General contact interactions allow you to define contact between many or all regions of the model with a single interaction. General contact is also used to define contact between Lagrangian bodies and Eulerian materials in a coupled Eulerian-Lagrangian analysis (see “Defining contact in Eulerian-Lagrangian models,” Section 27.3). Typically, general contact interactions are defined for an all-inclusive surface that contains all exterior faces and—in Abaqus/Explicit—analytical rigid surfaces, shell perimeter edges, edges based on beams and trusses, and Eulerian material boundaries. To refine the contact domain, you can include or exclude specific surface pairs (surface pairs cannot include Eulerian material boundaries). Surfaces used in general contact interactions can span many disconnected regions of the model. Attributes, such as contact properties, surface properties, and contact formulation, are assigned as part of the contact interaction definition but independently of the contact domain definition, which allows you to use one set of surfaces for the domain definition and another set of surfaces for the attribute assignments. For detailed instructions on creating this type of interaction, see “Defining general contact,” Section 15.13.1.

General contact interactions and surface-to-surface or self-contact interactions can be used together in the same analysis. Only one general contact interaction can be active in a step during an analysis.

For more information, see “Contact interaction analysis: overview,” Section 31.1.1 of the Abaqus Analysis User's Manual; “Defining general contact interactions in Abaqus/Standard,” Section 31.2.1 of the Abaqus Analysis User's Manual; “Defining general contact interactions in Abaqus/Explicit,” Section 31.4.1 of the Abaqus Analysis User's Manual; and “Eulerian analysis,” Section 13.1.1 of the Abaqus Analysis User's Manual. The assignment of a penalty stiffness scale factor is not supported in Abaqus/CAE. In addition, node-based surfaces cannot be used in a general contact interaction in Abaqus/CAE.

Surface-to-surface contact interactions describe contact between two deformable surfaces or between a deformable surface and a rigid surface. Self-contact interactions describe contact between different areas on a single surface. For detailed instructions on creating these types of interactions, see “Defining surface-to-surface contact,” Section 15.13.6; “Defining self-contact,” Section 15.13.7; and “Using contact and constraint detection,” Section 15.16. For more information, see “Defining contact pairs in Abaqus/Standard,” Section 31.3.1 of the Abaqus Analysis User's Manual, and “Defining contact pairs in Abaqus/Explicit,” Section 31.5.1 of the Abaqus Analysis User's Manual.

If your model includes complex geometries and numerous contact interactions, you may want to customize the variables that control the contact algorithms to obtain cost-effective solutions. These controls are intended for advanced users and should be used with great care. For more information, see “Contact controls editors,” Section 15.9.4.

Cyclic symmetry enables you to model an entire 360° structure at considerably reduced computational expense by analyzing only a single repetitive sector of a model. You can create cyclic symmetry interactions only in the initial step. Once a cyclic symmetry interaction is created, cyclic symmetry applies to the entire analysis history. If you deactivate a cyclic symmetry interaction in a frequency step, Abaqus/CAE evaluates all possible nodal diameters being evaluated for that step. For detailed instructions on creating this type of interaction, see “Defining cyclic symmetry,” Section 15.13.13. For more information about cyclic symmetry in Abaqus, see “Analysis of models that exhibit cyclic symmetry,” Section 10.4.3 of the Abaqus Analysis User's Manual.

Elastic foundations allow you to model the stiffness effects of a distributed support on a surface without actually modeling the details of the support. You can create elastic foundation interactions only in the initial step. Once an elastic foundation is activated, you cannot deactivate it in later analysis steps. For detailed instructions on creating this type of interaction, see “Defining foundations,” Section 15.13.14. For more information, see “Element foundations,” Section 2.2.2 of the Abaqus Analysis User's Manual.

Cavity radiation interactions describe heat transfer due to radiation in enclosures. Two cavity radiation models are available in Abaqus/CAE: a fully implicit definition and an approximation. The full version can be used for heat transfer without deformation in two-dimensional, three-dimensional, and axisymmetric models. It can include open or closed cavities and accounts for symmetries and surface blocking, but it does not support surface motion within cavities. For detailed instructions on creating this type of interaction, see “Defining a cavity radiation interaction,” Section 15.13.15.

The cavity radiation approximation is defined using a surface radiation interaction. You can approximate cavity radiation in any heat transfer analysis, with or without deformation. However, approximate cavity radiation can be used only for closed cavities in three-dimensional models. The approximation treats the cavity as a black body enclosure with a temperature equal to the average temperature of the entire surface. Under these limited conditions, approximate cavity radiation can save considerable computational expense. For detailed instructions on creating this type of interaction, see “Defining a surface radiative interaction,” Section 15.13.18.

For more information on both types of cavity radiation, see “Cavity radiation,” Section 36.1.1 of the Abaqus Analysis User's Manual.

Film condition interactions define heating or cooling due to convection by surrounding fluids. Two types of film condition interaction are available in Abaqus/CAE: surface film conditions define convection from model surfaces, and concentrated film conditions define convection from nodes or vertices. You can define film condition interactions only during a heat transfer, fully coupled thermal-stress, or coupled thermal-electrical step. For detailed instructions on defining these types of interactions, see “Defining a surface film condition interaction,” Section 15.13.16, and “Defining a concentrated film condition interaction,” Section 15.13.17, respectively. For more information, see “Thermal loads,” Section 29.4.4 of the Abaqus Analysis User's Manual.

Radiation interactions describe heat transfer to a nonreflecting environment due to radiation. Two types of radiation interactions are available in Abaqus/CAE: surface radiation interactions describe heat transfer with a nonconcave surface, and concentrated radiation interactions describe radiation from nodes or vertices. You can define radiation interactions only during a heat transfer, fully coupled thermal-stress, or coupled thermal-electrical step. For detailed instructions on creating these types of interactions, see “Defining a surface radiative interaction,” Section 15.13.18, and “Defining a concentrated radiative interaction,” Section 15.13.19, respectively. For more information, see “Thermal loads,” Section 29.4.4 of the Abaqus Analysis User's Manual.

For an Abaqus/Standard to Abaqus/Explicit co-simulation, you must specify the interface region (region for exchanging data) and coupling schemes (time incrementation process and frequency of data exchange) for the co-simulation. In each model, you create a Standard-Explicit co-simulation interaction to define the co-simulation behavior; only one Standard-Explicit co-simulation interaction can be active in a model. The settings in each co-simulation interaction must be the same in the Abaqus/Standard model and the Abaqus/Explicit model.

A Standard-Explicit co-simulation interaction can be created only in a general static, implicit dynamic, or explicit dynamic step. The interaction is valid only in the step in which it is created and is not propagated to subsequent steps. For detailed instructions on creating this type of interaction, see “Defining a Standard-Explicit co-simulation interaction,” Section 15.13.10. For more information, see “Performing an Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 14.1.3 of the Abaqus Analysis User's Manual.

Incident wave interactions model incident wave loading due to external acoustic wave sources. For detailed instructions on creating this type of interaction, see “Defining incident waves,” Section 15.13.12. For more information, see “Acoustic and shock loads,” Section 29.4.5 of the Abaqus Analysis User's Manual.

An acoustic impedance specifies the relationship between the pressure of an acoustic medium and the normal motion at an acoustic-structural interface. For detailed instructions on creating this type of interaction, see “Defining acoustic impedance,” Section 15.13.11. For more information, see “Acoustic and shock loads,” Section 29.4.5 of the Abaqus Analysis User's Manual.

An actuator/sensor interaction models a combination of sensors and actuators and, therefore, allows for modeling control system components. Currently, this type of interaction allows sensing and actuation at just one point. For detailed instructions on creating this type of interaction, see “Defining an actuator/sensor interaction,” Section 15.13.20.

The interaction definition and its optional associated property are used to define the basic aspects of the interaction, but the user must provide user subroutine UEL to supply the specific formulae for how actuation depends on sensor readings. You specify the name of the file containing the user subroutine when you create the analysis job in the Job module.

Actuator/sensor interactions are available only for Abaqus/Standard analyses. For more information, see “User subroutines and utilities,” Section 14.2 of the Abaqus Analysis User's Manual.