Abaqus UMAT Stress

Coupling material to use Abaqus UMAT models in MOOSE

Description

AbaqusUMATStress provides an interface for using _Abaqus UMAT_ functions as constitutive models in MOOSE.

UMAT User subroutine interface

UMAT functions are commonly coded in Fortran, are located in the $(APPLICATION_DIR)/plugins and $(APPLICATION_DIR)/test/plugins directories, and are automatically compiled by the MOOSE build system.

A UMAT file my_umat.f can be loaded by the AbaqusUMATStress by providing the the full path and filename without an extension via the "plugin" parameter in the MOOSE input file.

A valid UMAT subroutine has the following call signature


SUBROUTINE UMAT(STRESS,STATEV,DDSDDE,SSE,SPD,SCD,
     1 RPL,DDSDDT,DRPLDE,DRPLDT,
     2 STRAN,DSTRAN,TIME,DTIME,TEMP,DTEMP,PREDEF,DPRED,CMNAME,
     3 NDI,NSHR,NTENS,NSTATV,PROPS,NPROPS,COORDS,DROT,PNEWDT,
     4 CELENTCELENT,DFGRD0,DFGRD1,NOEL,NPT,LAYER,KSPT,KSTEP,KINC)
C
      CHARACTER*80 CMNAME
      DIMENSION STRESS(NTENS),STATEV(NSTATV),
     1 DDSDDE(NTENS,NTENS),DDSDDT(NTENS),DRPLDE(NTENS),
     2 STRAN(NTENS),DSTRAN(NTENS),TIME(2),PREDEF(1),DPRED(1),
     3 PROPS(NPROPS),COORDS(3),DROT(3,3),DFGRD0(3,3),DFGRD1(3,3)


      user coding to define DDSDDE, STRESS, STATEV, SSE, SPD, SCD
      and, if necessary, RPL, DDSDDT, DRPLDE, DRPLDT, PNEWDT


      RETURN
      END

A description of the input and output parameters of the UMAT user subroutines can be found in the Abaqus user manual.

Note that the UMAT standard uses 1-based indexing for NOEL (element number) and NPT (integration point number), while MOOSE uses 0-based indexing internally. We therefore add one to the element and integration point numbers from MOOSE before passing them to the UMAT.

UMAT Time step control

Time step control within the UMAT subroutine is used together with MOOSE's general capabilities to control time steps based on material behavior. PNEWDT denotes a factor that can be modified in the UMAT routine to be less than one, to signal a cut in the time step, or more than one, to signal a local increment in the time step. Since these time step controls are local to the quadrature point, MOOSE provides a layer of objects to handle the information provided by UMAT's PNEWDT. First, we select a soft Terminator which will invalidate a time step if the time step increment used turns out to be larger than a computed maximum time step increment anywhere in the system:

[UserObjects]
  [time_step_size]
    type = TimestepSize
    execute_on = 'INITIAL LINEAR'
  []
  [terminator_umat]
    type = Terminator
    expression = 'time_step_size > matl_ts_min'
    fail_mode = SOFT
    execute_on = 'FINAL'
  []
[]

As a second step, we select the time stepper controls for the entire finite element system. These controls will apply to UMAT stepping as well as any other kernel or object in the system:

[Executioner]
  [TimeStepper]
    type = IterationAdaptiveDT
    optimal_iterations = 30
    iteration_window = 9
    growth_factor = 2.0
    cutback_factor = 1.0
    timestep_limiting_postprocessor = matl_ts_min
    dt = 1.0
  []
[]

The time step increment will be reduced as prescribed in the UMAT routine. However, the maximum increment will be limited by the selection of growth_factor. This avoids increasing the time step too much from one time step to the next. To further rely on UMAT's PNEWDT, one can choose to select a larger growth_factor.

A subroutine that acts on PNEWDT is chosen in the regression test:

[Materials]
  [umat]
    type = AbaqusUMATStress
    constant_properties = '1000 0.3'
    plugin = '../../../plugins/elastic_timestep'
    num_state_vars = 0
    use_one_based_indexing = true
  []
[]

UMAT Loading steps

When setting up an input file, it can be useful to organize it in terms of the loading and boundary conditions that the structural component will undergo throughout the numerical simulation. For example, a user may want to apply natural boundary conditions as a first step (Step 1), then apply gradually a permanent or long-term load, e.g. the internal pressure in a vessel (Step 2). Finally, other loads, such as those originated by wind, can be added to the existing step to obtain the desired final numerical results (Step 3). For this case, MOOSE steps need to be defined throughout the simulation in StepUserObject. This user object can be passed to AbaqusUMATStress to inform the UMAT routine of the value of step time at the beginning of the current increment (TIME(1) with Fortran indexing).

An example of how to pass the user object in an input file is given below:

[Materials]
  [umat]
    type = AbaqusUMATStress
    constant_properties = '1000 0.3'
    plugin = '../../../plugins/elastic_temperature'
    num_state_vars = 0
    temperature = temperature
    use_one_based_indexing = true
  []
[]

Note that the step capability is three-pronged: 1) It allows to pass the step number to the UMAT routine via the present object, 2) It allows to pass the step number to the AbaqusUExternalDB plugin, and 3) It allows to directly drive controls via step number in StepPeriod.

Example input file

[Materials]
  [constant]
    type = AbaqusUMATStress
    #                      Young's modulus,  Poisson's Ratio, Yield, Hardening
    constant_properties = '1000 0.3 10 100'
    plugin = ../../../plugins/linear_strain_hardening
    num_state_vars = 3
    use_one_based_indexing = true
  []
[]

Input Parameters

constant_propertiesConstant mechanical and thermal material properties (PROPS)
C++ Type:std::vector<double>
Unit:(no unit assumed)
Controllable:No
Description:Constant mechanical and thermal material properties (PROPS)
num_state_varsThe number of state variables this UMAT is going to use
C++ Type:unsigned int
Unit:(no unit assumed)
Controllable:No
Description:The number of state variables this UMAT is going to use
pluginThe path to the compiled dynamic library for the plugin you want to use
C++ Type:FileName
Unit:(no unit assumed)
Controllable:No
Description:The path to the compiled dynamic library for the plugin you want to use
use_one_based_indexingFalseParameter to control whether indexing for element and integration points as presented to UMAT models is based on 1 (true) or 0 (false). This does not affect internal MOOSE numbering. The option to use 0-based numbering is deprecated and will be removed soon.
Default:False
C++ Type:bool
Unit:(no unit assumed)
Controllable:No
Description:Parameter to control whether indexing for element and integration points as presented to UMAT models is based on 1 (true) or 0 (false). This does not affect internal MOOSE numbering. The option to use 0-based numbering is deprecated and will be removed soon.

Required Parameters

base_nameOptional parameter that allows the user to define multiple mechanics material systems on the same block, i.e. for multiple phases
C++ Type:std::string
Unit:(no unit assumed)
Controllable:No
Description:Optional parameter that allows the user to define multiple mechanics material systems on the same block, i.e. for multiple phases
blockThe list of blocks (ids or names) that this object will be applied
C++ Type:std::vector<SubdomainName>
Unit:(no unit assumed)
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>
Unit:(no unit assumed)
Controllable:No
Description:The list of boundaries (ids or names) from the mesh where this object applies
computeTrueWhen false, MOOSE will not call compute methods on this material. The user must call computeProperties() after retrieving the MaterialBase via MaterialBasePropertyInterface::getMaterialBase(). Non-computed MaterialBases are not sorted for dependencies.
Default:True
C++ Type:bool
Unit:(no unit assumed)
Controllable:No
Description:When false, MOOSE will not call compute methods on this material. The user must call computeProperties() after retrieving the MaterialBase via MaterialBasePropertyInterface::getMaterialBase(). Non-computed MaterialBases are not sorted for dependencies.
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
Unit:(no unit assumed)
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.
decomposition_methodTaylorExpansionMethod to calculate the strain kinematics.
Default:TaylorExpansion
C++ Type:MooseEnum
Unit:(no unit assumed)
Options:TaylorExpansion, EigenSolution, HughesWinget
Controllable:No
Description:Method to calculate the strain kinematics.
external_fieldsThe external fields that can be used in the UMAT subroutine
C++ Type:std::vector<VariableName>
Unit:(no unit assumed)
Controllable:No
Description:The external fields that can be used in the UMAT subroutine
external_properties
C++ Type:std::vector<MaterialPropertyName>
Unit:(no unit assumed)
Controllable:No
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.
step_user_objectThe StepUserObject that provides times from simulation loading steps.
C++ Type:UserObjectName
Unit:(no unit assumed)
Controllable:No
Description:The StepUserObject that provides times from simulation loading steps.
temperatureCoupled temperature
C++ Type:std::vector<VariableName>
Unit:(no unit assumed)
Controllable:No
Description:Coupled temperature
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
Unit:(no unit assumed)
Controllable:No
Description:For the old and older state use projected material properties interpolated at the quadrature points. To set up projection use the ProjectedStatefulMaterialStorageAction.

Optional Parameters

control_tagsAdds user-defined labels for accessing object parameters via control logic.
C++ Type:std::vector<std::string>
Unit:(no unit assumed)
Controllable:No
Description:Adds user-defined labels for accessing object parameters via control logic.
enableTrueSet the enabled status of the MooseObject.
Default:True
C++ Type:bool
Unit:(no unit assumed)
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
Unit:(no unit assumed)
Controllable:No
Description:Determines whether this object is calculated using an implicit or explicit form
seed0The seed for the master random number generator
Default:0
C++ Type:unsigned int
Unit:(no unit assumed)
Controllable:No
Description:The seed for the master random number generator
use_displaced_meshFalseWhether or not this object should use the displaced mesh for computing displacements and quantities based on the deformed state.
Default:False
C++ Type:bool
Unit:(no unit assumed)
Controllable:No
Description:Whether or not this object should use the displaced mesh for computing displacements and quantities based on the deformed state.

Advanced Parameters

output_propertiesList of material properties, from this material, to output (outputs must also be defined to an output type)
C++ Type:std::vector<std::string>
Unit:(no unit assumed)
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>
Unit:(no unit assumed)
Controllable:No
Description:Vector of output names where you would like to restrict the output of variables(s) associated with this object

Outputs Parameters

References

No citations exist within this document.

(moose/modules/solid_mechanics/test/tests/umat/time_step/elastic_timestep.i)

# Testing the UMAT Interface - linear elastic model using the large strain formulation.

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

[Mesh]
  [gen]
    type = GeneratedMeshGenerator
    dim = 3
    xmin = -0.5
    xmax = 0.5
    ymin = -0.5
    ymax = 0.5
    zmin = -0.5
    zmax = 0.5
  []
[]

[Functions]
  [top_pull]
    type = ParsedFunction
    expression = t/100
  []
[]

[Physics/SolidMechanics/QuasiStatic]
  [all]
    add_variables = true
    strain = FINITE
  []
[]

[BCs]
  [y_pull_function]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = top
    function = top_pull
  []
  [x_bot]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0.0
  []
  [y_bot]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0.0
  []
  [z_bot]
    type = DirichletBC
    variable = disp_z
    boundary = front
    value = 0.0
  []
[]

[Materials]
  [umat]
    type = AbaqusUMATStress
    constant_properties = '1000 0.3'
    plugin = '../../../plugins/elastic_timestep'
    num_state_vars = 0
    use_one_based_indexing = 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 = 100
  nl_max_its = 100
  nl_rel_tol = 1e-12
  nl_abs_tol = 1e-10
  l_tol = 1e-9
  start_time = 0.0
  end_time = 30

  [TimeStepper]
    type = IterationAdaptiveDT
    optimal_iterations = 30
    iteration_window = 9
    growth_factor = 2.0
    cutback_factor = 1.0
    timestep_limiting_postprocessor = matl_ts_min
    dt = 1.0
  []
[]

[UserObjects]
  [time_step_size]
    type = TimestepSize
    execute_on = 'INITIAL LINEAR'
  []
  [terminator_umat]
    type = Terminator
    expression = 'time_step_size > matl_ts_min'
    fail_mode = SOFT
    execute_on = 'FINAL'
  []
[]

[Postprocessors]
  [matl_ts_min]
    type = MaterialTimeStepPostprocessor
  []
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Outputs]
  exodus = true
[]

(moose/modules/solid_mechanics/test/tests/umat/time_step/elastic_timestep.i)

# Testing the UMAT Interface - linear elastic model using the large strain formulation.

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

[Mesh]
  [gen]
    type = GeneratedMeshGenerator
    dim = 3
    xmin = -0.5
    xmax = 0.5
    ymin = -0.5
    ymax = 0.5
    zmin = -0.5
    zmax = 0.5
  []
[]

[Functions]
  [top_pull]
    type = ParsedFunction
    expression = t/100
  []
[]

[Physics/SolidMechanics/QuasiStatic]
  [all]
    add_variables = true
    strain = FINITE
  []
[]

[BCs]
  [y_pull_function]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = top
    function = top_pull
  []
  [x_bot]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0.0
  []
  [y_bot]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0.0
  []
  [z_bot]
    type = DirichletBC
    variable = disp_z
    boundary = front
    value = 0.0
  []
[]

[Materials]
  [umat]
    type = AbaqusUMATStress
    constant_properties = '1000 0.3'
    plugin = '../../../plugins/elastic_timestep'
    num_state_vars = 0
    use_one_based_indexing = 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 = 100
  nl_max_its = 100
  nl_rel_tol = 1e-12
  nl_abs_tol = 1e-10
  l_tol = 1e-9
  start_time = 0.0
  end_time = 30

  [TimeStepper]
    type = IterationAdaptiveDT
    optimal_iterations = 30
    iteration_window = 9
    growth_factor = 2.0
    cutback_factor = 1.0
    timestep_limiting_postprocessor = matl_ts_min
    dt = 1.0
  []
[]

[UserObjects]
  [time_step_size]
    type = TimestepSize
    execute_on = 'INITIAL LINEAR'
  []
  [terminator_umat]
    type = Terminator
    expression = 'time_step_size > matl_ts_min'
    fail_mode = SOFT
    execute_on = 'FINAL'
  []
[]

[Postprocessors]
  [matl_ts_min]
    type = MaterialTimeStepPostprocessor
  []
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Outputs]
  exodus = true
[]

(moose/modules/solid_mechanics/test/tests/umat/time_step/elastic_timestep.i)

# Testing the UMAT Interface - linear elastic model using the large strain formulation.

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

[Mesh]
  [gen]
    type = GeneratedMeshGenerator
    dim = 3
    xmin = -0.5
    xmax = 0.5
    ymin = -0.5
    ymax = 0.5
    zmin = -0.5
    zmax = 0.5
  []
[]

[Functions]
  [top_pull]
    type = ParsedFunction
    expression = t/100
  []
[]

[Physics/SolidMechanics/QuasiStatic]
  [all]
    add_variables = true
    strain = FINITE
  []
[]

[BCs]
  [y_pull_function]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = top
    function = top_pull
  []
  [x_bot]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0.0
  []
  [y_bot]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0.0
  []
  [z_bot]
    type = DirichletBC
    variable = disp_z
    boundary = front
    value = 0.0
  []
[]

[Materials]
  [umat]
    type = AbaqusUMATStress
    constant_properties = '1000 0.3'
    plugin = '../../../plugins/elastic_timestep'
    num_state_vars = 0
    use_one_based_indexing = 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 = 100
  nl_max_its = 100
  nl_rel_tol = 1e-12
  nl_abs_tol = 1e-10
  l_tol = 1e-9
  start_time = 0.0
  end_time = 30

  [TimeStepper]
    type = IterationAdaptiveDT
    optimal_iterations = 30
    iteration_window = 9
    growth_factor = 2.0
    cutback_factor = 1.0
    timestep_limiting_postprocessor = matl_ts_min
    dt = 1.0
  []
[]

[UserObjects]
  [time_step_size]
    type = TimestepSize
    execute_on = 'INITIAL LINEAR'
  []
  [terminator_umat]
    type = Terminator
    expression = 'time_step_size > matl_ts_min'
    fail_mode = SOFT
    execute_on = 'FINAL'
  []
[]

[Postprocessors]
  [matl_ts_min]
    type = MaterialTimeStepPostprocessor
  []
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Outputs]
  exodus = true
[]

(moose/modules/solid_mechanics/test/tests/umat/steps/elastic_temperature_steps_uo.i)

# Testing the UMAT Interface - linear elastic model using the large strain formulation.

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

[Mesh]
  [gen]
    type = GeneratedMeshGenerator
    dim = 3
    xmin = -0.5
    xmax = 0.5
    ymin = -0.5
    ymax = 0.5
    zmin = -0.5
    zmax = 0.5
  []
[]

[Functions]
  [top_pull_step2]
    type = ParsedFunction
    expression = (t-5.0)/20
  []
  # Forced evolution of temperature
  [temperature_load]
    type = ParsedFunction
    expression = '273'
  []
[]

[AuxVariables]
  [temperature]
  []
[]

[AuxKernels]
  [temperature_function]
    type = FunctionAux
    variable = temperature
    function = temperature_load
  []
[]

[Physics/SolidMechanics/QuasiStatic]
  [all]
    add_variables = true
    strain = FINITE
    generate_output = 'stress_yy'
  []
[]

[BCs]
  [y_step1]
    type = DirichletBC
    variable = disp_y
    boundary = top
    value = 0.0
  []
  [y_pull_function_step2]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = top
    function = top_pull_step2
  []
  [x_bot]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0.0
  []
  [y_bot]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0.0
  []
  [z_bot]
    type = DirichletBC
    variable = disp_z
    boundary = front
    value = 0.0
  []
[]

[Controls]
  [step1]
    type = StepPeriod
    enable_objects = 'BCs::y_step1'
    disable_objects = 'BCs::y_pull_function_step2'
    step_user_object = step_uo
    step_number = 0
  []
  [step2]
    type = StepPeriod
    enable_objects = 'BCs::y_pull_function_step2'
    disable_objects = 'BCs::y_step1'
    step_user_object = step_uo
    step_number = 1
  []
[]

[UserObjects]
  [step_uo]
   type = StepUserObject
   step_start_times = '0 5'
  []
[]

[Materials]
  [umat]
    type = AbaqusUMATStress
    constant_properties = '1000 0.3'
    plugin = '../../../plugins/elastic_temperature'
    num_state_vars = 0
    temperature = temperature
    use_one_based_indexing = 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 = 100
  nl_max_its = 100
  nl_rel_tol = 1e-12
  nl_abs_tol = 1e-10
  l_tol = 1e-9
  start_time = 0.0
  num_steps = 10
  dt = 1.0
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Outputs]
  exodus = true
[]

(moose/modules/solid_mechanics/test/tests/umat/elastic_hardening/linear_strain_hardening.i)

# Testing the UMAT Interface - creep linear strain hardening model using the finite strain formulation - visco-plastic material.

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

[Mesh]
  [gen]
    type = GeneratedMeshGenerator
    dim = 3
    xmin = -0.5
    xmax = 0.5
    ymin = -0.5
    ymax = 0.5
    zmin = -0.5
    zmax = 0.5
  []
[]

[Functions]
  [top_pull]
    type = ParsedFunction
    expression = t/100
  []
[]

[Physics/SolidMechanics/QuasiStatic]
  [all]
    add_variables = true
    strain = FINITE
  []
[]

[BCs]
  [y_pull_function]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = top
    function = top_pull
  []
  [x_bot]
    type = DirichletBC
    variable = disp_x
    boundary = left
    value = 0.0
  []
  [y_bot]
    type = DirichletBC
    variable = disp_y
    boundary = bottom
    value = 0.0
  []
  [z_bot]
    type = DirichletBC
    variable = disp_z
    boundary = front
    value = 0.0
  []
[]

[Materials]
  [constant]
    type = AbaqusUMATStress
    #                      Young's modulus,  Poisson's Ratio, Yield, Hardening
    constant_properties = '1000 0.3 10 100'
    plugin = ../../../plugins/linear_strain_hardening
    num_state_vars = 3
    use_one_based_indexing = 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 = 100
  nl_max_its = 100
  nl_rel_tol = 1e-12
  nl_abs_tol = 1e-10
  l_tol = 1e-9
  start_time = 0.0
  num_steps = 30
  dt = 1.0
[]

[Preconditioning]
  [smp]
    type = SMP
    full = true
  []
[]

[Outputs]
  [out]
    type = Exodus
    elemental_as_nodal = true
  []
[]