Experimental and Numerical Investigation of an In-line TubeBank’s Cooling Potential

(1)

Link¨oping University | Division of Energy Systems Master’s thesis, 30 hp | MSc Mechanical Engineering Spring 2016 | LIU-IEI-TEK-A–16/02697—SE

Experimental and Numerical

Investigation of an In-line Tube

Bank’s Cooling Potential

Hanley La

Lars Petterson

Supervisor: Klas Ekel¨ow Examiner: Bahram Moshfegh

(2)

(3)

Abstract

Within this thesis, an experimental and numerical study was performed on cooling of a 5x5 in-line tube bank placed within a duct using impinging jets. The Reynolds numbers investigated using the main inlet as reference were Re∼2300 and Re∼4500. The Reynolds number corresponding to the impinging jets was Re∼147000.

The aim of the study was to replicate the thermal conditions in an industrial tunnel kiln used for pro-duction of cylindrical objects. As the current cooling was fairly unknown due to difficulties in conducting proper measurements a miniature tunnel oven model had been built. The experimental part of the thesis was done on said miniature tunnel oven model which was at the time located at G¨avle University (HiG). Prior to collecting the cooling data, an extensive groundwork was performed e.g. leakage test, jet and inlet velocity studies. The velocity measurements were conducted using a hot-wire anemometer.

The simulation part was conducted using computational fluid dynamics simulations (CFD). A pre-study was performed in order to study the effect of using different settings in the CFD-setup. The study resulted in the use of steady RANS together with k − ω SST as turbulence model. First order schemes were used except for the energy equation which used second order. A mesh independence study was performed and showed a better agreement to experiments with the increase in mesh density.

The experimental and numerical results showed good resemblance to each other for both the temperat-ure and the heat transfer coefficient of the cylinders. The average deviation of the simulations to the experiments were 8.3% and 11.0% for the cylinder temperature and heat transfer coefficient respectively. By studying the obtained temperature and heat transfer coefficient contours obtained through ANSYS a more evenly distributed cooling was obtained by placing the impinging jets between cylinders compared to directly facing cylinders in a cylinder package. This was also apparent by observing the obtained results from the experimental study.

(4)

(5)

Acknowledgements

We would like to express our gratitude to Klas Ekelöw (supervisor) for the opportunity to do this thesis as well as all the support and knowledge he has provided us throughout this thesis. Bahram Moshfegh as well as Höganäs AB have our sincere gratitude as they made this thesis possible.

We would like to thank the knowledgeable staff at G¨avle University (HiG) for their support and aid they provided us concerning the miniature model.

We also would like to thank Elisabeth Larsson for managing the administrative issues we encountered during this thesis.

Finally, we would like to thank Marcus Rowlands and Hugo Hardestam for the critical reviews and second opinion they have provided throughout the duration of this thesis.

(6)

(7)

List of Figures

1.1 Schematic drawing of the tunnel oven showing the iron powder entering through the tunnel

oven. . . 1

2.1 Schematic drawing of a Pitot tube. . . 4

2.2 Schematic drawing of a hot wire. . . 5

2.3 Yaw and pitch angles of the bulk flow in relation to the wire normal. . . 6

2.4 Illustration of a thermocouple . . . 6

2.5 Illustration of orifice plate . . . 7

2.6 Illustration of the boundary layer, shear layer and the vortices . . . 8

2.7 Illustration of the von K´arm´an vortex street phenomena . . . 8

2.8 Law of the wall. . . 13

2.9 Illustration of the Jacobian-ratio . . . 15

2.10 Illustration of differently skewed geometries . . . 15

2.11 Illustration of a quadrilateral with different aspect-ratio . . . 16

2.12 Drag coefficient (CD) for a circular cylinder with respect to Reynolds number. . . 17

2.13 Correlation for cross-flow forced convection from single circular cylinder in air. . . 18

2.14 Illustration of the domain for flow over an in-line tube bank . . . 19

2.15 Illustration of staggered and in-line tube bank configuration . . . 20

2.16 Illustration of an impinging jet hitting a flat plate . . . 21

2.17 Illustration of an impinging jet hitting a flat plate subjected to a cross-flow . . . 21

2.18 Illustration of velocity and turbulent kinetic energy varying with nozzle shape . . . 22

3.1 Schematic drawing of the complete miniature model in 3d. . . 24

3.2 Schematic drawings of the wind tunnel from different point of views. . . 24

3.3 Photos taken on the various devices and gear used for measuring . . . 26

3.4 Schematic drawing of the CTA equipment chain . . . 26

3.5 Photos taken on the miniature model and its individual components . . . 27

3.6 Leakage test performed on fan 2 . . . 28

3.7 Velocity calibration for the CTA . . . 29

3.8 Velocity recalibration . . . 30

3.9 Force measuring cylinder . . . 31

3.10 Illustration of a cross section of the thermal cylinder . . . 32

3.11 Schematic drawing of the three sensor cases . . . 33

3.12 Data point lines along the main inlet . . . 34

3.13 Non-dimensional main inlet velocity (U/Ub) profile, Ub=0.75m/s. . . 35

3.14 Main inlet turbulence intensity (Tu) at Y, Ub=0.75m/s. . . 35

3.15 3D main inlet velocity, Ub=0.75m/s. . . 36

3.16 3D main inlet turbulence intensity, Ub=0.75m/s. . . 36

3.17 Main inlet velocity, turbulence intensity and turbulence kinetic energy, Ub=0.75m/s. . . . 37

3.18 Data point lines along the impinging jet outlet . . . 38

3.19 Mean jet velocity and turbulence intensity profile. . . 39

3.20 Comparing merge impinging jet velocity and turbulence intensity distribution to fully developed pipe flow. . . 39

3.21 Velocity profile along the horizontal axis for each impinging jet, desired UJ et=40m/s . . . 40

3.22 Velocity profile along the vertical axis for each impinging jet, desired UJ et=40m/s . . . . 40

3.23 Illustration of the domain for a single cylinder indicating the size of the domain . . . 41

3.24 Illustration of the domain for a group of cylinders indicating the size of the domain . . . . 42

3.25 The meshed domain of the single cylinder . . . 42

3.26 The meshed domain of the group of cylinders . . . 43

3.27 Illustration of the computational domain and cross section of cylinder showing the boundaries 43 3.28 Numerical and empirical verification of single cylinder . . . 45

(10)

3.29 Illustration of a single cylinder inside the wind tunnel. . . 46

3.30 Comparison of heat transfer coefficient for each iteration of the mesh independence study 47 3.31 Contour plot of y+ _{values of the cylinder package, jets placed between cylinders. . . .} ₄₈

3.32 Y+ _{distribution, jets placed between cylinders. . . .} ₄₈

3.33 Contour plot of y+ _{values of the floor and wall, jets placed between cylinders. . . .} ₄₉

3.34 Y+ _{distribution, jets placed between cylinders. . . .} ₄₉

3.35 Contour plot of y+ _{values of the cylinder package, jets placed on cylinders.} _{. . . .} ₄₉

3.36 Y+ _{distribution, jets placed on cylinders.} _{. . . .} ₄₉

3.37 Contour plot of y+ _{values of the floor and wall, jets placed on cylinders. . . .} ₄₉

3.38 Y+ _{distribution, jets placed on cylinders.} _{. . . .} ₄₉

3.39 Residuals for simulation of impinging jet located between cylinder for different inlet velocities. 50 3.40 Residuals for simulation of impinging jet located on cylinder for different inlet velocities. . 50

3.41 Illustration of the nine positions of interest (grey) in a group of cylinders . . . 52

4.1 Cooling time of a single cylinder exposed to various flows . . . 53

4.2 Heat transfer coefficient and electric power from measurements in relation to cylinder position and fluid velocity, without impinging jets. . . 54

4.3 Heat transfer coefficient and electric power from measurements in relation to cylinder position and fluid velocity, impinging jets between cylinder. . . 55

4.4 Heat transfer coefficient and electric power in relation to cylinder position and fluid velocity 55 4.5 Heat transfer coefficient (h) from numerical simulation in relation to cylinder position and fluid velocity, no jet. . . 57

4.6 Heat transfer coefficient (h) from numerical simulation in relation to cylinder position and fluid velocity, jet between cylinder. . . 58

4.7 Heat transfer coefficient (h) from numerical simulation in relation to cylinder position and fluid velocity, jet on cylinder. . . 58

A.1 Non-dimensional main inlet velocity (U/Ub) profile, Ub=0.75m/s. . . 68

A.5 Non-dimensional main inlet velocity (U/Ub) profile at Y = 10, 50, 150, 250 and 290 mm . 70 A.6 Non-dimensional main inlet velocity (U/Ub) profile at Z = 10, 50, 150, 250 and 290 mm . 70 B.1 Main inlet turbulence intensity (Tu) at Y, Ub=0.75m/s. . . 71

B.2 Main inlet turbulence intensity (Tu) at Z, Ub=0.75m/s. . . 71

B.3 Main inlet turbulence intensity (Tu) at Y, Ub=1.5m/s. . . 72

B.5 Main inlet turbulence intensity (Tu) at Y, Ub=7.5m/s. . . 73

C.1 3D main inlet velocity, U∞=0.75m/s. . . 74

C.2 3D main inlet turbulence intensity profile, U∞=0.75m/s. . . 74

C.4 3D main inlet turbulence intensity profile, U∞=1.5m/s . . . 75

C.6 3D main inlet turbulence intensity profile, U∞=7.5m/s . . . 76

D.1 Main inlet velocity, turbulence intensity and turbulence kinetic energy, Ub=0.75m/s . . . 77

D.2 Main inlet velocity, turbulence intensity and turbulence kinetic energy, Ub=1.5m/s . . . . 78

D.3 Main inlet velocity, turbulence intensity and turbulence kinetic energy, Ub=7.5m/s . . . . 79

E.1 Velocity profile along the horizontal axis for each impinging jet, UJ et=25m/s . . . 80

(11)

List of Tables

2.1 Values of skewness and its corresponding quality . . . 15

2.2 Different flow regimes around a circular cylinder. . . 18

3.1 Insulation study on a single cylinder with three configurations. . . 32

3.2 Study regarding the influence in the temperature measurements due to the placement of the thermocouples. . . 33

3.3 Average velocity of the horizontal velocity profiles . . . 40

3.4 Average velocity of the vertical velocity profiles . . . 40

3.6 Solution methods . . . 46

3.7 Mesh quality for the first, coarser mesh containing 6834886 nodes, used during the mesh dependency study. . . 48

3.8 Mesh quality for the second, finer mesh containing 12527470 nodes, used during the mesh dependency study. . . 48

3.9 Mesh quality for the third, finest mesh containing 23747413 nodes, used during the mesh dependency study. . . 48

3.10 Impact of adjacent heated cylinders . . . 51

3.11 Different cases investigated in the cooling study of one cylinder. . . 51

3.12 Simulation overview . . . 52

4.1 Measurements on a single cylinder without impinging jets . . . 54

4.2 Results from the empirical study on the wind tunnel for bulk velocities of 0.75 m/s and 1.5m/s without impinging jet. . . 56

4.3 Results from the empirical study on the wind tunnel for bulk velocities of 0.75 m/s and 1.5m/s with impinging jet activated placed between cylinder. . . 56

4.4 Results from the empirical study on the wind tunnel for bulk velocities of 0.75 m/s and 1.5m/s with impinging jet activated placed on cylinder. . . 57

4.5 Result from the numerical study on the wind tunnel for bulk velocities of 0.75 m/s and 1.5 m/s without jet. . . 59

4.6 Result from the numerical study on the wind tunnel for bulk velocities of 0.75 m/s and 1.5 m/s with impinging jet located between cylinder. . . 59

4.7 Result from the numerical study on the wind tunnel for bulk velocities of 0.75 m/s and 1.5 m/s with impinging jet located on cylinder. . . 60

4.8 Comparison between the heat transfer coefficient obtained through experiments and nu-merically simulations I) . . . 60

4.9 Comparison between the heat transfer coefficient obtained through experiments and nu-merically simulations II) . . . 61

4.10 Comparison between the heat transfer coefficient obtained through experiments and nu-merically simulations III) . . . 61

5.1 Average heat transfer coefficient of the in-line tube bank for different configurations. . . . 65

E.1 Average velocity of the horizontal velocity profiles, . . . 80

(12)

Chapter 1

Introduction

This thesis was conducted on behalf of the division of energy (ENSYS), which in turn is a subdivision to the department of management and engineering (IEI), at Linköping Universitet (LiU) for Höganäs AB in cooperation with Gävle Högskola (HiG). This chapter will further introduce the reader to the background, goal and limitations of this thesis.

1.1 Background

Metallurgical cooling processes is an area of importance as efficient cooling will increase the productiv-ity, have a potential of improving material properties and increase energy efficiency. H¨ogan¨as AB is a company specialized in metal powder production and a tunnel oven is used as a part of their heating and cooling process. The heating process is achieved by traversing steel powder which is contained in circular cylinders made out of a ceramic material, in groups of 25 through the tunnel oven (Fig. 1.1). The cylinders are placed on top of a rail-bounded car which is traversed through the tunnel by pushing in more rail-bounded cars creating a continuous process. As the cars are travelling along the tunnel oven the cylinders will gradually be heated up to around 1200◦C. When the heating process is completed the cars moves further along the tunnel oven into the cooling area. The cooling area have two impinging jets on each of walls responsible for cooling the metal powder. In the cooling area the cylinders are finally cooled to about 250◦C.

As of now the cooling distribution of each group of cylinders is fairly unknown as measurements inside the oven are limited due to the high temperature. H¨ogan¨as AB has therefore expressed a need to investigate the current cooling performance and the possibilities of improvements as a basis for a remodeled tunnel oven, which will take shape and replace the old one in the next couple of years.

Figure 1.1: Schematic drawing of the tunnel oven showing the iron powder entering through the tunnel oven.

1.2 Aim of Study

The aim of this thesis is to use a miniature model of the tunnel oven in order to investigate the cylinder group’s (also known as in-line tube bank) cooling performance with and without impinging jets by doing

(13)

measurements. A computational fluid dynamics (CFD) model will be made in order to make comparisons with the collected data for verification of the models ability to predict the phenomena observed in the tunnel oven model. If the CFD model is able to replicate the results from the miniature model with good agreement, further tests may be conducted numerically and in the future lead to a new, improved tunnel oven at H¨ogan¨as. This thesis will end with suggestions for improvements and recommendations for further studies based on the discoveries made.

1.3 Limitations

Due to the test facility being located in G¨avle at the University of G¨avle without access to the required simulation software, measurements and simulations could not be done simultaneously. In addition with the number of different possible measurement combinations being plenty. Limitations had therefore to be made in order to keep the set time frame for a master’s thesis of 20 weeks. The implementation of the thesis work was therefore divided into two parts; the measuring part and the simulation part.

The time frame for the measuring part relied heavily on the success of acquiring the correct behaviour of the flow for both the main inlet and the side jets. The measurements were conducted on one of the possible three rail-bounded cars which can be mounted in the miniature tunnel model at the same time, i.e. 25 cylinders. This was done mainly out of concern for the computing power needed for the CFD simulations otherwise being too large and unwieldy. Out of the 25 cylinders only nine of the positions were chosen to be of interest (Fig. 3.41) as the distribution of these cylinder will be a good representation of the overall cooling performance. The positions are expected to include both highly and weakly cooled cylinders and therefore be enough to use as verification for the CFD model.

The CFD analyses will only concern steady state simulations due to time limitations. Transient simula-tions were predicted to be too time consuming regarding both simulation time as well as preparing the model to obtain satisfactory results.

As numerical investigations of this proportion had high demands on the computational power, a good computer was vital for the ongoing of the work. During the time of the project access to a computer cluster at the national supercomputer centre (NSC) with 20000 CPU-hours per month was available. The local computers used for less computational intensive analyses consisted of two four-core processors with 2.66 GHz each with 48 GB ram memory. The commercial CFD software used for the numerical investigation was ANSYS Fluent 16.1.

(14)

Chapter 2

Theory

This chapter is mainly divided into three parts where the first part deals with the theory regarding the measurement instruments used for measurements in the miniature tunnel oven model (also referred as wind tunnel), e.g. the Pitot tube and the hot wire anemometer to mention a few. The second part is concerning the theory of fluid dynamics, CFD and heat transfer with regard to the numerical investigation consisting of the CFD model. Some topics mentioned are flow characteristics around a circular cylinder, impinging jets and different turbulence models. Finally, the third part concerns earlier studies of related problems which will be used as a foundation for this thesis.

2.1 Measurement Methodology

In order to obtain reliable measurements of the speed of air flow measurements were carried out using both a pitot tube and a hot wire anemometer (CTA). The theory regarding these two measuring methods as well as for other measuring units will be discussed in this chapter.

2.1.1 Pitot Tube

The Pitot tube is a measuring instrument which uses the total pressure (pt) and the static pressure (ps) to

obtain the velocity of the air by use of Bernoulli’s equation, Eq. (2.1). By installing the pitot tube in-line with the air stream values for the total pressure are obtained. By connecting the tube to a manometer and by keeping the reference port open the atmospheric pressure as the static pressure is obtained.

P1 ρ + 1 2V 2 1 + gh1= P2 ρ + 1 2V 2 2 + gh2 (2.1)

Bernoulli’s equation can be simplified by making the assumption of constant air density (due to the low air speed) making ρ a constant as well as by making the assumption of having a negligible difference in height of the fluid, see Eq. (2.2). This also means that the temperature of the two points also must be constant.

h1= h2 (2.2)

Assuming that the air stagnates at the inlet of the Pitot tube isentropically, adiabatically, and frictionless making the total pressure equal to the stagnation pressure and therefore making the inlet velocity zero results in Eq. (2.3), which is a simplified form of the Bernoulli’s equation.

pt= ps+

1 2ρV

2

2 (2.3)

Finally, by rewriting equation (2.3) the equation for velocity is obtained as equation (2.4).

V = s

2(pt− ps)

(15)

𝐼𝐼)

𝐼)

𝑝𝑠 5

Figure 2.1: Schematic drawing of two kinds of Pitot tubes I) simple Pitot tube with the static pressure inlet located on the manometer and II) static-Pitot tube with the static pressure inlet located on the tube. Where 1) inlet, 2) outlet, 3) plastic tube connecting the tube to the manometer, 4) the manometer for displaying the pressure difference and 5) the static pressure inlet for the static-Pitot tube.

Although pitot tubes are commonly used in industry the knowledge of how to use it properly is not as widely known. As stated earlier there are a couple of assumptions made when deriving the equations for velocity and pressure. However, these assumptions are not always valid or could at least introduce errors depending on certain factors i.e. the surrounding environment, way of mounting the pitot tube, and temperature of the fluid. Thus may lead to a change in air density, clogging of the tube leading to errors in the pressure, and deviations from the assumption of a perfect gas. The type of pitot tube could also affect the measurements, if the static pressure inlet is located on the pitot tube itself instead of on the manometer for instance. By having the inlet located on the tube the importance of having the pitot tube in-line with the flow increases as the static pressure inlet needs to be perpendicular to the flow to avoid being influenced by the dynamic pressure. If the tube is correctly installed the difference between these two tubes are relatively small as the static pressure in the flow and the atmospheric pressure are almost equal. [1]

Pitot tubes however are considered a simple and cost effective way of measuring velocities. As the tube diameter can be as small as a few millimeters it can be inserted into narrow spaces and cause small disturbances to the flow. Earlier measurements and studies shows that the accuracy of a Pitot tube are within 1% agreement to hot wire anemometers in turbulent flows within Re of 11100 and 67000 [2].

2.1.2 Hot Wire Anemometer

The hot wire anemometer also referred to as a constant temperature anemometer (CTA) is another device used to measure the velocity of the flow as well as the turbulence. The CTA consists of a small wire sensor mounted between two plated stainless steel supports. The typical size of the wire sensor is 5 µm in diameter and approximately 1-3 mm in length. [3]

Due to the high electric resistance in the wire it will heat up when sending an electric current through it. The wire is then cooled by its surrounding flowing medium, in this case air. The general principle is that the heat transferred from the hot wire to the cold surrounding fluid, generates a relationship between the fluid velocity and the electric output. The wire is usually made out of tungsten or platinum which suits well due to its high temperature coefficient of resistance. [4]

(16)

1 2 3 4 5 6 𝑈∞

Figure 2.2: Schematic drawing of a hot wire, where 1) wire sensor, 2) wire supports, 3) the hot wire body, 4) hot wire fitting, 5) attachment of the hot wire fitting to the traverse unit and 6) wires connecting the hot wire to the A/D board.

The governing equation for a CTA can be seen in Eq. (2.5), where E is the energy stored in the wire, W is the power generated by the heater and H is the heat transferred to the surrounding. The CTA is kept at a constant temperature and therefore the energy does not change with time resulting in, Eq. (2.6). Equation (2.7) is used to describe the energy stored in the wire where Cw is the heat capacity of the

wire and Twis the temperature of the wire. Equation (2.8) is used to define the relationship between the

generated heat, electric current, and wire resistance (I and Rwrespectively). Heat can be transferred by

convection to the fluid, conduction to the wire supports, and radiation to the surroundings, Eq. (2.9). In an equilibrium case the heat storage is zero, which results in the heat generation is equal to the heat loss (majority in the form of convection). After some simplifications Eq. (2.10) and (2.11) can be derived, which explain the relation between heat transfer and Reynolds number (velocity) and the voltage drop and fluid temperature. A, B and n are determined through calibration, N u is the dimensionless number relation between the conductive and convective heat transfer, Re is the Reynolds number, U is the flow velocity. [5] dE dt = W − H (2.5) W = H (2.6) E = CwTw (2.7) W = I2Rw (2.8)

H =X(Convection, Conduction, Radiation) (2.9)

N u = A1+ B1· Ren= A2+ B2· Un (2.10)

I2Rw= (Tw− Ta)(A + B · Un) (2.11)

The CTA is capable of measuring velocities in varying amount of turbulence intensity depending on the type of sensor chosen. Miniature wires are used for intensities up to 5-10% while gold plated wires can be used to intensities up to 20-25%. The angle of which the anemometer is mounted also affects the heat transfer and thus the measured speed. Ideally the anemometer should be mounted with the normal to the wire parallel to the medium flow (θ = α = 0). This is due to the heat transfer varying with the cosine of the angle between the wire normal and the velocity vector see Fig. 2.3 and Eq. 2.12 & 2.13, where α is the yaw angle, θ is the pitch angle, U (0) is the actual velocity of the flow, k is the yaw factor and h is the pitch factor. For increase of yaw angles > 0 (α) the effects of the prongs increases as they will be cooled by the flowing medium as well as blocking the flow. [3]

U (α)2= U (0)2(cos2α + k2sin2α)), θ = 0 (2.12)

(17)

𝑦

𝑈

∞

𝑧

𝑥

𝛼

𝜃

Figure 2.3: Yaw (α) and pitch (θ) angles of the bulk flow (U∞) in relation to the wire normal (x-axis) of

the CTA.

Hot wire anemometers are one of the standard tools for measuring air flows and if treated carefully offers great spatial resolution as well as high sampling frequency and low flow disturbance. One of the weaknesses with the CTA is its sensitivity to impurities in the flowing medium and this puts demands on the cleanliness of the flowing medium. Due to the small thickness of the wire, it can easily burn out or get damaged if not handled with care. [3]

2.1.3 Thermocouples

A thermocouple is an instrument used for measuring temperatures. This is done by use of two different wires which are connected at one end (junction end) and the other end is connected to a body with a known temperature (reference end), see Fig. 2.4. By installing the junction end in the fluid or environment of interest a difference in voltage is obtained between the two ends. By having the two wires of different metals the Seebeck effect is used to obtain the temperature (Eq. 2.14). The Seebeck effect shows that an electromotive force (Emf) is generated at the junctions of two wires of different materials. The Emf (ε) is the voltage converted by other forms of energy into electric energy [6].

ε = Z T2 T1 S12dT = Z T2 T1 (S1− S2)dT (2.14)

Where T1 and T2 are the temperatures of the reference end and the junction end respectively. The

coefficients S12 and S1, S2 are the Seebeck coefficient of the thermocouple and the two thermo-elements

respectively. The Seebeck coefficient is a relation between electricity and heat carried by electrons, hence having the SI unit (V/K) [7].

V

𝑇1

Wire 1

Wire 2

Reference end Junction end

𝑇2> T1

Figure 2.4: Illustration of a thermocouple

2.1.4 Orifice Plate

Orifice plate (also referred to as a restriction plate) is a device used to measure flow rate and was used as a extra measuring device to make sure the flow rate was correct (Fig. 2.5). The orifice plate creates a pressure drop along the pipe which can be converted to a mass flow and later to a flow velocity. An orifice plate follows the Bernoulli’s principle which states that an increase in the speed of a fluid occurs simultaneously with a decrease in the internal pressure [8]. The relation between pressure drop and flow

(18)

rate have been experimentally found by the manufacturer for a range of pipe and orifice plate diameters. Particularly for the pipe diameters of 104 and 200 mm and orifice plate inner dimensions of 35 and 155 mm (which was used in the experiment). See Eq. (2.15) and Eq. (2.16) for the respective relation, note that the unit for flow rate is in [l · s−1_{]. To get the desired velocity Eq. (2.17) was used to calculate the}

flow rate and thus the pressure drop could be obtained.

Qmain= 19.029 · ∆p0.49169 (2.15)

Qjet= 0.77274 · ∆p0.49557 (2.16)

Q = U A · 1000 (2.17)

Figure 2.5: Illustration of how the air flow was controlled by use of an orifice plate and measuring the resulting pressure difference ∆p. Where 1) inlet pipe, 2) orifice plate, 3) outlet pipe, 4) annular slot, 5) carrier ring and 6) two outlets for measuring pressure difference.

2.2 Fluid Dynamics

This chapter will explain important quantities e.g. von K´arm´an street vortices and Reynolds number as well as common flow characteristics occurring in similar problems. The theory behind three different numerical models (k − ω, k − and SST) as well as their characteristics and limitations will also be included as well as underlying theory regarding the closure problem, Navier-Stokes equations and some mesh characteristics.

2.2.1 Flow Characteristics

Flow around a circular cylinder is a well-known subject and has been studied for some time. If the cylinder is not rigidly mounted the forces induced by the vortex shedding may cause vibrations in the cylinder. As the bulk velocity in this case is relatively low the vibrations created will not be an issue however the vortex shedding phenomenon is. This phenomena occurs due to a separation of the boundary layer as a result of the negative pressure gradient at the rear of the cylinder caused by the shape of the cylinder relative to the flow. The vortices in the boundary layer are moving into the shear layer (which is the layer formed after the point at which the boundary layer disconnects from the cylinder) causing the shear layer to form a larger vortex (Fig. 2.6). Similarly, a vortex rotating in the reverse direction is created on the opposite side of the cylinder [9]. As the vortices on each side of the cylinder does not disconnect simultaneously a repeated swaying motion is created behind the cylinder, a so called von K´arm´an vortex street, see Fig 2.7.

(19)

Figure 2.6: Illustration of the boundary layer, shear layer and the vortices where U∞ is the free stream

velocity.

𝑈∞

Figure 2.7: Illustration of the von K´arm´an vortex street phenomena.

2.2.2 Non-Dimensional Quantities

The non-dimensional quantity that describes flow characteristic around a circular cylinder is the Reynolds number (Re), see definition in Eq. (2.18), in which ρ is the density of the fluid, U∞is the bulk flow velocity,

Lc is the characteristic length and µ is the dynamic viscosity of the fluid. In the case of a circular cylinder

the characteristic length is the cylinder diameter. Re is defined as the ratio of the inertial forces to viscous forces. Where the inertial forces is the force due to the momentum of the fluid and will rise with increased density and velocity. The viscous forces are due to the shear forces or the friction forces related to a fluid layer and its surrounding fluid layers. The Reynolds number gives a ratio between the two forces to determine which is the dominating force acting upon the fluid.

Re = Inertia forces Viscous forces=

ρU∞Lc

µ (2.18)

The reason to use a dimensionless number like Re is because of the similarity principle with respect to the Reynolds number. This principle states that mechanical similarity of a flow exists if the Reynolds number is equal for both flows. Mechanical similarity of a flow is defined as similar development of streamlines. So in other words, flow past two geometrical similar objects (e.g. two circular cylinders) are mechanically similar for different fluids, velocities and body sizes if the Re is identical [10]. Because of the above mentioned principle dimensional consideration have been extended to other quantities like force and frequency of vortex shedding.

The dimensionless coefficients for forces acting upon a body are defined in Eq. (2.19) and (2.20). The component of the total force acting in the free stream direction is defined as FD, D for drag, and the

component of the total force perpendicular to the free stream FL, L for lift. U∞ and ρ are the bulk flow

velocity and density respectively, A is usually the characteristic surface projected frontal area, CL is the

(20)

CL= 2FL ρU2 ∞A (2.19) CD= 2FD ρU2 ∞A (2.20)

The frequency of vortex shedding is defined as in Eq. (2.21), in which f is the frequency of vortex shedding, L is the characteristic length (cylinder diameter), U∞is the bulk velocity and St is the Stanton

number. [10]

St = f L U∞

(2.21)

2.3 Computational Fluid Dynamics

Computational fluid dynamics (CFD) uses mathematical modeling to investigate problems related to fluid flow, heat transfer, and chemical reactions by computer simulations. CFD is widely used in many fields e.g. aerospace, power generation, food and beverage industry to mention a few. CFD had been widely used since the 1990s as powerful computers started to be more affordable. The advantages of using CFD software compared to performing experiments are decreased lead time and cost for new designs, ability to study large systems which can be very hard and costly to perform and able to acquire unlimited detail level of results. There are also disadvantages with the use of CFD software, the main disadvantages being the costly licence fee and the hardware requirements. Other drawbacks are uncertainties related the mathematical models used to describe turbulence and other simplifications/assumptions needed to ease or enable calculation. [11]

2.3.1 Governing Equations of Fluid Flow

The governing equations of fluid flow represent mathematical statements of the conservation laws of physics:

• The mass of a fluid is conserved

• Newton’s second law: The rate of change of momentum of a fluid particle is equal to the sum of forces acting on the fluid particle

• First law of thermodynamics: The rate of change of energy is equal to the sum of the rate of heat addition to and the rate of work done on a fluid particle

The equation that describes the conservation of mass is usually called the continuity equation. Within a domain, the mass stays constant which mean that mass can neither be created or destroyed. The continuity equation is defined in Eq. (2.22), where ρ is the density, u, v & w are the velocity components in x, y & z direction of the Cartesian coordinate system.

∂ρ ∂t + ∂(ρu) ∂x + ∂(ρv) ∂y + ∂(ρw) ∂z = 0 (2.22)

The three Navier-Stokes equations describes conservation of momentum, momentum remain constant within a problem domain, and therefore can neither be created or destroyed, only change by action of force which is described by Newton’s second law. Navier-Stokes equations or just the momentum equations written in tensor form can be seen below, Eq. (2.23).

∂ui ∂t + uj ∂ui ∂xj = −1 ρ ∂p ρ∂xi +µ ρ ∂2ui ∂x2 j (2.23) The energy equation describes the conservation of energy, energy can neither be created nor destroyed, it transforms from one form to another but the total energy remain the same. The energy equation can be written in many forms. Equation (2.24) is written for an incompressible flow, where E is the internal energy, Φ is the viscous dissipation function seen in Eq. (2.25), ν is the kinematic viscosity, k is the thermal conductivity and T is the temperature.

(21)

∂E ∂t + uj ∂E ∂xj = Φ +1 ρ ∂ ∂xj k∂T ∂xj (2.24) Φ = ν 2 ∂ui ∂xj +∂uj ∂xi ∂ui ∂xj +∂uj ∂xi (2.25)

2.3.2 The Closure Problem

Making predictions on turbulent flow is and has been a difficult and important problem to solve for many years. The flow of a turbulent fluid typically has two related characteristics; a complex variation of velocity with respect to position and time as well as an instability to small perturbations. This makes tracking a particular particle at any given time and location impossible [12]. An often used example explaining this phenomena is one with water flowing from one reservoir to another through a circular pipe. If the water is flowing slow enough to maintain a fully laminar flow the experiment is close to reproducible. This is not the case for a fully turbulent flow as the flow is too unstable and varying. The turbulent velocity field appears due to small fluctuations in e.g. temperature, fluid density and perturbations in adjacent walls. The Reynolds number (Re) is a dimensionless parameter for determining whether the flow is turbulent or not. For low values of the Reynolds number the perturbations in the fluid are damped away by the viscosity of the fluid. For high values of Re the viscosity is overpowered by the shearing effects of the perturbations in the fluid [12]. Engineering models and software based on these have been implemented in order to model a representation of turbulence. The Reynolds-Averaged Navier-Stokes (RANS) is an example of modeling strategy for turbulence [13]. As the RANS model is obtained by averaging the Navier-Stokes equations the velocity fluctuations will still appear and the problem of ”closing” appears. In order to explain the occurrence of this phenomenon further the so-called Reynolds averaging procedure will be followed. The fluctuations are averaged and compensated by additional terms representing the effects of the fluctuations which disappears during the averaging process [14].

ui(x, t) = ¯ui(x, t) + u0i(x, t) (2.26)

P (x, t) = ¯P (x, t) + P0(x, t) (2.27)

Where over bar and prime denotes time average and fluctuating respectively for the velocity u(x, t) and pressure fields (P (x, t)), i denotes a component in the velocity vector field. As per definition the average of the fluctuating part of the velocity is zero [13]. Inserting equations (2.26) and (2.27) into (2.23) yields an expression for the mean velocity (Eq. (2.28)). The fluid density (ρ) and averaging the kinematic viscosity (ν) are constant and the fluid is incompressible (∇· u = 0).

∂ ¯ui ∂t + ¯uj+ ∂ ¯ui ∂xj +∂u 0 iu0j ∂xj = −1 ρ ∂ ¯P ∂xi + ν∂ 2_u_¯ i ∂x2 j (2.28) Comparing Eq. (2.28) with Eq. (2.23) shows that they are similar except for the Reynolds stress tensor (Rij = u0iu0j) which represents the time average of the fluctuating parts of the velocity. As mentioned

earlier is it not possible to predict the fluctuations of a turbulent flow and therefore the fluctuations can not be calculated analytically (at this time) and for that reason must any reference to the fluctuations be removed (the closure problem). A work around this problem is to approximate the stress term, Eq. (2.29). Note that it is in the simplest form.

Rij = −νT(x)

∂ ¯ui

∂xj

(2.29) Where the variable νT(x) denotes the turbulent eddy viscosity. This simplification was proposed by

Joseph Valentin Boussinesq and have since be called the Boussinesq hypothesis.

2.3.3 Standard k − Turbulence Model

The model which is considered to be the simplest of the turbulence models and therefore commonly used in industry is the k- model. Thanks to its simplicity it is also considered to be one of the most well known models. The k- model is made up of two equations in which two extra transport equations are

(22)

included. The two variables which are thereby included are the turbulent kinetic energy (k or TKE ) and the turbulent dissipation (). By including these the diffusion and convection of turbulent energy are therefore taken into account i.e the turbulent properties of the flow, (Eqs. 2.30, 2.31) [15], some terms within the mathematical formulas are equations and are defined in Eq. (2.32) - (2.36). Note that in Eq. (2.32) the Reynolds stress tensors can be substituted by Eq. (2.29) resulting in Eq. (2.33), the substituted turbulent eddy viscosity term will in this case be defined as in Eq. (2.34). Sk and S are

user-defined source terms and finally the constants are presented. The model uses a so called zero based assumption for the boundaries which means that no extra boundary conditions needs to be specified for the wall boundaries. [16]

The k- model can be summarized as a robust model and commonly used model despite it being sensitive to large adverse pressure gradients. The low sensitivity to turbulence in the free stream and the accurate predictions of the wall boundary flow makes it a reliable model for its low cost. [17]

Even though the k − model is so widely used it has it’s limitations, where one of the biggest being the sensitivity to adverse pressure-gradients. Under these circumstances the model predicts too high levels of the the shear-stress causing separation be delayed or even neglected. This issue can however be improved by using certain corrections i.e replacing the -equation. [18]

∂ ∂t(ρk) + ∂ ∂xi (ρkui) = ∂ ∂xj h (µ +µt σk )∂k ∂xj i + Pk+ Pb− ρ + Sk (2.30) ∂ ∂t(ρ) + ∂ ∂xi (ρui) = ∂ ∂xj h (µ +µt σ ) ∂ ∂xj i + C1 k(Pk+ C3Pb) − C2ρ 2 k + S (2.31) Pk = −ρu 0 iu 0 j ∂uj ∂xi (2.32) Pk= ρνT(x) ∂uj ∂xi (2.33) νT = Cµ k2 (2.34) Pb= βgi µt P rt ∂T ∂xi (2.35) β = −1 ρ ∂ρ ∂T p (2.36) C1= 1.44, C2= 1.92, Cµ= 0.09, σk= 1.0, σ= 1.3

2.3.4 Standard k − ω Turbulence Model

One of the models created in order to resolve some of the limitations of the k − model is the k − ω model. One of these limitations being the adverse pressure-gradients discussed previously. The model is also accurate used in free shear flows and separated flows. However, the model has other limitations i.e. one of them being the free stream specific dissipation rate (ωf). By varying this variable the magnitude

of the eddy-viscosity rate can vary by more than 100 % [18].

In ANSYS Fluent the k−ω model uses the formulation made by Wilcox [19]. By adding two modifications; a cross-diffusion term and a built in stress-limiter modification some of the short comings of the model are remedied. The troublesome consequences caused by the values of ωf are one of them [20]. The turbulent

properties of the model, turbulence kinetic energy (k) and specific dissipation rate (ω), can be obtained from the transport equations (Eq. 2.37 2.38) [19], the definitions of the terms can be seen in Eq. (2.39) - (2.44). The k − ω model can be summarized as robust, relatively cheap and modifiable [20] [21].

∂ ∂t(ρk) + ∂ ∂xi (ρkui) = ∂ ∂xj Γk ∂k ∂xj + Gk− Yk+ Sk (2.37)

(23)

∂ ∂t(ρω) + ∂ ∂xi (ρωui) = ∂ ∂xj Γω ∂ω ∂xj + Gω− Yω+ Sω (2.38) Γk = µ + µt σk (2.39) Γω= µ + µt σω (2.40) Gk = −ρu 0 iu 0 j ∂uj ∂xi (2.41) Gω= α ω kGk (2.42) Yk = ρβ∗fβ∗kω (2.43) Yω= ρβfβω2 (2.44)

2.3.5 k − ω SST Turbulence Model

The shear stress transport (SST) model was derived from the new base line (BSL) model in order to eliminate the free stream dependency of the of the k − ω model. The transition from the BSL model to the SST model was inspired by the assumption used in the Johnson-King (JK) model. The assumption was that the principal turbulent shear-stress was proportional to the turbulent kinetic energy. This assumption makes it possible to use the k − ω model in the boundary layer and transformed into a k − formulation in the free shear-layer [22]. This is the fundamental idea behind the SST model; to use the best parts of the two models and combining them into one. Making the SST model usable for low Re without any extra damping and avoiding the sensitiveness of the k − ω model in the free stream region [16]. ∂(ρk) ∂t + ∂(ρUik) ∂xi = ePk− β∗ρkω + ∂ ∂xi h (µ + σkµt) ∂k ∂xi i (2.45) ∂(ρω) ∂t + ∂(ρUik) ∂xi = α1 νt e Pk− βρω2+ ∂ ∂xi h (µ + σωµt) ∂ω ∂xi i + 2(1 − F1)ρσw2 1 ω ∂k ∂xi ∂ω ∂xi (2.46) νt= a1k max(a1ω, SF2) ; S =p2SijSij (2.47) Pk = µt ∂Ui ∂xj ∂U_i ∂xj +∂Uj ∂xi → ePk= min(Pk, 10· β∗ρkω) (2.48) F1= tanh nn minhmax √ k β∗_ωy, 500ν y2_ω , 4ρσω2k CDkωy2 ioo (2.49) F2= tanh hh max2 √ k β∗_ωy, 500ν y2_ω i2i (2.50) CDkw = max 2ρωω2 1∂k∂ω ω∂xi∂xi , 10−10) (2.51)

Where k is the turbulence kinetic energy, ω is the specific turbulence dissipation, y is the distance to the nearest wall, S is the invariant measure of the strain rate, ρ is the density and Ui is the mean velocity

of the flow. F1 and F2 are the blending functions which makes the SST model switch between the two

(24)

2.3.6 Law of the Wall

The no-slip condition imply that a viscous fluid at a surface boundary will ”stick” to the surface and therefore the velocity will be zero, see Fig. 2.6. The rapid change of velocity close to the surface, also called velocity gradient, is of importance to understand because how the velocity change with variation of distance to a wall. The law of the wall describe this relationship, see Eq. (2.52) and (2.53), in which the non-dimensional velocity and distance are called u-plus, u+_{, and y-plus, y}+_{, respectively, (Eq. (2.54)}

and (2.55)). κ is the Von K´arm´an constant (≈0.41), ln is the natural logarithm and C+ _{a constant}

(≈5.1), U∞ is the free stream velocity, uτ is the friction velocity which is defined in Eq. (2.56), ρ is the

fluid density, y is the distance to the wall and µ is the dynamic viscosity. The relation in Eq. (2.52) is applicable for distances close to the wall while Eq. (2.53), sometimes called the log law of the wall, is used further away from the wall, see Fig. 2.8. [11]

u+= y+ (2.52) u+= 1 κlny +_{+ C}+ _(2.53) u+=U∞ uτ (2.54) y+= ρuτy µ (2.55) uτ= r τw ρ (2.56)

Figure 2.8: The law of the wall can be seen with Eq. (2.52) and (2.53), which are a good representation within their distinct interval to the wall [24].

2.3.7 Boundary Layer Theory

The y+ values are usually divided into three intervals due to the dominant forces acting upon the fluid. The viscous/linear sub-layer (y+< 5), the buffer layer (5 < y+< 30) and log-law layer (30 < y+< 500).

(25)

In the viscous sub-layer the fluid is in contact with a wall and the shear stress is relatively constant and equivalent to the wall shear stress. The fluid closest to the wall is dominated by viscous effects. In the buffer layer, viscous and turbulent stresses are comparable in magnitude. In the log-law layer the turbulent (Reynolds) stresses dominate and the shear stress τ varies with distance from the wall. [11]

2.3.8 Wall Function

Wall functions use the relationship between the non-dimensional velocity and distance from a wall (uni-versal behaviour of near-wall flows) in order to predict the near wall flow. By the use of the wall function the mesh requirement close to the wall can be reduced. Ansys [16], recommends the use of enhanced wall treatment. This enhancement makes the transition from the two-layer approach smoother under the condition that y+ ≈ 1, For y+ _{< 5 the two-layer approach uses the law of the wall as the relation}

between u+_{and y}+_{, Eq. 2.52, in the viscous sublayer,. Further away from the wall at the second layer of}

the two-layer approach where the viscous effects are negligible the relation between u+ _{and y}+ _{is derived}

using the log law of the wall, Eq. 2.53. The enhanced wall function in Fluent however requires that the law of the wall are formulated in one expression and therefore applicable for the entire wall region, see Eq. (2.57), where (Γ) is the blending function (Eq. 2.58). [16] [11]

u+= eΓu+_lam+ eΓ1u+ turb (2.57) eΓ= −a(y +₎4 1 + by+, a = 0.01, b = 5 (2.58)

2.3.9 Mesh

To resolve fluid flow in a domain using mathematical models, the flow domain has to be divided into smaller sub-domains. The shapes of these sub-domains are usually in the form of triangle or quadrilateral for two dimensional domains and in the shapes of tetrahedron, pyramid, triangular prism and hexahedron for tree dimensional domains. Although more complicated shapes exist they are not as commonly used as the ones mentioned above. The sub-domains are usually called cells or elements, while all cells or elements is called mesh or grid. The density of the mesh is of importance as a denser mesh is usually able to more accurately resolve the fluid flow inside a fluid domain. Furthermore local refinements are often a necessity, specifically at wall boundaries, as the velocity gradient are often higher around those areas.

2.3.10 Mesh Characteristics

The first step in making a good mesh is to understand the problem and create the mesh thereafter as there are no perfect mesh that will suit every problem. There are numerous mesh quality criterion’s used as guidance for creating a suitable mesh. Three of these are presented below with tables explaining the numerical intervals as they are presented in ANSYS and its corresponding quality.

The Jacobian-ratio is a measure of how close to ideal shape a cell is by values from 1 (being a perfect shape) and increasing as the shape degenerates. The Jacobian-ratio can be increased until the cell col-lapses, leading to errors, see Fig 2.9.

(26)

1 30

100

Figure 2.9: Illustration of the Jacobian ratios for quadrilateral cells with a Jacobian ratio of 1, 30 and 100 respectively [16].

Skewness is a measure of how close to an ideal shape each element is. The measure of skewness ranges from 0 to 1 where 0 indicates an ideal, equilateral, shape and 1 indicates the furthest from ideal shape, the most degenerate shape. See Tab. 2.1 and Fig. 2.10

Table 2.1: Values of skewness and its corresponding quality Value of skewness Cell quality

1 Degenerate 0.9 - < 1 Bad (sliver) 0.75 - 0.9 Poor 0.5 - 0.75 Fair 0.25 - 0.5 Good > 0 - 0.25 Excellent 0 Equilateral 𝐼) 𝐼𝐼) 𝐼𝐼𝐼) 𝐼𝑉)

Figure 2.10: Illustration of different skewness level on triangular and quadratic elements. Where I) is an equilateral triangle, II) is a skewed triangle, III) is a equiangular quad and IV) is a skewed quad [16]. The ratio is a measure on how uniformly shaped the cells are. For a quadrilateral cell an aspect-ratio of 1 corresponds to a square with sides of equal length. As the aspect-aspect-ratio increases the more rectangular the shape becomes. A high aspect-ratio has its uses especially near walls where high accur-acy is required, i.e. to capture a boundary layer.

(27)

1 20

Figure 2.11: Illustration of a quadrilateral with different aspect-ratio [16].

2.4 Heat Transfer

The three basic mechanisms of heat transfer are conduction, convection and radiation. Conduction is the transfer of energy (heat) by microscopic collisions from the more energetic particles of a body to the adjacent, less energetic ones. Convection is the transfer of energy between a surface and the adjacent fluid that is in motion. Radiation is by which energy is emitted in the form of electromagnetic waves from a heated surface in all directions. Unlike conduction and convection, radiation does not need a medium in order for the heat transfer to take place. [25]

Fourier’s law of heat conduction Eq. (2.59) is used to describe the heat transfer mode of conduction. In which ˙Qcond is the rate of heat transfer [W], k is the thermal conductivity [W m−1K−1] which measure

the ability of a material to conduct heat. A is the area [m2_{] and dT/dx is the temperature gradient.}

˙

Qcond= −kA

dT

dx (2.59)

Convection can be described by Newton’s law of cooling Eq. (2.60), in which h is the convection heat transfer coefficient [W m−2K−1], Asis the surface area where convection heat transfer take place, Ts is

the surface temperature, and T∞is the free stream temperature. The heat transfer coefficient have to be

experimentally determined and the value depend on surface geometry, fluid motion, fluid properties and bulk fluid velocity. Convection is usually divided into natural or free convection and forced convection. The difference between the two is that in forced convection the fluid is forced to flow around the surface by external factor like a fan. Natural convection on the other hand, is due to the buoyancy effect of the fluid caused by temperature differences that result in density differences. Typical values of h range from 25-250 [W m−2K−1] for forced convection of gases. [25]

˙

Qconv= hAs(Ts− T∞) (2.60)

h = q

TS− T∞

(2.61) Radiation can be in an ideal case described by Stefan-Boltzmann law Eq. (2.62) in this case the surface emit radiation at a maximum rate. The surface in this ideal case is called a black body. σ = 5.670 · 10−8

[W m−2_K4_{] is the Stefan-Boltzmann constant, A}

sis the surface area and Tsis the surface temperature.

However all real surfaces emit less than that of a black body of the same temperature and is therefor described by Eq. (2.63). is the emissivity of a surface and range from 0 ≤ ≤ 1. [25]

˙

Qemit,max= σAsTs4 (2.62)

˙

Qemit= σAsTs4 (2.63)

For earlier mentioned reasons it is usually more convenient to use dimensional variables and the non-dimensional variable used for the heat transfer coefficient (h) is the Nusselt number (Nu). The Nusselt number is named after Wilhelm Nusselt and is considered as the dimensionless convection heat transfer coefficient. The expression for Nu is obtained by the ratio of convective to conductive heat transfer (Eq. 2.64), where k is the thermal conductivity of the fluid and Lc the characteristic length.

(28)

˙ Qconv ˙ Qcond =hLc k = N u (2.64)

As the Nusselt number increases so does the effective convection and pure conduction is obtained as Nu=1 [25].

2.5 Earlier Studies

Results from related previous studies are presented in this section, where some results have been used as a basis within this thesis. Other studies are presented solely for the purpose of providing a glance at the solutions, that are not locked to a specific configuration, to give a broader perspective to the reader.

2.5.1 Flow Passing a Circular Cylinder

Extensive experimental and numerical studies had been conducted on flow passing a circular cylinder. In the study by Mittal & Balachander [26], have compared two and three-dimensional simulation and found that three-dimensional simulation matched well with the experiment and thus indicating that it is the three-dimensionality of the flow that that create the difference between experimentally measured lift and drag forces and two-dimensional simulation. The three-dimensionality of the flow was identified at Re>180. The study by Cox et al. [27], have summarized experiment data and showed that the Strouhal number, Eq. (2.21) is around 0.2 over a large range of Re number ranging from around 200 - 100000. A general suggestion is to have a computation domain that is at least 5D (where D is the diameter of the cylinder) in the inflow direction to the cylinder, 15D in the outflow direction and 10D in the lateral direction [28]. Apelt & Fox [29] did experiments on cylinders with aspect ratio (A) ranging from 4 to 40 at Reynolds number 4.4 × 104 _{and have found that at A<7 vortex shedding does not occur. Aspect}

ratio is defined as a cylinder’s length divided by the cylinder diameter. Luo, Gan and Chew [30] did experiment on circular cylinder at Reynolds number 3.33 × 104 _{with aspect ratios of 4, 6 and 8. The}

drag coefficient, at various span wise locations was calculated by integrating the circumferential pressure distribution and was found to increase toward the free end but was most of the time smaller in magnitude than the drag coefficient of an infinitely long cylinder. Figure 2.12 and Tab. 2.2 show an overview of the flow regimes and the characteristics of each flow regime.

Figure 2.12: Drag coefficient (CD) for a circular cylinder with respect to Reynolds number [10].

(29)

Table 2.2: Different flow regimes around a circular cylinder [10]. Reproduced with permission.

The study by Morgan [31] have summarized experimental results for convective heat transfer of circular cylinders in cross-flow. The simplified equation for convective heat transfer is dependent on the Reynolds number and can be seen below, Eq. (2.65), D2 and n1 are constants and are determined experimentally,

N u is the Nusselt number (Eq. (2.64)) and Re is the Reynolds number. Morgan used the summarized experimental data to propose constants which are dependent on the range of Reynolds number, see Fig. 2.13. (N u)D,f = D2(Re)n_D,f1 (2.65) 10-4 10-2 100 102 104 106 Reynolds number [-] 10-1 100 101 102 103 Nusselt number [-]

Correlation for crossflow forced convection from cylinders in air

Figure 2.13: Proposed correlation for cross-flow forced convection from single circular cylinder in air. Recreated from [31].

(30)

2.5.2 Flow Passing a Tube Bank

The heat transfer depending on the position and pressure drop is an important function to study as this will determine the performance depending on e.g. the inlet velocity. Ikpotokin et al. [32] investigated a tube bank consisting of four columns of five parallel cylinders. The tube bank is placed in the middle of the tunnel spaced 12.5 mm from the walls with 25 mm spacing between the cylinders in the span wise direction, 18.75 mm in the in-line direction with a diameter of 12.5 mm. The height of the cylinders were the same height as the tunnel. It was shown that the heat transfer coefficient increased for each column in the down stream direction of the tube bank. The Nusselt number increased by 12.49 %, 11.85 %, 5.27 % from the first to the second, the second to the third and the third to the forth column respectively. This was occurring due to the turbulence increasing for each column but its rate were diminishing for each column. It is therefore more efficient to have more compact tube banks. As most of the flow travels between the cylinder the most optimal position in a heat transfer point of view is the middle row and farthest back in the stream wise direction [32].

Bae et al. [33] conducted a 3d numerical study on an in-line tube bank consisting of 10 rows of cylinders. A longitudinal pitch-to-diameter of SL/d=1.5, 1.75, 2, 2.25 and 2.5 with a transverse pitch-to-diameter

of ST/d=1.5. The domain consisted of one row of full rods and two rows of half rods (Fig. 2.14).

The periodic boundary conditions were applied for both the span-wise and transverse directions. The simulations where conducted using the Large Eddy Simulations (LES) method at a Reynolds number of 6300. The simulations show two flow regions appearing as expected; a high velocity region between the pipes in the stream-wise direction and a re-circulation area behind every pipe. The re-circulation tends to be containing asymmetric vortex patterns of one larger and one smaller vortex (which is in agreement with [34] [33]. 𝑈𝑈∞ 𝑦𝑦 𝑥𝑥 _𝑆𝑆 𝐿𝐿 𝑆𝑆𝑇𝑇 3𝑑𝑑 𝑃𝑃𝑃𝑃𝑃𝑃𝑃𝑃𝑃𝑃𝑑𝑑𝑃𝑃𝑃𝑃 𝑏𝑏𝑃𝑃𝑏𝑏𝑏𝑏𝑑𝑑𝑏𝑏𝑃𝑃𝑃𝑃𝑃𝑃𝑏𝑏 Figure 2.14: Illustration of the domain for flow over an in-line tube bank.

2.5.3 Tube Bank Configuration

Studies regarding the configuration of a tube bank shows that the two most commonly used are staggered configuration (right) and in-line configuration (left) (Figure 2.15). In a heat transfer perspective studies have shown that the staggered configuration is preferable as the flow collides more with the cylinders. This leads to an increase in the heat exchange i.e the ratio of convective to conductive ratio (Nusselt number, N u) [35]. Khan, Culham and Yovanovich showed that there is an increase in N u by ˜60% for the staggered configuration for a case with SL/D = ST/D = 1.25, where SLand ST are the longitudinal

and transverse distances between two adjacent tubes respectively. It is also shown that by increasing the spacing between the cylinders to SL/D = ST/D = 3 the N u number decreases indicating that an

(31)

𝑈∞ 𝑈∞

Figure 2.15: Illustration of in-line tube bank (left) and staggered tube bank (right) configuration.

2.5.4 Impinging Jet

Plenty of research has been conducted on jet impingement due to its high heat and mass transfer rate. By impinging a fluid upon a surface efficient and rapid cooling, drying or heating of the surface can be obtained. Therefore, the impinging jets are such a popular application in many engineering fields such as cooling of turbine blades, tempering metals and drying of textiles [36]. The impinging jet is usually divided into three different regions due to the different characteristics of the flow; the free flow region, the stagnation region and the wall jet region. The free flow region can further be divided into three different zones; the potential core zone, the developing zone and the fully developed zone (Fig. 2.16). The length and size of the free jet region is dependent on the distance between the impingement plate and the jet nozzle plate. For small distances between these two plates the developing and the fully developed zone may not exist. The fluid exiting the jet sets the ambient fluid into motion which in turn produces entrainment of mass, momentum and energy. This has multiple effects on the jet flow as well as the flow of the ambient fluid i.e. the behavior of the jet, increase of mass flow rate and temperature increase. The increase in temperature occurs only if the ambient fluid temperature is higher than the incoming jet [37]. The cone-like shape of the potential core, for a circular jet nozzle, is due to the increase of the shear layer ambient to the core. The inlet speed remains constant throughout the core and the length of the core varies with the turbulence intensity and the velocity profile of the nozzle [38]. The potential core zone turns in to the developing zone, a zone at which the flow starts to destabilize and the potential core has disappeared. The flow difference in the axial direction starts to decrease and a more evenly distributed velocity profile takes shape (fully developed) as the flow progresses into the third and final zone of the free jet region.

The stagnation region as well as the wall jet region are highly dependent on the obstacle obstructing the flow. As the flow hits the obstructing wall the axial transport of the turbulent normal stress and the axial momentum turns into static pressure [39]. The flow velocity of the wall jet region will decrease as the distance to the stagnation region increases [40]. It was also shown that the turbulence intensities as well as the Reynolds shear stresses is higher in this region than in the boundary layer or the free jet region. As indicated in the figure the angle of the stream lines in relation to the impingement plate increases as the distance [40].

(32)

Free jet region Potential core zone Developing zone Impingement plate Stagnation region Wall jet region Fully developed zone Potential core Boundary layer Jet

Figure 2.16: Illustration of an impinging jet hitting a flat plate with indications of each zone of the developing flow.

An impinging jet subjected to a cross-flow has slightly other characteristics than an undisturbed jet (Fig. 2.17). The free jet region remains similar as well as the stagnation region. The wall jet region however is deflected due to the pressure gradient across the jet. The wall jet forms a vortex wrapping around the jet on both sides rotating in opposite direction to each other and continues downstream as it decays [41].

Figure 2.17: Illustration of an impinging jet hitting a flat plate subjected to a cross-flow [41].

2.5.5 Jet Nozzle Shape

Investigations on how the heat transfer from a heated cylinder depend on the shape of the nozzle for an impinging jet has been carried out [42]. Experimental and numerical studies were conducted using three different shapes; circular, rectangular and square. The heated cylinder was kept at a constant heat flux while the hydraulic Reynolds number (Rehyd) was varied from 10000 to 25000. A modified Reynolds

number ( fRehyd) was also used were the mass flow rate is kept the same for all the shapes, as the mass flow

rate differs depending on the shape of the nozzle. The hydraulic diameter (dhyd/D) was kept constant

at 0.2 while the non-dimensional distance (h/dhyd) between the nozzle exit and the cylinder was varied

(33)

was preferable. Under that criteria the circular shaped nozzle showed better performance, higher Nusselt number at the stagnation point and adjacent regions. As the distance between the cylinder and the nozzle increases the Nusselt number decreases as the jet velocity decreases, which is true for all three shapes. [42] The shape of the associated body of the nozzle also affects the characteristics of the flow (Fig. 2.18). The velocity profile originating from a circular pipe indicates an increase in TKE at the edges due to the friction of the walls. The funnel shaped pipe however produces a homogeneous profile where the TKE is evenly spread over the cross-section. Over a sharp edged cross-section, i.e. an orifice plate, the highest velocity and TKE is obtained at the edges of the profile. [37]

u

r

u

r

u

r

Figure 2.18: Illustration of velocity (solid line) and turbulent kinetic energy (dashed line) varying with nozzle shape.

2.5.6 Influence Of Nozzle Arrangement

In industrial applications one impinging jet is usually not enough. The effects of different arrangements of multiple impinging jets has therefore been subjected to several studies. In-line and staggered arrange-ments with 24 nozzles with H = 2D (nozzle-to-plate distance) and S = 3D (jet-to-jet distance) where D is the orifice diameter has been studied by Makatar et al. [43]. The Reynolds number used during the study was Re=5000, 7500 and 13400. Numerical and experimental tests were conducted on an impingement surface. The distribution of temperature, Nusselt number and flow characteristics were measured. As the study was conducted in a confined volume with one outlet located at the end the cross-flow increased in the down-stream direction. The staggered configuration blocked the cross-flow more than the in-line con-figuration as the flow could easier pass between the jets for the latter. This resulted in a greater pressure difference for the staggered configuration resulting in a higher cross-flow velocity. Studies showed that a moderate cross-flow velocity is optimal for a high heat transfer as the cross-flow increases the intensity of the turbulence as it collides with the jet. As a result of this the in-line configuration had approximately 13 − 14% higher average Nusselt-number than the staggered configuration for Re=5000-13400. [43]

Experimental and Numerical Investigation of an In-line TubeBank’s Cooling Potential