ComputeLagrangianStrain

Compute strain in Cartesian coordinates.

Overview

The ComputeLagrangianStrain class calculates the basic kinematic quantities used by the new mechanics kernels mechanics kernels. The theory section on the new material system describes this class's role in greater detail, the following gives a brief description.

The class calculates the strain measures available for the constitutive models to use to define the stress update and the kinematic tenors required to setup the stress equilibrium problem for large deformation simulations. The stabilize_strain averages the volumetric/dilatational part of these strain measures using an $var element = document.getElementById("moose-equation-6400ad67-635a-47a2-820f-5daf114b63bd");katex.render("\\bar{F}", element, {displayMode:false,throwOnError:false});$ stabilization approach to prevent locking of linear quad and hex elements for problems experiencing incompressible deformation. This class also adds in the extra deformation gradient imposed by the homogenization system.

The calculations differ somewhat between small and large deformation kinematic theory. The large_kinematics flag selects between the two theories. This flag should be consistent between the strain calculator and the kernels. The stabilize_strain flag determines if the calculator uses the $var element = document.getElementById("moose-equation-83c46e52-0ff4-4e03-83f0-6aea5f39a9af");katex.render("\\bar{F}", element, {displayMode:false,throwOnError:false});$ stabilization Souza Neto et al. (1996).

Step-by-step the class:

Calculates the deformation gradient as $var element = document.getElementById("moose-equation-b59589f3-25c4-4d93-9166-b4c36e0c0d9e");katex.render("F_{iJ} = \\delta_{iJ} + \\frac{\\partial u_i}{\\partial X_J}", element, {displayMode:false,throwOnError:false});$ for large deformations or $var element = document.getElementById("moose-equation-677ed23f-5ac3-4d63-b929-17d247dfd16a");katex.render("F_{ij} = \\delta_{ij} + \\frac{\\partial u_i}{\\partial x_j}", element, {displayMode:false,throwOnError:false});$ for small deformations.
If stabilize_strain is set, average the volumetric parts of the deformation gradient, as described in the stabilization documentation.
If active, add the extra gradient to this displacement-based deformation gradient calculated in the ComputeLagrangianHomogenizedLagrangianStrain.
For large deformations only, calculate the kinematic tensors used to define the equilibrium problem in the right frame of reference in the kernels. For small deformations these measures are set to the identity.
Calculate the increment in the spatial velocity gradient: $var element = document.getElementById("moose-equation-2b0e9f1a-a1ef-4f29-9371-68863eb22baa");katex.render("\\Delta l_{ij} = \\delta_{ij} - F^{(n)}_{iK} F^{(n+1)-1}_{Kj}", element, {displayMode:false,throwOnError:false});$ for large deformations and $var element = document.getElementById("moose-equation-09e2adbd-5271-4c70-9405-8df8bab84459");katex.render("\\Delta l_{ij} = F_{ij}^{(new)} - F_{ij}^{(old)}", element, {displayMode:false,throwOnError:false});$ for small deformations.
Calculate the total strain increment as $var element = document.getElementById("moose-equation-02d21ee2-7793-4d0d-8dc3-ee3a9f4ac1d1");katex.render("\\Delta d_{ij} = \\frac{1}{2} \\left( l_{ij} + l_{ji} \\right)", element, {displayMode:false,throwOnError:false});$ .
Sum up and subtract the eigenstrain increment over the step to fine the mechanical strain increment, $var element = document.getElementById("moose-equation-754e65e9-14a6-49bb-a76a-46863af00bb9");katex.render("\\Delta \\varepsilon_{ij} = \\Delta d_{ij} - \\Delta \\varepsilon_{ij}^{(eigen)}", element, {displayMode:false,throwOnError:false});$ .
Use the previous step values of total and mechanical strain to calculate the updated strain values: $var element = document.getElementById("moose-equation-d767991e-8d47-435b-b7dd-739c50ce66d2");katex.render("d_{ij}^{(new)} = d_{ij}^{(old)} + \\Delta d_{ij}", element, {displayMode:false,throwOnError:false});$ and $var element = document.getElementById("moose-equation-0555d6be-176f-4254-bee3-7c7c62a9aeb8");katex.render("\\varepsilon_{ij} = \\varepsilon_{ij}^{(old)} + \\Delta \\varepsilon_{ij}", element, {displayMode:false,throwOnError:false});$ .

note

The strain calculator does not apply the eigenstrains to the deformation gradient, only the incremental and integrated strain measures.

tip

stabilize_strain should be set to true for problems using linear quad or hex elements where the material model produces incompressible or near-incompressible deformation. It should be set to false for higher order elements. The $var element = document.getElementById("moose-equation-75fac068-9518-417c-bd73-3160a5ef416b");katex.render("\\bar{F}", element, {displayMode:false,throwOnError:false});$ stabilization is ineffective for linear triangle or tet elements and these elements should not be used for incompressible or near-incompressible problems.

The calculator requires use_displaced_mesh=false and enforces this with an error.

Example Input File Syntax

The following example sets up the ComputeLagrangianStrain object for a large deformation problem without stabilization. For small deformations the only change would be large_kinematics=false.

[Materials]
  [elastic_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 1000.0
    poissons_ratio = 0.25
  []
  [compute_stress]
    type = ComputeLagrangianLinearElasticStress
    large_kinematics = true
  []
  [compute_strain]
    type = ComputeLagrangianStrain
    displacements = 'disp_x disp_y disp_z'
    large_kinematics = true
  []
[]

Input Parameters

displacementsDisplacement variables
C++ Type:std::vector<VariableName>
Controllable:No
Description:Displacement variables

Required Parameters

base_nameMaterial property base name
C++ Type:std::string
Controllable:No
Description:Material property base name
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
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
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
Options:NONE, ELEMENT, SUBDOMAIN
Controllable:No
Description:When ELEMENT, MOOSE will only call computeQpProperties() for the 0th quadrature point, and then copy that value to the other qps.When SUBDOMAIN, MOOSE will only call computeQpProperties() for the 0th quadrature point, and then copy that value to the other qps. Evaluations on element qps will be skipped
declare_suffixAn optional suffix parameter that can be appended to any declared properties. The suffix will be prepended with a '_' character.
C++ Type:MaterialPropertyName
Controllable:No
Description:An optional suffix parameter that can be appended to any declared properties. The suffix will be prepended with a '_' character.
eigenstrain_namesList of eigenstrains to account for
C++ Type:std::vector<MaterialPropertyName>
Controllable:No
Description:List of eigenstrains to account for
homogenization_gradient_namesList of homogenization gradients to add to the displacement gradient
C++ Type:std::vector<MaterialPropertyName>
Controllable:No
Description:List of homogenization gradients to add to the displacement gradient
large_kinematicsFalseUse large displacement kinematics in the kernel.
Default:False
C++ Type:bool
Controllable:No
Description:Use large displacement kinematics in the kernel.
prop_getter_suffixAn optional suffix parameter that can be appended to any attempt to retrieve/get material properties. The suffix will be prepended with a '_' character.
C++ Type:MaterialPropertyName
Controllable:No
Description:An optional suffix parameter that can be appended to any attempt to retrieve/get material properties. The suffix will be prepended with a '_' character.
stabilize_strainFalseAverage the volumetric strains
Default:False
C++ Type:bool
Controllable:No
Description:Average the volumetric strains

Optional Parameters

control_tagsAdds user-defined labels for accessing object parameters via control logic.
C++ Type:std::vector<std::string>
Controllable:No
Description:Adds user-defined labels for accessing object parameters via control logic.
enableTrueSet the enabled status of the MooseObject.
Default:True
C++ Type:bool
Controllable:Yes
Description:Set the enabled status of the MooseObject.
implicitTrueDetermines whether this object is calculated using an implicit or explicit form
Default:True
C++ Type:bool
Controllable:No
Description:Determines whether this object is calculated using an implicit or explicit form
seed0The seed for the master random number generator
Default:0
C++ Type:unsigned int
Controllable:No
Description:The seed for the master random number generator

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>
Controllable:No
Description:List of material properties, from this material, to output (outputs must also be defined to an output type)
outputsnone Vector of output names where you would like to restrict the output of variables(s) associated with this object
Default:none
C++ Type:std::vector<OutputName>
Controllable:No
Description:Vector of output names where you would like to restrict the output of variables(s) associated with this object

Outputs Parameters

References

EA de Souza Neto, D Perić, M Dutko, and DRJ Owen. Design of simple low order finite elements for large strain analysis of nearly incompressible solids. International Journal of Solids and Structures, 33(20-22):3277–3296, 1996.

@article{de1996design,
    author = "de Souza Neto, EA and Peri{\'c}, D and Dutko, M and Owen, DRJ",
    title = "Design of simple low order finite elements for large strain analysis of nearly incompressible solids",
    journal = "International Journal of Solids and Structures",
    volume = "33",
    number = "20-22",
    pages = "3277--3296",
    year = "1996",
    publisher = "Elsevier"
}

(moose/modules/tensor_mechanics/test/tests/lagrangian/cartesian/updated/patch/large_patch.i)

[Mesh]
  [base]
    type = FileMeshGenerator
    file = 'patch.xda'
  []
  [sets]
    input = base
    type = SideSetsFromPointsGenerator
    new_boundary = 'left right bottom top back front'
    points = '    0 0.5 0.5
                  1 0.5 0.5
                  0.5 0.0 0.5
               '
             '   0.5 1.0 0.5
                  0.5 0.5 0.0
                  0.5 0.5 1.0'
  []
[]

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

[Variables]
  [disp_x]
  []
  [disp_y]
  []
  [disp_z]
  []
[]

[Kernels]
  [sdx]
    type = UpdatedLagrangianStressDivergence
    variable = disp_x
    displacements = 'disp_x disp_y disp_z'
    component = 0
    use_displaced_mesh = true
    large_kinematics = true
  []
  [sdy]
    type = UpdatedLagrangianStressDivergence
    variable = disp_y
    displacements = 'disp_x disp_y disp_z'
    component = 1
    use_displaced_mesh = true
    large_kinematics = true
  []
  [sdz]
    type = UpdatedLagrangianStressDivergence
    variable = disp_z
    displacements = 'disp_x disp_y disp_z'
    component = 2
    use_displaced_mesh = true
    large_kinematics = true
  []
[]

[AuxVariables]
  [strain_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_yy]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_zz]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_xy]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_xz]
    order = CONSTANT
    family = MONOMIAL
  []
  [strain_yz]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_xx]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_yy]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_zz]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_xy]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_yz]
    order = CONSTANT
    family = MONOMIAL
  []
  [stress_xz]
    order = CONSTANT
    family = MONOMIAL
  []
[]

[AuxKernels]
  [stress_xx]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_xx
    index_i = 0
    index_j = 0
    execute_on = timestep_end
  []
  [stress_yy]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_yy
    index_i = 1
    index_j = 1
    execute_on = timestep_end
  []
  [stress_zz]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_zz
    index_i = 2
    index_j = 2
    execute_on = timestep_end
  []
  [stress_xy]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_xy
    index_i = 0
    index_j = 1
    execute_on = timestep_end
  []
  [stress_xz]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_xz
    index_i = 0
    index_j = 2
    execute_on = timestep_end
  []
  [stress_yz]
    type = RankTwoAux
    rank_two_tensor = cauchy_stress
    variable = stress_yz
    index_i = 1
    index_j = 2
    execute_on = timestep_end
  []

  [strain_xx]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_xx
    index_i = 0
    index_j = 0
    execute_on = timestep_end
  []
  [strain_yy]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_yy
    index_i = 1
    index_j = 1
    execute_on = timestep_end
  []
  [strain_zz]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_zz
    index_i = 2
    index_j = 2
    execute_on = timestep_end
  []
  [strain_xy]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_xy
    index_i = 0
    index_j = 1
    execute_on = timestep_end
  []
  [strain_xz]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_xz
    index_i = 0
    index_j = 2
    execute_on = timestep_end
  []
  [strain_yz]
    type = RankTwoAux
    rank_two_tensor = mechanical_strain
    variable = strain_yz
    index_i = 1
    index_j = 2
    execute_on = timestep_end
  []
[]

[BCs]
  [left]
    type = DirichletBC
    preset = true
    variable = disp_x
    boundary = left
    value = 0.0
  []

  [bottom]
    type = DirichletBC
    preset = true
    variable = disp_y
    boundary = bottom
    value = 0.0
  []

  [back]
    type = DirichletBC
    preset = true
    variable = disp_z
    boundary = back
    value = 0.0
  []

  [front]
    type = DirichletBC
    preset = true
    variable = disp_z
    boundary = front
    value = 0.1
  []
[]

[Materials]
  [elastic_tensor]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 1000.0
    poissons_ratio = 0.25
  []
  [compute_stress]
    type = ComputeLagrangianLinearElasticStress
    large_kinematics = true
  []
  [compute_strain]
    type = ComputeLagrangianStrain
    displacements = 'disp_x disp_y disp_z'
    large_kinematics = true
  []
[]

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

[Executioner]
  type = Transient
  dt = 1

  solve_type = 'newton'

  petsc_options_iname = -pc_type
  petsc_options_value = lu

  nl_abs_tol = 1e-10
  nl_rel_tol = 1e-10

  end_time = 1
  dtmin = 1.0
[]

[Outputs]
  exodus = true
[]