Exponential Softening

Softening model with an exponential softening response upon cracking. This class is intended to be used with ComputeSmearedCrackingStress.

Description

The material ExponentialSoftening computes the reduced stress and stiffness in the direction of a crack according to a exponential function. The computed cracked stiffness ratio softens the tensile response of the material once the principle stress exceeds the cracking stress threshold of the material.

As with the other smeared cracking softening models, which all follow the nomenclature convention of using the Softening suffix, this model is intended to be used with the ComputeSmearedCrackingStress material.

Softening Model

The tensile stress response to cracking is calculated as an exponential function of the crack strain $(1)var element = document.getElementById("moose-equation-e8ea2263-7d34-4c3c-a269-2c4ed927239d");katex.render(" \\sigma = \\sigma_c \\cdot \\left( \\sigma_{res} + (1 - \\sigma_{res}) \\cdot \\exp \\left[ \\frac{\\alpha \\beta}{\\sigma_c} \\cdot \\left( \\epsilon_c^{max} - \\epsilon_c^{init} \\right) \\right] \\right)", element, {displayMode:true,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ where the calculated stress, $var element = document.getElementById("moose-equation-b6d8ff4e-19ea-4e08-b46e-9a50c78e4275");katex.render("\\sigma", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is the principle stress along the direction of the crack, $var element = document.getElementById("moose-equation-47051250-7669-4039-bc49-8f111c7689cd");katex.render("\\sigma_c", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is the stress threshold beyond which cracking occurs, $var element = document.getElementById("moose-equation-d27833a3-8678-428a-904d-f683409a0eec");katex.render("\\sigma_{res}", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is the residual stress retained after full softening due to the crack is completed, $var element = document.getElementById("moose-equation-cd2f691f-75d2-41d6-ba5f-e24fed8f53f1");katex.render("\\alpha", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is the initial slope of the exponential curve, $var element = document.getElementById("moose-equation-4eea48a7-91e9-4b1b-9801-3028b850cc7a");katex.render("\\beta", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is a fitting parameter, $var element = document.getElementById("moose-equation-5941c3a1-4269-4499-bd8d-e7d5f1049384");katex.render("\\epsilon_c^{max}", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is the maximum strain in the direction of crack, and $var element = document.getElementById("moose-equation-4f23564d-1c6d-4581-9bf8-196dade2e9f9");katex.render("\\epsilon_c^{init}", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is the strain in direction of crack when crack initiation occurred. The ratio of the current stiffness to the original material stiffness is computed using the result of Eq. (1) $(2)var element = document.getElementById("moose-equation-b1f1e613-d3f5-430a-a50b-d99cd4d24fc7");katex.render(" R = \\sigma \\cdot \\frac{\\epsilon_c^{init}}{\\epsilon_c^{max}\\sigma_c}", element, {displayMode:true,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ where the definitions for the variables are the same here as in Eq. (1). The stiffness ratio is passed back to the ComputeSmearedCrackingStress to compute the softened cracked material stiffness.

Example Input File

[./exponential_softening]
  type = ExponentialSoftening
[../]

ExponentialSoftening must be run in conjunction with the fixed smeared cracking material model as shown below:

[./cracking_stress]
  type = ComputeSmearedCrackingStress
  shear_retention_factor = 0.1
  cracking_stress = 3.e9
  cracked_elasticity_type = FULL
  softening_models = exponential_softening
[../]

Input Parameters

alpha-1Initial slope of the exponential softening curve at crack initiation. If not specified, it is equal to the negative of the Young's modulus.
Default:-1
C++ Type:double
Controllable:No
Description:Initial slope of the exponential softening curve at crack initiation. If not specified, it is equal to the negative of the Young's modulus.
beta1Multiplier applied to alpha to control the exponential softening behavior.
Default:1
C++ Type:double
Controllable:No
Description:Multiplier applied to alpha to control the exponential softening behavior.
blockThe list of blocks (ids or names) that this object will be applied
C++ Type:std::vector<SubdomainName>
Controllable:No
Description:The list of blocks (ids or names) that this object will be applied
boundaryThe list of boundaries (ids or names) from the mesh where this object applies
C++ Type:std::vector<BoundaryName>
Controllable:No
Description:The list of boundaries (ids or names) from the mesh where this object 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
Controllable:No
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
declare_suffixAn optional suffix parameter that can be appended to any declared properties. The suffix will be prepended with a '_' character.
C++ Type:MaterialPropertyName
Controllable:No
Description:An optional suffix parameter that can be appended to any declared properties. The suffix will be prepended with a '_' character.
prop_getter_suffixAn optional suffix parameter that can be appended to any attempt to retrieve/get material properties. The suffix will be prepended with a '_' character.
C++ Type:MaterialPropertyName
Controllable:No
Description:An optional suffix parameter that can be appended to any attempt to retrieve/get material properties. The suffix will be prepended with a '_' character.
residual_stress0The fraction of the cracking stress allowed to be maintained following a crack.
Default:0
C++ Type:double
Controllable:No
Description:The fraction of the cracking stress allowed to be maintained following a crack.
use_interpolated_stateFalseFor the old and older state use projected material properties interpolated at the quadrature points. To set up projection use the ProjectedStatefulMaterialStorageAction.
Default:False
C++ Type:bool
Controllable:No
Description:For the old and older state use projected material properties interpolated at the quadrature points. To set up projection use the ProjectedStatefulMaterialStorageAction.

Optional Parameters

control_tagsAdds user-defined labels for accessing object parameters via control logic.
C++ Type:std::vector<std::string>
Controllable:No
Description:Adds user-defined labels for accessing object parameters via control logic.
enableTrueSet the enabled status of the MooseObject.
Default:True
C++ Type:bool
Controllable:Yes
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
Controllable:No
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
Controllable:No
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
Controllable:No
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>
Controllable:No
Description:List of material properties, from this material, to output (outputs must also be defined to an output type)
outputsnone Vector of output names where you would like to restrict the output of variables(s) associated with this object
Default:none
C++ Type:std::vector<OutputName>
Controllable:No
Description:Vector of output names where you would like to restrict the output of variables(s) associated with this object

Outputs Parameters

Input Files

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_multiple_softening.i)
(modules/solid_mechanics/test/tests/smeared_cracking/cracking_rotation.i)
(modules/solid_mechanics/test/tests/smeared_cracking/cracking_plane_stress.i)
(modules/solid_mechanics/test/tests/smeared_cracking/cracking_xyz.i)
(modules/solid_mechanics/test/tests/smeared_cracking/cracking_rz_exponential.i)
(modules/solid_mechanics/test/tests/smeared_cracking/cracking_exponential.i)

References

No citations exist within this document.

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_rotation.i)

# This test is to ensure that the smeared cracking model correctly handles finite
# rotation of cracked elements.

# This consists of a single element that is first  subjected to tensile loading
# in the y-direction via a prescribed displacement. This loading is sufficiently
# high to crack the material in that direction, but not completely unload. The
# prescribed displacement is then reversed so that the element is returned to its
# original configuration.

# In the next phase of the analysis, this element is then rotated 90 degrees by
# prescribing the displacement of the bottom of the element. The prescribed
# displacement BC used to crack the element in the first phase is deactivated.

# Once the element is fully rotated, a new BC is activated on what was originally
# the top surface (but is now the surface on the right hand side) to pull in
# the x-direction.

# If everything is working correctly, the model should re-load on the original
# crack (which should be rotated along with the elemnent) up to the peak stress
# in the first phase of the analysis, and then continue the unloading process
# as the crack strains continue to increase. Throughout this analysis, there should
# only be a single crack, as manifested in the crack_flags variables.

[Mesh]
  file = cracking_test.e
[]

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

[Physics/SolidMechanics/QuasiStatic]
  [./all]
    strain = FINITE
    add_variables = true
    generate_output = 'stress_xx stress_yy stress_zz stress_xy stress_yz stress_zx'
  [../]
[]

[AuxVariables]
  [./crack_flags1]
    order = CONSTANT
    family = MONOMIAL
  [../]
  [./crack_flags2]
    order = CONSTANT
    family = MONOMIAL
  [../]
  [./crack_flags3]
    order = CONSTANT
    family = MONOMIAL
  [../]
[]

[AuxKernels]
  [./crack_flags1]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags1
    component = 0
  [../]
  [./crack_flags2]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags2
    component = 1
  [../]
  [./crack_flags3]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags3
    component = 2
  [../]
[]

[BCs]
  [./x_pin]
    type = DirichletBC
    variable = disp_x
    boundary = '15 16'
    value = 0.0
  [../]
  [./y_pin]
    type = DirichletBC
    variable = disp_y
    boundary = '15 16'
    value = 0.0
  [../]
  [./z_all]
    type = DirichletBC
    variable = disp_z
    boundary = '11 12 13 14 15 16 17 18'
    value = 0.0
  [../]
  [./x_lb]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '11 12'
    function = 'if(t<10,0,if(t>=100,1,1-cos((t-10)*pi/180)))'
  [../]
  [./y_lb]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = '11 12'
    function = 'if(t<10,0,if(t>=100,1,sin((t-10)*pi/180)))'
  [../]
  [./x_lt]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '13 14'
    function = '2+(t-100)*0.01'
  [../]
  [./x_rt]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '17 18'
    function = '1+(t-100)*0.01'
  [../]
  [./top_pull]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = '13 14 17 18'
    function = 'if(t<5,t*0.01,0.05-(t-5)*0.01)'
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 100.e9
    poissons_ratio = 0.
  [../]
  [./cracking_stress]
    type = ComputeSmearedCrackingStress
    shear_retention_factor = 0.1
    cracking_stress = 3.e9
    cracked_elasticity_type = FULL
    softening_models = exponential_softening
  [../]
  [./exponential_softening]
    type = ExponentialSoftening
  [../]
[]

[Executioner]
  type = Transient

  petsc_options_iname = '-ksp_gmres_restart -pc_type'
  petsc_options_value = '101                lu'
  line_search = 'none'

  l_max_its = 100
  l_tol = 1e-5

  nl_max_its = 100
  nl_abs_tol = 1e-5
  nl_rel_tol = 1e-12

  start_time = 0
  end_time = 110
  dt = 1
[]

[Controls]
  [./p1]
    type = TimePeriod
    start_time = 0.0
    end_time = 10.0
    disable_objects = 'BCs/x_lt BCs/x_rt'
    enable_objects = 'BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
  [./p2]
    type = TimePeriod
    start_time = 10.0
    end_time = 101.0
    disable_objects = 'BCs/x_lt BCs/x_rt BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
  [./p3]
    type = TimePeriod
    start_time = 101.0
    end_time = 110.0
    enable_objects = 'BCs/x_lt BCs/x_rt'
    disable_objects = 'BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
[]

[Outputs]
  exodus = true
[]

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_rotation.i)

# This test is to ensure that the smeared cracking model correctly handles finite
# rotation of cracked elements.

# This consists of a single element that is first  subjected to tensile loading
# in the y-direction via a prescribed displacement. This loading is sufficiently
# high to crack the material in that direction, but not completely unload. The
# prescribed displacement is then reversed so that the element is returned to its
# original configuration.

# In the next phase of the analysis, this element is then rotated 90 degrees by
# prescribing the displacement of the bottom of the element. The prescribed
# displacement BC used to crack the element in the first phase is deactivated.

# Once the element is fully rotated, a new BC is activated on what was originally
# the top surface (but is now the surface on the right hand side) to pull in
# the x-direction.

# If everything is working correctly, the model should re-load on the original
# crack (which should be rotated along with the elemnent) up to the peak stress
# in the first phase of the analysis, and then continue the unloading process
# as the crack strains continue to increase. Throughout this analysis, there should
# only be a single crack, as manifested in the crack_flags variables.

[Mesh]
  file = cracking_test.e
[]

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

[Physics/SolidMechanics/QuasiStatic]
  [./all]
    strain = FINITE
    add_variables = true
    generate_output = 'stress_xx stress_yy stress_zz stress_xy stress_yz stress_zx'
  [../]
[]

[AuxVariables]
  [./crack_flags1]
    order = CONSTANT
    family = MONOMIAL
  [../]
  [./crack_flags2]
    order = CONSTANT
    family = MONOMIAL
  [../]
  [./crack_flags3]
    order = CONSTANT
    family = MONOMIAL
  [../]
[]

[AuxKernels]
  [./crack_flags1]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags1
    component = 0
  [../]
  [./crack_flags2]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags2
    component = 1
  [../]
  [./crack_flags3]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags3
    component = 2
  [../]
[]

[BCs]
  [./x_pin]
    type = DirichletBC
    variable = disp_x
    boundary = '15 16'
    value = 0.0
  [../]
  [./y_pin]
    type = DirichletBC
    variable = disp_y
    boundary = '15 16'
    value = 0.0
  [../]
  [./z_all]
    type = DirichletBC
    variable = disp_z
    boundary = '11 12 13 14 15 16 17 18'
    value = 0.0
  [../]
  [./x_lb]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '11 12'
    function = 'if(t<10,0,if(t>=100,1,1-cos((t-10)*pi/180)))'
  [../]
  [./y_lb]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = '11 12'
    function = 'if(t<10,0,if(t>=100,1,sin((t-10)*pi/180)))'
  [../]
  [./x_lt]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '13 14'
    function = '2+(t-100)*0.01'
  [../]
  [./x_rt]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '17 18'
    function = '1+(t-100)*0.01'
  [../]
  [./top_pull]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = '13 14 17 18'
    function = 'if(t<5,t*0.01,0.05-(t-5)*0.01)'
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 100.e9
    poissons_ratio = 0.
  [../]
  [./cracking_stress]
    type = ComputeSmearedCrackingStress
    shear_retention_factor = 0.1
    cracking_stress = 3.e9
    cracked_elasticity_type = FULL
    softening_models = exponential_softening
  [../]
  [./exponential_softening]
    type = ExponentialSoftening
  [../]
[]

[Executioner]
  type = Transient

  petsc_options_iname = '-ksp_gmres_restart -pc_type'
  petsc_options_value = '101                lu'
  line_search = 'none'

  l_max_its = 100
  l_tol = 1e-5

  nl_max_its = 100
  nl_abs_tol = 1e-5
  nl_rel_tol = 1e-12

  start_time = 0
  end_time = 110
  dt = 1
[]

[Controls]
  [./p1]
    type = TimePeriod
    start_time = 0.0
    end_time = 10.0
    disable_objects = 'BCs/x_lt BCs/x_rt'
    enable_objects = 'BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
  [./p2]
    type = TimePeriod
    start_time = 10.0
    end_time = 101.0
    disable_objects = 'BCs/x_lt BCs/x_rt BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
  [./p3]
    type = TimePeriod
    start_time = 101.0
    end_time = 110.0
    enable_objects = 'BCs/x_lt BCs/x_rt'
    disable_objects = 'BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
[]

[Outputs]
  exodus = true
[]

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_multiple_softening.i)

# Test of cracking with direction-specific release models in 3
# directions. Block is first pulled in one direction, and then
# held while it is sequentially pulled in the other two
# directions. Poisson's ratio is zero so that the cracking in one
# direction doesn't affect the others.

# Softening in the three directions should follow the laws for the
# prescribed models in the three directions, which are power law (x),
# exponential (y), and abrupt (z).

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

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

[Functions]
  [./displx]
    type = PiecewiseLinear
    x = '0 1 2 3'
    y = '0 1 1 1'
  [../]
  [./disply]
    type = PiecewiseLinear
    x = '0 1 2 3'
    y = '0 0 1 1'
  [../]
  [./displz]
    type = PiecewiseLinear
    x = '0 1 2 3'
    y = '0 0 0 1'
  [../]
[]

[Physics/SolidMechanics/QuasiStatic]
  [./all]
    strain = FINITE
    add_variables = true
    generate_output = 'stress_xx stress_yy stress_zz stress_xy stress_yz stress_zx'
  [../]
[]

[BCs]
  [./pullx]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = right
    function = displx
  [../]
  [./pully]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = top
    function = disply
  [../]
  [./pullz]
    type = FunctionDirichletBC
    variable = disp_z
    boundary = front
    function = displz
  [../]
  [./left]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0.0
  [../]
  [./bottom]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0.0
  [../]
  [./back]
    type = DirichletBC
    variable = disp_z
    boundary = back
    value = 0.0
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 2.8e7
    poissons_ratio = 0
  [../]
  [./elastic_stress]
    type = ComputeSmearedCrackingStress
    cracking_stress = 1.68e6
    cracked_elasticity_type = FULL
    softening_models = 'power_law_softening exponential_softening abrupt_softening'
    prescribed_crack_directions = 'x y z'
  [../]
  [./power_law_softening]
    type = PowerLawSoftening
    stiffness_reduction = 0.3333
  [../]
  [./exponential_softening]
    type = ExponentialSoftening
  [../]
  [./abrupt_softening]
    type = AbruptSoftening
  [../]
[]

[Executioner]
  type = Transient

  petsc_options_iname = '-ksp_gmres_restart -pc_type -sub_pc_type'
  petsc_options_value = '101                asm      lu'

  line_search = 'none'

  l_max_its = 100
  nl_max_its = 100
  nl_rel_tol = 1e-8
  nl_abs_tol = 1e-8
  l_tol = 1e-5
  start_time = 0.0
  end_time = 3.0
  dt = 0.01
[]

[Outputs]
  exodus = true
[]

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_rotation.i)

# This test is to ensure that the smeared cracking model correctly handles finite
# rotation of cracked elements.

# This consists of a single element that is first  subjected to tensile loading
# in the y-direction via a prescribed displacement. This loading is sufficiently
# high to crack the material in that direction, but not completely unload. The
# prescribed displacement is then reversed so that the element is returned to its
# original configuration.

# In the next phase of the analysis, this element is then rotated 90 degrees by
# prescribing the displacement of the bottom of the element. The prescribed
# displacement BC used to crack the element in the first phase is deactivated.

# Once the element is fully rotated, a new BC is activated on what was originally
# the top surface (but is now the surface on the right hand side) to pull in
# the x-direction.

# If everything is working correctly, the model should re-load on the original
# crack (which should be rotated along with the elemnent) up to the peak stress
# in the first phase of the analysis, and then continue the unloading process
# as the crack strains continue to increase. Throughout this analysis, there should
# only be a single crack, as manifested in the crack_flags variables.

[Mesh]
  file = cracking_test.e
[]

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

[Physics/SolidMechanics/QuasiStatic]
  [./all]
    strain = FINITE
    add_variables = true
    generate_output = 'stress_xx stress_yy stress_zz stress_xy stress_yz stress_zx'
  [../]
[]

[AuxVariables]
  [./crack_flags1]
    order = CONSTANT
    family = MONOMIAL
  [../]
  [./crack_flags2]
    order = CONSTANT
    family = MONOMIAL
  [../]
  [./crack_flags3]
    order = CONSTANT
    family = MONOMIAL
  [../]
[]

[AuxKernels]
  [./crack_flags1]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags1
    component = 0
  [../]
  [./crack_flags2]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags2
    component = 1
  [../]
  [./crack_flags3]
    type = MaterialRealVectorValueAux
    property = crack_flags
    variable = crack_flags3
    component = 2
  [../]
[]

[BCs]
  [./x_pin]
    type = DirichletBC
    variable = disp_x
    boundary = '15 16'
    value = 0.0
  [../]
  [./y_pin]
    type = DirichletBC
    variable = disp_y
    boundary = '15 16'
    value = 0.0
  [../]
  [./z_all]
    type = DirichletBC
    variable = disp_z
    boundary = '11 12 13 14 15 16 17 18'
    value = 0.0
  [../]
  [./x_lb]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '11 12'
    function = 'if(t<10,0,if(t>=100,1,1-cos((t-10)*pi/180)))'
  [../]
  [./y_lb]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = '11 12'
    function = 'if(t<10,0,if(t>=100,1,sin((t-10)*pi/180)))'
  [../]
  [./x_lt]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '13 14'
    function = '2+(t-100)*0.01'
  [../]
  [./x_rt]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = '17 18'
    function = '1+(t-100)*0.01'
  [../]
  [./top_pull]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = '13 14 17 18'
    function = 'if(t<5,t*0.01,0.05-(t-5)*0.01)'
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 100.e9
    poissons_ratio = 0.
  [../]
  [./cracking_stress]
    type = ComputeSmearedCrackingStress
    shear_retention_factor = 0.1
    cracking_stress = 3.e9
    cracked_elasticity_type = FULL
    softening_models = exponential_softening
  [../]
  [./exponential_softening]
    type = ExponentialSoftening
  [../]
[]

[Executioner]
  type = Transient

  petsc_options_iname = '-ksp_gmres_restart -pc_type'
  petsc_options_value = '101                lu'
  line_search = 'none'

  l_max_its = 100
  l_tol = 1e-5

  nl_max_its = 100
  nl_abs_tol = 1e-5
  nl_rel_tol = 1e-12

  start_time = 0
  end_time = 110
  dt = 1
[]

[Controls]
  [./p1]
    type = TimePeriod
    start_time = 0.0
    end_time = 10.0
    disable_objects = 'BCs/x_lt BCs/x_rt'
    enable_objects = 'BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
  [./p2]
    type = TimePeriod
    start_time = 10.0
    end_time = 101.0
    disable_objects = 'BCs/x_lt BCs/x_rt BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
  [./p3]
    type = TimePeriod
    start_time = 101.0
    end_time = 110.0
    enable_objects = 'BCs/x_lt BCs/x_rt'
    disable_objects = 'BCs/top_pull'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]
[]

[Outputs]
  exodus = true
[]

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_plane_stress.i)

################################################################################
#
# 1x1x1 cube, single element
# simulate plane stress
# pull in +y direction on right surface to produce shear strain
#
#
#
#          ____________
#         /|          /|
#        / |  5      / |                       -X  Left   1
#       /__________ /  |                       +X  Right  4
#      |   |    3  |   |                       +Y  Top    5
#      | 1 |       | 4 |                       -Y  Bottom 2
#      |   |_6_____|___|           y           +Z  Front  6
#      |  /        |  /            ^           -Z  Back   3
#      | /    2    | /             |
#      |/__________|/              |
#                                  ----> x
#                                 /
#                                /
#                               z
#
#
#
#################################################################################

[Mesh]
  file = cube.e
[]

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

[Functions]
  [./displ]
    type = PiecewiseLinear
    x = '0 0.1 0.2 0.3 0.4'
    y = '0 0.0026 0 -0.0026 0'
  [../]
  [./pressure]
    type = PiecewiseLinear
    x = '0 0.1 0.2 0.3 0.4'
    y = '0 0   0    0   0'
  [../]
[]

[Physics/SolidMechanics/QuasiStatic]
  [./all]
    strain = FINITE
    add_variables = true
    generate_output = 'stress_xx stress_yy stress_zz stress_xy stress_yz stress_zx'
  [../]
[]

[BCs]
  [./pull_y]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = 4
    function = displ
  [../]
  [./pin_x]
    type = DirichletBC
    variable = disp_x
    boundary = '1  4'
    value = 0.0
  [../]
  [./pin_y]
    type = DirichletBC
    variable = disp_y
    boundary = 1
    value = 0.0
  [../]
  [./back]
    type = DirichletBC
    variable = disp_z
    boundary = '3'
    value = 0.0
  [../]
  [./front]
    type = Pressure
    variable = disp_z
    boundary = 6
    function = pressure
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 200.0e3
    poissons_ratio = .3
  [../]
  [./elastic_stress]
    type = ComputeSmearedCrackingStress
    cracking_stress = 120
    cracked_elasticity_type = DIAGONAL
    shear_retention_factor = 0.1
    softening_models = exponential_softening
  [../]
  [./exponential_softening]
    type = ExponentialSoftening
    residual_stress = 0.1
    beta = 0.1
  [../]
[]

[Executioner]
  type = Transient
  #Preconditioned JFNK (default)
  solve_type = 'PJFNK'

  petsc_options_iname = '-ksp_gmres_restart -pc_type -sub_pc_type'
  petsc_options_value = '101                asm      lu'

  line_search = 'none'

  l_max_its = 100
  nl_max_its = 100
  nl_rel_tol = 1e-12
  nl_abs_tol = 1e-8
  l_tol = 1e-5
  start_time = 0.0
  end_time = 0.4
  dt = 0.04
[]

[Outputs]
  exodus = true
[]

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_xyz.i)

#

[Mesh]
  file = cracking_test.e
[]

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

[Functions]
  [./displx]
    type = PiecewiseLinear
    x = '0 1'
    y = '0 0.00175'
  [../]
  [./velocity_y]
    type = ParsedFunction
    expression = 'if(t < 2, 0.00175, 0)'
  [../]
  [./velocity_z]
    type = ParsedFunction
    expression = 0.00175
  [../]
[]

[Physics/SolidMechanics/QuasiStatic]
  [./all]
    strain = FINITE
    add_variables = true
    generate_output = 'stress_xx stress_yy stress_zz stress_xy stress_yz stress_zx'
  [../]
[]

[BCs]
  [./fix_x]
    type = DirichletBC
    variable = disp_x
    boundary = 1
    value = 0.0
  [../]
  [./move_x]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = 4
    function = displx
  [../]

  [./fix_y]
    type = DirichletBC
    variable = disp_y
    boundary = 2
    value = 0.0
  [../]
  [./move_y]
    type = PresetVelocity
    variable = disp_y
    boundary = 5
    function = velocity_y
#    time_periods = 'p2 p3'
  [../]

  [./fix_z]
    type = DirichletBC
    variable = disp_z
    boundary = 3
    value = 0.0
  [../]
  [./move_z]
    type = PresetVelocity
    variable = disp_z
    boundary = 6
    function = velocity_z
#    time_periods = 'p3'
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 186.5e9
    poissons_ratio = .316
  [../]
  [./elastic_stress]
    type = ComputeSmearedCrackingStress
    cracking_stress = 119.3e6
    cracked_elasticity_type = FULL
    softening_models = exponential_softening
  [../]
  [./exponential_softening]
    type = ExponentialSoftening
  [../]
[]

[Executioner]
  type = Transient

  petsc_options_iname = '-ksp_gmres_restart -pc_type'
  petsc_options_value = '101                lu'


  line_search = 'none'


  l_max_its = 100
  l_tol = 1e-5

  nl_max_its = 100
  nl_abs_tol = 1e-6
  #nl_rel_tol = 1e-4
  nl_rel_tol = 1e-8

  start_time = 0.0
  end_time = 3.0
  dt = 0.01
[]

[Controls]
  [./p1]
    type = TimePeriod
    start_time = 0.0
    end_time = 1.0
    disable_objects = 'BCs/move_y BCs/move_z'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]

  [./p2]
    type = TimePeriod
    start_time = 1.0
    end_time = 2.0
    disable_objects = 'BCs/move_z'
    enable_objects = 'BCs/move_y'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
  [../]

  [./p3]
    type = TimePeriod
    start_time = 2.0
    end_time = 3.0
    enable_objects = 'BCs/move_y BCs/move_z'
    reverse_on_false = false
    execute_on = 'initial timestep_begin'
    set_sync_times = true
  [../]
[]

[Outputs]
  exodus = true
[]

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_rz_exponential.i)

#
# Test to exercise the exponential stress release
#
# Stress vs. strain should show a linear relationship until cracking,
#   an exponential stress release, a linear relationship back to zero
#   strain, a linear relationship with the original stiffness in
#   compression and then back to zero strain, a linear relationship
#   back to the exponential curve, and finally further exponential
#   stress release.

[Mesh]
  file = cracking_rz_test.e
[]

[Problem]
  coord_type = RZ
[]

[GlobalParams]
  displacements = 'disp_x disp_y'
[]

[Functions]
  [./disply]
    type = PiecewiseLinear
    x = '0 1       2  3      4 5       6'
    y = '0 0.00175 0 -0.0001 0 0.00175 0.0035'
  [../]
[]

[Physics/SolidMechanics/QuasiStatic]
  [./all]
    strain = FINITE
    add_variables = true
    generate_output = 'stress_xx stress_yy stress_zz stress_xy stress_yz stress_zx'
  [../]
[]

[BCs]
  [./pully]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = 4
    function = disply
  [../]
  [./bottom]
    type = DirichletBC
    variable = disp_y
    boundary = 3
    value = 0.0
  [../]

  [./sides]
    type = DirichletBC
    variable = disp_x
    boundary = 1
    value = 0.0
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 186.5e9
    poissons_ratio = 0.316
  [../]
  [./elastic_stress]
    type = ComputeSmearedCrackingStress
    cracking_stress = 119.3e6
    cracked_elasticity_type = FULL
    softening_models = exponential_softening
  [../]
  [./exponential_softening]
    type = ExponentialSoftening
  [../]
[]

[Executioner]
  type = Transient

  solve_type = 'PJFNK'

  petsc_options_iname = '-ksp_gmres_restart -pc_type'
  petsc_options_value = '101                lu'

  line_search = 'none'
  l_max_its = 100
  l_tol = 1e-5

  nl_max_its = 10
  nl_rel_tol = 1e-8

  nl_abs_tol = 1e-3

  start_time = 0.0
  end_time = 6.0
  dt = 0.005
  dtmin = 0.005
[]

[Outputs]
  exodus = true
[]

(modules/solid_mechanics/test/tests/smeared_cracking/cracking_exponential.i)

#
# Test to exercise the exponential stress release
#
# Stress vs. strain should show a linear relationship until cracking,
#   an exponential stress release, a linear relationship back to zero
#   strain, a linear relationship with the original stiffness in
#   compression and then back to zero strain, a linear relationship
#   back to the exponential curve, and finally further exponential
#   stress release.
#

[Mesh]
  file = cracking_test.e
[]

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

[Functions]
  [./displx]
    type = PiecewiseLinear
    x = '0 1       2  3      4 5       6'
    y = '0 0.00175 0 -0.0001 0 0.00175 0.0035'
  [../]
  [./disply]
    type = PiecewiseLinear
    x = '0 5 6'
    y = '0 0 .00175'
  [../]
  [./displz]
    type = PiecewiseLinear
    x = '0 2 3'
    y = '0 0 .0035'
  [../]
[]

[Physics/SolidMechanics/QuasiStatic]
  [./all]
    strain = FINITE
    add_variables = true
    generate_output = 'stress_xx stress_yy stress_zz stress_xy stress_yz stress_zx'
  [../]
[]

[BCs]
  [./pullx]
    type = FunctionDirichletBC
    #type = FunctionDirichletBC
    variable = disp_x
    boundary = 4
    function = displx
  [../]
  [./left]
    type = DirichletBC
    variable = disp_x
    boundary = 1
    value = 0.0
  [../]

  [./fix_y]
    type = DirichletBC
    variable = disp_y
    boundary = '11 12'
    value = 0.0
  [../]

  [./move_y]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = '15 16'
    function = disply
  [../]

  [./back]
    type = DirichletBC
    variable = disp_z
    boundary = '3'
    value = 0.0
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 186.5e9
    poissons_ratio = .316
  [../]
  [./elastic_stress]
    type = ComputeSmearedCrackingStress
    cracking_stress = 119.3e6
    cracked_elasticity_type = FULL
    softening_models = exponential_softening
  [../]
  [./exponential_softening]
    type = ExponentialSoftening
  [../]
[]

[Executioner]
  type = Transient

  petsc_options_iname = '-ksp_gmres_restart -pc_type'
  petsc_options_value = '101                lu'

  line_search = 'none'
  l_max_its = 100
  l_tol = 1e-6

  nl_max_its = 10
  nl_rel_tol = 1e-12
  nl_abs_tol = 1.e-4

  start_time = 0.0
  dt = 0.02
  dtmin = 0.02
  num_steps = 300
[]

[Outputs]
  exodus = true
[]

Description
Example Input File
Input Parameters
Input Files
References