CFD Analysis of Flow Induced Vibration of Offshore Structures

German Institute of Science and
Technology – TUM Asia Pte. Ltd.
CFD analysis of Flow Induced Vibration of Cylinders
and Offshore Structures
Submitted by
Isaac Mark Joseph Manasseh
Master of Science in Aerospace Engineering
August 2013/2014

CFD analysis of Flow Induced vibration of Cylinders and Offshore
Structures
A dissertation submitted to Nanyang Technological University in
partial fulfillment of the requirement for the degree of Master of
Science in Aerospace Engineering
Supervised by
Assistant Professor Martin Skote
School of Mechanical and Aerospace Engineering
Nanyang Technological University
2016

i
ABSTRACT
Flow induced vibration is one of the major contributors to reduction in fatigue life of
offshore structures. The two phenomena associated with fluid-structure interaction
are: The vortex Induced Vibration, observed in structures with high aspect ratio like
the risers and mooring systems; the Vortex Induced Motion of offshore platforms
with low aspect ratio. A high fidelity fluid dynamics simulation is required to study
the above phenomena and the corresponding data is recommended for the
manufacture of structures which are not susceptible to Flow Induced Vibrations.
kOmegaSST and kEpsilon employing RANS have proven to be reliable turbulence
models to calculate hydrodynamic forces. The objective of the thesis is firstly, to
investigate the effects of flow around cylinders at various Reynolds numbers and
secondly, to propose a universal methodology to capture the VIM phenomenon. In
this thesis the OpenFOAM software’s groundwork is investigated concerning its
capability to perform transient simulations.
The simulations for cylinders were run at various flow regimes and the results were
found to be satisfactory. The force coefficient – Reynolds number relationship have
good conformity with other experimental results. The snappyHexMesh utility has
proven to generate converged results for complex grids with low values of
dimensionless wall distance 𝑦+
.
The main recommendation from the present work is to employ OpenFOAM’s mesh
utility for meshing complex offshore models and transient simulation capabilities for
predicting hydrodynamic forces.

ii
Acknowledgement
I wish to express my sincere gratitude to Dr. Nguyen Vinh Tan, Scientist, Capability
Group Manager for providing me an opportunity to work on his project and for his
continual support and guidance during my time as Research Intern at A*STAR-IHPC.
I would like to express my thanks to Assistant Professor Martin Skote for accepting
my Thesis proposal and guiding me through the period of my Thesis. His instant and
calm natured reply to my queries provided me the encouragement and the reassurance
to reach out to him during any part of the day.
I would also like to express my appreciation and thanks to Dr. Lou Jing, Department
director, Principal Scientist at A*STAR IHPC for taking the first initiatives to provide
me a research project for my Thesis.
Finally, I would like to thank my fellow research Intern Mr. Anand Sudhi, for his
valuable input and guidance concerning the ground work involved in Computational
Fluid Dynamics. I have immensely benefitted by working alongside him at A*STAR-
Institute of High Performance Computing.

iii
Table of Contents
ABSTRACT................................................................................................................................ i
Acknowledgement ................................................................................................................. ii
Nomenclature ........................................................................................................................ v
Abbreviation........................................................................................................................... v
Symbols..................................................................................................................................vi
List of Figures ........................................................................................................................vii
List of Tables...........................................................................................................................ix
CHAPTER 1: INTRODUCTION.................................................................................................. 1
1.1Background and motivation:......................................................................................... 1
1.2 Scope:........................................................................................................................... 2
1.3 Objectives:.................................................................................................................... 3
1.4 Organization of the report:.......................................................................................... 3
CHAPTER 2: LITERATURE REVIEW .......................................................................................... 4
2.1 Flow around Cylinders: ................................................................................................ 4
2.1.1 Fixed Cylinders: ..................................................................................................... 6
2.1.2 Oscillating cylinders: ........................................................................................... 10
2.3 Validation for computational fluid dynamics studies: ............................................... 13
2.4 Literature on flow around semi-submersible Structures:.......................................... 15
2.4.1 A review on experimental semi-submersible model: ......................................... 17
2.4.2 Model and experimental setup:.......................................................................... 19
2.4.3 Hydrodynamic forces and experimental validation:........................................... 22
CHAPTER 3: Computational Fluid Dynamics ........................................................................ 24
3.1 CFD methodology:...................................................................................................... 24
3.1.1 Governing Equations:.......................................................................................... 24
3.1.2: Turbulence Models: ........................................................................................... 28
3.1.3 Wall Function: ..................................................................................................... 30
3.2 Introduction to OpenFOAM:...................................................................................... 33
3.2.1 OpenFOAM case directory:................................................................................. 35
3.2.2 Discretization Schemes and Solver control:........................................................ 40
3.2.3 Steps involved in solving transport equation & working of the PISO loop:........ 42
CHAPTER 4: METHODOLOGY ............................................................................................... 46
4.1.1 Selection of Reynolds number for the Simulation:............................................. 48

iv
4.1.2 Mesh used for simulations:................................................................................. 49
4.1.4 Initial Flow conditions:........................................................................................ 52
4.1.5 Refined mesh for high Reynolds number simulation:......................................... 53
4.2 Procedure for VIM simulation of semi-submersibles: ............................................... 56
4.2.1 Design of deep-draft semi-submersible:............................................................. 57
4.2.2 3Dimensional mesh:............................................................................................ 59
4.2.4 Projection area and Reynolds number: .............................................................. 64
CHAPTER 5: RESULTS & DISCUSSION ................................................................................... 66
5.1 Flow over cylinders: ................................................................................................... 66
5.1.1 REYNOLDS NUMBER = 30:................................................................................... 66
5.1.2 REYNOLDS NUMBER = 200:................................................................................. 67
5.1.3 REYNOLDS NUMBER = 3500................................................................................ 68
5.1.4 REYNOLDS NUMBER = 10000:............................................................................. 70
5.1.5 High Reynolds number simulation using a coarse mesh: ................................... 75
5.1.6 High Reynolds number simulation using a refined mesh (Non-orthogonal mesh):
...................................................................................................................................... 76
5.2 CFD analysis of the semi-submersible model: ........................................................... 83
5.2.1 Discussion on the mesh parameters:.................................................................. 83
5.2.2 simpleFoam simulation (Steady state simulation):............................................. 86
Chapter 6: Conclusion and Future Work.............................................................................. 90
6.1 Thesis Summary: ........................................................................................................ 90
6.1.1: VIV simulation:................................................................................................... 90
6.1.2: VIM simulation:.................................................................................................. 91
6.2 Recommendations: .................................................................................................... 92
References ........................................................................................................................... 93
Appendix A – Mesh Generation........................................................................................... 96
Appendix B – fvSchemes & fvSolution:.............................................................................. 108
Appendix C –Turbulent boundary conditions:................................................................... 118
Appendix D: Mesh and Initial Conditions........................................................................... 125

v
Nomenclature
𝐴 𝑃 Projection Area
𝐶 𝐷 Drag Coefficient
𝐶 𝐷𝑚𝑒𝑎𝑛 Mean Coefficient of Drag
𝐶𝐿𝑟𝑚𝑠 Root Mean Square of Lift Coefficient
D Diameter of the Cylinder/Characteristic Length of the semi-submersible
𝐹𝐷 Drag Force
𝐹𝐿 Lift Forces
St Strouhal Number
𝑉𝑟 Reduced Velocity
Re Reynolds Number
𝐴
𝐷⁄ Non-dimensional Amplitude
𝑓𝑣𝑠 Frequency of Vortex Shedding
𝐶 𝑝 Coefficient of Pressure
𝑓𝐿 Frequency of Lift
𝑓𝑛 Natural Frequency of the Cylinder
𝑓𝑓 Forcing Frequency
L Turbulent Length Scale
𝑓𝑁 Natural Frequency in Still Water
𝑇 𝑁 Natural Period in Still Water
X In-line direction
Y Transverse direction
𝑘 𝑥/𝑘 𝑦 Spring Stiffness
T DDS Column Height
S DDS Column Spacing
P DDS Pontoon Height
𝑚 𝑟 Mass Ratio
Abbreviation
VIV Vortex Induced Vibration
VIM Vortex Induced Motion

vi
DDS Deep-Draft Semi-Submersible
RANS Reynolds Averaged Navier-Stokes Equation
DES Detached Eddy Simulation
LES Large Eddy Simulation
Symbols
𝜙 Transport Property
𝜌 Density
𝜐 Kinematic Viscosity
𝜏 Viscous Stress
𝜃 Phase angle of the Cylinder/Heading angle of the DDS
Γ Diffusion Coefficient
𝑦+
Dimensionless Wall Distance
𝜔 Specific Turbulence Dissipation Rate
𝜖 Turbulent Dissipation

vii
List of Figures
Figure 2.1: Vortex Shedding behind a Cylinder……………………………………………………..……….….6
Figure 2.2: Strouhal number versus Reynolds number.........................................................8
Figure 2.3: Coefficient of Lift and Drag……………………………..…...…………………………..………….…9
Figure 2.4: Frequency of Oscillation and Vortex shedding frequency……..……………………....12
Figure 2.5: DDS strucutre…………………………………………………………………………………………….....17
Figure 2.6: Towing tank……………………………..……………………………………………………………….…..19
Figure 2.7: Deep-draft Semi-submersible models……..……………………………………………….……20
Figure 2.8: Equal Spring Stiffness………………………………………..…………………………………….…….20
Figure 2.9: Charecteristic Length…………………………………………………..………………………….…….21
Figure 2.10: Force Coefficient plot (DDS Experimental plots)………..……..………………….……..23
Figure 3.1: Control Volume Cells………………………………………………………………………………….….26
Figure 3.2: Turbulence fluctuations……………………………………………..…………………………….……28
Figure 3.3: Dimensionless Wall Function………………………………..……………………………………….31
Figure 3.4: Turbulence Model (Wall Function & Resolved Grid)………..…………………………….32
Figure 3.5: OpenFOAM Directory…………………………………………………………………………………….36
Figure 4.1: 𝐶 𝐷 plot; Zdravkovich (1990) & Massey (1989) ……………………………………………….45
Figure 4.2: CL plot; Norgberg (2003); Stringer et al. (2016)…………………………………….……….46
Figure 4.3: Strouhal Number VS Reynolds number plot…………………..………………………………46
Figure 4.4: Flow Regimes around a Circular Cylinder………………………………………..……………..47
Figure 4.5: Coarse Mesh………………………………………………………………………………………………….49
Figure 4.6: Hover Cylinder Mesh……………………………………………………………………………………..50
Figure 4.7: Boundary Conditions…………………………………………………..…………………………………50
Figure 4.8: blockMeshDict…………………………………………………………..………………………………....53
Figure 4.9: Refined blockMesh……………………………………………………..…………………………………54
Figure 4.10: CAD Model (DDS scaled model)……………………………………………………………………57
Figure 4.11: Calculation of Moment of Inertia………………………………..……………………………….57
Figure 4.12: snappyHexMesh of DDS Geometry……………………………………………………..……….60
Figure 4.13: Uniform Mesh (Cross-Sectional view of the vertical Columns)………..…...……..61
Figure 4.14: Mesh Properties……………………………………………………………………………..…………..61
Figure 4.15: Projection Area………………………………………………………………………………………..….63
Figure 4.16: Mooring System……………………………………………………………………………..…………..63
Figure 5.1: Flow over Cylinder (Re = 30)………………………………………………………………..………..65

viii
Figure 5.2: Flow Over Cylinder (Re = 200)……………………….……………..………………….…….........66
Figure 5.3: Force Coefficients (Re = 200)………………………..…..………….……………………….……...66
Figure 5.4: Strouhal Number (Re = 200 )……………………………….……..………………………………….67
Figure 5.5: Force Coefficients (Re = 3500)……………………..………….…..………………………………..68
Figure 5.6: Force Coefficients (Re = 10000)…………………………..…………………………..….…………70
Figure 5.7: Flow Domain - DES Simulation (Re = 40000)…………………..………………….…………..71
Figure 5.8: Over Prediction of CL…………………………………………………..………………………………..75
Figure 5.9: Coefficient of Lift (kEpsilon Turbulence Model)………….……..………….…………….…77
Figure 5.10: Coefficient of Drag (kEpsilon Turbulence Model)……..…………………….…..……....77
Figure 5.11: Force Coefficient using FFT matlab Code (kEpsilon Turbulence M..del)….….…78
Figure 5.12: Strouhal Number…………………………………………………..………………………………….…78
Figure 5.13: Mesh Convergence Study……………………………….……………………………..……..…….79
Figure 5.14: CLrms plot (Numerical Values vs Experimental Values)..…….….…...……..……….80
Figure 5.15: CDmean plot (Numerical Values vs Experimental Values)…..…….…………………..81
Figure 5.16: Coarse mesh (DDS Geometry)………………………………..……………………………………82
Figure 5.17: Non-uniform mesh………………………………………………………..…………………………….83
Figure 5.18: Wrong Projection Area……………………………………………..…………………………………85
Figure 5.19: Pressure Residual (simpleFoam)…………………………………..……………………………..86
Figure 5.20: Coefficient of Drag for the Correct Projection Area……..……….……………………..86
Figure 5.21: pimpleFoam Pressure Residual……………………………………..…………………………….87
Figure 5.22: Force Coefficient for Transient Simulation………..……..………………………….……..87
Figure 5.23: Coefficient of Lift Fluctuations…………………………………..…….………………………….88

ix
List of Tables
Table 2.1: Deep-draft Semi-submersible Dimensions..........................................................21
Table 2.2: Reduced Velocity.................................................................................................21
Table 4.1: Boundary Conditions...........................................................................................51
Table 4.2: Experimental Force Coefficient Values................................................................52
Table 4.3: Scaled Geometry DDS Dimension........................................................................56
Table 4.4: Turbulence Properties.........................................................................................62
Table 5.1: DES Simulation.....................................................................................................72
Table 5.2: Mesh Convergence Study....................................................................................79

1
CHAPTER 1: INTRODUCTION
1.1 Background and motivation:
The flow around a cylinder has been an area of intense research and from time to time
has posed several fundamental problems to researchers, owing to the complex and
transitory nature of the wake vortices. These wake vortices appear are a result of
vortex shedding from a body, due to fluid-structure interaction. The motivation to
comprehensively examine vortex shedding is its presence in the offshore application.
Be it a riser system transporting oil from the sea bed or a huge floating offshore
platform; each of these structures experience vortex shedding in a unique manner. On
closer analysis, Flow induced vibration due to fluid-structure interaction can be
categorized mainly as the following, they are:
 Vortex Induced Vibration and
 Vortex Induced Motion
The vortex shedding behind cylindrical bodies, with high aspect ratio, induce motion
as a result of fluid-structure interaction. This is called the Vortex Induced Vibration
and is observed among flexible risers and mooring systems. The other category of
offshore structures which experience vortex shedding, possess low aspect ratio. They
are notably floatable structures in the form of Monocolumns, TLPs and the semi-
submersibles. Any or all of the vortex shedding phenomenon affect the fatigue life of
a structure. Although, this study covers the area of research conducted on semi-
submersible structures only. The structure is made up of four vertical square columns,
each attached to a base pontoon. The pontoon imparts buoyancy to the overall
structure. The vortex shedding behind each of these columns may differ as a
consequence of wake interference between them. The motion induced due to this type
of shedding is called the Vortex Induced Motion. The VIM is a complex phenomenon
because it is characterised by both Vortex Induced Vibration and Wake Induced
Vibration.

2
The CFD analysis is aimed at studying the two phenomena:
 VIV of cylinders at various Reynolds numbers and
 VIM of deep-draft semi-submersible structure.
The literature throws light on previous experimental work in this domain and
formulates the properties which govern the hydrodynamic effects. But in order to
examine the susceptibility of new offshore designs, high fidelity fluid dynamics
validation is required. There is also ample support for the claims that previous
experimental research needs numerical validation. The simulation in this thesis
advances chronologically into solving two problems. Firstly, The CFD analysis of
cylinders are compiled using an open source application called the OpenFOAM. This
then lays down the platform for inspecting more complex structures like the deep-
draft semi-submersibles. The objective of the thesis is to propose a universal CFD
methodology by which the vibration phenomenon can be studied. So then the
objective is not to present detailed VIM response of the model, but to capture the
phenomenon of Vortex Induced Motion without missing the physics of the flow.
For this purpose, three experimental papers are chosen for examining the VIV
phenomenon in cylindrical structures (Ong, Utnes, Holmedal, & Dag Myrhaung,
2009), (Stringer, Zang, & Hillis, 2014) and (Norberg, 2003). Secondly, another three
papers are selected for validating the VIM phenomenon observed among the semi-
submersible structures (Goncalves, Fujarra, Rosetti, Kogishi, & Koop, 2015),
(Rodolfo T. Goncalves, 2012) and (Fujarra, Goncalves, Rosetti, jr., & Koop, 2015).
1.2 Scope:
The simulations in this thesis is divided into two parts:
1. Simulation of flow around cylinders
 Low Reynolds flow simulations: CFD analysis were carried out for
various low Reynolds number flows (Re < 1000) using a 3D mesh.
 High Reynolds flow Simulation: CFD flow simulations were
performed for high Reynolds numbers (3500 < Re < 2 ∗ 106
), using
2D and 3D mesh.

3
 A special super-critical flow simulation was performed to analyse the
flexibility of the OpenFOAM solvers at High Reynolds numbers.
2. Simulation of flow around semi-submersibles
Static and transient simulations were performed on a 3D snappyHexMesh for
Reynolds number = 60,000 (Heading angle = 45°
)
1.3 Objectives:
The objectives of the thesis are as follows:
 To study the VIV phenomenon of cylinders and to measure the force
coefficients at various Reynolds numbers.
 To calculate Strouhal number for each of the simulation.
 To validate and analyse the relationship between force coefficients, Strouhal
number and the Reynolds number, using an experimental plot.
 To analyse the behaviour of the OpenFOAM solvers and the capability of
transient simulations to study the VIV phenomenon,
 To set up a complex 3D mesh with low non-orthogonality and skewed cells
and
 To numerically analyse the VIM phenomenon in the semi-submersible using
a complex 3D grid.
1.4 Organization of the report:
 Chapter 2: Literature review is presented for the flow around cylinders and
flow over deep-draft semi-submersible model.
 Chapter 3: Presents ground work for CFD methodology and Introduction to
OpenFOAM.
 Chapter 4: Presents methodology for setting up simulations for cylinders and
deep-draft semi-submersibles structures.
 Chapter 5: Discussion of results from the flow simulations.
 Chapter 6: Conclusion and future recommendations.

4
CHAPTER 2: LITERATURE REVIEW
2.1 Flow around Cylinders:
A flow past a cylinder will result in recurrent shedding of vortices. These shed
vortices induce motion on the body in the form of oscillatory Lift and drag, popularly
known as the Vortex Induced Vibration. The oscillatory motion of the cylinder is
altered as the velocity of the fluid varies. Cylinders represent marine structures with
high aspect ratio, like offshore oil risers and mooring systems. VIV can reduce the
fatigue life of these structures drastically. It is thus important to analyse the flow
around a cylinder as an initiative to reduce the susceptibility to flow induced
vibration. Below is a literature presented for flow around both fixed and flexible
cylinders, which then leads to a more specific method used for measuring
hydrodynamic forces around cylinders. The latter part of the literature is the main
focus for Computational Fluid dynamics simulation and validation. The flow around
cylinders can be classified into two categories, namely:
 Flow over a fixed cylinder and
 Flow over an oscillating cylinder.
The flow over an oscillating cylinder can be further classified on the basis of the
Nature of Vibration. They are:
1. Forced Vibration: Here the cylinder is made to oscillate at a specific
frequency as it comes in contact with the fluid flow. Example: A person
producing swivel motions in a wire, simultaneously immersed in a tank of
continuous fluid flow.
2. Free Vibration: Here there is no forced oscillations given to the cylinder,
whereas the Cylinder oscillates naturally as a result of fluid-structure
interaction.

5
Non-Dimensional Quantities:
Non-dimensional amplitude: 𝐴
𝐷⁄ , 𝐴 is the amplitude of the Oscillatory motion
and 𝐷 is the diameter of the cylinder.
Reduced Velocity: Reduced Velocity can be defined as the free stream velocity
flowing over a cylinder of diameter D, oscillating with a frequency ‘f’’. In other
words it can be interpreted as the incoming free stream velocity divided by a
component 𝐷𝑓.
𝑉𝑟 =
𝑈∞
𝐷𝑓
Reynolds number: The Reynolds number is defined as the ratio of inertial force
by the viscous force. At low Reynolds number the flow is dominated by the viscous
force and at high Reynolds number the flow is dominated by the inertial force. The
formula is given by:
𝑅𝑒 =
𝑈∞ 𝐷
𝜈
Mass Ratio: It is defined as the ratio of mass of the structure to the mass of the fluid
displaced. This ratio plays a very crucial role in the motion of oscillating cylinders
due to its influence on the damping factor.
𝑚 𝑟 =
𝑚 𝑠
𝑚 𝑓
An important quantity to measure during the study of cylinders is the non-
dimensional amplitude. There are other fluid flow quantities which have a profound
impact on the amplitude. They are written as a functional expression below:
𝐴
𝐷⁄ = 𝑓( 𝑙
𝐷⁄ , 𝑉𝑟, 𝑅𝑒, 𝑚 𝑟)

6
2.1.1 Fixed Cylinders:
As mentioned earlier, research establishments have expanded their computational
capabilities in order to understand the nature of Vortex shedding. In that, the
computational fluid dynamics of fixed cylinders is sufficient enough to understand
the transient nature of the flow over bluff bodies. Aerodynamic quantities such as
coefficient of Lift, coefficient of drag and Strouhal number can be analysed. It
provides compelling ideas to choosing the right combination of discretization
schemes and solutions to solve unsteady flows. The same technique can be adopted
for the study of flow over complex geometries in the likes of semi-submersible
models. During the course of the thesis, computational fluid dynamics of fixed
cylinders were carried out and validated with the experimental results. But before
moving into the computational aspect of the cylindrical body, it is good to know the
previous experimental methods and their drawbacks.
Figure 2.1: Vortex shedding behind a cylinder (Kármán, 1994)
The literature study enables good understanding of the mechanisms for developing a
mathematical reduced order model for impersonating Vortex Induced Vibration. In
the above figure, a vortex street is visible. The reason for vortex is the interaction
between the two shear layers arising from the sides of the cylindrical body. This
vortex generated from the side grows in size due to rotatory accumulation of fluid
called the circulation zone, and stops when it is strong enough to attract the opposing

7
wake vortex to cut across it. This then moves downstream as ‘shed’ vortex. Since the
wake structure for the overall shedding involves interaction between two oppositely
signed vortices, the strength of the wake is less in magnitude when compared to the
strength of the circulation zone appearing from one side of the bluff body. The rate
of circulatory shedding at the separation points is given by the formula:
𝑑𝛤
𝑑𝑡
=
1
2
𝑉𝑏
2
(2.1)
Here 𝑉𝑏 is the mean velocity at the boundary edge where the separation takes place.
The mean velocity is given by the formula: 𝑉𝑏
2
= 𝑉2
(1 − 𝐶 𝑝𝑏). Where the
component 𝐶 𝑝𝑏 is called the mean base pressure coefficient.
Strouhal Number: This number is defined as the ratio of the product of frequency
and the cylinder diameter, divided by free stream velocity.
𝑆𝑡 =
𝑓𝑣𝑠 𝐷
𝑈∞
(2.2)
The above formula illustrates that the Strouhal number is basically the inverse of the
reduced velocity. Here 𝑓𝑣 𝑠 represents the vortex shedding frequency. It is crucial to
note that the definition of Strouhal number for an oscillating cylinder differs from a
fixed cylinder with regards to the frequency exhibited. And so, careful attention is
required to understand the notations. Firstly, for a fixed cylinder the frequency of the
Coefficient of lift 𝑓𝐿 is equal to the vortex shedding frequency mentioned above. It
is by this argument that we claim that vortex shedding is the reason why the cylinder
exhibits oscillatory lift. The Strouhal number for a fixed cylinder is bound to increase
as the Reynolds number or the reduced velocity is increased. On considering the flow
over a fixed rigid cylinder, there is an increase in Strouhal number after the subcritical
Reynolds Number is surpassed. But overall, there exits something called the linear
dependency of shedding frequency, which is illustrated in the figure 2.2.It is because
of this dependency that the Strouhal number stays at a value of 0.2 for a wide range
of Reynolds numbers. That is to say the frequency 𝑓𝑣 𝑠 increases in the numerator of
the Strouhal number when the denominator free stream velocity also increases. After
the subcritical Reynolds number the vortex shedding frequency starts to dominate.

8
Figure 2.2: Strouhal number Vs Reynolds number (Zahari)
The Aerodynamic Coefficients:
The coefficient of lift is calculated using the change in pressure across the bluff body.
It is given by the equation:
𝐶 𝑝 =
𝑝−𝑝∞
1
2
𝜌∞ 𝑈∞
2
(2.3)
The Coefficient of Lift and Drag is given by the formulation,
𝐶𝑙(𝑡) =
𝐿(𝑡)
1
2⁄ 𝜌𝑉∞
2 𝐷
= √2𝐶𝐿
𝑟𝑚𝑠
𝑆𝑖𝑛(
𝑆𝑡2𝜋𝑈∞
𝐷
𝑡) (2.4)
𝐶 𝐷(𝑡) =
𝐷(𝑡)
1
2⁄ 𝜌𝑉∞
2 𝐷
= √2𝐶 𝐷
𝑚𝑒𝑎𝑛
𝑆𝑖𝑛(2
𝑆𝑡2𝜋𝑈∞
𝐷
𝑡) (2.5)
From the above equations, the frequency of Drag oscillates twice that of the
frequency of Lift i.e. 𝑓𝐷~2𝑓𝑣 𝑠 ≅ 2𝑓𝐿. This is due to the fact that one lift oscillation
period is produced when two alternate oppositely signed vortices are shed, whereas
one drag oscillation period is produced when a single vortex is shed from the side of
the body. One can perceive this as the generation of one fluctuating drag for every
vortex shed and one fluctuating lift generated after two counter rotating vortices are
shed. This is presented in the figure 2.3.

9
Figure 2.3: Coefficient of Lift & Drag (Sumer & Fredsøe, 1997)
It is also crucial to know why a root mean square value for coefficient of lift and
mean value for coefficient of drag is considered for calculation. The reason is that the
coefficient of lift oscillates about zero and thus calculating an average would
eventually equal zero. On the other hand, Coefficient of Drag oscillates about a
specific value other than zero. This is quite evident from the above illustration in
Figure 2.3. In our representation, lift and drag coefficients are detonated by the
expressions 𝐶𝐿,𝑟𝑚𝑠 and 𝐶 𝐷,𝑚𝑒𝑎𝑛.
The shape of the geometry is primarily responsible for the feedback effect between
the wake and the circulation at the separation points. This is the popularly acclaimed
reason for why the frequency of the fluctuating lift is almost equal to that of the vortex
shedding, 𝑓𝐿~𝑓𝑣𝑠. The vortex shedding depends on several other factors other than
the Reynolds number. They are,
 Surface roughness,
 Aspect ratio,
 Turbulence Intensity,
 Acoustic perturbation,
 Blockage ratio, etc.

10
While studying the vortex generated by a 2D bluff body, one will arrive to a
realization that the wake shedding primarily isn’t a 2D phenomenon. This calls for
adopting a parameter that represents the span wise flow similarity, called the
Correlation length (Bearman, 1984) and (Norberg, 2003). This Correlation length
throws light on the span wise variation of quantities such as the fluctuating surface
pressures, Lift force and the fluctuating velocity. Consider a cylinder having a span
wise extension. Now the distance between two points: a and b along the span wise
direction is measured as ‘Z’ If ‘e’ represents the quantity to be measured, then the
Correlation is given by the expression:
𝑅(𝑒, 𝑧) = 𝑒1 𝑒2̅̅̅̅̅̅/𝑒2̅ (2.6)
The Correlation Length is given by the expression:
𝐿 = ∫ 𝑅(𝑒, 𝑧) 𝑑𝑧
∞
0
(2.7)
There is another important phenomenon associated with high Reynolds number flow
over cylinders. It is the Drag crisis. Drag crisis is marked by a sudden drop in the
drag coefficient 𝐶 𝐷.The point of separation, measured in degrees from the stagnation
point, moves forward to 80°
with increasing Reynolds Number from Re = 103
to
105
. Then, unexpectedly, through the transition from laminar to turbulent phase, the
point of separation moves back from 80°
to 140°
and there is a sudden drop of the
coefficient of drag. This zone is called the critical Reynolds number, Re = 105
. This
low drag is captured in the CFD analysis performed later. The point of crisis is
denoted by a dip in the drag value.
2.1.2 Oscillating cylinders:
Oscillating cylinders can be mimicked experimentally by considering two options.
 Rigid cylinders placed on flexible mounts or
 Using flexible structures like riser pipes and cables.
In the flexibly mounted case, the response is uniform along the span wise length
because only at the mounts the cylinder oscillates. In the case of cables and risers,
vibration takes place at several range of modes and there is span wise variation of
hydrodynamic loading. For experimental studies a rigid cylinder placed on flexible
mount is often used.

11
Freely oscillating cylinder inside a fluid medium:
This is the category of vibrating cylinders where there is absence of prescribed or
imposed oscillations and the cylinder is free to respond to the hydrodynamic loading.
There are three frequencies that come into existence on discussing freely oscillating
cylinder (Blevins, 2001). They are:
 The natural frequency of the cylinder, 𝑓𝑛,
 The vortex shedding frequency, 𝑓𝑣 𝑠 and
 The frequency of the lift oscillation, 𝑓𝑳
It is generally agreed that the vortex shedding frequency of the cylinder is equal to
the frequency of the oscillating lift. Which is to say: 𝑓𝐿 = 𝑓𝑣 𝑠 and this condition is
normally away from 𝑓𝑛/ 𝑓𝑣 𝑠 = 1. As the velocity is increased, there will come a point
when the vortex shedding frequency of the cylinder is equivalent to the natural
frequency of the cylinder, 𝑓𝑛 = 𝑓𝑣 𝑠 . When this happens, a phenomenon popularly
known as Lock-In takes place. The amplitude of the transverse oscillation reaches the
maximum during this period. When compared to transverse oscillations, the in-line
oscillation is very small. This lock-in phenomenon does not increase in magnitude
due to the fact that it is limited by the drag component.
From the Equation of motion:
𝑌 𝑚
𝐷
= 𝐶 𝑦 𝑚
𝑠𝑖𝑛𝜙(
1
4𝜋3
)(
1
𝑚∗ 𝜁
)(
𝑈
𝑓𝑛 𝐷
)2
(
𝑓𝑛
𝑓
) (2.8)
𝑓
𝑓𝑛
= [1 − 𝐶 𝑦𝑚 𝑐𝑜𝑠𝜙(1 2⁄ 𝜋3
)(1 𝑚∗
)⁄ (𝑈 𝑓𝑛 𝐷⁄ )2(𝑦 𝑚 𝐷⁄ ) − 1]
1 2⁄
(2.9)
𝑌 𝑚
𝐷
Is the amplitude of the transverse vibration and 𝐶 𝑦 𝑚
is the amplitude of the
transverse fluid force coefficient (Bearman, 2011). For transverse oscillations the
fluid force leads the response by a phase 𝜙, but oscillate with the same frequency.
For there to exist an amplitude response, 𝜙 should be anywhere
between 0°
𝑎𝑛𝑑 180°
.
𝑓 < 𝑓𝑛 when 0°
< 𝜙 < 90°
; 𝑓 > 𝑓𝑛 when 90°
< 𝜙 < 180°

12
Cylinders with prescribed or imposed oscillations:
The cylinder is given imposed oscillations; which also experiences hydrodynamic
forces from the flowing fluid medium. Example: Beating motion given to a cable
immersed in a fluid flow medium. Now the cable or cylinder observes two
frequencies; One being the forcing frequency 𝑓𝑓 and another being the frequency of
vortex shedding 𝑓𝑣𝑠. Here the strouhal number is given by the formula:
𝑆𝑡 =
𝑓𝑣𝑠 𝐷
𝑈∞
(2.10)
Another new term is called the non-dimensional frequency 𝑓∗
=
𝑓𝑓
𝑓𝑣 𝑠
⁄ . Keeping the
reduced velocity and imposed amplitude at a constant value, increasing forced
frequency will thereby lead to a point where the forcing frequency 𝑓𝑓 and the
frequency of shedding 𝑓𝑣𝑠 are similar. This phenomenon is called the Lock-In. One
may also observe that the linear growth of the Strouhal number is no longer valid.
This can be illustrated in the image below:
Figure 2.4: Frequency of oscillation & vortex shedding frequency
From the above illustration, during the lock-in phenomenon, the frequency of
shedding does not follow the Strouhal number definition.
𝑆𝑡 ≠
𝑓𝑣𝑠 𝐷
𝑈∞
(2.11)
From the above illustration, 𝑓𝑣𝑠
0
is the frequency of shedding of the cylinder at rest,
which follows the Strouhal number formulation. At Lock-in
𝑓𝑓
𝑓𝑣𝑠
0⁄ ~ 1 .

13
2.3 Validation for computational fluid dynamics studies:
The review mentioned before this title, is concerned with the effect of hydrodynamic
effects of fluid-structure interaction; a brief description of terms and definitions. The
review material mentioned under the section (2.3) is exclusively meant for selection
of turbulence models and validation of force coefficient results. The turbulence
models and past research of the flow over bluff bodies is specified in paper by (Rawat,
Gupta, & Sarviya, 2013). A review of coefficient of lift values over a wide range of
Reynolds number is compiled by (Norberg, 2003). In this paper, the author addresses
the concept of fluctuating lift for Reynolds number ranging from 47 to 2*10^5. He
also explains the span wise variation of flow properties under the subject titled:
correlation length. In order to understand how the openFOAM solver responds to the
flow around cylinders, unsteady computational simulations were carried out for the
following Reynolds numbers: 30, 200, 3500, 10,000, 40,000, 5,50,000 and 2,00,000.
The results are validated through an experimental plot from the paper by (Stringer,
Zang, & Hillis, 2014). The force coefficient plot is a compilation of experimental
results from several other research papers. The three quantities to validate are:
 𝐶 𝐷𝑚𝑒𝑎𝑛
 𝐶𝐿𝑟𝑚𝑠and
 Strouhal Number
All of the above quantities are computed in the post processing phase by extracting
the pressure force calculated during the simulation.
𝐶 𝐷 =
𝐹 𝐷
0.5𝜌𝑈2 𝐷
(2.12)
𝐶𝐿𝑟𝑚𝑠 =
√
1
𝑛
(𝐹𝐿1
2 +⋯𝐹𝐿 𝑛
2 )
0.5𝜌𝑈2 𝐷
(2.13)
𝑆𝑡 =
𝑓𝐷
𝑈
(2.14)
All the above equations are calculated at definite time intervals, which is Non-
dimensionalized using the Equation below:
𝑡+
=
𝑡𝑈
𝐷
(2.15)

14
The three experimental plots for validating the above quantities are taken from
(Stringer, Zang, & Hillis, 2014) and listed below as the following:
 The experimental values for the 𝐶 𝐷𝑚𝑒𝑎𝑛 plot by Zdravkovich (1990), Massey
(1989) and (1980).
 The experimental values for the 𝐶𝐿𝑟𝑚𝑠 can be obtained using the plot by
Norberg.
 The experimental Strouhal number plot can be extracted from the plot by
Norberg( 2003) and Achenbach (1981).
Two other papers are referred for carrying out simulations at the supercritical range
of Reynolds numbers (Re = 1 ∗ 106
& 2 ∗ 106
). These simulations are based on
unsteady Reynolds-Averaged Navier-Stokes 𝑘−∈ turbulence model. It also reasons
out why the 𝑘−∈ turbulence model is the widely used turbulence model in the
industry. The reviews are comprehensively presented in the paper by (Ong, Utnes,
Holmedal, & Dag Myrhaung, 2009) and (Sangamesh.M.Hosur, D.K.Ramesha, &
Basu, 2014).

15
2.4 Literature on flow around semi-submersible Structures:
This literature review is based on the Vortex Induced Motion of the deep-draft semi-
submersible structure or DDS. The offshore profession is a briskly growing field of
Engineering. Several structures have been designed and developed to serve various
purposes. Most important application is: the drilling for crude oil and extraction.
Offshore structures fall under two crucial categories (Gokce & Keyder, 1991). They
are:
 Movable structures and
 Fixed structures.
The movable structures are known for their ease of portability and cost effectiveness.
Jack-ups, floating ship structures and semi-submersibles fall under this category. The
Jack-ups make up 60% of the floating offshore applications. It can be set-up to a
depth of 100 metres. The floating hull structures have deck platforms and equipment
mounted on manoeuvrable ships. They can work up to a depth of 1500-2000 metres
in relatively calm waters. Before studying semi-submersible offshore structures the
definition of conventional submersibles have to be understood. The submersible rigs
work in shallow waters, and make contact with the ocean floor. It works similar in
principle to the Jack-up structures. The submersible rig consists of two hull platforms,
placed one on top of each other. One of the hull holds the working deck, another hull
is either filled with water or Air. Filled with air during transport and with water during
the application. The semi-submersibles can carry relatively higher loads and work in
harsher environments. It serves many roles like crane-lift, drilling rigs, oil production.
The semi-submersible structure consists of four hull appendages which connect the
working deck with the pontoon structure. The pontoon structure gives buoyancy to
the semi-submersible in deep waters but does not come in contact with the ocean bed.
A deep-draft semi-submersible (DDS) has its columns submerged deep in the water
to provide stability against rough sea currents and waves. In the thesis, a scaled model
of DDS is used for computational fluid dynamics analysis, validated by scaled model
experiments conducted by (Fujarra, Goncalves, Rosetti, jr., & Koop, 2015).

16
Vortex Induced Motion of floating columns:
The Vortex Induced Motion in floating offshore structures such as TLPs, spars and
semi-submersibles are set up as a consequence of vortex shedding behind the
columns. The response motions take place at a region very close to the six degree of
freedom resonance, but predominantly exhibit inline and transverse motion. Vortex
Induced Vibration, in one sense, is different from Vortex Induced Motion. The former
is observed in rigid and flexible cylinders where the aspect ratio (L/D) is large
(Rodolfo T. Gonç alves & Meneghini, 2011). The phenomenon is observed among
flexible offshore risers, steel catenary risers, mooring systems, etc. Whereas, the
Vortex Induced Motion is a phenomenon pertaining to flow around rigid bodies with
low aspect ratio. These are also seen among slender buoys, Mono-column platforms.
In particular, the semi-submersible structure with increased geometry show complex
VIM phenomenon. VIM is a vibrational phenomenon that happens over an increased
period of time. This complex interaction between the flow current and the
submersible throws light on the design consideration for offshore structures. As per
the journal issues, many such full scale geometry cannot be tested and so model test
programmes are initiated to compile data for various designs and their VIM responses
respectively. In this thesis, research has been done to set up a computational fluid
dynamics methodology which can predict VIM behaviour for various design
variations.
The study has treated VIM of offshore structures as a primary problem and VIV of
flexible risers as a secondary problem due to the nature of the vortex shedding
associated with four-column platforms. This complex nature arises due to both
Vortex Induced Vibration and Wave Induced Vibration present within the VIM
phenomenon of the semi-submersible. This is illustrated in the Figure 2.5. VIV of
risers is altogether a separate topic and is not dealt in the Thesis.

17
Figure 2.5: Semi-submersible Structure (Antony, et al., 2015)
In the above image, the foremost column experiences Vortex Induced Vibration and
the other columns experience Wake Induced Vibration due to the column ahead of
them. These interactions come together to produce Vortex Induced Motion of the
entire platform. Hence, it is right to say that mooring systems not only encounter VIM
effects of the semi-submersible but also Vortex Induced Vibration on their own.
2.4.1 A review on experimental semi-submersible model:
The two research papers exceedingly referred for experimental data and literature
review are (Fujarra, Goncalves, Rosetti, jr., & Koop, 2015) and (Goncalves, Fujarra,
Rosetti, Kogishi, & Koop, 2015). Modelling of the semi-submersible and
methodology for CFD simulations are adopted based on the information provided in
these papers. There are several factors which affect the VIM response of the semi-
submersible
 The Geometry of the column structure, whether circular or square shaped,
 The angle of incidence between the free stream current and the
semisubmersible,
 Reduced Velocity or Reynolds number,
 Wake interference (When semi-submersible columns are placed in tandem),
 Corner edges of the square column,
 Surface roughness of the structure and Mooring stiffness.

18
There are other factors too, but the above highlighted ones are pivotal in determining
the nature of the VIM response. There are flow parameters which define the
magnitude of the hydrodynamic forces. One such parameter is the reduced velocity.
It is given by the expression, 𝑉𝑟 =
𝑈
𝑓𝐷
. 𝑈 is the flow velocity, 𝑓 is the frequency of
vibration and 𝐷 is the diameter or the characteristic length of the structure. In the
current case, frequency takes the notation 𝑓0 which is representative of the calm water
natural frequency. Therefore, 𝑉𝑟 =
𝑈
𝑓0 𝐷
. There are two phenomena associated with
Vortex Induced Motion. They are,
 Lock-In and
 Galloping.
Lock-In is observed when the vortex shedding frequency is equal in magnitude to the
natural frequency of the structure, 𝑓𝑛 = 𝑓𝑣 𝑠. Lock-In phenomenon does not increase
with increasing reduced velocity because it limited by drag effects. On the other hand,
Galloping is a low frequency phenomenon where the vortex shedding frequency is
greater than the structural response frequency (Waals, Phadke, & Bultema, 2007).
Galloping is observed due to Lift effects on the floating pontoons.
In the test experiment referred for literature, the model is a scaled version of the
original geometry. The model is scaled down to 1:100 of its original size. The viscous
effects of such a reduced model is addressed later. VIM of the semi-submersible is
predominantly two degree of freedom response, In-line oscillation (Surge) and
Transverse (sway) oscillations. Another motion the ‘Yaw’, is also addressed in the
experimental study recorded in the flow induced motions of multiple column floaters
(Rijken & Leverette, 2009) and (Goncalves, Fujarra, Rosetti, Kogishi, & Koop,
2015). The reduced velocity in terms of frequency was defined earlier. One other way
of describing reduced velocity is in terms of time period. The expression for the time
period reduced velocity is given by, 𝑉𝑟 =
𝑈𝐷
𝑇
where T is the oscillation period of surge
or sway. The designated range of reduced velocities and its corresponding Reynolds
numbers are mentioned later.

19
2.4.2 Model and experimental setup:
The most recent experimental study of offshore structures is exacted to a domain
covering semi-submersibles. This is largely due to the fact that cylindrical structures
are susceptible to VIM (such as TLPs and mono-columns); (Rijken & Leverette,
2009). (Hong, Choi, & Lee, 2008) performed experiments to study the VIM
phenomena of the deep-draft semi-submersible models. A review of this trend is
given in the paper by (Rodolfo T. Goncalves, 2012) which is used for validating CFD
results. In order to mimic the ocean environment and sea currents a towing tank is
set-up, where experiments on the scaled DDS is performed (The Society of Petroleum
Engineers).
Figure 2.6: Towing Tank (Fujarra, Goncalves, Rosetti, jr., & Koop)
Towing tank is basically a basin containing water, few feet wide and several feet long.
The erect side walls of the tank consists of rails which run along the length of the
basin. These rails guide the scaled model to and fro to mimic the ocean environment.
The tow is fitted with actuators, sensors and other devices to measure the
hydrodynamics forces on the semi-submersible. The tow allows manoeuvrability,
thrust for the model to meet the prescribed speed of the experiment, heading angle of
the flow. Measuring devices like the planar motion mechanism and computerized
planar motion carriage help in measuring hydrodynamic forces on the DDS when
they are submerged, offset or staggered. There are two DDS models prescribed for
the study of VIM. They are:
 SCR-model: Rounded square sections and
 CC-model: Circular columns

20
Figure 2.7: Deep-draft semi-submersible models (Goncalves, Fujarra, Rosetti,
Kogishi, & Koop, 2015)
These models are scaled down to 1:100 in conjugation with the geometry of the semi-
submersible presented in experimental study. These models are fitted with a circular
deck at the top. This provision ensures that the DDS experiences equal distribution
of spring stiffness from the mooring system. This is well depicted in the Fig. 2.8. The
mooring system is made up of 4 springs with equivalent spring stiffness along the X-
direction and the Y-direction, 𝑘 𝑥 = 𝑘 𝑦 = 23.9 gf/cm.
Figure 2.8: Equal Spring stiffness
The co-ordinate system is adopted in such a way that the transverse oscillation is
observed along the y-axis and the in-line oscillations are observed along the x-axis.
The yaw motion is observes in the x-y plane. The span wise length of the vertical
columns are observed along the z-axis. The CFD analysis also follows the above co-
ordinate system and axis measurements. Although a review for the CC-model is given
in the literature, the CFD analysis is performed only for the SRC-model. Information
regarding the corner edges of the semi-submersibles can be gathered from (Chen &
Chen, 2015). The dimension of the geometry is given in the Table 2.1.

21
Table 2.1: DDS Dimensions
QUANTITY SRC-model CC-model
SPACING BETWEEN
COLUMNS(S)
0.6096 m 0.6096 m
FACE SIDE LENGTH
OF THE COLUMN(L)
0.1524 m 0.1524 m
HEIGHT OF THE
PONTOON BASE(H)
0.0853 m 0.0853 m
HEIGHT OF THE
COLUMN DRAFT(T)
0.3353 m 0.3353 m
WEIGHT OF THE
STRUCTURE
49.9 kg 45.1 kg
The experimental analysis of the DDS was selected for reduced velocities from 4 to
30, which corresponds to Reynolds number from 7,000 to 80,000. The Reynolds
number is issued in the research paper with interest to complete the benchmark
database for CFD validations. The reduced velocity is calculated using the formula:
𝑉𝑟 = (𝑈. 𝑇0) 𝐷⁄ (2.16)
Where U is the free stream incident velocity, 𝑇0 is the natural period of motion in the
transverse and yaw motion and 𝐷 is called the characteristic length of the semi-
submersible which sees the incoming flow as the true face projection. It is given by
the formula:
𝐷 = 𝐿(|sin ∅| + |cos ∅|) (2.17)
Where L is the dimension of the face of the square column and ∅ is the angle of
incidence of the freestream current.
Figure 2.9: Characteristic Length
The reduced velocities tested for the bare SRC-DDS model at the 45° angle of
incidence is given in the table 2.2.
Table 2.2: Reduced velocity/Reynolds number
Hull Surface ∅ [deg] Reduced velocity (𝑉𝑟) # of Tests
SRC-model 45 4,5,6,7,8,9,10,12,14,16,18,20 12

22
Reynolds number can be calculated using the formula:
𝑅𝑒 =
𝜌𝑈𝐷
𝜇
(2.18)
In the above formula, free stream velocity 𝑈 can be calculated by inserting the known
quantities of 𝑉𝑟, 𝑇0 and 𝐷 into the Eqs. 2.16. The Reynolds number can be calculated
using the known value of free stream velocity from the Eqs. 2.18.
2.4.3 Hydrodynamic forces and experimental validation:
In the experimental analysis of Vortex Induced Motion of semi-submersibles, the
Hilbert-Huand Transform method (HHT) is used to extract peak values of amplitude.
Instead of validating the CFD method using the peak values of amplitude,
hydrodynamic force coefficients: 𝐶𝐿 and 𝐶 𝐷 can be used in conjunction with results
given in the following paper (Rodolfo T. Goncalves, 2012).
The equation of motion due to hydrodynamic force in the in-line and transverse
direction is discussed in (Sarpkaya, 2004):
𝑚𝑋̈(𝑡) + 𝐶𝑋̇ + 𝑘 𝑥 𝑋(𝑡) = 𝐹 𝐻𝑥(𝑡) (2.19)
𝑚𝑌̈(𝑡) + 𝐶𝑌 + 𝑘 𝑥 𝑌(𝑡) = 𝐹 𝐻𝑦(𝑡) (2.20)
Where C is the ratio of the critical damping; 𝑚 is the semi-submersible mass; 𝐹 𝐻𝑥(𝑡)
hydrodynamic fluid force in the in-line direction and 𝐹 𝐻𝑦(𝑡) is the hydrodynamics
fluid force in the transverse direction. Structural force are given on the left side of the
equation and the fluid force is given on the right hand side of the equation. Lift
coefficient is calculated from the equation:
𝐹 𝐻𝑦(𝑡) =
1
2
𝜌𝐴 𝑃 𝑈2
𝐶𝐿 (2.21)
𝐶𝐿(𝑡) =
2𝐹 𝐻𝑦(𝑡)
𝜌𝐴 𝑃 𝑈2
(2.22)
Where 𝜌 is the density of the fluid, 𝐴 𝑃 is the submerged projection Area
corresponding to the angle of the incidence of the flow. Similarly, coefficient of drag
can be calculated. The two crucial plots which will be used to validate the
computational fluid dynamics results is given below and attention has to be paid to

23
choose the correct projection Area of the semi-submersible. An error of 5-7% is
allowable while calculating the hydrodynamic force coefficients owing to the fact
that the dimensions for experimental semi-submersible is a little different from the
scaled model of the deep-draft semi-submersible model. This allowable error
percentage also accounts for the absence of data regarding the corner radius of the
scaled model.
Figure 2.10: Force Coefficient plots (DDS) (Fujarra, Goncalves, Rosetti, jr., &
Koop)
From the plot, after converting reduced velocity to Reynolds number (refer eqn.
2.18), the value of coefficient of drag 𝐶 𝐷 = 0.94-1.15 (For Reynolds number = 60000).
This value of coefficient of drag has to be predicted in order to validate the simulation
for the above Reynolds number.

24
CHAPTER 3: Computational Fluid Dynamics
3.1 CFD methodology:
Computational fluid dynamics is an inexpensive means by which real flows can be
simulated by solving governing equations. These come as desktop applications, some
commercialized and some being freely available to the public as open source
applications. The governing equations together which represent the physics of the
flow are called the Navier-Stokes equation. Since these are reduced order models,
research is being done to accurately mimic the real time flows. Experimental methods
have played a vital role in validating the results produced by the numerical
simulations. Navier-Stokes Equations are represented by a set of partial differential
terms. These differential terms are converted to algebraic equations and later solved
and visualized using computers.
3.1.1 Governing Equations:
The N.S equations is the foundation for modelling the physics of the fluid flow. In
other words, the modelling of the fluid motion within the numerical domain is
accomplished through Navier-Stokes equation. The fluid under steady may contain
information regarding pressure, temperature, viscosity, etc., all of which is
propagated through the entire length of the domain. These equations can also be
modelled to mimic turbulent flows. In the current CFD analysis, the material is
restricted to deal only with incompressible flows and the corresponding N-S
equations are given by:
𝜕𝑢
𝜕𝑥
+
𝜕𝑣
𝜕𝑦
+
𝜕𝑤
𝜕𝑧
= 0 (3.1)
𝜌 (
𝜕𝑢
𝜕𝑡
+ 𝑢
𝜕𝑢
𝜕𝑥
+ 𝑣
𝜕𝑢
𝜕𝑦
+ 𝑤
𝜕𝑢
𝜕𝑧
) = −
𝜕𝑝
𝜕𝑥
+ 𝜇 (
𝜕2 𝑢
𝜕𝑥2 +
𝜕2 𝑢
𝜕𝑦2 +
𝜕2 𝑢
𝜕𝑧2) (3.2)
𝜌 (
𝜕𝑣
𝜕𝑡
+ 𝑢
𝜕𝑣
𝜕𝑥
+ 𝑣
𝜕𝑣
𝜕𝑦
+ 𝑤
𝜕𝑣
𝜕𝑧
) = −
𝜕𝑝
𝜕𝑦
+ 𝜇 (
𝜕2 𝑣
𝜕𝑥2
+
𝜕2 𝑣
𝜕𝑦2
+
𝜕2 𝑣
𝜕𝑧2
) (3.3)
𝜌 (
𝜕𝑤
𝜕𝑡
+ 𝑢
𝜕𝑤
𝜕𝑥
+ 𝑣
𝜕𝑤
𝜕𝑦
+ 𝑤
𝜕𝑤
𝜕𝑧
) = −
𝜕𝑝
𝜕𝑧
+ 𝜇 (
𝜕2 𝑤
𝜕𝑥2
+
𝜕2 𝑤
𝜕𝑦2
+
𝜕2 𝑤
𝜕𝑧2
) (3.4)

25
Let the x-momentum equation alone be represented
Continuity equation: ∇. 𝑢 = 0
Momentum equation:
𝜕𝑢
𝜕𝑡
+ ∇. (𝑢. 𝑢) = −
1
𝜌
∇𝑝̅ + ∇. 𝜐 [2𝑆]
The first term in the momentum equation symbolises the transient nature of the
problem, the second term represents the convective term, the third term is the pressure
and the last term corresponds to the diffusion term of the equation.
In computational studies there are three major types of discretization. They are,
 The finite difference method,
 The finite volume methods and
 The finite element method.
The thesis operates an open source CFD application called the OpenFOAM. This
application is based on Finite volume method. A conservative discretization is
automatically satisfied through direct use of conservation law. Some of the important
highlights of the finite volume methodology are:
 It is the most widely used discretization method,
 No requirement of a structured grid,
 Very general and flexible in approach,
 It uses integral formulation of conservation laws
 It is based on the principle of interpolating cell-centred values.
 The discretization of the flux is also conservative.
This flux is responsible for transportation of the fluid property. The N-S equations
can be represented as transport equations when a source term and a flux term is
invoked.
𝜕(𝜌𝜙)
𝜕𝑡
+ ∇(𝜌𝜙𝑢) − ∇(Γ∇𝜙) = 𝑆 𝜙 (3.5)
The first term represents the rate of change of property 𝜙 with time, the second term
symbolizes the convection of the property 𝜙, and the third term defines the diffusion
of the property 𝜙. The final term on the right hand side of the equation is the source
term.

26
The flux term 𝜙 can be any of the fluid property. It can take up the role of temperature
when 𝜙 = 𝑇. The second term in the eqs. (3.5) becomes ∇(𝜌𝑇𝑢). Here the
temperature T is transported by the velocity component 𝑢. Now when the flux term
take the role of fluid velocity 𝑢, the second term in the eqs. (3.5) is represented
as ∇(𝜌𝑢𝑢). This implies that the velocity is transport by itself.
The integral form of the N-S equation can be explained through control volume cell
blocks.
Figure 3.1: Control volume cells (Haddadi, 2012)
Above figure has two control volume cells, whose one of the centre is at point P and
the neighbouring cell centre is at the point N. The normal vector is 𝑆̅. For an
orthogonal grid, the vector connecting point P and N should be parallel to the normal
surface vector 𝑆̅. Finite Integral over a volume for a cell is formulated as:
∫ ∫
𝜕𝜌𝜙
𝜕𝑡𝑣
𝑡+Δ𝑡
𝑡
𝑑𝑣𝑑𝑡 + ∫ ∫ ∇. (𝜌𝑢𝜙)
𝑣
𝑣
𝑡+Δ𝑡
𝑡
𝑑𝑣𝑑𝑡 = ∫ ∫ ∇. (𝐷∇𝜙)𝑣
𝑡+Δ𝑡
𝑡
𝑑𝑣𝑑𝑡 (3.6)
The volume integral of the divergence term has both spatial integration and spatial
derivation. Gauss Theorem is invoked in the eqs. (3.6). It states that the volume
integral over a divergence of a given value of 𝜙 is equal to the surface integral of the
value.
∫ ∇. 𝜙𝑑𝑣
𝑣
𝑣
= ∫ 𝑑𝑠. 𝜙
𝑠
𝑠
(3.7)
Inserting Eqn. (3.7) in (3.6), we get the divergence term and the diffusion term.

27
Divergence term:
∫ ∇(𝜌𝑢𝜙)𝑑𝑣 = ∫ 𝑑𝑠(𝜌𝑢𝜙) ≈ ∑ 𝑆(𝜌𝑢) 𝑓 𝜙 𝑓 =𝑓𝑠𝑣
∑ 𝐹𝜙 𝑓𝑓 (3.8)
Diffusion term:
∫ ∇(𝐷∇𝜙)𝑑𝑣 = ∫ 𝑑𝑠(𝐷∇𝜙) ≈ ∑ 𝐷𝑓(𝑆. ∇𝜙) 𝑓𝑓𝑠𝑣
(3.9)
Where the integral ∫ is the volume integral and𝑣
∫ denotes the surface integral𝑠
.
The above equations are solved inside the fluid domain consisting of initial conditions
and boundary condition. The discretization in eqs. (3.6) is of the second order. For
good accuracy it is necessary that the order of the discretization is equal or higher.

28
3.1.2: Turbulence Models:
Turbulence is a measure of randomness and chaos. Fluid flows in engineering
applications are often turbulent. Even working within the bounds of laminar flows, it
is impossible to control the turbulence. One such turbulent flow is considered and the
mean velocity measure at a certain time interval is given by:
Figure 3.2: Turbulence fluctuations (Sayma, 2009)
𝑢̅ =
1
Δ𝑡
∫ 𝑢𝑑𝑡
𝑡+Δ𝑡
𝑡
(3.10)
Therefore, velocity 𝑢 = 𝑢̅ + 𝑢′
. Similarly pressure can be defined as 𝑝 = 𝑝̅ + 𝑝′
.
Substituting Eqs. (3.10) into the N-S equation the following formulation is obtained.
𝜕𝑢̅𝑖
𝜕𝑡
+ 𝑢̅𝑗
𝜕𝑢̅𝑖
𝜕𝑥 𝑗
= −
1
𝜌
𝜕𝑝̅
𝜕𝑥 𝑖
+
1
𝜌
𝜕
𝜕𝑥 𝑗
[𝜇
𝜕𝑢̅ 𝑖
𝜕𝑥 𝑗
− 𝜌𝑢𝑖
′ 𝑢𝑗
′̅̅̅̅̅̅] (3.11)
The above equation is called the Reynolds Averaged Navier-stokes equation and the
last term is called the Reynolds stress term. The main objective of the turbulence
modelling is to calculate these Reynolds stresses, which are unspecified in the
momentum equation.
The Reynolds stresses in the Eqn. (3.11) can be likened to shear stresses present in
the momentum equation. When the momentum flow is averaged, they further
introduce more and more unspecified terms. As a result closure problem arises due
to presence of non-linearity in the RANS equation of unknowns. Since large volumes
of data has to be processed to solve the unspecified terms, modelling of Reynolds
stresses become inevitable. Thus the turbulence models arrive into the picture. RANS
models can work on comparatively unstructured, coarse grids and the disturbance

29
fluctuations are not resolved but modelled successfully. If not modelled, these RANS
turbulence models become steady state simulations.
Distinguished examples for RANS models are the 𝑘−∈ turbulence model; this model
is used in the thesis for performing high Reynolds number 2D refined grid
simulations. This is the most commonly used industrial turbulence model. Next in
line is the 𝑘 − 𝜔 − 𝑆𝑆𝑇 turbulence models. This model is adopted for most part of
the simulation present in the CFD analysis of cylinders.
The Detached Eddy Simulation is used for flow around a cylinder, which switched
into sub grid scale formulation where LES calculations can be performed. Also the
wake pattern is resolved clearly. The LES turbulence model is more accurate and
definitive, when compared to the RANS models. This model can be employed to
flows which possess unsteady turbulent fluctuations and the grid has to be resolved
well in order to capture the energy exchange between the Eddies (Energy cascade).
DNS simulation is based on a turbulence model which can be applied to any scale
flows, and it is not modelled correspondingly to meet the requirements. It is by far
the simplest approach to turbulent flow but that which require tremendous
computational effort.
RANS
DES
LES
DNS
Increasing complexity & Grid
resolution

30
3.1.3 Wall Function:
The wall mixing length for high Reynolds number flow is a place where the viscous
effects are felt. The viscous effect, away from the wall is subdivided into 3 layers
 Viscous sublayer,
 Buffer layer and
 Log-law region or Inner layer.
Beyond this is the outer layer and the free stream grid where one can observe free
stream velocity. At high Reynolds number flows, the first viscous sublayer is so thin
that it is very hard to resolve in the grid. To resolve this fine grid, the law of wall was
defined, which states: That the average velocity of the flow at a specific point in the
grid wall is directly proportional to the logarithmic distance from the point to the wall
(Ferziger & Perić, 1999). Because of the law of Wall, the velocity distribution for
almost all the turbulent flows, near the wall, is identically the same. In the simulation,
an important parameter to define the grid resolution is called the non-dimensional
wall distance, 𝒚+
𝑦+
=
𝑦𝑢 𝜏
𝜈
(3.12)
The distance y to the wall is made dimensionless with the friction velocity 𝑢 𝜏
And kinematic viscosity 𝜈 .
𝑢 𝜏 = √
𝜏 𝑤
𝜌
(3.13)
𝜏 𝑤 is the wall shear stress and 𝜌 is the density of the fluid.
𝑢+
=
𝑢
𝑢 𝜏
(3.14)
𝑢+
is the dimensionless Velocity. In that, velocity 𝑢 is parallel to the wall as a
function of 𝑦, divided by the friction velocity 𝑢 𝜏.

31
Figure 3.3: Dimensionless Wall Function (Wikipedia)
For the viscous sub-layer:
𝑦+
< 5; 𝑢+
= 𝑦+
; 𝑦+
is the wall co-ordinate and 𝑢+
is the dimensionless Velocity.
Assigning 𝑦+
= 12 for viscous sublayer, is an error of over 25%.
For Buffer layer:
5 < 𝑦+
< 30; 𝑦+
≠ 𝑢+
;
𝑢+
≠ 1 𝑘⁄ (𝑙𝑛 𝑦+
) + 𝑐 ;
For log-law region:
𝑦+
> 30 𝑡𝑜 60;
Wall Function is an approach of calling a function when the grid cannot be resolved
down to the viscous sub-layer (Kalitzin, Medic, Iaccarin, & Durbin, 2004). A
schematic representation is illustrated in figure 3.4.

32
Figure 3.4: Turbulence Model- Wall function and resolved grid (Skoda)
On the right hand side, the mesh is resolved down to the first cell layer. In the left
hand grid, the mesh is not resolved down to the viscous sublayer and so a wall
function is used to bridge the unresolved grid. High-Re number turbulence model can
be used in the wall Function case. Various turbulence models use wall Function for a
specific value of 𝑦+
. Normally, the 𝑦+
> 30. Turbulence models with different
spatial resolution of the grid would imply different 𝑦+
values for using wall function.
No wall-function must be applied when the 𝑦+
= 1; this is most desirable for near-
wall modelling. In the introduction to OpenFOAM two turbulence models with wall
Function is discussed.

33
3.2 Introduction to OpenFOAM:
OpenFoam is an open source application, available to download over the web. It
works on the Linux operating platform and whose acronym stands for Open Source
Field Operation and Manipulation. Numerical simulations can offer crucial insight
and information that are expensive to obtain due to the commercial nature of the
software. But OpenFoam has transcended the cost aspect, as it is a freely available
CFD tool employed to perform flow simulations. Initially, OpenFoam as a software
had flaws in terms of standard representation of the library due to discontinuity in the
way code was being handled by the researchers, year after year. Finally, due to bulk
investments, the online OpenFOAM forum was established and contains a
compilation of standard base code and other resources dedicated solely for extending
the horizon of the availability of computational resources. OpenFoam also gets
continuous support from repositories like (SourceForge), (GitHub). OpenFoam is
based on finite volume discretization, where the fluid property values are interpolated
at the cell centres and is compiled using C++ object oriented programming language,
mimicking scalar-vector-tensor operations. The OpenFoam CFD toolbox consists of
a wide range of numerical solvers for applications such as aero-acoustics, turbulence
modelling, heat transfer, stress analysis, etc. OpenFoam is an initiative of standard
compilation of base codes and no other individual researcher’s contribution is
accepted into the main documentation (Chen, Xiong, Morris, & Paterson, 2014). The
most important advantage of OpenFoam is the solver manipulation and
customization, where a student or a researcher can manipulate the solver to work for
a certain specific application. The software is not only a standalone application but
can also be used in conjunction with other commercial software. This can be
facilitated by executing a set of OpenFOAM commands. For post-processing and
visualization, tools such as paraview, tecplot, etc., can be used.The Navier-stokes
transport equation can be represented as the following:
𝜕𝜌𝑢
𝜕𝑡
+ ∇𝜙𝑢 − ∇. 𝜇∇𝑢 = −∇𝑝 (3.15)

34
The code in the eqn. 3.15 is represented in OpenFOAM using the C++ object oriented
programing as:
solve
(
fvm :: ddt (rho , U)
+ fvm :: div (phi , U)
- fvm :: laplacian (mu , U)
==
- fvc: grad (p)
);
The fvm stands for finite volume matrix and fvc stands for finite volume calculus. In
the above code, the laplacian operator and the divergence operator are implicitly
solved. Whereas, the gradient operator is solved explicitly using the finite volume
calculus (Weller, Tabor, Jasak, & Fureby, 1998). The most important equation to
compute in CFD is the Navier-Stokes equation. In that, the momentum equation is
expressed as:
𝜕𝑢
𝜕𝑡
+ 𝛻(𝑢. 𝑢) = −
1
𝜌
𝛻𝑝̅ + 𝛻. 𝜈[2𝑠] (3.16)
In the above equation the first term exhibits the transient behaviour, the second term
∇(𝑢. 𝑢) is called the convection term. The third term is called the pressure gradient
term. The forth term is called the diffusion term. It has got a laplacian operator. This
equation in OpenFoam is called the Transport Equation:
𝜕(𝜌𝜑)
𝜌𝑡
+ ∇(𝜌𝜑𝑢) = −∇(Γ∇𝜑) = 𝑆𝜑 (3.17)
𝜑 is called the fluid property which is being transported. First term specifies the rate
of change of property with time. Second term is the convection of the property 𝜑. The
third specifies the diffusion of the property 𝜑. Finally the last term is called the source
term. By setting the diffusion coefficient 𝛤 to zero, the above equation becomes a
pure convection.
𝜕(𝜌𝜑)
𝜌𝑡
= −∇(𝜌𝜑𝑢) (3.18)

35
When the convection term is equal to zero, it is called a pure diffusion term.
𝜕(𝜌𝜑)
𝜌𝑡
= −∇(Γ∇𝜑) (3.19)
When 𝜑 = 𝑢, then the transport equation becomes the following:
𝜕(𝜌𝑢)
𝜌𝑡
+ ∇(𝜌𝑢𝑢) = −∇(Γ∇𝑢) = 𝑆 𝑢 (3.20)
In the above equation, ∇(𝜌𝑢𝑢) is interpreted as velocity being transported by itself.
Let us consider 𝜑 = 𝑇, where 𝑇 is called a transport scalar. This then implies:
𝜕𝑇
𝜌𝑡
+ ∇𝑢𝑇 = 𝐷 𝑇∆𝑇 (3.21)
3.2.1 OpenFOAM case directory:
Each OpenFOAM case is constructed on three directories. They are:
 0 directory,
 constant directory and
 system directory
OpenFOAM simulations are never perceived as 2D simulations because even while
the simulations is of the type 2 dimensional, there is always one cell thickness along
the third direction. The above mentioned directories have sub-directories inside them
and there are several files attached to a single sub directory. An OpenFOAM case file
with its description is as follows:
 0 directory: 0 directory houses information regarding the initial conditions for
the simulation. Each of the file in the directory represents a flow property
assigned to boundary patches before the commencement of the simulation.
Here the T file represents temperature, p file represents pressure, epsilon
represents kinematic energy dissipation, U represents velocity, k represents
kinematic energy.

36
Figure 3.5: OpenFOAM directory
 constant directory: constant directory houses information regarding fluid
properties, physics of the flow, turbulence models contained in the following
files: transportProperties, turbulenceProperties and RASProperties. The
directory also contain a sub directory called /polyMesh which enlists
information regarding the topology and the mesh.
 System directory: system directory comprises of three main directories which
every other openFOAM case set-up has to possess. They are:
1. fvSchemes: This file contains information regarding the discretization
schemes used for the simulation. It contains the divergence scheme,
the laplacian scheme, the gradient scheme, etc,. These schemes are
basically first order accurate or second order accurate.

37
2. fvSolution: It contains details regarding the pressure-velocity coupling
methods (solver identification), preconditioners, residual control,
solver relaxations.
3. controlDict: This files controls the start time and end time of the
simulation. It contains information regarding ∆𝑡 of the simulation,
courant number, time interval for the simulation data and calls a
function which calculates the forceCoefficients. Some of the other
parameters include: startFrom, stopAt, writeInterval, writeFormat,
writePrecision.
An important feature of OpenFOAM is its capability to allow changes while the
simulation is running. This option is executed through runTimeModifiable.
The mesh utility such as blockMesh and snappyHexMesh are executed and the mesh
is constructed. The mesh is made up of a number of objects. These are specified inside
the /polyMesh sub directory. They are
 points: Two points represented by a vector cannot share the exact same
position.
 faces: Faces inside a mesh are constructed using several points across the co-
ordinates. There are internal faces and external faces. The external faces are
made of cells which make up the boundary. Connecting two faces of a cell is
the internal face category.
 boundary: The boundary is a set of patches assigned after the mesh utility is
executed. These patches are assigned to every fluid property given in the /0
directory with its initial condition.
There are several boundary conditions assigned to the patches generated by executing
the mesh utility; either blockMesh or snappyHexMesh. Most commonly used B.Cs
are listed below:
 fixedValue: This is also known as the Dirichlet boundary condition. The flow
variable, at a boundary patch, is assigned a specific value. At the no-slip
boundary wall, fixedValue takes up the value zero.

38
 zeroGradient: This is also called the Neuman boundary condition. This
condition is mostly observed at the wall boundary, where normal gradient of
the flow variable is assigned a value zero.
 slip: Slip boundary condition is applied to patches where the shear stress is
considered zero. This is usually observed among the top & bottom patches.
 empty: This boundary condition is applied to sides of the 2D simulation in
order to indicate that the front and back patches are empty.
 symmetryPlane: At a boundary patch when symmetryPlane is applied, there
is no presence of normal velocity component observed. It is used for a
symmetry plane.
There are two important mesh utilities associated with OpenFOAM. They are:
 blockMesh and
 snappyHexMesh
The parameters of the blockMesh utility is controlled inside the file named
blockMeshDict and the snappyHexMesh utility is controlled inside the parametric file
called snappyHexMeshDict.
blockMesh: This utility reads the topology and mesh properties from the file
blockMeshDict. The blockMeshDict is made up of parameters such as vertices,
blocks, boundary patches. The mesh boundary and the object are made up of co-
ordinates called the vertices. The entire mesh is broken up into several smaller
components called the blocks. The mesh distribution within a block is controlled by a
parameter called simpleGrading. The vertex co-ordinates are either assigned in
millimetres or centimetres or meters. For example:
convertToMeters 0.001
Indicates that the dimension is in millimetres and is converted to meters by
multiplying by a factor of 0.001.

39
snappyHexMesh: Another mesh in openFOAM is the automatically generating hex
mesh utility called the snappyHexMesh. The parameters of this utility is controlled
inside the file named snappyHexMeshDict. Here, the object to be meshed is modelled
inside a CAD interface and is saved as STL file. The utility makes use of blockMesh
to create a background mesh and a volume mesh is built around the STL geometry
inside the fluid domain (Maric, Hopken, & Mooney, 2014). During the mesh
execution the STL object is chiselled out and only the impression of the geometry
remains inside the mesh. The snappyHexMesh utility requires the following:
 An STL file which is created using a CAD interface and saved in the ASCII
format,
 A background mesh created using blockMesh and
 All the mesh parameters are controlled inside the file called the
snappyHexMeshDict.
In order to refine the STL objects’ edge, another file is used as a parameter inside the
mesh utility. This is called the surfaceFeatureExtract. The resolution of the STL
geometry depends on the background mesh. The cell splitting along the geometry is
bad when the backgrounds mesh is coarse.

40
3.2.2 Discretization Schemes and Solver control:
Choosing a proper scheme is vital in controlling the force coefficient values and the
overall convergence of the simulation. Discretization scheme is defined within the
directory system/fvSchemes and the solver control is defined inside
system/fvSolution. The working of the finite volume discretization through the
transport equation is executed by the discretization and interpolation schemes. When
the grid has highly non-orthogonal and skewed cells, it is important to choose good
grad schemes and laplacian schemes to adjust the simulation (Moraes & Lage, 2013).
The schemes are given in detail in the Appendix.
The fvScheme file has the following schemes:
 ddtSchemes;
 gradSchemes;
 divSchemes;
 laplacianSchemes;
 interpolationSchemes;
ddtSchemes are used for the temporal discretization. Some common choices of this
scheme includes:
 CrankNicolson,
 Euler (transiet simulation)
 steadystate (steady state simulation).
gradSchemes are parametric schemes that determine the sharpness of the gradient
interpolation across the grid, which is used in conjunction with the solver.
 Gauss;
 cellLimited;
 cellMDLimited;
 faceMDLimited;
 faceLimited;
divSchemes are used for discretizing convective terms in the finite volume model.
Less diffusive direction

41
For a highly non-orthogonal grid Gauss upwind; and for a good mesh Gauss
linerUpwind default; can be used as the divergence schemes. Solvers and
preconditioning technique will dictate the computational costs and time. The
fvSolution file in the system directory contains these parameters. The finite volume
discretization leads to an algebraic equation of the form Ax = b. These system of
equations are solved by either employing direct or iterative methods. All the matric
equations and the pressure-velocity coupling equations are manipulated inside the file
named fvSolution. The pressure equation demands a lot of computational time and
effort and based on how one wants the simulation to proceed, the pre-conditions are
selected. The geometric-algebraic multi-grid solver, also known as GAMG is often
used as a pre-conditioner to solve the pressure equation. The solver uses only few
number of cells to produce the solution and is later interpolated across the finer mesh.
Because the accurate solution is obtained in the finer mesh. In general, GAMG
commences with a specified mesh and whether the grid is coarsened or refined
depends on the simulation. The preconditioned conjugate (PCG) is used to solve
pressure equations used in conjunction with GAMG as the pre-conditioner to speed-
up the calculation, instead of using DIC as pre-conditioner. The other preconditioners
are Preconditioned Bi-conjugate (PBiCG) solvers. During a transient simulation like
the pimpleFoam, nCorrectors = 1; would mean that the simulation is running in the
piso mode and nCorrectors = 2; would mean that the simulation is running in the
pimple mode. According to the non-orthogonality of the grid, values for the
parameter nNonOrthogonalCorrectors can be assigned. Tolerance and relTol
parameters define the exit criterion for the solver for every iteration. Another
important point to remember is that while the simulation is running on piso mode, the
relaxation factors cannot be altered and has to be assigned the values 1; a detailed
review of fvSchemes and fvSolution is given in the Appendix B.
relaxationFactors
U 1.0;
k 1.0;
omega 1.0;

42
3.2.3 Steps involved in solving transport equation & working of the PISO loop:
The header file 'solver.c' is studied. Here the header files are included. The ones that
are predominantly observed are:
#include "createTime.H"
#include "createMesh.H"
#include "createFields.H"
The createFields.H file is opened. In the file, the code that calls in the transport
properties from the /constant Folder is:
(
transportProperties.lookup("nu")
);
The pressure and velocity is then calculated. The values of which are provided in
the /0 folder. The code responsible for achieving this is:
volScalarField p
(pressure)
(
IOobject
(
"p",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
Info<< "Reading field Un" << endl;
(Velocity)
volVectorField U
(
IOobject
(
"U",

43
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);
The above information creates the flux, by including the following header file:
# include "createPhi.H".
This Phi then enters a time loop inside the icoFoam.C header file. Here the finite
Volume vector matrix is set up to solve for the transport equation.
fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
- fvm::laplacian(nu, U)
);
solve(UEqn == -fvc::grad(p));
In the above code the partial time derivative, the divergence term (convection) and
the laplacian term (diffusion) is solved. The three terms inside the matrix is solved
using the pressure gradient expression on the last line. The function under the
namespace fvm discretizes the divergence and the laplacian operator implicitly. This
operator returns co-efficients for the matrix equation. The fvc:: grad is an explicit
finite volume discretization for the gradient operator. And this returns field variables.
This part of the code can be manipulated using the fvSchemes provided inside the
/system directory. The field variables then enter the two for loops; the inner loop and
the outer loop, prescribed under the PISO loop.

44
for (int corr=0; corr<nCorr; corr++) (Firstloop)
{ (Outerloop)
volScalarField rAU(1.0/UEqn.A());
volVectorField HbyA("HbyA", U);
HbyA = rAU*UEqn.H();
surfaceScalarField phiHbyA
(
"phiHbyA",
(fvc::interpolate(HbyA) & mesh.Sf())
+ fvc::interpolate(rAU)*fvc::ddtCorr(U, phi)
);
adjustPhi(phiHbyA, U, p);
for (int nonOrth=0; nonOrth<=nNonOrthCorr;nonOrth++)(Secondloop)
{ (Innerloop)
fvScalarMatrix pEqn
(
fvm::laplacian(rAU, p) == fvc::div(phiHbyA) (3.22)
);
pEqn.setReference(pRefCell, pRefValue);
pEqn.solve();
if (nonOrth == nNonOrthCorr)
{
phi = phiHbyA - pEqn.flux();
}
}
#include "continuityErrs.H"
U = HbyA - U*fvc::grad(p); (3.23)
U.correctBoundaryConditions();
The number of iterations within a loop depends on the value assigned to nCorrectors
and nNonorthogonalCorrectors inside fvSolution. For example if the nCorrectors = 2,
nNonorthogonalCorrectors = 2; the solution enters the inner loop and solves for
Pressure thrice using the Eqn. (3.22) and updates the value of velocity given in the

45
Eqn. (3.23). As the nOuterCorrectors = 2, the outer loop once again enters for the
second iteration and calculates the value of pressure inside the inner loop with the
recently updated velocity. The loop finally ends with a new value of velocity U.

46
CHAPTER 4: METHODOLOGY
In this chapter, the methodology for setting up OpenFOAM simulations is described
in detail. The objective of the research resounds through the chapter; that is to propose
a standard methodology for performing numerical simulations for capturing Vortex
Induced Vibration of cylindrical structures and Vortex Induced Motion of semi-
submersible offshore structures.
4.1 Procedure for VIV simulation of cylinders:
The aim of the study was to numerically analyse Vortex shedding behind fixed
Cylinders at various Reynolds numbers. Correspondingly, the values of 𝐶𝐿𝑟𝑚𝑠,
𝐶 𝐷𝑚𝑒𝑎𝑛 and Strouhal number are recorded and compared with the experimental
results. The right Refinement of mesh required for the simulation to produce good
results is chronologically mentioned in this chapter. The plots used for experimental
validations are given below:
Figure 4.1: 𝐶 𝐷 plot; Zdravkovich (1990), Massey (1989).

47
Figure 4.2: 𝐶𝐿 plot; Norgberg (2003), Stringer et al. (2014)
Figure 4.3: 𝑆𝑡 vs 𝑅𝑒 plot; (Norberg, 2003), (Achenbach, 1981)

48
4.1.1 Selection of Reynolds number for the Simulation:
This study was intended to cover simulation results over a wide range of Reynolds
numbers. Before selecting the Reynolds number for the simulation, a good
understanding of the various flow regimes is required; a review is done on how a flow
around a cylinder behaves at various Reynolds numbers by (Lienhard, 1966). It is
illustrated below:
Figure 4.4: Flow regimes around a circular cylinder (Lienhard, 1966)
The Reynolds number for the simulation is selected. The simulation is grouped as
per the turbulence model used and also categorized under 2D/3D simulation.
 Reynolds number of 30, 200 and 3,500 are selected for the k-Omega SST
URANS turbulence model under the category of 3D simulations.
 Reynolds number of 10,000 and 40,000 are selected for DES turbulence
model, using a 3D mesh.
 Reynolds numbers 5 ∗ 105
and 2 ∗ 106
are selected for k-Omega SST
turbulence model simulations using a two dimensional mesh.
 Reynolds number of 2 ∗ 106
is selected for 𝑘−∈ turbulence model for
2Dimensional simulation.

49
In the flow over a fixed cylinder the vortex starts to initiate at Re > 40. And so one
simulations is compiled at Re = 30 in order to capture the circulation zones, void of
any completely formed vortices. This phase is also called the steady separation phase.
The next simulation is performed for Re = 300. The following number is where the
laminar flow show signs of turbulence in the vortex street. There is also a jump in the
𝐶𝐿𝑟𝑚𝑠 value. This phase is called the laminar periodic shedding. There are four
simulations carried out at four different subcritical Reynolds numbers, one being Re
= 300, where the 𝐶𝐿𝑟𝑚𝑠 curve observes a dip and then starts to increase gradually.
Another simulation is performed at Re = 3,500 where the 𝐶𝐿𝑟𝑚𝑠 value sees a steady
increase in the curve. The other two subcritical Reynolds number simulations is
carried out at Re = 10,000 and Re = 40,000, where the 𝐶𝐿𝑟𝑚𝑠 value is almost a
constant.
The final two simulations are compiled in the area where Reynolds number is critical
and supercritical respectively. The purpose of the simulation is also to capture the
Drag Crisis where there is a steady drop in 𝐶 𝐷𝑚𝑒𝑎𝑛 value, which can also be
interpreted as the turbulent re-attachment of the flow. There is also a drop in the
𝐶𝐿𝑟𝑚𝑠 value which starts to increase when the Reynolds number attains super-
criticality. All the above simulations are compared with the experimental results put
forward by the research papers mentioned earlier.
4.1.2 Mesh used for simulations:
The entire set of simulations is carried out using 4 meshes, namely:
 2D coarse mesh created using blockMesh,
 2D hover cylinder mesh using snappyHexhMesh,
 3D hover cylinder mesh using snappyHexMesh and
 2D refined Mesh created using blockMesh.

50
2D Coarse mesh: Initially, the 2D coarse mesh had a Cylinder Diameter = 2m and
span wise length = 1m. This was recognized to have a very slow transition to vortex,
due to the large dimensions of the cylinder. This implies reduction in the velocity, to
account for the unchanging Reynolds number. So the Dimensions of the above
Cylinder was scaled down using the command transformPoints –scale. And the
reduced dimensional changes were as follows: Diameter = 0.06m and Span wise
length = 0.03m. The 2D coarse Mesh has a first nodal distance value of 1e-03 (The
distance from the cylinder wall to the centre of the first cell). The domain has a cell
count of 9200.
Figure 4.5: Coarse Mesh
2D & 3D hover cylinder mesh: The 2D hover mesh is created using snappyHexMesh
and then extruded to complete the 2D configuration. The cylinder dimensions are as
follows: D = 0.03155m and Span wise length = 0.05m. The 3D Mesh has an extension
of 0.5m in the span wise direction. The first cell spacing is of the approximate value

51
3.3e-05 with a considerably good wall layer refinement. The total number of cell
count in the domain is around 15,000 for the 2D case and 1175480 cells for the 3D
case respectively (refer Appendix, section A.1)
Figure 4.6: Hover cylinder mesh (snappyhexMesh)
4.1.3 Boundary conditions & Initial flow conditions:
A schematic representation of the Boundary condition is illustrated below.
Figure 4.7: Boundary conditions
At the Inlet of the domain, velocity 𝑈 is specified along with turbulent kinetic energy
𝑘 and turbulent dissipation 𝜔. Pressure is zero gradient at the inlet. At the wall-
cylinder wall the flow properties are zero gradient. At the outlet, the velocity,
turbulent kinetic energy and dissipation are zero gradient. Whereas, the pressure has

52
fixed value. Top and bottom patches always take slip boundary conditions. Front and
back are designated slip boundary condition or empty as per whether the simulation
is 2 dimensional or 3 Dimensional simulation.
Inlet Outlet Top &
Bottom
Cylinder
Velocity
(U)
fixed
Value
zeroGradient slip zeroGradient
Pressure zero
Gradient
fixedValue slip zeroGradient
Turbulent
kinetic
energy (𝑘)
fixed
Value
inletOutlet slip zeroGradient
Specific
dissipation
(𝜔)
fixed
Value
inletOutlet slip zeroGradient
Turbulent
Viscosity
(𝑛𝑢𝑡)
calculated
(0)
calculated (0) calculated
(0)
nutLowRe
WallFunction
Table 4.1 Boundary conditions
4.1.4 Initial Flow conditions:
The initial flow conditions are calculated using the below formula:
Turbulent viscosity 𝑛𝑢=1e − 06;
Velocity 𝑈 =
𝑅𝑒𝐷 ∗ 𝑛𝑢
𝐷
;
Turbulence Intensity 𝐼 = 0.16 ∗ 𝑅𝑒𝐷(−1
8⁄ )
;
Turbulence Length scale 𝐿 = 𝐷; 𝑙 = 0.07𝐿;
Turbulent kinetic Energy 𝑘 =
3
2
∗ (𝑈 ∗ 𝐼)2
;
Turbulence dissipation rate ∈= 0.093 4⁄
∗ 𝑘3 2⁄
/𝑙;

53
4.1.5 Refined mesh for high Reynolds number simulation:
Later in the fluid dynamics simulation of Reynolds number = 5.5 ∗ 106
and 2 ∗ 106
,
it has been found that a coarse mesh in conjunction with 𝑘 − 𝜔 − 𝑆𝑆𝑇 turbulence
model had yielded a coefficient of lift value with an error of over 15%. Instead of
correcting the values, another Reynolds number was chosen between the above two
Reynolds numbers; and a supercritical turbulence simulation was performed. Here a
refined mesh was used in conjunction with the 𝑘−∈ turbulence model. The force
coefficients along with the Strouhal Number was validated for the Reynolds number
= 1 ∗ 106
given in the paper (Ong, Utnes, Holmedal, & Dag Myrhaung, 2009).
Table 4.2: Experimental force coefficient values
Also a mesh convergence study was performed. A refined mesh is created after
changing the parameters inside the blockMeshDict and executing the command:
blockMesh.
Only few years back, obtaining good results at such high Reynolds number meant
publishing a journal paper. Many students struggle to compute good values for
𝐶 𝐷𝑚𝑒𝑎𝑛 and 𝐶𝐿𝑟𝑚𝑠, mostly because the lift value tends to be high and the drag crisis
is not captured properly. Due to time constraints and limited computational resources,
a two dimensional cylinder is used. Although, a 3D validation is required because the
wake vortices are primarily a 3D phenomenon. The kOmegaSST turbulence model is
also employed. Of the two models, kEpsilon turbulence model is computationally
cheap but less accurate; can be used only for a completely turbulent case and is not

54
suited for the capturing transition. On the other hand, kOmegaSST turbulence model
is accurate and robust. But the latter is not easy to control and so the fvSchemes and
the fvSolution have to be selected with good working precision. Initially, a coarse
mesh is adopted for the cylinder vortex vibration. The mesh parameters can be
changed inside the file blockMeshDict. The first cylinder blockMesh was adopted
from the website (WolfDynamics). The website uses the blockMesh utility to analyse
the Vortex Induced vibration of cylinders at high Reynolds flows, but with Air as the
fluid medium. Hence, the coarse nature of the Mesh. Now on the second attempt,
refineMesh command was used on the coarse Mesh and the simulation was run with
kOmegaSST turbulence model. On the third attempt, the Mesh parameters were
altered using the blockMeshDict and a good Mesh was thus created. The description
of the mesh is illustrated in the Figure 4.8.
Figure 4.8: blockMeshDict (Refined Mesh)

55
The complete details of the file is given in the appendix (refer section A.2). The above
parameters are presented for a blockMesh of 𝑦+
= 60 with a cylinder Diameter =
2m. Now another command is used to scale down the blockMesh. Scaling down a
mesh will felicitate the convergence process much faster. The command used was:
transformPoints –scale “(0.015 0.015 0.015)”
In an attempt to run the simulation using kEpsilon turbulence model, incorporating a
standard wall Function, the above blockMeshDict was altered and a mesh of 𝑦+
> 30
was generated. The refined Mesh is illustrated in the Figure 4.9.
Figure 4.9: Refined Mesh
Now after setting up the mesh, initial conditions for pressure, Velocity and the
turbulence properties are set inside the /0 directory of the OpenFOAM case. The
information on the fvSchemes and fvSolution for the high Reynolds number
simulation is given in the Appendix (refer section B.2).

56
4.2 Procedure for VIM simulation of semi-submersibles:
The computational fluid dynamics analysis of flow around cylinders enabled the
study of vortex Induced Vibration. These simulations laid foundation for the later
analysis of Vortex Induced Motion of the DDS structure. The difference between the
two terms, VIV and VIM, is explained in the chapter 2 (section 2.4). The aim of the
semi-submersible simulation is not the validation of all the VIM force coefficients,
like in the case of the cylinders. Although, an attempt is made to authenticate the CFD
results using the force coefficient plots mentioned in chapter 2 (refer Figure 2.9). The
primary objective of the simulation is to put forward a universal methodology to
capture the VIM phenomenon during the CFD analysis. The list of tasks performed
is as follows:
MODEL TESTS
(Experimental analysis)
DESIGN OF DDS MODEL
IN SolidWorks
3D MESH USING
snappyHexMesh
CFD ANALYSIS STATIC
CASE (simpleFoam)
CFD ANALYSIS QUASI-
STATIC CASE (pimpleFoam)
CFD ANALYSIS DYNAMIC
CASE (pimpleDYMFoam)
METHODOLOGY FOR DDS

57
4.2.1 Design of deep-draft semi-submersible:
The deep-draft semi-submersible model (SR-columns), was created using the CAD
program SolidWorks. The dimensions of the DDS are given in the Table 4.3
Table 4.3: Geometry dimensions
QUANTITY VALUE
SPACING BETWEEN COLUMNS 0.6096 m
FACE SIDE LENGTH OF THE COLUMN 0.1524 m
HEIGHT OF THE PONTOON BASE 0.0853 m
HEIGHT OF THE COLUMN 0.3353 m
WEIGHT OF THE STRUCTURE 49.9 kg
The experimental VIM tests were carried out for 3 angles of incidence:
0°
, 22°
and 45°
. Due to shortage of time, only the 45°
angle of incidence is covered
in the CFD validation. The DDS model is drawn to precision and radius of the corner
edges are obtained from the paper on CFD analysis (Antony, et al., 2015). The stagger
angle of the submersible is fixed inside the solidWorks, or can be manipulated in the
OpenFOAM environment using the following commands:
transformPoints –translate
transformPoints –rotate
transformPoints -rollPitchYaw
The information regarding the STL surface file; the orientation, co-ordinate origin
and the span wise extension can be interpreted using a visualization software like the
paraview. Attention has to be paid to make sure that the CAD model is written in the
ASCII code and saved as a surface STL file. During the mesh set-up, the ASCII code
enables the user to extract the patch name into the dictionary file
snappyHexMeshDict. Without the patch name from the STL file, snapping and layer
addition process of the mesh cannot be performed.

CFD Analysis of Flow Induced Vibration of Offshore Structures

CFD Analysis of Flow Induced Vibration of Offshore Structures

Recommended

Recommended

More Related Content

Similar to CFD Analysis of Flow Induced Vibration of Offshore Structures

Similar to CFD Analysis of Flow Induced Vibration of Offshore Structures (20)

CFD Analysis of Flow Induced Vibration of Offshore Structures