add documents

.raw/AbaqusAnalysisUserGuide3/AbaqusAnalysisUserGuide3_056.md

@@ -0,0 +1,218 @@
+<!-- source-page: 551 -->
+
+where the damaged elasticity matrix, $\mathbf { C _ { d } }$ , is computed using viscous values of damage variables for each failure mode. 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 $t / \eta \to \infty$ , where t represents time.
+
+Viscous regularization is also available in Abaqus/Explicit. Viscous regularization slows down the rate of increase of damage and leads to increased fracture energy with increasing deformation rates, which can be exploited as an effective method of modeling rate-dependent material behavior.
+
+In Abaqus/Standard the approximate amount of energy associated with viscous regularization over the whole model or over an element set is available using output variable ALLCD.
+
+# Defining viscous regularization coefficients
+
+You can specify different values of viscous coefficients for different failure modes.
+
+Input File Usage: Use the following option to define viscous coefficients:
+
+\*DAMAGE STABILIZATION
+
+$\eta _ { f t } , \eta _ { f c } , \eta _ { m t } , \eta _ { m c }$
+
+where , , , are viscosity coefficients for fiber tension, fiber compression, matrix tension, and matrix compression failure modes, respectively.
+
+Abaqus/CAE Usage: Use the following input to define the viscous coefficients for fiber-reinforced materials:
+
+Property module: material editor: Mechanical→Damage
+
+for Fiber-Reinforced Composites→Hashin Damage:
+
+Suboptions→Damage Stabilization
+
+Applying a single viscous coefficient in Abaqus/Standard
+
+Alternatively, in Abaqus/Standard you can specify the viscous coefficients as part of a section controls definition. In this case the same viscous coefficient will be applied to all failure modes. For more information, see “Using viscous regularization with cohesive elements, connector elements, 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.
+
+# Material damping
+
+If stiffness proportional damping is specified in combination with the damage evolution law for fiberreinforced materials, Abaqus calculates the damping stresses using the damaged elastic stiffness.
+
+# Elements
+
+The damage evolution law for fiber-reinforced materials must be used with elements with a plane stress formulation, which include plane stress, shell, continuum shell, and membrane elements.
+
+<!-- source-page: 552 -->
+
+Output 
+
+<table><tr><td colspan="2">In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables relate specifically to damage evolution in the fiber-reinforced composite damage model:</td></tr><tr><td>STATUS</td><td>Status of the element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). The value of this variable is set to 0.0 only if damage has occurred in all the damage modes.</td></tr><tr><td>DAMAGEFT</td><td>Fiber tensile damage variable.</td></tr><tr><td>DAMAGEFC</td><td>Fiber compressive damage variable.</td></tr><tr><td>DAMAGEMT</td><td>Matrix tensile damage variable.</td></tr><tr><td>DAMAGEMC</td><td>Matrix compressive damage variable.</td></tr><tr><td>DAMAGESHR</td><td>Shear damage variable.</td></tr><tr><td>EDMDDEN</td><td>Energy dissipated per unit volume in the element by damage.</td></tr><tr><td>ELDMD</td><td>Total energy dissipated in the element by damage.</td></tr><tr><td>DMENER</td><td>Energy dissipated per unit volume by damage.</td></tr><tr><td>ALLDMD</td><td>Energy dissipated in the whole (or partial) model by damage.</td></tr><tr><td>ECDDEN</td><td>Energy per unit volume in the element that is associated with viscous regularization.</td></tr><tr><td>ELCD</td><td>Total energy in the element that is associated with viscous regularization.</td></tr><tr><td>CENER</td><td>Energy per unit volume that is associated with viscous regularization.</td></tr><tr><td>ALLCD</td><td>The approximate amount of energy over the whole model or over an element set that is associated with viscous regularization.</td></tr></table>
+
+# Additional reference
+
+• 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.
+
+<!-- source-page: 553 -->
+
+# 24.4 Damage and failure for ductile materials in low-cycle fatigue analysis
+
+• “Damage and failure for ductile materials in low-cycle fatigue analysis: overview,” Section 24.4.1   
+• “Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2   
+• “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3
+
+<!-- source-page: 554 -->
+
+<!-- source-page: 555 -->
+
+# 24.4.1 DAMAGE AND FAILURE FOR DUCTILE MATERIALS IN LOW-CYCLE FATIGUE ANALYSIS: OVERVIEW
+
+Product: Abaqus/Standard
+
+# References
+
+• “Progressive damage and failure,” Section 24.1.1   
+• “Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2   
+• “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3   
+• “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7   
+• \*DAMAGE INITIATION   
+• \*DAMAGE EVOLUTION
+
+# Overview
+
+Abaqus/Standard offers a general capability for modeling progressive damage and failure of ductile materials due to stress reversals and the accumulation of inelastic strain energy in a low-cycle fatigue analysis using the direct cyclic approach. In the most general case this requires the specification of the following:
+
+• the undamaged ductile materials in any elements (including cohesive elements based on a continuum approach) whose response is defined in terms of a continuum-based constitutive model (“Material library: overview,” Section 21.1.1);   
+• a damage initiation criterion (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2); and   
+• a damage evolution response (“Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3).
+
+A summary of the general framework for progressive damage and failure in Abaqus is given in “Progressive damage and failure,” Section 24.1.1. This section provides an overview of the damage initiation criteria and damage evolution law for ductile materials in a low-cycle fatigue analysis using the direct cyclic approach.
+
+# General concepts of damage of ductile materials in low-cycle fatigue
+
+Accurately and effectively predicting the fatigue life for an inelastic structure, such as a solder joint in an electronic chip packaging, subjected to sub-critical cyclic loading is a challenging problem. Cyclic thermal or mechanical loading often leads to stress reversals and the accumulation of inelastic strain, which may in turn lead to the initiation and propagation of a crack. The low-cycle fatigue analysis capability in Abaqus/Standard uses a direct cyclic approach (“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7) to model progressive damage and failure based on a continuum
+
+<!-- source-page: 556 -->
+
+damage approach. The damage initiation (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2) and evolution (“Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3) are characterized by the stabilized accumulated inelastic hysteresis strain energy per cycle proposed by Darveaux (2002) and Lau (2002).
+
+The damage evolution law describes the rate of degradation of the material stiffness per cycle once the corresponding initiation criterion has been reached. For damage in ductile materials Abaqus/Standard assumes that the degradation of the stiffness can be modeled using a scalar damage variable, . At any given cycle during the analysis the stress tensor in the material is given by the scalar damage equation
+
+$$
+\pmb {\sigma} = (1 - D) \bar {\pmb {\sigma}},
+$$
+
+where is the effective (or undamaged) stress tensor that would exist in the material in the absence of damage computed in the current increment. The material has lost its load carrying capacity when .
+
+# Elements
+
+The failure modeling capability for ductile materials can be used with any elements (including cohesive elements based on a continuum approach) in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom).
+
+# Additional references
+
+• Darveaux, R., “Effect of Simulation Methodology on Solder Joint Crack Growth Correlation and Fatigue Life Prediction,” Journal of Electronic Packaging, vol. 124, pp. 147–154, 2002.   
+• Lau, J., S. Pan, and C. Chang, “A New Thermal-Fatigue Life Prediction Model for Wafer Level Chip Scale Package (WLCSP) Solder Joints,” Journal of Electronic Packaging, vol. 124, pp. 212–220, 2002.
+
+<!-- source-page: 557 -->
+
+# 24.4.2 DAMAGE INITIATION FOR DUCTILE MATERIALS IN LOW-CYCLE FATIGUE
+
+Product: Abaqus/Standard
+
+# References
+
+• “Progressive damage and failure,” Section 24.1.1   
+• \*DAMAGE INITIATION
+
+# Overview
+
+The material damage initiation capability for ductile materials based on inelastic hysteresis energy:
+
+• is intended as a general capability for predicting initiation of damage in ductile materials in a lowcycle fatigue analysis;   
+• can be used in combination with the damage evolution law for ductile materials described in “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3; and   
+• can be used only in a low-cycle fatigue analysis using the direct cyclic approach (“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7).
+
+# Damage initiation criteria for ductile materials
+
+The damage initiation criterion is a phenomenological model for predicting the onset of damage due to stress reversals and the accumulation of inelastic strain in a low-cycle fatigue analysis. It is characterized by the accumulated inelastic hysteresis energy per cycle, $\Delta w$ , in a material point when the structure response is stabilized in the cycle. The cycle number in which damage is initiated is given by
+
+$$
+N _ {0} = c _ {1} \Delta w ^ {c _ {2}},
+$$
+
+where $c _ { 1 }$ and $c _ { 2 }$ are material constants. The value of $c _ { 1 }$ is dependent on the system of units in which you are working; some care is required to modify $c _ { 1 }$ when converting to a different system of units.
+
+The initiation criterion can be used in conjunction with any ductile material.
+
+Input File Usage: \*DAMAGE INITIATION, CRITERION=HYSTERESIS ENERGY
+
+# Elements
+
+The damage initiation criteria for ductile materials can be used with any elements in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom). This includes cohesive elements based on a continuum approach (“Modeling of an adhesive layer of finite thickness” in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5).
+
+<!-- source-page: 558 -->
+
+# Output
+
+In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variable has special meaning when a damage initiation criterion is specified:
+
+CYCLEINI
+
+Number of cycles to initialize the damage at the material point.
+
+<!-- source-page: 559 -->
+
+# 24.4.3 DAMAGE EVOLUTION FOR DUCTILE MATERIALS IN LOW-CYCLE FATIGUE
+
+Product: Abaqus/Standard
+
+# References
+
+• “Progressive damage and failure,” Section 24.1.1   
+• \*DAMAGE EVOLUTION
+
+# Overview
+
+The damage evolution capability for ductile materials based on inelastic hysteresis energy:
+
+• assumes that damage is characterized by the progressive degradation of the material stiffness, leading to material failure;   
+• must be used in combination with a damage initiation criterion for ductile materials in low-cycle fatigue analysis (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2);   
+• uses the inelastic hysteresis energy per stabilized cycle to drive the evolution of damage after damage initiation; and   
+• must be used in conjunction with the linear elastic material model (“Linear elastic behavior,” Section 22.2.1), the porous elastic material model (“Elastic behavior of porous materials,” Section 22.3.1), or the hypoelastic material model (“Hypoelastic behavior,” Section 22.4.1).
+
+# Damage evolution based on accumulated inelastic hysteresis energy
+
+Once the damage initiation criterion (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2) is satisfied at a material point, the damage state is calculated and updated based on the inelastic hysteresis energy for the stabilized cycle. The rate of the damage in a material point per cycle is given by
+
+$$
+\frac {d D}{d N} = \frac {c _ {3} \Delta w ^ {c _ {4}}}{L},
+$$
+
+where $c _ { 3 }$ and $c _ { 4 }$ are material constants, and is the characteristic length associated with an integration point. The value of $c _ { 3 }$ is dependent on the system of units in which you are working; some care is required to modify $c _ { 3 }$ when converting to a different system of units.
+
+For damage in ductile materials Abaqus/Standard assumes that the degradation of the elastic stiffness can be modeled using the scalar damage variable, . At any given loading cycle during the analysis the stress tensor in the material is given by the scalar damage equation
+
+$$
+\boldsymbol {\sigma} = (1 - D) \bar {\boldsymbol {\sigma}},
+$$
+
+<!-- source-page: 560 -->
+
+where is the effective (or undamaged) stress tensor that would exist in the material in the absence of damage computed in the current increment. The material has completely lost its load carrying capacity when . You can remove the element from the mesh if all of the section points at all integration locations have lost their loading carrying capability.
+
+Input File Usage: \*DAMAGE EVOLUTION, TYPE=HYSTERESIS ENERGY
+
+# Mesh dependency and characteristic length
+
+The implementation of the damage evolution model requires the definition of a characteristic length associated with an integration point. The characteristic length is based on the element geometry and formulation: it is a typical length of a line across an element for a first-order element; it is half of the same typical length for a second-order element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness. This definition of the characteristic length is used because the direction in which fracture occurs is not known in advance. Therefore, elements with large aspect ratios will have rather different behavior depending on the direction in which the damage occurs: some mesh sensitivity remains because of this effect, and elements that are as close to square as possible are recommended. However, since the damage evolution law is energy based, mesh dependency of the results may be alleviated.
+
+# Maximum degradation and element removal
+
+You can control how Abaqus/Standard treats elements with severe damage.
+
+# Defining the upper bound to the damage variable
+
+By default, the upper bound to all damage variables at a material point is $D _ { m a x } = 1 . 0$ . You can reduce this upper bound as discussed in “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4.
+
+Input File Usage: \*SECTION CONTROLS, MAX DEGRADATION=
+
+# Controlling element removal for damaged elements
+
+By default, in Abaqus/Standard an element is removed (deleted) once D reaches $D _ { \mathrm { m a x } }$ at all of the section points at all integration locations in the element. If an element is removed, the output variable STATUS is set to zero for the element, and it offers no resistance to subsequent deformation. However, the element still remains in the Abaqus/Standard model and may be visible during postprocessing. In the Visualization module of Abaqus/CAE, you can suppress the display of elements based on their status (see “Selecting the status field output variable,” Section 42.5.6 of the Abaqus/CAE User’s Guide, in the HTML version of this guide).
+
+Alternatively, you can specify that an element should remain in the model even after all of the damage variables reach $D _ { m a x }$ . In this case, once all the damage variables reach the maximum value, the stiffness remains constant.