Beam modeling consists of: choosing a beam cross-section (Choosing a beam cross-section and Beam cross-section library); choosing the appropriate beam element type (Choosing a beam element and Beam element library); defining the beam cross-section orientation (Beam element cross-section orientation); determining whether or not numerical integration is needed to define the beam section behavior (Beam section behavior); and defining the beam section behavior (Using a beam section integrated during the analysis to define the section behavior or Using a general beam section to define the section behavior). The following topics are discussed:

Abaqus offers a wide range of beam modeling options.

## Determining whether beam modeling is appropriate

Beam theory is the one-dimensional approximation of a three-dimensional continuum. The reduction in dimensionality is a direct result of slenderness assumptions; that is, the dimensions of the cross-section are small compared to typical dimensions along the axis of the beam. The axial dimension must be interpreted as a global dimension (not the element length), such as

• distance between supports,

• distance between gross changes in cross-section, or

• wavelength of the highest vibration mode of interest.

In Abaqus a beam element is a one-dimensional line element in three-dimensional space or in the XY plane that has stiffness associated with deformation of the line (the beam's “axis”). These deformations consist of axial stretch; curvature change (bending); and, in space, torsion. (Truss elements are one-dimensional line elements that have only axial stiffness.) Beam elements offer additional flexibility associated with transverse shear deformation between the beam's axis and its cross-section directions. Some beam elements in Abaqus/Standard also include warping—nonuniform out-of-plane deformation of the beam's cross-section—as a nodal variable. The main advantage of beam elements is that they are geometrically simple and have few degrees of freedom. This simplicity is achieved by assuming that the member's deformation can be estimated entirely from variables that are functions of position along the beam axis only. Thus, a key issue in using beam elements is to judge whether such one-dimensional modeling is appropriate.

The fundamental assumption used is that the beam section (the intersection of the beam with a plane that is perpendicular to the beam axis; see the discussion in Choosing a beam cross-section) cannot deform in its own plane (except for a constant change in cross-sectional area, which may be introduced in geometrically nonlinear analysis and causes a strain that is the same in all directions in the plane of the section). The implications of this assumption should be considered carefully in any use of beam elements, especially for cases involving large amounts of bending or axial tension/compression of non-solid cross-sections such as pipes, I-beams, and U-beams. Section collapse may occur and result in very weak behavior that is not predicted by beam theory. Similarly, thin-walled, curved pipes exhibit much softer bending behavior than would be predicted by beam theory because the pipe wall readily bends in its own section—another effect precluded by this basic assumption of beam theory. This effect, which must generally be considered when designing piping elbows, can be modeled by using shell elements to model the pipe as a three-dimensional shell (see About shell elements) or, in Abaqus/Standard, by using elbow elements (see Pipes and pipebends with deforming cross-sections: elbow elements).

In addition to beam elements, frame elements are provided in Abaqus/Standard. These elements provide efficient modeling for design calculations of frame-like structures composed of initially straight, slender members. They operate directly in terms of axial force, bending moments, and torque at the element's end nodes. They are implemented for small or large displacements (large rotations with small strains) and permit the formation of plastic hinges at their ends through a “lumped” plasticity model that includes kinematic hardening. See Frame elements for details.

In addition to the various beam elements, Abaqus also provides pipe elements to model beams with pipe cross-sections that are subject to internal stress due to internal and/or external pressure loading. Abaqus provides a choice of two formulations for pipe elements:

• the thin-walled formulation, where the hoop stress is assumed to be constant and the radial stress is neglected, is available in Abaqus/Explicit and Abaqus/Standard; and

• the thick-walled formulation, where the hoop and radial stress vary through the cross-section, is available only in Abaqus/Standard.

The pipe elements are a specialized form of the corresponding beam elements that allow for internal and/or external pressure load specification and take the resulting hoop stress (as well as radial stress for thick-walled pipes) into account for the material constitutive calculations. Usage of the pipe elements is identical to that of the corresponding beam elements with respect to the section definition, boundary conditions at the element nodes, surface definitions, interactions such as tie constraints, etc.

## Using beam elements in dynamic and eigenfrequency analysis

The rotary inertia of a beam cross-section is usually insignificant for slender beam structures, except for twist around the beam axis. Therefore, Abaqus/Standard ignores rotary inertia of the cross-section for Euler-Bernoulli beam elements in bending. For thicker beams the rotary inertia plays a role in dynamic analysis, but to a lesser extent than shear deformation effects.

For Timoshenko beams the inertia properties are calculated from the cross-section geometry. The rotary inertia associated with torsional modes is different from that of flexural modes. For unsymmetric cross-sections the rotary inertia is different in each direction of bending. Abaqus allows you to choose the rotary inertia formulation for Timoshenko beams. When an approximate isotropic formulation is requested, the rotary inertia associated with the torsional mode is used for all rotational degrees of freedom in Abaqus/Standard, and a scaled flexural inertia with a scaling factor chosen to maximize the stable time increment is used for all rotational degrees of freedom in Abaqus/Explicit. The center of mass of the cross-section is taken to be located at the beam node. When the exact (anisotropic) formulation is requested, the rotary inertia associated with bending and torsion differ and the coupling between the translational and rotational degrees of freedom is included for beam cross-section definitions where the beam node is not located at the center of mass of the cross-section. For Timoshenko beams with the exact (default) rotary inertia formulation, you can define an additional mass and rotary inertia contribution to the beam's inertia response that does not add to its structural stiffness; see Adding inertia to the beam section behavior for Timoshenko beams.