Connector Plastic Behavior

Abaqus allows for the following three types of behaviors associated with a plasticity definition when the connector is not actively yielding:

• Linear elastic behavior, shown in Figure 1(a), is the most common case since similar behavior can be modeled in metal plasticity, for example, by specifying the Young's modulus. Elastic motion occurs prior to plasticity onset, and unloading from a plastic state occurs on a straight line parallel to the initial loading.

  Figure 1. Linear elastic-plastic (a), rigid plastic (b), and nonlinear elastic-plastic (c) response.
  
  

• Rigid behavior, shown in Figure 1(b), assumes that the slope in the linear elastic behavior is infinite; thus, the elastic motion prior to plasticity onset is zero, and unloading from a plastic state occurs on a vertical line. In practice, the rigid behavior is enforced using an automatically chosen high penalty stiffness.

• Nonlinear elastic behavior, shown in Figure 1(c), in which the initial elastic loading occurs along the defined nonlinear path. Elastic unloading occurs along a nonlinear curve (C $\to$ O_c) that is simply the user-defined nonlinear elastic curve motion shifted such that it passes through point C. The user-defined nonlinear elastic behavior must be such that the unloading path (C $\to$ O_c) does not intersect with the loading path (O $\to$ I $\to$ C); otherwise, a local instability will occur.

Other behaviors (such as damping or friction) can be specified in addition to the elastic/rigid/plastic specifications but will not be considered in the plasticity calculations since they are considered to be in parallel with the elastic-plastic/rigid plastic behavior (see the conceptual model in Connector Behavior).

If the coupled plasticity definition includes at least two terms in the associated potential definition (see Defining Derived Components for Connector Elements), a mode mix ratio can be defined to reflect the relative weight of the first two terms in their contribution to the potential. The mode mix ratio can be used in connector hardening definitions to specify dependencies in equivalent yield force or moment and, in plastic motion-based connector damage definitions (see Connector Damage Behavior), to specify dependencies in both damage initiation and damage evolution. It is defined as

where $F_I$ is the force/moment in the first component specified for the plasticity potential and $F_{II}$ is the force/moment in the second component specified for the same potential. ${\mathrm{\Psi }}_m=0.0$ if $F_I=0.0$ , ${\mathrm{\Psi }}_m=1.0$ if $F_{II}=0.0$ , and ${\mathrm{\Psi }}_m$ is somewhere in between −1.0 and 1.0 if neither is 0.0.

Perfect plasticity means that the yield force does not change with plastic relative motion.

CONNECTOR HARDENING
${F|}_0$

Interaction module: connector section editor: AddPlasticity: Specify isotropic hardening, Isotropic Hardening, and enter the Yield Force/Moment in the data table

Isotropic hardening behavior defines the evolution of the yield surface size, $F^0$ , as a function of the equivalent plastic relative motion, ${\overline{u}}^{pl}$ . This evolution can be introduced by specifying $F^0$ directly as a function of ${\overline{u}}^{pl}$ in tabular form or by using the simple exponential law

where ${F|}_0$ is the yield value at zero plastic relative motion and $Q_{inf}$ and b are material parameters. $Q_{inf}$ is the maximum change in the size of the yield surface, and b defines the rate at which the size of the yield surface changes as plastic deformation develops. When the equivalent force defining the size of the yield surface remains constant ($F^0={F|}_0$), there is no isotropic hardening.

CONNECTOR HARDENING, TYPE=ISOTROPIC, DEFINITION=TABULAR (default)

CONNECTOR HARDENING, TYPE=ISOTROPIC, DEFINITION=TABULAR (default), MODE MIX DEPENDENT

Interaction module: connector section editor: AddPlasticity: Specify isotropic hardening, Isotropic Hardening, Definition: Tabular

Mode mix dependent connector hardening behavior is not supported in Abaqus/CAE.

CONNECTOR HARDENING, TYPE=ISOTROPIC, DEFINITION=EXPONENTIAL LAW

Interaction module: connector section editor: AddPlasticity: Specify isotropic hardening, Isotropic Hardening, Definition: Exponential law

When nonlinear kinematic hardening is specified, the center of the yield surface is allowed to translate in the force space. The backforce, $\mathit{\alpha }$, is the current center of the yield surface and is interpreted similar to the backstress $\mathit{\alpha }$ discussed in Classical Metal Plasticity.

The yield surface is defined by the function

where $F^0$ is the yield value and $P\left(\mathbf{f}-\mathit{\alpha }\right)$ is the potential with respect to the backforce $\mathit{\alpha }$.

The kinematic hardening component is defined to be an additive combination of a purely kinematic term (the linear Ziegler hardening law) and a relaxation term (the recall term) that introduces the nonlinearity. When temperature and field variable dependencies are omitted, the hardening law is

where C and $\gamma$ are material parameters that must be calibrated from cyclic test data. C is the initial kinematic hardening modulus, and $\gamma$ determines the rate at which the kinematic hardening modulus decreases with increasing plastic deformation. When C and $\gamma$ are zero, the model reduces to an isotropic hardening model. When $\gamma$ is zero, the linear Ziegler hardening law is recovered. Refer to Models for Metals Subjected to Cyclic Loading for a discussion of calibrating the material parameters.

Defining the Kinematic Hardening Component by Specifying Half-Cycle Test Data

If limited test data are available, C and $\gamma$ can be based on the force-constitutive motion data obtained from the first half cycle of a unidirectional tension or compression experiment. An example of such test data is shown in Figure 2.

Figure 2. Half-cycle of force-motion data.

This approach is usually adequate when the simulation will involve only a few cycles of loading.

For each data point ($F_j,u_j^{pl}$) a value of ${\alpha }_j$ is obtained from the test data as

$${\alpha }_j=F_j-F_j^0,$$

where $F_j^0$ is the user-defined size of the yield surface at the corresponding plastic motion for the isotropic hardening definition or the initial yield force if the isotropic hardening component is not defined.

Integration of the backforce evolution law over a half cycle yields the expression

$$\alpha =\frac{C}{\gamma }\left(1-e^{-\gamma u^{pl}}\right),$$

which is used for calibrating C and $\gamma$.

When test data are given as functions of temperature and/or field variables, it is recommended that a data check analysis be run first. During the data check run, Abaqus will determine several pairs of material parameters (C, $\gamma$), where each pair will correspond to a given combination of temperature and/or field variables. Since Abaqus requires the parameter $\gamma$ to be a constant, the data check analysis will terminate with an error message if $\gamma$ is not a constant. However, an appropriate constant value of $\gamma$ may be determined from the information provided in the data file during the data check run. The values for the parameter C and the constant $\gamma$ can then be entered directly as described below.

Input File Usage

CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=HALF CYCLE (default)

Abaqus/CAE Usage

Interaction module: connector section editor: AddPlasticity: Specify kinematic hardening, Kinematic Hardening, Definition: Half-cycle

Defining the Kinematic Hardening Component by Specifying Test Data from a Stabilized Cycle

Force-constitutive motion data can be obtained from the stabilized cycle of a specimen that is subjected to symmetric cycles. A stabilized cycle is obtained by cycling the specimen over a fixed motion range $\mathrm{\Delta }u$ until a steady-state condition is reached; that is, until the force-motion curve no longer changes shape from one cycle to the next. Such a stabilized cycle is shown in Figure 3.

Figure 3. Force-motion data for a stabilized cycle.

See Models for Metals Subjected to Cyclic Loading for information on how the data should be processed before they are specified in the connector hardening definition.

Input File Usage

CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=STABILIZED

Abaqus/CAE Usage

Interaction module: connector section editor: AddPlasticity: Specify kinematic hardening, Kinematic Hardening, Definition: Stabilized

CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=PARAMETERS

Interaction module: connector section editor: AddPlasticity: Specify kinematic hardening, Kinematic Hardening, Definition: Parameters

The evolution law of the combined isotropic/kinematic model consists of two components: an isotropic hardening component, which describes the change in the equivalent force defining the size of the yield surface, $F^0$, as a function of plastic relative motion, and a nonlinear kinematic hardening component, which describes the translation of the yield surface in force space through the backforce, $\mathit{\alpha }$.

At most two connector hardening definitions, one isotropic and one kinematic, can be associated with a connector plasticity definition. If only one connector hardening definition is specified, it can be either isotropic or kinematic.

CONNECTOR HARDENING, TYPE=KINEMATIC
CONNECTOR HARDENING, TYPE=ISOTROPIC

Interaction module: connector section editor: AddPlasticity: Specify isotropic hardening and Specify kinematic hardening

Consider a SLOT connector that you have used to model a physical device efficiently. You have examined the reaction forces enforcing the SLOT constraint in the local 2- and 3-directions; since they appear to be quite large, you need to assess whether plastic deformations in the device may occur. One option that you have is to create detailed meshes for the slot and the pin in the device, define the contact interactions between them, and use elastic-plastic material definitions for the underlying materials. While this is the most accurate modeling solution, it may be impractical, especially when the device you are modeling is part of a larger model. Alternatively, you can do the following:

• use a CARTESIAN connection type instead of the SLOT connection with the first axis aligned with the slot direction;

• define components 2 and 3 as rigid; and

• define rigid plasticity separately in each of the components.

The following input can be used:

CONNECTOR SECTION, BEHAVIOR=slot
CARTESIAN
 orientation at node a
CONNECTOR BEHAVIOR, NAME=slot
CONNECTOR ELASTICITY, RIGID
 2, 3
CONNECTOR PLASTICITY, COMPONENT=2
CONNECTOR HARDENING, TYPE=ISOTROPIC
 100, 0.0
 110, 0.12
CONNECTOR PLASTICITY, COMPONENT=3
CONNECTOR HARDENING, TYPE=ISOTROPIC
 50, 0.0
 75, 0.23

The yield forces that you specify in the connector hardening definitions are obtained from an experimental result or are assessed from a “virtual experiment,” as follows:

• Use the meshed model of the slot discussed above.

• Run two simple separate analyses by constraining the slot part of the device and driving the pin into the slot walls using a boundary condition.

• Plot the reaction force at the pin node against its motion.

• Use these data to create the force-motion hardening curve to be specified in the connector hardening definition.

Referring to the spot weld shown in Figure 4 and to the yield function described in Defining Connector Potentials,

you could complete the plasticity definition, for example, by specifying tabular isotropic hardening and kinematic hardening via parameters.

Figure 4. Spot weld connection.

PARAMETER
$R_n$=0.02
$R_s$=0.05
CONNECTOR ELASTICITY, RIGID
CONNECTOR PLASTICITY
CONNECTOR POTENTIAL, EXPONENT=a
normal, $R_n$, , MACAULEY
shear, $R_s$, , ABS
CONNECTOR HARDENING, TYPE=ISOTROPIC
$F_1^0$, ${\overline{u}}_1^{pl}$
$F_2^0$, ${\overline{u}}_2^{pl}$
CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=PARAMETERS
C, $\gamma$