<!-- source-page: 811 -->

# 32.3 Flexible joint elements

• “Flexible joint element,” Section 32.3.1   
• “Flexible joint element library,” Section 32.3.2

<!-- source-page: 812 -->

<!-- source-page: 813 -->

# 32.3.1 FLEXIBLE JOINT ELEMENT

Product: Abaqus/Standard

# References

• “Flexible joint element library,” Section 32.3.2   
• \*JOINT   
• \*DASHPOT   
• \*SPRING

# Overview

JOINTC elements:

• are used to model joint interactions; and   
• are made up of translational and rotational springs and parallel dashpots in a local, corotational coordinate system.

Details of the element formulation can be found in “Flexible joint element,” Section 3.9.6 of the Abaqus Theory Guide.

# Typical applications

The JOINTC element is provided to model the interaction between two nodes that are (almost) coincident geometrically and that represent a joint with internal stiffness and/or damping (such as a rubber bushing in a car suspension system) so that the second node of the joint can displace and rotate slightly with respect to the first node.

Joints that have only one or two axes of rotation and no relative displacement are better modeled by the REVOLUTE- or UNIVERSAL-type MPCs (see “General multi-point constraints,” Section 35.2.2).

Similar functionality is available using connectors; see “Connectors: overview,” Section 31.1.1.

# Defining the joint behavior

The joint behavior consists of linear or nonlinear springs and dashpots in parallel, coupling the corresponding components of relative displacement and of relative rotation in the joint. You define the spring and dashpot behavior as described in “Springs,” Section 32.1.1, and “Dashpots,” Section 32.2.1.

Each spring or dashpot definition defines the behavior for one of the six local directions; up to six spring and six dashpot definitions can be included. If no specification is given for a particular local relative motion in the joint, the joint is assumed to have no stiffness with respect to that component.

The joint behavior can be defined in a local coordinate system that rotates with the motion of the first node of the element (“Orientations,” Section 2.2.5). If a local coordinate system is not defined, the global system is used.

<!-- source-page: 814 -->

You must associate the joint behavior with a set of JOINTC elements.

The kinematic behavior of JOINTC elements is described in detail in “Flexible joint element,” Section 3.9.6 of the Abaqus Theory Guide.

Input File Usage: Use the following options to define the joint behavior:
*JOINT, ELSET=name, ORIENTATION=name
*DASHPOT
*SPRING
Up to six *SPRING and *DASHPOT options can appear.

# Using JOINTC elements in large-displacement analyses

In large-displacement analysis the formulation for the relationship between moments and rotations limits the usefulness of these elements to small relative rotations. The relative rotation across a JOINTC element should be of a magnitude to qualify as a small rotation.

<!-- source-page: 815 -->

# 32.3.2 FLEXIBLE JOINT ELEMENT LIBRARY

Product: Abaqus/Standard

References 

<table><tr><td>• “Flexible joint element,” Section 32.3.1</td></tr><tr><td>• *JOINT</td></tr></table>

Overview

This section provides a reference to the flexible joint elements available in Abaqus/Standard.

Element types

JOINTC Joint interaction element

Active degrees of freedom 1, 2, 3, 4, 5, 6

Additional solution variables None.

Nodal coordinates required

None. The element nodes do not need to have coordinates defined since the action associated with these elements is defined by specifying the degrees of freedom involved.

Element property definition

Input File Usage: \*JOINT

Element-based loading

None.

Element output 

<table><tr><td>S11</td><td>Total direct force in the first local direction.</td></tr><tr><td>S22</td><td>Total direct force in the second local direction.</td></tr><tr><td>S33</td><td>Total direct force in the third local direction.</td></tr><tr><td>S12</td><td>Total moment about the first local direction.</td></tr><tr><td>S13</td><td>Total moment about the second local direction.</td></tr><tr><td>S23</td><td>Total moment about the third local direction.</td></tr></table>

<!-- source-page: 816 -->

The relative displacements and rotations corresponding to the forces and moments above are chosen by requesting the corresponding “strains.”

# Nodes associated with the element

Two nodes. The rotation at the first node of the element defines the rotation of the local axis system.

![](images/page-816_c3bd42da5887123569edc223c9b612830eab7e3540e4fa715003e75f8fcc967a.jpg)

<details>
<summary>text_image</summary>

z'
y'
1
2
x'
JOINT C
</details>

( local system, defined by a local orientation, attached to node 1 )

<!-- source-page: 817 -->

# 32.4 Distributing coupling elements

• “Distributing coupling elements,” Section 32.4.1   
• “Distributing coupling element library,” Section 32.4.2

<!-- source-page: 818 -->

<!-- source-page: 819 -->

# 32.4.1 DISTRIBUTING COUPLING ELEMENTS

Product: Abaqus/Standard

# References

• “Distributing coupling element library,” Section 32.4.2   
• \*DISTRIBUTING COUPLING

# Overview

Distributing coupling elements:

• can be used to distribute forces and moments on a reference node to a collection of nodes;   
• can be used to prescribe an average displacement and rotation to a collection of nodes;   
• can control the force distribution through the use of weight factors specified for each coupling node;   
• can be used to create a flexible coupling between structural and solid elements; and   
• can be used with two- or three-dimensional stress/displacement elements.

The preferred method for defining a distributing constraint is described in “Coupling constraints,” Section 35.3.2.

# Typical applications

The distributing coupling element constrains the motion of the coupling nodes to the translation and rotation of the element node. This constraint is enforced in an average sense and in a way that enables control of the transmission of loads. These characteristics make the distributing coupling element useful in a number of applications:

• The element can be used to prescribe a displacement and rotation condition on a boundary in cases where relative motion among the nodes on the boundary is required. An example of such a case is prescribing a twist on the end of a structure that is expected to warp and/or deform within the end surface (see Figure 32.4.1–1).   
• The element can be used to provide, through the motion of the reference node, a weighted average of the motion of the coupling nodes.   
• The element can be used to distribute loads, where the load distribution can be described with moment-of-inertia expressions. Examples of such cases include the classic bolt-pattern and weldpattern load distribution expressions.   
• The element can be used as a coupling between two parts (structural-solid) to transfer forces and moments. In comparison to MPCs and the kinematic coupling constraint, the distributing coupling element can be considered a more “flexible” connection.

<!-- source-page: 820 -->

![](images/page-820_ee87cf40367b3dc50feafb510c44b2652c8364b06a3a64ea7dd365c145c63e6a.jpg)

<details>
<summary>text_image</summary>

z
y
x
DCOUP3D
element node
(NODE 1)
prescribed
rotation
warping is permitted
by the coupling element
Group of coupling
nodes (COUPLESET)
</details>

Figure 32.4.1–1 DCOUP3D element used to impart a rotation on the surface of a structure without constraining motion within the surface.

# Choosing an appropriate element

Two- and three-dimensional distributing coupling elements are available. Element DCOUP2D describes behavior only in the global X–Y plane. Element DCOUP2D can be used in an axisymmetric analysis; however, its use requires care in selecting the load distributing weight factors. For example, a uniform axial load distribution to a structure would require specification of load distribution weight factors in proportion to the radius of the coupling nodes. Since the radius of these nodes will change with deformation, this use of DCOUP2D would only approximate the correct load distribution behavior in a large-displacement analysis.

# Defining the distributing coupling

To define a distributing coupling, you specify the coupling nodes to which loads are to be distributed, along with the corresponding weighting of the distribution. A minimum of two coupling nodes is required.

Input File Usage: \*DISTRIBUTING COUPLING, ELSET=name node number or node set, weight\_factor\_1 node number or node set, weight\_factor\_2
