87 CHAPTER 7 ANALYTICAL PROGRAMME USING ABAQUS 7.1 GENERAL With the advances in modern computing techniques, finite element analysis has become a practical and powerful tool for engineering analysis and design. In Structural Engineering, development of structural design code equations or redeveloping them is a continuous process and requires a wide range of experimental studies. Performing many number of experiments is costly, time consuming and hence uneconomical. On the other hand conducting experiments is a compulsion for the research to progress. The problem gets enormously simplified with the use of ABAQUS 6.9 (2009). ABAQUS is a highly sophisticated, general purpose finite element program, designed primarily to model the behaviour of solids and structures under externally applied loading. 7.2 FEATURES OF ABAQUS SOFTWARE ABAQUS includes the following features: Capabilities for analysing both static and dynamic problems The ability to model very large changes in shape of solids, in both two and three dimensions A very extensive element library, including a full set of continuum elements, beam elements, shell and plate elements.
88 A sophisticated capability to model contact between solids An advanced material library, including the usual elastic and elastic plastic solids; models for foams, concrete, soils, piezoelectric materials and many others Capabilities to model a number of phenomena of interest, including vibrations, coupled fluid/structure interactions, acoustics, buckling problems and so on. 7.3 ABAQUS MODELLING Figures 7.1 and 7.2 show the modelling of ordinary and seismic joint and fibre reinforced joint. By using partition command the ordinary model is separated in the joint region. Figure 7.1 Modelling of Concrete in Ordinary Joint Figure 7.2 Modelling of Concrete in Fibrous Joint
89 Figures 7.3 and 7.4 show the modelling of longitudinal and lateral reinforcement in ordinary and fibre reinforced joint and seismic joint. In ordinary joint the spacing of shear reinforcement is 40 mm. In the seismic joint the spacing of shear reinforcement is 20 mm up to a distance of 180 mm (2d b ) in the beam from the face of the column and 90 mm (d b ) from the top and bottom face of the beam in column and for the remaining the spacing was 40 mm, where d b is the effective depth of beam. Figure 7.3 Modelling of Reinforcement in Ordinary and Fibrous Joint Figure 7.4 Modelling of Reinforcement in Seismic Joint 7.4 ELEMENTS USED Solid 3D elements 8-node brick (C3D8) were used to model ordinary concrete and 4-node linear tetrahedron (C3D4) were used to model fibre reinforced concrete in the joint. Two node linear 3D truss element (T3D2) were used to model the reinforcement steel.
90 7.4.1 Solid Element C3D8 and C3D4) The Figure 7.5 shows C3D8 element which is an 8-noded brick element having eight nodes at their corners. These elements use linear interpolation in each direction and are often called linear elements or firstorder elements. These elements have only three displacement degrees of freedom and are Stress/displacement elements. C3D4 is a 4-node linear tetrahedron element and three degrees of freedom at each node. Figure 7.5 Linear Element Figure 7.6 Truss Element (8- Node Brick Element) (T3D2) 7.4.1.1. Reason for Choosing the Element These are the standard volume elements of ABAQUS. These elements can be composed of a single homogeneous material or can include several layers of different materials for the analysis of laminated composite solids. These are Stress/displacement elements and used in the modelling of linear or complex nonlinear mechanical analyses. Stress/displacement elements can be used for static and quasi-static analysis. However, good meshes of hexahedral elements usually provide a solution of equivalent accuracy at less cost. Quadrilaterals and hexahedra (C3D8) have a better convergence rate than triangles and tetrahedra, and sensitivity to mesh orientation in regular meshes. However, triangles and tetrahedra are less
91 sensitive to initial element shape, whereas first-order quadrilaterals and hexahedra perform better if their shape is approximately rectangular. For stress/displacement analyses the first-order tetrahedral element C3D4 is a constant stress tetrahedron, which should be avoided as much as possible; the element exhibits slow convergence with mesh refinement. This element provides accurate results only in general cases with very fine meshing. Therefore, C3D4 is recommended only for filling in regions of low stress gradient in meshes of C3D8. 7.4.2 3-D Truss Element (T3D2) Figure 7.6 shows the 3-D truss element (T3D2). These are three dimensional truss element having two degrees of freedom. Truss elements are used in two and three dimensions to model slender, line-like structures that support loading only along the axis or the centerline of the element. No moments or forces perpendicular to the centerline are supported. A 2-node straight truss element, which uses linear interpolation for position and displacement, has a constant stress. It is defined that the cross-sectional area associated with the truss element as part of the section definition. When truss elements are used in large-displacement analysis, the updated cross-sectional area is calculated by assuming that the truss is made of an incompressible material, regardless of the actual material definition. Truss elements have no initial stiffness to resist loading perpendicular to their axis. 7.4.2.1 Assigning a Material Definition to a Set of Truss Elements A set is a named region or collection of entities on which we can perform various operations such as assign section properties in the Property module, create contact pairs with contact node sets and surfaces in the
92 Interaction module, define loads and boundary conditions in the Load module and request output from specific regions of the model in the Step module. A geometry set contains geometric objects (cells, faces, edges and vertices) that are selected from one of the following types of parts or from instances of these parts. Geometry set is created for a set of reinforcement bars in each part. A material definition is associated with each solid section definition for each set. No material orientation is permitted with truss elements. 7.4.2.2 Embedded Element The embedded element technique is used to specify that an element or groups of elements are embedded in host elements. The embedded element technique can be used to model rebar reinforcement. ABAQUS searches for the geometric relationships between nodes of the embedded elements and the host elements. If a node of an embedded element lies within a host element, the translational degrees of freedom at the node are eliminated and the node becomes an embedded node. The translational degrees of freedom of the embedded node are constrained to the interpolated values of the corresponding degrees of freedom of the host element. Embedded elements are allowed to have rotational degrees of freedom, but these rotations are not constrained by the embedding. 7.5 MATERIAL PROPERTY Property module is used to perform the following tasks: Define materials Define beam section profiles Define sections Assign sections, orientations, normals, and tangents to parts
93 A material definition specifies all the property data relevant to a material. A material definition is specified by including a set of material behaviours and the property data is supplied with each material behaviour. The material editor is used to specify all the information that defines each material. ABAQUS/CAE assigns the properties of a material to a region of a part when a section referring to that material is assigned to the region. 7.6 MATERIAL BEHAVIOUR 7.6.1 Concrete Concrete damaged plasticity model (CDP) was used for defining concrete in plastic range. The concrete damaged plasticity model provides a general capability for modelling concrete and other quasi-brittle materials in all types of structures. This model uses concepts of isotropic damaged elasticity in combination with isotropic tensile and compressive plasticity to represent the inelastic behaviour of concrete. The concrete damaged plasticity model is based on the assumption of scalar (isotropic) damage and is designed for applications in which the concrete is subjected to arbitrary loading conditions, including cyclic loading. The model takes into consideration the degradation of the elastic stiffness induced by plastic straining both in tension and compression. It also accounts for stiffness recovery effects under cyclic loading. Concrete stress- strain behaviour under uniaxial compression after elastic range (0.7f c ) should be defined in terms of stress versus inelastic strain (crushing strain) (Danesh et al. 2008). 7.6.2 Reinforcement Longitudinal and transverse steel reinforcement behaviour was defined as an elastic-plastic material using a bilinear curve. Slope of the plastic range (Danesh et al. 2008) was assumed to be about one percent of steel modulus of elasticity. To introduce plasticity, kinematic hardening option was used.
94 7.7 MESHING ABAQUS/CAE provides with a variety of tools for controlling mesh characteristics. The density of a mesh is specified by creating seeds along the edges of the model to indicate where the corner nodes of the elements should be located and the shape of the mesh elements are also selected. Figure 7.7 Meshing Model of Ordinary Figure 7.8 Meshing Model and Seismic Joint of Fibrous Joint The meshing technique is chosen-free, structured or swept where applicable. The element type is selected and assigned to the mesh by choosing the element family, geometric order and shape along with specific element controls. In the present study the fibre portion in the joint is meshed using free meshing and remaining concrete portion is meshed with structured meshing. Figures 7.7 and 7.8 show the meshing model of ordinary and seismic joint and fibre reinforced joint. Tie constraint is used to tie the interface between
95 ordinary concrete and fibre concrete. A tie constraint ties two separate surfaces together so that there is no relative motion between them. This type of constraint allows us to fuse together two regions even though the meshes created on the surfaces of the regions may be dissimilar. 7.8 LOADING AND BOUNDARY CONDITIONS The numerical model is used to simulate the same conditions of the test specimens. The cyclic load is applied on a node which is at a distance of 50 mm from the free end of the top and bottom of the beam in eight to ten steps. Displacement at the point of load is obtained after the Finite Element Analysis. Displacement/rotation boundary condition is used to constrain the movement of the selected degrees of freedom to zero or to prescribe the displacement or rotation for each selected degree of freedom. In the present study on the both the ends of the column the displacement in the two directions were set to zero (both ends of the columns were hinged). 7.9 FINITE ELEMENT ANALYSIS RESULTS 7.9.1 General A numerical simulation makes sense only if it corresponds to the real model. Therefore, a numerical model specimen with the same properties of the experimental specimen was analyzed to verify its accuracy. 7.9.2 Number of Nodes and Elements used in the Analysis In the above analysis we have modelled three beam column joints. In the model the joint was modelled for ordinary concrete. The concrete was modelled in a single part as a solid element. The reinforcements were modelled by using 3D wires (T3D2). The reinforcements were modelled as three sets such as beam main reinforcement, column main reinforcement and
96 beam and column transverse reinforcement. For each set, different material properties have been assigned. The second model was used to model seismic joint. The concrete was modelled as like the first model. The steel reinforcements were modelled in four sets such as such as beam main reinforcement, column main reinforcement, beam and column transverse reinforcement in the joint region and other regions. The third model was used to model fibre joint. In this model five joints were modelled by changing various material properties of fibre concrete in the joint region. The concrete was modelled in three parts as shown in Figure 7.2. Table 7.1 Number of Nodes and Elements used in the Finite Element Model Sl.No Name Model 1 (Ordinary Model 2 (Seismic Model 3 (Fibre Joint) Joint) Joint) 1 No of Nodes 2399 2564 2721 2 No of Elements a) C3D8 b) C3D4 1092-1092 - 897 Element No 898 to 4103 (3205) c) T3D2 Element No 1093 to 1813(720) Element No 1093 to 1978 (885) Element No 4104 to 4849 (745)
97 Different material properties were assigned for fibre concrete in the joint regions and ordinary concrete in the other regions. The reinforcements were modelled as like the first model. The fibre concrete was meshed by using tetrahedron element. So the number of nodes and elements were different for each model. The Table 7.1 shows the actual number of nodes and elements used in the above three models. 7.9.3 Finite Element Analysis Results Figures 7.9 to 7.15 show the deformed configuration of all the specimens modelled using M25 concrete. Figure 7.16 shows the overall load deflection curves obtained from the ABAQUS analysis. The deflection is obtained by applying load at a distance of 50 mm from the beam tip at each cycle up to failure. A good correlation was observed with the experimental values in Figure 8.35. In the experimental specimen, when the loading reaches the maximum value, a rearrangement in the load resisting mechanisms occurs. When one of the load resisting mechanism reaches its capacity, the rearrangement occurs again and the load decreases. The numerical model cannot represent this phenomenon, thus near to this maximum level of loading, numerical instabilities appear in some areas of the mesh and the model cannot continue converging. 7.9.4 Global Structural Failure Global structural failure is defined as a large discontinuity in the composite structure s overall vertical load-displacement curve. (http://www.firehole.com/documents/ HeliusMCT-Example-Problem- Abaqus.pdf). The overall vertical deformation of the composite structure is quantified by using the vertical displacement at the load application point as shown in Figure 7.9. A large discontinuity in the load-displacement curve is indicative of very rapid growth (spreading) of localized material failures that
98 occur during a particular load increment, resulting in a large degradation of the overall stiffness of the composite structure. This definition of global structural failure is chosen in this analysis since most experimental tests are stopped at this point to prevent damage to expensive test equipment. Global structural Failure Figure 7.9 Vertical Load-Displacement Curve for the Prediction of Failure Figure 7.10 Displacement Pattern and Values of the Specimen II O2
99 Figure 7.11 Displacement Pattern and Values of the Specimen II S2 Figure 7.12 Displacement Pattern and Values of the Specimen II F12
100 Figure 7.13 Displacement Pattern and Values of the Specimen II F22 Figure 7.14 Displacement Pattern and Values of the Specimen II F32
101 Figure 7.15 Displacement Pattern and Values of the Specimen II F42 Figure 7.16 Displacement Pattern and Values of the Specimen II F52
102 Figure 7.17 Overall Load-Displacement Curves for M25 Obtained from ABAQUS Concrete Table 7.2 Finite Element Analysis Result for Specimens Cast in M25 Concrete Sl. No Specimen Id Ultimate load (P u ) kn Ultimate Deflection u (mm) Upward Downward Upward Downward 1 II O2 12 12 26.57 29.48 2 II S2 16 16 29.73 32.24 3 II F12 20 20 36.25 40.08 4 II F 22 20 20 46.53 48.97 5 II F32 16 16 42.87 44.72 6 II F 42 16 16 35.65 38 7 II F 52 12 12 31.68 32.24 7.10 SUMMARY The nonlinear finite element model was developed to simulate the same conditions of the test specimen, using ABAQUS to compare the experimental results. Elements used to model the steel and concrete, their properties and behaviour, number of nodes and elements used in the model were discussed. Reverse cyclic load was applied and its corresponding displacement was found. The displacement pattern for each specimen and overall load deflection curve for all the specimens were plotted.