Development, Calibration and Verification of Finite Element Models of Laboratory Structures
This thesis is presented in part submission as a requirement of the Bachelor of Engineering (Honours) in Civil Engineering in the Department of Civil, Construction & Civil Mineral Engineering, Athlone Institute of Technology.
Luke Molloy
2012
Project Supervisor Dr. Paul Archbold
Project Coordinator Dr. Paul Archbold
Head of Department Mr. Fergal Sweeney
Declaration I declare that the dissertation submitted by me, in whole or in part, has not been submitted to any other university, institute or college as an exercise for a degree or any other qualification. I further declare that, except where reference is given in the text, it is entirely my own work.
Signed:______________________
Date:____________
Acknowledgements
I would like to express my sincerest appreciation to my supervisor Dr. Paul Archbold for his guidance and instruction throughout the production of this dissertation. Also I would like to thank Athlone Institute of Technology for the use of the Software and Heavy Structures Laboratories which allowed me to conduct this project with the highest standard of equipment. I would like to thank everyone who was involved in this project for their assistance and support throughout above all my wife for her continuing support.
Abstract
This dissertation sets out to develop and verify finite element models created in ANSYS of two laboratory structures. The structures modelled were a T shaped aluminium beam and a scaled 3 hinge arch bridge. The structures were tested in the Athlone Institute of Technology Heavy Structures Laboratory. The T shaped beam was tested for strain associated with incremental loading and the bridge was tested for horizontal reaction forces associated with a transient load across the bridge deck. Both structures were tested physically and their geometries replicated in 3D finite element modelling code ANSYS. The models were subjected to the same loading and support conditions as the experimental setup to verify the accuracy of the finite element models. Model updating parameters implemented were the changing of Young’s modulus for the beam model based on an experimentally obtained value and structure geometry for the bridge model. Both models were verified with the experimental data which showed a successful result from the updating process. The updated beam model showed an average increase in the model maximum tensile strain went from 87% to 102% of the experimental value and an average increase in the model maximum compressive strain went from 88% to 100% of the experimental value while the 3 hinge arch bridge updated model results showed the model exceeding the horizontal reaction force by only 4% of the experimental result.
Table of Contents Table of Contents ......................................................................................................i List of Figures .......................................................................................................... iv List of Tables............................................................................................................ ix 1.
Introduction .................................................................................................... 1
2
Literature Review ............................................................................................ 3
2.1 Introduction .................................................................................................... 3 2.2 Background to finite element analysis............................................................ 4 2.3 Fundamental structural concepts ................................................................... 6 2.3.1 Material stiffness..................................................................................... 7 2.3.2 Principle of superposition ..................................................................... 10 2.3.3 Virtual work ........................................................................................... 11 2.4 Finite element direct stiffness method for framed structures ..................... 12 2.5 Matrix representation ................................................................................... 14 2.6 Continuous medium finite element method ................................................ 15 2.7 Model analysis............................................................................................... 17 2.8 Development of finite element models ........................................................ 18 2.9 Model updating ............................................................................................. 22 2.10
Model validity and verification ................................................................. 30
2.11
Model calibration ...................................................................................... 34 i
2.12
FE analysis studies ..................................................................................... 35
2.13
Element type selection.............................................................................. 43
2.14
Unit gravity load check .............................................................................. 45
2.15
Conclusion ................................................................................................. 45
3
Methodology ................................................................................................. 47
3.1 Introduction .................................................................................................. 47 3.2 Experimental data: T shaped aluminium beam ............................................ 48 3.2.1 Experimental strain data ....................................................................... 49 3.2.2 Experimentally derived Young’s modulus............................................. 51 3.2.3 Mathematically calculated deflection data .......................................... 55 3.2.4 Macaulay’s method ............................................................................... 55 3.2.5 Finite element stiffness method ........................................................... 58 3.3 Experimental data: 3 hinge arch bridge transient load ................................ 62 3.3.1 Experimental procedure ....................................................................... 63 3.3.2 Mathematically calculated data ............................................................ 64 3.4 Finite element modelling .............................................................................. 65 3.4.1 ANSYS self-learning ............................................................................... 65 3.4.2 Modelling methodology ........................................................................ 66 3.4.3 T shaped aluminium beam .................................................................... 70 3.4.4 Transient load on 3 hinge arch bridge .................................................. 79 4
Results ........................................................................................................... 95
4.1 T shaped aluminium beam results ................................................................ 95 4.1.1 Experimentally determined strain values ............................................. 95 4.1.2 Experimentally derived Young’s modulus............................................. 99 ii
4.1.3 Theoretical strain values ..................................................................... 100 4.1.4 Compressive strain results (ANSYS) .................................................... 101 4.1.5 Tensile strain results (ANSYS).............................................................. 104 4.1.6 Experimental strain investigation ....................................................... 107 4.1.7 Elastic beam bending deflection results ............................................. 110 4.1.8 Deflection results from finite element stiffness method ................... 113 4.1.9 Deflection results from Macaulay’s method ...................................... 118 4.1.10
Finite element model summery ...................................................... 120
4.1.11
Material data ................................................................................... 120
4.2 Three hinge arch bridge results .................................................................. 121 4.2.1 Experimental reaction results ............................................................. 121 4.2.2 ANSYS finite element model results ................................................... 122 4.2.3 Mesh results details ............................................................................ 126 4.2.4 Material data ....................................................................................... 127 4.2.5 Model results ...................................................................................... 128 5
Discussion .................................................................................................... 131
5.1 T shaped aluminium beam .......................................................................... 131 5.1.1 Finite element model .......................................................................... 133 5.1.2 Model updating ................................................................................... 138 5.2 Three hinge arch bridge .............................................................................. 140 5.2.1 Finite element model .......................................................................... 140 6
Conclusion and recommendations ............................................................. 146
7
Bibliography ................................................................................................ 148
8
Appendices .................................................................................................. 152
iii
List of Figures Figure 2.1 – Explanation of Young’s modulus (Hyperphysics 2012) ........................8 Figure 2.2 – Three-member example truss (Colorado 2012) ................................12 Figure 2.3 – Disconnection step (Colorado 2012) .................................................13 Figure 2.4 – Generic truss member (Colorado 2012) ............................................14 Figure 2.5 – Triangular mesh applied to a bracket (VKI 2012) ..............................16 Figure 2.6 – Cross section of corrugated webs (Chan et al. 2002) ........................19 Figure 2.7 – FE mesh representation of beams (Chan et al. 2002) ......................20 Figure 2.8 – Finite element model (Chan et al. 2002) ...........................................20 Figure 2.9 – Experimental setup (Chan et al. 2002) ..............................................21 Figure 2.10 – Elevation of the experimental modal (Zapico-Valle et al. 2010) .....26 Figure 2.11 – Truss geometry (Esfandiari et al. 2010) ...........................................27 Figure 2.12 – Degrees of freedom of model (Esfandiari et al. 2010) ....................27 Figure 2.13 – Steel framed scaled benchmark structure (Wu and Li 2006) ..........28 Figure 2.14 – Elevation of the Svinesund Bridge (Schlune et al. 2009) .................29 Figure 2.15 – Finite element model of the bridge (Schlune et al. 2009) ...............29 Figure 2.16 – Test setup arrangement (Han et al. 2008) .......................................32 Figure 2.17 – Test results from lateral load v displacement (Han et al. 2008) ......33 Figure 2.18 – Specimen geometry (McCarthy et al. 2005) ....................................36 Figure 2.19 – Finite element model (McCarthy et al. 2005) ..................................36 iv
Figure 2.20 – Modified gripping boundary conditions (McCarthy et al. 2005) .....37 Figure 2.21 – Test rig setup (McCarthy et al. 2005)...............................................38 Figure 2.22 – ISO tank container (Fahy and Tiernan 2001) ...................................39 Figure 2.23 – Geometry created with ANSYS (Fahy and Tiernan 2001) ................40 Figure 2.24 – Meshed model (Fahy and Tiernan 2001) .........................................41 Figure 2.25 – Single span slab deck (O’Brien and Keogh 1998) .............................42 Figure 2.26 – Up-stand FE model (O’Brien and Keogh 1998) ................................42 Figure 2.27 – Overlapping valid ranges of element types (Akin 2012)..................44 Figure 3.1 – Beam test rig setup ............................................................................49 Figure 3.2 - Cross section dimensions (mm) and strain gauge locations ..............49 Figure 3.3 - Experimental test rig setup schematic ...............................................50 Figure 3.4 – Stress/strain curve (Beal 2000) ..........................................................52 Figure 3.5 - Second moment of area reference data ............................................54 Figure 3.6 – Position of x for moment expression .................................................57 Figure 3.7 – Experimental setup ............................................................................59 Figure 3.8 – Beam discretised into 4 elements and 5 nodes .................................59 Figure 3.9 – Numbered system variables ..............................................................60 Figure 3.10 – Beam element stiffness matrix (Djafour et al. 2010).......................60 Figure 3.11 – Three hinged arch bridge with transient loading ............................62 Figure 3.12 – Schematic view of bridge sowing main dimensions (mm) ..............62 v
Figure 3.13 – Free body diagram of arch bridge....................................................63 Figure 3.14 – Cylinder dimensions (mm) ...............................................................63 Figure 3.15 – Force transducer located at horizontal support ..............................64 Figure 3.16 – ANSYS analysis systems toolbox ......................................................67 Figure 3.17 – Static structural stand alone system................................................68 Figure 3.18 – Von Mises stress criterion (Bolognese 2012) ..................................69 Figure 3.19 – Von Mises yield envelope (Bolognese 2012) ...................................69 Figure 3.20 – ANSYS workbench project schematic screenshot ...........................70 Figure 3.21 – ANSYS design modeller screenshot .................................................72 Figure 3.22 – Extruded beam .................................................................................73 Figure 3.23 – Meshed beam ..................................................................................74 Figure 3.24 – Solid 186 element ............................................................................74 Figure 3.25 – Solid 185 element ............................................................................75 Figure 3.26 – View of a quadratic hexahedron Solid 185 element in beam .........76 Figure 3.27 – Extruded solid structure...................................................................81 Figure 3.28 – Solid structure after meshing ..........................................................82 Figure 3.29 – Remote displacement support 1 .....................................................84 Figure 3.30 – Remote displacement support 2 .....................................................84 Figure 3.31 – Body parts 1 and 2 ...........................................................................86 Figure 3.32 – Body parts 2 and 3 ...........................................................................87 vi
Figure 3.33 – Experimental setup ..........................................................................87 Figure 3.34 – Revolute joint connection No's 1 & 2 ..............................................88 Figure 3.35 – MPC-184 revolute joint (ANSYS) ......................................................89 Figure 3.36 – 3-D model after meshing .................................................................90 Figure 3.37 – First load stage applied to bridge deck ............................................93 Figure 4.1 – Graphical representation for test No. 1 .............................................95 Figure 4.2 - Graphical representation of experimental load versus strain for test No. 2 ...........................................................................................................96 Figure 4.3 - Graphical representation of experimental load versus strain for test No. 3 ...........................................................................................................97 Figure 4.4 - Graphical representation of experimental load versus strain for average values............................................................................................98 Figure 4.5 – ANSYS compressive strain graphic, updated model ........................102 Figure 4.6 – Maximum compressive strain values...............................................103 Figure 4.7 – ANSYS tensile strain graphic, post-updated ....................................105 Figure 4.8 – Maximum tensile strain values ........................................................105 Figure 4.9 - % Variation between experimental strain gauge readings and theoretical values .....................................................................................108 Figure 4.10 – Modified maximum tensile strain values (Gauge 1) ......................109 Figure 4.11 – ANSYS maximum deflection graphic ..............................................111 Figure 4.12 – Maximum deflection values per load step ....................................112
vii
Figure 4.13 –Beam discretised into 4 elements and 5 nodes ..............................113 Figure 4.14 – Numbered system variables, degrees of freedom ........................117 Figure 4.15 – Deflection results using FE method maximum displacement .......118 Figure 4.16 – Mathematically computed deflections comparison ......................119 Figure 4.17 – First approach half arch .................................................................122 Figure 4.18 – Load located at 0.2m from centre .................................................123 Figure 4.19 – Resulting reaction for load at 0.2 meters ......................................124 Figure 4.20 – Von-Mises stress for load at 0.2m from centre .............................124 Figure 4.21 – Full bridge model ...........................................................................125 Figure 4.22 – Meshed connection at centre of bridge ........................................126 Figure 4.23 – Load positioned at 800mm from left end ......................................129 Figure 4.24 – Equivalent von-Mises stress for load location ...............................130 Figure 4.25 – Left and right hand support reactions graphic ..............................130 Figure 5.1 – Load versus strain experimental results ..........................................132 Figure 5.2 – Initial loading arrangement..............................................................134 Figure 5.3 – Resulting maximum compressive strain ..........................................137 Figure 5.4 – Resulting maximum deflection ........................................................137 Figure 5.5 – Applied moment ..............................................................................138 Figure 5.6 – Remote displacement supports 1 & 2 .............................................140
viii
List of Tables Table 3.1 - Second moment of area calculations ..................................................55 Table 3.2 – Sample material data for aluminium ..................................................71 Table 3.3 – Table of applied moments ..................................................................78 Table 3.4 – Structural steel material properties ....................................................80 Table 3.5 – Tabular data for supports ...................................................................83 Table 3.6 – Centre hinge revolute joint data .........................................................91 Table 3.7 – Remote displacement support details ................................................92 Table 4.1 – Experimental strain values for test No.1 ............................................95 Table 4.2 – Experimental strain values for test No.2 ............................................96 Table 4.3 – Experimental strain values for test No. 3............................................97 Table 4.4 – Experimental strain values averaged ..................................................98 Table 4.5 – Experimentally derived Young’s modulus ...........................................99 Table 4.6 – Theoretical strain values for Young’s modulus of 64GPa .................100 Table 4.7 – ANSYS produced minimum elastic strain ..........................................101 Table 4.8 – Compressive strain comparison ........................................................103 Table 4.9 – ANSYS maximum principal elastic strain ...........................................104 Table 4.10 – Tensile strain comparison ...............................................................106 Table 4.11 – Modified tensile strain comparison ................................................110 Table 4.12 – ANSYS total deformation results .....................................................110 ix
Table 4.13 – Deflection comparison ....................................................................112 Table 4.14 – Element stiffness matrices ..............................................................114 Table 4.15 – Combined structure stiffness matrix ..............................................115 Table 4.16 – Structure stiffness matrix multiplied by EI ......................................115 Table 4.17 – Computed 10 x 10 inverse matrix ...................................................116 Table 4.18 – Constants for use in FE method (example values) ..........................116 Table 4.19 – Results from FE method maximum displacement ..........................117 Table 4.20 – Required table of values .................................................................118 Table 4.21 – Results from double integration method .......................................119 Table 4.22 – ANSYS element summery ................................................................120 Table 4.23 – Pre-updating isotropic elasticity .....................................................121 Table 4.24 – Updated isotropic elasticity ............................................................121 Table 4.25 – Horizontal reaction force at right hinge (N) ....................................121 Table 4.26 – Horizontal and vertical model results .............................................123 Table 4.27 – Bodies summery ..............................................................................127 Table 4.28 – Element type summery ...................................................................127 Table 4.29 – Material constants ..........................................................................128 Table 4.30 – Isotropic elasticity ...........................................................................128 Table 4.31 – Reaction force results from FE model .............................................128 Table 5.1 – Initial load and support values ..........................................................135 x
Table 5.2 – Point loads 1 & 2 stepped load values ..............................................136 Table 5.3 – Applied moment at left end ..............................................................138 Table 5.4 – Mathematically calculated force reactions .......................................141 Table 5.5 –Maximum reactions at left hand support ..........................................142 Table 5.6 – Minimum reactions at left hand support ..........................................143 Table 5.7 – Maximum reactions at right hand support .......................................143 Table 5.8 – Minimum reactions at right hand support........................................144
xi
Molloy 2012
1. Introduction This dissertation aims to develop, calibrate and verify finite element (FE) models of certain types of structures present in the Heavy Structures Laboratory within Athlone Institute of Technology. The accuracy in representing the real structure geometry, supports and loading systems applied in the finite element model are essential in achieving accurate results in a structural design process. The structural analysis finite element code used was ANSYS which was available to use at the institute. Model verification procedures are important especially when designing large scale structural elements that depend on the integrity of the component to keep the structure from collapse. Developing the finite element model in whichever code is a process that needs to be carried out by an analyst having a good understanding of structural mechanics concepts in order to competently design a structure or structural element. Background checks are essential and the use of test structures can verify the FE model output results. In the absence of a test structure, mathematical procedures can indicate whether or not the model results are of the correct magnitude or sense. This dissertation looks at both the test structure and some mathematical procedures for validation and subsequent updating of FE models. Chapter 2 looks at some literature on uses of the finite element method (FEM) as a structural design tool and the background to its origin. Some basic structural concepts are explained in the lead up to a simple example of a basic finite element procedure. The uses of model updating are looked at and the validation, verification and calibration procedures that are often employed when utilising finite element analysis software. Chapter 3 outlines the methodology used which is divided into 2 sections. The first deals with the experimental setup of both structures while the second describes the methodology employed for the development of each finite element model in ANSYS. 1
Molloy 2012 Chapter 4 is the results chapter which produces the results from the experimental setup, mathematical calculations and results from the finite element modelling. Chapter 5 is a discussion chapter where the results from each experimental setup are compared to the original finite element model and the updated models. Results are compared in graphic form and a comparison in percentage form is produced as to how the updated model compared to the pre-updated and experimental setup. Finally the dissertation conclusions are stated and some recommendations for further study are produced in Chapter 6.
2
Molloy 2012
2 Literature Review 2.1
Introduction
Structural analysis is a procedure performed by engineers in order to evaluate maximum loading that can be applied to a structure for example, static and dynamic loading on a bridge, lateral wind loading on a wall or bridge truss reactions to loading. Many methods of analysing structures have been developed over the years and slow tedious hand calculations can sometimes be large and complex. In recent years a new method, the finite element Method (FEM), has been developed and speeds up the process of structural analysis coupled with the use of increasingly powerful computers which is accelerating the process even further. A review of literature from published books and scientific journals is presented in this chapter of the possible variations in producing finite element models and the results of forces obtained from finite element analysis software packages, the verification of these results and the methods of model updating that are used to calibrate the original models to act more like the real situation. Commencing with a brief history as to how the method came about and then an explanation of the basic structural concepts adopted by the method is reviewed. As many text books refer to the finite element method in the same manner they do have some different methods of explaining it. Once the fundamental theory behind the method is dealt with, topics covered will contain reviewed literature material on previously conducted experiments using the finite element method. There are many studies and journal articles published that deal with all of the above topics related to finite element analysis and the ones that relate to this project will be focused on in order to understand the task at hand.
3
Molloy 2012 2.2
Background to finite element analysis
The finite element method is widely used in structural analysis along with a wide use in a range of physical problems including heat transfer, seepage, flow of fluids and electromagnetic problems. Within this method, a continuum is idealised as an assemblage of finite elements with specific nodes where an infinite number of degrees of freedom (displacements, moments, or forces) of the continuum are replaced by specified known or unknowns at the node location (Ghali 2009). The use of the finite element method to solve engineering problems can be traced back to the early 1900’s when A.A. Griffith (1893–1963) introduced fracture mechanics while working on stress concentrations around elliptical holes in glass. By using strain energy equations and the interaction between internal elements within the structure of the glass he was able to compute the quantity of energy released for a specific crack depth (Roylance 2012). Also during that time some investigators were approximating and modelling elastic continua using discrete equivalent elastic bars. The finite element method (FEM) is a numerical procedure that can be applied to obtain solutions to many different problems that engineers in a wide range of study encounter. These problems may vary from steady, transient, linear or nonlinear problems in such areas as stress analysis, heat transfer, fluid flow and electromagnetism. It was not until 1943 that Richard Courant developed the mathematical method for an early version of finite element analysis. He used piecewise polynomial interpolation over triangular sub regions in the investigation of torsion problems by estimating unknown function values from known values at nearby points. Moaveni (1999) writes about what took place after Courant by explaining that the next significant step in the utilization of finite element methods was taken by Boeing in the 1950’s when they, followed by others, used triangular stress elements to model airplane wings. Yet it was not until 1960 that Professor Ray W Clough made the term “finite element” popular.
4
Molloy 2012 In a speech by professor Ray W Clough entitled ‘Early History of the Finite Element Method from the Viewpoint of a Pioneer’ Clough (2004), in which Clough addresses the Fifth World Congress on Computational Mechanics (WCCM V), he comprehensively discusses the subject of the FEM and its origin. In his speech Clough explains how he came upon problems with the analysis of the vibration properties of a large ‘delta’ wing structure that had been fabricated in the Boeing workshop. He was working in a Boeing summer faculty job in June of 1952 at the time. The problem he faced was different in that standard beam theory applied to typical aircraft wing stress analysis but could not be applied to this ‘delta’ wing design. It was this problem that prompted Clough to formulate a mathematical model of the ‘delta’ wing in which he represented it as an assemblage of 1 dimensional beam components. The results were disappointing and it was not until 1953 that his boss, John Turner, suggested using an assemblage of 2 dimensional plate elements connected at the corners to evaluate the vibration properties of the ‘delta’ wing. This concept was the essential definition of the FEM. From there Clough went on to derive stiffness matrices for these 2 dimensional elements with corner connections and indeed extended them to triangular plates also. With using the assemblage of triangular elements being the more accurate representation of the ‘delta’ wing structure Clough was able to get good agreement between the results of mathematical model vibration analysis and those measured with a physical model in the lab. He discovered as the mesh of triangular elements was refined the results of the model converged with those of the physical laboratory test results. The coining of the name ‘Finite Element Method’ was to come thereafter. During the 1960’s, investigators began to apply the finite element method to other areas of engineering, such as heat transfer and seepage flow problems. Zienkiewicz and Cheung (1967) wrote the first book entirely devoted to the finite element method. To understand the method we must appreciate some basic structural concepts.
5
Molloy 2012 2.3
Fundamental structural concepts
In order to understand the principles behind the finite element method we must take a look at some basic structural concepts, relating specifically to deflections of structures and some simple stress/strain relationships when external loads are applied to a structure of a given material and size. Any external loading causing a force on a structure will have results. Kong (1997) says that in any structure the application of some general force system consisting of both independently variable actions and some dependent reactions will produce both a system of internal actions and a pattern of deformation. All points in the structure will move (unless prevented by some postulated external restraint or by some unexpected combination of effects) and calculations must involve consideration of the three vector systems of actions (applied forces), internal actions and displacements, which sums up the basis of a large section of structural analysis by containing within it reference to Newton’s three laws of motion which are: 1.
Every object in a state of uniform motion tends to remain in that state of
motion unless an external force is applied to it 2.
The relationship between an object's mass m, its acceleration a, and the
applied force F is F = ma. Acceleration and force are vectors (as indicated by their symbols being displayed in slant bold font); in this law the direction of the force vector is the same as the direction of the acceleration vector 3.
For every action there is an equal and opposite reaction
With this in mind it is possible to move forward to examining the effect of a force on a structure of certain material, with elastic properties.
6
Molloy 2012 2.3.1 Material stiffness Within the method of finite element analysis there lays a fundamental property of a material which is an integral part of any structural member. This property is the stiffness of the member. A significant relationship between the stress ( and strain (
)
is stated by Kong (1997) relating to Robert Hooke’s
experimental observations which it is known, for example, that if a rectangular block is subjected to uniformly distributed normal stresses σx, then the normal strain εx which occurs as a result of the application of σx is proportional to σx. Stress and strain are linked by Young’s modulus which is a material property and varies with each material.
7
Molloy 2012 Each different material will have a different Young’s modulus as they will strain at different levels of stress as a result of an applied force. Figure 2.1 shows a graphical explanation of Young’s modulus and some common material values.
Figure 2.1 – Explanation of Young’s modulus (Hyperphysics 2012)
Any material that contains elastic properties and obey Hooke’s law will have the relationship between stress and strain as explained in section 2.3.1, this will lead to the approximate behavioural assumption that when the average stress in a member is σ then:
σ = where F is an applied force and A is the cross section of an element,
and the average strain:
ε=
where ΔL is the change in length and L is the original length of the
element. Since the relationship over the elastic region governed by Hooke’s law by the equation:
σ = Eε, then the combination of these equations will give:
F=
8
Molloy 2012 If we compare this equation with the equation for a linear spring which takes the form:
F = kx where k is a spring constant, x is the extension and rearranging the
previous equation to state that:
K=
K in this equation is known as the stiffness of a member and as can be seen that there is a relationship between cross-sectional area A, Young’s modulus E and the member length L. This will play an important role in the FEM and will form the basis for the matrix stiffness method which is used widely in finite element analysis (Moaveni 1999).
9
Molloy 2012 2.3.2 Principle of superposition An important principal in using finite element analysis for the basis of this project, i.e. linear elastic, 2 dimensional analyses, will be the principle of superposition. Caprani (2007) identifies the principle of superposition as for linear elastic structures, to be the load effects caused by two or more loadings, are equal to the sum of the load effects caused by each loading separately. He moves on to identify some limiting conditions namely: 1.
Linearly behaving material only
2.
Structures that undergo very small deformations only
It is worth noting that for this project, deformations of individual members will not be added into the calculations nor will they be considered when establishing the FE model using the software thus the principle of superposition will apply. The analysis of a structure by the finite element method is an application of the displacement method. In frames, trusses and grids, the elements will be bars connected at the nodes; these elements are considered to be one dimensional (Ghali 2009).
10
Molloy 2012 2.3.3 Virtual work The process of finding deflections and force reactions by the finite element method is fine when dealing with bars which consist within the method exact element matrices which cannot be generated. The displacements within the elements are expressed in terms of displacements at the nodes. To establish element matrices in these cases, the use of assumed displacement fields where the corresponding strains are determined by differentiation and the stresses by Hooke’s law. Here the use of the principle of virtual work with respect to nodal displacement gives the desired nodal displacement (Ghali 2009). When the elements become very small, the nodal displacements approach the actual displacement field. In practice, the element sizes are finite, not infinitesimal; hence the name finite element method (Imechanica 2012). Kong (1997) while describing the principle of virtual work relates the application to any structure of a generalised force system that can be represented by a vector force P will produce both a reaction system accompanied by an internal stress system characterised by a vector σ. There are several key components of any structural analysis:
Equilibrium equations (conservation)
Kinematics and compatibility requirements
Constitutive relations
Boundary conditions
There are straightforward ways of deriving equilibrium equations and compatibility requirements, but solving the resulting equations is not easy (maybe not even possible) for most realistic engineering structures. Hence, alternative ways of describing the requirements for equilibrium and compatibility have been devised that are easier to work with. Two of these ways are based on an imaginary (virtual) disturbance of a body that is in the deformed state (i.e. loaded). They are: 11
Molloy 2012 1.
The principle of virtual work => alternate way to describe equilibrium
requirements 2.
The principle of complementary virtual work => alternate way to describe
compatibility requirements
2.4
Finite element direct stiffness method for framed structures
The direct stiffness method is the most common implementation of the finite element method. Most commercial computer packages utilize the direct stiffness method (DSM). The following example taken from Colorado (2012) and explains the stiffness method quite well. To keep calculations to minimum a simple a three member truss is used as seen in Figure 2.2 below.
Figure 2.2 – Three-member example truss (Colorado 2012)
To make the transition from the frame truss to the mathematical model it will be necessary to rename the overall body ‘parts’. This will result in calling individual members as ‘elements’ and the joints being termed ‘nodes’. To keep the 12
Molloy 2012 housekeeping in order it is necessary to set up a co-ordinate system, a global system as pictured in red in Figure 2.2. This will be the master co-ordinates that will represent deflections of nodes in either the x or y direction. Within the frame an element axis co-ordinate system must also be established for local deflections. The breakup of the frame into individual elements is known as ‘discretization’ and can be seen in Figure 2.3. This is sometimes known as the breakdown stage or disconnection stage.
Figure 2.3 – Disconnection step (Colorado 2012)
At this stage it is possible to compute the stiffness matrixes for each element based on its area and modulus of elasticity, both of which are individual material properties. It can be seen from Figure 2.3 given the supporting conditions that there can be no displacement at node 1, horizontal displacement at node 2 and the possibility of both horizontal and vertical displacements at node 3. The pin at node 1 will have no displacement assuming that the pin is attached to infinitely stiff grounds. Figure 2.4 describes the fundamental principle that allows the numerical values to be assigned to the matrix. As shown in Figure 2.4, a generic plane truss member has four joint force components and four joint displacement components (the member degrees of freedom). The member properties are 13
Molloy 2012 length L, elastic modulus E and cross-section area A. In this member the local axis of the element lies in the same plane as the global axis. This will result in any local displacements in the x and y local direction will be transferred without any change to the global directions. The frame shown in Figure 2.3 will have three node locations and there are 2 degrees of freedom (DOF) at each node so that leads to a 6x6 matrix.
Figure 2.4 – Generic truss member (Colorado 2012)
2.5
Matrix representation
If the truss member in Figure 2.4 were to be connected firmly to a support at one end and pulled by a force at the other, with the member having a constant cross section and a member stiffness k, of
then based on the theory explained
earlier the force applied can be written as F = k x ΔL. Since the member cannot displace, say at i, then the two remaining displacements at j can be written in matrix form. The matrix for this frame will be in the order of:
A 1x6 matrix for the forces
A 6x6 matrix for the structure stiffness and
A 1x6 matrix for the displacements.
14
Molloy 2012 If the stiffness matrix for each individual element (member in this case) can be computed then the overall structure stiffness will be the summation of each of the individual element matrixes. Solving for the unknowns will solve the variables in the system such as deflections and forces. A solution can be found for the unknowns based on having some known values at node locations thus leading to a set of simultaneous equations which are easily solvable. The process becomes more complicated when variations in material properties are introduced and with the increase in member numbers. If a third dimension is added then the process is too complex to be undertaken by hand and a computer is needed to deal with the large number of calculations involved. The method outlined above is ideal for trusses and can lead to direct solutions for deflections and forces, however, to analyse a continuous medium such as a plate to compute stresses within it, further techniques need to be adapted.
2.6
Continuous medium finite element method
When an ‘I’ beam is subjected to loading from either a point load or uniformly distributed load its web is immediately under stress. These stresses are experienced throughout the web of the beam. The centre section of the beam resembles a steel plate subjected to the applied forces which may be acting in any direction on the beam. The structure then can be seen as a continuum and not as an assemblage of discrete elements connected at nodes, making it impossible at first glance to apply the same techniques as previously explained. The finite method of idealising a continuum as a connection of triangular plates can be attributed to R. Clough while he worked with Boeing in the 1950’s analysing stresses induced in airplane wings. The assembly of triangular plates proved to have a great advantage in analysing the ‘delta wing’. Clough (2004) states “Moreover, the derivation of the in-plane stiffness of a triangular plate was far simpler than that for a rectangular plate, so very soon I shifted the emphasis 15
Molloy 2012 of my work to the study of assemblages of triangular plate ‘elements’, as I called them” The steps involved in this method are as follows: 1.
Idealization of the structure, where the plate is idealized as a gathering of
a large number of discrete elements connected only at the nodes 2.
Specifying the relation between the internal displacements of each
element and the nodal displacements (based on a mathematical displacement function relating to expected deformation patterns) 3.
Using standard matrix stiffness methods, the analysis of the idealized
assemblage of discrete elements is performed The process for deriving stresses and stain values over the assemblage of finite triangular elements involves the placing of virtual loadings in order to establish element stiffness matrixes and is complex. Figure 2.5 below shows a typical bracket used in an engine block. The triangular elements are visible as a superimposed mesh onto the geometry of the shape being analysed.
Figure 2.5 – Triangular mesh applied to a bracket (VKI 2012)
16
Molloy 2012 Each individual element acts like a plate and will have similar physical properties as the material being tested. The elements here are most likely 3D tetrahedrons.
2.7
Model analysis
Structural analysis must depend on the idealization of structural form and the various aspects of material behaviour, in order that both maybe reduced to a form which permits handling by the computational methods available. It is obviously true that the form of computing equipment available influences the type of problem which may be tackled. The existence of the computer allows us to tackle more complicated structures than would be possible with conventional alone. It is less obvious, but equally true, that the extended computing facilities now available, and the ease of calculation which they imply, allow computations to be made with several different idealizations to determine which represents most adequately the behaviour of the structure. It would frequently be helpful, however, to have a model of the structure available in order that its behaviour under load could be readily ascertained and there are cases (even in the structure in which linear behaviour can be assumed), in which the model can provide the most ready answer to a problem of analysis. These models take two forms, depending on the method of use and of interpretation of the results, they are a) direct methods and b) indirect methods as referred to by Kong (1997)
17
Molloy 2012 2.8
Development of finite element models
Finite element analysis (FEA) or the finite element method (FEM) is a process for finding a numerical solution to a field or global problem. These field problems might consist of finding the distribution of heat in an engine or distribution of displacements in a concrete slab. For this project FEA will be used for the calculation of stress distributions within structural elements like beams and bridge decks along with associated deflections. Mathematically a field problem is described by differential equations or by an integral expression, of which are made up of the collection individual elements. Either description may be used to formulate finite elements. Finite elements formulations, in ready-to-use form, are contained in general purpose FEA programs. It is possible to use FEA programs while having little knowledge of the analysis method or the problem to which it is applied, inviting consequences that may range from embarrassing to disastrous, as stated by Cook (2002). Cook also explains that to understand the method one must visualize a structure not as a single entity but as a collection of individual finite elements. The term finite alludes to the elements having known measurable physical properties, like length, mass, thermal conductivity and thickness etc. with measurable quantities of deflection or stress among others, as opposed to infinite quantities apportioned within calculus. Within each of these individual elements a field quantity is only allowed to have a simple spatial variation which might be described in terms by polynomials terms up to x2, xy and y2. In this simple case x and y might be horizontal or vertical global deflections of a node within a truss frame. In general the variation in the region that is affected by a single element is much more complicated to solve and this is where FEA provides approximate solutions close to the true overall variation. However, the basic principles underlying the finite element method are simple when you consider a body in which the distribution of an unknown variable such as displacement is required. The difficulty arises when a body has many parts to it. This leads to a multiple of calculations and is time consuming by hand therefore the use of a computer program to do the calculations is superlative. 18
Molloy 2012 In order to represent a real structure to perform finite element analysis upon a mathematical model must be developed. The accurate representation of any structure, by a model which is to be analysed, depends on the type of finite element model used to represent the structural members and the structural properties assigned to the elements (ZĂĄrate and Caicedo 2008). A similar model is developed for the project undertaken in this dissertation, conducted by Chan et al. (2002) who conducts an experiment where beams of different formations of web design are loaded to failure and the results are compared to that of a FE analysis model. In this study the authors propose testing beams with a plane web, vertically and horizontally corrugated webs and the results obtained from both the experimental and finite element methods are compared to verify the finite element models created and to see if it could closely reflect the behaviour of such beams in the real condition. The various types of webs are pictured in Figure 2.6 below.
Figure 2.6 – Cross section of corrugated webs (Chan et al. 2002)
The sections shown in Figure 2.6 are the geometric shapes of the different web configurations with the FE model mesh pictured in Figure 2.7 below.
19
Molloy 2012
Figure 2.7 – FE mesh representation of beams (Chan et al. 2002)
The finite element model for type VCR is shown in Figure 2.8 below.
Figure 2.8 – Finite element model (Chan et al. 2002)
20
Molloy 2012 It can be seen that the developed FE model is represented as series of trigonometrical shapes which are all joined at points called nodes. Note that there is in an increased number of elements at turning sections which will refine the resulting data an increase convergence on the true value of stress at these locations. It is possible to modify the mesh concentration at sensitive areas; however, this can lead to a demand on computing power as the calculations become quite large. The accurate development of the model will reflect in the results obtained. With the FE model developed the test rig is setup to manually test each specimen and record actual deflections and stresses. This resulting measured data is then used to calibrate the FE model. The test rig is pictured below in Figure 2.9
Figure 2.9 – Experimental setup (Chan et al. 2002)
21
Molloy 2012 Son and Fam (2008) develop a non-linear FE model to study the flexural behaviour of hollow and concrete filled fibre reinforced polymer tubes. The model is developed to account for the geometric and non-linearity of the tubes and the material to predict the flexural behaviour of both the fibre reinforced polymer and concrete filled tubes. The model is developed using the FE analysis program ANSYS, which will also be used for this dissertation. The authors explain that a finer mesh was used around the lower part of the pole where failure was expected and gradually changed to a coarser mesh further away to the top of the pole, accomplished by using the automatic meshing capabilities of the computer program. The development of the model to represent reality as much as possible is also explained in the simulation of the translation and rotational degrees of freedom being restrained along the bottom base of the pole, to mimic a fixed support condition.
2.9
Model updating
FE models of structures are usually created by simplifying the real structure from engineering drawings and designs. This simplification process my not exactly represent fully all of the physical aspects of the original structure. For these situations the finite element model would need to be calibrated by modification of the inaccuracies and the possible elimination of such discrepancies wherever possible. The lesser the level of discrepancy then truer model results can be predicted. This process is termed ‘model updating’. Updated finite element models still need to be verified by comparing the calculated results of the updated model with experimental data so as to address the extent of differences between the final model and the true value of the structure (Chan et al. 2009). Model updating can extend from relatively simple models that represent a simple truss or beam structure in a static two-dimensional analysis to vey complex dynamic three-dimensional structural analysis problems. It is difficult to find literature on some of the basic updating techniques for simple problems as much of the material published focuses on results of vibration analysis and 22
Molloy 2012 dynamic responses by structures which are highly mathematical in nature and maybe beyond the scope of this project. However, creating a model of a simple structural setup for analysis can entail some parameters which might need to updated in the model such as Young’s modulus, fabrication errors, connection stiffness, possible non-linearity of materials and so forth. Existing FE models can be updated based on test data. The initial model data used to design a bridge structure may represent the material properties and structural response for the bridge in the early years of its existence. As time passes however these properties might deteriorate and structural damage may be caused to the structure. Maintenance, upgrading, repair, and replacement of bridges may lead to high costs and considerable disruption of traffic. For effective bridge management, accurate and reliable information about the safety and condition of bridges is essential. In current practice, however, existing bridges are analysed and evaluated by means of highly simplified structural models. Structural models that are verified, refined, and tuned with respect to actual measurements can reduce these uncertainties and provide a better basis for management decisions. Schlune et al. (2009) explain that FE model updating can be deceptively simple for small amounts of experimental data when a large amount of uncertain structural parameters exist. This could lead to the risk of having an undetermined or ill-posed problem, in which there might be several non-unique solutions. It is for this reason that a large amount of experimental data is required to effectively update the FE model. It is noted that physical phenomena might have to be introduced into the model to obtain a more realistic description of what is going on in reality. The finite element method and the models involved have become a widely used tool in structural mechanics and dynamics, reproducing numerically the static or dynamic reaction of a structure to the real effects of loading systems. The values used in the FE model are derived to replicate the physical parameters and are usually taken from previous tests or experiences similar to the current model. Model updating consists of estimating some parameters of the model on the 23
Molloy 2012 basis of similar dynamic testing on actual corresponding structures (Zapico-Valle et al. 2010). In a study carried out by Chan et al. (2009) the sensitivity based parameter model updating procedure as applied to model updating concurrent multi-scale model of structural behaviour of civil infrastructure and was successfully implemented on a steel truss which formed the basis for their study entitled ‘Concurrent multi-scale modelling of civil infrastructures for analyses on structural deteriorating—Part II: Model updating and verification’. In this study, dynamic and static load responses were recorded and a multi-scale FE model created. The method for model updating of a steel truss in the laboratory subjected to similar loading was applied to the model for predicting stresses at locations of the Runyang cable-stayed bridge. More traditional model updating techniques optimize an objective function; that is they limit a series of equations to get the best result that fit a mathematical expression, in order to calculate one single optimal model that replicates the behaviour of the real structure and represents the physical characteristics of that structure. Two examples of model updating are reported on by Zárate and Caicedo (2008) in a paper called ‘Finite Element Model Updating: Multiple Alternatives’ the first is not of relevance here but the second identifies model updating alternatives for a finite element model of the Bill Emerson Memorial Bridge. The proposal in this paper was to create a set of models which hold similar dynamic characteristics but are physically different and depending on the final use the analysis can decide on one or more models for further analysis. This method relies on the experience of the analyst to make an informed decision as to which model best suits the real setup. Open to traffic on December 13, 2003, the Bill Emerson Memorial Bridge is a 1206 m long cable-stayed structure. It carries four lanes of vehicular traffic along Missouri State Highway 34, Missouri State Highway 74 and Illinois Route 146 across the Mississippi River between Cape Girardeau, Missouri, and East Cape Girardeau, Illinois. The bridge consists of 128 cables, two longitudinal stiffened 24
Molloy 2012 steel girders, and two towers in the cable-stayed spans, and 12 additional piers in the Illinois approach span. In addition to four pot bearings at two towers, the superstructure of the cable-stayed span is constrained to the substructure with 16 longitudinal earthquake shock transfer devices at two towers, four tie-down devices at two ends of the cable-stayed span, and six lateral earthquake restrainers (UTC 2012). There are many methods for updating FE models, in essence the physical variables can be measured at several locations on a structure that is being modelled and recorded in real time during testing. This data can be transferred to the model in such a way that discrepancies between the experimental data and the computed predictions of the model are minimized thus leading to a more realistic result from the model. Any discrepancies between FEA results and reference data e.g. test result data, can be due to uncertain available physical data. Governing physical relations like modelling non-linear behaviour within the finite element model coupled with inaccurate boundary conditions will lead to the creation of errors in the FE results. There exists many different types of model updating techniques and many articles have been published on the various methods, though most are related to dynamic modelling using the finite element method. In a study by Zapico-Valle et al. (2010), a new method of finite element model updating of a small scale bridge was attempted. The model was created and a corresponding prototype of the experimental model of a multispan continuous deck motorway bridge with four identical spans with an irregular distribution of the bridge piers. The scaled bridge was tested for its reaction to seismic activity by subjecting it to movement on a shaking table. Figure 2.10 shows the experimental model on the shaking table.
25
Molloy 2012
Figure 2.10 – Elevation of the experimental modal (Zapico-Valle et al. 2010)
In this study minimisation of an error function in the time domain is carried out by a novel adaptive sampling algorithm. A different model updating technique is described by Esfandiari et al. (2010) as the utilization of the Frequency Response Function (FRF) and measured natural frequencies as part of a structural damage detection method. Using a non destructive technique to identify damage to a an existing structure the authors study the structural model updating using FRF data and measured natural frequencies of the damaged structure while not enlarging the measured data or reducing the finite element model. This process involves the excitation of a structure and recording the response of the structure to the excitation frequency. Each part of the structure will have a distinctive natural frequency and frequency response function, thus a change in the response function of the tested structure is correlated to change of stiffness, mass and dampening through a change in measured frequencies of the damaged structure. The effect of excitation frequencies on finite element modelling has been successfully addressed through a truss model example which the authors describe in the article. Figure 2.11 and Figure 2.12 below show the geometry of the truss used and the nodal degrees of freedom respectively.
26
Molloy 2012
Figure 2.11 – Truss geometry (Esfandiari et al. 2010)
Figure 2.12 – Degrees of freedom of model (Esfandiari et al. 2010)
A two stage finite element model updating method presented by Wu and Li (2006) in which the authors use the procedure for structural parameter identification and damage detection of a steel structure, seen here in Figure 2.13, using ambient vibration measurements. The first stage focuses on the structural parameter identification for the benchmark structure by the finite element updating approach. The steel structure in question is phase II of the IASC-ASCE benchmark steel frame structure which is a four-storey; two-bay by two-bay steel framed scaled structure built by the Earthquake Engineering Research Laboratory at the University of Colombia.
27
Molloy 2012
Figure 2.13 – Steel framed scaled benchmark structure (Wu and Li 2006)
A methodology for FE model updating proposed by Schlune et al. (2009) where the choice of measurements, model simplifications, accuracy and reliability of updated parameters and the analysis of untested load conditions were examined. The importance of modelling errors, other than model parameters, was highlighted. The article refers to the complete procedure of modifying a FE model to better correspond to measured data by methods including manual model refinement which describes all types of changes which are introduced manually into the model. In the article a FE model updating through non-linear optimization is proposed by minimising an objective function. Typical uncertainties commented on are where elastic modulus is used as a parameter to model the stiffness changes of a bridge deck in any direction, which is used to summarise effects, such as the railing system and the asphalt layer, on the structural performance of the bridge which will lead to uncertainties. Four multiresponse objective functions for FE model updating were proposed and tested in 28
Molloy 2012 the article where modelling the behaviour of the bridge bearings proved it was not possible to use the same data for static analysis as dynamic analysis for the updating procedure. The model updating methodology was applied to the Svinesund Bridge, which connects Norway and Sweden across the Ide Fjord diagrammatically pictured in Figure 2.14 with the FE model of the bridge pictured in Figure 2.15 below.
Figure 2.14 – Elevation of the Svinesund Bridge (Schlune et al. 2009)
Figure 2.15 – Finite element model of the bridge (Schlune et al. 2009)
29
Molloy 2012 2.10 Model validity and verification The development of FE models is a means of predicting future performance of a structure be it a displacement, moment, stress or reaction to some applied force or force system. The question could be asked then as to how accurate the model is performing to the real life action or reaction of the structure. This will depend on how valid the model is and how well it replicates the given situation. In a study on The National Cathedral, Washington, DC, by Hinojoso (2010), the vibration response of arches is experimentally measured to assess the effect of structural damage. The measurements provide acceleration time series which are then used to verify and validate predictions of the numerical simulation. They refer to model validity saying that when a FE analysis model reproduces a match to a set of physical evidence from tested results, the model is typically considered validated. However, when there is disagreement between model predictions and physical evidence, the numerical model can be calibrated. Korunovic (2011) attempts to validate the results of a FE model of a tyre steady rolling on a drum relating to cornering and braking behaviour, the use of a specially developed Computer Aided Design (CAD) package to create geometry and propagate it to the FE model proved suitable to their study. Two FE models were used and were performed in FE code ABAQUS. The CAD model contains a parameterized network of lines and points while following the dimensional changes of the tyre profile and its structural components, this forms the basis for the mapped finite element mesh. In this study the authors claim that the results of the finite element analysis conducted on the model have been directly compared to experimental results, thus validating the model to a certain degree. The equipment used and the methods for the experimental determination of breaking and cornering characteristics of the tire along with experimental determination of a friction coefficient were shown in the study. The results of the study show the difference between experimental and numerical results was smaller after the calibration of the friction coefficient had been included in the model. This would not have been possible to achieve had they not conducted a 30
Molloy 2012 physical experiment. It is assumed that if tire rolling behaviour is effectively modelled and verified on one kind of surface for a range of operating parameters, it may also be used to predict its behaviour in different road conditions. The use of a drum in this type of tyre performance testing takes up less space than flat testing systems leading to more efficient testing. The verification of the FEM used in this experiment proves the model to be effective and tyre design can be simplified further. Han et al. (2008) in comparison looks at the behaviour of composite frames made with square hollow sections (SHS) filled with concrete as column to steel beams. These types of frames are ideal for construction projects in areas of the world where there is a high risk of seismic activity. Also known as concrete filled steel tubular (CFST) columns they possess properties such as high strength and stiffness, large energy absorption and high ductility. They make reference in the study as to the complexity in modelling the concrete confinement effect for the concrete filled tubes leading to limited success in the development of an accurate model. In order for the authors to establish a valid model that would replicate the true properties, five components of the frame needed to be modelled. The components were; 1.
The confined concrete of the square columns
2.
The interface and the contact between the concrete and the steel tube
3.
The actual steel tubing (hollow steel section)
4.
The connection details between the column and the steel
5.
The actual steel beams.
Figure 2.16 shows the testing setup for the lateral loading by the MTS actuator. This is the physical setup and it is necessary to have a valid model to replicate the true parameters which can then be entered into the FEA software. 31
Molloy 2012
Figure 2.16 – Test setup arrangement (Han et al. 2008)
In addition to the physical setup being correctly modelled, the appropriate mesh must be applied to the model along with the correct element type, mesh size, boundary conditions and load applications to provide accurate and reasonable results which are important in simulating the behaviour of structural frames. In a paper presented by Han et al. (2008) entitled “Behaviour of steel beam to concrete-filled SHS column frames: Finite element model and verifications� it was seen that good agreement was achieved between the experimental curves from the lateral loading effects on displacement and the numerical curves produced by the FEM. Figure 2.17 shows how close the FEM predicted values for displacement were compared to the actual tested results.
32
Molloy 2012
Figure 2.17 – Test results from lateral load v displacement (Han et al. 2008)
It is also noted that some of the reasons for variations between the model results and the measured results which are caused at higher load levels, causing higher axially compressive loads and an increase in the effects of imperfections caused by unexpected fabrication imperfections in the testing setup, parameters that might not have been allowed for in the FEM. The finite element method is an approximation technique and thus will entail errors. For this reason researchers have designed several pathological tests to validate any new finite element analysis. The tests should be able to display most of the parameters which affect finite element accuracy. A representative set of tests should include patch tests, beam, plate and shell problems. Rao and Sharinvasa (2012) propose a problem set to help developers of finite element programs to ascertain the accuracy of particular finite elements in various applications. This problem set cannot however be used as a bench mark for cost comparison since the problems are too small for this purpose. Inaccuracies of the elements are brought in by the presence of spurious mechanisms, locking (excessive stiffness for particular loadings and or irregular shapes), elementary 33
Molloy 2012 defects like violation of rigid body property and invariance to node numbering etc. Parameters which affect accuracy are loading, element geometry, problem geometry, material properties etc. The member being analysed should be subjected to significant loadings and boundary conditions, for each type of deformation like: extension, bending, in-plane shear, out-of-plane shear and twist etc. 2.11 Model calibration The term model calibration refers to the process of adjusting the finite element model to better represent field test data. It is the result of the model updating process and is sometimes referred to as both in some literature. Kangas et al. (2012) use the process of generating a 3 dimensional finite element model then calibrating it to field test data. The results of the calibrated model are used to rate a represented bridge for the University of Cincinnati Infrastructure Institute (UCII) for condition assessment. The authors choose a bridge in Butler County, Ohio in America as a case study to illustrate the process. Bridge rating is very important because a failure to evaluate the health of a bridge correctly may lead to a catastrophe in the worst case. There is significant importance in defining model calibration in a larger context and trying to emphasise its role in relation to model verification and validation. The terms calibration, validation, and verification are used interchangeably in some literature, hindering the adequate communication of these principles. For clarification, the factors to which the accuracy of the FE solutions is dependent on are listed as: 1.
The adequacy of the governing equations involved in the analysis, i.e.,
mathematical definitions for dynamic behaviour of shells or plate elements 2.
The precision of numerical solution, i.e., fineness of discretization
3.
The accuracy of the physical parameters, i.e., values for material
properties and definitions for boundary conditions, and 34
Molloy 2012 4.
The adequacy of the constitutive element models, i.e., assuming linearity
only when the response is predominantly linear (Hinojoso 2010). Liu (2004) proposes an automatic calibration strategy for 3 dimensional FE models, going on to say that model calibration starts from a nominal bridge model and experimental data which is processed from a bridge field test and is then used for calibration reference. Many of the differences between experimental and analytic results are due to modelling limitations and experimental error, thus giving the reason why model calibration is needed to replicate current bridge structure conditions.
2.12 FE analysis studies A good example of a combination of the above topics is described in an experimental study of single lap composite bolted joints by McCarthy et al. (2005). The paper covers many of the topics previously discussed. In the paper the authors develop three-dimensional finite element models to study the effects of bolt-hole clearance on the mechanical behaviour of bolted composite joints. In this study a single-bolt, single-lap joint type model is constructed in the non-linear finite element code MSC Marc which is a powerful, general-purpose, nonlinear finite element analysis solution to precisely simulate the response of desired products under static, dynamic and multi-physics loading situations. It’s adaptability in modelling nonlinear material behaviours and transitory surrounding conditions make it ideal to solve complex design problems. The specific geometry of the joint is depicted in Figure 2.18.
35
Molloy 2012
Figure 2.18 – Specimen geometry (McCarthy et al. 2005)
The model mesh is displayed in Figure 2.19.
Figure 2.19 – Finite element model (McCarthy et al. 2005)
36
Molloy 2012 Five separate parts were meshed including:
Two laminates
Two washers, one top and one bottom
A combined nut-bolt
It can be seen that there is a high radial mesh density near the hole under the washer where high strain gradients exist. The increase in mesh density will cause a convergence on the true strains experienced at this location. The washers are modelled separately which has the disadvantage of increasing the model size due to the increase in number of elements. It does provide a more accurate representation of the real scenario though. The authors explain that improving the model to replicate the real situation improves the FE results. One of the examples of better modelling is representation of the clamped section of the plates illustrated in Figure 2.20
Figure 2.20 – Modified gripping boundary conditions (McCarthy et al. 2005)
It is seen that assuming a fixed nodal system on the surfaces of the plates where the grips are improves the FE model results and gives a closer result to that of the experimental data obtained.
37
Molloy 2012 The method for testing the joint stiffness is illustrated below in Figure 2.21.
Figure 2.21 – Test rig setup (McCarthy et al. 2005)
The main aim of the experiment was to study the effects of bolt-hole clearance on the mechanical behaviour of the joint. In their concluding remarks the authors explain that a valid model was developed and results verified by experimental testing in the lab. Efficiencies in the model were found to have improved by defining the contact bodies as sub-parts of the joint components to see which bodies would come into contact. The contact tolerance’s and the way in which they are modelled seem quite important. The results were also compared to other FE modelling packages such as ABAQUS and STRIPE. Fahy and Tiernan (2001) attempt to develop a valid FE model of the ISO tank containers which are used to transport bulk liquids by road, rail and sea and can contain volumes of 25,000 litres at any one time. The design of these tanks has arisen by trial and error, due to the lack of a definitive method to analyse the stiffness of the tank and frame. The main area of concern is where the tank is attached to the frame as this is difficult to analyse by traditional methods, with fatigue and vibration analysis being left to the manufacturer which can 38
Molloy 2012 sometimes mean excessively strengthened sections without any analysis. Using the computer package ANSYS 5.4 the authors model the tank container both statically and dynamically for road, rail and sea use. During the study the authors aim to:
Analyse the existing design to determine its safety
Validate the results by conducting static and dynamic tests
Improve the efficiency of the design
The typical ISO tank container is shown in Figure 2.22 and the geometric model created in ANSYS in Figure 2.23.
Figure 2.22 – ISO tank container (Fahy and Tiernan 2001)
39
Molloy 2012
Figure 2.23 – Geometry created with ANSYS (Fahy and Tiernan 2001)
The size of the tank diameter being 2.285m and length of 6.085m and comparing this to the thickness of 6mm indicated that plate or shell elements would give the best results from the FE analysis. Shell63 was chosen for the entire model and is the simplest shell element having four nodes and six degrees of freedom: translations in the x, y and z directions and rotations about the nodal x, y and z directions. Selection of an appropriate mesh is of paramount importance, starting with an initial course mesh and refining it in areas of interest with high stresses. The meshed model can be seen in Figure 2.24.
40
Molloy 2012
Figure 2.24 – Meshed model (Fahy and Tiernan 2001)
The results of the FE model and the verification of the results from testing by Fahy and Tiernan (2001) proved that a valid model had been developed and behaves in a similar manner to the actual tank however research is ongoing. The up-stand FE grillage analogy is used by O’Brien and Keogh (1998) in an effort to improve modelling of bridge decks with wide transverse edge cantilevers. Plane grillage analogy is a popular method with bridge designers modelling slabs in two dimensions, involving the idealisation of the bridge slab as a mesh of longitudinal and transverse beams located within the same plane. Assuming a constant neutral axis depth throughout, FE analysis is limited to planar analysis using plate bending elements similar to the plane grillage method. The slabs in this study have neutral axes of varying depth so applying the up-stand grillage analogy improves FE results. Figure 2.25 shows the single slab bridge deck with cantilevers and Figure 2.26 shows the up-stand grillage FE model of the bridge deck.
41
Molloy 2012
Figure 2.25 – Single span slab deck (O’Brien and Keogh 1998)
Figure 2.26 – Up-stand FE model (O’Brien and Keogh 1998)
To address the problem of a varying neutral axis elements of infinite flexural rigidity are placed between the edge cantilever and the base of the deck. Then depths of the elements were taken to be equal to the depth of the portion of slab which they represented. The up-stand FEA gave both bending moments and axial forces in each element ant the total stress value was arrived at by adding the stress components’ of each of each of these effects. The results compare well to three dimensional FE analyses. 42
Molloy 2012 2.13 Element type selection The previous examples of finite element modelling utilize many capabilities of the method ranging from simple, linear, static analysis to more complex, nonlinear and transient dynamic analysis. In order to correctly model the structure it is important to resemble it as accurately as possible in the computer program. This dissertation uses the FE modelling software ANSYS and for that reason the following section will use terminology associated with this package alone. ASNSYS element library contains over 150 element types which is very large considering most structural problems will only ever use a variety of 3 or 4 of these (Moaveni 1999). The most up to date version of ANSYS (release 14) utilises the workbench simulation software which is more user friendly that the classic programme (ANSYS 2012). ANSYS Workbench in itself is not a product, rather it is a product development platform and user GUI built for analysis needs with the objective of providing elegant next generation functionality and intelligent automation to the engineering community. The analysis used in this project contains the use of more than one type of element as the difference in the results will be analysed to see if they will mimic the true situation. With today’s advances in computing power there may seem never to be enough computational resources to solve all the problems that present themselves. Frequently solid elements are not the best choice for computational efficiency as a similar result may be obtained from the use of a 2D element and may save computing power demand. The person analysing the problem should learn when other element types can be applicable or when they can be utilized to authenticate a study carried out with a different element type. Solid Works Simulation offers a small element library that includes bars, trusses, beams, frames, thin plates and shells, thick plates and shells, and solid elements. There are also special connector elements called rigid links or multipoint constraints 43
Molloy 2012 however ANSYS element library is far more extensive. Shells and solid elements are considered to be continuum elements. Plate elements are a special case of flat shells with no initial curvature. Solid element formulations include the stresses in all directions and demand more computing power when solving. Shells are a mathematical simplification of solids of special shape. Thin shells (like thin beams) do not consider the stress in the direction perpendicular to the shell surface. Thick shells (like deep beams) do consider the stresses through the thickness on the shell, in the direction normal to the middle surface, and account for transverse shear deformations. It is important to choose the correct element type as to obtain the desired result depending on the analysis required. The following is a means of choosing a particular type of element. Let h represent the typical thickness of a component while its typical length is represented by L. The thickness to length ratio, h/L, gives some guidance as to when a particular element type is valid for an analysis. When h/L is large then shear deformation is at its maximum importance and solid elements should be used. Conversely, when h/L is small then transverse shear deformation is un important and thin shell elements are the most effective element choice. In the intermediate range of h/L the thick shell elements will be most effective. The thick shells are extensions of thin shell elements that contain additional strain energy terms. The overlapping h/L ranges for the three continuum element types are recommended in Figure 2.27.
Figure 2.27 – Overlapping valid ranges of element types (Akin 2012)
44
Molloy 2012 The thickness of the lines suggests that the regions where a particular element type is generally considered to be the preferred element of choice. The overlapping ranges suggest where one type of element calculation can be used to validate a calculated result obtained with a different element type. Validation calculations include the different approaches to boundary conditions and loads required by different element formulations (Akin 2012). 2.14 Unit Gravity Load check The Unit Gravity Loading validity check verifies that the model will provide accurate displacements and reactions forces under gravity loading. This is a good check to perform if a model will be used for quasi-static loads analysis. These are known as static analysis checks and can be performed simply and quickly to check a model. The resulting displaced shape should be inspected for its soundness in terms of whether or not any parts of the structure show any signs of suspicious displacements or dose the displaced shape look reasonable as expected under a unit load (NASA 1995).
2.15 Conclusion The literature reviewed here has described briefly the principles behind the finite element analysis method of analysing structures. Literature has been reviewed which covers the main issues that arise when dealing with finite element analysis. These issues include the initial development of a finite element model, the calibration and verification of the model in order to have the model produce results similar to that of measured test data. The main topics are how to correctly model such variables as: material stiffness, joint stiffness, loading arrangement and non-linearity among others. Some examples are given of the dynamic modelling of structures, which will not form part of the analysis of structures in this dissertation, given its significance it could not be overlooked. Vibration analysis of structures and the FE model updating techniques applicable to structural damage detection form a large part 45
Molloy 2012 of journal material. More research on this could be conducted in future but given the high level of mathematical knowledge required it will not be for some time. With background research conducted the project problem of developing, calibrating and verifying static FE models should be a less complicated process. Models can now be developed to test structures for elastic and plastic bending and the results compared to laboratory experimental data.
46
Molloy 2012
3 Methodology 3.1
Introduction
Finite element (FE) modelling software (ANSYS) produces results based on the entered data representing a physical setup for analysis. The results however need to be proved by some form of hand calculations or experimental test data in order to ensure the results are within the expected direction or magnitude. The process of updating FE models can only be accurately conducted by means of acquiring experimental data from similar physical tests. This data can then be entered into the FE model to change parameters such as material or section properties, support conditions, loading arrangements etc. This chapter has two objectives. The first describes the methods in which the experimental data was obtained from loading each structure in turn with mathematical methods included. The second describes the methodology involved in creating finite element models, in ANSYS simulation software package, of each structure and how to represent as close as possible the actual physical scenario. The physical testing took place in the Heavy Structures Laboratory of Athlone Institute of Technology. The geometry for the FE models will be created with ANSYS Workbench Design Modeller release 14 based on measured physical data from each of the test rig setups.
47
Molloy 2012 3.2
Experimental data: T shaped aluminium beam
This structure consists of an aluminium T shaped section 1000mm long supported at each end giving an effective length of beam of 805mm. Experimental values of strain were required along the centre of the longitudinal axis at 9 locations around the face in order to assess how the material reacts to the applied loading and also used to compute the Young’s Modulus of elasticity for the material, this value is used later in the ANSYS material properties (isotopic elasticity) as a model updating parameter. The measured strain values are used to compare values with those produced in the FE model. The averaged strain values will be used from the experimental test results to compare with the FE model to evaluate error percentages. There is also a mathematically calculated theoretical value for each strain location worked out for the structure as a further comparison.
48
Molloy 2012 3.2.1 Experimental strain data The test rig shown in Figure 3.1 was supplied by Hi-Tech Educational Equipment and consists of a universal frame where the beam was supported as shown.
Figure 3.1 – Beam test rig setup
Load was applied through a turn screw device located under the rig and is transferred to two locations centred on the beam at C and D identified in the schematic in Figure 3.3 Strain was recorded for the 9 locations, as indicated in Figure 3.2, for 15 load cases from 10N to 150N (or closest possible load) in 10N increments.
Figure 3.2 - Cross Section Dimensions (mm) and Strain Gauge Locations
49
Molloy 2012 Deflection was measured centrally on the beam for each load step by the deflection gauge located centrally on the top side of the beam. The test was carried out three times and the average strain values used. Results can be seen in Chapter 4. Simple supports were used at A and B which provides vertical reactions indicated in Figure 3.3. The beam is free to rotate at these locations giving only two reactions which will make the beam statically determinate. A load cell is attached to the loading mechanism which measures loading values and sends the information back to the HDA200 display. Nine strain gauges are located in the centre of the beam in positions described in Figure 3.2 and these send information back to the display in units of micro strain (¾ξ). Deflection is measured via a digital dial gauge placed on the upper surface of the beam centrally positioned over the load points. A schematic of the test setup is displayed in Figure 3.3 showing beam dimensions, load locations, support positions and strain gauge position.
Figure 3.3 - Experimental Test Rig Setup schematic
50
Molloy 2012 3.2.2 Experimentally derived Young’s modulus Young’s Modulus which applies to materials that obey Hooke’s Law is described as the ratio of tensile or compressive stress to tensile or compressive strain in a specimen subject to uni-axial loading as: E=
(1)
where: E is Young’s Modulus σ is tensile/compressive stress ε is tensile/compressive strain and is unitless and: σ=
(2)
where: F is axial force A is cross sectional area and: ε=
(3)
where: ΔL is change in length L is original length
These equations can be manipulated in order to find either value, if the stress is known, and the related strain measured, then E, the Young’s Modulus, can be derived for a particular material (Davis and Selvadori 1996). In bending however the strain is not easily measured physically, as the values are usually quite small,
51
Molloy 2012 so the use of electronic strain gauges are used to quantify it. Equation 1 can be graphically represented indicating the relationship between stress and strain. The elastic zone in Figure 3.4 shows that where the angle the line makes with the strain axis is representative of the modulus of elasticity within the elastic limit (slope of the line).
Figure 3.4 – Stress/Strain Curve (Beal 2000)
When materials are subjected to a normal or bending stresses, and elastic behaviour is experienced, the strain developed is recovered immediately the stress is removed. The limiting value of stress applied in order for this to happen is noted in Figure 3.4 as the elastic limit. Any further application of stress after this will result in the strain not fully recovering thus leaving a permanent deformation of the material. In 1678 Robert Hooke defined his law stating that the strain developed is directly proportional to the stress producing it. This law holds for most materials within certain limits (John 1978). The beam was tested by applying a load causing the beam to bend and recording the produced strain via electronic strain gauges and subsequently using the
52
Molloy 2012 bending moment equations and calculating the second moment of area for the shape a value for the Young’s Modulus was obtained.
Bending moment equations The bending moment equations for a beam can be equated as:
=
(4)
where: M is the bending moment I is the second moment of area σ is the bending stress y is the distance to the N/A where values are measured
rearranging equation 4 to make bending stress the subject gives: σ=
(5)
substituting equation 5 into equation 1 will yield a value for E: E=
(6)
Equation 6 now represents a value for the Young’s Modulus of the material being tested and since the strain can be recorded as the load increased, all that needs to be calculated is I, the second moment of area about the neutral axis.
Second moment of area The second moment of area section property for the bam is calculated with reference to Figure 3.5.
53
Molloy 2012
Figure 3.5 - Second Moment of Area Reference Data
Second moment of area calculations using the parallel axis theorom are evaluated by the the equations:
Ix,Total = Ix,1 + Ix,2
(7)
where:
Ix,1 and Ix,2 are the second moment of areas of shapes 1 and 2 respectivle Values for each Ix are given as:
Ix,1,2 =
+ b.d.天 2
(8)
Section property results with reference to Figure 4 for the beam cross section are presented in Table 3.1.
54
Molloy 2012 Table 3.1 - Second Moment of Area Calculations Section Dimensions (mm) b1
25.5
d1
3.2
b2
3.2
d2
47.5
y1
16.5
y2
8.85
Second Moment of Area (mm4) Ix,1=
22285
Ix,2=
40484
Ix,Total= 62769
The second moment of area arrived at will be used in Equation 6 and the recorded strain gauge readings to evaluate Young’s Modulus of elasticity of this material. 3.2.3 Mathematically calculated deflection data To check the validity of the deflection values which were obtained in the ANSYS finite element model, theoretical data for displacements were computed by two different methods as follows: 1.
Double integration (Macaulay’s method)
2.
Finite element stiffness method for deflection
3.2.4 Macaulay’s method Macaulay’s method, also known as the double integration method, is a structural analysis technique used to analyse deflections of Euler-Bernoulli beams and is very useful for discontinuous or discrete loading systems. The Euler-Bernoulli beam bending theory was developed in the mid 1800’s by Leonard Euler and Daniel Bernoulli to address the problem of finding deflections in beams subject to loading. Two key assumptions have to be made, the material 55
Molloy 2012 is linear elastic according to Hooke’s law and that the plane sections remain plane and perpendicular to the neutral axis during bending (Haukaas 2012). Macaulay’s Method enables the writing of a single equation of the bending moment for the full length of the beam. When coupled with the Euler-Bernoulli theory, we can then integrate the expression for bending moment to find the equation for deflection. This will allow the deflection to be found at any location on the beam, for the purposes of this experiment only the maximal deflection, expected at the centre of the beam, will be utilised. The method of finding the deflection of the beam will give deflected values which can be compared to the finite element stiffness method and then compared to deflection values obtained by ANSYS in the modelling stage.
From the Euler-Bernoulli Theory of Bending:
=
(9)
Where: R is the radius of curvature
For small displacements:
=
(10)
Where: y is the deflection at the point x is the distance of the point along the beam
This leads to the fundamental deflection equation: 56
Molloy 2012
=
(11)
M = EI
(12)
This can be rewritten as:
In order to find the deflection, y, at any point on the beam, a bending moment expression needs to be written from a position on the extreme right end of the beam in terms of x, the distance from the left end, which takes into account for all the different loading being applied and the reactions. Figure 3.6 shows the setup of the beam and the general location for the variable x.
Figure 3.6 – Position of x for moment expression
The general bending moment equation for the location x is:
Mx = RvA(x) – P1(x – 0.325) – P2(x – 0.48)
(13)
Where: RVA is the vertical reaction at the left end A P1 and P2 are the applied loads X is the variable distance from end A L is the beam length from A to B 57
Molloy 2012 Substituting Equation 13 into Equation 12 and integrating twice to solve for the deflection in terms of x which introduces two constants of integration, and using the boundary conditions:
1. Slope:
= 0 at x = L/2 due to symetrical loading
2. Deflection: y = 0 at x = 0 and x = L
This only leaves the second constant of integration and this stays at zero because of the simplistic nature of the loading arrangement. The result is an expression for the deflection at any point along the beam by entering a value for x. This process is simplified by the use of Microsoft Excel to do the calculations. Values for the constants and the computed deflections for each of the 15 load stages are presented in the results chapter.
3.2.5 Finite element stiffness method The finite element method as described in Chapter 2 of this dissertation can be used in a very simple manner to compute a 1 dimensional deflection value for the beam being modelled. This will involve descritizing the structure into a series of finite elements which are connected by nodes. As the beam will have two support points, two load points and one required deflection location, a 4 element structure with 5 nodes will be required. Figure 3.7 shows the beam in place in the experimental setup according to how the experimental test was conducted.
58
Molloy 2012
Figure 3.7 – Experimental setup
The beam was then broken down, or descritized, into 4 elements connected by 5 nodes as indicated in Figure 3.8. Nodes are located at locations of applied loading, reactions or points of interest for the required measured values. In this case there is no force, applied or reacted, at node 3. This node is required however as deflection was measured in the experimental setup at this location which was where the maximum deflection was expected.
Figure 3.8 – Beam discretised into 4 elements and 5 nodes
59
Molloy 2012 The system variables were assigned as seen in Figure 3.9.
Figure 3.9 – Numbered system variables
Each node has two degrees of freedom, which in turn are represneted as a vertical force or vertical displacement, a moment force or rotation. Each of the 4 elements individual stiffness matrixes is computed using methods of superposition as outlined in Chapter 2 and the summation of fixed end moments the following member stiffness matrix can be computed for each of the four members based on the matrix in Figure 3.10.
Figure 3.10 – Beam element stiffness matrix (Djafour et al. 2010)
The results of each member stiffness matrix and the resulting 10 x 10 structure stiffness matrix are presented in Chapter 4. There are many known’s associated with the structure, being: 1.
Reaction forces at each end: equal to the load due to symmetry 60
Molloy 2012 2.
No deflection at the supports
3.
Zero moment at supports: simply supported
4.
Moments across nodes 2,3 and 4 are equal and opposite: equilibrium
conditions These known values simplify the solving process significantly thus only leaving three values of interest to be solved for namely the deflection value at node 3 (max deflection) and both rotation values at nodes 1 and 5 represented in the global matrix as D3, D6 and D10 respectively.
61
Molloy 2012 3.3
Experimental data: 3 hinge arch bridge transient load
This structure represents a three hinged closed spandrel arch bridge and was supplied by Hi-Tech Educational Equipment. The bridge set up consists of a bridge fixed by pin supports at both ends and a third pin at the centre of the bridge span within the frame as depicted in Figure 3.11.
Figure 3.11 – Three Hinged Arch Bridge with Transient Loading
Dimensions of the experimental setup are shown in the schematic in Figure 3.12.
Figure 3.12 – Schematic View of Bridge Sowing Main Dimensions (mm)
62
Molloy 2012 Hinges are located at A, B and C thus forming the three hinged arch bridge. The forces involved internally and externally are depicted in Figure 3.13. Force FBX is where the load measuring cell is located.
Figure 3.13 – Free Body Diagram of Arch Bridge
3.3.1 Experimental procedure Load was applied by placing a metal cylinder of know mass at 10 equally spaced locations, identified in Figure 3.12 along the bridge and recording the resulting horizontal force at end B. Details of the metal cylinder which was the moving mass can be seen in Figure 3.14.
Figure 3.14 – Cylinder Dimensions (mm)
63
Molloy 2012 Horizontal force was measured through a force transducer located on one of the supports as seen in Figure 3.15.
Figure 3.15 – Force Transducer located at horizontal support
Three sets of test results were recorded for each of the eleven load positions and the average value for the horizontal reaction force for each location was used.
3.3.2 Mathematically calculated data The mathematically determined data was obtained form a simple 3 hinge arch bridge analysis using the standard three equilibrium equations:
Σ Moments = 0
Σ Horizontal Forces = 0
Σ Vertical Forces = 0
These equations are fine but on analysing the structure and the force reactions it is visible to see that there are 4 reactions present as a result of the applied vertical loading, see Figure 3.13. These are: 1.
Left hand vertical force – Fay
2.
Left hand horizontal force – Fax 64
Molloy 2012 3.
Right hand vertical force – Fby
4.
Right hand horizontal force – Fbx
Having 4 reactions and only 3 equations is not enough to solve for the resulting reaction forces. In the 3 hinge arch bridge analysis a further equation is required and this takes the form of:
Σ Moments about the centre hinge
This method is used to calculate the horizontal and vertical reactions for the given load of 24.8N at each of the 11 equally spaced locations along the top of the bridge. Tables of the resulting reactions are presented in the Results Chapter.
3.4
Finite Element Modelling
In order to conduct the finite element model of the given structures a knowledge of the computer programme ANSYS was required. As this was not part of any module within the Civil Engineering course a self-educate approach was taken. This would involve getting to know the basic commands and features of ANSYS in order to complete the modelling.
3.4.1 ANSYS self-learning The task of embarking along the self-educate route to have a working understanding of the ANSYS program seemed daunting initially. This task was made simpler though by taking a project management approach to the process with the aim of the project being to gain a fundamental user level as described in the Fundamental FEA Concepts and Applications publication by ANSYS (2012). Planning and scoping the project (self-educate) in order to provide clarity on the overall objectives included defining the project scope and evaluating if it would be possible to learn enough about the computer programme in order to complete the dissertation within the given timeframe. This process involved 65
Molloy 2012 searching through the ANSYS help website along with many forums that exist online. This proved invaluable research as the current version of ANSYS Workbench was installed in the computer lab within Athlone Institute of Technology and this version appeared to be more user friendly than the ANSYS classic version. It was decided at that stage to proceed with the Workbench element of the computer package and sufficiently educate myself in order to complete the project objectives. The initial procedure was to complete some basic tutorials which are easily accessible either from the ANSYS help section or online tutorials on the internet. In searching the internet there was many videos on the internet website Youtube.com which lead to the completion of the modelling process.
3.4.2 Modelling methodology The finite element models for simple 2 dimensional and 3dimensional problems are usually generated via the Mechanical ANSYS Parametric Design Language (APDL) command interface. For complicated assemblies the ANSYS Workbench product is used as it allows one to define the geometry natively and to set up a project workflow that allows the entire analysis from model generation to results processing to occur in a well-defined manner. Finite Element Analysis is a mathematical representation of a physical system comprising of an assembly of parts as the model, material properties, and applicable boundary conditions collectively referred to as pre-processing, the solution of that mathematical representation known as solving, and the study of results of that solution known as post-processing. Simple shapes and simple problems can be, and often are, done by hand. Most real world parts and assemblies are far too complex to do accurately, let alone quickly, without use of a computer and appropriate analysis software. The process involved can be broken down into basic steps including: 1.
Creating the geometry 66
Molloy 2012 2.
Selection of element type
3.
Assigning material properties
4.
Defining and generating the mesh
5.
Establishment of boundary conditions (supports and load arrangement)
6.
Post processing (solving)
7.
Analysis of results
To get to the geometry stage an analysis system must be set up first. On entering the ANSYS Workbench initial screen a list of items is presented in the Toolbox section. The project has to be built from these initial setting depending on the type of analysis being conducted. ANSYS Workbench Toolbox is displayed in Figure 3.16 where the static structural system can be seen amongst several other analysis type systems should they be required.
Figure 3.16 – ANSYS analysis systems toolbox
67
Molloy 2012 The type of analysis system used for the purpose of this project was the Static Structural (ANSYS) template. This template is then dragged to the Project Schematic, seen in Figure 3.20, and creates a standalone system. Other systems can be added or linked to a current system which will allow the sharing of data between analysis templates, say for instance the geometry could be the same for two types of analysis so there is no need to create the geometry twice. Once the system is in the project schematic there are options available to be completed in sequential order. The process will not allow the user to continue until the previous component in the project system is completed correctly. The static structural system comprises of the following components: 1.
Engineering data
2.
Geometry
3.
Model
4.
Setup
5.
Solution
6.
Results
A static structural analysis system graphic is shown in Figure 3.17. Note all the cells have a green tick indicating the data has been entered successfully along with a successful result.
Figure 3.17 – Static structural stand alone system
68
Molloy 2012 The completion of each step is a process in itself and establishing the correct data to be entered is paramount to a successful result. The methodology outlined here will be followed through for both of the structures modelled.
Von Mises Yield Criteria Von Mises postulated in 1913 that a material will yield when the distortional energy at the point in question reaches a critical value. The distortional energy written in terms of the 2D principal stresses and the yield stress can be seen in Figure 3.18.
Figure 3.18 – Von Mises stress criterion (Bolognese 2012)
The associated yield envelope is pictured in Figure 3.19.
Figure 3.19 – Von Mises Yield Envelope (Bolognese 2012)
These are the stresses that are viewed in relation to the principal stresses and are colour contoured in the ANSYS output as an indication of where the most 69
Molloy 2012 significant concentration of stress is to show where possible failure of a structure might occur. 3.4.3 T shaped aluminium beam As discussed in the previous section the structures are to be modelled as 3 dimensional solid structures. The T shaped aluminium beam will be modelled as a 3 dimensional solid structure. For the purpose of this analysis a static structural analysis system was used. This type of system determines the displacements, stresses, strains, and forces in a structure caused by loads that do not induce significant inertia and damping effects. Steady loading and response conditions are assumed which means the loads and the structures response are assumed to vary slowly with respect to time. Figure 3.20 shows three separate stand-alone static structural systems which were created for this project.
Figure 3.20 – ANSYS workbench project schematic screenshot
70
Molloy 2012 Stage 1: Engineering data The initial stage in the project system is entering of the engineering data. This component comprises of material properties of the solid to be modelled. The material is assumed to be homogenous, linear isotropic. The more relevant material properties for aluminium alloy set in the default values are presented in Table 3.2.
Table 3.2 – Sample material data for aluminium Temperature C
Young's Modulus Pa
22 7.1e+010 Compressive Yield Strength Pa 2.8e+008 Tensile Yield Strength Pa 2.8e+008 Tensile Ultimate Strength Pa 3.1e+008
Poisson's Ratio 0.33
Bulk Modulus Pa 6.9608e+010
Shear Modulus Pa 2.6692e+010
These material properties are set as default and are assumed by the programme until such time as experimental data is obtained from testing and entered into the relevant cells. These values are assigned to the individual elements and effect their interaction with each other and the overall behaviour of the solid structure as load is applied. Identifying differences in these properties by physical testing or theoretical assumptions will form part of the updating process as discussed earlier. Stage 2: Geometry Prior to initialising the geometry stage a detailed look at the problem is needed. This is done to fully understand the structure being analysed to arrive at the most economical yet thorough way the model can represent the actual structure. Advantages can be taken of symmetry if possible about the structure which will reduce the overall time and computer power required to solve the problem.
71
Molloy 2012 The geometry creation is started by opening the Design Modeller by double clicking in the system cell named geometry. After selecting the desired drawing units to construct the geometry, the cross section is drawn in the x-y plane as shown in Figure 3.21.
Figure 3.21 – ANSYS design modeller screenshot
Dimensions are assigned to create a cross section which represents the true shape of the beam being tested. It is important to ensure that the model is being created in a 3 dimensional analysis mode. Once the outline of the cross section is created it is possible to extrude the shape in the Z axis to form a 3 dimensional solid body. The computer now understands this to be a solid body made of the pre assigned material. Figure 3.22 shows the extruded body. Note the scale bar on the bottom of the figure which is there to compare relative size so as not to be out of scale by some multiple factor. The global coordinates are also displayed in the corner and clicking on an axis here will rotate the body to a desired view for inspection.
72
Molloy 2012
Figure 3.22 – Extruded beam
This completes the geometry stage and the model is now ready to setup with the required loading arrangement and support conditions which will correctly represent the real scenario. This is done by launching the mechanical application by clicking on the Model cell in the project schematic. Stage 3: Mechanical (model) Launching the mechanical application takes the newly generated solid body and places it in an environment where the body can be assigned a mesh of elements. The tree outline in the mechanical window displays the current body part as created in the geometry application. This is highlighted and the mesh control is activated by clicking ‘generate mesh’. ANSYS Workbench is ideal for the fundamental user as the programme chooses the size and type of element mesh best suited to the body being analysis. In this case 451 quadratic hexahedron (solid 186) elements are selected by the programme. The meshed solid body can be seen in Figure 3.23.
73
Molloy 2012
Figure 3.23 – Meshed beam
The quantity of elements can be specified by the programmer as the mesh tool allows an element size to be selected. For this application a size of 20mm per element was selected. Depending on the result required and the accuracy more elements can be specified by reducing the element size, however, this increases solving time. An example of a solid 186 element is outlined in Figure 3.24.
Figure 3.24 – Solid 186 element 74
Molloy 2012 This type of element is described as a higher order 3 dimensional 20 node solid element that exhibits quadratic displacement behaviour and is defined by 20 nodes having 3 degrees of freedom per node: translations in the nodal x, y and z directions. This element is probably a little too advanced for the required analysis but as the programme has chosen this element it was decided to run with it though the solve time will increase. Midside nodes
(nodes
A,B,Y,Z,V,X,R,T,Q,S,U,W in Figure 3.24 could be dropped for this type of analysis thus giving linear solution at element edges. This will become a model updating parameter in itself as lowering the order of the element by allowing the midside nodes to be dropped will change the element from a Solid 186 element to a Solid 185 element as shown in Figure 3.25.
Figure 3.25 – Solid 185 element
This element is described in the ANSYS element library as being defined by eight nodes having three degrees of freedom at each node: translation in the nodal x, y and z directions. This will be an adequate element type to use and should lower the solve time while still producing the data required. A view of this element can be seen in Figure 3.26 from the ANSYS finite element modeller.
75
Molloy 2012
Figure 3.26 – View of a quadratic hexahedron Solid 185 element in beam
Stage 4: Setup Once the body has a mesh allocated to it the loads and support conditions can be assigned. This is done in the setup stage by clicking on the static structural item in the tree menu. This activates several options in the main menu ribbon close to the top of the screen. There is no preference as to whether the load is placed first or the support. The selection of the type of support and boundary conditions will be determined by the actual scenario in which the model is to exist in real life. The model in this case was represented by a remote displacement support on each end face of the beam. This option, with reference to the global coordinates, constrains the movement of the beam at the supports to:
No movement in the X direction
No movement in the Y direction
Free movement in the Z direction (axially)
With regard to rotations: 76
Molloy 2012 
No rotation in the Y plane

No rotation in the Z plane

Free rotation in the X plane
This behaviour allows the supports to act as simple supports at the ends which are representative of the experimental situation. With the support conditions setup the loading is next to be applied. As the resulting values obtained from mathematical analysis, as described in section 3.2.2, use moment values in bending stress equations it was thought adequate to apply moments to each end of the beam to represent a point load as indicated in the experimental setup. The bending moment values will be applied in a series of steps. This is known as time history or time dependent tabular loading. Essentially it means that loads can be placed on the body at a designated time step. This will allow the 15 load increments to be applied to the body over a 16 second interval, the first being zero. Once the moment load is assigned to each end face, the amount of load steps to be applied must be specified in the analysis settings in the tree menu. This is set to 16 steps which is representative of the experimental setup loading from 0 to 150N or nearest values for increments of 10N. The true values recorded on the day of the experiment were converted into moments and entered into the tabular data for each load increment. Table 3.3 below shows the values of applied moment to each axis as calculated from applied loads which were used in the experimental setup.
77
Molloy 2012 Table 3.3 – Table of applied moments Moments applied LHS (Nm) Time(s) x y z 0 0 0 0 1 -2.04 0 0 2 -3.5 0 0 3 -4.9 0 0 4 -6.7 0 0 5 -8.4 0 0 6 -9.7 0 0 7 -11.5 0 0 8 -13.2 0 0 9 -14.6 0 0 10 -16.3 0 0 11 -18 0 0 12 -19.8 0 0 13 -21.3 0 0 14 -22.7 0 0 15 -24.6 0 0 16 0 0 0
Moments applied RHS (Nm) Time(s) x y z 0 0 0 0 1 2.04 0 0 2 3.5 0 0 3 4.9 0 0 4 6.7 0 0 5 8.4 0 0 6 9.7 0 0 7 11.5 0 0 8 13.2 0 0 9 14.6 0 0 10 16.3 0 0 11 18.04 0 0 12 19.8 0 0 13 21.3 0 0 14 22.7 0 0 15 24.6 0 0 16 0 0 0
Stage 5: Solution This stage of the analysis allows for the input of solution parameters in which results will be solved for. The solutions needed for this analysis contain:
Total deformation
Minimum principal elastic strain (compressive strain)
Maximum principal elastic strain (tensile strain)
As these were the only parameters required, where the expected maximum of the tensile strain was at the bottom most fibres and the maximum compressive strain was at the top most fibres of the beam, no other parameters were entered into the solver solution process. Stage 6: Results The final stage in the static structural analysis system is to solve the analysis. This is done by clicking the solve icon
and allowing the programme to solve 78
Molloy 2012 in its own time. During this time the computer generates the mathematical model and solves the thousands of differential equations relating to each node of each element in the mesh in order to arrive at a solution for the required parameters. The results are available in graphic format and also tabular data for each value at a minimum and maximum value for each time step which represents the moment increments. The results are presented in the results chapter. The results from this analysis were compared to the experimental results, and where possible, changes were made to the FE model in an updating procedure to calibrate the model to the experimental setup. The results of these are also presented in the results section.
3.4.4 Transient load on 3 hinge arch bridge The 3 hinge arch bridge was modelled in ANSYS following the same procedures as with the T shaped beam described in the previous section. The use of a static structural analysis system was used again. Each stage is described here assuming the same procedure but with some differences which were made to the process to make it specific to the arch bridge model. The method of analysing this structure with the load changing position along the top from one end to the other in stages of 100mm was done by firstly setting up the first 3 stages in the static structural system. It is possible to link the setup of one analysis system to that of many others. This allowed the use of the first setup arrangement to be linked to each stage of the load position which was 6 in this case.
Stage 1: Engineering data There was no way of assessing the material properties of the steel which makes up the bridge in the experiment, however, an assumption was made to give it 79
Molloy 2012 the same properties as structural steel. It was decided that the load being applied was on such a small scale compared to the structural capacity of the material to resist any real deformations that the use of the preset values were sufficient. During the experimental data collection process the self weight of the bridge was not considered when analysing the horizontal reactions due to the applied vertical loading, this was done by setting the reading on the force readout to zero prior to applying the load thus neglecting any horizontal loading from the self weight. The data used was that which was set as default in the ANSYS material library and was as follows in Table 3.4.
Table 3.4 – Structural steel material properties Temperature C
Young's Poisson's Bulk Modulus Pa Ratio Modulus Pa 2.e+011 0.3 1.6667e+011 Compressive Yield Strength Pa 2.5e+008 Tensile Yield Strength Pa 2.5e+008 Tensile Ultimate Strength Pa 4.6e+008
Shear Modulus Pa 7.6923e+010
The engineering data presented here was applicable to two design attempts. For the rest of this section there are two designs attempts presented which were subsequently analysis for their accuracy in replicating the experimental setup described in section 3.3 Stage 2: Geometry The creation of this structure in geometrical terms is dependent on the perception and understanding as to how best replicate the existing model in ANSYS. As the aim of this dissertation is to create finite element models, which 80
Molloy 2012 behave as close as possible to the experimental setup data of each tested structure, different approaches to the modelling of the 3 hinge arch bridge were attempted. The problems and the subsequent solutions are dealt with in the results and discussion chapter. Here each of the modelling attempt methods is described in detail. Attempt 1 This attempt was created as a 3 dimensional model of only half of the bridge. The model was constructed in the Design Modeller function of the Model static structural cell where 3 sketches were generated. The first sketch was one of the side plates of the bridge and this was then extruded to a depth of 6mm. The extruded sketch was then copied via the tools dropdown menu and copied to a distance equal to the experimental bridge. This allowed the correct gap between the plates to be established. Then the pin, highlighted in green in Figure 3.27 was drawn and extruded to the same value as the plates were offset. The final sketch drawn was the 6 connecting rods along the top and these were subsequently extruded to the same amount. The result is shown in Figure 3.27.
Figure 3.27 – Extruded solid structure
81
Molloy 2012 Stage 3: Mechanical (model) This stage involves as before the application of the mesh to the newly created bodies. ANSYS Workbench makes an attempt at creating a mesh which is most suited to the type of analysis and geometric shape being tested. The choice of element selected was the Linear Tetrahedron element type. The model mesh was then generated to take the form pictured in Figure 3.28.
Figure 3.28 – Solid structure after meshing
The size of elements could be controlled by the user and a size of 30mm was deemed to be substantial as stresses or strains were not of concern in this model, only reactions at the hinge of the structure were needed. Supporting conditions and loadings were applied to the model in the setup stage of the analysis.
82
Molloy 2012 Stage 4: Setup On initial observations one half of the arch bridge seemed to be sufficient so modelling the part would have to bear resemblance to the actual experimental setup in as much as possible. The following support conditions shown in Table 3.5 were applied to the model.
Table 3.5 – Tabular data for supports X Coordinate Y Coordinate Z Coordinate Location Definition Type X Component Y Component Z Component Rotation X Rotation Y Rotation Z Suppressed Behaviour Define By Rotation X Rotation Y Rotation Z
1.1556e-032 m 0.2123 m 3.e-003 m
1.e-002 m 0.225 m 4.5e-002 m Defined
0.5025 m 1.e-002 m 4.65e-002 m
Remote Displacement 0. m (ramped) Free 0. m (ramped)
Remote Force
Remote Displacement 0. m (ramped) 0. m (ramped) 0. m (ramped)
0. N (ramped) -12.4 N (ramped) 0. N (ramped) 0. ° (ramped) 0. ° (ramped) Free No Deformable Rigid Components 0. ° (ramped) 0. ° (ramped) Free
Remote displacements and the conditions as outlined in Table 3.5 were applied to the faces of the solid as shown in Figure 3.29 and Figure 3.30.
83
Molloy 2012
Figure 3.29 – Remote displacement support 1
The second support was applied to the hinge face as seen in Figure 3.30.
Figure 3.30 – Remote displacement support 2
84
Molloy 2012 The next stage was to apply the loading. As described at the outset of this subsection there needed to be 6 stages of loading to account for the variable load location on the structure. Each system had the same model, mesh, support conditions and material data. Loading was the only variable in 6 stages from distances of 0mm (centre of the bridge) to 500mm (over support) in each separate system. Stage 5: Solution The solution requirements of this model were only to assess the support reaction due to the varying load position. It was thought proper to allow the solution to contain the equivalent (von-Mises) stress analysis to see if they look like the predicted distribution. The support reaction was allocated to the hinge location at the lower right hand side of the model where the remote displacement support was located.
Stage 6: Results The results from the model are obtained by solving the model in order to produce a post-processed result. The required results are decided on in the setup stage. The results required for this model for each 15 load steps were: 
Remote displacement support 1 horizontal and vertical reactions

Remote displacement support 2 horizontal and vertical reaction

Von-Misses stress distribution (for information only)
Results for each load step are displayed and discussed in the results chapter. Issues in relation to this method are discussed in detail later. Problems with vertical reaction values prompted a rethink of the modelling setup. A second attempt was made to represent the true experimental setup as close as possible. The second attempt follows.
85
Molloy 2012 Attempt two Stage 1: Engineering data The material properties in stage one of the analysis setup, engineering data, remains as structural steel for the second attempt with the same isotropic elasticity properties. The critical difference is the model geometry which is attempted to recreate the experimental setup more accurately.
Stage two: Geometry This second attempt posed a significant challenge as it involved having two bodies connected by joints. The issues relating to the first attempt needed to be rectified and a more true representation of the experimental structure was needed. This was achieved by creating 4 separate body parts shown in Figure 3.31 and Figure 3.32 below highlighted in green.
Figure 3.31 – Body parts 1 and 2
86
Molloy 2012
Figure 3.32 – Body parts 2 and 3
As can be seen by the 3 dimensional solid created in ANSYS Design Modeller, there is a close representation to the experimental setup displayed in Figure 3.33.
Figure 3.33 – Experimental setup
Stage 3: Mechanical (model) The solid model consists of 4 body parts which are connected at the centre by two bodies which need to act as a joint or hinge. This need allows the structure to behave exactly like the experimental setup of the 3 hinge arch bridge. The 87
Molloy 2012 setting up of the joint types is done in the model stage of the analysis. In order to replicate the 3 hinge arch structure the interface between the two solid pins at the centre of the bridge and both sides of the bridge need to be modelled with a revolute, solid to multiple joint MPC184 element connection between the bodies at the centre of the bridge on both sides with freedom of rotation about the “Z� axis as pictured in Figure 3.34 below.
Figure 3.34 – Revolute joint connection No's 1 & 2
MPC184 Revolute Joint Element Description: The MPC184 revolute joint is a two-node element that has only one primary degree of freedom, the relative rotation about the revolute (or hinge) axis. This element imposes kinematic constraints such that the nodes forming the element have the same displacements. Additionally, only a relative rotation is allowed about the revolute axis, while the rotations about the other two directions are fixed which is visible from Figure 3.35 below.
88
Molloy 2012
Figure 3.35 – MPC-184 revolute joint (ANSYS)
This condition allows the connection at this location to only allow rotation about the Z axis while still maintaining a transmission of shear across the connection. There should be zero moment experienced at this location also which is representative of the experimental setup. The created model consisting of 4 body parts was meshed using the ANSYS automatic meshing capability which is program controlled to a large extent. The mesh size was set at 20mm. The meshing of the body parts took the form depicted in Figure 3.36 below.
89
Molloy 2012
Figure 3.36 – 3-D model after meshing
Once these conditions were completed the next stage in the analysis was to set boundary conditions and loading in the setup stage. Stage 4: Setup To adequately represent the model as the true structure it was important to mimic the real conditions experienced by the model. The provision of revolute joints in the setup stage allows for one of the hinges of the three required for this type of structure.
90
Molloy 2012 Table 3.6 outlines the properties of the joints at the bridge centre.
Table 3.6 – Centre hinge revolute joint data Object Name Revolute - Solid To Multiple Revolute - Solid To Multiple State Fully Defined Definition Connection Type Body-Body Type Revolute Torsional Stiffness 0. N·m/° Torsional Damping 0. N·m·s/° Suppressed No Reference Scoping Method Geometry Selection Scope 1 Face Body Solid Coordinate System Reference Coordinate System Behaviour Rigid Pinball Region All Mobile Scoping Method Geometry Selection Scope 8 Edges Body Multiple Initial Position Unchanged Behavior Rigid Pinball Region All Stops RZ Min Type None RZ Max Type None
In order to provide the two remaining hinges the use of remote displacements is required at the two pins at the lower sides of the model with constraints listed in Table 3.7.
91
Molloy 2012 Table 3.7 – Remote displacement support details Object Name State Scoping Method Geometry Coordinate System X Coordinate Y Coordinate Z Coordinate Location Type X Component Y Component Z Component Rotation X Rotation Y Rotation Z Suppressed Behaviour Rotation X Rotation Y Rotation Z Define By Coordinate System
Remote Displacement
Remote Displacement 2 Fully Defined Scope Geometry Selection 1 Face Global Coordinate System
-0.5025 m 1.5e-002 m 4.8e-002 m Defined Definition Remote Displacement 0. m (ramped) 0. m (ramped) 0. m (ramped) 0. ° (ramped) 0. ° (ramped) Free No Deformable 0. ° (ramped) 0. ° (ramped) Free
Force
0.5025 m
Pinball Region
Force 0. N (ramped) -24.8 N (ramped) 0. N (ramped)
Components Global Coordinate System Advanced All
The remote displacement boundary conditions outlined in Table 3.7 are representative of a hinge support. Neither support allows translations in X, Y or Z directions. The only allowable movement by the hinge supports is the free rotation about the Z plane. This allows the body attached to each of these supports to rotate freely which is representative of the experimental setup. The application of these boundary conditions ensures reactions in the horizontal and vertical directions at these locations but no transfer of moment, reflective conditions of the true scenario. Loading in the model will be in accordance with the physical experiment and will be a unit mass of 2536 grams which equates to approximately 24.8N placed at 100mm intervals along the top surface of the ridge deck. This is replicated by 92
Molloy 2012 allowing the load to be placed on each of the connecting pins which for part of the solid structure. The first load stage is depicted in Figure 3.37.
Figure 3.37 – First load stage applied to bridge deck
The surface of the connecting pin is selected as the application surface then by entering the load direction using the components selection and entering 0 for Z and X directions and a value of -24.8N in the Y direction. As there are 11 load positions to be solved for it is possible to use the same model and meshing for all stages by linking a separate static structural analysis system for each load. This keeps all the supporting boundary conditions the same and there is no need to set these up for each load step. The load application is repeated for the remaining load steps from 0mm to 1000mm in 100mm intervals, which is the extent of the bridge deck.
93
Molloy 2012 Stage 5: Solution Solution results for this structure only require support reactions in the horizontal and vertical sense as there is no moment reaction capability at any of the 3 hinges. The required information for this structure was horizontal and vertical reactions at each lower end of the bridge at the remote displacement supports. As a monitoring exercise the distribution of stresses was selected as a solution parameter to allow a general comparison with expected locations of maximum and minimum von-Mises (failure criteria) stresses which are an indication of the possible failure of the material due to a combination of stresses in the x, y and z directions. Stage 6: Results Solving the model produces the desired results after the computer calculates and solves the mathematical equations. Based on the data required in the solution stage the following results were processed: 
Remote displacement support 1 horizontal and vertical reactions

Remote displacement support 2 horizontal and vertical reaction

Von-Mises stress distribution (for information only)
94
Molloy 2012
4 Results 4.1
T shaped aluminium beam results
4.1.1 Experimentally determined strain values Experimental strain values at the locations on the beam for test number 1 values are in Table 4.1 with the graphical representation shown in Figure 4.1. Table 4.1 – Experimental strain values for test No.1 Stage 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16
Applied Load (N) Desired Actual 0 0 10 16 20 22 30 29 40 42 50 53 60 60 70 69.6 80 83 90 90 100 101 110 110 120 122 130 131 140 140 150 151
1 0 14 25 37 54 65 73 95 103 110 120 133 146 163 180 192
2 0 2 8 13 21 31 32 38 47 54 62 66 76 82 90 95
Channel Number 4 5 6 0 0 0 -6 -16 -4 -12 -24 -9 -16 -29 -16 -24 -42 -26 -35 -51 -34 -37 -58 -36 -40 -66 -42 -50 -79 -55 -57 -85 -61 -62 -93 -73 -65 -103 -76 -72 -111 -85 -79 -118 -95 -79 -124 -103 -87 -129 -109
3 0 -4 -5 -8 -13 -14 -19 -19 -26 -28 -33 -33 -37 -39 -41 -45
7 0 -3 -7 -13 -26 -26 -32 -40 -50 -51 -63 -69 -75 -84 -89 -96
8 0 -5 -9 -10 -14 -18 -19 -24 -30 -30 -35 -37 -41 -44 -48 -50
9 0 6 13 15 28 35 40 46 56 62 72 77 84 90 99 104
Deflection Centre(mm) 0 0.04 0.06 0.09 0.15 0.18 0.21 0.24 0.29 0.31 0.35 0.39 0.43 0.46 0.49 0.52
Test No. 1- µε v Load 300
Microstrain(µε)
1 200
2
100
3
0 -10 -100
4
-200
10
30
50
70
90
110
130
150
5 6
Load(N)
7
Figure 4.1 – Graphical representation for test No. 1
95
Molloy 2012 The results from test number 2 are displayed in Table 4.2 with the graphical representation displayed in Figure 4.2. Table 4.2 – Experimental strain values for test No.2 Stage 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16
Applied Load (N) Desired Actual 0 0 10 10.7 20 21.2 30 29.5 40 39 50 51.6 60 59.3 70 70.3 80 82.2 90 89.9 100 101 110 112 120 122 130 133 140 141 150 151
1 0 14 25 37 54 65 73 95 115 120 125 133 146 163 180 195
3 0 -3 -5 -8 -11 -13 -15 -18 -21 -24 -28 -30 -34 -37 -39 -40
Channel Number 4 5 6 0 0 0 -4 -5 -11 -13 -17 -15 -18 -23 -22 -27 -31 -26 -25 -33 -32 -27 -40 -38 -35 -45 -44 -40 -56 -52 -46 -64 -61 -52 -70 -67 -55 -81 -72 -66 -86 -83 -69 -94 -89 -73 -99 -91 -80 -107 -97
7 0 -5 -12 -17 -26 -31 -36 -39 -50 -51 -59 -67 -73 -81 -87 -93
8 0 -3 -4 -6 -10 -12 -11 -17 -24 -27 -28 -30 -34 -37 -39 -44
9 0 6 16 22 34 41 46 56 62 68 75 85 92 99 107 112
Deflection Centre(mm) 0 0.03 0.08 0.12 0.16 0.21 0.24 0.28 0.32 0.35 0.39 0.43 0.47 0.5 0.53 0.56
Test No. 2- µε v Load
250
Microstrain(µε)
2 0 7 12 18 27 33 37 44 52 59 67 73 81 90 94 96
200
1
150
2
100
3
50
4
0 -10 -50
5 10
30
50
70
90
110
130
150
6 7
-100 -150
8
Load(N)
9
Figure 4.2 - Graphical representation of experimental load versus strain for test No. 2
96
Molloy 2012 The results from test number 3 are displayed in Table 4.3 with the graphical representation shown in Figure 4.3. Table 4.3 – Experimental strain values for test No. 3 Stage 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16
Applied Load (N) Desired Actual 0 0 10 11 20 21.4 30 32 40 42 50 50 60 59 70 73 80 79 90 89 100 99 110 111 120 122 130 129 140 138 150 152
1 0 14 25 37 54 65 73 90 110 120 125 133 146 163 180 199
2 0 9 12 17 26 28 36 45 50 56 64 71 77 84 88 100
3 0 -1 -7 -8 -17 -15 -18 -22 -27 -28 -33 -39 -39 -41 -46 -46
Channel Number 4 5 6 0 0 0 -7 -5 -9 -14 -14 -17 -19 -22 -24 -28 -31 -38 -35 -38 -43 -37 -45 -48 -44 -56 -60 -52 -60 -65 -29 -71 -73 -63 -76 -80 -70 -85 -92 -75 -94 -101 -79 -101 -107 -83 -106 -111 -91 -118 -112
7 0 -6 -18 -22 -26 -31 -38 -48 -50 -57 -64 -72 -78 -82 -88 -97
8 0 -2 -10 -13 -16 -17 -18 -26 -22 -28 -33 -36 -40 -41 -47 -50
9 0 4 11 19 25 35 38 50 54 65 70 78 89 90 97 108
Deflection Centre(mm) 0 0.05 0.09 0.13 0.17 0.2 0.23 0.29 0.31 0.34 0.38 0.42 0.46 0.48 0.51 0.55
Test No 3- µε v Load 250 1
Microstrain(µε)
200 150
2
100
3
50
4
0 -10 -50
5 10
30
50
70
-100 -150
90
110
130
150
6 7
Load(N)
8
Figure 4.3 - Graphical representation of experimental load versus strain for test No. 3
97
Molloy 2012 The resulting average strain values from the 3 tests are presented in Table 4.4 with the corresponding graphical representation shown in Figure 4.4. Table 4.4 – Experimental strain values averaged Stage 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16
Applied Load (N) Desired Actual 0 0 10 13 20 22 30 30 40 41 50 52 60 59 70 71 80 81 90 90 100 100 110 111 120 122 130 131 140 140 150 151
1 0 14 25 37 54 65 73 93 100 117 123 133 146 163 178 195
2 0 6 11 16 25 31 35 42 50 56 64 70 78 85 91 97
3 0 -3 -6 -8 -14 -14 -17 -20 -25 -27 -31 -34 -37 -39 -42 -44
Channel Number 4 5 6 0 0 0 -6 -9 -8 -13 -18 -14 -18 -25 -21 -26 -35 -30 -32 -41 -36 -34 -48 -41 -40 -56 -49 -47 -65 -57 -44 -73 -65 -59 -80 -73 -63 -90 -80 -71 -97 -90 -76 -104 -97 -78 -110 -102 -86 -118 -106
7 0 -5 -12 -17 -26 -29 -35 -42 -50 -53 -62 -69 -75 -82 -88 -95
8 0 -3 -8 -10 -13 -16 -16 -22 -25 -28 -32 -34 -38 -41 -45 -48
9 0 5 13 19 29 37 41 51 57 65 72 80 88 93 101 108
Deflection Centre(mm) 0.00 0.04 0.08 0.11 0.16 0.20 0.23 0.27 0.31 0.33 0.37 0.41 0.45 0.48 0.51 0.54
Experimental Averaged - µε v Load 250 1
Microstrain(µε)
200
2
150
3
100
4
50 0 -5 -50
5
15
35
55
75
95
115
135
155
7
-100 -150
6
8 Load(N)
9
Figure 4.4 - Graphical representation of experimental load versus strain for average values
98
Molloy 2012 4.1.2 Experimentally derived Young’s modulus Based on the averaged experimentally derived values for strain, the experimental value for the modulus of elasticity was derived using Equation 6 from the Methodology Chapter. The values in Table 4.5 are average values for each strain gauge location over the 15 load stages: Table 4.5 – Experimentally derived Young’s modulus Gauge No. Dist. To NA(mm)
Young's Modulus of Elasticity 2 (N/mm )
Average:
1
2
3
4
5
6
7
8
9
33.96
16.84
6.96
13.93
17.12
17.12
13.93
6.96
16.84
78917
91310
84912
79975
64266
69621
97112
67930
102724
75726
88010
68470
59735
52057
69833
62964
50608
70408
71681
82197
67945
61579
54204
64695
62763
56230
70455
66752
72464
54055
56148
52418
60572
56868
55407
61636
69703
73261
66325
58687
56164
62863
63356
59269
60721
71579
74031
61782
63663
55262
64774
60660
66931
62687
66849
73084
65019
64519
56503
64630
60455
57256
61064
71565
71451
59461
62018
55504
62926
58710
57896
61897
67546
69367
60565
73464
54173
61118
60989
57002
60118
71522
67992
57697
61327
55819
60640
58360
56495
60472
73375
69131
58825
63205
54866
61496
57735
58254
60490
73465
68189
59952
61967
55744
60303
58403
57346
60212
70658
66927
60524
62435
55649
59857
57379
58043
61410
68984
67158
59918
64299
56446
60887
57236
56341
60287
68114
68016
62446
63459
56841
63276
57247
56808
61089
63959
Max value
102724
Min value
50608
99
Molloy 2012 4.1.3 Theoretical strain values Based on the experimentally derived Young’s modulus of 64GPa, the following theoretical strain values were computed for the 15 load stages are presented in Table 4.6. Table 4.6 – Theoretical strain values for Young’s modulus of 64GPa Gauge No. Dist. To N/A (mm)
Theoretical strain -6 x10 values determined from experimentally derived Young's modulus
1
2
3
4
5
6
7
8
9
33.96
16.84
6.96
13.93
17.12
17.12
13.93
6.96
16.84
17
9
-4
-7
-9
-9
-7
-4
9
30
15
-6
-12
-15
-15
-12
-6
15
41
21
-8
-17
-21
-21
-17
-8
21
56
28
-12
-23
-28
-28
-23
-12
28
71
35
-15
-29
-36
-36
-29
-15
35
82
40
-17
-33
-41
-41
-33
-17
40
97
48
-20
-40
-49
-49
-40
-20
48
112
55
-23
-46
-56
-56
-46
-23
55
123
61
-25
-51
-62
-62
-51
-25
61
138
68
-28
-57
-69
-69
-57
-28
68
152
76
-31
-63
-77
-77
-63
-31
76
168
83
-34
-69
-84
-84
-69
-34
83
180
89
-37
-74
-91
-91
-74
-37
89
192
95
-39
-79
-97
-97
-79
-39
95
208
103
-43
--85
-105
-105
-85
-43
103
100
Molloy 2012 4.1.4 Compressive strain results (ANSYS) The results produced by ANSYS are conveniently output in tabular form. Table 4.7 shows the results for the minimum principal elastic strain values for each of the load steps which are the measure of the compressive strain experienced by the beam as a result of the loading.
Table 4.7 – ANSYS produced minimum elastic strain Time [s] Minimum [m/m] Maximum [m/m] 1. -9.2184e-006 -1.5716e-007 2. -1.5816e-005 -2.6964e-007 3. -2.2142e-005 -3.7749e-007 4. -3.0276e-005 -5.1616e-007 5. -3.7958e-005 -6.4713e-007 6. -4.3833e-005 -7.4728e-007 7. -5.1966e-005 -8.8595e-007 8. -5.9648e-005 -1.0169e-006 9. -6.5975e-005 -1.1248e-006 10. -7.3657e-005 -1.2557e-006 11. -8.152e-005 -1.3898e-006 12. -8.9473e-005 -1.5254e-006 13. -9.6251e-005 -1.6409e-006 14. -1.0258e-004 -1.7488e-006 15. -1.1116e-004 -1.8952e-006 16. 0. 0.
The result from the ANSYS finite element model of the beam under the maximum load condition at load step 15 is shown in Figure 4.5. This figure shows the minimum principal elastic strain, the dark blue colour indicating the minimum value, which is negative and represents the maximum compressive strain produced in the beam by the applied maximum loading as it is the lower value. The dark red colour running through the beam is indicative of the largest value which indicates the maximum of the values of negative strain, which is the larger number, indicating the location of least strain and is coincident with the neutral axis, as expected.
101
Molloy 2012
Figure 4.5 – ANSYS compressive strain graphic, updated model
Each individual strain gauge value from the experimental setup was not obtained from the ANSYS model. The values obtained from the model concerned only the maximum compressive and tensile strain values. Maximum compressive strain values are graphed in Figure 4.6 and are taken directly from the output file from the ANSYS report. The full report can be seen on the CD in Appendix D. The experimental values were obtained by averaging the values from Gauges 5 and 6 (located on the top face of real beam) and are compared to the pre and postupdated finite element models.
102
Molloy 2012 0.00012 0.0001
Strain
0.00008 Pre-Updated
0.00006
Updated
0.00004
Experimental Data 0.00002 0 0 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 Load Step
Figure 4.6 – Maximum compressive strain values
The results obtained from the finite element modelling are tabulated in Table 4.8 is a percentage comparison basis between the pre and post-updating model values and the experimental compressive strain results. It can be seen that the updating procedure has resulted in the model returning on average 100% of the experimental strain produced by the maximum loading. Table 4.8 – Compressive strain comparison Model % of Experimental Max Compressive Strain Load Step Pre-updating Post-updating 1 100 113 2 89 101 3 88 100 4 84 96 5 89 101 6 89 102 7 90 102 8 88 100 9 86 98 10 87 99 11 87 98 12 86 98 13 86 98 14 88 99 15 89 102 Average 88 100
103
Molloy 2012
4.1.5 Tensile strain results (ANSYS) Results for tensile strain obtained from the ANSYS model are produced as maximum principal elastic strain values. Table 4.9 shows the results tubulised for each of the load steps. Table 4.9 – ANSYS maximum principal elastic strain Time [s] Minimum [m/m] Maximum [m/m] 1. 4.7491e-007 1.6563e-005 2. 8.1479e-007 2.8417e-005 3. 1.1407e-006 3.9784e-005 4. 1.5597e-006 5.4399e-005 5. 1.9555e-006 6.8201e-005 6. 2.2581e-006 7.8756e-005 7. 2.6772e-006 9.3371e-005 8. 3.0729e-006 1.0717e-004 9. 3.3988e-006 1.1854e-004 10. 3.7946e-006 1.3234e-004 11. 4.1997e-006 1.4647e-004 12. 4.6094e-006 1.6076e-004 13. 4.9586e-006 1.7294e-004 14. 5.2845e-006 1.8431e-004 15. 5.7268e-006 1.9973e-004 16. 0. 0.
The graphical results from the ANSYS finite element model for maximum tensile strain at load step 15 are shown in Figure 4.7 where the red colour running along the extreme bottom of the beam is the maximum positive strain which indicates tensile strain. This is where the maximum tensile strain value was expected. The dark blue running through the beam is the minimum value of tensile strain and is coincident with the neutral axis which is to be expected.
104
Molloy 2012
Figure 4.7 – ANSYS tensile strain graphic, post-updated
Results for the maximum experimental tensile strain are from the average maximum value of strain gauge number 1. The values for the finite element model were transferred from ANSYS to Excel and then compared to the experimental values. The results are compared graphically in Figure 4.8. 0.00025
Strain
0.0002 0.00015 Pre-Updated 0.0001
Updated Experimental Data
0.00005 0 0 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 Load Step
Figure 4.8 – Maximum tensile strain values 105
Molloy 2012 It can be seen from Figure 4.8 that the experimental maximum tensile strain lies almost midway between the pre and post-updated values. This was noted as being inconsistent with expectations. When the values were compared as percentage values of the experimental results, seen in Table 4.10, the finite element pre-updated model is actually closer to the experimental data than the post-updated value. Inaccuracies in the performance of gauge number 1 were witnessed on the day of the experiment.
Table 4.10 – Tensile strain comparison Model % of Experimental Max Tensile Strain Load Step
Pre-updating
Post-updating
1 2 3 4 5 6 7
107 102 97 91 95 97 90
124 119 113 106 110 113 105
8 9 10 11 12 13 14 15
97 92 97 99 99 96 93 92 96
113 107 113 116 116 111 109 107 113
Average
Following the identification of a possible problem with the experimental strain values for gauge number 1, the following investigation took place.
106
Molloy 2012 4.1.6 Experimental strain investigation To highlight possible inaccuracies in the measuring equipment a comparison of the theoretical values as a percentage of the experimental values are displayed in Figure 4.9. The values obtained for theoretical strain are based on the experimentally derived Young’s modulus which was derived in Table 4.5. Using this value the theoretical strain values were computed as shown in Table 4.6 which was then used as the basis for the graph in Figure 4.9. This graph gives an indication as to how each strain gauge performed during the experimental testing. It was noted on the day of the test that Gauge number 1 was displaying inconsistent readings which highlighted the need for further investigation. As the reading from this gauge has high significance in being the position of maximum tensile strain on the beam, the investigation was warranted. Gauge number 1 is highlighted in yellow and can be seen to be exceeding the 100% mark in all load steps. As the values shown in Figure 4.9 are the relationship of how much larger the theoretical strain values were compared to the measured values of gauge number 1, the conclusion is that the performance of strain gauge 1 was below that of the expected values. The result was an average required increase of 11% in the experimental strain data for gauge number 1.
107
Molloy 2012
15 14 13 12 11 10 9 8
Load Step
9
7 6
8
5 7
4
3 6
2 1
5 4 3 2 1
60
80
100
120
140
160
% Variation
Figure 4.9 - % Variation between experimental strain gauge readings and theoretical values
108
Molloy 2012 Following the % error calculated in Figure 4.9 a percentage error of 11% was computed in the experimental data for strain gauge No 1 which lead to an adjustment of the experimental data for this gauge reading. When the adjustment was accounted for the following graph was produced seen in Figure 4.10 which shows a closer relationship between the experimental tensile strain and the updated finite element model result.
0.00025 0.0002 0.00015
Strain
Pre-updated Updated
0.0001
Experimental
0.00005 0 0
1
2
3
4
5
6
7
8
9
10 11 12 13 14 15
Load Step
Figure 4.10 – Modified maximum tensile strain values (Gauge 1)
Table 4.11 shows the comparison between the pre and post-updating and how the tensile strain values compare to the experimental result. The post-updating value is almost 100% of the experimental result which was encouraging.
109
Molloy 2012 Table 4.11 – Modified tensile strain comparison Model % of Experimental Max Tensile Strain Load Step
Pre-updating
Post-updating
1 2 3 4 5 6 7 8 9 10 11 12 13 14 15
96 92 87 82 85 88 81 87 83 87 89 89 86 84 83 87
112 108 102 95 99 102 95 101 96 102 104 104 100 98 97 102
Average
4.1.7 Elastic Beam Bending Deflection Results As with the previous strain values, ANSYS produces a table of the recorded deformation values, Table 4.12 shows the maximum and minimum deflection values for each load step. Table 4.12 – ANSYS total deformation results Time [s] 1. 2. 3. 4. 5. 6. 7. 8. 9. 10. 11. 12. 13. 14. 15.
Minimum [m] 1.9114e-007 3.2795e-007 4.5913e-007 6.2779e-007 7.8708e-007 9.0889e-007 1.0775e-006 1.2368e-006 1.368e-006 1.5273e-006 1.6903e-006 1.8553e-006 1.9958e-006 2.127e-006 2.305e-006
Maximum [m] 4.1156e-005 7.061e-005 9.8854e-005 1.3517e-004 1.6946e-004 1.9569e-004 2.3201e-004 2.663e-004 2.9455e-004 3.2884e-004 3.6395e-004 3.9945e-004 4.2971e-004 4.5796e-004 4.9629e-004
110
Molloy 2012 The graphical result from ANSYS modeller for the maximum deflection is pictured in Figure 4.11. As expected the maximum deflection occurs at the centre of the beam. There are 16 images showing each load step increment of approximately 10N and it is not feasible to reproduce every one of them as they all show the maximum value of deflection for each load step at the midpoint of the beam. The video clip showing the transition through the load steps is visible on the CD in Appendix D.
Figure 4.11 – ANSYS maximum deflection graphic
Figure 4.12 shows the relationship between the experimentally produced deflections at the centre of the beam with those obtained from the finite element modelling pre and post-updating stages.
111
Molloy 2012 0.60
Deflection (mm)
0.50 0.40
Updated FE Model
0.30
Pre-Updated FE Model 0.20
Experimental Data
0.10 0.00 0
1
2
3
4
5
6
7
8
9 10 11 12 13 14 15
Load Step
Figure 4.12 – Maximum deflection values per load step
To compare the results in percentage form Table 4.13 displays the relationship between the pre and post-updated finite element models to the experimental measured deflection. While the measured deflection was still greater than the updated model, an improvement was seen in the post-updated model. Table 4.13 – Deflection comparison Model % of Experimental Deflection Load Step
Pre-updating
Post-updating
1 2 3 4 5 6 7 8 9 10 11 12 13 14 15
93 83 79 76 78 78 77 78 80 79 79 79 81 81 82 80
103 92 87 84 86 86 86 87 88 88 88 88 90 90 91 89
Average
112
Molloy 2012 As a further check on the performance of the finite element model on the deflection values, two other methods were implemented to predict the maximum deflection as described in the Methodology chapter. They were the finite element direct stiffness method and the double integration or Macaulay’s method for deflection. The following section is the results produced from those mathematical calculations.
4.1.8 Deflection results from finite element stiffness method Following the procedure outlined in the Methodology chapter the beam was broken down, or discretised into 4 elements and 5 nodes as seen in Figure 4.13.
Figure 4.13 –Beam discretised into 4 elements and 5 nodes
Based on the discretisation of the beam into 4 elements, an individual element stiffness matrix was computed and all 4 element stiffness matrices are produced in Table 4.14.
113
Molloy 2012 Table 4.14 – Element stiffness matrices Element 1 k1 L = .325
k2 L = 0.0775
1 350 56.8 -350 56.8
2 25779 1000 -25779 1000
6 56.8 12.3 -56.8 6.15 Element 2 7 1000 51.6 -1000 25.8
2 -350 -56.8 350 -56.8
7 56.8 6.1 -56.8 12.3
1 6 2 7
3 -25779 -1000 25779 -1000
8 1000 25.8 -1000 51.6
2 7 3 8
Element 3 k3 L = 0.0775
k4 L = .325
3 25779 1000 -25779 1000
4 350 56.8 -350 56.8
8 1000 51.6 -1000 25.8 Element 4 9 56.8 12.3 -56.8 6.15
4 -25779 -1000 25779 -1000
9 1000 25.8 -1000 51.6
3 8 4 9
5 -350 -56.8 350 -56.8
10 56.8 6.1 -56.8 12.3
4 9 5 10
Combining all 4 element matrices into 1 single structure matrix results in a 10 x 10 structure stiffness matrix and is presented in Table 4.15.
114
Molloy 2012 Table 4.15 – Combined structure stiffness matrix
1 2 3 4 5 6 7 8 9 10
1
2
3
4
5
6
7
8
9
10
350
-350
0
0
0
56.8
56.8
0
0
0
-350
26129
-25779
0
0
-56.8
943.2
1000
0
0
23
-25779
51558
-25779
0
0
-1000
0
1000
0
0
0
-25779
26129
-350
0
0
-1000
-943.2
56.8
0
0
0
-350
350
0
0
0
-56.8
-56.8
56.8
-56.8
0
0
0
12.3
6.15
0
0
0
56.8
943.2
-1000
0
0
6.15
63.9
25.8
0
0
0
1000
0
-1000
0
0
25.8
103.2
25.8
0
0
0
1000
-943.2
-56.8
0
0
25.8
63.9
6.15
0
0
0
56.8
-56.8
0
0
0
6.15
12.3
The combined structure stiffness matrix was then multiplied by the Young’s modulus (E) and the second moment of area (I) and results in the 10 x 10 matrix produced in Table 4.16.
Table 4.16 – Structure stiffness matrix multiplied by EI 6
7
1 2
1405250
1
-1E+06
0
0
0
228052
228052
0
0
0
-1E+06
1E+08
-1E+08
0
0
-228052
3786948
4015000
0
0
3 4
92345
-1E+08
2.1E+08
-1E+08
0
0
-4E+06
0
4E+06
0
0
0
-1E+08
1E+08
-1E+06
0
0
-4E+06
-4E+06
228052
0
0
0
-1E+06
1405250
0
0
0
-228052
-228052
228052
-228052
0
0
0
49384.5
24692.3
0
0
0
228052
3786948
-4E+06
0
0
24692.3
256559
103587
0
0
0
4015000
0
-4E+06
0
0
103587
414348
103587
0
0
0
4015000
-4E+06
-228052
0
0
103587
256559
24692.3
0
0
0
228052
-228052
0
0
0
24692
49384.5
5 6 7 8 9 10
2
3
4
5
8
9
10
The inverse of the matrix displayed in Table 4.16 was computed using the matrix function in Excel and the result is produced in Table 4.17 and is required as part of the solving process.
115
Molloy 2012 Table 4.17 – Computed 10 x 10 inverse matrix 1
2
3
4
5
1
1.1E-05
1.1E-05
1.1E-05
1.1E-05
1.1E-05
2E-19
7.1E-20
-2E-20
-7E-20
-2E-19
2 3 4 5 6 7 8 9
5.5E-05
2E-05
1.1E-05
1.4E-06
-4E-05
-0.0001
-0.0001
-0.0001
-0.0001
-0.0001
6.6E-05
2.2E-05
1.1E-05
-8E-07
-5E-05
-0.0001
-0.0001
-0.0001
-0.0002
-0.0002
7.8E-05
2.4E-05
1.1E-05
-3E-06
-6E-05
-0.0002
-0.0002
-0.0002
-0.0002
-0.0002
0.00013
3.4E-05
1.1E-05
-1E-05
-0.0001
-0.0003
-0.0003
-0.0003
-0.0003
-0.0003
0.00013
2.8E-05
-3E-18
-3E-05
-0.0002
-0.0003
-0.0004
-0.0004
-0.0004
-0.0004
0.00014
2.8E-05
-3E-18
-3E-05
-0.0002
-0.0004
-0.0004
-0.0004
-0.0004
-0.0004
0.00015
2.9E-05
-3E-18
-3E-05
-0.0001
-0.0004
-0.0004
-0.0004
-0.0004
-0.0004
0.00015
2.9E-05
-3E-18
-3E-05
-0.0001
-0.0004
-0.0004
-0.0004
-0.0004
-0.0004
0.00015
2.9E-05
-3E-18
-3E-05
-0.0001
-0.0004
-0.0004
-0.0004
-0.0004
-0.0003
10
6
7
8
9
10
To simplify the method the use of known constants wherever possible is a huge advantage. In the case of the beam being considered, and given the symmetrical nature of the beam itself, loading and support conditions, the reaction force at each end equated to half the total loading for each individual load step. Table 4.18 shows an example of the application of the total load applied in the experimental setup and entered into the cell which returns the required values for forces F1, F2, F4 and F5, refer to Figure 4.14 for force numbers. Full details of the method are available in CD format on in Appendix D. Table 4.18 – Constants for use in FE method (example values) Total Point load (N)
-151.3
Constants F1 F2
75.6 -75.6
F3 F4
0 -75.6
F5 F6 F7 F8 F9 F10
75.6 0 0 0 0 0
116
Molloy 2012
Figure 4.14 – Numbered system variables, degrees of freedom
A sample of the results produced from the previously mentioned data entry is produced in Table 4.19. The letter D in the table represents displacements, D3 and D10 being rotational displacements measured in radians and the required maximum deflection value in meters displayed as D3.
Table 4.19 – Results from FE method maximum displacement
Solution of Displacements
Deflection (m)
Rotation(Radians)
Rotation(Radians)
-1.95156E-18 -0.000368818
D1 D2
-0.000387258
D3
-0.000368818 8.67362E-17
D4 D5
-0.001465468
D6
-0.000475381 1.14492E-16 0.000475381
D7 D8 D9
0.001465468
D10
Centre of beam deflection
Rotation of beam at left end
Rotation of beam at right end
To represent the deflection data graphically a graph is produced in Figure 4.15 where only the maximum load step of 151.3N is applied to the method. The maximum value of displacement being – 0.387mm as a result.
117
Molloy 2012 0.0002
Displacement (m)
-4E-18 -0.095 0.005
Beam Length 0.105
0.205
0.305
0.405
0.505
0.605
0.705
0.805
-0.0002 -0.0004 -0.0006 -0.0008 -0.001
Figure 4.15 – Deflection results using FE method maximum displacement
4.1.9 Deflection results from Macaulay’s method Using the double integration method described in the Methodology chapter the following Table 4.20 shows the required table of values. Px1 is the position of the first point load from the left support and Px2 is the position of the second point load from the left support. L is the length of the beam.
Table 4.20 – Required table of values EI
L (m)
Px 1 (m)
Px 2 (m)
4015
0.805
0.325
0.48
Table 4.21 shows the resulting maximum deflection for each load step. The calculations were performed using Excel which can be seen on the spreadsheet in Appendix D.
118
Molloy 2012 Table 4.21 – Results from double integration method Constant A
Load(N)
0 -0.4901 -0.8398 -1.1765 -1.599 -2.0098 -2.3179 -2.7677 -3.1746 -3.4957 -3.913 -4.329 -4.758 -5.109 -5.447 -5.8968
0.00 12.57 21.53 30.17 41.00 51.53 59.43 70.97 81.40 89.63 100.33 111.00 122.00 131.00 139.67 151.33
Load each point(N) 0.00 6.28 10.77 15.08 20.50 25.77 29.72 35.48 40.70 44.82 50.17 55.50 61.00 65.50 69.83 75.60
Deflection (m) 0.00000 -0.00003 -0.00006 -0.00008 -0.00011 -0.00013 -0.00015 -0.00018 -0.00021 -0.00023 -0.00026 -0.00028 -0.00031 -0.00034 -0.00036 -0.00039
The comparison between the experimental, Macaulay’s, finite element stiffness method and the ANSYS updated model for the beam deflections are produced in graphical form in Figure 4.16.
0.6
Deflection (mm)
0.5 0.4 Experimental
0.3
Machauly
0.2
FE Method
0.1
Updated Model
0 0
1
2
3
4
5
6
7
8
9 10 11 12 13 14 15
Load Step
Figure 4.16 – Mathematically computed deflections comparison
119
Molloy 2012 Both the stiffness method and Macaulay’s method are in agreement with each other but differ to some extent to the experimental and updated ANSYS model of the beam. The close relationship between the experimental deflection results and the updated finite element model results are encouraging. The variation of the mathematical results is discussed later in the following chapter.
4.1.10 Finite element model summery Table 4.22 shows the summery description of the element types used by ANSYS in the meshing section of the setup.
Table 4.22 – ANSYS element summery Description Total Nodes Total Elements Total Body Elements Total Contact Elements Total Spot Weld Elements Element Types Coordinate Systems Materials Generic Element Type Name Quadratic Hexahedron
Quantity 3420 451 451 0 0 1 0 1 Mechanical APDL NASTRAN ABAQUS STL Name Name Name Name Solid186 CHEXA C3D20 N/A
4.1.11 Material data One of the updating parameters of this model was the material data. For this reason there are two material data sets. The manual changes to the Young’s modulus formed part of the model updating procedure. Table 4.23 shows the isotropic elasticity pre-updating while Table 4.24 shows the updated values.
120
Molloy 2012 Table 4.23 – Pre-updating isotropic elasticity Temperature C 22
Young's Modulus Pa 7.1e+010
Poisson's Ratio 0.33
Bulk Modulus Pa 6.9608e+010
Shear Modulus Pa 2.6692e+010
Bulk Modulus Pa 6.2745e+010
Shear Modulus Pa 2.406e+010
Table 4.24 – Updated isotropic elasticity Temperature C
4.2
Young's Modulus Pa 6.4e+010
Poisson's Ratio 0.33
Three hinge arch bridge results
4.2.1 Experimental reaction results The results from experimentally testing the three hinge arch bridge are not many as only the horizontal reactions from the resulting loading at the 11 locations were to be recorded. The values recorded by the force transducer of the HDA 200 interface are produced in Table 4.25 and are expressed in Newtons. The position for each load location is from the left end of the bridge. The values do not contain the self weight of the bridge as the force readings were set to zero prior to loading.
Table 4.25 – Horizontal reaction force at right hinge (N) Load Position (mm) 0 100 200 300 400 500 600 700 800 900 1000
Test 1 1 6.3 11.4 16.7 21.7 26.9 23.6 18.2 12.4 6.1 0.2
Test 2 1.8 6.9 12.1 18 22.8 28.5 24.9 19 13.1 6.8 0.9
Test 3 1.6 6.8 11.9 17.7 22.2 28 24.1 18.7 12.9 6.8 0.6
Test 4 0 4.7 10.2 15.5 20.3 26.2 22.3 16.6 10.9 4.6 1.2
Test 5 1.1 6.4 11.6 17.4 22 27.7 24 18.4 13 6.4 0.5
Average 1.1 6.22 11.44 17.06 21.8 27.46 23.78 18.18 12.46 6.14 0.68
121
Molloy 2012 4.2.2 ANSYS finite element model results First approach The three hinge arch was modelled by two different approaches as outlined in the Methodology section. The first is pictured in Figure 4.17 and represents only half of the bridge. The idea was to only model the setup as half the bridge as it was assumed that symmetry could be taken advantage of.
Figure 4.17 – First approach half arch
The results of placing the load, (12.4N) which was deemed half of the experimental load due to only using half of the bridge, are presented in Table 4.26. It was noted the value of the vertical reaction should change as the load is being moved along the bridge; this prompted a change in methodology.
122
Molloy 2012 Table 4.26 – Horizontal and vertical model results Load distance (m) Horizontal (N) Vertical (N)
0 30.189 12.4
0.1 24.059 12.4
0.2 17.93 12.4
0.3 11.79 12.4
0.4 5.66 12.4
0.5 0.15 12.4
Some of the other results for the bridge were also obtained such as the equivalent von-Misses stress. As an example of this the load at one section, 0.2 meters from the centre is chosen. The load being applied is depicted in Figure 4.18 with the right end support resulting reaction shown in Figure 4.19.
Figure 4.18 – Load located at 0.2m from centre
123
Molloy 2012
Figure 4.19 – Resulting reaction for load at 0.2 meters
The associated stress is depicted in Figure 4.20.
Figure 4.20 – Von-Mises stress for load at 0.2m from centre
124
Molloy 2012 Using the von-Mises stress failure criterion ANSYS produces a colour contour of the relevant stresses which are lightly to cause failure. The model showed agreement in such that the curved arch area was where concentrations of stresses were mostly felt. This was indicated by the dark red colour visible in Figure 4.20.
Second approach Following the errors witnessed in the first attempt, a second attempt was made to replicate the experimental setup and to have the model bridge perform like a three hinge arch bridge as close as possible. Reasons for doing so are outlined later in the discussion chapter. Figure 4.21 depicts the full 3 hinge arch bridge as modelled in ANSYS Design Modeller. The modelled bridge consist of 4 separate parts, the two main sections which make up the body of the bridge and two small hinges at the centre of the bridge which connect the two parts.
Figure 4.21 – Full bridge model
125
Molloy 2012 The types of joints which connect the body parts are outlined in the Methodology Chapter and their implications are discussed later in the Discussion Chapter. This method of modelling the bridge as a whole allows the structure to act like the experimental setup by the functioning revolute joint at the centre.
4.2.3 Mesh results details Meshing was performed automatically by ANSYS during the mechanical stage of the modelling process as outlined in the Methodology section. On closer examination of the centre of the bridge, as seen in Figure 4.22, there consist different element types for the hinges.
Figure 4.22 – Meshed connection at centre of bridge
It was possible to view the results of the elements by the use of the Finite Element Modeller as a system in the project schematic which allows details to be 126
Molloy 2012 viewed of the various types of elements being implemented by ANSYS and if adjustment needs to be made to the type of element it can be done here. Figure 4.22 above shows the blue elements as linear tetrahedron elements while the grey pins are linear hexahedron elements. The method of achieving a hinge at this point is by creating a joint element type for the pins as discussed in the Methodology Chapter.
Table 4.27 and Table 4.28 show a breakdown of the bodies and element types respectively. The larger element number is the main body while the smaller number is the pin connections at the centre of the bridge.
Table 4.27 – Bodies summery Body Name Solid Solid Solid Solid
Nodes 867 874 27 27
Elements 2229 2245 8 8
Table 4.28 – Element type summery Generic Element Type Mechanical APDL NASTRAN Name Name Name Linear Tetrahedron Mesh200 CTETRA Linear Hexahedron Mesh200 CHEXA
ABAQUS STL Name Name C3D4 N/A C3D8 N/A
4.2.4 Material data The material used in the model was structural steel and was pre-setup in the ANSYS material library. Table 4.29 and Table 4.30 show the values for the material constants and isotropic elasticity respectively.
127
Molloy 2012 Table 4.29 – Material constants Density 7850 kg m^-3 Coefficient of Thermal Expansion 1.2e-005 C^-1 Specific Heat 434 J kg^-1 C^-1 Thermal Conductivity 60.5 W m^-1 C^-1 Resistivity 1.7e-007 ohm m
Table 4.30 – Isotropic elasticity Temperature o C 22
Young's Modulus Pa 2.e+011
Poisson's Ratio 0.3
Bulk Modulus Pa 4.1667e+011
Shear Modulus Pa 1.9231e+011
4.2.5 Model results Table 4.31 shows the model results of the reaction forces at the supports for the applied loading at each position from the left end of the bridge.
Table 4.31 – Reaction force results from FE model Position (mm)
Load (N)
0 100 200 300 400 500 600 700 800 900 1000
24.8 24.8 24.8 24.8 24.8 24.8 24.8 24.8 24.8 24.8 24.8
Left Horizontal Reaction(N) 0.14811 6.4385 12.673 18.677 24.094 27.598 24.048 18.662 12.612 6.3426 0.022441
Left Vertical Reaction(N) 24.751 22.283 19.815 17.348 14.879 12.4 9.8698 7.4033 4.9353 2.4676 -5.48E-05
Right Horizontal Reaction(N) 0.14811 6.4385 12.673 18.677 24.094 27.598 24.048 18.662 12.612 6.3426 2.24E-02
Right Vertical Reaction (N) 4.94E-02 2.5171 4.9847 7.452 9.9208 12.4 14.93 17.397 19.865 22.332 24.8
The loading was applied at 11 locations along the bridge. The full report output from ANSYS can be viewed on the accompanying CD as the report is quite 128
Molloy 2012 detailed. For an example, one load location is presented here and the full results for that load. The load location chosen is at 800mm from the left end support. Figure 4.23 shows the load position on the model.
Figure 4.23 – Load positioned at 800mm from left end
The equivalent von-Mises stress is represented in Figure 4.24 where it can be seen that the largest area of stress is where the load is located which is to be expected.
129
Molloy 2012
Figure 4.24 – Equivalent von-Mises stress for load location
The resultant force reactions at the supports are depicted in Figure 4.25 showing the direction of the reaction force. The corresponding values for the horizontal and vertical components of the resultants are shown in Table 4.31 next to the 800mm distance.
Figure 4.25 – Left and right hand support reactions graphic
130
Molloy 2012
5 Discussion 5.1
T shaped aluminium beam
The aluminium T shaped beam is relatively simple structure however it has many significant important uses in construction and engineering. The process of designing beams for use as structural elements is mostly done nowadays by computers which utilise finite element analysis in their computation of resulting reactions, stresses and strains which occur due to applied loading. It is not a difficult process to setup a model of the required structure, nor is it complicated to apply the desired loading arrangement. It is however very important to know and understand the results that are being produced by such computer programs such as ANSYS or similar finite element analysis packages. The question of understanding the results and knowing where the finite element analysis program might be returning errors is the subject of this dissertation. The best way to compare the results from such finite element analysis programs is to conduct an experiment which is similar to the model, or in this case a model similar to the experimental setup. The first structure to be experimentally tested was the T shaped aluminium beam which was to be examined for the level of strain which was experienced in the beam at certain locations due to successive incremental loading. The beam was then modelled using ANSYS finite element analysis software to assess the performance of the model and compare the strain results with real data recorded from the experimental setup. The beam was subjected to loading increments of 10 Newtons (N) from zero up to approximately 150 N in the experiment. As this loading was not large enough to cause the material to yield, the results were linear as expected obeying Hooke’s Law.
131
Molloy 2012 Figure 5.1 shows the graph of the averaged values of strain recorded as the load was increased. It can be seen that the lines are generally strait indicating the material linearly elastic. The value for gauge number 1 appeared to be higher than the other values which prompted an investigation early on in the experiment as to the functionality of this gauge. This gauge reading was important as it was the location of maximum tensile strain experienced by the beam at each individual load increment. The results from Excel and the supporting graph are discussed in Section 4.1.6 in the Results chapter.
Experimental Averaged - µε v Load 250
1
Microstrain(µε)
200
2
150
3
100
4
50 0 -5 -50
5 15
35
55
75
95
115
135
6 7
-100 -150
155
8 Load(N)
9
Figure 5.1 – Load versus strain experimental results
The graph in Figure 5.1 shows 3 strain gage values as positive, positive strain indicating the tensile zone below the neutral axis and this is where gauges 1, 2 and 9 are located. The rest of the gauge values are negative, negative strain indicating shortening which is where the beam is experiencing compressive strain. Theoretically all lines on the graph should be straight in the case of a linear elastic isotropic material but in the case of these results there is some variation in the lines. This is mainly due to the electronic strain gauges
132
Molloy 2012 themselves showing variations as the extension or contraction of the various gauges is diminutive. Based on the experimental recorded strain values and the relationship between stresses, strain and Young’s modulus as described in Section 4.1.2, an average value for Young’s modulus was computed. This was found to be approximately 64 Gigapascals (GPa’s). This experimentally derived value is of significant importance to the model setup as the value is a material property and affects the bending behaviour of the material subjected to loading. 5.1.1 Finite element model The initial stage of the modelling was trial and error to some degree. Several attempts were made at creating a model to replicate the actual setup and some were with limited success. One issue was the supports at either end; the beam was tending to be adequately responsive to the loading and experienced lateral twisting when loading was applied. The problem was solved later with the application of remote displacement supports which allowed free or fixed rotation of the beam at either end in any desired plane. This lead to the selection of the plane normal to the length of the beam to be the only plane of rotation thus the other two planes could remain fixed in rotation. The remote displacement supports also allow the free or fixed condition for translation in the X, Y and Z directions to be selected. Allowing the relevant directions to be fixed resulted in the supports replicating a simple support condition which was representative of the experimental setup. The application of loading in the 3D model had its own difficulties. The initial method of applying the loads as two point loads pictured in Figure 5.2, which is representative of the experimental situation, proved to be inadequate.
133
Molloy 2012
Figure 5.2 – Initial loading arrangement
The location of the loads was set by applying a remote force but the method in which ANSYS applies the load did not produce the desired strain or displacement results. It seemed irrelevent where the point loads were placed on the beam, via entering coordinates entered in the remote displacement field, as to the possition of maximum deformation or strain values. The problem was with the selection of a reference edge or face in order to apply the load. The face selected was the top face shown as red in Figure 5.2 and this face becomes the origin point for the load being applied. This was not representative of the real situation. A possible future approach would be to create a small raised face at the points of loading and select this face as the reference for load application. Table 5.1 shows the allocation of the loadings Points 1 & 2 at their respective Z coordinates and the geomotry selection required as being 1 face.
134
Molloy 2012 Table 5.1 – Initial load and support values Object Name
Point Load 1
State Scoping Method Geometry Coordinate System X Coordinate Y Coordinate Z Coordinate Location
Point Load 2
Remote Displacement Fully Defined Scope Geometry Selection 1 Face Global Coordinate System
Remote Displacement 2
1.275e-002 m 4.75e-002 m 0.805 m 0. m Defined Definition Remote Force Remote Displacement Components 0. N (ramped) 0. m (ramped) Tabular Data 0. m (ramped) 0. N (ramped) Free No Deformable Free 0. ° (ramped) 0. ° (ramped) Free 0. ° (ramped) 0. ° (ramped) Advanced All
5.07e-002 m 0.327 m 0.478 m
Type Define By X Component Y Component Z Component Suppressed Behaviour Rotation X Rotation Y Rotation Z Rotation X Rotation Y Rotation Z Pinball Region
The tabular data in Table 5.1 for the Y directional compnent of the applied forces refers to the stepped incremental load application in ANSYS which is how the loading was applied in the experimental setup. Load steps of 1 second intervals were adopted and the values entered corresponded to the experimental values. The values corresponding to the applied loadings recorded in the experimental setup were entered as negative loading in the Y direction and are displayed in Table 5.2. The values in the table are half of the load recorded on the HDA 200 from the experiment as the load was applied in two locations in the real and experimental setup.
135
Molloy 2012 Table 5.2 – Point loads 1 & 2 stepped load values Steps Time [s] X [N] 1 0. 0. 1. 2 2. = 0. 3 3. 4 4. 5 5. 6 6. 7 7. 8 8. 9 9. 10 10. 11 11. 12 12. 13 13. 14 14. 15 15. 16 16.
Y [N] Z [N] 0. 0. -6.3 -12.25 = 0. -15.1 -20.5 -25.75 -29.7 -35.5 -40.7 -44.8 -50.15 -55.5 -61. -65.5 -69.85 -75.65 0.
The resulting strain at each load step is graphed in Figure 5.3 which shows the largest difference in the model compressive strain, at the maximum total applied load of approximately 151 N, is 61% less than the same experimental strain under the same conditions. This was an important observation as a difference of this magnitude could have significant replications if it was not noticed in a design process. Under estimation of strain values could lead to the beam being over strained if put into service under false data from design modelling software.
136
Molloy 2012 120 100
Strain x10-6
80 60
Two loads Experimental
40 20 0 0
1
2
3
4
5
6
7 8 9 Load Step
10 11 12 13 14 15
Figure 5.3 – Resulting maximum compressive strain
The resulting maximum deflection for each load step is presented in Figure 5.4 where a 51% lower value was experienced by the model beam compared to that of the experimental setup.
0.6
Max Delection(mm)
0.5 0.4
0.3 Two Loads
0.2
Experimental 0.1 0
0
1
2
3
4
5
6
7
8
9
10 11 12 13 14 15
Load Step
Figure 5.4 – Resulting maximum deflection
137
Molloy 2012 5.1.2 Model updating To update the model a different approach to the loading situation was adopted. Since the theoretical strain and experimental strain are linked to bending theory and beam bending equations the application of moment at each beam support was considered. Some analysis of the loading and support reactions was needed first, a simple static analysis. As the load applied in the experimental setup was applied in a symmetrical manner, being an equal distance from each support which gave an equal reaction at both supports, an equivalent moment could be applied at each end of the beam to replicate the effects of the combined point loads. The value for each moment, opposite in sense at either end, was a simple calculation of the force reaction at that end multiplied by the distance of the point load location from that end. This was computed in Excel for each of the applied loads for the 15 load steps and the results for the moment at the left end are presented in Table 5.3 with the corresponding ANSYS model graphic presented in Figure 5.5. The similar values, except positive in sense, were applied to the far end of the beam.
Table 5.3 – Applied moment at left end Steps Time [s] X [N·m] Y [N·m] Z [N·m] 1 0. 0. 0. 0. 1. -2.04 2 2. -3.5 = 0. = 0. 3 3. -4.9 4 4. -6.7 5 5. -8.4 6 6. -9.7 7 7. -11.5 8 8. -13.2 9 9. -14.6 10 10. -16.3 11 11. -18.04 12 12. -19.8 13 13. -21.3 14 14. -22.7 15 15. -24.6 16 16. 0.
Figure 5.5 – Applied moment
138
Molloy 2012 The resulting strain and deflection values from the application of the moments as the representative applied load moved closer to the experimental strain values. The initial values from this approach were still not close enough to the experimental results so another model updating technique was implemented. It was noticed that the isotropic elastic properties, Young’s modulus value, of the ANSYS material library value for aluminium was set at 71GPa’s which was resulting in a stiffer material being used by the model elements. The results from the experimentally derived Young’s modulus as seen in section 4.1.2 returned a value of 64GPa’s. This new value was used as a model updating parameter and proved to bring a closer correlation between the maximum tensile and compressive strain values of the model and the experimental results. The change in the maximum compressive strain experienced by the model beam went from 88% of the experimental compressive strain in the pre-updated model to 100% in the updated model. The change in the maximum tensile strain went from 87% to 102% of the experimental tensile strain values recorded. This proved a successful model updating procedure based on these results. Deflection values at the centre of the beam in the model also correlated well with the experimental results and were almost identical in the updated model. The deflection results from the mathematical methods, double integration and finite element stiffness, showed good correlation with each other but were on average for each load step 77% of the updated model deflection and were only 69% of the experimental deflection values. This could indicate a possible over estimation of the model deflection results but this can be ruled out by the correlation between the experimental results for deflection and the updated model values being almost equal. The remaining observation then is to assume the finite element stiffness method and Macaulay’s method for beam deflections under estimate the true deflection due to the assumptions made in section 3.2.3
139
Molloy 2012 5.2
Three hinge arch bridge
The three hinge arch bridge is a significant structural form which is more economical in terms of performance in wide spans than beams. The horizontal reactions produced at the supports reduce the bending moment experienced in the bridge. The experimental setup for the bridge recorded horizontal reactions at one end only as a known mass was positioned at 100mm intervals from one end to the far end. These results were compared to mathematically calculated values for verification before they were used to verify the ANSYS finite element model of the bridge. 5.2.1 Finite element model The first approach to the modelling of the bridge is explained in section 3.4.4 and outlines the initial model as half of the experimental bridge. The attempt was hoped to make use of the symmetrical nature of the real bridge geometry and by utilising remote displacements shown in Figure 5.6.
Figure 5.6 – Remote displacement supports 1 & 2
The remote displacement in the graphic on the left in Figure 5.6 was modelled as having zero translation in the X and Z directions with free translation in the Y 140
Molloy 2012 direction and free rotation in the Z plane which was aimed at replicating a pin type connection at this location like in the experimental setup. A similar remote displacement supporting condition was placed at the right hand hinge but free rotation in the Z plane was allowed here thus providing horizontal and vertical reactions like the experimental setup but allowing rotational hinge like behaviour. The results output for the ANSYS finite element model of the bridge did not compare well with the expected results based on the experimental setup. The vertical reaction remained a constant value even though the load was moved in 100mm increments from one end to the other; this should not be the case as shown in the mathematically calculated values based on the principles of the 3 hinge arch bridge displayed in Table 5.4 which were calculated in Excel.
Table 5.4 – Mathematically calculated force reactions Position (mm)
Load (N)
Left Left Vertical Right Horizontal Reaction(N) Horizontal Reaction(N) Reaction(N) 0.00 24.8 0.00
Right Vertical Reaction (N)
0
24.8
100
24.8
5.51
22.32
5.51
2.48
200
24.8
11.02
19.84
11.02
4.96
300
24.8
16.53
17.36
16.53
7.44
400
24.8
22.04
14.88
22.04
9.92
500
24.8
27.56
12.4
27.56
12.4
600
24.8
22.04
9.92
22.04
14.88
700
24.8
16.53
7.44
16.53
17.36
800
24.8
11.02
4.96
11.02
19.84
900
24.8
5.51
2.48
5.51
22.32
1000
24.8
0.00
0.00
0.00
24.8
0.00
It is clear to see from the results in Table 5.4 that both end support reactions (vertical and horizontal) of the bridge change reciprocally with the varying position of the mass. This was the data which prompted a new and more detailed approach to the modelling of the bridge as a full bridge. 141
Molloy 2012 The full bridge was modelled as described in section 3.4.4 attempt two. The model represented the function of a three hinge arch bridge as shown by the results in Table 4.31 in the Results Chapter. To assess the performance of the finite element analysis a percentage comparison between the experimental, mathematical and model reaction results was performed. The following tables make use of Excel to analyse the data from each result origin. Maximum and minimum values of both the horizontal and vertical reaction were searched for and the resulting maximum or minimum value was returned in a cell with the corresponding origin of that result placed in the cell next to it. A sample of the formula used was: =IF(Z22=H29,"Experimental",(IF(Z22=Z7,"Mathematical",(IF(Z22=AJ7,"Model"))))) The following Table 5.5, Table 5.6, Table 5.7 and Table 5.8 are the results from the analysis and compare the performance of the ANSYS model support reaction results to those of the experimental and mathematically calculated results.
Table 5.5 –Maximum reactions at left hand support Load Stage (m) 0
Max value of LH Hz (Newtons) 1.10 Exp
% Exp 100.00
% Model 742.69
Max value of LH V % % (Newtons) Math Model 24.8 Math 100 100.2
0.1
6.44
Model
103.51
100.00
22.32
Math
100
100.2
0.2
12.67
Model
110.78
100.00
19.84
Math
100
100.1
0.3
18.68
Model
109.48
100.00
17.36
Math
100
100.1
0.4
24.09
Model
110.52
100.00
14.88
Math
100
100.0
0.5
27.60
Model
100.50
100.00
12.4
Math
100
100.0
0.6
24.05
Model
101.13
100.00
9.92
Math
100
100.5
0.7
18.66
Model
102.65
100.00
7.44
Math
100
100.5
0.8
12.61
Model
101.22
100.00
4.96
Math
100
100.5
0.9
6.34
Model
103.30
100.00
2.48
Math
100
100.5
1
0.68
Exp
100.00
3030.17
0
Math
100
0.0
142
Molloy 2012 Table 5.6 – Minimum reactions at left hand support Load Stage (m) 0
Min Value of LH Hz (Newtons) 0.00 Math
% Exp 0.00
% Model 0.00
Min value of LH V (Newtons) 24.751 Model
% % Math Model 99.8 100
0.1
5.51
Math
88.60
85.60
22.283
Model
99.8
100
0.2
11.02
Math
96.35
86.97
19.815
Model
99.9
100
0.3
16.53
Math
96.91
88.52
17.348
Model
99.9
100
0.4
21.80
Exp
100.00
90.48
14.879
Model
100.0
100
0.5
27.46
Exp
100.00
99.50
12.4
Math
100.0
100
0.6
22.04
Math
92.70
91.67
9.8698
Model
99.5
100
0.7
16.53
Math
90.94
88.59
7.4033
Model
99.5
100
0.8
11.02
Math
88.46
87.39
4.9353
Model
99.5
100
0.9
5.51
Math
89.76
86.89
2.4676
Model
99.5
100
1
0.00
Math
0.00
0.00
-5.5E-05
Model
0.0
100
Table 5.7 – Maximum reactions at right hand support Load Stage(m) 0
Max Value of RH Hz % (Newtons) Exp 1.10 Exp 100.00
% Model 742.69
Max Value of RH V % % (Newtons) Math Model 4.94E-02 Model 100.0 100
0.1
6.44
Model
103.51
100.00
2.52E+00
Model 101.5
100
0.2
12.67
Model
110.78
100.00
4.98E+00
Model 100.5
100
0.3
18.68
Model
109.48
100.00
7.45E+00
Model 100.2
100
0.4
24.09
Model
110.52
100.00
9.92E+00
Model 100.0
100
0.5
27.60
Model
100.50
100.00
1.24E+01
Math 100.0
100
0.6
24.05
Model
101.13
100.00
1.49E+01
Model 100.3
100
0.7
18.66
Model
102.65
100.00
1.74E+01
Model 100.2
100
0.8
12.61
Model
101.22
100.00
1.99E+01
Model 100.1
100
0.9
6.34
Model
103.30
100.00
2.23E+01
Model 100.1
100
1
0.68
Exp
100.00 3030.17
2.48E+01
Math 100.0
100
143
Molloy 2012 Table 5.8 – Minimum reactions at right hand support Load Stage 0
Min Value of RH Hz (Newtons) 0.00 Math
% Exp 0.00
% Model 0.00
Min Value of RH V % % (Newtons) Math Model 0.00E+00 Math 100 0.0
0.1
5.51
Math
88.60
85.60
2.48E+00
Math
100
98.5
0.2
11.02
Math
96.35
86.97
4.96E+00
Math
100
99.5
0.3
16.53
Math
96.91
88.52
7.44E+00
Math
100
99.8
0.4
21.80
Exp
100.00
90.48
9.92E+00
Math
100
100.0
0.5
27.46
Exp
100.00
99.50
1.24E+01
Math
100
100.0
0.6
22.04
Math
92.70
91.67
1.49E+01
Math
100
99.7
0.7
16.53
Math
90.94
88.59
1.74E+01
Math
100
99.8
0.8
11.02
Math
88.46
87.39
1.98E+01
Math
100
99.9
0.9
5.51
Math
89.76
86.89
2.23E+01
Math
100
99.9
1
0.00
Math
0.00
0.00
2.48E+01
Math
100
100.0
The tables were created using Microsoft Excel with the following abbreviations used:
Math: mathematical results
Exp: experimentally recorded results
Model: ANSYS finite element modelled results
Three result origins are represented in the results tables above which show the model results for the maximum left hand horizontal reaction being returned for almost all loading positions. When compared to the experimental result for the same reaction the model exceeds the experimental result by approximately 4%. The left hand vertical reaction maximum value was returned by the mathematically obtained value but only exceeded the model result by 0.3% on average for each load location. This result shows the successful outcome from the modelling process. There were no experimental vertical reaction results for the bridge. The minimum reaction values show good correlation between the results with a slight variation the horizontal results which show the mathematically calculated results being the minimum value for almost all of the load stages. The model 144
Molloy 2012 value was never a minimum value for this reaction. The minimum reaction values of the left hand vertical reactions show good correlation between the mathematical and model results. In a similar fashion the reactions for the right hand supports show good correlation between model, mathematical and experimental results. It can be deduced from this that the modelling procedure implemented in the second attempt is representative of the experimental setup and could be used as a design tool with confidence.
145
Molloy 2012
6 Conclusion and recommendations This dissertation shows methods of verifying the results output from finite element analysis software for structural analysis. The finite element analysis code ANSYS was used. Two laboratory structures were tested and a 3D model of each was created in ANSYS and the loads applied in a similar manner to the experimental setup. The result of each model output was then compared to the experimental results for verification. Simple model updating was performed to calibrate each model to replicate the physical experimental setup such as material properties and actual model representation. The first structure to be experimentally tested was a T shaped aluminium section of beam 805mm long. This structure was tested for the strain effects at the centre of the beam while being subjected to 10 Newton (N) incremental loads from 0N up to 150N. The strain was tested using electronic strain gauges at 9 locations around the periphery of the beam face. The resulting strain from each location was then used to assess the Young’s modulus of the material. A 3D finite element model was created in ANSYS and the load applied, using a similar moment value to replicate the point loading, and maximum compression and tensile strain values and maximum deflection were recorded. It was observed that the initial results were of less magnitude than the experimental result. This was due to the ANSYS isotropic material properties for aluminium as set by the program for Young’s modulus was 71GPa’s. Having obtained a value of 64GPa’s for the experimental beam this became a model updating parameter. The updated model showed an average increase in the model maximum tensile strain from 87% to 102% of the experimental value and an average increase in the model maximum compressive strain from 88% to 100% of the experimental value thus showing a successful model updating procedure. The second structure to be experimentally tested was the three hinge arch bridge. The bridge was tested for horizontal support reactions at one end while a 146
Molloy 2012 mass of 2.536kg (24.8N) was moved to 11 locations along the bridge deck. Self weight of the bridge was ignored in the test. The bridge was then modelled with ANSYS to compare its performance with the experimental results. The main issue with this structure was the method of modelling in ANSYS which lead to two separate attempts at modelling. The first was attempt was modelled as half the bridge with an attempt at replicating a hinge at the centre by the use of remote displacements and setting up the appropriate boundary conditions. This proved to be unsuccessful as the vertical reactions in the model were unresponsive to the changing load position. The second attempt updated the model itself by creating a modified geometry of the entire 3 hinge arch bridge. The main feature of the model was the application of revolute joints (MPC 184, ANSYS library element) at the centre connection of the bridge to allow the joint to function as a hinge. This proved a successful model updating procedure as the updated results showed the model exceeding the horizontal reaction force by only 4% of the experimental result. The validity of finite element models is essential in trusting the output results. Proving the results is not always made possible by replicating a physical test similar to the model. For this reason more study needs to conducted as to the actual performance of individual element types by other means. The effects of static loading were only tested here but more emphasis on the dynamic effects on structures like bridges subjected to moving vehicles or seismic activity need to be conducted and a means of calibrating these effects without conducting physical experiments on the structure. The analyst must convey apt knowledge of the procedures involved in producing finite element models In spite of the great power of FEA, the disadvantages of computer solutions must be kept in mind when using this method as they do not necessarily reveal how the output values are influenced by important problem variables such as materials properties and geometrical features, and errors in input data can produce wildly incorrect results that may be overlooked revealing drastic consequences. 147
Molloy 2012
7 Bibliography
Akin, J. (2012) FEA Concepts. Concepts of Stress Analysis. [Online].
Available
at:
http://www.clear.rice.edu/mech403/HelpFiles/FEM_stress_concepts.pdf [Accessed:25/11/2012].
Ansys
(2012)
Fundimental
FEA
Concepts
and
Applications.http://www.see.ed.ac.uk/~fmill/CAE3/ANSYSstuff/ANSYS%20Materi als/ANSYS_Workbench-fea_concepts.pdf [Accessed.20/09/2012].
Beal, A. (2000) Who Invented Young's Modulus. [Online]. Available at:
http://anbeal.co.uk/TSE2000YoungsModulus.pdf [Accessed: 10/10/2012].
Bolognese,
J.
(2012)
FEMCI
Book.http://femci.gsfc.nasa.gov/femcibook.html.
Caprani, C. (2007) Structural analysis III Compatibility of displacements &
the principle of superposition.
Chan, C.L., Khalid, Y.A., Sahari, B.B. & Hamouda, A.M.S. (2002) Finite
element analysis of corrugated web beams under bending. Journal of Constructional Steel Research, 58 (11) pp. 1391-1406.
Chan, T.H.T., Li, Z.X., Yu, Y. & Sun, Z.H. (2009) Concurrent multi-scale
modeling of civil infrastructures for analyses on structural deteriorating—Part II: Model updating and verification. Finite Elements in Analysis and Design, 45 (11) pp. 795-805.
Clough, R. (2004) Early history of the finite element method from the
viewpoint of a pioneer. Internation journal for numerical methods in engineering, 60 (1).
Colorado (2012) Direct Stiffness Method. [Online]. Available at:
http://www.colorado.edu/engineering/cas/courses.d/IFEM.d/IFEM.Ch02.d/IFEM .Ch02.pdf [Accessed: 13/02/2012].
Cook, R. (2002) Concepts and Applications of Finite Element Analysis. New
Jersy: John Wiley and Sons 148
Molloy 2012
Davis, R.O. & Selvadori, A. (1996) Elasticity and Geomechanics. New York:
Press Syndicate
Djafour, M., Djafour, N., Megnounif, A. & Kerdal, D.E. (2010) A
constrained finite strip method for open and closed cross-section members. Thin-Walled Structures, 48 (12) pp. 955-965.
Esfandiari, A., Bakhtiari-Nejad, F., Sanayei, M. & Rahai, A. (2010)
Structural finite element model updating using transfer function data. Computers & Structures, 88 (1–2) pp. 54-64.
Fahy, M. & Tiernan, S. (2001) Finite element analysis of ISO tank
containers. Journal of Materials Processing Technology, 119 (1–3) pp. 293-298.
Ghali, A. (2009) Structural Analysis. Oxon: Spon
Han, L.-H., Wang, W.-D. & Zhao, X.-L. (2008) Behaviour of steel beam to
concrete-filled SHS column frames: Finite element model and verifications. Engineering Structures, 30 (6) pp. 1647-1658.
Haukaas, T. (2012) Euler-Bernoulli Beams. [Online]. Available at:
www.inrisk.ubc.ca. [Accessed:24/12/12].
Hinojoso, H. (2010) Calibration under uncertainity for finite element
models of masonary monuments. Washington: Los Almos national laboratory.
Hyperphysics (2012) Elasticity, Elastic Properties. [Online]. Available at:
http://hyperphysics.phy-astr.gsu.edu/hbase/permot3.html
[Accessed:
21/02/2012].
Imechanica (2012) Principal of virtual work and the finite element
method.
[Online].
Available
at:
http://imechanica.org/files/3_Principle%20of%20virtual%20work%20and%20FE M.pdf [Accessed: 17/04/2012].
John, V. (1978) Materials for Technology Students. London: Macmillan
Press
Kangas, S., Wang, X., Hunt, V. & Swanson, J. (2012) Field test based
calibration of bridge finite element models for condition assesment. [Online]. Available
at:
http://www.uc.edu/ucii/pubs/CONF%20-%20ASNT%20149
Molloy 2012 %202003%20-%20Field%20TestBased%20Calibration%20of%20Bridge%20Finite%20Element%20Models%20for% 20Condition%20Assessment%20%20Kangas,%20Wang,%20Padur,%20Li,%20Lui,%20Helmicki,%20Swanson,%20H unt.pdf.
Kong, F.K. (1997) Structural Analysis. Hong Kong: Chapman and Hall
Korunovic, N. (2011) Finite Element Analysis of a Tire Steady Rolling on
the Drum. Journal of Mechanical Engineers.
Liu, L.E.I. (2004) AN AUTOMATIC CALIBRATION STRATEGY FOR 3D FE
BRIDGE MODELS. Thesis. University of Cincinnati.
Mccarthy, M.A., Mccarthy, C.T., Lawlor, V.P. & Stanley, W.F. (2005) Three-
dimensional finite element analysis of single-bolt, single-lap composite bolted joints: part I—model development and validation. Composite Structures, 71 (2) pp. 140-158.
Moaveni, S. (1999) Finite Element Analysis. New Jersy: Prentice Hall
Nasa (1995) A Verification Procedure for MSC/NASTRAN Finite Element
Models. NASA Contractor Report. [Online]. Available at.
O’brien, E.J. & Keogh, D.L. (1998) Upstand finite element analysis of slab
bridges. Computers & Structures, 69 (6) pp. 671-683.
Rao, K. & Sharinvasa, U. (2012) A set of pathelogical tests to validate new
finite elements. Sadhana, 26 (6) pp. 549-590.
Roylance, D. (2012) Introduction to Fracture Mechanics. [Online].
Available at: http://ocw.mit.edu/courses/materials-science-and-engineering/311-mechanics-of-materials-fall-1999/modules/frac.pdf [Accessed.
Schlune, H., Plos, M. & Gylltoft, K. (2009) Improved bridge evaluation
through finite element model updating using static and dynamic measurements. Engineering Structures, 31 (7) pp. 1477-1485.
Son, J.-K. & Fam, A. (2008) Finite element modeling of hollow and
concrete-filled fiber composite tubes in flexure: Model development, verification
150
Molloy 2012 and investigation of tube parameters. Engineering Structures, 30 (10) pp. 26562666.
Utc (2012) Assesment of the Bill Emerson Memorial Cable-Stayed Bridge.
Vki (2012) Visual Kinematics, Inc. Home Page. [Online]. Available at:
http://www.vki.com/ [Accessed: 14/04/2012].
Wu, J.R. & Li, Q.S. (2006) Structural parameter identification and damage
detection for a steel structure using a two-stage finite element model updating method. Journal of Constructional Steel Research, 62 (3) pp. 231-239.
Zapico-Valle, J.L., Alonso-Camblor, R., González-Martínez, M.P. & García-
Diéguez, M. (2010) A new method for finite element model updating in structural dynamics. Mechanical Systems and Signal Processing, 24 (7) pp. 2137-2159.
Zhu, J.-H. & Young, B. (2006) Aluminum alloy circular hollow section
beam-columns. Thin-Walled Structures, 44 (2) pp. 131-140.
Zárate, B.A. & Caicedo, J.M. (2008) Finite element model updating:
Multiple alternatives. Engineering Structures, 30 (12) pp. 3724-3730.
151
Molloy 2012
8 Appendices
Appendix A – Dissertation Mind Map.................................................................A-1 Appendix B – ANSYS Full Report: Beam....................................Separate Document Appendix C – ANSYS Full Report: 3 Hinge Arch Bridge ............Separate Document Appendix D – CD Containing Electronic Support Information.....Inside Front Cover
152
Molloy 2012 A.
Appendix A – Dissertation Mind Map
Appendix A – Dissertation Mind Map
Figure A.1 – Dissertation Mind Map
A-1