Step 1 - Basic Thermal/Mechanical Coupling
In the tutorials for the Heat Conduction and Tensor Mechanics modules, basic thermal and mechanical problems were developed. The Heat Conduction tutorial culminated with a model that solves the heat equation on a simple rectangular domain, including terms for heat conduction, time-dependent effects, and volumetric heating.
The Tensor Mechanics tutorial includes a model that shows how thermal expansion can be accounted for using a prescribed temperature field.
The model shown here builds on these thermal and mechanical models by simultaneously solving for the thermal and mechanical response. As will be evident from examining this file, coupled physics models are defined by combining the components from all of the physics in a single input file, and defining interactions between the physics.
#
# Single block coupled thermal/mechanical
# https://mooseframework.inl.gov/modules/combined/tutorials/introduction/thermoech_step01.html
#
[GlobalParams]
displacements = 'disp_x disp_y'
[]
[Mesh]
[generated]
type = GeneratedMeshGenerator
dim = 2
nx = 10
ny = 10
xmax = 2
ymax = 1
[]
[pin]
type = ExtraNodesetGenerator
input = generated
new_boundary = pin
coord = '0 0 0'
[]
[]
[Variables]
[T]
initial_condition = 300.0
[]
[]
[Kernels]
[heat_conduction]
type = HeatConduction
variable = T
[]
[time_derivative]
type = HeatConductionTimeDerivative
variable = T
[]
[heat_source]
type = HeatSource
variable = T
value = 5e4
[]
[]
[Modules/TensorMechanics/Master]
[all]
add_variables = true
strain = FINITE
automatic_eigenstrain_names = true
generate_output = 'vonmises_stress'
[]
[]
[Materials]
[thermal]
type = HeatConductionMaterial
thermal_conductivity = 45.0
specific_heat = 0.5
[]
[density]
type = GenericConstantMaterial
prop_names = 'density'
prop_values = 8000.0
[]
[elasticity]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 1e9
poissons_ratio = 0.3
[]
[expansion1]
type = ComputeThermalExpansionEigenstrain
temperature = T
thermal_expansion_coeff = 0.001
stress_free_temperature = 300
eigenstrain_name = thermal_expansion
[]
[stress]
type = ComputeFiniteStrainElasticStress
[]
[]
[BCs]
[t_left]
type = DirichletBC
variable = T
value = 300
boundary = 'left'
[]
[t_right]
type = FunctionDirichletBC
variable = T
function = '300+5*t'
boundary = 'right'
[]
[pin_x]
type = DirichletBC
variable = disp_x
boundary = pin
value = 0
[]
[bottom_y]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0
[]
[]
[Preconditioning]
[smp]
type = SMP
full = true
[]
[]
[Executioner]
type = Transient
petsc_options_iname = '-pc_type'
petsc_options_value = 'lu'
end_time = 5
dt = 1
[]
[Outputs]
exodus = true
[]
Input file
Variables
The Variables block in this input files looks just like it does for a thermal-only problem. A single variable,T, is defined, with an initial condition of 300 Kelvin. An obvious question is why no variables are defined for mechanics. Coupled physics problems are usually defined in MOOSE by defining multiple variables and their associated Kernels. This is actually done in this model, but the Modules/TensorMechanics/Master Action block automatically sets up the displacement variables, so they don't explicitly appear in the Variables block in the input file. That Action sets up variables with the names defined by the displacements parameter, which is defined in GlobalParams. In this case, there are thus three solution variables: T, disp_x, and disp_y.
[Variables]
[T]
initial_condition = 300.0
[]
[]
Kernels
Similar to the Variables block, only the kernels related to the temperature solution are defined in the Kernels block in this case. This is again due to the fact that the Modules/TensorMechanics/Master Action automates setting up the Kernels associated with the displacement variables, so they don't explicitly appear in the input file. This model includes kernels for the conduction, time derivative, and volumetric terms in the heat equation.
[Kernels]
[heat_conduction]
type = HeatConduction
variable = T
[]
[time_derivative]
type = HeatConductionTimeDerivative
variable = T
[]
[heat_source]
type = HeatSource
variable = T
value = 5e4
[]
[]
Modules/TensorMechanics/Master
This block automates the process of setting up multiple objects related to solution of a mechanics problem. The objects set up by this block include the Variables and Kernels for the displacement solution, the Material that computes the strain, and objects associated with outputing stresses. In addition to simplifying the input, this ensures that a consistent set of options are selected for the desired formulation.
[all]
add_variables = true
strain = FINITE
automatic_eigenstrain_names = true
generate_output = 'vonmises_stress'
[]
Materials
Material properties must be defined for both the thermal and mechanical models. For the thermal model, the thermal conductivity, specific heat, and density are needed. For the mechanical model, the elasticity tensor, thermal eigenstrain, and stress are computed. The models listed here are essentially a combination of the models that were used for the single-physics thermal and mechanical models.
[Materials]
[thermal]
type = HeatConductionMaterial
thermal_conductivity = 45.0
specific_heat = 0.5
[]
[density]
type = GenericConstantMaterial
prop_names = 'density'
prop_values = 8000.0
[]
[elasticity]
type = ComputeIsotropicElasticityTensor
youngs_modulus = 1e9
poissons_ratio = 0.3
[]
[expansion1]
type = ComputeThermalExpansionEigenstrain
temperature = T
thermal_expansion_coeff = 0.001
stress_free_temperature = 300
eigenstrain_name = thermal_expansion
[]
[stress]
type = ComputeFiniteStrainElasticStress
[]
[]
BCs
Boundary conditions must be prescribed for the individual physics in the same way that they are for single-physics models. The variable parameter in each of these boundary condition blocks defines the variable that the boundary condition is applied to.
[BCs]
[t_left]
type = DirichletBC
variable = T
value = 300
boundary = 'left'
[]
[t_right]
type = FunctionDirichletBC
variable = T
function = '300+5*t'
boundary = 'right'
[]
[pin_x]
type = DirichletBC
variable = disp_x
boundary = pin
value = 0
[]
[bottom_y]
type = DirichletBC
variable = disp_y
boundary = bottom
value = 0
[]
[]
Preconditioning
The Preconditioning block is used here to define that a full matrix with coupling between all variables is used for preconditioning. This is more memory intensive than the default block-diagonal matrix, but typically results in improved convergence for multiphysics models.
The remaining blocks (Executioner and Outputs) are the same as they would be for single-physics models in this case.
Questions
Where is coupling introduced between the thermal and mechanical solutions in this model?
Once you've answered the questions and run this example we will move on to Step 2 in which we introduce a third block participating in the contact problem.