Hill Plasticity Stress Update

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

Description

This class computes Hill plasticity via a generalized radial return mapping algorithm Versino and Bennett (2018). It requires that the elastic behavior of the material is isotropic, whereas any departure from the yield function is anisotropic. The Hill yield function can be defined as: $(1)var element = document.getElementById("moose-equation-e6ee8b37-db34-4a6a-aab8-905074973e36");katex.render("f := \\frac{1}{2} \\boldsymbol{s}^{\\boldsymbol{T}} \\boldsymbol{A} \\boldsymbol{s} - {s_y}^2 \\left(\\alpha, \\dot{\\alpha}, T \\right) ", element, {displayMode:true,throwOnError:false});$ where $var element = document.getElementById("moose-equation-dab66c30-1d41-4ad0-be1e-a9c165e7a136");katex.render("\\boldsymbol{s}", element, {displayMode:false,throwOnError:false});$ is the deviatoric stress tensor in Voigt form, $var element = document.getElementById("moose-equation-3a7daee3-9027-4449-b859-19943480e082");katex.render("\\boldsymbol{A}", element, {displayMode:false,throwOnError:false});$ is the anisotropy (Hill) tensor, $var element = document.getElementById("moose-equation-872f8a3b-8e0b-41bf-9d2c-012d5fa9bfd6");katex.render("T", element, {displayMode:false,throwOnError:false});$ is the temperature and $var element = document.getElementById("moose-equation-30df7164-106f-48e5-a547-dcc094b34ec6");katex.render("\\alpha", element, {displayMode:false,throwOnError:false});$ is an internal parameter that can be used, for example, to prescribe strain hardening through a plasticity modulus. Hill's tensor is defined as a six by six matrix using the unitless constants $var element = document.getElementById("moose-equation-24f2a7aa-3f12-41d1-a9db-82c6e669f869");katex.render("F", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-cfedb8fe-9ba7-4732-b99f-d125c863d3b2");katex.render("G", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-7a99b3d9-f418-4661-a82f-1ab6df9f5330");katex.render("H", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-b5f0fb6d-802b-424c-ba8a-766633b72e36");katex.render("L", element, {displayMode:false,throwOnError:false});$ , $var element = document.getElementById("moose-equation-1cc4f4d4-8b3e-4bd9-a275-af81fa76104c");katex.render("M", element, {displayMode:false,throwOnError:false});$ and $var element = document.getElementById("moose-equation-43caa094-b6ca-4e83-ad87-790e3289a406");katex.render("N", element, {displayMode:false,throwOnError:false});$ as following:

$(2)var element = document.getElementById("moose-equation-ff829520-c6b6-474b-a589-6c0872e0cdd8");katex.render("\\boldsymbol{A} := \\begin{bmatrix} G+H & -H & -G & 0 & 0 & 0\\\\ -H & F+H & -F & 0 & 0 & 0\\\\ -G & -F & F+G & 0 & 0 & 0\\\\ 0 & 0 & 0 & 2N & 0 & 0\\\\ 0 & 0 & 0 & 0 & 2L & 0\\\\ 0 & 0 & 0 & 0 & 0 & 2M\\\\ \\end{bmatrix} ", element, {displayMode:true,throwOnError:false});$

The model currently uses power law hardening:

$(3)var element = document.getElementById("moose-equation-8b4bb590-4954-4052-a687-f695770c658d");katex.render("\\sigma_y = \\sigma_{yo} + K \\alpha^n ", element, {displayMode:true,throwOnError:false});$

where $var element = document.getElementById("moose-equation-d8eca4ab-6941-44b6-b5e9-723a32b1322e");katex.render("K", element, {displayMode:false,throwOnError:false});$ is the hardening constant and $var element = document.getElementById("moose-equation-90c6748e-e314-4f99-ac1c-53fc71de4e0d");katex.render("n", element, {displayMode:false,throwOnError:false});$ is the hardening exponent. The hardening exponent has a default value of 1.0 and this value can be modified by the user by setting the parameter "hardening_exponent". The "yield_stress" ( $var element = document.getElementById("moose-equation-4066a018-7865-4f9e-bdd5-24afbaef74df");katex.render("\\sigma_{yo}", element, {displayMode:false,throwOnError:false});$ ) and "hardening_constant" ( $var element = document.getElementById("moose-equation-8440edf2-27d7-4bd6-b37c-3160a7557ff1");katex.render("K", element, {displayMode:false,throwOnError:false});$ ) are the required parameters to be supplied by the user.

Verification

With $var element = document.getElementById("moose-equation-bd2e9315-0a40-46d0-9189-2d2eae4a7ae0");katex.render("f", element, {displayMode:false,throwOnError:false});$ being the yield condition, $var element = document.getElementById("moose-equation-6c152c1f-dd56-4079-8beb-3e82c3e29010");katex.render("\\boldsymbol{s}", element, {displayMode:false,throwOnError:false});$ the deviatoric stress and $var element = document.getElementById("moose-equation-e0a2db8b-1445-4e31-8686-c9ba14376008");katex.render("\\gamma", element, {displayMode:false,throwOnError:false});$ the plastic multiplier, the plastic strain rate is given as:

$(4)var element = document.getElementById("moose-equation-f1bec2bc-f50a-4efa-a2ad-64edca9d9f50");katex.render("\\dot{\\boldsymbol{\\epsilon}}^{\\boldsymbol{p}} = \\dot{\\gamma}\\frac{\\partial f}{\\partial \\boldsymbol{s}} ", element, {displayMode:true,throwOnError:false});$

Eq. (4) is a statement of normality condition, i.e., the associative flow rule. Using Eq. (1), the associative flow rule in Eq. (4) can be written as:

$(5)var element = document.getElementById("moose-equation-a497556e-4a56-4f20-a2b4-c54b4860f44d");katex.render("\\dot{\\boldsymbol{\\epsilon}}^{\\boldsymbol{p}} = \\dot{\\gamma} \\boldsymbol{A} \\boldsymbol{s} ", element, {displayMode:true,throwOnError:false});$

which can be written in incremental form as:

$(6)var element = document.getElementById("moose-equation-4f1996aa-f95b-4e4d-8f25-dab70dd059e9");katex.render("\\Delta\\boldsymbol{\\epsilon}^{\\boldsymbol{p}} = \\Delta\\gamma \\boldsymbol{A} \\boldsymbol{s} ", element, {displayMode:true,throwOnError:false});$

If $var element = document.getElementById("moose-equation-b646f0d7-f100-4826-af2a-894a5be178fd");katex.render("\\alpha", element, {displayMode:false,throwOnError:false});$ is the internal state variable associated with isotropic hardening, and $var element = document.getElementById("moose-equation-eff768fe-2d96-4edf-a5de-f521be1eb0c8");katex.render("\\beta", element, {displayMode:false,throwOnError:false});$ is the energy conjugate to the $var element = document.getElementById("moose-equation-bcfa7329-c760-4672-96d6-d56a449b7dd4");katex.render("\\dot{\\alpha}", element, {displayMode:false,throwOnError:false});$ , the $var element = document.getElementById("moose-equation-95bc89f7-3289-4e73-bc2f-dc0ea83d5375");katex.render("\\dot{\\alpha}", element, {displayMode:false,throwOnError:false});$ is written as:

$(7)var element = document.getElementById("moose-equation-c9431108-7c66-4a82-88b0-29b3386d4b98");katex.render("\\dot{\\alpha} = - \\dot{\\gamma}\\frac{\\partial f}{\\partial \\beta} ", element, {displayMode:true,throwOnError:false});$

The thermodynamic variable $var element = document.getElementById("moose-equation-07c3442e-c843-47cc-a6d5-1b9a5fad1458");katex.render("\\beta", element, {displayMode:false,throwOnError:false});$ is $var element = document.getElementById("moose-equation-d8f6b192-5b5e-4e44-bd96-23f9af41ec5b");katex.render("s_y", element, {displayMode:false,throwOnError:false});$ here (see Versino and Bennett (2018) for details). Equation Eq. (7) can be written in integrated incremental form as:

$(8)var element = document.getElementById("moose-equation-e9606e17-1d6f-412b-86c7-51492ade7c1e");katex.render("\\Delta\\alpha = 2 s_y \\Delta\\gamma ", element, {displayMode:true,throwOnError:false});$

Using Eq. (8) in Eq. (6), taking the partial derivative of $var element = document.getElementById("moose-equation-6834f643-a9c4-45ea-99c6-7525de1eef6e");katex.render("\\Delta\\boldsymbol{\\epsilon}^{\\boldsymbol{p}}", element, {displayMode:false,throwOnError:false});$ with respect to $var element = document.getElementById("moose-equation-4c5d23e8-2558-456b-b983-b17d9d9ba9ae");katex.render("\\boldsymbol{s}", element, {displayMode:false,throwOnError:false});$ , and applying chain rule, we obtain:

$(9)var element = document.getElementById("moose-equation-b1127023-fa97-415c-96a9-a21fab11467e");katex.render("\\frac{\\partial \\Delta\\boldsymbol{\\epsilon}^{\\boldsymbol{p}}}{\\partial \\boldsymbol{s}} = \\frac{\\partial \\Delta\\boldsymbol{\\epsilon}^{\\boldsymbol{p}}}{\\partial \\Delta\\alpha} \\frac{\\partial \\Delta\\alpha}{\\partial \\boldsymbol{s}} = \\frac{\\boldsymbol{A} \\boldsymbol{s}}{2s_y} \\frac{\\partial \\Delta\\alpha}{\\partial \\boldsymbol{s}} ", element, {displayMode:true,throwOnError:false});$

$(10)var element = document.getElementById("moose-equation-96627ef0-7b83-4097-871c-a610c526551a");katex.render("\\Rightarrow \\frac{\\partial \\boldsymbol{s}}{\\partial \\Delta\\boldsymbol{\\epsilon}^{\\boldsymbol{p}}} = \\frac{2s_y}{\\boldsymbol{A} \\boldsymbol{s}} \\frac{\\partial \\boldsymbol{s}}{\\partial \\Delta\\alpha} ", element, {displayMode:true,throwOnError:false});$

For the case where flow rule involves linear hardening with hardening constant $var element = document.getElementById("moose-equation-e7163c9b-eaee-4d35-a5ba-4e5f7c744084");katex.render("K", element, {displayMode:false,throwOnError:false});$ :

$(11)var element = document.getElementById("moose-equation-f0c36af6-23ad-44ef-b0c8-67035b1961e3");katex.render("\\frac{\\partial \\boldsymbol{s}}{\\partial \\Delta\\alpha} = K ", element, {displayMode:true,throwOnError:false});$

Substituting Eq. (11) in Eq. (10) we obtain:

$(12)var element = document.getElementById("moose-equation-788b5861-f85f-4b53-87e2-6e71dbc0dbca");katex.render("\\Rightarrow \\frac{\\partial \\boldsymbol{s}}{\\partial \\Delta\\boldsymbol{\\epsilon}^{\\boldsymbol{p}}} = \\frac{2s_y}{\\boldsymbol{A} \\boldsymbol{s}} K ", element, {displayMode:true,throwOnError:false});$

The left hand side of Eq. (12) gives the slope of the stress vs plastic strain curve. This equation can be written for the direct components of stress ( $var element = document.getElementById("moose-equation-c1cba17b-6434-4454-a8a1-7506592a90f1");katex.render("s_{ii}", element, {displayMode:false,throwOnError:false});$ ) as:

$(13)var element = document.getElementById("moose-equation-ce13e1c7-c815-49f3-9b6c-b2c0bd897dfa");katex.render("\\Rightarrow \\frac{\\partial s_{xx}}{\\partial \\Delta\\epsilon^p_{xx}} = \\frac{2s_y}{(G+H) s_{xx}} K ", element, {displayMode:true,throwOnError:false});$

For a uniaxial tensile test with monotonically increasing load, the stress always lies on the yield surface once the plastic deformation starts (for loading in x-direction $var element = document.getElementById("moose-equation-99b1518d-b4b4-4f10-8437-ad972e673efe");katex.render("s_{xx}", element, {displayMode:false,throwOnError:false});$ = $var element = document.getElementById("moose-equation-9c407e06-330f-45ed-bbd1-d861136599c9");katex.render("s_y", element, {displayMode:false,throwOnError:false});$ ) which simplifies Eq. (13) to:

$(14)var element = document.getElementById("moose-equation-978d7de9-ab65-4b66-916a-b3c00c5d4875");katex.render("\\Rightarrow \\frac{\\partial s_{xx}}{\\partial \\Delta\\epsilon^p_{xx}} = \\frac{2K}{(G+H)} ", element, {displayMode:true,throwOnError:false});$

Similarly, for uniaxial loading in y-direction we obtain:

$(15)var element = document.getElementById("moose-equation-288c1aa4-8530-4d91-94d0-351ac8a2ae9e");katex.render("\\Rightarrow \\frac{\\partial s_{yy}}{\\partial \\Delta\\epsilon^p_{yy}} = \\frac{2K}{(F+H)} ", element, {displayMode:true,throwOnError:false});$

These simplified equations (Eq. (14) & Eq. (15)) can be used in the verification tests for this material model.

warning

The combination of elastic isotropy and plastic anisotropy should be solved by the more efficient HillPlasticityStressUpdate class.

The effective plastic strain increment is obtained within the framework of a generalized (Hill plasticity) radial return mapping, see GeneralizedRadialReturnStressUpdate.

Example Input File Syntax

[trial_plasticity]
  type = ADHillPlasticityStressUpdate
  hardening_constant = 2000.0
  yield_stress = 0.001
  absolute_tolerance = 1e-14
  relative_tolerance = 1e-12
  base_name = trial_plasticity
  internal_solve_full_iteration_history = true
  max_inelastic_increment = 2.0e-6
  internal_solve_output_on = on_error
[]

Input Parameters

effective_inelastic_strain_nameeffective_plastic_strainName of the material property that stores the effective inelastic strain
Default:effective_plastic_strain
C++ Type:std::string
Controllable:No
Description:Name of the material property that stores the effective inelastic strain
hardening_constantHardening constant (H) for anisotropic plasticity
C++ Type:double
Controllable:No
Description:Hardening constant (H) for anisotropic plasticity
inelastic_strain_rate_nameplastic_strain_rateName of the material property that stores the inelastic strain rate
Default:plastic_strain_rate
C++ Type:std::string
Controllable:No
Description:Name of the material property that stores the inelastic strain rate
yield_stressYield stress (constant value) for anisotropic plasticity
C++ Type:double
Controllable:No
Description:Yield stress (constant value) for anisotropic plasticity

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.
hardening_exponent1Hardening exponent (n) for anisotropic plasticity
Default:1
C++ Type:double
Controllable:No
Description:Hardening exponent (n) for anisotropic plasticity
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
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

Daniele Versino and Kane C Bennett. Generalized radial-return mapping algorithm for anisotropic von mises plasticity framed in material eigenspace. International Journal for Numerical Methods in Engineering, 116(3):202–222, 2018.

@article{versino2018generalized,
    author = "Versino, Daniele and Bennett, Kane C",
    title = "Generalized radial-return mapping algorithm for anisotropic von Mises plasticity framed in material eigenspace",
    journal = "International Journal for Numerical Methods in Engineering",
    volume = "116",
    number = "3",
    pages = "202--222",
    year = "2018",
    publisher = "Wiley Online Library"
}

(moose/modules/tensor_mechanics/test/tests/anisotropic_plasticity/ad_aniso_plasticity_y.i)

[Mesh]
  [gen]
    type = GeneratedMeshGenerator
    dim = 3

    # Original verification nx = 2, ny = 10, nz = 2
    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
  []
  [plastic_strain_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [plastic_strain_xy]
    order = CONSTANT
    family = MONOMIAL
  []
  [plastic_strain_yy]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_yy]
    order = CONSTANT
    family = MONOMIAL
  []
  [elastic_strain_yy]
    order = CONSTANT
    family = MONOMIAL
  []
[]

[AuxKernels]
  [hydrostatic_stress]
    type = ADRankTwoScalarAux
    variable = hydrostatic_stress
    rank_two_tensor = stress
    scalar_type = Hydrostatic
  []
  [plasticity_strain_xx]
    type = ADRankTwoAux
    rank_two_tensor = trial_plasticity_plastic_strain
    variable = plastic_strain_xx
    index_i = 0
    index_j = 0
  []
  [plasticity_strain_xy]
    type = ADRankTwoAux
    rank_two_tensor = trial_plasticity_plastic_strain
    variable = plastic_strain_xy
    index_i = 0
    index_j = 1
  []
  [plasticity_strain_yy]
    type = ADRankTwoAux
    rank_two_tensor = trial_plasticity_plastic_strain
    variable = plastic_strain_yy
    index_i = 1
    index_j = 1
  []
  [elastic_strain_yy]
    type = ADRankTwoAux
    rank_two_tensor = elastic_strain
    variable = elastic_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 1e1 1e8'
    y = '0 -4e2 -4e2'
  []
[]

[Modules/TensorMechanics/Master]
  [all]
    strain = FINITE
    use_automatic_differentiation = true
    add_variables = true
  []
[]

[Materials]

  [elasticity_tensor]
    type = ADComputeIsotropicElasticityTensor
    youngs_modulus = 70000
    poissons_ratio = 0.25
  []

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

  [hill_tensor]
    type = ADHillConstants
    # F G H L M N
    hill_constants = "0.5829856 0.364424 0.6342174 2.0691375 2.3492325 1.814589"
    base_name = trial_plasticity
  []

  [trial_plasticity]
    type = ADHillPlasticityStressUpdate
    hardening_constant = 2000.0
    yield_stress = 0.001
    absolute_tolerance = 1e-14
    relative_tolerance = 1e-12
    base_name = trial_plasticity
    internal_solve_full_iteration_history = true
    max_inelastic_increment = 2.0e-6
    internal_solve_output_on = on_error
  []
[]

[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]
    [Side1]
      boundary = top
      function = pull
    []
  []
[]

[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 = 1e-11
  nl_abs_tol = 1.0e-14
  l_max_its = 90
  num_steps = 25
  [TimeStepper]
    type = IterationAdaptiveDT
    optimal_iterations = 30
    iteration_window = 9
    growth_factor = 1.05
    cutback_factor = 0.5
    timestep_limiting_postprocessor = matl_ts_min
    dt = 1e-5
    time_t = '0 3.2e-5 10'
    time_dt = '1e-5 1.0e-7 1.0e-7'
  []
  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
  []
  [plasticity_strain_yy]
    type = ElementalVariableValue
    variable = plastic_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
  perf_graph = true
[]