Transient Analysis of Flow Unsteadiness and Noise Characteristics in a Centrifugal Compressor with a Novel Vaned Diffuser ^†

Abstract

The demands to apply transonic centrifugal compressor have increased in the advanced gas turbine engines. Various techniques are used to increase the aerodynamic performance of the centrifugal compressor. The effects of the inclined leading edges in diffuser vanes of a transonic centrifugal compressor on the flow-field unsteadiness and noise generation are investigated by solving the compressible, three-dimensional, transient Navier–Stokes equations. Diffuser vanes with various inclination angles of the leading edge from shroud-to-hub and hub-to-shroud are numerically modeled. The results show that the hub-to-shroud inclined leading edge improves the compressor performance (2.6%), and the proper inclination angle is effective to increase the stall margin (3.88%). In addition, in this study, the transient pressure variations and radiated noise prediction at the design operating point of the compressor are emphasized. The influences of the inclined leading edges on the pressure waves were captured in time/space domain with different convective velocities. The pressure fluctuation spectra are calculated to investigate the tonal blade passing frequency (BPF) noise, and it is shown that the applied inclination angles in the diffuser blades are effective, not only to improve the aerodynamic performance and stall margin, but also to reduce the BPF noise (7.6 dB sound pressure level reduction). Moreover, it is found that the diffuser vanes with inclination angles could suppress the separation regions and eddy structures inside the passages of the diffuser, which results in reduction of the overall sound pressure level and the broadband noise radiated from the compressor.

1. Introduction

Industrial compression systems are increasingly demanded in various applications, which include petrochemical, automotive engines, power plants, and aircraft gas turbine. Single or multistage centrifugal compressors play an important role in such applications to compress the working fluid [1,2,3]. The growth of global air traffic and increasing number of constraints in relation to fuel consumption require the stage loading to be increased, and the centrifugal compressor size to be reduced. Therefore, the centrifugal compressors with higher efficiency, higher pressure ratio, and higher mass flow rate are necessarily needed.

To obtain higher pressure recovery and also to stabilize the flow, vaned diffusers are used in many centrifugal compressors [4,5,6,7,8]. Although, the efficiency of the diffuser is significantly dependent on the outflow condition from the impeller exit, and the radial vaneless distance between the leading edge of the diffuser vanes and the trailing edge of the impeller blades, which is called as interaction region. The impeller–diffuser interaction causes complicated, unsteady flow structures between the exit of impeller and the throat of the diffuser, in which unsteady transonic flow structures are believed to impact the operating range and the aerodynamic performance of centrifugal compressors [9,10,11,12]. Therefore, understanding of the flow variations in the impeller–diffuser interaction region with respect to the circumferential and spanwise directions is a fundamental factor to enhance the compressor efficiency in various operating points.

More recently, several theoretical and experimental researches have been carried out to realize the transient flow-field and radiated noise mechanism within the impeller and diffuser passages of centrifugal compressors [13,14,15,16,17]. Ziegler et al. [5,6] revealed that the interactions between the impeller and diffuser play important roles in the aerodynamic performance of centrifugal compressor. They showed that in most cases, smaller radial gaps between the impeller exit and diffuser vane inlet lead to a more uniform flow-field and higher pressure recovery coefficient at the diffuser outlet, which results in improvement in compressor performance. Vogel et al. [18] experimentally and numerically investigated the pressure variations in a centrifugal compressor with a vaned diffuser. They showed that these variations exist from the leading edge toward the trailing edge of the diffuser channels, and the maximum value of the pressure oscillations is reached to 30% of the pressure at the compressor inlet.

Nowadays, numerical simulations have been extensively used to investigate the complex flow characteristics within the turbomachines, due to development of high-performance computers and advanced computational fluid dynamics algorithms [19,20,21,22,23]. Everitt et al. [19] quantified the role of outflow from the impeller exit in the compressor performance with vaned diffusers. They found that the effectiveness is well correlated to the mixed-out average flow angle. Incidence angle was considered as the main effective factor on the compressor performance, which increases the separation regions inside the diffuser passages at off-design operating points, leading to an increase in loss and decrease in diffuser pressure recovery. Shum et al. [24] numerically analyzed the influence of impeller–diffuser interaction on the performance of a centrifugal compressor stage. The unsteady effects of impeller exit on diffuser loss and pressure recovery coefficients are similar to those from axial distortion at the inlet of the diffuser. It was found that both have negligible effects in comparison with the spatially and time-averaged flow incidence at the diffuser throat. Anish et al. [25] studied the time-dependent interaction influences on the diffuser efficiency of a centrifugal compressor. They showed that the circumferential variations of flow angle at the leading edge of the diffuser blade affect the diffuser efficiency. Fontanesi et al. [26] numerically studied the acoustic field of a centrifugal compressor. They found that the experimental whistle at the compressor inlet near the compressor surge is caused by the flow pulsations, detached and re-attached flow regions within the compressor passages. Although numerous investigations have been conducted to predict the noise generation and acoustic behaviors in turbomachines, most of them performed to the axial turbomachinery components because of their wide range applications in the aircraft engine industry. Additionally, most of the measurements and computational researches on the centrifugal compressors were performed to low-speed compressors, and few publications are provided for high-speed radial compressors [27,28].

One of the primary and complicated aerodynamic flow behaviors within the turbomachinery components is unsteadiness, which is also known as the key parameter in noise generation. Both tonal (discrete) and broadband noise are typically generated in the centrifugal compressors. The generated broadband noise in the centrifugal compressors is caused by the interaction between the three-dimensional turbulent structures and separation regions with the impeller and diffuser blades, and the secondary flow-field within the compressor channels. On the other side, the interaction between the impeller trailing edge and diffuser vane generates the tonal noise, which is known as the dominant noise in the centrifugal compressors. This tonal noise is related to the blade passing frequency, and depends on the impeller rotational speed, as well as the blade counts. Therefore, the effect of interaction between the impeller and diffuser on the compressor efficiency and acoustic performance is an important factor which needs to be taken into account.

Few approaches have been proposed in the literature to reduce the tonal noise in the centrifugal compressors by changing the geometry of the impeller and diffuser components. Shahin et al. [12] showed that the hub cavity affects the aero-acoustically generated noise in a compressor using large eddy simulation and the Ffowcs Williams-Hawkings model, for which expensive computational resources are required. Ohta et al. [14] investigated the influences of the tapered diffuser blade of the centrifugal compressor on the flow structure and noise generation. Although the tapered vanes can attenuate the level of the tonal noise, producing the tapered vanes is complicated and expensive.

In a previous study by the authors [11], applying the inclination angle in diffuser vane leading edges was found to enhance the pressure recovery coefficient and reduce the loss characteristics. However, in that study, a steady Reynolds-averaged Navier–Stokes approach (RANS) was only considered to analyze the aerodynamic performance at the design point, and the influences of inclined leading edges on the unsteady interactions between the trailing edges of the impeller blades and leading edges of the diffuser vanes were neglected. The main objective of the current study is to analyze the influences of the inclined diffuser vanes on the transient interaction between the impeller and diffuser blades as one of the main sources of the unsteadiness in the centrifugal compressors. Therefore, a numerical approach using the unsteady Reynolds-averaged Navier–Stokes (URANS) method was conducted to investigate the turbulent flow unsteadiness and characteristics of the generated noise of the centrifugal compressor by applying the inclined diffuser vanes. Finally, the inclined leading edge effects on the stall margin improvement were analyzed. The numerical data evaluated in the present study can be utilized to enhance the compressor efficiency and also to control the interaction strength between the impeller and diffuser, which leads to reduce the centrifugal compressor loss and level of the generated noise.

The present work shows the numerical results of applying the inclined leading edges in the diffuser vanes of a transonic centrifugal compressor. Section 2 describes the numerical methodology including the compressor geometry, computational domain, governing equations, and numerical validation. The influences of the inclined leading edges on the aerodynamic performance, stall margin, and flow unsteadiness are extensively investigated in Section 3. Finally, Section 4 reports the conclusions.

2. Numerical Methods

2.1. Compressor Geometry

The centrifugal compressor model used in the numerical simulations is the single-stage NASA CC3 centrifugal compressor [29]. The NASA CC3 is a transonic centrifugal compressor with high-compression ratio (4:1). The meridional view of the compressor stage is shown in Figure 1. The computational domain includes three separated parts: stationary inlet domain including a pipe and impeller eye; rotating impeller, with 15 main blades and 15 splitter blades; stationary vaned diffuser domain, including 24 two-dimensional wedge-type vanes. The leading edges of the splitter blades are located at the 50% and 30% of the pitch and chord of the main blades, respectively. In addition, to provide a uniform split flow between the main blade and splitter passages, the splitters are offset toward the suction side of the main blades. The leading edge of the diffuser vanes is placed at 108% of the impeller exit radius with a 7.8° divergence angle. McKain and Holbrook [30] describe the compressor design in detail, consisting of the geometrical parameters of the impeller and diffuser. The impeller rotational speed and the compressor mass flow rate are 21,789 rpm and 4.536 kg/s, respectively, at the design point.

Table 1. NASA CC3 centrifugal compressor specifications.

Operating condition
Inlet temperature	288 K
Inlet pressure	101,325 Pa
Total pressure ratio	4:1
Rotational speed at design point	21,789 rpm
Mass flow rate at design point	4.536 kg/s
Impeller configuration
Number of main blades	15
Number of splitter blades	15
Radius at impeller inlet (R1)	105 mm
Inlet blade height	64 mm
Radius at impeller exit (R2)	215.5 mm
Tip speed	492 m/s
Blade height at exit	17 mm
Backsweep angle	50°
Vaned diffuser configuration
Number of vanes	24
Divergence angle	7.8°
Vane height	17 mm
Inlet diameter	431 mm
Outlet diameter	714 mm

summarizes the centrifugal compressor operating conditions as well as the dimensions of the impeller and diffuser.

Figure 2 shows the numerical domain used in the current study for the computational simulations. As shown in the figure, the inlet pipe has been extended in the axial direction (about two times of the diameter of the impeller inlet) to provide a uniform and developed flow at the inlet of the compressor impeller. In addition, in order to minimize the influences of the imposed boundary condition at the diffuser outlet on the flow-field solution within the diffuser passages, the exit domain has been also extended in the radial direction about one chord of the diffuser vanes. A 120° sector computational domain (1/3 model) was applied for the numerical simulations instead of full-annulus modelling to reduce the computational cost and time. A partial computational model consists of five impeller passages and eight diffuser passages as illustrated in Figure 2a. Applying a partial numerical domain could reduce the computational time and on the other side by using more mesh points, the resolution of the computational grid was also improved. The full-annulus of the compressor stage including the impeller and diffuser blades are shown in Figure 2b.

2.2. Computational Grid

Commercial software, ANSYS TurboGrid V19.3 was used to generate the multi-block hexahedral structured grid in the current numerical simulations. Figure 3 shows the numerical mesh for the impeller and diffuser passages in detail. It should be noted that the main blades and splitter blades are indicated by yellow and red colors, respectively. The computational domain consists of 9,700,000 grid points: 5,400,000 and 3,500,000 hexahedral meshes for the impeller and diffuser, respectively, and 800,000 tetrahedral elements including 12 prism mesh layers at the wall surfaces for the inlet stationary domain. This grid was selected based on the grid independence test, which will be discussed later in Section 2.4. As shown in Figure 3a, the high-resolution meshes were radially generated in the vaneless gap between the impeller and diffuser to be able to resolve the pressure fluctuations at the interaction region. The details of the computational grid near the impeller blade leading edge and diffuser vane are shown in Figure 3b,c, respectively. In order to properly capture the tip leakage vortices, 30 grid points were generated at the tip clearances of the main and splitter blades of the impeller. Figure 3b shows the distribution of the structured mesh at the tip clearance of the main blade, which is indicated by the red plane.

In the case of compressible flows, one of the important factors is grid resolution at the wall surfaces to preserve the influences of the boundary layer. Therefore, the refined hexahedral grid is generated at the inner walls of the impeller and diffuser passages to keep the non-dimensional wall distance of y⁺ value less than 1 (y⁺ < 1). Figure 4 clearly shows that the distribution of y⁺ contour at the impeller blades and hub surfaces is less than 1.

2.3. Numerical Scheme and Boundary Condition

In the present study, the ANSYS CFX V19.3 solver was applied to obtain the numerical results. CFX solver is a finite volume, coupled implicit pressure based solution approach. In CFX software for the compressible flows, the 3D URANS equations, energy equation, and the equation of the state are simultaneously solved for the working fluid. In this study, the working fluid is air, which is assumed as an ideal gas. The mass, momentum and energy equations are given as follows:

$$\frac{\partial \rho }{\partial t}+\frac{\partial }{\partial x_j}\left(\rho U_j\right)=0$$

(1)

$$\frac{\partial \rho U_i}{\partial t}+\frac{\partial }{\partial x_j}\left(\rho U_i{U}_j\right)=-\frac{\partial p}{\partial x_i}+\frac{\partial }{\partial x_j}\left({\tau }_{ij}-\rho \overline{u_i{u}_j}\right)$$

(2)

$$\frac{\partial \rho h_{tot}}{\partial t}-\frac{\partial p}{\partial t}+\frac{\partial }{\partial x_j}\left(\rho U_j{h}_{tot}\right)=\frac{\partial }{\partial x_j}\left(\lambda \frac{\partial T}{\partial x_j}-\rho \overline{u_{j}h}\right)+\frac{\partial }{\partial x_j}\left[(U_i\left({\tau }_{ij}-\rho \overline{u_i{u}_j}\right)\right]$$

(3)

where $\rho$ presents the density, $U$ the vector of velocity $U_{x,y,z}$, $p$ the pressure, ${\tau }_{ij}$ the molecular stress tensor, T the temperature, $\lambda$ the thermal conductivity, u the velocity fluctuation component, and the mean total enthalpy is given by:

$$h_{tot}=h+\frac{1}{2}{U}_i{U}_i+k$$

(4)

where, $k$ is the turbulent kinetic energy.

The selected turbulence closure model is the $k-\omega$ shear stress transport model (SST). The $k-\omega$ SST turbulence model is widely used in the numerical simulations of the aerodynamic performance in the turbomachinery research area, due to its accuracy and efficiency in prediction of the flow separations [31,32,33,34].

In order to reduce the diffusion errors in the computational procedure [35], for discretizing the convection terms in the governing equations, a hybrid first-order and second-order upwind numerical schemes, which is known as high-resolution scheme was applied. The total pressure (101,325 Pa) and the total temperature (288 K) were the inlet boundary conditions, and the outlet boundary condition was the constant non-reflective static pressure boundary condition. To simulate the rotational effects of the impeller, a moving reference frame (MRF) for compressible flows was used. Rotational speed of the MRF was set to 21,789 rpm which is the speed of the compressor impeller at the design point condition. The adiabatic no slip boundary condition was chosen for all the walls. In order to preserve the stationary effects of the impeller shroud, a wall velocity boundary condition using the counter rotating option was applied.

As the pitch ratio between the impeller and diffuser passages was 1, the frozen rotor interface was selected for the steady simulation. Although, this type of the interface model transfers the flow from one side of the interface to another side by changing the reference frame, but the relative position of the variables through the interface surfaces is unchanged. For unsteady simulations, the interface between the impeller and diffuser was treated by the transient rotor-stator interface, which includes all of the unsteady behaviors of the flow-field.

Table 2. Solver setting specification.

Flow Solver		ANSYS CFX V19.3
Spatial discretization		High resolution scheme (a hybrid of first order and second order upwind scheme)
Temporal discretization		First order backward Euler scheme (steady) Second order backward Euler scheme (unsteady)
Turbulence model		$k-\omega$ SST
Working fluid		Air (treated as an ideal gas)
Boundary conditions	Inlet duct	Total pressure (101,325 Pa) Total temperature (288 K)
	Inlet duct/Impeller Impeller/Diffuser	Frozen rotor interface (steady) Transient rotor-stator interface (unsteady)
	Diffuser exit	Average static pressure

summarizes the solver setting used in the current study. For time discretization in the unsteady simulations, the backward Euler scheme was conducted, which is a second-order scheme. In order to take into account the effects of the relative positions of the impeller blades and diffuser vanes, a small time step of one-degree angular rotation was used with respect to the rotational speed of the impeller. The numerical simulations were carried out on a cluster including 256 CPU (3.3 GHz), and the unsteady simulation was performed until the flow-field fluctuations at various locations in the computational domain were time-periodic.

2.4. Numerical Sensitivity Analysis

A computational model was carried out for various numerical grids and various turbulence models and then compared with the measurement [29] to ensure the accuracy of the computational method. For the grid independency test, three different types of computational meshes, coarse (4.2 million grids), moderate (9.7 million grids), and fine (12.15 million grids) were tested with the $k-\omega$ SST turbulence model using the RANS approach. In order to generate various computational grid domains, the number of grid points was changed in the spanwise, streamwise, and radial directions to ensure y⁺ < 1 at the wall surfaces.

Table 3. Grid independence test.

	Pressure Ratio	Efficiency (%)	Pressure Ratio % Difference	Efficiency % Difference
Coarse	4.124	84.32	3.33%	1.48%
Moderate	3.998	83.04	0.17%	0.06%
Fine	3.991	83.09	-	-

compares the total pressure ratio and isentropic efficiency of the tested compressor at the design point condition, computed by Equations (5) and (6) for different grid resolutions.

$$TPR=\frac{P_{t,outlet}}{P_{t,inlet}}$$

(5)

$$\eta =\frac{\left(TP{R}^{\frac{\gamma -1}{\gamma }}-1\right)T_{t,inlet}}{T_{t,outlet}-T_{t,inlet}}$$

(6)

where $\gamma$ is the specific heat ratio of gas. It should be noted that the mass-flow averaged pressure and temperature are measured at the inlet duct and 1.7 R₂ planes, respectively. Fine grid case was taken as the reference case and the calculated pressure ratio and efficiency of the fine mesh were compared to the other two meshes. As summarized in Table 3, it is observed that by increasing the number of grid elements, the percentage differences in the total pressure ratio and efficiency are considerably less for the moderate mesh. Therefore, the moderate mesh (9.7 million elements) was selected as the computational grid in the current study for all of the numerical simulations to reduce the numerical cost.

Moreover, to ensure the verification of the numerical results regarding the turbulence closure, $k-\epsilon$ and $k-\omega$ SST turbulence models were conducted for the selected moderate mesh in the grid independency analysis.

Table 4. Influence of turbulence model on pressure ratio and efficiency of the compressor.

	$\mathit{k}-\mathit{\epsilon }$	$\mathit{k}-\mathit{\omega } \mathbf{SST}$	Exp
Pressure ratio	4.252	3.998	3.97
Efficiency (%)	86.17	83.04	83.2

compares the pressure ratio and efficiency of the compressor for the two various turbulence models. It is observed that the $k-\epsilon$ turbulence model overestimates both the pressure ratio and efficiency compared to those of the $k-\omega$ SST. This could be caused by the $k-\epsilon$ turbulence model limitations in predictions of the detached and re-attached regions in the flow separation zones especially in the diffuser passages.

2.5. Validation and Consistency of the Numerical Simulation

In order to compare the computational results and experimental data, steady simulations were first conducted from choke to surge at the design speed, to get the full compressor map. Each calculation of the steady solution was converged when the variation of the inlet mass flow rate was less than 0.001 kg/s per 500 iterations and the variation of the total-to-total efficiency was less than 0.2% per 200 iterations. Many other researchers have also used the same convergence criteria for the stall point prediction [32,36]. To obtain the compressor performance characteristic from choke to stall mass flow rate, the exit static pressure was varied in sufficiently small increment of the back pressure as 500 Pa, allowing the solution to converge at each back pressure. Figure 5 compares the aerodynamic performances of the compressor calculated by the numerical method and the experimental data [29] with respect to the mass flow rate, and shows that both the magnitude and trend of the computational data are well matched in comparison to those of the measurements at various operating points. Figure 5 also confirms that the time-averaged data from the unsteady simulations at two different operating points, one near surge and the other at design condition, are also well predicted compared to the experimental data [29] (indicated by the red circle symbols in Figure 5).

Moreover, Figure 6 compares the time-averaged velocity profile computed by the current URANS approach from hub to shroud with the experimental data measured by laser anemometry [37] at the compressor design point. This figure shows the accuracy of our unsteady simulations in prediction of the transient flow-field. It should be noted that the velocity profile is normalized by the tip velocity of the impeller and it is measured at the exit of the impeller (1.05 R₂). It can be concluded from Figure 6 that the unsteady computational data are in a good agreement with the experimental data.

2.6. Inclined Leading Edge in the Diffuser Vane

Generally in centrifugal compressor with vaned diffuser, the leading edges of the vanes are perpendicularly extended in the spanwise direction with respect to the direction of the upstream incoming flow. Therefore, a high incidence flow angle is generated near the leading edge of the diffuser vane, which results in the formation of separated flows within the diffuser channels. These separation regions lead to the significant loss in aerodynamic performance of the compressor. In this research, diffuser vanes with the inclination angles in the spanwise direction with respect to the height of the vane are proposed.

Two types of inclined leading edge of diffuser vanes with different angles from hub-to-shroud ($+\alpha$) and shroud-to-hub ($-\alpha$) were presented, and numerically analyzed. Figure 7 shows the parameter $\alpha$ and configuration of various types of inclined leading edges applied in the diffuser vanes compared to the original leading edge. As shown in Figure 7, the diffuser vane profiles for various inclination angles are exactly the same, and the only difference is observed at the vane leading edges. First, the performance map was calculated using steady simulations for two cases of $\alpha =$ (30 and −30)°, to evaluate the stall margin improvement. Then, transient simulations for different inclination angles of $\pm \alpha$ = (30 and 75)° were numerically analyzed, and were compared to the original diffuser. It should be noted that all the unsteady simulations were conducted at the design condition (21,789 rpm and 4.536 kg/s).

3. Results and Discussions

3.1. Aerodynamic Performance and Stall Margin

In a previous study by the authors [11], the inclined leading edges were found to suppress the separated flows near the throats of the diffuser, which can enhance the aerodynamic efficiency of the transonic centrifugal compressor. The pressure ratio and efficiency of the compressor at the design point condition for various inclined leading edges are shown in Figure 8a,b, respectively. While decreasing the magnitude of the inclination angle for the shroud-to-hub inclined vanes increases the pressure ratio, the values of area are always lower than those obtained for the original diffuser vane. In the case of hub-to-shroud inclined leading edges in the range of 0 < $\alpha$ < 45, the pressure ratio is larger in comparison with the original diffuser vane; but for $\alpha$ > 45, the pressure ratio is significantly dropped. A similar trend is also observed for the compressor performance in the case of shroud-to-hub ($-\alpha$) inclination angles, and 30° inclined leading edge showed the best efficiency compared to the other cases. In addition, the efficiency curve is also dramatically decreased for inclination angles bigger than 45.

Turbulence kinetic energy is one of the most important variables, which measures the intensity of the turbulence and velocity fluctuations in turbulent flows. Figure 9 shows the time-averaged non-dimensional turbulence kinetic energy distributions near impeller exit for the original centrifugal compressor. The turbulent kinetic energy is normalized by the tip velocity. As shown in the figure, there is a high magnitude region of turbulence kinetic energy near the impeller shroud, between the pressure side of the impeller main blade and splitter suction side (indicated by with circles in Figure 9). This high magnitude region indicates that there are more turbulent flows and more velocity fluctuations near the impeller shroud, which later these high-turbulence kinetic energy region enters into the impeller–diffuser vaneless gap. Therefore, by applying the inclination angles on the leading edge from hub-to-shroud, the vanless gap between the impeller and diffuser close to the shroud is increased, which leads to provide a more uniform flow within the vaneless region and diffuser throats.

In order to evaluate the effect of the inclined leading edge on the stall margin, the total pressure ratio and total-to-total efficiency curves were calculated for two different inclined leading edges (−30° and 30°), and compared with the reference case as shown in Figure 10a,b, respectively. In the case of the −30° case, the efficiency near stall and the stall margin are dramatically reduced in comparison to those of the original vaned diffuser. However, the 30° inclination angle can effectively increase the stall margin, compared to the original diffuser, and simultaneously improve the efficiency of compressor.

The stall margin improvement can be calculated by Equation (7) for a test case compared to the reference case, which was suggested by Cumpsty [38].

$$\Delta SM\left(\%\right)=\left[{\left(1-\frac{P{R}_{peak}}{P{R}_{stall}}\times \frac{{\dot{m}}_{stall}}{{\dot{m}}_{peak}}\right)}_{test}-{\left(1-\frac{P{R}_{peak}}{P{R}_{stall}}\times \frac{{\dot{m}}_{stall}}{{\dot{m}}_{peak}}\right)}_{ref.}\right]\times 100$$

(7)

where $P{R}_{peak}$ and ${\dot{m}}_{peak}$ represent the pressure ratio and mass flow rate at the peak efficiency point, respectively. $P{R}_{stall}$ is the pressure ratio at the stall, and the mass flow rate at the stall is denoted by ${\dot{m}}_{stall}$.

Figure 11 shows the stall margin improvement for the different inclination angles from hub-to-shroud. The inclination angle in the range of 15 < $\alpha$< 45 can significantly increase the stall margin. However, further increase in the hub-to-shroud inclination angle dramatically reduces the stall margin improvement, due to increase in the length of the impeller–diffuser gap. The maximum value in stall margin improvement is at 30°, and reaches about 3.88%.

Figure 12 compares the Mach number and static pressure distributions on the 50% span of the impeller–diffuser interface near stall between the original and 30° diffuser vanes. In the case of the original diffuser, a high Mach number region indicated by black circle in Figure 12a is observed in the diffuser throat, which causes a shock, and a large loss. Therefore, as shown in the pressure contour (Figure 12c), the magnitude of the pressure is decreased in the front part of the diffuser, and slowly recovers thereafter. However, in the case of 30° as shown in Figure 12b, this kind of shock wave is not observed within the passages, and the static pressure increases steadily and continuously. Figure 10, Figure 11 and Figure 12 confirm that the 30° inclination from hub-to-shroud not only can improve the pressure ratio and compressor performance at the design point condition, but also can significantly increase the compressor operating range and stall margin.

3.2. Flow-Field Analysis

The effect of the inclination angles of the diffuser vanes on the compressor aerodynamic performance was already evaluated with steady simulations in the previous work [11]. In steady calculations, while the impeller and diffuser locations are changed during the numerical simulation, the relative position of the impeller and diffuser across the interface is fixed (frozen rotor interface), which is known as clocking effect. Therefore, as it was shown in [11], the flow-field distributions within the diffuser passages are different at the design point. In addition, in the steady simulations, the transient effects between the impeller and diffuser are not taken into account. For these reasons, in order to have time-averaged and symmetric flow patterns within the compressor passages and also to realize the transient behaviors of the inclined leading edges on the flow physics, and clearly identify the radiated noise generated within the compressor, the unsteady simulations were carried out at the design point for five various cases, with $\alpha$= (0, $\pm$30, and $\pm$75)°.

Figure 13 compares the time-averaged static pressure and velocity contours at mid-span cutting plane for various inclination angles with those of the original diffuser vanes. The pressure and velocity magnitudes shown in Figure 13 are normalized by the inlet pressure and tip velocity, respectively. It is clearly observed that the highest pressure ratio within the diffuser passages is related to 30° inclined leading edge. However for −30° inclination angle, the magnitude of the static pressure is reduced compared to the original diffuser and 30°. The lowest pressure ratio distribution was found for the −75° inclined leading edges. The velocity contours demonstrates that by using 30° hub-to-shroud inclined leading edge, the separated regions generated on the pressure sides of the diffuser vanes are reduced in comparison to other cases. However, for −30° inclined leading edge in diffuser vane, the separation and low-momentum flow zones are clearly identified within the diffuser passages, especially close to the trailing edges. Figure 13 showed that the hub-to-shroud inclination angles are more effective to improve the efficiency of the current centrifugal compressor. Moreover, in the case of 30° inclined leading edge, the high-momentum regions in the vaneless space are decreased compared to the original diffuser, and the flow-field is more uniform.

In order to show the effect of inclined leading edges on the flow-field, the time-averaged meridional velocity profiles are shown in Figure 14a. The velocity profiles are circumferentially averaged close to the diffuser vane leading edge. Figure 14a shows that the magnitude of velocity is decreased near the shroud for the 30° case and the difference between minimum and maximum of the velocity signal is decreased in the spanwise direction compared to the original diffuser vane. For 75° and −75° inclination angles, the velocity magnitude is significantly reduced near the shroud and hub, respectively. Moreover, the time-averaged pressure profiles at the midspan along the streamwise direction from inlet to outlet of the diffuser are shown in Figure 14b. It is observed that for 30° case, the pressure recovery along the diffuser passage is increased compared to other cases due to reduction of separations and low-momentum regions.

Figure 15 compares the time-averaged normalized entropy production distribution on the streamwise plane close to the leading edge of the original diffuser vane and various inclined vanes. The entropy production is normalized by the entropy at the impeller exit. The distributions of entropy production for all the cases are almost similar, except for the near hub region. In the cases of the original and −30° inclined vanes, the higher entropy production region close to the pressure side of the diffuser vane hub, indicated by the red circles, is observed, which is caused by the pressure side separations. However, for the 30° inclination angle, the high-entropy region near the hub is significantly reduced, which confirms that the separation flows are postponed inside the diffuser passages.

The time-averaged streamline on the diffuser vane pressure sides for various inclined leading edges are shown in Figure 16. In the case of 30° inclination angle, no recirculation or separated regions are observed on the diffuser vane pressure side, which confirms the hub-to-shroud inclination angles applied in the leading edge of the diffuser vanes can significantly affect the separated flow regions generated by the interaction between the upstream entering flow and the diffuser vane leading edges. It is clear that the hub-to-shroud inclination angle is effective at mixing the low and high momentum flow regions. Therefore, the separated flows are postponed, which leads to enhance the aerodynamic performance of the centrifugal compressor.

In order to visualize the reattached and separation flow regions, time sequences of the Q_criterion iso-surface for different diffuser vanes during one impeller revolution are shown in Figure 17. The Q_criterion is defined as the second invariant of the velocity gradient tensor, which can be calculated by Equation (8) [39]:

$$Q_{criterion}=\frac{1}{2}\left({\Vert \mathsf{\Omega }\Vert }^2-{\Vert S\Vert }^2\right)$$

(8)

where $\mathsf{\Omega }$ and $S$ are vorticity and the rate of deformation tensors, respectively. As indicated by circles in Figure 17a,c, for the original diffuser vane and −30° inclination angle, separation bubbles close to the pressure side of the diffuser vanes, are formed by the impeller–diffuser interaction. These separation bubbles are developed, become larger, and are convected toward the downstream of the diffuser passages by the rotation of impeller with respect to time. However, as shown in Figure 17b for the 30° case, these separation bubbles are not observed within the diffuser passage during the impeller revolution, which confirms the effects of the hub-to-shroud inclined leading edge on postponing the separated flows.

Figure 18a,b shows the time-averaged normalized entropy production and pressure ratio curves, respectively, with respect to the circumferential direction at 1.08 R₂ at various spanwise locations for different inclination angles. In the case of the 30° inclination angle, the range between the minimum and maximum entropy production is decreased and the entropy profiles become more uniform in comparison to the original case. In addition, the values of the entropy production are lower with respect to the other cases, which leads to the reduction of the velocity fluctuations at the diffuser throats, and less separated flows inside the diffuser channels. In addition, as depicted in Figure 18b, increasing the inclination angle increases the static pressure at various locations in the spanwise direction.

Figure 19 shows the time/space dimensionless pressure distributions on the 50% span of the suction and pressure sides of diffuser vanes, for various inclined leading edge during one impeller rotational period. It should be noted that the y axis is normalized by the diffuser vane chord length. It is evident that in all cases, the unsteady pressure fluctuations are well captured.

Figure 19a shows that in the case of the original diffuser vanes, from the leading edge (LE) to trailing edge (TE), the magnitude of pressure is increased due to the diffuser effects. As shown in the figure, the transient effects of the pressure fluctuations are identified near the diffuser inlet on the suction side in −0.3 < $x/c_D$ < 0, which are generated by the reattached and separated flows within the diffuser passages. In addition, near the leading edge of the diffuser vane, there are high-pressure regions, which are caused by the stagnation point and interaction of the impeller and diffuser blades. The generated pressure disturbances by the impeller–diffuser interactions are clearly observed in Figure 19, and are extended from the leading edges toward the trailing edges of the diffuser vanes [40,41,42]. Fifteen main blade pressure waves are clearly visible on the each side of the diffuser vane. Moreover, between these pressure waves, there are other fifteen pressure waves with lower pressure magnitude, which are generated by the splitter blades. As shown in Figure 19, the slope of these generated waves by interactions between the impeller blades and diffuser vanes is constant along the diffuser channel, and is well-known as the convective velocity. From leading edge toward the trailing edge of the diffuser vane, as the main flow travels toward downstream, the magnitude of the pressure waves is decreased, and near the vane trailing edge, the magnitude of these waves is almost uniform. It should be noted that these pressure fluctuations inside the diffuser channels reveal the strong connections between the aerodynamic and acoustic fields, which are called as the dominant discrete noise sources in the centrifugal compressors. In addition, the existence of these pressure waves, which are periodically generated inside the diffuser channels with respect to time confirms the flow pulsation inside the diffuser passages.

It is interesting to note that there are also some other waves with different slopes compared to those of the impeller blades, which are generated along the streamwise direction on the pressure and suction sides of the diffuser vane, as indicated by the arrows in Figure 19. These waves are caused by the unsteady movements of the separated flow regions within the diffuser passages (see Figure 17), which are named as separation pressure waves. These waves are related to shear layer motions inside the diffuser channels as well as the enlargement and concentration of the separation bubbles toward the diffuser exit.

The maximum and minimum values of the static pressure contours were obtained in 30° and −75° inclined leading edges, respectively, which are in a good agreement with Figure 13; Figure 14. Moreover, in the case of 30° inclination angle in the leading edge, no significant separation wave is observed at the pressure and suction sides of the diffuser vane (see Figure 19b). However, in the case of $\alpha =$ −30°, the magnitude of the pressure is lower compared to that of the original diffuser, as well as two big separation waves on the pressure and suction sides are clearly observed as shown in Figure 19c, which are formed at the leading edge, and developed along the diffuser passage throughout the one revolution of the impeller. Figure 19d,e show that for $\alpha = \pm$75°, not only the pressure magnitude is significantly reduced compared to that of the original one, but also as indicated by the yellow arrows in the figure, large number of separation waves inside the diffuser channel are generated.

3.3. Spectral Analysis

Various studies regarding the prediction of noise sources in centrifugal compressors showed that the pressure fluctuations generated by the interactions between the impeller and diffuser blades and turbulent structures inside the compressor channels are the dominant factors, which affect the far-field acoustics [12]. Therefore, the unsteady static pressure at mid-span point of 1.08 R₂ near the impeller–diffuser interface is monitored with respect to time. Figure 20 shows the pressure signal at the compressor design point, for which the time periodic of the pressure fluctuations confirms the convergence of the transient simulation. Figure 20 shows that the current URANS approach has predicted the pressure fluctuations with a good accuracy in terms of magnitude and pattern compared to those calculated by LES in [43].

Figure 21a,b shows the spectra of the near-field pressure fluctuations computed by the current URANS approach for the original leading edge and various inclined leading edges. The sound pressure level (SPL) is evaluated using the fast Fourier transform approach on the pressure fluctuations. The SPL is used to investigate the different contributions of the transient pressure variations in the frequency domain. It should be noted that the SPL spectra of all the inclined leading edge cases were compared to the spectrum of the original diffuser vane, and the horizontal axis is normalized by BPF. As shown in Figure 21, there are clear fundamental peaks in the spectra, which corresponded to the BPF noise and its harmonics. The first and second harmonics of BPF noise are observed at 5.4 kHz and 10.8 kHz, respectively, which are indicated in Figure 21. Figure 21 clearly confirms that the tonal BPF noise and its harmonics, generated by the interaction between the impeller and diffuser, are the dominant noise sources in the current centrifugal compressor.

Figure 21 shows that by applying 30° inclination angle to the leading edge of the diffuser vane, not only the tonal peak at the first BPF is decreased by 7.6 dB, but also the spectrum level is decreased. In addition, Figure 21a shows that the 30° inclined leading edge in the diffuser vane reduces the overall sound pressure level (OASPL) by 5.74 dB. While the 75° inclined leading edge reduces the first BPF tonal noise, the OASPL is increased, due to transient and separated flows inside the diffuser channels. For the original diffuser vanes with the straight leading edges, a spanwise uniformly distributed pressure profiles from the upstream flow are impinged on the leading edges of the diffuser vanes. Therefore, the pressure fluctuations are generated on the vane surfaces and then are propagated toward inside the diffuser passages, which result in separated flows inside the diffuser channels. However, by applying the hub-to-shroud inclination angle on the leading edge of the diffuser vanes, the incoming pressure profiles from upstream are not uniformly distributed in the spanwise direction compared to that of the straight leading edge. This is caused by the pressure variations close to the inclined leading edge region, which could lead to the tonal noise reduction. However, as shown in Figure 21, for the shroud-to-hub inclination angles (−30° and −75°), the tonal noise and OASPL are not reduced. It can be concluded that the 30° inclination angle applied on the leading edges in the diffuser vanes of the current centrifugal compressor is an effective technique to reduce the BPF noise and OASPL, and also to improve the aerodynamic efficiency.

4. Conclusions

A compressible URANS method was performed to numerically predict the flow structures in a transonic centrifugal compressor with pressure ratio of 4. The aerodynamic performance of the original diffuser vane computed by the numerical simulation was validated by the measurements at various operating point conditions. Two types of the inclined leading edges with respect to the diffuser vane height, from hub-to-shroud and shroud-to-hub, were proposed.

(1)

The numerical results of various inclined leading edges showed that the inclination angles are effective tools for improving the efficiency of compressor and stall margin. With the optimal inclination angle of $\alpha$= 30° from hub-to-shroud, the performance at the design point increased by 2.6% and the stall margin by 3.88%, in comparison with the original diffuser. However, for accurate prediction of detailed flow physics near the stall point, transient approaches would be required. Detailed flow investigation inside the diffuser channels confirms that using the hub-to-shroud inclination angles can suppress the separated and secondary flows within the diffuser passage, especially on the vane pressure side.

(2)

The distribution of the static pressure and velocity contours in the diffuser channels demonstrated that the hub-to-shroud inclination angles reduced the flow unsteadiness. In addition, time-averaged streamlines on the surfaces of the diffuser vanes showed that the inclination angle in diffuser vane affects the boundary layer growth inside the diffuser channels, which leads to reduction of the recirculation zones, and thus the flow separations are postponed. It is evident that the hub-to-shroud inclined leading edges are very useful in mixing low and high-momentum flow regions.

(3)

The time/space pressure distribution at the midspan of the diffuser revealed that transient pressure waves mainly occur near the leading edges of the diffuser vanes, and decay very quickly along the diffuse passages. The number of these waves is the same as the number of impeller main and splitter blades, and their slope denotes the convective velocity. Instantaneous time/space distributions of the static pressure for various inclined leading edges confirmed that the 30° inclined leading edge had the maximum pressure level. Additionally, in the case of 30° inclination angle, in contrast with other cases, the pressure oscillations generated by the pseudo-periodic transient separation bubbles with various slopes were not observed on the time/space pressure distributions.

(4)

The spectrum of the near-field pressure fluctuation well predicted the fundamental frequencies corresponding to the first (5.4 kHz) and second (10.8 kHz) BPF harmonics. It is shown that the BPF tonal noise and its harmonics, generated by the interactions between the impeller and diffuser blades, are the dominant noise sources in the centrifugal compressors. The BPF noise and OASPL were decreased by 7.6 dB and 5.74 dB, respectively, by applying 30° inclination angle on the leading edges of the diffuser vanes. This confirms that the inclined leading edges are very effective technique, not only for the reduction of the tonal noise and OASPL, but also for the improvement of the aerodynamic performance.