Application of the Finite Element Method Using MARC and Mentat 3-1 Chapter 3: Tapered Bar Keywords: 1D elasticity, 2D elasticity, plane stress, model symmetry, convergence Modeling Procedures: ruled surface, convert 3.1 Problem Statement and Objectives A tapered bar subjected to an axial load will be analyzed in order to predict the distributions of stress and displacement in the bar. The geometrical, material, and loading specifications for the bar are given in Figure 3.1. The thickness of the bar is 2h inches, where h is described by the equation: hxx=−+4060032.. 3.2 Analysis Assumptions • Because the bar is thin in the width (out-of-plane) direction, a state of plane stress can be assumed. • Even though the load is exclusively axial, the taper in the bar may cause the state of stress to be two-dimensional in nature. The effect of taper on the stress state depends upon the degree of the taper, and is difficult to assess a-priori. Therefore, both a 2D plane stress elasticity analysis and a 1D elasticity analysis will be performed. Geometry: Material: Steel Length: L=10” Yield Strength: 36 ksi Width: b=1” (uniform) Modulus of Elasticity: 29 Msi Thickness: 2h (a function of x) Poisson’s Ratio: 0.3 Density = 0.0088 slugs/in3 Loading: Axial Load: P=10,000 lbs Figure 3.1 Geometry, material, and loading specifications for a tapered bar. P 2h L xApplication of the Finite Element Method Using MARC and Mentat 3-2 3.3 Mathematical Idealization Based on the assumptions above, two different models will be developed and compared. The first model is a 1D elasticity analysis. In this model, the main axis of the bar is discretized using linear two-noded 1D bar/truss finite elements having a uniform thickness within each element. Thus, the geometry is idealized as having a piecewise constant cross-section, as shown in Figure 3.2. The uniform thickness within each element is taken to be equal to the actual thickness of the tapered bar at the x-coordinate corresponding to the centroid of that element. The second model is a 2D plane stress model of the geometry as shown in Figure 3.1. The 2D finite element model of this structure will be developed using 2D plane stress bilinear four-noded quadrilateral finite elements. The present analysis can be greatly simplified by taking advantage of the horizontal plane of symmetry in the bar. The geometry, material properties, and loading conditions are all symmetric about this plane. Therefore, the response of the structure (i.e., displacements, strains, and stresses) will also be symmetric about this plane. Hence, it is necessary to model only a one-half of the bar, as shown in Figure 3.3. The boundary conditions on the symmetry plane are those that occur naturally on this plane, as can be verified by obtaining a solution using the entire bar domain. In particular, the vertical displacement and the shear traction are zero along the symmetry plane. Taking advantage of symmetry reduces the modeling effort, the amount of computer memory, and the amount of CPU time required to obtain a solution. Figure 3.2 Idealized geometry for a tapered bar. P L xApplication of the Finite Element Method Using MARC and Mentat 3-3 3.4 Finite Element Model The procedure for creating the finite element model and obtaining the finite element solution for each type of model is presented at the end of this chapter. The 1D analysis should be performed three times, each with a different mesh. Meshes consisting of 1, 2 and 3 elements should be developed. The 2D analysis should be performed only one time, using the mesh described within the procedure. 3.5 Model Validation Simple hand calculations can be performed to estimate the stresses and deflections in this bar structure. The results of these calculations should be used to assess the validity of the finite element results (i.e., to make sure that the finite element results are reasonable and do not contain any large error due to a simple mistake in the model). The displacement at the end of the bar can be approximated by assuming the bar is of uniform cross-sectional shape. The cross-sectional shape used in this calculation may be, for example, the cross-sectional shape at the mid-point of the bar (at x=5”). Then the displacement can be estimated using the well-known relation: δ=PLEA where δ is the tip displacement of the bar, A is the (uniform) cross-sectional area, and the other parameters are defined in Figure 3.1. The axial stress at any cross-section in the bar can be estimated by neglecting all other stress components and assuming that the axial stress is uniformly distributed over the cross-section. This assumption is not strictly valid for a tapered bar, but such an assumption should allow a reasonably accurate solution to be obtained for the purpose of validation. From equilibrium, it is Figure 3.3 One-half domain to be modeled using 2D plane stress representation. 0.5P h LApplication of the Finite Element Method Using MARC and Mentat 3-4 found that the resultant force at any cross-section is P, so the axial stress can be estimated using the relation: σ=PA where A is the actual cross-sectional area at the section under consideration. 3.6 Post Processing A total of four finite element models were developed – three using 1D two-noded linear truss/bar elements, and one using 2D four-noded bilinear plane stress elements. Based on the results of these analyses, perform and submit the following postprocessing steps. (1) Complete the following table: Model ID Tip Displacement Stress at x = 5.0 1D – one element 1D – two elements 1D – three elements 2D – plane stress elements Validation hand calculation (2) Create a plot of the distribution of displacement along the x-axis as predicted by the four models. Put all of the results on a single plot so that comparisons among the solutions can be made. (3) Create a plot of the distribution of axial stress along the x-axis as predicted by the four models. Put all of the results on a single plot so that comparisons among the solutions can be made. (4) Comment on the convergence of displacement and stress in the 1D