Numerical Investigation of Pressure Fluctuation in Centrifugal Pump Volute Based on SAS Model and Experimental Validation

Abstract

This paper presents an investigation of pressure fluctuation of a single-suction volute-type centrifugal pump, particularly volute casing, by using numerical and experimental methods. A new type of hybrid Reynolds-averaged Navier-Stokes/Large Eddy Simulation, referred to as the shear stress transport-scale-adaptive simulation (SAS) model, is employed to study the unsteady flow. Statistical analysis method is adopted to show the pressure fluctuation intensity distribution in the volute channel. A test rig for pressure pulsation measurement is built to validate the numerical simulation results using eight transient pressure sensors in the middle section of the volute wall. Results show that the SAS model can accurately predict the inner flow field of centrifugal pumps. Radial force acting on the impeller presents a star distribution related to the blade number. Pressure fluctuation intensity is strongest near the tongue and shows irregular distribution in the pump casing. Pressure fluctuation is distributed symmetrically at the cross-section of the volute casing because the volute can eliminate the rotational movement of the liquid discharged from the impeller. Blade passing frequency and its multiples indicate the dominant frequency of the monitoring points within the volute, and the low-frequency pulsation, particularly in the shaft component, increases when it operates at off-design condition, particularly with a small flow rate. The reason is that the vortex wave is enhanced at the off-design condition, which has an effect on the axle and is presented in the shaft component in the frequency domain.

1. Introduction

Centrifugal pumps, as essential energy-conversion and fluid-transporting devices, have been widely used in industry, agriculture, ship propulsion, and daily life [1]. Owing to the rotor-stator interaction between the asymmetric structure of the volute and the high-speed rotating impeller as well as a highly viscous fluid, the operation of centrifugal pumps can generate instability and pressure pulsations, which may be detrimental to the integrity and performance of the pump and may result in component fatigue, excessive vibration, and noise. With the trend in increasing rotation speed and power, pressure fluctuation in centrifugal pumps has become an urgent concern [2, 3].

Numerous studies on unsteady flow have compared experimental and numerical results in centrifugal pumps [4, 5]. Generally, the volute of the centrifugal pump is one of the major parts because it is directly connected to the external space. It is always designed as an Archimedes spiral, which could result in better pump performance, that is, strongest collection of water out of the impeller. However, limited studies have been conducted on pressure fluctuation of the inner flow in the volute. Furthermore, because the experimental method is time consuming and costly, investigation methods for complex fluid flow can be replaced or complemented by numerical simulation with the development of computational fluid dynamics (CFD). Today, most CFD simulations are conducted with traditional Reynolds-averaged Navier-Stokes (RANS) equations. Using RANS for many flows is not suitable because the turbulent part can be extremely large and have the same order as the mean. Examples are unsteady flow in general, particularly flows with large separation in centrifugal pumps. For this type of flows, using large eddy simulation (LES) is more appropriate. Numerous studies have been conducted on flow in rotating machinery based on the LES method [6–8]. However, the LES method remains too costly for industrial application. Pure LES also requires extremely fine grids, particularly in boundary layers, and the generation of boundary conditions is more complex. For this reason, the hybrid RANS/LES concept has been developed, such as detached eddy simulation in which the attached turbulent boundary layer is modeled with standard RANS and the separated regions are considered in an LES-like model. This concept has shown promising results. For example, Feng et al. [9] have used it to study the part-load condition of the radial diffuser pump, but the switching between the LES and RANS modes depends on the local grid size and may lead to grid-induced separation in attached boundary layers. Therefore, a model named scale-adaptive simulation (SAS) is proposed to solve this problem. SAS is an improved URANS model, with LES capability in unstable flow regions, which is the extension of Menter's SST k-ω model to a SAS formulation, according to Menter and Egorov [10, 11]. This concept has provided significant insights, such as those presented in the work of Lucius and Brenner [12] and Zhang et al. [13].

In our study, a new type of hybrid RANS/LES, SAS based on the SST method, is employed to examine the unsteady flow in the centrifugal pump, particularly the volute casing. A new method called pressure pulsation intensity analysis is proposed to exhibit the performance of the pressure pulsation on the entire volute casing. A test rig for pressure pulsation measurement is built to validate the numerical simulation results using eight transient pressure sensors in the middle section of the volute wall. Mathematical statistics and frequency domain analysis of pressure are conducted at the eight monitoring points distributed in the middle span of the pump flow field.

2. Numerical Modeling

2.1. SAS Based on SST k-ω Model Approaches

To resolve the unsteady turbulence flow in the centrifugal pumps, we adopt a type of SAS in the ANSYS CFX 14.5 based on the SST model, which is also a single rotating frame method. The SAS model was invented by Menter and colleagues [10, 11]. The idea behind the SST-SAS k-ω model is to add a production term, the SAS term, in the ω equation, which is sensitive to resolved (i.e., unsteady) fluctuations. The governing equations of the SST-SAS model differ from those of the SST RANS model because of the additional SAS source term Q_SAS in the transport equation for the turbulence eddy frequency ω, which is expressed as follows:

$\begin{array}{c}\frac{\partial \rho k}{\partial t}+\frac{\partial }{\partial x_j}\left(\rho U_{j}k\right)\hspace{1em}=P_k-\rho c_{\mu }k\omega \hspace{1em}\hspace{1em}+\frac{\partial }{\partial x_j}\left[\left(\mu +\frac{{\mu }_t}{{\sigma }_k}\right)\frac{\partial k}{\partial x_j}\right],\\ \frac{\partial \rho \omega }{\partial t}+\frac{\partial }{\partial x_j}\left(\rho U_j\omega \right)=\alpha \frac{\omega }{k}{P}_k-\rho \beta {\omega }^{\mathrm{2}}+Q_{\text{SAS}}\phantom{\text{hhhhhhhhhhhhhhhh}}+\frac{\partial }{\partial x_j}\left[\left(\mu +\frac{{\mu }_t}{{\sigma }_{\omega }}\right)\frac{\partial \omega }{\partial x_j}\right]\phantom{\text{hhhhhhhhhhhhhhhh}}+\left(\mathrm{1}-F_{\mathrm{1}}\right)\frac{\mathrm{2}\rho }{{\sigma }_{\omega \mathrm{2}}}\frac{\mathrm{1}}{\omega }\frac{\partial k}{\partial x_j}\frac{\partial \omega }{\partial x_j},\\ Q_{\text{SAS}}=\max [\rho {\xi }_{\mathrm{2}}\kappa S^{\mathrm{2}}{\left(\frac{L}{L_{\nu K}}\right)}^{\mathrm{2}}-C\phantom{\text{hhhhhhhhhh}}·\frac{\mathrm{2}\rho k}{{\sigma }_{\Phi }}\max (\frac{\mathrm{1}}{{\omega }^{\mathrm{2}}}\frac{\partial \omega }{\partial x_j}\frac{\partial \omega }{\partial x_j},\phantom{hhhhhhhhh\text{h}hhhhhhhhh}\frac{\mathrm{1}}{k^{\mathrm{2}}}\frac{\partial k}{\partial x_j}\frac{\partial k}{\partial x_j}),0].\end{array}$

(1)

Interpretation of the equations and details of the models can be found in the work of Davidson et al. [14–16]. When the flow equations resolve turbulence, the length scale based on velocity gradients is considerably smaller than that based on time-averaged velocity gradients. Thus, the von Karman length scale, L _vK , is an appropriate quantity to use as a sensor to detect unsteadiness. In regions where the flow tends to be unsteady, the objective of the SAS term is to increase ω. The result is that k and v _t are reduced so that the dissipating (damping) effect of the turbulent viscosity on the resolved fluctuations is reduced, thereby promoting the momentum equations to switch from steady to unsteady mode.

To model the flow near the wall, automatic near wall treatment has been used in the SST-SAS model and unsteady SST model. In the LES simulation, the Van Driest wall damping function is used to model the flow near the wall. The transient term is discretized through second-order backward Euler method. The advection term is discretized through high-resolution scheme in ANSYS CFX 14.5. It is blended between central differencing and upwind differencing locally.

2.2. Calculation Model and Grid Generation

A commercial single-stage, single-suction, horizontal-orientated low specific speed centrifugal pump with a six-blade impeller was selected as the model. The design parameters of the pump are shown in Table 1. The casing of the pump is typically combined with a spiral-volute unvaned annulus. In design process of such low specific speed centrifugal pump, the increased flow rate design method was used to improve the efficiency at the design point. The pump was divided into component parts such as the suction inlet, pump impeller, and volute to build a numerical model for a complete pump, as shown in Figure 1. This process would allow each mesh to be individually generated and tailored to the flow requirements in that particular component. The influence of boundary conditions was investigated to discard any effect on the numerical results, particularly on the discharge channel, and to verify the capabilities of the model. Therefore, we assumed that the flow closer in a fully developed condition at the inlet and outlet would provide better results for pressure amplitude levels, whereas a pressure outlet imposed at the inlet and outlet would significantly influence pressure variations [17].

Table 1:

Pump parameters.

Parameters	Value
Flow rate Q d /m3·h−1	25
Head H d /m	32
Rotation speed n d /r·min−1	2900
Blade width at the impeller outlet b2/mm	7
Suction diameter D s /mm	65
Exhaust diameter D d /mm	50
Outer diameter of the impeller D2/mm	165
Base diameter of volute D3/mm	176

Figure 1:

3D model of numerical domain.

The grids for the computational domains were generated using the grid generation tool ICEM-CFD 14.5 with blocking method. The grid details in the rotating domain and the volute wall are partially shown in Figure 2. The independence of the solutions from the number of grid elements was proven by simulating the flow field with different numbers of grid elements. The resulting pump model consisted of 3564 708 elements for rotating and stationary domains in total. Structured hexahedral cells were used to define the inlet, impeller, and volute domains, which had 748 274, 1488 384, and 1328 050 elements, respectively. The maximum nondimensional wall distance y⁺ < 10 was obtained in the complete flow field, which could satisfy the requirement of all turbulence modeling methods used in this paper. For temporal discretization, the time step size for unsteady flow was set to 2.87E − 5 seconds, equivalent to the time for the impeller to rotate at 0.5 degree. The total simulation time is for the impeller rotating 8 revolutions. The flow field was statically stable after 5 revolutions and data on the last 3 revolutions were maintained for pressure analysis.

Figure 2:

Details of grid view.

2.3. Statistical Analysis Theory of Pressure Fluctuation Intensity

Identifying the pressure pulsation intensity distribution at the flow channel can help us optimize the volute design. In previous studies, only a few monitoring points were set on the computational domains to study the unsteady pressure fluctuations as the time and frequency domains were analyzed. Thus, pressure fluctuations could not be easily investigated in the entire domain. In this paper, statistical methods were adopted to analyze the pressure fluctuation intensity on each grid node in the fluid domains. In statistics, standard deviation generally shows how much dispersion exists compared with the average. A lower standard deviation value indicates that the data points are closer to the mean value during a specified period. A higher pressure standard deviation value indicates larger pressure fluctuations [18].

The pressure fluctuations are presented in a normalized form to allow the scaling of pressure pulsation data with respect to size and speed. Therefore, a nondimensional pressure coefficient, C _P , is defined in (2) to determine the magnitude of the pressure fluctuations for an entire revolution period. C _P is calculated using the standard deviation of the unsteady pressure normalized by the dynamic pressure based on the impeller tip speed, U₂. The pressure on any grid node i can be given as P _i (x,y,z,t). The pressure coefficient, which represents the normalized pressure, is defined as follows:

$C_{P_i}=\frac{\left(P_i-P_{\text{ref}}\right)}{{\mathrm{0.5}\rho U}_{\mathrm{2}}^{\mathrm{2}}}.$

(2)

The average pressure coefficient in any period can be calculated with the following equation:

$\overline{C_P}=\frac{\mathrm{1}}{N}{\displaystyle \sum }_{n=\mathrm{0}}^{N-\mathrm{1}}{C}_P\left(x,y,z,\frac{n}{N}T\right),$

(3)

where T is the period of one impeller revolution and N, equal to 720 in this paper, is the recorded number of one impeller revolution.

The standard deviation of the pressure coefficient, which can describe pressure fluctuation intensity, can be calculated with the following equation:

$C_{Psdv}=\sqrt{\frac{{{\displaystyle \sum }}_{n=\mathrm{0}}^N{\left(C_P(x,y,z,(n/N\left)T\right)-\overline{C_P}\right)}^{\mathrm{2}}}{N-\mathrm{1}}.}$

(4)

In the CFX solver, most variables, such as pressure, are global variables that can be read from each grid node in the calculation domain. Therefore, using the expression language in CFX and the frozen copy function, we can express all of the statistical coefficients related to the results for the entire impeller revolution period, and we can establish the corresponding global variables. Then, the statistical results on each grid node can be obtained by reading the variables.

3. Results of Numerical Calculation

3.1. Analysis of Radial Force Acting on the Impeller

The traditional theory of centrifugal pump design assumes no radial force acting on the impeller in the most efficient operating condition because pressure is distributed uniformly in every cross-section of the spiral volute. Moreover, the radial force appears because the flow velocity in the impeller and volute is unequal when the pump does not operate in the most efficient condition and remains constant [19]. In fact, changing pressure is distributed in the centrifugal pump cavity because of the interference effects between the impeller and volute tongue, which results in unsteady radial force. Figure 3 illustrates the changing law of the radial force acting on the impeller in five operating conditions, where vector coordinates of a point represent the magnitude and direction of the radial force at a specific time. The radial force is present in every condition and appears as a hexagram with the impeller rotating in a circle. The radial force variation is bound up with the rotor-stator interaction that presents six cycles in one impeller revolution, and the interaction effect is enhanced whenever the impeller blade sweeps across the volute tongue, thereby resulting in a stronger radial force. This law also exhibits the advantage of the SAS numerical simulation model, which can capture the transient flow more accurately. The value of the radial force diminishes as the flow increases, reaching the lowest at 1.2Q _d and growing at larger flow rate conditions. The probable reason is that 1.2Q _d is the most efficient operating condition. When the pump operates at 0.6Q _d , the flow velocity outside the impeller far outweighs the velocity at the volute entrance, and the outflow liquid from the impeller continuously hits the liquid in the volute chamber, forcing out the liquid receiving energy and causing a large pressure gap of the liquid and stronger radial force acting on the impeller.

Figure 3:

Radial force acting on the impeller in various operating conditions.

3.2. Analysis of Pressure Fluctuation Intensity

The standard deviation and average pressure coefficient values at each grid node in the flow domain are calculated in CFD-Post. The unsteady pressure fluctuation distribution and intensity are evaluated directly and comprehensively using statistical methods. The distribution of pressure fluctuation intensity is presented in Figure 4. An asymmetrical distribution of fluctuation magnitudes in the volute domain can be obtained. Pressure fluctuation intensity decreases along with the spiral line, reaches the lowest when it locates farthest from the tongue, and then increases. However, low fluctuation intensity areas can be observed soon afterwards. The highest gradient of fluctuation magnitudes can be observed near the tongue. Also, higher fluctuation intensity can be found in the discharge tube of the volute channel. Fluctuation intensity at the outlet of the impeller appears larger than that near the volute wall.

Figure 4:

Pressure fluctuation intensity in the volute at mid span z = 0.

Eight axial cross-sections of the volute are presented in Figure 5. The distributions of pressure fluctuation intensity at four cross-sections are analyzed, as shown in Figure 6. The figure indicates that the intensity distributions are approximately symmetrical and the intensity decreases with increasing radial distance because the volute wall is far from the rotating blades. Thus, the volute geometry is vital to the distribution of pressure fluctuation intensity. Pressure fluctuation intensity in every section is at its maximum near the impeller exit, and the flow flattens as the fluid enters the internal volute channel. Pressure pulsation intensity distribution around the sections is symmetrical based on the middle cross-section, which can ensure that the volute has a stable relative movement to reduce hydraulic losses within the impeller. The flow around the middle section pulsates more strongly because it is the place where direct flow from the impeller occurs.

Figure 5:

Sketch of the eight axial cross-sections in the volute.

Figure 6:

Pressure fluctuation intensity distribution at four cross-sections in the volute at Q _d .

3.3. Pressure Characteristics of the Monitoring Points

To observe the flow features along with the spiral channel of the volute and to record the pressure information, we arranged eight monitoring points in the middle cross-section. The position of points A to G are illustrated in Figure 5. Point A stands at the tongue of the volute. Points B to G are located at the intersection between the spiral line and sections II to VII. Point H is located at the volute diffuser with the same horizontal height as point A. The pressure data for the last three revolutions at the monitoring points are saved for time-domain and frequency-domain analysis.

The time-domain and frequency-domain characteristics of point A in five operating conditions are presented in Figure 7. As shown in Figure 7(a), the pressure changes periodically in all five operating conditions, that is, a period of one rotation of the impeller, which includes six periods with negligible differences. Fluctuation amplitudes decrease as the flow increases, dropping to the lowest at Q _d and growing at larger flow rate conditions. As Figure 7(b) indicates, the pressure pulsation in the frequency spectrum in various operating conditions shows discrete spectral characteristics and blade passing frequency (290 Hz), and its multiples represent the main frequency. Broadband characteristics appear in the frequency spectrum, particularly at 0.6Q _d and 1.4Q _d , but also take a smaller proportion. Amplitudes after fast Fourier transform at blade passing frequency also diminish as the flow increases, dropping to the lowest at Q _d and growing at larger flow rate conditions. Results indicate that the blade-tongue interaction causes the pressure fluctuation in centrifugal pumps rather than the vortex fluctuation by turbulence disturbance.

Figure 7:

Pressure characteristics of point A in five operating conditions.

The time-domain and frequency-domain characteristics of points B to H in the design condition are shown in Figure 8. As Figure 8(a) indicates, the pressure changes periodically over time in all seven monitoring points. The value of the pressure increases from point B to point H, which is consistent with the supercharged principle of the pump volute. According to Figure 8(b), the pressure pulsation in the frequency spectrum of various operating conditions exhibits discrete spectral characteristics and blade passing frequency (290 Hz), and its multiples are the main frequency. The pulsation amplitude of monitoring points decreases along with the spiral line and reaches the lowest at the point located farthest from the tongue and then grows.

Figure 8:

Pressure characteristics of various monitoring points at 1.2Q _d .

4. Experimental Verification of Pressure Fluctuation

4.1. Test Rig Setup

Experiments were conducted in a closed-loop system composed of two parts: water circulation and data acquisition. The water circulation system supplies the necessary environment for centrifugal pump operation, and the data acquisition system changes all types of physical quantities in different conditions to the corresponding electrical signals by using sensors. The final data are directly discernible after processing. The installation diagram of the test system is shown in Figure 9(a). The pump, together with the motor, is fixed on a solid base. The meter, torque meter, and static pressure sensors are used to calculate the pump performance. Eight dynamic pressure sensors are used to transduce the transient pressure. The positions of these dynamic pressure sensors are set as the monitoring points, as shown in Figure 9(b). The data acquisition system is designed using LabVIEW based on a virtual instrument development platform that we made previously [17]. The component structure of the measurement system is illustrated in Figure 9(c).

Figure 9:

Test rig of experiment system.

The inlet gate valve is kept open during the measurement and the outlet gate valve is used to regulate the flow. A turbine flow meter is used to measure the flow Q. The turbine flow meter precision is ±0.3%, and the output standard electrical signal is in the 4 mA to 20 mA range. During the experiment, two static pressure sensors (CYG1401) were used to measure the inlet pressure (P _s ) and the outlet pressure (P _d ). The precision of CYG1401 was ±0.2%, which could produce standard electrical signals. The measurement range at the inlet was −100 kPa to 100 kPa, and that at the outlet was 0 MPa to 1 MPa. The twisting moment (M) imposed on the pump shaft was measured using HBM T5 (Germany), with measurement range of 20 N·m. Eight dynamic pressure sensors (CYG1145) were equipped to collect transient pressure signals in the volute flow channel at the 0 Hz to 0.1 MHz range. The precision grade of these sensors was 0.5. All transient signals were synchronously collected using NI-PXI-6251, a multifunctional acquisition card. The NI-PXI-6251 resolution was 16 bits and the maximum sampling rate was 250 kHz. Based on the Nyquist sampling theorem and the obtained test range of dynamic pressure, the time interval Δt was 5 × 10⁻⁵ s, hits N were 80 000, and the corresponding sampling rate (f _s ) at the moment was 10 000 Hz.

4.2. Comparison of Pump Performance Curves

The comparison of the delivery head curves obtained from numerical calculations and from the experiments for all five operational conditions of nominal speed is shown in Figure 10. For the CFD results, the delivery head was obtained from one averaged revolution of the unsteady calculation. Data from static pressure sensors were used in the experimental head calculation. Pump head was calculated based on the following equation:

$H=\frac{\mathrm{1}}{\rho g}\left({P_{\text{tot}}|}_{\text{outlet}}-{P_{\text{tot}}|}_{\text{inlet}}\right)\hspace{1em}\hspace{1em}+\frac{\mathrm{1}}{\mathrm{2}g}\left(v_{\text{out}}^{\mathrm{2}}-v_{\text{in}}^{\mathrm{2}}\right)+\left(z_{\text{out}}-z_{\text{in}}\right).$

(5)

With regard to pump efficiency, the total efficiency is the product of hydraulic efficiency, mechanical efficiency, and volumetric efficiency, given by (10). Only the hydraulic loss was considered in the numerical simulation; thus, the total efficiency should be calculated by (6) to (10). All of these equations are presented in the literature [19]:

$\eta ={\eta }_h{\eta }_m{\eta }_v,$

(6)

${\eta }_h=\frac{\rho gQH}{M\omega },$

(7)

${\eta }_m=\mathrm{1}-\mathrm{0.07}\frac{\mathrm{1}}{{\left(n_s/\mathrm{100}\right)}^{\mathrm{7}/\mathrm{6}}}-\mathrm{0.02}=\mathrm{0.866},$

(8)

${\eta }_v=\frac{\mathrm{1}}{{\mathrm{1}+\mathrm{0.68}n}_s^{-\mathrm{2}/\mathrm{3}}}=\mathrm{0.96},$

(9)

$n_s=\frac{\mathrm{3.65}n\sqrt{Q}}{H^{\mathrm{3}/\mathrm{4}}}.$

(10)

Based on most conditions, the numerical head is slightly lower than that of the corresponding experimental results, which may be due to the head loss in the longer pipe at the inlet and outlet. The numerical efficiency is slightly higher than that of the corresponding experimental results, which may be due to the neglected roughness. The agreement at the part-load operating points was worse than that at the design and over-load operating points. The maximum relative errors in the head and efficiency calculations were 3.8% and 3.3%, respectively. Moreover, numerical values are closer to experiment when we choose SAS model other than normal SST model, especially at part-load. Thus, the performance of the pump can be predicted accurately using the numerical method based on the SST-SAS model.

Figure 10:

Performance curves of numerical simulation and experiment.

4.3. Comparison of Pressure Fluctuation

In the data analysis process, the pressure data were transformed to pulsation coefficient K _P according to the following equation:

$K_P=\frac{\sqrt{\left(1/N\right){{\displaystyle \sum }}_{i=1}^N{\left(P_i-\overline{P}\right)}^2}}{\overline{P}},$

(11)

where P _i represents the transient pressure recorded at the monitoring points. N is the number of collected data and $\mathrm{\hspace{0.17em}\hspace{0.17em}}\overline{P}$ is the time-averaged pressure of the sampling data.

As shown in Figure 11, both numerical and experimental pulsation coefficients K _P of every monitoring point exhibits the same law with the flow rate variation, which first diminishes with the flow increase, reaching the lowest at Q _d and growing at larger flow rate conditions. The pulsation coefficient of monitoring point A is the maximum of all eight points. The difference between numerical and experimental values may be caused by the roughness of the volute wall, which can influence the measurement of the pressure on one side. On the other side, the numerical simulation ignores the influence of the roughness of the wall and the impaction from the pump casings to the flow. Therefore, adopting a full flow field model as the calculation domain to process the numerical simulation is recommended for further study.

Figure 11:

Comparison of pulsation coefficients.

Frequency-domain results of experimental data on the eight monitoring points at various operating conditions are reported in Figure 12. Zoom-FFT was used for spectrum zooming treatment. The advantage of Zoom-FFT is a higher frequency resolution than that of common FFT in the same Fourier transform point [20]. At pump design flow and over, the blade passing frequency (290 Hz) and multiples are the main discrete frequencies. The amplitude at blade passing frequency (290 Hz) is the maximum in the frequency area at all eight monitoring points, which is in accordance with the simulation. Instead of exhibiting most of these characteristics, the pump operating at small flow conditions shows more peaks at low frequency, such as shaft frequency and multiples. The amplitude value at shaft frequency is even higher than that at the blade passing frequency at some monitoring points because of the unsteady flow, such as back flow and cavitation, in the off-condition, particularly small operating conditions. This unsteady flow affects the impeller, which displays shaft frequency in the pressure frequency domain. By comparing the peak value at blade passing frequency, we observe an upward trend with the flow increasing at most of the monitoring points except points D and E. Steeper drop appears at points A and B located at the beginning of the volute spiral line, which is most influenced by the blade-tongue interaction.

Figure 12:

Characteristics of experimental pressure fluctuations in the frequency domain.

5. Conclusions

1. The comparison results between the experimental and numerical simulations in the pump performance and pressure pulsation show that the SAS model can accurately predict the inner flow field of the centrifugal pumps. The radial force that acts on the impeller exhibits a star distribution, which is related to the blade number.

2. The pressure fluctuation intensity is strongest near the tongue, appears to decrease initially, and then increases along with the spiral line. The main function of the volute is to collect the high energy outflow from the impeller, reduce the flow speed of the liquid, and transform the kinetic energy into pressure energy. However, reduction of the pressure fluctuation does not indicate a steady flow because of the blade-tongue interaction.

3. As shown by the pressure fluctuation distribution at cross-sections in the volute, a symmetrical phenomenon appears based on the middle-section plane. However, the outflow from the impeller is three-dimensionally disordered because the volute can eliminate the rotational movement of the liquid discharged from the impeller to prevent hydraulic losses, thereby ensuring a stable relative movement.

4. The blade passing frequency and its multiples are the dominant frequency of the monitoring points within the volute, which are mainly caused by the movement between the impeller and the volute, namely, the rotor-stator interaction. The low frequency pulsation, particularly that of the shaft component, increases when it operates at off-design condition, particularly at a small flow rate, mainly because of the unstable flow. The vortex wave improves in off-design condition, which affects the axle and is shown in the shaft component in the frequency domain.