<%BANNER%>

Computational Fluid Dynamics Investigation of Air Velocity and Temperature Distribution in a Room Equipped with Active C...

Permanent Link: http://ufdc.ufl.edu/UFE0042995/00001

Material Information

Title: Computational Fluid Dynamics Investigation of Air Velocity and Temperature Distribution in a Room Equipped with Active Chilled Beam Air-Conditioning
Physical Description: 1 online resource (68 p.)
Language: english
Creator: VEMPATI,ABHIJYOTH REDDY
Publisher: University of Florida
Place of Publication: Gainesville, Fla.
Publication Date: 2011

Subjects

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

Notes

Abstract: 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 COMPUTATIONAL FLUID DYNAMICS INVESTIGATION OF AIR VELOCITY AND TEMPERATURE DISTRIBUTION IN A ROOM EQUIPPED WITH ACTIVE CHILLED BEAM AIR-CONDITIONING By: Abhijyoth Reddy Vempati May 2011 Chair: H.A. (Skip) Ingley Major: Mechanical Engineering Chilled beam air-conditioning technology evolved in Europe in the late 1970s, but its presence in the United States heating ventilation and air conditioning market has not been felt until recently. These systems are supposedly more energy efficient and are claimed to be reducing electricity usage by about 20-30% because of reduced fan power requirement. The unit makes use of a "nozzle concept" which uses the high velocity of primary air coming from nozzles inside the beam unit to create a low pressure region which induces part of the room air into the air-conditioning unit. The high speed primary air jet induces about two-thirds of the total air requirement from the room itself. This induced air is cooled and then mixed with primary which is sent back for air conditioning. Because of the reduced fan power requirement to pump the air, the chilled beam unit turns out to be energy efficient. Their added advantages are less noisy operation, reduced CO2 emissions, easier customization and high comfort levels. The objective of the present research was to investigate the velocity and temperature distribution inside a room fitted with two active chilled beams (TROX 612B-HC active chilled beam unit) by use of numerical simulations. For the study purpose, a test room with the dimensions 40ft?10ft?10ft (l?w?h) was considered. The room environment was simulated by creating and preprocessing the model in GAMBIT 2.4.6 and using FLUENT 6.3.26 for solving, analyzing and post processing the results. The study was focused on summer air-conditioning. Key input parameters such as the type of chilled beam used, amount of primary air supplied, primary air temperature, nozzle type, room conditions, water temperature etc were taken from data sheets obtained from Affiliated Engineers Inc, Gainesville Branch. Numerical results have been validated by velocity measurements obtained from TROX DID 612B-HC active chilled beam selection program. The results obtained from the numerical simulations agreed well with the data available from the TROX selection program. In the end, a two dimensional simulation of a room with a multi-cone diffuser was performed for comparison of airflow distribution between an active chilled beam and a multi-cone diffuser. It was found out that with the active chilled beams, there was an almost uniform temperature distribution inside the room and quicker response to changes in heat load. Though the numerical simulation provides considerable insight into the theoretical indoor airflow distribution, the underlying assumptions that went into the modeling are questionable. Experimental studies will be necessary to develop a more accurate model.
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 ABHIJYOTH REDDY VEMPATI.
Thesis: Thesis (M.S.)--University of Florida, 2011.
Local: Adviser: Ingley, Herbert A.
Electronic Access: RESTRICTED TO UF STUDENTS, STAFF, FACULTY, AND ON-CAMPUS USE UNTIL 2011-10-31

Record Information

Source Institution: UFRGP
Rights Management: Applicable rights reserved.
Classification: lcc - LD1780 2011
System ID: UFE0042995:00001

Permanent Link: http://ufdc.ufl.edu/UFE0042995/00001

Material Information

Title: Computational Fluid Dynamics Investigation of Air Velocity and Temperature Distribution in a Room Equipped with Active Chilled Beam Air-Conditioning
Physical Description: 1 online resource (68 p.)
Language: english
Creator: VEMPATI,ABHIJYOTH REDDY
Publisher: University of Florida
Place of Publication: Gainesville, Fla.
Publication Date: 2011

Subjects

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

Notes

Abstract: 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 COMPUTATIONAL FLUID DYNAMICS INVESTIGATION OF AIR VELOCITY AND TEMPERATURE DISTRIBUTION IN A ROOM EQUIPPED WITH ACTIVE CHILLED BEAM AIR-CONDITIONING By: Abhijyoth Reddy Vempati May 2011 Chair: H.A. (Skip) Ingley Major: Mechanical Engineering Chilled beam air-conditioning technology evolved in Europe in the late 1970s, but its presence in the United States heating ventilation and air conditioning market has not been felt until recently. These systems are supposedly more energy efficient and are claimed to be reducing electricity usage by about 20-30% because of reduced fan power requirement. The unit makes use of a "nozzle concept" which uses the high velocity of primary air coming from nozzles inside the beam unit to create a low pressure region which induces part of the room air into the air-conditioning unit. The high speed primary air jet induces about two-thirds of the total air requirement from the room itself. This induced air is cooled and then mixed with primary which is sent back for air conditioning. Because of the reduced fan power requirement to pump the air, the chilled beam unit turns out to be energy efficient. Their added advantages are less noisy operation, reduced CO2 emissions, easier customization and high comfort levels. The objective of the present research was to investigate the velocity and temperature distribution inside a room fitted with two active chilled beams (TROX 612B-HC active chilled beam unit) by use of numerical simulations. For the study purpose, a test room with the dimensions 40ft?10ft?10ft (l?w?h) was considered. The room environment was simulated by creating and preprocessing the model in GAMBIT 2.4.6 and using FLUENT 6.3.26 for solving, analyzing and post processing the results. The study was focused on summer air-conditioning. Key input parameters such as the type of chilled beam used, amount of primary air supplied, primary air temperature, nozzle type, room conditions, water temperature etc were taken from data sheets obtained from Affiliated Engineers Inc, Gainesville Branch. Numerical results have been validated by velocity measurements obtained from TROX DID 612B-HC active chilled beam selection program. The results obtained from the numerical simulations agreed well with the data available from the TROX selection program. In the end, a two dimensional simulation of a room with a multi-cone diffuser was performed for comparison of airflow distribution between an active chilled beam and a multi-cone diffuser. It was found out that with the active chilled beams, there was an almost uniform temperature distribution inside the room and quicker response to changes in heat load. Though the numerical simulation provides considerable insight into the theoretical indoor airflow distribution, the underlying assumptions that went into the modeling are questionable. Experimental studies will be necessary to develop a more accurate model.
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 ABHIJYOTH REDDY VEMPATI.
Thesis: Thesis (M.S.)--University of Florida, 2011.
Local: Adviser: Ingley, Herbert A.
Electronic Access: RESTRICTED TO UF STUDENTS, STAFF, FACULTY, AND ON-CAMPUS USE UNTIL 2011-10-31

Record Information

Source Institution: UFRGP
Rights Management: Applicable rights reserved.
Classification: lcc - LD1780 2011
System ID: UFE0042995:00001


This item has the following downloads:


Full Text

PAGE 1

1 C OMPUTATIONAL F LUID D YNAMICS INVESTIGATION OF AIR VELOCITY AND TEMPERATURE DISTRIBUTION IN A ROOM EQUIPPED WITH ACTIVE CHILLED BEAM AIR CONDITIONING By ABHIJYOTH REDDY VEMPATI 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 Abhijyoth Reddy Vempati

PAGE 3

3 T o my parents and my sister

PAGE 4

4 ACKNOWLEDGEMENTS First and foremost, I would like to thank my parents Mr.Obula Reddy Vempati and Mrs. Lalita Vempati and my sister M/s Deepti Vempati for their emotional and financial support, without which I would not have been a part of the rich and competitive graduate program offered by th e Department of Mechanical and Aerospace Engineering at the University of Florida. I t gives me great pleasure to place on record my deep sense of gratitude for my committee chair Dr. H. A. (Skip) Ingley, for his inspiring and valuable guidance and untiri ng interest given at every stage of this work right up to the preparation of this dissertation. I wish to thank Dr. S. A. Sherif for his constant encouragemen t during the course of the project and for agreeing to be a member in my committee My s pecial than ks are due to Dr.Subrata Roy for his invaluable suggestions and his lab members : James, Navya Mastanaiah and Jignesh Soni for guiding me in the right direction whenever I faced problems regarding numerical simulations and CFD techniques My heartfelt thanks are due to Dr. Chin Cheng (James) Wang and doctoral candidate T ae Sook Lee for graciously allocating me their valuable time to answer my queries. It was because of some interesting discussions with them, this research was possible. I wo uld also like to thank Laurence Goodall (P.E) from Affiliated Engineers Inc, Gaine sville Branch for teaching me the concept of chilled beam air conditioning and providing me with the necessary data to carry out the numerical simulation. Finally, I take this opportunity to thank my beloved friends Uday Kiran Mahakali Anand Ankala Bhageerath Bogi Deept h i Thanigundala to name a few who have always been there for me

PAGE 5

5 TABLE OF CONTENTS page ACKNOWLEDGEMENTS ................................ ................................ ............................... 4 LIST OF TABLES ................................ ................................ ................................ ............ 7 LIST OF FIGURES ................................ ................................ ................................ .......... 8 LIST OF ABBREVIATIONS ................................ ................................ ........................... 10 ABSTRACT ................................ ................................ ................................ ................... 11 CHAPTER 1 INTRODUCTION ................................ ................................ ................................ .... 13 1.1 Chilled Beam Air Conditioning ................................ ................................ .......... 13 1.2 Objectives of Present Study ................................ ................................ .............. 14 1.3 Proposed Investigation and Scope of Research ................................ ............... 15 2 LITERATURE REVIEW ................................ ................................ .......................... 16 2.1 History of Chilled Beams ................................ ................................ ................... 16 2.2 Types of Chilled Beams ................................ ................................ .................... 16 2.3 Nu merical and Experimental Studies of Indoor Air Conditioning ...................... 19 3 PROBLEM STATEMENT ................................ ................................ ........................ 27 3.1 Data Acquisition and Physical Calculations ................................ ...................... 27 3.2 Identifying the Physical Domain and Input Parameters Required ..................... 28 4 CFD SIMULATION OF TEST ROOM ................................ ................................ ..... 30 4.1 Steps Involved In the Simulation Process ................................ ......................... 30 4.1.1 Pre processing. ................................ ................................ ....................... 31 4.1.2 Solving ................................ ................................ ................................ ..... 33 4.2 Setting the So lution Controls and Obtaining a Converged Solution .................. 37 5 RESULTS AND OBSERVATIONS ................................ ................................ ......... 41 5.1 Remarks and Observations ................................ ................................ .............. 41 5.2 Simulation Results ................................ ................................ ............................ 42 6 VALIDATIONS ................................ ................................ ................................ ........ 53

PAGE 6

6 7 CONCLUSIONS AND RECOMMENDATIONS ................................ ....................... 56 7.1 Conclusions ................................ ................................ ................................ ...... 56 7.2 Recommendati ons for Further Studies ................................ ............................. 57 APPENDIX A SOLID ROOM AND MESHED GEOMETRIC MODELS ................................ ......... 58 B MESH CONVERGENCE STUDY ................................ ................................ ........... 61 C COMPAR ISION WITH A MULTI CONE DIFFUSER ................................ ............... 63 LIST OF REFERENCES ................................ ................................ ............................... 66 BIOGRAPHICAL SKETCH ................................ ................................ ............................ 68

PAGE 7

7 LIST OF TABLES Table page 4 1 Solver settings for 2 D simulation ................................ ................................ ....... 39 4 2 Solver settings for 3 D simulation ................................ ................................ ....... 39 4 3 Descritization scheme for 2 D simulation ................................ ........................... 39 4 4 Descritization scheme for 3 D simulation ................................ ........................... 39 4 5 Under relaxation factors for both 2 D and 3 D simulations ................................ 40 6 1 Parameters V 1 and V 2 predicted by various models ................................ ........... 54 6 2 Error in prediction of V 1 and V 2 by the turbulence models ................................ .. 54 B 1 Comparison of the effect of grid on solution ................................ ....................... 62

PAGE 8

8 LIST OF FIGURES Figure page 1 1 Active chilled beam ................................ ................................ ............................. 15 2 1 Passive chilled beam ................................ ................................ .......................... 25 2 2 Active chilled beam ................................ ................................ ............................. 26 3 1 Room air velocity and temperatures parameters used in the design .................. 28 3 2 Schematic showing the location of lights and the air conditioning unit ............... 29 4 1 Schematic show ing the boundary conditions employed ................................ ..... 40 5 1 Velocity vectors of airflow inside the room ................................ .......................... 44 5 2 Temperature of airflow inside the room ................................ .............................. 44 5 3 Path lines showing the velocity magni tude of airflow inside the room ................ 45 5 4 Path lines showing the temperat ure of airf low inside the room ........................... 45 5 5 Plot of velocity magnitude (at a height of 1.7 m) across the room ...................... 46 5 6 Velocity vectors of airflow inside the room ................................ .......................... 46 5 7 Temperature of airflow inside the room ................................ .............................. 47 5 8 Path lines showing the velocity magnitude of airflow inside the room ................ 47 5 9 Path lines showing the temperature of airflow inside the room ........................... 48 5 10 Plot of velocity magnitude (at a height of 1.7 m) across the room ...................... 48 5 11 Velocity vectors of airflow inside the room ................................ .......................... 49 5 12 Temperature of airflow inside the room ................................ .............................. 49 5 13 Path lines showing the velocity magni tude of airflow inside the room ................ 50 5 14 Path lines showing the temperature of airflow inside the room ........................... 50 5 15 Velocity vectors of airflow (at the later al mid section) across the room .............. 51 5 16 Temperature of airflow (at the later al mid section) across the room ................... 51 5 17 Plot of velocity magnitude of airflow across the room ................................ ......... 52

PAGE 9

9 6 1 Locations showing the points of interest where the data is to be compared ....... 54 6 2 TROX active chilled beam calculation program ................................ .................. 55 A 1 Isometric view of the room model showing the gradient in x direction ................ 58 A 2 Isometric view of the meshed room mo del ................................ ......................... 58 A 3 Top View of the solid room model obtained from gambit ................................ .... 59 A 4 Isometric view of the solid room model obtained from gambit ............................ 59 A 5 Isometric view of the meshed room model obtained from gambit ....................... 60 B 1 Plot of velocity parameters as the mesh density varies ................................ ...... 62 C 1 Front view of the meshed 2 d room model fitted with a multi cone diffuser ........ 63 C 2 Velocity vectors of airflow inside the room ................................ .......................... 64 C 3 Temperature of airflow inside the room ................................ .............................. 64 C 4 Plot of velocity magnitude of airf low (at a height of 1.7m) across the room ........ 65

PAGE 10

10 LIST OF ABBREVIATION S CFD Computational Fluid Dynamics HVAC Heating Ventilation and Air Conditioning Btuh British Thermal Unit/hour SIMPLE Semi Implicit Method for Pressure Linked Equations RNG Re Normalization Group FEM Finite Element Methods SST Shear Stress Transport DNS Direct Numerical Simulation LES Large Eddy Simulation RANS Reynolds Averaged Navier Stokes Re Reynolds Number k Turbulent Kinetic Energy Turbulent Dissipation Rate Turbulent Specific dissipation rate V iscosity k k epsilon k k omega V 1 Local velocity at the top of the occupied zone at a distance of two inches from the wall V2 Local velocity at the top of the occupied zone directly below the point of collision of opposing air streams A Centerline distance between two active beams with opposing blows X Distance between active beam centerline and an adjacent wall H Mounting height of active chilled beam

PAGE 11

11 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 C OMPUTATIONAL F LUID D YNAMICS INVESTIGATION OF AIR VELOCITY AND TEMPERATURE DISTRIBUTION IN A ROOM EQUIPPED WITH ACTIVE CHILLED BEAM AIR CONDITIONING By Abhijyoth Reddy Vempati May 2011 Chair: H.A ( Skip ) Ingley Major: Mechanical Engineering Chilled be am air conditioning technology evolved in Europe in the late 1970 s, b ut its presence in the U nited S tates heating ventilation and air conditioning market has not been felt until recently. These systems are supposedly more energy efficient and are claimed to be reducing electricity usage by about 20 30% because of reduced fan power requirement. The high velocity of primary air coming from nozzles inside the beam unit to create a low pressure region which induces part of the room air into the air conditioning unit. The high speed primary air jet induces about two thirds of the total air requirement f r o m the room itself. This induced air is cooled and then mixed with primary which is sent back for air conditioning Because of the reduced fan power requirement to pump the air, the chilled beam unit turns out to be energy ef ficient Their added advantages are less noisy operation, reduced CO2 emissions, easie r customization and high comfort levels. The objecti ve of the present research wa s to investigate the velocity and temperature distribution inside a room fitte d with two active chilled beams ( TROX 612B HC active chilled beam unit ) by use of numerical simulations For the study purpose, a

PAGE 12

12 test room with the dimensions 40ft 10ft 10ft (l w h ) wa s considered. The room environment wa s simulated by creating and preprocessing the model in GAMBIT 2.4.6 and using FLUENT 6.3.26 for solving, analyzing and post processing the results The study wa s focused on summer air conditioning Key input parameters such as the type of chilled beam used, amount of primary air supplied, primary air temperature, nozzle type, room condition s water temperature etc wer e taken from data sheets obtained from Affiliated Engineers Inc, Gainesville Branch. Numerical results have been validated by velocity measurements obtained from TROX DID 612B HC a cti ve chilled b eam selection program. The results obtained from the numerica l simulations agreed well with the data available from the TROX selection program. In the end, a two dimensional simulation of a room with a multi cone diffuser was performed for comparison of airflow distribution between an active chilled beam and a multi cone diffuser. It was found out that with the active chilled beams, there was a n almost uniform temperature distribution inside the room and quicker response to changes in heat load. Though the numerical simulation provides considerable insight into the theoretical indoor airflow distribution, the underlying assumptions that went into the modeling are questionable. Experimental studies will be necessary to develop a more accurate model.

PAGE 13

13 CHAPTER 1 INTRODUCTION 1.1 Chilled Beam Air Conditioning An air conditioner is a mechanical appliance which supplies and maintains desirable internal atmospheric conditions for human comfort, irrespective of e xternal conditions. It is a system which effectively controls the temperature, humidity, purity and motion of air. It typically consists of cooling and dehumidifying processes for summer air conditioning or heating and humidification process for winter air conditioning. A system which performs the task of heating, ventilation and air conditioning may be called an HVAC system. A c hilled beam forms a part of an HVAC system which uses chilled water flow through a hollow beam (heat exchanger) to remove heat from a room It brings the chilled water closer to the occupied space than central air handlers a nd limits the utilization of fan power which ultimately leads to energy savings and cost cutting They are capable of handling only sensible ( dry) loads and hence must be connected to a source of primary dry air to provide dehumidification Fresh air must be supplied with the primary air for ventilation purposes. The water flowing in the beam unit needs to be heated/cooled outside of the conditioned space and care must be taken to maintain the water temperature higher than the room dew point temperature so as to avoid condensation on the coil. A rule of thumb is to keep the water flowing through the chilled beam at a temperature approximately one deg ree Fahrenheit above the room dew point temperature. Hence the water is usually supplied at 55 59F .This results in considerable energy savings and gives scope for geothermal cooling i.e. use of water reservoirs for cooling. [2 ]

PAGE 14

14 Advantages of Chilled Beam Technology are reported to include: a) Reduction in carbon emissions by about 15% b) Sustainability: chilled beams can utilize chilled water supplied at 57 F and returned at 62 F .Hence for a fair amount of the year, ground water; evaporative cooled water etc. can be utilized eliminating the need for usin g mechanical refrigeration for further cooling of the water c) No need for suspended ceilings. Chilled beams can be directly fitted in to a soffit and left exposed. d) L ower noise levels e) Mechanical system and duct r eductions f) Reduced or e limin ated r eheat requirement g) Pump energy instead of fan e nergy h) Can fit in to tight s pace Disadvantages of Chilled Beam Technology include: a) Difficult to handle r ooms w ith high heat l oads without supplemental air b) Condensation can be an issue i f not installed properly c) High first c ost ($80/ ) 1.2 Objectives of Present Study The present investigation aims at simulating an ai r conditioned room fitted with two Active Chilled Beam s ( T ROX DID 612B HC ) The velocity and temperature distribution inside the room will then be investigated to rate the performance of chilled beam air conditioning in terms of occupant comfort. The computational stud ies are performed on a 40ft 10ft 10ft room (12.192m 3.048m 3.048m) (l w h) by creating and pre processing the room model in GAMBIT 2.4.6 and analyzing and post processing the results in FLUENT 6.3.26 a commercial CFD code.

PAGE 15

15 1.3 Proposed Investigation and Scope of Research Both two dimensional and three dimensional simulations of the room with active chilled beam are performed. The airflow velocity and temperature distribution inside the room is of interest in the present research. The velocities and temperatures at certain locations inside the room will be evaluated to compare the results of the numerical simulation with those obtained from a TROX Active chilled beam selection program. To reduc e the computational intensity and complexity of the problem, a simplified geometrical model of the chilled beam will be considered. The suitability of various turbulence models will also be investigated in terms of achieving well converged solutions for the given problem set up A two dimensional simulation of a room fitted with a multi cone diffuser will also be performe d in the end for comparison with the results obtained with a chilled beam unit .This will give a qualitative idea about the performance of chilled beam air conditioning compared to conventional diffusers. Figure 1 1. Active chilled beam ( adapted from: CPD module [1] )

PAGE 16

16 CHAPTER 2 LITERATURE REVIEW 2.1 History o f Chilled Beams Chilled beams appeared in the E uropean market in the late 1970 s.They combine air supply with cooling or heating. The main principle of the active chilled beam s is induction of room air caused by the high velocity of primary supply air. Inducted room air is drawn into the beam through a water air heat exchanger where it is cooled or heated and subsequently mixed with the fresh a ir and supplied to the room t h rough slot diffusers The air flows from the beam over the ceiling, cascading down into the room In case of parallel positioning of the beams the jets can meet in the middle, lose momentum and fall down to the occupied zone. 2.2 Types of Chilled Beams Chilled beam technology uses closed circuit water based systems to facilitate heat transfer. Water flows through the cooling system absorbing and removing heat from the occupied space. Instead of radiation, chilled beams rely on convection heat transfer to delive r cooling. [1] The chilled beams can be broadly classified into four categories depending on the working principle as follows: a) Chilled ceilings b) Passive chilled Beams c) Active chilled Beams d) Multi Service Chilled Beams Chilled ceilings Also r eferred to as the original chilled beam syste m ; the chilled ceilings work on the principle of radiation. They exchange heat with the occupied space by radiation instead of introducing cold air These systems resemble a standard suspended metal

PAGE 17

17 ceiling system and are constr ucted from a copper cooling element bonded to the rear of a metal ceiling tile. Alternatively, these systems can also be used for heating purposes. Advantages: a) The most energy efficient of all the chilled beam systems Disadvantages: a) Lack of control of the humidity inside the room and hence need to be cou pled with a forced air system to tackle latent heat loads b) Very low sensible cooling capacity of 75.7 24 BTUH/square foot ) of linear beam c) Do not provide fresh air without an auxiliary outdoor air system. Passive chilled Beams Also referred to as the second generation of chilled beams, these were the first to use a pipe surrounded by fins in order to form a radiator system and are often used with under floor air distribution system s Rather th an radiation, these rely on the phenomenon of natural convection to provide cooling. As the room air gets h ot, it rises through the chilled beam where it is cooled and falls back to the occupied space Thus its efficiency increases as the room temperature increases (refer to Figure 2 1). Advantages: a) Increased cooling and heating capacity b) Extremely effective in taking care of solar heat load and sensible heat load. c) Moderate sensible cooling capacity of 384.6 400 BTUH/ ft. ) of linear beam Disadvantages: a) Lack of control of the humidity inside the room and hence need to be coupled with a forced air system to tackle latent heat loads b) Do not provide ventilation air

PAGE 18

18 Active chilled Beams Also known as high induction diffusers, these entered the H VAC industry in the early 1990 s and thus represent the third generation of chilled beams. These work on the principle of forced air induction and hence can provide both heating and cooling. All the HVAC functions are taken care of by a single unit .The ven tilation air is ducted through the chilled beam as part of the primary air It induces air movement over the coil, mixes it with the conditioned air and sends it back to the occupied space ( refer to Figure 2 2) Advantages: a) T akes care of both sensible and latent heat loads by providing ventilation air b) V ery high cooling capacity of 576.911 ( 600 BTUH/linear foot ) of beam Multi Service Chilled Beams Referred to as the fourth generation of chilled beam systems, these are new to the US market. An active o r passive chilled beam system can be made a multi service beam unit. These combine building operations to a single unit containing lighting fixtures, sprinkler systems, smoke detectors, security sensors etc. Advantages: a) D ecrease in building construction t ime by about 25% due to decrease in installation time b) Reduced ceiling space requirement. In some five floors were built in the same space occupied by a standard four story building Disadvantages a) Suitable for offices, labs, schools, hotels etc but not for residential areas because of lack of humidity control in case of multi service beams fi tted with passive chilled beams b) If a window is left open, condensation can occur on the coil

PAGE 19

19 2.3 Numerical and Experimental Studie s of Indoor Air Conditioning The history of using CFD as a tool to analyze indoor airflows dates back to 1974 with Neilsen being the pioneer in initiating such studies. Jelena and Qingyan [ 2 ] ASHRAE Members, came up with a manual illustrating the various steps involved in the verification, validation and reporting of CFD simulations of indoor air flows by citing references of numerous papers published in Roomvent (2000). The following can be deduced from their manual: a) Use a stea dy state simulation and star t with a simpler tur bulence model such as standard k model. The low Reynolds number turbulence mo dels took longer computing time b) Use of f irst order differencing scheme and SIMPLE algorithms (for pressure velocity compounding) seem to be more stable c) Zero pressure and zero gradient for all other flow parameters were used as boundary conditions for the exhaust fro m the space d) For a complicated analysis, grid independent results are very difficult to obtain. Hence there is a tradeoff between the grid resoluti on and computational intensity so as to a ttain sensible physical results e) Uncertainty and error in the measurement of turbulent intensity is the largest in both the CFD model and experimental methods. It is difficult to judge which of them is accurate Zhu Li, Yuan [ 3 ] researched indoor airflow by cold air distribution systems. They used Fluent to perform numerical simulation s of indoor cold air distribution under different conditions and compared their results with an experimental setup. They threw light on the possible mathematical model and boundary conditions t hat are appropriate for simulations of indoor airflow They made the following assumptions: a) Incompressible, invariable, steady state flow which coincides with Boussinesq assumption an d finite volume approach b) Velocity inlet boundary condition for the diffuser inlets c) Negligible air leakage throughout the conditioned space

PAGE 20

20 d) Negligible solar radiation and internal heat sources e) High Reynolds number 2 equation k turbulence model combi ned wi th wall function Their experimental set up involved a room of dimensions 23.6ft 18.3ft 10.5ft ( 7.2m 5.6m 3.2m ) .T hey made use of a thermo static multi anemometer to measure the temperature and velocity of air in the room. Their experimental results matched very well with the numerical simulations carried out in FLUENT validating the appropriate way of setting up indoor airflow problems in a commercial CFD code like FLUENT. Juan,Daniel,Marcelo,Benoit [4 ] researched airflow modeling and comfort levels in a computer room .They used GAM B IT for pre processing the model, FLUENT 6.0.2 to carryout numerical simulations and Vu for post processing the results. They considered species transport as well as radiation conversation equations along with mass, momentum, e nergy and turbulence equations They validated their numerical re sults with a MINIBAT experimental set up by considering a k realizabl e model with a two layer approach near the walls. They made the following assumptions : a) Segregated ( pressure based) solver, SIMPLE pressure velocity c ouplin g and finite volume approach b) R enormalization group ( RNG ) k turbulence model to treat turbulence near the ai r supply c) Discrete Ordinates (DO ) radiation model and H2 0 was used in species transport equ ations d) M odeled computers and human beings ( through thermal mannequins) e) Room boundaries were modeled as adiabatic walls and were considered diffuse 1.0 f) V elocity inlet boundary conditions for diffuser inlets

PAGE 21

21 Through numerical simulations, they estimated four indoor air quality parameters mean age of air, m ean radiant temperature p redicted mean vote, p redicted percentage of dissatisfied. Their investigation revealed that boundary conditions and inclusion of real world geometries like diffuser inlets have a major impact on fluid flow Awbi [ 5 ] investigated the application of CFD in room ventilation by using a computer program based on finite difference approach to solve 2 D AND 3 D ventilation problems. Arsen Boryana, Lyuben, Viktor and Risto [6 ] studied the impact of airflow interactions on comfort in a full scale test room 17.7ft 13.7ft 8.2ft (5.4m 4.2m 2.5m ) fitted with four active chilled beams. They researched the impact of primary air flow rate and heat load strength o n the thermal environment created in the occupied space. They used thermal mannequins, artificial windows, ceiling lights as heat sources inside the room. The air speed and temperature measurements were used to calculate air diffusion performance index ( AD PI ) and draught rating index ( DR).They found out that the supplied air flow rate has a significant impact on DR. Th ey concluded that: a) Substantial changes of local thermal conditions at different workplaces occurred in the room when he at load and supply flow rate were changed b) Higher heat load and higher supplied flow rates increase the risk of draught discomfort in the occupied zone Ristom Pekka, Hannu and Alex [7 ] researched the impact of heat load location and strength on air flow pattern s in a mock up office 11.8ft 10.8f 10.8ft (3.6m 3.6m 3.3m) fitted with two passive chilled beams, three light fittings and a swirl diffuser. They used human dummies and computers as heat sources inside the room. Their findings are summarized as follows:

PAGE 22

22 a) Negligible buoya ncy force. The plumes from the heat loads were not powerful enough to fight the downward flow from the be am. Instead the heated air was c ounter acted by the downward cold flow from the beam .T he human dummy only acted as a flow obstacle. Hence the shape of the occupant simulator is important b) T he point of occurrence of the maximum velocity in the occupied zone depends on the strength of the heat source and its distribution in the room c) L ayout of internal equipment had a minor impact on air distribution d) Full scale studies and CFD simulations are important for complex intera ctions of flows Cammarata and Petrone [8 ] studied the thermodynamic and fluid dynamic performance of an active chilled beam for indoor air conditioning by investigating 2D and 3D models in a n FEM based software, COSMOL Multiphysics. They evaluated the maximum airflow velocity and horizontal and vertical temperature gradient. A n incompressible, steady state fluid flow with a two equation k turbulence model was used. They concluded that there is an a lmost constant velocity distribution in the occupied portion of the conditioned space. Jan, Viktor Risto and Arsen [9 ] came up with practical guidelines to minimize draught discomfort in rooms with four active chilled beams. They focused on factor s affecting thermal comfort. They conducted experiments in a full scale te st room with the dimensions 17.7ft 13.7ft 8.2ft ( 5.4 m 4.2 m 2.5m ). The chilled beams had a velocity control device to control the induced airflow rate. They experimented with different strengths of heat load and locations, different layout of chilled beams, heat generated by occupants, primary and induced airflow rate. They came up with the following guidelines: a) The room height with chilled beams should be no more than 11.48ft ( 3.5m ) which could otherwise lead the thermal forces to cause draught risks in the occupied zone, when there is a high cooling load

PAGE 23

23 b) Chilled beams installed in a lengthwise position can cause unnecessary draught risks c) Higher airflow rate causes higher mean v elocity leading to greater draught risk d) Chilled beams should be installed perpendicular to window faade s to avoid flow interaction between heated surface s and flow s from chilled beam Posner Buchanan, Rankin [1 0 ] studied the measurement and prediction of indoor airflow in a model room. They compare d 3 dimensional CFD simulations carried out in FLUENT with experimental results obtained from a one tenth sub scale isothermal model room. They used lased Doppler anemom etry ( LDA) and particle image velocimetry ( PIV) to measure temperature and velocity fields in the sub scaled room made of anodized aluminum of dimensions 30ft 15ft 10ft ( 9 .1 4 m 4 .5 7 m 3 .05 m ) having four plain glass windows They focused more on the impact of obstructions in the airflow distribution. For numerical simulation, their problem set up involved the following: a) Fluid flow was modeled using three different configurations as: laminar, standard k turbulence model and RNG k turbulence model Default values for constants were used b) A p ower law s cheme of descritization was used and transient simulation was carr ied out to achieve convergence c) Buoyancy effects were neglected. There were no heat sources and no heating/cooling by ventilated air They conclud e d that laminar and RNG model s compare better with experimental measurements than the standard turbulence model. The standard model tends to smooth out steep gradients in the flow field. Stamou and Katsiris [12 ] studied the suita bility of SST k model for numerical simulation of indoor air conditioning and compared it with laminar and k turbulence models, by use of CFX, a commercial CFD code. Already available e xperimental results on displacement ventilation were used to rate the suitability of all these models. They

PAGE 24

24 showed that an SST model with a suitable grid shows the best agreement. The following can be deduced from their paper : a) Of the three main types of CFD methods i.e. Direct Numerical Simulation (DNS), La rge Eddy S imulatio n (LES) and Reynolds A veraged Navier S tokes (RANS), the RANS method was the least computationally intensive b) The standard k model wa s valid only for fully turbulent flows and often fail ed to capture low velocity (especially near wall) re gions. It over estimated the turbulent diffusion. Hence, one must resort to using low Re models such as the RNG k model. Many researchers claim this model to be more stable than any other k model in predi cting indoor airflow simulation c) The low Re number version of the k model wa s claimed to be more numerically stable and it gave faster converged solutions than the corresponding k models. However, its applicability to an indoor environment wa s not suitable due to its strong sensit ivity to free s tream conditions d) The k SST model combined the k model us ing a blending function and used the k model for near wall regions and k model for the rest of the flow e) The Reynolds Stress model (RSM) enabled detection of the presence and the loc alization of separated flow and correctly predicted airflow patterns b ut storage and execution times we re computationally intens ive for 3D indoor flows In the numerical simulation, they made the following assumptions for problem set up: a) A fully implicit coupled solver ( density based) was used b) The diffusers were modeled as velocity inlets c) At the outlet, the average static pressure wa s set to atmospheric and vertical gr adients of all other variables we re set to zero d) They modeled thermal m annequins, PC simulator and lighting simulator to simu late heat loads inside the room They concluded that t here are vertical temperature gradients and negligible horizontal temperature gradients .A steady state solution was not obtained for the standard k k and laminar flow models. Their calculations show ed that all the tested turbulent models predict ed satisfactorily the main qualitative features of the flow and the layered ty pe of temperature fields. Thus, all these models can be used for

PAGE 25

25 practical purposes. Calculations with the SST k based model show ed the best agreement with measurements and the laminar model the worst. Kotani, Yamanaka, Momoi [13 ] carried out 3 D CFD s imulations of airflow in a room with a multi cone ceiling diffuser and validated the results with the measurements obtained from an experimental set up They used a constant temperature hot film anemometer to measure the velocities, turbulent kinetic energ ies and length scales around the diffuser and ultra sonic anemometer to investigate airflow velocities and turbulent kinetic energies in the room. They concluded that a CFD simulation using the measured values as the supply boundary condition in the box me thod can predict the airflow pattern inside the room, except for the decay of axial jet velocity in the heating condition. A summary of their problem set up in, STREAM, Version 4, a commercial CFD code, is given below: a) Standard k turbulence mo del and measured velocities, turbulent parameters were used as boundary condit ions to perform the experiments b) A t hird or der QUICK descritization scheme was used c) The geometry of the multi cone diffuser was to capt ure both radial and axial flows Figure 2 1. Passive chilled beam (adapted from: CPD module [1] )

PAGE 26

26 Figure 2 2. Active chilled beam (adapted from: CPD module [1] )

PAGE 27

27 CHAPTER 3 PROBLEM STATEMENT 3.1 Data Acquisition and Physical Calculations Key input parameters such as the type of chilled beam used, amount of primary air supplied, primary air temperature, sensible cooling capacities, nozzle type, room conditions, water temperature etc were taken from data sheets obtained from Affiliated Eng ineers Inc, Gainesville Branch. The roo m geometry was modeled similar to the model room considered in the chilled beam design guide. The same figure wa s used in the TROX DID 612B HC Active Chilled Beam selection program. For details, refer to th e figure 3 1 The parameters X and A /2 in the figure are both 10ft (3.048m) and the room height is also 10ft (3.048m) The width of the room is considered to be 10ft (3.048m). Hence, the room dimensions 40ft 10ft 10ft (12.192m 3.048m 3.048m ) i.e. 400 sq ft (37.16 sqm) Two Trox DID 612B H C active chilled beams were modeled .The beam units are 6ft long with g type nozzles. The primary airflow rate is 125 cfm In order to find the total airflow rate, the amount of induced air is calculated using the following relations: Where, qcoil =sensible coolin g capacity of the coil=4205 Btuh GPM =chilled water flow rate= 2 GPM T room=room temperature = 74 F (23.3C) T entering chw= chilled water supply temperature=56 F (13.3C)

PAGE 28

28 Using thes e values, the amount of induced air was found out to be Q induced=277.1 cfm Thus the total airflow becomes Q total=Q primary + Q induced=402.1 cfm (0 .19 /s) Thi s 400 cfm of air is being supplied by each beam unit corresponding to 2cfm/ sq. ft. which is typical for laboratory applications. 3.2 Identifying the Ph y s ical Domain and Input Parameters Required Both 2 D and 3 D simulations were performed. The physical domain is the area within whi ch the fluid flow is to be studied, which is the room in the present study. For 2 D numerical simulation s an empty room with the dimensions 40ft 10ft ( 12.192m 3.048 m ) is modeled The present research is focused on the airflow distribution in an empty room. The room is fitted with two active chilled beams and f our light simulators. For the 3 D simulation, the room dimensions are 40ft 10ft 10ft ( 12.192m 3.048m 3.048m) Lights are e ach 4ft 1ft ( 1.2192m 0.3048m ) (l w) The beam unit is 6ft long and for the rest of the dimensions are as shown in the Figure 3 2 Input parameters required: Total airflow through each beam unit: 402 cfm (0.19 /s ). The heat emitted by each tube light i s 33 Figure 3 1. Room air velocity and temperatures parameters used in the design (adapted from: chilled beam design guide [14] )

PAGE 29

29 Figure 3 2 Schematic showing the location of lights and the air conditioning unit

PAGE 30

30 CHAPTER 4 CFD SIMULATION OF TE ST ROOM The re are several commercial CFD software packages in the market. The University of Florida maintains a license for FLUENT 6.3.26 from Fluent Inc. Hence this software was employe d for the present research. It has already been tried and tested in the field of indoor air conditioning 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 Navier 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, making it suitable for indoor airflow simulation The fluid flow solver, FLUENT provides solutions for incompressible / compressible, steady state / transient, laminar / turbulent single phase fl uid flow in complex geometries. 4.1 Steps Involved In the Simulation Process T he outline of the simulation process is summarized as follows: a) Pre processing Model ing the geometry and the flow domain Establish ing the boundary and initial conditions Mesh generation b) Solving Reading the mesh file and grid check Establish ing the s imulation strategy Establish ing the input parameters and files Perform ing the simulation Monitor ing the simulation for convergence c) Post processing Post process ing the simulation to get results gr aphs, plots, contour plots etc.(this will be dealt in the next chapter)

PAGE 31

31 4.1.1 Pre p rocessing For modeling the geometry, GAMBIT 2.4.6 software is used. It is a general purpose pre processor for CFD analysis which provides meshing capabilities wherein the model can be meshed and subsequently imported into FLUENT and solved. GAMBIT is designed for the creation of high quality computational meshes. Predefined grid topology templates are used to minimize grid setup time and optimize the m esh for the given application. GAMBIT enables the user to generate computationa l grids quickly through the automatic management of grid topology and grid attachment. Modeling p rocedure ( approximation and simplification of geometry ) In numerical simulations, approximations of the geometry and simplifications may be required in an analysis to ease the computational effort Especially, for the case of indoor air simulations, it is very difficult to model the diffusers, nozzles, vents etc of the air conditioning unit because these are much smaller compared to the room dimensions and a lso because of their complicated geometry It increases the computational effort because of the increased number of nodes and meshed elements making the problem set up complicated. Srebric and Chen said user should not be afraid of making assumption s. Good assumptions can simplify the complex physical phenomena in the real world with negligible effect on the accuracy of the [2] Keeping this in mind, t he inlets and the induction unit of the chilled beams were modeled as flat, plane ope nings through which the fluid flows at an angle set by the actual geometry of the chilled beam unit. 2 D modeling T he room dimensions are 40ft 10ft ( 12.192m 3.048m ) The chilled beam units and light simulators were modeled as edges along the ceiling of the room.

PAGE 32

32 All the edges forming the room boundary we re defined as a single face. This model wa s saved as .dbs file. Mesh g eneration T he entire face 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 (more elements) the better is the scope for analysis since it gives us more number of points to st udy the behavior of parameters. In GAMBIT, the 2 D mesh elements can be of two types namely Triangular and Quadrilatera l. Use of triangular element creates an unstructured mesh whereas; the use of a quadrilateral element creates a structured mesh. To create a mesh, either the element count (number of elements) or the element size can be specified. Gambit also provides us w ith size functions which allow us to control the size of mesh element edges for the geometric edges and for faces or volumes that are meshed. Since an empty room is considered with no complex structures such as thermal mannequins or pc simulators, a unifor m structured mesh of 0 .02m was employed. Establishing the boundary c onditions O nce the mesh is generated, various edges of the grid are given names for easy understanding and for setting the appropriate boundary conditions while solving. The continuum type (fluid/solid) is also specified. Finally this meshed model is exported as .msh file in a format that can be directly into FLUENT. 3 D m odeling T he room dimensions are 40ft 10ft 10ft ( 12.192m 3.048m 3.048m ) The chilled beam units and light simulator s were modeled

PAGE 33

33 as faces along the ceiling of the room. All the faces forming the room boundary are stitched to form a single connected volume This model wa s saved as .dbs file. Mesh g eneration 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. In GAMBIT, the 3 D mesh elements can be of two types na mely Tetrahedral (unstructured) and Hexagonal (structured) In the present model, a uniform structured mesh of 0 .15 m has been used for meshing the face. Establishing the boundary c onditions O nce the mesh is generated, various faces of the domain are given names for easy understanding and for setting the appropriate boun dary conditions while solving. The continuum type (fluid/solid) is also specified. Finally, this meshed model is exported as .msh file in a format that can be read directly into FLUENT. A schematic of the boundary conditions used is shown in the figure 4 2 4.1.2 Solving Solving is an important phase in CFD analysis. The software used for solving in the present study is FLUENT6.3.26. The .msh file is read into FLUENT and a routine grid check is performed to detect the presence of any skewed cells. Skewness 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 destabilize the solution. These skewed cells can be weeded out either by use of smooth/swap grid opt ion in FLUENT or by re meshing the model in GAMBIT .Then, we may proceed to setting up the problem. Establishing the simulation s trategy T o perform the simulation, we must lay out some rules that affect the physics of the problem. The problem is then set up based on

PAGE 34

34 these under lying assumptions. The present study is based on the following assumptions: a) Incompressible fluid flow and finite volume approach b) Steady state summer air conditioning simulation of the room environment c) Negligible buoyancy effects d) Negligible air leakage t hroughout the conditioned space e) Negligible solar radiation and internal heat sources f) Semi Implicit Method for Pressure Linked Equations ( SIMPLE pressure velocity coupling) g) Negligible radiation and species transport h) Room boundari es were modeled as adiabatic walls i) Two solvers are available in FLUENT namely: j) Pressure based (Segregated) solver k) Density based (Coupled) solver The pressure based solver is used for low speed incompressible flows while the density based solver is used fo r high speed compressible flows, where the velocity and pressure are strongly coupled (high pressures and high velocities) The indoor airflow simulation falls under the category of low speed incompressible flow which can be deduced fro m extensive literatu re survey .The air velocities at th e inlets, also indicate the same. Thereby, in the present study a pressure based solver has been employed. In this method, governing equations are solved sequentially (i.e. segregated from one another). Because the govern ing equations are non linear, several iterations of the solution loop must be performed before a converged solution is obtained. Once the grid is checked, the pressure based implicit solver is applied.

PAGE 35

35 Viscous m odel T he following turbulence models are applicable to indoor air flow analysis: a) k epsilon b) k omega The k epsilon (k equation turbulence model for industrial applications. The model computes the Reynolds stresses by solving two transport equations: one for the turbulent kinetic energy and one for the rate of computational resources and gives a solution of good accuracy. Just like the k models, the k model computes the Reynolds stresses by solving two transport equations: one for the turbulent kinetic energy and one for the specific dissipation rate, wh turbulent viscosity is then calculated as a function of k and The major difference in performance between the k models and the k models is found in the fact that the k models are primarily valid for turbulent core flow (i.e., flow in regions relatively far from walls) whereas the k models are created to be applicable through the boundary layer close to the wall. There exists one variant of the standard k model in FLUENT: the SST (Shear Stress Transport) k model. This model combines the features of the standard k and the standard k model by using the former for the flow somewhat far away from walls and the latter when modeling the flow close to a wall. It uses slightly greater computation al resources than k epsilon but gives a solution of better accuracy as it also includes the boundary layer for mation effects in the solution. Reynolds stress

PAGE 36

36 model uses seven equations and require 50 % to 60 % greater computational resources than k omega. It gives a solution of the highest accuracy among the solvers mentioned above. T he k epsilon solver was chosen for the analysis over k omega as it captures the effects of swirl flows effectively. FLUENT provides three k epsilon models: a) Standard b) RNG(Renormalizing Group Theory) c) Realizable To make the most appropriate choice of model for our application, we need to understand the capabilities and limitations of the various options. The choice of turbulence model will depend on considerations such as the physics encompassed in the flow, the established practice for a specific class of problem, the level of accuracy required, the available computational resources, and the amount of tim e available for the simulation. Among these models, the k epsilon Re alizable has the latest additions which include new formulation for turbulent viscosity and a new transport equ ation for the dissipation rate. Hence, t o treat turbulence near the air supply, realizable k turbulence model is employed with standard wall treatment option enabled. However, it will be interesting to see the performance of other turbulence models in terms of convergence time, solution predic tion and higher order accuracies. Hence, the standard and RNG k Establishing t he input p arameters (material properties, boundary conditions definition) T he fluid inside the room is air with the default proper ties as defined in the FLUENT library of materials. The boundary conditions employed in this model can be grouped into three categories:

PAGE 37

37 Mass flow inlet: The inlets of the chilled beam unit have been defined as mass flow inlets with a direction set by the actual geometry of the chilled beam. The air flow comes out through the slot diffusers at an angle of 32.47 with respect to normal with a discharge of 402 cfm through each beam unit. The air inlet temperature was taken to be 57 F (287K ). Pressure outlet: Zero pressure and zero gradient for all other flow parameters were used as boundary conditions for the exhaust and the induction unit. The air leaving the room was assumed to be at room temperature i.e. 74 F (296K ) Wall: the lig ht simulators and the room were defined as adiabatic walls. The room walls were set to a temperature of 80 F (300K ). The lights were given a heat flux corresponding to a heat flow of 3 3 4.2 Setting the Solution C ontrols and O btaining a Converged Solu tion A summary of the options set in FLUENT is included in tables 4 1 through 4 5. The rest of the options were all set to default. With these settings and boundary conditions, the solution was initialized and iterated till convergence. Iteration consists of the following steps: a) Fluid properties are updated, based on the current solution. And if the calculation has just begun, the fluid properties will be updated ba sed on the initialized solution b) Three momentum equations are solved in turn using current value of the pressure and face mass fluxes, in ord er to update the velocity field c) The velocity obtained in first step may not satisfy the continuity equation locally. A Poisson type equation for the pressure correction is derived from continuity equation a nd the linearized momentum equation. This pressure correction equation is then solved to obtain the necessary corrections to the pressure and velocity fields and the face mass fluxes su ch that continuity is satisfied

PAGE 38

38 d) When interface coupling is to be includ ed, the source terms in the appropriate continuous phase equations may be updated with a discrete phase trajectory calculation e) A check for convergence of the equation set is made Above steps re occur until convergence criterion is achieved. 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 of conti nuity, momentum, energy, k and which indicate that a certain level of convergence has been achieved. 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 ze ro value that, under normal circumstances, decreases as the solution progresses. If the residuals for all problem variables fall below the conve rgence criteria but are still declining the n the solution is still changing to a greater or lesser degree. A be tter indicator occurs when the residuals flatten in a traditional residual plot (of residual value vs. iteration). This point, sometimes referred to as convergence at the level of machine accuracy, takes time to reach and sometimes may be beyond what is ne eded. For this reason, the convergence is said to be achieved when all the residues fall below the order of a micro level ( 10 6 ) .A lternative tools such as reports of mass balances have also been employed A mesh convergence study was performed to arrive a t an optimal mesh size, such that the results do not change by an appreciable amount even after further reduction in mesh size. For details, refer to appendix B.

PAGE 39

39 Table 4 1. Solver settings for 2 D simulation Feature Status Space 2D Formulation Implicit Time Steady Energy equation Enabled Viscous Realizable k model, standard and RNG k model. Near wall treatment Standard wall functions Viscous heating Disabled Table 4 2. Solver s ettings for 3 D simulation Feature Status Space 3D Formulation Implicit Time Steady Energy equation Enabled Viscous Standard k model. Near wall treatment Standard wall functions Viscous heating Disabled Table 4 3 Descritization scheme for 2 D simulation Variable Discretization scheme Pressure Standard Momentum Second Order Upwind Turbulent kinetic energy Second Order Upwind Turbulent dissipation rate Second Order Upwind Energy Second Order Upwind Pressure velocity coupling Simple Table 4 4 Descritization scheme for 3 D simulation Variable Discretization scheme Pressure Standard Momentum First Order Upwind Turbulent kinetic energy QUICK Turbulent dissipation rate QUICK Energy QUICK Pressure velocity coupling Simple Note: Because of limited computational resources, only first order discretization scheme was employed for solving momentum equation while third order QUICK scheme was used for the rest in the 3 D simulation.

PAGE 40

40 Table 4 5. Under relaxation factors for both 2 D and 3 D simulations Variable Relaxation factor Pressure 0.3 Density 1 Body forces 1 Momentum 0.7 Turbulent kinetic energy 0.8 Turbulent dissipation rate 0.8 Turbulent viscosity 1 Energy 1 Figure 4 1. Schematic showing the boundary conditions employed ; Info: co ordinates x=0 40ft; y=0 10ft; z=0 10ft

PAGE 41

41 CHAPTER 5 RESULTS AND OBSERVATIONS Post p rocessing The data obtained from iterations carried out in FL UENT is analyzed in this chapter Since the primary objective of this study was to focus on the airflow distribution inside the room, the vectors of air velocity and temperatures are plotted along with a few remarks and observations ab out the simulation. 5.1 Remarks and Observations a) First order descr itization scheme was used initially .It was not ed that the RNG k model took the longest time to give a converged solution( 4338 iterations),while the standard and realizable models converged after 1100 and 1700 iterations respectively. Similar phenomenon was observed by Jelena et al [2] b) The simulation was performed on an Intel core 2 Duo CPU T6500 6.1 GHz processor 4GB RAM desktop. It took almost about 30 hrs of computational time to reach a 3 D first order converged solution. c) The first order descritization schemes are often inaccurate in predicting the actual physics of the problem and can be used only as an initial solution. Hence second order schemes were employed for 2 D simulation whereas only first order scheme was used for 3 D simulation because of limited computational resources. Both standard and realizable turbulence model simulations using second order descritization scheme were made. The RNG model failed to provide a converged solution with the present mesh. The realizable model conv erged to a greater extent than compared to a standard model. d) There is a considerable difference in the velocity and temperature distribution predicted by the standard and realizable models. e) The realizable model depicts two uniform vortices in the left half of the room portion while the standard model depicts a single large vortex in that portion. f) The plot of static temperature across the room shows that there is a horizontal gradient in temperature across the room with a realizable k simulation while the standard k uniform temperature distribution inside the room. g) The path lines predicted by a 2 D realizable model show a small vortex region forming between the inducer and the return which is absent in a standard model simulation.

PAGE 42

42 5.2 Simulation Results 2 D Standard k The Figure s 5 1 through 5 5 show the air velocity and temperature distribution inside a 2 D room with a standard k model. The standard model gave quicker num erical results when compared to the rest of the models. A single large vortex in the left half of the room can be noticed while a stagnant region can be observed in the top right portion of the room near the inducer and the exhaust A part of the stream go es through the inducer while the rest goes out through the exhaust/return. There is an almost uniform temperature distribution inside the room even though the colored visuals of temperature gradient may indicate otherwise. The temperature scale in the imag e shows that most of the room is at 288 K. As one moves to the right, the temperature is in the higher range of 288 K. This minute variation in temperature can only be detected through numerical simulations and may not be detected at all in experimental re sults. Hence, one might say that there is an almost uniform temperature distribution inside the room. The F igure 5 5 shows the plot of velocity magnitude of airflow inside the room with a standard k 1.7 m from the bottom of the room. T he velocity magnitude at locations 1 and 2 can be obtained from this plot which will later be used for validation of the results. The maximum velocity in the occupied zone was found out to be 96 fpm. 2 D Realizable k The Figu res 5 6 through 5 7 show the air velocity and temperature distribution inside a 2 D room with a realizable k model. T wo uniform vortices in the left half of the room can be noticed (as against a single large vortex with a standard model) while a stagnant region can be observed in the top right portion of the room near the exhaust. The path lines indicate a small vortex region formation between the inducer and the exhaust. A horizontal gradient in

PAGE 43

43 temperature (288 289 K) can be noticed This gradient in te mperature is again very small even though the colored visuals of temperature gradient may indicate otherwise. The temperature scale in the image shows that most of the room is at 288 K. As one moves to the right, the temperature is in the higher range of 2 88 K and 289K. This minute variation in temperature can only be detected through numerical simulations and may not be detected at all in experimental results. The Figure 5 10 shows the plot of velocity magnitude of airflow inside the room with a realizable k m from the bottom of the room. The velocity magnitude at locations 1 and 2 can be obtained from this plot which will later be used for validation of the results. 3 D Standard k turbulence model simulation The Figures 5 11 thr ough 5 17 show the air velocity and temperature distribution of airflow inside a room with a standard k The path lines of air velocity indicate that the flow comes out through the diffusers and leaves through the induction unit and the exhaust/ret urn. The flow comes out the through the diffuser, hits the wall and cascades down along the wall. The flows coming from two opposing chilled beam nozzles meet at the mid section of the room; they reinforce and cascade down to form a vortex of cold air whic h effectively cools the room. The air then moves to the rest of the room and part of it goes through the inducer where it is re treated and sent back into the occupied space while the rest of it exits through the return/exhaust. The air velocity in the occ upied zone is less than 60 fpm An almost uniform temperature distribution can be noticed except for the ceiling where heat sources and diffusers are located

PAGE 44

44 Figure 5 1 Velocity vectors of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y a xis: height of the room (0 3.048m) ; 2 D Standard k Turbulence Model Simulation Figure 5 2. Temperature of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; 2 D Standard k T urbulence Model Simulation

PAGE 45

45 Figure 5 3. Path lines showing the velocity magnitude of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; 2 D Standard k Turbulence Model Simulation Figure 5 4. Path lines showing the temperature of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; 2 D Standard k Turbulence Model Simulation

PAGE 46

46 Figure 5 5 Plot of velocity magnitude (at a height of 1.7 m) across the room ; Info: X axis: l ength of the room (0 12.192m); Y axis : velocity magnitude of airflow inside the room (0 0.6 m /s ) ; 2 D Standard k Turbulence Model Simulation Figure 5 6 Velocity vectors of airflow inside the room ; Info: X axis: length of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; 2 D Realizable k Turbulence Model Simulation

PAGE 47

47 Figure 5 7 Temperature of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m) ; Y axis: height of the room (0 3.048m) ; 2 D Realizable k Turbulence Model Simulation Figure 5 8 Path lines showing the velocity magnitude of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; 2 D Realizable k Turbulen ce Model Simulation

PAGE 48

48 Figure 5 9 Path lines showing the temperature of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; 2 D Realizable k Turbulence Model Simulation Figure 5 10 Plot of velocity magnitude (at a height of 1.7 m) across the room ; Info: X axis: l ength of the room (0 12.192m); Y axis : velocity magnitude of airflow inside the room (0 0.7 m /s ) ; 2 D Realizable k Turbulence Model Simulation

PAGE 49

49 Figure 5 11 Velocity vectors of a irflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; Z axis: width of the room (0 3.048 m); 3 D Standard k Turbulence Model Simulation Figure 5 12 Temperature of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; Z axis: width of th e room (0 3.048 m); 3 D Standard k Turbulence Model Simulation

PAGE 50

50 Figure 5 13 Path lines showing the velocity magnitude of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; Z axis: width of the r oom (0 3.048 m); 3 D Standard k Turbulence Model Simulation Figure 5 14 Path lines showing the temperature of airflow inside the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; Z axis: width of the room (0 3.04 8 m); 3 D Standard k Turbulence Model Simulation

PAGE 51

51 Figure 5 15 Velocity vectors of airflow (at the lateral mid section) across the room ; Info: X axis : l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; Z axis: width o f the room (0 3.048 m); 3 D Standard k Turbulence Model Simulation \ Figure 5 16 T emperature of airflow (at the lateral mid section) across the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: height of the room (0 3.048m) ; Z axis: width of th e room (0 3.048 m); 3 D Standard k Turbulence Model Simulation

PAGE 52

52 Figure 5 17 Plot of velocity magnitude of airflow (at the lateral mid section) across the room ; Info: X axis: l ength of the room (0 12.192m); Y axis: velocity magnitude of airflow inside the room (0 0.7 m /s ) ; 3 D Standard k Turbulence Model Simulation

PAGE 53

53 CHAPTER 6 VALIDATIONS This chapter contains information about the data obtained fro m numerical simulations and TROX selection program which are then compared with each other to validate the numerical model. The accuracy of the physics depicted by a numerical simulation is predicted by comparing the results obtained from the simulation with already a vailable standard results present in the form of a) experimental data or b) numerical results from a reliable source or c) empirical data. In the present case, because of lack of experimental data, the results are validated with the data obtained from TROX DID 612B HC active chilled beam calculation (version 1.1) which is a sp readsheet downloadable from TROX website. The spreadsheet provides information regarding the velocities at certain locations inside the room which is believed to be empirical data. The data used for validation of the p resent results is shown in the F igure 6 2 From the spread sheet, the velocity values at locations 1 and 2 (denoted as L and H 1 by TROX) are supposedly V 1 =104.2 fpm V 2 =98.3 fpm From the velocity plots shown in figure 5 .5 and 5.11, the velocity magnitude at locations 1 and 2 predicted by the standard and realizable k Standard k V 1 = 0.488 m/s =96.2 FPM V 2 = 0.483m/s =95.2 FPM

PAGE 54

54 Realizable k V 1 =0.605 m/s= 118 FPM V 2 = 0.48 m/s=94 .5 FPM T hese results are summarized in the table 6 1. Table 6 1. Parameters V 1 and V 2 predicted by various models Parameter Empirical model Standard model Realizable model V 1 (fpm) 104.2 96.2 118 V 2 (fpm) 98.3 95.2 95.2 Table 6 2. Error in prediction of V 1 and V 2 by the turbulence models Parameter Standard model Realizable model V 1 (% error) 7.67 13.24 V 2 (% error) 3.15 4.02 Figure 6 1. Locations showing the points of interest where the data is to be compared (adapted from: chilled beam design guide [14] )

PAGE 55

55 Figure 6 2 TROX active chilled beam calculation program

PAGE 56

56 CHAPTER 7 CONCLUSIONS AND RECO MMENDATIONS 7.1 Conclusions a) The velocity parameters (V 1 and V 2 ) predicted by the standard k turbulence model match closely with those of the 2 D empirical model with an error of about 7% for V 1 and 3% for V 2 b) The velocity parameters (V 1 and V 2 ) predicted by the realizable k turbulence model match with those of the 2 D empirical model with an er ror of about 13% for V 1 and 4% for V 2 c) Based on the above figures, it seems that the standard model which is actually a realizable model ,which is a more refined k turbulenc e model intended to suit a variety of practical turbulent flow cases d) The Laminar model failed to give a converged solution for both the two dimensional as well as the three dimensional simulation. This makes sense because most of indoor airflow problems fall under the turbulent regime. Similar phenomenon was observed by Stamou et al [12] e) There is an almost uniform temperature distribution inside the room with a horizontal temperature gradient of about 1.8 F (1 K) across the room with activ e chilled beam air conditioning f) The 3 D simulation shows that the velocity across the occupied zone is less than 60 FPM and that the roo m temperature is almost uniform g) Based on 2 D simulations, an attempt has been made to compare the performance in terms of air velocitie s and temperature distribution inside the room for a conventional multi cone diffuser and an active chilled beam. It may be concluded that the chilled beam provides a more uniform temperature distribution. (For details refer to Appendix B) h) The air velocit ies with an active chilled beam are higher than those observed with a multi cone diffuser which should results in a quicker response to changes in heat load (For details refer to Appendix C)

PAGE 57

57 7.2 Recommendations for Further Studies a) Unsteady state s imulat ions can be performed to capture the dynamic variation of velocity and temperature inside the room b) The present study is focused on an empty room and neglects buoyancy effects .However, it will be interesting to simulate a real life laboratory by placing ob structions (desks and chairs) and heat sources (like computers, people, burners etc.) and see how the airflow gets affected due to the presence of these factors c) There is a lack of lack of experimental data for comparisons to validate the results obtained f rom 3 D simulation. Also, it would be unfair to say that the standard model predicts the actual physics of the problem better than the realizable model just based on two data points because the actual flow field depends on a lot of parameters such as prese nce of obstructions, location of the return etc and the overall airflow may be a lot different Hence, experimental studies may be conducted to check the validity of the present numerical model and also to determine the correct tur bulence model which best s uits the present case d) Experimental studies may also be performed to check if the active chilled beams provide faster cooling than the multi cone diffusers e) Significant efforts were made to simplify the modeling of the chilled beam unit. Each of these trials are listed below which may be helpful fo r future research on this topic Trial 1: The first case involved modeling the actual geometry of the chilled beam, which resulted in a complex grid (unstructured mesh) and this also could not provide a converged sol ution. It requires a lot of computational intensity and time. Trial 2: The geometrical modeling of the chilled beam unit was simplified using a flat diffuser model i.e. modeling the geometry of the beam unit by identifying the mass flow inlet and exit port ions as flat openings on the ceiling. However, this must follow the wall) i.e. Instead of the jet diffusing out from the inlets and cascading down from the walls, it" hit the f loor and came towards the ce iling in the opposite direction Trial 3: The third and final model assumed the same flat opening as the one in the second trial. But this time, the boundary conditions were specified so as to make the airflow eject at an angle s et by the actual geometry of the beam unit. This reduced the computational intensity because of the luxury of being able to use a uniform structured mesh and also lead to good agreement with the coanda effect i.e. the air diffused out from the vents and casca ded down the walls

PAGE 58

58 APPENDIX A SOLID ROOM AND MESHE D GEOMETRIC MODELS Figure A 1 Isometric view of the room model showing the gradient in x direction Figure A 2 Isometric view of the meshed room model

PAGE 59

59 Figure A 3 Top View of the solid room model obtained from gambit Figure A 4 Isometric view of the solid room model obtained from gambit

PAGE 60

60 Figure A 5 Isometric view of the meshed room model obtained from gambit

PAGE 61

61 APPENDIX B MESH CONVERGENCE STU DY In any numerical study, it is important that we use a sufficiently refined mesh to ensure that the results obtained are accurate. Coarse meshes can yield inaccurate results in analyses. The numerical solution provided by the model tends to a unique solution as we increase the mesh density. But, a fi ner mesh also leads to an increase in computational resources required. The mesh is said to be refined when further mesh refinement produces a neg ligible change in the solution. Hence a mesh convergence study has been performed on the present 2 D model to determine the accuracy of the results. Since the primary focus is on velocity, the velocity magnitudes U 1 U 2, U obtained from various mesh sizes will be compared to arrive at an optimum mesh size (Refer to Table B 1). Where, U1= sum of all the velociti es at a certain section across the room U2=square root of summation of square of all the velocities at a certain section across the room ( ) U =Maximum velocity of all the velocities at a certain section across the room (U max) Four grids starting from .025m mesh edge length have been generated for the 2 D geometric model of the room and FLUENT runs have been conducted for the same case on these meshes. The velocity vectors at a certain section across the room were taken and the parameters U1, U2 and U were determined for each mesh. These velocities were then plott ed to check it they flatten out (Refer to Figure B 1).

PAGE 62

62 It can be deduced from the plot that after the 0 .02m mesh element length, the curve tends to flatten out for U 2 and U but the U1 is increasing. Hence, the 0 .02m mesh element edge size was chosen for this analysis as it is evident from the above table that there is not much change in the results for mesh element length less than the 0 .02m. Above decision was arrived at, t aking into consideration the time taken for the FLUENT runs and the accuracy of the results. Hence the 0 .02m mesh can be considered as a fine mesh for the present analysis Table B 1 Comparison of the effect of grid on solution Parameter 0 .025m mesh 0 .02m mesh 0 .018m mesh 0 .015m mesh U 1 3.370573 3.606919 3.704887 3.803583 U 2 0.919054 1.007596 1.029458 1.052654 U 0.478278 0.501668 0.51048 0.531936 Figure B 1 Plot of velocity parameters as the mesh density varies

PAGE 63

63 APPENDIX C COMPARISION WITH A MULTI CONE DIFFUSER For performing the 2 D numerical simulation of a room fitted with a multi cone diffuser, the box method suggested by Kotani et al [13] was used with Standard k turbulence modeling and third order QUICK discretization scheme. The same mass flow as that used for the active chilled beams was used for the simulation for proper comparison. Remarks and Observations a) From the numerical results, it may be deduced that the maximum velocity of airflow inside the 2 D room model with a multi cone diffuser is about 60 fpm whereas that with an active c hilled beam is about 90 100 fpm b) There is an almost uniform temperature distribution inside the room with an active chilled beam c) The portion of the room directly below the multi cone diffuser is cooler t han the other portions of the room d) Experimental studies on a multi cone diffuser and an active chilled beam unit may be performed for having a better understanding of the airflow properties for a fair comp arison between these two models Figure C 1 Front view of the meshed 2 d room model fitted with a multi cone diffuser

PAGE 64

64 Figure C 2 Velocity vectors of airflow inside the room Figure C 3 Temperature of airflow inside the room

PAGE 65

65 Figure C 4 Plot of velocity magnitude of airflow (at a height of 1.7m) acros s the room

PAGE 66

66 LIST OF REFERENCES 1. Dwyer T., and Staunton, J., chilled beams and integrated service modules alternative approaches to cooling CPD Collection SAS International, 11, 89 92 2. Srebric, J. and Chen, Q. examp le o f verification, validation, a nd re porting of indoor environment CFD ASHRAE Transactions 108(2), 185 194 3. Zhu, L., Li, R., and Yuan, D., 2006. analysis of a cold air distribution system HVAC Technologies for Energy Efficiency Vol.IV 2 3 4. Abanto, J., Barrero, D., Reggio, M., and Ozell B., 2004. A irflow modeling in a computer room Building and Environment 39, 1393 1402. 5. Awbi, H., 1989. A pplications of computational fluid dynamics in room ventilation Building and Environmen t 24(1), 73 84 6. Melikov, A., Yordanova, B., Bozkhov, L., Zboril V., and Kosonen, R., 2007. Impact o f the airflow in ith active chilled beams The 6th International Conference on Indoor Air Qua lity, Ventilation & Energy Conservation in Buildings IAQVEC 2007 Sendai, Japan 7. Kosonen R., Saarinen P., Koskela H., and Hole, A., 2010 Impact of heat load location and strength on air flow pattern with a passive chilled beam system International Conference on Building Energy and Environment COBEE2008 Vol.42 ( 1), 34 42. 8. Cammarata G and Petrone G 2008. A numerical investigation on active chilled beams for indoor air conditioning COSMOL Conference Hannover. 9. True, J., Zboril, V., Kosonen, R., and Melikov, A., 2007 Consideration for minimizing draught discomfort in rooms with active chilled Proceedings of Clima 2007 Wellb eing Indoors 10. Posner, J., Buchanan, C., and Rankin, D., 2003 and prediction of indoor a ir flow in a model room Energy and Buildings Vol. 35 (1) 515 526 11. Z boril V., Bozhkov, L., Y ordanova B., Melikov A., and Kosonen R., 2006. Airflow distribution in rooms w ith chilled beams 17th Air conditioning and Ventilation Conference Prague, Czech Republic 12. Stamou, A., and Katsiri s L., 2006. Verification of a CFD model for indoor airflow and heat t ransfer Building and Environment 41, 1171 1181

PAGE 67

67 13. Kotani, H., Yamanaka, T., and Momoi, Y., 2002. CFD simulation of airflow in room w i th multi cone ceiling diffuser using measured velocity and turbulent parameters i n large space Proceedings of the 8 th International Conference on Air Distributions in Rooms (RoomVent2002) Copenhagen, Denmark, 117 120. 14. Trox Inc., 2 design guide, USA. 15. Lobscheid, C., and Gadgil A., 2002. Mixing of a point source indoor pollutant: numeric al predictions and comparison w ith experiments Proceedings of Indoor Air2002 Vol.IV 223 228. 16. Cheong, K., Djunaedy, E., Chua, E., Tham, K., Sekhar, S., Wong, N., and Ullah, M., 2003. Thermal comfort study of a n a ir conditioned lecture theatre i n the tropics Building and Environment Vol. 38 (1) 63 73 17. Loomans M., 1998. of indoor air flow Doctoral Thesis, Dep artment of Mechanical Engineering, Eindhoven University of Technology 18. Fredriksson, J., Sandberg, M., Moshfegh, B., 2001. vestigation of the velocity field and airflow pattern generated b y cooling ceiling beams Building and Environment Vol. 36 (7) 891 899 19. ows induced by mechanical ventilation and air conditioning (MVAC) systems Applied Energy Vol. 68 (2) 135 159. 20. Melikov A., Y ordanova B., Bozkhov L., Zboril, V., and Kosonen R., 2007. Proceedings of Clima 2007 Wellb eing Indoors Helsinki.

PAGE 68

68 BIOGRAPHICAL SKETCH Abhijyoth Reddy Vempati was born in 1988 in Vijayawada, India He was brought up in Hyderabad, He is passionate about machines in general and automobiles in pa rticular which made him pursue mechanical e ngineering as his major in under graduate studies. He rec eived his ngineering from the Jawaharlal Nehru Technological University located in Hyderabad in 2009. In fall 2009, he joined the Mechanical and Aerospace Engineering Department at the University of Florida and started wo rking on his dissertation from s pring 2010 under the guidance of Dr.Ingley. Florida in the fall of 2011. H e plans to find a full time position as an engineer in the fields of Engine Manufacturing, Turbo Mac hinery or Thermal Analyses requiring C omputational F luid D ynamics Applic ation and is looking forward to the challenges that await him.