MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide4/AbaqusAnalysisUserGuide4_069.md

Tabular data are often used to define connector behaviors, such as nonlinear elasticity, isotropic hardening, etc. As shown in Figure 31.2.1–5, the data points make up a nonlinear curve in the constitutive space.

line

Displacement, u	Force, F
u₁	F(0)
u₂	F₂
u₃	F₃
u₄	F₄

Figure 31.2.1–5 Nonlinear connector behaviors defined as tabular data.

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 31.2.1–5.

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,” Section 21.1.2, 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” in “Connector plastic behavior,” Section 31.2.6) and plastic motion–based damage initiation criterion (“Plastic motion–based damage initiation criterion” in “Connector damage behavior,” Section 31.2.7) 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: Add→Plasticity: Isotropic Hardening: Definition: Tabular, Table Options button: Interpolation: Linear

Use the following input for damage initiation data:

Interaction module: connector section editor: Add→Damage: 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: Add→Plasticity: Isotropic Hardening: Definition: Tabular, Table Options button: Interpolation: Logarithmic

Use the following input for damage initiation data:

Interaction module: connector section editor: Add→Damage: 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 + \Delta t} = \omega \frac {\Delta \bar {u} ^ {p l}}{\Delta t} + (1 - \omega) \dot {\bar {u}} ^ {p l} | _ {t}

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

Input File Usage: Use either of the following options:

* \mathrm { C O N N E C T O R ~ H A R D E N I N G } , \mathrm { R A T E ~ F I L T E R ~ F A C T O R } = \omega *CONNECTOR DAMAGE INITIATION, RATE FILTER FACTOR=

Abaqus/CAE Usage: Use the following input for isotropic hardening data:

Interaction module: connector section editor: Add→Plasticity:

Isotropic Hardening: Definition: Tabular, Table Options

button: Filter factor: Specify:

Use the following input for damage initiation data:

Interaction module: connector section editor: Add→Damage: Initiation:

Table Options button: Filter factor: Specify:

31.2.2 CONNECTOR ELASTIC BEHAVIOR

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

References

• “Connectors: overview,” Section 31.1.1
• “Connector behavior,” Section 31.2.1
• *CONNECTOR BEHAVIOR
• *CONNECTOR ELASTICITY
• “Defining elasticity,” Section 15.17.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

Overview

Spring-like elastic connector behavior:

• can be defined in any connector with available components of relative motion;
• can be specified for each available component of relative motion independently, in which case the behavior can be linear or nonlinear;
• can be specified as dependent on relative positions or constitutive motions in several local directions; and
• can be specified for all available components of relative motion as coupled linear elastic behavior.

Alternatively, rigid-like behavior can be specified in any of the available components of relative motion using an automatically chosen stiff spring.

The directions in which the forces and moments act and the displacements and rotations are measured are determined by the local directions as described in “Connection-type library,” Section 31.1.5, for each connection type.

Defining linear uncoupled elastic behavior

In the simplest case of linear uncoupled elasticity you define the spring stiffnesses for the selected components ( \mathrm { i } . \mathrm { e } . , D _ { 1 1 } for component 1, D _ { 2 2 } for component 2, etc.), which are used in the equation

F _ {i} = D _ {i i} u _ {i} \quad (\text { no   sum   on   } i),

where F _ { i } is the force or moment in the i ^ { \mathrm { t h } } component of relative motion and u _ { i } is the connector displacement or rotation in the i ^ { \mathrm { t h } } direction. The elastic stiffness can depend on frequency (in Abaqus/Standard), temperature, and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of frequency, temperature, and field variables.

If a frequency-dependent damping behavior is specified in an Abaqus/Standard analysis procedure other than direct-solution steady-state dynamics, the data for the lowest frequency given will be used.

Input File Usage:

Use the following options to define linear uncoupled elastic connector behavior:*CONNECTOR BEHAVIOR, NAME=name*CONNECTOR ELASTICITY, COMPONENT=component number,DEPENDENCIES=n

Abaqus/CAE Usage:

Interaction module: connector section editor: Add→Elasticity: Definition: Linear, Force/Moment: component or components, Coupling: Uncoupled

Defining linear coupled elastic behavior

In the linear coupled case you define the spring stiffness matrix components, D _ { i j } , which are used in the equation

F _ {i} = \sum_ {j} D _ {i j} u _ {j},

where F _ { i } is the force in the i ^ { \mathrm { t h } } component of relative motion, u _ { j } is the motion of the j ^ { \mathrm { t h } } component, and D _ { i j } is the coupling between the i ^ { \mathrm { t h } } and j ^ { \mathrm { t h } } components. The D matrix is assumed to be symmetric, so only the upper triangle of the matrix is specified. In connectors with kinematic constraints the entries that correspond to the constrained components of relative motion will be ignored. The elastic stiffness can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables.

Input File Usage:

Use the following options to define linear coupled elastic connector behavior:*CONNECTOR BEHAVIOR, NAME=name*CONNECTOR ELASTICITY, DEPENDENCIES=n

Abaqus/CAE Usage:

Interaction module: connector section editor: Add→Elasticity: Definition: Linear, Force/Moment: component or components, Coupling: Coupled

Modeling coupled unsymmetric linear stiffness

By definition, linear elastic behavior should be defined by a symmetric spring stiffness matrix. However, Abaqus/Standard allows you to define an unsymmetric coupled spring stiffness matrix. The intended use case is to approximate fluid film bearings supporting a rotating structure in a rotordynamic analysis (see Genta, 2005, and “Distributed loads,” Section 34.4.3). Abaqus/Standard will not check the stability of an unsymmetric spring stiffness matrix; therefore, you must ensure that it is defined properly.

In the linear coupled case you define the spring stiffness matrix components, D _ { i j } , which are used in the equation

F _ {i} = \sum_ {j} D _ {i j} u _ {j},

where F _ { i } is the force in the i ^ { \mathrm { t h } } component of relative motion, u _ { j } is the motion of the j ^ { \mathrm { t h } } component, and D _ { i j } is the coupling between the i ^ { \mathrm { t h } } and j ^ { \mathrm { t h } } components. The D matrix in this case is assumed to be unsymmetric, so the entire matrix is specified. The entries that correspond to the constrained