Numerical Investigation of Impeller-Vaned Diffuser Interaction in a Centrifugal Compressor
Numerical Investigation of Impeller-Vaned Diffuser Interaction in a Centrifugal Compressor
Bardelli, Matteo;Cravero, Carlo;Marini, Martino;Marsano, Davide;Milingi, Omar
2019-04-18 00:00:00
applied sciences Article Numerical Investigation of Impeller-Vaned Diuser Interaction in a Centrifugal Compressor 1 1 2 , 1 1 Matteo Bardelli , Carlo Cravero , Martino Marini *, Davide Marsano and Omar Milingi Dipartimento di Ingegneria Meccanica, Energetica, Gestionale e dei Trasporti (DIME), Università di Genova, 16145 Genova, Italy; matteo.bardelli@edu.unige.it (M.B.); cravero@unige.it (C.C.); davide.marsano@edu.unige.it (D.M.); omar.milingi@gmail.com (O.M.) Dipartimento di Architettura, Design e Urbanistica (DADU), Università di Sassari, 07041 Alghero, Italy * Correspondence: marini@uniss.it; Tel.: +39-079-9720-409 Received: 5 February 2019; Accepted: 13 April 2019; Published: 18 April 2019 Abstract: The work presents the results of a CFD campaign to investigate the impeller–diuser interaction in a centrifugal compressor, taking advantage of experimental data from the open literature. Previous studies on the same turbomachine focused on an experimental investigation to understand the flow interaction between the impeller and the vaned diuser. These experimental data have been used to validate the simulation approach and discuss its results. Several CFD models with increasing complexity have been developed to take into account dierent aspects. The steady analysis has been performed to highlight the potentials and limitations of such models and to carry out a first study of the flow. In order to analyze the impeller–diuser interaction, a further model for the unsteady analysis has been set up. Two dierent operating points have been investigated: one on the surge limit and another in a more stable working zone. A good agreement with the experimental reference data has been obtained with the unsteady analysis and some insights in the complex flow field are deduced. Keywords: centrifugal compressor; CFD; impeller–diuser interaction 1. Introduction The interaction between impeller and diuser in centrifugal compressors is characterized by complex flow phenomena, which are still the focus of several research studies. Such an interaction, characterized by a set of mechanisms which causes distortions in the flow pattern, cannot be pinpointed if the respective components are studied independently. The impeller, because of secondary flows, gives rise to an outlet flow with a strongly unsteady character; the flow coming from the impeller would be non-uniform even after an ideal circumferential averaging, due to the above secondary flows which generate strong dierences of relative velocity and flow angle along the hub to shroud direction. When the eects of viscous transport phenomena are considerable, the flow at impeller exit is typically characterized with a jet and wake pattern (Dean and Senoo, 1960) [1]. As long as the mixing process takes place rapidly, it cannot be completed in the vaneless space, so that unsteady eects are more or less significant, depending on the radial gap. Despite the mixing process taking place rapidly, in the vaneless space the unsteady eects of the impeller are not damped before the diuser blade; these eects are significant and depend on the radial gap between impeller and diuser vane. On the other hand, the diuser vanes cause a speed decrease to ascribe to a potential flow eect (Dean, 1971) [2], unsteady pressure disturbances, and Mach number at the rotor-stator interface (Bulot and Trébinjac, 2009) [3]. Numerical investigations provide good chances to split the dierent phenomena, especially through the comparison between a steady calculation with a mixing plane at impeller–diuser interface Appl. Sci. 2019, 9, 1619; doi:10.3390/app9081619 www.mdpi.com/journal/applsci Appl. Sci. 2019, 9, 1619 2 of 16 and a transient rotor-stator calculation (Yamane et al., 1993 [4], Dawes, 1994 [5], Sato and He, 1999 [6], Shum et al., 2000 [7], Robinson et al., 2012 [8], Younsi et al., 2017 [9]). Many numerical simulations have been developed and applied to study the flow unsteadiness in vaned diusers (Krain, 2002) [10], in vaneless diusers (Kalinkevych and Shcherbakov, 2013) [11], and to compare the two types (Cui, 2005) [12]. The eect of the radial gap between the impeller and vaned diuser has been investigated also (Hosseini et al., 2017) [13]. In the last years, particular attention has been focused on the near surge conditions to better understand the stall mechanism (Bousquet et al., 2014 [14], Fujisawa and Ohta, 2017 [15]) and to devise some criteria to predict the surge limit in centrifugal compressors (Carretta et al., 2017 [16], Cravero and Marsano, 2017 [17]). The interaction between rotor and stator in a centrifugal compressor has also been extensively investigated through experimental analysis (Fisher and Inoue, 1981 [18], Rodgers, 1982 [19]). A previous study on this centrifugal compressor was presented in 2002 by Ziegler [20], who conducted an experimental investigation to understand the flow interaction between the impeller and the vaned diuser. In this paper, a CFD analysis of the compressor object of the Ziegler ’s studies is shown; the detailed geometry and experimental data are available for the test case called Radiver. The Ziegler ’s studies show that a better performance is obtained when the radial gap is small; in this condition, the rotor wake ingested by the diuser channel is capable of energizing the diuser boundary layer, preventing flow separation. For larger radial gaps the mixing processes cause a more radial wake flow in the vaneless space, reducing the above positive eect. In the following, the paper begins with an overview of the reference test case, then the CFD modelling is explained with mesh generation, pre-processing, and steady simulations. The second half of the paper is dedicated to the description of the numerical results, the comparison with experimental data and the discussion of the flow patterns, with special reference to the unsteady eects. 2. Validation of the CFD Approach 2.1. Reference Case The reference case is a centrifugal compressor part of a test rig that was described by Justen et al. (1999) [21], Ziegler et al. (2000) [22], and Ziegler et al. (2002) [23,24]. The data of the CFD test case can be obtained on request by the Institute of Jet Propulsion and Turbomachinery of Aachen. The impeller, developed by MTU Aero Engines, is unshrouded and has 15 backswept aluminum blades. The wedged diuser, designed at the Aachen institute, has 23 blades and allows a continuous adjustment of diuser vane angle ( ) and radial gap (r /r ). Some technical data are presented in 4SS 4 2 Table 1. The measurements of the test case were carried out at 80% rotational speed (N = 28,160 rpm) and the numerical simulations were consequently conducted at that speed. Unsteady measurements were carried out for two diuser geometries: [ = 16.5 , r /r = 1.04] and [ = 16.5 , r /r = 4SS 4 2 4SS 4 2 1.10]. Only the configuration [ = 16.5 , r /r = 1.04] has been considered for the CFD simulations. 4SS 4 2 The results that will be shown in the next sections are relative to the sections in Figure 1, so the CFD analysis can be compared to the experimental campaign taking into account such a nomenclature. 2.2. Mesh and Computational Domain The computational domain has been built on the basis of the geometrical coordinates of the hub, shroud and blade provided by Ziegler (2002) [20], for both the impeller and the vaned diuser. Structured grids have been generated with Turbogrid for the following parts, as reported in Figure 2: (A) single channel of impeller and a portion of the convergent duct, (B) single channel of vaned diuser and a portion of the vaneless diuser. Appl. Sci. 2019, 9, 1619 3 of 16 Table 1. Technical data of compressor for nominal speed and diuser reference geometry. Compressor: Rotational speed at design point N 35,200 rpm Maximum total pressure ratio 4.07 t,max Maximum isentropic eciency (tot/tot) 0.834 stt,max Mass flow at maximum eciency m 1.956 kg/s corr Impeller: Exit radius r 135 mm Number of blades Z 15 Blade backsweep angle at exit 38 bs Appl. Sci. 2019, 9, x 3 of 16 Diuser: Radial gap r4/r2 1.10 Radial gap r /r 1.10 4 2 Di Diffuser height user height b b 11.1 mm 11.1 mm Number of blades Z 23 Number of blades ZD 23 Vane angle 16.5 4SS Vane angle α4SS 16.5° Vane wedge angle 6.615 Vane wedge angle αV 6.615° Figure 1. Measurement planes in meridional (left) and blade to blade (right) view (Ziegler, 2002a) [23]. Figure 1. Measurement planes in meridional (left) and blade to blade (right) view (Ziegler, 2002a) [23]. Dimensions are in [mm] and referred to the configuration [ = 16.5 , r /r = 1.04]. Dimensions are in [mm] and referred to the configuration [α4SS = 16.5°, r4/r2 = 1.04]. 4SS 4 2 The computational domain upstream of the rotor is composed by a non-rotating subdomain from 2.2. Mesh and Computational Domain the inlet section to the rotor ogive where the rotating domain starts; at this point, an interface plane with The computational domain has been built on the basis of the geometrical coordinates of the hub, no mixing is defined. The impeller channel is discretized with an O-grid that consists of 40 elements shroud and blade provided by Ziegler (2002) [20], for both the impeller and the vaned diffuser. along the blade height. The tip clearance is subdivided into 30 mesh elements. The resulting y value Structured grids have been generated with Turbogrid for the following parts, as reported in Figure is 0.5 at the hub and 0.467 on the blade. The convergent duct is discretized with a coarser H-grid to 2: (A) single channel of impeller and a portion of the convergent duct, (B) single channel of vaned save grid elements in a zone without complex flow structures. The diuser channel is also discretized diffuser and a portion of the vaneless diffuser. with an O-grid with 45 elements along the height and this yields y = 0.5 at the hub and shroud walls + + and y = 0.631 on the blade. The above values of y are average values on the corresponding wall. The mesh of the convergent duct + impeller consists of 2.4 10 elements, while the mesh of the diuser has 0.5 10 elements. Appl. Sci. 2019, 9, 1619 4 of 16 Appl. Sci. 2019, 9, x 4 of 16 Figure 2. Mesh details of [convergent duct + impeller] (left) and diuser (right). Figure 2. Mesh details of [convergent duct + impeller] (left) and diffuser (right). All CFD simulations have been carried out with 2 impeller channels and 3 diuser vanes without The computational domain upstream of the rotor is composed by a non-rotating subdomain the volute. from the inlet section to the rotor ogive where the rotating domain starts; at this point, an interface This solution gives a ratio of the circumferential pitch of the rotor domain very close to the plane with no mixing is defined. The impeller channel is discretized with an O-grid that consists of circumferential pitch of the stator domain (diuser vanes) with a pitch ratio at the impeller–diuser 40 elements along the blade height. The tip clearance is subdivided into 30 mesh elements. The interface very close to one (PR = 1.02). With the above condition, the use of periodic flow option in the resulting y value is 0.5 at the hub and 0.467 on the blade. The convergent duct is discretized with a circumferential direction is also acceptable for unsteady simulations. The whole CFD model domain coarser H-grid to save grid elements in a zone without complex flow structures. The diffuser channel consists of 6.3 10 elements. A mesh sensitivity has been performed to check that the compressor is also discretized with an O-grid with 45 elements along the height and this yields y = 0.5 at the hub performance undergoes a variation of less than 1% with the dierent meshes. The mesh sensitivity and and shroud walls and y = 0.631 on the blade. The above values of y+ are average values on the mesh parameters have been tested according to previous experience (Carretta et al., 2017) [16]. corresponding wall. The mesh of the convergent duct + impeller consists of 2.4 × 10 elements, while the mesh of the diffuser has 0.5 × 10 elements. 2.3. CFD Models All CFD simulations have been carried out with 2 impeller channels and 3 diffuser vanes without The ANSYS CFX V17 software platform has been used for the CFD simulations. Figure 3 shows the volute. the dierent CFD models which have been tested: in each box the first row describes the analysis This solution gives a ratio of the circumferential pitch of the rotor domain very close to the type (steady or transient) and the interface option between impeller and diuser (Stage, i.e., mixing circumferential pitch of the stator domain (diffuser vanes) with a pitch ratio at the impeller–diffuser plane or transient), the second row denotes the advection scheme and the third row refers to the interface very close to one (PR = 1.02). With the above condition, the use of periodic flow option in turbulence model. The CFX nomenclature is used, in particular, for the advection upwind scheme, the circumferential direction is also acceptable for unsteady simulations. The whole CFD model which corresponds to a first order accuracy, while high resolution corresponds to a second order domain consists of 6.3 × 10 elements. A mesh sensitivity has been performed to check that the accuracy. The turbulence models adopted are the k-!, the SST and the model k-" with scalable wall compressor performance undergoes a variation of less than 1% with the different meshes. The mesh functions. The following boundary conditions have been set: inlet total pressure and temperature (T , t In sensitivity and mesh parameters have been tested according to previous experience (Carretta et al., p ), inlet turbulence intensity (5%), outlet mass-flow rate and a uniform impeller rotational speed. t In 2017) [16]. The mass flow rate at the exit boundary has been set, instead of the usual static pressure, because the analyses have been performed far from the choking condition. Moreover, a circumferential periodicity 2.3. CFD Models has been fixed because the model includes only a sector of the compressor, consisting of two impeller The ANSYS CFX V17 software platform has been used for the CFD simulations. Figure 3 shows channels and three diuser channels. Finally, all the solid walls have been modelled as adiabatic with the different CFD models which have been tested: in each box the first row describes the analysis no slip condition. type (steady or transient) and the interface option between impeller and diffuser (Stage, i.e., mixing plane or transient), the second row denotes the advection scheme and the third row refers to the turbulence model. The CFX nomenclature is used, in particular, for the advection upwind scheme, which corresponds to a first order accuracy, while high resolution corresponds to a second order accuracy. The turbulence models adopted are the k-ω, the SST and the model k-ε with scalable wall functions. The following boundary conditions have been set: inlet total pressure and temperature (Tt In, pt In), inlet turbulence intensity (5%), outlet mass-flow rate and a uniform impeller rotational speed. The mass flow rate at the exit boundary has been set, instead of the usual static pressure, because the Appl. Sci. 2019, 9, x 5 of 16 analyses have been performed far from the choking condition. Moreover, a circumferential periodicity has been fixed because the model includes only a sector of the compressor, consisting of Appl. two Sci. impeller channels and three 2019, 9, 1619 diffuser channels. Finally, all the solid walls have been modelled 5 of 16 as adiabatic with no slip condition. Figure 3. CFD simulation dataset for operating point M (close to design) and P1 (close to surge). Figure 3. CFD simulation dataset for operating point M (close to design) and P1 (close to surge). Two operating conditions have been simulated: point M (close to design) and point P1 (close to Two operating conditions have been simulated: point M (close to design) and point P1 (close to surge). The numerical simulations for the operating point M did not show stability problems. On the surge). The numerical simulations for the operating point M did not show stability problems. On the other hand, point P1 has been investigated with different models because of numerical instabilities other hand, point P1 has been investigated with dierent models because of numerical instabilities in in the original CFD settings. The activation of the turbulence model k-ω turned out to be necessary the original CFD settings. The activation of the turbulence model k-! turned out to be necessary in in order to dampen the instabilities. In Figure 3 a sketch of the simulation dataset for both operating order to dampen the instabilities. In Figure 3 a sketch of the simulation dataset for both operating points is shown. points is shown. Steady models have been validated after comparing the area averaged numerical results with Steady models have been validated after comparing the area averaged numerical results with the corresponding experimental results along the measurement planes, 2M and 7M, as suggested by the corresponding experimental results along the measurement planes, 2M and 7M, as suggested Ziegler [24]. In all the simulations, a maximum error lower than 5% for the main averaged flow by Ziegler [24]. In all the simulations, a maximum error lower than 5% for the main averaged flow quantities (p, pt, Tt, Ma, α) in the above sections has been obtained with respect to the experimental quantities (p, p , T , Ma, ) in the above sections has been obtained with respect to the experimental t t data. The only exception concerns the results with the model HR-SST in the operating point P1, where data. The only exception concerns the results with the model HR-SST in the operating point P1, where a a stall cell appeared in one of the three diffuser channels and errors for Mach number and flow angle stall cell appeared in one of the three diuser channels and errors for Mach number and flow angle are are much greater. The simulation interested by the stall has one low-velocity channel and two much greater. The simulation interested by the stall has one low-velocity channel and two channels channels with high velocity (because of redistribution of mass flow), as shown by the contours of with high velocity (because of redistribution of mass flow), as shown by the contours of Mach number Mach number in Figure 4. No stall is calculated if, in the operating point P1, a turbulence model k-ω in Figure 4. No stall is calculated if, in the operating point P1, a turbulence model k-! is used. The stall is used. The stall simulated in P1 with the model HR-SST induces an additional energy loss that is simulated in P1 with the model HR-SST induces an additional energy loss that is the cause of a lower the cause of a lower pressure ratio at the diffuser exit, as shown in Figure 5, where the predicted pressure ratio at the diuser exit, as shown in Figure 5, where the predicted overall performance is overall performance is compared with experimental data. However, it must be considered that the compared with experimental data. However, it must be considered that the stall in a three-diuser stall in a three-diffuser vane model has a much greater relative effect on the performance than it vane model has a much greater relative eect on the performance than it would have in a complete would have in a complete model. This occurs because the mass flow redistributes over three channels model. This occurs because the mass flow redistributes over three channels rather than over the whole rather than over the whole annulus, giving a more relevant change in incidence angle to the blade annulus, giving a more relevant change in incidence angle to the blade channels involved. channels involved. Transient simulations have been validated by checking that both area-averaged and local results Transient simulations have been validated by checking that both area-averaged and local results had their time-averaged values close to the corresponding values from steady analysis. Several had their time-averaged values close to the corresponding values from steady analysis. Several monitoring points have been defined at the same probe positions of the measurement devices. The stall monitoring points have been defined at the same probe positions of the measurement devices. The by adopting the turbulence model HR-SST in P1 is still present in the transient calculation and is stall by adopting the turbulence model HR-SST in P1 is still present in the transient calculation and confirmed inside the same diuser vane. The reason is due to the inability of a partial model to simulate is confirmed inside the same diffuser vane. The reason is due to the inability of a partial model to an unsteady circumferential phenomenon: a circumferential periodicity is imposed, which forces the simulate an unsteady circumferential phenomenon: a circumferential periodicity is imposed, which physical phenomenon (as previously observed, the mass flow rate blocked by the stall is redistributed forces the physical phenomenon (as previously observed, the mass flow rate blocked by the stall is in the 2 other channels of the domain and not in the remaining 22 of the complete diuser). In all the redistributed in the 2 other channels of the domain and not in the remaining 22 of the complete unsteady simulations, a time step of 8.87 10 [s] is set, discretizing the passage by a step of 1.5 . −6 diffuser). In all the unsteady simulations, a time step of 8.87 × 10 [s] is set, discretizing the passage These simulations have been carried out until a perfect periodicity of the flow phenomenon is detected. by a step of 1.5°. These simulations have been carried out until a perfect periodicity of the flow In particular, after ten complete revolutions of the impeller, the frequency observed on the signal at the phenomenon is detected. In particular, after ten complete revolutions of the impeller, the frequency impeller outlet is equal to the passage frequency. observed on the signal at the impeller outlet is equal to the passage frequency. Appl. Sci. 2019, 9, 1619 6 of 16 Appl. Sci. 2019, 9, x 6 of 16 Appl. Sci. 2019, 9, x 6 of 16 Figure 4. Mach number distribution at z/b = 0.5 for steady simulations HR k-ω (left) and HR-SST Figure 4. Mach number distribution at z/b = 0.5 for steady simulations HR k-! (left) and HR-SST Figure 4. Mach number distribution at z/b = 0.5 for steady simulations HR k-ω (left) and HR-SST (right) in the operating point P1. (right) in the operating point P1. (right) in the operating point P1. Figure 5. Total pressure ratio at plane 8M. Figure 5. Total pressure ratio at plane 8M. Figure 5. Total pressure ratio at plane 8M. 3. Analysis of the Impeller–Diuser Interaction 3. Analysis of the Impeller–Diffuser Interaction 3. Analysis of the Impeller–Diffuser Interaction 3.1. Steady Analysis at 2M 3.1. Steady Analysis at 2M 3.1. Steady Analysis at 2M The time-averaged quantities were compared to the corresponding values for the steady analysis The time-averaged quantities were compared to the corresponding values for the steady analysis and the The ti experimental me-averaged datqua a. Figur ntities were comp es 6 and 7 show ared to th the pitchwise e correspondin and spanwise g values for distributions the steady an of p for alysis the and the experimental data. Figures 6 and 7 show the pitchwise and spanwise distributions of pt for operating and the exp points erimM ent and al d P1. ataThe . Fignumerical ures 6 andand 7 show experimental the pitchwise data show and sp the anwi same se tr dist end, rib with utions a tendency of pt for the operating points M and P1. The numerical and experimental data show the same trend, with a the operating points M and P1. The numerical and experimental data show the same trend, with a of the numerical results to underestimate the total pressure values; the dierence is comparatively small tendency of the numerical results to underestimate the total pressure values; the difference is and tendency of reaches 10.9% the numeri at its maximum. cal resultIn s to theunderesti case of P1m point ate the total p (Figure 7), r the essure total value pressur s; the e is well-captur difference is ed comparatively small and reaches 10.9% at its maximum. In the case of P1 point (Figure 7), the total comparatively small and reaches 10.9% at its maximum. In the case of P1 point (Figure 7), the total using the k-! turbulence model for up to 50% of the span. The model results become less accurate pressure is well-captured using the k-ω turbulence model for up to 50% of the span. The model results moving pressure i near s we the ll-capt diuser ured fr usin ontg t wall. he k-Inω turbul this zone ence m (z/b o= del 0.7 foand r up to z/b 5= 0% 0.9), of the characterized span. The model by a resul strong ts become less accurate moving near the diffuser front wall. In this zone (z/b = 0.7 and z/b = 0.9), become less accurate moving near the diffuser front wall. In this zone (z/b = 0.7 and z/b = 0.9), whirling flow, the SST simulations seem to provide a better matching with the test case reference characterized by a strong whirling flow, the SST simulations seem to provide a better matching with values. characte Tri he zed spanwise by a strong distribution whirling of flow p , t has he S a maximum ST simulatiat ons z/b seem = 0.7 to provi for both de the a better ma operating tchi points ng wiM th the test case reference values. The spanwise distribution of pt has a maximum at z/b = 0.7 for both the the test case reference values. The spanwise distribution of pt has a maximum at z/b = 0.7 for both the and P1, while the circumferential distribution is almost constant: potential flow eects do not influence operating points M and P1, while the circumferential distribution is almost constant: potential flow the operat total ing po pressur intse M and distribution, P1, whil which e the cir is only cumferent determined ial distrib byuthe tion i impeller s almost geometry constant: pot and e operating ntial flow effects do not influence the total pressure distribution, which is only determined by the impeller effects do not influence the total pressure distribution, which is only determined by the impeller point (inlet conditions, rotational speed). The discussion of the z/b distributions needs a preliminary geometry and operating point (inlet conditions, rotational speed). The discussion of the z/b investigation geometry anon d operat the contributions ing point (inl of static et condit (p) and ions dynamic , rotati(dependent onal speed)on . The Ma) di components scussion of that the z make /b distributions needs a preliminary investigation on the contributions of static (p) and dynamic distributions needs a preliminary investigation on the contributions of static (p) and dynamic (dependent on Ma) components that make up the total pressure values. Only the simulation HR-KO (dependent on Ma) components that make up the total pressure values. Only the simulation HR-KO Appl. Sci. 2019, 9, x 7 of 16 Appl. Sci. 2019, 9, 1619 7 of 16 Appl. Sci. 2019, 9, x 7 of 16 will be considered for the point P1, because of its higher numerical stability and better coherence with will be considered for the point P1, because of its higher numerical stability and better coherence with the experimental data. up the total pressure values. Only the simulation HR-KO will be considered for the point P1, because the experimental data. of its higher numerical stability and better coherence with the experimental data. Figure 6. Total pressure at 2M, point M. Figure 6. Total pressure at 2M, point M. Figure 6. Total pressure at 2M, point M. Figure 7. Total pressure at 2M section, point P1P1. Figure 7. Total pressure at 2M section, point P1 Figure 7. Total pressure at 2M section, point P1 The maximum of p at z/b = 0.7 is merely caused by the dynamic component, as shown by the The maximum of pt at z/b = 0.7 is merely caused by the dynamic component, as shown by the corresponding maximum of Ma in Figure 8, because the static pressure is almost constant along z/b in The maximum of pt at z/b = 0.7 is merely caused by the dynamic component, as shown by the corresponding maximum of Ma in Figure 8, because the static pressure is almost constant along z/b 2M (z/b distribution of p in Figure 8). Because of the low meridional velocity at the surge limit, the flow corresponding maximum of Ma in Figure 8, because the static pressure is almost constant along z/b in 2M (z/b distribution of p in Figure 8). Because of the low meridional velocity at the surge limit, the is essentially tangential in 2M. Therefore, it attacks with a high incidence angle the stator blade leading in 2M (z/b distribution of p in Figure 8). Because of the low meridional velocity at the surge limit, the flow is essentially tangential in 2M. Therefore, it attacks with a high incidence angle the stator blade edge: the stator potential flow field causes a much greater blockage (i.e., higher pressure and lower flow is essentially tangential in 2M. Therefore, it attacks with a high incidence angle the stator blade leading edge: the stator potential flow field causes a much greater blockage (i.e., higher pressure and Mach number) near the diuser PS than near the SS, as can be seen in the pitchwise distributions of p leading edge: the stator potential flow field causes a much greater blockage (i.e., higher pressure and lower Mach number) near the diffuser PS than near the SS, as can be seen in the pitchwise and Ma (Figure 8). lower Mach number) near the diffuser PS than near the SS, as can be seen in the pitchwise distributions of p and Ma (Figure 8). Assuming the inviscid flow hypothesis, the velocity variations in the meridional and blade-to-blade distributions of p and Ma (Figure 8). Assuming the inviscid flow hypothesis, the velocity variations in the meridional and blade-to- planes can be calculated separately, as first proposed by Wu (1952) [25]. Neglecting the force due to the Assuming the inviscid flow hypothesis, the velocity variations in the meridional and blade-to- blade planes can be calculated separately, as first proposed by Wu (1952) [25]. Neglecting the force blade blade lean angle ( = 0), the hub to shroud velocity variation in the meridional plane is given by @n blade planes can be calculated separately, as first proposed by Wu (1952) [25]. Neglecting the force due to the blade lean angle ( 0 ), the hub to shroud velocity variation in the meridional plane the following relation, which has been applied at the impeller exit (n = z, R !1,
= 90 , u = constant): due to the blade lean angle ( 0 ), the hub to shroud velocity variation in the meridional plane is given by the following relation, which has been applied at the impeller exit (n = z, R →∞, γ = 90°, u is given by the following relation, which has been applied at the impeller exit (n = z, Rn→∞, γ = 90°, u = constant): @w w sin w cos @w @c = cos
cos 2W ) = = 0 (1) = constant): ∂w w ⋅ sin β @n R w ⋅ cos β ∂rw ∂c @z @z = − cosγ ⋅ cos β − 2Ω = = 0 2 ∂w w ⋅ sin β w ⋅ cos β ∂w ∂c (1) ∂n R r ∂z ∂z = − cosγ ⋅ cos β − 2Ω = = 0 (1) ∂n R r ∂z ∂z Appl. Sci. 2019, 9, 1619 8 of 16 Appl. Sci. 2019, 9, x 8 of 16 where n is the coordinate perpendicular to the axisymmetric streamsurface, Rn is the curvature radius where n is the coordinate perpendicular to the axisymmetric streamsurface, R is the curvature of the meridional streamline and γ is the angle between streamline and axial direction in the radius of the meridional streamline and
is the angle between streamline and axial direction in the meridional plane. meridional plane. Equation (1) suggests that, under the inviscid flow hypothesis, the hub to shroud velocity Equation (1) suggests that, under the inviscid flow hypothesis, the hub to shroud velocity distribution is constant at the impeller exit. Therefore, the variable distribution of Ma along z/b shown distribution is constant at the impeller exit. Therefore, the variable distribution of Ma along z/b shown in Figure 8 is due to viscous phenomena inside the impeller. in Figure 8 is due to viscous phenomena inside the impeller. Figure 8. Figure 8. Mach Mach nu number mber and pressu and pressur re e at 2M at 2M a and nd P1 po P1 point. int. 3.2. Impeller Flow Analysis 3.2. Impeller Flow Analysis Figure 9 shows the meridional velocity contours at five hub-to-shroud sections of the impeller and Figure 9 shows the meridional velocity contours at five hub-to-shroud sections of the impeller Figure 10 presents the corresponding turbulent kinetic energy contours. At surface 1, the meridional and Figure 10 presents the corresponding turbulent kinetic energy contours. At surface 1, the velocity is clearly influenced by blade loading (with a faster relative flow at SS) and by dierent meridional velocity is clearly influenced by blade loading (with a faster relative flow at SS) and by curvatures of the walls (which are the cause for the hub to shroud gradient). The meridional velocity different curvatures of the walls (which are the cause for the hub to shroud gradient). The meridional distribution is progressively distorted downstream by the increasing thickness of the shroud boundary velocity distribution is progressively distorted downstream by the increasing thickness of the shroud layer; this can be seen at surface 3 of Figure 11. The growth of this low momentum region corresponds boundary layer; this can be seen at surface 3 of Figure 11. The growth of this low momentum region to the increase of the high turbulence zone at the casing shown in Figure 10. A better knowledge corresponds to the increase of the high turbulence zone at the casing shown in Figure 10. A better of the complex phenomena inside the rotor can be achieved through the analysis of the vorticity knowledge of the complex phenomena inside the rotor can be achieved through the analysis of the contours of Figure 11. The dierent contributions to secondary flows can be seen clearly in surface vorticity contours of Figure 11. The different contributions to secondary flows can be seen clearly in 1: two blade surface vortices along the blade height (at SS: BVS, at PS: BVP, i.e., blade surface surface 1: two blade surface vortices along the blade height (at SS: BVS, at PS: BVP, i.e., blade surface vortices at the respective sides) and a strong vortex near the casing. This last vortex results from the vortices at the respective sides) and a strong vortex near the casing. This last vortex results from the merging of the passage vortex at shroud (PVS) and the Coriolis vortex (CV), as discussed by Van den merging of the passage vortex at shroud (PVS) and the Coriolis vortex (CV), as discussed by Van den Braembussche [26]. The blade vortex is stronger at the SS, due to the greater velocity gradient of the Braembussche [26]. The blade vortex is stronger at the SS, due to the greater velocity gradient of the boundary layer, and tends to vanish towards the radial exit, as shown in Figure 11. This is consistent boundary layer, and tends to vanish towards the radial exit, as shown in Figure 11. This is consistent with the conservation equation of the vorticity along a streamline derived by Smith [27] and developed with the conservation equation of the vorticity along a streamline derived by Smith [27] and by Hawthorne [28]. The blade vorticity carries low energy fluid along the blade, from the hub to the developed by Hawthorne [28]. The blade vorticity carries low energy fluid along the blade, from the hub to the tip. PVS (passage vortex at shroud) and CV (Coriolis vortex) contribute to the transport of Appl. Sci. 2019, 9, 1619 9 of 16 Appl. Sci. 2019, 9, x 9 of 16 Appl. Sci. 2019, 9, x 9 of 16 tip. PVS (passage vortex at shroud) and CV (Coriolis vortex) contribute to the transport of low energy low energy fluid from PS to SS along the shroud wall. The passage vortex is typically stronger in the fluid from PS to SS along the shroud wall. The passage vortex is typically stronger in the first half of low energy fluid from PS to SS along the shroud wall. The passage vortex is typically stronger in the first half of the impeller (because of higher blade-to-blade curvature) and at the shroud, while in the the impeller (because of higher blade-to-blade curvature) and at the shroud, while in the radial portion, first half of the impeller (because of higher blade-to-blade curvature) and at the shroud, while in the radial portion, the Coriolis force prevails (Kang and Hirsch, 2001) [29]; in this case, the effect at the the Coriolis force prevails (Kang and Hirsch, 2001) [29]; in this case, the eect at the hub is not clearly radial portion, the Coriolis force prevails (Kang and Hirsch, 2001) [29]; in this case, the effect at the hub is not clearly visible. The Coriolis vortex (CV) and the passage vortex (PV) have the same effect visible. The Coriolis vortex (CV) and the passage vortex (PV) have the same eect and are not always hub is not clearly visible. The Coriolis vortex (CV) and the passage vortex (PV) have the same effect and are not always distinguishable one from the other: they are often referred to as passage vortices. distinguishable one from the other: they are often referred to as passage vortices. The overall eect is a and are not always distinguishable one from the other: they are often referred to as passage vortices. The overall effect is a low energy fluid transport towards the shroud wall and the SS. Moreover, at low energy fluid transport towards the shroud wall and the SS. Moreover, at the casing, the above The overall effect is a low energy fluid transport towards the shroud wall and the SS. Moreover, at the casing, the above secondary flows interact with the tip vortex (TV). The passage vortex is well- secondary flows interact with the tip vortex (TV). The passage vortex is well-defined in the first part the casing, the above secondary flows interact with the tip vortex (TV). The passage vortex is well- defined in the first part of the impeller (Figure 11, surface 1) but it is clearly distorted by the trailing of the impeller (Figure 11, surface 1) but it is clearly distorted by the trailing vortex downward and defined in the first part of the impeller (Figure 11, surface 1) but it is clearly distorted by the trailing vortex downward and tends to move towards midspan. Weiss [30] described this phenomenon for tends to move towards midspan. Weiss [30] described this phenomenon for the same compressor. vortex downward and tends to move towards midspan. Weiss [30] described this phenomenon for the same compressor. The overall result is a thick high-turbulence region in the upper half of the The overall result is a thick high-turbulence region in the upper half of the channel (shown in Figure 10 the same compressor. The overall result is a thick high-turbulence region in the upper half of the channel (shown in Figure 10 for surface 5) that corresponds to the low relative velocity region in for surface 5) that corresponds to the low relative velocity region in Figure 12 (wake). The remaining channel (shown in Figure 10 for surface 5) that corresponds to the low relative velocity region in Figure 12 (wake). The remaining portion of the section has low turbulence level with high flow portion of the section has low turbulence level with high flow velocity and identifies the jet zone in the Figure 12 (wake). The remaining portion of the section has low turbulence level with high flow velocity and identifies the jet zone in the jet-wake model. jet-wake model. velocity and identifies the jet zone in the jet-wake model. Figure 9. Meridional velocity in the impeller, point P1. Figure 9. Meridional velocity in the impeller, point P1. Figure 9. Meridional velocity in the impeller, point P1. Figure 10. Figure 10. Turbulence kinetic energy in the i Turbulence kinetic energy in them impeller peller, point , point P1. P1. Figure 10. Turbulence kinetic energy in the impeller, point P1. Appl. Sci. 2019, 9, x 10 of 16 Appl. Sci. 2019, 9, 1619 10 of 16 Appl. Sci. 2019, 9, x 10 of 16 Figure 11. Vorticity in three hub-to-shroud surfaces of the impeller, point P1. PVS—passage vortex at shroud; BVS and BVP—blade surface vortices at SS and PS; CV—Coriolis vortex. The velocity contours in the relative frame are shown in Figure 12 in a plane close to the mixing- plane interface on the impeller side. On the same plane, the relative flow angle distribution shows a thin stripe near the casing; here, the relative flow is completely tangential because of the tip leakage vortex and the fixed (counter-rotating in the relative frame) shroud wall. Close to the blades, the relative angle becomes more and more affected by the trailing edge local distortion. The relative flow near PS is more tangential, while the relative flow near SS is more radial and they join downstream the trailing edge. Towards the channel midspan, the flow in the wake zone has a more radial character than in the jet zone, due to the low energy transport from pressure side to suction side caused by the Figure 11. Vorticity in three hub-to-shroud surfaces of the impeller, point P1. PVS—passage vortex at Figure 11. Vorticity in three hub-to-shroud surfaces of the impeller, point P1. PVS—passage vortex at passage vortex. shroud; BVS and BVP—blade surface vortices at SS and PS; CV—Coriolis vortex. shroud; BVS and BVP—blade surface vortices at SS and PS; CV—Coriolis vortex. The velocity contours in the relative frame are shown in Figure 12 in a plane close to the mixing- plane interface on the impeller side. On the same plane, the relative flow angle distribution shows a thin stripe near the casing; here, the relative flow is completely tangential because of the tip leakage vortex and the fixed (counter-rotating in the relative frame) shroud wall. Close to the blades, the relative angle becomes more and more affected by the trailing edge local distortion. The relative flow near PS is more tangential, while the relative flow near SS is more radial and they join downstream the trailing edge. Towards the channel midspan, the flow in the wake zone has a more radial character Figure 12. Relative velocity and angle at impeller exit in the relative frame of reference, point P1. Figure 12. Relative velocity and angle at impeller exit in the relative frame of reference, point P1. than in the jet zone, due to the low energy transport from pressure side to suction side caused by the passage vortex. The velocity contours in the relative frame are shown in Figure 12 in a plane close to the The flow structure in the absolute frame can be discussed with the aid of the local velocity mixing-plane interface on the impeller side. On the same plane, the relative flow angle distribution triangle sketched in Figure 13. High absolute velocities and tangential flow direction characterize the shows a thin stripe near the casing; here, the relative flow is completely tangential because of the tip wake zone (neglecting the flow distortion at the endwalls) while low absolute velocities and radial leakage vortex and the fixed (counter-rotating in the relative frame) shroud wall. Close to the blades, flow direction are encountered in the jet zone, as shown in Figure 14. The relative angle distortion the relative angle becomes more and more aected by the trailing edge local distortion. The relative close to the blades is the reason for lower PS and higher SS absolute velocities. The absolute velocity flow near PS is more tangential, while the relative flow near SS is more radial and they join downstream maximum value occurs approximately at 70% of the channel height. The above considerations the trailing edge. Towards the channel midspan, the flow in the wake zone has a more radial character explain the Mach number distribution along z/b direction presented in Figure 8 and the total pressure than in the jet zone, due to the low energy transport from pressure side to suction side caused by the curves of Figure 7. A very similar flow structure is observed for the operating point M (Milingi, 2016) passage vortex. [31]. Figure 12. Relative velocity and angle at impeller exit in the relative frame of reference, point P1. The flow structure in the absolute frame can be discussed with the aid of the local velocity triangle sketched in Figure 13. High absolute velocities and tangential flow direction characterize the wake The flow structure in the absolute frame can be discussed with the aid of the local velocity zone (neglecting the flow distortion at the endwalls) while low absolute velocities and radial flow triangle sketched in Figure 13. High absolute velocities and tangential flow direction characterize the direction are encountered in the jet zone, as shown in Figure 14. The relative angle distortion close to wake zone (neglecting the flow distortion at the endwalls) while low absolute velocities and radial the blades is the reason for lower PS and higher SS absolute velocities. The absolute velocity maximum flow direction are encountered in the jet zone, as shown in Figure 14. The relative angle distortion value occurs approximately at 70% of the channel height. The above considerations explain the Mach close to the blades is the reason for lower PS and higher SS absolute velocities. The absolute velocity number distribution along z/b direction presented in Figure 8 and the total pressure curves of Figure 7. maximum value occurs approximately at 70% of the channel height. The above considerations A very similar flow structure is observed for the operating point M (Milingi, 2016) [31]. Appl. explain the M Sci. 2019, 9, x ach number distribution along z/b direction presented in Figure 8 and the total pressure 11 of 16 curves of Figure 7. A very similar flow structure is observed for the operating point M (Milingi, 2016) [31]. Figure 13. Velocity triangle. Figure 13. Velocity triangle. Figure 14. Absolute velocity and angle at impeller exit in the relative frame of reference, point P1. 3.3. Unsteady Analysis at 2M In this section, the results from the transient analysis are discussed to understand the effect of the non-uniform rotating flow pattern coming from the impeller on the vaned diffuser. The analysis is focused on plane 2M for operating point P1 to get a direct comparison with the experimental data. Because of random sampling inherent to the L2F technique and due to the need for a constant time- step in the simulations, there is a minor shift between numerical and experimental instants (with absolute errors between 0.1% and 2.6%). The analysis is performed using the same rotor-stator positions from measurements. Figures 15 and 16 are diffuser-sided views in the absolute frame of reference: the impeller moves from right to left. The numerical results have been obtained from the transient simulation approach HR-KO discussed in the previous section. A good matching between the numerical and the experimental data can be observed with very similar flow patterns. The main difference takes place in the velocity distribution at the unsteady position φID/φtI = 0.595. At that instant, experimental results show a high velocity zone extending clearly from right to left along the front wall and spreading towards the rear wall; this stretching is not completely detected with the numerical simulation. On the other hand, a velocity pattern similar to the experimental data has been obtained for the two transient simulations using the SST model for the operating points M and P1. Nevertheless, in the operating point P1, the results with SST are shifted because of the stall appearing downstream in the diffuser channel, so consequently the flow is slower and more tangential at plane 2M. The results using the SST model are not used for further discussion because of the instability produced by the stalled channel in the diffuser, as previously discussed. Appl. Sci. 2019, 9, x 11 of 16 Appl. Sci. 2019, 9, 1619 11 of 16 Figure 13. Velocity triangle. Figure 14. Absolute velocity and angle at impeller exit in the relative frame of reference, point P1. Figure 14. Absolute velocity and angle at impeller exit in the relative frame of reference, point P1. 3.3. Unsteady Analysis at 2M In this section, the results from the transient analysis are discussed to understand the eect of the non-uniform rotating flow pattern coming from the impeller on the vaned diuser. The analysis 3.3. Unsteady Analysis at 2M is focused on plane 2M for operating point P1 to get a direct comparison with the experimental In this section, the results from the transient analysis are discussed to understand the effect of data. Because of random sampling inherent to the L2F technique and due to the need for a constant the non-uniform rotating flow pattern coming from the impeller on the vaned diffuser. The analysis time-step in the simulations, there is a minor shift between numerical and experimental instants is focused on plane 2M for operating point P1 to get a direct comparison with the experimental data. (with absolute errors between 0.1% and 2.6%). The analysis is performed using the same rotor-stator Because of random sampling inherent to the L2F technique and due to the need for a constant time- positions from measurements. Figures 15 and 16 are diuser-sided views in the absolute frame of step in the simulations, there is a minor shift between numerical and experimental instants (with reference: the impeller moves from right to left. The numerical results have been obtained from the absolute errors between 0.1% and 2.6%). The analysis is performed using the same rotor-stator transient simulation approach HR-KO discussed in the previous section. A good matching between positions from measurements. Figures 15 and 16 are diffuser-sided views in the absolute frame of the numerical and the experimental data can be observed with very similar flow patterns. The main reference: the impeller moves from right to left. The numerical results have been obtained from the dierence takes place in the velocity distribution at the unsteady position ' /' = 0.595. At that ID tI transient simulation approach HR-KO discussed in the previous section. A good matching between instant, experimental results show a high velocity zone extending clearly from right to left along the the numerical and the experimental data can be observed with very similar flow patterns. The main front wall and spreading towards the rear wall; this stretching is not completely detected with the difference takes place in the velocity distribution at the unsteady position φID/φtI = 0.595. At that numerical simulation. On the other hand, a velocity pattern similar to the experimental data has been instant, experimental results show a high velocity zone extending clearly from right to left along the obtained for the two transient simulations using the SST model for the operating points M and P1. front wall and spreading towards the rear wall; this stretching is not completely detected with the Nevertheless, in the operating point P1, the results with SST are shifted because of the stall appearing numerical simulation. On the other hand, a velocity pattern similar to the experimental data has been downstream in the diuser channel, so consequently the flow is slower and more tangential at plane obtained for the two transient simulations using the SST model for the operating points M and P1. 2M. The results using the SST model are not used for further discussion because of the instability Nevertheless, in the operating point P1, the results with SST are shifted because of the stall appearing Appl. Sci. 2019, 9, x 12 of 16 produced by the stalled channel in the diuser, as previously discussed. downstream in the diffuser channel, so consequently the flow is slower and more tangential at plane 2M. The results using the SST model are not used for further discussion because of the instability produced by the stalled channel in the diffuser, as previously discussed. Figure 15. Unsteady absolute velocity at 2M in the absolute frame of reference, point P1, comparison Figure 15. Unsteady absolute velocity at 2M in the absolute frame of reference, point P1, comparison between numerical results of HR-KO (left) and experimental results (right). between numerical results of HR-KO (left) and experimental results (right). Many of the effects studied separately in the previous sections using steady analysis can now be seen in the single unsteady analysis. Flow incidence at the diffuser is positive (i.e., absolute flow is more tangential with respect to the diffuser vane camber line) almost exclusively near the front wall where the wake generates a highly tangential absolute flow. On the other hand, the incidence angle becomes lower (and negative) towards the rear wall (jet zone). Furthermore, a thicker positive- incidence zone can be seen from the right to the left in the center of the wake zone moving with the impeller channel. The flow has a higher velocity close to the front wall because of the jet-wake flow pattern. The absolute velocity maximum values are located at about z/b = 70% as shown by the monitoring points and by the vortical structures analysis. The absolute velocity becomes lower and the flow more radial (negative incidence) at the diffuser vane leading edge on the right side because of the diffuser vane blockage; the opposite occurs on the left side, with respect to the vane leading edge. A velocity maximum can therefore be seen close to the front wall on the diffuser vane suction side, while a minimum is found at the opposite corner (between the rear wall and the pressure side). The velocity peak is more evident when the high-velocity zones in the impeller flow (Figure 13) are aligned with those caused by the potential flow field: this occurs at φID/φtI = 0.093. Appl. Sci. 2019, 9, 1619 12 of 16 Appl. Sci. 2019, 9, x 13 of 16 Figure 16. Unsteady incidence at 2M in the absolute frame of reference, point P1, comparison between Figure 16. Unsteady incidence at 2M in the absolute frame of reference, point P1, comparison between numerical results of HR-KO (left) and experimental results (right). numerical results of HR-KO (left) and experimental results (right). Many of the eects studied separately in the previous sections using steady analysis can now be A zone with high negative incidence values appears along the rear wall towards the vane seen in the single unsteady analysis. Flow incidence at the diuser is positive (i.e., absolute flow is more diffuser pressure side (see instants corresponding to φID/φtI = 0.093 − 0.843). It is clearly distorted by tangential with respect to the diuser vane camber line) almost exclusively near the front wall where the passage of the impeller blade trailing edge (see instants φID/φtI = 0.342 − 0.595) with high flow the wake generates a highly tangential absolute flow. On the other hand, the incidence angle becomes incidence. lower (and negative) towards the rear wall (jet zone). Furthermore, a thicker positive-incidence zone Figure 17 displays the pressure fluctuation in a monitoring point placed close to the center of can be seen from the right to the left in the center of the wake zone moving with the impeller channel. plane 2M, for the three transient calculations. The flow has a higher velocity close to the front wall because of the jet-wake flow pattern. The absolute velocity maximum values are located at about z/b = 70% as shown by the monitoring points and by the vortical structures analysis. The absolute velocity becomes lower and the flow more radial (negative incidence) at the diuser vane leading edge on the right side because of the diuser vane blockage; the opposite occurs on the left side, with respect to the vane leading edge. A velocity maximum can therefore be seen close to the front wall on the diuser vane suction side, while a minimum is found at the opposite corner (between the rear wall and the pressure side). The velocity peak is more evident when the high-velocity zones in the impeller flow (Figure 13) are aligned with those caused by the potential flow field: this occurs at ' /' = 0.093. ID tI A zone with high negative incidence values appears along the rear wall towards the vane diuser pressure side (see instants corresponding to' /' = 0.093 0.843). It is clearly distorted by the passage ID tI Figure 17. Pressure fluctuation in percentage at 2M for φ/φtD = 0.4145 (z/b = 0.5). of the impeller blade trailing edge (see instants ' /' = 0.342 0.595) with high flow incidence. ID tI Figure 17 displays the pressure fluctuation in a monitoring point placed close to the center of Two types of fluctuations are visible: a former with a high frequency and a latter with a low plane 2M, for the three transient calculations. frequency, which corresponds to three times the impeller rotational frequency. The former is caused Two types of fluctuations are visible: a former with a high frequency and a latter with a low by the impeller blade passage while the latter is probably due to downstream disturbances (e.g., fr diffuser v equency,awhich ne edges). The corresponds simulation for to three times the oper the impeller ating point rotational P1 wifr th equency the HR.-KO Themodel show former is caused s lower by the impeller blade passage while the latter is probably due to downstream disturbances (e.g., diuser fluctuations compared to the results with the HR-SST model. In the case of operating point M, the vane HR-Sedges). ST mod The el shows simulation simifor lar h the igh operating frequency point osci P1llwith ations but the HR-KO great model er low shows frequency lower osci fluctuations llations. compared to the results with the HR-SST model. In the case of operating point M, the HR-SST model Therefore, the SST tends to generate stronger downstream disturbances, as confirmed by the P1 with shows HR-SST case similarwhere high fr high frequency equen osci cllations y oscillation but gr s are also eater low much frequency more oscillations. evident. This is assessed as Therefore, the SST the tends to generate stronger downstream disturbances, as confirmed by the P1 with HR-SST case where reason for the stall detection at the operating point P1 using the SST model. The stall would be a high rotatifr ng equency stall, pa oscillations ssing to the neighboring di are also much mor ffuser e evident. vanes, but wi This is assessed th the 3-va asn the e periodic reason mod for the el, t stall he simulation of the phenomenon is inhibited. Appl. Sci. 2019, 9, x 13 of 16 Figure 16. Unsteady incidence at 2M in the absolute frame of reference, point P1, comparison between numerical results of HR-KO (left) and experimental results (right). A zone with high negative incidence values appears along the rear wall towards the vane Appl. Sci. 2019, 9, 1619 13 of 16 diffuser pressure side (see instants corresponding to φID/φtI = 0.093 − 0.843). It is clearly distorted by the passage of the impeller blade trailing edge (see instants φID/φtI = 0.342 − 0.595) with high flow detection at the operating point P1 using the SST model. The stall would be a rotating stall, passing to incidence. the neighboring diuser vanes, but with the 3-vane periodic model, the simulation of the phenomenon Figure 17 displays the pressure fluctuation in a monitoring point placed close to the center of is inhibited. plane 2M, for the three transient calculations. Figure 17. Pressure fluctuation in percentage at 2M for φ/φtD = 0.4145 (z/b = 0.5). Figure 17. Pressure fluctuation in percentage at 2M for '/' = 0.4145 (z/b = 0.5). tD 4. Conclusions Two types of fluctuations are visible: a former with a high frequency and a latter with a low frequency, which corresponds to three times the impeller rotational frequency. The former is caused The role and features of dierent CFD models to investigate the flow in the centrifugal stage by the impeller blade passage while the latter is probably due to downstream disturbances (e.g., configuration of a dynamic compressor have been discussed; a quite detailed comparison between the diffuser vane edges). The simulation for the operating point P1 with the HR-KO model shows lower numerical results obtained and corresponding experimental data has been possible thanks to the rich fluctuations compared to the results with the HR-SST model. In the case of operating point M, the dataset from Ziegler et al. (2002) [23,24]. The simplified approach with a reduced number of channels HR-SST model shows similar high frequency oscillations but greater low frequency oscillations. has been discussed with respect to the full annulus analysis. The steady simulations have allowed Therefore, the SST tends to generate stronger downstream disturbances, as confirmed by the P1 with by a first analysis to identify the main phenomena occurring at the impeller-vaned diuser interface. HR-SST case where high frequency oscillations are also much more evident. This is assessed as the Diuser potential flow field causes a lower absolute velocity at the stator leading-edge projection reason for the stall detection at the operating point P1 using the SST model. The stall would be a on plane 2M. At the operating point close to surge, the velocity deficit at the impeller outlet plane rotating stall, passing to the neighboring diffuser vanes, but with the 3-vane periodic model, the becomes more evident and moves towards the diuser pressure side because of a more tangential simulation of the phenomenon is inhibited. flow. A study of vortical structures in the rotor has helped to understand the impeller flow structure. A strong passage vortex, transferring low energy flow from pressure to suction side in the impeller channel, interacts with the opposite tangential flow due to the tip vortex. The final eect is an evident jet-wake flow pattern at the impeller exit with the wake zone placed in the upper half along the channel height (close to shroud) and with the jet zone in the remaining part. A good agreement with the experimental data has been obtained, with the unsteady analysis of impeller–diuser interaction and the instantaneous data giving a further insight into the flow structure at the impeller exit. A peak with high velocity value is detected close to the front wall and SS diuser vane with the lowest value placed at the opposite corner (rear wall and PS projection). The SST turbulence model has identified a stall cell in the diuser channel that was not detected by the k-! model and no clear evidence of this is shown in the experimental data. It could be a rotating stall, not highlighted by the experiments, that cannot be simulated with a periodic 3-vane model. The simulations in the operating point P1 using the k-! model show a good agreement with experimental data. Author Contributions: The contribution of all the authors has to be subdivided on to an equal basis. M.M. and C.C. designed the methodology and revised the draft; M.B., D.M. and O.M. contributed to calculations in dierent phases and interpretation of results. Funding: This research received no external specific funding. Acknowledgments: The above analysis has been possible thanks to the detailed data set (Radiver test case) provided by Niehuis. The authors are grateful to Niehuis, Ziegler, and Institute of Jet Propulsion and Turbomachinery for the sharing of their precious results and data. Conflicts of Interest: The authors declare no conflict of interest Appl. Sci. 2019, 9, 1619 14 of 16 Nomenclature c absolute velocity c meridional component of c i incidence angle to the diuser camber line k turbulent kinetic energy m ˙ mass flow rate Ma Mach number N shaft speed p pressure r radius T temperature u circumferential speed (W ) w relative velocity z/b relative coordinate normal to the diuser rear wall (Figure 1) Z number of blades absolute flow angle (Figure 17) relative flow angle (Figure 17) '/' circumferential coordinate relative to the diuser pitch (Figure 1) tD ' /' impeller unsteady position relative to the impeller pitch (see '/' in Figure 1) ID tI tI pressure ratio ! vorticity W angular velocity Subscripts D Diuser In Inlet I Impeller max maximum t total Acronyms HR High Resolution KE K-Epsilon (k-") KO K-Omega (k-!) PS Pressure Side SS Suction Side SST Shear Stress Transport UW Upwind Operating Points M stable (Figure 5) P1 near surge (Figure 5) References 1. Dean, R.C.; Senoo, Y. Rotating Wakes in Vaneless Diusers. ASME J. Basic Eng. 1960, 82, 563–570. [CrossRef] 2. Dean, R.C. On the Unresolved Fluid Dynamics of the Centrifugal Compressor. Advanced Centrifugal Compressors; ASME Gas Turbine Division: New York, NY, USA, 1971; pp. 1–55. 3. Bulot, N.; Trébinjac, I. Eect of the Unsteadiness on the Diuser Flow in a Transonic Centrifugal Compressor Stage. Int. J. Rotating Mach. 2009, 2009, 932593. [CrossRef] 4. Yamane, T.; Fujita, H.; Nagashima, T. Transonic Discharge Flows around Diuser Vanes from a Centrifugal Impeller; ISABE Paper 93-7053; ISABE: Tokyo, Japan, 1993. 5. Dawes, W.N. A Simulation of the Unsteady Interaction of a Centrifugal Impeller with its Vaned Diuser: Flow Analysis; ASME Paper 94-GT-105; ASME: New York, NY, USA, 1994. 6. Sato, K.; He, L. Eect of Rotor-Stator Interaction on Impeller Performance in Centrifugal Compressors. Int. J. Rotating Mach. 1999, 5, 135–146. [CrossRef] Appl. Sci. 2019, 9, 1619 15 of 16 7. Shum, Y.K.P.; Tan, C.S.; Cumpsty, N.A. Impeller-Diuser Interaction in Centrifugal Compressors. ASME J. Turbomach. 2000, 122, 777–786. [CrossRef] 8. Robinson, C.; Casey, M.; Hutchinson, B.; Steed, R. Impeller-Diuser Interaction in Centrifugal Compressors; ASME Paper GT2012-69151; ASME: New York, NY, USA, 2012. 9. Younsi, M.; Corneloup, C.; Moyroud, F.; Baldacci, A. Unsteady flow in a centrifugal compressor stage equipped with a vaned diuser and cavities. In Proceedings of the ASME Turbo Expo 2017: Turbomachinery Technical Conference and Exposition, Charlotte, NC, USA, 26–30 June 2017. 10. Krain, H. Unsteady Diuser Flow in a Transonic Centrifugal Compressor. Int. J. Rotating Mach. 2002, 8, 223–231. [CrossRef] 11. Kalinkevich, M.; Shcherbakov, O. Numerical Modeling of the Flow in a vaneless Diuser of Centrifugal Compressor Stage. ISRN Mech. Eng. 2013, 2013, 602384. [CrossRef] 12. Cui, M. Comparative Study of Unsteady Flows in a Transonic Centrifugal Compressor with Vaneless and Vaned Diusers. Int. J. Rotating Mach. 2005, 1, 90–103. [CrossRef] 13. Hosseini, M.; Sun, Z.; He, X.; Zheng, X. Eects of Radial Gap Ratio between Impeller and Vaned Diuser on Performance of Centrifugal Compressors. Appl. Sci. 2017, 7, 728. [CrossRef] 14. Bousquet, Y.; Carbonneau, X.; Dufour, G.; Binder, N.; Trébinjac, I. Analysis of the Unsteady Flow Field in a Centrifugal Compressor from Peak Eciency to Near Stall with Full-Annulus Simulations. Int. J. Rotating Mach. 2014, 2014, 729629. [CrossRef] 15. Fujisawa, N.; Ohta, Y. Transition Process from Diuser Stall to Stage Stall in a Centrifugal Compressor with a Vaned Diuser. Int. J. Rotating Mach. 2017, 2017, 2861257. [CrossRef] 16. Carretta, M.; Cravero, C.; Marsano, D. Numerical prediction of centrifugal compressor stability limit. In Proceedings of the ASME Turbo Expo 2017: Turbomachinery Technical Conference and Exposition, Charlotte, NC, USA, 26–30 June 2017. 17. Cravero, C.; Marsano, D. Numerical prediction of stability limit in centrifugal compressors with vaneless diuser. In Proceedings of the 23rd International Symposium on Air Breathing Engines (ISABE 2017), Manchester, UK, 3–8 September 2017. 18. Fisher, E.H.; Inoue, M. A study of diuser/rotor interaction in a centrifugal compressor. J. Mech. Eng. Sci. 1981, 23, 149–156. [CrossRef] 19. Rodgers, C. The performance of Centrifugal Compressor Channel Diusers. In Proceedings of the ASME 1982 International Gas Turbine Conference and Exhibit, London, UK, 18–22 April 1982. 20. Ziegler, K.U. CFD Test Case: Centrifugal Compressor “Radiver” with MTU Impeller of Aachen University; Institute of Jet Propulsion and Turbomachinery: Aachen, Germany, 2002. 21. Justen, F.; Ziegler, K.U.; Gallus, H.E. Experimental Investigation of Unsteady Flow Phenomena in a Centrifugal Compressor Vaned Diuser of Variable Geometry. ASME J. Turbomach. 1999, 121, 763–771. [CrossRef] 22. Ziegler, K.U.; Justen, F.; Rothstein, M.; Gallus, H.E.; Niehuis, R. Research on a Centrifugal Compressor of Variable Geometry. In Proceedings of the 15th International Compressor Engineering Conference, West Lafayette, IN, USA, 25–28 July 2000. 23. Ziegler, K.U.; Gallus, H.E.; Niehuis, R. A Study on Impeller-Diuser Interaction: Part I—Influence on the Performance. In Proceedings of the ASME Turbo Expo 2002: Power for Land, Sea, and Air, Amsterdam, The Netherlands, 3–6 June 2002. 24. Ziegler, K.U.; Gallus, H.E.; Niehuis, R. A Study on Impeller-Diuser Interaction: Part II—Detailed Flow Analysis. In Proceedings of the ASME Turbo Expo 2002: Power for Land, Sea, and Air, Amsterdam, The Netherlands, 3–6 June 2002. 25. Wu, C.H. A General Theory of 3D Flow in Subsonic and Supersonic Turbomachines of Axial, Radial and Mixed Flow Types. Available online: //apps.dtic.mil/dtic/tr/fulltext/u2/a380493.pdf (accessed on 17 April 2019). 26. Van den Braembussche, R.A. Description of Secondary Flow in Radial Flow Machines. Thermodyn. Fluid Mech. Turbomach. 1985, II, 665–684. 27. Smith, A.G. On the Generation of the Streamwise Component of Vorticity for Flows in a Rotating Passage. Aeronaut. Q. 1957, 8, 369–383. [CrossRef] 28. Hawthorne, W.R. Secondary Vorticity in Stratified Compressible Fluids in Rotating Systems; CUED/A-Turbo/TR 63; Engineering Department, Cambridge University: Cambridge, UK, 1974. Appl. Sci. 2019, 9, 1619 16 of 16 29. Kang, S.; Hirsch, C. Numerical Simulation and Theoretical Analysis of the 3D Viscous Flow in Centrifugal Impellers. Task Q. 2001, 5, 433–458. 30. Weiss, C.; Grates, D.R.; Thermann, H.; Niehuis, R. Numerical Investigation of the Tip Clearance on Wake Formation Inside a Radial Impeller. In Proceedings of the ASME Turbo Expo 2003, collocated with the 2003 International Joint Power Generation Conference, Atlanta, GA, USA, 16–19 June 2003. 31. Milingi, O. Numerical Investigation of Impeller-Vaned Diuser Interaction in a Centrifugal Compressor. Master ’s Thesis, University of Genoa, Genova, Italy, 2016. © 2019 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (http://creativecommons.org/licenses/by/4.0/).
http://www.deepdyve.com/assets/images/DeepDyve-Logo-lg.png
Applied Sciences
Multidisciplinary Digital Publishing Institute
http://www.deepdyve.com/lp/multidisciplinary-digital-publishing-institute/numerical-investigation-of-impeller-vaned-diffuser-interaction-in-a-zCcL74IEtl