김경종
8.4 KiB
40.5.1 RIGID SURFACE CONTACT ELEMENTS
Product: Abaqus/Standard
References
• “Axisymmetric rigid surface contact element library,” Section 40.5.2
• “Analytical rigid surface definition,” Section 2.3.4
• *INTERFACE
• *RIGID SURFACE
Overview
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 “master-slave” concepts for enforcing contact constraints that are used in the surfacebased contact capability in Abaqus/Standard.
For most problems the surface-based contact capability described in Chapter 36, “Defining Contact Interactions,” provides a more direct and general method for modeling contact between a rigid surface and a deformable body.
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,” Section 36.3.9), or
• when CAXA or SAXA elements are involved in contact (see “Contact modeling if asymmetricaxisymmetric elements are present,” Section 36.3.10).
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,” Section 2.3.4. 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” in “Analytical rigid surface definition,” Section 2.3.4.
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,” Section 37.1.5, for details.
• Modified “hard” contact, softened contact, and viscous damping. See “Contact pressure-overclosure relationships,” Section 37.1.2, and “Contact damping,” Section 37.1.3, for details.
40.5.2 AXISYMMETRIC RIGID SURFACE CONTACT ELEMENT LIBRARY
Product: Abaqus/Standard
References
• “Analytical rigid surface definition,” Section 2.3.4
• “Rigid surface contact elements,” Section 40.5.1
• *RIGID SURFACE
• *INTERFACE
Overview
This section provides a reference to the axisymmetric rigid surface contact elements available in Abaqus/Standard.
Element types
| IRS21A | Axisymmetric rigid surface contact element for use with first-order axisymmetric elements |
| IRS22A | Axisymmetric rigid surface contact element for use with second-order axisymmetric elements |
Active degrees of freedom
1, 2 at each node except the last node
1, 2, 6, the motion of the rigid body reference node, at the last node
Additional solution variables
Two additional variables at each node relating to the contact stresses.
Nodal coordinates required
r, z
Element property definition
Input File Usage: Use the following option to define the surface with which the elements interact: *RIGID SURFACE Use the following option to define the rigid surface element’s section properties: *INTERFACE
Element-based loading
| None. | |
| Element output | |
| S11 | Pressure between the element and the rigid surface in the direction of the normal to the rigid surface. |
| S12 | Shear component of the stress between the element and the rigid surface in the direction of the tangent to the rigid surface. |
| E11 | Separation of the surfaces in the direction of the normal to the rigid surface at the closest point of the surface to the integration point on the element. |
| E12 | Accumulated relative tangential displacement of the surfaces. |
| Node ordering on elements | |
The first two nodes in IRS21A and the first three nodes in IRS22A are on the deforming mesh. The last node is the rigid body reference node that defines the motion of the rigid body.
Numbering of integration points for output
The integration points are located at the nodes that lie on the surface of the deforming model and are numbered correspondingly.
41. Defining Cavity Radiation in Abaqus/Standard
Defining cavity radiation
41.1 Defining cavity radiation
• “Cavity radiation,” Section 41.1.1