Non-Linear Analysis of Base Plates in Automated Storage Systems

Transcription

1 Non-Linear Analysis of Base Plates in Automated Storage Systems Ph.D. Juan José del Coz Díaz, Fco. Suarez Domínguez, Paulino J.Garcia Nieto University of Oviedo. Construction and Applied Mathematics Area. Jose Luis Suárez Sierra, Juncal Guerrero Muñoz, Roberto Suárez Sierra AST-Ingeniería.-Spain Jesús Fernández García ESMENA-CTE.-Spain Abstract The present paper aims to describe the development of a numerical model to accurately simulate the connection between columns and foundation in metallic structures, which constitute any frame in automated storage systems. A nonlinear structural behavior of the model occurs, due to the changing status of the contact surfaces and node-to-node contacts, the geometric nonlinearities of the model (post-buckling and sliding response) and the material nonlinearities, such as plasticity and surface friction. The finite element approach has been carried out in two phases: First, a pre-buckling analysis has been accomplished and then, in a second phase of the study, the above-mentioned nonlinear analysis has been performed, updating the geometry of the finite element model to the deformed configuration for the first mode buckling. A total of four load cases were analyzed, with different compressive load and imposed lateral displacement. In order to validate the results some experimental models were tested to compare with the numerical model, so that better correlations and conclusions were obtained. The figures below show both the experimental model and the finite element model: Figure 1. Model tested M630 with E-type base plate

2 Figure 2. Numerical model of the specimen Introduction The European Standard FEM ([1]) establishes the approaches of tests to perform on base plates of storage systems to eventually determine their flexure stiffness. Thus, the main purpose of the simulation was to adequately reproduce the tests carried out on real models in the Technological Center of Esmena, designer and manufacturer of structural storage systems in Gijón (Asturias, Spain). The model tested was the named M630 from the selective rack system (shelving system designed for storing palletized loads), which includes an E-type base plate.

3 The analysis was performed through a sequence of multiple steps. A half-symmetry three-dimensional surface model of the assembly was initially created in SolidWorks The model was then imported to ANSYS 7.0 via IGES file. Once in ANSYS the geometry was completed, some details were added and, after a geometry checking, the model was meshed. Boundary conditions were included to suitably reproduce the laboratory tests and the load was applied in increasing levels, from 25 % to 100% of the beam ultimate load. A buckling analysis was subsequently performed to obtain the mode shapes and frequencies. The first mode shape was included to the model and a non-linear analysis was accomplished regarding the material and geometric non-linearities. Finally, the results were reviewed and the simulation was compared and validated with the experimental tests. The discussion of the results will be focused both in the values obtained for the stiffness in each model and in the failure modes. Geometric model As it was mentioned above the geometric model was initially designed in SolidWorks Symmetry, drills, holes and other construction details were added once the model was imported to ANSYS. The assembly consists of different parts, as shown in Figure 3 Figure 3. Geometric model Finite element model Based on the geometric model previously described, the finite element model was built, following a fourstep process. Step one was the definition of material properties. Step two was selecting the element types, formulations and real constants. The model was meshed ([2]) in a third step and lastly, in a fourth step, loads and boundary conditions were applied. 1. Material properties Different material properties and constitutive laws were defined in the model for each part of the assembly. Pure perfect isotropic elastic material behavior was assumed for the upper plate (Force plate) of the

4 specimen. However, the rest of the parts were subjected to plasticity. Thus the multilinear kinematic hardening option was selected to describe the material behavior and the data provided by the experimental tests (in form of stress-strain curves) were curve-fitted to a multilinear representation for beam, angles and base plate. Figure 4 shows the data curve fitting employed for the beam. Finally, for the contact pairs, a static coulomb friction coefficient of 0.3 was adopted for the material. M630-Tension test Stress [N/mm2] ,000 0,005 0,010 0,015 Strain [%] Figure 4. Data curve fitting for the multilinear kinematic hardening values 2. Element types The base plate, beam, force plate and angles were modeled using SHELL181. CONTA174 and TARGE 170 were utilized in different contact pairs throughout the model, such as the frontal and lateral contact between beam and angles or between base plate and foundation ([3], [4]). The frontal and lateral contact between angles and beam (see Figure 5) was modeled as flexible-flexible standard type, with beam/shell thickness effect, and the Augmented Lagrange method as the numerical algorithm. The values of normal penalty stiffness (FKN) and penetration tolerance (FTOLN) were 1 and 0.1 or 0.5 respectively. Figure 5. Contact pair between angles and beam

5 The contact between base plate and foundation was modeled as rigid-flexible standard type, with beam/shell thickness effect, and the Augmented Lagrange method as the numerical algorithm. The values of normal penalty stiffness (FKN) and penetration tolerance (FTOLN) were 1 and 0.1 respectively. Figure 6. Contact pair between base plate and foundation (left) and between beam and base plate (right) The contact between beam and base plate was modeled using CONTA178. It was assumed as node-to-node contact, with zero penetration value in the -Z-axis global direction, and pure Lagrange Multiplier Method as the numerical algorithm. The weak spring option was also considered for preventing rigid body motion, with a maximum tensile force of 1 Newton. The 8 mm diameter bolts were modeled using BEAM188. The nodal displacements were coupled in the three directions (UX, UY and UZ, see figure 7) so that they move accordingly to the nodes on the beam holes. Figure 7. Bolt and coupled degrees of freedom

6 3. Boundary conditions The boundary conditions should reproduce quite accurately those of the experimental tests performed on the laboratory. Therefore X and Y displacements were constrained in the point of application of the axial load and rotations around the longitudinal axis of the bolts were also constrained. The rest of the model remained unconstrained. Analysis The analysis was carried out in two phases: First, a pre-buckling analysis was accomplished and then, a nonlinear analysis was performed updating the geometry of the finite element model to the deformed shape for the first mode buckling. Pre-Buckling analysis A buckling analysis was carried out with the purpose of determining the eventual influence of geometric imperfections in the behavior of the model. Thus a compressive load, Nu, was applied on the force plate. The method chosen for mode extraction was Block Lanczos, with ten modes. Once the mode shapes were reviewed, the geometry of the finite element model was updated according to the displacement results of the previous analysis for the first mode shape. A displacement multiplier of 2 mm was applied. Nonlinear Analysis The following step consisted of applying on the model a compressive solicitation and a transversal displacement, in the direction in which was important to measure the value of the stiffness. Four compressive loads were applied on the pattern: N1 = N.; N2=50000 N.; N3=75000 N.; N4= N. Where the imposed displacement varied from 20 up to 35 mm. To avoid convergence problems the analysis was accomplished in two load steps. First, the compressive load was applied ramped, together with a small displacement of mm. Next, in a second load step, the corresponding displacement was imposed. The solution controls were also adjusted to improve convergence. Thus the parameter time was equaled to the value of the maximum displacement obtained, the geometric non-linearities were activated, the inertial effects were not included, the number of equilibrium iterations was specified and the tolerance convergence values of forces were delimited as well as the time step sizes for each load step. Analysis Results & Discussion The analysis results were retrieved and displayed by means of the time-history postprocessor, POST26.

7 Pre-buckling analysis 8.a) First mode buckling b) Second mode buckling Figure 8. Results of pre-buckling analysis The results of the buckling analysis show the mode shapes observed in the specimens subjected to compression. The imperfections derived from the first mode have been reflected in the numerical model, through a factor of imperfection of 2 mm. Nonlinear analysis The values of the moment at the base plate, M B, and the rotation of the beam, θ 0, were calculated as follows ([5]): F2 L 1 δ 1 δ 2 δ 3 δ 4 M B = + F1 ; θ 0 = d12 d34 Where: F 1 = Applied axial force F 2 = Resulted reaction of the imposed lateral displacement L/2= Beam length δ 1.. δ 4 = Relative displacements measured at the beam external borders d 12, d 34 = Distance between the points of measurement = Imposed lateral displacement See figure 9 for a scheme of the tests performed on the specimen.

8 θ 0 θ 0 F 2 /2 F 2 /2 F 1 F 1 L/2 F 2 L/2 Concrete block F 1 F 1 Beam Bearings δ 4 δ 5 δ 6 δ 1 d 12 F 1 F 1 d 34 δ 3 δ 2 F 2 Figure 9. Schematic representation of test forces and displacements In the numerical model, the magnitude of reactions and displacements were obtained from the ANSYS time-history results postprocessor. The relative displacements (δ 1.. δ 4 ) were calculated as an average value resultant from the displacement results obtained for a set of five nodes, each set positioned on the beam external borders, at similar positions on which the experimental measurement is usually performed. The value of the ultimate moment was estimated from the relationship: M = MAX M ; M θ = rad [ { }] (The ultimate moment is set as the moment at a beam rotation value of 0.02 radians providing the beam failure is not achieved before) And the corresponding design values: M d M = ;θ d = θ 1.1 { M } d Thus the stiffness was calculated as M d K = θ d

9 Several graphs moment-rotation were generated in Excel, for the different load cases. An example of the appearance of these graphs is shown below: M630-50% Load M % Load M ,00E+00 1,00E-02 2,00E-02 3,00E-02 Θ MOMENTO E E E E-02 GIRO 10.a) Graph moment-rotation, axial force= N. 10.b) Graph moment-rotation, axial force= N. Figure 10. Graphs moment-rotation A summary of the results obtained in the different load cases is tabulated below (Table 1), where the values of the estimated maximum design moment and stiffness are displayed for each load case. The specimen failure mode is also stated for each particular case. Table 1. Simulation results obtained from different load cases % LOAD Moment (Nmm) Stiffness (kgm) Failure mode 25 1,51E ,59 Base plate becomes unstuck 50 2,60E ,04 Base plate becomes unstuck 75 3,51E ,50 Base plate becomes unstuck 100 3,55E ,09 Local buckling Figures 11 and 12 display several results plots retrieved from the analyses in the different load cases.

10 Figure 11. Displacements in Z direction and stress plasticization ratio in the lower part of the specimen. Load value = N

11 Figure 12. Displacements in Z direction and stress plasticization ratio in the lower part of the specimen. Load value = N

12 Comparison with experimental results The previous information was contrasted with the experimental results obtained in the laboratory of the Technological Center of ESMENA, located in the Scientific and Technological Park of Gijón. Graphs representing both the numerical and experimental results obtained were built (Figure 13) in order to get a good comparison for the estimated stiffness and moment. M630 Base E - Stiffness Stiffness Compressive load (kn) M630 CTE M630 Ansys M630 Base E- Design moment Moment (kn.cm) Compressive load (kn) M630 CTE M630 Ansys Figure 13. Simulation and experimental data results comparison (CTE= Esmena Technological Center)

13 Conclusions After examining the results obtained numerical and experimentally it can be assumed that the computer aided simulation constitute a reasonable approach to describe the behavior of the system. The FE model may reproduce quite accurately the local buckling failure forms. Moreover the estimated stiffness values are similar to both cases (2-8 % deviation). Although the magnitudes of maximum design moments provided by ANSYS are moderately inferior (about 20 %) to those obtained in the CTE labs the comparison between both methods prove the finite element analysis as a reliable tool to get quite accurate results in a reasonable amount of time, which allows the designer of the assemblies to evaluate and optimize the design prior to manufacture and prototype testing. References [1] FEM RV11 Federación Europea de la Manutención-Sección X. Diseño de Sistemas estáticos de Acero de Rack Paletizado y Estantería. Marzo [2] K. Bathe, Finite Element Procedures, Prentice-Hall, Englewood Cliffs (New Jersey), [3] J.J. del Coz Díaz, P.J. García Nieto Design and finite element analysis of a wet cycle cement rotary kiln, Finite Elements in Analysis and Design, 39, (2002), [4] J.C. Simo, T.A. Laursen, An augmented Lagrangian treatment of contact problems including friction, Comp. Struct., 42, (1992), [5] O.C. Zienkiewicz, R.L. Taylor, The Finite Element Method: Solid and Fluid Mechanics and Nonlinearity, Vol. 2, McGraw-Hill Book Company (United Kingdom), 1991.