Processing math: 100%

Damage Evolution for Ductile Materials in Low-Cycle Fatigue

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);
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), the porous elastic material model (Elastic Behavior of Porous Materials), or the hypoelastic material model (Hypoelastic Behavior).

This page discusses:

Damage Evolution Based on Accumulated Inelastic Hysteresis Energy Density
Maximum Degradation and Element Removal
Elements
Output

Damage Evolution Based on Accumulated Inelastic Hysteresis Energy Density

Once the damage initiation criterion (Damage Initiation for Ductile Materials in Low-Cycle Fatigue) is satisfied at a material point, the damage state is calculated and updated based on the accumulated inelastic hysteresis energy density per cycle, $Δ w$ , for a stabilized cycle. The rate of the damage in a material point per cycle is given by

$\frac{d D}{d N} = \frac{c_{3} {(Δ w / Δ {\bar{w}}_{0})}^{c_{4}}}{L},$

where $c_{3}$ and $c_{4}$ are material constants, $L$ is the characteristic length associated with an integration point, and ${Δ \bar{w}}_{0}$ is a reference value of the accumulated inelastic hysteresis energy density per cycle.

The use of the reference energy density, ${Δ \bar{w}}_{0}$ , makes the above form of the damage evolution law different from the more standard Coffin-Manson type relations. It is recommended that for ${Δ \bar{w}}_{0}$ (which has units of energy density), you choose a value of 1.0 in the unit system in which the evolution law is calibrated to the available test data. If a different unit system is then used, you must convert the material constant $c_{3}$ based on its dimension of length per cycle. In this case, you must also convert ${Δ \bar{w}}_{0}$ appropriately to the new system to ensure that the physical results are invariant to the choice of the unit system.

For damage in ductile materials Abaqus/Standard assumes that the degradation of the elastic stiffness can be modeled using the scalar damage variable, $D$ . At any given loading cycle during the analysis the stress tensor in the material is given by the scalar damage equation

$σ = (1 - D) \bar{σ},$

where $\bar{σ}$ 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 $D = 1$ . 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

Use the following option to specify a reference accumulated inelastic hysteresis energy density per cycle:

DAMAGE EVOLUTION, TYPE=HYSTERESIS ENERGY, REF ENERGY= ${Δ \bar{w}}_{0}$

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.

Input File Usage

SECTION CONTROLS, MAX DEGRADATION= $D_{\max}$

Controlling Element Removal for Damaged Elements

A material point is considered to fail once D reaches $D_{\max}$ . By default, an element is deleted from a mesh upon material failure. Details for element deletion driven by material failure are discussed in Material Failure and Element Deletion. The status of an element can be determined by requesting output variable STATUS.

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 of the damage variables reach the maximum value, the stiffness remains constant.

Input File Usage

Use the following option to delete failed elements from the mesh (default):

SECTION CONTROLS, ELEMENT DELETION=YES

Use the following option to keep failed elements in the mesh computations:

SECTION CONTROLS, ELEMENT DELETION=NO

Elements

Damage evolution for ductile materials can be defined for any element that can be used with the damage initiation criteria for a low-cycle fatigue analysis in Abaqus/Standard (Damage Initiation for Ductile Materials in Low-Cycle Fatigue).

Output

In addition to the standard output identifiers available in Abaqus/Standard (Abaqus/Standard Output Variable Identifiers), the following variables have special meaning when damage evolution is specified:

STATUS: Status of the 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.