Rigid surface contact elements | |||||||||
|
| ||||||||
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:
when the deformable surface is on a substructure (see Contact modeling if substructures are present), or
when CAXA or SAXA elements are involved in contact (see Contact modeling if asymmetric-axisymmetric elements are present).
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 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 master-slave concept for rigid surface contact elements
Rigid surface contact elements use a “master-slave” concept to enforce the contact constraints. The rigid surface contact elements form the “slave” surface, and the nodes of these elements are constrained not to penetrate into the rigid (“master”) 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 slave 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:
Friction. See Frictional behavior for details.
Modified “hard” contact, softened contact, and viscous damping. See Contact pressure-overclosure relationships and Contact damping for details.