Efficient Design-Oriented Numerical Simulation of an Ejector

MISSING IMAGE

Material Information

Title:
Efficient Design-Oriented Numerical Simulation of an Ejector
Physical Description:
1 online resource (71 p.)
Language:
english
Creator:
Bogi,Bhageerath
Publisher:
University of Florida
Place of Publication:
Gainesville, Fla.
Publication Date:

Thesis/Dissertation Information

Degree:
Master's ( M.S.)
Degree Grantor:
University of Florida
Degree Disciplines:
Aerospace Engineering, Mechanical and Aerospace Engineering
Committee Chair:
Sherif, Sherif A
Committee Co-Chair:
Lear, William E
Committee Members:
Crisalle, Oscar D

Subjects

Subjects / Keywords:
Mechanical and Aerospace Engineering -- Dissertations, Academic -- UF
Genre:
Aerospace Engineering thesis, M.S.
bibliography   ( marcgt )
theses   ( marcgt )
government publication (state, provincial, terriorial, dependent)   ( marcgt )
born-digital   ( sobekcm )
Electronic Thesis or Dissertation

Notes

Abstract:
In order for the potential of ejector refrigeration systems to be realized for mobile applications, several important system level issues must be solved. One of the requirements placed on pulse refrigeration system operation is to operate satisfactorily under a wide range of compression ratios and entrainment ratio demands. Under some combinations of temperature, pressure and load, the stagnation pressure at which refrigerant is delivered by the ejector system is more than the stagnation pressure of the secondary inlet. Unless significant compression ratios are delivered, the ejector will serve no purpose, with potential catastrophic results and back flow. In this study, an analysis is shown which enables a designer to perform rapid-but-accurate CFD simulation of ejectors for design purposes; the method is to model the system using perfect gas assumptions by appropriately choosing scaled values of viscosity ? and specific heat constant Cp. The analysis is design dependent, geometrical variations in the ejector design change the scaled parameters with respect to the perfect gas model. Initially a mathematical model for an ejector is developed using FLUENT and is compared to experimental results and the numerical model is validated. A design-oriented approach is incorporated by changing the geometry and initial boundary conditions. Results indicate that moderate to high compression ratio operation will most likely decrease the entrainment ratio. The operating parameters of non-ideal components and subsystems change under varying operating conditions, which imposes additional limitations on achieving higher compression ratios. The effect of generating equivalent parameters for perfect gas model has been studied by considering certain specific design and operating regime choices and analyzing their effect on the performance of ejector. The results of this portion of study indicate that the efficiency of the perfect gas model with minimal computational effort. The magnitude of this effect is however design dependent and should be taken into account when considering a specific arrangement. The perfect gas model employs the method in which we appropriately choose scaled values of viscosity and specific heat using the linear fit generated as a part of this analysis, however the effect is more profound for the operational regime where compressibility is high. The significance of the study is that these findings can be used to guide the designer to obtain the best ejector system performance swiftly and with minimal computational effort. This analysis also predicts the performance of the system when operating conditions are different from the on design conditions.
General Note:
In the series University of Florida Digital Collections.
General Note:
Includes vita.
Bibliography:
Includes bibliographical references.
Source of Description:
Description based on online resource; title from PDF title page.
Source of Description:
This bibliographic record is available under the Creative Commons CC0 public domain dedication. The University of Florida Libraries, as creator of this bibliographic record, has waived all rights to it worldwide under copyright law, including all related and neighboring rights, to the extent allowed by law.
Statement of Responsibility:
by Bhageerath Bogi.
Thesis:
Thesis (M.S.)--University of Florida, 2011.
Local:
Adviser: Sherif, Sherif A.
Local:
Co-adviser: Lear, William E.
Electronic Access:
RESTRICTED TO UF STUDENTS, STAFF, FACULTY, AND ON-CAMPUS USE UNTIL 2012-08-31

Record Information

Source Institution:
UFRGP
Rights Management:
Applicable rights reserved.
Classification:
lcc - LD1780 2011
System ID:
UFE0043087:00001


This item is only available as the following downloads:


Full Text

PAGE 1

1 EFFICIENT DESIGN ORIENTED NUMERICAL SIMULATION OF AN EJECTOR By BHAGEERATH BOGI A THESIS PRESENTED TO THE GRADUATE SCHOOL OF THE UNIVERSITY OF FLORIDA IN PARTIAL FULFILLMENT OF THE REQUIREMENTS FOR THE DEGREE OF MASTER OF SCIENCE UNIVERSITY OF FLORIDA 2011

PAGE 2

2 2011 Bhageerath Bogi

PAGE 3

3 This document is dedicated to my parents who have supported me in all my endeavors

PAGE 4

4 ACKNOWLEDGMENTS First of all, I would like to thank Dr. S A Sherif the c h air m an of my graduate com m ittee, for providing m e with an opportunity to work under his guidance as a part of his research group. Dr Sherif s h ared with m e his extensive knowledge and always m otivated m e to perform better. I would also be grateful to D r. William Lear, t h e co chair of m y com m ittee for his efforts and his patience in assisting me. It was great working under his guidance as he shared a lot of his experiences and has been the back bone of this pr oject. I a m indebt ed to these two people for their moral a nd financial support in hardship I would also like to acknowledge D r Oscar Crisalle for being a part of my com m ittee and for the ti m e and attention that he pro vided. In addition, I would like to thank the m e mbers of the HVAC lab, my friends and colleagues from South Africa for their academic help. Above all I would like to express m y gra t itude to m y parents for their unwavering support and blessings.

PAGE 5

5 TABLE OF C ONTENTS page ACKNOWLEDGMENTS ................................ ................................ ................................ .. 4 LIST OF TABLES ................................ ................................ ................................ ............ 7 LIST OF FIGURE S ................................ ................................ ................................ .......... 8 LIST OF KEY SYMBOLS ................................ ................................ .............................. 10 ABSTRACT ................................ ................................ ................................ ................... 12 CHAPTER 1 INTRODUCTION ................................ ................................ ................................ .... 14 2 DESIGN OF EJECTOR ................................ ................................ .......................... 17 2.1 Description of System ................................ ................................ ....................... 17 2.2 Description of Ejector ................................ ................................ ........................ 18 2.2.1 Nozzle ................................ ................................ ................................ ..... 19 2.2.2 Suction Chamber ................................ ................................ ..................... 19 2.2.3 Mixing Chamber ................................ ................................ ...................... 19 2.2.4 Diffuser ................................ ................................ ................................ .... 20 2.2.5 Ejector Body Mixing Chamber and Diffuser ................................ ............. 20 2.3 Design Summary ................................ ................................ .............................. 21 3 COMPUTATIONAL EJECTOR MODEL ................................ ................................ .. 23 3.1 Benefits of Carrying out CFD Analysis ................................ .............................. 23 3.1.1 Low Cost ................................ ................................ ................................ 23 3.1.2 Speed ................................ ................................ ................................ ...... 23 3.1.3 Complete Information ................................ ................................ .............. 24 3.1.4 Ability to Simulate Realistic Conditions ................................ .................... 24 3.1.5 Ability to Simulate Ideal Conditions ................................ ......................... 24 3.1.6 Reduction of Failure Risks ................................ ................................ ....... 25 3.2 Steps for CFD Analysis ................................ ................................ ..................... 25 3.3 Identification of Flow Domain ................................ ................................ ............ 25 3.4 Grid Generation ................................ ................................ ................................ 27 3.5 Mesh ing Procedure ................................ ................................ ........................... 27 3.5.1 Importing Coordinates ................................ ................................ ............. 27 3.5.2 Creation of Edges ................................ ................................ .................... 27 3.5.3 Creation of Faces ................................ ................................ .................... 28 3.5. 4 Creation of Volumes ................................ ................................ ................ 28 3.5.5 Meshing ................................ ................................ ................................ ... 28 3.5.6 Reading the Case and Grid Check ................................ .......................... 30

PAGE 6

6 3.6 Solving ................................ ................................ ................................ .............. 31 3.6.1 Solvers ................................ ................................ ................................ .... 31 3.6.2 Convergence ................................ ................................ ........................... 33 3.6.3 Disc retization ................................ ................................ ........................... 34 3.6.4 Skewness ................................ ................................ ................................ 34 3.6.5 Residuals ................................ ................................ ................................ 34 3.7 Incorpor ating the Real Gas Model ................................ ................................ .... 35 3.8 Governing Equations ................................ ................................ ........................ 37 3.9 Boundary Conditions ................................ ................................ ......................... 39 3.10 Model Validation ................................ ................................ ............................. 44 3.11 Modeling Summary ................................ ................................ ......................... 48 4 RESULTS AND DISCUSSION ................................ ................................ ............... 50 4.1 Pressure Profiles ................................ ................................ ............................... 50 4.2 Velocity Profile ................................ ................................ ................................ .. 52 4.3 Mach Number Profile ................................ ................................ ........................ 54 4.4 Temperature Profile ................................ ................................ .......................... 55 4.5 Turbulence Intensity ................................ ................................ .......................... 56 5 MODELLING OF EQUIVALENT PERFECT GAS MODEL ................................ ..... 58 5.1 Algorithm to Estimate the Equivalent Viscosity ................................ ................. 58 5.2 Linear Fit for and ................................ ................................ ....................... 59 5.3 LINEST ................................ ................................ ................................ ............. 59 5.4 Verification of the Algorithm ................................ ................................ .............. 64 6 CONCLUSIONS ................................ ................................ ................................ ..... 66 7 RECOMMENDATIONS FOR FUTURE STUDY ................................ ..................... 68 LIST OF REFERENCES ................................ ................................ ............................... 69 BIOGRAPHIC AL SKETCH ................................ ................................ ............................ 71

PAGE 7

7 LIST OF TABLES Table page 2 1 Ejector geometries ................................ ................................ .............................. 21 3 1 Features of CFD analysis ................................ ................................ ................... 33 3 2 Proposed boundary conditions. ................................ ................................ .......... 43 3 3 Comparing experimental mass flow rate to simulated mass flow rate. ............... 44 5 1 List of boundary conditions used to make the fit. ................................ ................ 61 5 2 Normalized parameters ................................ ................................ ...................... 62 5 3 LINEST coefficient matrix ................................ ................................ ................... 63

PAGE 8

8 LIST OF FIGURES Figure page 2 1 Layout of pulse refrigeration system. ................................ ................................ .. 18 2 2 Ejector design schematic ................................ ................................ .................... 19 2 3 Ejector body for a 14 bar pulse and a mass flow rate of 0.002 kg/s ................... 21 3 1 Axisymmetric geometry of an ejector eith entry and exit zones .......................... 26 3 2 Growing boundary layer in the near wall region at nozzle exit ............................ 26 3 3 Meshed ejector geometry. ................................ ................................ .................. 29 3 4 Zoom in view of the near wall region. ................................ ................................ 3 0 3 5 Turbulence model ................................ ................................ ............................... 32 3 6 List of commands employed in FLUENT to activate real gas model ................... 36 3 7 List of commands employed in FLUENT to activate real gas model ................... 36 3 8 Example pressure inlet specification ................................ ................................ .. 40 3 9 Wall specifications ................................ ................................ .............................. 40 3 10 Geometry of ejector indicating the boundaries. ................................ .................. 41 3 11 Validation of model. ................................ ................................ ............................ 44 3 12 Velocity profiles for a 12 pulse, secondary inlet pressure of 8 and back pressure of (a) 8 (b) 8.5 and (c) 9 ................................ ........ 46 3 13 Graph of entrainment ratio vs. outlet pressure with the primary and secondary inlet pressures kept constant. ................................ ........................... 46 3 14 Mach number plot along the axis of the ejector ................................ .................. 47 3 15 Variation of Mach number along the axis. ................................ .......................... 48 4 1 Contours of total pressure. ................................ ................................ ................. 51 4 2 Contours of static pressure. ................................ ................................ ................ 52 4 3 Vectors of velocity. ................................ ................................ ............................. 53 4 4 Vectors of Mach number ................................ ................................ .................... 55

PAGE 9

9 4 5 Contours of static temperature. ................................ ................................ .......... 56 4 6 Contours of turbulence intensity. ................................ ................................ ........ 57 5 1 Histogram showing the variation using the linear fit and the actual values. Series 1 actual; Series 2 generated. ................................ ................................ ... 63 5 2 Percentage error for 40 data points. ................................ ................................ ... 64 5 3 Plot showing the trend line for the data points. ................................ ................... 65

PAGE 10

10 LIS T OF KEY SYMBOLS sonic velocity nozzle exit area area of constant area mixing chamber nozzle throat area flow velocity diameter of nozzle throa t pressure differential between boilers radial force / axial force / enthalpy turbulent kinetic energy / distance from nozzle exit to mixing chamber length of constant area mixing chamber system pressure total pressure static pressure in boiler 1,2 pressure at the o utlet of the diffuser pressure at the secondary inlet rate of change of specific mass / rate of dissipation density /

PAGE 11

11 viscosity / turbulent viscosity /

PAGE 12

12 Abstract of Thesis Presented to the Graduate School of the University of Florida in Partial Fulfillment of the Requirements for the Degree of Master of Science EFFICIENT DESIGN ORIENTED NUMERICAL SIMULATION OF AN EJECTOR By Bhageerath Bogi August 2011 Chair: S.A. Sherif Co chair: William E. Lear Major: Aerospace Engineering In order for the potential of ejector refrigeration systems to be realized for mobile applications, several important system level issues must be solved. One of the requirements pl aced on pulse refrigeration system operation is to operate satisfactorily under a wide range of compression ratios and entrainment ratio demands. Under some combinations of temperature, pressure and load the stagnation pressure at which refrigerant is del ivered by the ejector system is more than the stagnation pressure of the secondary inlet. Unless significant compression ratios are delivered, the ejector will serve no purpose, with potential catastrophic results and back flow. In this study, an analysis is shown which enable s a designer to perform rapid but accurate CFD simulation of ejectors for design purposes; the method is to model the system using perfect gas assumptions by appropriately choosing scaled values of viscosity and specific heat consta nt The analysis is design dependent, geometrical variations in the ejector design change the scaled parameters with respect to the perfect gas model. Initially a mathematical model for an ejector is developed using FLUENT and is compared to experimental results and the numerical model is validated. A design oriented approach is incorporated by changing the geometry and initial boundary

PAGE 13

13 conditions. Resul ts indicate that moderate to high compression ratio operation will most likely decrease the entrainment ratio. The operating parameters of non ideal components and subsystems change under varying operating conditions, which imposes additional limitations o n achieving higher compression ratios. The effect of generating equivalent parameters for perfect gas model has been studied by considering certain specific design and operating regime choices and analyzing their effect on the performance of ejector. The r esults of this portion of study indicate that the efficiency of the perfect gas model with minimal computational effort. The magnitude of this effect is however design dependent and should be taken into account when considering a specific arrangement. The perfect gas model employs the method in which we appropriately choose scaled values of viscosity and specific heat using the linear fit generated as a part of this analysis, however the effect is more profound f or the operational regime where compressibili ty is high. The significance of the study is that these findings can be used to guide the designer to obtain the best ejector system performance swiftly and with minimal computational effort. This analysis also predicts the performance of the system when operating conditions are different from the on design conditions

PAGE 14

14 CHAPTER 1 INTRODUCTION The exhaustion of the and the effect of conventional energy methods on the environment have become major concerns for energy industry in recent years. The supply of fossil fuels is reducing day by day and growing tension in the Middle East has led to a huge increase in petrol prices. In addition, environmental studies have shown that fossil f uels are causing major increase in the content of the temperatures and unwanted cl imatic changes. T he global drive towards sustainable and renewable energy technologies has fuelled research in solar powered ejector refrigeration systems. It is evident that most ejector based systems, whether driven by solar or waste heat require the refrigerant to be circulated by an electric pump Low grade thermal energies are widely available from many sources such as vehicle engines, fuel cell stacks, industrial processes and solar radiations, etc. To recover these energies through ejector based refrigeration cycle benefits o ur society both economically and environmentally The increased interest in space exploration, and the importance of a human presence in space, motivates space propulsion and thermal management improvements. One of the more important aspects of the desired enhancements is to have lightweight space power generation capabilities. Onboard power generation adds weight to the space platform not only due to its inherent weight, but also due to the increased weight of the required thermal management systems. This proposed work is a significant extension of prev ious projects, which relate to the analysis of an ejector based thermal management system.

PAGE 15

15 The ejector refrigeration system was firstly devel oped by Maurice Leblanc in 1910 This refrigeration system utilized low gra de thermal energy or waste heat instead of using electricity. The main advant age of this system is it has fewer moving parts i.e. no compressor is involved It is therefore very low in wear and significantly durable. It is also suitable to operate using water as a refrigerant. However, it usuall y has a very low coefficient of performance and this becomes the critical issue and disadvantage of this system. C omparing to the typical refrigeration cycle or vapor compression cycle, it can be seen that the ejector, the boiler and the circulating pump a re used to replace the compressor. The high pressure refrigerant, boiled in the boiler, is the primary fluid feeding to the primary nozzle. It then expands through the nozzle throat at supersonic speed and causes a low pressure area where it connects to th e evaporator. Therefore, the refrigerant in the evaporator can boil and evaporate easily. The heat absorbed at the evaporator is the refrigerating capacity. The evaporated refrigerant is called the secondary fluid The primary and secondary fluids are mixed and flow through the ejector to the condenser. The liquid refrigerant is pumped back to the boiler partly, and some portion is fed through the expansion valve and evaporator to complete the cycle. It can be seen that the refrigeration performanc e of the system depends much on the performance of the ejector to induce the refrigerant flow rate through the evaporator. In the present analysis a mathematical model for an ejector is being developed using numerical techniques provided by commercially av ailable computational fluid dynamics package FLUENT Initially geometry of the ejector is fixed considering appropriate scaling ratios from the literature and system requirements Flow regime of

PAGE 16

16 the ejector is simulated and the results are post processed t o study the performance of the system. Geometry of the ejector is chosen such that the flow is always over expanded facilitating a series of oblique shocks exiting the nozzle in order to achieve high compression ratios Flow field of the ejector is being e xamined under varying geometries and initial boundary conditions. In an effort to reduce the computational effort each time we perform a simulation incorporating a real gas model, an algorithm is being presented in this analysis which enable s a designer to perform rapid but accurate CFD simulation of ejectors for design purposes; the method is to model the system using perfect gas assumptions and by appropriately choosing viscosity and specific heat constant of the refrigerant Generation of this effective algorithm using the mathem atical tools is the basic motivation of the current study.

PAGE 17

17 CHAPTER 2 DE SIGN OF EJECTOR 2.1 Description of S ystem The ejector based pulse refrigeration system proposed by Brooks et al [ 1] is shown in Figure 2 1 .Primarily there are two loops the outer driving loop and a cooling loop. Two boilers are powered by waste heat or solar thermal energy generating a sustained series of high pressure pulses by alternately isolating, pressurizing and pulsing refrigerant R134a through the system. For the engineering test loop, the boiler absorption plate operates at approximately 90C.The ejector entrains a secondary flow from the cooling loop and provides the compression in the refrigeration sub system. The condenser removes heat from the system reducing the pressure and provides slightly sub cooled refrigerant to the boilers and the cooling loop. Initially, solenoid valves will direct the high pressure pulse of high vapor quality, through the ejector, entraining flow from the evapora tor and producing a cooling effect. After a predetermined time, control software will toggle the solenoid valves to direct the remainder of the pulse through the outer driving loop to replenish the boiler. In the proposed pulse refrigeration system, the d esign and performance of the ejector is critically important. This part of report describes the design of vapor ejectors proposed for use in the pulse driven system running on refrigeran t R134a. The ejector geometries design ed for different mass flow rate s are determined from an isentropic expansion analysis of R134a vapor using NIST RefProp data and geometric scaling ratios obtained in the literature. An assumption of pure vapor at the inlet to the ejector nozzle is being made as opposed to a two phase flu id as a part of this analysis.

PAGE 18

18 Figure 2 1 Layo ut of pulse refrigeration system 2.2 Description of E jector The ejector consists of four components the nozzle at the primary inlet, the suction chamber housing the secondary inlet, the constant area mixi ng ch amber and the recovery diffuser The primary motive flow isentropically expands and accelerates through the convergent divergent nozzle to reach supersonic velocity. The low pressure region at the outlet of the nozzle is necessary to entrain the secon dary flow. The two flows mix in the mixing chamber and the resulting stream regains pressure in the diffuser.

PAGE 19

19 Figure 2 2 Ejector design schematic 2.2.1 Nozzle The n ozzle is an essential component of the ejector, this allows the primary fluid to accelerate and assist in entraining the secondary flow fr om the evaporator; The Design of nozzle has a critical role in the working of ejector, a key design parameter is the nozzle exit to throat area ratio. Selvaraju et al [2] designed miniature ejectors with nozzle ex it to throat area ratios of approximately 2.6. This is comparable with other literature which give ratios between 2.5 and 3.1.The converging and diverging angles of the nozzle are not well documented in the literature and do n ot app ear to be key parameters. 2.2.2 Suction C hamber The suction chamber houses the secondary inlet to the ejector. Area ratios comparing the secondary inlet to other ejector geometry were not available from the literature. 2.2.3 Mixing C hamber The design of t he mixing chamber depends on three key dimensional ratios ( and The area ratio of the mixing chamber to the nozzle throat

PAGE 20

20 commonly ranges from 4 to 10.6 For optimal mixing of the two fluids to occur, the length to diam et er ratio of the mixing chamber is approximately 10 .The distance from the nozzle exit to the mixing chamber entrance ( ) is also important. It has been found experimentally that the ratio is approximately 1.5 for best ejector performance. The inlet angle into the mixing chamber is not critical but often ranges from 22 to 34 degrees. These values are absorbed from the literature. 2.2.4 Diffuser A pressure rise occurs in the diffuser due to the increasing cross sectional area. Th e diffusing angle commonly ranges from 6.3 to 9.4 degrees. Two ejector designs are presented which are based on the expected inlet conditions upstream of the nozzle. Based on work by Brooks [1] et al the expected mass flow rate of the pulse could be in th e range of 0.002 to 0.01 This depends on the boiler fill level and the duration of the pulse. An expected avera ge pulse pressure of 14 is selected for the inlet pressure, and mass flo w rate of 0.002 is delivered. 2 .2. 5 Ejecto r B ody Mixing Chamber and D iffuser Using the nozzle geometries and t he ratios identified in Table 2 1, the mixing chamber and the diff user geometries are calculated. The diffuser cone may need to be designed separately; however the internal geometries will remain the same. Table 2 1 summarizes the proposed designs for the ejectors. The dimensions, angles and ratios can be used to derive further scaled versions of the ejectors for use with A sample ejector body is shown in Figure 2 3 where in all th e dimensions are specified.

PAGE 21

21 Figure 2 3 Ejector body for a 14 bar pulse and a mass flow rate of 0.002 kg/s Table 2 1. Ejector geometries d t (mm) d 1 (mm) A 1 /A t Nozzle converging angle Nozzle diverging angle Chamber Inlet Angle D 3 A 3 /A t L 3 /D 3 L x /D 3 Chamber diffusing angle A 0.7 1.2 2.94 30 5 30 2.1 9 10 1.5 7 B 1.1 1.8 2.67 30 5 30 3.3 9 10 1.5 7 Table 2 1 compares ejector designs from the literature to ascertain key dimensional parameters. 2.3 Design Summary Two primary nozzle designs were developed for application in an ejector running on R134a. Geometric scaling ratios from literature were then used to complete the ejector designs. This analysis assumes that the fluid inlet condition to the ejector 3

PAGE 22

22 primary n ozzle is pure vapor, which may not accurately resemble the operating condition in a pulsed refrigeration system. Further investigation into two phase conditions at the inlet of the ejector, including friction losses will result in a more accurate analysis. Computational fluid dynamics analysis is pursued to develop the desig n further and model the ejector in order to arrive at the best design of the ejector optimizing in between compression and entrainment ratios.

PAGE 23

23 CHAPTER 3 COMPUTATIONAL EJECTO R MOD EL The software employed for the present work is FLUENT a commercially available CFD package which is wi dely used in the t urbo machinery industry to analyze flows in scrolls, volutes, compressors, water turbines, gas turbines, pumps, diffusers, rocket mot ors, pneumatic control devices, nozzles, cavities and ducts. The FLUENT software solves the 3 D Reynolds Navier Stokes equations for the mass averaged velocity and the time averaged pressure, energy and density. The software is an integrated and complex N avier Stokes fluid flow prediction system, capable of diverse and complex multi dimensional fluid flow problems. It uses a flexible, multi block grid system, a graphical interface and several sophisticated modeling tools, especially for rotating machinery and combustion applications. The fluid flow solver, FLUENT provides solutions for incompressible / compressible, steady state / transient, laminar / turbulent single phase fluid flow in complex geometries 3.1 Benefits of C arrying out CFD A nalysis 3.1.1 Low C ost The most important advantage of computational analysis is its low cost. In most applications, the cost of a computer simulation is much lower than the cost of a corresponding experimental analysis. This can reduce or even eliminate the need for expensive or large scale physical test facilities. 3.1.2 Speed A computational investigation can be performed with remarkable speed. A designer can study the implication of hundreds of different configurations quickly and choose the optimum design process; rapid evaluation of design alternatives can be

PAGE 24

24 made. On the other hand, a corresponding experimental investigation would take a long time. 3.1.3 Complete I nformation A computer solution to a problem gives detailed and complete information. It can provide the va lues of all relevant variables such as velocity, pressure, temperature, con centration, turbulence intensity throughout the domain of interest. This provides a better understanding of the flow phenomenon and the product performance. For this reason, even when an experiment is to be performed, there would be great value in obtaining a companion computer solution to supplement the experimental information. 3.1.4 Ability to Simulate Realistic C onditions In theoretical calculation, realistic conditions can be easily stimulated. There is no need to resort to small scale models. Through a computer program, there is lit tle difficulty in having a very large or very small dimension, in treating very low or very high temperatures, in handling toxic or flammable substances, or in following very fast or very slow processes. 3.1.5 Ability to Simulate Ideal Conditions A predict ion method is sometimes used to study a basic phenomenon, rather than a complex engineering application. In the study of phenomenon, one wants to focus attention on a few essential parameters and eliminates all irrelevant features. Thus many idealizations are desirable for example: two dimensionally constant densities an adiabatic surface of an infinite reaction rate. In a computation approach, such conditions can be setup with ease and precision, whereas even careful experimental can barely approximate the idealization.

PAGE 25

25 3.1.6 Reduction of F ailure R isks CFD can also be used to investigate configurations that may be too large to test or which pose a significant safety risk including pollutant spread and nuclear accident scenarios. This can often provide conf idence in operation, reduce or eliminate the cost of problem solving during installations, reduce product liability risks. 3.2 S teps for CFD A nalysis The basic steps involved in performing this simulation are 1. Identifying the flow domain and physical proce sses. 2. 2 D modeling and generating grid for the flow domain. 3. Specification of boundary conditions and initial guess. 4. Selection of solver parameters and convergence criterion. 5. Post processing and analysis of CFD results. The ejector is modeled and analysis is carried out by following the above steps. 3.3 Identific ation of Flow D omain It is required to understand the exact flow domain thoroughly before the construction of the grid. Present geometry has 2 pressure inlets, one pressure outlet and the geometry is being modeled as an axisymmetric case in order to reduce the computational effort as the geometry is symmetrical about the central axis. Flow domain has boundary layer growing on the walls of the geometry and an interior boundary layer on the walls of convergent divergent nozzle The flow analysis through any component under consideration will be having a flow entry zone as well as the exit zone ; in the present case we have two entry zones and one exit zone Thus the flow within the components should be analyzed along with inlet and outlet passages, and with realistic boundary conditions imposed

PAGE 26

26 Figure 3 1 Axisymmetric geometry of an ej ector eith entry and exit zones Figure 3 1 s hows the pressure inlets, the pressure outlet and the axis As the flow passes in the flow passages past the walled boundaries, a considerable boundary layer growth takes place with resulting frictional losses. The boundary layer is generally very thin initially, but grows thicker, with possible flow separation when adverse pressure gradients exist. Modeling this area very carefully is essential to ensure correct pres sure loss estimation. Thus sufficient number of grid lines within this region are incorporated with an initial size of 0 .001 and a growth rate of 1.1 0 to cap tu re the boundary layer in detail as shown in Figure 3 2. Figure 3 2 Growing boundary layer in the near wall region at nozzle exit Secondary inlet Outlet Primary inlet Axis Nozzle throat

PAGE 27

27 3.4 G rid G eneration The mesh for the present geometry is generated using GAMBIT it also provides meshing capabilities for boundary layer and the grid is subsequently imported into FLUENT and solved. GAMBIT is designed for the creation of high quality computational meshes for two dimensional geometries. Predefined grid topology templates are used to minimize grid setup time and optimize the mesh for the given application. GAMBIT enables the user to generate computationa l grids quickly through the automatic management of grid topology, periodic boundary conditions and grid attachment. The geometry is shown in two dimensional v iew with growing boundary layer in Figure 3 2 3.5 Meshing P rocedure 3.5.1 Importing C oordinates In GAMBIT, points can be created by specifying the coordinates, namely the x, y and z coordinates. But if the numbers of points are more, specifying the coordinates of each of these points becomes highly tedious. Instead, all the points can be imported int o GAMBIT at once in the form of a text document (*.txt). This test document contains the number of points in the first row followed by the x, y a nd z coordinates of the points. Ejector g eometry is constructed in gambit by importing the coordinates in a tex t document which is generated manually by analyzing the geometry of the ejector. 3.5.2 Creation of E dges The points imported are joined to form edges. In GAMBIT, points can be joined using straight lines or smooth curves. There are many kinds of curves tha t can be employed namely Conics, nurbs, lines etc. and in this study we use lines to join the points. Each of the points is to be selected in a systematic manner for the desired edges

PAGE 28

28 to be created. If the points are not sequentially selected, inappropriat e or irregular edges are created. 3.5.3 Creation of F aces In general, a face can be created by sweeping an edge along an axis or revolving it about an axis. In GAMBIT, faces can also be created by selecting the already formed edges in a sequential order c lock wise or anti clock wise Face formation can be confirmed by noticing a change in color from yellow to blue. 3.5.4 Creation of V olumes Volume generation in GAMBIT can be done in different ways. Volume can be created by sweeping a face along a direction, revolving a face about an axis or stitching the faces in a sequential manner. The volume generation can be confirmed by noticing a change in color from blue to green. For volume generation in case of Turbo machinery, there is a special feature called TURBO in GAMBIT. This feature creates periodic boundaries and breaks down the component into smaller similar elements. Now the analysis of o ne of these elements when integrated over the entire volume gives us the anal ysis of the complete component. 3.5.5 Meshing The entire volume is divided into innumerable small finite number of elements. This process is called meshing and the grid generated is called a mesh. Meshing gives us a scope to study the behavior of various parameters such as pressure, velocity etc at each of these elements. The finer the mesh the better is the scope for analysis since it gives us more number of points to study the b ehavior of parameters.

PAGE 29

29 In GAMBIT, the mesh elements can be of two types namely t rigonal and quadrilateral. To create a mesh, either the element count number or the element size can be specified. Gambit also provides us with size functions which allow us t o control the size of mesh for the geometric edges faces and volumes that are meshed. Size functions control the mesh characteristics in the proximity of the entities to which they are attached. Size functions control the fol lowing properties. Maximum mes h element edge lengths fixed type size function Angles between norma elements curvature type size function. Number of mesh elements employed in the gaps between two geometric entiti es proximity type size function From the above size functions the fixed size function has been used in meshing the ejector so as to capture the effect of boundary layer in the flow domain effectively. This allows us to have a finer mesh, with relatively less number of mesh elements for the flow domain which helps in capturing the flow effectively. Figure 3 3. Meshed ejector geometry

PAGE 30

30 Figure 3 4 Zoom in view of the near wall region The geometry of the ejector was developed usi ng the scaling ratios from Table 2 1. The model employs a 2 D axisymmetric mesh including only the upper half portion of the ejector as seen in Figure 3 3, the ejector design was plotted in Gambit and a Quad Map mesh was applied giving a total of 23742 cells. The mesh was then improved using the Thom Mi d smoothing tool in FLUENT. Once the mesh is generated, f or assigning values during solving, various surfaces of the grid are given names for easy understanding as primary inlet, secondary inlet, outlet, axis and wall The type of boundary conditions and t he continuum type are also specified. Finally, this meshed model is exported as file in a format that can be directly read into FLUENT as a case file. 3. 5.6 Reading the Case and Grid C heck First, the case file is read into FLUENT and its grid is checked for continuity and uniformity of the mesh. And the geometry is scaled appropriately into the required dimensions. Geometry is checked for negative volume which is an error if present. Nozzle throat

PAGE 31

31 3.6 Solving 3.6.1 Solvers Solving is an important phase in CFD analysis. The software used for solving in the present scenario is FLUENT a commercially available CFD tool Two solvers are available in FLUENT Segregated solver and Coupled solver In the present study, we use coupled implicit solver. Because the govern ing equations are non linear, several iterations of the solution loop must be performed before a converged solution is obtained. Supersonic flow requires the use of the density based implicit solver. The third order upwind discretization scheme is used for the momentum equations whilst a second order upwind discretization scheme is used for the turbulent kinetic and turbulent dissipation energy equations. Method of absolute formulation for velocity is employed in order to calculate the velocities at differe nt nodes. A G reen G auss cell based gradient option is used f or structured orthogonal grids, the gradient of a scalar at a given control volume centroid can be easily computed using the definition of the derivatives. The case becomes more complicated when g eneral unstructured grids are involved. The usual approach is to make use of Green Gauss theorem which states that the surface integral of a scalar function is equal to the volume integral over the volume bound by the surface of the gradient of the scalar function These schemes ensure satisfactory accuracy, stability and convergence of the model. Turbulence modeling was done using the model. The constants for the model were specified accordingly. Initially a gener al form of converged solution is obtained for the problem; the n the solution is refined using effective wall treatment functions in the boundary layer and near wall regions. Figure 3 5 shows the modeling

PAGE 32

32 parameters for turbulence. The convergence criteria is based on the residual value of the calculated variables which include the mass, velocity, turbulent kinetic energy and turbulent dissipation energy. In the present calculations, the threshold values were set to a of the initial resid ual value of ea ch variable. Figure 3 5. Turbulence model

PAGE 33

33 The features of the CFD analysis on the e je ctor are summarized in Table 3 1 Ta ble 3 1. Features of CFD a nalysis Number of cells 23742 Mesh type Quad Map Smoother Thom Mid Solver 2 D, Density based implicit solver Fluid Tetrafluroethane (R134a) Turbulence Model, Standard wall function Model NIST Real gas model Numerics Absolute velocity formulation 3.6.2 Convergence It is the point at which the solution no longer changes with successive iteration. Convergence criteria, along with reduction in residuals help in determining when the solution is complete. Convergence criteria are pre set conditions on the residuals which indicate that a certain level of convergence has been achieved. If the residuals for all problem variables fall below the convergence criteria but are still in decline, the solution is still changing to a greater or lesser degree. A better indicator occur s when the residuals flatten in a traditional res idual plot of residual value v s iteration This point, sometimes referred to as convergence at the level of machine accuracy, takes time to reach, however, and may be beyond our needs. For this reason, alter native tools such as reports of forces, heat balances, or mass balances are used instead. In the present simulation convergen ce criterion is set to be for all the variables. For each simulation, the solution is iterated until convergence is achieved s uch that the residue for each equation is less the n In general, it is observed that the residue for the momentum equations, the turbulent kinetic energy and turbulent energy dissipation rate are well below And the continuity equation residue i s below while the residue for the energy equation is below

PAGE 34

34 3.6.3 Discretization The act of replacing the differential equations that govern fluid flow with a set of algebraic equations that are to be solved at distinct points is called discretization Third order and second order discretization schemes are used in the current model depending on the importance of the property. The Pressure Implicit with Splitting of Operators PISO scheme is used fo r pressure velocity coupling A second order upwind scheme is adopted to discretize convective terms 3.6.4 Skewness It is the difference between the shape of the cell and the shape of an equilateral cell of an equivalent volume. Highly skewed cells can decrease accuracy and destabil ize the solution. Cells skewness is reduced after exp orting the mesh file into FLUENT 3.6.5 Residuals Residuals are the small imbalances that are created during the course of the iterative solution algorithm. This imbalance in each cell is a small, non z ero value that, under normal circumstances, decreases as the solution progresses. Each iteration consists of the following steps. Fluid properties are updated, based on the current solution. An d if the calculation has just begun, the fluid properties will be updated based on the initialized solution. Three momentum equations are solved in turn using current value of the pressure and face mass fluxes, in order to update the velocity field. The velocity obtained in first step may not satisfy the continui ty eq uation locally. A Poisson t ype equation for the pressure correction is derived from cont inuity equation and the lineariz ed momentum equation. This pressure correction equation is then solved to obtain the necessary corrections to

PAGE 35

35 the pressure and velocity fields and the face mass fluxes such that continuity is satisfied. When interface coupling is to be included, the source terms in the appropriate continuous phase equations may be updated with a discrete phase trajectory calculation. A check for convergence of the equation set is made. Above steps are continued until convergence criterion is achieved. Once the grid is checked, the solver is set to segregated and the viscous model is selected. There are two well known methods for numericall y solving the set of governing equations, the finite volume and the finite element approaches The governing equations for compressible fluid dynamics together with the initial and boundary conditions are solved using the density based solver to obtain a n umerical solution. Using th is solver the conservation of mass and momentum were solved iteratively along with the coupled energy equation 3.7 Incorpora ting the Real Gas M odel The simulation assumes that both the primary and secondary streams at the inlet to the ejector are in the gaseous phase. The properties of R134a were obtained from NIST REFPROP and the corresponding state equations for the real gas model were activated manually as shown in F igures 3 6 and 3 7. A Helmholtz equation of state has been used for solving states and the energy equation is also incorporated to calculate the temperatures across the flow domain.

PAGE 36

36 Figure 3 6 List of commands employed in FLUENT to activate real gas model Figure 3 7. List of commands employed in FLUENT to ac tivate real gas model

PAGE 37

37 3.8 Governing E quations The continuity equation for a 2D axisymme tric geometry is given in Eq. 3 1 T he axial and radial momentum conservati on equations are given by Eq. 3 2 and Eq.3 3, and combined in Eq. 3 4 ( 3 1 ) ( 3 2 ) ( 3 3 ) ( 3 4 ) Where is the axial coordinate, is the radial coordinate, is the axial velocity, is the radial velocity and v z is the swirl velocity. The Turbulence model is described in Eq 3 5 The dissipation rate of the turbulence kinetic energy is given by Eq 3 6 Constants: and ( 3 5 )

PAGE 38

38 ( 3 6 ) The above equations were solved using the finite volume method which is employed in the commercia l fluid flow solver FLUENT 6.3. Moreover, three turbulence models Realizable model Renormalization group RNG model and Shear stress trans port SST model, are tried out for solving the high velocity flow problem and then compared with the experimental results. The RNG mode l is finally selected in FLUENT for its ability to better predict ejector pe rformanc e than other turbulence models. The near wall treatment is treated with the standard wall functions which gives reasonably accurate results for the wall bounded with very high Reynolds number flow. A third order muscle iterative step scheme is used for the time marching of the momentum and continuity equations and second order discretization schemes are used for kinetic turbulence energy and dissipation rate. The time step is set up by a Courant Friedrichs Lewy CFL cond itions. The time step is controlled by a specified maximum value for the Cour ant number. The Courant number Co is defined as

PAGE 39

39 velocity. A maximum Courant number of 5 was set in the present simulation and a va riable time step based on the set Courant number was used. At the beginning of calculations, it is set to 0.5 because the solution is highly non linear, and it is increased up to 5 at the end due the full implicit time discretization. Moreover, proceeding to in depth analysis, a grid convergence study was performed to ensure overall mesh independent results In this investigation, structured squared shapes of grids were used for all simulations. In the previous study of the authors, it was observed that gr ids whose aspect ratios are different from unity produce non physical results. 3.9 B oundary C onditions The boundary conditions are sp ecified for stagnation pressure and stagnation temperature at the primary and secondary inlets and a static pressure for diffuser outlet. The diffuser outlet boundary condition is set up as a pressure boundary rather than a velocity boundary to avoid difficulties with backflow and to make sure the problem is not over specified Since we are modeling a geome try which is cylin drical and is symmetrical about the central axis, the centerline is specif ied as the axis of the geometry. An outlook of geometry where boundary conditions are specified is shown in Figure 3 10. The working fluid of the model is Freon R134a Its density is obtained using the ideal gas relationship. Other properties such as specific heat, thermal conductivity, viscosity and molecular weight are derived from R134a properties provided in NIST. Boundary conditions of the primary flow and the second adopted on the outlet of the ejector. P ressure inlet specification is shown in Figure 3 8.

PAGE 40

40 Figure 3 8. Example pressure inlet specification There are two wall regions in the present geometry, one is an interior wall encompassing the nozzle and the other is the outer case which covers the secondary inlet, mixed chamber and the diffuser Wall is specified as a stationary wall with no slip shear condition and has zero roughness coefficient. Material for the wall is chosen as Aluminuium with zero thickness and the heat generation rate being zero on the wall. Boundary conditions for wall are depicted in Figure 3 9. Figure 3 9 Wall specifications

PAGE 41

41 Figure 3 10. G eometry of ejector indicating the boundaries. The simulation solves for the velocity flow field pressure profile and entrainment ratio Pressure ratios are chosen such that the entrainment ratio is greater than zero and the compression ratio is greater than 1. The inlet conditions to the ejector simulation are dependent on numerous factors; power input to the PRS boilers, pressure di fferential between the boilers for a pulse to occur, and the effective cooling at the condenser. The ejector must be modeled as close to the expected operation of the refrigeration cycle as possible to ensure that the design is viable. The system pressure also resembles the initial pressure at the outlet of the ejector before the pulse occurs. Therefore the initial pressure at the ejector diffuser outlet is expected to be between 8 and 16 depending on the point in time of the cycle. The cooling loop and the condenser are in communication. Th e secondary inlet conditi on from the refrigeration loop is therefore dependent on the extent of cooling at the condenser and the conditions at the evaporator. Assuming that there is no load at the evaporator and that the expansion valve is fully open, the initial conditions follow from the condenser outlet. The refrigerant is sub cooled to 20.5 and has the corresponding system pressure which ranges from 8 to 16 depending on the point in time of the cycle. The pressure ratio is e ffectively equal to 1 and remains constant Blue inlets Red outlet Yellow axilsline White wall

PAGE 42

42 A recommended set of initial values to the computational model is provided in Table 3 2 and caters for a range of possible values. Simulating these input values will yield an operational envelope for the ejector and determine its effectiveness at inducing secondary flow

PAGE 43

43 Table 3 2 Proposed boundary conditions. Primary inlet dP = 2 bar dP=4 bar dP=6 bar Initial diffuser ou tlet Initial secondary inlet Initial diffuser outlet Initial secondary inlet Initial diffuser outlet Initial secondary inlet P (bar) T (C) P (bar) T (C) P (bar) T (C) P (bar) T (C) P (bar) T (C) P (bar) T (C) P (bar) T (C) 12 46.3 10 39.4 10 20.5 8 31.3 8 20.5 14 52.4 12 46.3 12 20.5 10 39.4 10 20.5 8 31.3 8 20.5 16 57.9 14 52.4 14 20.5 12 46.3 12 20.5 10 39.4 10 20.5 18 62.9 16 57.9 16 20.5 14 52.4 14 20.5 12 46.3 12 20.5 20 67.5 16 57.9 16 20.5 14 52.4 14 20.5

PAGE 44

44 3.10 Model V alidation F low entrainment to the ejector was extensively validated by the current authors in [1] using the num erical model developed in FLUENT. Table 3 3. Comparing experimental mass flow rate to simulated mass flow rate. Test Case Primary inlet pressure Secondary inlet pressure Outlet pressure Mass flow rate experimental N umerical model value 1 10 bar 6bar 6.3bar 0.002 kg/s 0.00173 kg/s 2 12 bar 8bar 8.4bar 0.005 kg/s 0.00442kg/s Figure 3 11 Validation of model. The experiment al mass flow rate is compared to the simulated mass flow rate for two cases with different primary and secondary inlet stagnation pressures keeping the compression ratio same. They were in good agreement with accuracy of 90 %. T he 0.0000 0.0010 0.0020 0.0030 0.0040 0.0050 0.0060 1.45 1.50 1.55 1.60 1.65 1.70 massflow rate primary to secondary inlet pressure ratio actual model

PAGE 45

4 5 slope of the trend line shoul d be 1 in order for the perfect match of the experimental data when compared to the theoretical data. Slope of the trend line is 0.9 from the equation of trend line generated. This comparison validates the current models performance with an experimental result. Now that mathematical model is in good agreement with the experimental results, this model can be used to perform simulations of on and off design conditions to optimize and select the best design conditions. The Mach number contours are plotted in Fig ure s 3 12 a, b and c for ejector design ed for a flow rate of 0.002 The initial boundary conditions are set to 12 for the primary pulse, 8 at the seconda ry inlet and varying diffuser back pressures of (a) 8 bar, (b) 8.5 and (c) 9 An entrainment ratio of 0.255 has been observed for case (a). The shock wave for this case is captured as shown in the pressure spike of figure 3 14 .Note that the c ode has the capability of handling transonic flow, as evidenced by the supersonic region in the primary nozzle, Figure 3 14 A pressure ratio greater than 1 results in backflow, shown in case (c). The simulation results are plotted in Figure 3 13 and show that the entrainment ratio is proportionally increased with a decrease in diffuser back pressure. This result indicates that the ejector is condenser limited; a sufficiently large condenser is required for the system to provide a lower ejector back pressur e to aid entrainment. The results are checked for various properties to test for the correctness of the modeling approach

PAGE 46

46 Figure 3 12. Velocity profiles for a 12 pulse, secondary inlet pressure of 8 and back pressure of (a) 8 (b) 8.5 and (c) 9 Vortices are observed in the flow field when the outlet pressure is increased to values greater than the secondary inlet pressure resulting in zero entrainment. Figure 3 13 Graph of entrainment ratio vs. outlet pressur e with the primary and secondary inlet pressures kept constant. 0.80 0.85 0.90 0.95 1.00 1.05 1.10 0.00 0.10 0.20 0.30 0.40 0.50 0.60 0.70 0.80 Pressure ratio Entrainment ratio r= priamry stagnation pressure inlet/ secondary stagnation pressure inlet r=1.5 r=1.6 r=1.8

PAGE 47

47 From the F igure 3 13 it is observed that e ntrainment ratio increases with a reduction in diffuser outlet pressure. Three plots are given for different pressure ratios as shown. In this figure each converged solution represents a point on the graph. Figure 3 14. Mach number plot along the axis of the ejector A grid independency analysis has also been performed by coarsening the mesh to double the size and fine tuning it to half. Variation in the res ults was found to be less than 3 % depicting that properties are independent of mesh. The number of cells in the model geometry was varied from 13582 to 54328 and simulated under the same conditions. The variation of x velocity Mach number along th e axis is plotted for 3 different grids halving and doubling the grid node points. The results were found to vary within 3 %, which indicates grid independence. The results for intermediate grid used for modeling purpose is much closer to the grid which is finer, which indicates the grid convergence as the mesh be comes finer, shown in F igure 3 15 The residuals w ere

PAGE 48

48 also examined to ensure that the convergence is steady and no sudden variation is found in the convergence of the solution. Series1 grid1 Series 2 grid 2 Series 3 grid 3. Figure 3 15 Variation of Mach number along the axis 3.11 Modeling Summary An ejector based pulsed refrigeration system is described which can be powered by solar or waste heat. A CFD model was developed in FLUENT and results confirm flow entrainment to the ejector and the model is validated with the experimental results The results also suggest that an optimally scaled condenser must be designed for the system to facilitate flow entrainment to the ejector. The careful design of the ejector will 0.00 0.20 0.40 0.60 0.80 1.00 1.20 1.40 -0.04 -0.02 0.00 0.02 0.04 0.06 Axis length in meters Series1 Series2 Series3 Mach number Series1 grid1 Series 2 grid 2 Series 3 grid 3 Grid 1 used for modeling Grid 2 coarse grid Grid 3 Fine grid

PAGE 49

49 enable the pulse refrigeration system to achieve active cooling at the evapor ator without the need for an electric circulation pump. High quality computational effort is put in to arrive at converged solutions. Now arises a need to develop a method which gives the same performance with minimal computational effort and negligible l oss es in the performance of the ejector.

PAGE 50

50 CHAPTER 4 RESULTS AND DISCUSSI ON Now that the model has been validated with the experimental results, computational model with minor variation in geometry is tested for various boundary conditions in an operational regime where the compressibility of is in the range 0.95~1 where in specific heat constant is a very weak function of temperature. The geometry is now designed such that we rule out the possibility of shock in the nozzle. It is done by replacing the convergent divergent nozzle with a convergent nozzle only so as to have a series of oblique shockwaves compressing the flow. The results are presented in this chapter with velocity, pressure, temperature and turbulence intensity contours being discussed. 4.1 Pressure P rofiles The stagnation pressure contours across the ejector interior are shown for a base case where the primary stagnation pressure is 1.0Mpa, secondary stagnation pressure is 0.5Mpa and outlet static pressure is 0.5Mpa in F igure 4 1. This contour plot illustrates a decrease in stagnation pressure downstre am of the primary nozzle exit due to the mixing of the two fluids. However there is rise in stagnation pressure of the secondary stream due to energy transfer between the two streams. Stagnation pressure is shifted along the ejector axis with an increase i n primary flow temperature. The explanation of this phenomenon is that the momentum of the fluid increases with elevation of boiler temperature. An increase in momentum of the primary flow results in higher flow velocities and consequently the mixing proce ss move dow nstream in the nozzle. Figure 4 1 elucidates that the stagnation pressure of outlet stream is higher than the stagnation pressure of the secondary stream with positive entrainment which is the desired result.

PAGE 51

51 It is observed that decre ase in sta tic pressure as shown in Figure 4 2 is more prominent than decrease in stagnation pressure at the nozzle exit. The reason for this phenomenon is that the magnitude of velocity is higher at the nozzle exit which is at the expense of static pressure. Figure 4 1 Contours of total pressure. P ressure in Pascal

PAGE 52

52 Figure 4 2 Contours of static pressure. 4.2 Velocity P rofile The velocity vectors across the ejector interior are shown for a base case where the primary stagnation pressure is 1.0Mpa, secondary stagnation pressure is 0.5Mpa and outlet static pressure is 0.55Mpa in F igure 4 3 The secondary fluid flow velocity is low at first, but speed s up as the two streams mix. A series of oblique shock waves Pressure in Pascal

PAGE 53

53 slows down the speed of the primary stream which results in increasing the pressure head. These shock waves are brought on by the non un iform mixing of the two streams The flow in the constant a rea duct is now at subsonic speeds and a diffuser at the end will help in gaining the static pressure. The ejector is now said to be operating in over expanded mode. Figure 4 3 Vectors of velocity. Velocity

PAGE 54

54 4.3 Mach Number P rofile A vector plot of the Mach number of the ejector is examined to investigate the expansion in the flow. The shock wave in this instance is pushed out of the primary nozzle this is the reason for choosing this geometry of only a converging nozzle and is now located where the primary flow is dispersed into the ejector. The form of the shock wave has also changed from normal to the ejector axis or direction of flow to a more oblique shape. A diamond shaped series of shock waves and expansion waves can be seen d ownstream of the primary nozzle. The supersonic converging duct found after the primary nozzle exit plane extends a distance into the ejector and serves to entrain fluid from the evaporator Mach number greater than one is observed at the exit of primary n ozzle. The reason for this phenomenon can be explained as the pressure behind the nozzle exit is more than the pressure at exit, the flow tries to expand and forms hypothetical aerodynamic diffuser section at the exit of the nozzle which allows the flow to expand, hence the increase in Mach number

PAGE 55

55 Figure 4 4 Vectors of Mach number 4.4 Temperature P rofile The static temperature profile for the base case is shown in Figure 4 5.Initiall y the primary stream is at 373 K and the secondary stream is at 288 K which interacts to gi ve a mixed temperature of 330 K Temperature profile s are similar to that of pressure contours Mach number

PAGE 56

56 Figure 4 5 Contours of static temperature. 4.5 Turbulence Intensity The turbulence intensity vectors are shown for the same base case in the Figure 4 7.The magnitude of turbulent intensity is varying from a minimum of 0% to a maximum of 8 % in the interaction regime. There is a region of higher turbulence intensity between the primary flow and sec ondary flow after the nozzle exit and it ultimately dies down as the flow enters into the mixing chamber. The reason behind this observation is the T emperature (K)

PAGE 57

57 viscous interaction between two streams, shear layers of primary stream are working on the secondary stream causing small eddies and vortices in the interaction region. Figure 4 6 Contours of turbulence intensity. Percentage

PAGE 58

58 CHAPTER 5 MODELLING OF EQUIVALENT PERFECT GAS MODEL In an effort to reduce the computational effort each time we perform a simulation using real gas assumptions an innovative approach is being discussed in this chapter. Specific heat constant and viscosity are the two major factors that vary according to the temperature in the flow domain of the real gas model w hereas these values will be kept constant in a perfect gas model. The computational effort and time that goes into a real gas model is of the order of ten times higher th an that of a simulation with perfect gas assumptions So in or der to speed up the convergence, save time and to reduce the computational effort by lessening the complexity of the equations used this approach is useful for the future designers. 5.1 Algorithm to Estimate t he Equivalent Viscosity The basic output of an y converged solution in the present simulation is the compression ratio and the entrainment ratio associated with it, these two components together constitute the performance of the system. In the perfect gas model for a given set of boundary conditions th at is for a given compression ratio, entrainment ratio is largely dependent upon the specific heat constant and viscosity. Holding these parameters as the key inputs we model the simulation. Some of the key steps involved are, Initially for a given set of boundary conditions a converged solution for real gas model is obtained. Entrainment ratio corresponding to the same is evaluated by post processing the results in F LUENT Now the perfect gas model is switched on with an initia l guess of viscosity and specific heat constant is made and the entrainment ratio is tabulated by varying the above key parameters. Now we search for such pair of values

PAGE 59

59 of and which gives the same entrainment ratio as that of the real gas model. N ow that we have a family of and , matching the performance of a real gas model, this combination is not unique. In order to make this combination unique, more in depth analysis is done by studying the sensitivity of these two parameters with respect to the entrainment ratio. In the operational regime of interest, does not vary much and is a weak function of temperature which is validated from the superheated tables of R134 a. So the value of is chosen such that it represents the value of the primary stream and an according value of is chosen which completes the pair and gives the performance of the real gas model. 5.2 Linear F it for and From the super heated tables of refrigerant a line of least squares fit is made for Depending upon the temperature of the primary stream value is calculated from the fit. Now let us assume depends upon the stagnation temperatures of the primary inlet secondary inlet ,stagnation pressure of primary inlet secondary inlet static p ressure of outlet and specific heat constant A linear fit for is generated using the following mathematical tool available in excel. 5.3 LINEST This tool is used to generate the fit for with the normalized val ues of pressure and temperature. B riefing about LINEST it calculates the statistics for a line by using the "least squares" method to calculate a straight line that best fits your data, and then returns an array that describes the line. LINEST is used with other functions to calculate the statistics for other types of models that are linear in the unknown parameters,

PAGE 60

60 including polynomial, logarithmic, exponential, and power series. Because this function returns an array of values, it must be entered as an array formula. The equation for the line is: o r (if there are multiple ranges of x values) where the dependent y value is a function of the independent x values. The m values are coefficients corresponding to each x value, and b is a constant va lue. Note that y, x, and m can be vectors. The array that LINEST returns is {mn,mn 1,...,m1,b}. LINEST can also return additional regression statistics. Now ou r unknown y is the viscosity and the parameters it depends on are , , and As discussed above, is fit as a linear combination of all the parameters stated from the data Table 5 2 Now the linear fit for can be written as = 0.971058 + 0.505967 + 0.763564 + 0.967391 0.05024 0.22698 from the coefficient matrix Table 5 3 Now a designer picks an operational regime and certain boundary conditions, the value of is calculated from the superheat tables of depending the primary flow temperature. The normalized pressure values are calculated by dividing the pressure with the critical pressure of and the same exercise is done with the temperature. Corresponding values are input to the linear fit generated using excel in order to calculate the value of normalized v iscosity. We get back the value of equivalent by multiplying it with the base of value of which gives the pe rformance of the model

PAGE 61

61 Table 5 1 List of boundary conditions used to make the fit. SNO 1 1000000 600000 660000 373 285 2 1000000 600000 650000 378 286 3 1000000 600000 660000 368 287 4 1000000 600000 650000 370 288 5 1000000 500000 550000 373 289 6 1000000 500000 550000 385 290 7 1000000 500000 550000 390 290 8 1000000 500000 550000 395 288 9 900000 500000 550000 373 285 10 900000 500000 540000 378 286 11 900000 500000 550000 368 287 12 900000 500000 540000 370 288 13 900000 450000 495000 373 289 14 900000 450000 500000 385 290 15 900000 450000 495000 390 290 16 900000 450000 500000 395 288 17 800000 420000 460000 373 285 18 800000 420000 450000 378 286 19 800000 420000 460000 368 287 20 800000 420000 450000 370 288 21 800000 400000 440000 373 289 22 800000 400000 440000 385 290 23 800000 400000 450000 390 290 24 800000 400000 450000 395 288 25 700000 400000 450000 373 285 26 700000 400000 440000 378 286 27 700000 400000 440000 368 287 28 700000 400000 450000 370 288 29 700000 350000 390000 373 289 30 700000 350000 385000 385 290 31 700000 350000 390000 390 290 32 700000 350000 385000 395 288 33 600000 350000 390000 373 285 34 600000 350000 385000 378 286 35 600000 350000 390000 368 287 36 600000 300000 330000 370 288 37 600000 300000 335000 373 289 38 600000 300000 333000 385 290 39 600000 300000 330000 390 290 40 600000 300000 332000 395 288

PAGE 62

62 Table 5 2 Normalized parameters 0.25 0 0.15 0 0.165 0.762 1.003 0.925 0.25 0 0.15 0 0.162 0.764 1.016 0.9 00 0.25 0 0.15 0 0.165 0.767 0.990 0.916 0.25 0 0.15 0 0.162 0.770 0.995 0.925 0.25 0 0.120 0.137 0.772 1.003 0.916 0.25 0 0.120 0.137 0.775 1.034 0.925 0.25 0 0.120 0.137 0.775 1.047 0.908 0.25 0 0.120 0.137 0.770 1.060 0.9 00 0.22 0 0.120 0.137 0.762 1.003 0.875 0.22 0 0.120 0.135 0.764 1.016 0.825 0.22 0 0.120 0.137 0.767 0.990 0.8 00 0.22 0 0.120 0.135 0.770 0.995 0.816 0.22 0 0.110 0.123 0.772 1.003 0.808 0.22 0 0.110 0.125 0.775 1.034 0.825 0.22 0 0.110 0.123 0.775 1.047 0.8 00 0.22 0 0.110 0.125 0.770 1.060 0.816 0.2 0 0 0.105 0.115 0.762 1.003 0.791 0.2 0 0 0.105 0.112 0.76 4 1.016 0.8 00 0.2 0 0 0.105 0.115 0.767 0.990 0.783 0.2 0 0 0.105 0.112 0.770 0.995 0.8 00 0.2 0 0 0.1 00 0.11 0 0.772 1.003 0.8 00 0.2 0 0 0.1 00 0.11 0 0.775 1.034 0.791 0.2 0 0 0.1 00 0.112 0.775 1.047 0.783 0.2 0 0 0.1 00 0.11 2 0.770 1.060 0.775 0.17 0 0.1 00 0.112 0.762 1.003 0.766 0.17 0 0.1 00 0.11 0 0.764 1.016 0.758 0.17 0 0.1 00 0.11 0 0.767 0.990 0.8 00 0.17 0 0.1 00 0.112 0.770 0.995 0.766 0.17 0 0.080 0.097 0.772 1.003 0.758 0.17 0 0.08 0 0.096 0.775 1.034 0.775 0.17 0 0.080 0.097 0.775 1.047 0.758 0.17 0 0.080 0.096 0.770 1.060 0.766 0.15 0 0.080 0.097 0.762 1.003 0.733 0.15 0 0.080 0.096 0.764 1.016 0.716 0.15 0 0.080 0.097 0.767 0.990 0.733 0.15 0 0.070 0.082 0.770 0.995 0.725 0.15 0 0.070 0.083 0.772 1.003 0.741 0.15 0 0.070 0.083 0.775 1.034 0.716 0.15 0 0.070 0.082 0.775 1.047 0.733 0.15 0 0.070 0.083 0.770 1.060 0.708

PAGE 63

63 Table 5 3 LINEST coefficient matrix 0.05024 0.967391 0.763564 0.505967 0.971058 0.22698 #N/A 0.18724 1.11982 2.866043 3.195672 0.408336 0.862776 #N/A 0.895987 0.022655 #N/A #N/A #N/A #N/A #N/A 58.57619 34 #N/A #N/A #N/A #N/A #N/A 0.150327 0.017451 #N/A #N/A #N/A #N/A #N/A Figure 5 1 Histogram showing the variation using the linear fit and the actual values Series 1 actual; Series 2 generated. 0.00 0.05 0.10 0.15 0.20 0.25 0.30 0.35 0.40 0.45 0.50 0.55 0.60 0.65 0.70 0.75 0.80 0.85 0.90 0.95 1.00 each bar shows a data point Series1 Series2 ACTUAL (series1) VS CALCULATED (series2)

PAGE 64

64 5.4 Verification of the Algorithm In order to prove the efficacy of the algorithm, it is tested for wide range of boundary conditions and the results are shown in th e form of histograms in F igure 5 1 showing the variation of calculated value with the actual value of normalized viscosity Figure 5 2 Percentage error for 40 data points. Thirty six data points lie within a pe rcentage error of 4% to 0% in the data sheet, which shows the accuracy of the linear fit generated using method of least squares. Figure 5 3 illustrates that the data fit generated for viscosity is 89.6 % accurate. The trend line slope should be actually 1 in order for the expe rimental data to be in perfect match with the theoretical data, it is 0.896 from the equation of trendline shown. 0 1 2 3 4 5 6 7 0 5 10 15 20 25 30 35 40 45 P e r c e n t a g e E r r o r

PAGE 65

65 Figure 5 3. Plot showing the trend line for the data points. From F igures 5 2 and 5 3, it can be concluded that we gain computational effort and time with minimal loss in performance of the system using this algorithm y = 0.896x + 0.0836 R = 0.896 0.70 0.75 0.80 0.85 0.90 0.95 0.70 0.75 0.80 0.85 0.90 0.95 calculated actual

PAGE 66

66 CHAPTER 6 CONCLUSIONS In this study an integrated and a balanced CFD model study was presented for a sup ersonic ejector working with In this work, good validation results have been obtained for a wide range of operating conditions and were generally in a better quantitative agreement that those found in literature, especially for the off design operation A lit erature study was conducted to explain the ph enomenon and behavior of the eje ctor in greater detail. The axi symmet ric geometry of the ejector was modeled and tested for grid independencies and the solutions were validated by examining the convergence of the solution residuals. The outcome of a conver ged solution was studied and it was found that the simulation gave meaningful results, consistent with the theoretical operation and functioning of an ejector. Potential outcomes of this analysis are stated below 1. A functional ejector is capable of operatin g u nder varying initial and boundary conditions in an operating regime of where compressibility is high enough so that assumption of both streams being vapors is valid and it can replace a compressor in a vapor compression refrigeration system. 2. Rea l vapor data and scaling ratios obtained from literature were used to design two prototype ejectors for the pulse refrigeration system running on 3. A numerical model was then developed in FLUENT a commercial computational fluid dynamics package and is compared to an experimental rig, the results confirm flow entrainment in the ejector Numerical model is validated 4. A CFD model for perfect gas flow regime was then developed in order to achieve highly efficient computation effort and more speed in con vergence of results This is compared to a real gas model with two parameters and held as the keys to the perfect gas model. 5. Using the mathematical tools an algorithm is designed to minimize the computational effort and the time that goes into real gas modeling with minimal loss in the performance.

PAGE 67

67 6. Algorithm is tested and validated for the particular geometry of the ejector. The results were in good agreem ent with less than 3% loss in the performance of the ejector.

PAGE 68

68 CHAPTER 7 RECOMMENDATIONS FOR FUTURE STUDY Similar analysis and algorithms can be extended to different geometries of ejectors by varying nozzle exit position, converging angle, nozzle to throat area ratio an d to different refrigerants as well. A good model for ejectors operating with refrigerants should take into account possible nucleation, growing of condensation droplets, m eta stable states, and should be consistent in terms of the mixture speed of sound. To our knowledge, there is no such works published in the open literature A comparison can be made for a boiler inlet temperature equal to the evaporator inlet temperature in the boundary conditions so as to have similar cooling loads at similar temperatures. For the pulse refrigeration system configuration discussed in this paper, different refrigerants will be considered. It appears that a refrigerant with a higher critical temperature will allow for higher entrainment ratios and thus better system performance. A low critical point pressure i s also desirable to allow for thinner pipe walls. This can be investigated at a higher order of magnitude. Flow field can be further made complex by incorporating two phase regime in the mixing chamber which makes the simulation more demanding and closer t o reality The model should be reconstructed in a full 3 D form and this should be compared with the axisymmetric geometry used in this study to compare the results. The turbulence model used for the iterative calculations can be changed to investigate the dependence of the solution on this.

PAGE 69

69 LIST OF REFERENCES 1. Michael Brooks, S. du Clou, Bhageerath. Bogi, W.E. Lear and S.A. Sherif refrigeration syste 25 28 July 2010. 2. International Journal of Refrigeration vol. 29, no. 7, 2006, pp. 1160 1166. 3. No. 3, pp. 216 226, 1974. 4. Fluids Engineering, Vol. 117, No. 2, pp. 309 316, 1995. 5. 444, 1991. 6. iments on Air to Air Supersonic TM 1410, September, 1958a. 7. Mechanics, Vol. V, H.L. Dryden and Th, von Karman (editors), Academic Press, New York, pp. 1 33, 1958b. 8. April June, pp. 285 291, 1995. 9. s of a Flow Proposal, NASA Marshall Space Flight Center, Thermal and Life Support Division, Huntsville, Alabama, 1996. 10. the Lockheed 1626, June, 1987. 11. Hydraulic Jet Pumping of Two Engineering, Vol. 5, No.4, pp. 361 364, 1990.

PAGE 70

70 12. Considerations of Jet Pumps with Supersonic Two AIAA 37th Aerospace Sciences Meeting, Reno, Nevada, January 11 14, AIAA Paper 99 0461, 1999. 13. Jet Pump Performance with and without Cavitat Eng ineering, Vol. 114, No. 4, pp. 626 631, 1992. 14. Ph of Multiphase Flow, Vol. 17, No. 2, pp. 267 272, 1991. 15. Sherif, S.A., Lear, W.E., Steadham, J.M., Hunt, P.L., and Holladay, J.B., Phase Jet Pump of a Thermal Management System for Aerospac Reno, Nevada, January 12 15, AIAA Paper 98 0360, 1998.

PAGE 71

71 BIOGRAPHICAL SKETCH Bhageerath Bogi was bo rn in Warangal, India Bhageerath co m pleted his Bachelor of Technology degree from National Ins titute of Technology ,Warangal, Andhra Pradesh, India, on July 2009 after which he joined University of Florida to pursue his Master of Science degree in Aerospace Engineering Bhageerath st a rt e d working t o wards his maste r a t the University of Florida f r om the f all of 2009. Later, he got the opportunity to be a part of the HVAC lab under the guidance of Dr. S.A.Sherif and Dr. W E. Lear Upon completion of his m August 2011, Bhageerath plans to continue contrib u ting to the energy industry and build on his knowledge and experience.