Defining tied contact in Abaqus/Standard

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 secondary surface to have the same value of displacement, temperature, pore pressure, or electrical potential as the point on the main surface that it contacts;
allows for rapid transitions in mesh density within the model;
requires a nondefault setting to control the treatment of small initial overclosures and gaps; and
cannot be used with self-contact or symmetric main-secondary contact.

It is often preferable to use the surface-based tie constraint capability instead of tied contact (see Mesh tie constraints for details).

This page discusses:

Defining tied contact for a contact pair
The tied contact formulation
Unconstrained nodes in tied contact pairs

Defining tied contact for a contact pair

To “tie” the surfaces of a contact pair together for an analysis, you must specify a nondefault control such that small initial overclosures (and optionally small initial gaps) are resolved by either adjusting the surface positions automatically or storing a contact offset distance per tied secondary node such that the initial penetration is zero. See Contact initialization for contact pairs in Abaqus/Standard for details on adjusting surfaces. As always, you must associate the contact pair with a contact interaction property definition.

Input File Usage

Use one of the following options to adjust surface positions as necessary for tied regions, where a is the threshold initial gap distance that is tied:

CONTACT PAIR, TIED, ADJUST=a or node_set_label, INTERACTION=name

CONTACT PAIR, TIED, ADJUST=YES, POSITION TOLERANCE=a, INTERACTION=name

Use the following option to store an offset distance (instead of adjusting surface positions) as necessary for tied regions, where a is the threshold initial gap distance that is tied:

CONTACT PAIR, TIED, ADJUST=NO, POSITION TOLERANCE=a, INTERACTION=name

Abaqus/CAE Usage

Interaction module: InteractionCreate: select a Secondary Node/Surface Adjustment option: toggle on Tie adjusted surfaces

Storing penetration offsets in the contact penetration calculations is not supported in Abaqus/CAE.

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 secondary nodes are within the adjustment zone (see Adjusting initial surface positions to resolve small initial gaps or overclosures), accounting for any shell or membrane thickness by default. Abaqus/Standard then either adjusts these secondary nodes' positions or determines a contact offset distance such that the revised initial penetration distance is zero. It forms constraints between these secondary nodes and the surrounding nodes on the main surface, using 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 About contact pairs in Abaqus/Standard and Assigning surface properties for contact pairs in Abaqus/Standard).

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). 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) 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 secondary nodes to the main surface unless they are precisely in contact with the main surface at the start of the analysis. Any secondary 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 main surface. In mechanical simulations an unconstrained secondary node can penetrate the main surface freely. In a thermal, electrical, or pore pressure simulation an unconstrained secondary node will not exchange heat, electrical current, or pore fluid with the main surface.

To avoid such unconstrained nodes in tied contact pairs, use the capability for adjusting the surfaces of a contact pair described in Contact initialization for contact pairs in Abaqus/Standard. This capability moves secondary nodes onto the main surface before Abaqus/Standard checks for the initial contact state. It is intended only for nodes that are close to the main surface and is not intended to correct large errors in the mesh geometry.

Checking that secondary nodes are constrained

Abaqus/Standard prints a table in the data (.dat) file identifying the predominant secondary node and other nodes involved in each constraint. If Abaqus/Standard cannot form a constraint for a given secondary node acting as a predominant secondary node, either because it is not in contact with the main surface or it cannot “see” the main surface, it will issue a warning message in the data file. For an explanation of when a secondary node would not “see” a main surface and how to correct this problem, see Contact formulations in Abaqus/Standard. 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.