Defining tied contact in Abaqus/Standard | ||
| ||
ProductsAbaqus/StandardAbaqus/CAE
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 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: : select a Slave Node/Surface Adjustment option: toggle on Tie adjusted surfaces
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), 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 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 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. 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. 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.