In ABAQUS/Explicit a rigid body is a collection of nodes and elements whose motion is governed by the motion of a single node, known as the rigid body reference node, as shown in Figure 4–7. The shape of the rigid body is defined either as an analytical rigid surface obtained by revolving or extruding a two-dimensional geometric profile or as a discrete rigid body obtained by meshing the body with nodes and elements. The shape of the rigid body does not change during a simulation but can undergo large rigid body motions. The mass and inertia of a discrete rigid body can be calculated based on the contributions from its elements, or they can be assigned specifically.
The motion of a rigid body can be prescribed by applying boundary conditions at the rigid body reference node. Loads on a rigid body are generated from concentrated loads applied to nodes and distributed loads applied to elements that are part of the rigid body or from loads applied to the rigid body reference node. Rigid bodies interact with the rest of the model through nodal connections to deformable elements and through contact with deformable elements.
In dynamic analyses rigid bodies can be used to model very stiff components that are either fixed or undergoing large dynamic motions. They can also be used to model constraints between deformable components, and they provide a convenient method of specifying certain contact interactions. When ABAQUS/Explicit is used for quasi-static forming analyses, rigid bodies are ideally suited for modeling tooling (such as punch, die, drawbead, blank holder, roller, etc.) and may also be effective as a method of constraint.
It may be useful to make parts of a model rigid for verification purposes. For example, in complex models where all potential contact conditions cannot be anticipated, elements far away from the impact region could be included as part of a rigid body, resulting in faster run times while developing a model. When the user is satisfied with the model and contact pair definitions, rigid body definitions can be removed and an accurate deformable finite element representation can be incorporated throughout.
The principal advantage to representing portions of a model with rigid bodies rather than deformable finite elements is computational efficiency. Element-level calculations are not performed for elements that are part of a discrete rigid body. Although some computational effort is required to update the motion of the nodes of the discrete rigid body and to assemble concentrated and distributed loads, the motion of the rigid body is determined completely by a maximum of six degrees of freedom at the rigid body reference node.
Rigid bodies are particularly effective for modeling relatively stiff parts of a model for which tracking waves and stress distributions is not important. Element stable time increment estimates in the stiff region can result in a very small global time increment. Since rigid bodies and elements that are part of a rigid body do not affect the global time increment, using a rigid body instead of a deformable finite element representation in a stiff region can result in a much larger global time increment, without significantly affecting the overall accuracy of the solution.
Rigid bodies defined with analytical rigid surfaces are slightly cheaper in terms of computational cost than discrete rigid bodies. Contact with analytical rigid surfaces tends to be less noisy than contact with discrete rigid bodies because analytical rigid surfaces can be smooth, whereas discrete rigid bodies are inherently faceted. However, the shapes that can be defined with analytical rigid surfaces are limited.
To create a discrete rigid body, use the *RIGID BODY option as the property reference for the elements forming the rigid body. Use the REF NODE parameter to assign a rigid body reference node to the rigid body. A rigid body reference node has both translational and rotational degrees of freedom and must be defined for every rigid body.
*RIGID BODY, REF NODE=<node>, ELSET=<element set name>, PIN NSET=<node set name>, TIE NSET=<node set name> <thickness>,
In addition to the rigid body reference node, discrete rigid bodies consist of a collection of nodes that are generated by assigning elements and nodes to the rigid body. These nodes provide a connection to other elements. Nodes that are part of a rigid body are one of two types:
Pin nodes, which have only translational degrees of freedom.
Tie nodes, which have both translational and rotational degrees of freedom.
The rigid body node type is determined by the type of elements on the rigid body to which the node is attached. The node type also can be specified or modified when assigning nodes directly to a rigid body. For pin nodes only the translational degrees of freedom are part of the rigid body, and the motion of these degrees of freedom is constrained by the motion of the rigid body reference node. For tie nodes both the translational and rotational degrees of freedom are part of the rigid body and are constrained by the motion of the rigid body reference node.
The rigid body capability in ABAQUS/Explicit allows any elements—not just rigid elements—to be part of a rigid body. For example, shell elements or rigid elements can be used to model the same effect if a *RIGID BODY option refers to the element set that contains the elements forming the rigid body. 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 can be used to model the two-dimensional surfaces of a three-dimensional rigid body.
Two-node rigid elements are available for plane strain and plane stress (R2D2) as well as axisymmetric models (RAX2).
Physical properties
All rigid elements must reference a *RIGID BODY option. For the planar and beam elements the cross-sectional area can be defined on the data line. For the axisymmetric and three-dimensional elements the thickness can be defined on the data line. The default thickness is zero. Alternatively, the NODAL THICKNESS parameter defines an average facet thickness based on the thickness at the nodes. These data are required when applying body forces or when the thickness is needed for the contact definition.
