Step 4 - Multiple submeshes

Mesh

We again are using multiple mesh generators to set up a more complex mesh. You could also use a meshing software, such as Cubit or Gmsh to create your geometry and mesh - and will most definitely have to do so when modeling complex geometries for which no specialized mesh generators are provided. It is crucial to assign block and boundary IDs and names to your meshes so you can apply material models and boundary conditions.

Here we are using the familiar GeneratedMeshGenerator, but with a few more options than last time. Note how we're specifying the extent of the mesh with the "xmin" and "xmax" parameters (we keep the default value for "ymin", which is 0). We also use the "bias_y" parameter to have the element height in the mesh gradually shrink towards the top (you will see later why that is a good idea). "boundary_name_prefix" adds a prefix string to the names of the default boundaries that the GeneratedMeshGenerator sets up (left, right, top, bottom (for >=2D), front, and back (for 3D)). The generated block will create a mesh with the boundaries pillar1_left, pillar1_right, pillar1_top, and pillar1_bottom.

The generated2 generator will set up the second pillar and works very much like the first, except that we are also adding the "boundary_id_offset" to ensure that the boundaries of the second pillar have their own unique IDs (this is done by shifting the default IDs of the four boundaries by 4 so they don't overlap with the IDs of pillar1).

The MeshCollectionGenerator then combines the two separate pillar mesh objects into a single mesh object that contains all elements from both meshes. Note that this does not mean the two meshes are glued together or connected in any way! Also, in contrast to the previous step the mesh generators do not form a chain, but they form a tree structure. The important thing for MOOSE is that a single generator sits at the end of such a chain or root of such a tree (otherwise MOOSE will complain with an error message).

SolidMechanics QuasiStatic Physics

As discussed previously, when we expect large deformation we need to make sure we select the correct strain formulation. So here we select finite strain.

BCs

The boundary conditions should look familiar. Note how we can specify multiple boundaries for every boundary condition (or Pressure action).

Materials

We select ComputeFiniteStrainElasticStress as the elastic stress calculator for the finite strain formulation.

Executioner

Some more tweaks are made to the Executioner block:

• We disable "line_search". Line searches can accelerate the convergence of the linear system, but here it does more harm than good (check for yourself by commenting out this option).

• We add a predictor to accelerate the solve. The SimplePredictor extrapolates an initial guess for the current time step from the two previous time steps. Especially with a Newton solve a good initial guess can lead to drastically improved convergence.

Expected outcome

First off, run the simulation and look at the result.

What do you observe (does it meet your expectations)?

Click here for the answer.

Convergence

Getting a problem to converge optimally can be tricky. Try a few different things

• Remove all petsc options and check how the problem converges with the default ILU preconditioner

• comment out the line_search option

• remove the predictor

Check the consequence of these changes. You can inspect internal performance metrics of MOOSE by adding the option perf_graph = true in the [Outputs] block!

Iterative preconditioning

Check how the problem converges with the following PETSc options

petsc_options_iname = '-pc_type -pc_hypre_type'
petsc_options_value = 'hypre boomeramg'

This enables a very scalable algebraic multigrid (AMG) preconditioner, provided by the Hypre library.

Postprocessing results

MOOSE has a system of so called Postprocessors that can extract scalar quantities for a simulation while it runs. These quantities can be printed on the screen in real time or written to files for later analysis. You add postprocessors under the [Postprocessors] top level block.

File output of postprocessors is enabled by adding the csv = true option in the [Outputs] block.

Let's see if we can extract the x deflection of the left cantilever. It should be a positive value and the scalar we can extract is the maximum disp_x value in the simulation cell (the left cantilever has positive displacements as it bends right in the positive x direction, while the right cantilever has negative displacements as it bends left in the negative x direction). So we need a postprocessor object that gives us an extreme value of a given variable. Take a look at NodalExtremeValue and try to set it up to output the maximum positive x deflection.

Click here for the answer.

Sidebar: Volumetric locking

Volumetric locking can occur in mechanics simulations of near incompressible materials if the elements (and associated shape functions) cannot accommodate the incompressibility constraint.

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

• "uniform_refine" in the [Mesh] block

• "volumetric_locking_correction" in the solid mechanics quasi-static physics block

• "elem_type" in the GeneratedMeshGenerator blocks

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).

Click here for the sidebar on volumetric locking.

Once you've answered the questions and run this example we will move on to Step 1 of the contact tutorial, which builds on this step.