36.3.7 Defining tied contact in Abaqus/Standard
Products: Abaqus/Standard Abaqus/CAE
References
Overview
Tied contact in Abaqus/Standard:
ties two surfaces forming a contact pair together for the duration of a simulation;
can be used in mechanical, coupled temperature-displacement, coupled thermal-electrical-structural, coupled pore pressure-displacement, coupled thermal-electrical, or heat transfer simulations;
constrains each of the nodes on the slave surface to have the same value of displacement, temperature, pore pressure, or electrical potential as the point on the master surface that it contacts;
allows for rapid transitions in mesh density within the model;
requires the adjustment of the contact pair surfaces; and
cannot be used with self-contact or symmetric master-slave contact.
Defining tied contact for a contact pair
To “tie” the surfaces of a contact pair together for an analysis, you must also adjust the surfaces because, as described below, it is very important that the tied surfaces be precisely in contact at the start of the simulation. See “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 36.3.5, for details on adjusting surfaces. As always, you must associate the contact pair with a contact interaction property definition.
| Input File Usage: | *CONTACT PAIR, TIED, ADJUST=a or node_set_label, INTERACTION=name |
| Abaqus/CAE Usage: | Interaction module: Interaction |
The tied contact formulation
When a contact pair uses the tied contact formulation, Abaqus/Standard uses the undeformed configuration of the model to determine which slave nodes are within the adjustment zone (see “Adjusting the surfaces in a contact pair” in “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 36.3.5), accounting for any shell or membrane thickness by default. Abaqus/Standard then adjusts these slave nodes' positions into a zero-penetration state and forms constraints between these slave nodes and the surrounding nodes on the master surface. The constraints are formed with either a “surface-to-surface” or a “node-to-surface” approach, similar to small-sliding contact. The traditional node-to-surface approach is used by default for tied contact.
The user interface for selecting between the surface-to-surface and node-to-surface approaches and to avoid consideration of shell and membrane thickness for tied contact is the same as for small-sliding contact (see “Defining contact pairs in Abaqus/Standard,” Section 36.3.1, and “Assigning surface properties for contact pairs in Abaqus/Standard,” Section 36.3.2).
Use of tied contact in mechanical simulations
The tied contact formulation constrains only translational degrees of freedom in mechanical simulations. Abaqus/Standard places no constraints on the rotational degrees of freedom of structural elements involved in tied contact pairs.
Self-contact is not supported with tied contact. Self-contact is designed for finite-sliding situations in which it is not obvious from the original geometry which parts of the surface will come into contact during the deformation.
Mechanical constraints for tied contact are strictly enforced with a direct Lagrange multiplier method by default. Alternatively, you can specify that these constraints should be enforced with a penalty or augmented Lagrange constraint method (see “Contact constraint enforcement methods in Abaqus/Standard,” Section 38.1.2). The constraint enforcement method specified will be applied to the tangential constraints in addition to the normal constraints. Softened contact pressure-overclosure relationships (exponential, tabular, or linear—see “Contact pressure-overclosure relationships,” Section 37.1.2) are ignored for tied contact.
Use of tied contact in nonmechanical simulations
The tied contact capability can be used in models where the nodal degrees of freedom include electrical potential and/or temperature. Except for the nodal degree of freedom being constrained, Abaqus/Standard uses exactly the same formulation for tied contact in nonmechanical simulations as it does for mechanical simulations.
Unconstrained nodes in tied contact pairs
Abaqus/Standard does not constrain slave nodes to the master surface unless they are precisely in contact with the master surface at the start of the analysis. Any slave nodes not precisely in contact at the start of the analysis—e.g., either open or overclosed—will remain unconstrained for the duration of the simulation; they will never interact with the master surface. In mechanical simulations an unconstrained slave node can penetrate the master surface freely. In a thermal, electrical, or pore pressure simulation an unconstrained slave node will not exchange heat, electrical current, or pore fluid with the master surface.
To avoid such unconstrained nodes in tied contact pairs, use the capability for adjusting the surfaces of a contact pair described in “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 36.3.5. This capability moves slave nodes onto the master surface before Abaqus/Standard checks for the initial contact state. It is intended only for nodes that are close to the master surface and is not intended to correct large errors in the mesh geometry.
Checking that slave nodes are constrained
Abaqus/Standard prints a table in the data (.dat) file identifying the predominant slave node and other nodes involved in each constraint. If Abaqus/Standard cannot form a constraint for a given slave node acting as a predominant slave node, either because it is not in contact with the master surface or it cannot “see” the master surface, it will issue a warning message in the data file. For an explanation of when a slave node would not “see” a master surface and how to correct this problem, see “Contact formulations in Abaqus/Standard,” Section 38.1.1. When creating a model with tied contact, it is important to use this information provided by Abaqus/Standard to identify any unconstrained nodes and to make any necessary modifications to the model to constrain them.