Isoparametric bilinear quadrilateral element

2D Plane Elasticity:
Isoparametric Bilinear Quadrilateral
Lagrange type Element
with 4 Nodes
Filipe Amorim Gonçalves Giesteira
Supervisors:
Francisco Andrade Pires
José Fernando Dias Rodrigues
Finite Element Method (FEM) – EM065
Integrated Master in Mechanical Engineering
December, 2018

iii
Abstract
This report was developed with the main goal of gathering in one single and concise document, the
following three major tasks, namely: (i) review extensively and in detail, the fundamental concepts of
2D plane elasticity theory, from the displacement field definition to the static equilibrium equations of
a generic body; (ii) systematize the basic principles of the FEM, and the steps necessary to formulate
any quadrilateral element for plane elasticity; and finally (iii) produce a document (to be evaluated as
mandatory assignment) within the context of the Finite Element Method (FEM) course from the
Mechanical Engineering department, lectured at Faculty of Engineering of University of Porto (FEUP).
The basic concepts and formulae that govern the plane elasticity of linear elastic solids were first detailed
and several usually omitted demonstrations (in typical FEM technical literature) shown. Then, the FEM
equations were formulated using different variational principles and direct integral statements.
The finite element formulation was detailed specifically for the Isoparametric Bilinear (4-nodes)
Quadrilateral Lagrange type Element. However, all theoretical demonstrations, formulation steps and
isoparametric relations were kept as generic as possible for 2D plane elasticity.
The formulated element was implemented using MATLAB® software, and the algorithm was based on
the original script from BaPMEF (Base para Programação do Método dos Elementos Finitos) FEA tool.
From the present work, it is possible to underline the versatility, flexibility, and accuracy of the FEM
for simple and more complex engineering problems. Even though in real-life situations there are almost
no truly 2D problems, during this report the simplification power of 2D analysis and its prediction
capability was highlighted by exploring several engineering examples. The validation of the
quadrilateral finite element was successfully achieved by analytical formulas from linear plane elasticity
theory. Commercially available CAE suites with FEA integrated packages were also used to assess the
computational accuracy from the finite element formulated.
Keywords
2D Elasticity, Plane Elasticity, Plane Stress, Plane Strain, Strong Formulation, Weak Formulation, FEA,
Finite Element Analysis, FEM, Finite Element Method, Finite Element Formulation, Quadrilateral,
Isoparametric, Lagrange Family, Lagrangian Element, Bilinear, 4-nodes, Gauss Quadrature, MATLAB,
Abaqus

v
Contents
Contents .............................................................................................................................................v
List of Acronyms ............................................................................................................................... vii
List of Figures .................................................................................................................................... ix
List of Tables ................................................................................................................................... xiii
1 Introduction....................................................................................................................................1
1.1 Context of the Report ......................................................................................................................1
1.2 Report Structure..............................................................................................................................1
1.3 Basic Mathematical Nomenclature...................................................................................................2
2 Theory of Linear Elasticity for Continuum Medium ..........................................................................3
2.1 Introduction.....................................................................................................................................3
2.2 Stress Tensor .................................................................................................................................3
2.3 Strain Tensor..................................................................................................................................8
2.4 Generalized Hooke’s Law..............................................................................................................11
2.5 Transformation Matrix ...................................................................................................................14
2.6 2D Linear Elasticity .......................................................................................................................16
2.6.1 Types of Plane Linear Elastic Problems........................................................................16
2.6.2 Dynamic Equilibrium....................................................................................................17
2.6.3 Transformation Matrix..................................................................................................18
2.6.4 2D Hooke’s Law – Isotropic Material Behavior..............................................................19
2.6.5 Strain-Displacement Fields Relation.............................................................................22
2.6.6 Eliminating Stress and Strain in the z direction .............................................................23
3 Finite Element Formulation – Strong and Weak Formulation.........................................................25
3.1 Review of the Governing Equations for 2D Elasticity ......................................................................25
3.1.1 Displacement Field......................................................................................................25
3.1.2 Strain Field..................................................................................................................25
3.1.3 2D Hooke’s Law – Isotropic Material Behavior..............................................................26
3.1.4 2D Hooke’s Law – Orthotropic Material Behavior (Extra)...............................................26
3.1.5 Total Stress-Strain Relation (Extra) ..............................................................................27
3.1.6 Dynamic Equilibrium....................................................................................................28
3.2 Strong Formulation........................................................................................................................29
3.3 Weak Formulation – Direct Variational Formulations ......................................................................32
3.3.1 The Principle of Minimum Total Potential Energy (MTPE) .............................................33
3.3.2 The Principle of Virtual Work (PVW) or The Principle of Virtual Displacements (PVD) ....36
3.3.3 Hamilton’s Principle.....................................................................................................37
3.4 Weak Formulation – Weighted-Integral Formulations......................................................................39
3.4.1 Assumption #1 ............................................................................................................39
3.4.2 Assumption #2 ............................................................................................................40
4 Isoparametric Quadrilateral Lagrange Element with 4 nodes ........................................................47
4.1 Interpolation Functions – Introduction and Lagrange Family ...........................................................47
4.2 Interpolation Function - Generation................................................................................................49
4.3 Isoparametric 2D Mapping and Relations.......................................................................................54
4.4 Numerical Integration ....................................................................................................................64
5 Finite Element Method - Equations...............................................................................................69
5.1 Discretization by the Finite Element Method...................................................................................69
5.2 Properties of the Finite Element.....................................................................................................71
5.2.1 Stiffness Matrix of each element...................................................................................71
5.2.2 Equivalent Nodal Load Vector......................................................................................72
5.3 Discretized Global Model – Assembly of the Finite Elements ..........................................................76
5.4 Computation Step .........................................................................................................................80

vi
5.4.1 Application of the Fundamental Boundary Conditions ...................................................80
5.4.2 Displacement Field......................................................................................................80
5.5 Post-Processing Step ...................................................................................................................80
5.5.1 Strain and Stress Field ................................................................................................80
5.5.2 Dependent Post-Processing Variables .........................................................................84
6 BaPMEF Script ............................................................................................................................85
6.1 Introduction ..................................................................................................................................85
6.2 Data Input.....................................................................................................................................86
6.2.1 Tool Info .....................................................................................................................86
6.2.2 Body Geometry...........................................................................................................86
6.2.3 Type of 2D Plane Problem...........................................................................................87
6.2.4 Definition of the Body (Element) Thickness ..................................................................87
6.2.5 Type of Meshing Procedure.........................................................................................87
6.2.6 Type of Mesh ..............................................................................................................88
6.2.7 Materials.....................................................................................................................88
6.2.8 Input Mode – Nodal Coordinates, Nodal Connections and Fundamental Boundary
Conditions ............................................................................................................................89
6.2.9 Fundamental Boundary Conditions ..............................................................................89
6.2.10 Loading Conditions – Natural Boundary Conditions ......................................................93
6.2.11 Point Loads.................................................................................................................95
6.3 Global Stiffness Matrix ..................................................................................................................95
6.4 Global Equivalent Load Vector ......................................................................................................95
6.5 Static Solution and Plotting of Nodal Displacements.......................................................................96
6.6 Post-processing............................................................................................................................96
7 Finite Element Validation – Analytical Solutions from Plane Elasticity .........................................101
7.1 Introduction - Airy Stress Function and Biharmonic Equation........................................................ 101
7.2 Rectangular Cross-Section Beam with Constant Section - Pure Bending ...................................... 101
7.3 Rectangular Cross-Section Beam with Constant Section – Cantilever Beam with Shear Distributed
Load107
7.4 Rectangular Cross-Section Beam with Constant Section – Simple Supported Beam under Uniform
Surface Traction ......................................................................................................................... 115
8 FEM Tool – Applications ............................................................................................................125
8.1 Fracture Mechanics – Infinite Plane with Centered Crack............................................................. 125
8.2 Comparison with Commercially Available Software - Abaqus........................................................ 140
8.2.1 Generic Loading........................................................................................................140
9 Conclusions and Future Work ....................................................................................................149
References.....................................................................................................................................151

vii
List of Acronyms
1D – One Dimension/Dimensional
2D – Two Dimension/Dimensional
3D – Three Dimension/Dimensional
BaPMEF – Base para Programação do Método dos Elementos Finitos
BC – Boundary Condition(s)
CAD – Computer Aided Design
CAE – Computer Aided Engineering
FEA – Finite Element Analysis
FEM – Finite Element Method
FEUP – Faculty of Engineering of University of Porto
GP – Gauss Points
MTPE – Minimum Total Potential Energy
PDE – Partial Differential Equations
PVD – Principle of Virtual Displacement
PVW – Principle of Virtual Work
List of Acronyms

ix
List of Figures
Figure 1- Definition of the nomenclature adopted for shear stresses acting on the differential volume
element [1]......................................................................................................................................... 4
Figure 2- a) Cauchy tetrahedron formed by slicing a parallelepiped along an arbitrary plane define by
the normal vector 𝑛. b) Infinitesimal triangular portion of a generic 2D body. .................................... 6
Figure 3- Nomenclature adopted for the shear stress definition, for the distortion of the differential
Cartesian element..............................................................................................................................10
Figure 4- Illustration of the angles between the transformed 𝑥’-axis and the original cartesian coordinate
system. .............................................................................................................................................14
Figure 5- Illustration of the individual rotations of the Euler angles. Image adapted form [2]. ............14
Figure 6- Definition of the nomenclature used to define the coordinates transformation matrix. The 𝜃,
𝜑, and 𝜓, represent the rotation angle about the z, x and y axis respectively. .....................................15
Figure 7- a) Plane Stress schematic geometry. b) Plane Strain schematic geometry............................16
Figure 8- Representation of the transformation of the coordinate system by rotation along the z-axis: a)
Counter Clockwise rotation, and b) Clockwise rotation. ....................................................................18
Figure 9- Lagrange Quadrilateral Element of four nodes in its natural coordinates system and natural
coordinates values.............................................................................................................................48
Figure 10- 3D representation of the four shape functions of the Isoparametric Quadrilateral Lagrange
Element with four nodes. ..................................................................................................................52
Figure 11- 3D surface plot of the determinant of the Jacobian matrix for isoparametric bilinear
quadrilateral elements with multiple degrees of distortion..................................................................55
Figure 12- Illustration of the true area and shape of a differential element of area in Natural coordinate
system. Based on illustrations and equations from [4], [5], [6]...........................................................58
Figure 13- a) Tangential and normal tractions acting on the horizontal boundary of the real distorted
finite element (particular example shown for the upper boundary with 𝜂 = 1 ). b) Tangential and normal
tractions acting on the vertical boundary of the real distorted finite element (particular example shown
for the right boundary with 𝜉 = 1 ). Illustration adapted from [4]. .....................................................63
Figure 14- Illustration of different cases of surface traction load applied in the a) lower, b) upper, c) left,
and d) right boundaries. Adapted by the author from [4]....................................................................75
Figure 15- Schematic illustration of the process of construction of the Connectivity matrix. The
connection matrix is a rectangular matrix, usually with higher number of rows than columns. ...........79
Figure 16- Schematic illustration of the concept of sub-element used to take advantage of the knowledge
of the strains in the GP......................................................................................................................82
Figure 17- Schematic illustration of the process of smoothing the nodal values for the strains or stresses
after post-processing [4]....................................................................................................................83
Figure 18- Overall structure of the BaPMEF script [3].......................................................................85
Figure 19- First interface that immediately pops-up after running the FEA tool. It should be noticed the
several features of the tool that the user cannot control or change. .....................................................86
Figure 20- A. The input window for the geometric variables comes already with some default values,
to encourage the user to pay attention to the units of length used (mm). .............................................86
Figure 21- Interface used to specify the type of plane problem, in which the user only has to press the
button that contains the desired analysis. ...........................................................................................87

x
Figure 22- Illustration of the two different possibilities of GUI that the user can be face with, after the
user select the desired plane problem: a) After selection of plane stress problem, b) After selection of
plane strain problem..........................................................................................................................87
Figure 23- GUI used to specify the type of meshing procedure desired..............................................87
Figure 24- GUI to input the necessary parameters to define the mesh if: a) The automatic process was
selected, b) The semi-automatic process was selected........................................................................88
Figure 25- Graphic Interface for input of the material properties. ......................................................88
Figure 26- Message window used to inform the user that the input mode of the nodal coordinates and
connections is predefined as automatic and the user cannot control it. ...............................................89
Figure 27- Graphic interface used to choose the input mode of the fundamental BC. .........................89
Figure 28- a) Schematic representation of Essential BC used in simulation of fracture surface of length
2a in the center of a plate. b) Illustration of Symmetry Boundary Conditions.....................................90
Figure 29- GUI for definition of the fundamental Boundary Conditions in case it was selected: a)
Automatic input mode; and c) Manual input mode. b) Interface used to input half of the crack length.
.........................................................................................................................................................91
Figure 30- Graphic output of BaPMEF tool for: a) Default values; and b) Example of a 10x10 finite
element mesh....................................................................................................................................92
Figure 31- Graphic interface that allow the user to freely define the gravitational field and an additional
external field.....................................................................................................................................93
Figure 32- Graphic interface used to define the natural BC in the: a) Left edge, b) Right edge, c) Lower
edge, and d) Upper edge. The four windows appear sequentially after defining each edge. ................94
Figure 33- Graphic interface used to define the cartesian components of the surface traction acting on
the entire edge of the body. ...............................................................................................................94
Figure 34. Graphic interface used to define the surface traction per element. .....................................95
Figure 35- GUI used to define the point loads. ..................................................................................95
Figure 36- Example of the graphic representation of the nodal displacements after surface traction along
the upper edge in a cantilever beam...................................................................................................96
Figure 37- Sequential interface to choose which: a)-c) primary variables (displacements), and d)-i)
primary post-processing variable(s) to plot........................................................................................97
Figure 38- Sequential interface to choose which secondary post-processing variable(s) to plot. .........98
Figure 39- Sequential interface menu windows to choose which predefined example to plot..............98
Figure 40- Spectrum of plots for the displacements: a) Horizontal displacements in the x-direction; b)
Vertical displacements in the y-direction; c) Magnitude of the displacements. Spectrum of plots for the
Strains: d) Linear Strains in the x-direction; e) Linear Strains in the y-direction; f) Shear Strains in the
xy plane............................................................................................................................................99
Figure 41- Spectrum of plots for the Stresses: a) Normal Stresses in the x-direction; b) Normal Stresses
in the y-direction; c) Shear Stresses in the xy plane. Spectrum of plots for the secondary post-processing
variables: d) Von Mises Stresses; e) Safety Factor, f) Stress/Strain in z-direction.............................100
Figure 42- Schematic illustration of the problem too which the analytical solutions using plane elasticity
theory were developed. ...................................................................................................................101
Figure 43- a) Schematic illustration of the problem simulated, with the aim to model pure bending
state.in plane elasticity. Image adapted from [1]. b) Coordinate system used to compute the analytical
solution, in order to match the coordinate system of the FEA solver. ...............................................102
Figure 44- a) Deformed shape of the mesh from the beam under pure bending. b) Horizontal
displacements in the x-direction, determined by the BaPMEF FEA tool. c) Vertical displacements in the
y-direction, determined by the BaPMEF FEA tool. .........................................................................105

xi
Figure 45- Comparison of the horizontal displacements in the x-direction, determined by the BaPMEF
tool against the analytical solution, in: 3D plot a)-b), and in the 2D plot over the neutral axis c). .....106
Figure 46- Physical model of a Cantilever Beam loaded by a shear distributed load P in the left edge. a)
Original coordinate system of the analytical solution from [1]; b) Coordinate system adopted and used
in the FEA tool. ..............................................................................................................................107
Figure 47- a) Deformed shape of the mesh from the cantilever beam. b) Horizontal displacements in the
x-direction, determined by the BaPMEF FEA tool. c) Vertical displacements in the y-direction,
determined by the BaPMEF FEA tool. ............................................................................................110
Figure 48- Comparison of the horizontal displacements in the x-direction, determined by the BaPMEF
tool against the analytical solution in: 3D plot a)-b), and in the 2D plot over the neutral axis c). ......111
Figure 49- Comparison of the vertical displacements in the y-direction, determined by the BaPMEF tool
against the analytical solution in: 3D plot a)-b), and in the 2D plot over the neutral axis c). .............112
Figure 50- 2D Plot of the vertical displacements in the y-direction with a mesh: a) 1 x 2; b) 2 x 2; c) 4 x
2; d) 6 x 2. ......................................................................................................................................113
Figure 51- 2D Plot of the vertical displacements in the y-direction with a mesh: a) 8 x 2; b) 15 x 2; c)
15 x 4..............................................................................................................................................114
Figure 52- A ...................................................................................................................................115
Figure 53- Plot of the mesh 50x10 used to discretize the simple supported beam. ............................118
Figure 54- Plot of the deformed shape of the simple supported beam after uniform load in the upper
boundary.........................................................................................................................................119
Figure 55- a) Horizontal Displacements in x-direction. b) Vertical Displacements in y-direction. c)
Normal Stresses in x-direction.........................................................................................................119
Figure 56- a) Normal Stresses in x-direction. b) Normal Stresses in y-direction. c) Shear Stresses in xy
plane...............................................................................................................................................120
Figure 57- Comparison of the vertical displacements in the y-direction, determined by the BaPMEF tool
against the analytical solution in: 3D plot a)-b), and in the 2D plot over the neutral axis c). .............121
Figure 58- Comparison of the normal stresses in the x-direction, determined by the BaPMEF tool against
the analytical solution in: 3D plot a)-b), and in the 2D plot over the neutral axis c)..........................122
Figure 59- Comparison of the normal stresses in the y-direction, determined by the BaPMEF tool against
the analytical solution in: 3D plot a)-b), and in the 2D plot over the neutral axis c)..........................123
Figure 60- Comparison of the shear stresses in the xy plane, determined by the BaPMEF tool against
the analytical solution in: 3D plot a), and in the 2D plot over the neutral axis b). c) 3D plot of the Von
Mises Stresses.................................................................................................................................124
Figure 61- a) Infinite plate with a through crack in the center, loaded perpendicularly to the crack
direction. b) Geometry of the simulated problem by FEA. ...............................................................125
Figure 62- Graphic representation of Mesh#A, highlighting the mesh refinement control. ...............131
Figure 63- a) Plot of the Normal Stresses in the y-direction, and b)-c) different degrees of zoom near the
crack tip region. ..............................................................................................................................131
Figure 64- Comparison between the numeric results (achieved with mesh#A) and the analytical results
from different approximation solutions and the general analytical solution (iv): a) Normal Stress in the
y-direction near the crack tip. b) Vertical Displacement in the y-direction along the semi-crack length.
.......................................................................................................................................................132
Figure 65- Graphic representation of the Mesh#B, highlighting the local mesh refinement control...133
Figure 66- a) Zoom of the Normal Stresses in the y-direction, in the region near the crack tip. b) Vertical
displacements in the y-direction and c) a zoom near the center of the crack. ....................................133
Figure 67- Comparison between the numeric results (achieved with mesh#B) and the analytical results

xii
.......................................................................................................................................................134
Figure 68- Comparison between the numeric results (achieved with mesh#C) and the analytical results
.......................................................................................................................................................135
Figure 69- Comparison between the numeric results (achieved with mesh#D) and the analytical results
.......................................................................................................................................................137
Figure 70- Comparison between the numeric results (achieved with mesh#E) and the analytical results
.......................................................................................................................................................139
Figure 71- Schematic representation of the problem simulated in both Abaqus® FEA solver and
BaPMEF FEA tool..........................................................................................................................140
Figure 72- Plot of the finite element mesh 10 x 5 automatically created...........................................140
Figure 73- Graphic representation of the deformed mesh, computed by: a) FEA BaPMEF tool, and c)
Abaqus®. b) Illustration of the loading conditions and boundary conditions added to the Abaqus®
model. ............................................................................................................................................142
Figure 74- Horizontal displacements in x-direction, determined by: a) MATLAB® FEA tool; b)
Abaqus®. Vertical displacements in y-direction, determined by: c) MATLAB® FEA tool; d) Abaqus®.
.......................................................................................................................................................143
Figure 75- Magnitude of the displacements, determined by: a) MATLAB® FEA tool; b) Abaqus®.144
Figure 76- Linear Strains in the x-direction, determined by: a) MATLAB® FEA tool; b) Abaqus®.144
Figure 77- Linear Strains in the y-direction, determined by: a) MATLAB® FEA tool; b) Abaqus®.145
Figure 78- Shear Strains xy, determined by: a) MATLAB® FEA tool; b) Abaqus®. .......................145
Figure 79- Normal Stresses in the x-direction, determined by: a) MATLAB® FEA tool; b) Abaqus®.
.......................................................................................................................................................146
Figure 80- Normal Stresses in the y-direction, determined by: a) MATLAB® FEA tool; b) Abaqus®.
.......................................................................................................................................................146
Figure 81- Shear Stresses xy, determined by: a) MATLAB® FEA tool; b) Abaqus®.......................147
Figure 82- Von Mises Equivalent Stresses, determined by: a) MATLAB® FEA tool; b) Abaqus®..147
Figure 83- Normal Stress in z-direction, determined by: a) MATLAB® FEA tool; b) Abaqus®. .....148

xiii
List of Tables
Table 1- Summary of the most important and distinct mathematical nomenclature used throughout the
report................................................................................................................................................. 2
Table 2- Summary of all simplifications made to the general stiffness matrix. ...................................13
Table 3- Type of boundary-value problems for two-variable problems in 2D dimensions and the number
of possible combinations for the different boundary conditions..........................................................32
Table 4- Nomenclature used in the weak formulations.......................................................................32
Table 5- Modified Pascal’s triangle into a rectangular array abacus for Lagrange Quadrilateral Elements
[5].....................................................................................................................................................49
Table 6- Integration Gauss points and weight coefficients for both simple and double integration, up to
3 Gauss Points [6], [32], [35]. The total possible combinations of integration points that the natural
coordinates can assume is also detailed. ............................................................................................65
Table 7- Summary of 1D Gaussian Quadrature (easily extrapolated for 2D quadrature) for 4 and 5 Gauss
points [6],[32], [35]..........................................................................................................................65
Table 8- Gauss points (GP), weight coefficients, and possible combinations that the natural coordinates
can assume, for both simple and double integration, for 4 GP [6], [32], [35]......................................66
Table 9- Standard properties of the material used for finite element validation and comparison with
commercially available software [42]................................................................................................89
Table 10- Numerical data used in the analytical solution. ................................................................103
Table 11- Numerical data and other inputs of the FEM tool.............................................................103
Table 17- Unchanged numerical data and other inputs of the FEM tool. ..........................................127
Table 18- Several features for two different structured meshes with equally spaced elements. .........128
Table 19- Mesh properties of Mesh#A, introduced during the BaPMEF input routine. .....................129
Table 20- Mesh properties of Mesh#B, introduced during the BaPMEF input routine. .....................129
Table 21- Mesh properties of Mesh#C, introduced during the BaPMEF input routine. .....................130
Table 22- Mesh properties of Mesh#D, introduced during the BaPMEF input routine. .....................136
Table 23- Mesh properties of Mesh#E, introduced during the BaPMEF input routine. .....................138

2D Plane Elasticity: Isoparametric Bilinear Quadrilateral Lagrange type Element with 4 Nodes
1
1 Introduction
1.1 Context of the Report
This report was developed within the Finite Element Course, lectured in the Integrated Master
in Mechanical Engineering – Specialty Structural Engineering and Machine Design, at Faculty of
Engineering of University of Porto (FEUP). The first (but not necessarily major) goal of this report is
divided in: (i) formulate an isoparametric bilinear quadrilateral element of the Lagrange family; and (ii)
using the algorithm base of the BaPMEF (Base para Programação do Método dos Elementos Finitos)
MATLAB® script, implement and present the major changes and upgrades to the code and its potential
capabilities for simulating plane elasticity problems. However, the author was slightly beyond this task
and also sought to demonstrate the background behind some important features of finite element
discretization.
1.2 Report Structure
The present report is divided in 9 main chapters, being the last numbered chapter dedicated to
the conclusion. Chapter 2 is essentially theoretical, and can be seen as an extra topic that was exported
from any classic elasticity theory literature, but completely reformulated in order to demonstrate and
explain only the concepts fundamental to chapter 3 and necessary to really understand the Finite Element
Method. Thus, this chapter can be omitted if a more practical reading is desired, without risks of
misunderstanding the next chapters.
In chapter 3, first a brief summary of the formulae that govern the linear elastic behavior for 2D
problems is done. Then, with the concepts fresh and clear in the reader’s mind, the concepts of strong
and weak formulation are exposed and compared. In some FEM literature [4], the concept of strong and
weak form is derived generically (i.e. for specific and different finite elements such as bar elements,
triangular elements, etc.) and sometimes for problems different from solid mechanics (e.g. heat transfer
field). Thus, in order to better understand the FEM background, the author:
• Derived the final strong form of a 2D plane elasticity problem, which governs the mechanical
behavior of any plane geometry, and theoretically allows to compute the continuous
displacement field (only viable and practicable for simple geometries and boundary conditions);
• Derived the weak form of the system of coupled partial differential equations, using different
principles from solid mechanics and dynamics. Which, gives the reader different perspectives
of the physical and mathematical meaning of weak form or weak formulation.
Chapter 4, along with chapter 5 can be considered to be more closely related to the FEM
formulation in practical terms. In the first mentioned chapter, the formulae and relation used in the
discretizing process with the Isoparametric Quadrilateral bilinear Lagrange element were demonstrated
and summarized. The numerical integration additional subchapter was added since it helps to make the
bridge between chapter 4 and chapter 5.
The goal of chapter 5 is to merge all the specific information detailed in chapter 4 (regarding
the finite element used); with the weak form (ready to be discretized in finite domains) derived by last
in chapter 3.
Chapter 6 consists of a bullet list with all the modifications and changes added to the original
BaPMEF script. The major upgrades detailed can be summarized as:
• Pre-processing step – illustration of the interface created to easily introduce the input data by
user. And elucidation of the mesh generation capabilities and mesh controls;
• Processing – exposition of the major changes in the global stiffness matrix and global
equivalent nodal forces;
• Post-processing capabilities – illustration of the developed graphic representation capabilities
(3D surfaces and/or color-plots for: displacements, strains, stresses) and the computation of the

2
post-processing variables (strains or stresses in the z-direction, Von Mises equivalent stress,
and safety factor);
During Chapter 7, the formulated element and implemented code will be tested and validated.
For this, the coded FEA tool was run in academic problems of plane elasticity. The numerical solution
achieved, was compared with the known analytical solutions of the problem. The geometry and loading
conditions tested were simple (to allow analytical solutions) and their goal different from the next
chapter.
In the final chapter 8, some applications of the developed FEA tool were detailed. The main
difference between this chapter and the previous one, is that the physical problems run have no analytical
solution, or are outside the Solid Mechanics field. The chapter is divided in the following subchapters:
• Application 8.1 – Widen the spectrum of application, changing from the classic Solid
mechanics, to the field of Fracture Mechanics. Introducing to mesh control features and
study the effect of mesh refinement;
• Applications 8.2.1 – Problems without analytical solution and comparison with commercially
available FEA software (Abaqus)
1.3 Basic Mathematical Nomenclature
In order to ease the understanding of the (sometimes heavy) mathematical treatment, the author
slightly drifted away from the nomenclature usually seen in technical FEM classic literature [4], [5], [6],
[7], [8]. The nomenclature used was similar to the one adopted in the Kinematics and Dynamics course,
lectured at FEUP, and considered by the author more intuitive. Thus, in order to avoid
misunderstandings, Table 1 details the most relevant nomenclature adopted. This only concerns generic
nomenclature; each variable and symbol will be defined whenever necessary and convenient.
Table 1- Summary of the most important and distinct mathematical nomenclature used throughout the report.
| | Column Vector
| | 𝑇 Row Vector
[ ]
Matrix of any general dimension, with the exception of a
column vector
det() Determinant of a square matrix
∬ ( ) 𝑑𝐴
𝐴
= ∫ ( ) 𝑑𝐴
𝐴
Double Integral over a generic Area (A)
∭ ( ) 𝑑𝑉
𝑉
= ∫ ( ) 𝑑𝑉
𝑉
Triple Integral over a generic Volume (V)
∯ ( ) 𝑑𝑆
𝑆
= ∮ ( ) 𝑑𝑆
𝑆
Surface Integral over a generic surface (S)
∮ ()
𝑙
𝑑𝑠 Line Integral over a generic curve (l)
[ 𝐶 ] Stiffness tensor (or matrix) whose terms are material properties
[ 𝐾 ]
Stiffness matrix whose terms are structure/element properties
(depending on the geometry and material)

3
2 Theory of Linear Elasticity for Continuum Medium
2.1 Introduction
The linear elastic theory tries to model the mechanical behavior of continuum linear elastic
solids. And until the current century as proven its potential in a variety of engineering problems.
However, its usability lies on the capacity of assuming proper simplifications [9]
In this chapter, the basic constitutive equations for 2D linear elasticity will be derived. The
equations here demonstrated, are fundamental and will be directly used for the formulation of the finite
element. Thus, this chapter can be considered as a literature review section. And, if the reader already
masters the basic concepts of linear elasticity, it can skip directly to chapter 3.
The approach followed is similar to the one typically carried in solid mechanics or strength of
materials classic literature. Basic concepts (valid for generic 3D anisotropic behavior) are progressively
simplified and particularized aiming the physical or engineering application in hands, in this case, the
2D problem constitutive equations. The major difference might be the depth of study. The starting point
was the formulation of the stress and strain tensor in their generic form (considering already the linear
elastic assumptions). After deriving the two second order tensors, and underlining their assumptions,
the relation between the two was considered. Videlicet, the generalized Hooke’s Law was stated and
explored. Supported in concepts previously discussed, and some referred within the last subchapter, the
Generalized Hooke’s Law will be continuously simplified until reaching the most often used and refined
formula in 2D linear elasticity. The equations of motion will first be presented within the stress tensor
definition subchapter. However, later it will be dedicated a specific section for 2D dynamic equilibrium.
2.2 Stress Tensor
In terms of continuum mechanics, anisotropic materials are materials that have different
mechanical properties depending on the direction of measurement. Concerning the mechanical behavior,
only the stiffness moduli and limit elastic stress parameters will be relevant. Concerning others fields of
interest, the anisotropy concept can be generalized, and we end up with anisotropy throughout the solid
relating to: thermal conductivity, magnetic permeability, refraction index, etc. [10].
From the solid mechanics of homogeneous materials1
[10], the tension matrix is a second order
tensor with 3x3 dimension. This second order Cartesian tensor is also called the Cauchy Stress Tensor
and has the form [11]:
[ 𝜎 ] = [
𝜎𝑥𝑥 𝜏 𝑥𝑦 𝜏 𝑥𝑧
𝜏 𝑦𝑥 𝜎 𝑦𝑦 𝜏 𝑦𝑧
𝜏 𝑧𝑥 𝜏 𝑧𝑦 𝜎𝑧𝑧
] ( 2.1 )
The nomenclature adopted in the definition of the stresses, is illustrated in Figure 1. In index
notation, the stress ( )𝑖𝑗 corresponds to the stress component acting in the j-direction, on a surface or
plane normal to i-direction. In other words, the first subscript refers to the plane in which the stress acts;
and the second subscript the direction about which the stress acts. Regarding the algebraic value, the
positive sign will be left for tension stresses and the negative for compression stresses.
1
Homogeneous materials are materials in which the mechanical properties of any given point are
equal to the specific properties of the solid. In other words, macroscopically, the specific properties are
independent of the point of analysis [10].

4
The previous tensor shown in equation ( 2.1 ) has 9 terms; however, it can be shown that only
6 of them are independent. The stress matrix is symmetric to its main diagonal, and the symmetry
conditions or relations are also called the reciprocity property of the stress tensor. The symmetry
relations can be derived by the following principles or Cauchy Equations of Motion [1]:
• According to the principle of conservation of linear momentum, if the continuum body is in
static equilibrium it can be demonstrated that the components of the Cauchy stress tensor in
every material point in the body satisfies the linear equilibrium equation (equation of motion
for null acceleration)2
.
[ 𝜎 ] ∇ + | 𝑓 | = | 𝑎 | = | 0 | ⇒ ( 2.2 )
[
]
[
𝜕
𝜕𝑥
𝜕
𝜕𝑦
𝜕
𝜕𝑥 ]
𝜌𝑑𝑉 + |
𝑓𝑥
𝑓𝑦
𝑓𝑧
| 𝜌𝑑𝑉 = |
𝑎 𝑥
𝑎 𝑦
𝑎 𝑧
| 𝜌𝑑𝑉 = |
0
0
0
| ( 2.3 )
Or making explicit each component of the vector equation comes:
(
𝜕𝜎𝑥𝑥
𝜕𝑥
+
𝜕𝜏 𝑥𝑦
𝜕𝑦
+
𝜕𝜏 𝑥𝑧
𝜕𝑧
) + 𝑓𝑥 = 𝜌 ∙ 𝑎 𝑥 = 𝜌 ∙
𝜕2
𝜕𝑡2
𝑢(𝑥, 𝑦, 𝑧) = 0 ( 2.4 )
(
𝜕𝜏 𝑦𝑥
𝜕𝑥
+
𝜕𝜎 𝑦𝑦
𝜕𝑦
+
𝜕𝜏 𝑦𝑧
𝜕𝑧
) + 𝑓𝑦 = 𝜌 ∙ 𝑎 𝑦 = 𝜌 ∙
𝜕2
𝜕𝑡2
𝑣(𝑥, 𝑦, 𝑧) = 0 ( 2.5 )
(
𝜕𝜏 𝑧𝑥
𝜕𝑥
+
𝜕𝜏 𝑧𝑦
𝜕𝑦
+
𝜕𝜎𝑧𝑧
𝜕𝑧
) + 𝑓𝑧 = 𝜌 ∙ 𝑎 𝑧 = 𝜌 ∙
𝜕2
𝜕𝑡2
𝑤(𝑥, 𝑦, 𝑧) = 0 ( 2.6 )
𝑎 Total acceleration = local acceleration + convective acceleration
𝑓𝑥, 𝑓𝑦, 𝑓𝑧 Volume forces acting on the x, y, and z direction respectively
𝑑𝑉 Differential of Volume, 𝑑𝑉 = 𝑑𝑥𝑑𝑦𝑑𝑧
2
The Cauchy Equation for the Conservation of Linear Momentum will be important in the formulation of the finite
element.
𝜏 𝑦𝑥
𝜏 𝑥𝑦
𝑦
𝑥𝜏 𝑦𝑥
𝜏 𝑥𝑦
𝜏 𝑧𝑥
𝜏 𝑥𝑧
𝑧
𝑥𝜏 𝑧𝑥
𝜏 𝑥𝑧
𝜏 𝑧𝑦
𝜏 𝑦𝑧
𝑧
𝑦𝜏 𝑧𝑦
𝜏 𝑦𝑧
Figure 1- Definition of the nomenclature adopted for shear stresses acting on the differential volume element [1].

5
• According to the analogous principle regarding the conservation of angular momentum, the
angular equilibrium requires that the summation of moments with respect to an arbitrary axis is
null. Analytically it can be written:
[(𝜏 𝑦𝑧 +
𝜕𝜏 𝑦𝑧
𝜕𝑦
𝑑𝑦
2
) + (𝜏 𝑦𝑧 −
𝜕𝜏 𝑦𝑧
𝜕𝑦
𝑑𝑦
2
) − (𝜏 𝑧𝑦 +
𝜕𝜏 𝑧𝑦
𝜕𝑧
𝑑𝑧
2
)
− (𝜏 𝑧𝑦 −
𝜕𝜏 𝑧𝑦
𝜕𝑧
𝑑𝑧
2
)]
𝑑𝑥𝑑𝑦𝑑𝑧
2
= 0
( 2.7 )
[− (𝜏 𝑥𝑧 +
𝜕𝜏 𝑥𝑧
𝜕𝑥
𝑑𝑥
2
) − (𝜏 𝑥𝑧 −
𝜕𝜏 𝑥𝑧
𝜕𝑥
𝑑𝑥
2
) + (𝜏 𝑧𝑥 +
𝜕𝜏 𝑧𝑥
𝜕𝑧
𝑑𝑧
2
)
+ (𝜏 𝑧𝑥 −
𝜕𝜏 𝑧𝑥
𝜕𝑧
𝑑𝑧
2
)]
2
= 0
( 2.8 )
[(𝜏 𝑥𝑦 +
𝜕𝜏 𝑥𝑦
𝜕𝑥
𝑑𝑥
2
) + (𝜏 𝑥𝑦 −
𝜕𝜏 𝑥𝑦
𝜕𝑥
𝑑𝑥
2
) − (𝜏 𝑦𝑥 +
𝜕𝜏 𝑦𝑥
𝜕𝑦
𝑑𝑦
2
)
− (𝜏 𝑦𝑥 −
𝜕𝜏 𝑦𝑥
𝜕𝑦
𝑑𝑦
2
)]
2
= 0
( 2.9 )
The vector equilibrium equation will degenerate in the symmetry relations. They can now be
easily obtained by just solving the three angular momentum equilibrium equations. The final relations
are:
𝜏 𝑦𝑧 = 𝜏 𝑧𝑦
𝜏 𝑥𝑧 = 𝜏 𝑧𝑥
𝜏 𝑥𝑦 = 𝜏 𝑦𝑥
( 2.10 )
From equation ( 2.1 ) and ( 2.10 ) we can finally write:
[ 𝜎 ] = [
] = [
𝜏 𝑥𝑦 𝜎 𝑦𝑦 𝜏 𝑦𝑧
𝜏 𝑥𝑧 𝜏 𝑦𝑧 𝜎𝑧𝑧
] = [
𝜎 𝑥𝑥 𝜏 𝑥𝑦 𝜏 𝑥𝑧
… 𝜎 𝑦𝑦 𝜏 𝑦𝑧
… … 𝜎𝑧𝑧
] ( 2.11 )
As indexed in the definition of second order tensor, equation ( 2.1 ) encloses the cartesian
components for a surface perpendicular to each one of the cartesian coordinate axis, as detailed in the
following equation:
[ 𝜎 ] = [
] = [
| 𝑇 𝑒 𝑥 | 𝑇
| 𝑇 𝑒 𝑦 | 𝑇
| 𝑇 𝑒 𝑧 | 𝑇
] ( 2.12 )
Where:
| 𝑇 𝑒 𝑥 | Stress vector acting on plane normal to x-direction
| 𝑇 𝑒 𝑦 | Stress vector acting on plane normal to y-direction
| 𝑇 𝑒 𝑧 | Stress vector acting on plane normal to z-direction
In a similar manner, the Cauchy Equation [1], allows to compute the resulting stress vector,
perpendicular to any arbitrary plane, acting on a generic point of coordinates (x,y,z). The Cauchy relation

6
can be given in two matrix forms, a condensed and a more explicit form. The two are respectively given
by:
| 𝑇 | = [ 𝜎 ] 𝑇 | 𝑛 | ⇒ | 𝑇 | = [
| 𝑇 𝑒 𝑥 | 𝑇
| 𝑇 𝑒 𝑦 | 𝑇
| 𝑇 𝑒 𝑧 | 𝑇
]
𝑇
| 𝑛 | ( 2.13 )
|
𝑇𝑥
𝑇𝑦
𝑇𝑧
| = [
]
𝑇
|
𝑛 𝑥
𝑛 𝑦
𝑛 𝑧
| = [
𝜎𝑥𝑥 𝜏 𝑦𝑥 𝜏 𝑥𝑧
𝜏 𝑥𝑦 𝜎 𝑦𝑦 𝜏 𝑧𝑦
] |
𝑛 𝑥
𝑛 𝑦
𝑛 𝑧
| ( 2.14 )
Where:
| 𝑛 | Vector of the direction cosines perpendicular to an arbitrary plane
[ 𝜎 ] Stress tensor matrix
| 𝑇 | Stress vector acting on a plane with normal unit vector | 𝑛|
Or considering the symmetry stated in the final equation ( 2.11 ), by the properties of the transposition
operation of a matrix it results:
[
]
𝑇
= [
]
𝑇
= [
] ( 2.15 )
|
𝑇𝑥
𝑇𝑦
𝑇𝑧
| = [
]
𝑇
|
𝑛 𝑥
𝑛 𝑦
𝑛 𝑧
| = [
] |
𝑛 𝑥
𝑛 𝑦
𝑛 𝑧
|
( 2.16 )
The Cauchy equation can be usually demonstrated by writing the static equilibrium equations:
(i) for an infinitesimal interior tetrahedron element of a linear elastic body - in the case of 3D general
case; (ii) or for an infinitesimal triangle - in the case of 2D particular case. Figure 2 illustrates both cases.
z
x
y𝑑𝐴 𝑦
𝑑𝐴 𝑥
𝑑𝐴 𝑧
−𝑇 𝑒 𝑧
−𝑇 𝑒 𝑥
−𝑇 𝑒 𝑦
𝑇
𝑑𝑚 = 𝜌𝑑𝑉
a) b)
Figure 2- a) Cauchy tetrahedron formed by slicing a parallelepiped along an arbitrary plane define by the
normal vector | 𝑛|. b) Infinitesimal triangular portion of a generic 2D body.
𝑑𝛤
𝑑𝑥
𝑑𝑦
𝜏 𝑥𝑦
𝜏 𝑦𝑥
y
x
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝑛 𝑦
𝑛 𝑥
𝑛⃗ 𝑇

7
Regarding the 3D general case:
• By basic analytical geometry it is possible to derive the following relations between the
infinitesimal quantities [12]:
{
𝑑𝐴 𝑥 = 𝑑𝐴 𝑛 𝑥
𝑑𝐴 𝑦 = 𝑑𝐴 𝑛 𝑦
𝑑𝐴 𝑧 = 𝑑𝐴 𝑛 𝑧
⇒
{
𝑛 𝑥 =
𝑑𝐴 𝑥
𝑑𝐴
𝑛 𝑦 =
𝑑𝐴 𝑦
𝑑𝐴
𝑛 𝑧 =
𝑑𝐴 𝑧
𝑑𝐴
( 2.17 )
• Verifying the Static Equilibrium condition comes:
{
∑ 𝐹𝑥 = 0
∑ 𝐹𝑦 = 0
∑ 𝐹𝑧 = 0
⇒ {
−𝜎𝑥𝑥 𝑑𝐴 𝑥 − 𝜏 𝑦𝑥 𝑑𝐴 𝑦 − 𝜏 𝑧𝑥 𝑑𝐴 𝑧 + 𝑇𝑥 𝑑𝐴 = 0
−𝜏 𝑥𝑦 𝑑𝐴 𝑥 − 𝜎 𝑦𝑦 𝑑𝐴 𝑦 − 𝜏 𝑧𝑦 𝑑𝐴 𝑧 + 𝑇𝑦 𝑑𝐴 = 0
−𝜏 𝑥𝑧 𝑑𝐴 𝑥 − 𝜏 𝑦𝑧 𝑑𝐴 𝑦 − 𝜎𝑧𝑧 𝑑𝐴 𝑧 + 𝑇𝑧 𝑑𝐴 = 0
( 2.18 )
• Dividing both members of each equation by the area of the arbitrarily inclined surface ( dA ):
{
−𝜎𝑥𝑥
𝑑𝐴 𝑥
𝑑𝐴
− 𝜏 𝑦𝑥
𝑑𝐴 𝑦
𝑑𝐴
− 𝜏 𝑧𝑥
𝑑𝐴 𝑧
𝑑𝐴
+ 𝑇𝑥 = 0
−𝜏 𝑥𝑦
𝑑𝐴 𝑥
𝑑𝐴
− 𝜎 𝑦𝑦
𝑑𝐴 𝑦
𝑑𝐴
− 𝜏 𝑧𝑦
𝐴 𝑧
𝑑𝐴
+ 𝑇𝑦 = 0
−𝜏 𝑥𝑧
𝑑𝐴 𝑥
𝑑𝐴
− 𝜏 𝑦𝑧
𝑑𝐴 𝑦
𝑑𝐴
− 𝜎𝑧𝑧
𝑑𝐴 𝑧
𝑑𝐴
+ 𝑇𝑧 = 0
( 2.19 )
• By the relations between the infinitesimals, equation ( 2.17 ), and manipulating the terms comes:
{
−𝜎𝑥𝑥 𝑛 𝑥 − 𝜏 𝑦𝑥 𝑛 𝑦 − 𝜏 𝑧𝑥 𝑛 𝑧 + 𝑇𝑥 = 0
−𝜏 𝑥𝑦 𝑛 𝑥 − 𝜎 𝑦𝑦 𝑛 𝑦 − 𝜏 𝑧𝑦 𝑛 𝑧 + 𝑇𝑦 = 0
−𝜏 𝑥𝑧 𝑛 𝑥 − 𝜏 𝑦𝑧 𝑛 𝑦 − 𝜎𝑧𝑧 𝑛 𝑧 + 𝑇𝑧 = 0
⇒ {
𝑇𝑥 = 𝜎𝑥𝑥 𝑛 𝑥 + 𝜏 𝑦𝑥 𝑛 𝑦 + 𝜏 𝑧𝑥 𝑛 𝑧
𝑇𝑦 = 𝜏 𝑥𝑦 𝑛 𝑥 + 𝜎 𝑦𝑦 𝑛 𝑦 + 𝜏 𝑧𝑦 𝑛 𝑧
𝑇𝑧 = 𝜏 𝑥𝑧 𝑛 𝑥 + 𝜏 𝑦𝑧 𝑛 𝑦 + 𝜎𝑧𝑧 𝑛 𝑧
( 2.20 )
• In the matrix form comes:
|
𝑇𝑥
𝑇𝑦
𝑇𝑧
| = [
𝜎𝑥𝑥 𝜏 𝑦𝑥 𝜏 𝑧𝑥
𝜏 𝑥𝑦 𝜎 𝑦𝑦 𝜏 𝑧𝑦
] |
𝑛 𝑥
𝑛 𝑦
𝑛 𝑧
| = [
]
𝑇
|
𝑛 𝑥
𝑛 𝑦
𝑛 𝑧
| ( 2.21 )
Or regarding the 2D case:
• The previous relations between the infinitesimals come:
{
𝑑𝐴 𝑥 = 𝑑𝐴 𝑛 𝑥
𝑑𝐴 𝑦 = 𝑑𝐴 𝑛 𝑦
⇒ {
𝑑𝑦𝑑𝑧 = 𝑑𝛤𝑑𝑧 𝑛 𝑥
𝑑𝑥𝑑𝑧 = 𝑑𝛤𝑑𝑧 𝑛 𝑦
⇒ {
𝑑𝑥 = 𝑑𝛤 𝑛 𝑥
𝑑𝑦 = 𝑑𝛤 𝑛 𝑦
⇒
{
𝑛 𝑥 =
𝑑𝑦
𝑑𝛤
𝑛 𝑦 =
𝑑𝑥
𝑑𝛤
( 2.22 )

8
• Verifying the Static Equilibrium condition comes:
{
∑ 𝐹𝑥 = 0
∑ 𝐹𝑦 = 0
⇒ {
−𝜎𝑥𝑥 𝑑𝑦 − 𝜏 𝑦𝑥 𝑑𝑥 + 𝑇𝑥 𝑑𝛤 = 0
−𝜎 𝑦𝑦 𝑑𝑥 − 𝜏 𝑥𝑦 𝑑𝑦 + 𝑇𝑦 𝑑𝛤 = 0
( 2.23 )
• Dividing both members of each equation by the length of the arbitrarily inclined surface ( dΓ ):
{
−𝜎𝑥𝑥
𝑑𝑦
𝑑𝛤
− 𝜏 𝑦𝑥
𝑑𝑥
𝑑𝛤
+ 𝑇𝑥 = 0
−𝜎 𝑦𝑦
𝑑𝑥
𝑑𝛤
− 𝜏 𝑥𝑦
𝑑𝑦
𝑑𝛤
+ 𝑇𝑦 = 0
( 2.24 )
• By the relations between the infinitesimals, equation ( 2.22 ), and manipulating the terms comes:
{
−𝜎𝑥𝑥 𝑛 𝑥 − 𝜏 𝑦𝑥 𝑛 𝑦 + 𝑇𝑥 = 0
−𝜎 𝑦𝑦 𝑛 𝑦 − 𝜏 𝑥𝑦 𝑛 𝑥 + 𝑇𝑦 = 0
⇒ {
𝑇𝑥 = 𝜎 𝑥𝑥 𝑛 𝑥 + 𝜏 𝑦𝑥 𝑛 𝑦
𝑇𝑦 = 𝜏 𝑥𝑦 𝑛 𝑥 + 𝜎 𝑦𝑦 𝑛 𝑥
( 2.25 )
• In the matrix form comes:
|
𝑇𝑥
𝑇𝑦
| = [
𝜎𝑥𝑥 𝜏 𝑦𝑥
𝜏 𝑥𝑦 𝜎 𝑦𝑦
] |
𝑛 𝑥
𝑛 𝑦
| = [
𝜎𝑥𝑥 𝜏 𝑥𝑦
𝜏 𝑦𝑥 𝜎 𝑦𝑦
]
𝑇
|
𝑛 𝑥
𝑛 𝑦
| ( 2.26 )
2.3 Strain Tensor
The magnitude of the strains and displacements (linear displacements or rotations) can influence
the mathematical definition of strain. The main theories applied to the continuum mechanics are [13],
[14]:
• Small Strains and small Displacements/rotations theory or infinitesimal strain theory– used to
solve most practical engineering problems that deal with common materials like wood, steel and
other alloys;
• Small Strains and large Displacements theory – essential to model materials and structures that
can withstand large displacements without entering the plastic domain, i.e. remaining elastic;
• Finite Strains and Displacements theory – necessary to model structures and materials where
the deformed and undeformed configuration is significantly different. These arbitrarily large
strains and displacements (linear or angular) can occur in materials with the mechanical
behavior of elastomers, fluids, biological (or not) soft tissues.
For small strains and small displacements (both linear and angular) the change in the geometry
and constitutive properties of the structure, due to deformation, doesn’t need to be considered after the
force is applied. In other words, physical and mechanical properties of the material e.g. density, stiffness,
etc. at each point of the infinitesimally deformed solid, can be assumed constant [10]. This definition of
strain is also designed by Cauchy strains, and it will be the strain concept used throughout the report.
The strain tensor or Cauchy strain tensor is also a second order tensor, and its 3x3 matrix is given by:
[ 𝜀 ] = [
𝜀 𝑥𝑥 𝜀 𝑥𝑦 𝜀 𝑥𝑧
𝜀 𝑦𝑥 𝜀 𝑦𝑦 𝜀 𝑦𝑧
𝜀 𝑧𝑥 𝜀 𝑧𝑦 𝜀 𝑧𝑧
] ( 2.27 )

9
The nomenclature adopted in the definition of the strains is rather different from the stress
nomenclature. In index notation, the strain term ( )𝑖𝑗 means: when 𝑖 = 𝑗 , the term corresponds to
the extension along the 𝑖-direction; when 𝑖 ≠ 𝑗 , the term of the strain matrix corresponds to the rotation
about the ij plane. Regarding its algebraic value, as schematized in Figure 3, the positive sign will be
ascribed when the angle between the two faces of the conceptual parallelogram is reduced, and the
negative sign when the angle increases.
The geometric definition of strains is demonstrated and detailed in [11], [1]. The linear strain
(also designated by longitudinal strain, linear deformation, extension, etc.) is quantified by the on-
diagonal matrix components 𝜀 𝑥𝑥 , 𝜀 𝑦𝑦 , 𝜀 𝑧𝑧 . The remaining non-diagonal terms correspond to the
angular strain (also designated by shear strain, angular deformation, distortion, etc.). The relation of
each term of the strain tensor, with the displacement field is given by [1]:
𝜀 𝑥𝑥 =
𝜕𝑢
𝜕𝑥
; 𝜀 𝑦𝑦 =
𝜕𝑣
𝜕𝑦
; 𝜀 𝑧𝑧 =
𝜕𝑤
𝜕𝑧
( 2.28 )
𝜀 𝑥𝑦 = 𝜀 𝑦𝑥 =
1
2
(
𝜕𝑢
𝜕𝑦
+
𝜕𝑣
𝜕𝑥
) ; 𝜀 𝑦𝑧 = 𝜀 𝑧𝑦 =
1
2
(
𝜕𝑣
𝜕𝑧
+
𝜕𝑤
𝜕𝑦
) ; 𝜀 𝑥𝑧 = 𝜀 𝑧𝑥 =
1
2
(
𝜕𝑢
𝜕𝑧
+
𝜕𝑤
𝜕𝑥
) ( 2.29 )
The geometric relation between strain and displacements can also be written in matrix form as:
| 𝜀 | =
|
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝜀 𝑥𝑦
𝜀 𝑦𝑧
𝜀 𝑥𝑧
|
|
|
=
[
𝜕
𝜕𝑥
0 0
0
𝜕
𝜕𝑦
0
0 0
𝜕
𝜕𝑧
1
2
𝜕
𝜕𝑦
1
2
𝜕
𝜕𝑥
0
0
1
2
𝜕
𝜕𝑧
1
2
𝜕
𝜕𝑦
1
2
𝜕
𝜕𝑧
0
1
2
𝜕
𝜕𝑥 ]
|
𝑢(𝑥, 𝑦, 𝑧)
𝑣( 𝑥, 𝑦, 𝑧)
𝑤( 𝑥, 𝑦, 𝑧)
| ( 2.30 )
Other main contrast regarding the stress tensor and strain tensor, is the difference between
tensorial and engineering strain for angular distortion. The angular distortion can be quantified in terms
of engineering shear strain (also called global strain), or tensorial shear strain. The engineering shear
strain can be considered as the total rotation of the 2D cartesian element subjected to shear stresses or
the total change of the original angle formed by the undeformed element; whereas the tensorial shear
strain can be understood as the average of the two displacements or the amount that each edge rotates
in average. This difference is illustrated in Figure 3, and the two are related by the following vector
equation [11]:
|
|
|
𝛾𝑥𝑦
𝛾𝑦𝑥
𝛾𝑦𝑧
𝛾𝑧𝑦
𝛾𝑥𝑧
𝛾𝑧𝑥
|
|
|
=
|
|
|
2𝜀 𝑥𝑦
2𝜀 𝑦𝑥
2𝜀 𝑦𝑧
2𝜀 𝑧𝑦
2𝜀 𝑥𝑧
2𝜀 𝑧𝑥
|
|
|
( 2.31 )

10
Their importance arises from the convenience of replacing the general symmetry of the stiffness
matrix (after continuous simplifications), as it will be explored in the next subchapter (see Page 12). In
the matrix form, the previous relations can be written as:
[ 𝜀 ] = [
] =
1
2
[
2𝜀 𝑥𝑥 𝛾𝑥𝑦 𝛾𝑥𝑧
𝛾𝑦𝑥 2𝜀 𝑦𝑦 𝛾𝑦𝑧
𝛾𝑧𝑥 𝛾𝑧𝑦 2𝜀 𝑧𝑧
] ( 2.32 )
The properties of a tensor won’t be remembered in this report [10]; however, it is always worth
notice that the following matrix is not a tensor!!
[
𝜀 𝑥𝑥 𝛾𝑥𝑦 𝛾𝑥𝑧
𝛾𝑦𝑥 𝜀 𝑦𝑦 𝛾𝑦𝑧
𝛾𝑧𝑥 𝛾𝑧𝑦 𝜀 𝑧𝑧
] ( 2.33 )
The symmetry property for the strain tensor matrix is derived meticulously in [11]. By the
displacement field geometric definition, and neglecting the second order terms (for small strains and
displacements, both linear and angular) it’s possible to verify the strain tensor symmetry. The symmetry
relations relating the shear distortion come:
𝛾𝑦𝑧 = 𝛾𝑧𝑦
𝛾𝑥𝑧 = 𝛾𝑧𝑥
𝛾𝑥𝑦 = 𝛾𝑦𝑥
( 2.34 )
From equation ( 2.27 ), ( 2.32 ) and ( 2.34 ) it is possible to finally write the strain tensor in
tensorial strains or engineering strains as:
[ 𝜀 ] = [
] = [
𝜀 𝑥𝑦 𝜀 𝑦𝑦 𝜀 𝑦𝑧
𝜀 𝑥𝑧 𝜀 𝑦𝑧 𝜀 𝑧𝑧
] = [
… 𝜀 𝑦𝑦 𝜀 𝑦𝑧
… … 𝜀 𝑧𝑧
] ( 2.35 )
[ 𝜀 ] =
1
2
[
𝛾𝑦𝑥 2𝜀 𝑦𝑦 𝛾𝑦𝑧
𝛾𝑧𝑥 𝛾𝑧𝑦 2𝜀 𝑧𝑧
] =
1
2
[
𝛾𝑥𝑦 2𝜀 𝑦𝑦 𝛾𝑦𝑧
𝛾𝑥𝑧 𝛾𝑦𝑧 2𝜀 𝑧𝑧
] =
1
2
[
… 2𝜀 𝑦𝑦 𝛾𝑦𝑧
… … 2𝜀 𝑧𝑧
] ( 2.36 )
Figure 3- Nomenclature adopted for the shear stress definition, for the distortion of the differential Cartesian
element.
𝑦 𝜏 𝑥𝑦
𝜏 𝑥𝑦
𝜕𝑢
𝜕𝑦
𝑥
𝜕𝑣
𝜕𝑥
𝑦
𝑥
𝛾 =
𝜕𝑢
𝜕𝑦
+
𝜕𝑣
𝜕𝑥
𝛾/2
𝑦
𝑥
𝛾 =
𝜕𝑢
𝜕𝑦
+
𝜕𝑣
𝜕𝑥𝛾/2

11
2.4 Generalized Hooke’s Law
Cauchy Elastic Materials or Simple Elastic Materials are materials for which the stress at a given
point is just function of the instantaneous strain. In other words, the stresses don’t depend of the strain
path, strain history, strain rate, and the time taken to achieve a given deformation field [15]. Cauchy
materials theoretical definition also implies:
• Homogeneous materials – the constitutive properties are independent of the point of analysis,
i.e. the terms of the stiffness matrix are not point functions;
• Temperature effect is ignored – even if there are thermal strains and/or residual stresses, the
effect of the temperature change in the properties of the material is neglected.
Assuming the previous hypothesis, the stress second order tensor is related by a second order-
valued function with the strain second order tensor as follows:
[ 𝜎 ] = 𝑓 ( [ 𝜀 ] ) ( 2.37 )
Considering that the stresses are a linear and homogeneous combination or function of the
strains, the contribution factors are in fact the elastic coefficients that characterize the mechanical
behavior of the material, i.e. are a property of the material. Historically the British engineer Robert
Hooke was the first to study this linear relation between the stress and strain [1]. That’s why the
generalize relationship of anisotropic materials - for spatial or triaxial stresses and strains - is called
Generalize Hooke’s Law. It’s a constitutive model for infinitesimal deformation of a linear elastic
material, in which the relation between stress and strains is model by a 4th
order tensor that linearly maps
between second-order tensors [14].
The elasticity tensor will result in a 9x9 elastic coefficient matrix. Hooke’s law can be presented:
in terms of a stiffness tensor or matrix ([ 𝐶 ]), putting in evidence the stress; or in terms of compliance
tensor or matrix ([ 𝑆 ]), in which the response function linking strain to the deforming stress is the
compliance tensor of the material. The matrix form of Hooke’s Law can be written as:
| 𝜎 | = [ 𝐶 ] | 𝜀 | = [ 𝐷 ] | 𝜀 | ( 2.38 )
| 𝜀 | = [ 𝑆 ] | 𝜎 | ( 2.39 )
Or explicitly as:
|
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑦𝑧
𝜏 𝑥𝑧
𝜏 𝑥𝑦
𝜏 𝑧𝑦
𝜏 𝑧𝑥
𝜏 𝑦𝑥
|
|
|
=
[
𝐶 𝑥𝑥𝑥𝑥 𝐶 𝑥𝑥 𝑦𝑦 𝐶 𝑥𝑥 𝑧𝑧 𝐶 𝑥𝑥 𝑥𝑦 𝐶 𝑥𝑥 𝑦𝑧 𝐶 𝑥𝑥 𝑥𝑧 𝐶 𝑥𝑥 𝑦𝑥 𝐶 𝑥𝑥 𝑧𝑦 𝐶 𝑥𝑥 𝑧𝑥
𝐶 𝑦𝑦 𝑥𝑥 ⋱ ⋮
𝐶𝑧𝑧 𝑥𝑥 ⋱ ⋮
𝐶 𝑦𝑧 𝑥𝑥 ⋱ ⋮
𝐶 𝑥𝑧 𝑥𝑥 ⋱ ⋮
𝐶 𝑥𝑦 𝑥𝑥 ⋱ ⋮
𝐶𝑧𝑦 𝑥𝑥 ⋱ ⋮
𝐶𝑧𝑥 𝑥𝑥 ⋱ ⋮
𝐶 𝑦𝑥 𝑥𝑥 … … … … … … … 𝐶 𝑦𝑥 𝑦𝑥 ]
|
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝜀 𝑦𝑧
𝜀 𝑥𝑧
𝜀 𝑥𝑦
𝜀 𝑧𝑦
𝜀 𝑧𝑥
𝜀 𝑦𝑥
|
|
|
( 2.40 )
|
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝜀 𝑦𝑧
𝜀 𝑥𝑧
𝜀 𝑥𝑦
𝜀 𝑧𝑦
𝜀 𝑧𝑥
𝜀 𝑦𝑥
|
|
|
=
[
𝑆 𝑥𝑥𝑥𝑥 𝑆 𝑥𝑥 𝑦𝑦 𝑆 𝑥𝑥 𝑧𝑧 𝑆 𝑥𝑥 𝑥𝑦 𝑆 𝑥𝑥 𝑦𝑧 𝑆 𝑥𝑥 𝑥𝑧 𝑆 𝑥𝑥 𝑦𝑥 𝑆 𝑥𝑥 𝑧𝑦 𝑆 𝑥𝑥 𝑧𝑥
𝑆 𝑦𝑦 𝑥𝑥 ⋱ ⋮
𝑆𝑧𝑧 𝑥𝑥 ⋱ ⋮
𝑆 𝑦𝑧 𝑥𝑥 ⋱ ⋮
𝑆 𝑥𝑧 𝑥𝑥 ⋱ ⋮
𝑆 𝑥𝑦 𝑥𝑥 ⋱ ⋮
𝑆𝑧𝑦 𝑥𝑥 ⋱ ⋮
𝑆𝑧𝑥 𝑥𝑥 ⋱ ⋮
𝑆 𝑦𝑥 𝑥𝑥 … … … … … … … 𝑆 𝑦𝑥 𝑦𝑥 ]
|
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑦𝑧
𝜏 𝑥𝑧
𝜏 𝑥𝑦
𝜏 𝑧𝑦
𝜏 𝑧𝑥
𝜏 𝑦𝑥
|
|
|
( 2.41 )

12
The main root of the indexical notation is very similar for the coefficients of both stiffness and
compliance matrixes. However, its meaning is exactly the opposite:
• The generic stiffness coefficient 𝐶 𝑖𝑗, corresponds to the stress component acting on the i-
direction due to a strain imposed in j-direction, while constraining to zero the strains in the
remaining directions;
• Whereas the generic compliance coefficient 𝑆 𝑖𝑗, corresponds to the strain component about the
𝑖-direction due to a stress applied in the 𝑗-direction, while keeping null the remaining stresses.
Without making any further assumption, to apply the Generalized Hooke’s Law it would be
necessary to define 81 elastic terms to compute the coefficient matrix (whether in its Stiffness or
Compliance form). From the stress symmetry and strain symmetry relations (reciprocity relations),
detailed in subchapter 2.2 and 2.3 respectively, it is possible to further simplify this matrix to a more
treatable form, as schematized in the following schematic equation:
|
|
|
( ) 𝑥𝑥
( ) 𝑦𝑦
( ) 𝑧𝑧
( ) 𝑦𝑧
( ) 𝑥𝑧
( ) 𝑥𝑦
−
−
−
|
|
|
=
[
𝜑 𝑥𝑥 𝑥𝑥 𝜑 𝑥𝑥 𝑦𝑦 𝜑 𝑥𝑥 𝑧𝑧 𝜑 𝑥𝑥 𝑥𝑦 𝜑 𝑥𝑥 𝑦𝑧 𝜑 𝑥𝑥 𝑥𝑧 − − −
𝜑 𝑦𝑦 𝑥𝑥 𝜑 𝑦𝑦 𝑦𝑦 𝜑 𝑦𝑦 𝑧𝑧 𝜑 𝑦𝑦 𝑥𝑦 𝜑 𝑦𝑦 𝑦𝑧 𝜑 𝑦𝑦 𝑥𝑧 − − −
𝜑𝑧𝑧 𝑥𝑥 𝜑𝑧𝑧 𝑦𝑦 𝜑𝑧𝑧 𝑧𝑧 𝜑𝑧𝑧 𝑥𝑦 𝜑𝑧𝑧 𝑦𝑧 𝜑𝑧𝑧 𝑥𝑧 − − −
𝜑 𝑥𝑦 𝑥𝑥 𝜑 𝑥𝑦 𝑦𝑦 𝜑 𝑥𝑦 𝑧𝑧 𝜑 𝑥𝑦 𝑥𝑦 𝜑 𝑥𝑦 𝑦𝑧 𝜑 𝑥𝑦 𝑥𝑧 − − −
𝜑 𝑦𝑧 𝑥𝑥 𝜑 𝑦𝑧 𝑦𝑦 𝜑 𝑦𝑧 𝑧𝑧 𝜑 𝑦𝑧 𝑥𝑦 𝜑 𝑦𝑧 𝑦𝑧 𝜑 𝑦𝑧 𝑥𝑧 − − −
𝜑 𝑥𝑧 𝑥𝑥 𝜑 𝑥𝑧 𝑦𝑦 𝜑 𝑥𝑧 𝑧𝑧 𝜑 𝑥𝑧 𝑥𝑦 𝜑 𝑥𝑧 𝑦𝑧 𝜑 𝑥𝑧 𝑥𝑧 − − −
− − − − − − − − −
− − − − − − − − −
− − − − − − − − −]
|
|
|
( ) 𝑥𝑥
( ) 𝑦𝑦
( ) 𝑧𝑧
( ) 𝑦𝑧
( ) 𝑥𝑧
( ) 𝑥𝑦
−
−
−
|
|
|
( 2.42 )
In order to simplify equation ( 2.42 ), it is not possible to directly eliminate all unnecessary
terms. Thus, in order that equation ( 2.42 ) preserves its meaning, the reciprocity property from both
stresses and strains implies the addition of the term 2 (due to the equal in value missing terms that were
eliminated).
|
|
( ) 𝑥𝑥
( ) 𝑦𝑦
( ) 𝑧𝑧
( ) 𝑦𝑧
( ) 𝑥𝑧
( ) 𝑥𝑦
|
|
=
[
𝜑 𝑥𝑥 𝑥𝑥 𝜑 𝑥𝑥 𝑦𝑦 𝜑 𝑥𝑥 𝑧𝑧 𝟐𝜑 𝑥𝑥 𝑦𝑧 𝟐𝜑 𝑥𝑥 𝑥𝑧 𝟐𝜑 𝑥𝑥 𝑥𝑦
𝜑 𝑦𝑦 𝑥𝑥 𝜑 𝑦𝑦 𝑦𝑦 𝜑 𝑦𝑦 𝑧𝑧 𝟐𝜑 𝑦𝑦 𝑦𝑧 𝟐𝜑 𝑦𝑦 𝑥𝑧 𝟐𝜑 𝑦𝑦 𝑥𝑦
𝜑𝑧𝑧 𝑥𝑥 𝜑𝑧𝑧 𝑦𝑦 𝜑𝑧𝑧 𝑧𝑧 𝟐𝜑𝑧𝑧 𝑦𝑧 𝟐𝜑𝑧𝑧 𝑥𝑧 𝟐𝜑𝑧𝑧 𝑥𝑦
𝜑 𝑦𝑧 𝑥𝑥 𝜑 𝑦𝑧 𝑦𝑦 𝜑 𝑦𝑧 𝑧𝑧 𝟐𝜑 𝑦𝑧 𝑦𝑧 𝟐𝜑 𝑦𝑧 𝑥𝑧 𝟐𝜑 𝑦𝑧 𝑥𝑦
𝜑 𝑥𝑧 𝑥𝑥 𝜑 𝑥𝑧 𝑦𝑦 𝜑 𝑥𝑧 𝑧𝑧 𝟐𝜑 𝑥𝑧 𝑦𝑧 𝟐𝜑 𝑥𝑧 𝑥𝑧 𝟐𝜑 𝑥𝑧 𝑥𝑦
𝜑 𝑥𝑦 𝑥𝑥 𝜑 𝑥𝑦 𝑦𝑦 𝜑 𝑥𝑦 𝑧𝑧 𝟐𝜑 𝑥𝑦 𝑦𝑧 𝟐𝜑 𝑥𝑦 𝑥𝑧 𝟐𝜑 𝑥𝑦 𝑥𝑦]
|
|
( ) 𝑥𝑥
( ) 𝑦𝑦
( ) 𝑧𝑧
( ) 𝑦𝑧
( ) 𝑥𝑧
( ) 𝑥𝑦
|
|
( 2.43 )
After simplification of the 4th
order coefficients’ tensor, the matrix lost its symmetry. The
importance of the engineering strains can now be fully understood. Instead of using the tensorial strains,
if the engineering strains were used, the symmetry of the matrix is restored, as detailed in [16].
Applying any energetic theorem e.g. Virtual Work Theorem, Minimum Potential Energy,
Maxwell-Betti Theorem, etc. [17], it is possible to prove that the matrix from the 4th
order tensor that
relates stress and strains in an elastic and loaded rigid body is symmetric. However, a different approach
was taken. In order to prove the symmetry of the elastic coefficient matrix, the concept of strain energy
density function is introduced. Conservative materials or Green Materials or Hyper-elastic materials are
a special case of Cauchy elastic materials (or simple elastic material), for which the stress-strain relation
derives from a strain energy density function [18]:
• Conservative materials possess a strain energy density function or energy potential, and this
energy potential is given by,
𝜎𝑟𝑠 =
𝜕𝑈𝑟𝑠
𝜕𝜀 𝑟𝑠
( 2.44 )

13
• Assuming linear stresses and strains,
| 𝜎 | = [ 𝐶 ] | 𝜀 | ⇒ 𝜎𝑖𝑗 = 𝐶𝑖𝑗 𝑘𝑙 ∙ 𝜀 𝑘𝑙 ( 2.45 )
• The elastic energy is finally given by,
𝐶𝑖𝑗 𝑘𝑙 ∙ 𝜀 𝑟𝑠 =
𝜕𝑈𝑟𝑠
𝜕𝜀 𝑟𝑠
; 𝑟𝑠 = 𝑘𝑙 ( 2.46 )
• Differentiating the previous equation to respect to 𝜀 𝑘𝑙 or 𝜀𝑖𝑗 we get,
𝐶𝑖𝑗 𝑘𝑙 =
𝜕2
𝑈𝑖𝑗
𝜕𝜀𝑖𝑗 𝜕𝜀 𝑘𝑙
𝐶𝑘𝑙 𝑖𝑗 =
𝜕2
𝑈𝑖𝑗
𝜕𝜀 𝑘𝑙 𝜕𝜀𝑖𝑗
( 2.47 )
• Which finally ends up in the symmetry relation:
𝐶𝑖𝑗 𝑘𝑙 =
𝜕2
𝑈𝑖𝑗
𝜕𝜀𝑖𝑗 𝜕𝜀 𝑘𝑙
=
𝜕2
𝑈𝑖𝑗
𝜕𝜀 𝑘𝑙 𝜕𝜀𝑖𝑗
= 𝐶𝑘𝑙 𝑖𝑗 ⇒ 𝐶𝑖𝑗 𝑘𝑙 = 𝐶𝑘𝑙 𝑖𝑗 ( 2.48 )
The vast majority of engineering materials are conservative, as a result, the symmetry of the
stiffness and compliance matrices is verified for most of common engineering problems. After all
previous simplifications summarized in Table 2, the Generalized Hooke’s Law for a conservative
anisotropic material is a 6x6 elastic matrix, and now only involves the knowledge of 21 unknown elastic
terms or parameters (only 21 stiffness components are actually independent in Hooke's law), and it can
be written in the form bellow:
|
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑦𝑧
𝜏 𝑥𝑧
𝜏 𝑥𝑦
|
|
|
=
[
𝐶11 𝐶12 𝐶13 𝐶14 𝐶15 𝐶16
… 𝐶22 𝐶23 𝐶24 𝐶25 𝐶26
… … 𝐶33 𝐶34 𝐶35 𝐶36
… … … 𝐶44 𝐶45 𝐶46
… … … … 𝐶55 𝐶56
… … … … … 𝐶66 ]
|
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝛾𝑦𝑧
𝛾𝑥𝑧
𝛾𝑥𝑦
|
|
|
( 2.49 )
Table 2- Summary of all simplifications made to the general stiffness matrix.
Property
Number of
Dependent terms
Original Number of terms 81 = 9 x 9
Stress Reciprocity 18 + 9* After Reciprocity
Reduction
36 = 6 x 6
Strain Reciprocity 18 + 9*
Symmetry of the
Stiffness matrix
15
After Matrix Symmetry
Reduction 21 =
6 ∙ (6 + 1)
2
* 9 terms are automatically and simultaneously eliminated by the reciprocity property of both stresses and
strains

14
2.5 Transformation Matrix
The transformation matrix allows to change the stress, the strain, or even the
stiffness/compliance tensor from one coordinate system to another generically transformed coordinate
system. In its completely general form, the transformation matrix is given by:
[ 𝑇 ] =
[
cos( 𝛼 𝑥′ 𝑥) cos(𝛼 𝑥′ 𝑦) cos( 𝛼 𝑥′ 𝑧)
cos(𝛼 𝑦′ 𝑥) cos(𝛼 𝑦′ 𝑦) cos(𝛼 𝑦′ 𝑧)
cos( 𝛼 𝑧′ 𝑥) cos(𝛼 𝑧′ 𝑦) cos( 𝛼 𝑧′ 𝑧) ]
( 2.50 )
The mathematical meaning of the angles of
the transformation matrix, equation ( 2.50 ), is
illustrated in Figure 4 for the particular case of the
transformed 𝑥’-axis. Using a similar principle, the
remaining rotation angles could also be drawn.
Usually, the direction cosines from equation ( 2.50 ), are hard to compute individually. So, the
transformation matrix can also be determined by the combination of three (simpler) transformation in
respect to only one axis. The most used combination is designated as Euler Angles (or x-convention)
and is determined by:
[𝑇] = [ −
cos( 𝜓) sin( 𝜓) 0
sin( 𝜓) cos( 𝜓) 0
0 0 1
]
𝑧
[
1 0 0
0 cos( 𝜃) sin( 𝜃)
0 −sin( 𝜃) cos( 𝜃)
]
𝑥
[ −
cos( 𝜑) sin( 𝜑) 0
sin( 𝜑) cos( 𝜑) 0
0 0 1
]
𝑧
( 2.51 )
The physical meaning of the three rotation angles is given in Figure 5 and Figure 6. Since the
matrix multiplication operation isn’t commutative, the order of rotation matters, Counter-clockwise
rotation was considered as a positive rotation for all angles.
𝑧
𝑥
𝑦
𝑥′
𝛼 𝑥′ 𝑥
𝛼 𝑥′ 𝑦
𝛼 𝑥′ 𝑧
Figure 4- Illustration of the angles between the
transformed 𝑥’-axis and the original cartesian
coordinate system.
Figure 5- Illustration of the individual rotations of the Euler angles. Image adapted from [2].

15
Since this report is essentially dedicated to plane elasticity, for the 2D case, the only possible
transformation consists in a rotation around the z-axis, and the transformation matrix s given by:
[𝑇] = [ −
cos( 𝜓) sin( 𝜓) 0
sin( 𝜓) cos( 𝜓) 0
0 0 1
]
𝑧
( 2.52 )
If orthotropic or other material behaviors were considered, it would be necessary to apply the
transformation matrix to the stress, strain and stiffness tensor as follows [16]:
[ 𝜎′ ] = [ 𝑇 ] [ 𝜎 ] [ 𝑇 ] 𝑇
( 2.53 )
[ 𝜀′ ] = [ 𝑇 ] [ 𝜀 ] [ 𝑇 ] 𝑇 ( 2.54 )
[ 𝜑′ ] = [ 𝑇 ] [ 𝜑 ] [ 𝑇 ] 𝑇 ( 2.55 )
The demonstration won’t be detailed here [10], since it wasn’t necessary for this report and a similar
demonstration was conducted in subchapter 5.3. However, after the several simplifications applied to
all tensors, the stress vector, strain vector, and stiffness matrix, would be computed by [16]:
| 𝜎′ | = [ 𝑇∗ ] | 𝜎 | ( 2.56 )
| 𝜀′ | = [ 𝑇∗∗ ] | 𝜀 | ( 2.57 )
[ 𝐶′ ] = [ 𝑇∗ ] [ 𝐶 ] [ 𝑇∗∗ ] 𝑇 ( 2.58 )
A final comment should be done, regarding the misguiding meaning of the transformation
matrix in technical literature of different fields. In solid mechanics, the transformation matrix assumes
that the mathematical entities are static, while the coordinate system is changed. Whereas the rotation
matrix usually designated also as transformation matrix, changes the entities while the coordinate system
remains the same.
𝜓
𝑥′
𝑦′
𝑦
𝑥
𝜓
𝜃
𝑦′′
𝑧′
𝑧
𝑦
𝜃
Figure 6- Definition of the nomenclature
used to define the coordinates
transformation matrix. The 𝜃, 𝜑, and 𝜓,
represent the rotation angle about the z, x
and y axis respectively.
𝜑
𝑥′′
𝑦′′′
𝑦′′
𝑥′′
𝜑

16
2.6 2D Linear Elasticity
2D linear elasticity theory provides the mathematical model and the theoretical background by
which the behavior of a real 3D structure or body is represented by a 2D geometry. In order to facilitate
the understanding of this subchapter and the previous chapters, a brief comment regarding the specific
2D plane problems’ nomenclature will be made. In Figure 7, the definition of the body geometry (with
the designation of the main reference dimensions); and the coordinate system used (with the respective
displacements associated to it) is outlined.
The solution of any general 2D plane problem using the linear elasticity theory implies (in a
preliminary analysis), the determination for each point of the body, of 11 unknown variables: 𝜎𝑥𝑥 , 𝜎 𝑦𝑦 ,
𝜎𝑧𝑧 , 𝜏 𝑥𝑦 , 𝜀 𝑥𝑥 , 𝜀 𝑦𝑦 , 𝜀 𝑧𝑧 , 𝛾𝑥𝑦 , 𝑢( 𝑥, 𝑦), 𝑣( 𝑥, 𝑦), 𝑤( 𝑥, 𝑦). In other words, the main goal of a general solid
mechanics problem is to compute the stresses, strains, and displacement vector, compatible with the:
Body Forces, Surface Tractions, and Boundary Conditions. In order to determine these 11 variables, we
have only 10 independent equations: 2 equations from the dynamic equilibrium defined by the Cauchy
Vector Equation, 4 equations from the Generalized Hooke’s Law, and 4 equations from the geometric
definition of strains. Thus, in order to solve any problem from plane elasticity, it is necessary to introduce
an additional simplification, which may arise from a particular stress distribution or a particular strain
distribution. Hence, giving rise to the two types of plane problems: Plane Stress and Plane Strain
problems.
2.6.1 Types of Plane Linear Elastic Problems
Plane linear elastic problems are a class of situations that due to their geometry (sort of
prismatic), boundary conditions, and loading conditions, two unknown fields (Stresses and Strains)
don’t depend from the third coordinate (usually designated by z). There are two types of plane problems
of relevant practical interest in mechanical engineering:
• Plane stresses – particularly accurate for thin plates (ideally infinitely thin), deep beams and
walls under in-plane loading, buttress dams, etc. in which the two dimensions (length and width)
are much higher than their thickness. In this type of problems, the following
assumptions/simplifications are made [4], [1]:
𝜎𝑧𝑧(𝑥, 𝑦, 𝑧 = ± 𝑡/2) = 𝜏 𝑦𝑧(𝑥, 𝑦, 𝑧 = ± 𝑡/2) = 𝜏 𝑥𝑧(𝑥, 𝑦, 𝑧 = ± 𝑡/2) = 0 ( 2.59 )
𝑡 ≪ 𝑙 ⋀ 𝑡 ≪ 𝑤 ⇒ 𝜎𝑧𝑧(𝑥, 𝑦, 𝑧) = 𝜏 𝑦𝑧(𝑥, 𝑦, 𝑧) = 𝜏 𝑥𝑧(𝑥, 𝑦, 𝑧) = 0 ( 2.60 )
𝑡 ≪ 𝑙 ⋀ 𝑡 ≪ 𝑤 ⇒ {
𝜎𝑥𝑥 = 𝑓𝑥 𝑥(𝑥, 𝑦)
𝜎 𝑦𝑦 = 𝑓𝑦 𝑦( 𝑥, 𝑦)
𝜏 𝑥𝑦 = 𝑓𝑥 𝑦(𝑥, 𝑦)
( 2.61 )
Figure 7- a) Plane Stress schematic geometry. b) Plane Strain schematic geometry.
a) b)y
x
l t
w
z
𝑢⃗
𝑣
𝑤⃗⃗
y
xl
t
w z
𝑣
𝑢⃗
𝑤⃗⃗

17
• Plane Strains – particularly accurate for thick geometries (ideally infinitely long), such as
containing walls, gravity dams, pressurized pipes, geotechnical engineering problems (e.g.
tunnels, foundations, etc.), etc.in which the dimension of section development (generatrix) is
much higher than the remaining dimensions (length and width). In this type of problems, the
following assumptions/simplifications are made [4], [1]:
𝑡 ≫ 𝑙 ⋀ 𝑡 ≫ 𝑤 ⇒ 𝜎𝑧𝑧( 𝑥, 𝑦, 𝑧) = 𝐶 𝑡𝑒 ( 2.62 )
{
𝑤( 𝑥, 𝑦, ±𝑡/2) = 0
𝑤( 𝑥, 𝑦, 0) = 0, 𝑏𝑦 𝑠𝑦𝑚𝑚𝑒𝑡𝑟𝑦
⇒ 𝑤( 𝑥, 𝑦, 𝑧) ≈ 0 ( 2.63 )
𝑤( 𝑥, 𝑦, 𝑧) = 0 ⇒
{
𝜀 𝑧𝑧(𝑥, 𝑦, 𝑧) = 𝛾𝑦𝑧(𝑥, 𝑦, 𝑧) = 𝛾𝑥𝑧(𝑥, 𝑦𝑧, 𝑧) = 0
𝜀 𝑥𝑥 = 𝑓𝑥 𝑥(𝑥, 𝑦)
𝜀 𝑦𝑦 = 𝑓𝑦 𝑦(𝑥, 𝑦)
𝛾𝑥𝑦 = 𝑓𝑥 𝑦(𝑥, 𝑦)
( 2.64 )
In addition, both simplifications or type of plane problems also consider that
{
𝑓𝑥 = 𝑓𝑥( 𝑥, 𝑦)
𝑓𝑦 = 𝑓𝑦( 𝑥, 𝑦)
𝑓𝑧 = 0
( 2.65 )
After plane stress or plane strain simplification (as concluded in section 2.6.6), the solid
mechanics problem is resumed to the resolution of two coupled Partial Differential Equations (PDE),
for two dependent variables: the two terms of the displacement vector, u(x,y) and v(x,y).
2.6.2 Dynamic Equilibrium
The dynamic equilibrium equations are the same, to whether plane stress or plane strain is
concerned. The dynamic equilibrium of a generic 2D rigid body can be written as:
• The classic formulations seen in the majority of the technical literature:
[ 𝜎 ] ∇ + | 𝑓 | = 𝜌 | 𝑎 | ⇒ [
𝜎𝑥𝑥 𝜏 𝑥𝑦
𝜏 𝑥𝑦 𝜎 𝑦𝑦
]
[
𝜕
𝜕𝑥
𝜕
𝜕𝑦 ]
+ |
𝑓𝑥
𝑓𝑦
| = 𝜌 |
𝑢̈ (𝑥, 𝑦)
𝑣̈(𝑥, 𝑦)
| ⇒ ( 2.66 )
(
𝜕𝜎𝑥𝑥
𝜕𝑥
+
𝜕𝜏 𝑥𝑦
𝜕𝑦
) + 𝑓𝑥 = 𝜌 𝑢̈ (𝑥, 𝑦) = 𝜌 ∙
𝜕2
𝜕𝑡2
𝑢(𝑥, 𝑦) ( 2.67 )
(
𝜕𝜏 𝑥𝑦
𝜕𝑥
+
𝜕𝜎 𝑦𝑦
𝜕𝑦
) + 𝑓𝑦 = 𝜌 𝑣̈(𝑥, 𝑦) = 𝜌 ∙
𝜕2
𝜕𝑡2
𝑣(𝑥, 𝑦) ( 2.68 )
𝑓𝑥, 𝑓𝑦 Volume forces acting on the x, and y direction respectively
• Instead of using the Nabla operator, in the Finite Element Method (FEM) formulation, the
matrix formulation is adopted due to its computational calculation suitability. The matrix of the

18
partial derivatives operator will be designated by [ 𝐿 ], and corresponds to the transposed of the
same matrix used to relate strains and displacements.
[ 𝐿 ] 𝑇| 𝜎 | + | 𝑓 | = 𝜌 | 𝑎 | ⇒
[
𝜕
𝜕𝑥
0
0
𝜕
𝜕𝑦
𝜕
𝜕𝑦
𝜕
𝜕𝑥 ]
𝑇
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜏 𝑥𝑦
| + |
𝑓𝑥
𝑓𝑦
| = 𝜌 |
𝑢̈ (𝑥, 𝑦)
𝑣̈(𝑥, 𝑦)
| ( 2.69 )
2.6.3 Transformation Matrix
In the context of this report, the transformation matrix always refers to a matrix acting upon a
coordinate system. It is really important to outline this fact. Since in some literature this designation is
also misused to refer to geometric transformation matrices of vectors and matrices (e.g. rotation,
stretching, squeezing, shearing, reflection, etc.). The transformation matrices for 2D coordinate systems
are summarized below, along with its schematic illustration in Figure 8:
• Transformation Matrix of the coordinate system by Counter clockwise rotation of the coordinate
system:
[ 𝑇 ] = [
cos( 𝜓) sin( 𝜓)
− sin( 𝜓) cos( 𝜓)
] ( 2.70 )
• Clockwise rotation of the coordinate system
[ 𝑇 ] = [
cos( 𝜓) −sin( 𝜓)
sin( 𝜓) cos( 𝜓)
] ( 2.71 )
a) b)
𝜓
𝑥′
𝑦′
𝑦
𝑥
𝜓
𝜓
𝑥′
𝑦′
𝑦
𝑥
𝜓
Figure 8- Representation of the transformation of the coordinate system by rotation along the z-axis: a)
Counter Clockwise rotation, and b) Clockwise rotation.

19
2.6.4 2D Hooke’s Law – Isotropic Material Behavior
In 2D elasticity, the Generalized Hooke’s Law can be further simplified (by eliminating the
terms that account for the shear behavior in the third dimension), and the matrix relation can be simply
written in the stiffness and compliance form, respectively, as:
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑥𝑦
|
|
=
[
𝐶11 𝐶12 𝐶13 𝐶14
… 𝐶22 𝐶23 𝐶24
… … 𝐶24 𝐶34
… … … 𝐶44 ]
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝛾𝑥𝑦
|
|
( 2.72 )
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝛾𝑥𝑦
|
|
=
[
𝑆11 𝑆12 𝑆13 𝑆14
… 𝑆23 𝑆23 𝑆24
… … 𝑆33 𝑆34
… … … 𝑆44 ]
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑥𝑦
|
|
( 2.73 )
Isotropic material behavior results from two necessary conditions: (i) linear elastic deformation
of an (ii) isotropic material - hyperelastic material whose scaler components of the stiffness tensor are
invariant (symmetric) with respect to all possible orthogonal transformations [10]. As demonstrated in
detail by [16], the stiffness and compliance coefficients are related respectively by:
{
𝐶11 = 𝐶22 = 𝐶33
𝐶12 = 𝐶13 = 𝑠𝑦𝑚 = 𝐶21 = 𝐶31
𝐶44 =
𝐶11 − 𝐶22
2
𝐶14 = 𝐶24 = 𝐶34 = 0 = 𝑠𝑦𝑚 = 𝐶14 = 𝐶24 = 𝐶34 = 0
( 2.74 )
{
𝑆11 = 𝑆22 = 𝑆33
𝑆12 = 𝑆13 = 𝑠𝑦𝑚 = 𝑆21 = 𝑆31
𝑆44 = 2( 𝑆11 − 𝑆22)
𝑆14 = 𝑆24 = 𝑆34 = 0 = 𝑠𝑦𝑚 = 𝑆14 = 𝑆24 = 𝑆34 = 0
( 2.75 )
Examples of typical engineering materials that can be considered isotopic with reasonable
accuracy are the major metal alloys: machined steel, Cast Iron. Cast Aluminum, etc. Considering
isotropic behavior, the “2D” Generalized Hooke’s Law comes [19]:
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑥𝑦
|
|
=
[
𝐶11 𝐶12 𝐶12 0
… 𝐶11 𝐶12 0
… … 𝐶11 0
0 0 0 ( 𝐶11 − 𝐶12)/2 ]
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝛾𝑥𝑦
|
|
( 2.76 )
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝛾𝑥𝑦
|
|
=
[
𝑆11 𝑆12 𝑆12 0
… 𝑆11 𝑆12 0
… … 𝑆11 0
0 0 0 2( 𝑆11 − 𝑆12) ]
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑥𝑦
|
|
( 2.77 )

20
The stiffness or compliance coefficients are usually given in terms of engineering parameters.
Elastic engineering parameters or constants, are properties frequently and easily determined by Lab
testing e.g. Young Modulus, Poisson Ratio, Shear Modulus, etc. The most relevant engineering
constants within the context of this report are: Principal or Young’s Modulus in the 𝑖 direction ( 𝐸 𝑖𝑖) –
ratio of the stress in the 𝑖 direction, to a strain in the 𝑖 direction; Poisson Coefficient or Poisson Ratio
(𝑣 𝑖𝑗) – the negative of the ratio of the transverse strain in the 𝑗 direction when a stress is applied in the
𝑖 direction, to the longitudinal strain in the 𝑖 direction when a stress is applied in the 𝑖 direction [1]. The
mathematical definition of the elastic engineering coefficients or parameters is then given as [16]:
{
𝐸 𝑖𝑖 =
𝜎 𝑖
𝜀 𝑖
, 𝑙𝑜𝑛𝑔𝑖𝑡𝑢𝑑𝑖𝑛𝑎𝑙 𝑑𝑖𝑟𝑒𝑐𝑡𝑖𝑜𝑛
𝑣 𝑖𝑗 = −
𝑆 𝑗𝑖
𝑆 𝑖𝑖
, 𝑡𝑟𝑎𝑛𝑠𝑣𝑒𝑟𝑠𝑎𝑙 𝑑𝑖𝑟𝑒𝑐𝑡𝑖𝑜𝑛
( 2.78 )
Concerning the physical understanding of the elastic coefficients, it is usually easy to: i) write
the compliance coefficients in terms of the engineering constants; ii) compute the stiffness matrix by
inverting the compliance matrix; and finally, iii) define the stiffness coefficients by simply looking at
the components of the stiffness matrix. This has to do with the fact that the stiffness coefficients are
computed constraining the strains in the remaining directions (by applying external stresses), whereas
the compliance coefficients are computed by simply considering the remaining stresses null. Thus, it is
possible to construct the compliance matrix column by column considering the meaning of the
compliance coefficients, and the elastic engineering parameters can be calculated as:
{
𝑆11 =
𝜀 𝑥𝑥
𝜎 𝑥𝑥
=
1
𝐸11
=
1
𝐸
𝑆22 =
𝜀 𝑦𝑦
𝜎 𝑦𝑦
=
1
𝐸22
=
1
𝐸
𝑆33 =
𝜀 𝑧𝑧
𝜎𝑧𝑧
=
1
𝐸33
=
1
𝐸
( 2.79 )
{
𝑆12 =
𝜀 𝑥𝑥
𝜎 𝑦𝑦
=
𝜀 𝑥𝑥
𝜎 𝑦𝑦
(
𝜀 𝑦𝑦
𝜎 𝑦𝑦
∙
𝜎 𝑦𝑦
𝜀 𝑦𝑦
) =
𝜀 𝑥𝑥
𝜎 𝑦𝑦
(
𝜀 𝑦𝑦
𝜎 𝑦𝑦
∙ 1
𝜀 𝑦𝑦
𝜎 𝑦𝑦
⁄ ) =
𝜀 𝑥𝑥
𝜎 𝑦𝑦
𝜀 𝑦𝑦
𝜎 𝑦𝑦
⁄ ∙
𝜀 𝑦𝑦
𝜎 𝑦𝑦
𝑆21 =
𝜀 𝑦𝑦
𝜎𝑥𝑥
=
𝜀 𝑦𝑦
𝜎𝑥𝑥
(
𝜀 𝑥𝑥
𝜎 𝑥𝑥
∙
𝜎𝑥𝑥
𝜀 𝑥𝑥
) =
𝜀 𝑦𝑦
𝜎 𝑥𝑥
(
𝜀 𝑥𝑥
𝜎𝑥𝑥
∙ 1
𝜀 𝑥𝑥
𝜎 𝑥𝑥
⁄ ) =
𝜀 𝑦𝑦
𝜎𝑥𝑥
𝜀 𝑥𝑥
𝜎 𝑥𝑥
⁄ ∙
𝜀 𝑥𝑥
𝜎𝑥𝑥
⇒ ( 2.80 )
{
𝑆12 =
𝑆12
𝑆22
∙ 𝑆22 = −𝑣21 ∙ 𝑆22 = −𝑣21 ∙
1
𝐸22
= −
𝑣21
𝐸22
= −
𝑣
𝐸
𝑆21 =
𝑆21
𝑆11
∙ 𝑆11 = −𝑣12 ∙ 𝑆11 = −𝑣12 ∙
1
𝐸11
= −
𝑣12
𝐸11
= −
𝑣
𝐸
( 2.81 )
𝑆44 = 2( 𝑆11 − 𝑆12) = 2 (
1
𝐸11
+ 𝑣21 ∙ 𝑆22) = 2 (
1
𝐸11
+ 𝑣21 ∙
1
𝐸22
) =
2(1 + 𝑣)
𝐸
( 2.82 )
In the compliance form, the “2D” Generalized Hook’s Law for linear elastic isotropic materials
now comes:

21
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝛾𝑥𝑦
|
|
=
[
1
𝐸
−
𝑣
𝐸
−
𝑣
𝐸
0
−
𝑣
𝐸
1
𝐸
−
𝑣
𝐸
0
−
𝑣
𝐸
−
𝑣
𝐸
1
𝐸
0
0 0 0
2(1 + 𝑣)
𝐸 ]
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑥𝑦
|
|
( 2.83 )
The stiffness form of the “2D” Generalized Hook’s law for linear elastic isotropic materials is
calculated by simply inverting the previous equation ( 2.84 ) comes:
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑥𝑦
|
|
=
[
𝐸(1 − 𝑣)
(1 + 𝑣)(1 − 2𝑣)
𝐸𝑣
(1 + 𝑣)(1 − 2𝑣)
𝐸𝑣
(1 + 𝑣)(1 − 2𝑣)
0
𝐸𝑣
(1 + 𝑣)(1 − 2𝑣)
𝐸(1 − 𝑣)
(1 + 𝑣)(1 − 2𝑣)
𝐸𝑣
(1 + 𝑣)(1 − 2𝑣)
0
𝐸𝑣
(1 + 𝑣)(1 − 2𝑣)
𝐸𝑣
(1 + 𝑣)(1 − 2𝑣)
𝐸(1 − 𝑣)
(1 + 𝑣)(1 − 2𝑣)
0
0 0 0
𝐸
2(1 + 𝑣) ]
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝛾𝑥𝑦
|
|
( 2.84 )
The plane assumption (plane stress or plane strain), conditions the process used to determine
Hook’s Law for plane problems. In order to compute Hook’s Law for plane stress, the compliance matrix
of the Generalized Hook’s Law is used; whereas to compute Hook’s Law for plane strain, the stiffness
matrix of the Generalized Hook’s Law is used [4]:
• Plane Stress
Assuming 𝜎𝑧𝑧 = 0:
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝜀 𝑧𝑧
𝛾𝑥𝑦
|
|
=
[
1
𝐸
−
𝑣
𝐸
−
𝑣
𝐸
0
−
𝑣
𝐸
1
𝐸
−
𝑣
𝐸
0
−
𝑣
𝐸
−
𝑣
𝐸
1
𝐸
0
0 0 0
2(1 + 𝑣)
𝐸 ]
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
0
𝜏 𝑥𝑦
|
|
( 2.85 )
The Compliance matrix is determined simply by ignoring the columns, in the generalized
compliance matrix, associated with the zero stress entries in the stress vector, coming:
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝛾𝑥𝑦
| =
[
1
𝐸
−
𝑣
𝐸
0
−
𝑣
𝐸
1
𝐸
0
0 0
2(1 + 𝑣)
𝐸 ]
|
𝜎 𝑥𝑥
𝜎 𝑦𝑦
𝜏 𝑥𝑦
|
( 2.86 )

22
The Stiffness matrix is determined simply by inverting the compliance matrix, and is given by:
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜏 𝑥𝑦
| =
𝐸
(1 − 𝑣2)
[
1 𝑣 0
𝑣 1 0
0 0 (1 − 𝑣)/2
] |
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝛾𝑥𝑦
| ( 2.87 )
Comment: Note that the compliance matrix for plane stress can’t be found by removing columns
and rows from the general isotropic stiffness matrix
• Plane Strain
Assuming 𝜀 𝑧𝑧 = 0:
|
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜎𝑧𝑧
𝜏 𝑥𝑦
|
|
=
𝐸
(1 + 𝑣)(1 − 2𝑣)
[
(1 − 𝑣) 𝑣 𝑣 0
𝑣 (1 − 𝑣) 𝑣 0
𝑣 𝑣 (1 − 𝑣) 0
0 0 0 (1 − 2𝑣)/2 ]
|
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
0
𝛾𝑥𝑦
|
|
( 2.88 )
The Stiffness matrix is determined simply by ignoring the columns, in the generalized stiffness
matrix, associated with the zero strain entries in the strain vector, coming:
|
𝜎𝑥𝑥
𝜎 𝑦𝑦
𝜏 𝑥𝑦
| =
𝐸
(1 + 𝑣)(1 − 2𝑣)
[
(1 − 𝑣) 𝑣 0
𝑣 (1 − 𝑣) 0
0 0 (1 − 2𝑣)/2
] |
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝛾𝑥𝑦
| ( 2.89 )
The Compliance matrix is determined simply by inverting the stiffness matrix, and is given by:
|
𝜀 𝑥𝑥
𝜀 𝑦𝑦
𝛾𝑥𝑦
| =
1
𝐸
[
1 − 𝑣2
−𝑣(1 + 𝑣) 0
−𝑣(1 + 𝑣) 1 − 𝑣2
0
0 0 2(1 + 𝑣)
] |
𝜎 𝑥𝑥
𝜎 𝑦𝑦
𝜏 𝑥𝑦
| ( 2.90 )
Comment: Note that the compliance matrix for plane strain can’t be found by removing columns
and rows from the general isotropic compliance matrix.
2.6.5 Strain-Displacement Fields Relation
The geometric definition of infinitesimal strains, within the context of FEM, is usually written
in the matrix form. The strain in the z direction (𝜀 𝑧𝑧) will be considered for now, since the 𝜀 𝑧𝑧 isn’t null
for the case of plane stress. However, in the next section further details regarding this topic will be given.
The strain field can then be written as:

Isoparametric bilinear quadrilateral element

Isoparametric bilinear quadrilateral element

Recomendados

Recomendados

Mais conteúdo relacionado

Mais procurados

Mais procurados (20)

Semelhante a Isoparametric bilinear quadrilateral element

Semelhante a Isoparametric bilinear quadrilateral element (20)

Mais de Filipe Giesteira

Mais de Filipe Giesteira (20)

Último

Último (20)

Isoparametric bilinear quadrilateral element