Effect of High Temperature on the Strain Behavior in Post-Tensioning Concrete Beams by Using Finite Element Method (ANSYS Program)

Transcription

1 Journal of Civil Engineering Research 2016, 6(2): DOI: /j.jce Effect of High Temperature on the Strain Behavior in Post-Tensioning Concrete Beams by Using Finite Element Method (ANSYS Program) Amer Farouk Izzet, Zahra'a Hussein Dakel * B.Sc. in Civil Engineering, University of Baghdad College of Engineering Civil Engineering Department, Baghdad, Iraq Abstract This research is conducted to study the of effect of high temperature on the strain Behavior in post-tensioning concrete beams exposed to fire flame. The exposure of these beams to fire causes changes in their structural behavior. Finite element method was used to idealize the effect of burning by fire flame exposed to post-tensioning concrete beams. The beams that were subjected to fire flame at temperature levels of (300, 500 and 700 C ) for 1 hour period of exposure. A three-dimensional nonlinear finite element model was adopted to investigate the structural behavior of post-tensioning concrete beams specimens with and without exposure to burning. Good agreement was observed between the adopted finite element model results and experimental results of [11]. It is found that the theoretical values of beam strain exceeds values by a margin the experimental [11] ranging between (1-23%) after burning for the analyzed beams specimens. The adopted finite element analysis showed, also, good agreement with experimental results of [11] throughout the load-deflection behavior before and after burning. Keywords Post-Tension, Finite element, Burning 1. Introduction Pre-stressed concrete is widely used in the construction industry of buildings, bridges, towers, pressure vessels and offshore structures. For architecture requirements many buildings need long span with small depth, in this case the pre-stressed elements are the economic solution. Traditionally, laboratory testing was used to investigate the structural behavior of post-tensioned reinforced concrete beams under static loads. However, such reliance on time consuming and expensive laboratory testing has hindered progress in this area. The advances in the fields of computer aided engineering and finite element method during the last two decades have changed this situation significantly in many engineering fields. In the present study, three dimensional numerical analysis were used to analyses the tested seven pre-stressed post-tensioned concrete beams after exposing six of them to the effect of fire and static loads using finite element analysis (FEA) approach by using ANSYS 2011 software. The methodology and modeling techniques for the numerical analysis are presented in this paper. [10] Proposed relationships for normal concrete to * Corresponding author: engzahra67@yahoo.com (Zahra'a Hussein Dakel) Published online at Copyright 2016 Scientific & Academic Publishing. All Rights Reserved provide efficient modeling and to meet fire performance criteria of the behavior of concrete exposed to fire.the proposed relationships are for both the peak strain of concrete at elevated temperatures. max ^( 6)T (1) Applying equation (1) gives the following peak strain as shown in Table (1): Table (1). Peak strain for concrete Temperature 1.1. Numerical Methods Peak strain value 300 C C C There are many practical engineering problems for which the exact solution cannot be obtained. This may be attributed to either the complex nature of governing differential equations or the difficulties that arise from the boundary and initial conditions. To achieve the solution for this problem numerical approximation was adopted. There are two common numerical methods; these are: Finite difference method. Finite element method. Finite element method is a numerical procedure that can be applied to obtain solution to a variety of problems in

2 Journal of Civil Engineering Research 2016, 6(2): engineering steady, transient, linear, or nonlinear problems in stress analysis, heat transfer, fluid flow, and electromagnetism problems may be analyzed with finite element methods. 2. The Modeling 2.1. Material Properties The required parameters to identify the material models are listed in Table (2). Seven concrete beam models were presented regarding Solid65 element, the control beam has ƒ'c=40 MPa and the other models subjected to high temperature each has different concrete strength identical to the experimental value. Every model includes density, linear isotropic and multi-linear isotropic properties to properly model concrete material. For concrete, ANSYS computer program requires input data for material properties, as follows [9]. Elastic modulus (Ex=Ec). Ultimate uniaxial compressive strength (UnCompSt =ƒc'). Ultimate uniaxial tensile strength (modulus of rupture, UnTensSt = f r ). Poisson's ratio (PRXY=υ). Shear transfer coefficient for opened and closed cracks (ShrCf-Op=β o and ShrCf-Cl = β c respectively). Compressive uniaxial stress-strain relationship for concrete. [11] An experimental effort was made to estimate the ultimate uniaxial compressive and tensile strength ( and f r ) of test three of concrete cubes and three prisms specimens. From the ultimate uniaxial compressive strength ( f f c ), obtained from appropriate tests, the elastic modulus of concrete (Ec) for each beam was calculated according to (ACI ) by using equation (2). Poisson s ratio for concrete was assumed to be 0.2, [2] for all reinforced concrete beams. Ec 4700 fc' MPa (2) The shear transfer coefficient, β, represents conditions of the crack face. The value of β ranges from 0.0 to 1.0, with 0.0 representing a smooth crack (complete loss of shear transfer) and 1.0 representing a rough crack (no loss of shear transfer) [1]. The value of β o is used in many studies of reinforced concrete and composite steel-concrete structures, however, varied between 0.05 and 0.25, [2], [8] and [7]. A number of preliminary analyses were attempted in this study with various values for the shear transfer coefficient within this range, but convergence problems were encountered at low loads with β o less than 0.2. Therefore, the shear transfer coefficients for closed and opened cracks, used in this study, were taken equal from 0.5 to 0.85 for all beam specimens. c Table (2). Material models properties for beams that used in research Material model number 1 2,3 Element type 1 Link8 4 Link8 5 Solid 45 Point Material properties Linear Isotropic (MPa) PRXY 0.2 Multi-linear isotropic Strain Stress (MPa) Concrete ShrCf-Op 0.2 ShrCf-Cl 0.8 UnTensSt UnCompSt 3.5 (MPa) 40 (MPa) HydroPts 0 BiCompSt 0 UnTensSt 0 TenCrFac 0 Linear isotropic ( MPa) PRXY 0.3 Yield stress Tangent modulus Bilinear Isotropic Linear Isotropic 450 (MPa) (MPa) PRXY 0.3 Yield stress Bilinear Isotropic 1720 (MPa) Tangent modulus 0 Initial strain Linear Isotropic 5.9x10^ (MPa) PRXY 0.3 Where: Shear transfer coefficients for an open crack (ShrCf-Op). Shear transfer coefficients for a closed crack (ShrCf-Cl). Uniaxial tensile cracking stress (UnTensSt). Uniaxial crushing stress (UnCompSt). Biaxial crushing stress (BiCompSt).

3 42 Amer Farouk Izzet et al.: Effect of High Temperature on the Strain Behavior in Post-Tensioning Concrete Beams by Using Finite Element Method (ANSYS Program) 2.2. Compressive Uniaxial Stress-Strain Relationship for Concrete The ANSYS computer program requires the uniaxial stress-strain relationship for concrete in compression. For numerical expressions [4], the following equations (3) and (4), were used along with equation (5) Gere and Timoshenko, [6] and equation (3) (ACI ) to construct the uniaxial compressive stress-strain curve for concrete in this study. f = E cε 1+ ε εo ε o = 2f c 2 (3) E c (4) E c = σ (5) ε Where: =stress at any strain, MPa ε =strain at stress f. ε o =strain at the ultimate compressive strength. Figure (1) shows the simplified compressive uniaxial stress-strain relationship that was used in this study. The simplified stress-strain curve for concrete model is constructed from six points connected by straight lines. The curve starts at zero stress and strain. Point 1, at 0.30 ƒc', is calculated from the stress-strain relationship of concrete in the linear range. Points 2, 3, and 4 are obtained from equation (3), in which ε o is calculated from equation (4). Point 5 is at ε o and ƒc'. In this study, an assumption was made of perfectly plastic behavior after point 5., [8]. this discussion will mean the process of defining the geometric configuration of the model's nodes and elements. Element (SOILD65) used for concrete was chosen to represent every type of materials that depending on the agreements with experimental study [11] SOILD65 Element Description SOLID65 (or 3-D reinforced concrete solid) is used for the 3-D modeling of solids with or without reinforcing bars (rebar). The solid is capable of cracking in tension and crushing in compression. In concrete applications, for example, the solid capability of the element may be used to model the concrete, while the rebar capability is available for modeling reinforcement behavior. The element is defined by eight nodes having three degrees of freedom at each node: translations of the nodes in x, y, and z-directions. Up to three different rebar specifications may be defined. The most important aspect of this element is the treatment of nonlinear material properties. The concrete is capable of cracking (in three orthogonal directions), crushing, plastic deformation, and creep. The rebars are capable of tension and compression, but not shear. They are also capable of plastic deformation and creep. This 8-node brick element is used, in this study, to simulate the behavior of concrete (i.e. plain concrete). The element is defined by eight nodes and by the isotropic material properties. The geometry, node locations, and the coordinate system for this element are shown in Figure (2). Figure 2. SOLID65 Geometry [1] Figure 1. Simplified compressive uniaxial stress-strain curves for concrete [8] 2.3. Beams Modeling The ultimate purpose of a finite element analysis is to recreate mathematically the behavior of an actual engineering system. In other words, the analysis must use an accurate mathematical model of a physical prototype. In the broadest sense, this model comprises all the nodes, elements, material properties, real constants, boundary conditions, and other features that are used to represent the physical system. In ANSYS terminology [1], the term beams generation usually takes on the narrower meaning of generating the nodes and elements that represent the spatial volume and connectivity of the actual system. Thus, model generation in 2.5. Link8 Element Description (For Pre-Stressing Rebar, Main and Shear Reinforcements LINK8 is a spare (or truss) element which may be used in a variety of engineering applications. This element can be used to model trusses, sagging cables, links, springs, etc. The 3-D spare element is a uniaxial tension-compression element with three degrees of freedom at each node: translations of the nodes in x, y, and z-directions. As in a pin-jointed structure, no bending of the element is considered. Plasticity, creep, swelling, stress stiffening, and large deflection capacities are included. This element is used in this study, to simulate the behavior of steel reinforcement which works as main longitudinal, ties reinforcement and pre-stressing rebar. The geometry, node locations, and the coordinate system for this element are shown in Figure (3).

4 Journal of Civil Engineering Research 2016, 6(2): Real Constants The real constants for the elements used to model the pre-stressed concrete beam problems are shown in Table (3). Each element has its real constant. Figure 3. Link 8 geometry [1] 2.8. Create Beam's Volume The pre-stressing beams, anchorages, load plates, and support plates were modeled as a Key point's Lines Areas Volumes. The dimensions of the beams are shown in Fig Solid45 Element Description (For Bearing Plates and Load Points) An eight-node solid element, SOLID45, is used for the steel plates at the supports and bearing plates in the beams models. The element is defined with eight nodes having three degrees of freedom at each node-translation in the nodal x, y, and z directions. The geometry and node locations for this element type are shown in Figure (4). The element has plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities. A reduced integration option with hourglass control is available. Table 3. Real constant for the elements that used in this research Real constant set Element type Constants 1 2,3 4 Solid 65 Link8 (Main and shear rein.) Link8 Φ=7mm (pre-stress bar) 3. Mesh Generation of Post-Tensioned Concrete Beams Specimens As an initial step in the finite element analysis, the post-tensioned concrete beam specimens are divided into a number of small elements, after that the loads and boundary conditions are applied, and the stresses and strains are calculated at integration points of these elements. An important step in the finite element modeling is the selection of the mesh density. Description Real Constant for Rebar Material Number 0 Volume Ratio 0 Orientation Angle 0 Orientation Angle 0 Cross-sectional area, mm Cross-sectional area, mm Initial strain 5.94*10^-3 Figure 4. SOLID45 geometry [1]

5 44 Amer Farouk Izzet et al.: Effect of High Temperature on the Strain Behavior in Post-Tensioning Concrete Beams by Using Finite Element Method (ANSYS Program) Figure 6. Beams meshing 4. Loads and Boundary Conditions To ensure that the model acts in the same way as the experimental beam. The boundary conditions need to be applied at points of symmetry, and where the supports and loadings exist. Moreover, displacement boundary conditions are needed to constrain the model to get a unique solution. The model being used is symmetrical about XY planes. Hence, the applied boundary conditions include the supports and applied load conditions. Each support was modeled, in such a way, so that an hinge was created. All the nodes that lies on the middle line of the support plate were given a constraint value of zero in the UY, and UX directions. By doing this, the beam will be allowed to rotate at the support. The support condition is shown in Figure (7). The external load was applied by mean of equivalent nodal forces with the existence of steel plates on the top face of beam at two points see Figure (7). The application of the loads up to failure was done incrementally as required by Newton-Raphson procedure. Therefore, the total applied load was divided into a series of load increments (load steps), with in each load step, maximum of (100) iterations were permitted. Failure for all models was define when the solution for a minimum load increment still does not converge (convergence fails). Figure 5. Beam modeling Convergence of results is obtained when the structure is divided to adequate number of elements. This is practically achieved when an increase in the mesh density has a negligible effect on the results. Therefore, in the present finite element modeling, a convergence study was carried out to determine the appropriate mesh density. The convergence study was made by increasing the number of elements (mesh) in each direction Z, Y and X. When an increase in mesh density has a negligible effect on the results of deflection, it is assumed that the convergence of results is obtained. Figure (6) shows the mesh of beam specimens which is adopted in this study. This mesh is used for all beams. Figure 7. Loads and Boundary Conditions 5. Results and Discussion In the analysis, the beam specimens were exposed to fire flame from all sides. The beam specimens were burnt at

6 Journal of Civil Engineering Research 2016, 6(2): temperature levels (300, 500 and 700 C) for 60minutes period of exposure Results of Analysis of Beam Specimens To illustrate the validity of the proposed numerical method for the analysis of reinforced concrete beam specimens under two-point loading, the tested beams will be analyzed by using ANSYS computer program Pre-Stress Effect The deflections obtained from experimental work [11], hand calculations [11], and from the FE analysis due to the pre-stress effect are given in Table (4). Figure (8) shows the deflected shape due to pre-stress effect for each tested specimens. From Table (4) it is clear that there is a good agreement between the experimental [11] and FE. Analysis. The difference varies between 0% to 18% and it was about 26% with respect to the hand calculation Heating Effect on the Post Tensioning Concrete The strain of the concrete can be measured theoretically by using ANSYS software, because it is impossible practically measured due to the flame heat. The results shown in Figure (9). Table 4. Pre-stress effect (camber) for pre-stress beams Beams Status R G1 S1 G2 S2 G3 S3 Center line deflection at pre-stress stage, mm Experimental [11] ANSYS Hand calculation [11] Figure 8. Pre-stressing force effects Figure (9). Peak strain models of pre-stressed concrete at elevated temperatures with experimental data of other researches

7 46 Amer Farouk Izzet et al.: Effect of High Temperature on the Strain Behavior in Post-Tensioning Concrete Beams by Using Finite Element Method (ANSYS Program) 6. Conclusions 1. The three-dimensional finite element model used in the present work is able to simulate the behavior of post-tensioning concrete beam. 2. The results from testing and finite element analysis show that the prediction of the strain by the proposed analytical method show good agreement with the test results from the experimentally tested beam specimens [11]. 3. From all that noticed that the strain increased when the temperature increased that s because of the weakness in beams properties such as compressive strength, load capacity and large mid span deflection. REFERENCES [1] ANSYS, Copyright 2011, "ANSYS Help", Release 9.0. [2] Bangash, M.Y.H., 1989, "Concrete and Concrete Structures", Numerical Modeling and Applications, Elsevier Science Publishers Ltd, London, England. [3] Chen, W. F. and Saleeb, A. F., 1981, "Constitutive Equations for Engineering Materials", West Lafayette, Indiana, December, 580 pp. [4] Desayi, P. and Krishnan, S., 1964, "Equation for the Stress-Strain Curve of Concrete", Journal of the American Concrete Institute, Vol. 61, March, PP [5] Dong, Y. and Prasad, K., 2008, "Thermal and Structural Response of a Two-Story, Two-Bay Composite Steel Frame under Fire Loading", Proceedings of the Combustion Institute, 8pp. [6] Gere, J.M., and Timoshenko, S.P., 1997, "Mechanics of Materials", PWS Publishing Company, Boston, Massachusetts. [7] Hemmaty, Y., 1998, "Modeling of the Shear Force Transformed Between Cracks in Reinforced Concrete Structures" Proceeding of the ANSYS Conference, Vol.1, Pittsburgh, Pennsylvania, August. [8] Huyse, L., Hemmaty, Y., and Vandewalle, L., 1994, "Finite Element Modeling of Fiber Reinforced Concrete Beams", Proceeding of the ANSYS Conference, vol.2. Pittsburgh, Pennsylvania, May. [9] Kachlakev, D.I. and McCurry, D., Jr., 2000, "Simulated Full Scale Testing of Reinforced Concrete Beams Strengthened With FRP Composites: Experimental Results and Design Model Verification", Oregon Department of Transportation, Salem, Oregon, June. [10] Farhad Aslani, "Pre-stressed concrete thermal behavior", Magazine of Concrete Research, 2013, 65(3), , Volume 65 Issue 3. [11] Zahra 'a Hussein and Amer Izzat, "Effect of Fire Flame (High Temperature) on the Behavior of Post-Tensioned Concrete Beams", Master thesis, A Thesis Submitted to the College of Engineering University of Baghdad in Partial Fulfillment of the Requirements for The Degree of Master of Science on Civil Engineering, 2016.