김경종
210 lines
14 KiB
Markdown
210 lines
14 KiB
Markdown
<!-- source-page: 531 -->
|
||
|
||
Input File Usage: Use the following option to delete the element from the mesh (default):
|
||
|
||
\*SECTION CONTROLS, ELEMENT DELETION=YES
|
||
|
||
# Keeping the element in the computations
|
||
|
||
Optionally, you may choose not to remove the element from the mesh, except in the case of threedimensional beam elements. With element deletion turned off, the overall damage variable is enforced to be $D \leq D _ { \operatorname* { m a x } }$ . The default value is $D _ { \mathrm { m a x } } = 0 . 9 9$ if element deletion is turned off, which ensures that elements will remain active in the simulation with a residual stiffness of at least 1% of the original stiffness. The dimensionality of the stress state of the element affects which stiffness components can become damaged, as discussed below.
|
||
|
||
In a heat transfer analysis the thermal properties of the material are not affected by damage of the material stiffness.
|
||
|
||
Input File Usage: Use the following option to keep the element in the computation:
|
||
|
||
$* { \mathrm { S E C T I O N ~ C O N T R O L S } } , { \mathrm { E L E M E N T ~ D E L E T I O N { = } N O } }$
|
||
|
||
# Elements with three-dimensional stress states in Abaqus/Explicit
|
||
|
||
For elements with three-dimensional stress states (including generalized plane strain elements) the shear stiffness will be degraded up to a maximum value, $D _ { \mathrm { m a x } }$ , leading to softening of the deviatoric stress components. The bulk stiffness, however, will be degraded only while the material is subjected to negative pressures (i.e., hydrostatic tension); there is no bulk degradation under positive pressures. This corresponds to a fluid-like behavior. Therefore, the degraded deviatoric, , and pressure, p, stresses are computed as
|
||
|
||
$$
|
||
\mathbf {S} = (1 - D _ {\mathrm{dev}}) \bar {\mathbf {S}},
|
||
$$
|
||
|
||
$$
|
||
p = (1 - D _ {\mathrm{vol}}) \bar {p},
|
||
$$
|
||
|
||
where the deviatoric and volumetric damage variables are given as
|
||
|
||
$$
|
||
D _ {\mathrm{dev}} = D,
|
||
$$
|
||
|
||
$$
|
||
D _ {\mathrm{vol}} = \left\{ \begin{array}{l l} D & \text {if} \bar {p} \leq 0, \\ 0 & \text {if} \bar {p} > 0. \end{array} \right.
|
||
$$
|
||
|
||
In this case the output variable SDEG contains the value of $D _ { \mathrm { d e v } }$ .
|
||
|
||
# Elements with three-dimensional stress states in Abaqus/Standard
|
||
|
||
For elements with three-dimensional stress states (including generalized plane strain elements) the stiffness will be degraded uniformly until the maximum degradation, $D _ { \mathrm { m a x } }$ , is reached. Output variable SDEG contains the value of D.
|
||
|
||
<!-- source-page: 532 -->
|
||
|
||
# Elements with plane stress states
|
||
|
||
For elements with a plane stress formulation (plane stress, shell, continuum shell, and membrane elements) the stiffness will be degraded uniformly until the maximum degradation, $D _ { \mathrm { m a x } }$ , is reached. Output variable SDEG contains the value of D.
|
||
|
||
# Elements with one-dimensional stress states
|
||
|
||
For elements with a one-dimensional stress state (i.e., truss elements, rebar, and cohesive elements with gasket behavior) their only stress component will be degraded if it is positive (tension). The material stiffness will remain unaffected under compression loading. The stress is, therefore, given by $\sigma = ( 1 -$ $D _ { \mathrm { u n i } } \big ) \bar { \sigma }$ , where the uniaxial damage variable is computed as
|
||
|
||
$$
|
||
D _ {\mathrm{uni}} = \left\{ \begin{array}{c l} D & \text {if} \bar {\sigma} \geq 0, \\ 0 & \text {if} \bar {\sigma} < 0. \end{array} \right.
|
||
$$
|
||
|
||
In this case $D _ { \mathrm { m a x } }$ determines the maximum allowed degradation in uniaxial tension $( D \leq D _ { \mathrm { m a x } } )$ . Output variable SDEG contains the value of $D _ { \mathrm { u n i } }$ .
|
||
|
||
# Convergence difficulties in Abaqus/Standard
|
||
|
||
Material models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. Some techniques are available in Abaqus/Standard to improve convergence for analyses involving these materials.
|
||
|
||
# Viscous regularization in Abaqus/Standard
|
||
|
||
You can overcome some of the convergence difficulties associated with softening and stiffness degradation by using the viscous regularization scheme, which causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments.
|
||
|
||
In this regularization scheme a viscous damage variable is defined by the evolution equation:
|
||
|
||
$$
|
||
\dot {d} _ {v} = \frac {1}{\eta} (d - d _ {v}),
|
||
$$
|
||
|
||
where is the viscosity coefficient representing the relaxation time of the viscous system and d is the damage variable evaluated in the inviscid base model. The damaged response of the viscous material is computed using the viscous value of the damage variable. Using viscous regularization with a small value of the viscosity parameter (small compared to the characteristic time increment) usually helps improve the rate of convergence of the model in the softening regime, without compromising results. The basic idea is that the solution of the viscous system relaxes to that of the inviscid case as $t / \eta \infty$ , where t represents time.
|
||
|
||
In Abaqus/Standard you can specify the viscous coefficients as part of a section controls definition. For more information, see “Using viscous regularization with cohesive elements, connector elements,
|
||
|
||
<!-- source-page: 533 -->
|
||
|
||
and elements that can be used with the damage evolution models for ductile metals and fiber-reinforced composites in Abaqus/Standard” in “Section controls,” Section 27.1.4.
|
||
|
||
# Unsymmetric equation solver
|
||
|
||
In general, if any of the ductile evolution models is used, the material Jacobian matrix will be nonsymmetric. To improve convergence, it is recommended that the unsymmetric equation solver is used in this case.
|
||
|
||
# Using the damage models with rebar
|
||
|
||
It is possible to use material damage models in elements for which rebar are also defined. The base material contribution to the element stress-carrying capacity diminishes according to the behavior described previously in this section. The rebar contribution to the element stress-carrying capacity will not be affected unless damage is also included in the rebar material definition; in that case the rebar contribution to the element stress-carrying capacity will also be degraded after the damage initiation criterion specified for the rebar is met. For the default choice of element deletion, the element is removed from the mesh when at any one integration location all section points in the base material and rebar are fully degraded.
|
||
|
||
# Elements
|
||
|
||
Damage evolution for ductile metals can be defined for any element that can be used with the damage initiation criteria for ductile metals in Abaqus (“Damage initiation for ductile metals,” Section 24.2.2).
|
||
|
||
# Output
|
||
|
||
In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning when damage evolution is specified:
|
||
|
||
STATUS Status of element (the status of an element is 1.0 if the element is active, 0.0 if the element is not).
|
||
|
||
SDEG Overall scalar stiffness degradation, D.
|
||
|
||
# Additional reference
|
||
|
||
• Hillerborg, A., M. Modeer, and P. E. Petersson, “Analysis of Crack Formation and Crack Growth in Concrete by Means of Fracture Mechanics and Finite Elements,” Cement and Concrete Research, vol. 6, pp. 773–782, 1976.
|
||
|
||
<!-- source-page: 534 -->
|
||
|
||
<!-- source-page: 535 -->
|
||
|
||
# 24.3 Damage and failure for fiber-reinforced composites
|
||
|
||
• “Damage and failure for fiber-reinforced composites: overview,” Section 24.3.1
|
||
• “Damage initiation for fiber-reinforced composites,” Section 24.3.2
|
||
• “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3
|
||
|
||
<!-- source-page: 536 -->
|
||
|
||
<!-- source-page: 537 -->
|
||
|
||
# 24.3.1 DAMAGE AND FAILURE FOR FIBER-REINFORCED COMPOSITES: OVERVIEW
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Progressive damage and failure,” Section 24.1.1
|
||
• “Damage initiation for fiber-reinforced composites,” Section 24.3.2
|
||
• “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3
|
||
• \*DAMAGE INITIATION
|
||
• \*DAMAGE EVOLUTION
|
||
• \*DAMAGE STABILIZATION
|
||
• “Hashin damage” in “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
Abaqus offers a damage model enabling you to predict the onset of damage and to model damage evolution for elastic-brittle materials with anisotropic behavior. The model is primarily intended to be used with fiber-reinforced materials since they typically exhibit such behavior.
|
||
|
||
This damage model requires specification of the following:
|
||
|
||
• the undamaged response of the material, which must be linearly elastic (see “Linear elastic behavior,” Section 22.2.1);
|
||
• a damage initiation criterion (see “Progressive damage and failure,” Section 24.1.1, and “Damage initiation for fiber-reinforced composites,” Section 24.3.2); and
|
||
• a damage evolution response, including a choice of element removal (see “Progressive damage and failure,” Section 24.1.1, and “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3).
|
||
|
||
# General concepts of damage in unidirectional lamina
|
||
|
||
Damage is characterized by the degradation of material stiffness. It plays an important role in the analysis of fiber-reinforced composite materials. Many such materials exhibit elastic-brittle behavior; that is, damage in these materials is initiated without significant plastic deformation. Consequently, plasticity can be neglected when modeling behavior of such materials.
|
||
|
||
The fibers in the fiber-reinforced material are assumed to be parallel, as depicted in Figure 24.3.1–1. You must specify material properties in a local coordinate system defined by the user. The lamina is in the 1–2 plane, and the local 1 direction corresponds to the fiber direction. You must specify the undamaged material response using one of the methods for defining an orthotropic linear elastic material (“Linear elastic behavior,” Section 22.2.1); the most convenient of which is the method for defining an orthotropic material in plane stress (“Defining orthotropic elasticity in plane stress” in “Linear elastic behavior,”
|
||
|
||
<!-- source-page: 538 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>natural_image</summary>
|
||
|
||
Isometric diagram of a rectangular prism with multiple cylindrical rods arranged in a grid, labeled with axes 1, 2, and 3 (no text or symbols on the diagram itself)
|
||
</details>
|
||
|
||
Figure 24.3.1–1 Unidirectional lamina.
|
||
|
||
Section 22.2.1). However, the material response can also be defined in terms of the engineering constants or by specifying the elastic stiffness matrix directly.
|
||
|
||
The Abaqus anisotropic damage model is based on the work of Matzenmiller et. al (1995), Hashin and Rotem (1973), Hashin (1980), and Camanho and Davila (2002).
|
||
|
||
Four different modes of failure are considered:
|
||
|
||
• fiber rupture in tension;
|
||
• fiber buckling and kinking in compression;
|
||
• matrix cracking under transverse tension and shearing; and
|
||
• matrix crushing under transverse compression and shearing.
|
||
|
||
In Abaqus the onset of damage is determined by the initiation criteria proposed by Hashin and Rotem (1973) and Hashin (1980), in which the failure surface is expressed in the effective stress space (the stress acting over the area that effectively resists the force). These criteria are discussed in detail in “Damage initiation for fiber-reinforced composites,” Section 24.3.2.
|
||
|
||
The response of the material is computed from
|
||
|
||
$$
|
||
\sigma = \mathbf {C _ {d}} \varepsilon ,
|
||
$$
|
||
|
||
where is the strain and $\mathbf { C _ { d } }$ is the elasticity matrix, which reflects any damage and has the form
|
||
|
||
$$
|
||
\mathbf {C _ {d}} = \frac {1}{D} \left[ \begin{array}{c c c} (1 - d _ {f}) E _ {1} & (1 - d _ {f}) (1 - d _ {m}) \nu_ {2 1} E _ {1} & 0 \\ (1 - d _ {f}) (1 - d _ {m}) \nu_ {1 2} E _ {2} & (1 - d _ {m}) E _ {2} & 0 \\ 0 & 0 & (1 - d _ {s}) G D \end{array} \right],
|
||
$$
|
||
|
||
<!-- source-page: 539 -->
|
||
|
||
where $D = 1 - ( 1 - d _ { f } ) ( 1 - d _ { m } ) \nu _ { 1 2 } \nu _ { 2 1 } , d _ { f }$ reflects the current state of fiber damage, $d _ { m }$ reflects the current state of matrix damage, $d _ { s }$ reflects the current state of shear damage, $E _ { 1 }$ is the Young’s modulus in the fiber direction, $E _ { 2 }$ is the Young’s modulus in the direction perpendicular to the fibers, is the shear modulus, and $\nu _ { 1 2 }$ and $\nu _ { 2 1 }$ are Poisson’s ratios.
|
||
|
||
The evolution of the elasticity matrix due to damage is discussed in more detail in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3; that section also discusses:
|
||
|
||
• options for treating severe damage (“Maximum degradation and choice of element removal” in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3); and
|
||
• viscous regularization (“Viscous regularization” in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3).
|
||
|
||
# Elements
|
||
|
||
The fiber-reinforced composite damage model must be used with elements with a plane stress formulation, which include plane stress, shell, continuum shell, and membrane elements.
|
||
|
||
# Additional references
|
||
|
||
• Camanho, P. P., and C. G. Davila, “Mixed-Mode Decohesion Finite Elements for the Simulation of Delamination in Composite Materials,” NASA/TM-2002–211737, pp. 1–37, 2002.
|
||
• Hashin, Z., “Failure Criteria for Unidirectional Fiber Composites,” Journal of Applied Mechanics, vol. 47, pp. 329–334, 1980.
|
||
• Hashin, Z., and A. Rotem, “A Fatigue Criterion for Fiber-Reinforced Materials,” Journal of Composite Materials, vol. 7, pp. 448–464, 1973.
|
||
• Lapczyk, I., and J. A. Hurtado, “Progressive Damage Modeling in Fiber-Reinforced Materials,” Composites Part A: Applied Science and Manufacturing, vol. 38, no. 11, pp. 2333–2341, 2007.
|
||
• Matzenmiller, A., J. Lubliner, and R. L. Taylor, “A Constitutive Model for Anisotropic Damage in Fiber-Composites,” Mechanics of Materials, vol. 20, pp. 125–152, 1995.
|
||
|
||
<!-- source-page: 540 -->
|