Rigid Surface Contact Elements

Rigid surface contact elements:

  • can be used to model contact between a rigid surface and a deformable body;

  • are needed only for several special-purpose applications, such as when a substructure contacts a rigid surface or when CAXA or SAXA element types are involved in contact;

  • can be used in both geometrically linear and nonlinear simulations; and

  • use the same “main-secondary” concepts for enforcing contact constraints that are used in the surface-based contact capability in Abaqus/Standard.

For most problems the surface-based contact capability described in Defining Contact Interactions provides a more direct and general method for modeling contact between a rigid surface and a deformable body.

This page discusses:

See Also
Defining Contact Interactions
Axisymmetric Rigid Surface Contact Element Library
In Other Guides
Analytical Rigid Surface Definition
*INTERFACE
*RIGID SURFACE

ProductsAbaqus/Standard

Modeling Contact between Rigid Surfaces and Rigid Surface Contact Elements

Determining the location of the areas of contact and the surface tractions between contacting structures are common goals of Abaqus simulations. Rigid surface contact elements can be used to model contact when one of the structures is assumed to be rigid. These elements need to be used only for specific applications, outlined below, because the surface-based contact definitions in Abaqus can be used for most simulations.

Modeling Contact with Axisymmetric Rigid Surface Contact Elements

Axisymmetric rigid surface contact elements should be used only in the following specific applications:

Other planar, axisymmetric, or three-dimensional problems should use the surface-based contact capability.

Local Basis System for Contact Stress and Relative Motions of the Surfaces

Abaqus/Standard reports the contact stresses between the bodies and the relative motions of the bodies in a local basis system that is attached to the rigid surface. The normal n to the rigid surface, which is also the contact direction, is defined when the rigid surface is created. For details, see Analytical Rigid Surface Definition. In axisymmetric problems Abaqus/Standard defines the first local tangent to lie in the plane of the model and the second orthogonal to this plane.

The Main-Secondary Concept for Rigid Surface Contact Elements

Rigid surface contact elements use a “main-secondary” concept to enforce the contact constraints. The rigid surface contact elements form the “secondary” surface, and the nodes of these elements are constrained not to penetrate into the rigid (“main”) surface.

Defining the Rigid Surface

You define the analytical rigid surface using the methods described in Defining Analytical Rigid Surfaces When Drag Chain or Rigid Surface Elements Are Used.

Assigning a Rigid Body Reference Node to the Rigid Surface

The motion of a rigid surface is controlled by the motion of a single node, referred to as the rigid body reference node, that is associated with the rigid surface. When rigid surface contact elements are used in a model, the rigid body reference node is identified when defining the IRS elements (see below for details).

Defining the Rigid Surface Contact Elements

The rigid surface contact elements define the secondary surface. They also define the rigid body reference node for the rigid surface with which they interact. All IRS elements identify the rigid body reference node by including its node number as the last node in their connectivity. The nodes on the deformable body that form the IRS elements are always given first.

In a model defined in terms of an assembly of part instances, the rigid surface definition and the reference node must appear inside the same part definition as the rigid surface contact elements.

Example

For example, the following input would be used to define IRS elements 1 and 2 that consist of two nodes on the deformable body and assign node 1000 as the rigid body reference node: 

ELEMENT, TYPE=[IRS21A], ELSET=element_set_name
1, 10, 11, 1000
2, 11, 12, 1000
RIGID SURFACE, ELSET=element_set_name

A similar input structure is used for IRS22A elements.

Associating an Analytical Rigid Surface with a Set of Rigid Surface Contact Elements

You must identify the set of rigid surface contact elements that interact with a particular rigid surface.

Input File Usage

RIGID SURFACE, ELSET=element_set_name

Defining the Rigid Surface Element's Section Properties

You must associate the section properties with a set of rigid surface contact elements.

There are no section data for axisymmetric rigid surface contact elements.

Input File Usage

INTERFACE, ELSET=element_set_name

Defining Nondefault Mechanical Surface Interactions with Rigid Surface Contact Elements

By default, Abaqus/Standard uses a “hard,” frictionless mechanical surface interaction model with rigid surface contact elements. You can assign optional mechanical surface interaction models. The following mechanical surface interaction models are available: