Loading...

Methodology for the Numerical Characterization of a Radial Turbine under Steady and Pulsating Flow

Doctoral Thesis / Dissertation 2012 243 Pages

Engineering - Mechanical Engineering

Excerpt

Contents

1 Introduction
1.1 Introduction
1.1.1 CFD codes
1.1.2 Turbomachinery modeling
1.2 Objectives
1.3 Methodology

Chapter 1 bibliography

2 Set-up analysis and optimization of numerical simulations for radial turbines
2.1 Introduction
2.1.1 CFD in turbomachinery
2.2 Computational methodology. Definition of a reference case
2.2.1 Experimental methodology
2.2.2 Computational domain
2.2.3 Boundary conditions
2.2.4 Wheel rotation strategies
2.2.5 Viscous model
2.3 Mesh independence
2.3.1 Volute
2.3.2 Stator
2.3.3 Rotor
2.3.4 Outlet section
2.3.5 Final considerations and selected mesh
2.4 Set-up Comparison
2.4.1 Type of solver
2.4.2 Mesh motion strategy
2.4.3 Temporal discretization
2.5 Summary of the results: Turbine map
2.6 Summary and conclusions

Chapter 2 bibliography

3 Implementation of a 1D-3D coupling computational fluid dynamic boundary condition
3.1 Introduction
3.2 Coupling methodology
3.2.1 The method of characteristics
3.2.2 Homentropic flow
3.2.3 Non-Homentropic flow
3.3 Implementation
3.3.1 OpenWAM
3.3.2 ANSYS-FLUENT
3.4 Validation
3.4.1 Sod’s problem
3.4.2 Impulse test rig
3.5 Conclusions

Chapter 3 bibliography

4 Development of an anechoic boundary condition for compu- tational fluid dynamic codes
4.1 Introduction
4.2 Non-reflecting boundary conditions
4.2.1 Assessment of NRBCs available in ANSYS-FLUENT
4.2.2 Implementing a boundary condition in a CFD commer- cial code
4.3 Proposal of a new non-reflecting boundary condition for non- homentropic flow
4.3.1 Modifications for non-homentropic flow
4.3.2 Implementation of an anechoic condition
4.3.3 Incident pressure condition
4.4 Application to the analysis of the acoustic response of a muffler
4.4.1 Experimental facility
4.4.2 Full three-dimensional simulation
4.4.3 Proposed Methodology
4.5 Summary and conclusions

Chapter 4 bibliography

5 Analysis of the influence of real flow effects in computational fluid dynamics boundary conditions based on the method of characteristics
5.1 Introduction
5.2 Non-perfect gas
5.3 Viscous flow
5.4 Swirling flow
5.5 Possible applications of the developed boundary conditions
5.5.1 Anechoic BC
5.5.2 Coupled 1D-3D simulation
5.6 Conclusions

Chapter 5 bibliography

6 Computational analysis of pulsating flow in radial turboma- chinery and its application to engine modelling
6.1 Introduction
6.2 Computational methodology and steady flow results
6.3 Pulsating flow results
6.3.1 Overall behavior
6.3.2 Local behavior of the different components
6.4 Discussion of results
6.5 Application to engine modeling
6.5.1 Proposed model
6.5.2 Model calibration
6.5.3 Pulsating results
6.6 Conclusions

Chapter 6 bibliography

7 Conclusions and future works
7.1 Conclusions
7.1.1 Computational methodology: Case configuration
7.1.2 Developed boundary conditions
7.1.3 Pulsating flow
7.2 Original contributions
7.3 Future works

Chapter 7 Bibliography

Global bibliography

Appendix 1: UDF code

Appendix 2: OpenWAM CFD connection

List of symbols

Latin letters

Abbildung in dieser Leseprobe nicht enthalten

Greek letters

Abbildung in dieser Leseprobe nicht enthalten

Subscript

Abbildung in dieser Leseprobe nicht enthalten

Superscript

Abbildung in dieser Leseprobe nicht enthalten

Abbreviations

Abbildung in dieser Leseprobe nicht enthalten

Chapter 1 Introduction

Contents

1.1 Introduction

1.2 Objectives

1.3 Methodology

Chapter 1 bibliography

1.1 Introduction

compressible flow turbine is a flow device that extracts energy from a fluid by expanding it through a stator and rotor system. When the flow passes through the rotor, it has a high tangential velocity that causes the rotation of the blades. The fluid can be a gas or a liquid depending on the applications. Turbines, depending of their geometry, can be classified in various types: axial, radial, or mixed flow ones, are used in all kinds of power- plants. Different scales of turbines are used, from the large turbines usually used in aircraft propulsion or the steam turbines for electricity generation to the smaller ones used in micro gas turbines. The most common application of radial turbomachinery is probably as part of a turbocharger for internal combustion engines (ICEs).

In the last decades, the legislation on internal combustion engines has severely reduced the limits for pollutant and noise emissions. This fact, com- bined with the necessity to keep production costs bounded, has driven re- searchers to optimize the efficiency of ICEs. These requirements have estab- lished the research activity at design phase as a key stage in the engine produc- tion process. Therefore, an intensive investigation on ICEs has been carried out, focusing on the optimization of performances and fuel consumption. In particular, the improvement of gas exchange processes has been thoroughly investigated [100, 26, 110].

Turbocharging is one of the most important technologies for the automo- tive industry, and particularly for diesel engines[5]. In an ICE, the energy of the exhaust gases is about 30-40 percent of the chemical energy released by the combustion[85]. These gases are expanded trough the turbine of the turbocharger which drives the compressor connected through shaft. The com- pressor is used to increase the density of the air admitted to the cylinder. Thereby the power output of the engine can be increased or alternatively the engine size can be reduced, without decreasing the power output. This tech- nique is known as downsizing. The use of turbochargers allows one to reduce the engine cylinder volume and weight, without reducing the power and torque produced. At the same time, this technology decreases the fuel consumption and reduces emissions [71, 85], which is vital for successfully fulfilling the cur- rent restrictions imposed by legislation.

The increasing use of turbochargers is leading to an outstanding develop- 2 ment of turbocharging technology. For instance, turbine vanes have evolved greatly over the last years, from being just a flat plate to the aerodynamically- shaped profiles used in the most recent designs. Another development in turbochargers industry that has been rapidly introduced in the market are variable geometry turbines (VGT), which improve transient performance of the engine [2, 25]. In order to keep improving the efficiency of turbochargers, it is necessary to understand and fully characterize its internal flow behavior.

Unfortunately, the effect on an ICE performance due to modifications in gas exchange components cannot be predicted beforehand, since the interac- tions between the acoustic responses of the different elements involved (intake or exhaust systems, turbomachinery, etc.) are quite strong [91, 77]. In this way, the use of computational fluid dynamics (CFD) has helped researchers in understanding flow behavior inside these components [20, 72] and also in al- lowing predictions of the results of different configurations without the cost of testing them experimentally[9]. CFD simulations allow researchers to under- stand flow behavior and quantify important flow parameters such as mass flow rates or pressure drops, provided that the CFD tools had been properly val- idated against experimental results. For reasons such as the aforementioned, CFD simulations have become a valuable tool in helping both the analysis and design of the intake and exhaust systems of an ICE.

1.1.1 CFD codes

The CFD codes are usually used in a wide range of engineering applications. Probably the most used ones are the one-dimensional and the three dimen- sional CFD models.One-dimensional CFD codes allow to understand global behavior of a flow system in terms of flow rates and pressure, having a good resolution in unsteady compressible problems. These codes solve a simplified version of the fluid flow governing equations in cases that have a dominant direction. Their main advantage is their low computational cost. However, if a good geometrical resolution or a more detailed flow field is needed, 3D simulations become essential. Three-dimensional CFD codes allow one to ob- tain an accurate solution of the flow field of the studied system, but with a extremely higher computational cost, moreover if non-steady simulations are considered.

CMT-Motores Térmicos has developed a 1D CFD code, particularly design 3 for the calculation of pressure waves in the intake and exhausts systems of an ICE. OpenWAM is an open source one-dimensional gas dynamic model able to compute the air management of internal combustion engine 79. The code is based in assuming a one-dimensional flow and neglecting the effect of viscosity. The resulting system of equations is solved in the time domain using a Finite Difference 2-step Lax-Wendroff scheme. The code also includes lumped models to compute the filling and emptying process of other ICE elements as cylinders, plenums, heat exchanges, etc.

Dealing with three-dimensional computations, CMT-Motores Térmicos has experience with several commercial codes. In the current work, the computations have been performed using the code ANSYS-FLUENT. ANSYSFLUENT is a finite volume code, capable of simulating viscous 3-dimensional flows. ANSYS-FLUENT is used extensively in industries such as automotive, aerospace, chemical, etc. The use of a commercial code has the advantage of having been extensively validated, but it has the inconvenience of its lack of accessibility to the flow variables and to the code itself.

1.1.2 Turbomachinery modeling

As previously commented CMT-Motores Térmicos has a in-house open source 1D code called OpenWAM. This code computes the pipes composing an ICE by means of a discretization of the Navier-Stokes equations. Additionally, the code includes some zero dimensional subcomponents which allow to model the rest of the elements of an ICE, acting as boundary conditions, and thus acquiring the capacity of simulating the behavior of a whole engine. Partic- ularly interesting for this thesis are the models of the compressor[44], and specially, turbine[99]. The turbine model is based on two nozzles in series, separated by an intermediate reservoir, which reproduces mass accumulation in the system. The reaction degree is calculated by means of geometrical pa- rameters and the corrected variables, obtained from the turbine maps. Once reaction degree is determined, the pressure drops produced at the stator and at the rotor can be computed taking into account the turbine efficiency, and the type and the position of the stator vanes. The model has proved to give good results for fixed and variable geometry turbines. As input, the model requires the turbine maps. Those can be supplied by the manufacturer or mea- sured in a turbocharger test rig. CMT-Motores Térmicos has the capability of experimentally testing turbochargers in steady or pulsating flow conditions.

Currently two different types of testing rigs are available, a steady flow test bench which uses a rotary screw compressor or those based in mounting the turbo on a truck engine. The first ones allow testing in steady flow conditions, as it is commonly done by turbomachinery manufacturers. However, pulsating conditions can by achieved using a rotatory valve. On the contrary, the second type allow to test the turbocharger working on engine conditions. The current measurement techniques commonly used in radial turbomachinery only allow obtaining global values of the flow variables, but not a complete description of the flow field. In this frame of ideas, the use of three dimensional CFD turbomachinery computations seems interesting.

For the case of 3D simulations, CMT-Motores Térmicos has experience in this field, mostly on aspects dealing with the air management in cylinder, combustion process, and flow in diesel injectors and jets. However, this thesis is among the firsts works in the group dealing with CFD computations of turbomachinery.

Modeling turbomachinery poses particular problems: their geometrical complexity requires the use of viscous compressible three dimensional (3D) codes to capture the flow behavior properly. Additionally, a mesh motion pro- cedure is needed in order to truthfully reproduce the rotor flow. This mesh motion can be obtained using a steady approach (multiple reference frame) in which the mesh does not really moves or a fully transient procedure (sliding mesh model). The first approach has the advantage of its lower computa- tional cost, but typically unsteady flow effects are missed in the process and can only be captured if the mesh is really moved. However this makes the computational cost even higher, and additionally, an oscillation is induced in the flow variables. These fluctuations travel along the domain, and eventu- ally are reflected when reaching the boundaries. These reflections increase the computational time required to achieve a periodic solution.

Regarding CFD simulation, it is worth clarifying the difference between the type of solver used and the dependence with time of the boundary conditions. The solver can be steady or transient. In a steady solver the equations terms related to the temporal variation are not included, while the transient one does include these terms. If a sliding mesh model is used, then the solver must be transient. However, in a transient simulation the boundary conditions can be either steady or time dependent, depending on whether the turbine is analyzed under steady flow conditions or pulsating conditions.

If the objective of the computation is to obtain the acoustic response of a system the use of long ducts is needed in order to avoid any interference pro- duced by the boundaries. This fact can be easily understood when compared to the experimental procedure used to obtain the acoustic response in an im- pulse test rig, such as the one simulated in[20]. Including these long ducts in the computational domain leads to a dramatic increase of the computational cost[46].

In this frame, the idea of developing a non-reflecting boundary condition (NRBC) that behaves as a long duct seems interesting. Since the acoustic re- sponse of these long ducts is supposed to be the lack of wave reflection, several researchers [87, 7, 29] have tried to developed the so-called non-reflecting or anechoic boundary conditions (BCs), to be able to eliminate these components without any penalty in the accuracy. A similar reasoning can be followed if a turbocharger test rig has to be simulated, in which long ducts are needed in order to have uniform flow at the measurement sections. Their inclusion in the computational domain could represent even doubling the number of cells in some configurations.

1.2 Objectives

Since this is the first thesis in CMT-Motores Térmicos which has as a main core a CFD analysis of turbomachinery, the main objective of the present thesis is to develop a methodology to characterize the behavior of a radial turbine by means of CFD. Additionally, the methodology intends to optimize the use of the current computational resources available, obtaining the best resolution possible and reducing the total computational time required.

A second objective is to analyze the performances of a radial turbine under steady and pulsating flow conditions. The testing at steady flow conditions is the most common procedure followed by turbochargers manufacturers, while pulsating flow is more similar to the real conditions when the turbine is working on a reciprocating engine. The steady flow results are used to validate the numerical procedure and afterwards obtain the pulsating results to have a better understanding of the transient flow effects in the radial turbine.

The main advantage of the use of CFD is that the complete flow field can be analyzed, in contrast to the current experimental measurements, in which only global variables are obtained. The last objective is the use of this new information available to improve the turbine models that are currently in use, particularly for the transient flow regimen.

1.3 Methodology

Once the main objectives of the thesis have been established, the methodology followed in this thesis is now described.

Since this is the first thesis in the group whose based on CFD computations of turbomachinery, the first task was to develop a methodology of performing those computations using ANSYS-FLUENT. Additionally, an optimization of the case with the objective of obtain the best resolution possible with the available computational resources was conducted. In this frame the compu- tational domain, the mesh and the different configuration models need to be defined as done in chapter 2. In order to evaluate the mesh independence, and thus be able to optimize the cell distribution, an analysis was performed. The different models used in the simulations were described. Particularly, a comparison of the solver types and the moving mesh strategies was shown. In this chapter, an experimental test-stand for turbochargers is also describes. The measurements obtained in this facility are used to evaluate the results obtained with numerical simulations in steady flow conditions.

Generally, the test facilities employed for testing radial turbines have long inlet and outlet ducts. If these ducts need to be simulated, the computational cost can be severely increased. Similar argument might be done if a simulation of the turbine installed in a complete engine model is required. Due to the expected one-dimensionality of the internal flow in the ducts and the availabil- ity on a one-dimensional numerical code, which can model a whole turbine, as OpenWAM, the development of a boundary condition to connect the 3D domain in ANSYS-FLUENT with the domain in OpenWAM seems interest- ing. The use of this boundary condition will allow to perform 1D-3D coupled computations, where good geometrical resolution is achieved where required, while the rest of the domain can be computed using a less computationally expensive code. The development and implementation of this boundary condi- tion is presented in chapter 3. Following the same criteria, some problems can be found in which the modeling of a semi-infinite duct could be interesting. This could be the case of the analysis of the acoustic response of a system, in which the reflections of the pressure waves at the boundaries need to be avoided. In this case, the use of a so-called anechoic or non-reflecting bound- ary condition could reduce the computational requirements of the simulation. The non-reflecting conditions available in ANSYS-FLUENT were assessed and afterwards a new formulation has been proposed and implemented in chapter 4. The two developed boundary conditions are based in the method of charac- teristics. However, there use of this method relies on some assumptions that are not always fulfilled in turbomachinery simulations. Therefore, an analysis of the influence of real flow effects on them was conducted in chapter 5. The computational tools developed in this thesis could be use to optimize the use of the requirements of a simulation, allowing to increase the effort in the most interesting regions of the domain and reducing the resources needed in the rest on them.

The turbine has been characterized under steady flow conditions in chapter 2, as it is has been traditionally done for testing turbomachinery. This tradi- tion probably comes from the aeronautic field, where it is common to obtain the performance of turbomachinery under these conditions. However, when the turbine is installed in a reciprocating engine, the flow at the turbine inlet is modulated by the piston movement. In order to evaluate the behavior of the turbine under pulsating conditions, numerical simulations using sinusoidal pressure pulses at the inlet are presented in chapter 6. These data is used to increase the knowledge of the unsteady internal flow in the turbine, and in this way, contribute to radial turbine modeling.

Finally, in chapter 7 the main contributions and conclusions of the thesis are summarized. These conclusions lead to a series of future work to con- tinue with the current research in turbomachinery modeling. For the sake of clarity and to make easier the review of the bibliography, the references cited on each chapter are collected at the end of the respective chapter in order of appearance; while the whole bibliography is included in alphabetic order after chapter 7. The code developed implementing the boundary conditions presented in chapters 3 and 4 is included as appendix at the end of the present document.

Chapter Bibliography 1

[2] J. Andersen, E. Karlsson, and A. Gawell. “Variable turbine geometry on SI engines”. In: SAE 2006 World Congress. SAE 2006-01-0020. 2006 (cit. on pp. 3, 16)

[5] E. Arcaklioglu and I. ¸ elikten. “A diesel engine’s performance and exhaust emissions”. In: Applied Energy 80.1 (2005), pp. 11-22 (cit. on p. 2).

[7] O. V. Atassi. “Nonreflecting boundary conditions for the time-dependent convective wave equation in a duct”. In: Journal of Computational Physics 197.2 (2004), pp. 737-758. issn: 0021-9991 (cit. on pp. 6, 81, 108).

[9] N. C. Baines. “A meanline prrediction method for radial turbine ef- ficiency”. In: 6 th International Conference on Turbocharging and Air Management Systems, I Mech E. C554-6. Concepts ETI, Inc. Institution of Mechanical Engineers, 1998 (cit. on p. 3).

[20] A. Broatch, X. Margot, A. Gil, and F. D. Denia. “A CFD Approach to the Computation of the Acoustic Response of Exhaust Mufflers”. In: Journal of Computational Acoustic 13.2 (2005), pp. 301-316. doi: 10.1142/S0218396X05002682 (cit. on pp. 3, 6, 72, 80, 95, 97).

[25] H. Chen. “Turbine wheel design for Garrett advanced variable geom- etry turbines for commercial vehicle applications”. In: 8th Interna tional Conference on Turbochargers and Turbocharging, Institution of Mechanical Engineers. 2006 (cit. on pp. 3, 16).

[26] C. D. Copeland, R. Martinez-Botas, and M. Seiler. “Comparison Be- tween Steady and Unsteady Double-Entry Turbine Performance Using the Quasi-Steady Assumption”. In: Journal of Turbomachinery 133 (2011), pp. 031001-1/031001-10 (cit. on pp. 2, 126, 130).

[29] J. R. Dea, F. X. Giraldo, and B. Neta. “High-order non-reflecting boundary conditions for the linearized 2-D Euler equations: No mean flow case”. In: Wave Motion 46.3 (2009), pp. 210-220 (cit. on pp. 6, 81, 108).

[44] J. Galindo, JR Serrano, H. Climent, and A. Tiseira. “Experiments and modelling of surge in small centrifugal compressor for automotive engines”. In: Experimental Thermal and Fluid Science 32.3 (2008), pp. 818-826 (cit. on p. 4).

[46] J. Galindo, A. Tiseira, P. Fajardo, and R. Navarro. “Coupling method- ology of 1D finite difference and 3D finite volume CFD codes based on the Method of Characteristics”. In: Mathematical and Computer Modelling 54.7-8 (2011), pp. 1738-1746. doi: http://dx.doi.org/ 10.1016/j.mcm.2010.11.078 (cit. on pp. 6, 15, 62, 81, 88, 93, 112, 118, 167).

[71] K. Mollenhauer and H. Tschoeke. Handbook of Diesel Engines. Springer, 2010 (cit. on p. 2).

[72] G. Montenegro and A. Onorati. “Modeling of Silencers for IC Engine Intake and Exhaust Systems by Means of an Integrated 1D-multiD Approach”. In: SAE International Journal of Engines 1.1 (2009), p. 466. doi: 10.4271/2008-01-0677 (cit. on pp. 3, 62, 80).

[77] M. L. Munjal. Acoustics of ducts and mufflers with application to ex- haust and ventilation system design. Wiley-Interscience, 1987. isbn: 0471847380 (cit. on pp. 3, 95).

[79] OpenWAM. CMT- Motores Térmicos. Universidad Politécnica de Va- lencia. url: http : / / www . OpenWAM . org (cit. on pp. 4, 14, 63, 87, 98).

[85] F. Payri and J. M. Desantes, eds. Motores de combusti ó n interna al- ternativos. Reverté, 2011 (cit. on p. 2).

[87] F. Payri, J. M. Desantes, and A. J. Torregrosa. “Acoustic boundary condition for unsteady one-dimensional flow calculations”. In: Journal of Sound and Vibration 188.1 (1995), pp. 85-110. issn: 0022-460X (cit. on pp. 6, 15, 83, 87, 108).

[91] K. S. Peat, A. J. Torregrosa, A. Broatch, and T. Fernández. “An inves- tigation into the passive acoustic effect of the turbine in an automotive turbocharger”. In: Journal of Sound and Vibration 295.1-2 (2006), pp. 60-75 (cit. on p. 3).

[99] J. R. Serrano, F. J. Arnau, V. Dolz, A. Tiseira, and C. Cervelló. “A model of turbocharger radial turbines appropriate to be used in zero-and one-dimensional gas dynamics codes for internal combustion engines modelling”. In: Energy Conversion and Management 49.12 (2008), pp. 3729-3745 (cit. on pp. 4, 120, 141, 144, 149).

[100] J. R. Serrano, F. J. Arnau, P. Piqueras, A. Onorati, and G. Montenegro. “1D gas dynamic modelling of mass conservation in engine duct systems with thermal contact discontinuities”. In: Mathematical and Computer Modelling 49.5-6 (2009), pp. 1078-1088. doi: 10.1016/j.mcm.2008. 03.015 (cit. on pp. 2, 64, 69).

[110] M. Tancrez, J. Galindo, C. Guardiola, P. Fajardo, and O. Varnier. “Turbine adapted maps for turbocharger engine matching”. In: Ex- perimental Thermal and Fluid Science 35.1 (2011), pp. 146-153. doi: 10.1016/j.expthermflusci.2010.07.018 (cit. on p. 2).

Chapter 2 Set-up analysis and optimization of numerical simulations for radial turbines

Contents

2.1 Introduction

2.2 Computational methodology. Definition of a reference case

2.3 Mesh independence

2.4 Set-up Comparison

2.5 Summary of the results: Turbine map

2.6 Summary and conclusions

Chapter 2 bibliography

2.1 Introduction

over the last years, researchers have focused in trying to understand the fluid dynamic processes in a turbomachine [55, 11]. The research can be done in two different ways: experimental or computational. Experimental research is carried out by testing the turbo in a test rig [43, 106, 96]. Other researchers use CFD in order to analyze and understand the internal flow in the turbine 53, therefore it is becoming a valuable tool for studying this kind of systems 119. There have been some studies in order to characterize the internal flow in a radial turbine under steady flow conditions [31, 112, 51]. In order to increase the efficiency of radial turbines some improvements are used as the variable geometry stator, which allow having a better performance in a wider flow range 53.

There are 0D-1D models which allow to simulate a fluid system obtaining good temporal response even in supersonic regime [79, 88]. However there are some conditions in which a good geometrical resolution is needed and therefore 3D simulations are needed. 3D-CFD codes allow to obtain an accurate solution of the flow field of the studied system, but with considerable computational cost [1, 102]. In this chapter, a methodology to configure the computational case of a turbine is presented, focusing on the definition of the computational model, in terms of meshing, mesh movement algorithm and computational algorithm.

In this chapter, an analysis of the main works found on CFD in turbomachinery are analyzed next. Afterwards the procedures followed to define the case configuration used are presented.

2.1.1 CFD in turbomachinery

CFD is a valuable tool for researchers in all disciplines of fluid mechanics and particularly in turbomachinery. Its use is growing constantly due to the ad- vances in development of numerical methods and computational power. How- ever, concerning the design process of a new turbomachine, the direct use of CFD tools is still unfeasible with the current computational capabilities 6. The problem of designing a turbine (or the optimization of an existing one) reduces to the selection of reasonable values for the different geometric pa- rameters. Nowadays the know-how of the designer is still the main tool for designing and optimizing turbomachines [123, 10].

Generally, 1D approaches to design and analyze turbomachines can be considered well adapted and powerful enough for most applications, such as turbocharger matching with the ICE. However, design and research are reach- ing a point in which it is necessary to fully understand the internal flow of the turbine. In the literature, there are some papers showing a good correspon- dence between CFD computations and experimental results [28, 112, 102, 58]. It is possible to find more works concerning CFD in turbomachinery, Blanco- Marigorta et al. 16 studied the influence of the volute geometry and relative position between impeller and volute casing by means of an unsteady simu- lation, but with steady boundary conditions, using FLUENT. Palfreyman et al. studied the aerodynamic characteristics of a mixed-flow turbine [81, 97] or other CFD works on radial turbomachines 51.

When turbochargers are tested in an experimental rig, long ducts at the inlet and exit are needed, mainly when it comes to pulsating flow, in order to avoid spurious reflections on the boundaries and being able to decompose the pressure waves depending on their traveling direction 87. In the same way, long distances are needed in the computational model, increasing the size of the mesh and therefore the computational requirements. There are some situations in which the turbomachine works at highly unsteady condi- tions, requiring transient simulations, which increase the computational cost furthermore. In this case, it is necessary to simulate enough time in order to allow the different pressure waves to cross the domain. In order to mini- mize computational requirements the idea of performing 1D-3D co-simulations seems clear 46, which allows to simulate a complex system by using 3D simu- lations just in the zones of the domain where it is needed, while keeping most of the piping system with a 1D model.

The objective of this chapter is to optimize the set-up of a 3D simulation for a turbocharger turbine in order to maximize the efficiency of the compu- tations, that is, to achieve the higher resolution possible with the available computational resources. A second objective could be to present a list of good working practices to perform CFD simulations in turbomachinery for industry. Different aspects must be considered. An introduction of the uses of CFD in turbomachinery has been presented. The first thing that must be analyzed when dealing with 3D simulations is the geometry considered and more precisely the mesh. The mesh should be fine enough to truthfully reproduce the wanted geometry, this is usually achieved by searching the in- dependence of the solution with the mesh. This analysis is done later on the chapter. A commercial code as ANSYS-FLUENT has different discretization schemes implemented. A discussion on them is also presented on the chapter. A CFD turbomachinery simulation must also deal with other models as the viscous model and more importantly in the case of rotating machines, the mesh movement model, which will be also analyzed and discussed. As part of this methodology, the results obtained in the simulation should be compared with experimental result, in order to check, at least in a global way, the validity of the simulation.

2.2 Computational methodology. Definition of a reference case.

In this chapter, 3D CFD simulations have been performed using the real ge- ometry of a Garret GT15 Turbocharger’s radial variable geometry turbine. As it was mentioned before, the idea of this chapter is to analyze and opti- mize the set-up of a 3D CFD simulation of a radial turbine. In this particular case, the simulations have been performed using the commercial code ANSYS- FLUENT. In the process of setting-up the case, there are a lot of different parameters that must be considered, and therefore it seems reasonable to an- alyze the different effects one at a time. For this reason, a reference case is defined and it is used as reference for the different configurations.

In order to validate the computations some experimental measurements are taken in an experimental test rig, as the one shown in89. The experimental methodology is described in 2.2.1 and the measurements will be used in the following sections to calibrate the validity of the simulations. In this work, the computational domain is going to be considered as the one that can be found if the turbine is set in a turbocharger test rig.

The turbine used is a variable geometry turbine (VGT) [2, 25], this fact introduces a new uncertainty in the simulation since it is not clear how to determine the actual aperture of the stator nozzle once the turbine it set in the test rig both at high or low temperatures condition. At low temperatures there is some uncertainty due to the existence of mechanical play in the different elements of the mechanism. While at high temperatures the deformation of the elements that form the mechanism is unknown. In addition the existence of turbine vanes has influence in the operating conditions of the turbine and particularly the interaction between stator and rotor may have some influence in the simulation set-up as it will be commented later on.

In order to determine the requirements of the computational mesh used and to compare the different case set-ups a reference case is defined. In this way the results obtained with the different simulation methodologies could be compared. In this work, all the computations were performed using ideal gas model with variable thermal properties as air model, more information can be found in 4.

In the rest of the current section, the reference case is going to be de- scribed. First, the computational domain and the boundary conditions used are described, followed by some comments of two important aspects to deal with when performing turbomachinery simulation as the moving mesh strategy and the viscous model.

2.2.1 Experimental methodology

The test bench in which the experimental data were obtained is similar to the one developed in 24. This experimental facility is a steady or constant flow test bench which is used to test the whole turbo system. Therefore, this bench is formed by two separated flow lines: the one feeding the turbine at controlled pressure and temperature; and the second is the compressor feeding system.

2.2.1.1 Experimental facility

The turbine line supplies hot and pressurized air flow to the turbine. Air flow is pressurized using a rotary screw compressor, which produces up to 9.84 m3 · s 1 at a maximum pressure of 3.5 bar. After the compressor, the air passes through a group of 5 concentric electric resistances of 12.5 kW each. In this way, the generated flow is supplied at a similar thermodynamic conditions to those found in the exhaust manifold of an ICE. The flow passes through the turbine, inducing its rotation, driving the compressor. The compressor takes the air at atmospheric conditions from the inlet duct, and this flow is compressed as it passes through the compressor.

Both lines are instrumented to measure the mass-flow rate passing through 17

Table 2.1: Characteristic of the measurements sensors in the facility.

Abbildung in dieser Leseprobe nicht enthalten

them. Additionally, measurements of flow pressure and temperature at the ducts at the inlet and outlet of both compressor and turbine are taken 109. In the duct at the compressor outlet a valve is set to allow one to modify the compressor operating point (back-pressure). A control system to regulate the power injected to the turbine was developed. The system evaluates power from the measurements of the mass flow rate, the flow thermodynamic variables, and the rotational speed, which is also measured, and thus regulates the inflow conditions.

The flow variables of interest have been: pressure, temperature, mass flow rate, and rotational speed. The main characteristics in terms of range and accuracy of the different measurement sensors used in the facility are shown in table 2.1. Pressure measurements have been taken at different sections of the ducts and using two different types of sensors depending on the required temporal response.

Since the simulations were performed assuming adiabatic walls, when the measurements are taken in the test rig, the turbocharger is insulated to min- imize heat losses through the walls. Additionally, to reduce the internal heat transfer some adiabatic tests were performed, in which the temperature at the inlet of the turbine, compressor and oil are maintained at a similar value.

The small size of turbocharger turbines, and particularly for the case of the vaned ones, makes difficult the acquisition of measurements of the internal flow variables, and generally only global measures are available. This means that only pressure ratio, corrected mass-flow rate, rotational speed and enthalpy jump between the inlet and outlet of the turbine are available. The corrected mass flow rate is defined as:

Abbildung in dieser Leseprobe nicht enthalten

in this work, 101325 Pa and 288.15 K are taken as reference values to compute the corrected mass.

2.2.1.2 Angular position

It is worth to mention again that there exists an additional uncertainty when comparing the measurements and the simulations that is the position of the nozzle vanes of the VGT. The positioning system of the vanes presents some clearance in the mechanism, which introduces some uncertainty in the real position that is being tested. The problem here lays in the impossibility to view the position once the turbine is mounted.

In order to have an estimation of the position of the vanes during the test, a calibrated screw is used to move the rack mechanism of the stator vanes. In this way, the vanes are moved by rotating the screw. The position is then measured via the displacement of the rack. In order to calibrate the model some tests have been done dismounting the turbine, and measuring the vane angle in different positions. Figure 2.1 shows a picture the stator vanes for the most open position. Pictures can be taken at different positions and used to obtain the correspondent position.

The position of the vanes is measured with respect the radial coordinate passing through the rotation axis, as indicated in figure 2.1. The results obtained of the angular position of the vanes versus the rack position are presented in Fig. 2.2.

From the results of the angular position, it seems that a linear trend will fit well the behavior of the positing system. However, some comments about this positioning system should be made. The first one is about the dispersion found in the value of the angle for different stator vanes for a given position, which was of about ± 1 . This effect was not included in the CFD model, in which all the vanes are set at the same angle. The second comment is about the

Abbildung in dieser Leseprobe nicht enthalten

Figure 2.1: Picture of the stator vanes in the most open position. The reference radial direction is indicated for each vane.

previously mentioned mechanical play of the positioning mechanism. Once the position of the screw was set, the vanes cloud still be moved by hand about ± 5 , this means that during the operation the angular position of the vanes might change due to the aerodynamic forces. The mechanism has been probably designed with this play in order to be fixed one the turbine is working in real temperature conditions. The thermal behavior of the different materials increases this uncertainty, since it is not clear that the mechanism works in the same way in hot and cold flow.

All the above reasons introduce an uncertainty when comparing experimental measurements with simulations, and thus will make difficult the validation on the computational results as it will discussed later on. In the following, in order to reduce the number of parameters the stator position was kept constant at a value of 75 %.

Abbildung in dieser Leseprobe nicht enthalten

Figure 2.2: Evolution of the angular position of the stator vanes as a function of the position of the screw.

2.2.2 Computational domain

The turbine was considered as it was installed in the turbocharger test rig, as the one showed in 65 so that straight ducts were set at the inlet and at the outlet of the turbine. These ducts are also used to minimize the influence of the computational boundary conditions in the operation of the turbine. In figure 2.3 a sketch of the radial turbine is shown with one of the meshes used in this analysis. In figure 2.3 only part of the domain presenting the turbine is shown. However, as it was mentioned before two straight ducts are used, a 120 mm (about 4 diameters) one upstream of the volute inlet (section 1) and a 500 mm (about 12 diameters) one at the turbine outlet (section 5). Due to the complexity of the system, in the following analyses the turbine is going to be divided in different regions: volute, nozzles, rotor, and outlet. The interfaces between two consecutive regions, which also indicated in figure

2.3, are used as post-processing surfaces. These post-processing surfaces are numbered correlatively as identified in Table 2.2 and are used in all this work to analyze the computational results.

As previously stated, the simulations are performed neglecting the heat

Abbildung in dieser Leseprobe nicht enthalten

Figure 2.3: Schematic representation of the turbine geometry and 3D computational mesh for turbine simulations. The different post-processing stations are included.

Table 2.2: Situation of the different sections considered in the computational domain

Abbildung in dieser Leseprobe nicht enthalten

transfer through the walls. The effect of heat transfer in turbomachinery has been studied in the literature, mainly for axial turbomachinery as 104. The works described in [18, 101] also studied the heat transfer effects on the turbocharger performance, focusing on the effect on the performance of the compressor and on the results from a one dimensional model. In the current work, the heat transfer from the turbine is going to be considered negligible, mainly due to the insulation of the turbine case, and therefore the walls are going to be considered as adiabatic.

2.2.3 Boundary conditions

Testing turbochargers under steady flow conditions, although it does not truth- fully represent the actual operational conditions when the turbine is installed on engine, is the standard procedure followed by manufacturers. In this chap- ter, all the simulations are performed at steady inflow conditions, using as boundary conditions the total pressure and temperature at the inlet section and static pressure at the outlet. Another option could have been to impose mass flow rate at the inlet, instead of using total pressure. However, the combination of total pressure at the inlet and static pressure at the outlet has been found to provide good numerical stability and convergence rates in radial turbine simulations 102.

The pressure outlet boundary condition allows one to specify the gauge pressure at the outlet section of the computational domain when the flow is subsonic, while the pressure is extrapolated from the interior if supersonic regime is reached3.

2.2.4 Wheel rotation strategies

One of the main topics to deal with is the strategy of simulating the rotor motion. There are basically two different approaches: Multiple Reference Frame (MRF) and Sliding Mesh Model (SMM).

In the first one of them the mesh does not really move. Instead, it uses a coordinate system that rotates with the rotor and the equations are solved in this rotation reference frame. Therefore the Coriolis and centrifugal forces are introduced in the Navier-Stokes equations as source terms. The rest of the turbine, that does not rotate, and the ducts are expressed in a non-rotational (inertial) coordinate system. Some works on the literature as59 used this approach, which implies that some effects such as the blade passing and the interaction stator-rotor are not considered.

The main advantage of using the MRF approach is its reduced computa- tional cost. However, it cannot take into account typical unsteady flow effects, as for example, the vortex shedding. For the case of turbomachinery simu- lations, the multiple reference frame approach may have some impact on the results, as it was stated in 82. A similar conclusion was obtained by the work of Liu and Hill 64 in which different turbocompressors were analyzed, finding evidences of the importance of the mesh motion model in the cases in which the stator-rotor interaction needed to be considered. Additionally, Liu and Hill analyzed two different MRF methods, concluding that the differences found when using the frozen rotor one were larger than the ones when the circumferential averaging was considered. Other work 54 stated the frozen rotor model was not the most appropriate for radial compressor simulations. In the present work, the MRF simulations where performed using the frozen rotor approach available in ANSYS-FLUENT. Since the circumferential av- eraging approach was not considered, hereinafter frozen rotor and MRF are used indistinctly.

The second approach consists in using the Sliding Mesh Model (SMM), also known as moving mesh, in which one part of the mesh is rotating with respect to the stationary part. The connection between the two zones is done by means of sliding interfaces. This means that the connectivity for cells on either side of the interface changes at each time step. The SMM has been proved to give good results as reported in50. With the SSM approach the blade passing effect is captured. This fact can be notice in the pressure wave fluctuations propagating both upstream and downstream the rotor.

In this work, the rotational speed of the turbine has been kept constant in order to reduce the amount of parameters under study. The selected rotational speed for the analysis was 18953 rad · s −1.

2.2.5 Viscous model

A variety of papers can be found in the literature dealing with the different vis- cous models for turbomachinery simulations. With the current computational capacities a Direct Numerical Simulation, in which the whole Navier-Stokes equations are computed, is only affordable in simple cases (flat plate, pipes, ...). For the rest of the cases turbulence needs to be modeled. Turbulence modeling is a main issue in CFD simulations 121. At this step different ap- proaches can be followed: the use of an Unsteady Reynolds Averaged method (URANS) or the use of a Detached Eddy Simulation (DES) 107 or even a Large Eddy Simulation (LES) [103, 30].

In LES simulations the large eddies are explicitly resolved. This means that only the small scales need to be modeled, which results in a more accu- rate solution, since small scales are usually more isotropic and less affected by macroscopic flow effects. On the other hand in the Reynolds Averaging approach, Navier-Stokes equations are time averaged, thus an instantaneous quantity can be decomposed into a time-averaged plus a fluctuating quantity. With this approach RANS equations govern the averaged flow quantities, while the fluctuations terms are being modeled, thus defining the Reynolds stresses. Therefore a closure model is needed to define and compute this new unknowns and, in this way, to close the system of equations. The most common closure models available in CFD commercial codes might be classified as models based on Boussinesq approach and Reynolds Stress Model (RSM).

DES model is a mixture between LES simulation for the free stream flow, while the boundary layer is modeled using a RANS approach. More informa- tion about the turbulence modeling can be found in the book of Versteeg and Malalasekera 119.

DES and LES models are expected to be more precise, however they re quire much higher computational cost which is unaffordable for this kind of calculations of a whole radial turbine with the current computational capa- bilities. In the framework of URANS models, the most commonly used for engineering applications are those based on the Boussinesq approach, which establishes the proportionality between Reynolds stresses and mean rates of deformation (mean velocity gradient), thus creating the turbulence viscosity concept. The main difference between models based on the Bussinesq ap- proach and the RSM is that the latter one solves an equation for each term of the Reynolds Stress Tensor. Therefore, RSM is more suitable for problems in which the anisotropy of turbulence is important. However, the additional computational cost of the Reynolds Stress Model is generally not justified.

There have been many works dealing with the analysis of turbulence mod- els in turbomachinery simulations. In 116 an analysis of different RANS tur- bulence models in CFD computations of radial turbomachinery is performed. Among the RANS closure models, the more commonly used for internal flow problems are those defined with two equations. The main advantage of these models is their good performance, with just a small increase on the CPU time of about a 10 % when compared to the laminar solution. The most important two-equations turbulence models use the turbulent kinetic energy k. These models can be divided in those based on the turbulence dissipation rate, ϵ, based on the development of 56, or, the specific dissipation rate, ω, based on the work of Wilcox 121. k − ω model is more accurate than the k − ϵ in computing the near wall layers, since the ω function might be integrated to the viscous sublayer. These kind of models are commonly known as Low-Re, referring to the turbulent Reynolds number. The main problem of the stan- dard k − ω model by Wilcox is the strong sensitivity of the ω -function to the free stream properties 70.

Turbomachines are complex fluid dynamic systems in which adverse pres- sure gradients and flow separation might occur. In order to capture those phenomena and avoid the sensitivity of Wilcox’s k − ω model, without using more complex and more computationally expensive models, SST turbulence model developed by Menter 67 is used. The SST model blends the robust and accurate formulation of the κ − ω model in the near-wall region with the free-stream independence of the κ − ϵ model in the far field. In SST tur- bulence model the transport of the principal turbulent shear stress is taken into account, which allows obtaining the correct response to adverse pressure gradients.

The SST model has been applied over a wide range of validations cases 68 and, particularly, it has been used in most turbomachinery applications found in the literature. Menter et al. 69 applied the SST model for turbomachinery simulations, showing a good agreement between the computations and the experimental data for all the cases considered. These cases showed the ability of the model to capture the effects of the variations of Reynolds number and flow separation in a wide range of conditions. In 60 the SST model is used to perform CFD simulations in an axial fan. Other application of the SST model in turbomachinery simulations is found in 92 in which the uncertainty of transition prediction is analyzed. Simpson et al. 102 used the SST in CFD simulations of a vaned and a vaneless radial turbine showing good results. In view of the results found in the literature in which the κ − ω SST model has been proved to provide good results, this model is used for the computations performed in this work.

2.3 Mesh independence

The 3D meshes used for the computations are similar to that shown in Fig. 2.3. The main difficulty when dealing with real geometries is the achievement of an appropriate mesh. In this work a non-conformal mesh was used. The mesh has been built using a mixed polyhedral and extruded-polygonal mesh. FLUENT offers the possibility of generating a polyhedral mesh from a tetrahedral one using the algorithm described in 3. The main advantage of using polyhedral meshes is that they have better accuracy than the equivalent tetrahedral one or, in other words, is possible to achieve the same resolution with a reduced number of cells 38. Polyhedral meshes have been used in computational prob- lems in engineering, as for example in the work of Tritthart el al. 117, in which a method for solving Reynolds equations with polyhedral cells was de- veloped, showing a better behavior in some problems than the quadrilateral cells. Once the mesh typology has been chosen, a mesh independence analysis should be performed.

The mesh independence analysis is usually done by considering that the finer is the mesh the better are the results obtained. This can be explained analyzing the dicretization error, which decreases with the cell size. The usual procedure when dealing with turbomachinery simulations consists in using different meshes each one of them with a smaller cell size. This procedure has been used in the work of Zachos et al. 124 and Li et al. 61. The ex- plained procedure may seem straight forward in the case of a simple system, particularly if the cells are more or less uniformly distributed. However for a more complex system, and moreover if a real geometry is considered, this procedure may be not the most appropriate since not all the subdomains of the system need the same amount of cells. This can be illustrated in the case of the turbine, in which it could seem interesting to have a smaller cell size in the rotor section, where the momentum interchange occurs, than in the ducts, which could even be computed with a one-dimensional approximation. The procedure shown here intends to optimize the resources in terms of cell distribution.

Additionally it is worth to mention that even though in the ideal case the smaller the cells are, the better is the result, there are other issues that have not been taken into account. On the one hand, if the cell refinement is not properly done, it may cause an increase of cells aspect ratio, and the use of distorted cells can introduce convergence errors and even spurious solutions. On the other hand, it is well know that RANS turbulence models are usually applied in combination of wall-functions, which model the flow behavior near the wall. Although the k − ω turbulence model was chosen, and its automatic wall treatment37 has the advantage of ensuring as high degree of grid in- dependence as possible, it is necessary to evaluate that the value of y + is in the range of application of the wall-function 3. The y + is a function of the mesh size, its definition can be found in the book of Versteeg and Malalasekera 119:

Abbildung in dieser Leseprobe nicht enthalten

This might become a problem if the mesh is too refined during the mesh inde- pendence analysis. As previously stated, the turbine was divided in 4 different regions, namely: volute, stator, rotor, and outlet section. The process followed in this work to perform the mesh independence analysis is based in defining a reference case: geometry, mesh, and configuration. Starting with this case, each of the turbine zones were refined separately, substituting in the reference case just the region being analyzed. Several simulations are performed, each one with a finer mesh and the process continues until variation the solution of two consecutive cases is sufficiently small, as it is usually done in standard mesh independence analysis. At this point, the increase of the computational cost of an additional refinement will not be justified by the increase in resolu- tion. The process continues with the refinement of the following turbine zone. Once all the sections are analyzed the information obtained can be used to determine the regions in which the refinement is more worthwhile.

In order to study the mesh refinement effect two parameters are going to be studied for all the different refinements: the mass-flow through the current element and the total torque developed by the turbine. In the following subsections, the meshing procedure of each one of the turbine regions and the local mesh independence analysis in each one of them are shown.

2.3.1 Volute

The objective of the volute is to feed the stator in the most uniform way as possible. For this reason, the volute should be design as a convergent duct, in order to compensate the mass-flow towards the stator and keep the pressure at the volute-stator interface as constant as possible. As it was previously mentioned, a polyhedric mesh is used in the volute. Due to the importance of the volute’s tongue, a smaller cell size in this region might be of interest. An ANSYS-FLUENT size function was used centered in the tongue’s edge, as shown in Fig. 2.4. The size function was configured with a minimum size of half the default meshing size used for the original tetrahedral mesh, and a growth rate of 1.1. Therefore, all the meshes are size is defined by just one size parameter, the default meshing size.

Different volute sizes where analyzed, each one of them having about twice number of cells. The information about the size of the volute meshes used is gathered in Table 2.3. In the table, the reference case is also indicated.

As previously mentioned, each of the volutes was replaced in the reference. The results obtained with each one of them are plotted in figure 2.5. The figure shows the evolution of mass-flow and torque in percentage with the number of elements in the volute.

Abbildung in dieser Leseprobe nicht enthalten

Figure 2.4: Close-up of the mesh in the volute’s tongue.

Table 2.3: Size of the volute meshes used in the mesh independence analysis

Abbildung in dieser Leseprobe nicht enthalten

2.3.2 Stator

As previously mentioned, the turbine subjected to study was a vaned turbine. In the current analysis the vanes were kept at a constant position. Due to the particular shape of the nozzle section, it has two different characteristic lengths which are important for the meshing procedure. On one hand, the faces that

Abbildung in dieser Leseprobe nicht enthalten

Figure 2.5: Mesh independence analysis for the volute section.

form the stator wall, whose mesh will define the resolution obtained in the stator vanes. On the other hand, the transversal length or stator thickness that is important to describe the profiles in the stator. Due to this reason, the chosen topology for the stator mesh was extruded polygons.

This means that the faces forming the stator wall were meshed using tri- angular cells, which were extruded in the transversal direction. Afterwards, ANSYS-FLUENT converts these triangles in polygons. Therefore, the mesh of the stator is defined with the cell size used in the stator walls, both upper and lower faces were meshed in the same way, and the number of rows in the transversal direction. Dealing with the stator wall meshes, it may seem interesting to have a better resolution, finer mesh, in the regions close to the stator vanes and screws, therefore a size function with the same configuration than in the volute was used.

In the following analysis two different parameters are used to describe the mesh: the number of cells in the stator wall and the number of rows in the transversal direction. The combinations used are gathered in Table 2.4.

Table 2.4: Size of the stator meshes used in the mesh independence analysis

Abbildung in dieser Leseprobe nicht enthalten

First, the mesh independence is directly performed using the total number of cells, some trends can be seen in Fig. 2.6 showing that if the number of cells is increased the dispersion of the values decreases. However it is not clear whether it is worthier to increase the number of cells in the face or the number of rows.

In Fig. 2.7, the evolution of the analyzed parameters with the number of rows is shown. The different curves are grouped together according to the number of elements in the stator wall.

From the previous results, it is clear that for the face meshes with 43396 and 79302 elements, the evolution with the number of cells is almost the same. Additionally, the increase in computational cost from 15 to 30 transversal rows does not justify the change in the solution of about 0 . 4% in the torque developed by the turbine. In any case, the intermediate value of 22 rows might represent a good trade-off solution.

Details

Pages
243
Year
2012
ISBN (Book)
9783656507239
File size
4.3 MB
Language
English
Catalog Number
v232675
Institution / College
Universidad Politécnica de Valencia – Departamento de M´aquinas y Motores T´ermicos
Grade
Tags
methodology numerical characterization radial turbine steady pulsating flow

Author

Share

Previous

Title: Methodology for the Numerical Characterization of a Radial Turbine under Steady and Pulsating Flow