You use the Edit Material dialog box to specify material damage initiation criteria and associated damage evolution. Once an initiation criterion is met, Abaqus applies the associated damage evolution law to determine the material degradation. You can specify the following types of damage in Abaqus/CAE:
Ductile; see “Ductile damage”
FLD; see “Forming limit diagram (FLD) damage”
FLSD; see “Forming limit stress diagram (FLSD) damage”
Johnson-Cook; see “Johnson-Cook damage”
Maxe or Quade; see “Maximum or quadratic nominal strain damage”
Maxs or Quads; see “Maximum or quadratic nominal stress damage”
Maxps or Maxpe; see “Maximum principal stress or strain damage”
M-K; see “Marciniak-Kuczynski (M-K) damage”
MSFLD; see “Müschenborn-Sonne forming limit diagram (MSFLD) damage”
Shear; see “Shear damage”
Hashin; see “Hashin damage”
Mullins Effect; see “Mullins effect”
In addition to damage initiation and evolution, Abaqus/Standard uses a viscous regularization scheme to improve convergence as fiber-reinforced composite materials (Hashin damage model) are damaged. “Damage stabilization” lists the viscous coefficients required for this scheme.
For more information on material damage, see Chapter 24, “Progressive Damage and Failure,” of the Abaqus Analysis User's Guide.
The Ductile damage initiation criterion is a model for predicting the onset of damage due to nucleation, growth, and coalescence of voids in ductile metals. The model assumes that the equivalent plastic strain at the onset of damage is a function of stress triaxiality and strain rate. The ductile criterion can be used in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models, including equation of state.
For more information, see “Damage initiation for ductile metals,” Section 24.2.2 of the Abaqus Analysis User's Guide.
To define ductile damage:
From the menu bar in the Edit Material dialog box, select Mechanical
Damage for Ductile MetalsDuctile Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
Fracture Strain
Equivalent fracture strain at damage initiation.
Stress Triaxiality
The stress triaxiality is defined as 
, where p is the pressure stress and q is the Mises equivalent stress.
Strain Rate
The equivalent plastic strain rate, 
.
Temp
Temperature, 
.
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Click OK to exit the material editor.
A forming limit diagram (FLD) is a plot of the forming limit strains in the space of principal (in-plane) logarithmic strains. The FLD damage initiation criterion is intended to predict the onset of necking instability in sheet metal forming. The maximum strains that a sheet material can sustain prior to the onset of necking are referred to as the forming limit strains.
Damage due to bending deformation cannot be evaluated using this model. For more information, see “Damage initiation for ductile metals,” Section 24.2.2 of the Abaqus Analysis User's Guide.
To define FLD damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Ductile MetalsFLD Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
Major Principal Strain
The maximum value of the in-plane principal limit strain.
Minor Principal Strain
The minimum value of the in-plane principal limit strain.
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Click OK to exit the material editor.
The FLSD damage initiation criterion is intended to predict the onset of necking instability in sheet metal forming. The strain-based forming limit curves (as used in the FLD criterion) are converted to stress-based curves to reduce the dependence on the strain path. This improves the performance of the FLSD damage model under conditions of arbitrary loading.
Similar to the FLD criterion, damage due to bending deformation cannot be evaluated using this model. For more information, see “Damage initiation for ductile metals,” Section 24.2.2 of the Abaqus Analysis User's Guide.
To define FLSD damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Ductile MetalsFLSD Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
Major Principal Stress
The maximum value of the in-plane principal limit stress.
Minor Principal Stress
The minimum value of the in-plane principal limit stress.
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Click OK to exit the material editor.
The Johnson-Cook damage initiation criterion is a special case of the ductile damage criterion model for predicting the onset of damage due to nucleation, growth, and coalescence of voids in ductile metals. The model assumes that the equivalent plastic strain at the onset of damage is a function of stress triaxiality and strain rate. The Johnson-Cook criterion can be used in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models, including equation of state.
For more information, see “Damage initiation for ductile metals,” Section 24.2.2 of the Abaqus Analysis User's Guide.
To define Johnson-Cook damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Ductile MetalsJohnson-Cook Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Enter damage parameters in the Data table:
–
Failure parameters.
Melting temperature
.
Transition temperature
.
Reference strain rate
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Click OK to exit the material editor.
The Maxe and Quade damage initiation criteria are used to predict damage initiation in cohesive elements where the cohesive layers are defined in terms of traction-separation. Both forms evaluate the strain ratios between a given strain value and the peak nominal strain value in each of three directions. 
, 
, and 
represent the peak values of the nominal strain when the deformation is either purely normal to the interface or purely in the first or the second shear direction, respectively. The Maxe criterion is based on the maximum value of the three ratios, whereas the Quade criterion is based on a quadratic combination of all three ratios.
For more information, see “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6 of the Abaqus Analysis User's Guide.
To define Maxe or Quade damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Traction Separation LawsMaxe Damage or Quade Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
If you are using the extended finite element method (XFEM) to model fracture, you can specify the crack propagation direction when the damage initiation criterion is satisfied. The crack can extend at a direction Normal to the local 1-direction (default) or Parallel to the local 1-direction.
Enter the Tolerance. The value should be equal to the tolerance within which the damage initiation criterion must be satisfied.
Select the arrow to the right of the Position field, and select the method for computing the stress/strain fields ahead of the crack tip to determine if the damage initiation criterion is satisfied and to determine the crack propagation direction (if needed):
Select Centroid to use the stress/strain at the element centroid.
Select Crack tip to use the stress/strain extrapolated to the crack tip.
Select Combined to use the stress/strain extrapolated to the crack tip to determine if the damage initiation criterion is satisfied and to use the stress/strain at the element centroid to determine the crack propagation direction (if needed).
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
Nominal Strain Normal-only Mode
Nominal strain at damage initiation in a normal-only mode.
Nominal Strain Shear-only mode First Direction
Nominal strain at damage initiation in a shear-only mode that involves separation only along the first shear direction.
Nominal Strain Shear-only mode Second Direction
Nominal strain at damage initiation in a shear-only mode that involves separation only along the second shear direction.
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Select SuboptionsDamage Stabilization Cohesive to enter viscous coefficients and improve the model convergence.
For more information, see “Damage stabilization.”
Click OK to exit the material editor.
The Maxs and Quads damage initiation criteria are used to predict damage initiation in cohesive elements where the cohesive layers are defined in terms of traction-separation. Both forms evaluate the stress ratios between a given stress value and the peak nominal stress value in each of three directions. 
, 
, and 
represent the peak values of the nominal stress when the deformation is either purely normal to the interface or purely in the first or the second shear direction, respectively. The Maxs criterion is based on the maximum value of the three ratios, whereas the Quads criterion is based on a quadratic combination of all three ratios.
For more information, see “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6 of the Abaqus Analysis User's Guide.
To define Maxs or Quads damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Traction Separation LawsMaxs Damage or Quads Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
If you are using the extended finite element method (XFEM) to model fracture, you can choose the crack propagation direction when the damage initiation criterion is satisfied. The crack can extend at a direction normal to the element local 1-direction (default) or parallel to the element local 1-direction.
Enter the Tolerance. The value should be equal to the tolerance within which the damage initiation criterion must be satisfied.
Select the arrow to the right of the Position field, and select the method for computing the stress/strain fields ahead of the crack tip to determine if the damage initiation criterion is satisfied and to determine the crack propagation direction (if needed):
Select Centroid to use the stress/strain at the element centroid.
Select Crack tip to use the stress/strain extrapolated to the crack tip.
Select Combined to use the stress/strain extrapolated to the crack tip to determine if the damage initiation criterion is satisfied and to use the stress/strain at the element centroid to determine the crack propagation direction (if needed).
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
Maximum Nominal Stress Normal-only Mode
Nominal stress at damage initiation in a normal-only mode.
Maximum Nominal Stress Shear-only mode First Direction
Nominal stress at damage initiation in a shear-only mode that involves separation only along the first shear direction.
Maximum Nominal Stress Shear-only mode Second Direction
Nominal stress at damage initiation in a shear-only mode that involves separation only along the second shear direction.
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Select SuboptionsDamage Stabilization Cohesive to enter viscous coefficients and improve the model convergence.
For more information, see “Damage stabilization.”
Click OK to exit the material editor.
The Maxps and Maxpe damage initiation criteria are used to predict damage initiation in the XFEM enriched region.
For more information, see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1 of the Abaqus Analysis User's Guide.
To define Maxps or Maxpe damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Traction Separation LawsMaxps Damage or Maxpe Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Enter the Tolerance. The value should be equal to the tolerance within which the damage initiation criterion must be satisfied.
Select the arrow to the right of the Position field, and select the method for computing the stress/strain fields ahead of the crack tip to determine if the damage initiation criterion is satisfied and to determine the crack propagation direction (if needed):
Select Centroid to use the stress/strain at the element centroid.
Select Crack tip to use the stress/strain extrapolated to the crack tip.
Select Combined to use the stress/strain extrapolated to the crack tip to determine if the damage initiation criterion is satisfied and to use the stress/strain at the element centroid to determine the crack propagation direction (if needed).
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
Maximum Principal Stress or Maximum Principal Strain
Maximum principal stress or strain at damage initiation.
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Select SuboptionsDamage Stabilization Cohesive to enter the viscous coefficient and improve the model convergence.
For more information, see “Damage stabilization.”
Click OK to exit the material editor.
The M-K damage initiation criterion is used to predict sheet metal forming limits for arbitrary loading paths. The model introduces thickness imperfections, in the form of grooves, in the sheet material to simulate defects. Damage occurs when the ratio of deformation in the grooves relative to deformation in the original sheet thickness exceeds a critical value. By default, Abaqus evaluates four grooves at equally spaced angles of 0°, 45°, 90°, and 135° with respect to the local 1-direction of the material at each time increment and uses the worst result to determine damage initiation. The M-K criterion can be used in conjunction with the Mises and Johnson-Cook plasticity models, including kinematic hardening.
For more information, see “Damage initiation for ductile metals,” Section 24.2.2 of the Abaqus Analysis User's Guide.
To define M-K damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Ductile MetalsM-K Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
If desired, modify the critical deformation severity factors 
, 
, and 
.
The severity factors each have a default value of 10 and are related to the ratios of equivalent plastic, normal, and tangential strain in the groove area compared to the nominal thickness area. Abaqus/Explicit will ignore severity factors that are set to 0. If all of these parameters are set equal to zero, the M-K criterion is based solely on nonconvergence of the equilibrium and compatibility equations.
Select the Frequency—the number of increments between calculating the M-K criterion.
Using the default frequency, 1, can be expensive since Abaqus evaluates each groove at every increment.
Select the Number of imperfections—the number of angular groove positions to evaluate.
The groove positions are equally spaced, starting at 0° and ending at 
with respect to the local 1-direction of the material.
Enter damage parameters in the Data table:
Groove Size
The ratio of the thickness at the groove to the nominal material thickness.
Angle
The starting angle (in degrees) with respect to the 1-direction of the local material orientation.
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Click OK to exit the material editor.
The MSFLD damage initiation criterion is used to predict sheet metal forming limits for arbitrary loading paths. The model works on the basis of equivalent plastic strain and assumes that the forming limit curve represents the sum of the highest attainable equivalent plastic strains. The approach requires transforming the original forming limit curve (without predeformation effects) from the space of major versus minor strains to the space of equivalent plastic strain, 
, versus ratio of principal strain rates, 
.
Damage due to bending deformation cannot be evaluated using this model. For more information, see “Damage initiation for ductile metals,” Section 24.2.2 of the Abaqus Analysis User's Guide.
To define MSFLD damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Ductile MetalsMSFLD Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Choose one of the following Definitions:
Select MSFLD to enter data in the form of equivalent plastic strains and ratios of minor to major strain rates.
Select FLD to enter data in the form of major and minor principal strains and the equivalent plastic strain and to have Abaqus transform the data into the Müschenborn-Sonne form.
If desired, you can change the value of 
(
). Omega is used to filter the ratio of principal strains rates, preventing the ratio from jumping to a higher value due to sudden changes in the strain direction (deformation path); the default value is 
.
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data area (parameters followed by MSFLD or FLD are used only for that definition type):
Plastic Strain at Initiation (MSFLD)
Equivalent plastic strain at initiation of localized necking.
Ratio of Principal Strains (MSFLD)
Ratio of minor to major principal strains, 
.
Major Principal Strain (FLD)
Major principal strain at damage initiation.
Minor Principal Strain (FLD)
Minor principal strain at damage initiation.
Plastic Strain Rate
Equivalent plastic strain rate.
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Click OK to exit the material editor.
The Shear damage initiation criterion is a model for predicting the onset of damage due to shear band localization. The model assumes that the equivalent plastic strain at the onset of damage is a function of the shear stress ratio and strain rate. The shear criterion can be used in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models, including equation of state.
For more information, see “Damage initiation for ductile metals,” Section 24.2.2 of the Abaqus Analysis User's Guide.
To define shear damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Ductile MetalsShear Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Enter the material parameter, 
.
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
Fracture Strain
Equivalent fracture strain at damage initiation.
Shear Stress Ratio
The shear stress ratio is defined as 
, where q is the Mises equivalent stress, p is the pressure stress, and 
is the maximum shear stress.
Strain Rate
The equivalent plastic strain rate, .
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Click OK to exit the material editor.
The Hashin damage model predicts anisotropic damage in elastic-brittle materials. It is primarily intended for use with fiber-reinforced composite materials and takes into account four different failure modes: fiber tension, fiber compression, matrix tension, and matrix compression.
For more information, see “Damage initiation for fiber-reinforced composites,” Section 24.3.2 of the Abaqus Analysis User's Guide.
To define Hashin damage:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for Fiber-Reinforced CompositesHashin Damage.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Select 
to use the model proposed in 1973 and 
to use the 1980 model. (For more information, see “Damage initiation for fiber-reinforced composites,” Section 24.3.2 of the Abaqus Analysis User's Guide.)
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
Fiber Tensile Strength
Fiber tensile strength.
Fiber Compressive Strength
Fiber compressive strength.
Matrix Tensile Strength
Matrix tensile strength.
Matrix Compressive Strength
Matrix compressive strength.
Longitudinal Shear Strength
Longitudinal shear strength.
Transverse Shear Strength
Transverse shear strength.
Temp
Temperature, .
Field n
Predefined field variables.
Select SuboptionsDamage Evolution to define the material degradation that takes place once damage begins.
For more information, see “Damage evolution.”
Select SuboptionsDamage Stabilization to enter viscous coefficients and improve the model convergence.
For more information, see “Damage stabilization.”
Click OK to exit the material editor.
The Mullins effect material behavior models stress softening of filled rubber elastomers under quasi-static cyclic loading. Abaqus provides three methods to define the Mullins effect in a material:
Specify the Mullins effect parameters directly as functions of temperature and/or field variables.
Use experimental unloading-reloading test data to calibrate the Mullins effect parameters.
Use user subroutine UMULLINS in Abaqus/Standard and VUMULLINS in Abaqus/Explicit.
For more information about the Mullins effect, including the meaning of the Mullins coefficients 
, 
, and 
, see “Stress softening in elastomers,” Section 22.6 of the Abaqus Analysis User's Guide.
To define the Mullins effect model:
From the menu bar in the Edit Material dialog box, select MechanicalDamage for ElastomersMullins Effect.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
To define the Mullins data using material constants only, perform the following steps:
From the Definition field, select Constants.
To define material damage data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage parameters in the Data table:
r
Value of the coefficient in the Mullins effect model. must be greater than 1.
m
Value of the coefficient in the Mullins effect model. must be greater than or equal to zero, and the values of and cannot both be zero.
beta
Value of the coefficient in the Mullins effect model. must be greater than or equal to zero, and the values of and cannot both be zero.
Temp
Temperature, .
Field n
Predefined field variables.
To specify experimental unloading-reloading test data to calibrate the parameters for the Mullins effect, perform the following steps:
From the Definition field, select Test Data Input.
If desired, enter values for one or two of the damage parameters , , and from the Define Parameters options. For this type of Mullins effect definition, Abaqus/CAE uses test data you provide to calculate the remaining damage parameters.
To provide a value for a damage parameter, toggle it on and specify its value in the appropriate field:
r
Value of the coefficient in the Mullins effect model. must be greater than 1.
m
Value of the coefficient in the Mullins effect model. must be greater than or equal to zero, and the values of and cannot both be zero.
beta
Value of the coefficient in the Mullins effect model. must be greater than or equal to zero, and the values of and cannot both be zero.
From the Add Test menu in the Edit Material dialog box, select Biaxial Test, Planar Test, or Uniaxial Test to add the selected type of unloading-reloading curve to the material model.
You can add multiple versions of each type of test to the material model. Abaqus/CAE names each test you create according to its type and the order in which it was created, so the first two uniaxial material tests you define would be named Uniaxial Test 1 and Uniaxial Test 2.
In the Test data table, enter the test data for the selected test:
Nominal Stress
Nominal stress, 
.
Nominal Strain
Nominal strain, 
.
Repeat the previous two steps to specify additional data calibration tests.
If you want to delete a calibration test, highlight its name in the Tests list and click Delete Test. When you delete a test, Abaqus/CAE removes the test from the list and renames the existing tests so that the test numbering remains consecutive. For example, if you create three biaxial tests and delete the first one (Biaxial Test 1), Biaxial Test 2 is renamed Biaxial Test 1, and Biaxial Test 3 is renamed Biaxial Test 2.
To define the Mullins effect by specifying the damage variable in the user subroutine UMULLINS in Abaqus/Standard and VUMULLINS in Abaqus/Explicit, perform the following steps:
See the following sections for more information:
Click OK to exit the material editor.
The damage evolution definition defines how the material degrades after one or more damage initiation criteria are met. Multiple forms of damage evolution may act on a material at the same time—one for each damage initiation criterion that was defined.
For more information on the types of damage evolution available in the Property module, see “Damage evolution and element removal for ductile metals,” Section 24.2.3 of the Abaqus Analysis User's Guide; “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3 of the Abaqus Analysis User's Guide; and “Connector damage behavior,” Section 31.2.7 of the Abaqus Analysis User's Guide.
The procedure below includes data entries for every type of damage evolution available in the Property module. The selections vary with the current damage initiation form.
To define damage evolution:
When you create a damage initiation criterion in the Edit Material dialog box, select SuboptionsDamage Evolution to specify the associated damage evolution parameters.
(For information on entering damage initiation criteria, see Defining damage, Section 12.9.3 .)
Select the Type of damage evolution:
Displacement
Displacement damage evolution defines damage as a function of the total (for elastic materials in cohesive elements) or the plastic (for bulk elastic-plastic materials) displacement after damage initiation. This type corresponds to the Displacement at Failure field in the Data table.
Energy
Energy damage evolution defines damage in terms of the energy required for failure (fracture energy) after the initiation of damage. This type corresponds to the Fracture Energy field in the Data table.
Select the Softening method:
Linear
Linear softening specifies a linear softening stress-strain response for linear elastic materials or a linear evolution of the damage variable with deformation for elastic-plastic materials. Linear softening is the default method.
Exponential
Exponential softening specifies an exponential softening stress-strain response for linear elastic materials or an exponential evolution of the damage variable with deformation for elastic-plastic materials.
Tabular
Tabular softening specifies the evolution of the damage variable with deformation in tabular form and is available only when you select Displacement for the type. The Displacement at Failure field in the Data table is replaced by a Damage Variable field and a Displacement field, and you can add additional rows to define the displacements.
Select the Mixed mode behavior (for materials associated with cohesive elements only):
Mode-Independent
Mode-independent is the default selection.
Tabular
Tabular mixed mode behavior specifies the fracture energy or displacement (total or plastic) directly as a function of the shear-normal mode mix for cohesive elements. This method must be used when you select the Displacement type with cohesive elements.
Power Law
Power law mixed mode behavior specifies the fracture energy as a function of the mode mix by means of a power law mixed mode fracture criterion; it is available only when you select the Energy type with cohesive elements. The Fracture Energy field in the Data table is replaced by fracture energy in the normal mode and first direction and second direction shear mode components.
BK
The BK mixed mode behavior specifies the fracture energy as a function of the mode mix by means of the Benzeggagh-Kenane mixed mode fracture criterion. The Data table entries are the same as those for the Power Law.
Select the Degradation to determine how Abaqus combines damage evolution when multiple forms are active:
Maximum
The maximum degradation form indicates that the current damage evolution mechanism will interact with other damage evolution mechanisms in a maximum sense to determine the total damage from multiple mechanisms. Maximum is the default selection.
Multiplicative
The multiplicative degradation form indicates that the current damage evolution mechanism will interact in a multiplicative manner with other damage evolution mechanisms defined using this form to determine the total damage from multiple mechanisms. Other damage evolution mechanisms defined using the maximum degradation will interact with the combination of those using the multiplicative form.
Select the Mode Mix Ratio to use in conjunction with the Mixed mode behavior definition (for cohesive elements):
Energy
The energy mixed mode ratio defines the mode mix in terms of a ratio of fracture energy in the different modes. This definition is the default, and it must be used when you select Power Law or BK for the Mixed mode behavior.
Traction
The traction mixed mode ratio defines the mode mix in terms of a ratio of traction components.
When you select Power Law or BK for the Mixed mode behavior for cohesive elements, toggle on Power and enter the exponent in the power law or the Benzeggagh-Kenane criterion that defines the variation of fracture energy with mode mix for cohesive elements.
For the Hashin damage evolution model, the Data table contains the following fields:
Fiber Tensile Fracture Energy
Fiber Compressive Fracture Energy
Matrix Tensile Fracture Energy
Matrix Compressive Fracture Energy
To define damage evolution data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define damage evolution data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
Enter damage evolution parameters in the Data table.
You may need to expand the dialog box to see all the columns in the Data table. For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
Click OK to save the damage evolution data and return to the material editor.
This option is used to specify viscosity coefficients used in the viscous regularization scheme for the damage model for traction separation laws and fiber-reinforced materials. Viscous regularization is intended to improve convergence as the material fails.
Damage stabilization is available for use with the following damage models for traction separation laws:
Maxe and Quade damage models. (For information on entering the Maxe and Quade damage initiation criterion in Abaqus/CAE, see “Maximum or quadratic nominal strain damage.”)
Maxs and Quads damage models. (For information on entering the Maxs and Quads damage initiation criterion in Abaqus/CAE, see “Maximum or quadratic nominal stress damage.”)
Maxps and Maxpe damage models. (For information on entering the Maxps and Maxpe damage initiation criterion in Abaqus/CAE, see “Maximum principal stress or strain damage.”)
Damage stabilization is available for use with the following damage model for fiber-reinforced materials:
Hashin damage model. (For information on entering the Hashin damage initiation criterion in Abaqus/CAE, see “Hashin damage.”)
You define damage stabilization for fiber-reinforced materials by entering viscosity coefficients for each of the potential failure modes:
Fiber tensile failure
Fiber compressive failure
Matrix tensile failure
Matrix compressive failure