Finite Element Simulation and Parametric Studies of Perfobond Rib Connector

Simulating the push-out test and conducting parametric study using finite element model are conducted using perfobond connectors. The finite element model was verified through comparing with push-out test results. The verified finite element model was then used to conduct parametric study aiming to investigate the effect of several parameters, such as height and thickness of connector, cross sectional area and yield strength of transverse reinforcement, concrete compressive strength and rib holes, on resistance capacity. The results of the parametric study are treated statistically to produce a mathematical model suggested to estimate the resistance capacity of the perfobond connector.


INTRODUCTION
Development of bridges includes developing materials, method of design and method of construction. The design of steel-concrete composite bridge includes the design of steel beam, concrete slab and connectors. Nowadays, several types of connectors are available such as stud, channel, spiral, tendon and perfobond connectors [1][2][3] .
Enhancing steel-concrete composite bridge can be conducted through improving connection between concrete slab and steel beam, which allows the composite action to be more effective [4] . The perfobond connector is one of the newly development connectors which give a good connection behavior comparative with the stud connector [5] . Since, design equations available to calculate resistance of perfobond connectors are mainly based on experimental investigation through performing push-out tests [6] . Connection between the two parts of bridges is investigated through push out test using perfobond connector [5] .
Comparing the results of push out test with the available equations shows large difference in estimating ultimate resistance of perfobond connector. Moreover, performing push out test each time is required to estimate the ultimate resistance for each proposed project. Thus, it is proposed to model the push out test using finite element method and establish a parametric study to investigate the behavior of the perfobond connector and connector's ultimate resistance. The study attempts to consider the height and thickness of connector, concrete compressive strength, steel yield strength and the area of concrete dowels. The objectives of the present work can be stated as: (1) Modeling push-out specimens using finite element analysis package ANSYS. (2) Verifying the model's accuracy in simulating push-out test comparing with experiments.
(3) Using the verified model to perform parametric study considering the effects of the above parameters on ultimate resistance capacity of perfobond connector.

Perfobond connectors' historical review:
The perfobond shear connector is a steel plate with holes positioned vertically and welded to steel beam flange, steel reinforcement bars are placed through rib holes then concrete placed around and through connectors, shown in Fig. 1. An investigation was carried out by Oguejiofor and Hosain [6] on modeling the push-out test using finite element predicting a numerical model for resisting capacity calculation of connector resistance [6] . The push test results were presented for connector resistance of concrete deck plates with precast concrete slab used as a shuttering [7] . Experimental tests were carried out with lightweight concrete describing connection behavior, measuring slip between steel profile and concrete slab, defining connection ductility and considering concrete strength, reinforcement disposition and rib existence [8] . Test program for composite bridge decks with perfobond rib shear connectors was presented for composite deck with profiled steel sheeting, perfobond ribs, concrete and steel reinforcements. Push-out, full-scale flexural and deck-to-girder connection tests were presented, shown that, perfobond ribs can effectively used for connecting steel-concrete composite bridge decks [9] .

Experimental and theoretical works
Push-out test: A push-out specimen consists of short steel beam section held in a vertical position by two identical reinforced concrete slabs attached to the beam flanges by shear connectors, Fig. 1. The overall system is subjected to vertical load, using hydraulic jack, producing shear load along the interface between concrete slab and beam flange on both sides. Top plate is used to ensure that the load applied uniformly. The push-out test was conducted using a total of 12 specimens. The 150×150×150mm concrete cubes were placed and cured at the same conditions, tested at 28days give an average value of concrete cube compressive strength f cu =54.60MPa. The beam and connector steel yielding stress used are Fy b =345MPa. The reinforcement steel yielding stress is Fy r =345MPa. Four dial gages are fixed at four points at the same level which used to measure the relative displacement between steel and concrete. The load was applied slowly in several steps to failure of each specimen, measuring the applied loads and the relative displacements at each load step, drawing the load-slip curves for each specimen. The results of the experiments are then compared with the available equations used to calculate the shear resistance of perfobond connector. Usually, a series of push-out specimens are tested to study the effect of a number of parameters on the performance of the connector [3,5] . Modeling the test using finite element model is used. After verifying the model, parametric study is conducted to investigate the above parameters effects on resistance capacity of shear connector. tension and crushing in compression in three orthogonal directions, as well as incorporating plastic and creep behavior, using an iterative solution for nonlinear analysis and the stiffness matrix is reformulated after each iteration. Each load step is judged as converged by satisfying three convergence criteria, these are the bilinear elements status, large deflection and plasticity criteria. The three-dimensional shell element, (Shell43), Fig. 2b, is defined by four nodal points with six translational degrees of freedom per node, four nodal thicknesses, material direction angle and orthotropic material properties, having in-plane and out-of-plane stiffness, which adopted to model the steel beam section and perfobond rib connector. The three dimensional spar element (Link8) is used to model the reinforcement, which is a uniaxial tension-compression element with three degrees of freedom at each node: translations in the nodal x,y and z directions. As a pinjointed structure, no bending of the element is considered. Plasticity, creep, swelling, stress stiffening and large deflection capabilities are included [10] . The adopted finite elements model discretization is shown in Fig. 3. The nonlinear elastic option (MELAS) is adopted to be used for concrete material, through entering uniaxial stress-strain curve for concrete. The typical stress-strain curve for concrete is linearly elastic up to 30% of the maximum compressive strength f c '. This was used to establish the first point of the stressstrain curve, where fc=fc'/3 and the corresponding strain is defined by ε=fc'/Ec, where Ec is the Young's modulus of elasticity for concrete. The other points in the stress-strain curve are established by using the numerical expressions given by Oguejiofor and Hosain [6] . The Bilinear Kinematics Hardening (BKIN) is adopted for steel beam, perfobond ribs and reinforcements. The material behavior is described by bilinear total stress-total strain curve starting at the origin and with positive stress and strain values. The initial slope of the curve is taken as the elastic modulus of the material. At the specified yield stress, the curve continues along the second slope defined by the tangent modulus [10] . In discretizing the specimen, nodes are numbered in natural and convenient manner. The nodes for slab portion are numbered from 1 to 3234; for reinforcement from 3235 to 3319; for steel section and perfobond rib connector were numbered from 3320 to 3657. A uniformly distributed load applied at top of beam flanges, all nodes at top steel section are constraints to have a uniform displacement in load direction, whereas, in the actual test the load was applied through thick steel plate. Similarly, all nodes at the bottom of concrete slabs are constrained. Coincident nodes at the junction of perfobond rib elements and steel flange and web elements and at connector and concrete slab are merged to simulate the rigid connection of these elements replacing all nodes lie at the same coordinate location with only one node and the lowest node number of all the nodes merged is retained. The coincident concrete and steel flange element nodes are coupled in both x and z directions. The numbering scheme adopted where then changed after merging nodes, changing the total nodes number to be 3507 nodes. Similar to actual test, loads are applied slowly in several sub-steps to failure, a constant step of 3kN is used, 140 iterations for each load step are allowed, full Newton-Raphson method is applied and the solution automatically proceeded to the next load step if convergence is achieved after only a few iterations. Each analysis is continued until the solution no longer converged, at which point the ultimate load is deemed to have been attained. Table 1 shows the ultimate capacity results of push-out specimens obtained experimentally for NP2 group and ANSYS models at ultimate stage as well as Table 2 shows the relative displacements of experiments and ANSYS models at ultimate stage for the same specimens. The experimentally obtained load-relative displacement curves results of group NP2, (etc. NP2-1, NP2-2 and NP2-3), with those obtained by finite element model are shown in Fig. 4 Numerical analysis and parametric study: Various analyses are conducted, classified as three main groups A, B and C using variables of compressive and tensile strengths of concrete; the amount and yield strength of Experiment Experiment

Finite element model's verification:
Av  concrete slab and initiated by longitudinal splitting of slab [5] . Cracks are normally induced in concrete members by tensile stresses that develop due to applied loads or as a result of restraint to volumetric change. Load-deformation behavior of concrete under compressive and tensile loads is closely linked to formation and propagation of these cracks. The numerically generated results were fitted to regression model accounts for the contribution of bearing, concrete dowels and splitting resistance and transverse reinforcement.
The regression mode1 was of the form:  The term (htf c' ) accounts for contribution of concrete bearing, while the term (A r f y ) accounts for transverse reinforcement contribution as well as term ' c sc f A accounts the contributions of concrete dowels formed through holes of perfobond rib connector, which fail in double shear, hence the total shear area of dowels, A sc , is =2n(πD 2 /4), where n is number of rib holes, D diameter of rib holes. Using multiple linear regressions with least squares procedure the β 0 , β 1 , β 2 and β 3 are determined and given as [11] : Equation (2) is suggested to estimate shear resistance of perfobond connector within the limits of the parameters investigated.

CONCLUSION AND RECOMMENDATIONS
From the previous works, it can be concluded that: 1. Using finite element method to simulate push-out test is acceptable. 2. The sensitivity of the perfobond connector to the variation of the area of transverse reinforcement is too small. 3. The numerical model used to estimate the shear resistance of the perfobond connector is suggested to be used within the limit of the investigated parameters. It is also recommended that, perfobond resistance capacity need to be investigated by more detailed study by experiments and computer simulations.