MeshCut2DFractureUserObject

XFEM mesh cutter for 2D models that defines cuts with amesh and uses fracture integrals to determine growth

Overview

This class is used to define an evolving cutting plane for 2D XFEM simulations based on a mesh that defines the initial crack and uses fracture integrals to grow that crack. It (1) reads in a mesh describing the crack surface, (2) uses the mesh to do initial cutting of 2D elements, and (3) grows the mesh incrementally based on fracture domain integrals to allow nonplanar crack growth based on propagation directions also determined by fracture integrals.

The crack propagates if the failure criterion is met, given by: $var element = document.getElementById("moose-equation-db8f25ed-cb7d-4e5c-85f0-3a6061eb1757");katex.render("K_c \\le \\sqrt{K^2_I+K^2_{II}}", element, {displayMode:true,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ where $var element = document.getElementById("moose-equation-148434fd-65b2-4800-b519-8fc1f60a75a7");katex.render("K_I", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ and $var element = document.getElementById("moose-equation-e238a775-6850-496f-aeda-2e5185fb49ae");katex.render("K_{II}", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ are the mode I and II stress intensity factors provided by the fracture integral and the material property $var element = document.getElementById("moose-equation-8bbf23da-e8e7-405e-994f-81287273c495");katex.render("K_c", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is given defined in the input file by "k_critical". The crack growth direction is given by the direction the maximized the crack-tip hoop stress, given by Equation 5 in Jiang et al. (2020). The growth increment is a user provided input given in the defined by "growth_increment".

Quasistatic behavior is assumed, and an iterative approach is taken to repeatedly solve the equilibrium equations, evaluate the fracture integrals, and as indicated by the failure criterion, incrementally advance the crack until the failure criterion is no longer met. To iteratively repeat the solution in this manner for each step, "max_xfem_update" must be set in the Executioner block, and should be large enough to allow a sufficient number of iterations for crack growth to cease during each timestep.

Example Input Syntax

[UserObjects]
  [cut_mesh2]
    type = MeshCut2DFractureUserObject
    mesh_file = make_edge_crack_in.e
    k_critical = 80
    growth_increment = 0.1
  []
[]

Input Parameters

growth_incrementLength to grow crack if k>k_critical
C++ Type:double
Controllable:No
Description:Length to grow crack if k>k_critical
k_criticalCritical fracture toughness.
C++ Type:double
Controllable:No
Description:Critical fracture toughness.
mesh_fileMesh file for the XFEM geometric cut; currently only the Exodus type is supported
C++ Type:MeshFileName
Controllable:No
Description:Mesh file for the XFEM geometric cut; currently only the Exodus type is supported

Required Parameters

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
execute_onXFEM_MARKThe list of flag(s) indicating when this object should be executed, the available options include XFEM_MARK, FORWARD, ADJOINT, HOMOGENEOUS_FORWARD, ADJOINT_TIMESTEP_BEGIN, ADJOINT_TIMESTEP_END, NONE, INITIAL, LINEAR, NONLINEAR, TIMESTEP_END, TIMESTEP_BEGIN, MULTIAPP_FIXED_POINT_END, MULTIAPP_FIXED_POINT_BEGIN, FINAL, CUSTOM.
Default:XFEM_MARK
C++ Type:ExecFlagEnum
Options:XFEM_MARK, FORWARD, ADJOINT, HOMOGENEOUS_FORWARD, ADJOINT_TIMESTEP_BEGIN, ADJOINT_TIMESTEP_END, NONE, INITIAL, LINEAR, NONLINEAR, TIMESTEP_END, TIMESTEP_BEGIN, MULTIAPP_FIXED_POINT_END, MULTIAPP_FIXED_POINT_BEGIN, FINAL, CUSTOM
Controllable:No
Description:The list of flag(s) indicating when this object should be executed, the available options include XFEM_MARK, FORWARD, ADJOINT, HOMOGENEOUS_FORWARD, ADJOINT_TIMESTEP_BEGIN, ADJOINT_TIMESTEP_END, NONE, INITIAL, LINEAR, NONLINEAR, TIMESTEP_END, TIMESTEP_BEGIN, MULTIAPP_FIXED_POINT_END, MULTIAPP_FIXED_POINT_BEGIN, FINAL, CUSTOM.
heal_alwaysFalseHeal previous cuts at every time step
Default:False
C++ Type:bool
Controllable:No
Description:Heal previous cuts at every time step
nucleate_uoThe MeshCutNucleation UO for nucleating cracks.
C++ Type:UserObjectName
Controllable:No
Description:The MeshCutNucleation UO for nucleating cracks.
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.
ring_number1Fracture integral ring number
Default:1
C++ Type:unsigned int
Controllable:No
Description:Fracture integral ring number
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

allow_duplicate_execution_on_initialFalseIn the case where this UserObject is depended upon by an initial condition, allow it to be executed twice during the initial setup (once before the IC and again after mesh adaptivity (if applicable).
Default:False
C++ Type:bool
Controllable:No
Description:In the case where this UserObject is depended upon by an initial condition, allow it to be executed twice during the initial setup (once before the IC and again after mesh adaptivity (if applicable).
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.
execution_order_group0Execution order groups are executed in increasing order (e.g., the lowest number is executed first). Note that negative group numbers may be used to execute groups before the default (0) group. Please refer to the user object documentation for ordering of user object execution within a group.
Default:0
C++ Type:int
Controllable:No
Description:Execution order groups are executed in increasing order (e.g., the lowest number is executed first). Note that negative group numbers may be used to execute groups before the default (0) group. Please refer to the user object documentation for ordering of user object execution within a group.
force_postauxFalseForces the UserObject to be executed in POSTAUX
Default:False
C++ Type:bool
Controllable:No
Description:Forces the UserObject to be executed in POSTAUX
force_preauxFalseForces the UserObject to be executed in PREAUX
Default:False
C++ Type:bool
Controllable:No
Description:Forces the UserObject to be executed in PREAUX
force_preicFalseForces the UserObject to be executed in PREIC during initial setup
Default:False
C++ Type:bool
Controllable:No
Description:Forces the UserObject to be executed in PREIC during initial setup
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

Input Files

(modules/xfem/test/tests/nucleation_uo/nucleate_edge_crack_2d.i)
(modules/xfem/test/tests/nucleation_uo/nucleate_AllEdgeCracks.i)
(modules/xfem/test/tests/solid_mechanics_basic/edge_crack_2d_propagation_mhs.i)
(modules/xfem/test/tests/nucleation_uo/nucleate_2edge_cracks_2d.i)

References

Wen Jiang, Benjamin W. Spencer, and John E. Dolbow. Ceramic nuclear fuel fracture modeling with the extended finite element method. Engineering Fracture Mechanics, 223:106713, 2020. URL: http://www.sciencedirect.com/science/article/pii/S0013794419307568, doi:https://doi.org/10.1016/j.engfracmech.2019.106713.

@article{jiang2020,
    author = "Jiang, Wen and Spencer, Benjamin W. and Dolbow, John E.",
    title = "Ceramic nuclear fuel fracture modeling with the extended finite element method",
    journal = "Engineering Fracture Mechanics",
    volume = "223",
    pages = "106713",
    year = "2020",
    issn = "0013-7944",
    doi = "https://doi.org/10.1016/j.engfracmech.2019.106713",
    url = "http://www.sciencedirect.com/science/article/pii/S0013794419307568"
}

(modules/xfem/test/tests/solid_mechanics_basic/edge_crack_2d_propagation_mhs.i)

[GlobalParams]
  displacements = 'disp_x disp_y'
  volumetric_locking_correction = true
[]

[XFEM]
  geometric_cut_userobjects = 'cut_mesh2'
  qrule = volfrac
  output_cut_plane = true
[]

[Mesh]
[gen]
  type = GeneratedMeshGenerator
  dim = 2
  nx = 45
  ny = 15
  xmin = -1.5
  xmax = 1.5
  ymin = 0.0
  ymax = 1.0
  elem_type = QUAD4
[]
[dispBlock]
  type = BoundingBoxNodeSetGenerator
  new_boundary = pull_set
  bottom_left = '-0.1 0.99 0'
  top_right = '0.1 1.01 0'
  input = gen
[]
[]

[DomainIntegral]
  integrals = 'Jintegral InteractionIntegralKI InteractionIntegralKII'
  displacements = 'disp_x disp_y'
  crack_front_points_provider = cut_mesh2
  2d=true
  number_points_from_provider = 2
  crack_direction_method = CurvedCrackFront
  radius_inner = '0.15'
  radius_outer = '0.45'
  poissons_ratio = 0.3
  youngs_modulus = 207000
  block = 0
  incremental = true
  used_by_xfem_to_grow_crack = true
[]

[UserObjects]
  [cut_mesh2]
    type = MeshCut2DFractureUserObject
    mesh_file = make_edge_crack_in.e
    k_critical=80
    growth_increment = 0.1
  []
[]

[Modules/TensorMechanics/Master]
  [./all]
    strain = FINITE
    planar_formulation = plane_strain
    add_variables = true
    generate_output = 'stress_xx stress_yy vonmises_stress'
  [../]
[]

[BCs]
  [top_y]
      type = DirichletBC
      boundary = pull_set
      variable = disp_y
      value = 0.001
  []
  [bottom_x]
    type = DirichletBC
    boundary = bottom
    variable = disp_x
    value = 0.0
  []
  [bottom_y]
    type = DirichletBC
    boundary = bottom
    variable = disp_y
    value = 0.0
  []
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 207000
    poissons_ratio = 0.3
    block = 0
  [../]
  [./stress]
    type = ComputeFiniteStrainElasticStress
    block = 0
  [../]
[]

[Executioner]
  type = Transient

  solve_type = 'PJFNK'
  petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
  petsc_options_value = '201                hypre    boomeramg      8'

  line_search = 'none'

  [./Predictor]
    type = SimplePredictor
    scale = 1.0
  [../]

# controls for linear iterations
  l_max_its = 100
  l_tol = 1e-2

# controls for nonlinear iterations
  nl_max_its = 15
  nl_rel_tol = 1e-8
  nl_abs_tol = 1e-9

# time control
  start_time = 0.0
  dt = 1.0
  end_time = 1
  max_xfem_update = 100
[]

[Outputs]
  exodus = true
  execute_on = TIMESTEP_END
  [xfemcutter]
    type=XFEMCutMeshOutput
    xfem_cutter_uo=cut_mesh2
  []
  # console = false
  [./console]
    type = Console
    output_linear = false
    output_nonlinear = false
  [../]
[]

(modules/xfem/test/tests/nucleation_uo/nucleate_edge_crack_2d.i)

[GlobalParams]
  displacements = 'disp_x disp_y'
  volumetric_locking_correction = true
[]

[XFEM]
  geometric_cut_userobjects = 'cut_mesh2'
  qrule = volfrac
  output_cut_plane = true
[]

[Mesh]
[gen]
  type = GeneratedMeshGenerator
  dim = 2
  nx = 20
  ny = 10
  xmin = 0
  xmax = 2
  ymin = 0.0
  ymax = 1.0
  elem_type = QUAD4
[]
[top_left]
  type = BoundingBoxNodeSetGenerator
  new_boundary = pull_top_left
  bottom_left = '-0.01 0.99 0'
  top_right = '0.11 1.01 0'
  input = gen
[]
[top_right]
  type = BoundingBoxNodeSetGenerator
  new_boundary = pull_top_right
  bottom_left = '1.89 0.99 0'
  top_right = '2.01 1.01 0'
  input = top_left
[]
[top_middle_ss]
  type = SideSetsFromBoundingBoxGenerator
  input = top_right
  bottom_left = '0.79 0.89 0'
  top_right = '1.21 1.01 0'
  block_id = '0'
  boundary_new = top_middle_ss
  boundaries_old = top
[]
[nucleate]
  type = ParsedSubdomainMeshGenerator
  input = top_middle_ss
  combinatorial_geometry = 'y > 0.39 & y < 0.51'
  block_id = 10
[]
[]

[DomainIntegral]
  integrals = 'InteractionIntegralKI InteractionIntegralKII'
  displacements = 'disp_x disp_y'
  crack_front_points_provider = cut_mesh2
  2d=true
  number_points_from_provider = 0
  crack_direction_method = CurvedCrackFront
  radius_inner = '0.15'
  radius_outer = '0.45'
  poissons_ratio = 0.3
  youngs_modulus = 207000
  block = 0
  incremental = true
  used_by_xfem_to_grow_crack = true
[]

[UserObjects]
  [nucleate]
    type = MeshCut2DRankTwoTensorNucleation
    tensor = stress
    scalar_type = MaxPrincipal
    nucleation_threshold = nucleation_threshold
    initiate_on_boundary = 'left right'
    nucleation_length = .2
  []
  [cut_mesh2]
    type = MeshCut2DFractureUserObject
    mesh_file = make_edge_crack_in.e
    k_critical=230
    growth_increment = 0.11
    nucleate_uo = nucleate
  []
[]
[AuxVariables]
  [nucleation_threshold]
    order = CONSTANT
    family = MONOMIAL
  []
[]
[ICs]
   [nucleation_bulk]
     type = ConstantIC
     value = 10000
     variable = nucleation_threshold
     block = 0
   []
   [nucleation_weak]
    type = FunctionIC
    function = nucleation_x
    variable = nucleation_threshold
    block = 10
  []
[]

[Functions]
  [nucleation_x]
    type = ParsedFunction
    expression = '300+x*50'
  []
[]

[Modules/TensorMechanics/Master]
  [./all]
    strain = FINITE
    planar_formulation = plane_strain
    add_variables = true
    generate_output = 'stress_xx stress_yy vonmises_stress max_principal_stress'
  [../]
[]

[Functions]
  [bc_pull_top]
    type = ParsedFunction
    expression = 0.0005*t
  []
[]

[BCs]
  [top_edges]
      type = FunctionDirichletBC
      boundary = 'pull_top_left pull_top_right'
      variable = disp_y
      function = bc_pull_top
  []
  [top_middle]
    type = NeumannBC
    boundary = top_middle_ss
    variable = disp_y
    value = -2000
  []
  [bottom_x]
    type = DirichletBC
    boundary = bottom
    variable = disp_x
    value = 0.0
  []
  [bottom_y]
    type = DirichletBC
    boundary = bottom
    variable = disp_y
    value = 0.0
  []
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 207000
    poissons_ratio = 0.3
  [../]
  [./stress]
    type = ComputeFiniteStrainElasticStress
  [../]
[]

[Executioner]
  type = Transient

  solve_type = 'PJFNK'
  petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
  petsc_options_value = '201                hypre    boomeramg      8'

  line_search = 'none'

  [./Predictor]
    type = SimplePredictor
    scale = 1.0
  [../]

# controls for linear iterations
  l_max_its = 100
  l_tol = 1e-2

# controls for nonlinear iterations
  nl_max_its = 15
  nl_rel_tol = 1e-8
  nl_abs_tol = 1e-9

# time control
  start_time = 0.0
  dt = 1.0
  end_time = 5
  max_xfem_update = 100
[]

[Outputs]
  csv=true
  execute_on = TIMESTEP_END
  # [xfemcutter]
  #   type=XFEMCutMeshOutput
  #   xfem_cutter_uo=cut_mesh2
  # []
  # console = false
  [./console]
    type = Console
    output_linear = false
    output_nonlinear = false
  [../]
[]

(modules/xfem/test/tests/nucleation_uo/nucleate_AllEdgeCracks.i)

[GlobalParams]
  displacements = 'disp_x disp_y'
[]

[XFEM]
  geometric_cut_userobjects = 'cut_mesh2'
  qrule = volfrac
  output_cut_plane = true
[]

[Mesh]
[gen]
  type = GeneratedMeshGenerator
  dim = 2
  nx = 10
  ny = 20
  xmin = 0
  xmax = 1.0
  ymin = 0.0
  ymax = 2.0
  elem_type = QUAD4
[]
[top_left]
  type = BoundingBoxNodeSetGenerator
  new_boundary = pull_top_left
  bottom_left = '-0.01 1.99 0'
  top_right = '0.11 2.01 0'
  input = gen
[]
[]

[DomainIntegral]
  integrals = 'InteractionIntegralKI InteractionIntegralKII'
  displacements = 'disp_x disp_y'
  crack_front_points_provider = cut_mesh2
  2d=true
  number_points_from_provider = 0
  crack_direction_method = CurvedCrackFront
  radius_inner = '0.15'
  radius_outer = '0.45'
  poissons_ratio = 0.3
  youngs_modulus = 207000
  block = 0
  incremental = true
  used_by_xfem_to_grow_crack = true
[]

[UserObjects]
  [nucleate]
    type = MeshCut2DRankTwoTensorNucleation
    tensor = stress
    scalar_type = MaxPrincipal
    nucleation_threshold = 180
    initiate_on_boundary = 'left'
    nucleation_length = .2
    nucleation_radius = .21
  []
  [cut_mesh2]
    type = MeshCut2DFractureUserObject
    mesh_file = make_edge_crack_in.e
    k_critical=500000 #Large so that cracks will not grow
    growth_increment = 0.11
    nucleate_uo = nucleate
  []
[]

[Modules/TensorMechanics/Master]
  [all]
    strain = FINITE
    planar_formulation = plane_strain
    add_variables = true
    generate_output = 'stress_xx stress_yy vonmises_stress max_principal_stress'
  []
[]

[Functions]
  [bc_pull_top]
    type = ParsedFunction
    expression = 0.0005*t
  []
[]

[BCs]
  [top_edges]
      type = FunctionDirichletBC
      boundary = 'pull_top_left'
      variable = disp_y
      function = bc_pull_top
  []
  [bottom_x]
    type = DirichletBC
    boundary = bottom
    variable = disp_x
    value = 0.0
  []
  [bottom_y]
    type = DirichletBC
    boundary = bottom
    variable = disp_y
    value = 0.0
  []
[]

[Materials]
  [elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 207000
    poissons_ratio = 0.3
  []
  [stress]
    type = ComputeFiniteStrainElasticStress
  []
[]

[Executioner]
  type = Transient

  solve_type = 'PJFNK'
  petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
  petsc_options_value = '201                hypre    boomeramg      8'

  line_search = 'none'

  [./Predictor]
    type = SimplePredictor
    scale = 1.0
  [../]

  l_max_its = 100
  l_tol = 1e-2

  nl_max_its = 15
  nl_rel_tol = 1e-8
  nl_abs_tol = 1e-9

  start_time = 0.0
  dt = 1.0
  end_time = 5
  max_xfem_update = 100
[]

[Outputs]
  csv=true
  exodus=true
  execute_on = TIMESTEP_END
[]

(modules/xfem/test/tests/solid_mechanics_basic/edge_crack_2d_propagation_mhs.i)

[GlobalParams]
  displacements = 'disp_x disp_y'
  volumetric_locking_correction = true
[]

[XFEM]
  geometric_cut_userobjects = 'cut_mesh2'
  qrule = volfrac
  output_cut_plane = true
[]

[Mesh]
[gen]
  type = GeneratedMeshGenerator
  dim = 2
  nx = 45
  ny = 15
  xmin = -1.5
  xmax = 1.5
  ymin = 0.0
  ymax = 1.0
  elem_type = QUAD4
[]
[dispBlock]
  type = BoundingBoxNodeSetGenerator
  new_boundary = pull_set
  bottom_left = '-0.1 0.99 0'
  top_right = '0.1 1.01 0'
  input = gen
[]
[]

[DomainIntegral]
  integrals = 'Jintegral InteractionIntegralKI InteractionIntegralKII'
  displacements = 'disp_x disp_y'
  crack_front_points_provider = cut_mesh2
  2d=true
  number_points_from_provider = 2
  crack_direction_method = CurvedCrackFront
  radius_inner = '0.15'
  radius_outer = '0.45'
  poissons_ratio = 0.3
  youngs_modulus = 207000
  block = 0
  incremental = true
  used_by_xfem_to_grow_crack = true
[]

[UserObjects]
  [cut_mesh2]
    type = MeshCut2DFractureUserObject
    mesh_file = make_edge_crack_in.e
    k_critical=80
    growth_increment = 0.1
  []
[]

[Modules/TensorMechanics/Master]
  [./all]
    strain = FINITE
    planar_formulation = plane_strain
    add_variables = true
    generate_output = 'stress_xx stress_yy vonmises_stress'
  [../]
[]

[BCs]
  [top_y]
      type = DirichletBC
      boundary = pull_set
      variable = disp_y
      value = 0.001
  []
  [bottom_x]
    type = DirichletBC
    boundary = bottom
    variable = disp_x
    value = 0.0
  []
  [bottom_y]
    type = DirichletBC
    boundary = bottom
    variable = disp_y
    value = 0.0
  []
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 207000
    poissons_ratio = 0.3
    block = 0
  [../]
  [./stress]
    type = ComputeFiniteStrainElasticStress
    block = 0
  [../]
[]

[Executioner]
  type = Transient

  solve_type = 'PJFNK'
  petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
  petsc_options_value = '201                hypre    boomeramg      8'

  line_search = 'none'

  [./Predictor]
    type = SimplePredictor
    scale = 1.0
  [../]

# controls for linear iterations
  l_max_its = 100
  l_tol = 1e-2

# controls for nonlinear iterations
  nl_max_its = 15
  nl_rel_tol = 1e-8
  nl_abs_tol = 1e-9

# time control
  start_time = 0.0
  dt = 1.0
  end_time = 1
  max_xfem_update = 100
[]

[Outputs]
  exodus = true
  execute_on = TIMESTEP_END
  [xfemcutter]
    type=XFEMCutMeshOutput
    xfem_cutter_uo=cut_mesh2
  []
  # console = false
  [./console]
    type = Console
    output_linear = false
    output_nonlinear = false
  [../]
[]

(modules/xfem/test/tests/nucleation_uo/nucleate_2edge_cracks_2d.i)

[GlobalParams]
  displacements = 'disp_x disp_y'
  volumetric_locking_correction = true
[]

[XFEM]
  geometric_cut_userobjects = 'cut_mesh2'
  qrule = volfrac
  output_cut_plane = true
[]

[Mesh]
[gen]
  type = GeneratedMeshGenerator
  dim = 2
  nx = 30
  ny = 15
  xmin = -2
  xmax = -.2
  ymin = 0.0
  ymax = 1.0
  elem_type = QUAD4
[]
[dispBlock_top]
  type = BoundingBoxNodeSetGenerator
  new_boundary = pull_top_y
  bottom_left = '-2.1 0.99 0'
  top_right = '-1.9 1.01 0'
  input = gen
[]
[dispBlock_bot]
  type = BoundingBoxNodeSetGenerator
  new_boundary = pull_bot_y
  bottom_left = '-2.1 -.01 0'
  top_right = '-1.9 0.01 0'
  input = dispBlock_top
[]
[]

[DomainIntegral]
  integrals = 'Jintegral InteractionIntegralKI InteractionIntegralKII'
  displacements = 'disp_x disp_y'
  crack_front_points_provider = cut_mesh2
  2d=true
  number_points_from_provider = 1
  crack_direction_method = CurvedCrackFront
  radius_inner = '0.15'
  radius_outer = '0.45'
  poissons_ratio = 0.3
  youngs_modulus = 207000
  block = 0
  incremental = true
  used_by_xfem_to_grow_crack = true
[]

[UserObjects]
  #fixme, nucleate has to be before cut_mesh2 in the input file or cut_mesh2 can't finde the nucleate_uo
  [nucleate]
    type = MeshCut2DRankTwoTensorNucleation
    tensor = stress
    scalar_type = MaxPrincipal
    nucleation_threshold = nucleation_threshold
    initiate_on_boundary = 'left bottom'
    average = true
    nucleation_length = .1
  []
  [cut_mesh2]
    type = MeshCut2DFractureUserObject
    mesh_file = make_edge_crack_in.e
    k_critical=80
    growth_increment = 0.1
    nucleate_uo = nucleate
  []
[]
[AuxVariables]
  [nucleation_threshold]
    order = CONSTANT
    family = MONOMIAL
  []
[]
[ICs]
   [nucleation]
     type = FunctionIC
     function =  nucleation_x_y
     variable = nucleation_threshold
   []
  # [nucleation]
  #   type = VolumeWeightedWeibull
  #   variable = nucleation_threshold
  #   reference_volume = 0.01 #This is the volume of an element for a 100x100 mesh
  #   weibull_modulus = 2
  #   median = 5000.0
  # []
[]

[Functions]
  [nucleation_y]
    type = ParsedFunction
    expression = 'if(y>0.7,10000,if(y<0.5,10000,4000*(1-y)^2-10000))'
  []
  [nucleation_x]
    type = ParsedFunction
    expression = 'if(x>-0.9,10000,if(x<-1.1,10000,1000*(x)^2-10000))'
  []
  [nucleation_x_y]
    type = LinearCombinationFunction
    functions = 'nucleation_x nucleation_y'
    w = '1 1'
  []
[]

[Modules/TensorMechanics/Master]
  [./all]
    strain = FINITE
    planar_formulation = plane_strain
    add_variables = true
    generate_output = 'stress_xx stress_yy vonmises_stress max_principal_stress'
  [../]
[]

[Functions]
  [bc_pull_top]
    type = ParsedFunction
    expression = 'if(t<6,0.0008*t,0.0008*5+0.0004*(t-6))'
  []
  [bc_pull_bot]
    type = ParsedFunction
    expression = 0.0004*t
  []
[]

[BCs]
  [top_left]
      type = FunctionDirichletBC
      boundary = pull_top_y
      variable = disp_y
      function = bc_pull_top
  []
  [bot_left]
    type = FunctionDirichletBC
    boundary = pull_bot_y
    variable = disp_y
    function = bc_pull_bot
[]
  [bottom_x]
    type = DirichletBC
    boundary = right
    variable = disp_x
    value = 0.0
  []
  [bottom_y]
    type = DirichletBC
    boundary = right
    variable = disp_y
    value = 0.0
  []
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 207000
    poissons_ratio = 0.3
    block = 0
  [../]
  [./stress]
    type = ComputeFiniteStrainElasticStress
    block = 0
  [../]
[]

[Executioner]
  type = Transient

  solve_type = 'PJFNK'
  petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
  petsc_options_value = '201                hypre    boomeramg      8'

  line_search = 'none'

  [./Predictor]
    type = SimplePredictor
    scale = 1.0
  [../]

# controls for linear iterations
  l_max_its = 100
  l_tol = 1e-2

# controls for nonlinear iterations
  nl_max_its = 15
  nl_rel_tol = 1e-8
  nl_abs_tol = 1e-9

# time control
  start_time = 0.0
  dt = 1.0
  end_time = 55
  max_xfem_update = 2
[]

[Outputs]
  # csv=true
  exodus = true
  execute_on = TIMESTEP_END
  # [xfemcutter]
  #   type=XFEMCutMeshOutput
  #   xfem_cutter_uo=cut_mesh2
  # []
  # console = false
  [./console]
    type = Console
    output_linear = false
    output_nonlinear = false
  [../]
[]

Overview
Example Input Syntax
Input Parameters
Input Files
References