ZANCO Journal of Pure and Applied Sciences The official scientific journal of Salahaddin University-Erbil ZJPAS (2016), 28 (6); 65-56 http://doi.org/10.21271/zjpas.28.6.7 Punching Strength of GFRP Reinforced Concrete Slab-Column Connections with Openings by the Finite Element Method Ali R. Yousif 1, Akram S. Mahmoud 2, Mohanad T. Abduljaleel 3 1 Civil Engineering Department-College of Eng.-University of Salahaddin-Erbil-Iraq 2 Civil Engineering Department-College of Eng.-University of Anbar-Iraq 3 Master Student, Civil Engineering Department-College of Eng.-University of Anbar-Iraq A R T I C L E I N F O Article History: Received: 06/ 04/2016 Accepted: 23/08/2016 Published:10/1 /2017 Keywords: Finite Element, Opening, GFRP bars, Flat Plate Slab, Punching Shear *Corresponding Author: Mohanad T. Abduljaleel Email: m.t.eng2012@gmail.com A B S T R A C T In flat slabs, a brittle failure mode can rise due to poor transfer capacity of shearing force and unsymmetrical moment. Existing of the opening around the vicinity of column increase the possibility of punching failure, in this case numerical analysis is necessary to understanding the structural behavior of such complex case. This study presents nonlinear finite element analysis of the slabcolumn connections reinforced with GFRP bars by using the ANSYS15 software, in addition, the summary of experimental test result. Solid 65 was used for modeling concrete element and GFRP bars were inputted by using link 180. Link 10 was used to overcome the rigidity of supporting which gave a good rotation in the both sides. For simplicity of analysis, only quarter-size have inputted. Only discrete model have considered to modeling reinforcement bars. Numerical result showed punching shear mode due to crashing of the concrete element before yielding the reinforcement bar. The numerical results were compared with the experimental data which obtained from testing four interior slab-column connections and gave a good agreement. Depending on the numerical and experimental result, existing of the openings reduced the punching shear capacity and increased the deflection of the specimens. Increasing of the reinforcement ratio improved punching capacity. Different stiffness have been observed between experimental and numerical model but have a liner behavior before first cracking. 1. INTRODUCTION Corrosion of steel reinforcement is a problem which faces the engineering in the hard condition situation and marine building. Researchers proposed more than one solution to overcome the corroding problem, for instance, increasing of concrete cover, epoxy coating, and using stainless steel bars. All those solutions do not provide the effective solution and at the same time, they are expensive. GFRPs bars are good alternative reinforcement and have significant properties that can be used in hard condition. Slab-column connections have a brittle failure with limited deflection and the forces and loads transfer from slab to the column, which creates a critical zone around the column lead to failure which called punching shear. Flat plate slabs reinforced with GFRP and with openings are a new subject which was not studied before according to our knowledge. Therefore the experimental and numerical investigation are required to understand the behavior of such slabs. This paper presents the numerical modeling of four slab-column connections reinforced with GFRP bars with and without openings by using ANSYS software.
57 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 2. Experimental Data A total of four (1100 1100 90) mm interior slab-column connections were reinforced with GFRP bars with reinforcement ratio ranged (1.3-2.2)%. All specimens were simply supported on the four edges and tested under axial load acting on the column from top to down. The column stub extended 200 mm from the top, and 100 mm from the bottom. Symmetrical opening (150 150) mm system was applied to avoid the effects of force and moment, which may appear due to the asymmetry of the opening. Figure (1) shows the details of the specimen. (b) Slab-column connection fabrication and test Fig. (1) Slab-column connection details 2.1. Materials and Tools The specimens were cast using normal strength concrete. Ordinary Portland cement, water, fine aggregate, and coarse aggregate were used. All these materials were compared with (ASTM C33, 1999) specification as shown in the Figures (2, 3). The target compressive strength of NSC was 30 MPa. The slump of fresh concrete was measured before casting, and was approximately equal to 20 mm. (a) Slab-column connection dimension Fig. (2) Fine aggregate sieve analysis
58 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 Fig. (3) Coarse aggregate sieve analysis 2.2. Glass Fiber Reinforced Polymer (GFRP) Bars Deformed surface GFRP bars of size No. 13 (12.7 mm) was used as flexural reinforcement of the two-way flat plate slabs. The modulus of elasticity (E f ) was 45 GPa. Ultimate tensile strength of the GFRP bars 800MPa. Table (1) demonstrates the physical properties of the GFRP bar. Table (1) Physical properties of GFRP bar Strain mm/mm 0 0.006 0.008 0.01 0.012 0.014 0.016 0.017 Stress MPa 0 200 288 411 550 660 775 802 2.3 Strain Gauge There are several methods for measuring strain; the most common is with metallic strain gauge. TML strain gauges were used to determine the strain in the reinforcement bar. Each specimen was provided with two strain gauges. The gauge type was FLA-6-11, which can be used for general purpose and applicable for metal, glass, and ceramic. Strain gauges were connected to Quarter Bridge and two-wire system. Figure (4) reveals the strain gauge after applied. Fig. (4) Strain gauge fixed on the GFRP bar 2.4. Experimental Result Simply support and monotonic load techniques were used for specimens test. Mechanical dial gauge at the mid span of specimen was used for measuring the deflection. As mentioned in previous Data logger was used to predict the strain of reinforcement bar. Table (2) displays the summary of the experimental result. Table (2) Summary of experimental test results Specimen X cone Strain at Ultimate Load MPa Slab's opening location kn mm SG1 2.2 136.2 16.20 3.6d 7120 29.8 N/A SGO1 1.3 67.7 14 2.4d 7935 37.3 At column face SGO3 2.2 80 17.70 4.0d 7757 30.5 At column face SGO4 2.2 100 11.30 3.4d 4691 35.4 2d from column face Note: X cone is distance from column face to observed failure, calculated by average around the column, and Ԑ is strain at ultimate load, u is deflection at mid span.
59 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 3. Simulation of Finite Element Model ANSYS software has many finite element analysis capabilities, simple static analysis as well as complex non-linear dynamic analysis. In general, a finite element solution passes through three main stages as follow (Alberta University, 2001). 1. Preprocessing Define keypoints, lines, areas, and volumes Define element type, material, and geometric properties mesh lines, areas, volumes 2. Solution Assigning loads Constraints Solving 3. Results review (post processing). The ANSYS software is capable of analyzing (numerically) nonlinear response of RC concrete under static and dynamic loading. Any model can be created using the command prompt line input or the Graphical User Interface (GUI) (Saber, M., 2013). ANSYS software version 15 was used for modeling quarter-size specimen. Three-dimensional element solid 65 which is capable of cracking and crushing along with the GFRP bar modeling were adopted to describe the behavior of the composite reinforced concrete material (concrete with GFRP bars). The construction of model using ANSYS is shown in Figure (5). Control point for 75 75 mm Fig. (5) ANSYS numerical model representation of experimental specimen Quarter-Size of specimen have been used due to the symmetrical case and reduce of the time inputting. In addition, it was found the modeling with Quarter-Size gives more flexible and accurate result compared with whole size. 3.1. Concrete Element (Solid65) Solid 65 which is an eight nodes element was used to model the concrete element with three degrees of freedom at each node, translations in the x, y, and z directions (Zhang, Q., 2004). The element is capable of plastic deformation, cracking in three orthogonal directions, and crushing. Figure (6) presents the solid 65 elements (ANSYS User s Manual Revision 15, 2015). 550 550 90 mm Fig. (6) Solid 65 element
60 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 The mechanical properties of the element (Solide 65) have been inputted depending on the experimental result Figure (7) demonstrates the test of compression strength. 3.3. Supporting Element (link10) Link 10 is a 3-D spar element having the unique feature of bilinear stiffness matrix resulting in tension only (or compression only) element. Link10 element is special nonlinear spring element in the transverse direction, which was employed along edges of slabs in the numerical model. The stiffness of spring elements is numerically set to be significantly high in compression and zero in tension, respectively (Zhang, Q., 2004). 3.4. Real Constants The real constants for this model are shown in Table (3). Fig. (7) Compression strength test 3.2. Reinforcement Bars (link180) Link180 is a three-dimensional spar used to model the GFRP and steel bars reinforcement. The element is uniaxial tension-compression, the geometry, and nodes location are shown in Figure (8). Two nodes are required for this element. Each node has three degrees of freedom, translation in the nodal x, y, and z directions. The plastic deformation is included in this element (ANSYS User s Manual Revision 15, 2015). Table (3) Real constants RC Set No. Element Type *link10 was given by command line **half-area of bar at plane of symmetry 3.5. Materials Properties 3.5.1. Concrete Material Material Value mm 2 1 Solid65 Concrete N/A 2 Link180 Steel Bar 113 3 Link10* Spring Sup. 2000 4 Link180 Stirrups 50 5 Link180 GFRP Bar 126 6 Link180 GFRP Bar ** 126/2 Concrete is a heterogeneous material consists of cement, mortar and aggregate. Its mechanical properties scatter widely and cannot be defined easily (Zhang, Q., 2004). For the convenience of analysis and design, however, concrete is often considered as a homogeneous material in the macroscopic sense. Figure (9) reveals the nonlinear response of the concrete material (Bangash, M., 1989). Fig. (8) Geometry of link180
61 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 Numerical expression equations were proposed by (Desayi and Krishnan, 1964); equations (1) and (2), were used along with equation (3) which was proposed by (Gere and Timoshenko, 1997). Fig. (9) Typical uniaxial compressive and tensile stress- strain of the concrete This curve can be divided into three stages, the uncracked elastic stage, the crack propagation stage, and the plastic stage. Development of a model for concrete behavior is not easy. The curve shows linear elastic behavior at about 30% of maximum compressive strength, and above this point crack takes place. After it reaches the maximum compressive strength, the curve descends into softening region, and crushing failure occurs at ultimate strain. For tension zone stress-strain curve shows linear behavior response, after this point concrete cracks and the strength decreases to zero (Bangash, M., 1989). ANSYS software requires some important data to construct stress-strain curve for the concrete. (Qi Zhang, 2004) investigated two stressstrain curves, linear and nonlinear, as shown in Figure (10). It was found that elastic-perfectly plastic model gives good convergence solution and reasonable results for load-deflection relationship. Fig. (11) Simplified uniaxial compressive stress-strain curve Nonlinear stress-strain curves created by these equations were used in the solution of the nonlinear models of flat plate slabs; Figure (12) demonstrates both curves. Fig. (10) Typical stress-strain relationship for normal concrete Fig. (12) Stress-strain curves
62 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 3.5.2. GFRP and Steel Reinforcement Bars GFRP bar was defined as linear elastic behavior with an elastic modulus of 45 GPa and Poisson`s ratio (0.3). The steel bar was defined as nonlinear behavior (bilinear) with elastic modulus 200 GPa, Poisson`s ratio (0.3), and yielding stress 530 MPa as shown in Figure (13). (a) smeared model SIG EPS (b) discrete model Fig. (13) Idealized stress-strain curve of steel reinforcement bar 3.6. Geometry and FE Modeling Due to the symmetry, only quarter of the specimen was used to simulate the flat plate slab; this approach reduced the computational time and effort. The model was built first by defining the nodes with careful numbering because the numbering is important to create an element. The nodes of a concrete element were created by copy process. Elements of the steel were built by the same way. This technique does not need any meshing. Modeling of bar reinforcement can be classified into three different techniques (Tavarez, F.A., 2001); as shown in Figure (14). a. The smeared model b. The discrete model c. The embedded model (c) embedded model Fig. (14) Reinforcement modeling types The smeared model (a) assumes that the reinforcement is uniformly spread through the concrete element in a defined region of the FE mesh. The discrete model (b) uses bar or beam elements that are connected to the concrete element nodes. The concrete and reinforcement elements share the same nodes. The discrete model was used in this study. The discrete model was used to model the reinforcement using link180 element with perfect bond between the concrete and the reinforcement. The dimensions of the model represent the same dimensions of the experimental specimen. The local failure of the supports will be avoided by using the spring elements.
63 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 3.7. Load and Boundary Conditions Automatic time stepping was used to solve the FE model with a specific number of substeps depending on the material properties, the value of loads, and element density. In this study, for reinforced concrete solid elements, convergence criteria were based on force only with the value of (0.05) to help the convergence of the solution. The constant load was applied on the top of the column in Y direction. Because a quarter of the slab was used for the model, planes of symmetry were required at the internal faces. At a plane of symmetry, the displacement in the direction perpendicular to the plane was held at zero (Kachlakev et al., 2001). All degrees of freedom (DOF) of support spring nodes were constrained to prevent the rotation and displacement. 4. Result of FE Analysis The ANSYS15 software was used to simulate four specimens SG1, SGO1, SGO3, and SGO4. The details of these specimens were shown in Figure (1) and Table (2). Numerical analysis was used to study the details of the slab-column connection behavior, and the following items were studied. 1. Load-deflection curves 2. Principal stresses 3. Shear stresses 4. Crack patterns 5. Load-strain curves Numerical analysis is different from the experimental results due to the assumptions made in the FE (ANSYS) modeling. The following are a number of such assumptions: 1. The concrete material is assumed to be homogenous. 2. The perfect bond between concrete and reinforcement. 3. The reinforcement is assumed to carry stress along its longitudinal axis. Figures from (15) to (18) show the contour plot of numerical analysis of specimen SGO3. Fig. (15) Deformed shape of SGO3 Fig. (16) Shear stress of SGO3 Fig. (17) 1st principal stress of SGO3
64 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 with experimental behavior specially at cracks initiation. (a) Specimen of SG1 without opening Fig. (18) GFRP stress of SGO3 5. Discussions Openings located near the column face lead to stress concentration due to the cutoff which decreased the punching perimeter and at the same time increased the deflection. Figure (16) showed that high stresses were concentrated near the opening sides which lead to splitting of the concrete, the fact which was seen experimentally. Depending on the experimental and FEM (ANSYS) results, the reinforcement did not reach yielding, and that explain the facts that all specimens failed by punching shear. In ANSYS software, cracking is shown with a circle outline in the plane of the crack, and crushing is shown with an octahedron outline. If the crack has opened and then closed, the circle outline will have an X through it. Each integration point can crack in up to three different planes. The first crack at an integration point is shown with a red circle outline, the second crack with a green outline, and the third crack with a blue outline (ANSYS User s Manual Revision 15, 2015). Cracks pattern of FEM (ANSYS) are shown in Figures (19) to (21). Specimen SGO3 showed cracks that concentrated at the opening's edges. Cracks pattern showed reasonable agreement (b) Specimen of SGO3 with opening Fig. (19) Cracks at 28% from ultimate load Fig. (20) Element crushed around column of the SGO3 specimen
65 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 Flat plate slabs reinforced with GFRP and with openings are new subject which was not studied before (according to our knowledge). The comparison between the FE (ANSYS) and experimental results is a good tool to check the accuracy of the numerical analysis of flat plate slabs. Table (3) shows the results of such comparisons. Fig. (21) Cracks initiation from opening's edges of SGO3 Slab No. Experimental Results Finite Element Results Finite Element/ Experimental P u u * Ԑ* P u u Ԑ P u u Ԑ (kn) (mm) (Micro) (kn) (mm) (Micro) SG1 136.2 16.2 7120 135.1 18.2 6915 0.99 1.12 0.97 SGO1 67.7 14 7935 69 14 7200 1.01 1 0.90 SGO3 80 17.7 7757 85.3 19.1 7200 1.06 1.07 0.92 SGO4 100 11.3 4691 93.2 10.8 5300 0.93 0.95 1.12 *deflection and strain at ultimate load only. Table (3) Comparison of FE analysis and experimental results The following figures show the load-deflection responses of FE ANSYS results. Figures (23) to (26) show the comparison between the numerical and experiential loaddeflection relationships. Fig. (22) Load-deflection relationships of FE models Figure (22) shows that the load deflection of numerical analysis of all models is exactly the same (linear) before cracking, and the behavior changed after the first cracks. The specimens which reinforced with GFRP and with openings showed a more ductile behavior, because existing of the openings. Fig. (23) Load-deflection relationships of SG1 Fig. (24) Load-deflection relationships of SGO1
66 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 results showed good agreement with the experimental results. Fig. (25) Load-deflection relationships of SGO3 Fig. (26) Load-deflection relationships of FE SGO4 In general, numerical models give lower deflection due to the perfect bond of the reinforcement. The best results of numerical model was that of the SGO4 specimen, which showed good agreement with experimental results. Figure (27) shows the reinforcement strains of the numerical models. 2. In general, the numerical load-deflections curves were somewhat stiffer than the companion experimental curves. This can be attributed, to some extent, to the assumed perfect bond between the concrete and the reinforcement, and also due to disregarding of the micro cracks that exist in the concrete. Notations The following symbols are used in this study: d = Average effective depth (mm) h = Slab thickness (mm) E c = Modulus of elasticity of the concrete (MPa) (E c =4700 ) E f = Modulus of elasticity of GFRP reinforcing bars (MPa) E s = Modulus of elasticity of steel reinforcing bars (MPa) A f = Area of the reinforcing bars (mm 2 ) f c Cylinders concrete compressive strength (MPa) f y = Yield strength of steel bars (MPa) f u = Ultimate tensile strength of steel bars (MPa) f fu = Ultimate tensile strength of FRP bars (MPa) V u = Ultimate punching shear load (kn) u = Deflection at ultimate load (mm) = Reinforcement ratio X cone = Distance from column face to observed failure surface (mm) Ԑ o = Strain at the ultimate compressive strength Fig. (27) Load-strain response of numerical model 6. Conclusion The main conclusions derived from this study may be summarized as follows: 1. The numerical investigation by ANSYS software provided a good tool for analyzing the GFRP reinforced slab specimens, and the Acknowledgements The author would like to thank staff of the civil engineering department of Salahaddin university-erbil and concrete laboratory for their facilities and patient throughout investigating of the experimental part of the manuscript of this paper. REFERENCES ANSYS, (2015) ANSYS User s Manual Revision 15, ANSYS, Inc., United States. AlbertaUniversity ANSYSTutorials, http://www.mece.u alberta.ca/tutorials/ansys/au/ Intro/Intro.html, copyright 2001.
67 Yousif, A. et al./zjpas: 2016, 28(6): 65-56 ASTM C33, (1999) Standard Specification for Concrete Aggregate American Society for Testing and Material. Bangash, M. Y. H. (1989), Concrete and Concrete Structure: Numerical Modeling and Applications, London: Elsevier Science Publishers Ltd. Desayi, P. and Krishnan, S. (1964), Equation for the Stress-Strain Curve of Concrete, Journal of the American Concrete Institute, Vol. 61: 345-350. Gere, J.M. and Timoshenko, S. P. (1997), Mechanics of Materials, PWS Publishing Company, Boston, Massachusetts. Kachlakev, D., Miller, T., Yim, S., Chansawat, K., and Potisuk, T. (2001), Finite Element Modeling of Reinforced Concrete Structures Strengthened with FRP Laminates, Final Report SPR 316, Oregon Department of Transportation, Salem, Oregon, 111p. Saber, M. (2013), Flexural Behavior of High Strength Self-Compacting Concrete Beam Reinforced with FRP Bars, University of Technology, Baghdad, Iraq. Tavarez, F.A. (2001), Simulation of Behavior of Composite Grid Reinforced Concrete Beams Using Explicit Finite Element Methods, M.Sc. Thesis University of Wisconsin-Madison, Madison, Wisconsin. Zhang, Q. (2004), Finite Element Application to Slab- Column Connection Reinforced with Glass Fiber Reinforced Polymers, Research report, 52 p.