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