- activation_energyActivation energy
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Activation energy
- coefficientLeading coefficient in power-law equation
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Leading coefficient in power-law equation
- n_exponentExponent on effective stress in power-law equation
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Exponent on effective stress in power-law equation
Power Law Creep Stress Update
This class uses the stress update material in a radial return isotropic power law creep model. This class can be used in conjunction with other creep and plasticity materials for more complex simulations.
Description
In this numerical approach, a trial stress is calculated at the start of each simulation time increment; the trial stress calculation assumed all of the new strain increment is elastic strain:
The algorithms checks to see if the trial stress state is outside of the yield surface, as shown in the figure to the right. If the stress state is outside of the yield surface, the algorithm recomputes the scalar effective inelastic strain required to return the stress state to the yield surface. This approach is given the name Radial Return because the yield surface used is the von Mises yield surface: in the deviatoric stress space, this yield surface has the shape of a circle, and the scalar inelastic strain is assumed to always be directed at the circle center.
Recompute Iterations on the Effective Plastic Strain Increment
The recompute radial return materials each individually calculate, using the Newton Method, the amount of effective inelastic strain required to return the stress state to the yield surface.
where the change in the iterative effective inelastic strain is defined as the yield surface over the derivative of the yield surface with respect to the inelastic strain increment.
The increment of inelastic strain is computed from the creep rate in this class.
(1)
where is the scalar von Mises trial stress, is the isotropic shear modulus, is the activation energy, is the universal gas constant, is the temperature, and are the current and initial times, respectively, and and are exponent values.
This class calculates an effective trial stress, an effective creep strain rate increment and the derivative of the creep strain rate, and an effective scalar inelastic strain increment; these values are passed to the ADRadialReturnStressUpdate to compute the radial return stress increment. This isotropic plasticity class also computes the plastic strain as a stateful material property.
This class is based on the implicit integration algorithm in Dunne and Petrinic (2005) pg. 146 - 149.
PowerLawCreepStressUpdate must be run in conjunction with an inelastic strain return mapping stress calculator such as ADComputeMultipleInelasticStress
Input Parameters
- absolute_tolerance1e-11Absolute convergence tolerance for Newton iteration
Default:1e-11
C++ Type:double
Unit:(no unit assumed)
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
Unit:(no unit assumed)
Controllable:No
Description:Factor applied to relative and absolute tolerance for acceptable convergence if iterations are no longer making progress
- adaptive_substeppingFalseUse adaptive substepping, where the number of substeps is successively doubled until the return mapping model successfully converges or the maximum number of substeps is reached.
Default:False
C++ Type:bool
Controllable:No
Description:Use adaptive substepping, where the number of substeps is successively doubled until the return mapping model successfully converges or the maximum number of substeps is reached.
- automatic_differentiation_return_mappingFalseWhether to use automatic differentiation to compute the derivative.
Default:False
C++ Type:bool
Controllable:No
Description:Whether to use automatic differentiation to compute the derivative.
- 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
Unit:(no unit assumed)
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
Unit:(no unit assumed)
Controllable:No
Description:Universal gas constant
- m_exponent0Exponent on time in power-law equation
Default:0
C++ Type:double
Unit:(no unit assumed)
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
Unit:(no unit assumed)
Controllable:No
Description:The maximum inelastic strain increment allowed in a time step
- maximum_number_substeps25The maximum number of substeps allowed before cutting the time step.
Default:25
C++ Type:unsigned int
Controllable:No
Description:The maximum number of substeps allowed before cutting the time step.
- relative_tolerance1e-08Relative convergence tolerance for Newton iteration
Default:1e-08
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Relative convergence tolerance for Newton iteration
- start_time0Start time (if not zero)
Default:0
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Start time (if not zero)
- temperatureCoupled temperature
C++ Type:std::vector<VariableName>
Unit:(no unit assumed)
Controllable:No
Description:Coupled temperature
- use_substep_integration_errorFalseIf true, it establishes a substep size that will yield, at most,the creep numerical integration error given by substep_strain_tolerance.
Default:False
C++ Type:bool
Controllable:No
Description:If true, it establishes a substep size that will yield, at most,the creep numerical integration error given by substep_strain_tolerance.
- use_substeppingNONEWhether and how to use substepping
Default:NONE
C++ Type:MooseEnum
Options:NONE, ERROR_BASED, INCREMENT_BASED
Controllable:No
Description:Whether and how to use substepping
Optional Parameters
- apply_strainTrueFlag to apply strain. Used for testing.
Default:True
C++ Type:bool
Controllable:No
Description:Flag to apply strain. Used for testing.
- 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.
- 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
- 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
- search_methodnearest_node_connected_sidesChoice of search algorithm. All options begin by finding the nearest node in the primary boundary to a query point in the secondary boundary. In the default nearest_node_connected_sides algorithm, primary boundary elements are searched iff that nearest node is one of their nodes. This is fast to determine via a pregenerated node-to-elem map and is robust on conforming meshes. In the optional all_proximate_sides algorithm, primary boundary elements are searched iff they touch that nearest node, even if they are not topologically connected to it. This is more CPU-intensive but is necessary for robustness on any boundary surfaces which has disconnections (such as Flex IGA meshes) or non-conformity (such as hanging nodes in adaptively h-refined meshes).
Default:nearest_node_connected_sides
C++ Type:MooseEnum
Options:nearest_node_connected_sides, all_proximate_sides
Controllable:No
Description:Choice of search algorithm. All options begin by finding the nearest node in the primary boundary to a query point in the secondary boundary. In the default nearest_node_connected_sides algorithm, primary boundary elements are searched iff that nearest node is one of their nodes. This is fast to determine via a pregenerated node-to-elem map and is robust on conforming meshes. In the optional all_proximate_sides algorithm, primary boundary elements are searched iff they touch that nearest node, even if they are not topologically connected to it. This is more CPU-intensive but is necessary for robustness on any boundary surfaces which has disconnections (such as Flex IGA meshes) or non-conformity (such as hanging nodes in adaptively h-refined meshes).
- 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
- substep_strain_tolerance0.1Maximum ratio of the initial elastic strain increment at start of the return mapping solve to the maximum inelastic strain allowable in a single substep. Reduce this value to increase the number of substeps
Default:0.1
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Maximum ratio of the initial elastic strain increment at start of the return mapping solve to the maximum inelastic strain allowable in a single substep. Reduce this value to increase the number of substeps
- 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
- 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
Unit:(no unit assumed)
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.
- 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.
Material Property Retrieval Parameters
Input Files
- (modules/solid_mechanics/test/tests/strain_energy_density/rate_model.i)
- (modules/solid_mechanics/test/tests/ad_viscoplasticity_stress_update/creep.i)
- (modules/solid_mechanics/test/tests/j_integral_vtest/c_int_surfbreak_ellip_crack_sym_mm_ad.i)
- (modules/solid_mechanics/test/tests/combined_creep_plasticity/combined_creep_plasticity.i)
- (modules/solid_mechanics/test/tests/power_law_creep/smallstrain.i)
- (modules/solid_mechanics/test/tests/power_law_creep/ad_restart2.i)
- (modules/solid_mechanics/test/tests/power_law_creep/ad_power_law_creep.i)
- (modules/solid_mechanics/test/tests/rom_stress_update/REG_finite_strain_power_law_creep.i)
- (modules/solid_mechanics/test/tests/recompute_radial_return/cp_affine_plasticity.i)
- (modules/solid_mechanics/test/tests/combined_creep_plasticity/combined_creep_plasticity_start_time.i)
- (modules/solid_mechanics/test/tests/substepping/power_law_creep.i)
- (modules/solid_mechanics/test/tests/rom_stress_update/AD_finite_strain_power_law_creep.i)
- (modules/solid_mechanics/test/tests/power_law_creep/ad_smallstrain.i)
- (modules/solid_mechanics/test/tests/combined_creep_plasticity/creepWithPlasticity.i)
- (modules/solid_mechanics/test/tests/combined_creep_plasticity/combined_stress_prescribed.i)
- (modules/solid_mechanics/test/tests/scalar_material_damage/ad_scalar_material_damage_creep_power.i)
- (modules/solid_mechanics/test/tests/domain_integral_thermal/interaction_integral_2d_c.i)
- (modules/solid_mechanics/test/tests/domain_integral_thermal/c_integral_2d.i)
- (modules/solid_mechanics/test/tests/strain_energy_density/nonAD_rate_model_weak_plane.i)
- (modules/solid_mechanics/test/tests/multi_power_law/power_law_creep.i)
- (modules/solid_mechanics/test/tests/power_law_creep/ad_restart1.i)
- (modules/solid_mechanics/test/tests/power_law_creep/power_law_creep.i)
- (modules/solid_mechanics/test/tests/combined_creep_plasticity/combined_stress_relaxation.i)
- (modules/combined/test/tests/inelastic_strain/creep/creep_nl1.i)
- (modules/solid_mechanics/test/tests/creep_tangent_operator/creep.i)
- (modules/solid_mechanics/test/tests/j_integral_vtest/c_int_surfbreak_ellip_crack_sym_mm.i)
- (modules/solid_mechanics/test/tests/strain_energy_density/ad_rate_model_weak_plane.i)
- (modules/solid_mechanics/test/tests/substepping/ad_power_law_creep.i)
- (modules/solid_mechanics/test/tests/power_law_creep/restart2.i)
- (modules/solid_mechanics/test/tests/material_limit_time_step/creep/nafems_test5a_lim.i)
- (modules/solid_mechanics/test/tests/ad_anisotropic_creep/ad_aniso_iso_creep_x_3d.i)
- (modules/solid_mechanics/test/tests/power_law_creep/cp_power_law_creep.i)
- (modules/solid_mechanics/test/tests/ad_plastic/power_law_creep.i)
- (modules/solid_mechanics/test/tests/ad_anisotropic_creep/aniso_iso_creep_x_3d.i)
- (modules/solid_mechanics/test/tests/ad_anisotropic_creep/anis_mech_hill_tensor_creep.i)
- (modules/solid_mechanics/test/tests/power_law_creep/restart1.i)
- (modules/solid_mechanics/test/tests/ad_return_mapping/ad_return_mapping_derivative.i)
- (modules/solid_mechanics/test/tests/strain_energy_density/rate_model_small.i)
- (modules/contact/test/tests/mortar_dynamics/block-dynamics-friction-creep.i)
- (modules/solid_mechanics/test/tests/scalar_material_damage/scalar_material_damage_creep_power.i)
References
- Fionn Dunne and Nik Petrinic.
Introduction to Computational Plasticity.
Oxford University Press on Demand, 2005.[BibTeX]
@book{dunne2005introduction, author = "Dunne, Fionn and Petrinic, Nik", title = "Introduction to Computational Plasticity", year = "2005", publisher = "Oxford University Press on Demand" }
(modules/solid_mechanics/test/tests/strain_energy_density/rate_model.i)
# Single element test to check the strain energy density calculation
[GlobalParams]
displacements = 'disp_x disp_y'
volumetric_locking_correction = true
[]
[Mesh]
type = GeneratedMesh
dim = 2
nx = 1
ny = 1
xmin = 0
xmax = 1
ymin = 0
ymax = 2
[]
[AuxVariables]
[./SERD]
order = CONSTANT
family = MONOMIAL
[../]
[]
[Functions]
[./rampConstantUp]
type = PiecewiseLinear
x = '0. 1.'
y = '0. 1.'
scale_factor = -100
[../]
[]
[Physics/SolidMechanics/QuasiStatic]
[./master]
strain = FINITE
add_variables = true
incremental = true
generate_output = 'stress_xx stress_yy stress_zz vonmises_stress strain_xx strain_yy strain_zz'
planar_formulation = PLANE_STRAIN
[../]
[]
[AuxKernels]
[./SERD]
type = MaterialRealAux
variable = SERD
property = strain_energy_rate_density
execute_on = timestep_end
[../]
[]
[BCs]
[./no_x]
type = DirichletBC
variable = disp_x
boundary = 'left'
value = 0.0
[../]
[./no_y]
type = DirichletBC
variable = disp_y
boundary = 'bottom'
value = 0.0
[../]
[./Pressure]
[./top]
boundary = 'top'
function = rampConstantUp
[../]
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 206800
poissons_ratio = 0.0
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'powerlawcrp'
[../]
[./powerlawcrp]
type = PowerLawCreepStressUpdate
coefficient = 3.125e-21 # 7.04e-17 #
n_exponent = 4.0
m_exponent = 0.0
activation_energy = 0.0
# max_inelastic_increment = 0.01
[../]
[./strain_energy_rate_density]
type = StrainEnergyRateDensity
inelastic_models = 'powerlawcrp'
[../]
[]
[Executioner]
type = Transient
petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
petsc_options_value = '201 hypre boomeramg 4'
line_search = 'none'
l_max_its = 50
nl_max_its = 20
nl_abs_tol = 3e-7
nl_rel_tol = 1e-12
l_tol = 1e-2
start_time = 0.0
dt = 1
end_time = 1
num_steps = 1
[]
[Postprocessors]
[./epxx]
type = ElementalVariableValue
variable = strain_xx
elementid = 0
[../]
[./epyy]
type = ElementalVariableValue
variable = strain_yy
elementid = 0
[../]
[./epzz]
type = ElementalVariableValue
variable = strain_zz
elementid = 0
[../]
[./sigxx]
type = ElementAverageValue
variable = stress_xx
[../]
[./sigyy]
type = ElementAverageValue
variable = stress_yy
[../]
[./sigzz]
type = ElementAverageValue
variable = stress_zz
[../]
[./SERD]
type = ElementAverageValue
variable = SERD
[../]
[]
[Outputs]
csv = true
[]
(modules/solid_mechanics/test/tests/ad_viscoplasticity_stress_update/creep.i)
[GlobalParams]
displacements = 'disp_x disp_y'
[]
[Mesh]
type = GeneratedMesh
dim = 2
nx = 2
ny = 2
xmax = 0.002
ymax = 0.002
[]
[Physics/SolidMechanics/QuasiStatic/All]
strain = FINITE
add_variables = true
base_name = 'total'
generate_output = 'strain_xx strain_yy strain_xy hydrostatic_stress vonmises_stress'
use_automatic_differentiation = true
[]
[Functions]
[./pull]
type = PiecewiseLinear
x = '0 0.1'
y = '0 1e-5'
[../]
[]
[Materials]
active='elasticity_tensor porous_stress porosity creep'
[./elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 1e10
poissons_ratio = 0.3
base_name = 'total'
[../]
[./porous_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = creep
outputs = all
base_name = 'total'
[../]
[./regular_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = creep
outputs = all
base_name = 'total'
[../]
[./porosity]
type = ADGenericConstantMaterial
prop_names = porosity
prop_values = 0.1
outputs = all
[../]
[./creep]
type = ADPowerLawCreepStressUpdate
activation_energy = 4e4
temperature = 1200
coefficient = 1e-18
gas_constant = 1.987
n_exponent = 3
base_name = 'creep'
outputs = all
[../]
[]
[BCs]
[./no_disp_x]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[../]
[./no_disp_y]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[../]
[./pull_disp_y]
type = ADFunctionDirichletBC
variable = disp_y
boundary = top
function = pull
[../]
[]
[Executioner]
type = Transient
solve_type = NEWTON
dt = 0.01
end_time = 0.12
[]
[Postprocessors]
[./disp_x]
type = SideAverageValue
variable = disp_x
boundary = right
[../]
[./disp_y]
type = SideAverageValue
variable = disp_y
boundary = top
[../]
[./avg_hydro]
type = ElementAverageValue
variable = total_hydrostatic_stress
[../]
[./avg_vonmises]
type = ElementAverageValue
variable = total_vonmises_stress
[../]
[./dt]
type = TimestepSize
[../]
[./num_lin]
type = NumLinearIterations
outputs = console
[../]
[./num_nonlin]
type = NumNonlinearIterations
outputs = console
[../]
[./eff_creep_strain]
type = ElementAverageValue
variable = creep_effective_creep_strain
[../]
[./porosity]
type = ElementAverageValue
variable = porosity
[../]
[]
[Outputs]
csv = true
[]
(modules/solid_mechanics/test/tests/j_integral_vtest/c_int_surfbreak_ellip_crack_sym_mm_ad.i)
[GlobalParams]
order = FIRST
family = LAGRANGE
displacements = 'disp_x disp_y disp_z'
volumetric_locking_correction = true
[]
[Mesh]
file = c_integral_coarse.e
partitioner = centroid
centroid_partitioner_direction = z
[]
[AuxVariables]
[SED]
order = CONSTANT
family = MONOMIAL
[]
[resid_z]
[]
[]
[Functions]
[rampConstantUp]
type = PiecewiseLinear
x = '0. 0.1 100.0'
y = '0. 1 1'
scale_factor = -68.95 #MPa
[]
[dts]
type = PiecewiseLinear
x = '0 1'
y = '1 400000'
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[master]
strain = FINITE
add_variables = true
incremental = true
generate_output = 'stress_xx stress_yy stress_zz vonmises_stress'
use_automatic_differentiation = true
[]
[]
[AuxKernels]
[SED]
type = MaterialRealAux
variable = SED
property = strain_energy_density
execute_on = timestep_end
[]
[]
[BCs]
[crack_y]
type = ADDirichletBC
variable = disp_z
boundary = 6
value = 0.0
[]
[no_y]
type = ADDirichletBC
variable = disp_y
boundary = 12
value = 0.0
[]
[no_x]
type = ADDirichletBC
variable = disp_x
boundary = 1
value = 0.0
[]
[Pressure]
[Side1]
boundary = 5
function = rampConstantUp
[] # BCs
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 206800
poissons_ratio = 0.0
[]
[radial_return_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'powerlawcrp'
[]
[powerlawcrp]
type = ADPowerLawCreepStressUpdate
coefficient = 3.125e-21 # 7.04e-17 #
n_exponent = 4.0
m_exponent = 0.0
activation_energy = 0.0
# max_inelastic_increment = 0.01
[]
[]
[DomainIntegral]
integrals = CIntegral
boundary = 1001
crack_direction_method = CurvedCrackFront
crack_end_direction_method = CrackDirectionVector
crack_direction_vector_end_1 = '0.0 1.0 0.0'
crack_direction_vector_end_2 = '1.0 0.0 0.0'
radius_inner = '12.5 25.0 37.5'
radius_outer = '25.0 37.5 50.0'
intersecting_boundary = '1 2'
symmetry_plane = 2
incremental = true
inelastic_models = 'powerlawcrp'
use_automatic_differentiation = true
[]
[Executioner]
type = Transient
solve_type = 'NEWTON'
petsc_options = '-snes_converged_reason -ksp_converged_reason -pc_svd_monitor '
'-snes_linesearch_monitor -snes_ksp_ew'
petsc_options_iname = '-pc_type -pc_factor_shift_type'
petsc_options_value = 'lu NONZERO'
nl_max_its = 20
nl_abs_tol = 1e-3
nl_rel_tol = 1e-11
start_time = 0.0
end_time = 401
[TimeStepper]
type = FunctionDT
function = dts
min_dt = 1.0
[]
[]
[Postprocessors]
[_dt]
type = TimestepSize
[]
[nl_its]
type = NumNonlinearIterations
[]
[lin_its]
type = NumLinearIterations
[]
[react_z]
type = NodalSum
variable = resid_z
boundary = 5
[]
[]
[Outputs]
execute_on = 'timestep_end'
csv = true
[]
(modules/solid_mechanics/test/tests/combined_creep_plasticity/combined_creep_plasticity.i)
#
# This test is Example 2 from "A Consistent Formulation for the Integration
# of Combined Plasticity and Creep" by P. Duxbury, et al., Int J Numerical
# Methods in Engineering, Vol. 37, pp. 1277-1295, 1994.
#
# The problem is a one-dimensional bar which is loaded from yield to a value of twice
# the initial yield stress and then unloaded to return to the original stress. The
# bar must harden to the required yield stress during the load ramp, with no
# further yielding during unloading. The initial yield stress (sigma_0) is prescribed
# as 20 with a plastic strain hardening of 100. The mesh is a 1x1x1 cube with symmetry
# boundary conditions on three planes to provide a uniaxial stress field.
#
# In the PowerLawCreep model, the creep strain rate is defined by:
#
# edot = A(sigma)**n * exp(-Q/(RT)) * t**m
#
# The creep law specified in the paper, however, defines the creep strain rate as:
#
# edot = Ao * mo * (sigma)**n * t**(mo-1)
# with the creep parameters given by
# Ao = 1e-7
# mo = 0.5
# n = 5
#
# thus, input parameters for the test were specified as:
# A = Ao * mo = 1e-7 * 0.5 = 0.5e-7
# m = mo-1 = -0.5
# n = 5
# Q = 0
#
# The variation of load P with time is:
# P = 20 + 20t 0 < t < 1
# P = 40 - 40(t-1) 1 < t 1.5
#
# The analytic solution for total strain during the loading period 0 < t < 1 is:
#
# e_tot = (sigma_0 + 20*t)/E + 0.2*t + A * t**0.5 * sigma_0**n * [ 1 + (5/3)*t +
# + 2*t**2 + (10/7)*t**3 + (5/9)**t**4 + (1/11)*t**5 ]
#
# and during the unloading period 1 < t < 1.5:
#
# e_tot = (sigma_1 - 40*(t-1))/E + 0.2 + (4672/693) * A * sigma_0**n +
# A * sigma_0**n * [ t**0.5 * ( 32 - (80/3)*t + 16*t**2 - (40/7)*t**3
# + (10/9)*t**4 - (1/11)*t**5 ) - (11531/693) ]
#
# where sigma_1 is the stress at time t = 1.
#
# Assuming a Young's modulus (E) of 1000 and using the parameters defined above:
#
# e_tot(1) = 2.39734
# e_tot(1.5) = 3.16813
#
#
# The numerically computed solution is:
#
# e_tot(1) = 2.39718 (~0.006% error)
# e_tot(1.5) = 3.15555 (~0.40% error)
#
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Physics/SolidMechanics/QuasiStatic]
[./all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy elastic_strain_yy creep_strain_yy plastic_strain_yy'
[../]
[]
[Functions]
[./top_pull]
type = PiecewiseLinear
x = ' 0 1 1.5'
y = '-20 -40 -20'
[../]
[./dts]
type = PiecewiseLinear
x = '0 0.5 1.0 1.5'
y = '0.015 0.015 0.005 0.005'
[../]
[]
[BCs]
[./u_top_pull]
type = Pressure
variable = disp_y
boundary = top
factor = 1
function = top_pull
[../]
[./u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[../]
[./u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[../]
[./u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
block = 0
youngs_modulus = 1e3
poissons_ratio = 0.3
[../]
[./creep_plas]
type = ComputeMultipleInelasticStress
block = 0
tangent_operator = elastic
inelastic_models = 'creep plas'
max_iterations = 50
absolute_tolerance = 1e-05
combined_inelastic_strain_weights = '0.0 1.0'
[../]
[./creep]
type = PowerLawCreepStressUpdate
block = 0
coefficient = 0.5e-7
n_exponent = 5
m_exponent = -0.5
activation_energy = 0
[../]
[./plas]
type = IsotropicPlasticityStressUpdate
block = 0
hardening_constant = 100
yield_stress = 20
[../]
[]
[Executioner]
type = Transient
#Preconditioned JFNK (default)
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 6
nl_rel_tol = 1e-6
nl_abs_tol = 1e-10
l_tol = 1e-5
start_time = 0.0
end_time = 1.5
[./TimeStepper]
type = FunctionDT
function = dts
[../]
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/power_law_creep/smallstrain.i)
# 1x1x1 unit cube with uniform pressure on top face for the case of small strain.
# This test does not have a solid mechanics analog because there is not an equvialent
# small strain with rotations strain calculator material in solid mechanics
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Variables]
[temp]
order = FIRST
family = LAGRANGE
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = SMALL
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = '0 1'
y = '1 1'
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = Pressure
variable = disp_y
boundary = top
factor = -10.0e6
function = top_pull
[]
[u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
tangent_operator = elastic
[]
[power_law_creep]
type = PowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp_ew'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.0
end_time = 1.0
num_steps = 10
dt = 0.1
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/power_law_creep/ad_restart2.i)
# 1x1x1 unit cube with uniform pressure on top face
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Variables]
[temp]
order = FIRST
family = LAGRANGE
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
use_automatic_differentiation = true
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = '0 1'
y = '1 1'
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = ADPressure
variable = disp_y
boundary = top
factor = -10.0e6
function = top_pull
[]
[u_bottom_fix]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = ADDirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
constant_on = SUBDOMAIN
[]
[radial_return_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
[]
[power_law_creep]
type = ADPowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.6
end_time = 1.0
num_steps = 12
dt = 0.1
[]
[Outputs]
exodus = true
[]
[Problem]
restart_file_base = ad_restart1_out_cp/0006
# temp has an initial condition despite the restart
allow_initial_conditions_with_restart = true
[]
(modules/solid_mechanics/test/tests/power_law_creep/ad_power_law_creep.i)
# 1x1x1 unit cube with uniform pressure on top face
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
[]
[Variables]
[temp]
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
use_automatic_differentiation = true
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = ADPressure
variable = disp_y
boundary = top
factor = -10.0e6
[]
[u_bottom_fix]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = ADDirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
constant_on = SUBDOMAIN
[]
[radial_return_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
[]
[power_law_creep]
type = ADPowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Preconditioning]
[smp]
type = SMP
full = true
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.0
end_time = 1.0
num_steps = 10
dt = 0.1
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/rom_stress_update/REG_finite_strain_power_law_creep.i)
[GlobalParams]
displacements = 'disp_r disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 2
xmin = 1
xmax = 2
nx = 50
ny = 50
coord_type = RZ
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
eigenstrain_names = 'thermal'
use_automatic_differentiation = false
[]
[]
[AuxVariables]
[temp]
initial_condition = 1000.0
[]
[]
[AuxKernels]
[cooling]
type = FunctionAux
variable = temp
function = '1000-10*t*x'
[]
[]
[BCs]
[top_pull]
type = FunctionNeumannBC
variable = disp_z
boundary = top
function = '1e7*t'
use_displaced_mesh = true
[]
[bottom_fix]
type = DirichletBC
variable = disp_z
boundary = bottom
value = 0.0
[]
[left_fix]
type = DirichletBC
variable = disp_r
boundary = left
value = 0.0
[]
[]
[Materials]
[eigenstrain]
type = ComputeThermalExpansionEigenstrain
eigenstrain_name = 'thermal'
stress_free_temperature = 1000
thermal_expansion_coeff = 1e-4
temperature = temp
[]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'creep'
[]
[creep]
type = PowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Postprocessors]
[nl_its]
type = NumNonlinearIterations
[]
[total_nl_its]
type = CumulativeValuePostprocessor
postprocessor = nl_its
[]
[]
[Executioner]
type = Transient
solve_type = 'NEWTON'
petsc_options_iname = '-pc_type'
petsc_options_value = 'lu'
line_search = 'none'
end_time = 10
dt = 1
automatic_scaling = true
[]
[Outputs]
print_linear_converged_reason = false
print_nonlinear_converged_reason = false
print_linear_residuals = false
perf_graph = true
[]
(modules/solid_mechanics/test/tests/recompute_radial_return/cp_affine_plasticity.i)
# Affine Plasticity Test for Transient Stress Eigenvalues with Stationary Eigenvectors
# This test is taken from K. Jamojjala, R. Brannon, A. Sadeghirad, J. Guilkey,
# "Verification tests in solid mechanics," Engineering with Computers, Vol 31.,
# p. 193-213.
# The test involves applying particular strains and expecting particular stresses.
# The material properties are:
# Yield in shear 165 MPa
# Shear modulus 79 GPa
# Poisson's ratio 1/3
# The strains are:
# Time e11 e22 e33
# 0 0 0 0
# 1 -0.003 -0.003 0.006
# 2 -0.0103923 0 0.0103923
# The expected stresses are:
# sigma11:
# -474*t 0 < t <= 0.201
# -95.26 0.201 < t <= 1
# (189.4+0.1704*sqrt(a)-0.003242*a)
# --------------------------------- 1 < t <= 2
# 1+0.00001712*a
# -189.4 t > 2 (paper erroneously gives a positive value)
#
# sigma22:
# -474*t 0 < t <= 0.201
# -95.26 0.201 < t <= 1
# -(76.87+1.443*sqrt(a)-0.001316*a)
# --------------------------------- 1 < t <= 2 (paper gives opposite sign)
# 1+0.00001712*a
# 76.87 t > 2
#
# sigma33:
# 948*t 0 < t <= 0.201
# 190.5 0.201 < t <= 1
# -(112.5-1.272*sqrt(a)-0.001926*a)
# --------------------------------- 1 < t <= 2 (paper has two sign errors here)
# 1+0.00001712*a
# 112.5 t > 2
#
# where a = exp(12.33*t).
#
# Note: If planning to run this case with strain type ComputeFiniteStrain, the
# displacement function must be adjusted. Instead of
# strain = (l - l0)/l0 = (u+l0 - l0)/l0 = u/l0
# with l0=1.0, we would have
# strain = log(l/l0) = log((u+l0)/l0)
# with l0=1.0. So, for strain = -0.003,
# -0.003 = log((u+l0)/l0) ->
# u = exp(-0.003)*l0 - l0 = -0.0029955044966269995.
#
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
block = '0'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
# This test uses ElementalVariableValue postprocessors on specific
# elements, so element numbering needs to stay unchanged
allow_renumbering = false
[]
[Functions]
[disp_x]
type = PiecewiseLinear
x = '0. 1. 2.'
y = '0. -0.003 -0.0103923'
[]
[disp_y]
type = PiecewiseLinear
x = '0. 1. 2.'
y = '0. -0.003 0.'
[]
[disp_z]
type = PiecewiseLinear
x = '0. 1. 2.'
y = '0. 0.006 0.0103923'
[]
[stress_xx]
type = ParsedFunction
# The paper gives 0.201 as the time at initial yield, but 0.20097635952803425 is the exact value.
# The paper gives -95.26 MPa as the stress at yield, but -95.26279441628823 is the exact value.
# The paper gives 12.33 as the factor in the exponential, but 12.332921390339125 is the exact value.
# 189.409039923814000, 0.170423791206825, -0.003242011311945, 1.711645501845780E-05 - exact values
symbol_names = 'timeAtYield stressAtYield expFac a b c d'
symbol_values = '0.20097635952803425 -95.26279441628823 12.332921390339125 189.409039923814000 0.170423791206825 -0.003242011311945 1.711645501845780E-05'
value = '1e6*
if(t<=timeAtYield, -474*t,
if(t<=1, stressAtYield,
(a+b*sqrt(exp(expFac*t))+c*exp(expFac*t))/(1.0+d*exp(expFac*t))))' # tends to -a
[]
[stress_yy]
type = ParsedFunction
# The paper gives 0.201 as the time at initial yield, but 0.20097635952803425 is the exact value.
# the paper gives -95.26 MPa as the stress at yield, but -95.26279441628823 is the exact value.
# The paper gives 12.33 as the factor in the exponential, but 12.332921390339125 is the exact value.
# -76.867432297315000, -1.442488120272900, 0.001315697947301, 1.711645501845780E-05 - exact values
symbol_names = 'timeAtYield stressAtYield expFac a b c d'
symbol_values = '0.20097635952803425 -95.26279441628823 12.332921390339125 -76.867432297315000 -1.442488120272900 0.001315697947301 1.711645501845780E-05'
value = '1e6*
if(t<=timeAtYield, -474*t,
if(t<=1, stressAtYield,
(a+b*sqrt(exp(expFac*t))+c*exp(expFac*t))/(1.0+d*exp(expFac*t))))' # tends to -a
[]
[stress_zz]
type = ParsedFunction
# The paper gives 0.201 as the time at initial yield, but 0.20097635952803425 is the exact value.
# the paper gives 190.5 MPa as the stress at yield, but 190.52558883257645 is the exact value.
# The paper gives 12.33 as the factor in the exponential, but 12.332921390339125 is the exact value.
# -112.541607626499000, 1.272064329066080, 0.001926313364644, 1.711645501845780E-05 - exact values
symbol_names = 'timeAtYield stressAtYield expFac a b c d'
symbol_values = '0.20097635952803425 190.52558883257645 12.332921390339125 -112.541607626499000 1.272064329066080 0.001926313364644 1.711645501845780E-05'
value = '1e6*
if(t<=timeAtYield, 948*t,
if(t<=1, stressAtYield,
(a+b*sqrt(exp(expFac*t))+c*exp(expFac*t))/(1.0+d*exp(expFac*t))))' # tends to -a
[]
[]
[Variables]
[disp_x]
order = FIRST
family = LAGRANGE
[]
[disp_y]
order = FIRST
family = LAGRANGE
[]
[disp_z]
order = FIRST
family = LAGRANGE
[]
[]
[AuxVariables]
[./stress_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./stress_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./stress_zz]
order = CONSTANT
family = MONOMIAL
[../]
[./vonmises]
order = CONSTANT
family = MONOMIAL
[../]
[./plastic_strain_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./plastic_strain_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./plastic_strain_zz]
order = CONSTANT
family = MONOMIAL
[../]
[]
[Kernels]
[SolidMechanics]
[../]
[]
[AuxKernels]
[./stress_xx]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_xx
index_i = 0
index_j = 0
execute_on = 'timestep_end'
[../]
[./stress_yy]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_yy
index_i = 1
index_j = 1
execute_on = 'timestep_end'
[../]
[./stress_zz]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_zz
index_i = 2
index_j = 2
execute_on = 'timestep_end'
[../]
[./vonmises]
type = RankTwoScalarAux
rank_two_tensor = stress
variable = vonmises
scalar_type = vonmisesStress
execute_on = 'timestep_end'
[../]
[./plastic_strain_xx]
type = RankTwoAux
rank_two_tensor = plastic_strain
variable = plastic_strain_xx
index_i = 0
index_j = 0
execute_on = 'timestep_end'
[../]
[./plastic_strain_yy]
type = RankTwoAux
rank_two_tensor = plastic_strain
variable = plastic_strain_yy
index_i = 1
index_j = 1
execute_on = 'timestep_end'
[../]
[./plastic_strain_zz]
type = RankTwoAux
rank_two_tensor = plastic_strain
variable = plastic_strain_zz
index_i = 2
index_j = 2
execute_on = 'timestep_end'
[../]
[]
[BCs]
[fixed_x]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[fixed_y]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[fixed_z]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[disp_x]
type = FunctionDirichletBC
variable = disp_x
boundary = right
function = disp_x
[]
[disp_y]
type = FunctionDirichletBC
variable = disp_y
boundary = top
function = disp_y
[]
[disp_z]
type = FunctionDirichletBC
variable = disp_z
boundary = front
function = disp_z
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 210666666666.666667
poissons_ratio = 0.3333333333333333
[../]
[./strain]
type = ComputeIncrementalStrain
[../]
[creep]
type = PowerLawCreepStressUpdate
coefficient = 0
n_exponent = 1
m_exponent = 1
activation_energy = 0
temperature = 1
[]
[isotropic_plasticity]
type = IsotropicPlasticityStressUpdate
yield_stress = 285788383.2488647 # = sqrt(3)*165e6 = sqrt(3) * yield in shear
hardening_constant = 0.0
[]
[radial_return_stress]
type = ComputeCreepPlasticityStress
tangent_operator = elastic
creep_model = creep
plasticity_model = isotropic_plasticity
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp_ew'
petsc_options_iname = '-pc_type'
petsc_options_value = 'lu'
nl_abs_tol = 1e-10
l_max_its = 20
start_time = 0.0
dt = 0.01 # use 0.0001 for a nearly exact match
end_time = 2.0
[]
[Postprocessors]
[analytic_xx]
type = FunctionValuePostprocessor
function = stress_xx
[]
[analytic_yy]
type = FunctionValuePostprocessor
function = stress_yy
[]
[analytic_zz]
type = FunctionValuePostprocessor
function = stress_zz
[]
[stress_xx]
type = ElementalVariableValue
variable = stress_xx
elementid = 0
[]
[stress_yy]
type = ElementalVariableValue
variable = stress_yy
elementid = 0
[]
[stress_zz]
type = ElementalVariableValue
variable = stress_zz
elementid = 0
[]
[stress_xx_l2_error]
type = ElementL2Error
variable = stress_xx
function = stress_xx
[]
[stress_yy_l2_error]
type = ElementL2Error
variable = stress_yy
function = stress_yy
[]
[stress_zz_l2_error]
type = ElementL2Error
variable = stress_zz
function = stress_zz
[]
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/combined_creep_plasticity/combined_creep_plasticity_start_time.i)
#
# This test is Example 2 from "A Consistent Formulation for the Integration
# of Combined Plasticity and Creep" by P. Duxbury, et al., Int J Numerical
# Methods in Engineering, Vol. 37, pp. 1277-1295, 1994.
#
# The problem is a one-dimensional bar which is loaded from yield to a value of twice
# the initial yield stress and then unloaded to return to the original stress. The
# bar must harden to the required yield stress during the load ramp, with no
# further yielding during unloading. The initial yield stress (sigma_0) is prescribed
# as 20 with a plastic strain hardening of 100. The mesh is a 1x1x1 cube with symmetry
# boundary conditions on three planes to provide a uniaxial stress field.
#
# In the PowerLawCreep model, the creep strain rate is defined by:
#
# edot = A(sigma)**n * exp(-Q/(RT)) * t**m
#
# The creep law specified in the paper, however, defines the creep strain rate as:
#
# edot = Ao * mo * (sigma)**n * t**(mo-1)
# with the creep parameters given by
# Ao = 1e-7
# mo = 0.5
# n = 5
#
# thus, input parameters for the test were specified as:
# A = Ao * mo = 1e-7 * 0.5 = 0.5e-7
# m = mo-1 = -0.5
# n = 5
# Q = 0
#
# The variation of load P with time is:
# P = 20 + 20t 0 < t < 1
# P = 40 - 40(t-1) 1 < t 1.5
#
# The analytic solution for total strain during the loading period 0 < t < 1 is:
#
# e_tot = (sigma_0 + 20*t)/E + 0.2*t + A * t**0.5 * sigma_0**n * [ 1 + (5/3)*t +
# + 2*t**2 + (10/7)*t**3 + (5/9)**t**4 + (1/11)*t**5 ]
#
# and during the unloading period 1 < t < 1.5:
#
# e_tot = (sigma_1 - 40*(t-1))/E + 0.2 + (4672/693) * A * sigma_0**n +
# A * sigma_0**n * [ t**0.5 * ( 32 - (80/3)*t + 16*t**2 - (40/7)*t**3
# + (10/9)*t**4 - (1/11)*t**5 ) - (11531/693) ]
#
# where sigma_1 is the stress at time t = 1.
#
# Assuming a Young's modulus (E) of 1000 and using the parameters defined above:
#
# e_tot(1) = 2.39734
# e_tot(1.5) = 3.16813
#
#
# The numerically computed solution is:
#
# e_tot(1) = 2.39718 (~0.006% error)
# e_tot(1.5) = 3.15555 (~0.40% error)
#
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Physics/SolidMechanics/QuasiStatic]
[./all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy elastic_strain_yy creep_strain_yy plastic_strain_yy'
[../]
[]
[Functions]
[./top_pull]
type = PiecewiseLinear
x = ' 10 11 11.5'
y = '-20 -40 -20'
[../]
[./dts]
type = PiecewiseLinear
x = '10 10.5 11.0 11.5'
y = '0.015 0.015 0.005 0.005'
[../]
[]
[BCs]
[./u_top_pull]
type = Pressure
variable = disp_y
boundary = top
factor = 1
function = top_pull
[../]
[./u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[../]
[./u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[../]
[./u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
block = 0
youngs_modulus = 1e3
poissons_ratio = 0.3
[../]
[./creep_plas]
type = ComputeMultipleInelasticStress
block = 0
tangent_operator = elastic
inelastic_models = 'creep plas'
max_iterations = 50
absolute_tolerance = 1e-05
combined_inelastic_strain_weights = '0.0 1.0'
[../]
[./creep]
type = PowerLawCreepStressUpdate
block = 0
coefficient = 0.5e-7
n_exponent = 5
m_exponent = -0.5
activation_energy = 0
start_time = 10
[../]
[./plas]
type = IsotropicPlasticityStressUpdate
block = 0
hardening_constant = 100
yield_stress = 20
[../]
[]
[Executioner]
type = Transient
#Preconditioned JFNK (default)
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 6
nl_rel_tol = 1e-6
nl_abs_tol = 1e-10
l_tol = 1e-5
start_time = 10.0
end_time = 11.5
[./TimeStepper]
type = FunctionDT
function = dts
[../]
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/substepping/power_law_creep.i)
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
[gen]
type = GeneratedMeshGenerator
dim = 3
nx = 2
ny = 2
nz = 2
[]
[]
[AuxVariables]
[temp]
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
add_variables = true
generate_output = 'stress_zz elastic_strain_zz creep_strain_zz'
use_automatic_differentiation = false
[]
[]
[Functions]
[front_pull]
type = PiecewiseLinear
x = '0 1'
y = '0 1'
scale_factor = 0.5
[]
[]
[BCs]
[u_front_pull]
type = ADFunctionDirichletBC
variable = disp_z
boundary = front
function = front_pull
[]
[uz_back_fix]
type = ADDirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[u_yz_fix]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xz_fix]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
[]
[power_law_creep]
type = PowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 0.0
temperature = temp
# options for using substepping
substep_strain_tolerance = 0.1
max_inelastic_increment = 0.01
[]
[]
[Executioner]
type = Transient
solve_type = 'NEWTON'
petsc_options_iname = '-pc_type '
petsc_options_value = 'lu '
line_search = 'none'
nl_max_its = 10
nl_rel_tol = 1e-6
nl_abs_tol = 1e-10
end_time = 0.1
dt = 0.1
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/rom_stress_update/AD_finite_strain_power_law_creep.i)
[GlobalParams]
displacements = 'disp_r disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 2
xmin = 1
xmax = 2
nx = 50
ny = 50
coord_type = RZ
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
eigenstrain_names = 'thermal'
use_automatic_differentiation = true
[]
[]
[AuxVariables]
[temp]
initial_condition = 1000.0
[]
[]
[AuxKernels]
[cooling]
type = FunctionAux
variable = temp
function = '1000-10*t*x'
[]
[]
[BCs]
[top_pull]
type = ADFunctionNeumannBC
variable = disp_z
boundary = top
function = '1e7*t'
use_displaced_mesh = true
[]
[bottom_fix]
type = ADDirichletBC
variable = disp_z
boundary = bottom
value = 0.0
[]
[left_fix]
type = ADDirichletBC
variable = disp_r
boundary = left
value = 0.0
[]
[]
[Materials]
[eigenstrain]
type = ADComputeThermalExpansionEigenstrain
eigenstrain_name = 'thermal'
stress_free_temperature = 1000
thermal_expansion_coeff = 1e-4
temperature = temp
[]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'creep'
[]
[creep]
type = ADPowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Postprocessors]
[nl_its]
type = NumNonlinearIterations
[]
[total_nl_its]
type = CumulativeValuePostprocessor
postprocessor = nl_its
[]
[]
[Executioner]
type = Transient
solve_type = 'NEWTON'
petsc_options_iname = '-pc_type'
petsc_options_value = 'lu'
line_search = 'none'
end_time = 10
dt = 1
automatic_scaling = true
[]
[Outputs]
print_linear_converged_reason = false
print_nonlinear_converged_reason = false
print_linear_residuals = false
perf_graph = true
[]
(modules/solid_mechanics/test/tests/power_law_creep/ad_smallstrain.i)
# 1x1x1 unit cube with uniform pressure on top face for the case of small strain.
# This test does not have a solid mechanics analog because there is not an equvialent
# small strain with rotations strain calculator material in solid mechanics
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Variables]
[temp]
order = FIRST
family = LAGRANGE
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = SMALL
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
use_automatic_differentiation = true
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = '0 1'
y = '1 1'
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = ADPressure
variable = disp_y
boundary = top
factor = -10.0e6
function = top_pull
[]
[u_bottom_fix]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = ADDirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
constant_on = SUBDOMAIN
[]
[radial_return_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
[]
[power_law_creep]
type = ADPowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Preconditioning]
[smp]
type = SMP
full = true
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp_ew'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.0
end_time = 1.0
num_steps = 10
dt = 0.1
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/combined_creep_plasticity/creepWithPlasticity.i)
#
# This test is Example 2 from "A Consistent Formulation for the Integration
# of Combined Plasticity and Creep" by P. Duxbury, et al., Int J Numerical
# Methods in Engineering, Vol. 37, pp. 1277-1295, 1994.
#
# The problem is a one-dimensional bar which is loaded from yield to a value of twice
# the initial yield stress and then unloaded to return to the original stress. The
# bar must harden to the required yield stress during the load ramp, with no
# further yielding during unloading. The initial yield stress (sigma_0) is prescribed
# as 20 with a plastic strain hardening of 100. The mesh is a 1x1x1 cube with symmetry
# boundary conditions on three planes to provide a uniaxial stress field.
#
# In the PowerLawCreep model, the creep strain rate is defined by:
#
# edot = A(sigma)**n * exp(-Q/(RT)) * t**m
#
# The creep law specified in the paper, however, defines the creep strain rate as:
#
# edot = Ao * mo * (sigma)**n * t**(mo-1)
# with the creep parameters given by
# Ao = 1e-7
# mo = 0.5
# n = 5
#
# thus, input parameters for the test were specified as:
# A = Ao * mo = 1e-7 * 0.5 = 0.5e-7
# m = mo-1 = -0.5
# n = 5
# Q = 0
#
# The variation of load P with time is:
# P = 20 + 20t 0 < t < 1
# P = 40 - 40(t-1) 1 < t 1.5
#
# The analytic solution for total strain during the loading period 0 < t < 1 is:
#
# e_tot = (sigma_0 + 20*t)/E + 0.2*t + A * t**0.5 * sigma_0**n * [ 1 + (5/3)*t +
# + 2*t**2 + (10/7)*t**3 + (5/9)**t**4 + (1/11)*t**5 ]
#
# and during the unloading period 1 < t < 1.5:
#
# e_tot = (sigma_1 - 40*(t-1))/E + 0.2 + (4672/693) * A * sigma_0**n +
# A * sigma_0**n * [ t**0.5 * ( 32 - (80/3)*t + 16*t**2 - (40/7)*t**3
# + (10/9)*t**4 - (1/11)*t**5 ) - (11531/693) ]
#
# where sigma_1 is the stress at time t = 1.
#
# Assuming a Young's modulus (E) of 1000 and using the parameters defined above:
#
# e_tot(1) = 2.39734
# e_tot(1.5) = 3.16813
#
#
# The numerically computed solution is:
#
# e_tot(1) = 2.39718 (~0.006% error)
# e_tot(1.5) = 3.15555 (~0.40% error)
#
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy elastic_strain_yy creep_strain_yy plastic_strain_yy'
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = ' 0 1 1.5'
y = '-20 -40 -20'
[]
[dts]
type = PiecewiseLinear
x = '0 0.5 1.0 1.5'
y = '0.015 0.015 0.005 0.005'
[]
[]
[BCs]
[u_top_pull]
type = Pressure
variable = disp_y
boundary = top
factor = 1
function = top_pull
[]
[u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
block = 0
youngs_modulus = 1e3
poissons_ratio = 0.3
[]
[creep_plas]
type = ComputeCreepPlasticityStress
block = 0
tangent_operator = elastic
creep_model = creep
plasticity_model = plasticity
max_iterations = 50
relative_tolerance = 1e-8
absolute_tolerance = 1e-8
[]
[creep]
type = PowerLawCreepStressUpdate
block = 0
coefficient = 0.5e-7
n_exponent = 5
m_exponent = -0.5
activation_energy = 0
temperature = 1
[]
[plasticity]
type = IsotropicPlasticityStressUpdate
block = 0
yield_stress = 20
hardening_constant = 100
[]
[]
[Executioner]
type = Transient
#Preconditioned JFNK (default)
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 6
nl_rel_tol = 1e-6
nl_abs_tol = 1e-10
l_tol = 1e-5
start_time = 0.0
end_time = 1.5
[TimeStepper]
type = FunctionDT
function = dts
[]
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/combined_creep_plasticity/combined_stress_prescribed.i)
#
# 1x1x1 unit cube with time-varying pressure on top face
#
# The problem is a one-dimensional creep analysis. The top face has a
# pressure load that is a function of time. The creep strain can be
# calculated analytically. There is no practical active linear
# isotropic plasticity because the yield stress for the plasticity
# model is set to 1e30 MPa, which will not be reached in this
# regression test.
#
# The analytic solution to this problem is:
#
# d ec
# ---- = a*S^b with S = c*t^d
# dt
#
# d ec = a*c^b*t^(b*d) dt
#
# a*c^b
# ec = ----- t^(b*d+1)
# b*d+1
#
# where S = stress
# ec = creep strain
# t = time
# a = constant
# b = constant
# c = constant
# d = constant
#
# With a = 3e-24,
# b = 4,
# c = 1,
# d = 1/2, and
# t = 32400
# we have
#
# S = t^(1/2) = 180
#
# ec = 1e-24*t^3 = 3.4012224e-11
#
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
volumetric_locking_correction = true
[]
[Physics/SolidMechanics/QuasiStatic]
[./all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_yy'
[../]
[]
[Functions]
[./pressure]
type = ParsedFunction
expression = 'sqrt(t)'
[../]
[./dts]
type = PiecewiseLinear
y = '1e-2 1e-1 1e0 1e1 1e2'
x = '0 7e-1 7e0 7e1 1e2'
[../]
[]
[BCs]
[./top_pressure]
type = Pressure
variable = disp_y
boundary = top
function = pressure
[../]
[./u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[../]
[./u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[../]
[./u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2.8e7
poissons_ratio = 0.3
[../]
[./creep_plas]
type = ComputeMultipleInelasticStress
inelastic_models = 'creep plas'
tangent_operator = elastic
[../]
[./creep]
type = PowerLawCreepStressUpdate
coefficient = 3.0e-24
n_exponent = 4
m_exponent = 0
activation_energy = 0
[../]
[./plas]
type = IsotropicPlasticityStressUpdate
hardening_constant = 1
yield_stress = 1e30
[../]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options_iname = '-pc_type -pc_factor_mat_solver_package'
petsc_options_value = ' lu superlu_dist'
line_search = 'none'
l_max_its = 100
nl_max_its = 100
nl_rel_tol = 1e-10
nl_abs_tol = 1e-7
l_tol = 1e-6
start_time = 0.0
end_time = 32400
dt = 1e-2
[./TimeStepper]
type = FunctionDT
function = dts
[../]
[]
[Postprocessors]
[./timestep]
type = TimestepSize
[../]
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/scalar_material_damage/ad_scalar_material_damage_creep_power.i)
# This is a basic test of the system for continuum damage mechanics
# materials. It uses ScalarMaterialDamage for the damage model,
# which simply gets its damage index from another material. In this
# case, we prescribe the evolution of the damage index using a
# function. A single element has a fixed prescribed displacement
# on one side that puts the element in tension, and then the
# damage index evolves from 0 to 1 over time, and this verifies
# that the stress correspondingly drops to 0.
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
elem_type = HEX8
[]
[AuxVariables]
[damage_index]
order = CONSTANT
family = MONOMIAL
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = SMALL
incremental = true
add_variables = true
generate_output = 'stress_xx strain_xx creep_strain_xx'
use_automatic_differentiation = true
[]
[]
[AuxKernels]
[damage_index]
type = ADMaterialRealAux
variable = damage_index
property = damage_index_prop
execute_on = timestep_end
[]
[]
[BCs]
[symmy]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0
[]
[symmx]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0
[]
[symmz]
type = ADDirichletBC
variable = disp_z
boundary = back
value = 0
[]
[axial_load]
type = ADDirichletBC
variable = disp_x
boundary = right
value = 0.01
[]
[]
[Functions]
[damage_evolution]
type = PiecewiseLinear
xy_data = '0.0 0.0
0.1 0.0
2.1 2.0'
[]
[]
[Materials]
[damage_index]
type = ADGenericFunctionMaterial
prop_names = damage_index_prop
prop_values = damage_evolution
[]
[damage]
type = ADScalarMaterialDamage
damage_index = damage_index_prop
[]
[stress]
type = ADComputeMultipleInelasticStress
damage_model = damage
inelastic_models = 'creep'
[]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 140000
poissons_ratio = 0.3
[]
[creep]
type = ADPowerLawCreepStressUpdate
coefficient = 1.1e-12 #
n_exponent = 8.7
m_exponent = 0
activation_energy = 0.0
[]
[]
[Postprocessors]
[stress_xx]
type = ElementAverageValue
variable = stress_xx
[]
[strain_xx]
type = ElementAverageValue
variable = strain_xx
[]
[creep_strain_xx]
type = ElementAverageValue
variable = creep_strain_xx
[]
[damage_index]
type = ElementAverageValue
variable = damage_index
[]
[]
[Preconditioning]
[smp]
type = SMP
full = true
[]
[]
[Executioner]
type = Transient
l_max_its = 50
l_tol = 1e-8
nl_max_its = 20
nl_rel_tol = 1e-10
nl_abs_tol = 1e-8
dt = 0.1
dtmin = 0.001
end_time = 1.1
[]
[Outputs]
csv = true
[]
(modules/solid_mechanics/test/tests/domain_integral_thermal/interaction_integral_2d_c.i)
#This problem from [Wilson 1979] tests the thermal strain term in the
#interaction integral
#
#theta_e = 10 degrees C; a = 252; E = 207000; nu = 0.3; alpha = 1.35e-5
#
#With uniform_refine = 3, KI converges to
#KI = 5.602461e+02 (interaction integral)
#KI = 5.655005e+02 (J-integral)
#
#Both are in good agreement with [Shih 1986]:
#average_value = 0.4857 = KI / (sigma_theta * sqrt(pi * a))
#sigma_theta = E * alpha * theta_e / (1 - nu)
# = 207000 * 1.35e-5 * 10 / (1 - 0.3) = 39.9214
#KI = average_value * sigma_theta * sqrt(pi * a) = 5.656e+02
#
#References:
#W.K. Wilson, I.-W. Yu, Int J Fract 15 (1979) 377-387
#C.F. Shih, B. Moran, T. Nakamura, Int J Fract 30 (1986) 79-102
[GlobalParams]
order = FIRST
family = LAGRANGE
displacements = 'disp_x disp_y'
volumetric_locking_correction = False
[]
[Mesh]
file = crack2d.e
displacements = 'disp_x disp_y'
# uniform_refine = 3
[]
[AuxVariables]
[./SED]
order = CONSTANT
family = MONOMIAL
[../]
[./SERD]
order = CONSTANT
family = MONOMIAL
[../]
[./temp]
order = FIRST
family = LAGRANGE
[../]
[]
[Functions]
[./rampConstantUp]
type = PiecewiseLinear
x = '0. 0.1 100.0'
y = '0. 1 1'
scale_factor = -68.95 #MPa
[../]
[]
[Physics/SolidMechanics/QuasiStatic]
[./master]
strain = FINITE
add_variables = true
incremental = true
generate_output = 'stress_xx stress_yy stress_zz vonmises_stress'
planar_formulation = PLANE_STRAIN
[../]
[]
[AuxKernels]
[./SED]
type = MaterialRealAux
variable = SED
property = strain_energy_density
execute_on = timestep_end
[../]
[./SERD]
type = MaterialRealAux
variable = SERD
property = strain_energy_rate_density
execute_on = timestep_end
[../]
[]
[BCs]
[./crack_y]
type = DirichletBC
variable = disp_y
boundary = 100
value = 0.0
[../]
[./no_y]
type = DirichletBC
variable = disp_y
boundary = 400
value = 0.0
[../]
[./no_x1]
type = DirichletBC
variable = disp_x
boundary = 900
value = 0.0
[../]
[./Pressure]
[./crack_pressure]
boundary = 700
function = rampConstantUp
[../]
[../]
[] # BCs
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 206800
poissons_ratio = 0.0
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'powerlawcrp'
[../]
[./powerlawcrp]
type = PowerLawCreepStressUpdate
coefficient = 3.125e-21 # 7.04e-17 #
n_exponent = 3.0
m_exponent = 0.0
activation_energy = 0.0
[../]
[]
[DomainIntegral]
integrals = 'CIntegral InteractionIntegralKI'
boundary = 800
crack_direction_method = CrackDirectionVector
crack_direction_vector = '1 0 0'
2d = true
axis_2d = 2
radius_inner = '60.0 80.0 100.0 120.0'
radius_outer = '80.0 100.0 120.0 140.0'
symmetry_plane = 1
incremental = true
# interaction integral parameters
block = 1
youngs_modulus = 207000
poissons_ratio = 0.3
inelastic_models = 'powerlawcrp'
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options_iname = '-pc_type -ksp_gmres_restart -sub_ksp_type -sub_pc_type -pc_asm_overlap'
petsc_options_value = 'asm 31 preonly lu 1'
line_search = 'none'
l_max_its = 50
nl_max_its = 40
nl_rel_step_tol= 1e-10
nl_rel_tol = 1e-10
start_time = 0.0
dt = 1
end_time = 1
num_steps = 1
[]
[Outputs]
exodus = true
csv = true
[]
[Preconditioning]
active = 'smp'
[./smp]
type = SMP
pc_side = left
ksp_norm = preconditioned
full = true
[../]
[]
(modules/solid_mechanics/test/tests/domain_integral_thermal/c_integral_2d.i)
[GlobalParams]
order = FIRST
family = LAGRANGE
displacements = 'disp_x disp_y'
volumetric_locking_correction = true
[]
[Mesh]
file = crack2d.e
[]
[AuxVariables]
[./SERD]
order = CONSTANT
family = MONOMIAL
[../]
[]
[Functions]
[./rampConstantUp]
type = PiecewiseLinear
x = '0. 0.1 100.0'
y = '0. 1 1'
scale_factor = -68.95 #MPa
[../]
[]
[Physics/SolidMechanics/QuasiStatic]
[./master]
strain = FINITE
add_variables = true
incremental = true
generate_output = 'stress_xx stress_yy stress_zz vonmises_stress'
planar_formulation = PLANE_STRAIN
[../]
[]
[AuxKernels]
[./SERD]
type = MaterialRealAux
variable = SERD
property = strain_energy_rate_density
execute_on = timestep_end
[../]
[]
[BCs]
[./crack_y]
type = DirichletBC
variable = disp_y
boundary = 100
value = 0.0
[../]
[./no_y]
type = DirichletBC
variable = disp_y
boundary = 400
value = 0.0
[../]
[./no_x1]
type = DirichletBC
variable = disp_x
boundary = 900
value = 0.0
[../]
[./Pressure]
[./crack_pressure]
boundary = 700
function = rampConstantUp
[../]
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 206800
poissons_ratio = 0.0
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'powerlawcrp'
[../]
[./powerlawcrp]
type = PowerLawCreepStressUpdate
coefficient = 3.125e-21 # 7.04e-17 #
n_exponent = 2.0
m_exponent = 0.0
activation_energy = 0.0
[../]
[]
[DomainIntegral]
integrals = CIntegral
boundary = 800
crack_direction_method = CrackDirectionVector
crack_direction_vector = '1 0 0'
2d = true
axis_2d = 2
radius_inner = '60.0 80.0 100.0 120.0'
radius_outer = '80.0 100.0 120.0 140.0'
incremental = true
inelastic_models = 'powerlawcrp'
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options_iname = '-pc_type -ksp_gmres_restart -sub_ksp_type -sub_pc_type -pc_asm_overlap'
petsc_options_value = 'asm 31 preonly lu 1'
line_search = 'none'
l_max_its = 50
nl_max_its = 40
nl_rel_step_tol= 1e-10
nl_rel_tol = 1e-10
start_time = 0.0
dt = 1
end_time = 1
num_steps = 1
[]
[Outputs]
exodus = true
[]
[Preconditioning]
[./smp]
type = SMP
pc_side = left
ksp_norm = preconditioned
full = true
[../]
[]
(modules/solid_mechanics/test/tests/strain_energy_density/nonAD_rate_model_weak_plane.i)
# Single element test to check the strain energy density calculation
[GlobalParams]
displacements = 'disp_x disp_y'
volumetric_locking_correction = true
out_of_plane_strain = strain_zz
[]
[Mesh]
type = GeneratedMesh
dim = 2
nx = 1
ny = 1
xmin = 0
xmax = 1
ymin = 0
ymax = 2
[]
[Variables]
[./strain_zz]
[]
[]
[AuxVariables]
[./SERD]
order = CONSTANT
family = MONOMIAL
[../]
[]
[Functions]
[./rampConstantUp]
type = PiecewiseLinear
x = '0. 1.'
y = '0. 1.'
scale_factor = -100
[../]
[]
[Physics/SolidMechanics/QuasiStatic]
[./master]
strain = FINITE
add_variables = true
incremental = true
generate_output = 'stress_xx stress_yy stress_zz vonmises_stress strain_xx strain_yy'
planar_formulation = WEAK_PLANE_STRESS
[../]
[]
[AuxKernels]
[./SERD]
type = MaterialRealAux
variable = SERD
property = strain_energy_rate_density
execute_on = timestep_end
[../]
[]
[BCs]
[./no_x]
type = DirichletBC
variable = disp_x
boundary = 'left'
value = 0.0
[../]
[./no_y]
type = DirichletBC
variable = disp_y
boundary = 'bottom'
value = 0.0
[../]
[./Pressure]
[./top]
boundary = 'top'
function = rampConstantUp
[../]
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 206800
poissons_ratio = 0.0
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'powerlawcrp'
[../]
[./powerlawcrp]
type = PowerLawCreepStressUpdate
coefficient = 3.125e-21 # 7.04e-17 #
n_exponent = 4.0
m_exponent = 0.0
activation_energy = 0.0
# max_inelastic_increment = 0.01
[../]
[./strain_energy_rate_density]
type = StrainEnergyRateDensity
inelastic_models = 'powerlawcrp'
[../]
[]
[Executioner]
type = Transient
petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
petsc_options_value = '201 hypre boomeramg 4'
line_search = 'none'
l_max_its = 50
nl_max_its = 20
nl_abs_tol = 3e-7
nl_rel_tol = 1e-12
l_tol = 1e-2
start_time = 0.0
dt = 1
end_time = 1
num_steps = 1
[]
[Postprocessors]
[./SERD]
type = ElementAverageValue
variable = SERD
[../]
[]
[Outputs]
csv = true
[]
(modules/solid_mechanics/test/tests/multi_power_law/power_law_creep.i)
[Mesh]
type = GeneratedMesh
dim = 2
nx = 2
ny = 2
second_order = true
[]
[GlobalParams]
displacements = 'disp_x disp_y'
volumetric_locking_correction = false
[]
[Functions]
[pull]
type = PiecewiseLinear
x = '0 10'
y = '0 1e-3'
[]
[]
[AuxVariables]
[strain_energy_rate_density]
order = CONSTANT
family = MONOMIAL
[]
[]
[AuxKernels]
[strain_energy_rate_density]
type = MaterialRealAux
variable = strain_energy_rate_density
property = strain_energy_rate_density
execute_on = timestep_end
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = SMALL
incremental = true
add_variables = true
use_automatic_differentiation = true
generate_output = 'hydrostatic_stress vonmises_stress'
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 1e10
poissons_ratio = 0.3
[]
[elastic_strain]
type = ADComputeMultipleInelasticStress
inelastic_models = "creep_nine creep_one"
[]
[creep_one]
type = ADPowerLawCreepStressUpdate
coefficient = 1e-24
n_exponent = 4
m_exponent = 0
activation_energy = 0
base_name = creep_one
[]
[creep_nine]
type = ADPowerLawCreepStressUpdate
coefficient = 9e-24
n_exponent = 4
m_exponent = 0
activation_energy = 0
base_name = creep_nine
[]
[strain_energy_rate_density]
type = ADStrainEnergyRateDensity
inelastic_models = 'creep_nine'
[]
[]
[BCs]
[no_disp_x]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[no_disp_y]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[pull_disp_y]
type = ADFunctionDirichletBC
variable = disp_y
boundary = top
function = pull
[]
[]
[Preconditioning]
[smp]
type = SMP
full = true
[]
[]
[Executioner]
type = Transient
petsc_options_iname = -pc_hypre_type
petsc_options_value = boomeramg
line_search = 'none'
nl_rel_tol = 1e-11
nl_abs_tol = 1e-11
num_steps = 5
dt = 1e-1
[]
[Postprocessors]
[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
[]
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/power_law_creep/ad_restart1.i)
# 1x1x1 unit cube with uniform pressure on top face
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Variables]
[temp]
order = FIRST
family = LAGRANGE
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
use_automatic_differentiation = true
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = '0 1'
y = '1 1'
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = ADPressure
variable = disp_y
boundary = top
factor = -10.0e6
function = top_pull
[]
[u_bottom_fix]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = ADDirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
constant_on = SUBDOMAIN
[]
[radial_return_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
[]
[power_law_creep]
type = ADPowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.0
end_time = 1.0
num_steps = 6
dt = 0.1
[]
[Outputs]
exodus = true
[out]
type = Checkpoint
num_files = 1
[]
[]
(modules/solid_mechanics/test/tests/power_law_creep/power_law_creep.i)
# 1x1x1 unit cube with uniform pressure on top face
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Variables]
[temp]
order = FIRST
family = LAGRANGE
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = '0 1'
y = '1 1'
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = Pressure
variable = disp_y
boundary = top
factor = -10.0e6
function = top_pull
[]
[u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
tangent_operator = elastic
[]
[power_law_creep]
type = PowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.0
end_time = 1.0
num_steps = 10
dt = 0.1
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/combined_creep_plasticity/combined_stress_relaxation.i)
#
# 1x1x1 unit cube with constant displacement on top face
#
# This problem was taken from "Finite element three-dimensional elastic-plastic
# creep analysis" by A. Levy, Eng. Struct., 1981, Vol. 3, January, pp. 9-16.
#
# The problem is a one-dimensional creep analysis. The top face is displaced 0.01
# units and held there. The stress relaxes in time according to the creep law.
#
# The analytic solution to this problem is (contrary to what is shown in the paper):
#
# / (E*ef)^3 \^(1/3)
# stress_yy = |---------------------|
# \ 3*a*E^4*ef^3*t + 1 /
#
# where E = 2.0e11 (Young's modulus)
# a = 3e-26 (creep coefficient)
# ef = 0.01 (displacement)
# t = 2160.0 (time)
#
# such that the analytical solution is computed to be 2.9518e3 Pa
#
# Averaged over the single element block, MOOSE calculates the stress in the yy direction to be
# to be 3.046e3 Pa, which is a 3.2% error from the analytical solution.
#
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Functions]
[./dts]
type = PiecewiseLinear
y = '1e-2 1e-1 1e0 1e1 1e2'
x = '0 7e-1 7e0 7e1 1e2'
[../]
[]
[Physics/SolidMechanics/QuasiStatic]
[./all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
[../]
[]
[BCs]
[./u_top_pull]
type = DirichletBC
variable = disp_y
boundary = top
value = 0.01
[../]
[./u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[../]
[./u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[../]
[./u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2.0e11
poissons_ratio = 0.3
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
tangent_operator = elastic
inelastic_models = 'power_law_creep'
[../]
[./power_law_creep]
type = PowerLawCreepStressUpdate
coefficient = 3.0e-26
n_exponent = 4
activation_energy = 0.0
relative_tolerance = 1e-14
absolute_tolerance = 1e-14
[../]
[]
[Postprocessors]
[./stress_yy]
type = ElementAverageValue
variable = stress_yy
[../]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 100
nl_max_its = 100
nl_rel_tol = 1e-5
nl_abs_tol = 1e-8
l_tol = 1e-5
start_time = 0.0
end_time = 2160
[./TimeStepper]
type = FunctionDT
function = dts
[../]
[]
[Outputs]
exodus = true
[]
(modules/combined/test/tests/inelastic_strain/creep/creep_nl1.i)
#
# Test for effective strain calculation.
# Boundary conditions from NAFEMS test NL1
#
# This is not a verification test. This is the creep analog of the same test
# in the elas_plas directory. Instead of using the IsotropicPlasticity
# material model this test uses the PowerLawCreep material model.
#
[GlobalParams]
temperature = temp
order = FIRST
family = LAGRANGE
volumetric_locking_correction = true
displacements = 'disp_x disp_y'
[]
[Mesh]
file = one_elem2.e
[]
[Variables]
[./disp_x]
[../]
[./disp_y]
[../]
[./temp]
initial_condition = 600.0
[../]
[]
[AuxVariables]
[./stress_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./stress_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./stress_zz]
order = CONSTANT
family = MONOMIAL
[../]
[./stress_xy]
order = CONSTANT
family = MONOMIAL
[../]
[./vonmises]
order = CONSTANT
family = MONOMIAL
[../]
[./pressure]
order = CONSTANT
family = MONOMIAL
[../]
[./elastic_strain_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./elastic_strain_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./elastic_strain_zz]
order = CONSTANT
family = MONOMIAL
[../]
[./creep_strain_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./creep_strain_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./creep_strain_zz]
order = CONSTANT
family = MONOMIAL
[../]
[./tot_strain_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./tot_strain_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./tot_strain_zz]
order = CONSTANT
family = MONOMIAL
[../]
[./eff_creep_strain]
order = CONSTANT
family = MONOMIAL
[../]
[]
[Kernels]
[./TensorMechanics]
use_displaced_mesh = true
decomposition_method = EigenSolution
[../]
[./heat]
type = HeatConduction
variable = temp
[../]
[./heat_ie]
type = HeatConductionTimeDerivative
variable = temp
[../]
[]
[AuxKernels]
[./stress_xx]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_xx
index_i = 0
index_j = 0
execute_on = timestep_end
[../]
[./stress_yy]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_yy
index_i = 1
index_j = 1
execute_on = timestep_end
[../]
[./stress_zz]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_zz
index_i = 2
index_j = 2
execute_on = timestep_end
[../]
[./stress_xy]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_xy
index_i = 0
index_j = 1
execute_on = timestep_end
[../]
[./vonmises]
type = RankTwoScalarAux
rank_two_tensor = stress
variable = vonmises
scalar_type = VonMisesStress
execute_on = timestep_end
[../]
[./pressure]
type = RankTwoScalarAux
rank_two_tensor = stress
variable = pressure
scalar_type = Hydrostatic
execute_on = timestep_end
[../]
[./elastic_strain_xx]
type = RankTwoAux
rank_two_tensor = elastic_strain
variable = elastic_strain_xx
index_i = 0
index_j = 0
execute_on = timestep_end
[../]
[./elastic_strain_yy]
type = RankTwoAux
rank_two_tensor = elastic_strain
variable = elastic_strain_yy
index_i = 1
index_j = 1
execute_on = timestep_end
[../]
[./elastic_strain_zz]
type = RankTwoAux
rank_two_tensor = elastic_strain
variable = elastic_strain_zz
index_i = 2
index_j = 2
execute_on = timestep_end
[../]
[./creep_strain_xx]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xx
index_i = 0
index_j = 0
execute_on = timestep_end
[../]
[./creep_strain_yy]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_yy
index_i = 1
index_j = 1
execute_on = timestep_end
[../]
[./creep_strain_zz]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_zz
index_i = 2
index_j = 2
execute_on = timestep_end
[../]
[./tot_strain_xx]
type = RankTwoAux
rank_two_tensor = total_strain
variable = tot_strain_xx
index_i = 0
index_j = 0
[../]
[./tot_strain_yy]
type = RankTwoAux
rank_two_tensor = total_strain
variable = tot_strain_yy
index_i = 1
index_j = 1
[../]
[./tot_strain_zz]
type = RankTwoAux
rank_two_tensor = total_strain
variable = tot_strain_zz
index_i = 2
index_j = 2
[../]
[./eff_creep_strain]
type = MaterialRealAux
property = effective_creep_strain
variable = eff_creep_strain
[../]
[]
[Functions]
[./appl_dispy]
type = PiecewiseLinear
x = '0 1.0 2.0'
y = '0.0 0.25e-4 0.50e-4'
[../]
[]
[BCs]
[./side_x]
type = DirichletBC
variable = disp_x
boundary = 101
value = 0.0
[../]
[./origin_x]
type = DirichletBC
variable = disp_x
boundary = 103
value = 0.0
[../]
[./bot_y]
type = DirichletBC
variable = disp_y
boundary = 102
value = 0.0
[../]
[./origin_y]
type = DirichletBC
variable = disp_y
boundary = 103
value = 0.0
[../]
[./top_y]
type = FunctionDirichletBC
variable = disp_y
boundary = 1
function = appl_dispy
[../]
[./temp_fix]
type = DirichletBC
variable = temp
boundary = '1 2'
value = 600.0
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
block = 1
youngs_modulus = 250e9
poissons_ratio = 0.25
[../]
[./strain]
type = ComputePlaneFiniteStrain
block = 1
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
block = 1
inelastic_models = 'powerlawcrp'
[../]
[./powerlawcrp]
type = PowerLawCreepStressUpdate
block = 1
coefficient = 3.125e-14
n_exponent = 5.0
m_exponent = 0.0
activation_energy = 0.0
[../]
[./thermal]
type = HeatConductionMaterial
block = 1
specific_heat = 1.0
thermal_conductivity = 100.
[../]
[./density]
type = Density
block = 1
density = 1.0
[../]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
nl_rel_tol = 1e-10
nl_abs_tol = 1e-12
l_tol = 1e-6
l_max_its = 100
nl_max_its = 20
dt = 1.0
start_time = 0.0
num_steps = 100
end_time = 2.0
[]
[Postprocessors]
[./stress_xx]
type = ElementAverageValue
variable = stress_xx
[../]
[./stress_yy]
type = ElementAverageValue
variable = stress_yy
[../]
[./stress_zz]
type = ElementAverageValue
variable = stress_zz
[../]
[./stress_xy]
type = ElementAverageValue
variable = stress_xy
[../]
[./vonmises]
type = ElementAverageValue
variable = vonmises
[../]
[./pressure]
type = ElementAverageValue
variable = pressure
[../]
[./el_strain_xx]
type = ElementAverageValue
variable = elastic_strain_xx
[../]
[./el_strain_yy]
type = ElementAverageValue
variable = elastic_strain_yy
[../]
[./el_strain_zz]
type = ElementAverageValue
variable = elastic_strain_zz
[../]
[./crp_strain_xx]
type = ElementAverageValue
variable = creep_strain_xx
[../]
[./crp_strain_yy]
type = ElementAverageValue
variable = creep_strain_yy
[../]
[./crp_strain_zz]
type = ElementAverageValue
variable = creep_strain_zz
[../]
[./eff_creep_strain]
type = ElementAverageValue
variable = eff_creep_strain
[../]
[./tot_strain_xx]
type = ElementAverageValue
variable = tot_strain_xx
[../]
[./tot_strain_yy]
type = ElementAverageValue
variable = tot_strain_yy
[../]
[./tot_strain_zz]
type = ElementAverageValue
variable = tot_strain_zz
[../]
[./disp_x1]
type = NodalVariableValue
nodeid = 0
variable = disp_x
[../]
[./disp_x4]
type = NodalVariableValue
nodeid = 3
variable = disp_x
[../]
[./disp_y1]
type = NodalVariableValue
nodeid = 0
variable = disp_y
[../]
[./disp_y4]
type = NodalVariableValue
nodeid = 3
variable = disp_y
[../]
[./_dt]
type = TimestepSize
[../]
[]
[Outputs]
exodus = true
[./console]
type = Console
output_linear = true
[../]
[]
(modules/solid_mechanics/test/tests/creep_tangent_operator/creep.i)
[Mesh]
type = GeneratedMesh
dim = 2
nx = 2
ny = 2
second_order = true
[]
[GlobalParams]
displacements = 'disp_x disp_y'
volumetric_locking_correction = false
[]
[Functions]
[./pull]
type = PiecewiseLinear
x = '0 10'
y = '0 1e-3'
[../]
[]
[Physics/SolidMechanics/QuasiStatic]
[./all]
strain = FINITE
add_variables = true
use_finite_deform_jacobian = true
generate_output = 'hydrostatic_stress'
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 1e10
poissons_ratio = 0.3
[../]
[./elastic_strain]
type = ComputeMultipleInelasticStress
# inelastic_models = ''
tangent_operator = nonlinear
[../]
[./creep_ten]
type = PowerLawCreepStressUpdate
coefficient = 10e-24
n_exponent = 4
activation_energy = 0
base_name = creep_ten
[../]
[./creep_ten2]
type = PowerLawCreepStressUpdate
coefficient = 10e-24
n_exponent = 4
activation_energy = 0
base_name = creep_ten2
[../]
[./creep_one]
type = PowerLawCreepStressUpdate
coefficient = 1e-24
n_exponent = 4
activation_energy = 0
base_name = creep_one
[../]
[./creep_nine]
type = PowerLawCreepStressUpdate
coefficient = 9e-24
n_exponent = 4
activation_energy = 0
base_name = creep_nine
[../]
[./creep_zero]
type = PowerLawCreepStressUpdate
coefficient = 0e-24
n_exponent = 4
activation_energy = 0
base_name = creep_zero
[../]
[]
[BCs]
[./no_disp_x]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[../]
[./no_disp_y]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[../]
[./pull_disp_y]
type = FunctionDirichletBC
variable = disp_y
boundary = top
function = pull
[../]
[]
[Preconditioning]
[./smp]
type = SMP
full = true
[../]
[]
[Executioner]
type = Transient
petsc_options_iname = '-pc_type'
petsc_options_value = 'lu'
line_search = 'none'
nl_rel_tol = 1e-5
num_steps = 5
dt = 1e-1
[]
[Postprocessors]
[./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
[../]
[]
[Outputs]
csv = true
perf_graph = true
[]
[Debug]
show_var_residual_norms = true
[]
(modules/solid_mechanics/test/tests/j_integral_vtest/c_int_surfbreak_ellip_crack_sym_mm.i)
[GlobalParams]
order = FIRST
family = LAGRANGE
displacements = 'disp_x disp_y disp_z'
volumetric_locking_correction = true
[]
[Mesh]
file = c_integral_coarse.e
partitioner = centroid
centroid_partitioner_direction = z
[]
[AuxVariables]
[./SED]
order = CONSTANT
family = MONOMIAL
[../]
[./resid_z]
[../]
[]
[Functions]
[./rampConstantUp]
type = PiecewiseLinear
x = '0. 0.1 100.0'
y = '0. 1 1'
scale_factor = -68.95 #MPa
[../]
[./dts]
type = PiecewiseLinear
x = '0 1'
y = '1 400000'
[../]
[]
[Physics/SolidMechanics/QuasiStatic]
[./master]
strain = FINITE
add_variables = true
incremental = true
generate_output = 'stress_xx stress_yy stress_zz vonmises_stress'
[../]
[]
[AuxKernels]
[./SED]
type = MaterialRealAux
variable = SED
property = strain_energy_density
execute_on = timestep_end
[../]
[]
[BCs]
[./crack_y]
type = DirichletBC
variable = disp_z
boundary = 6
value = 0.0
[../]
[./no_y]
type = DirichletBC
variable = disp_y
boundary = 12
value = 0.0
[../]
[./no_x]
type = DirichletBC
variable = disp_x
boundary = 1
value = 0.0
[../]
[./Pressure]
[./Side1]
boundary = 5
function = rampConstantUp
[../]
[../]
[] # BCs
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 206800
poissons_ratio = 0.0
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'powerlawcrp'
[../]
[./powerlawcrp]
type = PowerLawCreepStressUpdate
coefficient = 3.125e-21 # 7.04e-17 #
n_exponent = 4.0
m_exponent = 0.0
activation_energy = 0.0
# max_inelastic_increment = 0.01
[../]
[]
[DomainIntegral]
integrals = CIntegral
boundary = 1001
crack_direction_method = CurvedCrackFront
crack_end_direction_method = CrackDirectionVector
crack_direction_vector_end_1 = '0.0 1.0 0.0'
crack_direction_vector_end_2 = '1.0 0.0 0.0'
radius_inner = '12.5 25.0 37.5'
radius_outer = '25.0 37.5 50.0'
intersecting_boundary = '1 2'
symmetry_plane = 2
incremental = true
inelastic_models = 'powerlawcrp'
[]
[Executioner]
type = Transient
# Two sets of linesearch options are for petsc 3.1 and 3.3 respectively
#Preconditioned JFNK (default)
solve_type = 'NEWTON'
# petsc_options = '-snes_ksp_ew'
petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
petsc_options_value = '201 hypre boomeramg 4'
line_search = 'none'
l_max_its = 50
nl_max_its = 20
nl_abs_tol = 1e-3
nl_rel_tol = 1e-11
l_tol = 1e-2
start_time = 0.0
end_time = 401
[./TimeStepper]
type = FunctionDT
function = dts
min_dt = 1.0
[../]
[]
[Postprocessors]
[./_dt]
type = TimestepSize
[../]
[./nl_its]
type = NumNonlinearIterations
[../]
[./lin_its]
type = NumLinearIterations
[../]
[./react_z]
type = NodalSum
variable = resid_z
boundary = 5
[../]
[]
[Outputs]
execute_on = 'timestep_end'
csv = true
[]
(modules/solid_mechanics/test/tests/strain_energy_density/ad_rate_model_weak_plane.i)
# Single element test to check the strain energy density calculation
[GlobalParams]
displacements = 'disp_x disp_y'
volumetric_locking_correction = true
out_of_plane_strain = strain_zz
[]
[Mesh]
type = GeneratedMesh
dim = 2
nx = 1
ny = 1
xmin = 0
xmax = 1
ymin = 0
ymax = 2
[]
[AuxVariables]
[SERD]
order = CONSTANT
family = MONOMIAL
[]
[]
[Variables]
[strain_zz]
[]
[]
[Functions]
[rampConstantUp]
type = PiecewiseLinear
x = '0. 1.'
y = '0. 1.'
scale_factor = -100
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[master]
strain = FINITE
add_variables = true
incremental = true
generate_output = 'stress_xx stress_yy stress_zz vonmises_stress strain_xx strain_yy'
planar_formulation = WEAK_PLANE_STRESS
use_automatic_differentiation = true
[]
[]
[AuxKernels]
[SERD]
type = MaterialRealAux
variable = SERD
property = strain_energy_rate_density
execute_on = timestep_end
[]
[]
[BCs]
[no_x]
type = ADDirichletBC
variable = disp_x
boundary = 'left'
value = 0.0
[]
[no_y]
type = ADDirichletBC
variable = disp_y
boundary = 'bottom'
value = 0.0
[]
[Pressure]
[top]
boundary = 'top'
function = rampConstantUp
[]
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 206800
poissons_ratio = 0.0
[]
[radial_return_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'powerlawcrp'
[]
[powerlawcrp]
type = ADPowerLawCreepStressUpdate
coefficient = 3.125e-21 # 7.04e-17 #
n_exponent = 4.0
m_exponent = 0.0
activation_energy = 0.0
# max_inelastic_increment = 0.01
[]
[strain_energy_rate_density]
type = ADStrainEnergyRateDensity
inelastic_models = 'powerlawcrp'
[]
[]
[Executioner]
type = Transient
petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
petsc_options_value = '201 hypre boomeramg 4'
line_search = 'none'
l_max_its = 50
nl_max_its = 20
nl_abs_tol = 3e-7
nl_rel_tol = 1e-12
l_tol = 1e-2
start_time = 0.0
dt = 1
end_time = 1
num_steps = 1
[]
[Postprocessors]
[SERD]
type = ElementAverageValue
variable = SERD
[]
[]
[Outputs]
csv = true
[]
(modules/solid_mechanics/test/tests/substepping/ad_power_law_creep.i)
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
[gen]
type = GeneratedMeshGenerator
dim = 3
nx = 2
ny = 2
nz = 2
[]
[]
[AuxVariables]
[temp]
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
add_variables = true
generate_output = 'stress_zz elastic_strain_zz creep_strain_zz'
use_automatic_differentiation = true
[]
[]
[Functions]
[front_pull]
type = PiecewiseLinear
x = '0 1'
y = '0 1'
scale_factor = 0.5
[]
[]
[BCs]
[u_front_pull]
type = ADFunctionDirichletBC
variable = disp_z
boundary = front
function = front_pull
[]
[uz_back_fix]
type = ADDirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[u_yz_fix]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xz_fix]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[radial_return_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
[]
[power_law_creep]
type = ADPowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 0.0
temperature = temp
# options for using substepping
substep_strain_tolerance = 0.1
max_inelastic_increment = 0.01
[]
[]
[Executioner]
type = Transient
solve_type = 'NEWTON'
petsc_options_iname = '-pc_type '
petsc_options_value = 'lu '
line_search = 'none'
nl_max_its = 10
nl_rel_tol = 1e-6
nl_abs_tol = 1e-10
end_time = 0.1
dt = 0.1
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/power_law_creep/restart2.i)
# 1x1x1 unit cube with uniform pressure on top face
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Variables]
[temp]
order = FIRST
family = LAGRANGE
initial_condition = 1000.0
[]
[]
[Problem]
allow_initial_conditions_with_restart = true
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = '0 1'
y = '1 1'
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = Pressure
variable = disp_y
boundary = top
factor = -10.0e6
function = top_pull
[]
[u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
tangent_operator = elastic
[]
[power_law_creep]
type = PowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.6
end_time = 1.0
num_steps = 12
dt = 0.1
[]
[Outputs]
# file_base = power_law_creep_out
exodus = true
[]
[Problem]
restart_file_base = restart1_out_cp/0006
[]
(modules/solid_mechanics/test/tests/material_limit_time_step/creep/nafems_test5a_lim.i)
[GlobalParams]
temperature = temp
order = FIRST
family = LAGRANGE
volumetric_locking_correction = true
displacements = 'disp_x disp_y'
[]
[Mesh]
file = plane1_mesh.e
[]
[Problem]
type = ReferenceResidualProblem
extra_tag_vectors = 'ref'
reference_vector = 'ref'
group_variables = 'disp_x disp_y'
[]
[Variables]
[./disp_x]
[../]
[./disp_y]
[../]
[]
[AuxVariables]
[./temp]
initial_condition = 1500.0
[../]
[./creep]
order = CONSTANT
family = MONOMIAL
[../]
[./stress_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./stress_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./stress_zz]
order = CONSTANT
family = MONOMIAL
[../]
[./vonmises]
order = CONSTANT
family = MONOMIAL
[../]
[./pressure]
order = CONSTANT
family = MONOMIAL
[../]
[./invariant3]
order = CONSTANT
family = MONOMIAL
[../]
[./creep_strain_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./creep_strain_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./creep_strain_zz]
order = CONSTANT
family = MONOMIAL
[../]
[./creep_strain_xy]
order = CONSTANT
family = MONOMIAL
[../]
[./elastic_strain_xx]
order = CONSTANT
family = MONOMIAL
[../]
[./elastic_strain_yy]
order = CONSTANT
family = MONOMIAL
[../]
[./elastic_strain_zz]
order = CONSTANT
family = MONOMIAL
[../]
[]
[Kernels]
[SolidMechanics]
use_displaced_mesh = true
extra_vector_tags = 'ref'
[../]
[]
[AuxKernels]
[./creep_aux]
type = MaterialRealAux
property = effective_creep_strain
variable = creep
[../]
[./stress_xx]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_xx
index_i = 0
index_j = 0
[../]
[./stress_yy]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_yy
index_i = 1
index_j = 1
[../]
[./stress_zz]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_zz
index_i = 2
index_j = 2
[../]
[./vonmises]
type = RankTwoScalarAux
rank_two_tensor = stress
variable = vonmises
scalar_type = VonMisesStress
[../]
[./pressure]
type = RankTwoScalarAux
rank_two_tensor = stress
variable = pressure
scalar_type = Hydrostatic
[../]
[./invariant3]
type = RankTwoScalarAux
rank_two_tensor = stress
variable = invariant3
scalar_type = ThirdInvariant
[../]
[./creep_strain_xx]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xx
index_i = 0
index_j = 0
[../]
[./creep_strain_yy]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_yy
index_i = 1
index_j = 1
[../]
[./creep_strain_zz]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_zz
index_i = 2
index_j = 2
[../]
[./creep_strain_xy]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xy
index_i = 0
index_j = 1
[../]
[./elastic_str_xx_aux]
type = RankTwoAux
rank_two_tensor = elastic_strain
variable = elastic_strain_xx
index_i = 0
index_j = 0
[../]
[./elastic_str_yy_aux]
type = RankTwoAux
rank_two_tensor = elastic_strain
variable = elastic_strain_yy
index_i = 1
index_j = 1
[../]
[./elastic_str_zz_aux]
type = RankTwoAux
rank_two_tensor = elastic_strain
variable = elastic_strain_zz
index_i = 2
index_j = 2
[../]
[]
[BCs]
[./bot_y]
type = DirichletBC
variable = disp_y
boundary = 1
value = 0.0
[../]
[./side_x]
type = DirichletBC
variable = disp_x
boundary = 2
value = 0.0
[../]
[./top_press]
type = Pressure
variable = disp_y
boundary = 3
factor = -100.0
[../]
[./side_press]
type = Pressure
variable = disp_x
boundary = 4
factor = -200.0
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
block = 1
youngs_modulus = 200e3
poissons_ratio = 0.3
[../]
[./strain]
type = ComputePlaneFiniteStrain
block = 1
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
block = 1
inelastic_models = 'powerlawcrp'
[../]
[./powerlawcrp]
type = PowerLawCreepStressUpdate
block = 1
coefficient = 3.125e-14
n_exponent = 5.0
m_exponent = 0.0
activation_energy = 0.0
max_inelastic_increment = 0.01
[../]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options_iname = '-pc_type -pc_factor_mat_solver_package'
petsc_options_value = ' lu superlu_dist'
line_search = 'none'
l_max_its = 50
nl_max_its = 100
end_time = 1000.0
num_steps = 10000
l_tol = 1e-3
[./TimeStepper]
type = IterationAdaptiveDT
dt = 1e-6
time_t = '1e-6 2e-6 3e-6 5e-6 9e-6 1.7e-5 3.3e-5 6.5e-5 1.29e-4 2.57e-4 5.13e-4 1.025e-3 2.049e-3 4.097e-3 8.193e-3 1.638e-2 3.276e-2 5.734e-2 0.106 0.180 0.291 0.457 0.706 1.08 1.64 2.48 3.74 5.63 8.46 12.7 19.1 28.7 43.0 64.5 108.0 194.0 366.0 710.0 1000.0'
time_dt = '1e-6 1e-6 2e-6 4e-6 8e-6 1.6e-5 3.2e-5 6.4e-5 1.28e-4 2.56e-4 5.12e-4 1.024e-3 2.048e-3 4.096e-3 8.192e-3 1.6384e-2 2.458e-2 4.915e-2 7.40e-2 0.111 0.166 0.249 0.374 0.560 0.840 1.26 1.89 2.83 4.25 6.40 9.6 14.3 21.5 43.0 86.1 172.0 344.0 290.0 290.0'
optimal_iterations = 30
iteration_window = 9
growth_factor = 2.0
cutback_factor = 0.5
timestep_limiting_postprocessor = matl_ts_min
[../]
[]
[Postprocessors]
[./matl_ts_min]
type = MaterialTimeStepPostprocessor
[../]
[./sigma_xx]
type = ElementAverageValue
variable = stress_xx
[../]
[./sigma_yy]
type = ElementAverageValue
variable = stress_yy
[../]
[./sigma_zz]
type = ElementAverageValue
variable = stress_zz
[../]
[./vonmises]
type = ElementAverageValue
variable = vonmises
[../]
[./pressure]
type = ElementAverageValue
variable = pressure
[../]
[./invariant3]
type = ElementAverageValue
variable = invariant3
[../]
[./eps_crp_xx]
type = ElementAverageValue
variable = creep_strain_xx
[../]
[./eps_crp_yy]
type = ElementAverageValue
variable = creep_strain_yy
[../]
[./eps_crp_zz]
type = ElementAverageValue
variable = creep_strain_zz
[../]
[./eps_crp_mag]
type = ElementAverageValue
variable = creep
[../]
[./disp_x2]
type = NodalVariableValue
nodeid = 1
variable = disp_x
[../]
[./disp_x3]
type = NodalVariableValue
nodeid = 2
variable = disp_x
[../]
[./disp_y3]
type = NodalVariableValue
nodeid = 2
variable = disp_y
[../]
[./disp_y4]
type = NodalVariableValue
nodeid = 3
variable = disp_y
[../]
[./_dt]
type = TimestepSize
[../]
[./elas_str_xx]
type = ElementAverageValue
variable = elastic_strain_xx
[../]
[./elas_str_yy]
type = ElementAverageValue
variable = elastic_strain_yy
[../]
[./elas_str_zz]
type = ElementAverageValue
variable = elastic_strain_zz
[../]
[]
[Outputs]
print_linear_residuals = true
perf_graph = true
csv = true
[./out]
type = Exodus
elemental_as_nodal = true
[../]
[./console]
type = Console
max_rows = 25
[../]
[]
(modules/solid_mechanics/test/tests/ad_anisotropic_creep/ad_aniso_iso_creep_x_3d.i)
[Mesh]
[gen]
type = GeneratedMeshGenerator
dim = 3
nx = 10
ny = 2
nz = 2
xmin = 0.0
ymin = 0.0
zmin = 0.0
xmax = 10.0
ymax = 1.0
zmax = 1.0
[]
[corner_node]
type = ExtraNodesetGenerator
new_boundary = '100'
nodes = '3 69'
input = gen
[]
[corner_node_2]
type = ExtraNodesetGenerator
new_boundary = '101'
nodes = '4 47'
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
[]
[creep_strain_xz]
order = CONSTANT
family = MONOMIAL
[]
[creep_strain_yz]
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_zz
index_i = 2
index_j = 2
[]
[creep_strain_xz]
type = ADRankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xz
index_i = 0
index_j = 2
[]
[creep_strain_yz]
type = ADRankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_yz
index_i = 1
index_j = 2
[]
[sigma_xx]
type = ADRankTwoAux
rank_two_tensor = stress
variable = stress_xx
index_i = 1
index_j = 1
[]
[]
[Functions]
[pull]
type = PiecewiseLinear
x = '0 1.0e-9 1.0'
y = '0 -4e1 -4e1'
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
generate_output = 'elastic_strain_xx stress_xx'
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_iso'
max_iterations = 50
[]
[hill_tensor]
type = ADHillConstants
# F G H L M N
hill_constants = "0.5 0.5 0.5 1.5 1.5 1.5"
[]
[trial_creep_aniso_iso]
type = ADHillCreepStressUpdate
coefficient = 1e-16
n_exponent = 9
m_exponent = 0
activation_energy = 0
max_inelastic_increment = 0.00003
relative_tolerance = 1e-20
absolute_tolerance = 1e-20
internal_solve_output_on = never
# Force it to not use integration error
max_integration_error = 1.0
[]
[trial_creep_iso]
type = ADPowerLawCreepStressUpdate
coefficient = 1e-16
n_exponent = 9
m_exponent = 0
activation_energy = 0
# F G H L M N
max_inelastic_increment = 0.00003
relative_tolerance = 1e-16
absolute_tolerance = 1e-16
internal_solve_output_on = never
[]
[]
[BCs]
[no_disp_x]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[no_disp_y]
type = ADDirichletBC
variable = disp_y
boundary = 100
value = 0.0
[]
[no_disp_z]
type = ADDirichletBC
variable = disp_z
boundary = 101
value = 0.0
[]
[Pressure]
[Side1]
boundary = right
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-13
nl_abs_tol = 1.0e-14
l_max_its = 90
num_steps = 10
dt = 5.0e-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_xx]
type = ElementalVariableValue
variable = creep_strain_xx
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_yy]
type = ElementalVariableValue
variable = creep_strain_yy
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_zz]
type = ElementalVariableValue
variable = creep_strain_zz
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_xy]
type = ElementalVariableValue
variable = creep_strain_xy
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_yz]
type = ElementalVariableValue
variable = creep_strain_yz
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_xz]
type = ElementalVariableValue
variable = creep_strain_xz
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[elastic_strain_xx]
type = ElementalVariableValue
variable = elastic_strain_xx
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[sigma_xx]
type = ElementalVariableValue
variable = stress_xx
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[]
[Outputs]
csv = true
exodus = true
perf_graph = true
[]
(modules/solid_mechanics/test/tests/power_law_creep/cp_power_law_creep.i)
# 1x1x1 unit cube with uniform pressure on top face
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Variables]
[temp]
order = FIRST
family = LAGRANGE
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = '0 1'
y = '1 1'
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = Pressure
variable = disp_y
boundary = top
factor = -10.0e6
function = top_pull
[]
[u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[radial_return_stress]
type = ComputeCreepPlasticityStress
creep_model = power_law_creep
plasticity_model = isotropic_plasticity
tangent_operator = elastic
[]
[power_law_creep]
type = PowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[isotropic_plasticity]
type = IsotropicPlasticityStressUpdate
yield_stress = 1e30
hardening_constant = 0.0
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.0
end_time = 1.0
num_steps = 10
dt = 0.1
[]
[Outputs]
exodus = true
[]
(modules/solid_mechanics/test/tests/ad_plastic/power_law_creep.i)
[Mesh]
type = GeneratedMesh
dim = 2
nx = 2
ny = 2
second_order = true
[]
[GlobalParams]
displacements = 'disp_x disp_y'
volumetric_locking_correction = false
[]
[AuxVariables]
[./hydrostatic_stress]
order = CONSTANT
family = MONOMIAL
[../]
[]
[AuxKernels]
[./hydrostatic_stress]
type = ADRankTwoScalarAux
variable = hydrostatic_stress
rank_two_tensor = stress
scalar_type = Hydrostatic
[../]
[]
[Variables]
[./disp_x]
order = SECOND
scaling = 1e-10
[../]
[./disp_y]
order = SECOND
scaling = 1e-10
[../]
[]
[Functions]
[./pull]
type = PiecewiseLinear
x = '0 10'
y = '0 1e-3'
[../]
[]
[Kernels]
[./stress_x]
type = ADStressDivergenceTensors
component = 0
variable = disp_x
[../]
[./stress_y]
type = ADStressDivergenceTensors
component = 1
variable = disp_y
[../]
[]
[Materials]
[./elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 1e10
poissons_ratio = 0.3
[../]
[./strain]
type = ADComputeIncrementalStrain
[../]
[./elastic_strain]
type = ADComputeMultipleInelasticStress
[../]
[./creep_ten]
type = ADPowerLawCreepStressUpdate
coefficient = 10e-24
n_exponent = 4
activation_energy = 0
base_name = creep_ten
[../]
[./creep_ten2]
type = ADPowerLawCreepStressUpdate
coefficient = 10e-24
n_exponent = 4
activation_energy = 0
base_name = creep_ten2
[../]
[./creep_one]
type = ADPowerLawCreepStressUpdate
coefficient = 1e-24
n_exponent = 4
activation_energy = 0
base_name = creep_one
[../]
[./creep_nine]
type = ADPowerLawCreepStressUpdate
coefficient = 9e-24
n_exponent = 4
activation_energy = 0
base_name = creep_nine
[../]
[./creep_zero]
type = ADPowerLawCreepStressUpdate
coefficient = 0e-24
n_exponent = 4
activation_energy = 0
base_name = creep_zero
[../]
[]
[BCs]
[./no_disp_x]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[../]
[./no_disp_y]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[../]
[./pull_disp_y]
type = ADFunctionDirichletBC
variable = disp_y
boundary = top
function = pull
[../]
[]
[Preconditioning]
[./smp]
type = SMP
full = true
[../]
[]
[Executioner]
type = Transient
petsc_options_iname = -pc_hypre_type
petsc_options_value = boomeramg
line_search = 'none'
nl_rel_tol = 1e-5
num_steps = 5
dt = 1e-1
[]
[Postprocessors]
[./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
[../]
[]
[Outputs]
csv = true
[]
(modules/solid_mechanics/test/tests/ad_anisotropic_creep/aniso_iso_creep_x_3d.i)
[Mesh]
[gen]
type = GeneratedMeshGenerator
dim = 3
nx = 10
ny = 2
nz = 2
xmin = 0.0
ymin = 0.0
zmin = 0.0
xmax = 10.0
ymax = 1.0
zmax = 1.0
[]
[corner_node]
type = ExtraNodesetGenerator
new_boundary = '100'
nodes = '3 69'
input = gen
[]
[corner_node_2]
type = ExtraNodesetGenerator
new_boundary = '101'
nodes = '4 47'
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
[]
[creep_strain_xz]
order = CONSTANT
family = MONOMIAL
[]
[creep_strain_yz]
order = CONSTANT
family = MONOMIAL
[]
[]
[AuxKernels]
[hydrostatic_stress]
type = RankTwoScalarAux
variable = hydrostatic_stress
rank_two_tensor = stress
scalar_type = Hydrostatic
[]
[creep_strain_xx]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xx
index_i = 0
index_j = 0
[]
[creep_strain_xy]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xy
index_i = 0
index_j = 1
[]
[creep_strain_yy]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_yy
index_i = 1
index_j = 1
[]
[creep_strain_zz]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_zz
index_i = 2
index_j = 2
[]
[creep_strain_xz]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xz
index_i = 0
index_j = 2
[]
[creep_strain_yz]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_yz
index_i = 1
index_j = 2
[]
[sigma_xx]
type = RankTwoAux
rank_two_tensor = stress
variable = stress_xx
index_i = 1
index_j = 1
[]
[]
[Functions]
[pull]
type = PiecewiseLinear
x = '0 1.0e-9 1.0'
y = '0 -4e1 -4e1'
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
generate_output = 'elastic_strain_xx stress_xx'
add_variables = true
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 700
poissons_ratio = 0.0
[]
[elastic_strain]
type = ComputeMultipleInelasticStress
# inelastic_models = 'trial_creep_iso'
max_iterations = 50
[]
[hill_tensor]
type = HillConstants
# F G H L M N
hill_constants = "0.5 0.5 0.5 1.5 1.5 1.5"
[]
[trial_creep_aniso_iso]
type = HillCreepStressUpdate
coefficient = 1e-16
n_exponent = 9
m_exponent = 0
activation_energy = 0
max_inelastic_increment = 0.00003
relative_tolerance = 1e-20
absolute_tolerance = 1e-20
internal_solve_output_on = never
# Force it to not use integration error
max_integration_error = 1.0
[]
[trial_creep_iso]
type = PowerLawCreepStressUpdate
coefficient = 1e-16
n_exponent = 9
m_exponent = 0
activation_energy = 0
# F G H L M N
max_inelastic_increment = 0.00003
relative_tolerance = 1e-16
absolute_tolerance = 1e-16
internal_solve_output_on = never
[]
[]
[BCs]
[no_disp_x]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[no_disp_y]
type = DirichletBC
variable = disp_y
boundary = 100
value = 0.0
[]
[no_disp_z]
type = DirichletBC
variable = disp_z
boundary = 101
value = 0.0
[]
[Pressure]
[Side1]
boundary = right
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-13
nl_abs_tol = 1.0e-14
l_max_its = 90
num_steps = 10
dt = 5.0e-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_xx]
type = ElementalVariableValue
variable = creep_strain_xx
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_yy]
type = ElementalVariableValue
variable = creep_strain_yy
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_zz]
type = ElementalVariableValue
variable = creep_strain_zz
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_xy]
type = ElementalVariableValue
variable = creep_strain_xy
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_yz]
type = ElementalVariableValue
variable = creep_strain_yz
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[creep_strain_xz]
type = ElementalVariableValue
variable = creep_strain_xz
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[elastic_strain_xx]
type = ElementalVariableValue
variable = elastic_strain_xx
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[sigma_xx]
type = ElementalVariableValue
variable = stress_xx
execute_on = 'TIMESTEP_END'
elementid = 39
[]
[]
[Outputs]
csv = true
exodus = true
perf_graph = true
[]
(modules/solid_mechanics/test/tests/ad_anisotropic_creep/anis_mech_hill_tensor_creep.i)
[Mesh]
type = GeneratedMesh
dim = 2
nx = 128
ny = 128
second_order = true
[]
[GlobalParams]
displacements = 'disp_x disp_y'
volumetric_locking_correction = false
[]
[AuxVariables]
[hydrostatic_stress]
order = CONSTANT
family = MONOMIAL
[]
[]
[AuxKernels]
[hydrostatic_stress]
type = ADRankTwoScalarAux
variable = hydrostatic_stress
rank_two_tensor = stress
scalar_type = Hydrostatic
[]
[]
[Variables]
[disp_x]
order = SECOND
scaling = 1e-10
[]
[disp_y]
order = SECOND
scaling = 1e-10
[]
[]
[Functions]
[pull]
type = PiecewiseLinear
x = '0 10e3'
y = '0 1e-4'
[]
[]
[Kernels]
[stress_x]
type = ADStressDivergenceTensors
component = 0
variable = disp_x
[]
[stress_y]
type = ADStressDivergenceTensors
component = 1
variable = disp_y
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
add_variables = true
generate_output = 'elastic_strain_xx elastic_strain_yy elastic_strain_xy'
use_automatic_differentiation = true
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeElasticityTensor
fill_method = orthotropic
C_ijkl = '2.0e3 2.0e5 2.0e3 0.71428571e3 0.71428571e3 0.71428571e3 0.4 0.2 0.004 0.004 0.2 0.4'
[]
[elastic_strain]
type = ADComputeMultipleInelasticStress
inelastic_models = "trial_creep"
max_iterations = 300
[]
[hill_tensor]
type = HillConstants
# F G H L M N
hill_constants = "0.5 0.5 0.3866 1.6413 1.6413 1.2731"
base_name = trial_creep
[]
[trial_creep]
type = ADHillCreepStressUpdate
coefficient = 1e-24
n_exponent = 4
m_exponent = 0
activation_energy = 0
# internal_solve_output_on = always
base_name = trial_creep
[]
[creep_one]
type = ADPowerLawCreepStressUpdate
coefficient = 1e-24
n_exponent = 4
activation_energy = 0
base_name = creep_one
[]
[creep_nine]
type = ADPowerLawCreepStressUpdate
coefficient = 9e-24
n_exponent = 4
activation_energy = 0
base_name = creep_nine
[]
[]
[BCs]
[no_disp_x]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[no_disp_y]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[pull_disp_y]
type = ADFunctionDirichletBC
variable = disp_y
boundary = top
function = pull
[]
[]
[Preconditioning]
[smp]
type = SMP
full = true
[]
[]
[Executioner]
type = Transient
solve_type = Newton
petsc_options_iname = '-ksp_gmres_restart -pc_type -sub_pc_type'
petsc_options_value = '101 asm lu'
line_search = 'none'
nl_rel_tol = 1e-5
nl_abs_tol = 1.0e-13
num_steps = 200
dt = 1.0e2
automatic_scaling = true
[]
[Postprocessors]
[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
[]
[]
[Outputs]
csv = true
exodus = true
[]
(modules/solid_mechanics/test/tests/power_law_creep/restart1.i)
# 1x1x1 unit cube with uniform pressure on top face
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
[]
[Variables]
[temp]
order = FIRST
family = LAGRANGE
initial_condition = 1000.0
[]
[]
[Problem]
allow_initial_conditions_with_restart = true
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
incremental = true
add_variables = true
generate_output = 'stress_yy creep_strain_xx creep_strain_yy creep_strain_zz elastic_strain_yy'
[]
[]
[Functions]
[top_pull]
type = PiecewiseLinear
x = '0 1'
y = '1 1'
[]
[]
[Kernels]
[heat]
type = Diffusion
variable = temp
[]
[heat_ie]
type = TimeDerivative
variable = temp
[]
[]
[BCs]
[u_top_pull]
type = Pressure
variable = disp_y
boundary = top
factor = -10.0e6
function = top_pull
[]
[u_bottom_fix]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[u_yz_fix]
type = DirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xy_fix]
type = DirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[temp_fix]
type = DirichletBC
variable = temp
boundary = 'bottom top'
value = 1000.0
[]
[]
[Materials]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[radial_return_stress]
type = ComputeMultipleInelasticStress
tangent_operator = elastic
inelastic_models = 'power_law_creep'
[]
[power_law_creep]
type = PowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 3.0e5
temperature = temp
[]
[]
[Executioner]
type = Transient
solve_type = 'PJFNK'
petsc_options = '-snes_ksp'
petsc_options_iname = '-ksp_gmres_restart'
petsc_options_value = '101'
line_search = 'none'
l_max_its = 20
nl_max_its = 20
nl_rel_tol = 1e-6
nl_abs_tol = 1e-6
l_tol = 1e-5
start_time = 0.0
end_time = 1.0
num_steps = 6
dt = 0.1
[]
[Outputs]
exodus = true
[out]
type = Checkpoint
num_files = 1
[]
[]
(modules/solid_mechanics/test/tests/ad_return_mapping/ad_return_mapping_derivative.i)
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
[gen]
type = GeneratedMeshGenerator
dim = 3
nx = 2
ny = 2
nz = 2
[]
[]
[AuxVariables]
[temp]
initial_condition = 1000.0
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = FINITE
add_variables = true
generate_output = 'stress_zz elastic_strain_zz creep_strain_zz'
use_automatic_differentiation = true
scaling = 1.06364e-11
[]
[]
[Functions]
[front_pull]
type = PiecewiseLinear
x = '0 1'
y = '0 1'
scale_factor = 0.5
[]
[]
[BCs]
[u_front_pull]
type = ADFunctionDirichletBC
variable = disp_z
boundary = front
function = front_pull
[]
[uz_back_fix]
type = ADDirichletBC
variable = disp_z
boundary = back
value = 0.0
[]
[u_yz_fix]
type = ADDirichletBC
variable = disp_x
boundary = left
value = 0.0
[]
[u_xz_fix]
type = ADDirichletBC
variable = disp_y
boundary = bottom
value = 0.0
[]
[]
[Materials]
[elasticity_tensor]
type = ADComputeIsotropicElasticityTensor
youngs_modulus = 2e11
poissons_ratio = 0.3
[]
[radial_return_stress]
type = ADComputeMultipleInelasticStress
inelastic_models = 'power_law_creep'
[]
[power_law_creep]
type = ADPowerLawCreepStressUpdate
coefficient = 1.0e-15
n_exponent = 4
activation_energy = 0.0
temperature = temp
# options for using substepping
use_substepping = INCREMENT_BASED
substep_strain_tolerance = 0.1
max_inelastic_increment = 0.01
automatic_differentiation_return_mapping = true
[]
[]
[Executioner]
type = Transient
solve_type = 'NEWTON'
petsc_options_iname = '-pc_type '
petsc_options_value = 'lu '
line_search = 'none'
nl_max_its = 10
nl_rel_tol = 1e-10
nl_abs_tol = 1e-10
end_time = 0.1
dt = 0.1
[]
[Outputs]
exodus = true
file_base = reference
[]
(modules/solid_mechanics/test/tests/strain_energy_density/rate_model_small.i)
# Single element test to check the strain energy density calculation
[GlobalParams]
displacements = 'disp_x disp_y'
volumetric_locking_correction = true
[]
[Mesh]
type = GeneratedMesh
dim = 2
nx = 1
ny = 1
xmin = 0
xmax = 1
ymin = 0
ymax = 2
[]
[AuxVariables]
[./SERD]
order = CONSTANT
family = MONOMIAL
[../]
[]
[Functions]
[./rampConstantUp]
type = PiecewiseLinear
x = '0. 1.'
y = '0. 1.'
scale_factor = -100
[../]
[./ramp_disp_y]
type = PiecewiseLinear
x = '0. 1. 2.'
y = '0. 6.8e-6 1.36e-5'
[../]
[]
[Physics/SolidMechanics/QuasiStatic]
[./master]
strain = SMALL
add_variables = true
incremental = true
generate_output = 'stress_xx stress_yy stress_zz vonmises_stress elastic_strain_xx elastic_strain_yy elastic_strain_zz strain_xx strain_yy strain_zz'
planar_formulation = PLANE_STRAIN
[../]
[]
[AuxKernels]
[./SERD]
type = MaterialRealAux
variable = SERD
property = strain_energy_rate_density
execute_on = timestep_end
[../]
[]
[BCs]
[./no_x]
type = DirichletBC
variable = disp_x
preset = false
boundary = 'left'
value = 0.0
[../]
[./no_y]
type = DirichletBC
variable = disp_y
preset = false
boundary = 'bottom'
value = 0.0
[../]
[./top_disp]
type = FunctionDirichletBC
variable = disp_y
preset = false
boundary = 'top'
function = ramp_disp_y
[../]
[]
[Materials]
[./elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 206800
poissons_ratio = 0.0
[../]
[./radial_return_stress]
type = ComputeMultipleInelasticStress
inelastic_models = 'powerlawcrp'
[../]
[./powerlawcrp]
type = PowerLawCreepStressUpdate
coefficient = 3.125e-21 # 7.04e-17 #
n_exponent = 4.0
m_exponent = 0.0
activation_energy = 0.0
# max_inelastic_increment = 0.01
[../]
[./strain_energy_rate_density]
type = StrainEnergyRateDensity
inelastic_models = 'powerlawcrp'
[../]
[]
[Executioner]
type = Transient
petsc_options_iname = '-ksp_gmres_restart -pc_type -pc_hypre_type -pc_hypre_boomeramg_max_iter'
petsc_options_value = '201 hypre boomeramg 4'
line_search = 'none'
l_max_its = 50
nl_max_its = 20
nl_abs_tol = 3e-7
nl_rel_tol = 1e-12
l_tol = 1e-2
start_time = 0.0
dt = 1
end_time = 2
num_steps = 2
[]
[Postprocessors]
[./etxx]
type = ElementalVariableValue
variable = strain_xx
elementid = 0
[../]
[./etyy]
type = ElementalVariableValue
variable = strain_yy
elementid = 0
[../]
[./etzz]
type = ElementalVariableValue
variable = strain_zz
elementid = 0
[../]
[./sigxx]
type = ElementAverageValue
variable = stress_xx
[../]
[./sigyy]
type = ElementAverageValue
variable = stress_yy
[../]
[./sigzz]
type = ElementAverageValue
variable = stress_zz
[../]
[./SERD]
type = ElementAverageValue
variable = SERD
[../]
[]
[Outputs]
csv = true
[]
(modules/contact/test/tests/mortar_dynamics/block-dynamics-friction-creep.i)
starting_point = 1e-1
offset = -0.095
[GlobalParams]
displacements = 'disp_x disp_y'
[]
[Mesh]
file = long-bottom-block-1elem-blocks.e
[]
[Variables]
[normal_lm]
block = 3
use_dual = true
[]
[frictional_lm]
block = 3
use_dual = true
[]
[]
[AuxVariables]
[creep_strain_xx]
order = CONSTANT
family = MONOMIAL
block = '2'
[]
[creep_strain_yy]
order = CONSTANT
family = MONOMIAL
block = '2'
[]
[creep_strain_xy]
order = CONSTANT
family = MONOMIAL
block = '2'
[]
[]
[AuxKernels]
[creep_strain_xx]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xx
index_i = 0
index_j = 0
block = '2'
[]
[creep_strain_yy]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_yy
index_i = 1
index_j = 1
block = '2'
[]
[creep_strain_xy]
type = RankTwoAux
rank_two_tensor = creep_strain
variable = creep_strain_xy
index_i = 0
index_j = 1
block = '2'
[]
[]
[ICs]
[disp_y]
block = 2
variable = disp_y
value = '${fparse starting_point + offset}'
type = ConstantIC
[]
[]
[Physics/SolidMechanics/Dynamic]
[all]
add_variables = true
hht_alpha = 0.0
newmark_beta = 0.25
newmark_gamma = 0.5
mass_damping_coefficient = 0.0
stiffness_damping_coefficient = 0.01
displacements = 'disp_x disp_y'
generate_output = 'stress_xx stress_yy'
block = '1 2'
strain = FINITE
[]
[]
[Materials]
[elasticity_2]
type = ComputeIsotropicElasticityTensor
block = '2'
youngs_modulus = 1e6
poissons_ratio = 0.3
[]
[elasticity_1]
type = ComputeIsotropicElasticityTensor
block = '1'
youngs_modulus = 1e8
poissons_ratio = 0.3
[]
[multiple_inelastic]
type = ComputeMultipleInelasticStress
inelastic_models = 'creep'
block = '2'
[]
[creep]
type = PowerLawCreepStressUpdate
coefficient = 1.0e-23 # 10e-24
n_exponent = 4
activation_energy = 0
block = '2'
[]
[stress]
type = ComputeFiniteStrainElasticStress
block = '1'
[]
[density]
type = GenericConstantMaterial
block = '1 2'
prop_names = 'density'
prop_values = '775'
[]
[]
# User object provides the contact force (e.g. LM)
# for the application of the generalized force
[UserObjects]
[weighted_vel_uo]
type = LMWeightedVelocitiesUserObject
primary_boundary = 20
secondary_boundary = 10
primary_subdomain = 4
secondary_subdomain = 3
lm_variable_normal = normal_lm
lm_variable_tangential_one = frictional_lm
secondary_variable = disp_x
disp_x = disp_x
disp_y = disp_y
[]
[]
[Constraints]
[weighted_gap_lm]
type = ComputeDynamicFrictionalForceLMMechanicalContact
primary_boundary = 20
secondary_boundary = 10
primary_subdomain = 4
secondary_subdomain = 3
variable = normal_lm
friction_lm = frictional_lm
disp_x = disp_x
disp_y = disp_y
use_displaced_mesh = true
c = 1e4
c_t = 1e4
mu = 0.5
interpolate_normals = false
newmark_beta = 0.25
newmark_gamma = 0.5
capture_tolerance = 1e-04
[]
[normal_x]
type = NormalMortarMechanicalContact
primary_boundary = 20
secondary_boundary = 10
primary_subdomain = 4
secondary_subdomain = 3
variable = normal_lm
secondary_variable = disp_x
component = x
use_displaced_mesh = true
compute_lm_residuals = false
weighted_gap_uo = weighted_vel_uo
[]
[normal_y]
type = NormalMortarMechanicalContact
primary_boundary = 20
secondary_boundary = 10
primary_subdomain = 4
secondary_subdomain = 3
variable = normal_lm
secondary_variable = disp_y
component = y
use_displaced_mesh = true
compute_lm_residuals = false
weighted_gap_uo = weighted_vel_uo
[]
[tangential_x]
type = TangentialMortarMechanicalContact
primary_boundary = 20
secondary_boundary = 10
primary_subdomain = 4
secondary_subdomain = 3
variable = frictional_lm
secondary_variable = disp_x
component = x
use_displaced_mesh = true
compute_lm_residuals = false
weighted_velocities_uo = weighted_vel_uo
[]
[tangential_y]
type = TangentialMortarMechanicalContact
primary_boundary = 20
secondary_boundary = 10
primary_subdomain = 4
secondary_subdomain = 3
variable = frictional_lm
secondary_variable = disp_y
component = y
use_displaced_mesh = true
compute_lm_residuals = false
weighted_velocities_uo = weighted_vel_uo
[]
[]
[BCs]
[botx]
type = DirichletBC
variable = disp_x
boundary = 40
value = 0.0
[]
[boty]
type = DirichletBC
variable = disp_y
boundary = 40
value = 0.0
[]
[topy]
type = FunctionDirichletBC
variable = disp_y
boundary = 30
function = '${starting_point} * cos(2 * pi / 4 * t) + ${offset}'
[]
[leftx]
type = FunctionDirichletBC
variable = disp_x
boundary = 30 # 50
function = '1e-2*t' #'0.1 *sin(2 * pi / 12 * t)'
[]
[]
[Executioner]
type = Transient
end_time = 0.25
dt = 0.05
dtmin = 0.05
solve_type = 'PJFNK'
petsc_options = '-snes_converged_reason -ksp_converged_reason -pc_svd_monitor '
'-snes_linesearch_monitor -snes_ksp_ew'
petsc_options_iname = '-pc_type -pc_factor_shift_type -pc_factor_shift_amount -mat_mffd_err '
petsc_options_value = 'lu NONZERO 1e-15 1e-5'
nl_max_its = 50
line_search = 'none'
snesmf_reuse_base = false
[TimeIntegrator]
type = NewmarkBeta
beta = 0.25
gamma = 0.5
[]
[]
[Debug]
show_var_residual_norms = true
[]
[Outputs]
exodus = true
checkpoint = true
[]
[Preconditioning]
[smp]
type = SMP
full = true
[]
[]
[Postprocessors]
active = 'num_nl cumulative contact'
[num_nl]
type = NumNonlinearIterations
[]
[cumulative]
type = CumulativeValuePostprocessor
postprocessor = num_nl
[]
[contact]
type = ContactDOFSetSize
variable = normal_lm
subdomain = '3'
execute_on = 'nonlinear timestep_end'
[]
[]
(modules/solid_mechanics/test/tests/scalar_material_damage/scalar_material_damage_creep_power.i)
# This is a basic test of the system for continuum damage mechanics
# materials. It uses ScalarMaterialDamage for the damage model,
# which simply gets its damage index from another material. In this
# case, we prescribe the evolution of the damage index using a
# function. A single element has a fixed prescribed displacement
# on one side that puts the element in tension, and then the
# damage index evolves from 0 to 1 over time, and this verifies
# that the stress correspondingly drops to 0.
[GlobalParams]
displacements = 'disp_x disp_y disp_z'
[]
[Mesh]
type = GeneratedMesh
dim = 3
nx = 1
ny = 1
nz = 1
elem_type = HEX8
[]
[AuxVariables]
[damage_index]
order = CONSTANT
family = MONOMIAL
[]
[]
[Physics/SolidMechanics/QuasiStatic]
[all]
strain = SMALL
incremental = true
add_variables = true
generate_output = 'stress_xx strain_xx creep_strain_xx'
[]
[]
[AuxKernels]
[damage_index]
type = MaterialRealAux
variable = damage_index
property = damage_index_prop
execute_on = timestep_end
[]
[]
[BCs]
[symmy]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0
[]
[symmx]
type = DirichletBC
variable = disp_x
boundary = left
value = 0
[]
[symmz]
type = DirichletBC
variable = disp_z
boundary = back
value = 0
[]
[axial_load]
type = DirichletBC
variable = disp_x
boundary = right
value = 0.01
[]
[]
[Functions]
[damage_evolution]
type = PiecewiseLinear
xy_data = '0.0 0.0
0.1 0.0
2.1 2.0'
[]
[]
[Materials]
[damage_index]
type = GenericFunctionMaterial
prop_names = damage_index_prop
prop_values = damage_evolution
[]
[damage]
type = ScalarMaterialDamage
damage_index = damage_index_prop
[]
[stress]
type = ComputeMultipleInelasticStress
damage_model = damage
inelastic_models = 'creep'
[]
[elasticity_tensor]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 140000
poissons_ratio = 0.3
[]
[creep]
type = PowerLawCreepStressUpdate
coefficient = 1.1e-12 #
n_exponent = 8.7
m_exponent = 0
activation_energy = 0.0
[]
[]
[Postprocessors]
[stress_xx]
type = ElementAverageValue
variable = stress_xx
[]
[strain_xx]
type = ElementAverageValue
variable = strain_xx
[]
[creep_strain_xx]
type = ElementAverageValue
variable = creep_strain_xx
[]
[damage_index]
type = ElementAverageValue
variable = damage_index
[]
[]
[Preconditioning]
[smp]
type = SMP
full = true
[]
[]
[Executioner]
type = Transient
l_max_its = 50
l_tol = 1e-8
nl_max_its = 20
nl_rel_tol = 1e-10
nl_abs_tol = 1e-8
dt = 0.1
dtmin = 0.001
end_time = 1.1
[]
[Outputs]
csv = true
[]