김경종
11 KiB
Depending on what is being modeled, permanent set may be defined as the true permanent set seen in the material after recovery of viscoelastic strains or it may include viscoelastic strains. In either case, an initial yield stress is required, below which there will be no permanent set and the behavior of the material will be fully elastic. In the case of filled rubbers this initial yield stress may correspond to a small nonzero stress; whereas for the family of thermoplastic materials, there may be a more marked value of initial yield stress.
Input File Usage: *PLASTIC, HARDENING=ISOTROPIC
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic
Processing test data
If you have uniaxial and/or biaxial test data, as shown in Figure 23.7.1–1, you can use an interactive Abaqus/CAE plug-in to obtain the hyperelasticity, plasticity, and Mullins effect data. For information about the plug-in and instructions about its usage, see “Abaqus/CAE plug-in application for processing cyclic test data of filled elastomers and thermoplastics” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base.
Limitations
The model is intended to capture permanent set under multiaxial stress states and mild reverse loading conditions, as illustrated by Govindarajan, Hurtado, and Mars (2007). This model is not intended to capture deformation under complete reverse loading. Any rate effects apply only to the plastic part of the material definition.
Elements
Permanent set can be modeled with all element types that support the use of the hyperelastic material model.
Procedures
Permanent set modeling can be carried out in all procedures that support the use of the hyperelastic material model with the exception of the steady-state transport procedure. In linear perturbation steps in Abaqus/Standard, the current material tangent stiffness corresponding to the elastic part is used to determine the response, while ignoring any plasticity effects.
Output
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) corresponding to other isotropic hardening plasticity models can be obtained for permanent set models.
Additional references
• Govindarajan, S. M., J. A. Hurtado, and W. V. Mars, “Simulation of Mullins Effect in Filled Elastomers Using Multiplicative Decomposition,” European Conference for Constitutive Models for Rubber, September 2007, Paris, France.
• Simo, J. C., “Algorithms for Static and Dynamic Multiplicative Plasticity that Preserve the Classical Return Mapping Schemes of the Infinitesimal Theory,” Computer Methods in Applied Mechanics and Engineering, vol. 99, p. 61–112, 1992.
• Weber, G., and L. Anand, “Finite Deformation Constitutive Equations and Time Integration Procedure for Isotropic Hyperelastic-Viscoplastic Solids,” Computer Methods in Applied Mechanics and Engineering, vol. 79, p. 173–202, 1990.
24. Progressive Damage and Failure
Progressive damage and failure: overview 24.1
Damage and failure for ductile metals 24.2
Damage and failure for fiber-reinforced composites 24.3
Damage and failure for ductile materials in low-cycle fatigue analysis 24.4
24.1 Progressive damage and failure: overview
• “Progressive damage and failure,” Section 24.1.1
24.1.1 PROGRESSIVE DAMAGE AND FAILURE
Abaqus provides the following models to predict progressive damage and failure:
• Progressive damage and failure for ductile metals: Abaqus offers a general capability for modeling progressive damage and failure in ductile metals. The functionality can be used in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models (“Damage and failure for ductile metals: overview,” Section 24.2.1). The capability supports the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), Müschenborn-Sonne forming limit diagram (MSFLD), and Marciniak-Kuczynski (M-K) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The progressive damage models allow for a smooth degradation of the material stiffness, which makes them suitable for both quasi-static and dynamic situations, a great advantage over the dynamic failure models (“Dynamic failure models,” Section 23.2.8).
The Johnson-Cook and Marciniak-Kuczynski (M-K) damage initiation criteria are not available in Abaqus/Standard.
• Progressive damage and failure for fiber-reinforced materials: Abaqus offers a capability to model anisotropic damage in fiber-reinforced materials (“Damage and failure for fiber-reinforced composites: overview,” Section 24.3.1). The response of the undamaged material is assumed to be linearly elastic, and the model is intended to predict behavior of fiber-reinforced materials for which damage can be initiated without a large amount of plastic deformation. The Hashin’s initiation criteria are used to predict the onset of damage, and the damage evolution law is based on the energy dissipated during the damage process and linear material softening.
• Progressive damage and failure for ductile materials in low-cycle fatigue analysis: Abaqus/Standard offers a capability to model progressive damage and failure for ductile materials due to stress reversals and the accumulation of inelastic strain in a low-cycle fatigue analysis using the direct cyclic approach (see “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7). The damage initiation criterion and damage evolution are characterized by the accumulated inelastic hysteresis energy per stabilized cycle (see “Damage and failure for ductile materials in low-cycle fatigue analysis: overview,” Section 24.4.1). After damage initiation, the elastic material stiffness is degraded progressively according to the specified damage evolution response.
In addition, Abaqus offers a concrete damaged model (“Concrete damaged plasticity,” Section 23.6.3), dynamic failure models (“Dynamic failure models,” Section 23.2.8), and specialized capabilities for modeling damage and failure in cohesive elements (“Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6) and in connectors (“Connector damage behavior,” Section 31.2.7).
This section provides an overview of the progressive damage and failure capability and a brief description of the concepts of damage initiation and evolution. The discussion in this section is limited to damage models for ductile metals and fiber-reinforced materials.
Abaqus offers a general framework for material failure modeling that allows the combination of multiple failure mechanisms acting simultaneously on the same material. Material failure refers to the complete loss of load-carrying capacity that results from progressive degradation of the material stiffness. The stiffness degradation process is modeled using damage mechanics.
To help understand the failure modeling capabilities in Abaqus, consider the response of a typical metal specimen during a simple tensile test. The stress-strain response, such as that illustrated in Figure 24.1.1–1, will show distinct phases. The material response is initially linear elastic, a \mathrm { ~ - ~ } b , , followed by plastic yielding with strain hardening, b - c . Beyond point c there is a marked reduction of load-carrying capacity until rupture, c - d . . The deformation during this last phase is localized in a neck region of the specimen. Point c identifies the material state at the onset of damage, which is referred to as the damage initiation criterion. Beyond this point, the stress-strain response c - d is governed by the evolution of the degradation of the stiffness in the region of strain localization. In the context of damage mechanics c - d can be viewed as the degraded response of the curve c - d ^ { \prime } that the material would have followed in the absence of damage.
text_image
σ a b c d d' ε
Figure 24.1.1–1 Typical uniaxial stress-strain response of a metal specimen.
Thus, in Abaqus the specification of a failure mechanism consists of four distinct parts:
• the definition of the effective (or undamaged) material response ( { \bf e . g . } , \ a \ - \ b \ - \ c \ - \ d ^ { \prime } in Figure 24.1.1–1),
• a damage initiation criterion (e.g., c in Figure 24.1.1–1),
• a damage evolution law ( \boldsymbol { \mathrm { e } } . \boldsymbol { \mathrm { g } } . , c - d in Figure 24.1.1–1), and
• a choice of element deletion whereby elements can be removed from the calculations once the material stiffness is fully degraded (e.g., d in Figure 24.1.1–1).
These parts will be discussed separately for ductile metals (“Damage and failure for ductile metals: overview,” Section 24.2.1) and fiber-reinforced materials (“Damage and failure for fiber-reinforced composites: overview,” Section 24.3.1).
Mesh dependency
In continuum mechanics the constitutive model is normally expressed in terms of stress-strain relations. When the material exhibits strain-softening behavior, leading to strain localization, this formulation results in a strong mesh dependency of the finite element results in that the energy dissipated decreases upon mesh refinement. In Abaqus all of the available damage evolution models use a formulation intended to alleviate the mesh dependency. This is accomplished by introducing a characteristic length into the formulation, which in Abaqus is related to the element size, and expressing the softening part of the constitutive law as a stress-displacement relation. In this case the energy dissipated during the damage process is specified per unit area, not per unit volume. This energy is treated as an additional material parameter, and it is used to compute the displacement at which full material damage occurs. This is consistent with the concept of critical energy release rate as a material parameter for fracture mechanics. This formulation ensures that the correct amount of energy is dissipated and greatly alleviates the mesh dependency.