Mazars Damage

Mazars scalar damage model

Description

The MazarsDamage model is an implementation of the isotropic damage model for concrete described in Mazars (1984) and Pijaudier-Cabot and Mazars (2001). It is based on the theory of elasticity coupled with the isotropic damage. It describes the elastic stiffness degradation and the softening behavior of concrete under both uniaxial tension and uniaxial compression using an isotropic scalar damage variable $var element = document.getElementById("moose-equation-898e4949-df2e-4f59-a39a-e41e36f10d14");katex.render("d", element, {displayMode:false,throwOnError:false});$ . The damage depends only on the effective stresses applied to an undamaged area.

The evolution of the damage is determined by an equivalent strain $var element = document.getElementById("moose-equation-6fde52a7-6d9f-458b-9e81-a8f501aa98eb");katex.render("\\tilde{\\varepsilon}", element, {displayMode:false,throwOnError:false});$ that quantifies the amount of the local extension state during the mechanical loading. It is calculated from the positive eigenvalues of the strain tensor as follows: $var element = document.getElementById("moose-equation-fb126062-e74f-4845-a0b9-3b44b4acfe27");katex.render("\\tilde{\\varepsilon}=\\sqrt{\\sum_{i=1}^3\\bigl(\\langle\\varepsilon_i\\rangle_+\\bigr)^2}", element, {displayMode:true,throwOnError:false});$ where $var element = document.getElementById("moose-equation-1ce81a27-2ad5-46eb-8dd1-f4b6403b9dc5");katex.render("\\varepsilon_i", element, {displayMode:false,throwOnError:false});$ are the components of principal strain and $var element = document.getElementById("moose-equation-c44427c0-7f37-41ed-b73a-108e7e747301");katex.render("\\langle.\\rangle_+", element, {displayMode:false,throwOnError:false});$ is the Macualay bracket, defined as $var element = document.getElementById("moose-equation-9b944796-ca89-4c1e-a2ed-2d3af444c5fd");katex.render("\\langle\\varepsilon_i\\rangle_+ = \\Bigg\\{ \\begin{array}{cc} \\varepsilon_i & \\varepsilon_i>0\\\\ 0 & \\varepsilon_i<=0 \\end{array}", element, {displayMode:true,throwOnError:false});$

The damage loading function is: $var element = document.getElementById("moose-equation-48d2d1ab-c352-4663-9fd4-985f453e7622");katex.render("f(\\tilde{\\varepsilon},\\kappa)=\\tilde{\\varepsilon}-\\kappa", element, {displayMode:true,throwOnError:false});$ where $var element = document.getElementById("moose-equation-55042db1-16ee-4def-b915-0b256a687da9");katex.render("\\kappa", element, {displayMode:false,throwOnError:false});$ is the parameter defining the threshold of damage growth. Initially, $var element = document.getElementById("moose-equation-d280fe04-9fda-4825-91a7-d8a748c3809b");katex.render("\\kappa", element, {displayMode:false,throwOnError:false});$ is equal to $var element = document.getElementById("moose-equation-de615548-d607-476d-a45f-34e6e8b479ae");katex.render("f_t/E_0", element, {displayMode:false,throwOnError:false});$ , where $var element = document.getElementById("moose-equation-e64b83e1-a886-40a7-999a-8bb23018d28a");katex.render("f_t", element, {displayMode:false,throwOnError:false});$ is the tensile strength and $var element = document.getElementById("moose-equation-d60f2d56-41c3-4e93-9126-db75ab95fa4c");katex.render("E_0", element, {displayMode:false,throwOnError:false});$ is the initial Young's modulus of the material. During subsequent steps, it takes on the maximum value of the equivalent strain during the entire load history: $var element = document.getElementById("moose-equation-de6e89ee-ff96-4e3b-aea4-16d89e8700f6");katex.render("\\kappa = \\max(\\tilde{\\varepsilon},\\kappa_0)", element, {displayMode:true,throwOnError:false});$

To account for the differing behavior of the concrete in tension and in compression, the scalar damage $var element = document.getElementById("moose-equation-b60cc96a-5495-4969-8675-3ec22fbdc30e");katex.render("d", element, {displayMode:false,throwOnError:false});$ is expressed as a combination of two damage modes: $var element = document.getElementById("moose-equation-f81bd836-8fc7-4eae-8511-636f49664fc8");katex.render("d=\\alpha_td_t + \\alpha_cd_c", element, {displayMode:true,throwOnError:false});$ where $var element = document.getElementById("moose-equation-73cfc7b4-e22f-4ae0-96fc-8233e5c5f13a");katex.render("\\alpha_t", element, {displayMode:false,throwOnError:false});$ and $var element = document.getElementById("moose-equation-d7280538-6b0b-40fc-9f86-0ba91ef0bec4");katex.render("\\alpha_c", element, {displayMode:false,throwOnError:false});$ are dimensionless coefficients and represent the contribution of each loading mode such that $var element = document.getElementById("moose-equation-5812263b-1dab-4284-83c5-16350caa7d40");katex.render("\\alpha_t=1", element, {displayMode:false,throwOnError:false});$ and $var element = document.getElementById("moose-equation-3d9d3c7d-553c-4402-938f-4458f6187913");katex.render("\\alpha_c=0", element, {displayMode:false,throwOnError:false});$ under uniaxial tension, and $var element = document.getElementById("moose-equation-cab05fd6-d177-4838-8fae-e2a9e5d7be6b");katex.render("\\alpha_t=0", element, {displayMode:false,throwOnError:false});$ and $var element = document.getElementById("moose-equation-a56cb8e1-425a-49ab-a757-01d020b7f812");katex.render("\\alpha_c=1", element, {displayMode:false,throwOnError:false});$ under uniaxial compression. These coefficients are defined as functions of the principal components of the strain tensors $var element = document.getElementById("moose-equation-e75a3999-5f79-46c1-b75e-981debca1e84");katex.render("\\varepsilon_{ij}^t", element, {displayMode:false,throwOnError:false});$ and $var element = document.getElementById("moose-equation-903e2c54-100a-4b8b-be7b-e80c2ac66a60");katex.render("\\varepsilon_{ij}^c", element, {displayMode:false,throwOnError:false});$ that result from the tensile and compressive components of the stress tensor, respectively, defined as: $var element = document.getElementById("moose-equation-1c9260d1-c2d4-49e0-a001-b62e33b19779");katex.render("\\varepsilon_{kl}^t=(1-d)C_{ijkl}^{-1}\\sigma_{ij}^t", element, {displayMode:true,throwOnError:false});$ $var element = document.getElementById("moose-equation-9bd14d28-d3e5-454b-baa7-b7bf4863e320");katex.render("\\varepsilon_{kl}^c=(1-d)C_{ijkl}^{-1}\\sigma_{ij}^c", element, {displayMode:true,throwOnError:false});$ $var element = document.getElementById("moose-equation-be5fb39f-2ade-4918-9dcb-b3b65c8618a1");katex.render("\\alpha_t", element, {displayMode:false,throwOnError:false});$ and $var element = document.getElementById("moose-equation-2f1f4f1c-f7f9-46c1-a916-029630d10170");katex.render("\\alpha_c", element, {displayMode:false,throwOnError:false});$ are then computed as: $var element = document.getElementById("moose-equation-14212321-796d-4bed-9c92-71692d91b7ce");katex.render("\\alpha_t=\\sum_{i=1}^3\\biggl(\\frac{\\langle\\varepsilon_i^t\\rangle\\langle\\varepsilon_i\\rangle}{\\tilde{\\varepsilon}^2}\\biggr)^\\beta", element, {displayMode:true,throwOnError:false});$ $var element = document.getElementById("moose-equation-e23ae0d8-fa6c-47b1-8301-0873df1a0e1a");katex.render("\\alpha_c=\\sum_{i=1}^3\\biggl(\\frac{\\langle\\varepsilon_i^c\\rangle\\langle\\varepsilon_i\\rangle}{\\tilde{\\varepsilon}^2}\\biggr)^\\beta", element, {displayMode:true,throwOnError:false});$ The exponent $var element = document.getElementById("moose-equation-fa143d73-47f9-4f49-81b7-7206000705c6");katex.render("\\beta", element, {displayMode:false,throwOnError:false});$ in these equations is a parameter that can be tuned to fit experimental data for shear response, and is recommended initially to be set to 1. The current implementation of the model has this parameter hard-coded to 1, and it cannot be set by the user.

The scalar damage variables $var element = document.getElementById("moose-equation-d0dcfb7e-5776-440e-af83-648ff2025fae");katex.render("d_t", element, {displayMode:false,throwOnError:false});$ and $var element = document.getElementById("moose-equation-1457a111-c83f-48f7-8071-11fa4654b557");katex.render("d_c", element, {displayMode:false,throwOnError:false});$ for tension and compression, respectively, are computed as: $var element = document.getElementById("moose-equation-9fcf5110-9eff-4771-85e6-7047ae2a7335");katex.render("d_t=1 - \\frac{\\kappa_0(1-A_t)}{\\kappa} - \\frac{A_t}{\\exp[B_t(\\kappa-\\kappa_0)]}", element, {displayMode:true,throwOnError:false});$ $var element = document.getElementById("moose-equation-0ad689d2-536b-4d7c-9438-462e9fbe9015");katex.render("d_c=1 - \\frac{\\kappa_0(1-A_c)}{\\kappa} - \\frac{A_c}{\\exp[B_c(\\kappa-\\kappa_0)]}", element, {displayMode:true,throwOnError:false});$ where $var element = document.getElementById("moose-equation-e5a7127d-8340-4378-95be-a98adec7d793");katex.render("A_t", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-8f9fa36e-9b31-4a61-8dc6-742b0a787a0a");katex.render("A_c", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-afda2e79-0989-4f17-a427-c0ae36f1709c");katex.render("B_t", element, {displayMode:false,throwOnError:false});$ , and $var element = document.getElementById("moose-equation-8dec0e8a-913a-4c7c-b7f7-dffcdcf6d07e");katex.render("B_c", element, {displayMode:false,throwOnError:false});$ are material parameters that control the shape of the nonlinear response and are determined using compression and tension tests.

Implementation and Usage

Damage models such as this do not directly compute the stress, but are used in conjunction with a stress calculator to modify the stress computation that takes other phenomena into account as well. The damage models derive from a common base class that defines functionality that a damage model must supply. The ComputeDamageStress model is a stress calculating model that computes the behavior of materials that only exhibit damaged isotropic elastic behavior. The example below shows how the damage and stress models are used in conjunction with each other.

Example Input Syntax

[damage]
  type = MazarsDamage
  tensile_strength = 1e6
  a_t = 0.87
  a_c = 0.65
  b_t = 20000
  b_c = 2150
[]

MazarsDamage is run in conjunction with a stress calculator that supports the use of a damage model, (ComputeDamageStress in this case), as shown:

[stress]
  type = ComputeDamageStress
  damage_model = damage
[]

Input Parameters

a_cA_c parameter that controls the shape of the response in compression
C++ Type:double
Options:
Description:A_c parameter that controls the shape of the response in compression
a_tA_t parameter that controls the shape of the response in tension
C++ Type:double
Options:
Description:A_t parameter that controls the shape of the response in tension
b_cB_c parameter that controls the shape of the response in compression
C++ Type:double
Options:
Description:B_c parameter that controls the shape of the response in compression
b_tB_t parameter that controls the shape of the response in tension
C++ Type:double
Options:
Description:B_t parameter that controls the shape of the response in tension
tensile_strengthTensile stress threshold for damage initiation
C++ Type:std::vector<VariableName>
Options:
Description:Tensile stress threshold for damage initiation

Required Parameters

base_nameOptional parameter that allows the user to define multiple mechanics material systems on the same block, i.e. for multiple phases
C++ Type:std::string
Options:
Description:Optional parameter that allows the user to define multiple mechanics material systems on the same block, i.e. for multiple phases
blockThe list of block ids (SubdomainID) that this object will be applied
C++ Type:std::vector<SubdomainName>
Options:
Description:The list of block ids (SubdomainID) that this object will be applied
boundaryThe list of boundary IDs from the mesh where this boundary condition applies
C++ Type:std::vector<BoundaryName>
Options:
Description:The list of boundary IDs from the mesh where this boundary condition applies
constant_onNONEWhen ELEMENT, MOOSE will only call computeQpProperties() for the 0th quadrature point, and then copy that value to the other qps.When SUBDOMAIN, MOOSE will only call computeQpProperties() for the 0th quadrature point, and then copy that value to the other qps. Evaluations on element qps will be skipped
Default:NONE
C++ Type:MooseEnum
Options:NONE, ELEMENT, SUBDOMAIN
Description:When ELEMENT, MOOSE will only call computeQpProperties() for the 0th quadrature point, and then copy that value to the other qps.When SUBDOMAIN, MOOSE will only call computeQpProperties() for the 0th quadrature point, and then copy that value to the other qps. Evaluations on element qps will be skipped
damage_index_namedamage_indexname of the material property where the damage index is stored
Default:damage_index
C++ Type:MaterialPropertyName
Options:
Description:name of the material property where the damage index is stored
maximum_damage_increment0.1maximum damage increment allowed for simulations with adaptive time step
Default:0.1
C++ Type:double
Options:
Description:maximum damage increment allowed for simulations with adaptive time step
residual_stiffness_fraction1e-08Minimum fraction of original material stiffness retained for fully damaged material (when damage_index=1)
Default:1e-08
C++ Type:double
Options:
Description:Minimum fraction of original material stiffness retained for fully damaged material (when damage_index=1)
use_old_damageFalseWhether to use the damage index from the previous step in the stress computation
Default:False
C++ Type:bool
Options:
Description:Whether to use the damage index from the previous step in the stress computation

Optional Parameters

control_tagsAdds user-defined labels for accessing object parameters via control logic.
C++ Type:std::vector<std::string>
Options:
Description:Adds user-defined labels for accessing object parameters via control logic.
enableTrueSet the enabled status of the MooseObject.
Default:True
C++ Type:bool
Options:
Description:Set the enabled status of the MooseObject.
implicitTrueDetermines whether this object is calculated using an implicit or explicit form
Default:True
C++ Type:bool
Options:
Description:Determines whether this object is calculated using an implicit or explicit form
seed0The seed for the master random number generator
Default:0
C++ Type:unsigned int
Options:
Description:The seed for the master random number generator
use_displaced_meshFalseWhether or not this object should use the displaced mesh for computation. Note that in the case this is true but no displacements are provided in the Mesh block the undisplaced mesh will still be used.
Default:False
C++ Type:bool
Options:
Description:Whether or not this object should use the displaced mesh for computation. Note that in the case this is true but no displacements are provided in the Mesh block the undisplaced mesh will still be used.

Advanced Parameters

output_propertiesList of material properties, from this material, to output (outputs must also be defined to an output type)
C++ Type:std::vector<std::string>
Options:
Description:List of material properties, from this material, to output (outputs must also be defined to an output type)
outputsnone Vector of output names were you would like to restrict the output of variables(s) associated with this object
Default:none
C++ Type:std::vector<OutputName>
Options:
Description:Vector of output names were you would like to restrict the output of variables(s) associated with this object

Outputs Parameters

Input Files

(test/tests/mazars_damage/mazars.i)
(test/tests/mazars_tensile_bar/tensile_bar.i)

References

Jacky Mazars. Application de la mécanique de l'endommagement au comportement non linéaire et à la rupture du béton de structure. PhD thesis, Université Paris 6, France, 1984.

@phdthesis{mazars_application_1984,
    Author = "Mazars, Jacky",
    School = "Universit{\'e} Paris 6, France",
    Title = "Application de la m{\'e}canique de l'endommagement au comportement non lin{\'e}aire et {\`a} la rupture du b{\'e}ton de structure",
    Year = "1984"
}

Gilles Pijaudier-Cabot and Jacky Mazars. Damage models for concrete. In Jean Lemaitre, editor, Handbook of Materials Behavior Models. Academic Press, 2001.

@incollection{pijaudier-cabot_damage_2001,
    Author = "Pijaudier-Cabot, Gilles and Mazars, Jacky",
    Editor = "Lemaitre, Jean",
    Booktitle = "Handbook of Materials Behavior Models",
    Publisher = "Academic Press",
    Title = "Damage Models for Concrete",
    Year = "2001"
}

(test/tests/mazars_damage/mazars.i)

# Test MazarsDamage model in uniaxial tension and compression.
# This test is a single element with imposed Dirichlet BCs to
# pull or push on the element and verify that it follows the
# expected hardening/softening behavior.

[GlobalParams]
  displacements = 'disp_x disp_y disp_z'
[]

[Mesh]
  type = GeneratedMesh
  dim = 3
  nx = 1
  ny = 1
  nz = 1
  elem_type = HEX8
[]

[AuxVariables]
  [stress_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [damage_index]
    order = CONSTANT
    family = MONOMIAL
  []
[]

[Modules/TensorMechanics/Master]
  [all]
    strain = SMALL
    incremental = true
    add_variables = true
  []
[]

[AuxKernels]
  [stress_xx]
    type = RankTwoAux
    variable = stress_xx
    rank_two_tensor = stress
    index_j = 0
    index_i = 0
    execute_on = timestep_end
  []
  [strain_xx]
    type = RankTwoAux
    variable = strain_xx
    rank_two_tensor = total_strain
    index_j = 0
    index_i = 0
    execute_on = timestep_end
  []
  [damage_index]
    type = MaterialRealAux
    variable = damage_index
    property = damage_index
    execute_on = timestep_end
  []
[]

[BCs]
  [symmy]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0
  []
  [symmx]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0
  []
  [symmz]
    type = DirichletBC
    variable = disp_z
    boundary = back
    value = 0
  []
  [axial_load]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = right
    function = pull
  []
[]

[Functions]
  [push]
    type = ParsedFunction
    value = '-t'
  []
  [pull]
    type = ParsedFunction
    value = 't'
  []
[]

[Materials]
  [damage]
    type = MazarsDamage
    tensile_strength = 1e6
    a_t = 0.87
    a_c = 0.65
    b_t = 20000
    b_c = 2150
  []

  [stress]
    type = ComputeDamageStress
    damage_model = damage
  []
  [elasticity]
    type = ComputeIsotropicElasticityTensor
    poissons_ratio = 0.2
    youngs_modulus = 10e9
  []
[]

[Postprocessors]
  [stress_xx]
    type = ElementAverageValue
    variable = stress_xx
  []
  [strain_xx]
    type = ElementAverageValue
    variable = strain_xx
  []
  [damage_index]
    type = ElementAverageValue
    variable = damage_index
  []
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Executioner]
  type = Transient

  l_max_its  = 50
  l_tol      = 1e-8
  nl_max_its = 20
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-8

  dt = 0.0001
  dtmin = 0.0001
  end_time = 0.001
[]

[Outputs]
  exodus = true
  csv = true
[]

(test/tests/mazars_damage/mazars.i)

# Test MazarsDamage model in uniaxial tension and compression.
# This test is a single element with imposed Dirichlet BCs to
# pull or push on the element and verify that it follows the
# expected hardening/softening behavior.

[GlobalParams]
  displacements = 'disp_x disp_y disp_z'
[]

[Mesh]
  type = GeneratedMesh
  dim = 3
  nx = 1
  ny = 1
  nz = 1
  elem_type = HEX8
[]

[AuxVariables]
  [stress_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [damage_index]
    order = CONSTANT
    family = MONOMIAL
  []
[]

[Modules/TensorMechanics/Master]
  [all]
    strain = SMALL
    incremental = true
    add_variables = true
  []
[]

[AuxKernels]
  [stress_xx]
    type = RankTwoAux
    variable = stress_xx
    rank_two_tensor = stress
    index_j = 0
    index_i = 0
    execute_on = timestep_end
  []
  [strain_xx]
    type = RankTwoAux
    variable = strain_xx
    rank_two_tensor = total_strain
    index_j = 0
    index_i = 0
    execute_on = timestep_end
  []
  [damage_index]
    type = MaterialRealAux
    variable = damage_index
    property = damage_index
    execute_on = timestep_end
  []
[]

[BCs]
  [symmy]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0
  []
  [symmx]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0
  []
  [symmz]
    type = DirichletBC
    variable = disp_z
    boundary = back
    value = 0
  []
  [axial_load]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = right
    function = pull
  []
[]

[Functions]
  [push]
    type = ParsedFunction
    value = '-t'
  []
  [pull]
    type = ParsedFunction
    value = 't'
  []
[]

[Materials]
  [damage]
    type = MazarsDamage
    tensile_strength = 1e6
    a_t = 0.87
    a_c = 0.65
    b_t = 20000
    b_c = 2150
  []

  [stress]
    type = ComputeDamageStress
    damage_model = damage
  []
  [elasticity]
    type = ComputeIsotropicElasticityTensor
    poissons_ratio = 0.2
    youngs_modulus = 10e9
  []
[]

[Postprocessors]
  [stress_xx]
    type = ElementAverageValue
    variable = stress_xx
  []
  [strain_xx]
    type = ElementAverageValue
    variable = strain_xx
  []
  [damage_index]
    type = ElementAverageValue
    variable = damage_index
  []
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Executioner]
  type = Transient

  l_max_its  = 50
  l_tol      = 1e-8
  nl_max_its = 20
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-8

  dt = 0.0001
  dtmin = 0.0001
  end_time = 0.001
[]

[Outputs]
  exodus = true
  csv = true
[]

(test/tests/mazars_damage/mazars.i)

# Test MazarsDamage model in uniaxial tension and compression.
# This test is a single element with imposed Dirichlet BCs to
# pull or push on the element and verify that it follows the
# expected hardening/softening behavior.

[GlobalParams]
  displacements = 'disp_x disp_y disp_z'
[]

[Mesh]
  type = GeneratedMesh
  dim = 3
  nx = 1
  ny = 1
  nz = 1
  elem_type = HEX8
[]

[AuxVariables]
  [stress_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [damage_index]
    order = CONSTANT
    family = MONOMIAL
  []
[]

[Modules/TensorMechanics/Master]
  [all]
    strain = SMALL
    incremental = true
    add_variables = true
  []
[]

[AuxKernels]
  [stress_xx]
    type = RankTwoAux
    variable = stress_xx
    rank_two_tensor = stress
    index_j = 0
    index_i = 0
    execute_on = timestep_end
  []
  [strain_xx]
    type = RankTwoAux
    variable = strain_xx
    rank_two_tensor = total_strain
    index_j = 0
    index_i = 0
    execute_on = timestep_end
  []
  [damage_index]
    type = MaterialRealAux
    variable = damage_index
    property = damage_index
    execute_on = timestep_end
  []
[]

[BCs]
  [symmy]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0
  []
  [symmx]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0
  []
  [symmz]
    type = DirichletBC
    variable = disp_z
    boundary = back
    value = 0
  []
  [axial_load]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = right
    function = pull
  []
[]

[Functions]
  [push]
    type = ParsedFunction
    value = '-t'
  []
  [pull]
    type = ParsedFunction
    value = 't'
  []
[]

[Materials]
  [damage]
    type = MazarsDamage
    tensile_strength = 1e6
    a_t = 0.87
    a_c = 0.65
    b_t = 20000
    b_c = 2150
  []

  [stress]
    type = ComputeDamageStress
    damage_model = damage
  []
  [elasticity]
    type = ComputeIsotropicElasticityTensor
    poissons_ratio = 0.2
    youngs_modulus = 10e9
  []
[]

[Postprocessors]
  [stress_xx]
    type = ElementAverageValue
    variable = stress_xx
  []
  [strain_xx]
    type = ElementAverageValue
    variable = strain_xx
  []
  [damage_index]
    type = ElementAverageValue
    variable = damage_index
  []
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Executioner]
  type = Transient

  l_max_its  = 50
  l_tol      = 1e-8
  nl_max_its = 20
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-8

  dt = 0.0001
  dtmin = 0.0001
  end_time = 0.001
[]

[Outputs]
  exodus = true
  csv = true
[]

(test/tests/mazars_tensile_bar/tensile_bar.i)

# This tests a bar pulled in tension from one side.
# The material is modeled using the MazarsDamage model,
# and a single band of elements is given a slightly lower
# tensile strength to force damage localization.

[GlobalParams]
  displacements = 'disp_x disp_y disp_z'
[]

[Mesh]
  type = GeneratedMesh
  dim = 3
  nx = 10
  ny = 2
  nz = 2
  xmax = 0.05
  ymax = 0.01
  zmax = 0.01
  elem_type = HEX8
[]

[AuxVariables]
  [react_x]
  []
  [react_y]
  []
  [react_z]
  []
  [tensile_strength]
    order = CONSTANT
    family = MONOMIAL
  []
[]

[Modules/TensorMechanics/Master]
  [all]
    strain = FINITE
    incremental = true
    add_variables = true
    generate_output = 'stress_xx strain_xx'
    save_in = 'react_x react_y react_z'
  []
[]

[AuxKernels]
  [damage_index]
    type = MaterialRealAux
    variable = damage_index
    property = damage_index
    execute_on = timestep_end
  []
  [tensile_strength]
    type = FunctionAux
    variable = tensile_strength
    function = 'if(x<0.005,0.99e6,1.0e6)'
    execute_on = initial
  []
[]

[BCs]
  [symmy]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0
  []
  [symmx]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0
  []
  [symmz]
    type = DirichletBC
    variable = disp_z
    boundary = back
    value = 0
  []
  [axial_load]
    type = FunctionDirichletBC
    preset = true
    variable = disp_x
    boundary = right
    function = 't'
  []
[]

[Materials]
  [damage]
    type = MazarsDamage
    tensile_strength = tensile_strength
    a_t = 0.87
    a_c = 0.65
    b_t = 20000
    b_c = 2150
    use_old_damage = true
    outputs = exodus
    output_properties = damage_index
  []
  [stress]
    type = ComputeDamageStress
    damage_model = damage
  []
  [elasticity]
    type = ComputeIsotropicElasticityTensor
    poissons_ratio = 0.2
    youngs_modulus = 10e9
  []
[]

[Postprocessors]
  [react]
    type = SideAverageValue
    variable = react_x
    boundary = right
  []
  [disp]
    type = SideAverageValue
    variable = disp_x
    boundary = right
  []
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Executioner]
  type = Transient

  l_max_its  = 50
  l_tol      = 1e-8
  nl_max_its = 20
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-8

  dt = 5e-7
  dtmin = 5e-7
  end_time = 1e-5
[]

[Outputs]
  exodus = true
  csv = true
[]

Description
Implementation and Usage
Example Input Syntax
Input Parameters
Input Files
References