BORANG PENGESAHAN STATUS TESIS

UNIVERSITI TEKNOLOGI MALAYSIA PSZ 19:16 (Pind. 1/ 97) BORANG PENGESAHAN STATUS TESIS JUDUL : FINITE ELEMENT ANALYSIS ON THE STRENGTH OF FLUSH ENDPLATE CONNECTION WITH TRAPEZOID WEB PROFILE BEAM USING LUSAS SOFTWARE SESI PENGAJIAN : 2007/2008 Saya _ MUHAMMAD JOHAN BIN JOHARI _ (HURUF BESAR) mengaku membenarkan tesis (PSM/Sarjana/Doktor Falsafah)* ini disimpan di Perpustakaan Universiti Teknologi Malaysia dengan syarat-syarat kegunaan seperti berikut : 1. Hakmilik tesis adalah di bawah nama penulis melainkan penulisan sebagai projek bersama dan dibiayai oleh UTM, hakmiliknya adalah kepunyaan UTM. 2. Perpustakaan Universiti Teknologi Malaysia dibenarkan membuat salinan untuk tujuan pengajian sahaja. 3. Perpustakaan dibenarkan membuat salinan tesis ini sebagai bahan pertukaran di antara institusi pengajian tinggi. 4. ** Sila tandakan ( ) SULIT TERHAD (Mengandungi maklumat yang berdarjah keselamatan atau kepentingan Malaysia seperti yang termaktub didalam AKTA RAHSIA RASMI 1972.) (Mengandungi maklumat TERHAD yang telah ditentukan oleh organisasi/badan di mana penyelidikan dijalankan.) TIDAK TERHAD Disahkan oleh, (TANDATANGAN PENULIS) (TANDATANGAN PENYELIA) Alamat Tetap : 23 Jln Padi Ria 8, Bandar Baru Uda, P. M. DR. SARIFFUDDIN BIN SAAD (Nama Penyelia) 81200 Johor Bahru, Johor. Tarikh : 22 NOVEMBER 2007 Tarikh : 22 NOVEMBER 2007 Catatan * Potong yang tidak berkenaan. ** Jika tesis ini SULIT atau TERHAD, sila lampirkan surat daripada pihak berkuasa/ organisasi berkenaan dengan menyatakan sekali tempoh tesis ini perlu dikelaskan sebagai SULIT atau TERHAD. Tesis dimaksudkan sebagai tesis bagi Ijazah Doktor Falsafah dan Sarjana secara penyelidikan, atas disertasi bagi pengajian secara kerja kursus dan penyelidikan, atau Laporan Projek Sarjana Muda (PSM).

I hereby declare that I have read this thesis and in my opinion this thesis is sufficient in terms of scope and quality for the award of the degree of Master of Engineering (Civil Structure) Signature :... Name of Supervisor : P. M. DR. SARIFFUDDIN BIN SAAD Date : 22 NOVEMBER 2007

FINITE ELEMENT ANALYSIS ON THE STRENGTH OF FLUSH ENDPLATE CONNECTION WITH TRAPEZOID WEB PROFILE BEAM USING LUSAS SOFTWARE MUHAMMAD JOHAN BIN JOHARI A project report submitted in partial fulfillment of the requirements for the award of the degree of Master of Engineering (Civil Structure) Faculty of Civil Engineering Universiti Teknologi Malaysia NOVEMBER 2007

ii I declare that this thesis entitled Finite Element Analysis on the Strength of Flush Endplate Connection With Trapezoid Web Profile Beam Using LUSAS Software is the result of my own research except as cited in the references. The thesis has not been accepted for any degree and is not concurrently submitted in candidature of any other degree. Signature :... Name : MUHAMMAD JOHAN BIN JOHARI Date : 22 NOVEMBER 2007

Ayahanda, bonda dan adik-adik tercinta Pengorbanan dan kasih sayang Menjadi dorongan iii

iv ACKNOWLEDGEMENT First of all, I would like to take this opportunity to express my sincerest appreciation to my project supervisor, P. M. Dr. Sariffuddin bin Saad for his advices and guidance throughout the course of this research. Thank you for all your support and kindness. Next, I would like to thank all my friends who have helped me throughout my postgraduate study. Special thanks goes towards Mr. Tai Wai Yau and Miss Fuang Siew Lu, who have extended their hands in helping me in completing this research. My most heartfelt gratitude and appreciation goes to my beloved family, who are always there when I needed them most. Muhammad Johan bin Johari

v ABSTRACT Conventional design for steel constructions utilize simple or full strength connection between beam to column connections. However, a majority of the actual connections show a partial strength behaviour. Lack of use of partial strength design is mainly due to lack of understanding of their behaviour, and full scale laboratory tests have been done for this reason. However, full scale tests are expensive and time consuming, and finite element modeling using existing software is a preferred alternative. The flush endplate is used in this research for the partial strength connection, with Trapezoid Web Profiled steel section as beam and hot rolled UC section as column. Three dimensional finite element model of flush endplate connection has been developed and analyzed using LUSAS, to develop the momentrotation relationship of the connection and to determine its moment resistance. Validation of the finite element result was done by comparing them with existing experimental results. It was found that the finite element moment resistance, M R, was 28.17% more than the test result. The moment-rotation (M-Ф) of both methods show similar characteristics. The modes of failure for both experimental and finite element models are also similar.

vi ABSTRAK Rekabentuk struktur keluli biasanya dilakukan dengan menggunakan sambungan mudah atau sambungan tegar bagi sambungan di antara rasuk dan tiang. Bagaimanapun, kebanyakan kelakuan sambungan sebenar adalah separa tegar. Kekurangan penggunaan sambungan separa tegar di dalam rekabentuk sambungan keluli adalah disebabkan oleh kurangnya pemahaman mengenai kelakuan sambungan itu sendiri, dan ujikaji makmal berskala penuh telah dijalankan untuk tujuan itu. Ujikaji makmal berskala penuh adalah mahal dan mengambil masa yang panjang, oleh itu permodelan menggunakan kaedah unsur terhingga menggunakan perisian sedia ada lebih digemari. Sambungan keluli jenis plat hujung sedatar telah diambil sebagai sambungan di dalam projek ini, di samping rasuk berprofil trapezoid. Model unsur terhingga tiga dimensi telah dibina menggunakan perisian LUSAS, untuk mendapatkan lengkung momen-putaran dan rintangan momen bagi sambungan tersebut. Keputusan daripada analisis LUSAS telah dibandingkan dengan keputusan makmal untuk menentukan keberkesanan analisis menggunakan kaedah unsur terhingga bagi sambungan ini. Didapati bahawa momen rintangan bagi kaedah unsur terhingga adalah 28.17% lebih tinggi daripada keputusan makmal. Graf momenputaran (M-Ф) bagi ujikaji makmal dan analisis unsur terhingga menunjukkan ciriciri yang hampir sama. Mod kegagalan model yang diperolehi melalui kedua-dua kaedah juga adalah serupa.

vii TABLE OF CONTENTS CHAPTER TITLE PAGE DECLARATION ii DEDICATION iii ACKNOWLEDGEMENT iv ABSTRACT v ABSTRAK vi TABLE OF CONTENTS vii LIST OF TABLES xi LIST OF FIGURES xii LIST OF SYMBOLS xv LIST OF APPENDICES xvi 1 INTRODUCTION 1.1 Introduction 1 1.2 Problem Statement 3 1.3 Research Objective 3 1.4 Research Scope 3 2 LITERATURE REVIEW 2.1 Finite Element Method 5 2.1.1 Nonlinear Finite Element Analysis 6 2.1.1.1 Geometric Nonlinearity 7 2.1.1.2 Boundary Nonlinearity 8

viii 2.1.1.3 Material Nonlinearity 9 2.2 LUSAS 9 2.2.1 Nonlinear Solution Procedure in LUSAS 11 2.2.2 LUSAS Element Library 12 2.3 Connections 17 2.3.1 Rigid Connections 17 2.3.2 Simple Connections 18 2.3.3 Semi Rigid Connections 19 2.3.4 Bolted Flush Endplate Connection 22 2.4 Research Studies 24 2.4.1 Comparison of Partial Strength Connection Between Extended and Flush End-Plate Connections With Trapezoid Web Profiled Steel Sections [2] 24 2.4.2 Finite-Element Analysis of Unstiffened Flush End-Plate Bolted Joints [3] 25 2.4.3 Behavior of Flush End-Plate Connection Connected to Column Flange [11] 26 2.4.4 Modeling for Moment-Rotation Characteristics for End-Plate Connections [12] 27 2.4.5 Structural Behavior of End-Plate Bolted Connections to Stiffened Columns [15] 29 2.4.6 Refined Three-Dimensional Finite Element Model for End-Plate Connection [16] 30 2.4.7 Other Studies 31

ix 3 METHODOLOGY 3.1 Introduction 34 3.2 Experimental Test 35 3.2.1 Experimental Framework 35 3.2.2 Specimens 36 3.2.3 Test Procedure 39 3.3 Finite Element Model 40 3.3.1 Model Components 40 3.3.1.1 Endplate 41 3.3.1.2 Beam 42 3.3.1.3 Column 43 3.3.1.4 Bolts and Nuts 44 3.3.2 Element Types 45 3.3.2.1 HX8M (3D Continuum Element) 45 3.3.2.2 QTS4 (Thick Shell Element) 46 3.3.2.3 JNT4 (Joint Element) 47 3.3.3 Nonlinear Material Properties 48 3.3.4 Boundary Conditions 49 3.3.5 Loading 50 4 RESULTS AND DISCUSSION 4.1 Introduction 51 4.2 Experimental Results 51 4.3 Finite Element Analysis Results 53 4.3.1 Moment-Rotation (M-Ф) Curve 54 4.3.1.1 Moment, M 54 4.3.1.2 Rotation, Ф 55 4.3.2 Mode of Failure 62 4.4 Result Comparisons 63 4.4.1 Comparison of Moment-Rotation (M-Ф) Curve 63

x 4.4.2 Comparison of Moment Resistance M R 64 4.4.3 Comparison of Mode of Failure 65 4.5 Moment-Rotation Curves at Different Points Along the Beam 66 5 CONCLUSION 5.1 Conclusion 69 REFERENCES 71 Appendix A 74-85

xi LIST OF TABLES TABLE NO. TITLE PAGE 2.1 Element groups in LUSAS [8] 14 3.1 Geometrical configurations of the tested connections [2] 37 4.1 Calculation of the moments and corresponding rotations at each load increment for specimen FEP1P1-2 58 4.2 Comparison of moment resistance for specimen FEP1P1-2 between experimental and analytical results 65

xii LIST OF FIGURES FIGURE NO. TITLE PAGE 2.1 Example of geometric nonlinearity behavior [5] 8 2.2 Beam element connected to columns through the use of rigid connections [6] 18 2.3 Beam element connected to columns through the use of simple connections [6] 19 2.4 Moment-rotation characteristics of typical rigid, semi rigid and simple connections [9] 20 2.5 Moment-rotation (M-Ф) curves of semi rigid connections [13] 21 2.6 Semi rigid connection types [13] 22 2.7 Typical flush endplate connection 23 3.1 Testing rig used in the experiment [2] 36 3.2 Arrangement for specimen FEP1P1-2 38

xiii 3.3 Full LUSAS finite element model of specimen FEP1P1-2 41 3.4 Endplate model 42 3.5 Beam model 43 3.6 Column model 44 3.7 Bolt model 45 3.8 HX8M solid element [8] 46 3.9 QTS4 thick shell element [8] 47 3.10 JNT4 3D joint element [8] 48 3.11 Boundary conditions 50 4.1 Experimental moment-rotation curve for specimen FEP1P1-2 52 4.2 Mode of failure for specimen FEP1P1-2 [2] 53 4.3 Applied load P and the moment arm [6] 54 4.4 Location of inclinometers for specimen FEP1P1-2 [6] 55 4.5 Calculation of rotation 56 4.6 Moment-rotation curve for specimen FEP1P1-2 (model) 61

xiv 4.7 Mode of failure of the connection 62 4.8 Moment-rotation relationship for the experimental and model 64 4.9 Comparison of mode of failure for specimen FEP1P1-2 66 4.10 Moment-rotation curves for different points along the beam 68

xv LIST OF SYMBOLS M R - Moment resistance M - Bending moment Ф - Rotation M-Ф - Moment-rotation TWP - Trapezoid Web Profiled S j,ini - Initial stiffness p y - Design strength k c - Elastic spring stiffness P - Applied load dx - Displacement in X direction dy - Displacement in Y direction

xvi LIST OF APPENDICES APPENDIX TITLE PAGE A Tensile test results 74

CHAPTER 1 INTRODUCTION 1.1 Introduction Steel construction holds substantial advantages over reinforced concrete construction. These advantages can be based on factors such as flexibility, durability, quality and economy. The flexibility of steel construction can be discussed as its ability to be customized to suit the construction requirements, regardless of the size of the structure to be constructed. Steel is also more durable compared to reinforced concrete, in the sense that it can better withstand chemical and environmental attacks. Steel maintenance primarily focuses on corrosion whereby for reinforced concrete wider range of maintenance is needed. The quality of steel is also generally of higher standard, because they are manufactured in factories where the quality is controlled. Although the cost of steel is high, fast erection and elimination of falsework will provide a reduction in overall cost of construction. Also, because steel is lightweight, it is the most suitable material for high rise constructions.

2 Steel structures are built using many components, such as tension members, compression members, bending members, combined force members and connections [1]. Amongst the said components, connections are the most critical. Most steel structure failures are caused by inadequate and poorly designed connections, while failure due to main structural members is rare. Conventional steel constructions utilize pinned or rigid connection between beam to column connections, where only nominal moment is designed to be transferred from the beam to the column for the former, and full moment transfer is designed for the latter. Another type of connection can be designed for beam to column connections in steel construction, where it utilizes a condition between simple and rigid connection design. This type of design is known as semi rigid or partial strength connection design. However, as opposed to conventional design, the value of the moment resistance, M R, of the connection must be known prior to designing using the semi rigid design. Expensive laboratory work and testing is needed to determine the value of moment resistance for a specific connection and also to understand its behaviour, particularly the mode of failure. This experimental method is not only costly, but also time consuming. An alternative method is modelling of the connections by finite element method using computer software. Because of the developments in the fields of finite element analysis and computer technology, this method is not only made possible, it is also more economical, less time consuming, and various types of connections can be modeled with relative ease.

3 1.2 Problem Statement A semi rigid bolted flush endplate connection represents various complexity and undefined problems with many parameters affecting its behaviour and structural capacity. It is costly and time consuming to undertake laboratory testing to understand the real behaviour of the connection. To save time and cost, finite element analysis is an ideal approach in order to understand the characteristics of semi rigid flush endplate connections, such as moment resistance and mode of failure. However, the accuracy of the analytical results from finite element analysis needs to be validated by comparisons with the results of full scale laboratory tests. 1.3 Research Objective The objective of this research is to model a flush endplate connection using finite element method. From the results of the analysis, the moment-rotation (M-Ф) curve of the connection is to be plotted in order to determine the moment resistance (M R ) of the connection. Furthermore, comparisons need to made between the analytical results and the results obtained from full scale laboratory tests in order to determine its accuracy. 1.4 Research Scope In this research, a semi rigid beam to column connection will be analyzed using finite element analysis software, LUSAS 13.57 [2]. This research is focused

4 on a bolted flush endplate connection, and it is modeled by connecting the endplate of a trapezoid web profiled beam to the flange of an I section column. The dimensions for the model will follow the dimensions used in the full scale laboratory test, conducted by M. Md. Tahir et al. [3], in which the comparisons will also be referred to.

CHAPTER 2 LITERATURE REVIEW 2.1 Finite Element Method The finite element method has become a powerful tool for the numerical solution of a wide range of engineering problems. With the advances in computer technology, complex problems can be modeled with relative ease [4]. In this method of analysis, a complex region defining a continuum is discretized into simple geometric shapes called finite elements. The material properties and the governing relationships are considered over these elements and expressed in terms of unknown values at the nodes. An assembly process, considering the loading and constraints, results in a set of equations. Solution to these equations gives the approximate behaviour of the continuum [5]. The procedures for analysis using finite element method first involve idealization of the system, which involves the formulation of governing equations and boundary conditions. The system is then discretized into finite elements, and then appropriate interpolation functions are selected. The element properties are then determined and assembled to form a set of global equations. Solution of these

6 equations will give a numerical result which will then need to be interpreted and evaluated. Although finite element method can be used to solve any engineering problem provided the governing equation is determined, it is a very complex method. The governing differential equation may be very difficult even for a simple system. The engineer must practice extra care for generating error free input data for the software. Undetected errors in input data may result in error solutions that might appear acceptable. Hence, checking the accuracy of the results is an important phase for finite element analysis. Furthermore, finite element method is only an approximate numerical method, where assumptions are made in the formulation. Proper judgment needs to be practiced to generate acceptable results. 2.1.1 Nonlinear Finite Element Analysis In linear finite element analysis, assumptions made are that all materials in the structure are linearly elastic and that the deformations of the analyzed structure is sufficiently small to be insignificant when considering the overall behaviour of the structure. Even though very few situations in the real world adhere to this description, with some restrictions and assumptions, the majority of engineering problems can be applied with linear finite element analysis. However, cases requiring special attention to gross changes in geometry, permanent deformations, structural cracks, buckling, stresses greater than the yield stress and contact between component parts indicate that a nonlinear finite element analysis is required [2].

7 There are generally three types of nonlinear behaviour in a structure namely geometric nonlinearity, boundary nonlinearity and material nonlinearity [1], [2], [6]. There is also another type of nonlinear structural behaviour where the magnitude or direction of the applied forces changes with application to the structure (nonlinear force-deflection relationship) [7]. 2.1.1.1 Geometric Nonlinearity Geometric nonlinearities are due to significant changes in the structural configuration during loading [1], [2], [6]. In this problem a nonlinear straindisplacement relationship is observed [7]. Figure 2.1 illustrates a geometric nonlinearity problem. In the figure, the horizontal force causes the column to deform horizontally, and the linear solution would fail to consider the progressive eccentricity of the vertical force. Depending on how large the horizontal deformation is, serious errors could be introduced if the effect of geometric nonlinearity is neglected.

8 Figure 2.1 Example of geometric nonlinearity behaviour [2] 2.1.1.2 Boundary Nonlinearity Boundary nonlinearity occurs when the deformation of the structure causes the external restraints to deform. This will result in a nonlinear displacementdeformation relationship [6], [7]. In this problem the external restraints are needed to be modified, usually due to lift-off or smooth or frictional contact during the process within an analysis [2]. 2.1.1.3 Material Nonlinearity

9 Material nonlinearity occurs when the model exhibits a nonlinear stress-strain relationship. It can be observed in structures undergoing nonlinear elasticity, plasticity, viscoelasticity, creep or other inelastic effects [7]. 2.2 LUSAS LUSAS is a finite element analysis software product which can analyze all types of linear and nonlinear stress, dynamics, composite and thermal engineering problems. It was first developed in 1970 at London University as a research tool of finite element technology. Since then, LUSAS has become a powerful tool for the solution of various types of linear and nonlinear problems. The LUSAS software provides four specialist products, namely LUSAS Bridge, LUSAS Civil & Structure, LUSAS Composite and LUSAS Analyst. A complete finite element analysis involves three stages [2]: Pre-Processing Finite Element Solver Results Processing (post processing) The LUSAS finite element system consists of two parts to perform a full analysis; LUSAS Modeller will perform the pre-processing and post processing of the analysis and is fully graphical user interface, while LUSAS Solver will perform the actual finite element analysis.

10 In LUSAS, pre-processing involves creating a model for the structure to be analyzed, assigning its properties, and then outputting the information as a formatted data file suitable for processing by LUSAS. A model is a graphical representation of the structure to be analyzed, and for the LUSAS model, features such as points, lines, surfaces and volumes need to be defined in order to define its geometry. After that the model needs to be assigned with its attributes before it is ready to be analyzed. The basis of drawing the geometric model is by having points which will create lines, lines or combined lines will produce surfaces, and the combination of surfaces will produce volumes for a three dimensional model. An attribute is first defined by creating an attribute dataset. It is then assigned to appropriate features to define its properties. The LUSAS attribute types include geometric, mesh, materials, supports and loading. Once a model is completed the solution stage can begin, and using the data file from the model, LUSAS Finite Element Solver will solve the stiffness matrix and produce a results file. Some of the data that can be contained in the results file include stresses, strains, displacements, velocities, accelerations, reactions, potentials, fluxes, gradients, fatigue datasets and strain energy. Results processing in LUSAS involves a selection of tools for viewing and analyzing the results file produced by the LUSAS Finite Element Solver. Many different ways for viewing the results are supported, such as averaged/smoothed contour plots, unaveraged/unsmoothed contour plots, deformed/undeformed mesh plots, Wood-Armer deformation calculations, Animated display of modes or load increments, section line plots, yield flag plots, graph plotting, or vector plots.

11 2.2.1 Nonlinear Solution Procedure in LUSAS In nonlinear analysis, it is impossible to directly obtain a stress distribution which equilibrates a given set of external loads. A solution procedure is adopted in LUSAS is to apply the total required load in increments. Within each increment a linear prediction of the nonlinear response is made, and subsequent iterative corrections are performed in order to restore equilibrium by the elimination of the residual forces. The iterative corrections are referred to some form of convergence criteria which indicates to what extent an equilibrate state has been achieved. Such a solution procedure is therefore commonly referred to as an incremental-iterative method. In LUSAS, the nonlinear solution is based on the Newton-Rhapson procedure. The details of the solution procedure are controlled using the nonlinear control properties assigned to load case. For the analysis of nonlinear problems, the solution procedure adopted may be of significance to the results obtained. In order to reduce this dependence, wherever possible, nonlinear control properties in LUSAS incorporate a series of generally applicable default settings, and automatically activated facilities. In LUSAS the incremental-iterative solution is based on the Newton-Rhapson iterations. In the Newton-Rhapson procedure an initial prediction of the incremental

12 solution is based on the tangent stiffness from which the incremental displacements and their iterative corrections may be derived. Load incrementation for nonlinear problems in LUSAS may be specified in four ways. It can either be specified by manual incrementation where the loading data in each load increment is specified separately; automatic incrementation where a specified load case is factored using fixed or variable increments; mixed incrementation between manual and automatic incrementation; or load curves where the variation of one or more sets of loading data is specified as a load factor against load increment or time step load curve. The choice and level of incrementation will depend on the problem to be solved. Where an increment has failed to converge within the specified maximum number of iterations it will be automatically reduced and reapplied. This will be repeated according to values specified until the maximum number of reductions has been tried. In a final attempt to achieve a solution the load increment is then increased to try and step over a difficult point in the analysis. If the solution still fails to converge, the solution is then terminated. 2.2.2 LUSAS Element Library The LUSAS element library contains more than 100 element types. The elements are classified into groups according to their functions. The LUSAS element groups are: Bars Beams

13 2D Continuum Elements 3D Continuum Elements Plates Shells Membranes Joints Field Elements Interface Elements Each element group is sub-divided into element sub-groups according to the type of formulation. Within each sub-group, elements vary according to the geometry, the number of nodes, and the properties required for each element. The individual elements are referred to by their LUSAS name. Table 2.1 shows the various element groups available in the LUSAS element library.

Table 2.1 Element groups in LUSAS [8] 14

15 A brief description of each element group is given below. a. Bar Elements Bar elements are used to model plane and space frame structures, and stiffening reinforcement. LUSAS incorporates 2 and 3-dimensions bar elements which may either be straight and curved. Bar elements model axial force only. b. Beam Elements Beam elements are used to model plane and space frame structures. LUSAS incorporates a variety of thin and thick beams in 2 and 3-dimensions. In addition, specialized beam elements for modeling grillage or eccentrically ribbed plate structures are available. LUSAS beam element may be either straight or curved and may model axial force, bending and torsion behaviour. c. 2D Continuum Elements 2D continuum elements are used to model solid structures whose behaviour may reasonably be assumed to be two-dimensional. 2D continuum elements may be applied to plane stress, plane strain and axisymmetric solid problems. Triangular and quadrilateral elements are available. Fourier elements, which allow non axisymmetric loading to be applied to axisymmetric models, are considered a special case of the 2D continuum elements since the mesh is defined entirely in the xy-plane, but the resulting displacements, stresses and strains are purely three-dimensional. In addition, special crack tip elements are available to model the singularities encountered at crack openings, and explicit elements are available to model high speed dynamics problems efficiently. d. 3D Continuum Elements 3D continuum elements are used to model fully three-dimensional structures. Tetrahedral, pentahedral an hexahedral solid elements are available to model full three-dimensional stress fields.

16 e. Plate Elements Plate elements are used to model flat structures whose deformation can be assumed to be predominantly flexural. LUSAS incorporates both thick and thin plate elements. Triangular and quadrilateral flexural plate elements are available. Ribbed plate elements are also available to model 2D structures whose behaviour is dependent on both flexural and membrane behaviour. f. Shell Elements Shell elements are used to model three-dimensional structures whose behaviour is dependent upon both flexural and membrane effects. LUSAS incorporates both flat and curved shell elements, which may be either triangular or quadrilateral. Both thick and thin shell elements are available. g. Membrane Elements Membrane elements are used to model two and three-dimensional structures whose behaviour is dominated by in-plane membrane effects. LUSAS incorporates both axisymmetric and space membrane elements. Membrane elements incorporate in-plane behaviour only. h. Joint Elements Joint elements are used to model flexible joints between other LUSAS elements. LUSAS incorporates a variety of joint elements which are designed to match the nodal freedoms of their associated elements. Joint elements may also be used to model point masses, elasto-plastic hinges, or smooth and frictional element contacts.

17 i. Field Elements Field elements are used to model quasi-harmonic equation problems such as thermal conduction or potential distribution. LUSAS incorporates bar, plane, axisymmetric solid and three-dimensional solid field elements. Thermal link elements are also available. j. Interface Elements These elements should be used at places of potential delamination between 2D continuum elements for modeling delamination and crack propagation. 2.3 Connections In steel construction, individual members such as beams and columns are attached to each other to form a stable structure. The form of attachment utilizes the use of connections, which are the connecting elements of the steel structure. These elements such as angles and plates, are attached to other members through the process of welding or bolting. Connections can be categorized into three groups; rigid, semi rigid and simple connections [1], [3], [6], [7]. 2.3.1 Rigid Connections Rigid connections are connections with rigidity, sufficient to maintain the original angle between intersecting members that is virtually unchanged under the design load. Figure 2.2 shows a beam element connected to columns through the use of rigid connections. Rigid connections are designed to be fully restraint, in which

18 theoretically no relative rotation should occur between the connected members. In this connection, full continuity of the connection is maintained [3] where the bending moment is transferred fully from the beam to the column, along with shear and axial forces [6]. Figure 2.2 connections [6] Beam element connected to columns through the use of rigid 2.3.2 Simple Connections Simple connections are those connections that provide zero rotational restraint at the connections. Figure 2.3 shows a beam element connected to columns through the use of simple connections. In design, simple connections are assumed to transfer shear force only [7], from the beam to the column, besides nominal moment [3] and axial load [6]. This means that members with simple connection are free to rotate when load is applied. When designing using simple connections, the member is assumed to be simply supported, and care should be taken in construction so as not to provide extra strength to the connection, because the column might fail from buckling due to the extra moment transferred to it.

19 Figure 2.3 connections [6] Beam element connected to columns through the use of simple 2.3.3 Semi Rigid Connections Although it is common to design using either simple or rigid connections, a majority of the connections do not fall under this categories. This is because it is hard to maintain such idealized situation, where either no relative rotation should occur for rigid connections, and no moment is transferred in simple connections. Many connections transfer some bending moments and rotation occurs to a certain degree. This type of connection is called the semi rigid connection, or partial strength connection. Typical moment-rotation (M-Ф) relationships for rigid, semi rigid and simple connections are shown in Figure 2.4.

20 Figure 2.4 connections [9] Moment-rotation characteristics of typical rigid, semi rigid and simple A semi rigid connection have a moment resistance less than that of the connected beam. Such behaviour is termed partial strength by Eurocode 3 [10]. Partial strength is defined as a connection with moment resistance which is less than that of the member [11]. Beam to column connection is generally assumed to be either perfectly pinned or perfectly rigid [7]. This simplification leads to an incorrect estimation of the behaviour of the connection, where it is actually between the two assumptions. In order to be able to utilize the partial strength capability of these connections in design, the moment resistance of the connections is needed to be determined through their moment-rotation relationship [3]. Various researches have been done for this purpose [1], [3], [4], [6], [7], [11]. There are twelve basic classifications of semi rigid connections which are identified by connection type [6], [7]:

21 Web side plate (shear tab) Single web cleat (single angle) Double web cleats (double angle) Flange cleats (flange angles) Bottom flange cleat and web cleat (seat and web angle) Header plate (shear endplate) Flush endplate Extended endplate Combined web and flange cleats Tee stubs Top plate and seat cleat (angle) Tee stubs and web cleat (angle) However, the widely used semi rigid connections are of the angle cleat and the endplate connections [12]. Figure 2.5 shows the relative moment-rotation (M-Ф) curves of these semi rigid connections, while they are illustrated in Figure 2.6. Figure 2.5 Moment-rotation (M-Ф) curves of semi rigid connections [13]

22 Figure 2.6 Semi rigid connection types [13] 2.3.4 Bolted Flush Endplate Connection Bolted endplate connections are extensively used for connecting beams to columns in steel frame constructions. They have the advantage of requiring less supervision and a shorter assembly time than welded connections [14], [15]. The

23 popularity of these type of connections can be attributed to the fact that it results in handling of fewer pieces in the field [16]. These connections may be either flush or extended endplate types, depending mainly on their strength and stiffness requirements. A typical flush endplate bolted connection comprises a rectangular steel plate of nearly the same depth as the depth of the beam, which is welded to the end of a beam. This assembly is connected to the flange of the column by one or two pairs of high strength steel bolts near the beam compression flange [4]. The flush endplate bolted connection will be the focus of this research. The connection moment capacity is influenced by the endplate thickness [1], [6], [7] and column web stiffening [4], [6], [7]. The position of bolts in the tension area may also influence the connection moment capacity. Other types of parameters that may affect the behaviour of the endplate connection include column flange and web thickness, beam depth, and also bolt sizes and grades [1]. Figure 2.7 shows a typical flush endplate connection. Figure 2.7 Typical flush endplate connection

24 2.4 Research Studies 2.4.1 Comparison of Partial Strength Connection Between Extended and Flush End-Plate Connections With Trapezoid Web Profiled Steel Sections [3] This paper was prepared by Md. Tahir, et al. [3] at Universiti Teknologi Malaysia in 2006. In this study, four sets of partial strength connections were tested, two for flush endplate and two for extended endplate connections. The modes of failure for the specimens were limited to the tension region of the joint, whereas the form of deformation for the flush endplate connections was the translation of the tip of the endplate away from the face of the column, and for the extended endplate connections, the endplate was translated away from the face of the column in a Y-shape form. The curves for moment-rotation (M-Ф) relationships showed that the connections behaved linearly in the first stage followed by nonlinear behaviour whilst gradually losing its stiffness with the increase in rotation. The knee method was used to determine the moment resistance, M R of the connections from the moment-rotation curves. The overall results showed that the experimental values of moment resistance were greater than the theoretical values with the ratio ranged in between 0.77 to 1.17.

25 2.4.2 Finite-Element Analysis of Unstiffened Flush End-Plate Bolted Joints [4] This reported about the investigation on the behaviour of unstiffened flush endplate bolted joints by means of finite element analysis. The LUSAS package was chosen as the tool for the finite element analysis of the joints, and the accuracy of the results were verified through comparisons with the results of some full scale tests performed at the University of Abertay Dundee. For the LUSAS finite element model, three types of elements were used for modeling, namely BRS2 bar element, HX16 3D continuum element and JNT4 joint element. The bar element was used to model the bolts in both the tension and compression regions of the joint, the 3D continuum element was used to model the column webs and flanges, endplates, and also the beam webs and flanges. The joint element meanwhile was used to generate the prying force at the interface of the endplates and column flanges. The nonlinear solution procedure adopted in this study was the Newton- Rhapson procedure, which is an incremental iterative method, in which the total load is applied in a number of increments. In this study, automatic load incrementation was used, which is included in the LUSAS package. For the test program of the experiment, a total of six full scale tests were performed which incorporated two beam sizes, two connection details, two bolt sizes and two column sizes. It was noted that the bolts were hand tightened by a podger spanner, and no washers were used. Comparisons between analytical and test results were made in the form of moment-rotation characteristics and also bolt strains. The authors agreed that in

26 general, there was a good agreement between experimental and analytical results, although some discrepancies existed. This might be due to bolt tightening effect, imperfection of the test setup, thread stripping and lack of fit. The authors suggested that the European Standards were adopted to prevent failures due to thread stripping. It was concluded that a model of an unstiffened flush endplate joint applying the finite element method to carry out a three dimensional elastoplastic analysis of the joint was generated successfully, although the effects of welds, bolt heads and column fillets were not included in the model. This was because it was assumed that they generate insignificant contributions to the moment-rotation characteristics of the joints. 2.4.3 Behaviour of Flush End-Plate Connection Connected to Column Flange [11] This paper, prepared by Mahmood Md. Tahir, et al., was presented at the 8 th East Asia-Pacific Conference on Structural Engineering and Construction in 2001. The objective of this study is to predict the moment resistance, M R and initial stiffness, S j,ini of flush endplate connections connected to column flange in order to find the capacity of the connection used in semi continuous constructions. In this study, a total of seven tests were conducted at Universiti Teknologi Malaysia laboratory, which comprised of three column and beam sizes, two bolt sizes and various connection configurations. The connections were fabricated so that the study of the performance of the connections due to different geometry configurations were made possible.

27 In the test procedure, the load was applied incrementally sufficient enough to cause extensive inelastic deformation of the connection, unloaded, and then followed by reverse loading to study the complete response. However, since this paper only described the prediction of moment resistance and initial stiffness of the connection in the first phase of loading, the connections response in the second phase was not included. It is to note that the readings were only recorded after two minutes of time lapse, to allow the specimen to reach an equilibrium state. The moment-rotation curves showed that the connections behaved linearly in the first stage followed by nonlinear behaviour and gradually losing its stiffness with the increase in rotation. By adopting the knee method technique to the momentrotation curves of the connections, the moment resistance of the connection was established. The overall results showed that the experimental values of moment resistance were greater than the theoretical values with the ratio ranged from 1.02 to 1.68. 2.4.4 Modeling for Moment-Rotation Characteristics for End-Plate Connections [12] This paper was prepared to develop an elastoplastic model for bolted endplate connections based on the T-stub yield and beam theories and to model the connection resistance and the moment-rotation relationship of the connection. With this model, the difficulties of modeling some characteristics such as torque and lack of fit in finite element model can be overcome. This paper tried to find a simple and sufficiently accurate method to analyze the semi rigid connection behaviour that could be directly used in connection design and frame analysis.

28 The proposed deformation model included models for the deformations in the tension zone, compression zone, shear zone and also T-stub deformation and column web tension deformation. However, the beam deformation was not included. This paper argued that the beam curvature contributed little to the connection unless for stiff connections with higher bending moment. So, for the rotation of a partial strength and semi rigid connection, the effect of beam deformation could be neglected. The nonlinear moment-rotation relationship for a given connection detail was determined from the models of the deformations in the proposed deformation model. When verifying the proposed model with existing experimental results, it was seen that for extended endplate connections, the maximum moment resistance obtained from the theoretical analysis are much smaller than test results, while for flush endplates, the values were quite close. It was also observed that there were differences in moment resistance for thin endplates, these were attributed to strain hardening and post yield strength which were not considered in the model. This was because that the connection tests were loaded up to bolt fracture. For the model, the initial tangent stiffness is higher than the test result, and gradually reduced to zero at yield. It was argued that the tangent stiffness for the model was smaller than the test result when the moment approached the yield moment due to the neglected hardening effect. As for the moment capacity, smaller values were expected when comparing with test results, because the proposed model assumed the yield stress as the ultimate stress of the connection components except for the bolts. This conservative underestimation of the moment resistance leads to an overdesigned structure.

29 2.4.5 Structural Behaviour of End-Plate Bolted Connections to Stiffened Columns [15] This paper was prepared by Bahaari and Sherbourne [15]. In this paper, endplates connected to stiffened columns were analyzed and presented in terms of their moment-rotation behaviour, with particular attention towards prestressed and hand-tightened bolts. The authors argued that the purpose of bolt pretension in connections was to delay the contribution of bolts to the deformation and rotation of the joint, while hand-tightened bolts simply alloweed the plates to pull away and changed their curvature at low levels of load. It was found that the early stiffness of endplate connections with regard to the influence of bolt pretension was higher for thick endplates as compared to thin endplates. However, at low values of connection moment, two identical connections, one having pretensioned bolts while the other utilizes hand-tightened bolts, displayed identical initial stiffnesses. Meanwhile, near the connections ultimate capacity, the two connections shows similar characteristics. The comparison made to the moment-rotation curves of the connections between analytical and experimental values for the hand-tightened thin endplate connections show good agreement, while for thick endplates the experimental moment-rotation behaviour is more flexible. As for prestressed bolts, the analytical model for thin endplate is more flexible than the experimental data. The authors argued that the test data was unreliable, since its initial stiffness was threefold to that of hand-tightened model,

30 while for thin endplate the flexibility was gained through plate deformability, and bolts contributed about 25% at most. For thick endplates with prestressed bolts, the analytical model showed a more flexible behaviour at later stage. It was concluded that the flexibility of the model around the ultimate load was attributed to more bolt elongation in the model, as well as possible differences between the real and assumed material properties. 2.4.6 Refined Three-Dimensional Finite Element Model for End-Plate Connection [16] This paper is about the investigation on the behaviour of endplate connections through finite element analysis by using the ADINA code. A refined threedimensional finite element model was developed by incorporating a 3D nonconforming solid element developed by the authors, where the variable node transition solid elements are used for the effective connection between the refined and coarse regions in the local mesh refinement. Besides that, a contact algorithm also developed by the authors was employed to simulate the interaction between the endplate and column flange. The effects of bolt pretension and the shapes of the bolt shank, head and nut were also taken into consideration. The comparisons of moment-rotation relationship between the analytical models and test data shows that, coarse meshing of the analytical models gave more flexible curves and by using fine meshing, the results were better correlated with the

31 test data. Besides that, by using nonconforming element as opposed to conforming elements, the analytical results were better correlated. The finite element solution by the model with fine meshing and nonconforming elements provided nearly the same moment-rotation relationship as the test results, except at a higher load range where the torsional twisting was developed in the experiment. 2.4.7 Other Studies Numerous studies of experimental and analytical nature have been conducted to study the behaviour of semi rigid steel bolted endplate connections, particularly the flush endplate and the extended endplate types. Md. Tahir, et al. [11] conducted experiments to study the behaviour of flush endplate connection connected to column flange, with particular attention directed towards the results of moment and shear, comparing them with theoretical results conforming with the procedures based on Eurocode 3 [10] and BS 5950 [17]. Sulaiman, et al. [18] investigated the moment-rotation relationships of extended endplate connections incorporating beams with Trapezoidal Web Profiled (TWP) sections, in order to find the behaviour of partial strength joints in terms of the moment capacities of the joints. Md. Tahir, et al. [3] compared the behaviour of partial strength extended and flush endplate connections with TWP sections as beams, in terms of the three main

32 characteristics of partial strength connections; strength, rigidity and ductility. The experimental results were validated theoretically using the component method proposed by Steel Construction Institute. Meanwhile, various studies have also been conducted to investigate the behaviour of semi rigid connections analytically, incorporating various parameters such as flush and extended endplates, stiffened and unstiffened column flanges, hand-tightened and prestressed bolts, using various types of analysis including three dimensional finite element modeling. Shi, et al. [12] developed an elastoplastic model of bolted endplate connections based on the T-stub yield theory and beam theory. The model assumed that the yield stress as the ultimate stress of the connection components except for the bolts, which leads to the underestimation of the moment resistance of the connections and an overdesigned structure. Bahaari and Sherbourne [15] evaluated analytically the behaviour of endplate connections to stiffened columns using nonlinear finite element analysis, with particular attention to prestressed and hand-tightened bolts. By incorporating a half model of flush endplate joint in the LUSAS package, Bose, et al. [4] analyzed the flush endplate bolted joints using three-dimensional finite element analysis. A refined three dimensional finite element model for endplate connections was developed by Choi and Chung [16], incorporating a three dimensional nonconforming elements and contact algorithm with gap elements developed by the authors.

33 Although there are many analytical investigations conducted to study the behaviour of flush endplate bolted connections, there are still no studies conducted to investigate the same type of connection incorporating the TWP sections as beams, even though experimental studies have been conducted [3], [11], [18] to be used as validation.

CHAPTER 3 METHODOLOGY 3.1 Introduction In this research, the bolted flush endplate connection was investigated using finite element analysis method. Among the wide variety of commercial finite element software packages available that are able to carry out a nonlinear finite element analysis are LUSAS, ANSYS, COSMOS/M, ABAQUS and NASTRAN. In this research, LUSAS version 13.57 was selected as the tool for the purpose of analyzing the problem and determining the moment-rotation (M-Ф) curve of the proposed beam to column connection. In order to meet the research objective of determining the validity of finite element analysis using LUSAS software, full scale experimental moment-rotation (M-Ф) results were obtained from a previous research and used as reference, and compared with the analytical (M-Ф) results from the finite element analysis.

35 3.2 Experimental Test The experimental work was done by M. Md. Tahir et al. in the structural laboratory at Universiti Teknologi Malaysia [3]. It was a full scale laboratory test with a total of four sets of specimens and was done in conjunction with other research. For the purpose of this research, only one specimen, namely specimen FEP1P1-2 was focused on for the finite element modeling and for comparisons with the analytical results. 3.2.1 Experimental Framework The experimental framework was arranged in a situation similar to the arrangement of testing rig and frame components as shown in Figure 3.1. The experiment was set up by connecting a 3 m high column with a 1.5 m spanning beam. The bottom part of the column was restrained from any movement while the top of the column was supported by rollers which only allow the column to move freely in vertical direction. This means that the top of the column was free in vertical direction but fixed from movement in horizontal direction.

36 Figure 3.1 Testing rig used in the experiment [3] 3.2.2 Specimens Two sets of flush endplate connections, namely FEP1P1-2 and FEP2R20P1, and two sets of extended endplate connections, namely EEP2R20P1 and EEP3R20P1, were arranged for the testing, making up a total of four sets of specimens in this experimental work. Two sets of column sizes were used, 254 254 107 UC was used for the specimens with flush endplate connections, and 305 305 118 UC was used for the specimens with extended endplate connections. The beams used were of the Trapezoid Web Profiled (TWP) steel sections, with three different sizes. The endplates used were of the 200 12 size, and all the

37 bolts were of grade M20. The geometrical configurations of the tested connections are summarized in Table 3.1. Table 3.1 Geometrical configurations of the tested connections [3] For the particular specimen focused in this research, specimen FEP1P1-2, the column used was of the 254 254 107 UC size and 3 m high with a steel grade of S275. The beam was a Trapezoid Web Profiled steel section with a size of 400 170 49/12/6 and a length of 1.5 m with the flange s steel grade of S355 and the web s steel grade of S275. The endplate in use was of the size of 460 200 12 with a steel grade of S275. The bolts were of M20 grade with 22 mm diameter holes incorporated in the column flange and endplate to suit the M20 bolts. The base plate in use was of the size of 500 500 18 with p y = 265 N/mm 2. Figure 3.2 shows the arrangement for specimen FEP1P1-2 flush endplate connection.

38 Figure 3.2 Arrangement for specimen FEP1P1-2

39 3.2.3 Test Procedure After the instrumentation system had been set up and the specimen had been securely located in the rig, the load was applied at a distance of 1.3 m from the face of the column using a hydraulic jack. The specimen was then loaded up to twothirds of the predicted final loading value. A 5kN increment was adopted so that a uniform data and gradual failure of the specimen can be monitored. After reaching the two-third value, the specimen was unloaded back and reinitialized. This procedure was taken to ensure the specimen is in the equilibrium state prior to the actual testing. After reinitializing the instrumentation system, the specimen was loaded back as described above, but the load applied was not restricted to the two-third value. Instead, the specimen was further loaded until a substantial deflection of the beam can be observed. For each loading, a set of reading was taken for deflections, rotations and applied load. The load application was continuously applied at this point by increment in the deflection of 2 mm instead of as before. This procedure was continued until the specimen had reached its failure condition. The failure conditions was considered to have reached when an abrupt or significantly large reduction in the applied load and when a large increase in the deflection of the beam.

40 3.3 Finite Element Model LUSAS finite element software was used to model and analyze the specimen. In this research, the specimen considered for modeling and analysis was focused on the specimen FEP1P1-2. The dimensions and parameters of the connection in modeling were made as exactly as possible to the specimen in the full scale experimental work. However, some assumptions were made in these modeling processes. They are: The model undergoes material nonlinearity only. Spring stiffness contact occurs between the interface of the endplate and the column flange. Beam and endplate were modeled as one unit by assuming that the welds of the beam and the endplate were rigid. 3.3.1 Model Components In this research, there are four components modeled namely the endplate, beam, column and bolts. A full model of the system is shown in Figure 3.3.

41 Figure 3.3 Full LUSAS finite element model of specimen FEP1P1-2 3.3.1.1 Endplate The dimensions of the endplate for FEP1P1-2 were 460 200 12 mm. The endplate was modeled by using volume geometry because the endplate is a significant and important component in the system. Furthermore, its deformation could be clearly viewed by using the volume geometry. Figure 3.4 shows the endplate model.

42 Figure 3.4 Endplate model 3.3.1.2 Beam For FEP1P1-2, the beam size used was TWP 400 170 49/12/6 with a length of 1.5 m. The depth and width of the beam section were 400 mm and 170 mm respectively, while the thickness of the flange and the thickness of the web were 12 mm and 6 mm respectively. The beam length was modeled with the length of 1300 mm instead of using the actual length of 1500 mm. This was because the point load was applied at the distance of 1300 mm from the column face in the experimental work. Therefore, the extra length of 200 mm will not affect the strength of the connection. The beam flanges were modeled with volume geometry while the beam web was modeled with

43 surface geometry to simplify the modeling process. Figure 3.5 shows the model of the beam component. Figure 3.5 Beam model 3.3.1.3 Column The column size used for specimen FEP1P1-2 was 254 254 107 UC. The column was modeled with the full length of 3000 mm. As like the beam component, the column flange was modeled using volume geometry and the column web was modeled using surface geometry. Figure 3.6 shows the model of the column component.

44 Figure 3.6 Column model 3.3.1.4 Bolts and Nuts Six bolts of grade M20 were used in specimen FEP1P1-2. All bolt shanks, bolt heads and nuts were modeled using the volume geometry. Figure 3.7 shows the model of the bolt component.

45 Figure 3.7 Bolt model 3.3.2 Element Types Of the over 100 element types available in LUSAS element library, three are chosen to model the various components of the bolted flush endplate system. These elements are HX8M, QTS4 and JNT4 [4], [6], [7]. 3.3.2.1 HX8M (3D Continuum Element) HX8M elements are three dimensional, isoparametric solid hexahedral elements comprising of eight nodes with three degrees of freedom at each node [8]. These elements will be used to model the beam and column flanges, endplate and bolts [6], [7]. Figure 3.8 shows the HX8M element.

46 Figure 3.8 HX8M solid element [8] 3.3.2.2 QTS4 (Thick Shell Element) QTS4 elements are three dimensional, flat face quadrilateral elements with four nodes and five degrees of freedom for each node [8]. These elements will be used to model the beam and column webs [6], [7]. Figure 3.9 shows the QTS4 element.

47 Figure 3.9 QTS4 thick shell element [8] 3.3.2.3 JNT4 (Joint Element) JNT4 elements are three dimensional joint elements which connects two nodes by three springs in the local x-, y- and z-directions. These elements have a total of four number of nodes where the third and fourth nodes are used to define the local x-axis and the local xy-plane. The active first and second nodes have three degrees of freedom [8]. These elements will be used to model the interface between the endplate and column flange [4], [6], [7]. Figure 3.10 shows the JNT4 element.

48 Figure 3.10 JNT4 3D joint element [8] 3.3.3 Nonlinear Material Properties Material nonlinearity occurs when the stress-strain relationship ceases to be linear and the steel yields and become plastic. The values of these properties for each of the component in the model are obtained from the standard tensile tests carried out during the full scale experimental work (see Appendix A). Other material properties unspecified in the tensile tests are obtained from other sources [4], [6]. Other material properties are given below [6]: Mass density of steel = 7.85 10-5 N/mm 3 Initial yield stress of bolts = 600 N/mm 2

49 For the bolts, the data for the hardening gradient are given as follows [4]: Hardening gradient, slope 1 = 20000 Plastic strain 1 = 100 For contact line between endplate and column flange, the following data were used [1], [4], [6], : Elastic spring stiffness, k c = 10 9 N/mm 3.3.4 Boundary Conditions All nodes at the bottom of the column were fully restrained against displacement and rotation in the x, y and z directions while all nodes at the top of the column were free to move in the y direction. This is in accordance to the experimental work to which this research refers to [3]. Figure 3.11 shows the boundary conditions of the model.

50 Figure 3.11 Boundary conditions 3.3.5 Loading An initial point load of 5 kn was applied at the distance of 1300 mm from the column face. The load was then increased incrementally by LUSAS with the load factor to achieve the required range of the connection moment.

CHAPTER 4 RESULTS AND DISCUSSION 4.1 Introduction In this section, the moment-rotation (M-Ф) curve is plotted using the analytical results obtained from finite element analysis. From this curve, the moment resistance M R was obtained and then compared with the existing experimental results. The comparison of mode of failure between experimental work and the finite element model was also done. 4.2 Experimental Results Experimental results of moment-rotation (M-Ф) curve for specimen FEP1P1-2 is shown in Figure 4.1. The experimental value of moment resistance, M R was 142 knm. The mode of failure of the connection was observed as the translation of the tip of the endplate away from the face of the column. Further loading of the

52 Figure 4.1 Experimental moment-rotation curve for specimen FEP1P1-2

53 specimen resulted in more deformation of the tip of the endplate. Figure 4.2 shows the mode of failure for specimen FEP1P1-2. Figure 4.2 Mode of failure for specimen FEP1P1-2 [3] 4.3 Finite Element Analysis Results In this section, the moment-rotation (M-Ф) curve for the model is obtained from the analytical results of the finite element analysis of the model. The moment resistance M R of the bolted flush endplate connection is later obtained from the moment-rotation curve. Also, the mode of failure of the model is also obtained from the deformed mesh of the model in the post-processing phase.

54 4.3.1 Moment-Rotation (M-Ф) Curve LUSAS software is unable to directly produce the moment-rotation curve. This software can only provide raw data of displacements for the nodes with the corresponding load increments. Therefore, calculations of moment and rotation of the connection are needed to be done. 4.3.1.1 Moment, M The values of moment can be obtained by multiplying the applied loading at the end of the beam with the moment arm (see Figure 4.3). Figure 4.3 Applied load P and the moment arm [6]

55 Example of calculation: Moment, M = P 1.3 m = 5 kn 1.3 m = 6.5 knm 4.3.1.2 Rotation, Ф In the experimental work, the rotation of the connection due to applied load is measured using two inclinometers. Figure 4.4 shows the locations where the values of rotation were determined. Point A is located at a distance of 100 mm from the face of the column while Point B is located at the point of intersection between the centroidal line of the beam and the centroidal line of the column. Figure 4.4 Location of inclinometers for specimen FEP1P1-2 [6]

56 From the displacement results of the finite element analysis, the rotation values of the connection are calculated using the Pythagoras Theorem where the degree of rotation is approximately obtained using a triangular shape as seen in Figure 4.5. Figure 4.5 Calculation of rotation shown below. An example of the calculation to get the rotation at the first load increment is Point A: Displacement of X, dx A = 0.0005 mm Displacement of Y, dy A = -0.0430 mm Point B: Displacement of X, dx B = -0.0001 mm Displacement of Y, dy B = 0.0007 mm Total displacement in X direction = dx B dx A + 100 + 133.35 = -0.0001 0.0005 + 100 + 133.35 = 233.3506 mm Total displacement in Y direction = dy B dy A = 0.0007 (-0.0430) = 0.0437 mm Rotation, Ф = tan -1 (Total displacement in Y direction / Total displacement in X direction)

57 = 0.0001876 rad = 0.1876 mrad The analytical moment and rotation results for specimen FEP1P1-2 calculated from the displacement results of finite element modeling are shown in Table 4.1. The moment-rotation (M-Ф) curve for the specimen is shown in Figure 4.6.

58 Table 4.1 Calculation of the moments and corresponding rotations at each load increment for specimen FEP1P1-2 Displacement of Column Displacement of Beam Total Displacement Increment # Load Factor Load Moment dx dy dx dy DX DY Rotation (N) (knm) (mm) (mm) (mm) (mm) (mm) (mm) (mrad) 0 0 0 0.00 0.0000 0.0000 0.0000 0.0000 0.0000 0.0000 0.0000 1 1 5000 6.50-0.0001 0.0007 0.0005-0.0430 233.3506 0.0438 0.1876 2 2 10000 13.00-0.0002 0.0015 0.0010-0.0861 233.3512 0.0876 0.3752 3 3 15000 19.50-0.0002 0.0022 0.0015-0.1291 233.3517 0.1313 0.5628 4 4 20000 26.00-0.0003 0.0030 0.0020-0.1721 233.3523 0.1751 0.7505 5 5 25000 32.50-0.0004 0.0037 0.0025-0.2152 233.3529 0.2189 0.9381 6 6 30000 39.00-0.0005 0.0045 0.0030-0.2582 233.3535 0.2627 1.1257 7 7 35000 45.50-0.0006 0.0052 0.0035-0.3012 233.3541 0.3065 1.3133 8 8 40000 52.00-0.0007 0.0060 0.0040-0.3443 233.3547 0.3502 1.5009 9 9 45000 58.50-0.0007 0.0067 0.0045-0.3873 233.3552 0.3940 1.6885 10 10 50000 65.00-0.0008 0.0075 0.0050-0.4303 233.3558 0.4378 1.8761 11 11 55000 71.50-0.0009 0.0082 0.0055-0.4736 233.3564 0.4818 2.0648 12 12 60000 78.00-0.0009 0.0090 0.0057-0.5194 233.3566 0.5284 2.2644 13 13 65000 84.50-0.0008 0.0098 0.0057-0.5676 233.3565 0.5774 2.4743 14 14 70000 91.00-0.0008 0.0106 0.0056-0.6162 233.3564 0.6268 2.6861 15 15 75000 97.50-0.0006 0.0114 0.0053-0.6664 233.3560 0.6779 2.9049 16 16 80000 104.00-0.0005 0.0123 0.0042-0.7188 233.3547 0.7310 3.1326 17 17 85000 110.50-0.0002 0.0131 0.0020-0.7755 233.3521 0.7886 3.3796 18 18 90000 117.00 0.0002 0.0139 0.0000-0.8335 233.3497 0.8475 3.6317 19 19 95000 123.50 0.0006 0.0148-0.0026-0.8934 233.3468 0.9081 3.8917 20 20 100000 130.00 0.0011 0.0156-0.0060-0.9578 233.3430 0.9734 4.1715

59 Table 4.1 Calculation of the moments and corresponding rotations at each load increment for specimen FEP1P1-2 (continued) 21 21 105000 136.50 0.0015 0.0165-0.0107-1.0263 233.3378 1.0427 4.4688 22 22 110000 143.00 0.0021 0.0174-0.0167-1.1001 233.3312 1.1174 4.7890 23 23 115000 149.50 0.0026 0.0183-0.0225-1.1815 233.3249 1.1998 5.1422 24 24 120000 156.00 0.0032 0.0192-0.0279-1.2708 233.3188 1.2899 5.5285 25 25 125000 162.50 0.0039 0.0201-0.0355-1.3663 233.3106 1.3864 5.9422 26 26 130000 169.00 0.0046 0.0210-0.0452-1.4684 233.3002 1.4894 6.3838 27 27 135000 175.50 0.0053 0.0219-0.0570-1.5847 233.2878 1.6066 6.8865 28 28 140000 182.00 0.0059 0.0228-0.0632-1.7178 233.2809 1.7406 7.4614 29 25.2 126000 163.80 0.0061 0.0207-0.0646-1.5956 233.2793 1.6164 6.9288 30 26.2 131000 170.30 0.0061 0.0215-0.0641-1.6387 233.2799 1.6601 7.1164 31 27.2 136000 176.80 0.0060 0.0222-0.0636-1.6817 233.2804 1.7039 7.3041 32 28.1 140500 182.65 0.0059 0.0229-0.0633-1.7262 233.2808 1.7491 7.4976 33 26.6 133000 172.90 0.0061 0.0218-0.0640-1.6653 233.2799 1.6871 7.2321 34 27.6 138000 179.40 0.0060 0.0226-0.0635-1.7083 233.2805 1.7309 7.4197 35 28.3 141500 183.95 0.0061 0.0231-0.0634-1.7566 233.2805 1.7797 7.6289 36 28.7 143500 186.55 0.0065 0.0235-0.0634-1.8313 233.2801 1.8548 7.9509 37 29.3 146500 190.45 0.0068 0.0241-0.0637-1.9439 233.2796 1.9680 8.4361 38 30 150000 195.00 0.0069 0.0247-0.0654-2.1138 233.2777 2.1385 9.1669 39 30.9 154500 200.85 0.0064 0.0253-0.0677-2.3636 233.2760 2.3889 10.2404 40 31.9 159500 207.35 0.0057 0.0257-0.0673-2.6535 233.2771 2.6792 11.4846 41 32.8 164000 213.20 0.0045 0.0259-0.0617-2.9794 233.2838 3.0053 12.8817 42 33.8 169000 219.70 0.0026 0.0261-0.0449-3.3624 233.3024 3.3885 14.5229 43 34.7 173500 225.55 0.0003 0.0263-0.0115-3.8287 233.3382 3.8549 16.5193

60 Table 4.1 Calculation of the moments and corresponding rotations at each load increment for specimen FEP1P1-2 (continued) 44 35.6 178000 231.40-0.0022 0.0257 0.0452-4.3971 233.3975 4.4228 18.9475 45 36.6 183000 237.90-0.0060 0.0235 0.1151-5.0725 233.4711 5.0960 21.8236 46 37.5 187500 243.75-0.0114 0.0200 0.1935-5.8098 233.5549 5.8298 24.9558 47 38.5 192500 250.25-0.0210 0.0164 0.2772-6.6116 233.6482 6.6280 28.3597 48 39.4 197000 256.10-0.0234 0.0074 0.3711-7.4617 233.7445 7.4691 31.9431 49 40.4 202000 262.60-0.0341-0.0009 0.4763-8.4321 233.8604 8.4312 36.0365 50 40.8 204000 265.20-0.0397-0.0043 0.5565-9.0787 233.9462 9.0744 38.7689 51 40.8 204000 265.20-0.0404-0.0045 0.5677-9.1728 233.9581 9.1683 39.1678 52 40.8 204000 265.20-0.0406-0.0046 0.5709-9.2001 233.9615 9.1955 39.2833

61 Figure 4.6 Moment-rotation curve for specimen FEP1P1-2 (model)

62 4.3.2 Mode of Failure From the deformed mesh of the model in the post processing phase, it can be seen that the mode of failure of the connection is the deformation of the tip of the endplate away from the face of the column. Figure 4.7 shows the mode of failure for the connection. Figure 4.7 Mode of failure of the connection

63 4.4 Result Comparisons In this section, the analytical moment-rotation (M-Ф) results from the finite element analysis are compared with moment-rotation (M-Ф) results from the experimental work. Result comparisons are important in order to validate the accuracy of the finite element analysis of the connection. The comparisons are made in terms of the shape of the moment-rotation (M-Ф) curve, the moment resistance (M R ) and also in terms of the mode of failure. 4.4.1 Comparison of Moment-Rotation (M-Ф) Curve Figure 4.8 shows the moment-rotation curve for specimen FEP1P1-2 produced in the experimental work and also the moment-rotation curve of the same specimen produced in the finite element analysis of the model. By observing the two curves, it can be seen that they show similar trend. For the finite element analysis of the model, the moment-rotation relationship behaves linearly first followed by nonlinearly, as with the experimental results. The curves show two phases where they behave linearly at the beginning followed by a second phase of much reduced stiffness due to inelastic deformation of the connection. The initial slope of the experimental curve is less stiffer compared to that of the finite element curve. This is probably because the experimental model is more flexible during testing compared to the model used in the analysis.

64 Figure 4.8 model Moment-rotation relationship for the experimental and finite element 4.4.2 Comparison of Moment Resistance, M R The values of the moment resistance M R for both the experimental and finite element analysis were determined by estimating when a knee method formed in the moment-rotation curve. The comparison of the moment resistance values for specimen FEP1P1-2 is shown in Table 4.2. The experimental value of the moment resistance was 142 knm, whereas the moment resistance obtained from finite element analysis is taken to be 182 knm. This comparison gives a percentage of difference of 28.17%. The large difference percentage can be attributed to various assumptions made in the model, as well as flaws in the actual specimen and imperfections in the test setup.

65 Table 4.2 Comparison of moment resistance for specimen FEP1P1-2 between experimental and analytical results Specimen Moment Resistance (knm) Experimental Analytical Difference Percentage FEP1P1-2 182 142 28.17% 4.4.3 Comparison of Mode of Failure From the comparison of mode of failure between experimental and finite element analysis as shown in Figure 4.9, it can be seen that the connection have a similar mode of failure, where the tip of the endplate deformed away from the face of the column.

66 Figure 4.9 Comparison of mode of failure for specimen FEP1P1-2 4.5 Moment-Rotation Curves At Different Points Along the Beam In the laboratory test, the inclinometer is placed at a position of 100 mm from the face of the column flange. In this study, moment-rotation curves for different points along the beam is obtained to see the effects of various inclinometer placement on the moment resistance obtained. The points considered starts from the interface of the column flange and the endplate, taken as x = 0 mm, until x = 160 mm taken at 20 mm intervals.