Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
A linear multi-point constraint requires that a linear combination of nodal variables is equal to zero; that is, 
, where 
is a nodal variable at node 
, degree of freedom i; and the 
are coefficients that define the relative motion of the nodes.
In ABAQUS/Explicit linear constraint equations can be used only to constrain mechanical degrees of freedom.
A linear constraint equation is defined in ABAQUS by specifying:
the number of terms in the equation, 
;
the nodes, , and the degrees of freedom, i, corresponding to the nodal variables ; and
the coefficients, .
=3). =5, i=3, 
=1.0, 
=6, j=1, 
=–1.0, 
=1000, k=3, and 
=1.0.| Input File Usage: | *EQUATION |
For example, the following input could be used to define the equation constraint above:*EQUATION 3 5, 3, 1.0, 6, 1, -1.0, 1000, 3, 1.0 Either node sets or individual nodes can be specified as input. If node sets are used, corresponding set entries will be matched to each other. If sorted node sets are given as input, you must ensure that the nodes are numbered such that they will match up with each other correctly once sorted. The nodes in an unsorted node set will be used in the order that they are given in defining the set (see “Node definition,” Section 2.1.1). If the first entry is a single node, subsequent entries must be single nodes. If the first entry is a node set, subsequent entries can be either node sets or single nodes. The latter option is useful if a degree of freedom at each of a set of nodes depends on a degree of freedom of a single node, such as may occur in certain symmetry conditions or in the simulation of a rigid body. |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Equation |
| The nodes must be specified as sets. The first set can contain one or more points. If the first set contains one point, subsequent sets must contain only a single point. If the first set contains more than one point, subsequent sets can contain one or more points. |
In ABAQUS/Standard the first nodal variable specified ( corresponding to ) will be eliminated to impose the constraint (in the above equation constraint, degree of freedom 3 at node 5 will be eliminated); therefore, it should not be used to apply boundary conditions, nor should it be used in any subsequent multi-point constraint, kinematic coupling constraint, tie constraint, or equation constraint (see “Kinematic constraints: overview,” Section 20.1.1). This restriction does not apply in ABAQUS/Explicit.
In ABAQUS/Standard a linear multi-point constraint cannot be used to connect two rigid bodies at nodes other than the reference nodes, since multi-point constraints use degree-of-freedom elimination and the other nodes on a rigid body do not have independent degrees of freedom. In ABAQUS/Explicit a rigid body reference node or any other node on a rigid body can be used in an equation constraint definition.
Linear constraint equations lead to constraint forces at all degrees of freedom appearing in the equations. If you are checking the equilibrium of the model in ABAQUS/Standard, these constraint forces should be taken into account.
If a local coordinate system (“Transformed coordinate systems,” Section 2.1.5) is defined for any node involved in the equation, the variables at that node appear in the equation in the local system.
If an equation constraint is defined at the part (or part instance) level, the nodal variables are transformed initially according to the positioning data given for each instance of the part (see “Defining an assembly,” Section 2.9.1).
Note: Equation constraints cannot be defined at the part (or part instance) level in ABAQUS/CAE.
It is sometimes necessary to impose a constraint in the form
is a prescribed value that may vary with time, 
. This is easily done by rewriting the equation as
, that is not attached to any element in the model. Choosing 
to be some convenient degree of freedom 
at node allows the prescribed value to be imposed through a boundary condition specification. If necessary, an amplitude reference can be provided to give the variation with time (see “Boundary conditions,” Section 19.3.1); such an amplitude reference is required in ABAQUS/Explicit for prescribed displacements.For example, assume that node 1000 in the example above is a “dummy” node that appears only in this equation and is not attached to any other part of the model. Defining a boundary condition to constrain degree of freedom 3 at node 1000 to –12.5 would impose the constraint
The linear constraint generates constraint forces at all the degrees of freedom involved in the equation. For a given constraint equation these forces are proportional to their respective coefficients. To find the constraint forces, introduce a node that is not attached to any element in the model; rewrite the constraint equation as
of node . The reaction force obtained at node will be equal to the constraint force acting at node in degree of freedom 
. The constraint force in any term with coefficient 
in the constraint equation is obtained by multiplying the constraint force at node in degree of freedom with the ratio 
. For example, if the equation is 
is the opposite of the coefficient of 
, the constraint force at node 5 is the same as the reaction force at node 1000. Since the coefficient of 
is the same as the coefficient of , the constraint force at node 6 is the opposite of the reaction force at node 1000.Sometimes we may wish to impose an equation starting at a certain point in the analysis:
represents the change in displacement after time 
. The equation can be rewritten as 
is not attached to any element in the model. Prior to time (which is assumed to be at the end of a step), degree of freedom of node is left unrestrained. After time further changes in are restrained in ABAQUS/Standard by applying a boundary condition fixing the degree of freedom at its current values at the start of the step.The input for a linear constraint equation can be contained in a separate input file.
| Input File Usage: | *EQUATION, INPUT=file_name |
| If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line. |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Equation: click mouse button 3 while holding the cursor over the data table, and select Read from File |