Available contact algorithms in AbaqusAbaqus provides more than one approach for defining contact. Abaqus/Standard includes the following approaches for defining contact:
Abaqus/Explicit includes the following approaches for defining contact:
Each approach has somewhat unique advantages and limitations. The remainder of this section is organized as follows:
Defining a surface-based contact simulationA contact simulation using contact pairs or general contact is defined by specifying:
In many cases you do not need to explicitly specify many of the aspects listed above because the default settings are usually appropriate. SurfacesSurfaces can be defined at the beginning of a simulation or upon restart as part of the model definition (see About surfaces). Abaqus has five classifications of contact surfaces:
Surfaces of the same type can be combined to create new surfaces (see Operating on surfaces). However, with regard to contact a combined surface can be used only with general contact in Abaqus/Explicit. When the general contact algorithm is used, Abaqus also provides a default all-inclusive, automatically defined surface that includes all element-based surface facets (in Abaqus/Standard and in Abaqus/Explicit), all crack surfaces for enriched elements (in Abaqus/Standard only), all analytical rigid surfaces (in Abaqus/Explicit only), and all Eulerian materials (in Abaqus/Explicit only) in the model. Contact interactionsContact interactions for contact pairs and general contact 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. Additional restrictions and guidelines for contact surfaces are discussed for each contact definition approach. The definition of contact pairs is discussed in detail in About contact pairs in Abaqus/Standard and About contact pairs in Abaqus/Explicit. The definition of general contact interactions is discussed in detail in About general contact in Abaqus/Standard and About general contact in Abaqus/Explicit. Surface propertiesNondefault 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 in Abaqus/Explicit. Surface properties for contact pairs are discussed in ,Assigning surface properties for contact pairs in Abaqus/Standard and Assigning surface properties for contact pairs in Abaqus/Explicit. Surface properties for general contact are discussed in Surface properties for general contact in Abaqus/Standard and Assigning surface properties for general contact in Abaqus/Explicit. Contact propertiesContact 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 depend on the contact algorithm and whether Abaqus/Standard or Abaqus/Explicit is used (see About mechanical contact properties). Some of the available models are:
The thermal, thermal-electrical, and pore-fluid surface interaction models available in Abaqus are discussed in Thermal contact properties, Electrical contact properties, and Pore fluid contact properties, respectively. Contact interaction models are defined as model data except for contact pairs in Abaqus/Explicit, in which case they are defined as history data. Information on assigning contact properties to contact pairs can be found in Assigning contact properties for contact pairs in Abaqus/Standard and Assigning contact properties for contact pairs in Abaqus/Explicit. Information on assigning contact properties to general contact interactions can be found in Contact properties for general contact in Abaqus/Standard and Assigning contact properties for general contact in Abaqus/Explicit. Numerical controlsThe default algorithmic controls for contact analyses are usually sufficient, but you can adjust numerical controls for some special cases. For example, depending on the contact algorithm used, the numerical controls for the contact formulation, the master and slave roles for the contact surfaces, and the sliding formulation are provided. Information on contact formulations and numerical methods used by the contact algorithms is provided in Contact formulations in Abaqus/Standard and Contact formulations for contact pairs in Abaqus/Explicit. The available numerical controls for the various contact algorithms are discussed in Numerical controls for general contact in Abaqus/Standard, Adjusting contact controls in Abaqus/Standard, Contact controls for general contact in Abaqus/Explicit, and Contact controls for contact pairs in Abaqus/Explicit. Contact simulation capabilities in Abaqus/StandardAbaqus/Standard provides the following approaches for defining contact interactions: general contact, contact pairs, and contact elements. Contact pairs and general contact both use surfaces to define contact; comparisons of these approaches are provided later in this section. Contact elements are provided for certain interactions that cannot be modeled with either general contact or contact pairs; however, it is generally recommended to use general contact or contact pairs if possible. Capabilities of contact pairs and general contact in Abaqus/StandardContact pairs and general contact combine to provide the following capabilities in Abaqus/Standard:
Coupled thermomechanical and coupled thermal-electrical-structural interactions can be included in any of the above examples as long as both of the surfaces are deformable. Choosing between general contact or contact pairs in Abaqus/StandardFor most contact problems you have a choice of whether to define contact interactions using general contact or contact pairs. In Abaqus/Standard the distinction between general contact and contact pairs lies primarily in the user interface, the default numerical settings, and the available options. The general contact and contact pair implementations share many underlying algorithms. The contact interaction domain, contact properties, and surface attributes are specified independently for general contact, offering a more flexible way to add detail incrementally to a model. The simple interface for specifying general contact allows for a highly automated contact definition; however, it is also possible to define contact with the general contact interface to mimic traditional contact pairs. Conversely, specifying self-contact of a surface spanning multiple bodies with the contact pair user interface (if the surface-to-surface formulation is used) mimics the highly automated approach often used for general contact. In Abaqus/Standard traditional pairwise specifications of contact interactions may result in more efficient analyses as compared to an all-inclusive self-contact approach to defining contact. Therefore, there is often a trade-off between ease of defining contact and analysis performance. Abaqus/CAE provides a contact detection tool that greatly simplifies the process of creating traditional contact pairs for Abaqus/Standard (see Understanding contact and constraint detection). Default settings for general contact and contact pairsDifferences in default settings for general contact and contact pairs in Abaqus/Standard include the following:
Capabilities available only for general contact in Abaqus/StandardThe following capabilities are available only for general contact in Abaqus/Standard (they are not available for contact pairs in Abaqus/Standard):
Contact involving crack surfaces for enriched elements is available only using general contact. Capabilities available only for contact pairs in Abaqus/StandardThe following capabilities are available only for contact pairs in Abaqus/Standard (they are not available for general contact in Abaqus/Standard):
A single analysis can include general contact and contact pair definitions. For example, you may choose to model contact interactions involving analytical rigid surfaces with contact pairs and other contact interactions with general contact. General contact automatically avoids processing contact interactions that are treated by contact pairs. Using contact elements in contact simulationsAbaqus/Standard provides a library of contact elements that can be used to model certain classes of problems. Examples of such problems are:
Defining a contact simulation using contact elementsThe steps required for defining a contact simulation using contact elements are similar to those needed when defining a surface-based contact simulation:
The first three steps are discussed in Contact Elements in Abaqus/Standard in the sections for each type of contact element. The contact property models for contact elements are identical to those used for surface-based contact. Contact simulation capabilities in Abaqus/ExplicitAbaqus/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). 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). The general contact and contact pairs algoirthms in Abaqus/Explicit differ by more than the user interface; in general they use completely separate implementations with many key differences in the designs of the numerical algorithms. The two contact algorithms combine to provide the following capabilities in Abaqus/Explicit:
Choosing between general contact or contact pairs in Abaqus/ExplicitContact 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 in Abaqus/Explicit allows the following (none of which are allowed with the contact pair algorithm in Abaqus/Explicit):
Other benefits of the general contact algorithm in Abaqus/Explicit include the following:
See Knee bolster impact with general contact, Crimp forming with general contact, and Collapse of a stack of blocks with general contact for example analyses that use the general contact algorithm. 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 in Abaqus/Explicit only when the contact pair algorithm is used:
In addition, the general contact algorithm in Abaqus/Explicit places more restrictions on adaptive meshing than the contact pair algorithm (see Defining ALE adaptive mesh domains in Abaqus/Explicit). The choice of contact algorithm may affect the speedup factor if loop-level parallelization is used: the contact pair algorithm includes some loop-level parallelization, while the general contact algorithm has no loop-level parallelization. Contact output is more complete for a contact pair analysis. The two contact algorithms can be used together in the same Abaqus/Explicit analysis. The general contact algorithm automatically avoids processing interactions that are treated by the contact pair algorithm. Compatibility between Abaqus/Standard and Abaqus/ExplicitThere are fundamental differences in the mechanical contact algorithms in Abaqus/Standard and Abaqus/Explicit even though the input syntax is similar. The main differences are the following:
As a result of these differences, contact definitions specified in an Abaqus/Standard analysis cannot be imported into an Abaqus/Explicit analysis and vice versa (see Transferring results between Abaqus/Explicit and Abaqus/Standard). However, in many cases you can successfully respecify a contact definition in an import analysis. |