Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
The surface-based coupling constraint:
couples the motion of a collection of nodes on a surface to the motion of a reference node;
is of type kinematic when the group of nodes is coupled to the rigid body motion defined by the reference node;
is of type distributing when the group of nodes can be constrained to the rigid body motion defined by a reference node in an average sense by allowing control over the transmission of forces through weight factors specified at the coupling nodes;
automatically selects the coupling nodes located on a surface lying within a region of influence;
can be used with two- or three-dimensional stress/displacement elements; and
can be used in geometrically linear and nonlinear analysis.
The surface-based coupling constraint in ABAQUS provides coupling between a reference node and a group of nodes referred to as the “coupling nodes.” This option provides the same functionality as the kinematic coupling constraint and the distributing coupling elements (DCOUP2D, DCOUP3D) in ABAQUS/Standard with a surface-based user interface. The coupling nodes are selected automatically by specifying a surface and an optional influence region. The procedure used to define the coupling nodes is discussed below.
For a distributing coupling constraint, the distributing weight factors are calculated automatically if the surface is an element-based surface. In such a case the weight factors are based on the tributary area at each coupling node, except for a surface along a shell edge, where the weight factors are based on the tributary edge length. Furthermore, the distributing weight factors can be modified using one of several weighting methods, which allow the forces transferred to the coupling nodes to vary inversely with the radial distance from the reference node.
The coupling constraint is useful when a group of coupling nodes is constrained to the rigid body motion of a single node. The coupling constraint can be employed effectively in the following applications:
To apply loads or boundary conditions to a model. Figure 20.3.2–1 illustrates the use of a kinematic coupling constraint to prescribe a twisting motion to a model without constraining the radial motion.
Figure 20.3.2–2 illustrates a distributing coupling constraint used to prescribe a displacement and rotation condition on a boundary where relative motion between the nodes on the boundary is required. In this example a twist is prescribed at the end of the structure that is expected to warp and/or deform within the end surface.To distribute loads on a model, where the load distribution can be described with a moment-of-inertia expression. Examples of such cases include the classic bolt-pattern and weld-pattern distribution expressions.
To apply dimensionality transitions between continuum and structural elements. For example, a distributing coupling allows flexible coupling between structural and solid elements.
To model end conditions. For example, modeling a rigid end plate or modeling plane sections of a solid to remain planar can be done easily with a kinematic coupling definition.
To simplify modeling of complex constraints. In a kinematic coupling definition the degrees of freedom that participate in the constraint may be selected individually in a local coordinate system.
To model interactions with other constraints, such as connector elements. For example, a hinged part may be modeled more realistically by two distributing coupling definitions, whose reference nodes are connected by a hinge connector element. The load transfer then occurs between two “clouds” of nodes, rather than between two single nodes. “Substructure analysis of a one-piston engine model,” Section 4.1.10 of the ABAQUS Example Problems Manual, illustrates this use of connector elements in conjunction with coupling constraints to model a one-piston engine.
Defining a coupling constraint requires the specification of the reference node (also called the constraint control point), the coupling nodes, and the constraint type. The coupling constraint associates the reference node with the coupling nodes. A name must be assigned to the constraint and may be used in postprocessing with ABAQUS/CAE. A node number or node set name may be specified for the reference node. If a node set is specified, the node set must contain exactly one node. The reference node for a kinematic coupling constraint has both translational and rotational degrees of freedom. The surface on which the coupling nodes are located can be node-based; element-based; or, in ABAQUS/Explicit, a combination of both surface types. You can specify an optional radius of influence that limits the coupling nodes to a specific region on the surface. Details on how coupling nodes are defined by specifying an influence region are discussed below.
The constraint type can be either kinematic or distributing, as discussed below.
| Input File Usage: | Use the following options: |
*COUPLING, CONSTRAINT NAME=name, REF NODE=n, SURFACE=surface *KINEMATIC or *DISTRIBUTING |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Coupling type: Kinematic or Distributing |
A reference node for a distributing coupling constraint can be used as the reference node only for a single distributing coupling constraint definition. In addition, the reference node cannot be used as the reference node in any distributing coupling element definition or mesh-independent spot weld definition, and it cannot be a shell node involved in a shell-to-solid coupling constraint.
By default, coupling nodes belonging to the entire surface are selected for the coupling definition. You can limit the coupling nodes to lie within a spherical region centered about the reference node by defining a radius of influence.
The procedure by which coupling nodes are selected for the constraint definition depends on the surface type:
For a node-based surface, all the nodes defined by the surface definition that fall within the influence region are selected for the coupling definitions.
For an element-based surface, the surface facets that are either fully or partially inscribed by the influence region are determined. All nodes belonging to these facets, whether or not these nodes fall within the influence region, are selected for the coupling nodes. When the influence radius is less than the distance to the closest coupling node, ABAQUS selects all nodes belonging to the closest facet. If the projection of the reference node on the surface falls on an edge or a vertex of multiple facets, all nodes belonging to these facets adjoining the edge or vertex are included in the coupling definition.
A distributing coupling constraint must include at least two coupling nodes. If fewer than two coupling nodes are found, ABAQUS issues an error message during input file preprocessing.
| Input File Usage: | *COUPLING, CONSTRAINT NAME=name, REF NODE=n, SURFACE=surface, INFLUENCE RADIUS=r |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Influence radius: Specify |
Kinematic coupling constrains the motion of the coupling nodes to the rigid body motion of the reference node. The constraint can be applied to user-specified degrees of freedom at the coupling nodes with respect to the global or a local coordinate system.
Kinematic constraints are imposed by eliminating degrees of freedom at the coupling nodes. In ABAQUS/Standard once any combination of displacement degrees of freedom at a coupling node is constrained, additional displacement constraints—such as MPCs, boundary conditions, or other kinematic coupling definitions—cannot be applied to any coupling node involved in a kinematic coupling constraint. The same limitation applies for rotational degrees of freedom. This restriction does not apply in ABAQUS/Explicit. See “Kinematic constraints: overview,” Section 20.1.1, for more information.
| Input File Usage: | Use both of the following options to define a kinematic coupling constraint: |
*COUPLING *KINEMATIC first dof, last dof For example, the following coupling constraint is used to constrain degrees of freedom 1, 2, and 6 on surface surfA to reference node 1000: *COUPLING, CONSTRAINT NAME=C1, REF NODE=1000, SURFACE=surfA *KINEMATIC 1, 2 6, |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Coupling type: Kinematic: toggle on the degrees of freedom |
Translational degrees of freedom are constrained by eliminating the specified degrees of freedom at the coupling nodes. When all translational degrees of freedom are specified, the coupling nodes follow the rigid body motion of the reference node.
Rotational degrees of freedom are constrained by eliminating the specified degrees of freedom at the coupling nodes.
All combinations of selected rotational degrees of freedom result in rotational behavior identical to existing MPC types:
Selection of three rotational degrees of freedom along with three displacement degrees of freedom is equivalent to MPC type BEAM.
Selection of two rotational degrees of freedom is equivalent to MPC type REVOLUTE in ABAQUS/Standard.
Selection of one rotational degree of freedom is equivalent to MPC type UNIVERSAL in ABAQUS/Standard.
In ABAQUS/Standard internal nodes are created by the kinematic coupling to enforce the constraints that are equivalent to MPC types REVOLUTE and UNIVERSAL. These nodes have the same degrees of freedom as the additional nodes used in these MPC types and are included in the residual check for nonlinear analysis.
The kinematic coupling constraint can be specified with respect to a local coordinate system instead of the global coordinate system (see “Orientations,” Section 2.2.5). Figure 20.3.2–1 illustrates the use of a local coordinate system to constrain all but the radial translation degrees of freedom of the coupling nodes to the reference node. In this example a local cylindrical coordinate system is defined that has its axis coincident with the structure's axis. The coupling node constraints are then specified in this local coordinate system.
| Input File Usage: | *COUPLING, ORIENTATION=local |
For example, the following input is used to specify the kinematic coupling constraint shown in Figure 20.3.2–1:*ORIENTATION, SYSTEM=CYLINDRICAL, NAME=COUPLEAXIS 0.0, -1.0, 0.0, 0.0, 1.0, 0.0 *COUPLING, REF NODE=500, SURFACE=Endcap, ORIENTATION=COUPLEAXIS *KINEMATIC 2, 3 |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Edit: select local coordinate system |
In geometrically nonlinear analysis steps the coordinate system in which the constrained degrees of freedom are specified will rotate with the reference node regardless of whether the constrained degrees of freedom are specified in the global coordinate system or in a local coordinate system.
Distributing coupling constrains the motion of the coupling nodes to the translation and rotation of the reference node. This constraint is enforced in an average sense in a way that enables control of the transmission of loads through weight factors at the coupling nodes. The constraint distributes loads such that the resultants of the forces at the coupling nodes are equivalent to the forces and moments at the reference node. Forces and moments at the reference node are distributed as a coupling node-force distribution only. For cases of more than a few coupling nodes, the distribution of forces is not determined by equilibrium alone, and distributing weight factors are used to define the force distribution. In the general case of transmission of forces and moments, the force distribution follows that of a classic bolt-pattern analysis, where the weight factors can be considered to be the areas of particular bolt cross-sections. For further details, see “Distributing coupling elements,” Section 3.9.8 of the ABAQUS Theory Manual.
The moment constraint between the rotation degrees of freedom at the reference node and the average rotation of the cloud nodes can be released in one direction in a two-dimensional analysis and one, two, or three directions in a three-dimensional analysis. In a three-dimensional analysis you can specify the moment constraint directions in the global coordinate system or in a local coordinate system. All available translational degrees of freedom at the reference node are always coupled to the average translation of the coupling nodes.
In a three-dimensional ABAQUS/Standard analysis if all three moment constraints are released by specifying only degrees of freedom 1–3, only translation degrees of freedom will be activated on the reference node. If only one or two rotation degrees of freedom have been released, all three rotation degrees of freedom are activated at the reference node. In this case you must ensure that proper constraints have been placed on the unconstrained rotation degrees of freedom to avoid numerical singularities. Most often this is accomplished by using boundary conditions or by attaching the reference node to an element such as a beam or shell that will provide rotational stiffness to the unconstrained rotation degrees of freedom.
| Input File Usage: | *DISTRIBUTING first dof, last dof |
| If no degrees of freedom are specified, all available degrees of freedom are coupled. If you specify one or more rotation degrees of freedom but not all available translation degrees of freedom, ABAQUS issues a warning message and adds all available translation degrees of freedom to the constraint. For example, the following coupling constraint is used to constrain degrees of freedom 1–5 on the reference node 1000 to the average translation and rotation of surface surfA: *COUPLING, CONSTRAINT NAME=C1, REF NODE=1000, SURFACE=surfA *DISTRIBUTING 1, 5 In this example the moment constraint between the reference node and the coupling nodes will be released in the 6-direction but will be enforced in the 4- and 5-directions. This provides a “revolute-like” rotation connection between the reference node and the coupling nodes (see “General multi-point constraints,” Section 20.2.2). |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Coupling type: Distributing: toggle on the rotational degrees of freedom (ABAQUS/CAE automatically constrains the translational degrees of freedom) |
User-defined weight factors are used for node-based surfaces. The cross-sectional areas specified in the surface definition are used as the weight factors (see “Defining node-based surfaces,” Section 2.3.3).
For element-based surfaces the weight factors are calculated by ABAQUS. The default weight distribution is based on the tributary surface area at each coupling node, except for a surface along a shell edge where the weight distribution is based on the tributary edge length. The procedure used to calculate the default weight factors is designed to ensure that if a radius of influence is prescribed, the default weight distribution varies smoothly with the influence radius.
The procedure to calculate the distributing weight factors depends on whether or not an influence radius is specified.
If no influence radius is specified, the entire surface is used in the coupling definition. In this case all nodes located on the surface are included in the coupling definition and the distributing weight factor at each coupling node is equal to the tributary surface area.
If an influence radius is specified, the default distributing weight factors at the coupling nodes are calculated as follows:
A “participation factor” is calculated for each surface facet. The participation factor is defined below.
The tributary nodal area (or tributary edge length along a shell edge) at each facet node is computed and is multiplied by the facet participation factor.
The coupling node distributing weight factor is computed as the sum of the corresponding facet nodal areas (calculated above) for all joining facets.
The participation factor defines the proportion of the facet's area that contributes to the distributing weight factors when an influence radius is specified. The participation factor varies between zero and one.
To define the participation factor, the distance of the facet node closest to the reference node, 
, and the distance of the facet node farthest from the reference node, 
, are calculated.
If 
, where 
is the influence radius, all facet nodes lie within the influence region; and a participation factor of one is used.
If 
, none of the facet nodes lie within the influence region; and the participation factor is set to zero.
If 
, the facet is partially inscribed in the influence region; and the facet is assigned a participation factor equal to 
.
for all facets), ABAQUS selects all nodes belonging to the closest facets (as outlined under “Specifying a region of influence”) and uses a participation factor equal to one.You can modify the default weight distribution defined above. Various weighting methods are provided that monotonically decrease with radial distance from the reference node. For each case the default weight distribution that is based on the tributary surface area (or tributary edge length along a shell edge) is scaled by the weight factor 
. If the weighting method is not specified, a uniform weighting method is used in which all weight factors are equal to 1.0.
A linearly decreasing weighting scheme
is the weight factor at coupling node 
, 
is the coupling node radial distance from the reference node, and 
is the distance to the furthest coupling node.| Input File Usage: | *DISTRIBUTING, WEIGHTING METHOD=LINEAR |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Coupling type: Distributing: Weighting method: Linear |
A quadratic polynomial weight distribution defined by
| Input File Usage: | *DISTRIBUTING, WEIGHTING METHOD=QUADRATIC |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Coupling type: Distributing: Weighting method: Quadratic |
A monotonically decreasing weight distribution according to the cubic polynomial
| Input File Usage: | *DISTRIBUTING, WEIGHTING METHOD=CUBIC |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Coupling type: Distributing: Weighting method: Cubic |
The distributing coupling constraint can be specified with respect to a local coordinate system instead of the global coordinate system (see “Orientations,” Section 2.2.5). Figure 20.3.2–2 illustrates the use of a local coordinate system to release the moment constraints between the reference node and the coupling nodes in the local 4- and 6-directions, providing a “universal-like” rotation connection. In this example a local rectangular coordinate system is defined that has its local 
-axis coincident with the global 
-axis. The moment constraint is specified in this local coordinate system.
| Input File Usage: | *COUPLING, ORIENTATION=local |
For example, the following input is used to specify the distributing coupling constraint shown in Figure 20.3.2–2:*ORIENTATION, SYSTEM=RECTANGULAR, NAME=COUPLEAXIS 0.0, 1.0, 0.0, 0.0, 0.0, 1.0 *COUPLING, REF NODE=500, SURFACE=Endcap, ORIENTATION=COUPLEAXIS *DISTRIBUTING 1, 3 5, 5 |
| ABAQUS/CAE Usage: | Interaction module: Create Constraint: Coupling: Edit: select local coordinate system |
In geometrically nonlinear analysis steps the coordinate system of the degrees of freedom that define the moment release rotates with the reference node regardless of whether the global coordinate system or a local coordinate system is used.
The distributing coupling constraint transmits moments at the reference node as a force distribution among the coupling nodes, even if these nodes have rotational degrees of freedom. Thus, when the coupling node arrangement is colinear, the constraint is not capable of transmitting all components of a moment at the reference node. Specifically, the moment component that is parallel to the colinear coupling node arrangement will not be transmitted. When this case arises, a warning message is issued that identifies the axis about which the element will not transmit a moment.
A distributing coupling constraint cannot be used with axisymmetric elements with asymmetric deformation. This element type is not compatible with the distributing coupling constraint.
A distributing coupling definition with a large number of coupling nodes produces a large wavefront in ABAQUS/Standard. This may result in significant memory usage and a long solution time to solve the finite element equilibrium equations.
