Global Strain

The global strain system enables capturing the volume change, shear deformation etc. while still maintaining the periodicity. It relaxes the stresses along the periodic directions and allows the corresponding deformation. This, combined with the periodic displacement, enforces the strain periodicity.

The global strain is computed by setting integral of each of the stress components $\sigma_{ij}$ in the periodic direction to zero such that

$\int_\Omega {(\sigma_{ij} - \sigma^0_{ij})} d\Omega = 0$

Here, indices $i$ and $j$ corresponds to the periodic directions and associated periodic displacement components, respectively. $\sigma^0_{ij}$ denotes the components of the stress tensor representing the applied loads in the periodic directions. The components of the global strain are considered constant over the whole domain.

The total strain $\epsilon_{ij}^{total}$ at any point is calculated considering the contribution of the global strain tensor as,

$\epsilon_{ij}^{total} = \epsilon_{ij} + \epsilon_{ij}^{g} - \epsilon_{ij}^{0}$

where $\epsilon_{ij}$ are the strain components calculated from the displacement gradients, $\epsilon_{ij}^g$ are the global strain components, and $\epsilon_{ij}^0$ are the eigen strain components. An additional displacement field $\boldsymbol u^g$ is generated to visualize the effect of the global strain as

$\boldsymbol {u}^g = (\boldsymbol {r} - \boldsymbol {r}_{0}) \boldsymbol{\epsilon}^g$

where $\boldsymbol {r}$ is the position vector, $\boldsymbol{r}_{0}$ is the location of the reference point, and $\boldsymbol{\epsilon}^g$ is the global strain tensor. The reference point could be any fixed ( $\boldsymbol {u}^{total} = \boldsymbol {0}$ ) point in the domain. For maintaining periodicity, it is recommended to fix the center point of the simulation domain as the reference point.

The total displacement is represented as

$\boldsymbol {u}^{total} = \boldsymbol {u} + \boldsymbol {u}^g$

where $\boldsymbol u$ is the local displacement field calculated from the mechanical equilibrium.

GlobalStrainAction can be used to set up the model for global strain and corresponding displacement calculation. This action can be created using the following syntax.

Example Input File Syntax

[./GlobalStrain]
  [./global_strain]
    scalar_global_strain = global_strain
    displacements = 'u_x u_y u_z'
    auxiliary_displacements = 'disp_x disp_y disp_z'
    global_displacements = 'ug_x ug_y ug_z'
  [../]
[../]

Subblocks

The subblocks of the GlobalStrain action triggers MOOSE objects to be built. It can be applied to the whole domain using a single subblock

[Physics/SolidMechanics/GlobalStrain]
  [./all]
    ...
  [../]
[]

or multiple subblocks can be used to apply block restrictions to the objects

[Physics/SolidMechanics/GlobalStrain]
  [./block_a]
    ...
  [../]
  [./block_b]
    ...
  [../]
[]

Available Actions

Solid Mechanics App
GlobalStrainActionSet up the GlobalStrainAction environment

(contrib/moose/modules/solid_mechanics/test/tests/global_strain/global_strain_action.i)

[Mesh]
  [generated_mesh]
    type = GeneratedMeshGenerator
    dim = 3
    nx = 2
    ny = 2
    nz = 2
    xmin = -0.5
    xmax = 0.5
    ymin = -0.5
    ymax = 0.5
    zmin = -0.5
    zmax = 0.5
  []
  [cnode]
    type = ExtraNodesetGenerator
    coord = '0 -0.5 0'
    new_boundary = 100
    input = generated_mesh
  []
[]

[GlobalParams]
  displacements = 'u_x u_y u_z'
  block = 0
[]

[Variables]
  [./global_strain]
    order = SIXTH
    family = SCALAR
  [../]
[]

[Physics]
  [SolidMechanics]
    # QuasiStatic action for generating the tensor mechanics kernels, variables,
    # strain calculation material, and the auxilliary system for visualization
    [QuasiStatic]
      [./stress_div]
        strain = SMALL
        add_variables = true
        global_strain = global_strain #global strain contribution
        generate_output = 'strain_xx strain_xy strain_yy stress_xx stress_xy
                           stress_yy vonmises_stress'
      [../]
    [../]
    # GlobalStrain action for generating the objects associated with the global
    # strain calculation and associated displacement visualization
    [./GlobalStrain]
      [./global_strain]
        scalar_global_strain = global_strain
        displacements = 'u_x u_y u_z'
        auxiliary_displacements = 'disp_x disp_y disp_z'
        global_displacements = 'ug_x ug_y ug_z'
      [../]
    [../]
  [../]
[]

[BCs]
  [./Periodic]
    [./all]
      auto_direction = 'z'
      variable = 'u_x u_y u_z'
    [../]
  [../]

  # fix center point location
  [./centerfix_x]
    type = DirichletBC
    boundary = 100
    variable = u_x
    value = 0
  [../]
  [./centerfix_z]
    type = DirichletBC
    boundary = 100
    variable = u_z
    value = 0
  [../]
  # applied displacement
  [./appl_y]
    type = DirichletBC
    boundary = top
    variable = u_y
    value = 0.033
  [../]
  [./fix_y]
    type = DirichletBC
    boundary = bottom
    variable = u_y
    value = 0
  [../]
[]

[Materials]
  [./elasticity_tensor]
    type = ComputeElasticityTensor
    block = 0
    C_ijkl = '7 0.33'
    fill_method = symmetric_isotropic_E_nu
  [../]
  [./stress]
    type = ComputeLinearElasticStress
  [../]
[]

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

[Executioner]
  type = Transient
  scheme = bdf2
  solve_type = 'PJFNK'

  line_search = basic

  petsc_options_iname = '-pc_type -ksp_gmres_restart -sub_ksp_type -sub_pc_type -pc_asm_overlap'
  petsc_options_value = 'asm         31   preonly   lu      1'

  l_max_its = 30
  nl_max_its = 12

  l_tol = 1.0e-4

  nl_rel_tol = 1.0e-6
  nl_abs_tol = 1.0e-10

  start_time = 0.0
  num_steps = 2
[]

[Outputs]
  exodus = true
[]

Example Input File Syntax
Subblocks
Available Actions