Content uploaded by Efe Kinaci
Author content
All content in this area was uploaded by Efe Kinaci on Sep 09, 2015
Content may be subject to copyright.
University of Duisburg-Essen
Institute for Energy and Environmental Engineering
Chair of Fluid Mechanics
Bachelor Thesis
Numerical and Experimental Investigation of The Rotor
Blades of An HAWT With A Profile HKAS Inspired by a
Maple Seed
Supervisors: Prof. Dr. –Ing. Ernst von Lavante
Prof. Dr.-Ing. Wojciech Kowalczyk Dipl. –Ing. Harun Kaya
Dipl. Ing. Harun Kaya
Author: Kinaci, Mustafa Efe
Matriculation Number: 2232889
October 3, 2011
Eidesstattliche Erklärung
Ich versichere, dass ich die eingereichte Bachelorarbeit ohne fremde
Hilfe verfasst und andere als die in ihr angegebene Literatur nicht
benutzt habe und dass alle ganz oder annahernd übernommenen
Textstellen sowie verwendeten Grafiken und Tabellen kenntlich
gemacht sind; ausserdem versichere ich, dass die Ausarbeitung in dieser
oder ähnlicher Form noch nicht anderweitig als Prüfungsleistung
vorgelegt und bewertet würde.
Datum Unterschrift Unterschrift
Acknowledgments
Firstly, I would like to thank the head of Fluid Mechanics department Prof. Dr.-Ing.
Ernst von Lavante for introducing me to fluid mechanics and fluid dynamics. His
vast knowledge on these and many other subjects has captured my total attention
and made me advance in these subjects. I would also like to thank Prof. Dr.-Ing.
Wojciech Kowalczyk for his support.
This task could not have been completed without the help of Dipl. Ing. Harun Kaya,
who has given me this topic, and I thank him especially for showing me the support
to accomplish this task and giving me advices for my future endeavors. I would also
thank Dipl. Ing Ali Gedikli for giving me the start to learn the needed software’s
and helping me advance in them. I thank them for sharing their knowledge.
Last but not least I would like to thank all of my friends for morally helping me
during this hard period. I thank my family for always pushing me forward into a
more successful career and helping me in every aspect of my life, without their help
and support none of this could have been done. I thank them for picking me up
whenever I stumbled.
Table of Contents
1. Introduction 5
1.1 Motivation 5
1.2 Goal of Thesis 6
1.3 Overview 6
2. Theoretical Background 7
2.1 Wind Turbines 7
2.1.1 Origins 8
2.1.2 Aerodynamics of a Wind Turbine 12
2.2 Laminar and Turbulent Flows 18
2.3 Numerical and Experimental Setup 20
2.3.1 Gridgen 20
2.3.2 Star-CCM+ 24
2.3.3 Experimental Setup 32
3. Results and Comparison 34
3.1 Star-CCM+ 36
3.2 Experiment 42
3.3 Comparison of Results 44
4. Conclusion 46
5. Bibliography 47
List of Tables 2
List of Tables
Table 1: Continuum Physic Models and Definitions. 25
Table 2: The Different Regions and Their Explanations. 29
Table 3: Simulation Properties. 31
Table 4: The measurements gathered from experimental work. 43
Table 5: A table of the angle of attack for different installation angles. 44
List of Figures 3
List of Figures
Figure 1: Heron's Windmill Design. 8
Figure 2: Types of Vertical Axis Rotors. 10
Figure 3: Horizontal Axis Wind Turbine. 11
Figure 4: Detailed drawing of the parts of a HAWT. 11
Figure 5: Flow Model of Betz's Momentum Theory. 12
Figure 6: Figure of airfoil and the affecting forces. 15
Figure 7: A sketch of the boundary layer on an airfoil. 16
Figure 8: Angle of incidence. 17
Figure 9: Flow physics for a two-dimensional airfoil undergoing dynamic stall. 18
Figure 10: Laminar and Turbulent Flows. 19
Figure 11: The Database imported from Solid Works. 20
Figure 12: End top side view 21
Figure 13: The rotor domains' skewness. 22
Figure 14: The Volume Conditions 23
Figure 15: The length of the airfoil 27
Figure 16: Periodic Parts of the Model. 29
Figure 17: Outer Wall with Slip. 29
Figure 18: The turbine profile made out of maple seed. 32
Figure 19: The design of the experimental setup. 32
Figure 20: The experimental Set-up. 33
Figure 21: The location of the rotor profile inside the test tunnel. 33
Figure 22: Power Output for 30 Degree Installation Angle. 34
Figure 23: Power Output for 40 Degree Installation Angle. 35
Figure 24: Power Output for 60 Degree Installation Angle. 35
Figure 25: The velocity magnitude scene of 300rpm. 36
Figure 26: The velocity magnitude from negative y to plus z [the pressure outlet section]. 37
Figure 27: Velocity magnitude display right after the turbine. 38
Figure 28: Schematic diagram showing the air loads. 38
Figure 29: Pressure coefficient distributions of the HKAS airfoil for 0.03m, 0.05m, 0.07m,
0.08m and shows the streamline plots from CFD simulations for the corresponding
distances [0.03, 0.05, 0.07, 0.08 meters]. 40
Figure 30: Streamline results for 60 in the CFD simulation. 41
Figure 31: Streamline results for 30 in the CFD simulation. 41
Figure 32: Streamline results for 45 in the CFD simulation. 41
Figure 33: Streamline results for 70 in CFD simulation. 42
Introduction 5
1. Introduction
1.1 Motivation
The significant rise in the cost of petroleum oil and as the environment is becoming
worse the search for viable alternative technologies have increased. As one type of
renewable energy generation, wind power is not only environmental friendly but
also more mature in technology and able to be explored in larger scale compared
with other types of green energy. The EU has committed itself to the promotion of
renewable energy sources to tackle climate change [1]. National research programs
were initiated around the world to investigate the possibilities of using wind energy.
Wind turbines in Denmark generated 0.7 billion kwh in 1991, or 2.4% of
Denmark’s total electrical consumption. The California Energy Commission (CEC)
reports more than 15,000 turbines generated 2.5 billion kWh in California in 1990
[2]. Since August 2009, the first German offshore wind farm Alpha Ventus is also
operational [3].
Though wind turbines and windmills have been used for centuries, the application
of rotor aerodynamics technology to improve reliability and reduce costs of wind
generated energy has only been pursued in earnest for the past 25 years. Since wind
energy is a low-density source of power, it is important to maximize the efficiency
of wind turbines. Among other problems to be solved about wind turbines the
aerodynamic performance prediction is the basic one. With the development of
modern computer technology and simulation method of turbulence, numerical
simulation method has the potential to provide physically simulation of the wind
turbine flow field. Another critical aspect of the wind turbine that has not been
evaluated until recently is the blade itself. The blades angle of attack as well as its
shape has an effect on the performance of the turbine. A recurring problem is that
increasing the angle eventually forces the blade to stall.
If a technology could be developed to boost the operation of wind turbines, it would
be less stress on the countries with high dependence on fossil fuels and also an
environment friendlier solution for everyone.
Introduction 6
1.2 Goal of Thesis
Generating energy without harming the environment is one of the top priorities, and
using the earth’s wind power to do so is just another advantage. The accurate
prediction of the performance of wind turbines is of great importance when
designing economical and reliable wind turbines [4]. The aim of the present work is
to obtain aerodynamic predictions of HKAS turbine profile which is inspired by a
maple seed. The power output was to be determined off four different installation
angles [ and a constant velocity of 10 m/s. The simulation
results are compared with the experimental data from University Duisburg-Essen’s
laboratories, a small wind tunnel test, for validation. The testing tunnel size was 12
cm in diameter and the located turbine profile was approximately near that size.
Plexiglas was used as the material to craft this profile shape out of, with an
approximated thickness of 1.2 cm. The simulations were carried out in Star-CCM+
v6.04.014 and the design was created with Solid Works and meshing was done in
Gridgen V15.
1.3 Overview
The structure of this study is as follows. Information and detailed history of wind
turbine origins are stated at the first section of chapter 2. The following section
explains the different types of flows. At the end of chapter 2 the experimental set-up
as well as theory of the programs used and detailed information on how the
simulations were made is explained. The closing chapter summarizes and draws a
conclusion based also on these results. The results of the simulation and
experimental testing, and a comparison is also stated at the closing chapter.
Theoretical Background 7
2. Theoretical Background
2.1 Wind Turbines
The use of wind energy is not newly discovered. Simply, it was only easier to find
other more powerful means of energy rather than looking for alternate ways. The
procedures used to create energy from fossil fuels are slowly coming to a stopping
point. Most countries have realized the hazardous effects of these fuels. According
to the UK HM Treasuries’ Stern Review posted in 2006 the effective mitigation of
climate change will require deep reductions ,up to 60-80%, in greenhouse gas
emissions by 2050. Also the near depletion of fossil fuels is another reason for the
search of an effective and reliable energy sources.
Wind power all starts with the sun. When the sun heats up a certain area of land, the
air around that land absorbs the heat. After a certain temperature and due to the fact
that hot air is lighter than cold air, the heated air rises. When the hot air rises,
immediately the cooler air flows in to replace the free space and hence it creates
wind.
Wind turbines use the kinetic energy of the wind to generate electricity. In order to
capture this energy and convert it to electrical energy, one needs to have a device
that is capable of ‘touching’ the wind. This device, or turbine, is usually composed
of three major parts: the ‘rotor blades’, the drivetrain and the generator. The blades
are the part of the turbine that touches the wind and rotates about an axis. Extracting
energy from the wind is typically accomplished by first mechanically converting the
velocity of the wind into a rotational motion of the wind turbine by the means of the
rotor blades, and then converting the rotational energy of the blades into electrical
energy by using a generator [5].
Theoretical Background 8
2.1.1 Origins
The earliest example of windmills was first designed by the Greek engineer Heron
of Alexandria in the 1st century. It is also claimed that the Babylonian emperor
Hammurabi had planned the use of wind powered machines due to his interest in
irrigation projects around the 17th century B.C.
Figure 1: Heron's Windmill Design.
It is not entirely clear where the European’s have seen the windmills, but it has been
said that the Chinese were using windmills for draining rice fields. Some people
speculate that the European’s have learned about windmills from the Persians. The
first verifiable information about windmills in Europe is that they were used in the
Duchy of Normandy around the 1180’s [6]. Later on, Netherlands used these
windmills and made improvements on them. There are several kinds of windmills;
The first one is the Post mill. As the name suggests the mill’s main structure was
balanced on a large upright post so that it could turn to face the wind. The milling
machines were then stationed inside the hub. These windmills had four sails and
they were usually covered with fabric.
Theoretical Background 9
The other type of windmills used in Europe was Hollow-post mill or “Wipmolen”.
For this type of windmill, the body mounted is hollowed out to accommodate a
drive shaft. This type of windmill was used in the Netherlands first to drain the
wetlands, later for graining and wood cutting.
Tower windmill was widely spread in the Mediterranean regions. This structure had
no yaw, so it could only be turned in the direction of the wind manually.
The most advanced windmills were a type called the Dutch windmill. The entire
housing was a fixed structure, and only the top cap could rotate where the sails were
located. This allowed for the building of larger and more powerful windmills. The
model could support various machines like grain millstones and heavy pan grinders.
Naturally after the invention of steam engines the number of windmills started to
decrease all over Europe. Some new wind wheel ideas were thought of during the
Renaissance period but it wasn’t deeply considered until Wilhelm Leibniz, who
proposed numerous impulses for the construction of windmills. Bernoulli later on
applied his recently formulated basic laws of fluid mechanics to the design of
windmill sails. Also Euler did some research on the windmill sails. He was the first
to calculate the twist of the sails [7].
The turning point from wind wheels into modern wind turbines is marked by the
Danish scientist Poul la Cour. He was a pioneer of electricity generation by means
of wind power generation in the 19th century. He did many researches on how to
make the wind wheel more aerodynamic, and tested some of his ideas in a wind
tunnel which he had built himself. La Cour later on started building wind turbines,
which were widely used until the end of World War I, but afterwards the
construction decreased due to the fact that the oil prices became cheaper. However,
the dynamic properties of his wind turbines were not so high and needed to be
worked on. This job was taken gladly by many countries including Germany and
U.S.A.
Since the basic parts of a wind energy converter were known, the different types of
wind turbines were obtained mostly by the changes made in the wind rotor.
However, the wind rotor is not the only component. Gearbox, generator and control
systems are just as well necessary to change the rotational energy into electricity.
There are two main types of wind rotors, Vertical Axis Rotors and Horizontal Axis
Rotors. Vertical Axis Rotors were the earliest designs in wind turbines. These wind
turbines were not able to successfully use aerodynamic lift, until recently. French
engineer Darrieus modeled a new type of Vertical axis rotor known as the “Darrieus
Rotor”. This model was hard to build due to its shape and had no real advantages
Theoretical Background 10
with respect to horizontal axis rotors. The production costs were higher and the
power output could not be controlled by pitching the rotor blades. Another type for
vertical axis rotors is the Savonius design. This model is especially used for driving
small water pumps, but it has no real electricity generating value.
Figure 2: Types of Vertical Axis Rotors.
Horizontal axis wind turbine (HAWT) is the common equipment in wind turbine
generator systems in recent years. This is due to the fact that in propeller designs,
rotor speed and power output can be controlled by pitching the rotor blades about
their longitudinal axis. Rotor blade pitching is the most effective protection against
over speeding and extreme wind speeds. Another reason for the widely use of
HAWT is the rotor blade shape can be aerodynamically optimized. This is an
advantage because it can be optimized to achieve the highest efficiency, which is
known to be when the aerodynamic lift is exploited to a maximum degree.
Theoretical Background 11
Figure 3: Horizontal Axis Wind Turbine.
Every part of a wind turbine, even the oil can, be changed to have a better power
output but the most significant one is the rotor blades because of the aerodynamic
structure. Some description of the parts of a Horizontal Axis Wind Turbine is
shown in Figure 4. This figure also shows that the gearbox and the generator are
stationed in the nacelle of the turbine. The gearbox and the generator of a Vertical
Axis Wind Turbine are stationed at the base of the turbine.
Figure 4: Detailed drawing of the parts of a HAWT.
Theoretical Background 12
2.1.2 Aerodynamics of a Wind Turbine
The most effective change that can be done to the wind turbine is finding different
shapes for the rotor. The capability of the rotor to convert a maximum proportion of
the wind energy flowing through its swept area into mechanical energy is obviously
the direct result of its aerodynamic properties. With different shapes come different
properties.
The German aerodynamicist Albert Betz has formulated the physical laws of energy
conversion and the theory of wind rotor. Betz published writings in which he was
able to show that by applying elementary physical laws, the mechanical energy
extractable from air passing through a given cross sectional area is restricted to a
certain fixed proportion of the energy or power contained in the air stream. Betz’s
simple momentum theory, which assumes an energy converter working without
losses in a frictionless airflow, is based on the modeling of a two-dimensional flow
through the actuator disc. The airflow is slowed down and the flow lines are
deflected only in one plane. Although it contains simplifications its results are quite
usable for performing rough calculations.
Figure 5: Flow Model of Betz's Momentum Theory.
Theoretical Background 13
To understand the Betz’s momentum theory thoroughly, here are some background
calculations. The kinetic energy of an air mass m moving at velocity v can be
expressed as:
Considering a cross sectional area A, which the velocity v passes, the volume
flowing through a certain time unit, the so called volume flow is:
And the mass flow with the air density:
The equation expressing the kinetic energy of the moving air and the mass flow
yield the amount of energy passing through the cross section A per unit time.
However, as shown in Figure 5 the velocity before the converter () and the
velocity after the converter () are different. That is why we must consider the
conditions before and after the converter. Thereby changing the power P to:
Maintaining the mass flow (continuity equation) requires that the mass flow before
and after the converter is equal.
Thus;
From this equation it is shown that the maximum power is reached when is equal
to zero. However, this does not make sense physically. That would mean that the
velocity before the converter also has to be zero.
Theoretical Background 14
Using the law of conversation the force that air exerts on the converter can also be
calculated.
From the force we can calculate the power
With respect to this equation we can see that the flow velocity through the converter
is equal to the arithmetic mean of and:
Mechanical power output of the controller can be expressed as
The reference power for this output is the free-air stream power across the same
cross-sectional area but without the extraction of the mechanical power of the
converter.
The ratio between the mechanical power output and that of the undisturbed free-air
stream is the power coefficient.
According to Betz, the maximum ideal power coefficient should be 0.593. Since
Betz was the first to derive this value it is called the Betz factor. This value is the
maximum fraction of the power that can be extracted from the wind flow. To
calculate this value Betz had certain assumptions, the first one was that the rotor
does not have a hub, so an ideal rotor with infinite number of blades that does not
have any drag. Second, the flow would be incompressible so the density would be
constant, and heat transfer between the rotor and flow would not occur. Third, the
rotor has to be massless and the flow in and out of the rotor has to be axial. This
Theoretical Background 15
proves that the Betz factor is just an ideal coefficient. Reaching this value even with
today’s technology is hard because of the other constraints.
Today, the designing of an airplane wing or a rotor is simulated and experimented
upon by inspecting the airfoil cross-section of a blade element. If a horizontal blade
element is cut by a vertical plane parallel to the centerline the resulting section is
called airfoil section. The generated characteristics (generated lift and stall
characteristics) of the blade depend strongly on the geometry of the airfoil sections
that make up the blade [8].
Figure 6: Figure of airfoil and the affecting forces.
The motion of the air around the blade section produces pressure and velocity
variations which produce the aerodynamic forces and moments. It is possible to use
the equations of the motion for an inviscid flow to determine the pressure
distribution around the vehicle and hence the velocity of the air particles at the edge
of the boundary layers. For many high-Reynolds number flows, the flow field may
be divided into two regions: (1) a viscous boundary layer adjacent to the surface of
the rotor and (2) the essentially inviscid flow outside the boundary layer. The
Theoretical Background 16
Laminar boundary layer is a relatively thin layer with limited mass transfer and a
low velocity gradient near the wall can be seen. There is low skin friction in this
boundary layer. In Turbulent boundary layer the layer is thicker with considerable
amount of mass transfer, and with higher skin friction and higher velocity near the
surface [9].
Figure 7: A sketch of the boundary layer on an airfoil.
The shear and pressure forces can be resolved as the lift and drag forces along the
axis as shown in fig. 6. The lift force is the force component acting upward,
perpendicular to the direction of the undisturbed free-stream velocity. The
aerodynamic lift is produced primarily by the pressure forces acting on the vehicle
surface. The drag force is the net aerodynamic force acting in the same direction as
the undisturbed free-stream velocity. The aerodynamic drag is produced by the
pressure forces and by skin friction forces that act on the surface.
The lift and drag coefficients of an airfoil are functions of the angle of incidence
and fig. 8 shows the curves for a typical airfoil, the drag being drawn to five times
the scale of the lift. The lift coefficient varies linearly with the angle of incidence
for a certain range and then attains a maximum value at the critical angle of
incidence. The important working range of an airfoil is represented by the linear
part of the lift curve and in this range the drag is small compared with the lift, but
on approaching the critical angle the drag increases rapidly.
Theoretical Background 17
Figure 8: Angle of incidence.
After the critical angle of incidence of the airfoil is exceeded, stall starts to occur.
The stall occurs when the airflow separates from the upper side of the airfoil. The
Reynolds number dependency becomes smaller. The Reynolds number dependency
is related to the point on the airfoil where the boundary layer transition from
laminar to turbulent flow occurs [Fig. 7]. The way an airfoil stalls is very dependent
on the geometry. Thin airfoils with sharp nose tend to stall more abruptly than thick
airfoils. There are different stall behaviors and the explanation lies in the way the
boundary layer separates from the upper side of the airfoil.
The behavior of the viscous boundary layer is very complex and depends on the
curvature of the airfoil, the Re number, surface roughness and for high speed also
on the Mach number.
During the past decades, dynamic stall phenomenon has received a great deal of
attention of aerodynamicists and researchers from different research institutions all
over the world. Methodologies, through which the dynamic stall is represented,
mainly include three categories: experimental approaches, various semi-empirical
models, and computational fluid dynamics solutions.
Theoretical Background 18
Farren [10] first carried out
experiments on various British
airfoils in the 1930s to measure the
dynamic stall phenomenon. In the
1970s and the early 1980s,
Mc.Alister and McCroskey did
notable experimental dynamic stall
studies on different airfoils.
Schreck and Helin were the first to
provide a visual representation of
DSV (dynamic stall vortex) using
dye in a water tunnel and a detailed
set of surface pressure
measurements on a finite wing
[11].
2.2 Laminar and Turbulent
Flows
Experiments in flow pipes
demonstrated that two different
flow regimes exist – laminar and
turbulent. When laminar flow
exists in a system, the fluid flows in
smooth layers called laminae. A
fluid particle in one layer stays in
that layer. The layers of fluid slide
by one another without apparent
eddies or swirls. Turbulent flow, on
the other hand, exists at much
higher flow rates in the system. In this case eddies and vortices mix the fluid by
moving particles tortuously about
the cross section.
The existence of two types of flow is easily visualized by examining results of
experiments performed by Osborne Reynolds. In his experiments a transparent tube
is attached to a constant-head tank with water as the liquid medium. The opposite
end of the tube has a valve to control the flow rate. Dyed water is injected into the
Figure 9: Flow physics for a two-dimensional airfoil
undergoing dynamic stall.
Theoretical Background 19
water at the tube inlet and the resulting flow pattern is observed. For low rates of
flow the pattern is regular and forms a single line like thread. There is no lateral
mixing in any part of the tube, and the flow follows parallel streamlines. This type
of flow is called laminar or viscous flow.
As the flow rate of water is increased beyond a certain point, the dye is observed
not to follow a straight threadlike line but to disperse. The dyed water mixes
thoroughly with the pipe water as a result of erratic fluid behavior in the pipe. This
type of flow is called turbulent flow [12].
So the transition from the laminar to the turbulent state occurs if the momentum
exchange by molecular transport cannot compete sufficiently effectively with the
transport due to macroscopic fluctuations in flow velocity. Reynolds argued that the
transition from the laminar to the turbulent state occurs when a dimensionless
parameter exceeds a certain critical value [13]. The Reynolds number:
Where and v are the fluid density and viscosity, respectively and V and D are the
typical velocity and size scale of the flow, respectively. For straight circular pipes
the flow is always laminar for a Reynolds number less than about 2100. The flow is
usually turbulent for Reynolds numbers over 4000. However, the situation is also
more complex than what was originally presumed by Reynolds. For instance, the
numerical value of the critical Reynolds number depends on the flow and a number
of other factors such as the initial disturbance level.
Figure 10: Laminar and Turbulent Flows.
Theoretical Background 20
2.3 Numerical and Experimental Setup
In this chapter a brief introduction to the simulation programs that were used to do
this thesis is going to be given, as well as how it was done. The general programs
that are used to do are; Gridgen a meshing toolkit and for the simulation part Star-
CCM+ is used. The experimental part which took place at one of University of
Duisburg Essen’s laboratories is also shown in this chapter.
2.3.1 Gridgen
Gridgen is an interactive, graphical software package used to create 2D and 3D
quadrilateral, hexahedral, triangular, and tetrahedral grid meshes and finite element
models. Gridgen is employed in the construction of hybrid meshes as well, through
the use of prisms and pyramids. In this purpose, it serves as a preprocessor to
Computational Fluid Dynamics and Finite Element Analysis [14].
A database model from Solid Works was imported to Gridgen V15.10 R1. This
allowed the drawing of the outlining connectors for the project easier, thus making
the meshing easier as well. The most important aspect that had to be looked out for
was the meshing that had to be done around the turbine rotor. This area had to be
done with fine-structured meshing in order for the simulation to give the desired
results. The meshing can be thought of as the process of replacing a continuous
medium like air, water or metal with finite number of pieces. These pieces, called
cells, can be any shape. It’s a lot easier to solve CFD problems by dividing the
domain into these small cells.
Figure 11: The Database imported from Solid Works.
Theoretical Background 21
In our case there are in total of 605 connectors, 477 domains, in which 44 are
unstructured, and 118 blocks, in which 25 are unstructured. The amount of
structured meshes is greater than those of unstructured meshes since it is mostly
accepted that structured meshes are higher quality than unstructured meshes but it is
really hard to construct in hard topologies.
From the above given database the connectors were drawn using the create
connector on DB (database) entities tool. This gave the basic shape of the turbine
rotor and the 120 arc that it is in. The arc is only 120 because it is unnecessary for
all of the rotor blades to be drawn, when it could be done in Star-CCM+ digitally.
In the process of drawing the rest of the connectors dimensioning had to be taken
seriously. Dimensioning the connector’s shows at which point a node has to be
situated. The distance between these nodes had to be arranged so that the meshing
would flow continuously. The distance between the nodes had to be equal. This
dimensioning process is needed for the meshes to be structured. In general, when
there shouldn’t be a denser area switching into a less dense area. This would mean
an error in the simulation part.
Figure 12: End top side view
Theoretical Background 22
The designing of the domains, which are made by combining four dimensioned
connectors if structured or just combining the connectors to form a closed area for
unstructured, had to take the best skweness() into account. The skewness around
the rotor blades also had to be especially at the best ratio. This area is the most
important part since the fluid flow is going to be thoroughly examined in this part
for that reason even the structured meshes had to undergo some methods to better
the mesh. There also ways to improve the quality of structured grids by applying
Gridgen's elliptic PDE methods. These methods iteratively solve Poisson's equation.
While the defaults have been set to provide the nominal grid, the control functions
can be fine-tuned at any time using the following techniques [15]:
LaPlace (smoothness)
Thomas-Middlecoff (clustering)
Fixed Grid (smoothness)
von Lavante-Hilgenstock-White, and Steger-Sorenson (orthogonality).
Figure 13: The rotor domains' skewness.
Theoretical Background 23
The blocks are created after the domains. Domains can be considered as surface
areas, and blocks as the volume. Blocks are created by combining six domains, if
structured, together. When a block is made Gridgen automatically fills the blocks
with grids according to the grid structure of the domains. If an unstructured domain
exists inside a block, the block has to be unstructured as well. In this case the
volume just has to be closed and for the blocks to work another action has to be
taken, where we define to the program that these blocks also need to be filled with
meshes. Blocks are needed to define the volume conditions, and the domains to
define the boundary conditions. These conditions are defined for the comfort of the
user, so they are highly needed. Boundary conditions define the velocity inlet,
pressure outlet, periodic areas, etc. and volume conditions define the blocks in one
area in general.
This helps the user to see which area is the inlet and outlet. It also helps to do some
specific changes in Star-CCM+ such as the transformation or rotation of one
volume condition. If these conditions are not met problems would occur in the
simulation part. The simple task of just rotating on area would be more
complicated. Velocity inlet, pressure outlet, rotational part and wing section are the
four volume conditions for this work. The rotational part is the area where the
turbine will rotate when the simulation starts. The wing section is the circular area
which covers the rotor blade and this part is inside the rotational part. Wing section
had to be circular in order for us to change the angle of the turbine so that the
meshes wouldn’t overlap.
Figure 14: The Volume Conditions
Theoretical Background 24
The four volume conditions as shown in the figure above also had different
boundary layers. The boundary layers also needed to be separate even if they
defined the same thing, each area had to have their own pressure outlet wall, which
is the outer arc. Also there are in total of 6 periodic areas. These are the areas which
can be considered left and right parts of the triangular section of the design. The left
side is considered periodic left and had to be separated by 1-2-3 for the three
different areas used, and the right side is considered periodic right also as 1-2-3 for
the areas used. This periodicity allows the design to be completed to a 360 in Star-
CCM+.
After the VC and BC (volume and boundary conditions) were specified and all of
the meshes generated, the designing process was done. The output of the file was
made as a fluent model, which was specified at the startup of Gridgen so that Star-
CCM+ would be able to open it. Analysis S/W command of the program contains
the type of the model, whether it is a 2-D or 3-D model, and the output format of the
mesh design is also arranged here.
2.3.2 Star-CCM+
Star-CCM+ is an intuitive and modern analysis environment that guides users
effortlessly through setting up, running and analyzing complex engineering
simulations. The program has an easy to use and practical interface. The main usage
of this program is mainly computational fluid dynamics. The program’s main
advantages are:
CAD & PLM integration, fully integrated with most common design
programs such as Pro-Engineer, SolidWorks and Gridgen;
Built-in meshing technology, polyhedral meshing, which also will be used
later to see the results;
Intuitive simulation user environment;
Multi-disciplinary solutions; and
Engineering analysis, especially for fluid mechanics department [16].
Theoretical Background 25
The program has the capability of solving the most complex engineering problems,
with a good accuracy. For this the program has a wide range of usable physical
models. These physical models have to be determined by the user, and chosen at the
beginning of the simulation. The physical models cover time, flow, motion, regime
and even heat transfer and combustion.
The physics values used for this simulation were discussed with supervisors and the
conclusion was that;
Simulation Properties
Explanations
Continua
Physics 1
Models
Constant Density
Gas: Air with density 1.18415
kg/m^3 and dynamic viscosity of
1.85508E-5 Pa-s
Implicit Unsteady
Laminar
Segregated Flow
Three Dimensional
Reference
Values
Reference Pressure: 101325.0 Pa1
Initial
Conditions
Pressure: 0.0 Pa1
Velocity: [0.0, -10.0, 0.0] m/s2
Table 1: Continuum Physic Models and Definitions.
1. Default Values in Star-CCM+
2. Velocity is not negative; the minus sign defines the direction of the flow.
Theoretical Background 26
The model constant density was chosen because there is no change of density
happening during the experiment. Air cannot be treated as a steady flow; it has to be
regarded as implicit unsteady. In some cases of an airfoil simulation the model
turbulent is chosen instead of laminar. The reason for this is because of the critical
Reynolds number is 5*105. If we look at the Reynolds number equation
The critical length l can be calculated with the equation:
Where is fluid viscosity, the fluid density and the velocity. If the critical
length is greater than the length of the airfoil ( ) the flow is considered to be
laminar. If the critical length is smaller than the length of the airfoil ( the flow
is considered to be turbulent. So we can calculate as
The length L of the airfoil can be withdrawn from the drawing itself which is
. This makes the case of true, so the flow can be considered to be
laminar. The airfoil’s length is smaller than the laminar boundary layer, and the
flow cannot convert into a turbulent flow.
Theoretical Background 27
Figure 15: The length of the airfoil
The velocity, pressure and other properties of fluid flow can be functions of time
(apart from being functions of space). To determine if a flow is steady or unsteady,
these properties are taken into consideration. If a flow is such that the properties at
every point in the flow do not depend upon time, than the flow is considered to be
steady. Mathematically speaking for steady flows,
Where P is any property like pressure, velocity or density. Unsteady flow is one
where the properties do depend on time [17]. Turbulent flows are unsteady by
definition. The implicit unsteady approach is appropriate if the time scales of the
phenomena of interest are of the same order as the convection and/or diffusion
processes (for example, vortex shedding) or are due to some relatively low
frequency external excitation (for example, time-varying boundary conditions or
boundary motion). With implicit unsteady approach you are required to set the
physical time-step size, the Courant number, and the number of inner iterations to
be performed at each physical time-step [18].
The Segregated Flow model solves the flow equations (one for each component of
velocity, and one for pressure) in a segregated, or uncoupled, manner. The linkage
between the momentum and continuity equations is achieved with a predictor-
corrector approach. This model has its roots in constant-density flows. Although it
is capable of handling mildly compressible flows and low Raleigh number natural
Theoretical Background 28
convection, it is not suitable for shock-capturing, high Mach number and high
Raleigh-number applications [19].
After the correct continuum models have been chosen, the next step is to configure
the rest of the simulation properties. Some specifications were already given as
boundary and volume layers in Gridgen. Due to that after the imporing was done to
Star-CCM+ the regions were already separated as desired. The properties of these
regions are as shown in Table 2.
Simulation Properties
Explanations
Regions
Wing
Section Overview
Covers the Ahorn-Samen (Turbine Rotor) section
of the design and the general interface section. The
interface between the wing section and rotational
part.
Physics Values
Where the motion of the wing part can be chosen
as stationary or rotation. If for a rotational part a
stationary motion is chosen, the reference frame
can be arranged to be for rotation.
Pressure
Outlet
Section Overview
The section which is considered the end part of the
shape. The part which shows the pressure outlet.
Boundaries
Periodic Left &
Right
The boundaries which were specified as periodic
are chosen and made clear to the program that it
will be periodic.
Pressure Outlet
Wall
Physics Condition: Slip – in order for the program
not to recognize the part as a wall.
Rotation
Part
Section Overview
The middle part which covers also the wing
section. It has interface with all other sections. The
periodicity and wall physics are the same as
pressure outlet region.
Theoretical Background 29
Velocity
Inlet
Section Overview
It is the inlet of the shape. The direction of the
velocity is determined by the velocity physics
values. The periodicity and wall physics are the
same as pressure outlet region.
Table 2: The Different Regions and Their Explanations.
The figures 16 and 17 show the periodic regions and outer wall parts. As explained
on the table above the outer wall has to have slip condition for the program to not to
recognize it as a normal wall. Otherwise the data would change and the results
would not be symmetric.
Figure 16: Periodic Parts of the Model.
Figure 17: Outer Wall with Slip.
Theoretical Background 30
The wing section is the part that contains the turbine rotor. This part has the option
to be rotated using Star-CCM+. To compare results the rotors were rotated for four
different angles (30-45-60-70). However these angles are not the angle of attack
but they are the angle of installation. The angle which if the turbine was built the
rotors would have directly from construction. The results from four different
simulations were than taken into account for the experimental setup. This simple
action of rotating the wing part was also already concluded in the designing of the
mesh grids.
The rest of the simulation properties were all done so that the rotor blade would
have rotational motion. These properties can be seen in Table 3 below.
Simulation Properties
Explanations
Interfaces
There are in total of six interfaces created. Three
are in-place interfaces, which are in between the
four different areas (velocity inlet, pressure outlet,
rotational part and wing section). The other three
interfaces are periodic interfaces.
Derived
Parts
The parts which
are made by the
user. They show the
simulation area.
There are five derived parts created to determine
the results. One part is a cylindrical section that
covers from velocity inlet to pressure outlet. The
other four parts are on the wing section with
different distances (0.03m-0.05m-0.07m-0.08m).
These parts are necessary to get out the lift and
drag coefficients at different lengths of the rotor.
Solvers
The solvers are the implicit unsteady solver, in
which the time-step is determined to be 0.0010s,
and segregated flow solver.
Stopping Criteria
Stopping criteria as can be understood from the
name, is the property where the maximum inner
and maximum iteration number is decided.
Reports
Reports are created in order to plot the desired
force values in a certain direction and part. The
reports were created for drag coefficient, lift
coefficient, moment and moment coefficient. The
Theoretical Background 31
results of these reports are plotted.
Monitors
Reports are defined here to be simulated through
the simulation iterations.
Plots
Residuals and charts depending on the
reports/monitors were generated. An additional
pressure coefficient plot was generated for ever
derived part.
Scenes
Scalar and vector scenes were generated to view
the results.
Tools
Rotation with 2500rpm and 300rpm is added to
motions bar. The periodicity is also arranged here
with the transforms bar. It is decided on how many
times the periodic should continue, in this case 2
times.
Table 3: Simulation Properties.
By changing the simulation properties, the plots for desired coefficients were
created. With the data the lift and drag coefficients were calculated. After the
desired number of iterations was reached, by the help of derived cylindrical section
symmetry was controlled, this helped to check if the periodic parts were working as
desired. A vector scene was created to check the initial directions. This scene
creates an arrow like structure on the desired parts such as velocity inlet, the ahorn
samen or pressure outlet. The rotation of the blade is also controlled with this scene.
The rotation speed was set as 2500rpm for the beginning iterations, than changed to
300rpm. For normal 12 meter diameters, this speed is not reachable other. The
experimental setup would only allow for a 12 cm diameter blade. Due to that the
rotational speed was calculated with 2500 and 300(rpm).
Theoretical Background 32
2.3.3 Experimental Setup
Figure 18: The turbine profile made out of maple seed.
The experimental work took place after the simulations were finished. The
experiment took place in one of the University of Duisburg-Essen’s Essen
laboratories. The rotor blades were cut from a Plexiglas material, each blade with
the length of 6 cm. A cylindrical pipe not much wider than the blades combined was
connected to an air motor which gave out the desired the air at the desired velocity.
The desired value was determined by a turbine meter. The rotor blades were
connected to a nacelle-like structure (see Fig. 18), which also was connected to a
generator. The ammeter, voltmeter and resistor were connected to generate as
shown in Fig. 19 below.
Figure 19: The design of the experimental setup.
The resistance was changed manually, starting from 50Ω until 500Ω. With each
resistance a different voltage was calculated. The rotor blades were first run without
any resistance. This was done to find out the unloaded revolution speed of the
blades. The blade revolution was determined by using a stroboscope.
Theoretical Background 33
Figure 20: The experimental Set-up.
The Figure 20 shows the testing tunnel for experiment. The air motor is at the end
and blows air with a magnitude of 10 m/s. From a hole near the end the center of
the tunnel is measured and the speed is checked. The rotor blades are inserted at this
location afterwards and screwed down for stabilization. Figure 21 shows the
location and the ending of the pipe. The Turbine blades can be seen connected to
the tunnel and to the voltmeter and ampermeter. The turbine rotates inside the
tunnel with the incoming wind and shows how much voltage and current it creates.
With this information known a calculation of the power output for different angles
is made. General testing is done with normal edged profiles but as a comparison a
round edged profile type is also tested. The round edged profile has shown to have
better results than square-edged one, but since the simulation is done with only
square-edged profile type in the comparison between the experiment and simulation
the square-edge profile values are taken.
Figure 21: The location of the rotor profile inside the test tunnel.
Results and Comparison 34
3. Results and Comparison
In this chapter the results from the simulation part and the results of the
experimental work are explained. As it was previously stated the simulation and
experiment took place in four different angles with same velocity and revolution
speed. However, only the simulation results for 60 are explained since it was the
best power output that was gathered. The other simulation results are added to the
appendix section at the end. The power output of each angle starting from 30 and
ending at 60 are shown in the Figures 22-24. The power output of 70 could not be
calculated with the results from the simulation.
Figure 22: Power Output for 30 Degree Installation Angle.
-0.8
-0.7
-0.6
-0.5
-0.4
-0.3
-0.2
-0.1
0
0.1
0 500 1000 1500 2000 2500 3000 3500
P [W]
w [U/min]
Power-rotational speed
Results and Comparison 35
Figure 23: Power Output for 40 Degree Installation Angle.
Figure 24: Power Output for 60 Degree Installation Angle.
-0.45
-0.4
-0.35
-0.3
-0.25
-0.2
-0.15
-0.1
-0.05
0
0.05
0 1000 2000 3000 4000
P [W]
w [U/min]
Power-rotational speed
0
0.005
0.01
0.015
0.02
0.025
0.03
0 500 1000 1500 2000 2500 3000 3500
P [W]
w [U/min]
Power-rotational speed
Results and Comparison 36
3.1 Star-CCM+
The simulations are done with the same simulation properties which were described
in chapter 2.3.2. Maximum number of iterations for 60 is 5000 iterations for 300
rpm and 8000 iterations for 2500 rpm. These numbers of iterations are
approximately the same for all the other simulations. The first thing to check in the
simulations is the symmetry of the scalar scene of the velocity magnitude. The
accuracy of the simulation can also be checked with this, if the simulation
properties are wrong than the scene would not be symmetrical.
Since the velocity is flowing from positive to negative y, the perspective to best
look at these is from the positive x looking down onto negative z. As another
control method the scene looking up from negative y at 90 degrees is also
acceptable, since with this scene the pressure outlet can be seen from a straight
point of view (see Figure 26). The scalar scene for a velocity magnitude is plotted
upon the derived parts (see chapter 2.3.2). From the figure below it can be seen that
the flow continues from the upper part to the lower part. This means that the
periodicity has worked and that the program is calculating for three rotor blades.
Figure 25: The velocity magnitude scene of 300rpm.
Results and Comparison 37
Figure 26: The velocity magnitude from negative y to plus z [the pressure outlet section].
From the figure above the velocity is marked with the same colors that show the
same speed from left to right. Since the velocity is the same of the two sides it can
be called that this is symmetrical if the scene would not be symmetrical than the
simulation had to be started again with different properties. The above figure is
from the pressure outlet view, which is the end of the geometrical shape. The
vortexes that were created by the rotor have disappeared slowly. However if a
closer plane section is made, Figure 27, the exact shape of the wind after it has
made contact with the rotating turbine blade can be seen. The flow is distinctly
shown in these figures to be continuing form left to right in motion, which also
proves that the simulation is running periodically. After the simulation was
evaluated and the accuracy checked, the rest of the information needed could be
read from the other results that are calculated by the simulation. The air loads, lift,
drag and moment coefficients, that are acting on the rotor are plotted from the
reports created in the program. This is done for every angle of installation. The
details for these plots were given at the beginning of the simulation, and because of
how the rotor moved and the incoming way of velocity showed that the rotor was
moving on towards minus z axis. For the reports of these plots to be correct the
movement axis has to be defined before starting the simulation unlike other data.
Results and Comparison 38
Figure 27: Velocity magnitude display right after the turbine.
The results show that it is not possible to get
the data for the coefficients from a 45 degree
installation angle. For 45 degrees the values
for the coefficients do not stabilize at one
point but instead they are changing with
every iteration step. Figure 28 shows the
average values which are the results of the
reports for the other calculated installation
angles, 30-45-70 degrees. The lift and drag is
important for the stability of the rotor (see
chapter 2.2), because of stall.
As it can be seen from the graphs on the
Figure 28 the drag coefficient is rising as the
installation angle rises. It reaches a
maximum of 0.16 at 70 degrees, while at 60
degrees it is 0.14 and at 30 degrees it is
0.053. The drag is minimum at 30 degrees.
However, the lift is also minimum at 30
degrees, 0.07. The lift coefficient for 60
degrees is the highest with approximately
0.075. At 70 degrees the lift coefficient drops
to 0.015. This means that at 70 degrees the
drag is more than the lift coefficient which
would create a stall. The moment
coefficient, which is not the moment
Figure 28: Schematic diagram showing the air
loads.
Results and Comparison 39
generated, also rises as the installation angle closes to 90 degrees. The moment
coefficient for all the angles is a negative value. These are not the only coefficients
that were calculated with the simulation. The pressure coefficient at different
lengths was also calculated for all of the different installation angles. The derived
parts that were created at 0.03, 0.05, 0.07, 0.08 meters were the base of calculating
the pressure coefficients.
Results and Comparison 40
Figure 29: Pressure coefficient distributions of the HKAS airfoil for 0.03m, 0.05m, 0.07m, 0.08m and
shows the streamline plots from CFD simulations for the corresponding distances [0.03, 0.05, 0.07, 0.08
meters].
The above velocity magnitude scenes are only for the wing section. They show the
velocity change and distribution in different lengths of the rotor. The pressure
coefficient distribution plots are from the Ahorn-Samen section, which means the
pressure coefficients are from only around the rotor. These did not need to be made
for the whole system since the changes that are most important are in the areas near
the rotor. From the velocity magnitude diagrams we can see how the velocity is
changed by the shape of the rotor. The rotor is not a straight figure but it is a bended
figure which makes the location of the rotor from different cross-sections also
different. The red are in the velocity diagrams, which is the part where velocity is
highest, is changing according to the taken distance. The velocity around the tip can
be seen to be higher than the velocity at the hub. Also the separation lines of
velocities are distinctly seen (as the red color in the plots). A general streamline
function starting from velocity inlet and ending at pressure outlet, which also goes
over the rotor, is shown on Figure 30. The continuing figures (Fig. 31, Fig. 32 and
Fig. 33) show the streamline of the other installation angles, which are 30, 45 and
70 degrees. The streamline function is different for every installation angle since it
is different for every installation angle how the incoming velocity is affected. All of
the following streamline functions are simulated for the rotational speed of the
turbine blade as 300 rotations per minute.
Results and Comparison 41
Figure 30: Streamline results for 60 in the CFD simulation.
In this figure it can be seen that a vortex is created after the rotor blade. This
happens due to the pressure drop from the upper part of the rotor to the lower part.
The vortex however dissolves as it continues on.
Figure 31: Streamline results for 30 in the CFD simulation.
Figure 32: Streamline results for 45 in the CFD simulation.
Results and Comparison 42
Figure 33: Streamline results for 70 in CFD simulation.
The figures above show that the vortex is created in every installation angle, which
is a sign that a good meshing was done to be able to show these vortexes. The
streamline function change for every angle, and at 70 it is clearly depicted that the
vortex is too great and does not stabilize as the other angles.
3.2 Experiment
For the experimental work there was in total of eight different results for every
angle twice, and also four measurements were made with a round edged rotor blade
rather than a rectangular shaped one. The resistance was given by hand, but the
values that were read were the current, voltage and with the use of a stroboscope the
revolution speed was measured.First the revolution speed was read from the
stroboscope, for every angle with no resistance at all. Afterwards the resistance was
gradually increased starting from 50Ω and going up until 500Ω. All of the
measurements were taken with the constant velocity of 10m/s. The results of the
rectangular edged measurements are given at the table below.
30 with 10m/s.
Resistance Free Revolution Speed: 668rpm
[rpm]
R[Ω]
I[A]
U[V]
P[W]
553
50
0.008
0.4
0.0032
596
100
0.0059
0.6
0.00354
629
200
0.0039
0.8
0.00312
636
300
0.003
0.9
0.0027
645
400
0.0023
0.93
0.002139
652
500
0.0019
1
0.0019
Results and Comparison 43
45 with 10m/s
Resistance Free Revolution Speed: 1181 rpm
[rpm]
R[Ω]
I[A]
U[V]
P[W]
947
50
0.0135
0.67
0.00905
1001
100
0.0101
1.02
0.0103
1068
200
0.0067
1.36
0.00911
1101
300
0.0051
1.54
0.00785
1116
400
0.004
1.63
0.00652
1131
500
0.0034
1.7
0.00578
60 with 10m/s
Resistance Free Revolution Speed: 2077 rpm
[rpm]
R[Ω]
I[A]
U[V]
P[W]
1376
50
0.0202
1
0.0202
1580
100
0.0161
1.6
0.02576
1757
200
0.0112
2.23
0.02498
1843
300
0.0086
2.6
0.02236
1882
400
0.0069
2.77
0.01911
1933
500
0.0058
2.92
0.01694
70 with 10m/s
Resistance Free Revolution Speed: 2807 rpm
[rpm]
R[Ω]
I[A]
U[V]
P[W]
1266
50
0.0181
0.9
0.01629
1661
100
0.017
1.7
0.0289
2090
200
0.0132
2.67
0.03524
2292
300
0.0105
3.2
0.0336
2392
400
0.0087
3.5
0.03045
2471
500
0.0074
3.73
0.0276
Table 4: The measurements gathered from experimental work.
The results for the most power output for every installation angle are highlighted on
the table above. The power output is calculated by the simple multiplication of the
current with the generated voltage. The generated voltage is created with the
rotation of the turbine. The angle of installation is a different value than the angle of
attack. The angle of attack can be calculated by the use of and the position that
we want to calculate. For the highlighted power outputs an angle of attack for the
tip and hub of the rotor was calculated.
Results and Comparison 44
30 with 10m/s
Whub
Wtip
hub
tip
[rpm]= 596 rpm
1.36 m/s
5.055 m/s
7.74
26.81
45 with 10m/s
Whub
Wtip
hub
tip
[rpm]=1001 rpm
2.285 m/s
4.90 m/s
12.87
40.33
60 with 10m/s
Whub
Wtip
hub
tip
[rpm]= 1580
3.606 m/s
13.402 m/s
19.83
53.27
70 with 10m/s
Whub
Wtip
hub
tip
[rpm]= 2090
4.77 m/s
17.72 m/s
25.506
60.57
Table 5: A table of the angle of attack for different installation angles.
The table states that with the rising installation angle the angle of attack at the hub
and tip of the rotor blade rises. The angle of attack is an important factor that needs
to be checked in every turbine, propeller or rotor. A recurring problem is that
increasing the angle eventually forces the blade to stall, which is difficult to predict.
This results in manufacturers developing blades with limited operating angles to
ensure that stalling is minimized.
3.3 Comparison of Results
The results from experiment and the power outputs from the CFD simulation part
were put into graphs and evaluated. The graphs showed that the simulation and
experimental part had approximately the same power output for 30-45-60 degrees,
but for 70 degrees the simulation results were not correct. This proved that the CFD
simulations that were made are correct.
Results and Comparison 45
Figure 34: Simulation Results for HKAS51527
Figure 35: Experimental Results for HKAS51527
Conclusion 46
4. Conclusion
When the data gathered from both the simulation and experiment is compared, it
can be seen that the power output for 30, 45 and 60 degrees are nearly the same for
the simulation and experiment. The data from 70 degrees however did not show a
similarity as the other installation angles, the numerical results for 70 degrees
showed that the drag force was higher than the lift and the power output was lower.
Because of that the results for 70 degrees was not graphed as it was with the other
values.
The reason why the data’s from simulation and experiment are so similar is because
of the meshing that was used during the designing of the rotor blade. The whole
meshing was done with Gridgen as a structured mesh, which as a drawback
consumes more time than other methods. If a harder model was to be meshed the
polyhedral mesh system built in Star-CCM+ might be more of a use than other
candidates, since it is easier to construct and simulate. This mesh type also showed
tremendous results on this and other simulations that were done. The result for an
unstructed mesh is below average and would not be recommended. However if the
model is harder one might use unstructured meshing in some areas combined with
structured mesh creating a hybrid mesh.
The results showed that until 70 degrees as the installation angle increases the
power output increases in general as well. Though it must be reminded that the
installation angle is not the angle of attack, and the angle of attack is always
changing with time because of the rotational movement of the turbine. The angle of
attack for the best experimental results were calculated and shown on Table 5.
This simulation is made for a 6 cm long turbine blade. The testing of a larger blade
was not possible due to insufficient resources, and without a proper testing the
results of the simulation could not have been verified. If the resources were to be
found such as a bigger dimensional testing tunnel, the model can directly be
changed to match the new dimensions.
Bibliography 47
5. Bibliography
[1]
M. Carstei, "US - EU Dialogue on Sustainable Energy Security," 2011.
[2]
C. B. A.C. Hansen, "Aerodynamics of Horizontal-Axis Wind Turbines," Annu. Rev. Fluid
Mech., no. 25, pp. 115-149, 1993.
[3]
T. N. Annette Westerhellweg, "CFD Simulation of Wake Effects at the Alpha Ventus
Offshore Wind Farm," EWEA, Brussels, 2011.
[4]
X. Z. Z. D. GH Yu, "Numerical simulation of a wind turbine airfoil: dynamic stall and
comparison with experiments," pp. 657-677, 2010.
[5]
S. P. J. M. C.G. Gebhardt, "Numerical simulations of the aerodynamic behavior of
large horizontal-axis wind turbines," International Journal of Hydrogen Energy, pp.
6005-6010, 2009.
[6]
E. Hau, Wind Turbines, Berlin Heidelberg: Springer, 2006.
[7]
H.Glauert, The Elements of Aerofoil and Airscrew Theory, Melbourne: Cambridge
University Press, 1947.
[8]
H.Glauert, The Elements of aerofoil and airscrew theory.
[9]
J. J. B. a. M. L. Smith, Aerodynamics For Engineers, Eaglewood Cliffs: Prentice-Hall,
1979.
[10]
W.S.Farren, The reaction on a wing whose angle of attack is rapidly changing.
[11]
S. S. a. H.E.Helin, Unsteady vortex dynamics and surface pressure topologies on a
finite wing..
[12]
W. S.Jama, Introduction to Fluid Mechanics, CRC Press.
[13]
H. Oertel, Prandtl-Essentials of Fluid Mechanics, Springer.
Bibliography 48
[14]
"Pointwise," [Online]. Available: www.pointwise.com/archive/faq-v13.html.
[15]
J. A. John P. Steinbrenner, "Anisotropic Tetrahedral Meshing Based on Surface
Deformation Techniques," pp. 1-16.
[16]
M. Perić, "Future Developments of tar-CD and Star-CCM+," pp. 1-27.
[17]
[Online]. Available: www-mdp.eng.cam.ac.uk.
[18]
[Online]. Available: www.kxcad.net/STAR-CCM/online/116-CoupledFlowandEnergy-
11.html.
[19]
[Online]. Available: www.kxcad.net/STAR-CCM/online/117-SegregatedFlow-02.html.
