Contact

Description

The Contact block can be used to specify parameters related to mechanical contact enforcement in MOOSE simulations. The ContactAction is associated with this input block, and is the class that performs the associated model setup tasks. Use of the ContactAction is not strictly required, but it greatly simplifies the setup of a simulation using contact enforcement. A high-level description of the contact problem is provided here.

This block can be used to specify mechanical normal and tangential contact using several possible models for the physical behavior of the interaction:

frictionless
glued
coulomb (frictional)

Contact enforcement using node/face primary/secondary algorithms is available using the following mathematical formulations:

kinematic
penalty
tangential penalty (kinematic normal constraint with penalty tangential constraint)
augmented lagrange
reduced active nonlinear function set (RANFS)

In addition, face/face contact using a mortar method can also be specified using this block.

Constructed Objects

The primary task performed by this action is creating the Constraint classes that perform the contact enforcement. The type of Constraint class(es) constructed depend on the formulation and physical interaction model specified using the formulation and model parameters. Table 1 shows the Constraint classes that can be created for various types of contact enforcement.

Table 1: Constraint objects constructed by ContactAction

Formulation	Model	Constraint Object
kinematic	all	MechanicalContactConstraint
penalty	all	MechanicalContactConstraint
tangential_penalty	all	MechanicalContactConstraint
ranfs	frictionless	RANFSNormalMechanicalContact
mortar	all	MechanicalContactConstraint
mortar	all	NormalMortarMechanicalContact NormalMortarLMMechanicalContact
mortar	coulomb	TangentialMortarMechanicalContact TangentialMortarLMMechanicalContact

In addition to the Constraint class, several other objects are created, as shown in

Table 2: Other objects constructed by ContactAction

Constructed Object	Purpose
ContactPressureAux	Compute contact pressure and store in an AuxVariable
Penetration	Compute contact penetration and store in an AuxVariable
NodalArea	Compute nodal area and store in an AuxVariable

Notes on Node/Face Contact Enforcement

The node/face contact enforcement is based on a primary/secondary algorithm, in which contact is enforced at the nodes on the secondary surface, which cannot penetrate faces on the primary surface. As with all such approaches, for the best results, the primary surface should be the coarser of the two surfaces.

The contact enforcement system relies on MOOSE's geometric search system to provide the candidate set of faces that can interact with a secondary node at a given time. The set of candidate faces is controlled by the patch_size parameter and the patch_update_strategy options in the Mesh block. The patch size must be large enough to accommodate the sliding that occurs during a time step. It is generally recommended that the patch_update_strategy=auto be used.

The formulation parameter specifies the technique used to enforce contact. The DEFAULT option uses a kinematic enforcement algorithm that transfers the internal forces at secondary nodes to the corresponding primary face, and forces the secondary node to be at a specific location on the primary face using a penalty parameter. The converged solution with this approach results no penetration between the surfaces. The PENALTY algorithm employs a penalty approach, where the penetration between the surfaces is penalized, and the converged solution has a small penetration, which is inversely proportional to the penalty parameter.

Regardless of the formulation used, the robustness of the mechanical contact algorithm is affected by the penalty parameter. If the parameter is too small, there will be excessive penetrations with the penalty formulation, and convergence will suffer with the kinematic formulation. If the parameter is too large, the solver may struggle due to poor conditioning.

`System` Parameter

The system parameter is deprecated and currently defaults to Constraint.

Gap offset parameters

Gap offset can be provided to the current contact formulation enforced using the MechanicalContactConstraint. It can be either secondary_gap_offset (gap offset from secondary side) or mapped_primary_gap_offset (gap offset from primary side but mapped to secondary side). Use of these gap offset parameters treats the surfaces as if they were virtually extended (positive offset value) or narrowed (negative offset value) by the specified amount, so that the surfaces are treated as if they are closer or further away than they actually are. There is no deformation within the material in this gap offset region.

Example Input syntax

Node/face frictionless contact:

[Contact]
  [./leftright]
    secondary = 3
    primary = 2
    model = frictionless
    penalty = 1e+6
    normal_smoothing_distance = 0.1
  [../]
[]

Node/face frictional contact:

[Contact]
  [./leftright]
    secondary = 3
    primary = 2
    model = coulomb
    penalty = 1e+7
    friction_coefficient = 0.2
    formulation = penalty
    normal_smoothing_distance = 0.1
  [../]
[]

Normal (frictionless) mortar contact:

[Contact]
  [frictionless]
    mesh = simple_mesh
    primary = 2
    secondary = 1
    formulation = mortar
  []
[]

Normal and tangential (frictional) mortar contact:

[Contact]
  [frictional]
    mesh = revised_file_mesh
    primary = 20
    secondary = 10
    formulation = mortar
    model = coulomb
    friction_coefficient = 0.1
  []
[]

Gap offset:

[Contact]
  [./leftright]
    primary = 2
    secondary = 3
    model = frictionless
    penalty = 1e+6
    secondary_gap_offset = secondary_gap_offset
    mapped_primary_gap_offset = mapped_primary_gap_offset
  [../]
[]

Input Parameters

primaryThe primary surface
C++ Type:BoundaryName
Options:
Description:The primary surface
secondaryThe secondary surface
C++ Type:BoundaryName
Options:
Description:The secondary surface

Required Parameters

active__all__ If specified only the blocks named will be visited and made active
Default:__all__
C++ Type:std::vector<std::string>
Options:
Description:If specified only the blocks named will be visited and made active
al_frictional_force_toleranceThe tolerance of the frictional force for augmented Lagrangian method.
C++ Type:double
Options:
Description:The tolerance of the frictional force for augmented Lagrangian method.
al_incremental_slip_toleranceThe tolerance of the incremental slip for augmented Lagrangian method.
C++ Type:double
Options:
Description:The tolerance of the incremental slip for augmented Lagrangian method.
al_penetration_toleranceThe tolerance of the penetration for augmented Lagrangian method.
C++ Type:double
Options:
Description:The tolerance of the penetration for augmented Lagrangian method.
c_normal1Parameter for balancing the size of the gap and contact pressure
Default:1
C++ Type:double
Options:
Description:Parameter for balancing the size of the gap and contact pressure
c_tangential1Parameter for balancing the contact pressure and velocity
Default:1
C++ Type:double
Options:
Description:Parameter for balancing the contact pressure and velocity
capture_tolerance0Normal distance from surface within which nodes are captured
Default:0
C++ Type:double
Options:
Description:Normal distance from surface within which nodes are captured
displacementsThe displacements appropriate for the simulation geometry and coordinate system
C++ Type:std::vector<VariableName>
Options:
Description:The displacements appropriate for the simulation geometry and coordinate system
formulationkinematicThe contact formulation
Default:kinematic
C++ Type:MooseEnum
Options:ranfs, kinematic, penalty, augmented_lagrange, tangential_penalty, mortar
Description:The contact formulation
friction_coefficient0The friction coefficient
Default:0
C++ Type:double
Options:
Description:The friction coefficient
inactiveIf specified blocks matching these identifiers will be skipped.
C++ Type:std::vector<std::string>
Options:
Description:If specified blocks matching these identifiers will be skipped.
mapped_primary_gap_offsetOffset to gap distance mapped from primary side
C++ Type:VariableName
Options:
Description:Offset to gap distance mapped from primary side
meshThe mesh generator for mortar method
C++ Type:MeshGeneratorName
Options:
Description:The mesh generator for mortar method
modelfrictionlessThe contact model to use
Default:frictionless
C++ Type:MooseEnum
Options:frictionless, glued, coulomb
Description:The contact model to use
normal_lm_scaling1Scaling factor to apply to the normal LM variable
Default:1
C++ Type:double
Options:
Description:Scaling factor to apply to the normal LM variable
normal_smoothing_distanceDistance from edge in parametric coordinates over which to smooth contact normal
C++ Type:double
Options:
Description:Distance from edge in parametric coordinates over which to smooth contact normal
normal_smoothing_methodMethod to use to smooth normals
C++ Type:MooseEnum
Options:edge_based, nodal_normal_based
Description:Method to use to smooth normals
normalize_penaltyFalseWhether to normalize the penalty parameter with the nodal area.
Default:False
C++ Type:bool
Options:
Description:Whether to normalize the penalty parameter with the nodal area.
orderFIRSTThe finite element order: FIRST, SECOND, etc.
Default:FIRST
C++ Type:MooseEnum
Options:CONSTANT, FIRST, SECOND, THIRD, FOURTH
Description:The finite element order: FIRST, SECOND, etc.
penalty1e+08The penalty to apply. This can vary depending on the stiffness of your materials
Default:1e+08
C++ Type:double
Options:
Description:The penalty to apply. This can vary depending on the stiffness of your materials
ping_pong_protectionFalseWhether to protect against ping-ponging, e.g. the oscillation of the secondary node between two different primary faces, by tying the secondary node to the edge between the involved primary faces
Default:False
C++ Type:bool
Options:
Description:Whether to protect against ping-ponging, e.g. the oscillation of the secondary node between two different primary faces, by tying the secondary node to the edge between the involved primary faces
primary_secondary_jacobianTrueWhether to include Jacobian entries coupling primary and secondary nodes.
Default:True
C++ Type:bool
Options:
Description:Whether to include Jacobian entries coupling primary and secondary nodes.
secondary_gap_offsetOffset to gap distance from secondary side
C++ Type:VariableName
Options:
Description:Offset to gap distance from secondary side
tangential_lm_scaling1Scaling factor to apply to the tangential LM variable
Default:1
C++ Type:double
Options:
Description:Scaling factor to apply to the tangential LM variable
tangential_toleranceTangential distance to extend edges of contact surfaces
C++ Type:double
Options:
Description:Tangential distance to extend edges of contact surfaces
tension_release0Tension release threshold. A node in contact will not be released if its tensile load is below this value. No tension release if negative.
Default:0
C++ Type:double
Options:
Description:Tension release threshold. A node in contact will not be released if its tensile load is below this value. No tension release if negative.
use_dualFalseWhether to use the dual mortar approach
Default:False
C++ Type:bool
Options:
Description:Whether to use the dual mortar approach

Optional Parameters

(modules/contact/test/tests/sliding_block/sliding/frictionless_kinematic.i)

#  This is a benchmark test that checks constraint based frictionless
#  contact using the kinematic method.  In this test a constant
#  displacement is applied in the horizontal direction to simulate
#  a small block come sliding down a larger block.
#
#  The gold file is run on one processor
#  and the benchmark case is run on a minimum of 4 processors to ensure no
#  parallel variability in the contact pressure and penetration results.
#

[Mesh]
  file = sliding_elastic_blocks_2d.e
  patch_size = 80
[]

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

[AuxVariables]
  [./penetration]
  [../]
  [./inc_slip_x]
  [../]
  [./inc_slip_y]
  [../]
  [./accum_slip_x]
  [../]
  [./accum_slip_y]
  [../]
[]

[Functions]
  [./vertical_movement]
    type = ParsedFunction
    value = -t
  [../]
[]

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

[AuxKernels]
  [./zeroslip_x]
    type = ConstantAux
    variable = inc_slip_x
    boundary = 3
    execute_on = timestep_begin
    value = 0.0
  [../]
  [./zeroslip_y]
    type = ConstantAux
    variable = inc_slip_y
    boundary = 3
    execute_on = timestep_begin
    value = 0.0
  [../]
  [./accum_slip_x]
    type = AccumulateAux
    variable = accum_slip_x
    accumulate_from_variable = inc_slip_x
    execute_on = timestep_end
  [../]
  [./accum_slip_y]
    type = AccumulateAux
    variable = accum_slip_y
    accumulate_from_variable = inc_slip_y
    execute_on = timestep_end
  [../]
  [./penetration]
    type = PenetrationAux
    variable = penetration
    boundary = 3
    paired_boundary = 2
  [../]
[]

[Postprocessors]
  [./nonlinear_its]
    type = NumNonlinearIterations
    execute_on = timestep_end
  [../]
  [./penetration]
    type = NodalVariableValue
    variable = penetration
    nodeid = 222
  [../]
  [./contact_pressure]
    type = NodalVariableValue
    variable = contact_pressure
    nodeid = 222
  [../]
[]

[BCs]
  [./left_x]
    type = DirichletBC
    variable = disp_x
    boundary = 1
    value = 0.0
  [../]
  [./left_y]
    type = DirichletBC
    variable = disp_y
    boundary = 1
    value = 0.0
  [../]
  [./right_x]
    type = DirichletBC
    variable = disp_x
    boundary = 4
    value = -0.02
  [../]
  [./right_y]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = 4
    function = vertical_movement
  [../]
[]

[Materials]

  [./left]
    type = ComputeIsotropicElasticityTensor
    block = '1 2'
    youngs_modulus = 1e6
    poissons_ratio = 0.3
  [../]
  [./left_stress]
    type = ComputeFiniteStrainElasticStress
    block = '1 2'
  [../]
[]

[Executioner]
  type = Transient
  solve_type = 'PJFNK'

  petsc_options = '-snes_ksp_ew'
  petsc_options_iname = '-pc_type -sub_pc_type -pc_asm_overlap -ksp_gmres_restart'
  petsc_options_value = 'asm     lu    20    101'

  line_search = 'none'

  l_max_its = 100
  nl_max_its = 1000
  dt = 0.1
  end_time = 15
  num_steps = 1000
  l_tol = 1e-6
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-6
  dtmin = 0.01

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

[Outputs]
  interval = 10
  [./out]
    type = Exodus
    elemental_as_nodal = true
  [../]
  [./console]
    type = Console
    max_rows = 5
  [../]
[]

[Contact]
  [./leftright]
    secondary = 3
    primary = 2
    model = frictionless
    penalty = 1e+6
    normal_smoothing_distance = 0.1
  [../]
[]

(modules/contact/test/tests/sliding_block/sliding/frictional_02_penalty.i)

#  This is a benchmark test that checks constraint based frictional
#  contact using the penalty method.  In this test a constant
#  displacement is applied in the horizontal direction to simulate
#  a small block come sliding down a larger block.
#
#  A friction coefficient of 0.2 is used.  The gold file is run on one processor
#  and the benchmark case is run on a minimum of 4 processors to ensure no
#  parallel variability in the contact pressure and penetration results.
#

[Mesh]
  file = sliding_elastic_blocks_2d.e
  patch_size = 80
[]

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

[AuxVariables]
  [./penetration]
  [../]
  [./inc_slip_x]
  [../]
  [./inc_slip_y]
  [../]
  [./accum_slip_x]
  [../]
  [./accum_slip_y]
  [../]
[]

[Functions]
  [./vertical_movement]
    type = ParsedFunction
    value = -t
  [../]
[]

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

[AuxKernels]
  [./zeroslip_x]
    type = ConstantAux
    variable = inc_slip_x
    boundary = 3
    execute_on = timestep_begin
    value = 0.0
  [../]
  [./zeroslip_y]
    type = ConstantAux
    variable = inc_slip_y
    boundary = 3
    execute_on = timestep_begin
    value = 0.0
  [../]
  [./accum_slip_x]
    type = AccumulateAux
    variable = accum_slip_x
    accumulate_from_variable = inc_slip_x
    execute_on = timestep_end
  [../]
  [./accum_slip_y]
    type = AccumulateAux
    variable = accum_slip_y
    accumulate_from_variable = inc_slip_y
    execute_on = timestep_end
  [../]
  [./penetration]
    type = PenetrationAux
    variable = penetration
    boundary = 3
    paired_boundary = 2
  [../]
[]

[Postprocessors]
  [./nonlinear_its]
    type = NumNonlinearIterations
    execute_on = timestep_end
  [../]
  [./penetration]
    type = NodalVariableValue
    variable = penetration
    nodeid = 222
  [../]
  [./contact_pressure]
    type = NodalVariableValue
    variable = contact_pressure
    nodeid = 222
  [../]
[]

[BCs]
  [./left_x]
    type = DirichletBC
    variable = disp_x
    boundary = 1
    value = 0.0
  [../]
  [./left_y]
    type = DirichletBC
    variable = disp_y
    boundary = 1
    value = 0.0
  [../]
  [./right_x]
    type = DirichletBC
    variable = disp_x
    boundary = 4
    value = -0.02
  [../]
  [./right_y]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = 4
    function = vertical_movement
  [../]
[]

[Materials]
  [./left]
    type = ComputeIsotropicElasticityTensor
    block = '1 2'
    youngs_modulus = 1e6
    poissons_ratio = 0.3
  [../]
  [./stress]
    type = ComputeFiniteStrainElasticStress
    block = '1 2'
  [../]
[]


[Executioner]
  type = Transient
  solve_type = 'PJFNK'

  petsc_options = '-snes_ksp_ew'
  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 = 1000
  dt = 0.1
  end_time = 15
  num_steps = 1000
  l_tol = 1e-6
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-6
  dtmin = 0.01

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

[Outputs]
  interval = 10
  [./out]
    type = Exodus
    elemental_as_nodal = true
  [../]
  [./console]
    type = Console
    max_rows = 5
  [../]
[]

[Contact]
  [./leftright]
    secondary = 3
    primary = 2
    model = coulomb
    penalty = 1e+7
    friction_coefficient = 0.2
    formulation = penalty
    normal_smoothing_distance = 0.1
  [../]
[]

(modules/contact/test/tests/mechanical-small-problem/frictionless-nodal-lm-mortar-disp-action.i)

[GlobalParams]
  displacements = 'disp_x disp_y'
[]

[Mesh]
  [./simple_mesh]
    type = FileMeshGenerator
    file = mesh.e
  [../]
[]

[Problem]
  kernel_coverage_check = false
[]

[Variables]
  [./disp_x]
    block = '1 2'
  [../]
  [./disp_y]
    block = '1 2'
  [../]
[]

[BCs]
  [./left_x]
    type = DirichletBC
    variable = disp_x
    boundary = 'outside_left'
    value = 0.0
  [../]
  [./left_y]
    type = DirichletBC
    variable = disp_y
    boundary = 'outside_left'
    value = 0.0
  [../]
  [./right_x]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = 'outside_right'
    function = '-5e-3 * t'
  [../]
  [./right_y]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = 'outside_right'
    function = 0
  [../]
[]

[Kernels]
  [disp_x]
    type = Diffusion
    variable = disp_x
    block = '1 2'
  []
  [disp_y]
    type = Diffusion
    variable = disp_y
    block = '1 2'
  []
[]

[Debug]
  show_var_residual_norms = 1
[]

[Contact]
  [frictionless]
    mesh = simple_mesh
    primary = 2
    secondary = 1
    formulation = mortar
  []
[]

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

[Executioner]
  solve_type = PJFNK
  type = Transient
  num_steps = 10
  dt = 1
  dtmin = 1
  petsc_options_iname = '-pc_type -snes_linesearch_type -pc_factor_shift_type -pc_factor_shift_amount'
  petsc_options_value = 'lu       basic                 NONZERO               1e-15'
[]

[Outputs]
  exodus = true
  hide = 'contact_pressure nodal_area_frictionless penetration'
[]

[Postprocessors]
  [contact]
    type = ContactDOFSetSize
    variable = frictionless_normal_lm
    subdomain = '4'
    execute_on = 'nonlinear timestep_end'
  []
[]

(modules/contact/test/tests/bouncing-block-contact/frictional-nodal-min-normal-lm-mortar-fb-tangential-lm-mortar-action.i)

starting_point = 2e-1

# We offset slightly so we avoid the case where the bottom of the secondary block and the top of the
# primary block are perfectly vertically aligned which can cause the backtracking line search some
# issues for a coarse mesh (basic line search handles that fine)
offset = 1e-2

[GlobalParams]
  displacements = 'disp_x disp_y'
  diffusivity = 1e0
  scaling = 1e0
[]

[Mesh]
  [./original_file_mesh]
    type = FileMeshGenerator
    file = long-bottom-block-1elem-blocks-coarse.e
  [../]
  # These sidesets need to be deleted because the contact action adds them automatically. For this
  # particular mesh, the new IDs will be identical to the deleted ones and will conflict if we don't
  # remove the original ones.
  [./delete_3]
    type = BlockDeletionGenerator
    input = original_file_mesh
    block = 3
  [../]
  [./revised_file_mesh]
    type = BlockDeletionGenerator
    input = delete_3
    block = 4
  [../]
[]

[Variables]
  [./disp_x]
    block = '1 2'
    # order = SECOND
  [../]
  [./disp_y]
    block = '1 2'
    # order = SECOND
  [../]
[]

[Contact]
  [frictional]
    mesh = revised_file_mesh
    primary = 20
    secondary = 10
    formulation = mortar
    model = coulomb
    friction_coefficient = 0.1
  []
[]

[ICs]
  [./disp_y]
    block = 2
    variable = disp_y
    value = ${fparse starting_point + offset}
    type = ConstantIC
  [../]
[]

[Kernels]
  [./disp_x]
    type = MatDiffusion
    variable = disp_x
  [../]
  [./disp_y]
    type = MatDiffusion
    variable = disp_y
  [../]
[]

[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 / 40 * t) + ${offset}'
  [../]
  [./leftx]
    type = FunctionDirichletBC
    variable = disp_x
    boundary = 50
    function = '1e-2 * t'
  [../]
[]

[Executioner]
  type = Transient
  end_time = 200
  dt = 5
  dtmin = .1
  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'
  l_max_its = 30
  nl_max_its = 20
  line_search = 'none'
[]

[Debug]
  show_var_residual_norms = true
[]

[Outputs]
  exodus = true
  hide = 'contact_pressure nodal_area_frictional penetration'
[]

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

[Postprocessors]
  [./num_nl]
    type = NumNonlinearIterations
  [../]
  [./cumulative]
    type = CumulativeValuePostprocessor
    postprocessor = num_nl
  [../]
  [contact]
    type = ContactDOFSetSize
    variable = frictional_normal_lm
    subdomain = frictional_secondary_subdomain
    execute_on = 'nonlinear timestep_end'
  []
[]

(modules/contact/test/tests/mechanical_constraint/frictionless_kinematic_gap_offsets.i)

# this test is the same as frictionless_kinematic test but designed to test the gap offset capability
# gap offsets with value of 0.01 were introduced to both primary and secondary sides in the initial mesh
# these values were accounted using the gap offset capability to produce the same result as if no gap offsets were introduced
[Mesh]
  file = blocks_2d_gap_offset.e
[]

[GlobalParams]
  displacements = 'disp_x disp_y'
[]

[AuxVariables]
  [./inc_slip_x]
  [../]
  [./inc_slip_y]
  [../]
  [./accum_slip_x]
  [../]
  [./accum_slip_y]
  [../]
  [./primary_gap_offset]
  [../]
  [./secondary_gap_offset]
  [../]
  [./mapped_primary_gap_offset]
  [../]
[]

[Functions]
  [./vertical_movement]
    type = ParsedFunction
    value = -t
  [../]
[]

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

[AuxKernels]
  [./zeroslip_x]
    type = ConstantAux
    variable = inc_slip_x
    boundary = 3
    execute_on = timestep_begin
    value = 0.0
  [../]
  [./zeroslip_y]
    type = ConstantAux
    variable = inc_slip_y
    boundary = 3
    execute_on = timestep_begin
    value = 0.0
  [../]
  [./accum_slip_x]
    type = AccumulateAux
    variable = accum_slip_x
    accumulate_from_variable = inc_slip_x
    execute_on = timestep_end
  [../]
  [./accum_slip_y]
    type = AccumulateAux
    variable = accum_slip_y
    accumulate_from_variable = inc_slip_y
    execute_on = timestep_end
  [../]
  [./primary_gap_offset]
    type = ConstantAux
    variable = primary_gap_offset
    value = -0.01
    boundary = 2
  [../]
  [./mapped_primary_gap_offset]
    type = GapValueAux
    variable = mapped_primary_gap_offset
    paired_variable = primary_gap_offset
    boundary = 3
    paired_boundary = 2
  [../]
  [./secondary_gap_offset]
    type = ConstantAux
    variable = secondary_gap_offset
    value = -0.01
    boundary = 3
  [../]
[]

[BCs]
  [./left_x]
    type = DirichletBC
    variable = disp_x
    boundary = 1
    value = 0.0
  [../]
  [./left_y]
    type = DirichletBC
    variable = disp_y
    boundary = 1
    value = 0.0
  [../]
  [./right_x]
    type = DirichletBC
    variable = disp_x
    boundary = 4
    value = -0.02
  [../]
  [./right_y]
    type = FunctionDirichletBC
    variable = disp_y
    boundary = 4
    function = vertical_movement
  [../]
[]

[Materials]
  [./left]
    type = ComputeIsotropicElasticityTensor
    block = 1
    poissons_ratio = 0.3
    youngs_modulus = 1e7
  [../]
  [./right]
    type = ComputeIsotropicElasticityTensor
    block = 2
    poissons_ratio = 0.3
    youngs_modulus = 1e6
  [../]
  [./stress]
    type = ComputeFiniteStrainElasticStress
    block = '1 2'
  [../]
[]

[Executioner]
  type = Transient

  solve_type = 'PJFNK'

  petsc_options_iname = '-pc_type'
  petsc_options_value = 'lu'

  line_search = 'none'

  l_max_its = 100
  nl_max_its = 1000
  dt = 0.01
  end_time = 0.10
  num_steps = 1000
  l_tol = 1e-6
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-8
  dtmin = 0.01

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

[Outputs]
  file_base = frictionless_kinematic_gap_offsets_out
  [./exodus]
    type = Exodus
    elemental_as_nodal = true
  [../]
  [./console]
    type = Console
    max_rows = 5
  [../]
[]

[Contact]
  [./leftright]
    primary = 2
    secondary = 3
    model = frictionless
    penalty = 1e+6
    secondary_gap_offset = secondary_gap_offset
    mapped_primary_gap_offset = mapped_primary_gap_offset
  [../]
[]

Description
Constructed Objects
Notes on Node / Face Contact Enforcement
Parameter System
Gap offset parameters
Example Input syntax
Input Parameters

Install MOOSE

New Users

Examples and Tutorials

Application Usage

Physics and Syntax

Application Development

Framework Development

MOOSEDocs

Infrastructure

Questions

Information and Tools

INL Applications and Remote Access

Contact

Description

Constructed Objects

Notes on Node/Face Contact Enforcement

`System` Parameter

Gap offset parameters

Example Input syntax

Input Parameters

Required Parameters

Optional Parameters

Contact

Description

Constructed Objects

Notes on Node/Face Contact Enforcement

System Parameter

Gap offset parameters

Example Input syntax

Input Parameters

Required Parameters

Optional Parameters

(modules/contact/test/tests/sliding_block/sliding/frictionless_kinematic.i)

(modules/contact/test/tests/sliding_block/sliding/frictional_02_penalty.i)

(modules/contact/test/tests/mechanical-small-problem/frictionless-nodal-lm-mortar-disp-action.i)

(modules/contact/test/tests/bouncing-block-contact/frictional-nodal-min-normal-lm-mortar-fb-tangential-lm-mortar-action.i)

(modules/contact/test/tests/mechanical_constraint/frictionless_kinematic_gap_offsets.i)

`System` Parameter