ÇUKUROVA UNIVERSITY INSTITUTE OF NATURAL AND APPLIED ... · Anahtar Kelimeler: Aerodinamik,...

ÇUKUROVA UNIVERSITY

INSTITUTE OF NATURAL AND APPLIED SCIENCES

Ms. Sc. THESIS

Serkan MEZARCIÖZ

AERODYNAMICS OF A MODEL BUS

DEPARTMENT OF MECHANICAL ENGINEERING

ADANA, 2006

ÇUKUROVA ÜNİVERSİTESİ

FEN BİLİMLERİ ENSTİTÜSÜ


Serkan MEZARCIÖZ

MASTER TEZİ

MAKİNA MÜHENDİSLİĞİ ANABİLİM DALI

Bu Tez ..../..../2006 Tarihinde Aşağıdaki Jüri Üyeleri Tarafından

Oybirliği/Oyçokluğu İle Kabul Edilmiştir.

İmza: İmza: İmza:

Prof. Dr. Beşir ŞAHİN Doç. Dr. Hüseyin AKILLI Doç. Dr. Galip SEÇKİN DANIŞMAN ÜYE ÜYE

Bu Tez Enstitümüz Makina Mühendisliği Anabilim Dalında Hazırlanmıştır.

Kod No:

Prof. Dr. Aziz ERTUNÇ Enstitü Müdürü

Not: Bu tezde kullanılan özgün ve başka kaynaktan yapılan bildirişlerin, çizelge, şekil ve fotoğrafların kaynak gösterilmeden kullanımı, 5846 sayılı Fikir ve Sanat Eserleri Kanunundaki hükümlere tabidir.

ABSTRACT

M.Sc. THESIS


Serkan MEZARCIÖZ

DEPARTMENT OF MECHANICAL ENGINEERING INSTITUTE OF NATURAL AND APPLIED SCIENCES

UNIVERSITY OF ÇUKUROVA

Supervisor: Prof. Dr. Beşir ŞAHİN Year: 2006, Pages:67

Jury: Prof. Dr. Beşir ŞAHİN

:Doç. Dr. Hüseyin AKILLI : Doç. Dr. Galip SEÇKİN The ultimate goal of this work is to examine the turbulent, 3D flow around a

bus-shaped body by means of CFD. Another goal of this study is to show the accordance between the numerical and experimental results. In the present study, RANS k-ε turbulence model is employed to simulate the flow around the vehicle, and the results of the experiments performed by PIV are used to validate the corrections of the numerical simulation. A comparison of predicted results for time-averaged flow data, particularly, around the forward face of the model with the experimental results of Particle Image Velocimetry (PIV) showed that numerically predicted present results and experimental results agreed well. The flow is assumed to be incompressible, viscous, turbulent, and steady flow.

Key Words: Aerodynamics, Bus, Reynolds Average Navier Stokes (RANS), k-ε

Turbulence Model

I

ÖZ

YÜKSEK LİSANS TEZİ

BİR OTOBÜS MODELİNİN AERODİNAMİĞİ

Serkan MEZARCIÖZ

ÇUKUROVA ÜNİVERSİTESİ

FEN BİLİMLERİ ENSTİTÜSÜ

MAKİNA MÜHENDİSLİĞİ ANABİLİM DALI

Danışman: Prof. Dr. Beşir ŞAHİN

Yıl: 2006, Pages:67

Juri: Prof. Dr. Beşir ŞAHİN

:Doç. Dr. Hüseyin AKILLI

: Doç. Dr. Galip SEÇKİN

Bu çalışmanın ana amacı hesaplamalı akışkanlar mekaniği aracılığı ile otobüs

şeklindeki bir cismin etrafındaki 3 boyutlu, türbülanslı akışın incelenmesidir. Çalışmanın diğer bir amacı ise deneysel ve nümerik sonuçlar arasındaki benzerliklerin gösterilmesidir. Bu çalışmada araç etrafındaki akışın simülasyonu için k-ε türbülans modeli kullanılmış ve nümerik simülasyon sonuçlarının doğruluğunu teyit etmek için PIV deneylerinin sonuçları kullanılmıştır. Modelin ön yüzünün etrafındaki tahmin edilen akış özellikleri ile parçacık görüntülemeli hız ölçüm deneylerinin sonuçlarının karşılaştırması, nümerik olarak tahmin edilen mevcut sonuçların ve deneysel sonuçların birbirine uygun olduğunu göstermektedir. Akış sıkıştırılamaz, türbülanslı, sürekli kabul edilmiştir.

Anahtar Kelimeler: Aerodinamik, Otobüs, Reynolds Average Navier Stokes (RANS), k-ε Türbülans Modeli

II

ACKNOWLEDGMENT

I would like to express my gratitude to everyone who assisted in this study.

First and Foremost, I would like to thank my supervisor, Professor Beşir ŞAHİN,

who gave me the opportunity, support, and freedom that I needed to conduct this research.

I would like to thank Assist.Prof. Hüseyin AKILLI for his scientific and technical

guidance and his support during my graduate studies.

I would like to thank Tural TUNAY for transferring all his knowledge, for helping in

the study and for his friendship.

I would also like to thank Research Assistant Cahit GÜRLEK for his very useful

comments and experimental support.

I appreciate gratefully the help from my friends, İbrahim PEHLİVAN and

Serin MAVRUZ for their contributions to this project.

Finally, I am greatly indebted to my parents for nurturing and cherishing

my academic endeavors.

III

CONTENTS PAGE

ABSTRACT......................................................................................................... I

ÖZ......................................................................................................................... II

ACKNOWLEDGEMENT……………………………………………………… III

CONTENTS……………………………………………………………………. IV

LIST OF FIGURES ……………………………………………………………. VI

NOMENCLATURE……………………………………………………………. IX

1. INTRODUCTION…………………………………………………………… 1

1.1.Importance of Aerodynamics and Flow Around Road Vehicles………... 1

1.2. Importance of Aerodynamics for Buses………………………………... 10

2. PREVIOUS STUDIES AND SCOPE OF THE PRESENT STUDY……….. 12

2.1. Scope of the Present Study……………………………………………... 21

3. MATERIALS AND METHODS……………………………………………. 22

3.1. Vehicle Geometry and Dimensions…………………………………….. 23

3.2. Determination of Dimensions of the Flow Domain…………………..... 24

3.3. Grid Generation and Refinement Study………………………………... 26

3.4. Boundary Conditions…………………………………………………… 28

3.4.1. Boundary Conditions for Simulations……………………………. 29

3.5. Simulation of the Flow…………………………………………………. 29

3.5.1. Discretization……………………………………………………... 30

3.5.2. Convergence……………………………………………………… 32

3.6. Governing Equations for Fluid Flow…………………………………… 33

3.7. Reynolds Averaged Navier Stokes (RANS) Equations of Motion……... 34

3.8. Overview of Turbulence Modeling…………………………………….. 36

3.9. Turbulence Models……………………………………………………... 37

3.9.1. Time Averaged Turbulence Models……………………………… 37

3.9.1.1. Zero Equation Model……………………………………... 38

3.9.1.2. One Equation Model……………………………………… 38

3.9.1.3. Two Equation Models……………………………………. 39

3.10. Near Wall Treatment………………………………………………….. 44

IV

4. RESULTS AND DISCUSSION…………………………………………….. 46

5. CONCLUSIONS…………………………………………………………….. 60

5.1. Future Studies…………………………………………………………... 62

REFERENCES…………………………………………………………………. 63

CIRRICULUM VITAE………………………………………………………… 67

V

LIST OF FIGURES PAGE

Figure 1.1. An aerodynamically improved truck (MAN)…………………. 2

Figure 1.2. Induced air resistances in the case of a fully faired semi-trailer

outfit……………………………………………………………. 3

Figure 1.3. Induced air flow at the vehicle body…………………………... 4

Figure 1.4. Longitudinal swirls caused by induced draft…………………... 5

Figure 1.5. Air flow through a motor vehicle……………………………… 6

Figure 1.6. Application of Rear Flap to a Truck (MAN, 2004)……………. 7

Figure 1.7. Forces and moments in aerodynamic measurements…………... 8

Figure 1.8. Components of aerodynamic drag in an optimized bus body

(MAN, 2004)………………………………………………….…

9

Figure 1.9. Aerodynamic drag at oblique flow for different passenger cars

(BOSCH, 2002)…………………………………………………. 10

Figure 1.10. An application of rounded corner to a bus (TEMSA Diamond)... 11

Figure 1.11. A bus having sharp corners (TEMSA Tourmalin)……………… 11

Figure 2.1. Geometry of the vehicle body and computational domain used

by Krajnovic and Davidson (2001)……………………………... 15

Figure 2.2 Kinetic energy contours at the centerline (y=0) around the 25º

Ahmed body using the linear k-ε and cubic non-linear k-ε

models with specified Chieng and Launder wall functions Craft

et al (2001)……………………………………………………… 17

Figure 2.3. Geometry of the cube with its channel dimensions ( Krajnovic

and Davidson, 2002b)…………………………………………… 18

Figure 2.4. Schematic representation of the computational domain with

vehicle body (Krajnovic and Davidson, 2004a)……………..... 21

Figure 3.1. The dimensions of the vehicle model…………………………... 23

Figure 3.2. Schematic representation of the computational domain with

vehicle body (Krajnovic and Davidson, 2004a)………………… 24

Figure 3.3. Position of the bus in the channel (side view, dimensions in

mm)…………………………………………….……….………. 25

VI

Figure 3.4. Position of the bus in the channel (cross-sectional view)………. 25

Figure 3.5. 3D view of the computational domain………………………….. 25

Figure 3.6. Distribution of y* values for the grid having 442.496 nodes…... 27

Figure 3.7. Distribution of y* values for the grid having 786.586 nodes…... 27

Figure 3.8. Distribution of y* values for the grid having 1.186.819 nodes… 28

Figure 3.9. Convergence of the residuals to 10-5…………………………… 33

Figure 3.10. Subdivisions of near wall region (FLUENT, 1998)…………….. 44

Figure 4.1. The symmetry planes of the bus model…………………………. 46

Figure 4.2. Time-averaged patterns of experimental streamlines around

forward face of the bus model along the central axis in side view

plane(Gürlek,2006)…………………………………………….. 47

Figure 4.3. Time-averaged patterns of numerical streamlines around

forward face of the bus model in side view symmetry

plane……………………………………………………………. 48

Figure 4.4. Comparison of time–averaged experimental and numerical

patterns of streamlines in plan view planes around the forward

part of the bus model …………………….................................... 49

Figure 4.5. Comparison of time–averaged (a) experimental and

(b)numerical vorticity in plan view planes of forward portion of

the bus model.. ………………………………………………… 50

Figure 4.6. Comparison of time–averaged experimental and numerical

streamlines in plan view planes downstream of the bus model … 50

Figure 4.7. Time-averaged experimental velocity vector map downstream of

the bus model in horizontal symmetry plane……………………. 51

Figure 4.8. Time-averaged numerical velocity vector map downstream of

the bus model in horizontal symmetry plane……………………. 52

Figure 4.9. Time-averaged patterns of streamlines downstream of the bus

model, in side view plane. a: experimental data, b: numerical

data………………………………………………………………. 52

Figure 4.10. Time-averaged velocity vector map in side view symmetry

plane of the bus model……..…………………………………… 53

VII

Figure 4.11. Time-averaged velocity vectors in side view plane in the

forward face of the model………………………………………. 54

Figure 4.12. Time-averaged velocity vectors on the horizontal symmetry

plane near front of vehicle model………………………………. 54

Figure 4.13. Time-averaged velocity vector map in side view symmetry

plane downstream of the model…………………………………. 55

Figure 4.14. Contours of static pressure in the vertical symmetry plane…… 55

Figure 4.15. Contours of static pressure in the vertical symmetry plane near

the top of the model……………………………………………. 56

Figure 4.16. Velocity vectors on the vertical symmetry plane of the vehicle… 56

Figure 4.17. Time-averaged patterns of streamlines and corresponding

various plan views having different heights from the bottom of

the channel as a:Y/H=0.015, b:Y/H=0.045, c:Y/H=0.09,

d: horizontal symmetry plane of the vehicle, ………………….. 57

Figure 4.18. Time-averaged pattern of streamlines and corresponding

distribution of velocity contour in different planes having

different heights from the bottom of the channel as

a:Y/H=0.896, b:Y/H=1,045, c:top of the vehicle,

d:Y/H=1.433…………………………………………………….. 58

Figure 4.19. Planes mentioned in figure 4.17 and 4.18………………………. 58


velocity contour in side view plane……………………………... 59


velocity contour in plan view plane……………………………... 59

VIII

NOMENCLATURE

A surface area (m2)

B Width of the channel

vc specific heat at constant volume

F height of the channel

H Height of thevehicle

FD Drag force

I turbulence intensity (%)

k turbulent kinetic energy (m2/s2)

L length of the vehicle

l characteristic length scale of the turbulent flow

N frame number

p pressure (Pa)

np local pressure (Pa)

∞p free stream pressure (Pa)

q& heat flux

′′− ji uuρ Reynolds (turbulent) stress

jq− Reynolds (turbulent) heat flux

jq filtered heat flux

Pr Prandtl number

tPr turbulent Prandtl number

R specific gas constant

Re Reynolds number

S strain rate magnitude

T flow time (sec)

T temperature (K)

iu time averaged (mean) velocity components in the yx, and direction z

iu′ fluctuating velocity component in the yx, and direction z

IX

∞U free stream velocity (m/s)

iu velocity components ( for wvu ,, =i 1, 2 and 3 respectively)

ix independent space coordinates ( zyx ,, for =i 1, 2 and 3 respectively)

V volume of a computational cell (m3)

cw frequency (rad/s)

X non-dimensional x -distance ( DxX /= )

X1 Distance between inflow and model front face

X2 Distance between outflow and model back face

fX projected fin pattern length

Z non-dimensional −z coordinate ( sz /= )

Greek Symbols

ρ fluid density (kg/m3)

α thermal diffusivity (= )/( pCk ρ )

P∆ pressure drop

ν kinematic viscosity (m2/s2)

tν turbulent kinematic viscosity (m2/s2)

τ non-dimensional time (= ) sUt /

ε turbulent dissipation rate (m2/s3)

∆ averaged grid size

β frequency parameter

µ viscosity, kg/(ms)

tµ turbulent (eddy) viscosity

effµ effectivite viscosity ( teff µµµ += )

ijτ Reynolds stress tensor or SGS stress term or filtered stress

ϑ characteristic velocity of the turbulent flow

X

λ a second viscosity related to the dynamic viscosity )32( µλ −=

ϕ a flow property

Φ)

filtered variable

θ corrugation (wavy) angle (º)

κ von Karman constant

φ cell centered value of a flow variable (field variable)

ω time average square of the vorticity fluctuations

η ratio between the characteristic time scales of turbulence and mean flow field

subscripts

in at the inlet

w in the wall

exit at the exit

av average

crit critical

∞ free stream value

superscripts

* non-dimensional value

‘ fluctuating component

^ filtered variable −

time averaged (mean component)

XI

1.INTRODUCTION Serkan MEZARCIÖZ

1. INTRODUCTION

1.1. Importance of Aerodynamics and Flow Around Road Vehicles

Aerodynamic structure and the flow around the road vehicles have been

investigated for a long time. Significance of the aerodynamics is obvious, since it

affects the fuel consumption, wind noise, and vibration.

The complexity of the structures in this three dimensional flow makes

experimental studies very difficult. Furthermore experimental studies often provide

only information on some limited partition of the flow. (Point, line or a plain).

Computational Fluid Dynamics (CFD) gives a description of the flow in the entire

computational domain (Numerical Wind Tunnel) (Krajnovic and Davidson , 2002a).

The drag forces of importance to the vehicle designer are dominated primary

by the wake forces. Thus the prediction of the pressure coefficient at the rear of the

vehicle is of great importance. Although the RANS simulations have been successful

in predicting many parts of the flow around the vehicles, they have failed to predict

the effects of the unsteady wake on the body. It is believed that an unsteady

simulation such as Large Eddy Simulation (LES) will have greater success than

RANS in predicting the pressure at the rear of the vehicles and give better insight

into the flow around these bodies (Krajnovic and Davidson, 2001: Howard and

Pourquie, 2002).

Good aerodynamics is becoming more and more important, even for

commercial vehicles, as fuel prices rise. The characteristic value that describes the

air resistance is the drag coefficient (CD). Low CD values indicate low drag and allow

a higher terminal speed and lower fuel consumption. The air resistance and flow

characteristics around vehicle can be determined in a wind tunnel experiments or

Computational Fluid Dynamics (CFD) analysis. In this study a CFD analysis with a

Reynolds Average Navier Stokes (RANS) and k-ε turbulence model will be

employed in stead of experimental study.

As the speed of a vehicle increases, so does its drag. The increase in drag is as

the square of the speed, as can be seen from the formula of the drag force FDRAG

1


2...21. VACF DDRAG ρ= ( 1.1)

Where, CD :Coefficient of drag

ρ :Density of fluid

A :Cross-sectional area exposed to the flow

V : Velocity

Most of the vehicle manufacturers are focusing on the subject of

aerodynamics and they are making some researches to improve the aerodynamic

structure and gain lower CD values. (See Figure 1.1).

Figure 1.1. An aerodynamically improved truck (MAN)

Here are some examples of the researches;

Development of Truck and Bus Aerodynamics using Computational Fluid

Dynamics (Takeuchi and Kohri, 1997).

Aerodynamic Simulations by Using Discontinuous Interface Grid and

Solution Adaptive Grid Method (Uchida et al., 1998).

2


Development of Rear Spoiler for Hatchback Vehicles using Concurrent CFD

Method (Yamane et al., 1999).

The total drag of a vehicle is made up of the following components:

Pressurized-air resistance and induced air resistance, Surface air resistance, and

internal air resistance.

The induced air resistance is caused by the differences in air pressure that

arise between the top and bottom of the vehicle as it moves along Figure1.2.

Together, the pressurized-air resistance and the induced air resistance make up the

majority of the total drag, accounting for some 50-90 %.

Figure 1.2. Induced air resistances in the case of a fully faired semi-trailer outfit

Pressurized-air resistance is determined by the size of the areas of separated

flow. The main factor here is the size of the rear separation zone. At points where the

flow separates, a partial vacuum is formed, giving rise to the pressurized-air

resistance. Fundamentally, the aim is to ensure that the separation areas and hence

the partial vacuum zones are small (MAN, 2004).

The target should be to keep the separation zones and hence vacuum zones on

the vehicle as small as possible. By specifically influencing the turbulence on the

3


rear end separation, a smaller vacuum and hence a smaller pressure resistance can be

achieved. A “stretching” of the boundary layer in the rear-end area can also lead to a

significant reduction in resistance. The induced resistance is a part of the vehicle’s

pressure resistance. Air pressure differences between the vehicle’s upper and lower

side produce cross-flows (Figure 1.3) that form two large longitudinal swirls together

with the roof flow (Figure 1.4). (BOSCH, 2002).

Figure 1.3. Induced air flow at the vehicle body

In their immediate vicinity such swirls induce low pressures. The “dead water

area” at the rear end is extended and thus leads to an increased pressure resistance.

4


Figure 1.4. Longitudinal swirls caused by induced draft

The term surface air resistance is used to describe the frictional resistance of

the “outer skin” of the vehicle to air flow. It is more pronounced on long vehicles

such as semi-trailer outfits and buses. The surface air resistance makes up 3-30 % of

the total drag.

The internal resistance is the proportion of the air resistance to which the

vehicle is subject by virtue of the through-flow of air for cooling and for interior or

cabin ventilation (MAN, 2004). Air not only flows around a vehicle, but also through

the vehicle in order to cool down the aggregates and to ventilate the passenger

compartment. When air flows through the cooler, engine compartment, wheelhouses,

and passenger compartment (Figure 1.5), losses of momentum arise from friction as

well as turbulences and flow separation in the vehicle’s interior. The resulting

internal resistance which constitutes about 3-11% of the total aerodynamic drag only

makes up a small part. Internal air resistance accounts for 3-11 % of total drag.

(BOSCH, 2002). In this study internal resistance will not be considered.

5


Figure 1.5. Air flow through a motor vehicle

The drag coefficient of a vehicle can be significantly reduced by rounding the

front section and using a front apron, a roof spoiler and side skirts. Only a slight

improvement in the drag coefficient is possible by altering the external shape of a

commercial-vehicle body since rounding the corners and edges reduces the load

space and hence the payload.

An aerodynamically designed cab causes an increase in the flow impinging

on a non-optimized body. The CD value is then higher than that with a sharp-edged

cab and a non-optimized body. The reason is that the front section of the body in the

case of a sharp-edged cab lies in a separation zone and is thus subject to a lower air

resistance.

In combination with such air deflectors, an aerodynamically optimized cabin

provides significant reductions in the drag of the vehicle as a whole.

Another measure for reducing resistance is to enclose the exposed running

gear of the vehicle with fairings. This reduces the air resistance of the vehicle

especially in a cross-wind.

Turbulence and the associated separation of the air flow increase drag to a

considerable extent. The rear of a vehicle combination, e.g. a semi-trailer outfit, is a

particularly problematic zone.

In order to optimize this are too, vertical metal flaps hinged to the rear of the

vehicle were used, an application of this can be seen in Figure 1.6. These flaps open

6


at a speed of 50-55 km/h and reduce the size of the separation edge at the rear of the

vehicle.

To ensure that these flaps open and close automatically, there is a funnel on

each of the top corners at the rear of the vehicle. The airflow when the vehicle is in

motion blows through these funnels and inflates two air sacks situated behind the

flap, thereby opening the latter. When the vehicle slows down, the flaps close again

and reduce the length of the vehicle to the legal limits. TÜV, the German technical

testing organization, allows the prescribed vehicle length to be exceeded while the

vehicle is in motion (MAN, 2004).

Figure 1.6. Application of Rear Flap to a Truck (MAN, 2004)

Since the main dimensions of a vehicle are to a large extent regulated by law,

a reduction of the aerodynamic drag is possible only by means of a reduced CD-

value. Drag coefficients of CD=0.15 achieved in prototypes, indicate the high

potential for future development compared to today’s mass-produced passenger cars

(CD=0.26- 0.45) and commercial vehicles (CD= 0.6-0.8) (BOSCH, 2002).

7


In order to achieve an aerodynamic body design, it is still necessary to

undertake experimental tests in a wind tunnel despite the availability of computer-

aided computational methods.

Corresponding to the degrees of freedom in three-dimensional space, three

forces (force of aerodynamic drag, lateral force, and lift) and three moments

(pitching, rolling, and yawing moment) (Figure 1.7) act on the vehicle. They are

usually determined by measuring the three forces coordinates on each wheel of the

vehicle. By geometrically adding up the forces recorded in the wind tunnel, the

aerodynamic forces and moments can be determined. This will not be considered

here in more detail. Out of the measured forces, the aerodynamic coefficients, e.g.

CD-value, are computed by combining them with the remaining constants. In this

case the vehicle flow should not be changed and a nearly distance and friction-free

measurement should be made possible (BOSCH, 2002).

Figure 1.7. Forces and moments in aerodynamic measurements

8


Modern wind tunnels are used not only to determine the aerodynamic drag

and their coefficients, but also for the acoustical investigation of vehicles. The

increasing demand for noise comfort in passenger cars, in this respect requires

optimization and tests. The challenge involved in these tests lies in lowering the

ambient noise level in so-called aero-acoustic wind tunnels, to such a level that the

actual noise measurement on the vehicle cannot be falsified very much by the

tunnel’s own operating noise. Operating noise has been lowered down to 60dB

(BOSCH, 2002).

The vehicle’s surface resistance, in theory called frictional resistance, is of

significance in long vehicles, e.g. busses. Figure 1.8 shows the cumulative resistance

in an aerodynamically-efficient bus body consisting of negligible resistance at the

vehicle front, relatively high resistance at the rear end, and body resistance consisting

basically of frictional resistance which steadily increases with the length of vehicle

(BOSCH, 2002).

Figure 1.8.Components of aerodynamic drag in an optimized bus body (MAN, 2004)

When air flow attacks a vehicle at an angle, the drag coefficient significantly

changes. Figure 1.9 shows the influence of the angle of approach on the CD-value for

different passenger car designs (BOSCH, 2002). In this study oblique flow condition

is neglected.

9


Figure 1.9. Aerodynamic drag at oblique flow for different passenger cars (BOSCH, 2002)

Consequently, for passenger cars as well as for commercial vehicles, there are

considerable increases in the coefficients of resistance when they are approached by

a side wind. In this case the maxima of the angle of approach β =25°-35° can be

achieved. When the vehicle is driven, angles of approach greater than 15° are

however exceptional.

1.2. Importance of Aerodynamics for Buses

Aerodynamic structure of the commercial vehicles especially buses are very

important, because aerodynamic forces and flow around the bus will cause a noise

called aero-acoustic noise, and vibration. Since the intercity buses transport

passengers, wind noise and vibration are much important than the trucks and trailers,

but the aerodynamic structure is also important for the trailers and trucks, from the

point of view of fuel consumption.

The experiments show that the fuel consumption can be lowered by

improving aerodynamic structure of the vehicle. The front apron and an optimally

positioned roof spoiler alone reduce fuel consumption by about 1.5 litres/100 km

(MAN, 2004).

10


Also the flow characteristics around the elements of the bus such as mirrors,

wheels, air conditioning unit, escape hatches on the top of the bus, plays an important

role as a source of the noise and vibration. These parts must be designed and

positioned to the bus by considering the flow around the parts.

In order to improve the flow characteristics of the bus, the best way is to use

rounded corners in stead of sharp one. The flow characteristic of the bus, shown in

the Figure1.10, is better than the bus shown in Figure 1.11.

Figure 1.10. An application of rounded corner to a bus (TEMSA Diamond)

Figure 1.11. A bus having sharp corners (TEMSA Tourmalin)

11

2.PREVIOUS STUDIES Serkan MEZARCIÖZ

2. PREVIOUS STUDIES AND SCOPE OF THE PRESENT STUDY

The drag forces of importance to the vehicle designer are dominated primary

by the wake forces, thus the prediction of the pressure coefficient at the rear of the

vehicle is of great importance. Also since the flow around a vehicle has an important

effect on the fuel consumption, noise, and vibration, lots of scientists and automotive

companies pay attention to this subject.

Takeuchi and Kohri (1997) has preformed a study for Mitsubishi Motors

Cooperation. The name of the study was “Development of Truck and Bus

Aerodynamics using Computational Fluid Dynamics“. This paper describes a

prediction method of aerodynamic drag and engine cooling performance for trucks

and buses using CFD. In particular, to obtain the accuracy of wake flow behind the

body, which is a dominant component of the total drag, they developed an adequate

method by comparing the experiment with calculation. Furthermore a practical

method for engine cooling air flow rate with regard to radiator and cooling fan

characteristics was shown.

“Aerodynamic Simulations by Using Discontinuous Interface Grid and

Solution Adaptive Grid Method” by Uchida et al. (1998), was carried out by the

financial support of Daihatsu Motor Cooperation Ltd. Aerodynamic simulations of

an automobile with the air-flow type spoiler using a discontinuous interface grid

method and flow simulation around the rear view door mirror using a solution

adaptive grid method were presented in their work. Consequently, it has become

possible to capture the detailed phenomena around these parts, such as the spoiler

and rear view door mirror.

Kuriyama (1998) conducted a study of “Transient Aerodynamic Simulation in

Crosswind” for Daihatsu Motor Cooperation Ltd. In this study, transient

aerodynamic simulation by using a sliding mesh of discontinuous interface and the

Arbitrary Lagrangian-Eulerian method was presented. This method uses the k-ε

turbulence model and the third-order upwind scheme, in order to introduce the

convective term of Navier-Stokes Equation to improve the data of flow field and

12


pressure distribution. Computed Yaw characteristics in crosswind are in good

agreement with the experiments.

Sumitani and Murayama (1999) reported that, airflow effect is one of the

important functions demanded of a rear spoiler. It helps prevent mud or dust from

swirling up behind the running vehicle, or, in the case of driving in rain or snow,

helps prevent rain or snow from adhering to the rear window. They often decide on

the shape of a spoiler in a relatively short time, focusing primarily on its appearance.

Therefore, they established a design method using recently developed computational

fluid dynamics to determine the central cross sectional shape of spoiler that realizes a

desired airflow effect and verified its effectiveness through testing.

In order to determine the flow around a road vehicle there are different

techniques, the most commonly used are wind tunnel experiments, and numerical

analysis of Computational Fluid Dynamics, in the case of CFD analysis two

challenging techniques Reynolds-Average Navier Stokes (RANS) and Large Eddy

Simulation (LES) are used.

Comparison of LES and RANS calculations of the flow around bluff bodies

was conducted by (Rodi 1997). His work compares LES and RANS calculations of

vortex-shedding flow past a square cylinder at Re = 22.000 and of the 3D flow past a

surface-mounted cube at Re= 40.000. The RANS calculations were obtained with

various versions of the k-ε model and in the square-cylinder case also with Reynold-

stress models, the various calculation results are compared with detailed

experimental data and an assessment is given of the performance, the cost and the

potential of the various methods. As a result of this study, Calculations obtained with

a variety of LES and RANS methods have been presented for two basic bluff body

flows with relatively simple body geometries albeit complex flow behavior. The

comparison with detailed measurements has shown that the main features of these

complex flows can be predicted reasonably well, at least with some of the methods.

The square cylinder results are not entirely satisfactory and do not provide a uniform

picture. It is clear, however, that for this flow the Standard k-ε model produces rather

poor results. This is to a large extent due to the excessive turbulence production in

the stagnation flow resulting from the use of this model. The Kato-Launder

13


modification removes this problem and yields improved results; a further

considerable improvement can be obtained when this model is combined with the

two-layer approach resolving the near-wall region. The excessive turbulence

production problem is also absent when a Reynolds-stress model is used which,

however, tends to over predict the periodic motion. In all RANS calculations, the

turbulence fluctuations are severely under predicted; the fairly high value of these

fluctuations in the experiment may stem from low frequency variations of the

shedding motion due to 3D effects which cannot be accounted for in 2D RANS

calculations. LES seems to pick up these motions and in general gives a better

simulation of the details of the flow (Rodi 1997).

The price to be paid for this is a large increase in computing time: the

UKAHY2 LES calculations took 73 h on a SNI S600/20 vector computer while the

RANS calculations using wall functions took 2 h and the ones using the two-layer

approach 8 h on the same computer. Further, it was found that none of the LES

results are uniformly good and entirely satisfactory and there were large differences

between the individual calculations which are difficult to explain. Reasons for the

lack of agreement with the experiments include insufficient resolution near the side

walls of the cylinder where the separated shear layer undergoes transition and a thin

reverse flow region is present, neglect of the turbulence in the incoming stream,

numerical diffusion and insufficient domain extent and number of grid points in the

span wise direction. Hence, this flow was selected once more as a test case for a LES

workshop held in Grenoble in September 1996 (Rodi 1997).

For the cube flow, the same problem with the excessive k-production in the

stagnation region exists when the standard form of the k-ε. Model is employed; and

this leads to poor predictions of the flow over the roof. These are significantly

improved by introducing the Kato Launder modification and also when the two layer

approach is used, and only with the latter can the complex structure of the near-wall

streamlines be simulated. However, both modifications increase even further the

length of the separation region behind the cube which is too large already for the

standard model.

14


RANS methods with statistical turbulence models will be needed and used for

many years to come in engineering calculations of the flow past bluff bodies.

However, inaccuracies must be accepted, and this comparative study has

demonstrated that LES is clearly more suited and has great potential for calculating

these complex flows. Further development and testing is certainly necessary, but

with the recent advances in computing power LES will soon be ready and feasible

for practical applications (Rodi 1997).

Krajnovic and Davidson (2001), investigated two large eddy simulation of the

flow past a bus-like vehicle body, and they compared the results with the

experimental data of E.G. Duell and A.R. George (1999). “Experimental study of a

ground vehicle body unsteady near wake The effect of the near wall resolution and

the modeling of the unresolved coherent structures in the near wall flow were

studied. The purpose of this work was to present LES of the flow around a bus-like

bluff body at Re=210000. They compared two LES in which the near wall region

was treated in different ways. It was determined that, although the wall functions are

inadequate to represent the thin vortices close to the wall, their use leads to results in

a near wake region that are similar to those in the simulation with a sufficient wall

normal resolution. That study indicated that the wall normal resolution has little

influence on the pressure coefficient at the rear face.

The geometry used by Krajnovic and Davidson (2001), is shown in the

flowing figure.

Figure 2.1. Geometry of the vehicle body and computational domain used by

Krajnovic and Davidson (2001)

15


The relationship between the bus-like shape and the channel dimensions are;

A domain with an upstream length X1/H=8, a downstream length of X2/H=16, and a

span-wise width of B=5.92H, was used for the simulation. The values of the other

geometrical quantities are L=0.46m, H=0.125m, W=0.125m, S=0.3075m,

R=0.0.019m, r=0.0127m, c=0.01m, and C=0.5 m. The ground clearance of c/H=0.08

is similar to the clearance ratio of buses. The Reynolds number Re=U.H/υ was

210000 on the basis of the incoming mean velocity, U and the vehicle height, H. The

cross-section of the tunnel test section, the ground clearance and the position of the

model’s cross-section with respect to the tunnel were identical in LES and

experimental set-up (Krajnovic and Davidson 2001).

In the study “Computational Study of Flow around the AHMED Car Body”

carried out by Craft et al (2001). A number of RANS simulations of flow around the

Ahmed body have been undertaken on Refined Turbulence Modeling. The

simulations have involved two different turbulence methods: a linear and non-linear

k-ε model, and two different wall functions. In this study calculations were

converged until, velocity, mass and turbulence residuals were below 10-4. Grid used

is approximately 300.000 cells and the legs, or stilts, on which the model is

supported in the wind tunnel experiments, were not included in the computational

grid. Grid were adjusted to maintain y* values of as many as possible near-wall cells

around the body to within the limits 55


Figure 2.2. Kinetic energy contours at the centerline (y=0) around the 25º Ahmed body

using the linear k-ε and cubic non-linear k-ε models with specified Chieng and Launder wall functions Craft et al (2001)

The development of attached or separated flow over the rear slant is strongly

influenced by the presence of the side edge vortices which draw fluid out of the

boundary layer on the rear slant. The weaker, more defined vortices predicted by, the

non-linear model led to the separation of the boundary layer. The velocity field was

reasonable predicted by the linear k-ε model over the 25º Ahmed body. But the

predicted stream wise normal stress was an order-of-magnitude lower than the

experimental values. For the 35º Ahmed body, both linear and non-linear models

correctly predicted separated flow over the rear slant. The linear k-ε model gave

reasonable predictions for the wake dimensions and velocity, although the predicted

turbulent kinetic energy was too high. The wake predicted by the non-linear k-ε

model was both too high in the z-axis and too long in the x-axis. The relatively poor

prediction of the wake size with non-linear model is in agreement with an earlier

study of the flow over a square cylinder, Craft et al (2001).

The feasibility of use of large-eddy simulation (LES) in external vehicle

aerodynamics is investigated. The computational cost needed for LES of the full size

car at road conditions is beyond the capability of the computers in the near future

17


(Krajnovic, 2002). Since LES cannot be used for quantitative prediction of this flow,

i.e. obtaining the aerodynamic forces and moments, an alternative use of this

technique is suggested that can enhance the understanding of the flow around a car. It

is found that making LES of the flow around simplified car-like shapes at lower

Reynolds number can increase our knowledge of the flow around a car. Two

simulations are made, one of the flows around a cube and the other of the flow

around a simplified bus. The former simulation proved that LES with relatively

coarse resolution and simple inlet boundary condition can provide accurate results.

The latter simulation resulted in flow in agreement with experimental observations

and displayed some flow features that were not observed in experiments or steady

simulations of such flows. This simulation gave information to study the transient

mechanisms that are responsible for the aerodynamic properties of a car. The

knowledge gained from this simulation can be used by the stylist to tune the

aerodynamics of the car’s design but also by the CFD specialists to improve the

turbulence models (Krajnovic and Davidson, 2002b). Geometry of the cube with its

channel dimensions are shown in the Figure 2.3.

Figure 2.3. Geometry of the cube with its channel dimensions (Krajnovic and

Davidson, 2002b)

18


Turbulence modeling plays a vital role in any numerical simulation in terms

of accuracy and computational cost. Wurtzler (2003) presents a Spalart-Allamaras

based detached eddy simulation hybrid model and numerical results for the Ahmed

reference car model with 25º base slant angle. Highly three-dimensional and

unsteady wake flow behavior is documented by showing velocity vectors in the

trailing region. One-equation RANS model is also used for the same simulation.

Both techniques are compared by showing the capability of each technique in

capturing the minor flow details and in predicting the coefficient of drag (CD).

Finally, unsteady behavior of CD is studied in both cases. Average value of CD is

calculated and validated with the reported experimental data of Ahmed et al. and

numerical results of Gillieron and Chometon. Further, brief discussion about the

present day available turbulence modeling techniques including DNS, LES, RANS

and DES is also done in the study of Detached Eddy Simulation over a reference

Ahmed Car Model.

In the study of “a comparison of large eddy simulations with a standard k-ε

Reynolds-Averaged Navier Stokes model for the prediction of a fully developed

turbulent flow over a matrix of cubes” by Cheng et al (2003), a fully developed

turbulent flow over a matrix of cubes has been studied using the large Eddy

simulation (LES) and Reynolds-averaged Navier–Stokes (RANS) [more specifically,

the standard k–e model] approaches. A comparison of predicted model results for

mean flow and turbulence with the corresponding experimental data showed that

both the LES and RANS approaches were able to predict the main characteristics of

the mean flow in the array of cubes reasonably well. LES, particularly when used

with LDM, was found to perform much better than RANS in terms of its predictions

of the span-wise mean velocity and Reynolds stresses. Flow structures in the

proximity of a cube, such as separation at the sharp leading top and side edges of the

cube, recirculation in front of the cube, and the arch-type vortex in the wake are

captured by both the LES and RANS approaches. However, LES was found to give a

better overall quantitative agreement with the experimental data than RANS (Cheng

et al., 2003).

19


In journal of “LES as a powerful Engineering tool for predicting complex

turbulent flows and related phenomena” Inagaki (2004) reported the advantages of

LES over the k-ε model as follows; high prediction accuracy, capability of resolving

the unsteadiness of turbulent motion over a broad range of scales, and simplicity of

modeling the turbulent effects in the fluid phenomena containing multiphysics

(Inagaki, 2004).

In the present numerical study the dimensions of the channel was determined

by referencing the study carried out by Krajnovic and Davidson (2004a). The

relationship between the generic vehicle body and channel dimensions were chosen

in that study and the present numerical analysis to be the same as used in the

experiments by Ahmed et al (1984) and Lienhart and Becker (2003). The geometry

of the body and the computational domain used by Krajnovic and Davidson (2004a)

are given in Figure 2.4. The body is placed in the channel with cross section of

BxF=6.493Hx4.861H (Width x Height). The cross section of this channel is identical

with the open test section of the wind tunnel used in the experiments of Lienhart and

Becker (2003). The front face of the body is located at the distance of X1=7.3H from

the channel inlet and the downstream length between the rear face of the body and

the channel outlet is X2=21H. The body is lifted from the floor producing the ground

clearance of c/H=0.174, same as in the experiments. The Reynolds number, based on

the incoming velocity U and the car height H, of Re=7.68x10∞ 5 used in the

experiments Lienhart and Becker (2003) was reduced to Re=2x105.

Krajnovic and Davidson (2004a) have already demonstrated successful LES

of this lower Reynolds number case with no rear body slant angle, i.e. α=0º (generic

bus body). Krajnovic and Davidson expect that the slanted rear end will produce a

wider spectrum of turbulent scales that must be resolved in LES.

20


Figure 2.4. Schematic representation of the computational domain with vehicle body

(Krajnovic and Davidson, 2004a)

2.1. Scope of the Present Study

The purpose of the present study is to show a numerical study of a flow

around a bus-like shape taking into account the 3D geometry, the effect on the flow

around the bus. This study has been done with the commercial software package

FLUENT. This code uses FVM and solves 3D flows.

In the present study the dimensions of the model was the same as the

dimensions of the model which was used by Gürlek (2006) in his experimental work.

For the channel dimensions of the present study, we referenced the ratios of

dimensions which were used by Krajnovic and Davidson (2004a).

By using GAMBIT program grid generation and identification of boundary

condition were performed and using FLUENT program finite volume analysis was

executed by k-ε turbulence model.

In order to get more precise results, in the present numerical simulation,

calculations will be converged until residuals were below 10-5 and the grid used has

935.004 cells. As in the study of Craft et al (2001), we also did not include the legs

of the model for the computation domain, and the present y* value was in range of

Craft et al (2001).

The analysis performed numerically was compared to the experimental results

of Gürlek (2006).

21

3.MATERIALS AND METHODS Serkan MEZARCIÖZ

3. MATERIALS AND METHODS

Experimental fluid dynamics has played an important role in validating and

defining the limits of the various approximations to the governing equations. The

wind tunnel, for example, as a piece of experimental equipment, provides an

effective means of simulating real flows. Traditionally this gas provided a cost

effective alternative to full-scale measurement. However, in the design of equipment

that depends critically on the flow behavior, for example the aerodynamic design of

an aircraft or a bus, full-scale measurement, as part of the design process is

economically impractical. This situation has led to an increasing interest in the

development of numerical studies.

Computational Fluid Dynamics (CFD) has proven capability in predicting the

detailed flow behavior for wide-ranging engineering applications, leading typically

to an improved equipment or process design.

Most of the vehicle manufacturers are, now using CFD a simulation toll

originally developed for academic research and aerospace. CFD is used to solve the

RANS Equations that describe fluid flow and to generate a 3D model of that flow,

making possible more effective vehicles and minimizing the aero acoustic noise, and

vibration.

The object of CFD is to use computers to solve the previously intractable

conservation equations for fluids in order to accurately simulate flows. This typically

involves discretizing the problem in a finite set of elements, applying the

conservation of mass, momentum, energy, and chemical species (where necessary) to

these elements, placing additional boundary conditions at the edge of the

computational grids, and solving the resultant algebraic equations in an iterative

fashion (Öztürk, 2004).

Thus, CFD allows the analysis of fluid flow problems in detail, faster and

earlier in the design cycle than possible with experiments, costing less money and

lowering the risks involved in the design process. This trend is only likely to grow

more pronounced in the future as computers become increasingly cheaper and more

powerful while traditional forms of testing become increasingly expensive. For

22


improving aerodynamic structure of the ground vehicles, it is great importance to

carry out investigation on the flow behavior indeed. With the currently increasing

computer capability and CFD developed, numerical simulations of the 3D turbulent

flow around the road vehicles is becoming possible.

The purpose of the present study is to show a numerical study of a flow

around a bus-like shape taking into account the 3D geometry, the effect on the flow

around the bus. This study has been done with the commercial software package

FLUENT. This code uses FVM and solves 3D flows. For the solution, the grid was

generated by GAMBIT package program.

3.1. Vehicle Geometry and Dimensions

In the present study dimensions of the model geometry was the same as

dimensions which were used in the experiments of Gürlek (2006). The length of the

model L=175mm, the height of the model H is 67mm, and the width of the vehicle

W is 56 mm. The ground clearance of the vehicle c is taken as 9 mm. The geometry

of the model is shown in the Figure 3.1.

Figure 3.1. The dimensions of the vehicle model.

23


3.2. Determination of Dimensions of the Flow Domain

In order to perform a computer simulation of a physical flow problem, the

first step is to build a model of the flow domain. In the present study, to determine

the dimensions of the flow domain, the dimensions normalized by the vehicle height

H, is referenced as in Krajnovic and Davidson (2004a and 2004b). According to

Krajnovic and Davidson (2004a) the relationship between the channel dimensions

and vehicle height H, are as follows; The body was placed in the channel with cross

section of B x F=6.493H x 4.861H (Width x Height). The front face of the body is

located at the distance of X1=7.3H from the channel inlet and the downstream length

between the rear face of the body and the channel outlet is X2=21H and the distance

between the side walls of bus and channel S is 2.571H. Schematic representation of

the computational domain with vehicle body (Krajnovic and Davidson, (2004)) is

shown in Figure 3.2.

Figure 3.2. Schematic representation of the computational domain with vehicle body

(Krajnovic and Davidson, 2004a)

By referencing the ratios of Krajnovic and Davidson, (2004a), the present

flow geometry dimensions and the position of the vehicle model in the channel were

determined as follows;

Width of the channel (B) = 6.493xH = 6.493x 67=435 mm.

Height of the channel (F)= 4.861xH=4.861x67= 326 mm.

Distance between inflow and model front face (X1)= 7.3xH=7.3x67=489 mm

Distance between outflow and model back face (X2)= 21xH=21x67=1407mm

Overall length of the channel=X1+L+ X2= 489+ 175+1407=2071 mm.

24


With these results the dimensions of the computational domain and the

position of the model in the domain is determined and shown in the Figures 3.3 , 3.4

and 3.5.

Figure 3.3. Position of the bus in the channel (side view, dimensions in mm)

Figure 3.4. Position of the bus in the channel (cross-sectional view)

Figure 3.5. 3D view of the computational domain

25


3.3. Grid Generation and Refinement Study

A mesh is a set of points distributed over a calculation field for a numerical

solution of a set of partial differential equations. Essential CFD involves the setting

up partial differential equations and boundary conditions describing fluid flow over a

physical domain these equations are then solved numerically to generate the pressure

and velocity fields in the flow domain.

In order to perform the discretisation of the governing equations the physical

space must be subdivided into number of cells by means of a structured grid. The

grid can be constructed using a rectangular, a cylindrical or a body fitted coordinate

system.

In the present study the 3-D finite volume, rectangular mesh is built by using

GAMBIT computer code In order to build the models, firstly the geometry of the

flow domain is described by defining discrete set of points (nodes) and collection of

these points (elements). The points are joined to create lines, arcs, circles, and finally

the volumes are created.

To validate the numerical results, it is great importance to check whether the

grid that has been used to discretize the computational domain complies with the

requirements of the turbulence model used.

To check the grid used for the analysis, simulations were performed with

three different grids. The used firs second and third grids have 442.496, 786.586 and

1.186.819 nodes, respectively. The grids were compressed near the vehicle body

walls. The grids were adapted in order to further resolve the flow near the body wall

regions.

It is decided for the grid compatibility by checking the y* value, Craft et al

(2001) used a grid, which were adjusted to maintain y* values of as many as possible

near wall cells around the body within the limits 55


can not be used for this simulation. In the Figure 3.6, distribution of y* values for

442.496 nodes can be seen.

Figure 3.6. Distribution of y* values for the grid having 442.496 nodes

When the number of cells is 658.903 and nodes is 786.586, the value of y* is

in the range of 0


Lowering the y* value gives more precise results and provides us the grid

independency, but lowering the y* value, in other words refining the grid, is limited

by the computational cost of the simulation. In the present study y* value is lower to

the range of 0


3.4.1. Boundary Conditions for Simulations

1. Velocity Inlet boundary conditions are used at the inflow section of the

channel as approximately 90 km/h (25 m/s). it is assumed that only a constant and

uniform stream wise-direction velocity component exists and other velocity

components are assumed to be zero.

2. Free outflow boundary condition: The outflow boundary condition is used

to model flow exist where the details of the flow velocity and pressure are not known

prior to solution of the flow problem so that mass balance correction is applied at the

outflow boundary and other data at the exit plane is extrapolated from the interior.

Diffusion fluxes for all flow variables in the direction normal to the exit plane are to

be zero. Therefore the outflow velocity is consistent with a close to fully developed

flow assumption.

3. Wall boundary condition is used to bound fluid and solid regions at the

vehicle and channel surfaces. The boundary conditions are no- slip ( ) 0=== wvu

4. Fluid boundary condition at the fluid zone. Fluid zone is defined as group

of cells for which all active equations are solved. The fluid material is set as air.

3.5. Simulation of the Flow

In the present study, in order to simulate the flow around the bus-shape

model, a commercial package program FLUENT was employed.

For all flows, FLUENT solves conservation equations for mass and

momentum. For flows involving heat transfer or compressibility, an additional

equation for energy conservation is solved Additional transport equations are also

solved when the flow is turbulent. FLUENT employs the finite-volume-based

technique. In the finite volume method the solution domain is subdivided into a finite

number of discrete continuous control volumes (CVs) or cells, and the conservation

equations are applied to each CV. The governing conservation equations are

integrated on the individual control volumes to construct the algebraic equations for

the discrete dependent variables (unknowns) such as velocity, pressure, temperature

29


and scalars. The discretized equations are linearized and the resultant linear system

of equations is solved to yield updated values of the dependent variables (FLUENT,

1998).

3.5.1. Discretization

FLUENT uses a control volume based technique to convert the governing

equations to algebraic equations that can be solved numerically. This control volume

technique consist of integrating the governing equations about each control volume,

yielding discrete equations that conserve each quantity on a control-volume basis.

Discretization of the governing equations can be illustrated most easily by

considering the steady-state conservation equation for transport of a scalar quantity

φ . This is demonstrated by the following equation written in integral form for an

arbitrary control volume V as follows:

∫ Adrr

.νρ = ∫∫ +∇ΓV

dVSAd φφ φr

. (3.1)

where ρ is the density, νr is te velocity vector ( ), kwjviu ˆˆˆ ++= Ar

is the surface

area vector, is the diffusion coefficient for φΓ φ , φ∇ is the gradient of

,ˆˆˆ ⎟⎟⎠

⎞⎜⎜⎝

⎛⎟⎠⎞

⎜⎝⎛∂∂

+⎟⎟⎠

⎞⎜⎜⎝

⎛∂∂

+⎟⎠⎞

⎜⎝⎛∂∂

= kz

jy

ix

φφφφ and is the source of φS φ per unit volume.

Equation (3.6) is applied to each control volume, or cell, in the computational

domain. Discretization of Equation (3.2) on a given cell yields

(3.2) =∑ ffN

fff A

faces rr .φνρ VSAfN

fn

faces

φφ φ +∇Γ∑r

.)(

30


where is the number of faces enclosing cell, facesN fφ is the value of φ convected

through face fff Afrr ., νρ is the mass flux through the face, fA

r is the area of , f

nzyx kAjAiAA )(,ˆˆˆ φ∇++= is the magnitude of φ∇ normal to face , and V is the

cell volume.

f

Fluent stores discrete values of φ at the cell centers. However, face values of

fφ are required for the convection terms in Equation (3.1) and must be interpolated

from the cell center values. This is accomplished using an upwind scheme.

Then the discretized equations are linearized and resultant linear equation

system are solved to yield updated variables of the dependent variables.

In the segregated solution method, the governing equations are solved

sequentially. Because the governing equations are non-linear (and coupled), several

iterations of the solution loop must be performed before a converged solution is

obtained. Each iteration consists of the steps shown below:

1. Fluid properties are updated based on the current solution.

2. The and momentum equations are each solved in turn using

current values for pressure and face mass fluxes, in order to update the

velocity field.

vu, w

3. Since the velocities obtained in Step 2 may not satisfy the continuity

equation locally, a “Poisson-type” equation for the pressure correction is

derived from the continuity equation and the linearized momentum

equations. This pressure correction equation is then solved to obtain the

necessary corrections to the pressure and velocity fields and the face mass

fluxes such that continuity is satisfied.

4. Where appropriate, equations for scalars such as turbulence, energy,

species, and radiation are solved using the previously updated values of

the other variables.

5. A check for convergence of the equation set is made.

These steps are continued until the convergence criteria are met.

31


In the segregated solution method, the discrete, non-linear governing

equations are linearized to produce a system of equations for the dependent variables

in every computational cell. The resultant linear system is then solved to yield an

updated flow-field solution. Implicit means: For a given variable, the unknown value

in each cell is computed using a relation that includes both existing and unknown

values from neighboring cells. Therefore each unknown will appear in more than one

equation in the system, and these equations must be solved simultaneously to give

the unknown quantities.

In the segregated solution method, each discrete governing equation is

linearized implicitly with respect to that equation’s dependent variable. This will

result in a system of linear equations with one equation for each cell in the domain.

Because there is only one equation per cell, this is sometimes called a “scalar”

system of equations. A point implicit (Gauss-Seidel) linear equation solver is used in

conjunction with an algebraic multigrid (AMG) method to solve the resultant scalar

system of equation is linearized to produce a system of equations in which u

velocity is the unknown. Simultaneous solution of this equation system (using the

scalar AMG solver) yields an updated velocity field. u

In summary, the segregated approach solves for a single variable field

(e.g., p ) by considering all cells at the same time. It then solves for the next variable

field by again considering all cells at the same time, and so on (FLUENT, 1998).

3.5.2. Convergence

The convergence criterion for the continuity and momentum equations is set

as All the simulations are performed until the solution is converged with the

specified convergence criterions. The convergence of the residuals of the last 229

iterations can be seen in Figure 3.9.

510−

32


Figure 3.9. Convergence of the residuals to 10-5

3.6. Governing Equations for Fluid Flow

All physical systems obey three fundamental conservation laws: Mass is

conserved, Momentum is conserved, and Energy is conserved. The governing

equations of fluid flow and heat transfer represent mathematical statements of the

conservation laws of physics. The conservation equations are derived by considering

the mass, momentum and energy balances for an infinitesimal control volume. In the

absence of an external body force, differential forms of the governing continuity,

momentum and energy equations for the laminar case used in the present study can

be given as follows:

* Continuity Equation. The mass conservation or the continuity equation for

a time-dependent, three-dimensional, incompressible and Newtonian fluid is given in

Eqn. (3.3).

0=∂∂

i

i

xu

(3.3)

33


* Momentum Equation. The most useful form of the conservation of the

momentum equation is obtained by applying Newton’s Second Law of motion to an

infinitesimal fluid element and re-arranging the viscous stress terms yields the so

called Navier-Stokes Equation.

( )

⎥⎥⎦

⎤

⎢⎢⎣

⎡⎟⎟⎠

⎞⎜⎜⎝

⎛

∂

∂+

∂∂

∂∂

+∂∂

−=∂

∂+

∂∂

i

j

j

i

jij

iji

xu

xu

xxp

xuu

tu

νρ1 (3.4)

* Energy Equation. The energy of a fluid is defined as the sum of internal

(thermal) energy, kinetic energy and gravitational potential energy. The internal

energy equation for a time-dependent, three-dimensional, incompressible and

Newtonian fluid is given in Eqn. (3.5).

( )jj

ji x

Tx

Txt

T∂∂

∂∂

=∂∂∂

+∂∂ α (3.5)

3.7. Reynolds Averaged Navier Stokes (RANS) Equations of Motion

The Navier-Stokes Equations are a set of non-linear partial differential

equations and they can only be able to describe continuous and homogeneous fluid

flows approximately. However, at very small scales or under extreme conditions, real

fluids made out of mixtures of discrete molecules and other materials, such as

suspended particles and dissolved gases, produce different results form the

continuous and homogeneous fluids modeled by the Navier- Stokes Equations.

Although the full, unsteady Navier-Stokes Equations correctly describe nearly all

flows of practical interest, they are too complex for practical solution in many cases

and a special “reduced” form of the full equations is often used instead-these are the

Reynolds Averaged Navier Stokes (RANS) equations.

In Reynolds Averaging, the solution variables in the instantaneous (exact)

Navier-Stokes equations are decomposed into the mean (ensemble-averaged or time-

averaged) and fluctuating components. Now all flow variables in the equations can

34


be displaced by sum of a mean (ensemble) and a fluctuating component: Reynolds

averaging means replacing the time-varying quantities with time-averaged (mean)

and fluctuating components as

u=u + ; v = u′ vv ′+ ;w= ww ′+ ; p= pp ′+

Whereu v w , are mean velocity components, andu′ , v′ , w′ are fluctuating velocity

components.

The solution of the full steady Navier-Stokes Equations is sufficiently

accurate only for laminar cases of the fluid flow. For turbulent flows the Reynolds

averaged form of the equations are most commonly used. The RANS form of the

equations introduce new terms that reflect the additional modeling of the small

turbulent motions.

In the absence of an external body forces, the governing time averaged

conservation equations for an incompressible, Newtonian fluid of constant density

and constant viscosity take the following forms:

1)Time averaged continuity equation:

0=∂∂

i

i

xu

(3.6)

2) Time averaged momentum equation:

( )⎥⎥⎦

⎤

⎢⎢⎣

⎡ ′′−⎟⎟⎠

⎞⎜⎜⎝

⎛

∂

∂+

∂∂

∂∂

+∂∂

−=∂

∂+

∂∂

jii

j

j

i

jij

iji uuxu

xu

xxp

xuu

tu

νρ1 (3.7)

3) Time averaged energy equation:

( ) jjj

ji

qxT

xTu

xtT

−∂∂

∂∂

=∂∂

+∂∂ α (3.8)

35


Reynolds averaging introduces additional terms in the momentum and energy

equations which are known as “Reynolds (turbulent) stress”, - and the

“Reynolds (turbulent) heat flux”, - , which appear on the right-hand side of the

momentum and the energy equations, respectively. The task of turbulence modeling

is to model these unknown, higher-order, extra terms in the mean flow equations and

thus close the system of equations. The need to model these correlations is the

‘closure problem’. It is also possible to model a transport equation for the heat flux,

but this is not a common practice. Instead, a turbulent thermal diffusivity is defined

proportional to the turbulent viscosity. The constant of proportionality is called the

turbulent Prandtl number, Pr

,′′ ji uuρ

jq

t (0.85


1.Models that use the Boussinesq Approximation: These are the eddy

viscosity models.

2.Models that solve directly for the Reynolds Stresses. These become

complicated fast by introducing further terms requiring modeling.

3.Models not based on time-averaging: These are Large Eddy Simulation

(LES) and Direct Numerical Simulation (DNS) methods.

3.9. Turbulence Models

A turbulence model is a computational procedure to close the system of mean

flow equations so that a more or less wide variety of flow problems can be

calculated. For most engineering purposes it is unnecessary to resolve the details of

the turbulent fluctuations. Only the effects of the turbulence on the mean flow are

usually sought. The most common turbulence models are classified as follows:

3.9.1. Time Averaged Turbulence Models

Time Averaged Turbulence Models are also referred as RANS Equations

Based Turbulence Models or Classical Models. These are:

1. Zero Equation Model (Mixing Length Model)

2. One Equation Model

3. Two Equation Model (k-ε Model, k-w Model)

4. Reynolds Stress Model

5. Algebraic Stress Model

These models model all scales of eddies present in the flow. Zero, One and

Two Equation Models use Boussinesq Hypothesis to relate the Reynolds stresses to

the time averaged velocity gradients as shown below:

- =′′vuρ ⎟⎟⎠

⎞⎜⎜⎝

⎛∂∂

+∂∂

xv

yu

tµ (3.9)

37


Where tµ is the turbulent (eddy) viscosity. The advantage of this approach is

that relatively low computational cost is required to compute the turbulent viscosity.

3.9.1.1. Zero Equation Model

The Zero Equation Model was the first turbulence model proposed by Prandtl

in 1925 and is also known as Prandtl Mixing Length Model. In zero-equation model,

the flow is characterized by one velocity scale and one length scale and the turbulent

viscosity is assumed to be constant. Therefore no transport of turbulence is resolved

in the zero equation models. The eddy viscosity expressed as

yuLC mt ∂∂

= 2µρµ (3.10)

Where Lm is the mixing length and is a constant. The model can be

successively applied to the simple flows and the mixing length can be specified by an

empirical formula in most situations. However, the model fail for separating flows

and cannot be applied to the rapidly developing and recalculating flows where

convective or diffusive transport of turbulence are important.

µC

3.9.1.2. One Equation Model

In one- equation model a transport equation turbulent kinetic energy is solved

and some physically based arguments for the mixing length is solved. This means

that the turbulent eddy viscosity now becomes a dependent variable that varies

spatially and with time for unsteady flows. The turbulent kinetic energy is considered

to be the velocity scale it is contained in the large scale fluctuations and is expressed

as follows:

k = ( )22221 wvu ′+′+′ (3.11)

38


The turbulent eddy viscosity is modeled by

st LkCµρµ ′= (3.12)

where and represent empirical constant and length scale, respectively. The

length scale distribution cannot be specified empirically for complex flows. Although

theoretical formulae for determining the length scale are proposed based on the mean

flow, they are very dependent on the problem type, they have not been tested

sufficiently and they require rather expensive computing time.

µC ′ sL

3.9.1.3. Two Equation Models

In two equation models, the RANS equations are closed by assuming the

turbulent stresses are proportional to the mean velocity gradients and the constant of

proportionality is the turbulent viscosity (Boussinesq Hypothesis). The constant of

proportionality is allowed to vary through out of the flow field and has been

correlated in terms of the turbulent kinetic energy and dissipation rate. Various

transport equations are developed for the turbulent kinetic energy and dissipation

rate.

* Standard Linear Turbulence k-ε Model

The standard linear k-ε turbulence model is well known and the model has

been tested for vortex shedding flow by Majumdar and Rodi (1985) previously.

Turbulent kinematic viscosity, vt, is related to kinetic energy k and turbulent

dissipation ε by a following formula:

εµ2kCvt = (3.13)

39


The forms of the k and ε equation of the Standard Linear k-ε model are then

gives as follows:

ε−∂∂

⎟⎟⎠

⎞⎜⎜⎝

⎛

∂

∂+

∂∂

+⎟⎟⎠

⎞⎜⎜⎝

⎛

∂∂

∂∂∂

=j

i

i

j

j

it

j

k

k

t

j xu

xu

xu

vx

vxDt

Dk (3.14)

kC

xu

xu

xu

vk

Cx

vxDt

D

j

i

i

j

j

it

j

t

j

2

21εεε ε

ε

−∂∂

⎟⎟⎠

⎞⎜⎜⎝

⎛

∂

∂+

∂∂

+⎟⎟⎠

⎞⎜⎜⎝

⎛

∂∂

∂∂∂

= (3.15)

The coefficients εµ σσ ,,,, 21 kCCC are constants in the sense that they are not

changed in any calculation. However, these constants need to be changed in order to

accommodate the effects such as low Reynolds number, near wall, etc. these five

coefficients have a value as shown below for the Standard k -ε model:

09.0=µC

C1 = 1.44

C2 = 1.92

00.1=kσ

30.1=εσ

The turbulent heat transport on the other hand is modeled by using the

concept of Reynolds’ analogy to turbulent momentum transfer by the use of Eqn.

(3.6).

The standard linear k -ε turbulence model is extended by Launder and

Spalding (1972) and named by ω−k and k – L models where Ls is the length

characterizing the macro scale of turbulence and ω is the time average square of the

vorticity fluctuations as defined by Wilcox and Rubesin (1980):

( )22

kC f

εω = (3.16)

40


ii

jj

xxuu∂∂

′∂′∂=νε (3.17)

ε

2/3kCL fs = (3.18)

The standard linear and extended k -ε turbulence models are not sufficient

for the predictions of near wall flow at high Reynolds numbers.

* Non-Linear RNG k -ε Turbulence Model

The Renormalization Group (RNG) k -ε model is proposed by Speziale

(1987) and has been validated against internal flow and impinging jet problem by

Rabbit (1997) and later is developed by Yakhot et al. (1992). This model is very

similar in form to the standard and extended k -ε turbulence models, however the

RNG k -ε model differs from the standard model by the inclusion of an additional

sink term in the turbulence dissipation equation to account for non-equilibrium strain

rates and employs different values for the various model coefficients. The form of

the k equation remains same. The turbulence dissipation, ε equation of the RNG k -

ε model includes the following sink term

k

C 23

0

3

1

1 εβη

ηηηµ

+

⎟⎠⎞⎜

⎝⎛ −

(3.19)

In the above term employs the parameterη , which is the ratio between the

characteristic time scales of turbulence and mean flow field as follows:

εη kS=

41


where

S = t

ijijGSS µ=2

⎟⎟⎠

⎞⎜⎜⎝

⎛

∂

∂+

∂∂

=i

j

j

iij x

uxu

S21 (3.20)

The primary model coefficients of the RNG k -ε turbulence model are

εµ σσ ,,,, 21 kCCC and Von Karman constant κ . Recommended values of this model

coefficients are as follows:

085.0=µC

41.11 =C

68.12 =C

7179.0=kσ

7179.0=εσ

κ = 0.3875

* Realizable k -ε Turbulence Model

The term “realizable” means that the model satisfies certain mathematical

constrains on the normal stress, consistent with the physics of turbulent flows. The

realizable k -ε model proposed by Shih et al. (1995) intends to address the

shortcomings of traditional k -ε turbulence models by adopting a new eddy-viscosity

formula involving a variable originally proposed by Reynolds (1987) and a new

model equation for dissipation based on the dynamic equation of the mean-square

vorticity fluctuation. The kinetic energy equation is the same as that in the standard

Date post:	19-Oct-2020
Category:	Documents
Upload:	others
View:	4 times
Download:	0 times

ÇUKUROVA UNIVERSITY INSTITUTE OF NATURAL AND APPLIED ... · Anahtar Kelimeler: Aerodinamik,...

Documents