure of the profiles at a distance of 2 mm on the pressure side was greater than that at a distance of 0.5 mm on the pressure side, but the pressure of the profiles at a distance of 2 mm on the suction side was less than that at a distance of 0.5 mm on the suction side. For Q = 7 m3/h, 13 m3/h, and 20 m3/h, the pressure difference on the pressure sides between the radii of 20 mm to 60 mm was very little, and the pressure difference on the pressure sides between the radii of 60 mm to 73 mm became obvious. For Q = 7 m3/h and 13 m3/h, the pressure on the pressure sides of the near wall kept increasing. For Q = 20 m3/h, the pressure even decreased slightly with increasing radius. The pressure on the suction sides near the wall generally decreased with the increase of flow rates, especially when the flow rate increased to 20 m3/h, where the lowest pressure appeared

at the radius of 25 mm. Compared with the pressure on the suction side at Q = 7 m3/h, the pressure decreased to about 40,000 Pa, and the pressures at distances of 0.5 mm and 2 mm on the suction side interlaced, which shows the complexity of the flow.

**Figure 8.** Static pressure distributions of profiles near wall region at different flow rates.
