About Kinematic Constraints

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 independent 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 likely 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.

Abaqus/Explicit uses a penalty method to solve for constraints in certain situations. The penalties are weighted based on the masses of nodes participating in the constraint and the stable time increment. The penalty formulation attempts to satisfy the constraint approximately (i.e., a very small lack of compliance exists after imposition of the constraint). One situation in which the penalty approach is used to solve the constraint is when slave nodes of a tie constraint participate in other constraints such as multi-point constraints, kinematic coupling constraints, constraint equations, connector elements, rigid body constraints, or constraints due to boundary conditions. In this case the lack of compliance in the tie constraint is not carried across step boundaries; therefore, noisy accelerations and energy imbalance may be observed at step boundaries for certain problems. An alternative modeling approach (such as simply reversing the master and slave surfaces in the tie constraint) may switch to a different solution approach and thus resolve the above mentioned inaccuracies.

In Abaqus/Explicit when there are two or more overlapping distributed coupling constraints or overlapping distributed coupling and tie constraints, and the elements underlying the participating surfaces have very low densities, the lack of compliance may result in an inaccurate solution. Specifying reasonable density values for underlying elements may reduce the lack of compliance and improve solution accuracy.

Abaqus/Explicit always uses a geometrically nonlinear formulation for the enforcement of kinematic constraints. This is the case even when you have designated a particular analysis step as being geometrically linear. Consequently, results in these geometrically linear analyses could be hard to interpret, particularly when the loading in the model is high (displacements are large) and a geometrically nonlinear formulation should have been used.