Connector Behavior

Assigning a Connector Behavior to a Connector Element

You can assign the name of a connector behavior to particular connector elements.

Input File Usage

Use the following options to define the connector behavior:

CONNECTOR SECTION, ELSET=name, BEHAVIOR=behavior name
CONNECTOR BEHAVIOR, NAME=behavior name

Abaqus/CAE Usage

Interaction module: 
ConnectorSectionCreate: Name: connector section name: 
Behavior Options, Add
ConnectorAssignmentCreate: select wires: Section: connector section name

Connector Behavior Models

Connector behaviors allow for modeling of the following types of effects:

spring-like elastic behavior;
rigid-like elastic behavior;
dashpot-like (damping) behavior;
friction;
plasticity;
damage;
stops;
locks;
failure; and
uniaxial behavior.

Kinetic behavior can be specified only in available components of relative motion. The list of available components of relative motion for each connector type is given in Connection-Type Library. A connector behavior can be specified in any of the following ways:

uncoupled: the behavior is specified separately in individual available components of relative motion;
coupled: all or several of the available components of relative motion are used simultaneously in a coupled manner to define the behavior; or
combined: a combination of both uncoupled and coupled definitions are used simultaneously.

A conceptual model illustrating how connector behaviors interact with each other is shown in Figure 1. Most behaviors (elasticity, damping, stops, locks, friction) act in parallel. Plasticity models are always defined in conjunction with spring-like or rigid-like elasticity definitions. Degradation due to damage can be specified either for the elastic-plastic or rigid-plastic response alone or for the entire kinetic response in the connector. The failure behavior will apply to the entire connector response.

Multiple definitions for the same behavior type are permitted. For example, if connector elasticity (or damping) is defined several times in an uncoupled fashion for the same available component of relative motion, in a coupled fashion, or in both fashions, the spring-like (or dashpot-like) responses are added together. Multiple definitions of friction, plasticity, and damage behaviors are permitted as long as the rules outlined in the corresponding behavior sections are followed. Multiple uncoupled stop and lock definitions for the same component are permitted, but only one will be enforced at a time.

Defining Coupled and Uncoupled Connector Behavior

In many cases connector behavior is specified in an uncoupled manner in individual available components of relative motion. Coupled behavior can be defined for all or some of the available components of relative motion in a connector.

For coupled plasticity, damage, and, in certain situations, friction behavior, additional functions describing the nature of the coupling effects must be defined (see Connector Functions for Coupled Behavior). These functions do not define a behavior by themselves but are used as tools for building a desired behavior. For example, these functions may be used to define:

sophisticated yield functions in the connector force space for coupled plasticity behavior;
friction-generating contact forces for friction behavior; or
force or relative motion magnitude measures needed for damage behavior specifications.

Input File Usage

Use the following input to define uncoupled behavior:

*CONNECTOR BEHAVIOR OPTION, COMPONENT=n

Use the following input to define coupled behavior:

*CONNECTOR BEHAVIOR OPTION

Abaqus/CAE Usage

Interaction module: connector section editor: Addconnector behavior: Coupling: Uncoupled or Coupled

Defining Nonlinear Connector Behavior Properties to Depend on Relative Positions or Constitutive Displacements/Rotations

In all nonlinear uncoupled connector kinetic behaviors the independent variable is the connector available component in the direction for which the response is defined. When modeling the following connector behaviors, the properties can also depend on relative positions or constitutive displacements/rotations in several component directions:

connector elasticity,
connector damping,
connector derived components, and
connector friction.

When modeling connector uniaxial behavior, the properties can also depend on constitutive displacements/rotations in several component directions; see Connector Uniaxial Behavior for more information.

Input File Usage

Use the following option to specify that the connector behavior properties are dependent on components of relative position included in the behavior definition:

*CONNECTOR BEHAVIOR OPTION, 
INDEPENDENT COMPONENTS=POSITION (default)

Use the following option to specify that the connector behavior properties are dependent on components of constitutive relative displacements or rotations included in the behavior definition:

*CONNECTOR BEHAVIOR OPTION, 
INDEPENDENT COMPONENTS=CONSTITUTIVE MOTION

In either case the first data line identifies the independent component numbers to be used in determining the dependencies, and the additional data for the connector behavior definition begin on the second data line.

Abaqus/CAE Usage

For elasticity or damping behavior, use the following input to specify that connector behavior properties are dependent on relative position or constitutive relative displacements/rotations:

Interaction module: connector section editor: AddElasticity or Damping: Coupling: Coupled on position or Coupled on motion, select components and enter data

For connector derived components, use the following input to specify that connector behavior properties are dependent on relative position or constitutive relative displacements/rotations:

Interaction module: connector section editor: 
AddFriction, Plasticity, or Damage: Force Potential, Initiation
Potential, or Evolution Potential
Specify derived component, Use local directions: Independent
position components or Independent constitutive motion
components, select components and enter data

For friction behavior specifying internal contact forces, use the following input to specify that connector behavior properties are dependent on relative position or constitutive relative displacements/rotations:

Interaction module: connector section editor: AddFriction: Friction model: User-defined, Contact Force, Use independent components: Position or Motion, select components and enter data

Defining Reference Lengths and Angles for Constitutive Response

In many connector behavior definitions, material-like behavior has a reference position where the force or moment is zero, which is different from the initial position. This is the case, for example, in a spring that has nonzero force or moment in the initial configuration. In these situations the most convenient way to define the connector behavior is relative to the nominal or reference geometry where the forces or moments vanish.

You can define the translational or angular positions at which constitutive forces and moments are zero by specifying up to six reference values (one per component of relative motion): three lengths and three angles (in degrees). The reference lengths and angles affect only spring-like elastic connector behavior and, if the friction-generating contact force (moment) is a function of the relative displacement (rotation), connector friction behavior. By default, the reference lengths and angles are the length and angle values determined from the initial geometry. See Connection Types for the meaning of the reference lengths and angles for each connection type. Abaqus will not account for the energy stored as a result of precompressed or preextended behavior.

Input File Usage

CONNECTOR CONSTITUTIVE REFERENCE
length 1, length 2, length 3, angle 1, angle 2, angle 3

Abaqus/CAE Usage

Interaction module: connector section editor: AddReference Length: Length associated with CORM

Defining Precompressed or Preextended Linear Elastic Behavior

In many cases connectors are precompressed or preextended when installed in assemblies. In such cases the connector force is nonzero in the initial configuration. While nonlinear elasticity could be used to define nonzero force in the initial configuration, it is often more convenient to specify a (linear) spring stiffness plus a reference length or angle at which the force or moment is zero. For example, linear uncoupled elastic behavior defined with the connection type AXIAL would have force given by the equation

F_{1} = D_{11} u_{1}^{m a t},

where $u_{1}^{m a t} = l - l_{1}^{r e f}$ . $l$ is the current length of the AXIAL connection, and $l_{1}^{r e f}$ is the user-defined constitutive reference length. The connector constitutive displacement quantities, $u_{j}^{m a t}$ , are defined for different connection types as described in Connection Types.

Example

An input file template for a connector model of the shock absorber in Figure 2 is presented in About Connectors. A reference angle of 22.5° is defined for the nonlinear torsional spring as the fourth data item (corresponding to the connector's fourth component of relative motion) in the connector constitutive reference:

CONNECTOR BEHAVIOR, NAME=sbehavior
...
CONNECTOR CONSTITUTIVE REFERENCE
 , , , 22.5

The effect of this reference angle is that the nonlinear torsional spring has a zero moment at an angle of 22.5°.

Defining the Time Integration Method for Constitutive Response in Abaqus/Explicit

In Abaqus/Explicit kinematic constraints, stops, locks, and actuated motion in connector elements are treated with implicit time integration. By default, connector constitutive behavior (for example, elasticity, damping, and friction) is also integrated implicitly. The advantage of implicit time integration is that elements with these behaviors do not affect the stability or time incrementation of the analysis in any way.

When “soft” springs are modeled with connectors, a more traditional explicit time integration for the constitutive response can be used. This explicit time integration may lead to a small improvement in computational performance. However, explicit integration of relatively stiff springs will reduce the global time increment size, since such connector elements are included in the stable time increment size calculation.

Input File Usage

Use the following option to specify implicit integration of the constitutive response:

CONNECTOR BEHAVIOR, INTEGRATION=IMPLICIT

Use the following option to specify explicit integration of the constitutive response:

CONNECTOR BEHAVIOR, INTEGRATION=EXPLICIT

Abaqus/CAE Usage

Interaction module: connector section editor: AddIntegration: Integration: Implicit or Explicit

Defining Connector Behavior in Linear Perturbation Procedures

In linear perturbation procedures (see General and Perturbation Procedures) the connector element kinematics are linearized about the base state. Hence, linearized versions of kinematic constraints are applied, and the connector behavior is linearized about the state at the end of the previous general analysis step.

Using Several Connectors in Series or in Parallel

Connector element behaviors allow for proper modeling of most physical connection behaviors within a single connector element. However, in rare circumstances more complex connection behaviors may require multiple connector elements to be used in parallel or in series. You place connector elements in parallel by defining two or more connector elements between the same nodes. You place connectors in series by specifying additional nodes (most often in the same location as the nodes of interest) and then stringing connector elements between these nodes.

For example, assume that you would like to define a connector stop that exhibits elastic-plastic behavior upon contact. Since this is not permitted within the context of one connector behavior definition, you can circumvent the limitation by using two connector elements in series. This concept is illustrated in Figure 3. The first connector defines the stop, and the second defines the elastic-plastic behavior. Since both elements are subject to the same load (because they are in series), the desired behavior is obtained.

Connectors in parallel can be used as well to model complex kinetic behavior. For example, assume that you need to define an elastic-viscous connector with spring-like and dashpot-like behaviors in parallel (for example, the strut in an automotive suspension). Assume that damage can occur only in the dashpot once it is stretched/compressed beyond specified limits. Since this is not permitted within the context of one connector behavior definition, you can circumvent the limitation by using two connector elements in parallel. This concept is illustrated in Figure 4.

The first connector defines the elastic behavior, and the second defines the dashpot behavior. Since the two connector elements are in parallel, they undergo the same motion (stretching/compression). A motion-based damage behavior (see Connector Damage Behavior) can be used to degrade the entire behavior in the second element. Thus, only the dashpot behavior will eventually degrade.

Defining Connector Behavior Using Tabular Data

Tabular data are often used to define connector behaviors, such as nonlinear elasticity, isotropic hardening, etc. As shown in Figure 5, the data points make up a nonlinear curve in the constitutive space.

The options to define table lookups are described below.

Extrapolation Options

By default, the dependent variables are extrapolated as a constant (with a value corresponding to the endpoints of the curve) outside the specified range of the independent variables. This choice may cause a zero stiffness response, which may lead to convergence problems. You can specify linear extrapolation to extrapolate the dependent variables outside the specified range of the independent variables assuming that the slope given by the end points of the curve remains constant. The extrapolation behavior is illustrated in Figure 5.

You define the extrapolation choice globally for all connector behaviors but can redefine the extrapolation choice for the following connector behaviors individually:

connector elasticity;
connector plasticity (connector hardening);
connector damping;
derived components for connector elements;
connector friction;
connector damage (connector damage initiation and evolution);
connector locks; and
connector uniaxial behavior.

Tabular data for connector stop and lock behavior options are not supported in Abaqus/CAE.

Specifying Constant Extrapolation for All Connector Behaviors

You can specify constant extrapolation for tabular data for all connector behaviors.

Input File Usage

CONNECTOR BEHAVIOR, EXTRAPOLATION=CONSTANT (default)

Abaqus/CAE Usage

Interaction module: connector section editor: Table Options tabbed page: Extrapolation: Constant

Specifying Linear Extrapolation for All Connector Behaviors

You can specify linear extrapolation for tabular data for all connector behaviors.

Input File Usage

CONNECTOR BEHAVIOR, EXTRAPOLATION=LINEAR

Abaqus/CAE Usage

Interaction module: connector section editor: Table Options tabbed page: Extrapolation: Linear

Redefining the Extrapolation Choice for Individual Connector Behaviors

You can redefine the extrapolation choice for individual connector behaviors.

Input File Usage

Use either of the following options:

*CONNECTOR BEHAVIOR OPTION, EXTRAPOLATION=CONSTANT

*CONNECTOR BEHAVIOR OPTION, EXTRAPOLATION=LINEAR

For example, use the following options to use constant extrapolation for all connector behaviors except for connector elasticity:

CONNECTOR BEHAVIOR, EXTRAPOLATION=CONSTANT

CONNECTOR ELASTICITY, EXTRAPOLATION=LINEAR

Abaqus/CAE Usage

Use the following input for elasticity, damping, friction, plasticity, and damage behaviors:

Interaction module: connector section editor: Behavior Options tabbed page: Table Options button: Extrapolation: toggle off Use behavior settings and choose Constant or Linear

Use the following input for connector derived components:

Interaction module: derived component editor: Add: Table Options button: Extrapolation: toggle off Use behavior settings and choose Constant or Linear

Regularization Options for Abaqus/Explicit

By default, Abaqus/Explicit regularizes the data into tables that are defined in terms of even intervals of the independent variables since table lookups are most economical if the interpolation is from even intervals of the independent variables. In some cases, where it is necessary to capture sharp changes in connector behavior accurately, you can use the user-defined tabular connector behavior data directly by turning regularization off. However, the table lookups will be more computationally expensive compared to using regular intervals. Therefore, the use of regularization is almost always recommended.

Abaqus/Explicit uses an error tolerance to regularize the input data. The number of intervals in the range of each independent variable is chosen such that the error between the piecewise linear regularized data and each of your defined points is less than the tolerance times the range of the dependent variable. The default tolerance is 0.03. In some cases where the dependent quantities are defined at uneven intervals of the independent variables and the range of the independent variable is large compared to the smallest interval, Abaqus/Explicit may fail to obtain an accurate regularization of your data in a reasonable number of intervals. In this case Abaqus/Explicit stops after all data are processed and issues an error message that you must redefine the behavior data. See Material Data Definition for a more detailed discussion of data regularization.

You define the choice of regularization and regularization tolerance globally for all connector behaviors but can redefine the choice of regularization and regularization tolerance for the following connector behaviors individually:

connector elasticity;
connector plasticity (connector hardening)
connector damping;
derived components for connector elements;
connector friction;
connector damage (connector damage initiation and evolution);
connector locks; and
connector uniaxial behavior.

Tabular data for connector stop and lock behavior options are not supported in Abaqus/CAE.

Specifying the Regularization of User-Defined Tabular Data for All Connector Behaviors

You can specify regularization of tabular data and a regularization tolerance to be used globally for all connector behaviors.

Input File Usage

CONNECTOR BEHAVIOR, REGULARIZE=ON (default), 
RTOL=tolerance

Abaqus/CAE Usage

Interaction module: connector section editor: Table Options tabbed page: Regularization: toggle on Regularize data (Explicit only), Specify: tolerance

Specifying the Use of User-Defined Tabular Data without Regularization for All Connector Behaviors

You can specify the use of user-defined tabular data directly by turning regularization off for all connector behaviors.

Input File Usage

CONNECTOR BEHAVIOR, REGULARIZE=OFF

Abaqus/CAE Usage

Interaction module: connector section editor: Table Options tabbed page: Regularization: toggle off Regularize data (Explicit only)

Redefining the Regularization Options for Individual Connector Behaviors

You can redefine the choice of regularization and regularization tolerance for individual connector behaviors.

Input File Usage

Use either of the following options:

*CONNECTOR BEHAVIOR OPTION, REGULARIZE=ON, RTOL=tolerance

*CONNECTOR BEHAVIOR OPTION, REGULARIZE=OFF

For example, use the following options to regularize the user-defined data for all connector behaviors except for connector elasticity:

CONNECTOR BEHAVIOR, REGULARIZE=ON, RTOL=0.05

CONNECTOR ELASTICITY, REGULARIZE=OFF

Abaqus/CAE Usage

Use the following input for elasticity, damping, friction, plasticity, and damage behaviors:

Interaction module: connector section editor: Behavior Options tabbed page: Table Options button: Regularization: toggle off Use behavior settings; toggle on Regularize data (Explicit only) and Specify: tolerance, or toggle off Regularize data (Explicit only)

Use the following input for connector derived components:

Interaction module: derived component editor: Add: Table Options button: Regularization: toggle off Use behavior settings; toggle on Regularize data (Explicit only) and Specify: tolerance, or toggle off Regularize data (Explicit only)

Evaluation of Rate-Dependent Data

Data for the tabulated isotropic hardening in connector plasticity (Defining the Isotropic Hardening Component by Specifying Tabular Data) and plastic motion–based damage initiation criterion (Plastic Motion–Based Damage Initiation Criterion) can be specified as dependent on the equivalent relative plastic motion rate. Loading/unloading data for the rate-dependent connector uniaxial behavior model can be specified as dependent on the rate of deformation.

Specifying Linear Intervals for Interpolation of Rate-Dependent Data

By default, both Abaqus/Standard and Abaqus/Explicit interpolate rate-dependent data using linear intervals of the relative motion rate.

Input File Usage

Use the following option to specify linear interpolation for isotropic hardening data:

CONNECTOR HARDENING, RATE INTERPOLATION=LINEAR

Use the following option to specify linear interpolation for damage initiation data:

CONNECTOR DAMAGE INITIATION, RATE INTERPOLATION=
LINEAR

Use both of the following options to specify linear interpolation for uniaxial behavior loading/unloading data:

CONNECTOR UNIAXIAL BEHAVIOR
LOADING DATA, RATE INTERPOLATION=LINEAR

Abaqus/Standard always interpolates rate-dependent data using linear intervals of the equivalent relative plastic motion rate.

Abaqus/CAE Usage

Use the following input for isotropic hardening data:

Interaction module: connector section editor: AddPlasticity: Isotropic Hardening: Definition: Tabular, Table Options button: Interpolation: Linear

Use the following input for damage initiation data:

Interaction module: connector section editor: AddDamage: Initiation: Table Options button: Interpolation: Linear

Connector uniaxial behavior cannot be defined in Abaqus/CAE.

Specifying Logarithmic Intervals for Interpolation of Rate-Dependent Data in Abaqus/Explicit

In Abaqus/Explicit you can specify that logarithmic intervals of the relative motion rate be used for the interpolation of rate-dependent data if the rate dependence of the data is measured at logarithmic intervals.

Input File Usage

Use the following option to specify linear interpolation for isotropic hardening data:

CONNECTOR HARDENING, RATE INTERPOLATION=LOGARITHMIC

Use the following option to specify linear interpolation for damage initiation data:

CONNECTOR DAMAGE INITIATION, RATE INTERPOLATION=LOGARITHMIC

Use both of the following options to specify linear interpolation for uniaxial behavior loading/unloading data:

CONNECTOR UNIAXIAL BEHAVIOR
LOADING DATA, RATE INTERPOLATION=LOGARITHMIC

Abaqus/CAE Usage

Use the following input for isotropic hardening data:

Interaction module: connector section editor: AddPlasticity: Isotropic Hardening: Definition: Tabular, Table Options button: Interpolation: Logarithmic

Use the following input for damage initiation data:

Interaction module: connector section editor: AddDamage: Initiation: Table Options button: Interpolation: Logarithmic

Connector uniaxial behavior cannot be defined in Abaqus/CAE.

Filtering the Equivalent Plastic Motion Rate in Abaqus/Explicit

Rate-sensitive connector constitutive behavior may introduce nonphysical high-frequency oscillations in an explicit dynamic analysis. To overcome this problem, Abaqus/Explicit uses a filtered equivalent plastic motion rate

{{\dot{\bar{u}}}^{p l} |}_{t + Δ t} = ω \frac{Δ {\bar{u}}^{p l}}{Δ t} + (1 - ω) {{\dot{\bar{u}}}^{p l} |}_{t}

for the evaluation of rate-dependent data. $Δ {\bar{u}}^{p l}$ is the incremental change in equivalent plastic motion during the time increment $Δ t$ , and ${{\dot{\bar{u}}}^{p l} |}_{t}$ and ${{\dot{\bar{u}}}^{p l} |}_{t + Δ t}$ are the plastic motion rates at the beginning and end of the increment, respectively. The factor $ω$ ( $0 < ω \leq 1$ ) facilitates filtering high-frequency oscillations associated with rate-dependent connector behavior. You can specify the value of the rate filter factor, $ω$ , directly. The default value is 0.9. A value of $ω = 1$ provides no filtering and should be used with caution.

Input File Usage

Use either of the following options:

CONNECTOR HARDENING, RATE FILTER FACTOR= $ω$

CONNECTOR DAMAGE INITIATION, RATE FILTER FACTOR= $ω$

Abaqus/CAE Usage

Use the following input for isotropic hardening data:

Interaction module: connector section editor: AddPlasticity: Isotropic Hardening: Definition: Tabular, Table Options button: Filter factor: Specify:  $ω$

Use the following input for damage initiation data:

Interaction module: connector section editor: AddDamage: Initiation: Table Options button: Filter factor: Specify:  $ω$