Hill Creep Stress Update

This class uses the stress update material in a generalized radial return anisotropic power law creep model. This class can be used in conjunction with other creep and plasticity materials for more complex simulations.

Description

This class computes a creep strain rate based on an equivalent deviatoric stress function that is calculated as a function of Hill's function anisotropy parameters $var element = document.getElementById("moose-equation-f0220441-1ff9-4a37-bf7a-fd0023a10828");katex.render("F", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-c640b14c-71ed-46f4-9360-1db55aad17eb");katex.render("G", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-542b26ff-1a2d-45a4-8af2-d66c72e01a8c");katex.render("H", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-deb08ee0-a9ba-4355-8de6-27021bdf9828");katex.render("L", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-3944e299-79aa-4fdc-bd98-9f722b8ad70c");katex.render("M", element, {displayMode:false,throwOnError:false});$ , and $var element = document.getElementById("moose-equation-8a90baa1-dff3-4746-9d32-87e7b5ee7e5f");katex.render("N", element, {displayMode:false,throwOnError:false});$ : $var element = document.getElementById("moose-equation-c72f1671-49fa-4d09-a1e0-dd75a724e45c");katex.render("\\tilde{q}(\\sigma) = {[F(\\sigma_{22} - \\sigma_{33})^2 + G(\\sigma_{33} - \\sigma_{11})^2 + H(\\sigma_{11} - \\sigma_{22})^2 + 2L\\sigma_{23}^2 + 2M\\sigma_{13}^2 + 2N\\sigma_{12}^2]}^{1/2}", element, {displayMode:true,throwOnError:false});$

The equivalent creep strain rate function may then be obtained as $var element = document.getElementById("moose-equation-7f00e13d-a0f5-40cd-8365-816908739f36");katex.render("\\dot{\\epsilon} = A_{aniso} (\\tilde{q})^{n}", element, {displayMode:true,throwOnError:false});$

where $var element = document.getElementById("moose-equation-f007d168-1a54-4166-a8cc-88d9f06464e1");katex.render("A_{aniso}", element, {displayMode:false,throwOnError:false});$ is a creep coefficient and $var element = document.getElementById("moose-equation-697e2ef3-7ee0-41d2-962d-c78c43252ecd");katex.render("n", element, {displayMode:false,throwOnError:false});$ the creep exponent.

The effective creep strain increment is obtained within the framework of a generalized (Hill plasticity) radial return mapping, see GeneralizedRadialReturnStressUpdate. This class computes the generalized radial return inelastic increment.

More details on the Hill-type creep material model may be found in Stewart et al. (2011).

Numerical time integration error

The return mapping algorithm used to solve for elastic and inelastic strains relies on an additive decomposition. The stress increment can be determined, assuming a one-dimensional problem, as $var element = document.getElementById("moose-equation-c94cc203-166e-47f4-9d6c-54c9ed31aa77");katex.render("\\Delta\\sigma = E \\Delta\\epsilon^{elastic} = E (\\Delta\\epsilon^{total} - \\Delta\\epsilon^{creep})", element, {displayMode:false,throwOnError:false});$ , where $var element = document.getElementById("moose-equation-a08ab640-8fbd-4307-931c-31a06d20ba5e");katex.render("E", element, {displayMode:false,throwOnError:false});$ is a representative value of the Young's modulus. One way of limiting the error incurred in the numerical time integration is to compare it with the elastic strain increment during such an increment. Namely, we want to ensure that $var element = document.getElementById("moose-equation-bb28074e-a485-4e87-a14b-a078c7db8311");katex.render("err_{creep} \\ll \\frac{\\Delta\\sigma}{E}", element, {displayMode:false,throwOnError:false});$ . Estimating the creep numerical integration error as proportional to the increment of creep strain rates: $var element = document.getElementById("moose-equation-94f8f9be-6598-405f-9ee1-d204630e003e");katex.render("err_{creep} = (\\Delta\\dot{\\epsilon}_{t+\\Delta t} - \\Delta\\dot{\\epsilon}_{t}) \\cdot \\Delta t", element, {displayMode:false,throwOnError:false});$ , the recommended time step is

$(1)var element = document.getElementById("moose-equation-831ed645-d9cd-47a7-9a97-c88bb092999d");katex.render("\\Delta t_{limit} = \\frac{\\Delta t \\cdot E \\cdot userTolerance}{\\Delta\\sigma}, ", element, {displayMode:true,throwOnError:false});$

where $var element = document.getElementById("moose-equation-4ef9f152-6c17-4ca4-b085-a51684c1a494");katex.render("\\Delta t_{limit}", element, {displayMode:false,throwOnError:false});$ is the computed time step limit, $var element = document.getElementById("moose-equation-2d34f2e5-b7b4-44a7-8faf-d9196b1c9e7f");katex.render("\\Delta t", element, {displayMode:false,throwOnError:false});$ is the current time step, $var element = document.getElementById("moose-equation-00908528-55f0-499a-9cc1-cca22d27527b");katex.render("\\Delta\\sigma", element, {displayMode:false,throwOnError:false});$ denotes a stress time increment scalar, and $var element = document.getElementById("moose-equation-098a5668-cfca-4390-865c-022053e88c7d");katex.render("userTolerance", element, {displayMode:false,throwOnError:false});$ is the maximum numerical time integration error selected by the user. As Eq. (1) suggests, the creep error depends on the material stiffness and the given stress increment. For complex simulation scenarios, controlling this error by only prescribing a maximum inelastic strain increment may not be sufficient to limit creep error. Furthermore, too conservative selection of the maximum inelastic strain may lead to a large increase in the number of time steps required to finish the simulation.

warning:Selection of time step increments with creep

It is recommended to choose a max_inelastic_increment that guarantees that creep strain increments are well within the small strain increment assumption. Complementarily, max_integration_error must be selected such that the numerical time integration will not significantly affect the creep results. Usually, for most applications, values on the order of $var element = document.getElementById("moose-equation-815be1bb-8fa5-4655-84b2-63c2120512b9");katex.render("1.0\\cdot10^{-3}", element, {displayMode:false,throwOnError:false});$ - $var element = document.getElementById("moose-equation-18af9426-67b0-465e-b2a0-ef1ab0da47da");katex.render("1.0\\cdot10^{-5}", element, {displayMode:false,throwOnError:false});$ will suffice. For better results, these time integration limits may be combined with a soft Terminator.

For three-dimensional problems, a norm of the stress diference and a representative value for the Young's modulus is used internally.

Example Input File Syntax

[trial_creep_two]
  type = ADHillCreepStressUpdate
  coefficient = 1e-16
  n_exponent = 9
  m_exponent = 0
  activation_energy = 0
  max_inelastic_increment = 0.00003
  absolute_tolerance = 1e-20
  relative_tolerance = 1e-20
  # Force it to not use integration error
  max_integration_error = 0.000001
[]

Input Parameters

activation_energyActivation energy
C++ Type:double
Controllable:No
Description:Activation energy
coefficientLeading coefficient in power-law equation
C++ Type:double
Controllable:No
Description:Leading coefficient in power-law equation
effective_inelastic_strain_nameeffective_creep_strainName of the material property that stores the effective inelastic strain
Default:effective_creep_strain
C++ Type:std::string
Controllable:No
Description:Name of the material property that stores the effective inelastic strain
inelastic_strain_rate_namecreep_strain_rateName of the material property that stores the inelastic strain rate
Default:creep_strain_rate
C++ Type:std::string
Controllable:No
Description:Name of the material property that stores the inelastic strain rate
n_exponentExponent on effective stress in power-law equation
C++ Type:double
Controllable:No
Description:Exponent on effective stress in power-law equation

Required Parameters

absolute_tolerance1e-11Absolute convergence tolerance for Newton iteration
Default:1e-11
C++ Type:double
Controllable:No
Description:Absolute convergence tolerance for Newton iteration
acceptable_multiplier10Factor applied to relative and absolute tolerance for acceptable convergence if iterations are no longer making progress
Default:10
C++ Type:double
Controllable:No
Description:Factor applied to relative and absolute tolerance for acceptable convergence if iterations are no longer making progress
base_nameOptional parameter that defines a prefix for all material properties related to this stress update model. This allows for multiple models of the same type to be used without naming conflicts.
C++ Type:std::string
Controllable:No
Description:Optional parameter that defines a prefix for all material properties related to this stress update model. This allows for multiple models of the same type to be used without naming conflicts.
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.
gas_constant8.3143Universal gas constant
Default:8.3143
C++ Type:double
Controllable:No
Description:Universal gas constant
m_exponent0Exponent on time in power-law equation
Default:0
C++ Type:double
Controllable:No
Description:Exponent on time in power-law equation
max_inelastic_increment0.0001The maximum inelastic strain increment allowed in a time step
Default:0.0001
C++ Type:double
Controllable:No
Description:The maximum inelastic strain increment allowed in a time step
max_integration_error0.0005The maximum inelastic strain increment integration error allowed
Default:0.0005
C++ Type:double
Controllable:No
Description:The maximum inelastic strain increment integration error allowed
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.
relative_tolerance1e-08Relative convergence tolerance for Newton iteration
Default:1e-08
C++ Type:double
Controllable:No
Description:Relative convergence tolerance for Newton iteration
start_time0Start time (if not zero)
Default:0
C++ Type:double
Controllable:No
Description:Start time (if not zero)
temperatureCoupled temperature
C++ Type:std::vector<VariableName>
Controllable:No
Description:Coupled temperature
use_transformationTrueWhether to employ updated Hill's tensor due to rigid body or large deformation kinematic rotations. If an initial rigid body rotation is provided by the user in increments of 90 degrees (e.g. 90, 180, 270), this option can be set to false, in which case the Hill's coefficients are extracted from the transformed Hill's tensor.
Default:True
C++ Type:bool
Controllable:No
Description:Whether to employ updated Hill's tensor due to rigid body or large deformation kinematic rotations. If an initial rigid body rotation is provided by the user in increments of 90 degrees (e.g. 90, 180, 270), this option can be set to false, in which case the Hill's coefficients are extracted from the transformed Hill's tensor.

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

internal_solve_full_iteration_historyFalseSet true to output full internal Newton iteration history at times determined by `internal_solve_output_on`. If false, only a summary is output.
Default:False
C++ Type:bool
Controllable:No
Description:Set true to output full internal Newton iteration history at times determined by `internal_solve_output_on`. If false, only a summary is output.
internal_solve_output_onon_errorWhen to output internal Newton solve information
Default:on_error
C++ Type:MooseEnum
Options:never, on_error, always
Controllable:No
Description:When to output internal Newton solve information

Debug 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

References

Calvin M Stewart, Ali P Gordon, Young Wha Ma, and Richard W Neu. An anisotropic tertiary creep damage constitutive model for anisotropic materials. International Journal of Pressure Vessels and Piping, 88(8-9):356–364, 2011.

@article{stewart2011anisotropic,
    author = "Stewart, Calvin M and Gordon, Ali P and Ma, Young Wha and Neu, Richard W",
    title = "An anisotropic tertiary creep damage constitutive model for anisotropic materials",
    journal = "International Journal of Pressure Vessels and Piping",
    volume = "88",
    number = "8-9",
    pages = "356--364",
    year = "2011",
    publisher = "Elsevier"
}

(moose/modules/tensor_mechanics/test/tests/ad_anisotropic_creep/ad_aniso_creep_y_3d.i)

[Mesh]
  [gen]
    type = GeneratedMeshGenerator
    dim = 3
    nx = 2
    ny = 10
    nz = 2

    xmin = 0.0
    ymin = 0.0
    zmin = 0.0

    xmax = 1.0
    ymax = 10.0
    zmax = 1.0
  []
  [corner_node]
    type = ExtraNodesetGenerator
    new_boundary = '100'
    nodes = '4 10'
    input = gen
  []
  [corner_node_2]
    type = ExtraNodesetGenerator
    new_boundary = '101'
    nodes = '1 67'
    input = corner_node
  []
[]

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

[AuxVariables]
  [hydrostatic_stress]
    order = CONSTANT
    family = MONOMIAL
  []
  [creep_strain_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [creep_strain_xy]
    order = CONSTANT
    family = MONOMIAL
  []
  [creep_strain_yy]
    order = CONSTANT
    family = MONOMIAL
  []
  [creep_strain_zz]
    order = CONSTANT
    family = MONOMIAL
  []
[]

[AuxKernels]
  [hydrostatic_stress]
    type = ADRankTwoScalarAux
    variable = hydrostatic_stress
    rank_two_tensor = stress
    scalar_type = Hydrostatic
  []
  [creep_strain_xx]
    type = ADRankTwoAux
    rank_two_tensor = creep_strain
    variable = creep_strain_xx
    index_i = 0
    index_j = 0
  []
  [creep_strain_xy]
    type = ADRankTwoAux
    rank_two_tensor = creep_strain
    variable = creep_strain_xy
    index_i = 0
    index_j = 1
  []
  [creep_strain_yy]
    type = ADRankTwoAux
    rank_two_tensor = creep_strain
    variable = creep_strain_yy
    index_i = 1
    index_j = 1
  []
  [creep_strain_zz]
    type = ADRankTwoAux
    rank_two_tensor = creep_strain
    variable = creep_strain_yy
    index_i = 1
    index_j = 1
  []
  [sigma_yy]
    type = ADRankTwoAux
    rank_two_tensor = stress
    variable = stress_yy
    index_i = 1
    index_j = 1
  []
[]

[Functions]
  [pull]
    type = PiecewiseLinear
    x = '0 1.0e-11 1.0'
    y = '0 -4e1 -4e1'
  []
[]

[Modules/TensorMechanics/Master]
  [all]
    strain = FINITE
    generate_output = 'elastic_strain_yy stress_yy'
    use_automatic_differentiation = true
    add_variables = true
  []
[]

[Materials]
  [elasticity_tensor]
    type = ADComputeIsotropicElasticityTensor
    youngs_modulus = 700
    poissons_ratio = 0.0
  []

  [elastic_strain]
    type = ADComputeMultipleInelasticStress
    inelastic_models = "trial_creep_two"
    max_iterations = 50
    absolute_tolerance = 1e-16
  []

  [hill_tensor]
    type = ADHillConstants
    # F G H L M N
    hill_constants = "0.5 0.25 0.3866 1.6413 1.6413 1.2731"
  []

  [trial_creep_two]
    type = ADHillCreepStressUpdate
    coefficient = 1e-16
    n_exponent = 9
    m_exponent = 0
    activation_energy = 0
    max_inelastic_increment = 0.00003
    absolute_tolerance = 1e-20
    relative_tolerance = 1e-20
    # Force it to not use integration error
    max_integration_error = 0.000001
  []
[]

[BCs]
  [no_disp_x]
    type = ADDirichletBC
    variable = disp_x
    boundary = 101
    value = 0.0
  []

  [no_disp_y]
    type = ADDirichletBC
    variable = disp_y
    boundary = bottom
    value = 0.0
  []

  [no_disp_z]
    type = ADDirichletBC
    variable = disp_z
    boundary = 100
    value = 0.0
  []

  [pressure]
    type = ADPressure
    boundary = top
    function = pull
    variable = disp_y
    component = 1
  []
[]

[Executioner]
  type = Transient

  solve_type = NEWTON
  petsc_options_iname = '-pc_type -pc_factor_mat_solver_package'
  petsc_options_value = 'lu     superlu_dist'

  nl_rel_tol = 1.0e-13
  nl_abs_tol = 1.0e-13
  l_max_its = 90
  num_steps = 10
  dt = 1.0e-4
  start_time = 0
  automatic_scaling = true
[]

[Postprocessors]
  [matl_ts_min]
    type = MaterialTimeStepPostprocessor
  []
  [max_disp_x]
    type = ElementExtremeValue
    variable = disp_x
  []
  [max_disp_y]
    type = ElementExtremeValue
    variable = disp_y
  []
  [max_hydro]
    type = ElementAverageValue
    variable = hydrostatic_stress
  []
  [dt]
    type = TimestepSize
  []
  [num_lin]
    type = NumLinearIterations
    outputs = console
  []
  [num_nonlin]
    type = NumNonlinearIterations
    outputs = console
  []
  [creep_strain_yy]
    type = ElementalVariableValue
    variable = creep_strain_yy
    execute_on = 'TIMESTEP_END'
    elementid = 39
  []
  [elastic_strain_yy]
    type = ElementalVariableValue
    variable = elastic_strain_yy
    execute_on = 'TIMESTEP_END'
    elementid = 39
  []
  [sigma_yy]
    type = ElementalVariableValue
    variable = stress_yy
    execute_on = 'TIMESTEP_END'
    elementid = 39
  []
[]

[Outputs]
  csv = true
  exodus = true
  perf_graph = true
[]