Using a Beam Section Integrated during the Analysis to Define the Section Behavior

Use a beam section integrated during the analysis to define the section behavior when numerical integration over the section is required as the beam deforms. You can choose a section shape from the library of beam section shapes provided (see Beam Cross-Section Library) and define the section's dimensions. In addition, you can specify the number of section points to use for integration. The default number of section points is adequate for monotonic loading that causes plasticity. If reversed plasticity occurs, more section points are required.

You can also specify an offset for the section origin, as illustrated in Figure 1, for a rectangular cross-section. In Figure 1, the original cross-section axes ${\mathbf{n}}_1$ - ${\mathbf{n}}_2$ are always placed at the beam axis, while the local 1-2 system defines the shifted cross-section axes after offsets of $x_{1o}$ and $x_{2o}$ are applied in the ${\mathbf{n}}_1$ - and ${\mathbf{n}}_2$ -directions, respectively.

Figure 1. Offset for the section origin.

Use a material definition (Material Data Definition) to define the material properties of the section, and associate these properties with the section definition. Linear or nonlinear material behavior can be associated with the section definition. However, if the material response is linear, the more economic approach is to use a general beam section (see Using a General Beam Section to Define the Section Behavior).

You must associate the section properties with a region of your model.

BEAM SECTION, ELSET=name, SECTION=library_section, MATERIAL=name

BEAM SECTION OFFSET

Property module:
Create Profile: Name: library_section
Create Section: select Beam as the section Category and Beam as the section Type, Section integration: During analysis, Profile name: library_section, Material name: name, Offset for origin of cross-section: specify X1 and X2 values
AssignSection: select regions

In the shear flexible elements Abaqus provides for a possible uniform cross-sectional area change by allowing you to specify an effective Poisson's ratio for the section. This effect is considered only in geometrically nonlinear analysis (see Defining an Analysis) and is provided to model the reduction or increase in the cross-sectional area for a beam subjected to large axial stretch.

The value of the effective Poisson's ratio must be between −1.0 and 0.5. By default, this effective Poisson's ratio for the section is set to 0.0 so that this effect is ignored. Setting the effective Poisson's ratio to 0.5 implies that the overall response of the section is incompressible. This behavior is appropriate if the beam is made of a typical metal whose overall response at large deformation is essentially incompressible (because it is dominated by plasticity). Values between 0.0 and 0.5 mean that the cross-sectional area changes proportionally between no change and incompressibility, respectively. A negative value of the effective Poisson's ratio results in an increase in the cross-sectional area in response to tensile axial strains.

This effective Poisson's ratio is not available for use with Euler-Bernoulli beam elements.

BEAM SECTION, POISSON=${\nu }_{\mathrm{eff}}$

Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis, Section Poisson's ratio: ${\nu }_{\mathrm{eff}}$

When a beam section integrated during the analysis is used, damping can be introduced through the material behavior definition. See Material Damping for more information about the material damping types available in Abaqus.

Temperature and field variables can be specified at specific points through the section or by defining the value at the origin of the cross-section and specifying the gradients in the local 1- and 2-directions. The actual values of the temperature and field variables are specified as either predefined fields or initial conditions (see Predefined Fields or Initial Conditions).

In any element it is assumed that the temperature definitions at all the nodes of the element are compatible with the temperature definition method chosen for the element. For cases in which the temperature definition method changes from one element to the next, separate nodes must be used on the interface between elements with different temperature definition methods and MPCs must be applied to make the displacements and rotations the same at the nodes.