Step 4a - Volumetric locking

Keep the postprocessing modifications from the previous question, set the "poissons_ratio" of the cantilevers to 0.49. Then add and modify the following parameters

For convenience all those parameters may be listed under [GlobalParams] instead. Compare first order QUAD4 elements to second order QUAD8 elements, compare the cantilever deflection with and without volumetric locking correction (with QUAD4 elements), and compare the result for different levels of uniform refinement (1, 2, 3, 4).

#
# We study the effects of volumetric locking
# https://mooseframework.inl.gov/modules/solid_mechanics/tutorials/introduction/answer04b.html
#

[GlobalParams]
  displacements = 'disp_x disp_y'
  # elem_type applies to the GeneratedMeshGenerator blocks
  elem_type = QUAD4
  # volumetric_locking_correction applies to the SolidMechanics QuasiStatic Physics
  volumetric_locking_correction = false
  # uniform_refine applies to the final mesh
  uniform_refine = 0
[]

[Mesh]
  [generated1]
    type = GeneratedMeshGenerator
    dim = 2
    nx = 5
    ny = 15
    xmin = -0.6
    xmax = -0.1
    ymax = 5
    bias_y = 0.9
    boundary_name_prefix = pillar1
  []
  [generated2]
    type = GeneratedMeshGenerator
    dim = 2
    nx = 4
    ny = 15
    xmin = 0.1
    xmax = 0.6
    ymax = 5
    bias_y = 0.9
    boundary_name_prefix = pillar2
    boundary_id_offset = 4
  []
  [collect_meshes]
    type = MeshCollectionGenerator
    inputs = 'generated1 generated2'
  []
[]

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

[BCs]
  [bottom_x]
    type = DirichletBC
    variable = disp_x
    boundary = 'pillar1_bottom pillar2_bottom'
    value = 0
  []
  [bottom_y]
    type = DirichletBC
    variable = disp_y
    boundary = 'pillar1_bottom pillar2_bottom'
    value = 0
  []
  [Pressure]
    [sides]
      boundary = 'pillar1_left pillar2_right'
      function = 1e4*t
    []
  []
[]

[Materials]
  [elasticity]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 1e9
    # near incopmpressible material
    poissons_ratio = 0.49
  []
  [stress]
    type = ComputeFiniteStrainElasticStress
  []
[]

[Postprocessors]
  [x_deflection]
    type = NodalExtremeValue
    value_type = max
    variable = disp_x
  []
[]

[Executioner]
  type = Transient
  solve_type = NEWTON
  line_search = none
  petsc_options_iname = '-pc_type'
  petsc_options_value = 'lu'
  end_time = 5
  dt = 0.5
  [Predictor]
    type = SimplePredictor
    scale = 1
  []
[]

[Outputs]
  exodus = true
  csv = true
[]
(moose/modules/solid_mechanics/tutorials/introduction/mech_step04a.i)

We can run the various combinations of first/second order elements, active/deactivated volumetric locking correction, and levels of refinement and plot the resulting data.

Note that you can override input file parameters from the command line! That means you can run all the cases plotted below using these commands:


../../solid_mechanics-opt -i mech_step04a.i GlobalParams/elem_type=QUAD4
../../solid_mechanics-opt -i mech_step04a.i GlobalParams/elem_type=QUAD4 GlobalParams/volumetric_locking_correction=true
mpirun -n 4 ../../solid_mechanics-opt -i mech_step04a.i GlobalParams/elem_type=QUAD4 GlobalParams/volumetric_locking_correction=true GlobalParams/uniform_refine=1
mpirun -n 4 ../../solid_mechanics-opt -i mech_step04a.i GlobalParams/elem_type=QUAD8
mpirun -n 8 ../../solid_mechanics-opt -i mech_step04a.i GlobalParams/elem_type=QUAD4 GlobalParams/volumetric_locking_correction=true GlobalParams/uniform_refine=4
mpirun -n 8 ../../solid_mechanics-opt -i mech_step04a.i GlobalParams/elem_type=QUAD8 GlobalParams/uniform_refine=2

The point here is to make you aware that volumetric locking can occur in first order elements with certain material properties. It can be alleviated through

  • Refinement

  • Use of higher order elements (QUAD8)

  • Use of volumetric locking correction

Users are encouraged to carefully check their results through convergence studies.