**1. Introduction**

A submersible tubular pump is a kind of horizontal pump with a low head and large discharge, which uses a postpositive tubular-type structure with a motor and pump coaxial. It has the advantages of low cost, high efficiency, and easy-to-realize automatic or semi-automatic control [1,2]. In recent years, this type of pump has been widely used in small and medium-sized pumping stations, such as in agricultural irrigation and urban flood control, especially in the plain areas [3–5]. All pumps experience pressure pulsation due to changes, discontinuities, and variations that occur in their pumping or pressure generating action, and submersible tubular pumps are no exception. The pressure pulsation and unstable flow in the vane pump is mainly caused by the rotor–stator interaction between the

impeller and the guide vane. These pulsations can sometimes be very severe and cause damage to the piping or other components in a pumping system, which may give rise to vibration [6–9], generate hydraulic noise [10–12], and affect the performance of the pumping system, thus affecting the stable operation of the pumping system. Therefore, the distribution of pressure pulsations in the pump needs to be studied to ensure the safe, efficient, and stable operation of the pumping station.

With the development of computational fluid dynamics (CFD) technology, more scholars are using CFD to study complex flow fields in pumps [13–15], but the results of numerical simulation need to be verified by experimental data. Therefore, combining numerical simulation and experiments is more reliable. To ensure the safe and stable operation of pumping stations, many researchers are paying attention to the pressure pulsation and the unsteady flow inside the centrifugal pumps [16–23] and axial-flow pumps [24–29]. Studies on tubular pumps are relatively rare. Yang et al. [30] studied the pressure fluctuation of an S-shaped shaft extension tubular pumping system by CFD and experimentation, where the pressure fluctuations at 21 measurement locations in inlet and outlet passages were obtained and analyzed in time and frequency domains for three typical working conditions of different flow rates. Zhang et al. [31] investigated the three-dimensional turbulent flow and the pressure fluctuation in a submersible axial-flow pump by adopting the RNG (Renormalization Group) k-ε turbulence model and the SIMPLEC (Semi-Implicit Method for Pressure-Linked Equation) algorithm, with which the pressure pulsation distribution of the impeller inlet and outlet was obtained.

In this paper, an experimental system for model and pressure pulsation tests is built to validate the numerical simulation results using six transient pressure sensors in different sections of the pump. Unsteady numerical simulations are used to reveal the complex flow fluctuations, and the fast Fourier transform (FFT) method is used to obtain the amplitudes of pressure fluctuations. The results can provide references for further analysis of the pressure fluctuation of submersible tubular pumps, and ensure the safe and stable operation of submersible tubular pump stations.

#### **2. Numerical Simulation**

#### *2.1. Pump Geometry*

The simulated object is a submersible turbine pump device. Figure 1 shows a single-line diagram of the pump used in the numerical simulation and experiment, including the inlet passage, impeller, guide vane, bulb unit, and outlet passage. The dimensions given in the figure are values relative to the diameter D of the impeller. The main geometric parameters of the pump device are shown in Table 1.

**Figure 1.** Single-line diagram of the pumping system.


**Table 1.** Parameters of the model pump.

#### *2.2. Pump Modeling*

The numerical simulation study in this paper is for the entire submersible tubular pump device, in which the inlet passage, the outlet passage, and the bulb unit are modeled by Unigraphics NX (11.0, Siemens PLM Software, Shanghai, China, 2016) for 3-D solid modeling, as shown in Figure 2a. The impeller and guide vane components are generated automatically in the TurboGrid software (14.5, ANSYS Inc., Pittsburgh, PA, USA, 2013); as shown in Figure 2b, the distance between the blade tip and the impeller chamber is set to 0.2 mm.

**Figure 2.** A 3-D model of the pump device: (**a**) passages and bulb unit; (**b**) impeller and guide vane.

### *2.3. Numerical Model and Grid Generation*

The numerical simulation of this paper adopts the current common commercial CFD software ANSYS CFX-14.5 (14.5, ANSYS Inc., Pittsburgh, PA, USA, 2013), which performs the steady and unsteady calculations for the submerged tubular pump devices under different working conditions. The three-dimensional Reynolds-averaged Navier–Stokes equations were solved by CFX code. The turbulence effects were modeled by the standard k-ε turbulence model. The pressure–velocity coupling was performed using the SIMPLEC algorithm. The criterion for convergence was considered to be 10<sup>−</sup>4, allowing an optimal number of iterations for each time step.

In this calculation, structured hexahedral cells were used to define the computational domain. The grids of the inlet passage, bulb unit, and outlet passage were generated by ICEM-CFD (14.5, ANSYS

Inc., Pittsburgh, PA, USA, 2013), while the grids of the impeller and guide vane were generated by TurboGrid (14.5, ANSYS Inc., Pittsburgh, PA, USA, 2013). In order to ensure the grid quality, the grid independence calculation was carried out, and the total grid number was about 4.19 <sup>×</sup> 106. Figure 3 shows the grid details for each component of the pumping system.

The boundary conditions were set as follows: the inlet pressure was specified at the entrance of the inlet passage. The inlet adopts the total pressure and the pressure is set to 1 for the atmosphere. The mass outflow condition was defined at the exit of the outlet passage. The transient rotor–stator model was used for the unsteady calculation. The shroud of the impeller was set as absolutely stationary, and the blade and hub of the impeller were relatively stationary. No slip boundary conditions or wall functions were used for the solid walls.

In this paper, the result of the steady calculation was taken as the initial flow field of the unsteady calculation, and then the unsteady numerical simulation was carried out using the sliding mesh technique. The time step of the unsteady calculations was <sup>Δ</sup>*<sup>t</sup>* <sup>=</sup> 3.4483 <sup>×</sup> <sup>10</sup>−<sup>4</sup> s. The impeller rotated 3◦ at each time step, so it took 120 steps to complete the rotation. The chosen time step was small enough to get the necessary time resolution.

#### **3. Experiment System**
