MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide3/AbaqusAnalysisUserGuide3_053.md

Initial conditions

When we need to study the behavior of a material that has been previously subjected to deformations, such as those originated during the manufacturing process, initial equivalent plastic strain values can be provided to specify the initial work hardened state of the material (see “Defining initial values of state variables for plastic hardening” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1).

In addition, when the initial equivalent plastic strain is greater than the minimum value on the forming limit curve, the initial value of plays an important role in determining whether the MSFLD damage initiation criterion will be met during subsequent deformation. It is, therefore, important to specify the initial value of in these situations. To this end, you can specify initial values of the plastic strain tensor (see “Defining initial values of plastic strain” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). Abaqus will use this information to compute the initial value of as the ratio of the minor and major principal plastic strains; that is, neglecting the elastic component of deformation and assuming a linear deformation path.

Input File Usage: Use both of the following options to specify that material hardening and plastic strain have occurred prior to the current analysis:

*INITIAL CONDITIONS, TYPE=HARDENING

*INITIAL CONDITIONS, TYPE=PLASTIC STRAIN

Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step

Initial plastic strain conditions are not supported in Abaqus/CAE.

Elements

The damage initiation criteria for ductile metals can be used with any elements in Abaqus that include mechanical behavior (elements that have displacement degrees of freedom) except for the pipe elements in Abaqus/Explicit.

The models for sheet metal necking instability (FLD, FLSD, MSFLD, and M-K) are available only with elements that include mechanical behavior and use a plane stress formulation (i.e., plane stress, shell, continuum shell, and membrane elements).

Output

In addition to the standard output identifiers available in Abaqus (“Output variables,” Section 4.2), the following variables have special meaning when a damage initiation criterion is specified:

ERPRATIO Ratio of principal strain rates, , used for the MSFLD damage initiation criterion.

SHRRATIO Shear stress ratio, \theta _ { s } = ( q + k _ { s } p ) / \tau _ { \mathrm { m a x } } , used for the evaluation of the shear damage initiation criterion.

TRIAX Stress triaxiality, \eta = - p / q (available in Abaqus/Standard only in conjunction with damage initiation).

DMICRT	All damage initiation criteria components listed below.
DUCTCRT	Ductile damage initiation criterion, $\omega_{D}$ .
JCCRT	Johnson-Cook damage initiation criterion (available only in Abaqus/Explicit).
SHRCRT	Shear damage initiation criterion, $\omega_{S}$ .
FLDCRT	Maximum value of the FLD damage initiation criterion, $\omega_{FLD}$ , during the analysis.
FLSDCRT	Maximum value of the FLSD damage initiation criterion, $\omega_{FSLD}$ , during the analysis.
MSFLDCRT	Maximum value of the MSFLD damage initiation criterion, $\omega_{MSFLD}$ , during the analysis.
MKCRT	Marciniak-Kuczynski damage initiation criterion (available only in Abaqus/Explicit), $\omega_{MK}$ .

A value of 1 or greater for output variables associated with a damage initiation criterion indicates that the criterion has been met. Abaqus will limit the maximum value of the output variable to 1 if a damage evolution law has been prescribed for that criterion (see “Damage evolution and element removal for ductile metals,” Section 24.2.3). However, if no damage evolution is specified, the criterion for damage initiation will continue to be computed beyond the point of damage initiation; in this case the output variable can take values greater than 1, indicating by how much the initiation criterion has been exceeded.

Additional references

• Hooputra, H., H. Gese, H. Dell, and H. Werner, “A Comprehensive Failure Model for Crashworthiness Simulation of Aluminium Extrusions,” International Journal of Crashworthiness, vol. 9, no. 5, pp. 449–464, 2004.
• Bai, Y., and T. Wierzbicki, “A New Model of Metal Plasticity and Fracture with Pressure and Lode Dependence,” International Journal of Plasticity, vol. 24, no. 6, pp. 1071–1096, 2008.
• Johnson, G. R., and W. H. Cook, “Fracture Characteristics of Three Metals Subjected to Various Strains, Strain rates, Temperatures and Pressures,” Engineering Fracture Mechanics, vol. 21, no. 1, pp. 31–48, 1985.
• Keeler, S. P., and W. A. Backofen, “Plastic Instability and Fracture in Sheets Stretched over Rigid Punches,” ASM Transactions Quarterly, vol. 56, pp. 25–48, 1964.
• Marciniak, Z., and K. Kuczynski, “Limit Strains in the Processes of Stretch Forming Sheet Metal,” International Journal of Mechanical Sciences, vol. 9, pp. 609–620, 1967.
• Müschenborn, W., and H. Sonne, “Influence of the Strain Path on the Forming Limits of Sheet Metal,” Archiv fur das Eisenhüttenwesen, vol. 46, no. 9, pp. 597–602, 1975.
• Stoughton, T. B., “A General Forming Limit Criterion for Sheet Metal Forming,” International Journal of Mechanical Sciences, vol. 42, pp. 1–27, 2000.

24.2.3 DAMAGE EVOLUTION AND ELEMENT REMOVAL FOR DUCTILE METALS

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

References

• “Progressive damage and failure,” Section 24.1.1
• *DAMAGE EVOLUTION
• “Damage evolution” in “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

Overview

The damage evolution capability for ductile metals:

• 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 metals (“Damage initiation for ductile metals,” Section 24.2.2);
• uses mesh-independent measures (either plastic displacement or physical energy dissipation) to drive the evolution of damage after damage initiation;
• takes into account the combined effect of different damage mechanisms acting simultaneously on the same material and includes options to specify how each mechanism contributes to the overall material degradation; and
• offers options for what occurs upon failure, including the removal of elements from the mesh.

Damage evolution

Figure 24.2.3–1 illustrates the characteristic stress-strain behavior of a material undergoing damage. In the context of an elastic-plastic material with isotropic hardening, the damage manifests itself in two forms: softening of the yield stress and degradation of the elasticity. The solid curve in the figure represents the damaged stress-strain response, while the dashed curve is the response in the absence of damage. As discussed later, the damaged response depends on the element dimensions such that mesh dependency of the results is minimized.

In the figure \sigma _ { y 0 } and \bar { \varepsilon } _ { 0 } ^ { p l } are the yield stress and equivalent plastic strain at the onset of damage, and \bar { \varepsilon } _ { f } ^ { p l } is the equivalent plastic strain at failure; that is, when the overall damage variable reaches the value \dot { D } = 1 . The overall damage variable, D, captures the combined effect of all active damage mechanisms and is computed in terms of the individual damage variables, d _ { i } , as discussed later in this section (see “Evaluating overall damage when multiple criteria are active”).

The value of the equivalent plastic strain at failure, \bar { \varepsilon } _ { f } ^ { p l } , depends on the characteristic length of the element and cannot be used as a material parameter for the specification of the damage evolution law.

line

Point	ε	σ
(D=0)	0	σ_y0
(1-D)E	ε_f^pl	σ_f^pl
D σ̄	ε̅_0^pl	σ̄_0

Figure 24.2.3–1 Stress-strain curve with progressive damage degradation.

Instead, the damage evolution law is specified in terms of equivalent plastic displacement, \bar { u } ^ { p l } , or in terms of fracture energy dissipation, G _ { f } ; these concepts are defined next.

Mesh dependency and characteristic length

When material damage occurs, the stress-strain relationship no longer accurately represents the material’s behavior. Continuing to use the stress-strain relation introduces a strong mesh dependency based on strain localization, such that the energy dissipated decreases as the mesh is refined. A different approach is required to follow the strain-softening branch of the stress-strain response curve. Hillerborg’s (1976) fracture energy proposal is used to reduce mesh dependency by creating a stress-displacement response after damage is initiated. Using brittle fracture concepts, Hillerborg defines the energy required to open a unit area of crack, G _ { f } , as a material parameter. With this approach, the softening response after damage initiation is characterized by a stress-displacement response rather than a stress-strain response.

The implementation of this stress-displacement concept in a finite element model requires the definition of a characteristic length, L , associated with an integration point. The fracture energy is then given as

G _ {f} = \int_ {\bar {\varepsilon} _ {0} ^ {p l}} ^ {\bar {\varepsilon} _ {f} ^ {p l}} L \sigma_ {y} d \bar {\varepsilon} ^ {p l} = \int_ {0} ^ {\bar {u} _ {f} ^ {p l}} \sigma_ {y} d \bar {u} ^ {p l}.

This expression introduces the definition of the equivalent plastic displacement, \bar { u } ^ { p l } , as the fracture work conjugate of the yield stress after the onset of damage (work per unit area of the crack). Before damage initiation \dot { \bar { u } } ^ { p l } = \bar { 0 } ; after damage initiation \dot { \bar { u } } ^ { p l } = L \bar { \bar { \varepsilon } } ^ { p l } .

The definition of the characteristic length depends 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 they crack: some mesh sensitivity remains because of this effect, and elements that have aspect ratios close to unity are recommended. Alternatively, this mesh dependency could be reduced by directly specifying the characteristic length as a function of the element topology and material orientation in user subroutine VUCHARLENGTH (see “Defining the characteristic element length at a material point in Abaqus/Explicit” in “Material data definition,” Section 21.1.2).

Each damage initiation criterion described in “Damage initiation for ductile metals,” Section 24.2.2, may have an associated damage evolution law. The damage evolution law can be specified in terms of equivalent plastic displacement, \bar { u } ^ { p l } , or in terms of fracture energy dissipation, G _ { f } . Both of these options take into account the characteristic length of the element to alleviate mesh dependency of the results.

Evaluating overall damage when multiple criteria are active

The overall damage variable, D, captures the combined effect of all active mechanisms and is computed in terms of individual damage variables, d _ { i ; } , for each mechanism. You can choose to combine some of the damage variables in a multiplicative sense to form an intermediate variable, d _ { \mathrm { m u l t } } , as follows:

d _ {\mathrm{mult}} = 1 - \prod_ {k \in N _ {\mathrm{mult}}} (1 - d _ {k}).

Then, the overall damage variable is computed as the maximum of d _ { \mathrm { m u l t } } and the remaining damage variables:

D = \max \left\{d _ {\mathrm{mult}}, \max _ {j \in N _ {\mathrm{max}}} (d _ {j}) \right\}.

In the above expressions N _ { \mathrm { m u l t } } and N _ { \mathrm { m a x } } represent the sets of active mechanisms that contribute to the overall damage in a multiplicative and a maximum sense, respectively, with N _ { \mathrm { a c t } } = N _ { \mathrm { m u l t } } \cup N _ { \mathrm { m a x } } .

Input File Usage:

Use the following option to specify that the damage associated with a particular criterion contributes to the overall damage variable in a maximum sense (default):

* { \mathrm { D A M A G E ~ E V O L U T I O N } } , { \mathrm { D E G R A D A T I O N } } { \mathrm { = M A X I M U M } }

Use the following option to specify that the damage associated with a particular criterion contributes to the overall damage variable in a multiplicative sense:

*DAMAGE EVOLUTION, DEGRADATION=MULTIPLICATIVE

Abaqus/CAE Usage:

Use the following options to specify that the damage associated with a particular criterion contributes to the overall damage variable in a maximum sense (default) or in a multiplicative sense, respectively:

Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Degradation: Maximum or Multiplicative

Defining damage evolution based on effective plastic displacement

As discussed previously, once the damage initiation criterion has been reached, the effective plastic displacement, \bar { u } ^ { p l } , is defined with the evolution equation

\dot {\bar {u}} ^ {p l} = L \dot {\bar {\varepsilon}} ^ {p l},

where L is the characteristic length of the element.

The evolution of the damage variable with the relative plastic displacement can be specified in \bar { u } _ { f } ^ { p l } ular, linear, or exponential form. Instantaneous failure will occur if the plastic displacement at failure,, is specified as 0; however, this choice is not recommended and should be used with care because it causes a sudden drop of the stress at the material point that can lead to dynamic instabilities.

Tabular form

You can specify the damage variable directly as a tabular function of equivalent plastic displacement, d = d ( \bar { u } ^ { p l } ) , as shown in Figure 24.2.3–2(a).

Input File Usage: \mathrm { * D A M A G E ~ E V O L U T I O N } , \mathrm { T Y P E = D I S P L A C E M E N T } , \mathrm { S O F T E N I N G { = } T A B U L A R }

Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Type: Displacement: Softening: Tabular

Linear form

Assume a linear evolution of the damage variable with effective plastic displacement, as shown in Figure 24.2.3–2(b). You can specify the effective plastic displacement, \bar { u } _ { f } ^ { p l } , at the point of failure (full degradation). Then, the damage variable increases according to

\dot {d} = \frac {L \dot {\bar {\varepsilon}} ^ {p l}}{\bar {u} _ {f} ^ {p l}} = \frac {\dot {\bar {u}} ^ {p l}}{\bar {u} _ {f} ^ {p l}}.

This definition ensures that when the effective plastic displacement reaches the value \bar { u } ^ { p l } = \bar { u } _ { f } ^ { p l } , the material stiffness will be fully degraded ( ). The linear damage evolution law defines a truly linear stress-strain softening response only if the effective response of the material is perfectly plastic (constant yield stress) after damage initiation.

Input File Usage: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, \mathrm { S O F T E N I N G { = } L I N E A R }

(a) tabular

(b) linear

line

α	ū_f^pl	d
0	0	0
1	0.5	0.5
3	0.75	0.75
10	1	1

(c) exponential
Figure 24.2.3–2 Different definitions of damage evolution based on plastic displacement: (a) tabular, (b) linear, and (c) exponential.

Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Type: Displacement: Softening: Linear

Exponential form

Assume an exponential evolution of the damage variable with plastic displacement, as shown in Figure 24.2.3–2(c). You can specify the relative plastic displacement at failure, \bar { u } _ { f } ^ { p l } , and the exponent . The damage variable is given as

d = \frac {1 - e ^ {- \alpha (\bar {u} ^ {p l} / \bar {u} _ {f} ^ {p l})}}{1 - e ^ {- \alpha}}.

Input File Usage: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=EXPONENTIAL

Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Type: Displacement: Softening: Exponential

Defining damage evolution based on energy dissipated during the damage process

You can specify the fracture energy per unit area, G _ { f } , to be dissipated during the damage process directly. Instantaneous failure will occur if G _ { f } is specified as 0. However, this choice is not recommended and should be used with care because it causes a sudden drop in the stress at the material point that can lead to dynamic instabilities.

The evolution in the damage can be specified in linear or exponential form.

Linear form

Assume a linear evolution of the damage variable with plastic displacement. You can specify the fracture energy per unit area, G _ { f } . Then, once the damage initiation criterion is met, the damage variable increases according to

\dot {d} = \frac {L \dot {\bar {\varepsilon}} ^ {p l}}{\bar {u} _ {f} ^ {p l}} = \frac {\dot {\bar {u}} ^ {p l}}{\bar {u} _ {f} ^ {p l}},

where the equivalent plastic displacement at failure is computed as

\bar {u} _ {f} ^ {p l} = \frac {2 G _ {f}}{\sigma_ {y 0}}

and \sigma _ { y 0 } is the value of the yield stress at the time when the failure criterion is reached. Therefore, the model becomes equivalent to that shown in Figure 24.2.3–2(b). The model ensures that the energy dissipated during the damage evolution process is equal to G _ { f } only if the effective response of the material is perfectly plastic (constant yield stress) beyond the onset of damage.

Input File Usage: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=LINEAR

Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Type: Energy: Softening: Linear

Exponential form

Assume an exponential evolution of the damage variable given as

d = 1 - \exp \left(- \int_ {0} ^ {\bar {u} ^ {p l}} \frac {\bar {\sigma} _ {y} d \bar {u} ^ {p l}}{G _ {f}}\right).

The formulation of the model ensures that the energy dissipated during the damage evolution process is equal to G _ { f } , as shown in Figure 24.2.3–3(a). In theory, the damage variable reaches a value of 1 only asymptotically at infinite equivalent plastic displacement (Figure 24.2.3–3(b)). In practice, Abaqus/Explicit will set d equal to one when the dissipated energy reaches a value of 0 . 9 9 G _ { f } .

Input File Usage: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=EXPONENTIAL

Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Type: Energy: Softening: Exponential

text_image

σ_y σ_yo G_f ū^pl

(a)

line

| ū^pl | d | |------|-----| | 0 | 0 | | >0 | 1 |

(b)
Figure 24.2.3–3 Energy-based damage evolution with exponential law: evolution of (a) yield stress and (b) damage variable.

Maximum degradation and choice of element removal

You have control over how Abaqus treats elements with severe damage. You can specify an upper bound, D _ { \mathrm { m a x } } . to the overall damage variable, D; and you can choose whether to delete an element once maximum degradation is reached. The latter choice also affects which stiffness components are damaged.

Specifying the value of maximum degradation

The default setting of D _ { \mathrm { m a x } } depends on whether elements are to be deleted upon reaching maximum degradation (discussed next). For the default case of element deletion and in all cases for cohesive elements, D _ { \mathrm { m a x } } = 1 . 0 ; otherwise, D _ { \mathrm { m a x } } = 0 . 9 9 . The output variable SDEG contains the value of D. No further damage is accumulated at an integration point once D reaches D _ { \mathrm { m a x } } (except, of course, any remaining stiffness is lost upon element deletion).

Input File Usage: Use the following option to specify D _ { \mathrm { m a x } } :

* \text { SECTION   CONTROLS,   MAX   DEGRADATION } = D _ {\max}

Removing the element from the mesh

Elements are deleted by default upon reaching maximum degradation. Except for cohesive elements with traction-separation response (see “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6), Abaqus applies damage to all stiffness components equally for elements that may eventually be removed:

\boldsymbol {\sigma} = (1 - D) \bar {\boldsymbol {\sigma}}.

In Abaqus/Standard an element is removed from the mesh if D reaches D _ { \mathrm { m a x } } at all of the section points at all the integration locations of an element except for cohesive elements (for cohesive elements the conditions for element deletion are that D reaches D _ { \mathrm { m a x } } at all integration points and, for tractionseparation response, none of the integration points are in compression).

In Abaqus/Explicit an element is removed from the mesh if D reaches D _ { \mathrm { m a x } } at all of the section points at any one integration location of an element except for cohesive elements (for cohesive elements the conditions for element deletion are that D reaches D _ { \mathrm { m a x } } at all integration points and, for tractionseparation response, none of the integration points are in compression). For example, removal of a solid element takes place, by default, when maximum degradation is reached at any one integration point. However, in a shell element all through-the-thickness section points at any one integration location of an element must fail before the element is removed from the mesh. In the case of second-order reducedintegration beam elements, reaching maximum degradation at all section points through the thickness at either of the two element integration locations along the beam axis leads, by default, to element removal. Similarly, in modified triangular and tetrahedral solid elements and fully integrated membrane elements D reaching D _ { \mathrm { m a x } } at any one integration point leads, by default, to element removal.

In a heat transfer analysis the thermal properties of the material are not affected by the progressive damage of the material stiffness until the condition for element deletion is reached; at this point the thermal contribution of the element is also removed.