Rigid elements

The rigid body capability in Abaqus allows most element types to be part of a rigid body. In addition, there exists an element type specifically designated as a rigid element. The rules governing rigid bodies, such as how loads and boundary conditions are applied, pertain to all element types that form the rigid body, including rigid elements.

The names of all rigid elements begin with the letter “R.” The next characters indicate the dimensionality of the element. For example, 2D indicates that the element is planar; and AX, that the element is axisymmetric. The final character represents the number of nodes in the element.

Rigid element library

The three-dimensional quadrilateral (R3D4) and triangular (R3D3) rigid elements are used to model the two-dimensional surfaces of a three-dimensional rigid body. Another element—a two-node, rigid beam element (RB3D2)—is provided in Abaqus/Standard mainly to model components of offshore structures to which fluid drag and buoyancy loads must be applied.

Two-node, rigid elements are available for plane strain, plane stress, and axisymmetric models. A planar, two-node rigid beam element is also available in Abaqus/Standard and is used mainly to model offshore structures in two dimensions.

Degrees of freedom

Only the rigid body reference node has independent degrees of freedom. For three-dimensional elements, the reference node has three translational and three rotational degrees of freedom; for planar and axisymmetric elements, the reference node has degrees of freedom 1, 2, and 6 (rotation about the 3-axis).

The nodes attached to rigid elements have only secondary degrees of freedom. The motion of these nodes is determined entirely by the motion of the rigid body reference node. For planar and three-dimensional rigid elements the only secondary degrees of freedom are translations. The rigid beam elements in Abaqus/Standard have the same secondary degrees of freedom as the corresponding deformable beam elements: 1–6 for the three-dimensional rigid beam and 1, 2, and 6 for the planar rigid beam.

Physical properties

All rigid elements must refer to a section property.

The following applies only to Abaqus/Explicit: For the planar and rigid beam elements the cross-sectional area can be defined. For the axisymmetric and three-dimensional elements the thickness can be defined. The default thickness is zero. These data are required only if you apply body forces to the rigid elements or when the thickness is needed for the contact definition.

Formulation and integration

Since the rigid elements are not deformable, they do not use numerical integration points, and there are no optional formulations.

Element output variables

There are no element output variables. The only output from rigid elements is the motion of the nodes. In addition, reaction forces and reaction moments are available at the rigid body reference node.