Flexure of a deep beam

In this example the flexural response of a simply supported beam is modeled using continuum elements. The problem was originally used by Flanagan and Belystchko (1982) to test the hourglass control algorithms found in lower-order elements.

The half-symmetry model of the beam has a half-span of 0.4 and a depth of 0.1. The mesh consists of 32 elements (8 × 4). The material is linear elastic with Young's modulus = 1 × 10⁶, Poisson's ratio = 0.0, and density = 1000.

A pinned boundary condition (directions 1 and 2) is specified for the center node on the left boundary of the mesh. A symmetry condition (direction 1) is specified for all the nodes on the right boundary of the mesh. A constant pressure load of magnitude 720000 is applied instantaneously to the top surface of the beam at the beginning of the step.

This problem is modeled with both two-dimensional and three-dimensional elements. In the two-dimensional case all the elements are 4-node plane strain continuum elements (CPE4R). Figure 1 shows three meshes for the problem. The upper mesh is the standard case with 45 nodes. The center and lower mesh in the figure have been generated as two distinct parts each containing 16 elements (4 × 4) and 25 nodes. The two parts intersect along a vertical line of nodes where there are two nodes at each point with identical coordinates (coincident nodes). The mesh shown in the center is constrained to behave as the continuous mesh by using multi-point constraints to pin the coincident nodes along the interface between the two parts. In the lower mesh a surface-based tie constraint is used to constrain the nodes along the interface to have the same response as the original mesh. The three meshes should give identical results with these constraints. All the nodes that have boundary conditions or constraints are indicated in Figure 1 by circles.

The three-dimensional case is identical to the two-dimensional case except that 8-node continuum elements (C3D8R) are used to model the beam. In this case the out-of-plane displacements are constrained to be zero (plane strain). Three meshes are also used in the three-dimensional case with the same constraints (in three dimensions) as described for the two-dimensional case.

The above problems are solved with different section control options. For two-dimensional and three-dimensional solid elements the section control options in Abaqus/Explicit allow the user to choose between five different hourglass control options. In addition, three different kinematic assumptions can be chosen for the three-dimensional solid elements. A discussion of the accuracy and performance that can be obtained with the various section control options can be found in Section Controls. Viscous hourglass control should not be used in quasi-static or low-mode dynamics problems, and analyses with this option are not included here. The section controls option in Abaqus/Standard allows the user to pick between two different hourglass control options. The reduced-integration elements in Abaqus/Standard allow only average strain kinematic formulation with second-order accuracy. Table 1 lists the various options and their plot legend and file descriptors.