Proceedings of the ASME th Biennial Conference on Engineering Systems Design and Analysis ESDA2014 June 25-27, 2014, Copenhagen, Denmark

Transcription

1 Proceedings of the ASME th Biennial Conference on Engineering Systems Design and Analysis ESDA2014 June 25-27, 2014, Copenhagen, Denmark ESDA UNSTEADY FLOW SIMULATION IN SUCTION MUFFLER OF A HERMETIC RECIPROCATING COMPRESSOR Umut Can COSKUN and Hasan GUNES Department of Mechanical Engineering, Istanbul Technical University Gumussuyu Istanbul, TURKEY Kemal SARIOGLU and Husnu KERPICCI Arcelik Research and Development Center, Tuzla, 34950, Istanbul, TURKEY ABSTRACT In this study a numerical study of a suction muffler in a hermetic reciprocating compressor of a domestic refrigerator is performed using a finite volume based flow solver (Fluent). In order to reveal the behavior of the flow realistically, unsteady experimental pressure data has been used in the outlet boundary condition for the simulations. Detailed investigations are carried out to reveal the instantaneous flow behavior in different muffler sections such as channel and chambers based on the mass flow rate variation with respect to crankshaft angle. Power spectrum of pressure fluctuations at selected points help to reveal the noise characteristics of the muffler. This study gives a comprehensive insight into the interaction of muffler chambers with flow through the channel. In a previous study, the ratio of the chamber volumes were shown to be an important design parameter. To verify this assumption, three prototype muffler geometries were simulated. In these prototypes, the plate that divides the muffler into two chambers was moved by 7 mm and 10 mm in the direction to enlarge the second chamber. The flow through the prototype geometries were investigated numerically. The results showed that the aerodynamic performance increased while the aero-acoustic performance slightly decreased. Furthermore, this study aims to be an initial step to a more complicated optimization process which involves the inlet valve dynamics. Key words: Unsteady flow simulation, Hermetic compressor, suction muffler, Computational Fluid Dynamics (CFD) INTRODUCTION Due to their vast use in the world, the reciprocating compressors plays a significant role for the global energy consumption [1]. For this reason, European Union established a regulation of energy labeling [2] which encourage the compressor manufacturers to produce more efficient products. Thus, the detailed investigations on various components of reciprocating compressors are among the popular research subjects. In hermetic reciprocating compressors, pressure fluctuations in the cylinder and the suction muffler cause noise as well as a negative effect on the performance of the refrigeration. Therefore, the noise level should be kept at a minimum level for our comfort [3]. Suction muffler is an important compressor component mainly used for controlling the noise level. Many researchers have devoted their attention on suction mufflers with the aim of achieving high performance and low noise levels. Choi et al. (2000) optimized the suction muffler by analyzing the flow and sound fields for an optimum design of a suction muffler [4]. In the same study, it is shown that according to the spectral characteristics of the noise, either one chamber suction muffler or two-chamber suction muffler can be used for noise reduction. Recently, Sarioglu et al. (2012) investigated the refrigerant flow inside the suction muffler experimentally and numerically. They performed time-dependent flow analyses and found that the muffler's inner channel design is critical to reduce the overall pressure loss in the muffler. They also pointed out that after the expansion process, there are back flows during the exhaust period at muffler inlet [5]. Nakano et al. (2008) applied CFD simulations on several components of a reciprocating hermetic compressor including the lubrication system and the suction muffler. In their analysis, they solved three-dimensional unsteady compressible viscous flow with a commercial flow solver, taking pressure variations in the cylinder obtained from previous calculations where they 1 Copyright 2014 by ASME

2 have implemented these data as boundary conditions. They found that the mass flow rate of the suction muffler was increased due to the heat and pressure losses [6]. Pereira et al. (2008) investigated the performance of reciprocating compressors via CFD and validated their data with experiments. They investigated the effect of modification in the design of suction and discharge parts and analyzed energy losses in mufflers and valves aiming to increase the compressor efficiency [7]. In this study, the flow dynamics in a two-chamber suction muffler is simulated in order to improve the performance by increasing the mass flow rate through the muffler. The effect of the volumetric ratio of chambers is investigated numerically. Solutions have been validated with the available experimental data. A good agreement has been achieved with experimental results, i.e., numerical simulations predict average mass flow rate only 4% higher than the measured value. Crankshaft Suction Muffler Fig.2. A typical suction muffler. In this study, the possible effects of the volume ratio of chambers on the aerodynamic and aero-acoustic performances are investigated. In a previous study, it is shown that the pressure fluctuations caused by valve-piston motion decrease during a period [8]. Thus, it is suggested that by increasing the volume ratio of the chamber 2 to chamber 1, one can delay the flutter to a later time in the piston cycle. To verify this assumption, three prototype muffler geometries including the reference one were investigated. In these prototypes, the plate that divides the suction muffler into two chambers was moved by 7 mm and 10 mm in the direction to enlarge the second chamber. In Annex Fig.3 the cross-sections of the prototype suction mufflers are shown. Fig.1. Hermetic reciprocating compressor. COMPUTATIONAL DOMAIN AND BOUNDARY CONDITIONS Geometry and Boundary Conditions In a hermetic reciprocating compressor, the motion of the piston from top to bottom dead center causes the deformation of the valve reed due to the pressure differences between cylinder and the muffler. This deformation opens the path between muffler and the low pressure cylinder. To model the full system (muffler, piston-cylinder and valves), a sophisticated numerical procedure including fluid structure interaction and dynamic mesh has to be performed. However, in this study, we are interested in the flow inside the muffler thus, the flow domain is restricted by the muffler. This simplification is only viable if one can provide the correct cyclic pressure variation in the muffler exit as a boundary condition. Fig.4. The cross-section of the computational domain/mesh of the muffler. 2 Copyright 2014 by ASME

3 Fig.5. Mesh independency tests for steady simulations. The fluid used in our calculations is isobutene which is commonly used as a refrigerant in household refrigerators. Isobutene is assumed to be compressible ideal gas with constant physical properties. The operating pressure inside the compressor is bar. The blue arrow in Fig. 2 shows the pressure inlet and the red arrow shows the pressure outlet boundaries. One period of the fluid motion in the muffler is defined as one cycle of piston motion starting from the top dead center. Experimentally obtained pressure data at each crank angle is used as user specified transient pressure outlet boundary condition as shown in Fig. 7. The constant pressure boundary condition is specified at inlet. All other boundaries are stationary walls with no-slip condition. Due to the compressibility effects, the energy equation has to be solved and all of the wall boundaries are prescribed with constant temperature for simplicity. Mesh quality plays a significant role in the accuracy and the stability of the numerical simulations thus, extensive grid checks have been performed as shown in Fig. 5 to show mesh independence. Grid refinement has been made in flow regions where large gradients occur such as channel walls shown in Fig.6. Fig.7. The pressure data obtained by measurements is employed for outlet boundary condition Fig.6. A detailed view of the computational grid. A case study for choosing a suitable turbulence model and wall function has been performed in order to optimize the numerical model. In reference case (prototype I), the calculations are validated with experimentally available mass flow rate. Our numerical results agree with the experimental data with a deviation of 4%. As we consider a fully periodic flow, the outlet boundary has been prescribed with two kinds of boundary conditions depending on the crank angle. Experimentally it is shown in Fig.7 that the suction reed opens approximately at the crank angle 50 o and closes at 180 o. The intermittent closing and opening movement of the valve reed is called flutter which causes the pressure fluctuations between these angles (as indicated to the left of the red dotted lines in Fig.7. In the numerical simulations 50 o crank angle is determined as the beginning of the period and following 130 o has been chosen as pressure outlet boundary profile. During the remaining 230 o crank angle, the suction reed is considered closed for which we define the outlet boundary as wall with no-slip condition. 3 Copyright 2014 by ASME

4 Governing Equations and Numerical Procedure Our numerical results have been obtained using a finite volume based compressible transient flow solver. The governing equations to be solved are continuity, momentum and energy equations given in (1), (2) and (3) respectively [9]: V t p ij ui uiu j gi t x x x u i i j * i * ij ; t x j * T CpuiT xi xi xi * t (1) (2) (3) Fig.8. The variation of the mass flow rate at inlet section. In addition to conservation equations, equation of state has to be taken into account since the fluid is modeled as compressible ideal gas. Our former studies show that, of all the turbulent models available in Ansys-Fluent, the realizable k-ε turbulence model gives better comparison with the available experimental data, so the realizable k-ε turbulent model with non-equilibrium wall function for near wall treatment is used in our simulations. In the numerical solutions, SIMPLE algorithm is used for pressure-velocity coupling. The density, momentum and energy equations are discretized with second-order upwind scheme. In order to resolve each crank angle, the time step is taken at Δt = 5.67x10-5 seconds. Similar results are obtained when the time step is doubled. RESULTS The effect of piston and valve motions are included to the numerical model indirectly by using experimental pressure profile obtained for Prototype I. This transient profile (as shown in Fig. 7) is used as outlet boundary condition for other Prototypes investigated for comparison. Figure 8 and 9 show the mass flow rate at muffler inlet and outlet sections for the three prototypes. As it can be seen from Fig. 8 and 9, the mass flow rate through the muffler is increased in Prototype II and III. Table 1 shows the mean mass flow rates and the mass-averaged temperatures at outlet sections of each prototype. A suction muffler is desired to cause low pressure loss, provide high mass flow rate and cooler fluid at the outlet section. Based on the requirements above, Prototype II shows better results both aerodynamically and thermally. Fig.9. The variation of the mass flow rate at outlet section. Mean Values Prototype I Prototype II Prototype III Experimental [g/s] Mass F.R. [g/s] Numerical [g/s] Mass F.R. [g/s] (+ %3.34) (+ %2.41) Temp. [K] Table 1. The average mass flow rates and temperatures. Figure 10 and 11 show the variation of the mass flow rate of each prototype at chamber sections (I and II) respectively. Since the volume ratio of the chamber II to chamber I is increased, the contribution of chamber I to main flow is decreased while the contribution of chamber II is increased. Since the volume of the chamber II is increased and it contains higher amount of fluid in Prototype II & III, according to the Fig.11, the mass flow rate contribution of chamber II to main flow during the beginning of the period is increased in Prototype II and III. The instantaneous velocity distributions of Prototype I and III at 60 o crank angle are shown in Fig.12. The flow through the channel in Prototype III is more continuous than the Prototype I. Even though the pressure fluctuation magnitudes are greater in Prototype III, because the chamber I 4 Copyright 2014 by ASME

5 is smaller compared to Prototype I, the main (channel) flow is less effected from chamber I, therefore cooler fluid leaves from the suction muffler. Fig.13. The pressure fluctuations at chamber I. Fig.10. The variation of the mass flow rate at chamber I. Fig.14. The pressure fluctuations at chamber II. Fig.11. The variation of the mass flow rate at chamber II. Flutter of the suction valve is expected to be delayed in a further time in period. Since the same boundary profile is used for all prototypes, such effect cannot possibly be accurately observed. However, this numerical tests show the influence of the volume ratio of the chambers on the aerodynamic and aeroacoustic performance of the suction muffler without simulating the valve motion. In order to understand the aero-acoustic behavior of the muffler prototypes, the pressure fluctuations at chamber I and II are shown in Fig.13 and 14, respectively. We see in these figures that the pressure fluctuations of prototype II and III are very similar and slightly different than prototype I. In the beginning of a period (i.e. suction phase), the magnitude of pressure fluctuations are slightly higher in prototype II&III in both sections while this difference decreases towards the end of the period (compression phase). In any section of the suction muffler, the pressure fluctuations cannot be described with a constant frequency and magnitude. Figure 15 shows the power spectrum of the pressure fluctuations at channel section of each prototype. It can be seen that there are almost no differece between the three Prototypes for frequencies below 300 Hz. However, the frequency magnitudes of Prototype II and III are higher than Prototype I for higher frequencies (> 300 Hz). 5 Copyright 2014 by ASME

6 ACKNOWLEDGEMENT We gratefully acknowledge the financial support of Arçelik A.S. and Scientific Research Office (BAP) of Istanbul Technical University. Fig.15. Power spectrum of pressure fluctuations at channel section of three prototypes. CONCLUSION We present a numerical study to investigate the flow dynamics inside a muffler which is commonly used in hermetic reciprocating compressors. The computations have been performed using a finite volume based, compressible, transient flow solver (Fluent). We investigated the effect of volume ratio of chambers on the aerodynamic and aero-acoustic behavior of suction muffler. We found that the mass flow rate is increased in prototype II and III while the noise level is increased slightly as reflected for higher frequency amplitudes of the power spectrum of the pressure fluctuations. We show that in the absence of the piston-cylinder motion, the unsteady flow in the suction muffler can only be modeled accurately if the experimental data is available. This study aims to be an initial step to a more complicated optimization process involving the piston-cylinder system with valve motion. NOMENCLATURE ρ Density (kg/m 3 ) μ Dynamic viscosity (kg/m.s) g Gravitational acceleration (m/s 2 ) ṁ Mass flow rate (kg/s) τ Stress tensor (Pa) Cp Spesific heat at constant temperature (J/kg.K) T Temperature (K) λ Thermal diffusivity (m 2 /s) V Velocity (m/s) u Velocity component (m/s) REFERENCES [1] Lang, W., Almbauer, R. A, and Jajcevic, D., 2010, "Usage and validation of a fluid structure interaction methodology for the study of different suction valve parameters of a hermetic reciprocating compressor", Int. J. of Multiphysics, Vol 4. Num 1, pp [2] J. EU Commission Directive 2003/66 EG [3] Lee, J. H., An, K. H., and Lee, I., S., 2002, Design of the suction muffler of areciprocating compressor, Int. Compres. Eng. Conf.,Purdue Unv. [4] Choi, J. K., Joo, M. J., Oh, S. K., and Park, S. W., 2000, Smart suction mufflerdesign for a reciprocating compressor, Int. Compres. Eng. Conf.,Purdue Unv. [5] Sarioglu, K., Ozdemir A. R., Oguz, E., and Kaya, A., 2012, An experimental and numerical analysis of refrigerant flow inside the suction muffler of hermetic reciprocating compressor, Int. Compres. Eng. Conf., Purdue Unv. [6] Nakano, A., and Kinjo, K., 2008 CFD applications for development of reciprocating compressor, Int. Compres. Eng. Conf.,Purdue Unv. [7] Pereira, E. L. L., Deschamps, C. J., and Ribas, F. A., Jr, 2008, Performance analysis of reciprocating compressors through computational fluid dynamics, Proc. IMechE, vol. 222, Part E: J. Process Mechanical Engineering. [8] Coskun, U. C., Gunes, H., and Sarioglu, K., 2013, Numerical investigation of suction muffler in household refrigerator compressor, Proc. Int. Conf. of Mechanics, Fluids, Heat, Elasticity and Electromagnetic Fields, pp [9] Ansys-Fluent Theory Guide, Release Copyright 2014 by ASME

7 ANNEX PROTOTYPE GEOMETRIES AND INSTANTANEOUS VELOCITY FIELDS Fig.3. Prototype muffler geometries III, II and I, respectively. Chamber II Velocity [m/s] Chamber I Fig.12. The instantaneous velocity distributions at 60 o crank angle of Prototype I and III respectively. 7 Copyright 2014 by ASME