Hydrodynamic and structural analysis

Transcription

Inspection Capabilities for Enhanced Ship Safety
D3.3 (WP3): Hydrodynamic and structural analysis
Responsible Partner: RINA
Contributor(s): USG, LR, RINA, AES, DANAOS
Dissemination Level
PU
Public
PP
Restricted to other programme participants (including the Commission Services)
RE
Restricted to a group specified by the consortium (including the Commission Services)
CO
Confidential, only for members of the consortium (including the Commission Services)
x
This document is produced by the INCASS Consortium. The INCASS project is funded by the European
Commission under the Seventh Framework Programme (FP7/2007-2013). Grant Agreement n°605200
D3.3 (WP3) – Hydrodynamic and structural analysis
Document information table
Contract number:
605200
Project acronym:
INCASS
Project Coordinator:
University of Strathclyde Glasgow (USG)
Document Responsible Partner:
RINA Services SPA
Deliverable Type:
Report
Document Title :
Hydrodynamic and structural analysis
Document ID:
D3.3
Contractual Date of Delivery:
31/07/2014
Filename:
D3.3 Hydrodynamic and structural analysis
Status:
Final version
RINA
Version: 3
Actual Date of Delivery:
31/07/2014
Authoring & Approval
Prepared by
Modified
Author
Date
Adnan Kefal
05/06/2014
Adnan Kefal
18/07/2014
All
V1
Erkan Oterkus
28/07/2014
All
V2
Adnan Kefal
29/07/2014
21,25,28
V3
Minor comments
Page/Sections
Version
V0
Comments
Creation
of the
document
Description of the
software
Executive
summary
Approved by
Name
Role
Partner
Date
Document Manager
Erkan Oterkus
WP3 Leader
USG
31/07/2014
Document Approval
Iraklis Lazakis
Project Coordinator
USG
31/07/2014
This document is produced by the INCASS Consortium, funded by the European Commission (FP7/2007-2013).
Grant Agreement n° 605200.
Page 2 of 94
Executive Summary
Current INCASS structural mechanics platform is based on previously EU funded
RISPECT methodology. RISPECT approach used two different commercial software
for performing structural and hydrodynamics analyses. These are MAESTRO software
for structural analysis calculations and FD-Wave Load software for hydrodynamic
analysis. Although commerial software is generally powerful and beneficial, it may not
be practical to use them as part of a more general platform due to connectivity issues.
Hence, as part Task 3.3 of the INCASS project, two in-house finite element and
hydrodynamics analyses software, ADFEM and ADPAN, have been developed by
using the object-oriented Java programming language.
The Java language has several advantages. These are an object-oriented paradigm,
multiplatform support, ease of development, reliability and stability, the ability to use
legacy C or C++ code, good documentation, development-tool availability, etc.
Moreover, Java programs are less susceptible to bugs and security flaws.
The newly developed in-house panel method code, ADPAN, is a frequency-domain
hydrodynamic software which can be used to predict the motions and wave loads of any
vessel. The software first calculates the velocity potentials, source strengths, and flow
velocities at the centroids of the hydrodynamic panels for requested speed, heading, and
frequency. By using this data, the hydrodynamic motions and loads can be computed.
The approach used to calculate the hydrodynamic forces is based on 3D potential theory
with zero speed Green’s function.
The newly developed in-house finite element code, ADFEM, contains a finite element
library including truss, beam, plane, plate, shell and solid element types. By using the
developed tool, it is also possible to combine beam and shell elements or truss and plane
elements (for simple cases) to build the finite element model of a ship. This feature will
result in significant computational efficiency.
Page 3 of 94
Both the hydrodynamics tool and finite element analysis tool are validated extensively
by considering various problem cases. The numerical solutions obtained from in-house
software are compared against analytical solutions and the results generated by using
other available software including ANSYS, AQWA and PRECAL.
Utilization of ADPAN and ADFEM as an integrated tool allows solution of hydroelastic ship model in order to obtain both displacements and relevant stress distribution
of the hull structure. Then, these properties will be calibrated within INCASS platform
in order to calculate future conditions of the hull structure and predict the right
inspection intervals.
Page 4 of 94
Table of Contents
1
INTRODUCTION ............................................................................................... 12
2
PANEL METHOD CODE ................................................................................... 14
2.1
SHIP MOTIONS ........................................................................................... 15
2.2
PANEL METHOD ........................................................................................ 20
2.3
ADPAN SOFTWARE .................................................................................. 25
2.4
APPLICATIONS AND VALIDATION OF ADPAN ............................................. 26
2.4.1 Radiation Problem of a Floating Hemisphere............................................... 27
2.4.2 Diffraction Problem of a Submerged Spheroid ............................................ 30
2.4.3 Rigid Body Motions of a Long Barge .......................................................... 32
2.4.4 Hydrodynamic Analysis of WIGLEY III ..................................................... 34
2.4.5 Hydrodynamics of S175 Type Container Ship ............................................. 39
3
FINITE ELEMENT CODE .................................................................................. 46
3.1
FINITE ELEMENT METHOD ......................................................................... 46
3.2
ELEMENT TYPES ........................................................................................ 48
3.2.1 Truss Element ............................................................................................. 48
3.2.2 Beam Element ............................................................................................. 49
3.2.3 Plane Element ............................................................................................. 49
3.2.4 Shell Element .............................................................................................. 50
3.2.5 Solid Element .............................................................................................. 52
3.3
ADFEM SOFTWARE .................................................................................. 53
Page 5 of 94
3.4
APPLICATIONS AND VALIDATION OF ADFEM ............................................ 56
3.4.1 Truss Problem ............................................................................................. 56
3.4.2 Beam Problem ............................................................................................. 58
3.4.3 Frame Structure Problem ............................................................................. 60
3.4.4 Plane4 Problem ........................................................................................... 64
3.4.5 Plane8 Problem ........................................................................................... 67
3.4.6 Shell3 Element ............................................................................................ 69
3.4.7 Shell4 Element ............................................................................................ 73
3.4.8 Shell8 Element ............................................................................................ 78
3.5
GLOBAL FINITE ELEMENT ANALYSES OF SHIP AND COUPLING OF FINITE
ELEMENTS ............................................................................................................ 83
4
CONCLUSION .................................................................................................... 91
5
REFERENCES .................................................................................................... 92
Page 6 of 94
List of Figures
Figure 1
Hemisphere Mesh ...................................................................................... 28
Figure 2
Hemisphere added mass for (a) surge and (b) heave motion ....................... 29
Figure 3
Hemisphere damping for (a) surge and (b) heave motion ........................... 30
Figure 4
Spheroid geometry and orientation in space ............................................... 31
Figure 5
Spheroid mesh ........................................................................................... 31
Figure 6
(a) Real and (b) imaginary component of excitation force .......................... 32
Figure 7
Barge mesh representation ......................................................................... 32
Figure 8
Barge motion amplitudes ........................................................................... 33
Figure 9
Barge motion phase angles ........................................................................ 34
Figure 10 WIGLEY III sectional view ....................................................................... 35
Figure 11 WIGLEY III mesh ..................................................................................... 35
Figure 12 WIGLEY III pitch added mass .................................................................. 37
Figure 13 WIGLEY III pitch damping ....................................................................... 37
Figure 14 WIGLEY III motion amplitudes ................................................................ 38
Figure 15 WIGLEY III motion phase angles ............................................................. 38
Figure 16 WIGLEY III oscillatory pressure distribution (Unit: Pa) ............................ 39
Figure 17 S175 container ship profile view ............................................................... 40
Figure 18 S175 container ship waterlines .................................................................. 41
Figure 19 S175 container ship body plan ................................................................... 41
Figure 20 S175 container ship isometric mesh view .................................................. 42
Figure 21 S175 container ship added mass ................................................................ 42
Figure 22 S175 container ship damping ..................................................................... 43
Figure 23 S175 container ship motion amplitudes ..................................................... 43
Figure 24 S175 container ship motion phase angles ................................................... 44
Figure 25 S175 container ship pressure distribution ................................................... 44
Figure 26 Space truss isometric view......................................................................... 57
Figure 27 Beam mesh and cross section .................................................................... 58
Page 7 of 94
Figure 28 (a) Translational and (b) rotational displacement results of the beam problem
59
Figure 29 Key point locations and application of boundary conditions on frame
structure .............................................................................................................. 60
Figure 30 Frame structure translational displacements along (a) x- and (b) y- directions
of all nodes .......................................................................................................... 62
Figure 31 Frame structure (a) translational-z and (b) rotational-x displacements of all
nodes 62
Figure 32 Frame structure (a) rotational-y and (b) rotational-z displacements of all
nodes 63
Figure 33 Frame structure total translational displacement contour plot; .................... 63
Figure 34 Frame structure total rotational displacement contour plot; ........................ 64
Figure 35 A square plate mesh and boundary condition representation ...................... 64
Figure 36 Translational displacements along (a) x- and (b) y-directions of all nodes for
the Plane4 problem .............................................................................................. 65
Figure 37 Contour plot of translational displacement along x-direction for the Plane4
problem; (a) ADFEM and (b) ANSYS................................................................. 66
Figure 38 Contour plot of translational displacement along y-direction for the Plane4
Figure 39 A rectangular plate and its applied boundary conditions ............................ 67
the Plane8 problem .............................................................................................. 68
Figure 43 A clamped edge square plate and its discretization .................................... 70
Figure 44 Translational displacements along z-direction of all nodes for the Shell3
problem ............................................................................................................... 70
Figure 45 Rotational displacements along (a) x- and (b) y-directions of all nodes for
the Shell3 problem .............................................................................................. 71
Page 8 of 94
Figure 46 Contour plot of translational displacement along z-direction for the Shell3
Figure 47 Contour plot of rotational displacement along x-direction for the Shell3
problem; .............................................................................................................. 72
Figure 48 Contour plot of rotational displacement along y-direction for Shell3
problem; .............................................................................................................. 72
Figure 49 T beam mesh and its boundary conditions ................................................. 73
Figure 51 (a) Translational-z and (b) rotational-x displacements of all nodes for the
Shell4 problem .................................................................................................... 74
Figure 52 Rotational displacements along (a) y- and (b) z-directions of all nodes for
Figure 53 Contour plot of translational displacement along x direction for the Shell4
Figure 54 Contour plot of translational displacement along y direction for the Shell4
Figure 57 Contour plot of rotational displacement along y-direction for the Shell4
Figure 58 Contour plot of rotational displacement along z-direction for the Shell4
Figure 59 A clamped square plate modelled with Shell8 ............................................ 79
Figure 60 Translational displacements along z-direction of all nodes for the Shell8
problem ............................................................................................................... 79
Figure 61 Rotational displacements along (a) x- and (b) y-directions of all nodes for
Page 9 of 94
Figure 64 Contour plot of rotational displacement along y-direction for the Shell8
problem; .............................................................................................................. 82
Figure 65 Stiffened plate model................................................................................. 84
Figure 66 Stiffened plate boundary conditions ........................................................... 85
the stiffened plate ................................................................................................ 86
Figure 68 (a) Translational-z and (b) rotational-x displacements of all nodes for the
stiffened plate ...................................................................................................... 86
Figure 69 Rotational displacements along y- and z- directions of all nodes for the
stiffened plate ...................................................................................................... 87
Figure 70 Contour plot of translational displacement along x-direction for the stiffened
plate; (a) ADFEM and (b) ANSYS ...................................................................... 87
Figure 71 Contour plot of translational displacement along y-direction for the stiffened
Figure 72 Contour plot of translational displacement along z-direction for the stiffened
Figure 73 Contour plot of rotational displacement along x-direction for the stiffened
Figure 74 Contour plot of rotational displacement along y-direction for the stiffened
Figure 75 Contour plot of rotational displacement along z-direction for stiffened plate;
(a) ADFEM and (b) ANSYS ............................................................................... 90
Page 10 of 94
List of Tables
Table 1
WIGLEY III hull properties ...................................................................... 36
Table 2
S175 container ship properties ................................................................... 40
Table 3
Finite element library of ADFEM .............................................................. 55
Table 4
Displacement results of space truss problem .............................................. 57
Table 5
Strain and stress results of space truss problem .......................................... 58
Table 6
Key points of frame structure .................................................................... 61
Page 11 of 94
1 INTRODUCTION
RISPECT uses pre-calculated hydrodynamic and structural analyses of the intact ship. These
are not adequate for the rapid emergency decision response required for a damaged ship
structure. A new efficient hydrodynamic and structural analysis system needs to be merged to
existing RISPECT system. This process is done within INCASS Task 3.3 by replacing the
two commercially available computational tools used within the RISPECT system
(MAESTRO software for structural analysis calculations and FD-Wave Load software for
hydrodynamic analysis), with in-house finite element and panel-method codes.
An in-house finite element code, called ADFEM, together with a panel-method code, called
ADPAN, are implemented by using Java computer programming language based on objectoriented methodology. The Java language is selected for its numerous advantages: an objectoriented paradigm, multiplatform support, ease of development, reliability and stability, the
ability to use legacy C or C++ code, good documentation, development-tool availability, etc.
The Java runtime environment always checks subscript legitimacy to ensure that each
subscript is equal to or greater than zero and less than the number of elements in the array.
Even this simple feature is very important for developers. As a result, Java programs are less
susceptible to bugs and security flaws.
The panel method code, ADPAN, provides the user with an integrated frequency-domain
computational tool to predict the motions and wave loads of any vessel. To compute these
hydrodynamic motions and loads, ADPAN first calculates the velocity potentials, source
strengths, and flow velocities at the centroids of the hydrodynamic panels for each speed,
heading, and frequency requested. The computation of these hydrodynamic forces is based on
3D potential theory using the zero speed Green’s function.
The finite element code, ADFEM, offers the user a finite element library that includes
formulation of truss, beam, plane, plate, shell and solid element types. Combination of beam
and shell elements or truss and plane elements (for simple cases) can be used to build the
Page 12 of 94
finite element model of a ship. By applying the required boundary conditions, the solution of
hydro-elastic ship model can be performed in finite element code in order to obtain both
displacements and relevant stress distribution of the hull structure. Then, these properties will
be calibrated in INCASS software in order to calculate future conditions of the hull structure
and predict the right inspection intervals.
Page 13 of 94
2 PANEL METHOD CODE
The design of marine structures such as ships, offshore and coastal structures is intensively
affected by wave-body dynamics; therefore hydrodynamic analysis of rigid bodies that are
freely oscillating under the free water surface turns out to be extremely important for today’s
naval architects and marine engineers. The fundamental principle of setting up a complete
linear hydrodynamic analysis can be described by stating two different types of hydrodynamic
problems. First kind of these problems is the interaction of regular surface waves with a rigid
body which is called “diffraction problem.” Second kind of these problems is the fluid motion
resulting from the forced harmonic oscillation of the body in still water which is called
“radiation problem.” Although these problems physically seem very distinctive, they are
mathematically very similar. In fact, they can be treated simultaneously by a solution
procedure or computer program. Essentially, all formulated boundary value problems are of
combined type and therefore, the radiation-diffraction problem can be solved by the same
theoretical numerical schemes.
It is not easy to apply pure numerical approaches like finite differences methods, finite
element method etc. to solve radiation-diffraction problem since the boundary regions of the
wave-body domain needs to be modelled. However, the boundary element method, which is
often called as panel method, could be more suitable for the solution of integral equations
presented in below in terms of flexibility, efficiency and computational time. The presented
formulations deal with three dimensional bodies of arbitrary shape being freely oscillating in
water of infinite depth. It is assumed that the body moves at zero forward speed and is excited
by regular surface waves. The problem is formulated as boundary value problem of potential
theory with mixed boundary conditions such as free water surface region condition. The
numerical solution procedure involves a discretization of the body surface by plane triangular
or quadrilateral elements as they better fit the given body surface. An efficient calculation of
the relevant influence matrices and the solution of a set of linear algebraic equations are
described by standard algorithms. Sample problems are solved and the results of these
Page 14 of 94
problems are compared with those of other investigators, commercial software and analytical
results.
2.1
Ship Motions
The hydrodynamic forces acting on a ship in waves are solved using potential flow theory.
The present approach is similar to that is used by many other investigators including Beck and
Loken (1989), and Papanikolaou and Schellin (1992). In order to be able to compute all
responses of any vessel to regular waves, it is necessary to deal with six degrees of freedom
motion considering important couplings among them. It is desirable first to define an axis
system in order to calculate motions of ship at zero forward speed. The equation of motion is
solved with respect to the ship centre of gravity, although the defined coordinate system has
its origin in the still water plane aligned vertically with the ship centre of gravity. Global
coordinate system is fixed with respect to the earth having the origin at any desired point.
However it is better to choose the mid-ship as an origin of the system because one can easily
utilize the symmetry plane (x-z plane) of the ship. Moreover, x-y plane is coincident with
calm water level and z direction is positive upwards.
Deep water conditions are assumed for a ship moving with constant forward speed, U 0 , at
any angle,  , to regular sinusoidal waves of small amplitude. The frequency of the oscillation
will be shifted to the frequency of the wave encounter as stated in Equation (1) with
k0  2 /  , where k0 is the wave number and  is the wave length.
e  0  k0 U0 cos 
(1)
Ship’s frequency of encounter is higher than the absolute frequency for waves coming from
ahead where direction of wave is   180deg . In stern seas (   0deg ) the frequency of the
encounter is lower and may be equal to zero when the ship speed is equal to the phase
velocity of the waves. When direction of the wave propagation is   90deg , it is defined as
beam sea condition and waves come from starboard side of the ship. In case of ship has zero
forward speed, the frequency of the wave encounter equals to the regular waves of the
frequency. The ship is assumed to oscillate as a rigid body in six degree of freedom and the
Page 15 of 94
resulting oscillatory motions of the ship are assumed to be linear and harmonic. The harmonic
and complex responses of the vessel is  j (t ) where j  1, 2,3, 4,5, 6 refer to surge, sway,
heave, roll, pitch and yaw, respectively. These responses will be proportional to the amplitude
of the exciting forces and at the same frequency but with a phase shift. Consequently, the ship
motions will have the form given in Equation (2).
 j (t)   j cos(et   j )  Re  j ei t 
e
(2)
The general formula of the basic linearized equations (Euler’s equation of motion) in six
degrees of freedom is given in Equations (3) to (5).  jk are the components of the generalized
inertia matrix including all possible couplings for the ship in which z c and xc are the vertical
and longitudinal centre of gravity,  and I represents the mass and moment of inertia terms.
k (t ) are the accelerations in mode k and Fj (t ) represents the total forces or moments acting
on the body in direction j .
6

k 1
k (t )  Fj (t ) , j  1, 2...6
(3)
 j (t)  e2 j ei t
(4)
jk
e
 

 0
 0
 jk  
 0
 zc

 0
0

0
zc
0
xc
0
0

0
xc
0
0
zc
0
I 44
0
 I 46
zc
0
xc
0
I 55
0
0 

xc 
0 

I 46 
0 

I 66 
(5)
The total forces and moments for each direction of motion can be written in terms of
gravitational ( F jG ) and fluid force ( FjH ) acting on the ship. The hydrostatic ( FjHS ) and
hydrodynamic ( FjHD ) forces acting on the ship are obtained by integrating the fluid pressure
over the underwater portion of the hull. Therefore, the actual components of the fluid force
are hydrostatic and hydrodynamic forces. The gravitational forces are simply due to the
weight of the vessel applied to the centre of gravity. Since the mean gravitational force cancel
Page 16 of 94
the mean buoyant forces, they are usually combined with the hydrostatic part of the fluid
force to calculate the extended hydrostatic force ( FjEH ). As a result, Equations (6) to (9) can
be written in order to define the relationship between the described forces.
Fj  FjG  FjH
(6)
FjH  FjHS  FjHD
(7)
FjEH  FjG  FjHS
(8)
Fj  FjEH  FjHD
(9)
To determine the hydrostatic forces, we must integrate the static pressure over the underwater
hull surface. The details of the integral evaluation can be found in Newman (1977). Although
this integration seems straightforward, it is a tedious process. Therefore, it is much easier to
directly define the extended hydrostatic force for each direction. The Equations (11) to (15)
can be used to calculate the extended hydrostatic force where  is density, g is gravity,
B( x) is the full breadth of the water-plane at x,  is the total mass of the ship, GM T is the
transverse metacentric height, GM L is the longitudinal metacentric height, LCF is the
longitudinal centre of flotation.
FjEH  C jkk eiet
0

0
0
C jk  
0
0

0
0 0
0
0
0 0
0
0
0 C33 0 C35
0 0 C44 0
0 C35 0 C55
0 0
0
0
(10)
0

0
0

0
0

0 
(11)
C33   g  B( x)dx
(12)
L
C35    g  xB( x)dx
(13)
L
Page 17 of 94
C44  g GM T
C55  g GM L   g LCF
(14)
2
 B( x)dx
(15)
L
The hydrodynamic pressure at a point in the fluid can be written by Bernoulli’s equation for
unsteady flow where  is time-dependent velocity potential. Assuming the zero forward
speed condition and neglecting second and higher order term derivations of time-dependent
velocity potential, the oscillatory pressure acting on the ship hull is given in Equation (16).
The hydrodynamic force can then be evaluated by integration of defined oscillatory pressure
as stated in Equation (17). The components of the generalized unit normal for each motion
mode are expressed by Equations (18) and (19) in which nx , ny , nz are the directional cosines
for the unit normal pointing outward from the hull and z g is the height of the ship centre of
gravity above the waterline.
P  
FjHD    
S

t
(16)

n j ds
t
(17)
n1  nx , n2  ny , n3  nz
(18)
n4  ynz  ( z  zg )ny , n5  ( z  zg )nx  xnz , n6  xny  ynx
(19)
To accomplish calculating the hydrodynamic force acting on the ship hull, the total timedependent velocity potential for fluid flow needs to be calculated. The time-dependent total
velocity potential can be subdivided into a simple summation of the steady and unsteady
components. The steady part results from the steady forward speed of the vessel. Hence, it is
the combination of the free stream velocity and the steady perturbation potential of the ship
hull. The unsteady part of the time-dependent total velocity potential can be subdivided into
incident wave, the diffracted wave, and the radiation potentials due to the motion in each
degree of freedom. Note that incident wave, diffracted wave, and radiated wave potentials are
all independent of time and depend only on space variables, when the solution of these
potentials are done in frequency domain.
Page 18 of 94
The steady part of the velocity potential is omitted for hydrodynamic force calculation since it
has been assumed that ship is travelling at zero forward speed. Therefore, the hydrodynamic
force can be now described in terms of time-independent unsteady velocity potential
components as represented in Equations (20) to (23).
FjHD  FjI  FjD  FjR
(20)


FjI      ieI n j ds  eiet
S


(21)


FjD      ieD n j ds  eiet
S


(22)
6 
6

FjR       iek n j ds k eiet   (e 2 Ajk  ie B jk )k eiet
k 1 
k 1
S

(23)
Symbols of I , D , k denotes incident, diffracted, and radiated (for each motion mode k)
wave potentials whereas F jI , FjD , F jR symbolizes the incident, diffracted and radiated wave
forces, respectively. Radiated wave force can be written in terms of added mass ( A jk ) and
damping ( B jk ) coefficients. Added mass and damping coefficients can be mathematically
expressed as given in Equations (24) and (25), respectively.

Im(k )n j ds
e S
(24)
B jk    Re(k )n j ds
(25)
Ajk 
S
The incident wave force and diffracted wave force are the forces that excite the motion of the
vessel. Therefore, these forces are generally summed and called exciting forces ( FjEX ). The
expressions for all different forces can now be substituted back into equation (3) in order to
obtain a compact form of oscillatory rigid body motion equation as formulated in equation
(28) where  jk is the mass matrix, A jk is added mass matrix, B jk is the damping matrix,
Page 19 of 94
C jk is the hydrostatic restoring force coefficient matrix,  k is the unknown (complex)
vessel’s amplitudes, and FjEX is the total exciting force, for subscripts of j, k  1, 2,3, 4,5,6 .
FjEX  FjI  FjD
(26)
e2  jkk eiet  Fj  FjEH  FjEX  FjR
(27)
  
2
e
2.2
jk

 Ajk   ie B jk  C jk k   FjEX 
(28)
Panel Method
The equation of the oscillatory motion can only be solved if radiation and diffraction velocity
potentials are known. Therefore, these potentials need to be determined by solving a wellknown radiation and diffraction problem of a body with zero translational velocity performing
small steady oscillations in the presence of a free surface. The mathematical formulation is
explicitly given by Wehausen and Laitone (1960) and results will simply be stated in this
report with no attempt to derive the formulation.
The fluid field in the half-space z < 0 is assumed to be homogeneous, inviscid, and
incompressible and the fluid motion is irrotational. Thus the velocity is equal to the negative
gradient of a scalar potential function, ( x, y, z, t ) , which is a function of time t as well as the
position formulated by Wehausen and Laitone (1960) as given in Equations (29) to (32). In
these equations,
r
is distance between source and field points in three dimensional space, f
is the wave number for zero forward speed assumption, J 0 is the first kind Bessel’s function,
and R is the horizontal distance between source and field point.
R  ( x  a)2  ( y  b)2
(29)
r  R 2  ( z  c) 2
(30)
Page 20 of 94
e2 02
f 

 k0
g
g
(31)

1

k  f k (z c )
( x, y, z, t )    PV 
e
J 0 (kR)dk  cos et  2 fe f ( z c ) J 0 ( fR)sin et
k f
0
r

(32)
It is assumed that the fluid motion is harmonic with a single frequency
e . Thus the time-
dependent potentials ( x, y, z, t ) can be written as in equation (33) where the potential
 (x, y, z) is independent of time and corresponds to the steady potential. It should be noted
that the potential  that must be calculated for radiation, diffraction and incident waves. The
steady potential  satisfies the boundary conditions described by equations from (34) to (38)
for z < 0:
( x, y, z, t )  Re{ (x, y, z) eiet }
(33)
2  0
(34)

 ( x, y,0)

0
 ie  U 0   ( x, y,0)  g
x 
z

(35)
lim     0
(36)

 d  2  


lim  R  i

   0
R 


 dR g  

(37)
2
z 
n   

 f ( S ) on S
n
(38)
The physical significance of the above equations is as follows. Equation (34) is the partial
differential equation for 
and expresses the conditions of incompressibility and
irrotationality. Equations (35), (36) and (37) are the auxiliary conditions on  . Equation (35)
is the linearized free-surface condition, which requires that the pressure on the free-surface be
constant. Equation (36) expresses the vanishing of the disturbance at infinite depth, and
Equation (37) is the radiation condition that requires the disturbance to be an outgoing wave
at infinite horizontal distance. Equation (38) is the boundary condition on S. It expresses the
Page 21 of 94
fact that the normal fluid velocity on S must be specified as a function f(S) of position on the
surface. Often the fluid normal velocity is specified as equal to the normal velocity of the
surface S. However, in the case of a known incident wave,  denotes the disturbance
potential due to the body, and the boundary condition expresses the fact that the normal
velocity of the disturbance must cancel that of the incident wave on the body surface.
The method of solving the mathematical problem defined by equations (33) to (38), is based
on elementary solution or point source solution. The point source potential is defined as the
one that simultaneously satisfies the auxiliary conditions and the homogeneous partial
differential equation throughout space except at one point, where it is singular. The location
of the field point where the point source potential is singular is the location of the point
source. Expressions for the point source potential are given by Noblesse (1982) and Newman
(1985). A source distribution method (panel method or boundary element method) is used to
solve the radiation and diffraction potentials. The radiated or diffracted velocity potential at a
location in the fluid domain is expressed as follows:
  x, y, z  
1
G( x, y, z; a, b,c) (a, b,c) dS
4 S
(39)
where a, b, c is the source location on the surface of the ship, and  (a, b, c) is the strength of
the source at a, b, c . G( x, y, z; a, b, c) is the Green function, as given in Equation (40),
describing the flow at x, y, z caused by a source of unit strength at a, b, c ,

1
k  f k (z c )
G  x, y, z; a, b, c    PV 
e
J 0 (kR)dk  i 2 fe f ( z c ) J 0 ( fR)
r
k f
0
(40)
The Green function satisfies the continuity condition and all boundary conditions with the
exception of the normal velocity boundary condition on the hull surface given in equation
(41), where vn ( x, y, z ) is the flow normal velocity on the hull surface. The source strengths
are solved such that the equation (42) is satisfied and the hull boundary condition for radiation
potential is given by equation (43) while the hull boundary condition for the wave diffraction
problem is stated by equation (44).
Page 22 of 94
  x, y, z 
 vn ( x, y, z )
n
(41)
1
1 G( x, y, z; a, b,c)
  (a, b,c) 
 (a, b,c) dS  v n ( x, y, z)
2
4 S
n
(42)
k  x, y, z 
 ie nk
n
(43)
D  x, y, z 
  x, y, z 
 I
n
n
(44)
Solution of the three-dimensional radiation and diffraction potentials for zero forward speed is
discussed in detail by Hogben and Standing (1974), Faltinsen and Michelsen (1974), and
Garrison (1978). The ship hull should be discretized into flat panels, and the source strength is
taken as being constant over each panel. The normal velocity boundary condition should be
satisfied at the centroid of each panel. Panel source strengths for each radiation mode and for
wave diffraction needs to be solved by evaluation of the Green function and its derivatives
over each panel. Once the source strengths are solved, the potentials on the hull surface can be
calculated. When solving the radiation and diffraction potentials, evaluation of the Green
function is the most time consuming computational task. Telste and Noblesse (1986) and
Newman (1985) have developed efficient methods that are commonly used for evaluating the
Green function. Using an opposite sign convention with respect to the one provided by Telste
and Noblesse (1986), the composition of
their Green function with Newman (1985)
formulation of the Green function can be written as Equation (45) to (47).
1 1
G  x, y, z; a, b, c     2 fR0 (h, v)  i 2 fev J 0 (h)
r r1
(45)
2
2
h  fR , v  f ( z  c) , r1  R  ( z  c)
(46)
R0 (h, v) 

2


v
ev E0 (h)  Y0 (h)  
0
et v dt
(47)
h2  t 2
where r1 is the distance between the image of source point with respect to the free surface
and field point, h is non-dimensional horizontal distance between source and field points, v
Page 23 of 94
is the non-dimensional vertical distance between source and field points, R0 (h, v) is the
frequency dependent term that can be expressed by using Weber function, E0 (h) and second
kind Bessel’s function, Y0 (h) . The derivatives of the Green function can then be evaluated as
represented in Equations (48) to (52).
G( x, y, z; a, b, c) 
G G
G
G

nx 
ny 
nz
n x
y
z
(48)
G
( x  a) ( x  a)
( x  a)
( x  a) v


2f 2
R1 (h, v)  i 2 f 2
 e J1 (h)
3
3
x
r
r1
R
R
(49)
G
(y b) (y b)
(y b)
(y b) v
  3  3 2f 2
R1 (h, v)  i 2 f 2
 e J1 (h)
y
r
r1
R
R
(50)
G
(z c) (z c)
1
  3  3  2 f  2 f 2 R0 (h, v)  i 2 f 2 ev J 0 (h)
z
r
r1
r1
(51)
R1 (h, v) 

2


v
ev E1 (h)  Y1 (h)  h 
0
et v dt
h
2
t
(52)
3
2 2

where J1 (h) is the second order of first kind Bessel’s function, R1 (h, v) is the derivative of
frequency dependent term with respect to non-dimensional horizontal distance that can be
expressed by using second order of Weber function, E1 (h) and second order of second kind
Bessel’s function, Y1 (h) .
Garrison (1978) gives a detailed discussion on evaluation of influence matrix terms to
determine velocity potentials using panel sources. If a field point is in close proximity to a
source panel, then the variation of the Green function term 1/r over the source panel must be
considered. The variation of the term 1/r1 over the image source panel can also be significant
if the field point is close to the image source; however, this situation is less common.
Fortunately, the frequency dependent term of Green function can usually be considered
constant with location over the source panel. Garrison gives a comprehensive overview on the
application of panel methods to offshore structures in waves and provides useful guidelines
Page 24 of 94
for panelling of a body for computation of wave induced forces. For instance, there should be
sufficient number of panels to adequately model the geometry of the body. Adjacent panels
should have similar size, so that the source potential from a larger panel does not improperly
influence the adjacent smaller panels. Panel geometries should not be too elongated, with the
upper limit on the aspect ratio being approximately 5. In practice, the geometry of a ship hull
can often be adequately described with 200 panels on each side of the hull. The mesh size
should be based on the properties for the highest encounter frequency. Normally, the length of
the panels should be chosen such that one obtains about 5 panels per wave length for the
highest encounter frequency.
Hess and Smith (1964) is one of the earliest and most influential works on the application of
panel methods, since they describe the evaluation of panel normals and centroids. For a
triangular panel, the normal components are evaluated by taking the cross product of two of
its edges and then applying a normalization factor. The centroid coordinates are merely the
average of the coordinates of vertices. For a quadrilateral panel, the normal components are
evaluated by taking the cross product of the two diagonals, thus yielding the rotational
orientation of the panel plane. The location of the panel plane is fixed by specifying that it
passes through the mean of the four vertex coordinates. Vertex coordinates are then adjusted
to lie on the computed panel plane.
2.3
ADPAN Software
Based on the zero forward speed assumption and potential flow theory, a panel method
software, called ADPAN, has been generated in order to solve the hydrodynamic forces
acting on a ship in waves. The discretised body is one of the most important inputs for the
software. This discretization should be done by using either flat quadrilateral panels or flat
triangular panels. Once the nodes and corresponding panels are generated and written to an
input file, ADPAN reads these nodes and panels in order to calculate the panel properties.
Then, the radiation and diffraction source strengths of each panel are determined by using the
panel properties.
Page 25 of 94
ADPAN has been implemented by using JAVA language based on object-oriented
programming methodology. Five different Java packages are built and twenty six different
classes have been implemented in these Java packages. An external package called Jama has
been used to solve the linear matrix equation systems. This package involves LU
decomposition and it solves the linear equation system by using the LU decomposition
method. The remaining packages are called adpan, model, util, influence and
oscillatorymotion respectively. The “adpan” package controls the orientation of the other
packages during the compilation and run processes. The “model” package is a general storage
for the input file variables. The “util” package is an auxiliary package that mainly contains
file reading and file writing classes.
The most important packages are essentially “influence” and “oscillatorymotion”,since they
are implemented to solve Green function and equation of oscillatory motion in six degree of
freedom, respectively. In addition to the solution of equation of motion, “oscillatorymotion”
package is used to calculate the hydrodynamic panel pressures for each panel. The equation of
motion is solved with respect to the ship centre of gravity. However, the coordinate system in
ADPAN has its origin in the still water plane aligned vertically with the ship centre of gravity
because this selection makes the solution of the three-dimensional velocity potentials for a
ship hull easier. It is assumed that the ship hull has lateral symmetry thus radiation potentials
are evaluated only on the port side of the hull, while diffraction potentials are evaluated on
both sides of the hull.
2.4
Applications and Validation of ADPAN
To verify implementation of the three-dimensional panel method, sample computations have
been performed for several different problems by using ADPAN. First of all, a radiation
problem of a floating hemisphere is considered because it is very important to calculate
correct added mass and damping coefficients. Secondly, a diffraction problem has been
solved over a submerged spheroid in order to find out the corresponding real and imaginary
part of the excitation force in surge direction. Both the floating hemisphere and submerged
Page 26 of 94
spheroid problems can be solved analytically and the solutions are given by Hulme (1982)
and Wu and Eatock Taylor (1987), respectively. In addition to the analytical results, the
results generated by using AQWA, a commercial hydrodynamic software based on potential
flow theory, are used for validation purposes. For both problems, the numerical results
obtained by using ADPAN are in very good agreement with those found by using AQWA and
the analytical results. Once the results are validated for typical radiation and diffraction
problems, a simple long barge problem is solved in order to check the accuracy of the
implemented equation of rigid body motion. An analytical solution is not so simple for this
case, therefore an external tool, PRECAL developed by Lloyd’s Register, is used for
comparison purposes. Moreover, the hydrodynamic problems of more complicated
geometries such as WIGLEY III and S175 container ship are considered in both ADPAN and
PRECAL in order to demonstrate the capability of ADPAN. The problem descriptions,
results, and discussion of all these problems are given below.
2.4.1 Radiation Problem of a Floating Hemisphere
The radiation problem of a hemisphere with radius r = 1 m floating at zero forward speed in
head sea condition β = 180 degrees is considered to illustrate the capability of ADPAN in
obtaining the convergent values of the added mass and damping coefficient. The wave height
is H = 1 m and therefore the wave amplitude is a = 0.5 m. The vertical centre of the gravity of
hemisphere is selected at free surface z c = 0 and the longitudinal centre of gravity is located at
geometric centre of the hemisphere xc = 0.
Page 27 of 94
Figure 1
Hemisphere Mesh
Full model of hemisphere is discretised by flat quadrilateral panels as shown in Figure 1. The
total number of panels is 768 for full model, however ADPAN uses just half of it for solution
process. The radiation problem of floating hemisphere is solved for 28 different wave
frequencies by using ADPAN and AQWA. The convergence of the computed added mass and
damping results in surge and heave direction obtained from ADPAN, AQWA and the
analytical results given by Hulme (1982) are shown in Figures 2 and 3, respectively. The
variation of the ADPAN results for surge added mass A11 are in good agreement with other
solutions while ADPAN and other solutions of heave added mass A33 are almost identical for
each frequency as presented in Figure 2.
Page 28 of 94
1.4
1.9
1.2
1.7
1
1.5
0.8
1.3
0.6
1.1
0.4
0.9
0.2
0.7
0
2
4
6
8
10
0
2
4
6
8
ADPAN - A11
ADPAN - A33
ANALYTICAL - A11
ANALYTICAL - A33
AQWA - A11
AQWA - A33
AQWA_LID - A11
AQWA_LID - A33
(a)
Figure 2
10
(b)
Hemisphere added mass for (a) surge and (b) heave motion
The numerical results of surge damping B11 and heave damping B33 are plotted together with
the other solutions as shown in Figure 3. It can be seen from these figures that ADPAN
provides very good results when low frequency range is considered, however there are some
slight differences in high frequency range. However, this doesn’t mean that results obtained
from ADPAN are incorrect, since the results of AQWA and ADPAN are similar. This
difference is related to the irregular frequency phenomenon due to the resonant frequencies at
which a fictitious fluid motion inside the body breaks down.
Page 29 of 94
3.5
1.8
3
1.6
1.4
2.5
1.2
2
1
1.5
0.8
0.6
1
0.4
0.5
0.2
0
0
0
2
4
6
8
10
0
2
4
6
8
ADPAN - B11
ADPAN - B33
ANALYTICAL - B11
ANALYTICAL - B33
AQWA - B11
AQWA - B33
AQWA_LID - B11
AQWA _LID - B33
(a)
Figure 3
10
(b)
Hemisphere damping for (a) surge and (b) heave motion
The definite improvement in reducing the irregular frequency behaviour is noticeable, if lid
panels are added to the discretised domain. As it can be seen from Figure 3 that when the
problem is solved by adding lid panels as in AQWA, the results are very promising in
comparison to the analytical results. This observation is similar to the one obtained from a
different type of the B-spline panel method proposed by Maniar (1995).
2.4.2 Diffraction Problem of a Submerged Spheroid
ADPAN is also verified for the diffraction problem of a submerged spheroid in head seas.
The solution of this problem illustrates the accuracy of ADPAN for obtaining the reliable
values of the excitation force. The submerged spheroid used by Wu and Eatock Taylor (1987)
is chosen for comparison purposes. The radius and length of the submerged spheroid is 1 m
and 6 m, respectively. The submergence depth of the spheroid, which is the vertical distance
between the global coordinate system and mass centre of the spheroid, is 2 m. Figure 4 shows
Page 30 of 94
the general geometrical aspect ratio and orientation of the spheroid according to global
coordinate system.
Figure 4
Spheroid geometry and orientation in space
The spheroid is assumed to move at zero forward speed with the unit wave height, 1 m.
Hence, the wave amplitude is 0.5 m. The vertical centre of the gravity is at zc = -2 m and the
longitudinal centre of gravity is at xc = 0 according to global coordinate system. Although the
full model is discretised by 1176 different flat quadrilateral panels as shown in Figure 5,
ADPAN uses xz-plane symmetry condition to solve the diffraction problem.
Figure 5
Spheroid mesh
The variation of the diffraction potential over the spheroid body surface is calculated for 18
different wave frequencies. Figure 6 represents the computed real and imaginary parts of the
wave exciting forces in surge direction, respectively. The numerical results are in excellent
agreement with the analytical solutions obtained by Wu and Eatock Taylor (1987).
Page 31 of 94
0
-0.5
5
0.4
0.9
1.4
1.9
2.4
0
0.4
-1
0.9
1.4
1.9
2.4
-5
-1.5
-10
-2
-2.5
-15
-3
-20
Analytic Real Excitation
Analytic Imaginary Excitation
ADPAN Real Excitation
ADPAN Imaginary Excitation
(a)
Figure 6
(b)
(a) Real and (b) imaginary component of excitation force
2.4.3 Rigid Body Motions of a Long Barge
The accuracy of the implemented equations related to the rigid body motion are confirmed by
solving a long barge problem in head seas condition with β = 180 degrees. Length, breadth,
and draft of the barge is L = 100 m, B = 20 m, and T = 5 m, respectively.
Figure 7
Barge mesh representation
Page 32 of 94
Although the geometry presented in Figure 7 seems quite simple, generating an analytical
solution for this problem is very tedious and complex. Both ADPAN and PRECAL are used
to solve the barge problem for comparison purposes. The barge is assumed to move at zero
forward speed U = 0 m/s condition with the unit wave height H = 1 m. Hence, the wave
amplitude is a = 0.5 m. The vertical centre of the gravity is chosen as zc = -1 m, while the
longitudinal centre of gravity is set at xc = 0 according to the global coordinate system. The
full model is discretised by 1080 flat quadrilateral panels as shown in Figure 7; however
ADPAN uses 504 of them when xz-plane symmetry condition is taken account during the
solution process.
1.60
1.40
1.20
1.00
0.80
0.60
0.40
0.20
0.00
0.20
0.40
0.60
0.80
1.00
1.20
1.40
1.60
1.80
PRECAL - SURGE AMPLITUDE
ADPAN - SURGE AMPLITUDE
PRECAL - HEAVE AMPLITUDE
ADPAN - HEAVE AMPLITUDE
PRECAL - PITCH AMPLITUDE
ADPAN - PITCH AMPLITUDE
Figure 8
2.00
Barge motion amplitudes
First, the radiation - diffraction problem is solved over the body surface for 30 different wave
frequencies. Added mass and damping matrices are obtained from the solution of the radiation
problem, while excitation force vector is calculated by solving the diffraction problem. Then,
the corresponding hydrodynamic coefficient matrix together with the mass and inertia matrix
of the body are defined by using the surface panels. Once the required parameters are derived
Page 33 of 94
for the solution of the rigid body motion equation, motion amplitudes and phase angles are
determined for the directions of six degree of freedom.
200.00
150.00
100.00
50.00
0.00
0.20
-50.00
0.40
0.60
0.80
1.00
1.20
1.40
1.60
1.80
2.00
-100.00
-150.00
-200.00
PRECAL - SURGE PHASE
ADPAN - SURGE PHASE
PRECAL - HEAVE PHASE
ADPAN - HEAVE PHASE
PRECAL - PITCH PHASE
ADPAN - PITCH PHASE
Figure 9
Barge motion phase angles
The numerical results generated by using ADPAN and PRECAL are plotted in Figures 8 and
9. Since the barge is assumed to move in head sea condition, the numerical motion amplitudes
generated by both software in sway, roll and yaw directions can be negligibly small. In fact,
these result are theoretically zero. Therefore, there is no need to present these results.
According to the Figures 8 and 9, the variation of the motion amplitudes and phase angles in
surge, heave and pitch directions obtained from ADPAN are in excellent agreement with
those generated by using PRECAL.
2.4.4 Hydrodynamic Analysis of WIGLEY III
The body surfaces that are used to present the results so far are not as complex as a ship hull
surface. In addition to the simplicity of the body surface, these results are used to validate
subclasses of the whole software in a compact mode. Therefore, the accuracy of ADPAN in
Page 34 of 94
compact mode needs to be tested by solving hydrodynamics of a more complex surface which
looks more like a ship type. Such a validation of ADPAN can be done by solving the
hydrodynamics of WIGLEY III. The frame/cross section lines of the hull are shown in Figure
10.
Figure 10 WIGLEY III sectional view
WIGLEY III hull floating at zero forward speed U = 0 m/s in head sea condition, β = 180
degrees, properties are given in Table 1. The wave height is H = 2 m and therefore the wave
amplitude is a = 1 m. The vertical centre of the gravity of hull is located at z c = -1.250 m
while the longitudinal centre of gravity is set at xc = 0.
Figure 11 WIGLEY III mesh
Page 35 of 94
In addition to ADPAN, PRECAL is used to model the problem for comparison purposes.
Figure 11 shows the hull surface represented by flat quadrilateral panels and the orientation of
the hull with respect global coordinate system. Total number of panels is 2000 for full model
but ADPAN uses just half of the model to solve the hydrodynamic responses.
Table 1
WIGLEY III hull properties
Property
Value
Unit
LOA
100
m
LBP
100
m
B
20
m
T
6.25
m
VOL
2843.8
m3
AWP
691.32
m2
LCF
0
m
GML
125.42
m
GMT
0.333
m
KX
4.087
m
KY
25
m
KZ
25.332
m
KXZ
0
m
The radiation and diffraction problem of floating WIGLEY III hull is solved for 51 different
wave frequencies. Six degree of freedom motion amplitudes and phase angles are calculated
by using the parameters generated from radiation and diffraction problem. The numerical
results generated by using ADPAN are compared with those calculated by using PRECAL.
The variation of the heave added mass A33, pitch added mass A55, heave damping B33, and
pitch damping B55, with respect to wave frequencies are plotted in Figures 12 and 13,
respectively. The numerical results of ADPAN are in good agreement with those obtained
from PRECAL. Since the hull is assumed to move in head sea condition, the numerical
motion amplitudes generated by both software in sway, roll and yaw directions are
theoretically zero. Therefore, there is no need to present these results.
Page 36 of 94
6000
5500
5000
4500
4000
3500
3000
2500
2000
1500
1000
0.00
1600000
1400000
1200000
1000000
800000
600000
0.50
ADPAN - A33
1.00
1.50
400000
0.00
PRECAL - A33
0.50
ADPAN - A55
1.00
1.50
PRECAL - A55
Figure 12 WIGLEY III pitch added mass
The surge, heave and pitch motion amplitudes and motion phase angles for corresponding
wave frequencies are shown in Figure 14 and 15, respectively. The numerical results of
ADPAN match very well with those obtained from PRECAL.
900000
800000
2000
700000
600000
1500
500000
400000
1000
300000
200000
500
100000
0
0
0
0.5
ADPAN - B33
1
1.5
PRECAL - B33
0
0.5
ADPAN - B55
1
1.5
PRECAL - B55
Figure 13 WIGLEY III pitch damping
Page 37 of 94
2.000
1.500
1.000
0.500
0.000
0.00
0.20
0.40
0.60
0.80
1.00
1.20
1.40
Figure 14 WIGLEY III motion amplitudes
200.0
150.0
100.0
50.0
0.0
0.00
-50.0
0.20
0.40
0.60
0.80
1.00
1.20
1.40
-100.0
-150.0
-200.0
ADPAN - SURGE PHASE
ADPAN - HEAVE PHASE
ADPAN - PITCH PHASE
Figure 15 WIGLEY III motion phase angles
Page 38 of 94
Figure 16 WIGLEY III oscillatory pressure distribution (Unit: Pa)
Once the ship motions are determined, the variation of panel pressures for each frequency is
calculated. In order to demonstrate the dynamic pressure variation, each panel pressure for the
frequency of 0.32 rad/sec are exported from ADPAN. The resultant dynamic pressure
variation is plotted in Figure 16. Since the geometry of WIGLEY hull has two symmetry
planes and oscillatory waves are in head sea direction, the expected variation of dynamic
pressure is symmetric with respect to longitudinal centre of gravity which aligns with the
solution presented in Figure 16.
2.4.5 Hydrodynamics of S175 Type Container Ship
A final validation case is conducted by solving the hydrodynamic response of S175 container
ship. ADPAN results are compared with those obtained from PRECAL. S175 container ship
hull properties are given in Table 2. The profile view, waterlines, body plan, and isometric
view of hull surface represented by flat triangular and quadrilateral panels can be seen at
Figures 17 to 20, respectively. As it can be seen from the presented figures, the geometry of
Page 39 of 94
S175 container ship is more complex in comparison to the geometries used in previous
problems.
Table 2
S175 container ship properties
Property
Value
Unit
LOA
178
m
LBP
175
m
B
50.8
m
T
9.5
m
VOL
24067
m3
AWP
3155.9
m2
LCF
-7.048
m
GML
205.29
m
GMT
1.022
m
KX
9.167
m
KY
43.75
m
KZ
43.752
m
KXZ
0
m
A finer mesh and some triangular panels are needed to be used to overcome such a
complexity of the body surface during pre-processing stage. As a consequence, total number
of panels used for the full model is 2946 from which 2930 of them are quadrilateral panels
and the remaining 16 are triangular panels.
Figure 17 S175 container ship profile view
Page 40 of 94
ADPAN takes the advantage of the lateral symmetry condition and generates the results by
using 1473 panels. It is assumed that ship floats at zero forward speed in head sea condition.
The wave height is H = 2 m and therefore the wave amplitude is a = 1 m. The vertical centre
of the gravity is located at zc = 0 and the longitudinal centre of gravity is set at xc = -2.556.
Figure 18 S175 container ship waterlines
The radiation and diffraction problem of floating S175 container ship is solved for 37
different wave frequencies. Six degree of freedom motion amplitudes and phase angles are
calculated by using the parameters generated from radiation and diffraction problem.
Figure 19 S175 container ship body plan
The numerical results generated by using ADPAN are compared with those calculated by
using PRECAL. The variation of the heave added mass A33, pitch added mass A55, heave
damping B33, and pitch damping B55, with respect to wave frequencies are plotted in Figure
Page 41 of 94
21 and 22, respectively. The numerical results from ADPAN are in well agreement with those
obtained from PRECAL.
Figure 20 S175 container ship isometric mesh view
Since the hull is assumed to move in head sea condition, the numerical motion amplitudes
generated by both software in sway, roll and yaw direction are zero. Therefore there is no
need to present these results.
55000
50000
45000
40000
35000
30000
25000
20000
15000
60000000
55000000
50000000
45000000
40000000
35000000
30000000
25000000
20000000
15000000
0.3
0.8
ADPAN - A33
0.3
1.3
PRECAL - A33
0.8
ADPAN - A55
1.3
PRECAL - A55
Figure 21 S175 container ship added mass
The surge, heave and pitch motion amplitudes and motion phase angles for corresponding
wave frequencies are shown in Figures 22 and 23, respectively. According to the plotted
Page 42 of 94
motion results, the numerical results of ADPAN are in very good agreement when they are
compared with those obtained from PRECAL.
17000
20000000
15000
13000
15000000
11000
10000000
9000
7000
5000000
5000
3000
0
0.3
0.8
ADPAN - B33
1.3
0.3
PRECAL - B33
0.8
ADPAN - B55
1.3
PRECAL - B55
Figure 22 S175 container ship damping
1.2
1
0.8
0.6
0.4
0.2
0
0.3
0.5
0.7
0.9
1.1
1.3
1.5
Figure 23 S175 container ship motion amplitudes
Page 43 of 94
200
150
100
50
0
0.3
0.5
0.7
0.9
1.1
1.3
1.5
-50
-100
-150
-200
ADPAN - SURGE PHASE
ADPAN - HEAVE PHASE
ADPAN - PITCH PHASE
Figure 24 S175 container ship motion phase angles
Figure 25 S175 container ship pressure distribution
Page 44 of 94
In order to show the dynamic pressure variation, each panel pressure for the frequency of 0.4
rad/sec are exported from ADPAN. The resultant dynamic pressure variation is plotted in
Figure 25. Since the geometry of S175 has only one symmetry plane and oscillatory waves
are in head sea direction, the expected variation of dynamic pressure should be symmetric
with respect to xz-plane but should be non-symmetric with respect to yz-plane which aligns
with the solution presented in Figure 25.
Page 45 of 94
3 FINITE ELEMENT CODE
Designing ships too strong makes them heavy, slow and very costly to build and operate since
their cargo space is decreased. On the other hand, structural failures, hull damage, weather
conditions can easily cause a big injury or in extreme cases a catastrophic failure and sinking
of ships which are designed weak. Therefore, the structural strength of ships is a key topic
that affects the safety of crew, economic costs, and the pollution of the environment in which
ships are trading. The required structural management and safety of ship can be achieved by
performing appropriate inspections at the right intervals and repairing defects that are
identified. Structural management tools of INCASS project can achieve better prediction of
the right interval of ship inspections, if an in-house finite element code exists.
3.1
Finite Element Method
The finite element method (FEM) is a computational technique for solving problems that are
described by partial differential equations or can be formulated as functional minimization. A
domain of interest is represented as an assembly of finite elements. Interpolation functions in
finite elements are determined in terms of nodal values of a physical field that is sought. A
continuous physical problem is transformed into a discretized finite element problem with
unknown nodal values. For a linear problem, a system of linear algebraic equations should be
assembled and solved. Values within finite elements can be recovered by interpolating nodal
values. Piece-wise approximation of physical fields (a finer mesh of domain) on finite
elements provides good precision even with simple interpolation (shape) functions. An
arbitrary precision of results can be achieved by increasing the number of elements and nodes.
Theory, practice, and programming of the finite element method are described in many
textbooks, such has comprehensive books of Bathe (2006), Fish and Belytschko (2007),
Logan (2011), and Oñate (2013).
Page 46 of 94
Finite element procedure can be described by several steps. The first step is the discretization
of the domain by dividing a solution region (domain) into finite elements that are connected at
nodes. The finite element mesh is typically generated by a pre-processor program because of
the large amount of data. The description of a mesh consists of several arrays, the main of
which are nodal coordinates and element connectivity. Secondly, the logical determination of
interpolation functions is required for the finite element procedure. Interpolation functions are
used to interpolate the field variables over the element. Usually, polynomials are selected as
interpolation functions. The degree of the polynomial depends on the number of nodes
belonging to the element. Interpolation functions are commonly called shape functions since
they are also used for the definition of the element shape.
The third step is the computation of the element matrices and vectors. The matrix equation for
the finite element is established that relates the nodal values of the unknown function to
known parameters. For this task different approaches can be used. The most convenients are:
the variational approach and the Galerkin method. The fourth step is the assembly process of
the element equations. To find the global equation system for the whole solution region, one
must assemble all the element equations. In other words, local element equations must be
combined properly for all elements used for discretization. Element connectivity matrix is
used for the assembly process. Before starting the solution process, boundary conditions
(which are not accounted for in the element equations) should be imposed.
Solving the global equation system is the fifth step. The finite element global equation system
is typically sparse, symmetric and positive-definite. Direct and iterative methods can be used
for solution. The nodal values of the sought function are produced as a result of the solution.
The sixth and the last step is the computation of the additional results such as strains, stresses
etc. In many cases, we need to calculate additional parameters. For example, in mechanical
problems, strains and stresses are of interest in addition to displacements, which are obtained
after solution of the global equation system. It is important to mention that the displacements,
which represent the primary result function, are continuous, however its derivatives (strains
and stresses) have discontinuities at element boundaries. Therefore, the most reliable results
of the finite element method is the displacements. The stress and strain distribution might be
Page 47 of 94
slightly different depending on the assumption of the stress interpolation used to calculate
these values for the same problem, even though the displacement results are completely same.
3.2
Element Types
A finite element is the basic building block of finite element analysis. There are several basic
types of elements. Type of the finite element that is used to conduct a finite elements analysis
depends on the type of object that is to be modelled and the type of analysis that is going to be
performed. An element is a mathematical relation that defines how the degrees of freedom of
a node relate to the next. These elements can be in the form of lines (trusses or beams), areas
(2-D or 3-D plates and membranes) or volumes (brick or tetrahedral). It also relates how the
deflections create stresses. The following content will describe element types in more detail
which could possibly be used to perform a finite element analysis of an arbitrary problem.
3.2.1 Truss Element
Truss elements are two node members which allow arbitrary orientation in a rectangular
Cartesian coordinate system. In fact, the truss transmits only axial force and truss element has
three degree of freedom (three global translation components) at each node. Trusses are used
to model structures such as towers, bridges and buildings. The three-dimensional truss
element is assumed to have a constant cross-sectional area and can be used in linear elastic
analysis. Linear elastic material behaviour is defined only by the modulus of elasticity. Truss
elements cannot be subjected to a boundary condition that includes a rotational degree of
freedom, since they don’t have any rotational degrees of freedom. In order to model a
problem, truss elements can be used when the length of the element is much greater than the
width or depth (approximately 8-10 times). A truss is connected to the rest of the model with
hinges that do not transfer moments. The external applied forces can be only at joints. When
using truss elements, the axial cross-sectional area of the truss elements must be specified.
Page 48 of 94
3.2.2 Beam Element
A beam element is a slender structural member that offers resistance to forces and bending
under applied loads. A beam element differs from a truss element because a beam resists
moments (twisting and bending) at the connections. The classical beam theories based on
Bernoulli-Euler and Timoshenko beam kinematics can be used to formulate beam elements.
These two node elements are formulated in three-dimensional space and the nodes are
specified by the element geometry, for example nodes located at end of the element. A
maximum of three translational degrees of freedom and three rotational degrees-of-freedom
can be defined for beam elements. Three orthogonal forces (one axial and two shear) and
three orthogonal moments (one torsion and two bending) are calculated at each end of the
element. Optionally, the maximum normal stresses produced by combined axial and bending
loads are calculated. Uniform inertia loads in three directions, fixed-end forces, and
intermediate loads are the basic element based loadings. Beam element is used to model
structures when the length of the element is much greater than the width or depth. The
element has constant cross-sectional properties along its axial direction and the element must
be able to transfer moments. The element must also be able to handle a load distributed across
its length. Beam elements can be used for finite-element analysis of elastic spatial frame
structures.
3.2.3 Plane Element
Plane elements can be used for two dimensional modelling of solid structures. Plane elements
can have either triangular, rectangular or quadrilateral shapes. In fact, the development of a
quadrilateral element is very much the same as the rectangular element, except for an
additional procedure for coordinate mapping. The elements are connected at common nodes
and/or along common edges to form continuous structures. A quadrilateral element can be
defined by four nodes or eight nodes whereas a triangular shape plane element can be defined
by using either three nodes or six nodes. All of these nodes have two degrees of freedom at
each node: translations in the nodal x and y directions in plane element local coordinate
system. The formulation of these elements can differ depending on the problem state. In solid
Page 49 of 94
mechanics, plane elasticity can be referred as the set of mathematical models which describe
the behaviour of a body using only displacements on a plane. Two types of plane elasticity
needs to described, namely plane stress and plane strain. Plane stress is defined to be a state of
stress in which the normal stress and the shear stresses perpendicular to the plane are assumed
to be zero. Plane strain is defined to be a state of strain in which the strain normal to the x-y
plane and the shear strains except the shear strain in x-y plane are assumed to be zero.
Nodal displacement compatibility is enforced during the formulation of the nodal equilibrium
equations for two-dimensional elements. If proper displacement functions are chosen,
compatibility along common edges is also obtained. The two-dimensional element is
extremely important for (1) plane stress analysis, which includes problems such as plates with
holes, fillets, or other changes in geometry that are loaded in their plane resulting in local
stress concentrations and (2) plane strain analysis, which includes problems such as a long
underground box culvert subjected to a uniform load acting constantly over its length, pipes
subjected to loads that remain constant over their lengths.
3.2.4 Shell Element
Before discovering a shell type of element, a plate type of element need to be described since
a plate element is a simplified case of a shell element. Physically, a plate can be considered as
a two-dimensional extension of a beam in simple bending because both beams and plates
support loads transverse or perpendicular to their plane and through bending action. However,
a beam has a single bending moment resistance, while a plate resists bending about two axes
and has a twisting moment. Plate structures are geometrically similar to the structure of the
solid plane element for plane stress problem because both plane and plate structures are flat
(if a plate were curved, it would become a shell). As for the solid plane element, a plate
element can also be triangular, rectangular or quadrilateral in shape. Therefore, a plate
element can have different number of nodes depending on the shape as discussed in solid
plane elements description. In general, each node has three degrees of freedom, a translation
out of plane direction with two rotations in plane direction. The out-of-plane rotational degree
of freedom is not considered for plate elements.
Page 50 of 94
These elements are used to model and analyse objects such as pressure vessels, or structures
such as automobile body parts. To illustrate a plate example, consider the horizontal boards
on a bookshelf that support the books. Those boards can be approximated as a plate structure,
and the transverse loads are the weight of the books. The plate structure can be schematically
represented by its middle plane laying on the x–y plane. The deformation caused by the
transverse loading on a plate is represented by the deflection and rotation of the normals of
the middle plane of the plate, and they will be independent of z and a function of only x and y.
It is assumed that the element has a uniform thickness. If the plate structure has a varying
thickness, the structure can be divided into small elements, each of uniform thickness, to
approximate the overall variation in thickness.
There are a number of theories that govern the deformation of plates. In particular, Kirchhoff
plate theory that works for thin plates and Reissner–Mindlin plate theory that works for
thin/thick plates are well known. While many of the assumptions of Kirchhoff plate theory are
analogous to the classical beam theory or Euler–Bernoulli beam theory, Reissner-Mindlin’s
assumptions are analogous to the Timoshenko beam theory. Many structures may not be
considered as a “thin plate,” or rather their transverse shear strains cannot be ignored.
Chapelle and Bathe (2011) propose that Reissner–Mindlin plate theory is more suitable in
general, and the elements developed based on the Reissner–Mindlin plate theory are more
practical and useful.
Shell elements can be in the form of four or eight node quadrilaterals and three or six node
triangular elements in any three dimensional orientation. The four node elements require a
much finer mesh than the eight node elements to give convergent displacements and stresses
in models involving out-of-plane bending. A shell can be seen, in essence, as the extension of
a plate to a non-planar surface. The non-planarity introduces axial (membrane) forces in
addition to flexural (bending and shear) forces, thus providing a higher overall structural
strength. Shell-type structures are common in many engineering constructions such as roofs,
domes, bridges, containment walls, water and oil tanks and silos, as well as in airplane and
spacecraft fuselages, ship hulls, automobile bodies, mechanical parts, etc. The way in which a
shell supports external loads by the combined action of axial and flexural effects is similar to
that of arches and frame structures. Thus, while a beam and a plate typically resist the external
Page 51 of 94
forces by flexural effects only, frames, arches and shells offer a higher resistance to load due
to the coupled action of axial and flexural forces.
Shells are typically classified by the shape of their middle surface. The governing equations
of a curved shell (equilibrium and kinematic equations, etc.) are quite complex due to the
curvature of the middle surface. A way of overcoming this problem is considering the shell as
formed by a number of flat shells. Oñate (2013) states that a shell formulation doesn’t need to
be considered as curved shell, if a good number of flat shell elements are used to model the
structure. The flexural and in-plane states are typically decoupled at the element level when
the shell element is flat. This decoupling extends to the element stiffness matrix which is
formed by a simple superposition of the flexural and membrane contributions.
The full flexural-membrane coupling appears when flat elements meeting at different angles
are assembled in the global stiffness matrix. The superposition leads each nodes of a shell
element has five degrees of freedom: two translational in-plane deformations from in plane
(membrane) element and one translational out of plane deformation with two rotational
deformations from plate element. However, having five degrees of freedom might not be
practical enough to capture a logical deformed shape when a complex structure is tried to be
modelled in rectangular Cartesian coordinate system.
As a result, a rotational degree of freedom in out of plane direction, drilling rotation, needs to
be added to the general flat shell element formulation. Adding this drilling rotation not only
increases the robustness of the element, but also provides such a logical transformation
scheme when the superposition of the elements is done in global coordinates. As a
consequence, a general flat shell element has six degrees of freedom: three translations and
three rotations in x, y, z directions.
3.2.5 Solid Element
Solid elements are three-dimensional finite elements and can be used to model the structure
without any a priori geometric simplification. They are suitable for the stress analysis of
Page 52 of 94
general three-dimensional bodies that require more precise analysis than is possible through
two-dimensional analysis. Examples of three-dimensional problems are arch dams, thickwalled pressure vessels, and solid forging parts as used, for instance, in the heavy equipment
and automotive industries.
Finite element models of this type of element have the advantage of directness. Geometric,
constitutive and loading assumptions required to effect dimensionality reduction, for example
to planar or axisymmetric behaviour, are avoided. Boundary conditions on both forces and
displacements can be more realistically treated. However, utilization of solid elements is
costly. In terms of modelling, mesh preparation, computing and post processing effort. The
rapid increase in computer time as the mesh is refined should be noted. In fact, use of solid
elements should be restricted to problem and analysis stages, such as verification, where the
generality and flexibility of full three dimensional models is warranted. They should be
avoided during design stages. Furthermore, they should also be avoided in thin-wall
structures, since solid elements tend to perform poorly because of locking problems.
The tetrahedron shape is applicable for basic three-dimensional solid element and the
hexahedron shape is another option, but it requires a more complex formulation in
comparison to tetrahedron. The number of nodes used to formulate a solid element can be
different. Six or ten node tetrahedron shape, eight or twenty node hexahedron shape
formulations are commonly used. Each node of these solid element types has three degrees of
freedom: translation in the nodal x, y, and z directions.
3.3
ADFEM Software
A finite element software, called ADFEM, is developed by using Java language based on
object-oriented methodology. During program development, three different tasks of the finite
element analysis (pre-processing, processing, and post processing) are often implemented as
three separate computer programs. Since these tasks have many common data structures and
methods, the three modules contain duplicated or similar code fragments which complicates
support and modification. In Java language, it is possible to have several main methods. The
Page 53 of 94
code (classes) can be organized into packages. A package is a named collection of classes
providing encapsulation and modularity, which can eliminate code duplication and provide a
means for easy code reuse. ADFEM is organized into six class packages, namely adfem, util,
model, solver, element including and external package called Jama that is useful for matrix
operations.
From the data point of view the finite element solution is transformation of input data into
output data. Since data describing a finite element mesh is too large, input is usually
generated by a pre-processor. Currently, ADFEM does not have a mesh generation capability.
Once the mesh of a problem is generated by an external tool, the nodal coordinates and the
element connectivity should be set up as an input file for ADFEM. There is a robust scanner
class, called fescanner, implemented in order to read very large input data. ADFEM is
designed to solve elastic and static problems with displacement and force boundary
conditions. The data can be divided into the data related to the finite element model and the
data describing loading conditions. The finite element model data and loading conditions
don’t change during problem solution since we suppose that the model shape, material
properties, and boundary conditions are constant. The description of the finite element model
is listed below:

Program initiator

Element types

Scalar parameters such as section types, section properties etc.

Material properties

Nodal data such as coordinates of nodal points

Element data such as element materials and connectivity

Description of displacement boundary conditions

Surface and concentrated loads

Solution command
Page 54 of 94
Table 3
Finite element library of ADFEM
Element
Name
Truss
Element
Type
Truss
Total Number of Nodal Degree
Nodes
Freedom
2
Ux, Uy, Uz
of Element Degree of
Freedom
6
Beam
Beam
2
Plane3
Plane
3
Ux, Uy, Uz, Rotx, 12
Roty, Rotz
Ux, Uy
6
Plane4
Solid Plane
4
Ux, Uy
8
Plane6
Solid Plane
6
Ux, Uy
12
Plane8
Solid Plane
8
Ux, Uy
24
Shell3
Shell
3
Shell4
Shell
4
Shell8
Shell
8
Solid8
Solid
8
Roty, Rotz
Roty, Rotz
Roty, Rotz
Ux, Uy, Uz
24
Finite element types are considered as main objects in both mathematical and algorithmic
senses. In order to implement the main methods for a finite element, an abstract class Element
is designed. The class holds element data, methods common to all element types, and empty
methods specific to particular element types. Overriding of the parent methods allows one to
create new element types using standard procedures. Formulation of truss, beam, plane, plate,
shell and solid element types has been implemented into the ADFEM. The formulation of
these element types has already been discussed and purely generated by many authors such as
Logan (2011), Bathe (2006) and Oñate (2013). Therefore, instead of providing the details of
the finite element formulation for each element type, only the capability parameters are given
in Table 3 for each element implemented into ADFEM.
A math library called SuanShu is used to solve linear matrix equation system in ADFEM.
SuanShu is an object-oriented, high performance, extensively tested, and professionally
Page 55 of 94
documented library of numerical methods. A CPU parallelized Cholesky decomposition
implemented in SuanShu is the current solver method used in ADFEM.
3.4
Applications and Validation of ADFEM
To verify implementation of the finite element code, sample problems have been solved by
using ADFEM. In fact, the selection of the problem type is completely dependent on the
selection of the element type that will be used to model the problem. Hence, at least one
problem needs to be described for each element type. First of all, a space truss structure is
considered by using Truss element. Secondly, a basic I cross section beam problem is
modelled in order to validate Beam element formulation in ADFEM. Thirdly, solution of a
complex frame structure is discussed in order to illustrate the capability of Beam element in
more detail. Next, two different plate problems under axial loading condition are considered
to confirm the accuracy of both Plane4 and Plane8. Since Plane3 and Plane6 are
simplification case of Plane4 and Plane8, respectively, there is no need to model a problem
with these element types. Once the plane element formulations used in ADFEM is validated,
transverse loading case of these problems is considered in order to demonstrate the capability
of the Shell3, Shell4 and Shell8 element types. The numerical results obtained by using
ADFEM are compared with the results that are found by using a commercial finite element
code, ANSYS. Based on the validation cases, the results obtained by using ADFEM are very
reasonable because they are in very good agreement with those found by using ANSYS. The
problem descriptions, results, and discussion of all these problems are given below.
3.4.1 Truss Problem
The space truss problem as shown in Figure 26 is considered for validation of truss element
formulation in ADFEM. Cross section area is 2 cm2 and elastic modulus is 210000 MPa for
all elements. The coordinates of each node, in centimetres, are shown in the figure. Nodes 1–4
Page 56 of 94
are supported by ball-and-socket joints (fixed supports). The space truss is subjected to a 1000
N load in the x direction at node 5 and the aim is to determine the displacement of node 5.
Figure 26 Space truss isometric view
Table 4
Displacement results of space truss problem
ADFEM ADFEM ADFEM ANSYS ANSYS ANSYS
NODE UX
UY
UZ
UX
UY
UZ
5
0.040908 0.000000 -0.011979 0.040908 0.000000 -0.011979
Once the unknown displacement is found, the strain and the stresses in each element are
calculated. For comparison purposes, the same problem is modelled with a space truss
element, Link180, in order to solve the described problem in ANSYS. The displacement,
strain and stress results that are obtained from ADFEM and ANSYS are tabulated in Table 4
and 5, respectively. Displacement results are listed in millimetres, while the corresponding
stress results has unit of MPa. As it can be seen from both tables, the results completely agree
with each other. Therefore, it is should be indicated that Truss element in ADFEM is
analogous to Link180 element in ANSYS.
Page 57 of 94
Table 5
Strain and stress results of space truss problem
ADFEM
ELEMENT EXX
1
1.786E-05
2
-1.331E-05
3
-1.331E-05
4
1.786E-05
ADFEM
SXX
3.750E+00
-2.795E+00
-2.795E+00
3.750E+00
ANSYS
EXX
1.786E-05
-1.331E-05
-1.331E-05
1.786E-05
ANSYS
SXX
3.750E+00
-2.795E+00
-2.795E+00
3.750E+00
3.4.2 Beam Problem
A console beam problem with I type cross section as shown in Figure 27 is considered for
validation of Beam element implemented in ADFEM. According to Figure 27, I cross section
properties are b =200 mm, h = 200 mm, t f = 15 mm, and tw = 15 mm. The selected material’s
elastic modulus is 210000 MPa with the Poisson’s ratio of v = 0.3. Length of the beam is L =
2 m and it is divided into 20 finite elements. In order to apply displacement boundary
conditions, one end node of the beam is fixed for all degrees of freedom while the other nodes
are free to translate and rotate. Beam is subjected to -1000 N concentrated load in the z
direction at all nodes except the fixed node.
Figure 27 Beam mesh and cross section
The aim of this problem is to determine the unknown translational and rotational
displacement for each node. The same problem is also modelled in ANSYS by using
Beam188 which is a beam element working based on Timoshenko Beam Theory. Moreover,
it is also solved analytically based on Euler Beam Theory for comparison purposes. Euler
Page 58 of 94
Beam Theory as well as Timoshenko Beam Theory is implemented into the formulation of
beam element used in ADFEM. There is a specific key option that is defined to select the
appropriate theoretical approach when the input file is prepared. This problem is solved for
both cases and the both results are provided in below. The translational and rotational
displacement results that are obtained from ADFEM, ANSYS and analytical solution are
plotted in Figure 28 in order to emphasize the difference between Euler and Timoshenko
beam theory.
0.00
-0.20 0
1.40E-03
5
10
15
20
1.20E-03
-0.40
1.00E-03
-0.60
8.00E-04
-0.80
-1.00
6.00E-04
-1.20
4.00E-04
-1.40
2.00E-04
-1.60
-1.80
0.00E+00
-2.00
0
5
10
15
20
ADFEM Euler Beam
ADFEM Euler Beam
Analytical Result
Analytical Result
ADFEM Timoshenko Beam
ADFEM Timoshenko Beam
ANSYS Beam 188
ANSYS Beam 188
(a)
(b)
Figure 28 (a) Translational and (b) rotational displacement results of the beam problem
As shown in Figure 28 (a), the translational displacements obtained from ADFEM and
ANSYS are in good agreement, while those obtained from ADFEM and analytical solution
agree well as well. However, the results from Euler and Timoshenko Beam Theory are
slightly different since Timoshenko Beam Theory uses shear correction parameter in order to
indicate the transverse shear effects, which is especially important when a beam becomes
thicker. Hence, the definition of shear correction parameter affects the displacements in
translational degree of freedom. Moreover, this affect is negligibly small in rotational degree
Page 59 of 94
of freedom for this problem, since all the rotational displacement results are in very well
agreement as shown in right hand side of Figure 28 (b).
3.4.3 Frame Structure Problem
A frame structure is modelled in ADFEM by using a beam element based on Timoshenko
Beam Theory. The same model is built in ANSYS with Beam188 element as well in order to
validate the results. Key points of the frame structure are represented in Figure 29 (a). The
coordinates of key points are listed in Table 6. Circular solid cross section is selected for each
beam with a radius of r = 10 mm. The selected material’s elastic modulus is 210000 MPa with
the Poisson’s ratio of v = 0.3. The frame structure divided into beam elements and the length
of each beam element is 50 mm. Therefore, the total number of the nodes used to discretise
this problem becomes 466.
(a)
(b)
Figure 29 Key point locations and application of boundary conditions on frame structure
The applied displacement and loading boundary conditions for this problem including the
direction of the concentrated forces are shown in Figure 29 (b). The magnitude of all the
applied concentrated loads is 1000 N. The displacement results generated by using ADFEM
Page 60 of 94
and ANSYS are compared for each degree of freedom, namely translations and rotations in x,
y, z directions as shown in Figures 30-32, respectively.
Table 6
Key
Point
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
Key points of frame structure
X
Y
0
1500
3000
0
1500
3000
0
1500
3000
0
1500
3000
0
1500
3000
0
1500
3000
0
1500
3000
-500
-500
-500
0
0
0
500
500
500
-500
-500
-500
0
0
0
500
500
500
0
0
0
Z
(mm)
0
0
0
0
0
0
0
0
0
500
500
500
500
500
500
500
500
500
750
750
750
According to the figures, the results are perfectly coincident. Also, the variation of the total
translational and rotational displacement magnitudes over the structure obtained from
ADFEM and ANSYS are presented in Figure 33 and 34, respectively. According to the
comparison of these results, it can be concluded that the ADFEM beam element is equivalent
to the ANSYS Beam 188 element.
Page 61 of 94
6.00
3.00
5.00
2.50
4.00
2.00
3.00
1.50
2.00
1.00
1.00
0.50
0.00
0.00
0
100
200
300
400
500
-1.00
0
100
200
300
400
500
-0.50
ADFEM UX
ANSYS UX
ADFEM UY
(a)
ANSYS UY
(b)
Figure 30 Frame structure translational displacements along (a) x- and (b) y- directions of
all nodes
1.50
2.00E-03
1.00E-03
1.00
0.00E+00
-1.00E-03
0.50
0
100
200
300
400
500
-2.00E-03
-3.00E-03
0.00
0
100
200
300
400
500
-4.00E-03
-5.00E-03
-0.50
-6.00E-03
-7.00E-03
-1.00
-8.00E-03
-1.50
-9.00E-03
ADFEM UZ
ANSYS UZ
(a)
ADFEM ROTX
ANSYS ROTX
(b)
Figure 31 Frame structure (a) translational-z and (b) rotational-x displacements of all nodes
Page 62 of 94
1.20E-02
5.00E-04
1.00E-02
4.00E-04
3.00E-04
8.00E-03
2.00E-04
6.00E-03
1.00E-04
4.00E-03
0.00E+00
2.00E-03
-1.00E-04
0
100
200
300
400
500
-2.00E-04
0.00E+00
0
100
200
300
400
500
-3.00E-04
-2.00E-03
-4.00E-04
-4.00E-03
-5.00E-04
ADFEM ROTY
ANSYS ROTY
ADFEM ROTZ
(a)
ANSYS ROTZ
(b)
Figure 32 Frame structure (a) rotational-y and (b) rotational-z displacements of all nodes
(a)
(b)
Figure 33 Frame structure total translational displacement contour plot;
(a) ADFEM and (b) ANSYS
Page 63 of 94
(a)
(b)
Figure 34 Frame structure total rotational displacement contour plot;
3.4.4 Plane4 Problem
A square plate structure with 1 m edge length as shown in Figure 35 is considered to be
solved under tension loading by using ADPAN’s Plane4 element which is implemented based
on isoparametric formulation.
Figure 35 A square plate mesh and boundary condition representation
Page 64 of 94
The same problem is solved in ANSYS by using Plane182 as well for comparison purposes. It
is assumed that the plate will deform based on plane stress condition and the plate thickness is
10 mm. The selected material’s elastic modulus is 210000 MPa with the Poisson’s ratio of v =
0.3.The geometry is discretised by using 4489 elements and 4624 nodes as presented in
Figure 35. All nodes at the left edge of the plate are considered to be fixed and a nodal force
of 1000 N in x-direction is applied to each node at the right edge of the plate.
0.04
0.01
0.04
0.01
0.03
0.00
0.03
0.00
0.02
0.00
0.02
0
0.01
2000
3000
4000
5000
0.00
0.01
-0.01
0.00
-0.01
1000
0.00
0
1000
2000
ADFEM UX
3000
4000
5000
-0.01
ANSYS UX
(a)
ADFEM UY
ANSYS UY
(b)
Figure 36 Translational displacements along (a) x- and (b) y-directions of all nodes for the
Plane4 problem
Page 65 of 94
(a)
(b)
problem; (a) ADFEM and (b) ANSYS
The displacement results generated by using ADFEM and ANSYS are compared for each
degree of freedom, namely translations in x, y directions, as shown in Figure 36, respectively.
The displacement results are perfectly matching with each other according the figures. The
variation of the nodal translational displacement in x- and y-directions over the plate obtained
from ADFEM and ANSYS are presented in Figures 37 and 38. According to the comparison
of these variations, it can be concluded that the ADFEM Plane4 element is similar to the
ANSYS Plane182 element.
(a)
(b)
Page 66 of 94
3.4.5 Plane8 Problem
A rectangular plate structure with 1 m length and 0.5 m height is considered to be solved
under a loading condition as shown in Figure 39.
Figure 39 A rectangular plate and its applied boundary conditions
This problem is not just only modelled by using ADFEM’s Plane8 element, but also solved
with Plane183 element in ANSYS for validation purposes. It is assumed that the plate will
deform based on plane stress condition and the plate thickness is 10 mm. The selected
material’s elastic modulus is 210000 MPa with the Poisson’s ratio of v = 0.3. According to
the Figure 39, the plate is meshed by using 1250 elements and 3901 nodes and all nodes at
left edge of the plate are considered to be fixed.
Page 67 of 94
0.3
0.1
0.25
0
0.2
-0.1
0.15
0
1000
2000
3000
4000
-0.2
0.1
-0.3
0.05
-0.4
0
-0.05
0
1000
2000
3000
4000
-0.5
-0.1
-0.6
-0.15
-0.7
-0.2
-0.8
ANSYS UX
ADFEM UX
ANSYS UY
(a)
ADFEM UY
(b)
Plane8 problem
(a)
(b)
In addition to the displacement boundary condition, Figure 39 illustrates that nodal force of
1000 N in x-direction together with a nodal force of -1000 N in y-direction is applied to each
node at the right and upper edge of the plate, respectively. The displacement results generated
by using ADFEM and ANSYS are individually compared for each degree of freedom, namely
translations in x, y directions (see Figure 40). The displacement results are perfectly matching
Page 68 of 94
each other according the figures. The variation of the nodal translational displacement in x
and y direction over the plate obtained from ADFEM and ANSYS are respectively
demonstrated in Figure 41 and 42. According to the comparison of these variations, it can be
indicated that the ADFEM Plane8 element is good agreement with ANSYS Plane183.
3.4.6 Shell3 Element
Shell3 element has three nodes on the edges of the element and bending capability of the
elements is implemented based on Mindlin Plate Theory. Isoparametric shape functions are
used to formulate the element and the mathematical foundation that describes the flexural
capability of the element is provided by Tessler (1985) and Tessler and Hughes (1985).
Membrane stiffness of the element is identical to the Plane3 (constant strain triangle)
formulation in ADFEM.
solved under a distributed out of plane loading condition by using ADFEM’s Shell3 element.
For comparison purposes, the same problem is solved with Shell 181 which is a three or four
node shell element in ANSYS. The plate thickness is 10 mm. The selected material’s elastic
modulus is 210000 MPa with the Poisson’s ratio of v = 0.3.The geometry is discretised by
using 3200 elements and 1681 nodes as presented in Figure 43.
Page 69 of 94
Figure 43 A clamped edge square plate and its discretization
All the nodes at right, left, upper, and bottom edges of the plate are considered to be fixed,
and therefore, the clamped edge boundary condition is considered. Nodal force of -100 N in z
direction is applied to all nodes of the plate except the nodes that are already fixed.
0.000
0
500
1000
1500
-2.000
-4.000
-6.000
-8.000
-10.000
-12.000
ADFEM UZ
ANSYS UZ
Figure 44 Translational displacements along z-direction of all nodes for the Shell3 problem
Page 70 of 94
0.04
0.04
0.03
0.03
0.02
0.02
0.01
0.01
0.00
0.00
0
500
1000
0
1500
-0.01
-0.01
-0.02
-0.02
-0.03
-0.03
-0.04
-0.04
ADFEM ROTX
ANSYS ROTX
500
1000
ADFEM ROTY
(a)
1500
ANSYS ROTY
(b)
Figure 45 Rotational displacements along (a) x- and (b) y-directions of all nodes for the
Shell3 problem
(a)
(b)
The non-zero displacement results generated by using ADFEM and ANSYS are compared for
each degree of freedom, namely translation in z-direction and rotations in x and y directions,
respectively, as shown in Figure 44 and 45. The displacement results are perfectly matching
Page 71 of 94
with each other according the figures. The variation of the nodal translational displacement in
z-direction over the plate obtained from ADFEM and ANSYS are shown in Figure 46.
Furthermore, the variation of the nodal rotational displacement in x- and y-directions over the
plate are illustrated in Figures 47 and 48. According to the comparison of these variations, it
can be concluded that the ADFEM Shell3 element is working very well.
(a)
(b)
Figure 47 Contour plot of rotational displacement along x-direction for the Shell3 problem;
(a)
(b)
Figure 48 Contour plot of rotational displacement along y-direction for Shell3 problem;
Page 72 of 94
Shell4 element is a quadrilateral element with four nodes at its corners.
The bending
capability of the element is implemented based on the Mindlin Plate Theory. Isoparametric
shape functions are used to formulate the element and the mathematical foundation that
describes the flexural capability of the element is provided by Tessler and Hughes (1983).
Membrane stiffness of the element is identical to the Plane4 formulation in ADFEM. In
addition to the bending capability and membrane stiffness, drilling rotation degree of freedom
is added to Shell4 formulation based on the proposed formulation by Cook, R. D. (1994). It
should be noted Shell4 becomes very robust to solve complex problems after adding all these
capabilities.
Figure 49 T beam mesh and its boundary conditions
A beam problem which has a T type cross section is solved by using Shell4 as shown in
Figure 49. Two different plates are attached together in order to create the geometry of the
structure. These plates have the same length of 2000 mm together with different heights, 200
mm and 400 mm.
Page 73 of 94
0.800
2.000
0.600
0.000
0.400
-2.000
0.200
-4.000
500
1000
1500
2000
-6.000
0.000
-0.200
0
0
500
1000
ADFEM UX
1500
2000
-8.000
ADFEM UY
ANSYS UX
(a)
ANSYS UY
(b)
Shell4 problem
The same problem is modelled with Shell181 in ANSYS in order to show the capability of
Shell4 with respect to Shell181. Each plate has thickness of 10 mm. The selected material’s
elastic modulus is 210000 MPa with the Poisson’s ratio of v = 0.3.The geometry is discretised
by using 1920 elements and 2025 nodes as presented in Figure 49.
0.010
3.00E-04
2.00E-04
0.005
1.00E-04
0.00E+00
0.000
0
500
1000
1500
2000
0
-1.00E-04
500
1000
1500
2000
-0.005
-2.00E-04
-3.00E-04
-0.010
ADFEM UZ
ADFEM ROTX
ANSYS UZ
(a)
ANSYS ROTX
(b)
Figure 51 (a) Translational-z and (b) rotational-x displacements of all nodes for the Shell4
problem
Page 74 of 94
1.50E-04
0.00E+00
0
1.00E-04
500
1000
1500
2000
-1.00E-03
5.00E-05
-2.00E-03
0.00E+00
0
500
1000
1500
2000
-5.00E-05
-3.00E-03
-1.00E-04
-4.00E-03
-1.50E-04
-5.00E-03
ADFEM ROTY
ANSYS ROTY
ADFEM ROTZ
(a)
ANSYS ROTZ
(b)
Figure 52 Rotational displacements along (a) y- and (b) z-directions of all nodes for the
Shell4 problem
One end of the beam is fixed for all degrees of freedoms and a nodal force of -1000 N in ydirection is applied to other end nodes which are on symmetry plane of the structure as shown
in Figure 49. The unknown displacement results of ADFEM and ANSYS are compared for all
degree of freedom as shown in Figure 50-52. The variation of nodal translational and
rotational displacements over the plate are respectively presented in Figures 53-58.
(a)
(b)
Figure 53 Contour plot of translational displacement along x direction for the Shell4
Page 75 of 94
(a)
(b)
Figure 54 Contour plot of translational displacement along y direction for the Shell4
As it is shown in the figures that the displacement results are in perfect agreement for all
translational displacement and rotational displacement in x- and z-directions, although there is
a difference exists for the rotational displacement in y-direction. Actually, this difference is
due to the drilling rotation formulation used for Shell4. When the structure is considered to be
modelled by beam elements, it can be seen that drilling rotation degree of freedom is
rotational degree of freedom in y direction. Since the direction of load applied to the structure
is same as the direction of the drilling rotation degree of freedom, a very small contribution is
expected from rotational displacement in y-direction to the total rotational displacement.
Page 76 of 94
(a)
(b)
(a)
(b)
In ADFEM results, range of rotational displacements in y-direction is very small in
comparison to other rotational displacements, while corresponding ANSYS results are much
higher than ADFEM as shown in Figure 52. Furthermore, the variation of this displacement
over the structure for ADFEM is more reasonable than ANSYS as it can be seen from Figure
57. As a consequence, it can be concluded that the implemented drilling rotational stiffness
proposed by Cook (1994) is very promising and Shell4 element is robust enough to model
complex structures.
Page 77 of 94
(a)
(b)
Figure 57 Contour plot of rotational displacement along y-direction for the Shell4 problem;
(a)
(b)
Figure 58 Contour plot of rotational displacement along z-direction for the Shell4 problem;
Shell8 element has eight nodes on the edges of the element in total. Four of these nodes
located at the corner of the element while the remaining four of them located at the mid-point
Page 78 of 94
of the edges. Isoparametric shape functions are used to formulate both bending and membrane
stiffness of the element. Formulation of the bending capability is based on the Mindlin Plate
Theory while membrane capability of the element is equal to the Plane8 formulation in
ADFEM.
Figure 59 A clamped square plate modelled with Shell8
solved by using Shell8 when out of plane loading is applied to the structure. The same
problem is solved with Shell281 which is a six or eight node shell element in ANSYS for
validation process.
6.00
4.00
2.00
0.00
-2.00
0
500
1000
1500
2000
-4.00
-6.00
ADFEM UZ
ANSYS UZ
Figure 60 Translational displacements along z-direction of all nodes for the Shell8 problem
Page 79 of 94
The plate thickness is 10 mm. The selected material’s elastic modulus is 210000 MPa with
the Poisson’s ratio of v = 0.3.The geometry is discretised by using 625 elements and 1976
nodes. Figure 59 shows that all nodes at right, left, upper, and bottom edges of the plate are
considered to be fixed, and therefore the clamped edge boundary condition is considered.
Nodal force of -100 N in z direction is applied to all nodes below the centreline along x
direction of the plate, while the reverse of the same loading condition is applied to the nodes
above the centreline along x direction of the plate. The direction of the applied loading
condition can be seen in Figure 59 in more detail.
0.30
0.15
0.20
0.10
0.05
0.10
0.00
0.00
0
500
1000
1500
2000
-0.05
-0.10
-0.10
-0.20
-0.15
ADFEM ROTX
0
ANSYS ROTX
500
1000
ADFEM ROTY
(a)
1500
2000
ANSYS ROTY
(b)
Figure 61 Rotational displacements along (a) x- and (b) y-directions of all nodes for the
Shell8 problem
Page 80 of 94
(a)
(b)
The unknown displacement results found in ADFEM and ANSYS are compared for each
degree of freedom. The displacement results are perfectly identical to each other according to
Figures 60 and 61. The variation of the nodal translational displacement in z direction,
rotational displacement in x- and y- directions over the plate are demonstrated in Figures 63
and 64, respectively. According to the comparison of these variations, it can be concluded that
the Shell8 element gives reasonable results and can be used to build complex structures as
well as Shell4 element.
Page 81 of 94
(a)
(b)
(a)
(b)
Figure 64 Contour plot of rotational displacement along y-direction for the Shell8 problem;
Page 82 of 94
3.5
Global Finite Element Analyses of Ship and Coupling of Finite
Elements
The global three dimensional finite element model is a representative of the hull structures of
three cargo holds with the middle cargo hold within 0.4L amidships. It is used to determine
both the global response of the hull girder and local behaviour of the main supporting
structures. The stress results from such models must be suitable for strength evaluation of the
watertight boundaries of cargo holds and non-tight main supporting structures. The global
three dimensional finite element analyses establish the scantling requirements of plates and
stiffeners, and they are sufficient for establishing the steel weight estimate. Structural details
are evaluated by the subsequent local three dimensional finite element analyses.
To evaluate the vessel’s structures within 0.4L amidships with reasonable accuracy, the finite
element models ideally place the target cargo hold in the middle and extend approximately the
length of the adjacent holds fore and aft. In addition, there is a short extension beyond the
transverse bulkheads at both ends. Even though finite element analysis can be done by using
both full and half-width models, it is recommended that the finite element models should be
created with both the port and starboard sides of cargo hold structures, that are symmetrical
with respect to the centreline, for easier review, result analysis and subsequent strength In
general, the ship structural finite element model consists of four types of elements:
For stiffeners:

Truss element

Beam element
For plates:

Membrane plate element (simplified case of Shell Element).

Shell Element.
Page 83 of 94
Figure 65 Stiffened plate model
These four simple types of elements are considered sufficient to represent the hull structures
even though higher order element types exist. Ship structures consist of various stiffened
plates. These stiffened plates can be represented by a combination of membrane plates and
rod elements as long as only in-plane stress is calculated from the model. Combined use of
membrane plates and rod elements may simplify the modelling processes and reduce the total
number of degrees of freedom in the model. However, additional operations, such as shifting
load, may result in less accurate results for some elements.
As a consequence, combination of shell and beam elements is preferable in order to obtain
more realistic results. Appropriate properties of stiffeners are assigned by considering
equivalent beams model. Also, the required properties of plates are attached to the equivalent
shell model. The combination of beam model and shell model can be done by defining an
appropriate rigid link between them. Since ADFEM have the Beam and Shell element types,
portion of the side of a typical longitudinally and transverse framed (complex frame system)
ballast tank as shown in left hand side of Figure 65 can be modelled to demonstrate the
capability of the element combination. A stiffened square plate with 1 m edge length as
shown on right hand side of Figure 65 is considered to be solved under out of plane loading.
Page 84 of 94
Figure 66 Stiffened plate boundary conditions
The plate is modelled with Shell4 element, while longitudinal and transverse stiffeners are
modelled with Beam element based on Timoshenko Beam Theory. The required rigid links
between Shell4 and Beam elements are defined by using Beam element based on Euler Beam
Theory. The same problem is designed to be solved with Shell181 and Beam181 elements in
ANSYS for validation purposes.
1.50E-02
1.50E-02
1.00E-02
1.00E-02
5.00E-03
5.00E-03
0.00E+00
0.00E+00
0
500
1000
1500
2000
0
-5.00E-03
-5.00E-03
-1.00E-02
-1.00E-02
-1.50E-02
-1.50E-02
ADFEM - UX
ANSYS - UX
500
1000
ADFEM - UY
(a)
1500
2000
ANSYS - UY
(b)
Page 85 of 94
stiffened plate
1.60E-01
8.00E-04
1.40E-01
6.00E-04
1.20E-01
4.00E-04
1.00E-01
2.00E-04
8.00E-02
0.00E+00
6.00E-02
-2.00E-04
4.00E-02
0
500
1000
1500
2000
-4.00E-04
2.00E-02
-6.00E-04
0.00E+00
0
500
1000
ADFEM - UZ
1500
2000
-8.00E-04
ADFEM - ROTX
ANSYS - UZ
(a)
ANSYS - ROTX
(b)
Figure 68 (a) Translational-z and (b) rotational-x displacements of all nodes for the stiffened
plate
The plate thickness is 10 mm. Rectangular solid cross section is selected for each beam with
thickness of 10 mm and height of 100 mm The selected material’s elastic modulus is 210000
MPa with the Poisson’s ratio of v = 0.3.The geometry is discretised by using 1993 nodes
together with 2232 elements from which 1920 of them are Shell4 elements and 312 of them
are Beam elements.
Page 86 of 94
6.00E-04
6.00E-05
4.00E-04
4.00E-05
2.00E-04
2.00E-05
0.00E+00
0.00E+00
0
500
1000
1500
2000
0
-2.00E-04
-2.00E-05
-4.00E-04
-4.00E-05
-6.00E-04
-6.00E-05
ADFEM - ROTY
ANSYS - ROTY
500
1000
ADFEM - ROTZ
(a)
1500
2000
ANSYS - ROTZ
(b)
Figure 69 Rotational displacements along y- and z- directions of all nodes for the stiffened
plate
(a)
(b)
Figure 70 Contour plot of translational displacement along x-direction for the stiffened
plate; (a) ADFEM and (b) ANSYS
As shown in Figure 66, all nodes at the right, left, upper, and bottom edges of the plate are
considered to be fixed, and therefore the clamped edge boundary condition is considered.
Nodal force of 100 N in z direction is applied to nodes attached to the mid-plane of the plate.
Page 87 of 94
(a)
(b)
Figure 71 Contour plot of translational displacement along y-direction for the stiffened
The unknown displacement results of ADFEM and ANSYS are compared for each degree of
freedom in Figures 67-69. The variation of the nodal translational and rotational
displacements over the plate are demonstrated in Figures 70-75.
(a)
(b)
Figure 72 Contour plot of translational displacement along z-direction for the stiffened
Page 88 of 94
As it can be seen from the figures that the results are in perfect agreement for all translational
displacement. The results are very similar to each other as well for rotational displacements in
x- and y-directions, while a difference exists for the rotational displacement in z-direction due
to the drilling rotation formulation used for Shell4 which is clearly described earlier in Shell4
Problem section.
(a)
(b)
Figure 73 Contour plot of rotational displacement along x-direction for the stiffened plate;
Page 89 of 94
Figure 74 Contour plot of rotational displacement along y-direction for the stiffened plate;
As a summary, current finite elements implemented into ADFEM enables the coupling of
elements in finite element analysis sense. Therefore, this capability of ADFEM provides the
opportunity to conduct a three dimensional global finite element analysis of any type of ship
in a more computationally efficient manner.
Figure 75 Contour plot of rotational displacement along z-direction for stiffened plate; (a)
ADFEM and (b) ANSYS
Page 90 of 94
4 CONCLUSION
An in-house finite element code, ADFEM, together with a panel-method code, ADPAN, are
implemented by using Java language based on object-oriented methodology. The theoretical
background used to develop both software is described in detail. The finite element code is
examined and verified by solving a problem for each element type implemented into its finite
element library.
The procedures how to build a global three dimensional finite element model of the hull
structures are described. One of the most effective techniques for global finite element
analysis of ship structures is coupling suitable element types together. A portion of the side of
a typical longitudinally and transverse framed (complex frame system) ballast tank is
analysed in ADFEM to demonstrate the capability of finite element coupling.
Moreover, ADPAN is used to conduct hydrodynamic analysis of floating hemisphere,
submerged spheroid, long barge, WIGLEY III and S175 container ship in order to validate
and demonstrate the capability of ADPAN. For analysis of WIGLEY III and S175 container
ship, hydrodynamic pressure are calculated and exported from ADPAN for each panel that is
used to model the body surface. The variation of the hydrodynamic pressure is demonstrated
over the hull surfaces. The pressure calculation allows the user of the codes to perform a
hydro-elastic response analysis of the ship structure.
Page 91 of 94
5 REFERENCES
Bathe, K. J. (2006). Finite Element Procedures. Prentice-Hall.
Beck, R. F. and Loken, A. E. (1989). Three-dimensional effects in ship relative-motion
problems. Journal of Ship Research, 33(4), 261-268.
Chapelle, D. and Bathe, K. J. (2011). The finite element analysis of shells: Fundamentals
(Vol. 1). Berlin: Springer.
Cook, R. D. (1994). Four-node ‘flat’shell element: Drilling degrees of freedom, membranebending coupling, warped geometry, and behavior. Computers & Structures, 50(4), 549-555.
Faltinsen, O.M. and Michelsen, F.C. (1974). Motions of large structures in waves at zero
Froude number. In The Dynamics of Marine Vehicles and Structures in Waves, London.
Fish, J. and Belytschko, T. (2007). A First Course in Finite Elements. John Wiley & Sons.
Garrison, C.J. (1978). Hydrodynamic Loading of Large Offshore Structures. In Zienkiewicz,
O.C., Lewis, O.C., and Stagg, K.G., (Eds.), Numerical Methods in Offshore Engineering, pp.
87–139. Chichester, England: John Wiley & Sons.
Hess, J. L. and Smith, A. M. O. (1964) Calculation of nonlifting potential flow about arbitrary
three-dimensional bodies. Journal of Ship Research, 8, 2, 22–44.
Hogben, N. and Standing, R.G. (1974). Wave Loads on Large Bodies. In The Dynamics of
Marine Vehicles and Structures in Waves, London.
Hulme, A. (1982). The wave forces acting on a floating hemisphere undergoing forced
periodic oscillations. Journal of Fluid Mechanics, 121, 443–463.
Page 92 of 94
Logan, D. (2011). A first course in the finite element method. Cengage Learning.
Maniar , H. D. (1995). A three dimensional higher order panel method based on B-splines,
Ph.D. thesis, Massachusetts Institute of Technology, Cambridge, MA.
Newman, J. N. (1977). Marine hydrodynamics. MIT press.
Newman, J.N. (1985). The evaluation of free-surface Green functions. In Fourth International
Conference on Numerical Ship Hydrodynamics, Washington.
Noblesse, F. (1982). The Green function in the theory of radiation and diffraction of regular
water waves by a body. Journal of Engineering Mathematics, 16(2), 137-169.
Oñate, E. (2013). Structural Analysis with the Finite Element Method. Linear Statics: Volume
2: Beams, Plates and Shells (Vol. 2). Springer.
Papanikolaou, A. D. and Schellin, T. E. (1992). A three-dimensional panel method for
motions and loads of ships with forward speed.
Telste, J. G. and Noblesse, F. (1986). Numerical evaluation of the Green function of waterwave radiation and diffraction. Journal of Ship Research, 30(2), 69-84.
Tessler, A. and Hughes, T. J. (1983). An improved treatment of transverse shear in the
Mindlin-type four-node quadrilateral element. Computer Methods in Applied Mechanics and
Engineering, 39(3), 311-335.
Tessler, A. (1985). A priori identification of shear locking and stiffening in triangular Mindlin
elements. Computer Methods in Applied Mechanics and Engineering, 53(2), 183-200.
Tessler, A. and Hughes, T. J. (1985). A three-node Mindlin plate element with improved
transverse shear. Computer Methods in Applied Mechanics and Engineering, 50(1), 71-101.
Page 93 of 94
Wehausen, J. V. and Laitone, E. V. (1960). Surface waves (pp. 446-778). Springer Berlin
Heidelberg.
Wu, G. X., and Eatock Taylor, R. (1987) The exciting forces on a submerged spheroid in
regular waves. Journal of Fluid Mechanics, 182, 411–426.
Page 94 of 94

Hydrodynamic and structural analysis

Transcription

Similar documents

How to prepare succesful projects

Audemars Piguet - Case Study

hydrodynamic separation

FNU Highlights from the - Frontier Nursing University

User Manual of how to inquire about Traffic Fines by the Mobile

ANSYS® Mechanical™ Liebherr

Dynamic - Solartron Metrology

Mechanical Enterprise

RCD Insert -Kaleidoscope

SU-233/PVS M3X Tactical Illuminator