2.1. Sound Field Solving Theory
Similar to aerodynamic noise, hydrodynamic noise is an interdisciplinary field that combines unsteady fluid dynamics and acoustics [
20]. Currently, in the research of hydrodynamic noise, theoretical methods and tools predominantly originate from aerodynamic acoustics, with the exclusion of cavitation noise in water. Therefore, both domestic and international scholars generally classify hydrodynamic noise and aerodynamic noise under the discipline of aerodynamic acoustics.
The research in aerodynamic acoustics is widely acknowledged to have originated from Lighthill. In 1952, Lighthill [
21] introduced the acoustic analogy method and Lighthill equation, as shown in Equation (1):
where
represents the Hamilton operator,
;
ρ represents the fluid density, kg/m
3;
ρ0 represents the reference density, kg/m
3;
t represents time, s;
c0 is the speed of sound, m/s;
Tij refers to the Lighthill stress tensor;
x represents the spatial coordinates, with subscripts
i and
j denoting the components along the coordinate axes, following the summation convention of tensors;
u represents the fluid velocity, m/s;
p represents the pressure exerted on the fluid, Pa;
p0 represents the undisturbed pressure experienced by the fluid, Pa; and
δij is the unit tensor,
.
The acoustic analogy method, as envisioned in Lighthill’s work, assumes that the sources of sound in the flow field are independent and that sound propagation is unaffected by the fluid. By manipulating the N-S equations, one can derive the wave equation for sound in the fluid. Lighthill focused on free-field sound radiation and did not extend the integral solution form. To obtain the complete integral form solution of the Lighthill equation, Curle [
22] employed the Kirchhoff integral method, considering the influence of solid obstacles on the surface of the fluid. Curle derived the Curle equation, as shown in Equation (2):
where
τij is the viscous stress tensor;
r is the distance between the field point and the source point,
r = |
x −
y|;
x represents the field point; and
y represents the source point.
Williams et al. [
23] extended the Kirchhoff integral method to incorporate moving solid boundaries, thereby providing the most general form of the Lighthill acoustic analogy known as the FW-H equation. It is expressed by Equation (3):
where
δ(
f) is the Dirac delta function;
H(
f) is the Heaviside function;
ui is the component of fluid velocity;
vi is the component of surface velocity;
t is time, s; and
ni represents the unit normal vector along the exterior normal to the surface of the sound source.
By performing the integration of Equation (3), we obtain:
where
Mr is the Mach number of the moving source in the direction of the observer.
In Equation (4), the first term on the right-hand side represents the Lighthill acoustic source, which signifies the contribution of quadrupole sources to the acoustic field. The second term represents the pressure fluctuations within the boundary layer of the solid wall motion, indicating the contribution of dipole sources in the flow field to the acoustic field. The third term represents the interaction between the solid wall motion and the flow field, representing the contribution of monopole sources in the flow field to the acoustic field. Directly solving the FW-H equation is challenging, and early solution methods involved solving the FW-H equation in the frequency domain. However, these methods were infrequently used due to the complexity of the computational formulas. Subsequently, with the continuous improvement of computer performance, Farassat [
24] proposed a time-domain solution for the FW-H equation. By introducing the Green’s function formula and adjusting the FW-H equation, Farassat derived time-domain integral expressions for monopole and dipole noise sources. Farassat’s time-domain solution method enabled the widespread application of the FW-H equation in the engineering field.
Goldstein [
25] proposed a generalized form of the Lighthill equation for solving the sound generation problem in homogeneous moving media. The various methods based on Lighthill’s ideas mentioned above are collectively referred to as the acoustic analogy methods. Bailly [
26] analyzed plate noise using two methods: direct noise computation (DNC) and the acoustic analogy theory. The results showed that the acoustic analogy theory provided comparable results to DNC calculations at low Mach numbers, but with higher computational efficiency. Lighthill emphasized the compressible nature of fluids as an essential factor for sound propagation, which is why he incorporated density variations as an acoustic quantity in his equations. With the development of aeroacoustics, researchers have proposed various acoustic analogy equations based on different acoustic quantities, depending on their specific research areas. Powell [
27] introduced vorticity into the Lighthill equation and derived the Powell equation, as shown in Equation (5):
where
ω represents vorticity;
u is the velocity vector of fluid particles; and
ω ×
u represents the acoustic source, where a larger vorticity leads to a greater noise generation.
Powell developed the vorticity acoustic theory, which uses the magnitude of vorticity as a measure of acoustic source energy. He pointed out that for low Mach numbers in adiabatic and isentropic fluids, both fluid motion and sound radiation are generated by vorticity. The vorticity acoustic theory proposed by Powell is essentially an extension of Lighthill’s theory for low Mach numbers.
Howe [
28] further developed the vortex sounding theory by considering the effect of entropy change and mean flow on flow sounding and proposed Howe’s equation, as shown in Equation (6):
where
D is the Doppler amplification factor,
D = |1 −
Mr|;
E is the internal energy of the fluid;
T is the temperature, K;
s is the entropy;
B denotes the stagnation enthalpy of the fluid, defined as
;
cp is the specific heat capacity of pressure;
cv is the specific heat capacity of constant volume; and
γ is the ratio of specific heat, defined as
.
The Powell equation can be regarded as a modification of the Howe equation under the condition of low Mach numbers. Subsequently, Howe [
29] pointed out in his research that the transient pressure on solid surfaces is the primary cause of noise generation. He proposed a research approach that involves first calculating the flow field and then computing the sound field for studying the rotationally induced sound field by machinery. Timushev [
30] and others utilized the vorticity acoustic theory to solve the flow-induced noise within a centrifugal pump, and the results demonstrated good agreement with experimental data. In addition to Howe, several researchers [
31,
32,
33,
34] have investigated the aerodynamic noise mechanisms from different perspectives. The studies indicate that there exist interactions and correlations between acoustic waves, fluid vortices, and different vortices. According to the acoustic analogy theory, turbulent noise exhibits quadrupole source characteristics. For mixed-flow pumps, the Mach number of the internal flow is less than 1, which means that turbulent sound waves cannot reach the far field. However, during the dynamic and static interference between turbulence and the impeller, volute, and guide vanes of the pump, the quadrupole sources undergo scattering. This leads to intense pressure fluctuations on the surfaces of the rotor or stator, resulting in the generation of dipole sources and increased radiation efficiency. Therefore, in numerical simulation studies, the contribution of dipole sources to the sound field is often considered.
2.2. Numerical Calculation Model and Method
2.2.1. Flow Field Calculation Model and Grid Division
The research object of this study is a low specific speed mixed-flow pump with guide vanes. The computational domain covers the entire device section from the inlet section of the pump to the outlet section of the annular volute, as shown in
Figure 1. The design parameters are as follows: rated flow rate
Qdes = 380 m
3/h, rated head
H = 6 m, rated speed
n = 1450 r/min, specific speed
ns = 480, number of impeller blades
Z = 4, and number of guide vane blades
Zd = 7. The inlet diameter of the pump is
D1 = 250 mm, the outlet diameter is
D2 = 200 mm, and the blade tip clearance is
δ = 0.2 mm.
The physical model of the mixed-flow pump includes six parts: inlet section, impeller section, guide vane section, annular worm chamber section, and outlet section, with a large spatial structure. Therefore, the inlet section, impeller section, guide vane section, worm chamber section, and outlet section of the mixed-flow pump model are discretized separately during meshing, and in order to obtain more accurate results of the flow field, high-quality hexahedral structured meshes are drawn for all the computational domains. Among them, the water body domain inside the impeller section adopts the J/O type topology; in order to ensure that there are enough meshes in the gap of the blade rim, the mesh encryption process is realized by increasing the mesh nodes in the gap and at the same time adjusting the mesh scale in the near-wall area, controlling that the mesh Y
+ value of the gap area varies in the range of 100; Y
+ is the dimensionless coefficient representing the boundary layer mass. The mesh of each part of the mixed-flow pump is shown in
Figure 2. The number of grids in each part of the computational domain, inlet section, impeller section, guide vane section, annular worm chamber section, and the total number of grids are 246,048, 2,827,416, 2,298,345, 437,091, and 5,808,900, respectively.
In the process of numerical calculation of mixed-flow pump, it is necessary to quantitatively analyze the errors in numerical calculation, the causes of errors, and the influence range. In particular, the density and quality of the mesh largely determine the accuracy and reliability of the simulation. In order to take into account the accuracy and efficiency of the calculation, it is usually necessary to carry out grid independence verification before numerical calculation to determine the appropriate number of grids.
In this paper, by adjusting the number and position of grid nodes in the topology structure, 5 sets of structural grids with different grid numbers are obtained. The numerical calculation of 5 different quantities of grids under rated working conditions is carried out, and the pump head and efficiency are compared as reference standards, and the results are shown in
Figure 3. When the total grid number of the model is greater than 5.8 million, its head and efficiency are basically unchanged, which meets the requirement of the grid independence test. Therefore, considering the calculation accuracy and efficiency, a grid scheme with an overall grid number of 5.8 million was selected for the subsequent numerical calculation study.
2.2.2. Flow Field Calculation of Turbulence Model and Boundary Conditions
Based on ANSYS CFX, following the ITTC-CFD Uncertainty Analysis Guidelines, the SST k-ω turbulence model was selected for the model after validation. In the steady-state flow analysis, four operating conditions were considered: 0.6Qdes, 0.8Qdes, 1.0Qdes, and 1.2Qdes. For the unsteady flow analysis, the steady-state flow field results of the four flow rate conditions were used as initial conditions to simulate and solve the unsteady flow conditions inside the mixed-flow pump at the four operating points. In the numerical simulation, a multiple reference frame (MRF) approach was employed. The impeller domain was set as a rotating domain, while the remaining fluid domains were considered stationary. For steady-state simulations, data transfer between the stationary and rotating domains was accomplished using a frozen-rotor interface, while for unsteady simulations, a sliding mesh technique was utilized through a transient rotor/stator interface. The medium used in the simulations was clean water at a temperature of 25 °C. The solid walls of the entire computational domain were assigned as no-slip walls. The inlet boundary condition was specified as total pressure inlet, while the outlet boundary condition was set as a flow rate outlet.
Considering computation time and accuracy, in the steady-state simulations, the solver settings were kept consistent for all flow rate conditions. The time step size was set to 0.00025, the number of iterations per step was set to 2000, and the convergence criterion was set to 10−4. In the unsteady simulations, a time step size of 3° per step was used, which was sufficient to capture dynamic pressure signals. The impeller completed 10 revolutions, resulting in a total of 1600 time steps. The convergence criterion for the unsteady simulations was also set to 10−4. The calculation was considered converged when the monitored values exhibited periodic stability. For the analysis of the unsteady flow field, data extraction was performed starting from the 5th revolution, and a total of 5 revolutions’ worth of data were extracted.
2.2.3. Noise Numerical Simulation Methods
There are three main approaches for fluid acoustic simulation: direct numerical simulation, acoustic field prediction based on semi-empirical models, and hybrid numerical simulation. Among them, hybrid numerical simulation is the most commonly used in scientific research and engineering. The basic idea is to first use computational fluid dynamics (CFD) methods to obtain the internal flow field of the pump. Then, the temporal pressure fluctuation information in the flow field is converted into sound source information. Finally, by neglecting fluid viscosity, the acoustic field is predicted based on the acoustic wave propagation equation or acoustic analogy methods. Since the acoustic energy is much smaller than the fluid energy, this method does not consider the effect of the acoustic field on the flow field.
This study focuses on the contribution of pump wall dipole sources to the acoustic field. In rotating machinery, dipole sources include the guide vane, volute casing wall dipole, and impeller wall rotating dipole. Different computational approaches are used for these sources. In this paper, the guide vane and volute casing wall dipoles are referred to as stationary component dipoles, while the impeller wall dipole is referred to as the rotating component dipole.
Figure 4 illustrates the calculation approach for the noise generated by the stationary and rotating component dipoles. The acoustic field calculations were performed using the Acoustic module in LMS Virtual Lab. For both types of dipole sources, the internal acoustic field was obtained using the finite element method (FEM) in acoustics, including the distribution of flow-induced noise and sound power within the mixed-flow pump.
2.2.4. Stationary Component Dipole Noise
Figure 4e shows the acoustic finite element mesh, which has been coarsened. The size of the mesh elements needs to strictly adhere to the criterion that the number of grid cells per wavelength should be greater than 6. The wavelength is determined based on the highest frequency. In this numerical simulation, the mesh consists of 128,014 elements and 28,125 nodes, which adequately meet the requirements for acoustic field simulation calculations.
An important step in the calculation of the volute casing wall dipole acoustic field is pressure data mapping, which involves mapping the pressure data stored at the CFD grid nodes onto the acoustic grid as boundary conditions for sound propagation calculations. Therefore, the conservative maximum distance algorithm is used to compute the data mapping process, reducing energy losses during the mapping process. Additionally, following the frequency-domain calculation approach for sound propagation, the temporal pressure fluctuation data need to be Fourier-transformed during the data mapping process, converting the temporal signal of fluid pressure into frequency-domain data. The pressure fluctuation data from the 5th to the 10th revolution in the CFD simulation are used as the source signals. The inlet and outlet surface of the pump are set to have the AML attribute, while the inner wall surface of the volute casing grid is set as a fully reflective wall. Other parameter settings for sound propagation calculations are presented in
Table 1.
2.2.5. Rotating Component Dipole Noise
According to the FW-H theory, the noise generated by the rotating dipole is simulated, and it is converted into pressure fluctuations acting as blade loads, as shown in
Figure 5. When defining the sound source boundary conditions for the rotating dipole, all the surface elements in the CFD grid are simplified into a single point source. This point source contains the temporal signal information of the pressure fluctuations. Additionally, the equivalent source method is employed to compactly represent the rotating dipole as a compact sound source. The impeller is divided into segments, where each segment can be considered as a compact sound source relative to the wavelength of the sound wave. The loads on the surface of each segment are integrated to the centroid of that segment, resulting in the total load on the impeller. To obtain wideband noise, the temporal pressure fluctuation signals at each point are divided into equal duration segments. In the subsequent acoustic calculations, the calculation of wideband noise is achieved by setting the impeller speed and the number of subharmonics. To ensure that the impeller dipole noise spectrum has the same frequency resolution as the volute casing dipole noise spectrum, this study adopts a total duration of 5 revolutions as one time segment. The settings for the rotating dipole sound source definition are presented in
Table 2. For the configuration of other acoustic finite element meshes and field point grids, please refer to
Table 1.
2.2.6. Experimental Validation
By constructing a water pump test rig for external characteristic testing, the hydraulic performance of the pump was tested to verify the reliability of the numerical simulations. The obtained flow–head and flow–efficiency characteristic curves from the experiments were compared with the numerical simulation results, as shown in
Figure 6c,d. The results revealed that the simulated flow–head curve closely matched the experimental results. As the flow rate increased, the head gradually decreased, and the deviation between the experimental and simulated values also decreased. As for the flow–efficiency curve, the efficiency increased with increasing flow rate and reached its maximum at the design operating point. The efficiency values obtained from the experimental measurements were close to the simulated values. A comparison of the CFD numerical results indicated good agreement between the head and efficiency curves of the mixed-flow pump and the experimental results. The maximum deviation at the design operating point did not exceed 5%, as shown in
Table 3, demonstrating the reliability of the computed results.
In order to validate the current paper simulation model, the current model results are compared qualitatively and quantitatively with the published work [
35]. Therefore, the same geometric design is used at the inlet and outlet of the mixed-flow pump, and the meshing is performed in ANSYS ICEM with similar boundary conditions.
Figure 2a,b is the published work results. By comparing these results, it is found that they have a good agreement, thus qualitatively verifying the model.