- 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 master and slave 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
Pressure penetration loading.
- 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.
- 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
(Abaqus/Standard
only)
-
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
User Subroutines and Utilities.