Understanding interactions

You can use the Interaction module to define several types of interactions.

See Also
In Other Guides
Defining Contact Interactions

You can define the following types of interactions:

General contact

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). Typically, general contact interactions are defined for an all-inclusive surface that contains all exterior faces; feature edges; and—in Abaqus/Explicit—analytical rigid surfaces, edges based on beams and trusses, and Eulerian material boundaries. To refine the contact domain, you can include or exclude specific surface pairs. 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.

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 About Contact Interactions, About General Contact in Abaqus/Standard, About General Contact in Abaqus/Explicit, and Eulerian Analysis. 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, self-contact, and pressure penetration

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, Defining self-contact, and Using contact and constraint detection. For more information, see About Contact Pairs in Abaqus/Standard and About Contact Pairs in Abaqus/Explicit.

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.

A pressure penetration interaction allows you to simulate the pressure of a fluid penetrating between two surfaces involved in surface-to-surface contact. The fluid pressure is applied normal to the surfaces. You must create a surface-to-surface contact interaction to specify the main and secondary surfaces for the pressure penetration. The bodies forming the joint can both be deformable, as is the case with threaded connectors; or one can be rigid, as occurs when a soft gasket is used as a seal between stiffer structures. A pressure penetration interaction can be used only in an Abaqus/Standard analysis. For detailed instructions on creating pressure penetration interactions, see Defining pressure penetration. For more information, see Fluid Pressure Penetration Loads.

Fluid cavity

A fluid cavity interaction allows you to select and assign properties to a liquid- or gas-filled fluid cavity in the model. Fluid cavity selection includes a reference point and the surface that encloses the cavity. The properties are defined in a fluid cavity interaction property (for more information, see Understanding interaction properties). You can define fluid cavity interactions in the initial step of an Abaqus/Standard or an Abaqus/Explicit analysis. The fluid cavity interaction remains constant throughout all steps of an analysis; you cannot modify or deactivate it after the initial step. For detailed instructions on creating fluid cavity interactions, see Defining a fluid cavity interaction.

Fluid exchange

A fluid exchange interaction allows you to define movement of fluid between a cavity and the environment or between two cavities. To create a fluid exchange interaction, you must first select an existing fluid cavity interaction for each cavity (one for exchange to environment or two for exchange between cavities). Then you can select or create a fluid exchange interaction property (for more information, see Understanding interaction properties) and set the effective exchange area. For detailed instructions on creating fluid exchange interactions, see Defining a fluid exchange interaction.

Fluid inflator
A fluid inflator interaction allows you to inflate a fluid cavity to model the flow characteristics of inflators used for airbag systems. To create a fluid inflator interaction, you must first select an existing fluid cavity interaction. Then you can select or create a fluid inflator interaction property (for more information, see Understanding interaction properties). For detailed instructions on creating fluid inflator interactions, see Defining a fluid inflator interaction.
XFEM crack growth

An XFEM crack growth interaction allows you to activate or deactivate growth of a crack created using the extended finite element method. For detailed instructions on creating this type of interaction, see Deactivating and activating an XFEM crack growth.

Model change

A model change interaction allows you to remove and reactivate elements during an analysis. You can use model change interactions in all Abaqus/Standard analysis procedures except for the static, Riks procedure and linear perturbation procedures. For detailed instructions on creating this type of interaction, see Defining a model change interaction. For more information on removing and reactivating elements, see Element and Contact Pair Removal and Reactivation.

Cyclic symmetry

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. For more information about cyclic symmetry in Abaqus, see Analysis of Models that Exhibit Cyclic Symmetry.

Elastic foundation (Abaqus/Standard only)

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. For more information, see Element Foundations.

Cavity radiation (Abaqus/Standard only)

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.

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.

For more information on both types of cavity radiation, see Cavity Radiation in Abaqus/Standard.

Thermal film conditions

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, and Defining a concentrated film condition interaction, respectively. For more information, see Thermal Loads.

Radiation to and from the ambient environment

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, and Defining a concentrated radiative interaction, respectively. For more information, see Thermal Loads.

Abaqus/Standard to Abaqus/Explicit co-simulation

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. For more information, see Structural-to-Structural Co-Simulation.

Incident waves

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. For more information, see Acoustic and Shock Loads.

Acoustic impedance

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. For more information, see Acoustic and Shock Loads.

Actuator/sensor (Abaqus/Standard only)

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.

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.

Warning:

This feature is intended for advanced users only. Its use in all but the simplest test examples will require considerable coding by the user/developer. User-Defined Elements, should be read before proceeding.

Actuator/sensor interactions are available only for Abaqus/Standard analyses. For more information, see User Subroutines and Utilities.