Profiles for a Savonius Wind Turbine

MAT-VET-F 20014

Examensarbete 15 hp Juni 2020

Two-dimensional Study of Blade

Profiles for a Savonius Wind Turbine

Martina Lundberg

Aikaterini Manousidou Julia Solhed

Johanna Sundberg

Teknisk- naturvetenskaplig fakultet UTH-enheten

Besöksadress:

Ångströmlaboratoriet Lägerhyddsvägen 1 Hus 4, Plan 0

Postadress:

Box 536 751 21 Uppsala

Telefon:

018 – 471 30 03

Telefax:

018 – 471 30 00

Hemsida:

http://www.teknat.uu.se/student

Abstract

Two-dimensional Study of Blade Profiles for a Savonius Wind Turbine

Martina Lundberg, Aikaterini Manousidou, Julia Solhed, Johanna Sundberg

A Savonius wind turbine is a self-starting vertical axis rotor. It can be designed to be compact in size and also produces less noise which makes it suitable to integrate into urban spaces such as rooftops and sign-poles. These characteristics make it interesting from a sustainability point of view, especially when aiming to increase the

decentralization of electricity production.

This thesis aimed to investigate the aerodynamic performance of different two-bladed Savonius profiles by varying the blade arc angle and the overlap ratio. For evaluation, the dimensionless power coefficient and torque coefficient were investigated over different tip speed ratios. The study was conducted numerically with 2D simulations in Ansys Fluent. The partial differential equations describing the characteristics of the flow, including the flow turbulence effects, were solved with the Reynolds-average Navier Stokes in combination with the k-omega SST model.

A validation was performed by comparing data from simulated and experimental tests of a semi-circular profile and a Benesh profile. The investigation of the blade arc angle and overlap ratio was performed on a Modified Bach profile. The profile with a blade arc angle of 130 degrees and an overlap ratio of 0.56 generated a maximal power coefficient of 0.267 at a tip speed ratio of 0.9. This blade configuration generated the best performance of all conducted simulations in this project. However, this project contained uncertainties since simulations can never be an exact description of reality.

The project was also limited by the computational power available. Nevertheless, according to the conducted simulations, it was observed that a higher blade arc angle and a larger overlap ratio seem to generate higher efficiency.

ISSN: 1401-5757, MAT-VET-F 20014 Examinator: Martin Sjödin

Ämnesgranskare: Sandra Olsson

Handledare: Anders Goude, Victor Mendoza

Populärvetenskaplig sammanfattning

En Savonius vindturbin är en självstartande vertikalaxlade rotor som kan utformas i en kompakt design samtidigt som den producerar mindre oljud än horisontalaxlade vindkraftverk. Dagens hållbarhetssträvan i kombination med Savonius turbinens karakteristiska egenskaper gör den till ett potentiellt starkt vertyg för vindenergi. Då den kan placeras på exempelvis hustak eller skylt- stolpar, utan att störa närliggande omgivning, finns det många möjliga sätt att implementera och integrera den i samhällets infrastruktur.

Målet med detta projekt var att undersöka den aerodynamiska prestationen på Savoniusturbiner med två blad genom att variera bladvinkeln och överlappningsförhållandet. För att jämföra de olika profilerna användes den dimensionlösa effektkoefficienten och momentkoefficienten. Dessa koeffi- cienter beräknades i förhållande till löptalet. Studien utfördes numeriskt med 2D-simuleringar i Ansys Fluent. De partiella differentialekvationerna som beskriver flödets egenskaper, inkluderat turbulenseffekterna, löstes med Reynolds-average Navier Stokes i kombination med k-ω SST mod- ellen.

En validering utfördes genom att jämföra data med simulerade och experimentella värden av en Semi-circular profil och en Benesh profil. Studien av bladvinkel och överlappningsförhållandet ut- gick från en Modified Bach profil. Den mest effektiva profilen hade en bladvinkel av 130

och ett överlappsförhållande på 0,56. Den genererade en maximal effektkoefficient på 0,267 vid löptal 0,9.

Projektet innehöll en del osäkerheter då simuleringar aldrig kan beskriva verkligheten till fullo.

Den tillgängliga beräkningskapaciteten begränsade även projektet ytterligare. Trots vissa begrän-

sningar, visar ändå utförda simuleringar att ökad bladvinkel och ökat överlappningsförhållande

genererar högre effekt.

Contents

Populärvetenskaplig sammanfattning 3

Nomenclature 5

1 Introduction 6

1.1 Aim . . . . 7

2 Theory 7 2.1 Fundamentals of fluid mechanics . . . . 7

2.1.1 Navier Stokes equation . . . . 8

2.1.2 Computational fluid dynamics . . . . 8

2.2 Savonius turbines . . . . 8

2.2.1 General characteristics . . . . 8

2.2.2 Betz Theory . . . . 9

2.2.3 Blade profile geometries . . . . 11

2.2.3.1 Performance characteristics . . . . 11

2.2.3.2 Conventional semi-circular . . . . 12

2.2.3.3 Benesh . . . . 12

2.2.3.4 Modified Bach . . . . 12

2.3 Numerical Modelling . . . . 13

2.3.1 Software . . . . 13

2.3.1.1 Ansys . . . . 13

2.3.1.2 Fusion 360 . . . . 13

2.3.2 Methodology . . . . 13

2.3.2.1 Simulation domain . . . . 13

2.3.2.2 Meshing . . . . 14

2.3.2.3 Turbulence modelling . . . . 15

2.3.2.4 Boundary conditions . . . . 15

2.3.2.5 Yplus . . . . 16

2.3.2.6 Stability: CFL Criterion . . . . 17

2.3.2.7 Blockage factor . . . . 17

2.3.3 Validation . . . . 17

3 Method 18 3.1 Simulation set-up . . . . 18

3.2 Validation . . . . 19

3.2.1 Simulation domain sensitivity study . . . . 21

3.3 Study of the Modified Bach . . . . 22

4 Results 23 4.1 Validation . . . . 23

4.2 Blade study . . . . 24

5 Discussion 26 6 Conclusion 28 7 Appendix 31 7.1 Validation of rectangular cylinder . . . . 31

7.2 Simulation set-up guide . . . . 32

Nomenclature

∆t time step discretization [s]

∆x spatial discretization [m]

 blockage factor [-]

η

efficiency [-]

λ tip speed ratio [-]

ν kinematic viscosity [m

/s]

Ω turbine rotational speed [rad/s]

ρ density of fluid [kg/m

] τ

wall shear stress [P a]

A area normal to the flow [m

] C

drag coefficient [-]

C

power coefficient [-]

C

torque coefficient [-]

F

drag force [N/m]

L

variable slip length [m]

P

Produced power [N rad/s]

Q torque [N ]

R radius of rotor [m]

r radius of blades [m]

u

friction velocity [m/s]

v

freestream velocity [m/s]

y

dimensionless wall distance [-]

CFD Computational Fluid Dynamics CFL Courant-Friedrichs-Lewy condition OR overlap ratio [-]

RANS Reynolds Average Navier Stokes

SSWT Savonius-style wind turbine

1 Introduction

People have been harvesting wind for mechanical power since the 9th century when Persians cre- ated vertical-axis windmills to grind grain.[1] Windmills continued to flourish and were developed into what we now know as horizontal-axis windmills.[1] They were widely used during the late medieval and early modern times. With the introduction of fossil fuels such as coal and oil, the utility of windmills declined dramatically. However, the growing demand for electricity and the invention of the first airplane created an interest in the science of aerodynamics and as a result in other wind-driven machines as well. Between the years of 1888 and 1900, the United States and Denmark conducted experiments on the use of the mechanical structure of windmills for the gen- eration of electricity. Consequently, this resulted in the development of the first wind turbines.[2]

Two decades later, the Finnish engineer Sigurd Johannes Savonius invented the Savonius-style wind turbine (SSWT). The initial rotor was not designed to generate electricity but instead designed to power ships.[3] Sigurd Savonius aimed to take advantage of the Magnus effect by placing a vertical axis rotor on a ship and create a propulsion effect pushing it forward. Later on, the Savonius rotor was developed further and in 1926 a patent for an SSWT generating electricity was filed. However, SSWTs have been explored long before the 1920s and the first records of similar designs date back as early as the 17th century.[4]

Nowadays when discussing Savonius rotors in the field of wind energy, the term refers to a sub- division of vertical-axis wind turbines. A common characteristic of SSWTs is that they consist of two or more blades symmetrically placed around the vertical rotational axis. Some of the blade configurations studied by Sigurd Savonius in the 1920s are presented in figure 1. Horizontal-axis wind turbines are usually associated with producing a lot of noise. On the contrary, vertical-axis wind turbines create less noise.[5] One of the other primary advantages with the SSWT is that it does not need a yaw system to control its orientation in relation to the incoming wind direction.

It is also capable of self-starting even at low wind speeds.[5] However, the SSWT cannot extract as much of the wind’s energy compared to other wind turbines, making it less efficient.[4] Despite the lower efficiency, it has several advantages in addition to its independence of the incoming wind direction. Some benefits of the SSWT is that its generator can be located on the ground which allows for easier maintenance and that the turbine is less sensitive to wind speed variations and turbulence.[5] The SSWT can be designed to be very compact in size and can, therefore, be in- tegrated into urban spaces, for example by being placed on rooftops, sign-poles, and statues. As seen in figure 2, micro SSWT are implemented as leaves on the so-called Wind Tree. The Wind Tree was designed by a French company called New World Wind and several prototypes have been installed in France, Belgium and Germany between 2013 and 2016.[6] The UK start-up company Capture Mobility gives another great example of an implementation for the SSWTs. The company developed a small-scaled SSWT that would produce up to 1kW of electricity per turbine from the turbulence of passing cars near highly trafficked roads. The produced electricity could be used to power street lights and road signs.[7]

Figure 1: Wing profiles created and studied by Savonius in the 1920s.[3]

Figure 2: Savonius micro-turbines implemented as leaves on the Wind Tree.[6]

Europe has an excellent reputation in supporting renewable energy sources and had accounted for over 70% of global wind power installations by 2000. In 2009 the Swedish Parliament decided to set a goal of at least 50% of the total energy usage coming from renewable energy sources by 2020.[8] According to Wind Europe’s data, Sweden’s proportion of wind power in its electricity production was 15% in 2019 and Sweden more than doubled its wind power installations between 2018 and 2019.[9] Evidently, Sweden is one of the countries that prioritize minimizing their eco- logical footprint and clearly invest in wind power. It has been found that small scale renewable energy generation is more cost-effective since it efficiently utilizes the natural resources of the local community. That would also contribute to the increased decentralization of electricity and min- imized environmental degradation.[10][11] As shown above, the SSWT can be a powerful tool to further develop the sector of wind power and maximize the output capacity of the country. The SSWT can be designed with a variety of blade configurations, however, those need to be optimized towards obtaining an efficient Savonius rotor that also is commercially competitive.

1.1 Aim

The purpose of this project is to study how the variation of two different design parameters affect the performance of a specific two-bladed SSWT. The parameters will be varied one at a time but the modification of the first parameter that results in the best possible performance will be used when varying the second parameter. The study will be conducted numerically with two-dimensional simulations.

2 Theory

In this section, important theory regarding the SSWT is introduced including the fundamentals of fluid mechanics, Navier Stokes equation and Computational Fluid Dynamics (CFD). Betz the- ory and common comparison parameters along with blade profiles used in this project are also introduced and described. Thereafter the numerical modelling software is presented along with important concepts of setting up a simulation.

2.1 Fundamentals of fluid mechanics

Fluid mechanics is the science and study of the mechanics of liquids and gases at different states.

It can mainly be divided into two branches including fluid statics, which is the science of fluids in a stationary state, and fluid dynamics, which is the study of fluids in motion. Fluid dynamics de- scribe how the flow processes are influenced by outer forces and interactions with boundaries.[12].

The different characteristics of these flows can thereafter be described by several mathematical

equations such as the Navier Stokes equation in fluid mechanics, described in the next section.

2.1.1 Navier Stokes equation

Navier Stokes equation, in fluid mechanics, is a partial differential equation used to describe the flow of fluids. It provides a relation between the pressure, velocity, viscosity, and density of a moving fluid. In the early 18th century the mathematician, Leonard Euler, developed an equation used to describe the flows of incompressible and frictionless fluids, called the Euler equation. Over time, that equation has undergone improvements, firstly by the engineer Claude-Louis Navier in 1821 when he added the element of viscosity. This addition expanded the equation to also describe the flow of viscous fluids. Later in the 19th century, the mathematician and physicist Sir George Gabriel Stokes improved the equation further. This resulted in the Navier Stokes equation 1 where u is the fluid velocity vector, p the fluid pressure, ρ the fluid density and ν the kinematic viscosity.[13]

∂u

∂t + u · 5u = − 5p

ρ + ν 5

u (1)

Even though Stokes improved the equation, the analytic solution of the nonlinear partial differential equations can only be obtained in 2D for simple flows. For more complex 3D-flows, including turbulence and vortices, these solutions are too difficult to solve. For that reason the Navier Stokes is a part of the Millenium Problems, being one of seven mathematical problems rewarding one million dollars for the correct solution.[13] Since this has not been accomplished yet, the use of numerical methods is crucial. Instead of analytic solutions the field of computer science and mathematics analyzes and implements numerical algorithms to provide solutions. In problems regarding fluid flows, this area of study is called CFD, described in the next section.

2.1.2 Computational fluid dynamics

CFD is a branch of fluid mechanics that utilizes numerical analysis to investigate fluid flows. The use of CFD in solving complex problems in modern engineering has over the past years steadily increased. From only being used in areas of high-technology engineering such as astronautics and aeronautics, CFD is now integrated into multiple fields. CFD is for example widely used in the transport sector, where the airflow around cars and airplanes are studied.[14] Computer simulations make it possible to test prototypes in advance and see if the flow around the model is acceptable.

The use of CFD, for optimization and improvement of existing and development of new designs, results in lower costs and enhanced efficiency.

2.2 Savonius turbines

2.2.1 General characteristics

When conducting research and studies on the performance of wind turbines, dimensionless pa- rameters are used for the evaluation. The most frequently measured coefficients are the power coefficient (C

) and the torque coefficient (C

) which are presented in equations 2 and 3. The C

relates to the power produced by the turbine and the C

relates to the torque exerted on the turbine.

C

= QΩ

1

2

ρv

A (2)

C

= Q

1

2

ρv

AR (3)

In 3D the area normal to the flow would be the width of the rotor multiplied by the height of the

rotor. Since the simulations are two-dimensional the area in the XY-plane can be described as a

line as long as the diameter of the rotor, A = 2R. Thus equations 2 and 3 can be simplified to

equations 4 and 5.

C

= QΩ

ρv

R (4)

C

= Q

ρv

R

(5)

Another important parameter that is used when studying the performance of wind turbines is the tip speed ratio (λ). λ is defined as the ratio between the tip speed of the blades (ΩR) to the free stream velocity (v

) and can be seen in equation 6.

λ = ΩR v

(6) λ is closely related to the efficiency of a wind turbine since it describes the operational condition.

Turbines reach optimal performance at different λ. The measured or simulated C

and C

of a turbine is usually plotted against λ calculated as in equation 6.

The power that the turbine produces can be calculated using equation 7 and the efficiency can be calculated using equation 8. These equations are used to analyze the performance of the turbine.

There is a limit to how much power can be extracted from the wind by a turbine. This limit and the theory behind it is described in the next section.

P

= QΩ (7)

η

= C

(8)

2.2.2 Betz Theory

The discussion of wind energy and the efficiency of wind turbines inevitably references to the Betz theory. Albert Betz introduces this theory in 1919 in his publication ”Wind Energy and its Use by Windmills”.[15] The Betz theory specifies the maximum energy that can be collected by the given wind turbine in an open wind flow. The law is derived by using the conservation of energy principle. This principle is applied to a flow of wind going through a turbine. For the derivation, the turbine is assumed to have an infinite number of blades and retain no hub. In addition to this, the swept area (A) of the turbine and wind speed (v) flowing through the swept area is assumed to be uniform. A wind turbine extracts mechanical energy by reducing the kinetic energy of the wind flow, in other words by slowing down the wind.[15] In figure 3 an elementary sketch of a horizontal axis wind turbine along with wind speed and the swept area is presented. The velocity of the upstream wind v

of the turbine is larger than the downstream wind v

. The derivations of the Betz law, describe that for optimal application the downstream velocity v

should be one-third of the upstream velocity v

.

By using a wind turbine, the wind flow can be slowed down and thus induce a change of wind speed. As the wind flow is slowed down a change in pressure is also induced. The Betz theory depicts the important fact that a part of the wind flow will pass by the turbines sweep area, not through it. Furthermore, if the flow is decelerate even more, an even greater fraction of the flow will not pass through the turbines sweep area. Hence, it is reasonable that a turbine can only extract a part of the energy in the wind flow. Consequently, there is an optimal case where the turbine slows down the flow in a way that makes a maximum amount of the flow to pass through the turbine. For this ideal situation, the power coefficient is C

≈ 16/27 ≈ 0.59259 ≈ 59.26%.

This value is known as Betz limit or Betz coefficient. This coefficient propose that a maximum of

59.3% of the energy can be extracted in an open undisturbed flow of wind.[15]

Figure 3: Wind turbine with upstream and down stream wind speed (v) and sweep area (A) with ideal wind speed before and after the wind turbine. This figure also displays the velocity and pressure changes as the flow interacts with the turbine.[15]

The important concept the Betz theory implies, is that a change of wind speed and pressure is

necessary to collect energy. The wind needs to be slowed down and there needs to be a change in

pressure as the flow pass through the turbine. Every turbine has a characteristic λ where it reaches

an optimal C

, referred to as C

. The C

indicates the point where the flow interacts

with the blade in a way that generates the maximum effect possible. A pressure difference and

velocity change will be greater when the flow attaches and interacts with the blade. The SSWTs

operate at rather low λ compared to horizontal-axis wind turbines. In previous studies of SSWTs

λs between 0.2 to 2.0 are examined.[16] Operating λ and approximately generated C

for different

types of wind turbines are presented in figure 4. Experimental tests by Roy and Saha showed

SSWTs can generate a C

as high as 0.28 depending on the blade configuration.[17] The C

curve

of a turbine is usually parabolic as can be observed in figure 4. When designing and trying a

prototype of any wind turbine, the first thing to do is to generate a λ curve. This is done to find

where the turbine operates as optimal as possible. A C

at a large λ is favourable from a

mechanical point of view. A turbine operating at a larger λ implies it operates at larger rotational

speed, which means a smaller generator could be constructed and used for the device.

Figure 4: Graph over the variation curve of C

average to T SR in different types of wind tur- bines.[18]

2.2.3 Blade profile geometries

With the scope of improving efficiency, several blade profile geometries have been developed and researched. In this section, some common performance characteristics and designing parameters for SSWT blades are presented. Thereafter, three blade profiles known as conventional semi-circular, Benesh and Modified Bach are introduced in the sections below and seen in figure 5. These are three of an abundant amount of different blades that have been studied previously.

Figure 5: Two dimensional figure of the following wing profiles: (a) a conventional semi-circular, (b) Benesh type and (c) a modified Bach type.[17]

2.2.3.1 Performance characteristics

The performance of a turbine is affected by several design parameters. The parameters that have

proven to have an impact on the performance are the number of blades, the aspect ratio and the

overlap ratio (OR).[19] In the report written by Zemamou et al., it is concluded that two blades

are more beneficial, in comparison to a higher number of blades.[19] The aspect ratio is the height

of the rotor divided by its diameter (D). Many studies have been conducted within this area

and, generally, a ratio of between 1 and 2 gives a sufficiently good performance.[19] However, when

performing simulations in 2D this parameter does not have to be taken into consideration. The OR

affects the wind flow in the rotor and is the distance s, called the bucket gap width, divided with

the bucket diameter, d marked in figure 6. No clear mutual conclusion has been drawn regarding

the most effective ratio by previous studies.[19] Several more parameters could be investigated

regarding their effect on the performance of the SSWT.

Figure 6: A cross section of a semi circular turbine.

2.2.3.2 Conventional semi-circular

A conventional semi-circular rotor is one of the simpler models of the Savonius rotor. This rotor consists of two blades oppositely arranged in an s-formation fixed around the rotation axis.[20] In its simple construction, it is one of the most frequently described profiles when mentioning Savonius rotors. Many studies have analyzed the semi-circular rotors performance and efficiency by altering parameters such as the OR and the blade arc angle.[16][17] They have also added more blades and tried multi-staging, placing two turbines on the same rotational axis, with the conclusion that the improved results do not compensate for the complexity and costs of the altered profiles.[17]

2.2.3.3 Benesh

The Benesh rotor is an improved model of the SSWT, named after its creator Benesh Alvin H.[20]

It is like the semi-circular rotor, a vertical axis turbine including two blades whose outer edges define the rotor’s diameter. The blade’s shape differs from the semi-circular. Instead of having two blades in an s-shape, they have more of an airfoil-shaped blade profile. Close to the center and outwards to the edges of the rotor, the blades have a linear portion which passes to a curved portion towards the edges. Because of the shape of the blades, the Benesh rotor can contribute to better aerodynamic characteristics. The cross-section not only produces a higher lift but also a higher torque because its rotational speed is increased due to its shape. The greater torque, Q, also results in an increased C

value.[17]

2.2.3.4 Modified Bach

The Modified Bach rotor is a further developed model of the classical Bach profile. The classical

Bach profile has similar characteristics to the Benesh type but with a shorter linear portion. The

Modified Bach has the same airfoil-shaped blades but instead a larger OR than the original Bach. It

has a different overlap distance and blade arc angle which contributes to a higher flow acceleration

that enhances its performance.[17]

2.3 Numerical Modelling

To study the blade geometry configurations, 2D numerical modeling is used. In this section the software used and the methodology for this project are presented. The methodology introduces important theoretical concepts used when conducting numerical simulations. At last, the approach of validation for a numerical model is presented.

2.3.1 Software 2.3.1.1 Ansys

Simulations are carried out using the software Ansys Fluent, specifically the Ansys Student Pack- age. This free Student Package is powerful but has a limit of 512 000 computational cells and nodes.[21] Ansys Fluent is a software that makes it possible to perform CFD, with a broad spec- trum of tuning possibilities of parameters such as pressure and flow speed. First, the simulation domain and geometry is specified, this is done in the Design Modeler interface. Then in the Mesh interface, the mesh of the domain is created and tuned to serve the object and simulation of in- terest. Next, the computational set-up of the calculation is defined, which includes the choice of model for the flow and the spatial discretization to mention a few.

2.3.1.2 Fusion 360

Fusion 360 is the CAD program used to design the blade profile geometries. It is a free software for students and educators. Fusion 360 is a modeling software used for precise modeling of 3D and 2D objects. It is widely used within a range of businesses since the program has a lot of features that make it well suited for model designing and prototyping.

2.3.2 Methodology

In this section, some important theoretical concepts for the simulations are presented. The concepts are introduced in the same order as the Ansys workflow. The concepts include simulation domain, mesh, turbulence modeling, boundary conditions, y

, stability criterion, and blockage factor.

2.3.2.1 Simulation domain

A simulation domain is where the calculations will be performed and should include the object to be analyzed. There are three distances that need to be considered when creating a domain.

First of all, the distance between the object and the inlet. When the flow comes near the object

it will begin to change direction to get around it. Therefore, the space upstream of the object of

interest must be sufficiently large so that this change in direction and velocity is allowed to take

place without interruption. Second of all, when considering the distance from the object to the

sidewalls, it is important that the walls do not affect the flow. In reality, the wind turbine will

not be enclosed and therefore these walls should not interfere and be placed far enough from the

object. Third of all, the distance downstream of the object needs to be considered. The flow will

be affected downstream for some time after passing the object, usually by some sort of oscillations

or whirls depending on the shape. For this reason, the domain needs to be longer downstream

than upstream of the object.[22] An example of how the flow can be affected by an object in a

simulation can be seen in figure 7.

Figure 7: A turbine in a simulation domain with a flow entering the domain from the left. The color scheme depicts the velocity changes.

2.3.2.2 Meshing

A mesh is a network of discrete geometric units, also known as cells. The simulation time will be affected by the size of the cells and in certain cases, the simulation time can be far too long to be realistic. Therefore, the size of these cells should vary depending on their location in the simulation domain. A guideline to adhere to in the prioritization of the size of the cells is to have smaller cells where large velocity variances are expected and in the regions of interest.[22] For example, if the drag force of a tennis ball is to be investigated, the cells closest to it should be the smallest and could successively be increased further away.

When simulating in 2D, the simulation domain is usually rectangular. At the inlet of the do- main, the flow is mostly constant and only minor discrepancies are expected. The same applies to the outlet and the edges of the domain. Larger deviations are to be anticipated close to the object of interest. To effectively simplify the process, the domain is broken down into smaller blocks, re- ferred to as "areas of refinement", which can be designed to be of different sizes in different areas of the domain.[23] An additional layer of extra refined mesh cells is added around the studied object, this is called inflation, see figure 8. It is essential in the regions closest to the object because that is where the boundary layer of the object is located. Therefore it is important that the solution of the flow is accurate in this region. y

is a measurement of the resolution of the mesh in this region which is explained and introduced in section 2.3.2.5.

Figure 8: A turbine with inflation cells and triangular cells.

The choice of mesh model depends on the characteristics of the application. For 2D simulations in Ansys Fluent, the mesh cells can be chosen to be quadrilateral, triangular, or a mix of both, as seen in figure 9. The mesh can also be set up to be structured or unstructured.[24] According to the Ansys Fluent User Guide, two things that need to be taken into consideration are the set-up time and the computational expense. Quadrilateral structured mesh is known to give accurate results but can be time-consuming to set up. A structured mesh can also generate an inefficient mesh distribution. For example, a very refined mesh can be generated in an area where a finer mesh is not contributing to higher accuracy of the solution. A triangular unstructured mesh takes less time to set up but does not always contribute to the most accurate solutions. One advantage of the triangular unstructured mesh is the possibility to create areas of refinement in selected areas of the simulation domain. This makes it possible to save computational power as a triangular unstructured mesh can be created using fewer cells than the corresponding mesh of quadrilateral elements.[24]

Figure 9: Different types of mesh.[25]

2.3.2.3 Turbulence modelling

Turbulence is a concept used in fluid dynamics. It describes a fluid motion that behaves in a way that makes it impossible to predict what velocity the flow will have at a specific point. According to the Oxford Dictionary of Mechanical Engineering “turbulence, or turbulent flow, is a fluid motion which is distinguished by disorderly velocity variations along with rapid changes in pressure and other fluid properties”.[26] There are different ways of modeling turbulence and one method is the Reynolds Average Navier Stokes (RAN S).[22] The general idea of the RAN S model is to use average expressions of the different variables and then rewrite the Navier-Stokes equation with these expressions. This equation will look similar to the Navier Stokes equation but will contain one extra term which is denoted as the Reynolds Stress. Since this expression contains an extra unknown term, at least one more equation is required to solve this problem. These additional equations to express the Reynolds Stress term will be the specified RAN S turbulence model of choice. Depending on the geometry and fluid motion, there are different RAN S models that are more suitable than others.[22] Reviewing previous CFD studies of Savonius wind turbines the most frequently used models are the two equation-based models realizable k-ε and k-ω Shear Stress Transport (SST).[5][27]

2.3.2.4 Boundary conditions

Boundary conditions describe how the flow is acting in contact with the boundaries. They are

important to explain how the fluid behaves in all parts of the domain. Considering a pipe, for

example, a moving or a fixed boundary will certainly affect how the flow is behaving in the middle

of the pipe. Boundary conditions can be applied on different parameters such as velocity and pres-

sure.[28] In a simulation with a k-ω turbulence model, boundary conditions for velocity, pressure, k

and ω are predefined but can be redefined if necessary.[24] There are two kinds of commonly used

conditions when considering the velocity, called slip and no-slip boundary conditions. The slip

condition indicates that the velocity at the given boundary does not have to be zero. To explain

the difference of motion between the boundary and the fluid in contact with the boundary, the variable slip length L

is introduced. It is the distance from the edge of the boundary to a point inside the boundary where the continuum flow and the boundary would have the same velocity.

To clarify, this distance is a theoretical value. The difference in velocity of the boundary and the continuum can be calculated with equation 9 below. However, when considering incompressible fluids and solid boundaries, no-slip conditions can often be used. A no-slip condition means that the velocity at the boundary is zero. The two conditions are visualized in figure 10.[28]

∆v

= δv

δz |

L

(9)

Figure 10: Visualisation of a no-slip boundary condition in a) and a slip boundary condition in b).

2.3.2.5 Yplus

When using turbulence models such as k-ω to resolve all the viscosity-affected areas, it is also important to introduce the non-dimensional parameter y

. To solve the flow and turbulence in the boundary layer, wall functions are used. According to Fangqing Liu “wall functions are empirical equations used to satisfy the physics of the flow in the near-wall region”.[29] Determining the application of these wall functions, the most commonly used parameter is y

. It can be explained as the resolution needed for the turbulence model to solve the boundary layer.[29]

y

= y × u

ν (10)

u

= r τ

ρ (11)

y is the distance to the wall, ν and ρ the viscosity and density of the fluid in the tunnel, τ

the

wall shear stress and u

the friction velocity. The value of y

denotes the location of the first cell

center in a specific region. Depending on what method is used to model the behavior near the

wall, different wall functions are required, thus this location varies. Every type of wall function

builds its foundation on the universal law of the wall. This law states that regardless of the kind

of turbulent flow, the distribution of the velocity in the near wall-region is the same. As a result,

this region can be separated into three different parts: the viscous sub-layer, the logarithmic layer,

and the defect or buffer layer. Depending on the turbulence model of choice, the first cell center is

placed in one of these layers.[30]

2.3.2.6 Stability: CFL Criterion

In order to avoid that the numerical scheme produces incorrect results, a small enough time step needs to be chosen. By using the Courant–Friedrichs–Lewy condition (CFL-condition) the upper limit of time step size can be chosen to obtain a stable solution, see equation 12. The general idea of the CFL-condition is that the flow should not move past more than one mesh cell per time step as valuable information will then be lost.[27] As a result of this, the upper limit of the time step will also decrease when the size of the mesh cells is decreased.

CF L : v∆t

∆x < 1 (12)

Where v corresponds to the maximum velocity possible in the simulation domain, ∆t to the time step, and ∆x for the smallest size of a mesh element. This ratio is sometimes referred to as the Courant number.

2.3.2.7 Blockage factor

When wind tunnel measurements are performed on an object, it is blocking a part of the flow leading to a velocity increment. This velocity augmentation needs to be accounted for when processing the data. To handle this, a blockage factor  is used which is presented in equation 13. The blockage factor is used to correct for how much of a tunnel an object is blocking and the effect it has on the wind speed passing by the object. However,  for the Savonius rotor has a 50%

margin of error. This is mainly due to the shape of the rotor as the frontal area of the turbine, in reality, is changing continuously when rotating.[16]

 = Frontal area of turbine

4 × Test section area (13)

The blockage factor is applied in experiments and 3D simulations. However, in 2D simulations the frontal area of the turbine is not completely defined as only a cross-section of the tunnel is examined.

2.3.3 Validation

Validation can generally be explained as to how well experimental data agrees with the data

extracted from a simulation.[14] It basically explains a numerical model’s ability to describe physical

phenomena. However, the experimental data is not an exact description of reality since it is tested

in a contained environment. The experimental values are nonetheless the best description of reality

that is quantified. Another important aspect of the validation is to create a model with reasonable

settings in order to generate an accurate enough solution in an acceptable amount of time. The

focus is put on trying to identify and eliminate errors, which will then improve the accuracy of the

model. Parameters that can be changed in the model are for example the size of the domain, the

position of the studied object in the domain, and the mesh cell size. Thereby, validation also can

be said to prove that the model is solved correctly by the computer. [14]

3 Method

This section presents the method for conducting the study of two parameters of a blade geometry configuration. First, the process of setting up a simulation is introduced. Before a simulation can be deemed to produce any reasonable data, the simulation model has to be validated. The validation approach is presented along with a domain width sensitivity study. Thereafter the method of the blade arc angle and overlap ratio studies of the Modified Bach is presented.

3.1 Simulation set-up

The simulation set-up is presented in this section, for a detailed step-by-step simulation instruc- tion, see appendix 7.2. The rotor geometry was sketched in 2D using Fusion 360. The sketch was thereafter imported into Ansys Fluent where it was incorporated into a simulation domain. The simulation domain consequently consisted of two surfaces, the rotating rotor, and the stationary tunnel. When the simulation domain was created, the regions for refined mesh was also constructed.

The next step was to generate a mesh and make the appropriate refinements for the different areas of the simulation domain. The meshing method was set to triangular unstructured due to the time efficiency of the meshing process for this method. Previous similar studies have also used this meshing method.[31] The size of the cells in the different areas of the simulation domain and the inflation was also defined. Appropriate names for the different segments in the simulation domain were specified. Since the simulation domain consists of two surfaces, Ansys automatically creates a static connection between the two surfaces. This connection was deleted to enable an introduction of a sliding mesh interface later on.

Then the computational set-up was set to pressure based and time-dependant. The turbulence model was set to k-ω SST. This turbulence model was chosen since previous studies show that it depicts the effects of curved surfaces well, which made it a suitable model for simulations of the Savonius Rotor.[5][32] The k-ω SST model is known to perform well, not only in the fully developed turbulence areas but all the way down to the wall. As described in section 2.3.2.5, due to the choice of turbulence model the area closest to the wall will be a viscous sublayer. By using the k-ω SST method the behavior in the viscous sub-layer and the logarithmic layer needs to be resolved. In the logarithmic layer, no wall functions are needed. In the viscous sub-layer, on the surface of the blades, wall functions are however necessary. Due to the choice of turbulence model y

< 5 was required in this region to ensure good results.[29][30]

After the turbulence model was selected, a mesh interface was created. This mesh interface enabled a contact area between the mesh in the stationary region and the mesh in the rotating region. The rotor surface was given a rotational mesh motion. This mesh motion was set to the rotational speed of the turbine. Thereafter boundary conditions were defined. The inlet velocity was specified. On the blades, the no-slip boundary condition was applied and the blades were given the rotational speed of choice. The rotational speed was the same for the blades as for the mesh motion of the rotor. The slip boundary condition was used on the walls. This was done to minimize the walls’

influence on the performance of the turbine. For other parameters such as for k, ω, the pressure, and the gradient, the Ansys default boundary conditions were used.

Then the solution and discretization methods were selected. The pressure and velocity coupling were set to be solved using the coupled algorithm. For the spatial discretization, three different numerical schemes were used. To solve the gradient the least square cell-based method was im- plemented. For the pressure and momentum, the second-order upwind method was chosen. The first-order upwind scheme was used for the turbulent kinetic energy and the specific dissipation rate. The time discretization was conducted using the first-order implicit formulation.

Thereafter, the solution initialization was conducted using the hybrid initialization method. So-

lution graphics were created for the velocity and for y

. These were then added as solution

animations so that the simulations could be monitored continuously.

Figure 11: Torque exerted on a turbine. The initial phase of the simulation with Courant number of ≈ 4 and the stable phase with fulfilled stability condition.

Before starting the simulation a suitable time step was chosen using the CFL criterion. When starting a simulation the initial phase was conducted using a time step corresponding to a Courant number of approximately 4. After the initial unstable phase, the simulation was paused and the time step was reduced to fulfill the CFL criterion, as in equation 12. An example of this is presented in figure 11. This was done to save time as the simulations were expensive both in time and computational power.[27] The maximum number of iterations per time step was set to 20.

The number of time steps the simulation was set to run was also defined. In every time step, the torque exerted on the blades was extracted from the simulation and stored in a report file. The report file was exported to MATLAB where the post-processing took place.

3.2 Validation

The validation consisted of creating a simulation set-up model that could be applied when conduct- ing the studies further on in this project. The validation was performed on a rotating semi-circular SSWT with an OR of 0.20, see figure 12a. Values for the C

and C

for different λ with an inlet velocity of 7 m/s were calculated and compared to the experimental data from Blackwell et al.

and the simulated data from Ferrari et al. and Mendoza et al.[5][16][33]

Table 1: Simulation settings in simulation series 1, 2 and 3.

Simulation 1 Simulation 2 Simulation 3

Domain width [m] 6 8 12

Domain length [m] 11.9 11.9 17

Inflation 4 16 16

Areas of refinement 1 1 2

Distance inlet to turbine [m] 2 2 5

(a) Semi-circular rotor

(b) Benesh rotor

Figure 12: The two rotors studied in the validation (a) semi-circular blade from Blackwell et al.

and (b) Benesh type from Roy and Saha.[16][17]

Three series of simulations at different λ were conducted. The different simulation settings for these simulations are presented in table 1. The first simulations, referred to as simulation 1, were conducted with a domain corresponding to Blackwell et al. experiments. For these simulations there was one area of refined mesh and the inflation was set to 4 layers. Thereafter, simulations were conducted where one different setting was varied to see how it affected the results. Increasing the inflation, widening the simulation domain, and changing the size of the mesh were tested.

Thereafter another series of simulations were conducted, referred to as simulation 2. For these simulations, the inflation was increased to 16 layers and the simulation domain width was increased to 8 m. A final series was performed which are referred to as simulation 3. The domain width was set to 12 m and the length of the simulation domain was also increased to 17 m. Two refinement regions of mesh were added, in order to have a smooth transition from the largest to the smallest cell sizes. The distance from the inlet of the simulation domain to the turbine was also increased to 5 m. The simulation domain set-up is presented in figure 13, where all distances are expressed in terms of the rotor diameter D. The cell sizes of the different regions and around the blades are presented in table 2.

Table 2: Cell size percentages relative to the width of the domain.

Cell Region 1 Region 2 region 3 Interface Rotor Blade

Percentage 4.1% 1.67% 0.42% 0.17% 0.17% 0.0833%

To summarize the validation, the same simulation set-up was applied to a different SSWT blade

configuration, the Benesh type, see figure 12b. The same correlation of simulation domain size and

mesh cell size in relation to the turbine diameter was used. These measurements were conducted

to test the new simulation set-up and its applicability to another type of blade configuration. The

values for the C

and C

for different λ with an inlet velocity of 6.26 m/s were compared to the

experimental values of Roy and Saha.[17]

Figure 13: Dimensions of the simulation domain expressed in terms of the diameter of the turbine.

The two dotted rectangles represent areas for refined cell sizes.

3.2.1 Simulation domain sensitivity study

A sensitivity study was carried out to decide the appropriate width for the simulation domain. This was done in between simulations 2 and 3. The domain width was investigated as a substantial change in C

and C

was observed when varying it. The study was done by running a number of simulations with identical settings and only varying the width of the simulation domain. The different widths tested were 6, 8, 12, 15, and 25 meters. All simulations were made at λ = 1.0 and an inlet velocity of 7 m/s. The results of this study can be seen in figure 14. It was observed that the C

only decreases by 0.006 between the widths of 12 and 25 meters. The computational cost for performing simulations in the 25-meter wide domain was significantly higher compared to the 12 m wide domain. However, the increase in accuracy of the result was only 2.8% percent.

Therefore, it was decided that a 12-meter wide domain was to be used in simulation run 3.

6 8 10 12 14 16 18 20 22 24 26

Width [m]

0.2 0.21 0.22 0.23 0.24 0.25 0.26 0.27

C P

Simulation Blackwell

Figure 14: Results of the C

at λ=1.0 from the sensitivity study for different widths of the

simulation domain

3.3 Study of the Modified Bach

The blade geometry study concerns a Modified Bach turbine as seen in figure 15. Roy and Saha showed that the Modified Bach generated the second-highest C

for many different Reynolds num- bers.[17] This blade profile also had an easily replicated geometry which is why it was chosen to be studied further. The CFD set-up established in the validation was applied when conducting the simulations on this turbine.

Figure 15: Modified Bach type blade.

The current studies on SSWTs at Uppsala University are focusing on rotors of dimensions between 0.3 and 0.5 meters and velocities in the range of 7 to 9 m/s. In previous studies λ values between 0.2 to 2.0 are investigated, therefore this study was conducted within the same range. The di- ameter of the rotor studied in this project was chosen to be 0.5 m. The choice of diameter was made due to that smaller rotors took longer time to simulate. This was observed in the validation when simulations were carried out on the Benesh turbine, which had a smaller diameter than the semi-circular. The inlet velocity was chosen to be 8 m/s, since it is in the middle of the range studied by Uppsala University. The goal of the project was to investigate if and how changes in two design parameters affect the C

of the turbine. The two selected parameters were the blade arc angle and the OR between the blades.

Firstly, a C

to λ curve was generated for a Modified Bach with a diameter of 0.5 meters, an OR of 0.4, and a blade arc angle of 110

. λ was varied between 0.4 and 1.4. New rotors were sketched in Fusion 360 with arc angles of 80

to 150

, with 10

increments. Then, a new series of simulations were performed for λ values to find the C

peak for each blade. It was not necessary to produce the whole λ curve for each blade since the interesting part was if the C

peak had moved and how high the C

value got. When the simulations had been conducted for all blade arc angles, the generated curves were compared with each other. The aim was to find which blade arc angle that generated the highest C

value. The blade with the highest C

to λ curve was then used to vary the OR.

Secondly, two different ORs were investigated with the values of 0.22 and 0.56. The rotor diameter

was kept constant while the bucket gap was varied. As a result, the diameter of the buckets had to

fluctuate. The same procedure, in order to determine which OR that gave the highest C

value,

was used as for the first parameter. The new C

to λ curve with improved parameters was then

compared with the original curve for the Modified Bach with a 110

blade arc angle.

4 Results

4.1 Validation

The validation process of the semi-circular blade, presented in figure 16, shows simulation 1, 2 and 3. The changes implemented after simulation 1 resulted in an improvement of 11.2% in simulation 2. One of the improvements from simulation 1 to simulation 2 was the increase in inflation layers.

Increasing the inflation led to a significant decrease in the y

value. 16 inflation layers were chosen to be used in future simulations since it resulted in a y

that stayed under 5, as desired. Between simulation 2 and 3, an improvement of 37.2% was achieved. Simulation 3 in figure 16 corresponds to the same series of simulations as in figure 17. In figure 17 it can be observed that the simulation set-up generated a C

curve with a similar shape as the experimental values of Blackwell et al.

within a range of 20%. The validation for the semi-circular blade was then considered satisfactory and complete.

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 2

-0.1 0 0.1 0.2 0.3 0.4 0.5

CQ

Blackwell et al.

Simulation 1

Simulation 2 Simulation 3

(a) C

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8

-0.05 0 0.05 0.1 0.15 0.2 0.25 0.3 0.35 0.4

CP

Blackwell et al.

Simulation 1

Simulation 2 Simulation 3

(b) C

Figure 16: Results of the three series of simulations of C

and C

viewing the optimization process in comparison with Blackwell et al.[16]

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8 2

-0.1 0 0.1 0.2 0.3 0.4 0.5

CQ

Blackwell et al.

Ferrari et al. (2D)

Mendoza et al. (3D) Simulation 3

(a) C

0 0.2 0.4 0.6 0.8 1 1.2 1.4 1.6 1.8

-0.05 0 0.05 0.1 0.15 0.2 0.25 0.3

CP

Blackwell et al.

Ferrari et al. (2D)

Mendoza et al. (3D) Simulation 3

(b) C

Figure 17: Results of the verification of C

and C

, plotted with the experimental results of

Blackwell et al. and numerical results of Ferrari et al. and Mendoza et al. for a semicircular

Savonius turbine with OR of 0.20.[5][16][33]

When the validation of the semi-circular blade was considered satisfactory, the simulation set-up was applied to a Benesh type rotor. The results of the simulations in relation to Roy and Saha are presented in figure 18. The simulation values were in a range of 4% and followed the shape of the Roy and Saha values well. Therefore the simulation set-up application was considered satisfactory.

The diameter of the Benesh turbine was smaller than the semi-circular and this resulted in more time-consuming simulations.

0 0.2 0.4 0.6 0.8 1 1.2

0.15 0.2 0.25 0.3 0.35 0.4 0.45 0.5 0.55 0.6

CQ

Roy Simulation

(a) C

0 0.2 0.4 0.6 0.8 1 1.2

0.05 0.1 0.15 0.2 0.25 0.3

CP

Roy Simulation

(b) C

Figure 18: Results of three series of simulations of C

and C

for the validation against the experimental results of Roy and Saha.[17]

4.2 Blade study

The results of the blade arc angle study are displayed in figure 19. The curves of the initial 110

blade arc angle Modified Bach rotor are plotted in black.

0.4 0.5 0.6 0.7 0.8 0.9 1 1.1 1.2 1.3 1.4

0.1 0.15 0.2 0.25 0.3 0.35 0.4 0.45

CQ

80^° 90°

100^° 110°

120^° 130°

140^° 150°

(a) C

0.4 0.5 0.6 0.7 0.8 0.9 1 1.1 1.2 1.3 1.4

0.16 0.18 0.2 0.22 0.24 0.26 0.28

CP

80^° 90°

100^° 110°

120^° 130°

140^° 150°

(b) C

Figure 19: Results of the series of simulations for different blade angles.

In order to clearly determine the efficiency of each rotor, the C

and P

values achieved

for each curve along with the corresponding λ values are disclosed in table 3. Thereupon, the

highest C

attained was for the 130

degree profile. Thus, this profile was then chosen to

study different ORs.

Table 3: Maximum C

for different blade angles and the maximum generated power.

Blade angle

λ C

P

[W]

80 0.6 0.2165 33.95

90 0.6 0.2249 35.26

100 1.0 0.2407 37.75

110 1.0 0.2396 37.57

120 0.8 0.2533 39.72

130 0.9 0.2627 41.19

140 1.1 0.2532 39.70

150 1.0 0.2603 40.81

The results of the OR study are presented in figure 20 and the highest C

and P

values, as well as the λ values at which they were achieved at, are displayed in table 4.

0.4 0.5 0.6 0.7 0.8 0.9 1 1.1 1.2 1.3 1.4

0.1 0.15 0.2 0.25 0.3 0.35 0.4 0.45

CQ

OR = 0.22 OR = 0.40 OR = 0.56

(a) C

0.4 0.5 0.6 0.7 0.8 0.9 1 1.1 1.2 1.3 1.4

0.16 0.18 0.2 0.22 0.24 0.26 0.28

CP

OR = 0.22 OR = 0.40 OR = 0.56

(b) C

Figure 20: Results of the series of simulations for different ORs.

Table 4: Maximum C

for different ORs and the maximum generated power.

OR λ C

P

[W]

0.22 0.8 0.2310 36.22 0.40 0.9 0.2627 41.19 0.56 0.9 0.2670 41.87

According to both figure 20 and table 4, the rotor that obtained the highest C

was the one with

an OR of 0.56. The initial Modified Bach rotor with a 110

blade arc angle and an OR of 0.4 was

then plotted alongside the optimized one with a 130

blade arc angle and an OR of 0.56 in figure

21. An improvement of 8.15% was achieved in this blade study.

0.4 0.5 0.6 0.7 0.8 0.9 1 1.1 1.2 1.3 1.4 0.1

0.15 0.2 0.25 0.3 0.35 0.4 0.45

CQ

Angle = 110^°, OR = 0.4 Angle = 130^°, OR = 0.56

(a) C

0.4 0.5 0.6 0.7 0.8 0.9 1 1.1 1.2 1.3 1.4

0.16 0.18 0.2 0.22 0.24 0.26 0.28

CP

Angle = 110^°, OR = 0.4 Angle = 130^°, OR = 0.56

(b) C

Figure 21: The initial Modified Bach rotor with a blade arc angle of 110

and an OR of 0.4 plotted with the optimized rotor with a blade arc angle 130

and an OR of 0.56.

It is worth mentioning that for all performed simulations the obtained y

never exceeded the value of 5. On the contrary, the y

value fluctuated in the interval of 0 to 3, as seen in figure 22.

Figure 22: Example of the y

measured along the blades.

5 Discussion

The results for the different blade arc angles that were tested are presented in figure 19. From

this figure, it can be determined that the C

peak value for the initial blade arc angle of 110

is

approximately at λ = 1.0. Moreover, this curve has a wide peak, meaning that for a broad range

of λ values the C

does not vary a lot. In addition to this observation, the C

curves for the 80

and 90

blade arc angles are considerably lower than for the 110

profile. Thus, the C

is

lower for these angles compared with the 110

blade arc angle. Therefore, the 80

and 90

profiles

are considered less efficient. In the range between 0.6 and 1 of λ it is evident that the C

curve is

almost identical for the 100

and 110

profiles. However, after λ = 1.0 the curve for the 100

profile

drops much more than for 110

profile. Hence, it can be argued that the turbine with a blade arc

angle of 100

is not the better option because it has a narrower and sharper peak. For the blade

arc angles of larger values, it is clear that all the curves lay above the 110

profile curve. Therefore,

these angles can be seen as better options based on these results. The 140

profile and the 150

profile are also interesting to mention. In relation to the performance of the 130

profile the 140

profile generate lower values of C

while the 150

profile show almost a similar performance. The

130

profile results in the highest C

values for λ = 0.9 and λ = 1.0. Thus, this profile was chosen

when moving forward to investigate the second parameter, OR.

The results for the different ORs are presented in figure 20. The blade arc angle study was con- ducted for a blade with OR 0.4. In this part, ORs of 0.22 and 0.56 were tested. The OR of 0.22 generated a C

curve with considerably lower values than for the OR of 0.4. The OR of 0.56 generates a C

= 0.2651 at λ = 1.0 and this is somewhat larger than the OR of 0.4 which generates a C

= 0.2627 at λ = 0.9. Judging from these simulations, the increase of the OR to 0.56 generates a larger C

overall. Therefore the OR 0.56 is deemed to be the better one of the three ORs studied. The blade of the initial Modified Bach turbine in comparison to the blade with a 130

blade arc angle and an OR of 0.56 are presented in figure 21. However, only three different ORs were investigated and another OR might generate a large C

.

As the results of this study are based on simulations, they depend completely on how well the simulation model depicts reality. When simulations are performed there will always be uncertain- ties and the flow can never be calculated completely accurate at every point. The mesh could always be more refined and a larger simulation domain could be used. However, these types of changes would lead to a higher amount of cells which would contribute to a considerably longer simulation time and higher computational costs. The number of simulations was limited by the available computational power. The simulations in this project were conducted using laptops which were a restriction because of their computational capacities. In order to perform more precise simulations and at a higher rate, supercomputers would be a suitable and more efficient option to use. Ideally, more simulations for several more λ than the ones presented in figure 19 would have been performed to give more accurate results with smoother curves. However, due to the restrictions mentioned above, this was not possible. Considering figure 19b, the C

peak for the 130

profile could be between = 0.8 to = 1.1. The C

peak for the 150

profile could be higher than for the 130

at some values of λ around 1 that have not yet been investigated.

The same arguments could be made regarding figure 20b. Consequently, there are some uncer- tainties when analyzing the graphs which would have been eliminated if more λ values would have been simulated. It is also important to keep in mind that these simulations were two-dimensional.

Two-dimensional simulations do not take into account turbulence effects and swirls that may occur at the top and bottom of a turbine. These phenomenons may affect the performance of the turbine.

The final rotor that was concluded to give the highest performance in this report does not necessar- ily have to be the most beneficial one. There are several more interesting parameters to investigate further. For example, the gap ratio, which is the distance between the blades. Changes in this parameter would result in different flows inside the turbine that possibly could lead to higher C

values. It would also be of interest to study the performance of different blade geometries for

different inlet velocities. This could perhaps lead to changes in the rotors moment and therefore

affect the C

and C

either positively or negatively. If SSWTs are going to be used on a larger

scale in the future, they might be installed in groups and in close proximity to each other. There-

fore, it could be of interest to study the effects of several turbines close to each other. From the

simulations conducted it was observed that the turbines induced a wake. This was observed as

the velocity downstream of the turbine was decreased for a considerable distance. Hence, it would

not be beneficial to place additional turbines in this area. How to arrange multiple turbines in the

proximity of each other would be an interesting topic for further studies.

6 Conclusion

A simulation model was created and used in order to validate existing experimental data with nu- merical simulations. The simulated values for C

and C

corresponded well to the experimental ones after some adjustments in the model. This model was then used for studying two different design parameters, the blade arc angle and the OR.

In conclusion, the rotor that achieved the highest C

had a blade arc angle of 130

and an OR

of 0.56. It would have been preferred to study a wider range of ORs in order to better under-

stand their effect on the SSWT performance. However, that could not have been accomplished in

the time-frame given to complete this study. Furthermore, this study contains some uncertainties

mainly because it is based on simulations. There can always be made improvements in a simulation

model which can lead to better results. On the other hand, these types of changes are restricted

by computational power. It is hard to draw a clear conclusion from this study because of all the

uncertainties but a trend can be distinguished. A bigger blade arc angle and a bigger OR seems

to contribute to the pressure difference around the blades, which results in a higher C

.

References

[1] F. R. Eldridge, Wind Machines. United States: Van Nostrand Reinhold Inc., 1982.

[2] D. G. Shephered, “Historical development of the windmill”, 1990, NASA, United States En- ergy Research Development Administration.

[3] S. Savonius, The Wing-rotor in Theory and Practice. Finland: Savonius Co, 1925.

[4] F. Coyle, Introduction to Wind Power. United States: English Press International, 2011, ch. 9.

[5] V. Mendoza, E. Katsidoniotaki, and H. Bernhoff, “Numerical Study of Novel Concept for Manufacturing Savonius Turbines with Twisted Blades”, Energies, vol. 13, 2020.

[6] New World Wind, The Wind Tree, Available here.

[7] Shell, Sarah Kempe, Winds of change: Turbine turns Traffic into Energy, Available here.

[8] Regeringskansliet, The swedish national action plan for the promotion of the use of renewable energy in accordance with directive 2009/28/ec and the commission decision of 30.06.2009.

Available here, 2010.

[9] W. Europe, Data analysis, statistics, Available here, Feb. 2020.

[10] R.B. Hiremath and Bimlesh Kumar and P. Balachandra and N.H. Ravindranath and B.N.

Raghunandan, “Decentralised renewable energy: Scope, relevance and applications in the Indian context”, Energy for Sustainable Development, vol. 13, Oct. 2018.

[11] François Bouffard and Daniel S.Kirschen, “Centralised and distributed electricity systems”, Energy Policy, vol. 36, Oct. 2018.

[12] F. Coyle, Computational Fluid Dynamics - A Practical Approach. United States: English Press International, 2011, ch. 9.

[13] Encyclopedia Britannica Academic, Available here.

[14] W. Oberkampf and T. Trucano, “Verification and validation in computational fluid dynam- ics”, Progress in Aerospace Sciences, vol. 38, 2002.

[15] M. Ragheb and A. M. Ragheb, “Wind Turbines Theory - The Betz Equation and Optimal Rotor Tip Speed Ratio”, in Fundamental and Advanced Topics in Wind Power. Croatia:

InTech, 2011, ch. 2, isbn: 978-953-307-508-2.

[16] B. F. Blackwell, R. E. Sheldahl, and L. V. Feltz, “Wind Tunnel Performance Data for Two- and Three-Bucket Savonius Rotors”, NASA, United States Energy Research Development Administration, 1977.

[17] S. Roy and U. K. Saha, “Wind tunnel experiments of a newly developed two-bladed Savonius- style wind turbine”, Applied Energy, 2015.

[18] M. Ebrahimpour, R. Shafaghat, R. Alamian, and M. S. Shadloo, “Numerical Investigation of the Savonius Vertical Axis Wind Turbine and Evaluation of the Effect of the Overlap Parameter in Both Horizontal and Vertical Directions on Its Performance”, Symmetry, vol. 11, 2019.

[19] M. Zemamou, M. Aggour, and A. Toumi, “Review of Savonius wind turbine design and performance”, Energy Procedia, vol. 141, 2017.

[20] A. Moutsoglou and Y. Weng, “Performance Tests of a Benesh Wind Turbine Rotor and a Savonius Rotor”, Wind Engineering, vol. 19, 1995.

[21] Ansys, Ansys fluent, Available here, 2020.

[22] A. Goude, Simulering, Studentportalen, Tillämpad mekanik III med strömningslära, Uppsala University, 2019.

[23] R. Peyret, Handbook of Computational Fluid Mechanics. Elsevier Science, 1996, ch. 7, isbn:

9780125530101.

[24] Ansys, Ansys Fluent User Guide, Available here, 2011.