김경종
316 lines
19 KiB
Markdown
316 lines
19 KiB
Markdown
<!-- source-page: 741 -->
|
||
|
||
# Defining perfect plasticity
|
||
|
||
Perfect plasticity means that the yield force does not change with plastic relative motion.
|
||
|
||
Input File Usage: Use the following option to define perfect plasticity:
|
||
|
||
*CONNECTOR HARDENING $F|_{0}$
|
||
|
||
Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify isotropic hardening, Isotropic Hardening, and enter the Yield Force/Moment in the data table
|
||
|
||
# Defining nonlinear isotropic hardening
|
||
|
||
Isotropic hardening behavior defines the evolution of the yield surface size, $F ^ { 0 }$ , as a function of the equivalent plastic relative motion, $\bar { u } ^ { p l }$ . This evolution can be introduced by specifying $F ^ { 0 }$ directly as a function of $\bar { u } ^ { p l }$ in tabular form or by using the simple exponential law
|
||
|
||
$$
|
||
F ^ {0} = F | _ {0} + Q _ {\mathrm{inf}} (1 - e ^ {- b \bar {u} ^ {p l}}),
|
||
$$
|
||
|
||
where $F | _ { 0 }$ is the yield value at zero plastic relative motion and $Q _ { \mathrm { i n f } }$ and b are material parameters. $Q _ { \mathrm { i n f } }$ 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.
|
||
|
||
Defining the isotropic hardening component by specifying tabular data
|
||
|
||
Isotropic hardening can be introduced by specifying the equivalent force defining the size of the yield surface, $F ^ { 0 }$ , as a tabular function of the equivalent relative plastic motion, $\bar { u } ^ { p l }$ , and, if required, of the equivalent relative plastic motion rate, $\dot { \bar { u } } ^ { p l }$ , temperature, and/or other predefined field variables. The yield value at a given state is simply interpolated from this table of data.
|
||
|
||
Input File Usage: \*CONNECTOR HARDENING, TYPE=ISOTROPIC, DEFINITION=TABULAR (default)
|
||
|
||
Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify isotropic hardening, Isotropic Hardening, Definition: Tabular
|
||
|
||
Defining the isotropic hardening component using the exponential law
|
||
|
||
Specify the material parameters of the exponential law $( F | _ { 0 } , Q _ { \mathrm { i n f } }$ , and b) directly if they are already calibrated from test data. These parameters can be specified as functions of temperature and/or field variables.
|
||
|
||
Input File Usage: \*CONNECTOR HARDENING, TYPE=ISOTROPIC, DEFINITION=EXPONENTIAL LAW
|
||
|
||
Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify isotropic hardening, Isotropic Hardening, Definition: Exponential law
|
||
|
||
<!-- source-page: 742 -->
|
||
|
||
# Defining nonlinear kinematic hardening
|
||
|
||
When nonlinear kinematic hardening is specified, the center of the yield surface is allowed to translate in the force space. The backforce, , is the current center of the yield surface and is interpreted similar to the backstress discussed in “Classical metal plasticity,” Section 23.2.1.
|
||
|
||
The yield surface is defined by the function
|
||
|
||
$$
|
||
\phi := P (\mathbf {f} - \boldsymbol {\alpha}) - F ^ {0} \leq 0,
|
||
$$
|
||
|
||
where $F ^ { 0 }$ is the yield value and $P ( \mathbf { f } - \alpha )$ is the potential with respect to the backforce .
|
||
|
||
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
|
||
|
||
$$
|
||
\dot {\pmb {\alpha}} = C \frac {1}{F ^ {0}} (\mathbf {f} - \pmb {\alpha}) \dot {\bar {u}} ^ {p l} - \gamma \pmb {\alpha} \dot {\bar {u}} ^ {p l},
|
||
$$
|
||
|
||
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,” Section 23.2.2, 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 31.2.6–2. This approach is usually adequate when the simulation will involve only a few cycles of loading.
|
||
|
||
For each data point $( F _ { j } , u _ { j } ^ { p l } )$ 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
|
||
|
||
$$
|
||
\alpha = \frac {C}{\gamma} (1 - e ^ {- \gamma u ^ {p l}}),
|
||
$$
|
||
|
||
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
|
||
|
||
<!-- source-page: 743 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>line</summary>
|
||
|
||
| Point | u^pl | F |
|
||
|-------|------|-------|
|
||
| F₀ | 0 | F |
|
||
| F₁ | u₁^pl| F₁ |
|
||
| F₂ | u₂^pl| F₂ |
|
||
| F₃ | u₃^pl| F₃ |
|
||
</details>
|
||
|
||
Figure 31.2.6–2 Half-cycle of force-motion data.
|
||
|
||
field variables. Since Abaqus requires the parameter $\gamma$ to be a constant, the data check analysis will terminate with an error message $\operatorname { i f } \gamma$ is not a constant. However, an appropriate constant value of $\cdot _ { \gamma }$ 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: Add→Plasticity: 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 $\Delta u$ 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 31.2.6–3. See “Models for metals subjected to cyclic loading,” Section 23.2.2, 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: Add→Plasticity: Specify kinematic hardening, Kinematic Hardening, Definition: Stabilized
|
||
|
||
Defining the kinematic hardening component by specifying the material parameters directly
|
||
|
||
The parameters $c$ and $\gamma$ can be specified directly if they are already calibrated from test data. The parameter $\boldsymbol { c }$ can be provided as a function of temperature and/or field variables, but temperature and field variable dependence of $\cdot _ { \gamma }$ is not available. The algorithm currently used to integrate the nonlinear isotropic/kinematic hardening model does not provide accurate solutions if the value of $\gamma$ changes significantly in an increment due to temperature and/or field variable dependence.
|
||
|
||
<!-- source-page: 744 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
F
|
||
F₁ F₂ Fᵢ Fₙ
|
||
Δu
|
||
uᵢ u
|
||
uₚ⁰
|
||
uₚⁱ = uᵢ - (Fᵢ/E) - uₚ⁰
|
||
</details>
|
||
|
||
Figure 31.2.6–3 Force-motion data for a stabilized cycle.
|
||
|
||
Input File Usage: \*CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=PARAMETERS
|
||
|
||
Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify kinematic hardening, Kinematic Hardening, Definition: Parameters
|
||
|
||
# Defining nonlinear isotropic/kinematic hardening
|
||
|
||
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, , 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, .
|
||
|
||
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.
|
||
|
||
Input File Usage: Use the following two options to define nonlinear isotropic/kinematic hardening:
|
||
|
||
\*CONNECTOR HARDENING, TYPE=KINEMATIC
|
||
|
||
\*CONNECTOR HARDENING, TYPE=ISOTROPIC
|
||
|
||
Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify isotropic hardening and Specify kinematic hardening
|
||
|
||
# Using multiple plasticity definitions
|
||
|
||
Multiple connector plasticity definitions can be used as part of the same connector behavior definition. However, only one connector plasticity definition can be used to define plasticity for each available component of relative motion. At most one coupled plasticity definition can be associated with a connector behavior definition. Additional connector plasticity definitions are permitted for the same
|
||
|
||
<!-- source-page: 745 -->
|
||
|
||
connector behavior definition only if the two spaces do not overlap; for example, you could define uncoupled connector plasticity for components 1, 2, and 6 and have one coupled connector plasticity definition involving components 3, 4, and 5.
|
||
|
||
Each connector plasticity definition must have its own hardening definition.
|
||
|
||
# Examples
|
||
|
||
Illustrations of uncoupled and coupled plasticity behaviors are shown in the following examples.
|
||
|
||
# Uncoupled plasticity in a SLOT-like connector
|
||
|
||
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:
|
||
|
||
```csv
|
||
*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.
|
||
|
||
<!-- source-page: 746 -->
|
||
|
||
• 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.
|
||
|
||
# Coupled plasticity in a spot weld
|
||
|
||
Referring to the spot weld shown in Figure 31.2.6–4 and to the yield function described in “Defining connector potentials” in “Connector functions for coupled behavior,” Section 31.2.4,
|
||
|
||
$$
|
||
\phi (\mathbf {f}) = \left[ \left(\frac {\max (F _ {n} , 0)}{R _ {n}}\right) ^ {a} + \left(\frac {| F _ {s} |}{R _ {s}}\right) ^ {a} \right] ^ {1 / a},
|
||
$$
|
||
|
||
you could complete the plasticity definition, for example, by specifying tabular isotropic hardening and kinematic hardening via parameters.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
F_s
|
||
F
|
||
F_n
|
||
</details>
|
||
|
||
Figure 31.2.6–4 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 $F_{1}^{0}$ , $\bar{u}_{1}^{pl}$ $F_{2}^{0}$ , $\bar{u}_{2}^{pl}$ *CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=PARAMETERS
|
||
C, $\gamma$
|
||
|
||
<!-- source-page: 747 -->
|
||
|
||
# Defining plastic connector behavior in linear perturbation procedures
|
||
|
||
Plastic relative motions are not allowed during linear perturbation analyses. Therefore, the connector relative motions will be linear elastic perturbations about the plastically deformed base state, similar to metal plasticity.
|
||
|
||
# Output
|
||
|
||
The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following output variables are of particular interest when defining plasticity in connectors:
|
||
|
||
CUE Connector elastic displacements/rotations.
|
||
|
||
CUP Connector plastic displacements/rotations.
|
||
|
||
CUPEQ Connector equivalent plastic relative displacements/rotations. In addition to the usual six components associated with connector output variables, CUPEQ includes the scalar CUPEQC, which is the equivalent plastic relative motion associated with a coupled plasticity definition.
|
||
|
||
CALPHAF Connector kinematic hardening shift forces/moments.
|
||
|
||
<!-- source-page: 748 -->
|
||
|
||
<!-- source-page: 749 -->
|
||
|
||
# 31.2.7 CONNECTOR DAMAGE BEHAVIOR
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Connectors: overview,” Section 31.1.1
|
||
• “Connector behavior,” Section 31.2.1
|
||
• \*CONNECTOR BEHAVIOR
|
||
• \*CONNECTOR DAMAGE EVOLUTION
|
||
• \*CONNECTOR DAMAGE INITIATION
|
||
• \*CONNECTOR ELASTICITY
|
||
• \*CONNECTOR PLASTICITY
|
||
• \*CONNECTOR POTENTIAL
|
||
• \*SECTION CONTROLS
|
||
|
||
• “Defining damage,” Section 15.17.7 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
Connector damage behavior:
|
||
|
||
• can be specified in any connectors with available components of relative motion;
|
||
• can be used to degrade the elastic, elastic-plastic, or rigid plastic response in connector elements;
|
||
• can use a force-based, motion-based, or plastic motion–based damage initiation criterion upon which response degradation may be triggered;
|
||
• can use either a (plastic) motion-based or an energy-based damage evolution law to degrade the force response in the connector;
|
||
• can be defined in terms of several competing damage mechanisms; and
|
||
• can be used only as an indicator of proximity to the damage initiation point without degrading the connector response.
|
||
|
||
# Damage formulation in connectors
|
||
|
||
If relative forces or motions in a connection exceed critical values, the connector starts undergoing irreversible damage (degradation). Upon additional loading there is further evolution of damage leading to eventual failure. If damage has occurred, the force response in the connector component i will change according to the following general form:
|
||
|
||
$$
|
||
F _ {i} = (1 - d _ {i}) F _ {e f f _ {i}}, \quad 0 \leq d _ {i} \leq 1 \mathrm{nosumoni}
|
||
$$
|
||
|
||
<!-- source-page: 750 -->
|
||
|
||
where $d _ { i }$ is a scalar damage variable and $F _ { e f f _ { i } }$ is the response in the available connector component of relative motion i if damage were not present (effective response).
|
||
|
||
To define a connector damage mechanism, you specify the following:
|
||
|
||
• a criterion for damage initiation; and
|
||
• a damage evolution law that specifies how the damage variable d evolves (optional).
|
||
|
||
Prior to damage initiation, d has a value of 0.0; thus, the force response in the connector does not change. Once damage has been initiated, the damage variable will monotonically evolve up to the maximum value of 1.0 if damage evolution is specified. Complete failure occurs when $d = 1 . 0$ .
|
||
|
||
Abaqus allows you to specify a maximum degradation value (the default value is 1.0); damage evolution will stop when the damage variable reaches this value, and the element will be deleted from the mesh by default. Alternatively, you can specify that the damaged connector elements remain in the analysis with no further damage evolution. The maximum degradation value is used to evaluate the damaged stiffness in the remaining part of the analysis. This functionality is discussed in detail in “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4.
|
||
|
||
For connectors with purely elastic behavior, damage can be initiated and evolved in one direction only. If damage was initiated in tension, it will evolve in tension; if damage was initiated in compression, it will evolve in compression. Once damage initiates in tension, it cannot be initiated in compression and vice versa.
|
||
|
||
# Defining connector damage initiation
|
||
|
||
The degradation process in connectors initiates when forces or relative motions in the connector satisfy certain criteria. Three different criteria types can be used to trigger damage in connectors: criteria based on force, plastic motion, or constitutive motion. Connector damage initiation criteria for the available components of relative motion can be specified for each component independently (uncoupled). Alternatively, connector damage initiation criteria that couple all or some of the available components of relative motion in the connector can be defined.
|
||
|
||
The damage initiation criterion 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.
|
||
|
||
# Force-based damage initiation criterion
|
||
|
||
By default, the damage initiation criterion is specified in terms of forces/moments in the connector. Elastic or rigid connector behavior must be defined for the components involved in the initiation. You provide the lower (compression) limit, $f _ { m i n }$ , and the upper (tension) limit, $f _ { m a x }$ , for the force/moment damage initiation values. If the force is outside the range specified by the two limit values, damage is initiated. The output variable CDIF can be used to monitor the proximity to the damage initiation point.
|