This section presents an overview of the contact analysis capabilities in ABAQUS. The contact modeling capabilities available in ABAQUS/Standard and ABAQUS/Explicit differ significantly; therefore, they are discussed separately. A comparison of the capabilities is provided at the end of this section.
There are two methods for modeling contact interactions in ABAQUS/Standard: using surfaces or using contact elements.
Most contact problems are modeled by using surface-based contact. The following types of problems can be simulated with surface-based contact:
Contact between two deformable bodies. The structures can be either two- or three-dimensional, and they can undergo either small or finite sliding. Examples of such problems include the assembly of a cylinder head gasket and the slipping between the two components of a threaded connector.
Contact between a rigid surface and a deformable body. The structures can be either two- or three-dimensional, and they can undergo either small or finite sliding. Examples of such problems include metal forming simulations and analyses of rubber seals being compressed between two components.
Finite-sliding self-contact of a single deformable body. An example of such a problem is a complex rubber seal that folds over on itself.
Small-sliding or finite-sliding interaction between a set of points and a rigid surface. These models can be either two- or three-dimensional. An example of this type of problem is the pull-in of an underwater cable that is resting on the seabed, with the seabed modeled as a rigid surface.
Contact between a set of points and a deformable surface. These models can be either two- or three-dimensional. An example of this class of contact problem is the design of a bearing where one of the bearing surfaces is modeled with substructures.
Problems where two separate surfaces need to be “tied” together so that there is no relative motion between them. This modeling technique allows for joining dissimilar meshes.
Coupled thermal-mechanical interaction between deformable bodies with finite relative motion. The analysis of a disc brake is an example of such a problem.
Coupled pore fluid-mechanical interaction between bodies. An example of this type of problem is the analysis of the interfaces between layered soil material at a waste disposal site.
There are three steps in defining a surface-based contact simulation in ABAQUS/Standard:
defining the surfaces of the bodies that could potentially be in contact;
specifying which surfaces interact with one another; and
defining the mechanical and thermal property models that govern the behavior of the surfaces when they are in contact.
Surfaces are considered part of the model definition, so all surfaces that may be needed in an analysis must be defined at the beginning of the simulation.
ABAQUS has three classifications of contact surfaces:
element-based deformable and rigid surfaces (“Defining element-based surfaces,” Section 2.3.2);
node-based surfaces (“Defining node-based surfaces,” Section 2.3.3); and
analytical rigid surfaces (“Defining analytical rigid surfaces,” Section 2.3.4).
Once surfaces have been created, you must specify which pairs of surfaces can interact with each other during the analysis. At least one surface of the pair must be a non-node-based surface. The definition of these contact pairs is discussed in detail in “Defining contact pairs in ABAQUS/Standard,” Section 21.2.1.
Some of the mechanical contact property models available in ABAQUS/Standard include:
softened contact (“Contact pressure-overclosure relationships,” Section 22.1.2),
friction (“Frictional behavior,” Section 22.1.4), and
user-defined constitutive models for surface interaction (“User-defined interfacial constitutive behavior,” Section 22.1.5).
Surface interaction in thermal or coupled thermal-mechanical contact simulations can include heat exchange by conduction and radiation as well as the generation of frictional heat in coupled simulations. These contact property models are discussed in “Thermal contact properties,” Section 22.2.1.
Surface interaction in coupled thermal-electrical problems includes flow of electrical current between the surfaces in addition to the thermal property models mentioned previously. The thermal-electrical property model is discussed in “Electrical contact properties,” Section 22.3.1.
The contact property model for pore fluid simulations is discussed in “Pore fluid contact properties,” Section 22.4.1. The model includes pore fluid flow that is both normal and tangential to the surfaces.
The surface-based contact method cannot be used for certain classes of problems. ABAQUS/Standard provides a library of contact elements for these problems. Examples of such problems are:
Contact interaction between two pipelines or tubes modeled with pipe, beam, or truss elements where one pipe lies inside the other (such as a J-tube pull in offshore piping installation) or the pipes lie next to each other (available in both two and three dimensions; see “Tube-to-tube contact elements,” Section 23.3.1).
Contact between two nodes along a fixed direction in space. An example of such a problem is the interaction of a piping system with its supports (see “Gap contact elements,” Section 23.2.1).
Simulations using axisymmetric elements with asymmetric deformations, CAXAn and SAXAn elements. See “Contact modeling if asymmetric-axisymmetric elements are present,” Section 21.2.8, for details.
Heat transfer analyses where the heat flow is one-dimensional. An example of such a problem is the heat flow in a piping system that is discontinuous. The thermal interaction in this problem is one-dimensional, so no surfaces can be defined (see “Gap contact elements,” Section 23.2.1).
The steps required for defining a contact simulation using contact elements are similar to those needed when defining a surface-based contact simulation:
create the contact elements or slide lines;
assign element section properties to the contact elements;
associate sets of contact elements with the slide lines if applicable; and
define the contact property models for the contact elements.
ABAQUS/Explicit provides two algorithms for modeling contact interactions. The general (“automatic”) contact algorithm allows very simple definitions of contact with very few restrictions on the types of surfaces involved (see “Defining general contact in ABAQUS/Explicit,” Section 21.3). The contact pair algorithm has more restrictions on the types of surfaces involved and often requires more careful definition of contact; however, it allows for some interaction behaviors that currently are not available with the general contact algorithm (see “Defining contact pairs in ABAQUS/Explicit,” Section 21.4).
The two contact algorithms combine to provide the following capabilities in ABAQUS/Explicit:
Contact between rigid and/or deformable bodies.
Contact of a body with itself.
Finite-sliding or small-sliding contact.
Contact with eroding bodies (due to element failure). A node-based surface must be used to model the eroding body if contact pairs are used. General contact allows element-based surfaces to be defined on eroding bodies, so contact between any number of eroding bodies can be modeled.
General constitutive models for the contact behavior, relating constraint pressure and shear traction to penetration distance and relative tangential motion.
Thermal interaction at the surface of a body; for example, conductive heat transfer.
Contact definitions are not entirely automatic with the general contact algorithm but are greatly simplified. The generality of this algorithm is primarily in the relaxed restrictions on the surfaces that can be used in contact. The general contact algorithm allows the following (none of which are allowed with the contact pair algorithm):
A surface can span unattached bodies.
More than two surface facets can share a common edge (allowing “T-intersections” in shells, for example).
A surface can include deformable and rigid regions; furthermore, the rigid regions need not be from the same rigid body.
A surface can have mixed parent element types; for example, adjacent surface facets can be on shell and solid elements.
A surface can be based on combinations of surfaces of the same type.
An element-based surface can be defined on the interior of solid bodies for use in modeling erosion due to element failure.
The general contact algorithm can enforce edge-to-edge contact for geometric feature edges, perimeter edges of structural elements, and edges defined by beam and truss elements, unlike the contact pair algorithm. However, modeling of edge-to-edge contact is not allowed for analyses conducted with multiple parallel domains.
The general contact algorithm eliminates problematic, nonphysical “bull-nose” extensions that may arise at shell surface perimeters in the contact pair algorithm.
With the general contact algorithm each slave node can see contact with multiple facets per increment; with the contact pair algorithm each slave node can see contact with only one facet per increment unless multiple surface pairings are specified. Likewise, each contact edge can see contact with multiple edges per increment when the general contact algorithm is used.
The general contact algorithm has some built-in smoothing for element-based surfaces that can be beneficial for modeling contact near corners.
The general contact algorithm, unlike the contact pair algorithm, removes contact faces and contact edges from the contact domain and, if an interior surface is defined, activates newly exposed surface faces as elements fail. Thus, element-based surfaces can be used to describe eroding solids. This allows contact between multiple eroding solids to be modeled since a node-based surface does not need to be defined on the eroding solid. However, an analysis conducted with multiple parallel domains will not allow the contact domain to include any faces whose parent elements may fail.
Contact state information (such as the proper contact normal orientation for double-sided surfaces) is transferred across step boundaries in the general contact algorithm even if the contact domain is modified; in the contact pair algorithm, contact state information is transferred across step boundaries only for contact pairs with no modifications.
The contact interaction domain, contact properties, and surface attributes are specified independently for the general contact algorithm, offering a more flexible way to add detail incrementally to a model.
The general contact algorithm has been developed to minimize the need for algorithmic controls.
Although the general contact algorithm is more powerful and allows for simpler contact definitions, the contact pair algorithm must be used in certain cases where more specialized contact features are desired. The following features are available only when the contact pair algorithm is used:
Two-dimensional surfaces
Analytical rigid surfaces
Kinematically enforced contact (see “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4; the general contact algorithm uses only penalty enforcement)
Small-sliding contact (see “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4)
Exponential and no separation contact pressure-overclosure models
A friction coefficient defined in terms of average surface temperature and/or field variables
User subroutines VFRIC and VUINTER
Breakable bonds, such as spot welds (however, mesh-independent non-breakable spot welds can be used with either contact algorithm; see “Mesh-independent fasteners,” Section 20.3.4)
Thermal contact
The two contact algorithms can be used together in the same ABAQUS/Explicit analysis. For example, contact involving analytical rigid surfaces can be modeled with the contact pair algorithm while the rest of the contact definition is modeled with the general contact algorithm. The general contact algorithm automatically avoids processing interactions that are treated by the contact pair algorithm.
A contact simulation using either algorithm in ABAQUS/Explicit is defined by specifying:
surface definitions for the bodies that could potentially be in contact;
the surfaces that interact with one another (the contact interactions);
any nondefault surface properties to be considered in the contact interactions;
the mechanical and thermal contact property models, such as the pressure-overclosure relationship or the contact conduction coefficient;
any nondefault aspects of the contact formulation; and
any algorithmic contact controls for the analysis.
Surfaces can be defined at the beginning of a simulation or upon restart as part of the model definition (see “Surfaces: overview,” Section 2.3.1). ABAQUS has three classifications of contact surfaces:
element-based deformable and rigid surfaces (“Defining element-based surfaces,” Section 2.3.2);
node-based deformable and rigid surfaces (“Defining node-based surfaces,” Section 2.3.3); and
analytical rigid surfaces (“Defining analytical rigid surfaces,” Section 2.3.4).
When the general contact algorithm is used, ABAQUS/Explicit also provides a default element-based surface that includes all bodies in the model.
Contact interactions for both contact algorithms are defined by specifying surface pairings and self-contact surfaces. General contact interactions typically are defined by specifying self-contact for the default surface, which allows an easy, yet powerful, definition of contact. (Self-contact for a surface that spans multiple bodies implies self-contact for each body as well as contact between the bodies.)
At least one surface in an interaction must be a non-node-based surface, and at least one surface in an interaction must be a non-analytical rigid surface.
The definition of general contact interactions, including further restrictions on the surfaces that can be used in them, is discussed in detail in “Defining general contact interactions,” Section 21.3.1. The definition of contact pairs, including further restrictions on the surfaces that can be used in them, is discussed in detail in “Defining contact pairs in ABAQUS/Explicit,” Section 21.4.1.
Nondefault surface properties (such as thickness and, in some cases, offset) can be defined for particular surfaces in a contact model. In addition, you can control which edges of a surface will be included in the general contact domain. The general contact algorithm uses the surface property assignments specified for contact purposes (see “Surface properties for general contact,” Section 21.3.2); the contact pair algorithm uses the surface properties specified in the surface definition (see “Surface properties for ABAQUS/Explicit contact pairs,” Section 21.4.2).
Contact interactions in a model can refer to a contact property definition, in much the same way that elements refer to an element property definition. By default, the surfaces interact (have constraints) only in the normal direction to resist penetration. The other mechanical contact interaction models available in ABAQUS/Explicit depend on the contact algorithm used (see “Mechanical contact properties: overview,” Section 22.1.1). Some of the available models are:
softened contact (“Contact pressure-overclosure relationships,” Section 22.1.2, and “Frictional behavior,” Section 22.1.4);
contact damping (“Contact damping,” Section 22.1.3, and “Frictional behavior,” Section 22.1.4);
friction (“Frictional behavior,” Section 22.1.4);
a user-defined constitutive model for surface interactions (“User-defined interfacial constitutive behavior,” Section 22.1.5); and
spot welds bonding two surfaces together until the welds fail (“Breakable bonds,” Section 22.1.8).
Contact interaction models are defined as model data for general contact analyses and as history data for contact pair analyses. Information on assigning contact properties to specific contact interactions can be found in “Contact properties for general contact,” Section 21.3.3, and “Contact properties for ABAQUS/Explicit contact pairs,” Section 21.4.3.
The contact formulation includes the constraint enforcement method, the contact surface weighting, and the sliding formulation. Nondefault aspects of the contact formulation can be specified for particular interactions in a contact model, depending on the contact algorithm chosen. See “Contact formulation for general contact,” Section 21.3.4, for details on the formulation used with general contact. See “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4, for details on the formulation used with the contact pair algorithm.
The default algorithmic controls for contact analyses are usually sufficient, but additional solution controls are available for some special cases. The available solution controls depend on the contact algorithm used. See “Contact controls for general contact,” Section 21.3.6, for information on nondefault algorithmic controls for general contact. See “Defining contact pairs in ABAQUS/Explicit,” Section 21.4.1, and “Common difficulties associated with contact modeling using the contact pair algorithm in ABAQUS/Explicit,” Section 21.4.6, for information on nondefault algorithmic controls for the contact pair algorithm.
There are fundamental differences in the mechanical contact algorithms in ABAQUS/Standard and ABAQUS/Explicit, even though the input syntax for ABAQUS/Standard and the contact pair algorithm in ABAQUS/Explicit are similar. These differences are reflected in how and where contact conditions are defined in the input file. The main differences are the following:
Contact constraints in ABAQUS/Standard are model definition data; however, in ABAQUS/Standard once contact pairs have been created, they can be removed (see “Removing/reactivating ABAQUS/Standard contact pairs,” Section 21.2.4) for a portion of the analysis and added back to the model in a later step of the analysis. In the contact pair algorithm in ABAQUS/Explicit contact constraints are history definition data (see “Defining a model in ABAQUS,” Section 1.3.1); in the general contact algorithm in ABAQUS/Explicit contact definitions can be either model or history data.
ABAQUS/Standard uses a strict master-slave weighting when enforcing contact constraints (see “Defining contact pairs in ABAQUS/Standard,” Section 21.2.1); the nodes of the slave surface are constrained not to penetrate into the master surface. The nodes of the master surface can, in principle, penetrate into the slave surface. ABAQUS/Explicit includes this formulation but typically uses a balanced master-slave weighting by default (see “Contact formulation for general contact,” Section 21.3.4, and “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4).
ABAQUS/Standard and ABAQUS/Explicit both provide a finite-sliding contact formulation (see “Contact formulation for ABAQUS/Standard contact pairs,” Section 21.2.2, and “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4). However, the two-dimensional finite-sliding contact formulation in ABAQUS/Standard requires that the master surfaces be smooth; whereas in ABAQUS/Explicit the master surfaces are faceted, except for analytical rigid surfaces, which can be smoothed.
ABAQUS/Standard and ABAQUS/Explicit both provide a small-sliding contact formulation (see “Contact formulation for ABAQUS/Standard contact pairs,” Section 21.2.2, and “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4). However, the small-sliding contact formulation in ABAQUS/Standard transfers the load to the master nodes according to the current position of the slave node. ABAQUS/Explicit always transfers the load through the anchor point. Furthermore, a surface-to-surface approach to this formulation, which typically provides more accurate contact stresses, is available only in ABAQUS/Standard.
ABAQUS/Explicit can account for the current thickness and midsurface offset of shells and membranes in the contact logic, whereas ABAQUS/Standard accounts for these effects only in the surface-to-surface small-sliding contact formulation.
Many benefits of the ABAQUS/Explicit general contact algorithm are not available in ABAQUS/Standard.