NodalFrictionalConstraint

Frictional nodal constraint for contact

Only a penalty formulation is implemented. First, the previous time step tangential force is computed as:

var element = document.getElementById("moose-equation-ea92a7c2-db57-41cb-a69f-24b4a270019c");katex.render("F_{old} = \\text{tangeantial penalty} (u_{primary-old} - u_{secondary-old})", element, {displayMode:true,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});

If it is greater than the allowed frictional force (normal force times the friction coefficient), then the local nodes are in the slippage regime and the old force is recomputed as:

var element = document.getElementById("moose-equation-5ae026f0-ea6f-46f2-ab02-ff4dd6b530a9");katex.render("F_{old} = \\text{friction coefficient} * \\text{normal force} * \\dfrac{F_{old}}{|F_{old}|}", element, {displayMode:true,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});

From the previous time step force $var element = document.getElementById("moose-equation-d9ee67c6-f56d-4018-be3e-fd0a665bdbc7");katex.render("F_{old}", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ , and the previous and current values of $var element = document.getElementById("moose-equation-46265a5b-487d-42a8-907f-a717afae13b6");katex.render("u", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ on the primary and secondary side, the current force is computed as:

var element = document.getElementById("moose-equation-67f65a56-f265-4428-a750-90ead482a648");katex.render("F = F_{old} + ((u_{secondary-old} - u_{secondary}) - (u_{primary} - u_{primary-old})) * \\text{tangeantial penalty}", element, {displayMode:true,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});

If it is greater than the allowed frictional force (normal force times the friction coefficient), then the local nodes are in the slippage regime and the current force is recomputed as:

var element = document.getElementById("moose-equation-12b36973-3d3b-4954-a92b-6e76266e09dc");katex.render("F = \\text{friction coefficient} * \\text{normal force} * \\dfrac{F}{|F|}", element, {displayMode:true,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});

and the opposite on the secondary side, where $var element = document.getElementById("moose-equation-0efb1d49-b168-4e30-9dd1-79ef3c8637f4");katex.render("u", element, {displayMode:false,throwOnError:false,macros:{"\\eqc":"\\,,","\\eqp":"\\,.","\\pd":"\\frac{\\partial #1}{\\partial #2}","\\pr":"\\left(#1\\right)","\\ddt":"\\frac{d #1}{d t}"}});$ is usually the displacement component variable value for mechanical contact applications.

note

The primary and secondary variables must be different for this implementation of the nodal frictional constraint.

Input Parameters

boundaryThe primary boundary
C++ Type:BoundaryName
Unit:(no unit assumed)
Controllable:No
Description:The primary boundary
friction_coefficientFriction coefficient for slippage in the normal direction
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Friction coefficient for slippage in the normal direction
normal_forceNormal force used together with friction_coefficient to compute the normal frictional capacity.
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Normal force used together with friction_coefficient to compute the normal frictional capacity.
secondaryThe secondary boundary
C++ Type:BoundaryName
Unit:(no unit assumed)
Controllable:No
Description:The secondary boundary
tangential_penaltyStiffness of the spring in the tangential direction.
C++ Type:double
Unit:(no unit assumed)
Controllable:No
Description:Stiffness of the spring in the tangential direction.
variableThe name of the variable that this residual object operates on
C++ Type:NonlinearVariableName
Unit:(no unit assumed)
Controllable:No
Description:The name of the variable that this residual object operates on

Required Parameters

formulationpenaltyFormulation used to calculate constraint - penalty or kinematic.
Default:penalty
C++ Type:MooseEnum
Unit:(no unit assumed)
Options:penalty, kinematic
Controllable:No
Description:Formulation used to calculate constraint - penalty or kinematic.
variable_secondaryThe name of the variable for the secondary nodes, if it is different from the primary nodes' variable
C++ Type:NonlinearVariableName
Unit:(no unit assumed)
Controllable:No
Description:The name of the variable for the secondary nodes, if it is different from the primary nodes' variable

Optional Parameters

absolute_value_vector_tagsThe tags for the vectors this residual object should fill with the absolute value of the residual contribution
C++ Type:std::vector<TagName>
Unit:(no unit assumed)
Controllable:No
Description:The tags for the vectors this residual object should fill with the absolute value of the residual contribution
extra_matrix_tagsThe extra tags for the matrices this Kernel should fill
C++ Type:std::vector<TagName>
Unit:(no unit assumed)
Controllable:No
Description:The extra tags for the matrices this Kernel should fill
extra_vector_tagsThe extra tags for the vectors this Kernel should fill
C++ Type:std::vector<TagName>
Unit:(no unit assumed)
Controllable:No
Description:The extra tags for the vectors this Kernel should fill
matrix_tagssystemThe tag for the matrices this Kernel should fill
Default:system
C++ Type:MultiMooseEnum
Unit:(no unit assumed)
Options:nontime, system
Controllable:No
Description:The tag for the matrices this Kernel should fill
vector_tagsnontimeThe tag for the vectors this Kernel should fill
Default:nontime
C++ Type:MultiMooseEnum
Unit:(no unit assumed)
Options:nontime, time
Controllable:No
Description:The tag for the vectors this Kernel should fill

Tagging 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 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
Unit:(no unit assumed)
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

Input Files

(modules/solid_mechanics/test/tests/beam/constraints/frictional_constraint.i)
(modules/solid_mechanics/test/tests/beam/constraints/frictionless_constraint.i)
(modules/solid_mechanics/test/tests/beam/fric_constraint/2_block_common_cross.i)

(modules/solid_mechanics/test/tests/beam/constraints/frictional_constraint.i)

# Test for frictional beam constraint.
#
# Using a simple L-shaped geometry with a frictional constraint at the
# corner between the two beams. The longer beam properties and loading is
# taken from an earlier beam regression test for static loading. The maximum
# applied load of 50000 lb should result in a displacement of 3.537e-3. Since
# the constraint is frictional with a low normal force (1.0) and coefficient
# of friction (0.05) and the short beam is much less stiff, the
# y-dir displacement of the long beam is still 3.537e-3. However, the y-dir
# displacement of the short beam increases until the force exceeds the
# frictional capacity which in this case is 0.05 and then remains constant
# after that point.

[Mesh]
  file = beam_cons_patch.e
  displacements = 'disp_x disp_y disp_z'
[]

[Variables]
  [./disp_x]
    order = FIRST
    family = LAGRANGE
  [../]
  [./disp_y]
    order = FIRST
    family = LAGRANGE
  [../]
  [./disp_z]
    order = FIRST
    family = LAGRANGE
  [../]
  [./rot_x]
    order = FIRST
    family = LAGRANGE
  [../]
  [./rot_y]
    order = FIRST
    family = LAGRANGE
  [../]
  [./rot_z]
    order = FIRST
    family = LAGRANGE
  [../]
[]

[BCs]
  [./fixx1]
    type = DirichletBC
    variable = disp_x
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixy1]
    type = DirichletBC
    variable = disp_y
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixz1]
    type = DirichletBC
    variable = disp_z
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixr1]
    type = DirichletBC
    variable = rot_x
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixr2]
    type = DirichletBC
    variable = rot_y
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixr3]
    type = DirichletBC
    variable = rot_z
    boundary = '1001 1003'
    value = 0.0
  [../]
[]

[Constraints]
  [./tie_y_fuel]
    type = NodalFrictionalConstraint
    normal_force = 1.0
    tangential_penalty = 1.2e5
    friction_coefficient = 0.05
    boundary = 1005
    secondary = 1004
    variable = disp_y
  [../]
  [./tie_x_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = disp_x
  [../]
  [./tie_z_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = disp_z
  [../]
  [./tie_rot_y_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = rot_y
  [../]
  [./tie_rot_x_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = rot_x
  [../]
  [./tie_rot_z_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = rot_z
  [../]
[]

[Functions]
  [./force_loading]
    type = PiecewiseLinear
    x = '0.0 5.0'
    y = '0.0 50000.0'
  [../]
[]

[NodalKernels]
  [./force_x2]
    type = UserForcingFunctionNodalKernel
    variable = disp_y
    boundary = '1004'
    function = force_loading
  [../]
[]

[Preconditioning]
  [./smp]
    type = SMP
    full = true
  [../]
[]
[Executioner]
  type = Transient
  solve_type = PJFNK
  line_search = 'none'
  nl_max_its = 15
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-8

  dt = 1
  dtmin = 1
  end_time = 5
[]

[Kernels]
  [./solid_disp_x]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 0
    variable = disp_x
  [../]
  [./solid_disp_y]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 1
    variable = disp_y
  [../]
  [./solid_disp_z]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 2
    variable = disp_z
  [../]
  [./solid_rot_x]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 3
    variable = rot_x
  [../]
  [./solid_rot_y]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 4
    variable = rot_y
  [../]
  [./solid_rot_z]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 5
    variable = rot_z
  [../]
[]

[Materials]
  [./elasticity_pipe]
    type = ComputeElasticityBeam
    shear_coefficient = 1.0
    youngs_modulus = 30e6
    poissons_ratio = 0.3
    block = 1
    outputs = exodus
    output_properties = 'material_stiffness material_flexure'
  [../]
  [./strain_pipe]
    type = ComputeIncrementalBeamStrain
    block = '1'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    area = 28.274
    Ay = 0.0
    Az = 0.0
    Iy = 1.0
    Iz = 1.0
    y_orientation = '0.0 0.0 1.0'
  [../]
  [./stress_pipe]
    type = ComputeBeamResultants
    block = 1
    outputs = exodus
    output_properties = 'forces moments'
  [../]
  [./elasticity_cons]
    type = ComputeElasticityBeam
    shear_coefficient = 1.0
    youngs_modulus = 10e2
    poissons_ratio = 0.3
    block = 2
    outputs = exodus
    output_properties = 'material_stiffness material_flexure'
  [../]
  [./strain_cons]
    type = ComputeIncrementalBeamStrain
    block = '2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    area = 1.0
    Ay = 0.0
    Az = 0.0
    Iy = 1.0
    Iz = 1.0
    y_orientation = '0.0 0.0 1.0'
  [../]
  [./stress_cons]
    type = ComputeBeamResultants
    block = 2
    outputs = exodus
    output_properties = 'forces moments'
  [../]
[]

[Postprocessors]
  [./disp_y_n4]
    type = NodalVariableValue
    variable = disp_y
    nodeid = 3
  [../]
  [./disp_y_n2]
    type = NodalVariableValue
    variable = disp_y
    nodeid = 1
  [../]
  [./horz_forces_y]
    type = PointValue
    point = '9.9 60.0 0.0'
    variable = forces_y
  [../]
  [./forces_y]
    type = PointValue
    point = '10.0 59.9 0.0'
    variable = forces_y
  [../]
[]

[Outputs]
  csv = true
  exodus = true
[]

(modules/solid_mechanics/test/tests/beam/constraints/frictionless_constraint.i)

# Test for frictionless beam constraint.
#
# Using a simple L-shaped geometry with a frictionless constraint at the
# corner between the two beams. The longer beam properties and loading is
# taken from an earlier beam regression test for static loading. The maximum
# applied load of 50000 lb should result in a displacement of 3.537e-3. Since
# the constraint is frictionless, the y-dir displacement of the long beam is
# 3.537e-3 and the short beam y-dir displacement is zero.

[Mesh]
  file = beam_cons_patch.e
  displacements = 'disp_x disp_y disp_z'
[]

[Variables]
  [./disp_x]
    order = FIRST
    family = LAGRANGE
  [../]
  [./disp_y]
    order = FIRST
    family = LAGRANGE
  [../]
  [./disp_z]
    order = FIRST
    family = LAGRANGE
  [../]
  [./rot_x]
    order = FIRST
    family = LAGRANGE
  [../]
  [./rot_y]
    order = FIRST
    family = LAGRANGE
  [../]
  [./rot_z]
    order = FIRST
    family = LAGRANGE
  [../]
[]

[BCs]
  [./fixx1]
    type = DirichletBC
    variable = disp_x
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixy1]
    type = DirichletBC
    variable = disp_y
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixz1]
    type = DirichletBC
    variable = disp_z
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixr1]
    type = DirichletBC
    variable = rot_x
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixr2]
    type = DirichletBC
    variable = rot_y
    boundary = '1001 1003'
    value = 0.0
  [../]
  [./fixr3]
    type = DirichletBC
    variable = rot_z
    boundary = '1001 1003'
    value = 0.0
  [../]
[]

[Constraints]
  [./tie_y_fuel]
    type = NodalFrictionalConstraint
    normal_force = 1000
    tangential_penalty = 1.2e6
    friction_coefficient = 0.0
    boundary = 1005
    secondary = 1004
    variable = disp_y
  [../]
  [./tie_x_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = disp_x
  [../]
  [./tie_z_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = disp_z
  [../]
  [./tie_rot_y_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = rot_y
  [../]
  [./tie_rot_x_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = rot_x
  [../]
  [./tie_rot_z_fuel]
    type = NodalStickConstraint
    penalty = 1.2e14
    boundary = 1005
    secondary = 1004
    variable = rot_z
  [../]
[]

[Functions]
  [./force_loading]
    type = PiecewiseLinear
    x = '0.0 5.0'
    y = '0.0 50000.0'
  [../]
[]

[NodalKernels]
  [./force_x2]
    type = UserForcingFunctionNodalKernel
    variable = disp_y
    boundary = '1004'
    function = force_loading
  [../]
[]

[Preconditioning]
  [./smp]
    type = SMP
    full = true
  [../]
[]
[Executioner]
  type = Transient
  solve_type = PJFNK
  line_search = 'none'
  nl_max_its = 15
  nl_rel_tol = 1e-10
  nl_abs_tol = 1e-8

  dt = 1
  dtmin = 1
  end_time = 5
[]

[Kernels]
  [./solid_disp_x]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 0
    variable = disp_x
  [../]
  [./solid_disp_y]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 1
    variable = disp_y
  [../]
  [./solid_disp_z]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 2
    variable = disp_z
  [../]
  [./solid_rot_x]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 3
    variable = rot_x
  [../]
  [./solid_rot_y]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 4
    variable = rot_y
  [../]
  [./solid_rot_z]
    type = StressDivergenceBeam
    block = '1 2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    component = 5
    variable = rot_z
  [../]
[]

[Materials]
  [./elasticity_pipe]
    type = ComputeElasticityBeam
    shear_coefficient = 1.0
    youngs_modulus = 30e6
    poissons_ratio = 0.3
    block = 1
    outputs = exodus
    output_properties = 'material_stiffness material_flexure'
  [../]
  [./strain_pipe]
    type = ComputeIncrementalBeamStrain
    block = '1'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    area = 28.274
    Ay = 0.0
    Az = 0.0
    Iy = 1.0
    Iz = 1.0
    y_orientation = '0.0 0.0 1.0'
  [../]
  [./stress_pipe]
    type = ComputeBeamResultants
    block = 1
    outputs = exodus
    output_properties = 'forces moments'
  [../]
  [./elasticity_cons]
    type = ComputeElasticityBeam
    shear_coefficient = 1.0
    youngs_modulus = 10e2
    poissons_ratio = 0.3
    block = 2
    outputs = exodus
    output_properties = 'material_stiffness material_flexure'
  [../]
  [./strain_cons]
    type = ComputeIncrementalBeamStrain
    block = '2'
    displacements = 'disp_x disp_y disp_z'
    rotations = 'rot_x rot_y rot_z'
    area = 1.0
    Ay = 0.0
    Az = 0.0
    Iy = 1.0
    Iz = 1.0
    y_orientation = '0.0 0.0 1.0'
  [../]
  [./stress_cons]
    type = ComputeBeamResultants
    block = 2
    outputs = exodus
    output_properties = 'forces moments'
  [../]
[]

[Postprocessors]
  [./disp_y_n4]
    type = NodalVariableValue
    variable = disp_y
    nodeid = 3
  [../]
  [./disp_y_n2]
    type = NodalVariableValue
    variable = disp_y
    nodeid = 1
  [../]
  [./forces_y]
    type = PointValue
    point = '10.0 59.9 0.0'
    variable = forces_y
  [../]
[]

[Outputs]
  csv = true
  exodus = true
[]

(modules/solid_mechanics/test/tests/beam/fric_constraint/2_block_common_cross.i)

# Test for LineElementAction on multiple blocks by placing parameters
# common to all blocks outside of the individual action blocks

# 2 beams of length 1m are fixed at one end and a force of 1e-4 N
# is applied at the other end of the beams. Beam 1 is in block 1
# and beam 2 is in block 2. All the material properties for the two
# beams are identical. The moment of inertia of beam 2 is twice that
# of beam 1.

# Since the end displacement of a cantilever beam is inversely proportional
# to the moment of inertia, the y displacement at the end of beam 1 should be twice
# that of beam 2.

[Mesh]
  type = FileMesh
  file = test_fric_cross.e
  #displacements = 'disp_x disp_y disp_z'
[]

[BCs]
  [./fixx1]
    type = DirichletBC
    variable = disp_x
    boundary = '1 2 3'
    value = 0.0
  [../]
  [./fixy1]
    type = DirichletBC
    variable = disp_y
    boundary = '1 2 3'
    value = 0.0
  [../]
  [./fixz1]
    type = DirichletBC
    variable = disp_z
    boundary = '1 3'
    value = 0.0
  [../]
  [./fixr1]
    type = DirichletBC
    variable = rot_x
    boundary = '1 2 3'
    value = 0.0
  [../]
  [./fixr2]
    type = DirichletBC
    variable = rot_y
    boundary = '1 2 3'
    value = 0.0
  [../]
  [./fixr3]
    type = DirichletBC
    variable = rot_z
    boundary = '1 2 3'
    value = 0.0
  [../]
  [./move_z4]
    type = FunctionDirichletBC
    variable = disp_z
    boundary = 2
    function = pull
  [../]
[]

[Functions]
  [./pull]
    type = PiecewiseLinear
    x = '0.0 1.0 2.0  3.0  4.0  5.0  6.0  7.0   8.0  9.0 10.0 11.0 12.0 13.0'
    y = '0.0 0.0 -0.2 -0.4 -0.6 -0.8 -0.6 -0.4 -0.2  0.0 0.2 0.4  0.6 0.8'
  [../]
[]

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

[Executioner]
  type = Transient
  solve_type = NEWTON
  line_search = 'none'
  nl_max_its = 15
  nl_rel_tol = 1e-10
  nl_abs_tol = 5e-5
  l_max_its = 10

  dt = 1
  dtmin = 1
  end_time = 13
[]

[Physics/SolidMechanics/LineElement/QuasiStatic]
  # parameters common to all blocks

  add_variables = true
  displacements = 'disp_x disp_y disp_z'
  rotations = 'rot_x rot_y rot_z'

  # Geometry parameters
  area = 0.5
  y_orientation = '0.0 1.0 0.0'

  [./block_1]
    Iy = 1e-5
    Iz = 1e-5
    block = 1
  [../]
  [./block_2]
    Iy = 8e-4
    Iz = 8e-4
    block = '2 3'
  [../]
[]

[Materials]
  [./stress]
    type = ComputeBeamResultants
    block = '1 2 3'
  [../]
  [./elasticity_1]
    type = ComputeElasticityBeam
    youngs_modulus = 2.0
    poissons_ratio = 0.3
    shear_coefficient = 1.0
    block = '1 2 3'
  [../]
[]

[Constraints]
  [./tie_z]
    type = NodalFrictionalConstraint
    normal_force = 0.006
    tangential_penalty = 100
    friction_coefficient = 0.5
    boundary = 6
    secondary = 4
    variable = disp_z
  [../]
  [./tie_z2]
    type = NodalFrictionalConstraint
    normal_force = 0.006
    tangential_penalty = 100
    friction_coefficient = 0.2
    boundary = 6
    secondary = 5
    variable = disp_z
  [../]
[]

[Postprocessors]
  [./disp_x_1]
    type = NodalVariableValue
    nodeid = 1
    variable = disp_x
  [../]
  [./disp_x_2]
    type = NodalVariableValue
    nodeid = 2
    variable = disp_x
  [../]
  [./disp_z_1]
    type = NodalVariableValue
    nodeid = 1
    variable = disp_z
  [../]
  [./disp_z_2]
    type = NodalVariableValue
    nodeid = 2
    variable = disp_z
  [../]
[]

[Outputs]
  #file_base = '2_block_out'
  exodus = true
[]

Input Parameters
Input Files