Displacement Analysis of Cantilever I-beam

[ Problem Description ] [ I-Beam Cantilever ] [ Finite Element Analyses ] [ Input and Output Files ]


The purposes of this example are:


Displacements are computed for a cantilever beam having an I-shape cross section, and subject to two concentrated loads P = 1600 lb at the flanges of the free end in opposite direction along y axis.

Details of the I-beam geometry and externally applied loads are shown in Figure 1.

Figure 1 : Cantilever I-beam and Externally Applied Point Loads.

The cantilever beam has length L = 40 inches, height h = 5 inches, width w = 10 inches, and thickness t = 0.25 inches. It is constructed entirely from one material type -- Young's Modulus E = 10^7 psi and Poisson's Rate = 0.3.


Finite element analyses are computed for a variety of mesh geometrys, and compared against the results for ANSYS-5.0 shell element, and the SAP-90 shell element.

Each segment of the I-beam is modeled with five shell finite elements, four for the flanges, and 1 shell element for the I-beam web. The overall mesh geometry is controled by the parameter N in Figure 1. N = 2 means that the I-beam is modeled with only two sets of shell finite elements along its length (i.e. 10 finite elements in total).

The ANSYS-5.0 shell element is a four node flat shell element having six degrees of freedom per node in which a drilling degree of freedom based on an approach suggested by Kanok-Nukulchai [1]. The SAP-90 shell element is a quadrilateral flat shell element (six degrees of freedom per node).

Meshes N24816
ALADDIN's Shell Element (x 0.1) 2.451422.505282.514822.52135
ANSYS-5.0 Shell Element (x 0.1) 1.12801.89432.33782.5135
SAP-90 Shell Element (x 0.1) 2.02182.30102.45622.5195

Table 1 : Transverse Displacements at Point 1 (see Figure 1).

Meshes N24816
ALADDIN's Shell Element (x 0.01) 1.387531.465721.488241.49583
ANSYS-5.0 Shell Element (x 0.01) 0.62991.11121.37431.4601
SAP-90 Shell Element (x 0.01) 1.04341.31161.44071.4833

Table 2 : Horizontal Displacements at Point 1 (see Figure 1).

Tables 1 and 2 summarize the transverse and horizontal displacements at Point 1 (see Figure 1) for a variety of finite element meshes. For the purposes of numerical comparison, displacements are also shown for shell elements in the ANSYS-5.0 and SAP-90 finite element packages.



  1. Kanok-Nukulchai, "A Simple and Efficient Finite Element for General Shell Analysis," International Journal for Numerical Methods in Engineering , Vol. 14, 1979, pp. 179-200.


Developed in July 1996 by Lanheng Jin & Mark Austin
Last Modified September 27, 1996
Copyright © 1996, Lanheng Jin and Mark Austin, Department of Civil Engineering, University of Maryland