The following types of kinematic constraints can be defined:
Equations: Linear multi-point constraints can be given in the form of an equation (see “Linear constraint equations,” Section 20.2.1).
Multi-point constraints: Multi-point constraints (MPCs) specify linear or nonlinear constraints between nodes. These relations between nodes can be the default types that are provided in ABAQUS or, in ABAQUS/Standard, can be coded in the form of a user subroutine. “General multi-point constraints,” Section 20.2.2, explains the use of MPCs and lists the available default constraints.
Kinematic coupling: In ABAQUS/Standard a node or group of nodes can be constrained to a reference node. Similar to multi-point constraints, the kinematic coupling constraint allows general node-by-node specification of constrained degrees of freedom (see “Kinematic coupling constraints,” Section 20.2.3).
Surface-based tie constraints: Two surfaces can be tied together. Each node on the first surface (the slave surface) will have the same values for its degrees of freedom as the point on the second surface (the master surface) to which it is closest (see “Mesh tie constraints,” Section 20.3.1). In the case of surface elements tied to a beam surface, the offset distances between the surface elements and the beam are used in the definition of constraints, which include the rotational degrees of freedom of the beam.
Surface-based coupling constraints: A group of nodes located on a surface can be constrained to a reference node. This constraint may be kinematic, in which the group of coupling nodes can be constrained to the rigid body motion defined by the reference node, or distributing, in which the group of coupling nodes can be constrained to the rigid body motion defined by the reference node in an average sense (see “Coupling constraints,” Section 20.3.2).
Surface-based shell-to-solid coupling: An edge-based surface on a three-dimensional shell element mesh can be coupled to an element- or node-based surface on a three-dimensional solid mesh. The coupling is enforced by the creation of an internal set of distributing coupling constraints (see “Shell-to-solid coupling,” Section 20.3.3).
Mesh-independent spot welds: Two or more surfaces can be bonded together using fasteners such as spot welds (see “Mesh-independent fasteners,” Section 20.3.4). Distributed coupling constraints are created on each of the connected surfaces. The connection is modeled independent of the mesh.
Embedded elements: An element or a group of elements can be embedded in a group of host elements (see “Embedded elements,” Section 20.4.1). ABAQUS will search for the geometric relationships between nodes on the embedded elements and the host elements. If a node on an embedded element lies within a host element, the degrees of freedom at the node will be eliminated by constraining them to the interpolated values of the degrees of freedom of the host element. Host elements cannot be embedded themselves.
Release: In ABAQUS/Standard a local rotational degree of freedom or a combination of local rotational degrees of freedom can be released at one or both ends of a beam element (see “Element end release,” Section 20.5.1).
Boundary conditions are also a type of kinematic constraint in stress analysis because they define the support of the structure or give fixed displacements at nodal points. Specification of boundary conditions is discussed in “Boundary conditions,” Section 19.3.1.Connector elements can be used to impose element-based kinematic constraints for mechanism-type analysis. See “Connectors: overview,” Section 17.1.1.
Contact interactions, described in Part VIII, “Interactions,” can be used to enforce constraints between bodies that come into contact. Contact interactions can be used in mechanical as well as coupled thermal-mechanical and coupled pore fluid-mechanical analysis.
“Overconstraint checks,” Section 20.6.1, describes the overconstraint checks and the automatic resolution of some overconstraints performed in ABAQUS/Standard.
It is possible to use a single node in several multi-point constraints, kinematic coupling constraints, tie constraints, and constraint equations. However, the constraint dependencies are handled differently in ABAQUS/Standard and ABAQUS/Explicit.
In ABAQUS/Standard kinematic constraints are usually imposed by eliminating degrees of freedom at the dependent nodes. Once a variable has been eliminated, it cannot be referenced in any boundary condition or in any subsequent multi-point constraint, kinematic coupling constraint, tie constraint, or constraint equation. If you intend to use a variable that is eliminated in one constraint equation as the retained variable in another constraint equation, you must order the input so that the constraint equation in which the variable is eliminated follows the other constraint equations. MPC types BEAM, CYCLSYM, LINK, PIN, REVOLUTE, TIE, and UNIVERSAL, as well as the kinematic coupling and tie constraints, are sorted internally by ABAQUS/Standard to obtain a proper elimination order when possible.
Excessive chaining of multi-point constraints, kinematic coupling constraints, and constraint equations is not recommended and may result in a degradation in performance during analysis preprocessing. Whenever possible, it is best to relate the behavior of several nodes (grouped into a node set) to a single node by using one multi-point constraint, kinematic coupling constraint, or constraint equation.
Kinematic constraints in ABAQUS/Explicit can be defined in any order without regard to constraint dependencies. With the exception of constraints arising from kinematic contact pairs, ABAQUS/Explicit solves for all kinematic constraints simultaneously. Thus, nodes involved in a combination of multi-point constraints, constraint equations, connector element kinematic constraints, rigid body constraints, and constraints due to boundary conditions will simultaneously satisfy these constraints as long as they are not conflicting. Redundant and closed loop constraints are acceptable.
Since the above constraints are enforced independently of contact constraints, the penalty contact algorithm should be used for nodes involved in both kinematic constraints and contact pair definitions. The penalty contact algorithm introduces numerical softening through the use of penalty springs and does not interfere with kinematic constraints. If a node that participates in a kinematic constraint is used in a kinematic contact pair, the contact constraint will most often override the kinematic constraint. Except for rigid bodies, ABAQUS/Explicit will not prevent you from defining these conditions, but the results cannot be guaranteed. If a kinematic constraint is defined for a node on a rigid body, the penalty contact algorithm must be used for all contact pairs involving the rigid body.
To obtain accurate reaction force and moment output from ABAQUS/Explicit at nodes that are constrained by boundary conditions in addition to one or more of the kinematic constraints described above, it may sometimes be necessary to run the analysis in double precision. In such a situation a double precision run will also yield a better estimate of the work done by the reaction forces and moments, thereby providing a more accurate value of the energy due to the external work reported by ABAQUS/Explicit.