CHAPTER 7 FINITE ELEMENT ANALYSIS

Transcription

1 189 CHAPTER 7 FINITE ELEMENT ANALYSIS 7.1 SCOPE In Engineering applications, the physical response of the structure to the system of external forces is very much important. Understanding the response of these components during loading is crucial to the development of an overall efficiency and safe structure. Different methods have been utilized to study the response of structural components. Experimental programs are usually carried out to predict the physical responses of the structure. While this is a method that produces real life response, it is always necessary to validate the experimental results for better understanding of the structure. The finite element analysis can be effectively utilized to study these components. In recent years, the use of finite element analysis has increased due to the progressing knowledge and the capabilities of computer software and hardware. It has now become the choice method to analyze concrete structural components. The use of computer software to model these elements is much faster, and extremely cost-effective. Finite element analysis as used in structural engineering determines the overall behaviour of a structure by dividing it into a number of simple elements, each of which has well-defined mechanical and physical properties.

2 190 Taking into account the fact that the numerical models should be based on reliable test results and also experimental and numerical analyses should complement each other in the investigation of a particular structural phenomenon, Commercial finite element software ANSYS version 11.0 was chosen for this study. The present investigation focuses on the modelling of beams reinforced with Prefabricated Cage using the ANSYS. A threedimensional model is proposed in which all the main structural parameters and associated nonlinearities are included and the beams are analysed both in the linear and non-linear stage. In the linear stage, the deflections are found out and the deflection contour and deformed shape are plotted. In the non linear analysis, the failure loads and failure crack pattern are found out and are validated with that of the experimental and theoretical results. 7.2 ANSYS Advances in computational features and software have brought the finite element method within the reach of both academic research and engineers in practice by means of general-purpose nonlinear finite element analysis packages, with one of the most used package nowadays being ANSYS. The program offers a wide range of options regarding element types, material behaviour and numerical solution controls as well as graphic user interfaces, auto-meshers and sophisticated postprocessors and graphics to speed the analyses. ANSYS includes dedicated numerical models for the nonlinear response of concrete under loading. These models usually include a smeared crack analogy to account for the relatively poor tensile strength of concrete, a plasticity

3 191 algorithm to facilitate concrete crushing in compression regions and a method of specifying the amount, distribution and the orientation of any internal reinforcement. The internal reinforcement may be modelled as an additional smeared stiffness distributed through an element in a specified orientation or alternatively by using discrete strut or beam elements connected to the solid elements. The beam elements would allow the internal reinforcement to develop shear stresses but as these elements in ANSYS are linear, no plastic deformation of the reinforcement is possible. The smeared stiffness and link modelling options allow the elastic-plastic response of the reinforcement to be included in the simulation at the expense of the shear stiffness of the reinforcing bars. 7.3 ANSYS MODELLING OF PCRC BEAMS Modelling is one of the most important aspects in ANSYS Finite Element analysis. Accuracy in the modelling of element type and size, geometry, material properties, boundary conditions and loads are of absolute necessary for close numerical idealization of the actual member. A good idealization of the geometry reduces the running time of the solution considerably. A three dimensional structure can be easily analyzed by considering it as a two dimensional structure without any variation in results. Creative thinking in idealizing and meshing the structure helps not only in considerable reduction of time but also in less memory usage of the system. Finite element modeling of specimen in ANSYS consists of the following three phases:

4 192 Selection of element type Assigning material properties Modelling and meshing the geometry Element Types Selection of proper element types is another important criterion in finite element analysis. The following are the element types used in the ANSYS modelling of PCRC beams. Ansys element Type SOLID 65 SOLID 45 SHELL 63 Material Concrete Steel plates and supports Cold-formed steel sheet Solid 65 ANSYS provides a dedicated three-dimensional eight noded solid isoparametric element, Solid65, to model the nonlinear response of brittle materials based on a constitutive model for the triaxial behaviour of concrete after Williams and Warnke (Fanning 2001). This element is capable of cracking (in three orthogonal directions), crushing, plastic deformation, and creep. The geometry, node locations, and the coordinate system for this element are shown in Figure 7.1. Solid65 element is capable of incorporating one material property for concrete and up to three rebar materials for rebars, which are assumed to be uniformly distributed throughout the concrete element in a defined

5 193 region of the FE mesh. This type of smeared reinforcement model is mainly used in analyzing structures which are large in volume of concrete, e.g., foundations. Figure 7.1 SOLID65 3D Reinforced Concrete Solid Solid 45 SOLID 45 is a three dimensional brick element used to model isotropic solid problems. It has eight nodes, with each node having three translational degrees of freedom in the nodal X, Y, Z directions. This element may be used to analyze large deflection, large creep strain, plasticity and creep problems. The element is used to model the steel plates provided at support and loading plates. It has no real constants. This element is illustrated in Figure 7.2.

6 194 Figure 7.2 SOLID 45-3D Plain Concrete Solid Shell 63 SHELL 63 is used to model the thin walled structures effectively. This has both bending and membrane capabilities. Both inplane and normal loads were permitted. The element had six degrees of freedom at each node. The element is defined by four nodes, four thicknesses, elastic foundation stiffness and the orthotropic material properties. Stress stiffening and large deflection capabilities were included. For PCRC Beams, steel sheet was modeled by using SHELL 63. The geometry and node locations for this element type are shown in Figure 7.3.

7 195 Figure 7.3 SHELL 63 Elastic Shell MATERIAL PROPERTIES Concrete Development of a model for the behaviour of concrete is a challenging task. Concrete is a quasi-brittle material and has different behaviour in compression and tension. Figure 7.4 shows a typical stressstrain curve for normal weight concrete. Material nonlinearity was used in the analysis. For concrete the following nonlinear material properties were considered. Figure 7.4 Typical Stress-strain Curve for Normal Weight Concrete

8 196 As per the ANSYS concrete model, two shear transfer coefficients, one for open cracks and the other for closed ones are used to consider the amount of shear transferred from one end of the crack to the other. Following are the input data required to create the material model for concrete in ANSYS. Elastic Modulus, (E c ) Poisson s Ratio, ( ) Ultimate Uniaxial compressive strength, (f ck ) Ultimate Uniaxial tensile strength, (f t ) Shear transfer coefficient for opened crack, ( 0 ) Shear transfer coefficient for closed crack, ( c ) Poisson s ratio for concrete was assumed to be 0.2 for all the beams. Damien Kachlakev et. al. (2000) conducted numerous investigations on full-scale beams and they found out the shear transfer coefficient for opened crack was 0.2 and for closed crack was 1. The two shear transfer coefficients are used to consider the retension of shear stiffness in cracked concrete. Even though the above parameters are enough for the ANSYS non-linear concrete model, it is better to keep a stress-strain curve of concrete as a backbone for achieving accuracy in results. Hence it was attempted to input stress strain curve.

9 197 The stress-strain curve for concrete can be constructed by using the Desayi and Krishnan (1964) equations. Multi-linear kinematic behaviour is assumed for the stress-strain relationship of concrete which is shown in Figure 7.5. It is assumed that the curve is linear up to 0.3 f c. Therefore, the elastic stress-strain relation is enough for finding out the strain value. = = 0.3 (7.1) Figure 7.5 Simplified Compressive Uniaxial Stress-Strain Curve for Concrete formula. The Ultimate strain can be found out from the following = (7.2)

10 198 The total strain in the non-linear region is calculated and corresponding stresses for the strains are found out by using the following formula. & ) = (7.3) The above input values are given as material properties for concrete to define the non-linearity. In compression, the stress-strain curve of concrete is linearly elastic up to about 30% of the maximum compressive strength. Above this point, the stress increases gradually up to the maximum compressive strength, and then descends into a softening region and eventually crushing failure occurs at an ultimate strain cu. In tension, the stress-strain curve for concrete is approximately linearly elastic up to the maximum tensile strength. After this point, the concrete cracks and the strength decreases gradually to zero. ANSYS has its own non-linear material model for concrete. Its reinforced concrete model consists of a material model to predict the failure of brittle materials, applied to a three-dimensional solid element in which reinforcing bars may be included. The material is capable of cracking in tension and crushing in compression. It can also undergo plastic deformation and creep. Three different uniaxial materials, capable of tension and compression only may be used as a smeared reinforcement, each one in any direction. Plastic behaviour and creep can be considered in the reinforcing bars too. For plain cement concrete model, the reinforcing bars can be removed.

11 Failure Criteria for Concrete ANSYS non-linear concrete model is based on William- Warnke failure criteria. As per the William-Warnke failure criteria, at least two strength parameters are needed to define the failure surface of concrete. Once the failure is surpassed, concrete cracks if any principal stresses are tensile while crushing occurs if all the principal stresses are compressive. Tensile failure consists of a maximum tensile stress criterion. Unless plastic deformation is taken into account, the material behaviour is linearly elastic until failure. When the failure surface is reached, stresses in that direction have a sudden drop to zero, provided there is no strain softening neither in compression nor in tension. This indicates that the descending portion in strain-strain curve of concrete is not considered in ANSYS non-linear concrete model. Figure D Failure Surface for Concrete

12 200 A three-dimensional failure surface for concrete is shown in Figure 7.6. The most significant non-zero principal stresses are in the x and y directions respectively. Three failure surfaces are shown as the projections on the xp- yp plane. The modes of failure are the function of the sign of ZP (principal stress in Z direction). For example, if xp and yp, both are negative (compressive) and ZP is slightly positive (tensile), cracking would be predicted in a direction perpendicular to However, if ZP is zero or slightly negative, the material is assumed to crush. In a concrete element, cracking occurs when the principal tensile stress in any direction lies outside the failure surface. After cracking, the elastic modulus of concrete element is set to zero in the direction parallel to the principal tensile stress direction. Crushing occurs when all principal stresses are compressive and lie outside the failure surface. Subsequently, the elastic modulus is set to zero in all directions and the element effectively disappears. ZP Non-Linear Material Model for Steel The steel for the finite element models was assumed to be an elastic-perfectly plastic material (Deric John Oehlers 1993) and identical in tension and compression. Properties like young s modulus and yield stress, for the steel reinforcement used in this FEM study were found out by conducting the required tests on the sample specimens. Poisson s ratio of 0.3 was used for the steel reinforcement. Bilinear kinematic material model was adopted in this study. Figure 7.7 shows the stressstrain relationship used in this study.

13 201 Figure 7.7 Stress-Strain Curve for Steel A summary of material properties used for modeling all the beams are shown in Table 7.1. These values were used for calculating the important properties required for specifying material non-linearity. Table 7.1 Material Properties Series Material Properties (In N/ mm 2 ) f ck E c f t f y E A x B x C x D x E x F x Concrete G x H x I x J x K x L x A, B,C, CR sheet (1.6mm) x 10 5 D,E,F, CR sheet (2.0mm) x 10 5 G,H,I CR sheet (2.5mm) x 10 5 CR sheet (1.6mm) x 10 5 J,K,L CR sheet (2.0mm) x 10 5 CR sheet (2.5mm) x 10 5

14 Modelling the Geometric Shape A quarter of the full beam was used for modeling by taking advantage of the symmetry of the beam and loadings. Planes of symmetry were required at the internal faces. At a plane of symmetry, the displacement in the direction perpendicular to that plane was held at zero. The geometrical details of the beams modelled are given in Table 7.2. By taking advantage of the symmetry of the beams, a quarter of the full beam was modeled as in Figure 7.8. Ideally, the bond strength between the concrete and steel reinforcement should be considered. However, in this study, perfect bond between materials was assumed. Nodes of the CR sheet shell elements were connected to those of adjacent concrete solid elements in order to satisfy the perfect bond assumption. Figure 7.8 Quarter Beam Model

15 203 Table 7.2 Summary of the Beam Details Sl. No Beam Id t s mm B mm D mm Span m Yield Strength of Steel(N/mm 2 ) Ast (mm 2 ) Compressive of concrete (N/mm 2 ) 1 A A A B B B C C C D D D E E E F F F G G G H H H I I I J J J K K K L L L

16 Finite Element Discretization As an initial step, a finite element analysis requires meshing of the model. In other words, the model is divided into a number of small elements and after loading, stress and strain are calculated at integration points of these small elements. An important step in finite element modeling is the selection of the mesh density. A convergence of results is obtained when an adequate number of elements are used in a model. This is practically achieved when an increase in the mesh density has a negligible effect on the results. Therefore, in this finite element modelling, a convergence study was carried out to determine an appropriate mesh density. The finite element models dimensionally replicated the fullscale transverse beams. That is, a PCRC beam with a cross section of 150 x 200 x 2500mm with the same material properties were modeled in ANSYS with an increasing number of elements. A convergence of results is obtained when an adequate number of elements is used in a model. If the mesh density is increased higher, then convergence problems arise. Based on trial solutions only, the required mesh density is selected. For the PCRC beams, totally 1464 elements were provided. All the nodes were merged with one another to provide a stiff model. The merge operation is useful for tying separate, but coincident parts of a model together. By default, the merge operation retains the lowest numbered coincident item. Higher numbered coincident items are deleted. When merging entities in a model that has already been meshed, the order in which multiple NUMMRG commands are issued is

17 205 significant. If you want to merge two adjacent meshed regions that have coincident nodes and keypoints, always merge nodes (NUMMRG, NODE) before merging keypoints (NUMMRG,KP). Merging keypoints before nodes can result in some of the nodes becoming orphaned, i.e., the nodes lose their association with the solid model. Orphaned nodes can cause certain operations (such as boundary condition transfers, surface load transfers etc.) to fail. After a NUMMRG, NODE is issued and some nodes may be attached to more than one solid entity. As a result, subsequent attempts to transfer solid model loads to the elements may not be successful. Issue NUMMRG, KP to correct this problem. The Figures show the modelling and meshing of various parts of PCRC beams. Figure 7.12 shows FEM discretization of fabricated Prefabricated Cage with reinforcement in a beam and Figure 7.13 represents FEM discretization of concrete portion. Figure 7.9 Modelling of Profile I Figure 7.10 Modelling of Profile II

18 206 Figure 7.11 Modelling of Prefabricated Cage Profile III Figure 7.12 Prefabricated Cage meshed with Quadrilateral Free Meshing Figure 7.13 Concrete Block Meshed with Hexahedral Mapped Meshing

19 Loading and Boundary Conditions A steel plate of 10 mm thick and 50mm x 75mm cross section was provided at the support to avoid the concentration of stresses. Moreover, a single line support was placed under the centerline of the steel plate to allow rotation of the plate. In the quarter model, as the two sides of the beam are continuous, the displacement in the direction perpendicular to the planes was arrested (Figure 7.14). The full scale models were tested in two point loading. The finite element models were loaded at the same locations as in the fullsize beams. Steel plate of 10 mm thick and 50mm x 75mm cross section was provided at the point of loading to avoid concentration of stresses. The load was subdivided into a number of small loads called load step. Each load step was solved gradually and then the solution was obtained for each load step. Figure 7.14 PCRC Beam Model with Loading and Boundary Conditions

20 ANALYSIS Initially linear analysis was carried out. Having confirmed the results in the linear range then nonlinear analysis was performed Linear Analysis Results of the proposed finite element model are verified against the results experimentally obtained from beam tests. The behaviour of the model is investigated throughout the loading history from the first application of the load to service load. Table 7.3 compares the results obtained using the proposed finite element model with those obtained from the experimental tests. Table 7.3 Experimental and Numerical deflections at Service load f ck f y Sl.No Beam Series N/mm 2 N/mm 2 exp P s P s s mm mm 1 A A A B B B C C C D D D E E E F F F G

21 209 Table 7.3 (Continued) f ck f y Sl.No Beam Series N/mm 2 N/mm 2 exp P s P s s mm mm 20 G G H H H I I I J J J K K K L L L Non-linear Analysis In nonlinear analysis, the total load applied to a finite element model was divided into a series of load increments called load steps. At the completion of each incremental solution, the stiffness matrix of the model was adjusted to reflect nonlinear changes in structural stiffness before proceeding to the next load increment. The ANSYS programme uses Newton-Raphson equilibrium iterations for updating the model stiffness. Newton-Raphson equilibrium iterations provide convergence at the end of each load increment within tolerance limits. A force convergence criterion with a tolerance limit of 5% was adopted for avoiding the divergence problem. Equilibrium iterations to be performed were relaxed up to 100. Failure load of each beam was obtained and are presented in Table 7.4.

22 210 Table 7.4 Experimental and Numerical Results Beam Series Experimental Failure Load (kn) ANSYS Failure Load (kn) P exp / P ANSYS A A A B B B C C C D D D E E E F F F G G G H H H I I I J J J K K K L L L

23 RESULTS AND DISCUSSION This section compares the results from the ANSYS finite element analyses with the experimental data for the full-size beams. The following comparisons are made: deflection at service stage, Crack pattern and loads at failure. The data from the finite element analyses were collected at the same location as the load tests for the full-size beams. The following results were obtained from ANSYS for all the tested specimens. Deflection contours at service load Crack pattern Failure load Deflections were found out for various load values. The contours of deflection are shown for a selected specimen in Figure Deformed shapes for some of the specimens are shown in Figure The development of cracks was captured at various load intervals and failure crack pattern is presented in Figure The results from ANSYS were tabulated in Table 7.4. Figure 7.15(a) Deflection Contour for D1 Series Figure 7.15(b) Deflection Contour for D2 Series

24 212 Figure 7.15(c) Deflection Contour for E2 Series Figure 7.15(d) Deflection Contour for E3 Series Figure 7.15(e) Deflection Contour for G1 Series Figure 7.15(f) Deflection Contour for G2 Series Figure 7.16(a) Deformed Shape of A1 Series Figure 7.16(b) Deformed Shape of B1 Series

25 213 Figure 7.16(c) Deformed Shape of C1 Series Figure 7.16(d) Deformed Shape of H1 Series Figure 7.16(e) Deformed Shape of J1 Series Figure 7.16(f) Deformed Shape of K1 Series Figure 7.17 Experimental and ANSYS Crack Pattern of J3 Series

26 KEY FINDINGS A three dimensional finite element model of PCRC beams is proposed based on the use of the commercial software ANSYS version From the finite element analysis the following conclusions were drawn. Results of the numerical simulations are compared with the experimental findings. Apparently, good agreement is obtained from the comparison showing that the proposed numerical simulation method is applicable for analyzing the similar structures. Deflections at the centre line along with progressive cracking of the finite element model compare well to data obtained from experimental investigations. The failure mechanisms of PCRC beams is modelled quite well using finite element analysis and the failure load predicted is very close to the failure load measured during experimental testing. Verification and calibration of material models for coldformed sheet and concrete by PCRC beam test makes it possible to predict the failure load and deflection at service load with higher confidence. For concrete Multi linear kinematic material model is used whereas bilinear kinematic model gives excellent predictions for cold-formed sheet.