Copyright © 2020-2022 Garth N. Wells and Michal Habera

This demo solves the equations of static linear elasticity using a smoothed aggregation algebraic multigrid solver. The demo is implemented in demo_elasticity.py.

from contextlib import ExitStack

import numpy as np

import ufl
from dolfinx import la
from dolfinx.fem import (Expression, Function, FunctionSpace,
                         VectorFunctionSpace, dirichletbc, form,
from dolfinx.fem.petsc import (apply_lifting, assemble_matrix, assemble_vector,
from dolfinx.io import XDMFFile
from dolfinx.mesh import (CellType, GhostMode, create_box,
from ufl import dx, grad, inner

from mpi4py import MPI
from petsc4py import PETSc

dtype = PETSc.ScalarType

Operator’s nullspace

Smooth aggregation algebraic multigrid solvers require the so-called ‘near-nullspace’, which is the nullspace of the operator in the absence of boundary conditions. The below function builds a PETSc NullSpace object. For this 3D elasticity problem the nullspace is spanned by six vectors – three translation modes and three rotation modes.

def build_nullspace(V):
    """Build PETSc nullspace for 3D elasticity"""

    # Create list of vectors for building nullspace
    index_map = V.dofmap.index_map
    bs = V.dofmap.index_map_bs
    ns = [la.create_petsc_vector(index_map, bs) for i in range(6)]
    with ExitStack() as stack:
        vec_local = [stack.enter_context(x.localForm()) for x in ns]
        basis = [np.asarray(x) for x in vec_local]

        # Get dof indices for each subspace (x, y and z dofs)
        dofs = [V.sub(i).dofmap.list.array for i in range(3)]

        # Build the three translational rigid body modes
        for i in range(3):
            basis[i][dofs[i]] = 1.0

        # Build the three rotational rigid body modes
        x = V.tabulate_dof_coordinates()
        dofs_block = V.dofmap.list.array
        x0, x1, x2 = x[dofs_block, 0], x[dofs_block, 1], x[dofs_block, 2]
        basis[3][dofs[0]] = -x1
        basis[3][dofs[1]] = x0
        basis[4][dofs[0]] = x2
        basis[4][dofs[2]] = -x0
        basis[5][dofs[2]] = x1
        basis[5][dofs[1]] = -x2

    # Orthonormalise the six vectors
    assert la.is_orthonormal(ns)

    return PETSc.NullSpace().create(vectors=ns)

Create a box Mesh

msh = create_box(MPI.COMM_WORLD, [np.array([0.0, 0.0, 0.0]),
                                  np.array([2.0, 1.0, 1.0])], [16, 16, 16],
                 CellType.tetrahedron, GhostMode.shared_facet)

Create a centripetal source term (\(f = \rho \omega^2 [x_0, \, x_1]\))

ω, ρ = 300.0, 10.0
x = ufl.SpatialCoordinate(msh)
f = ufl.as_vector((ρ * ω**2 * x[0], ρ * ω**2 * x[1], 0.0))

Set the elasticity parameters and create a function that computes and expression for the stress given a displacement field.

E = 1.0e9
ν = 0.3
μ = E / (2.0 * (1.0 + ν))
λ = E * ν / ((1.0 + ν) * (1.0 - 2.0 * ν))

def σ(v):
    """Return an expression for the stress σ given a displacement field"""
    return 2.0 * μ * ufl.sym(grad(v)) + λ * ufl.tr(ufl.sym(grad(v))) * ufl.Identity(len(v))

A function space space is created and the elasticity variational problem defined:

V = VectorFunctionSpace(msh, ("Lagrange", 1))
u = ufl.TrialFunction(V)
v = ufl.TestFunction(V)
a = form(inner(σ(u), grad(v)) * dx)
L = form(inner(f, v) * dx)

A homogeneous (zero) boundary condition is created on \(x_0 = 0\) and \(x_1 = 1\) by finding all boundary facets on \(x_0 = 0\) and \(x_1 = 1\), and then creating a Dirichlet boundary condition object.

facets = locate_entities_boundary(msh, dim=2,
                                  marker=lambda x: np.logical_or(np.isclose(x[0], 0.0),
                                                                 np.isclose(x[1], 1.0)))
bc = dirichletbc(np.zeros(3, dtype=dtype),
                 locate_dofs_topological(V, entity_dim=2, entities=facets), V=V)

Assemble and solve

The bilinear form a is assembled into a matrix A, with modifications for the Dirichlet boundary conditions. The line A.assemble() completes any parallel communication required to computed the matrix.

A = assemble_matrix(a, bcs=[bc])

The linear form L is assembled into a vector b, and then modified by apply_lifting to account for the Dirichlet boundary conditions. After calling apply_lifting, the method ghostUpdate accumulates entries on the owning rank, and this is followed by setting the boundary values in b.

b = assemble_vector(L)
apply_lifting(b, [a], bcs=[[bc]])
b.ghostUpdate(addv=PETSc.InsertMode.ADD, mode=PETSc.ScatterMode.REVERSE)
set_bc(b, [bc])

Create the near-nullspace and attach it to the PETSc matrix:

null_space = build_nullspace(V)

Set PETSc solver options, create a PETSc Krylov solver, and attach the matrix A to the solver:

# Set solver options
opts = PETSc.Options()
opts["ksp_type"] = "cg"
opts["ksp_rtol"] = 1.0e-10
opts["pc_type"] = "gamg"

# Use Chebyshev smoothing for multigrid
opts["mg_levels_ksp_type"] = "chebyshev"
opts["mg_levels_pc_type"] = "jacobi"

# Improve estimate of eigenvalues for Chebyshev smoothing
opts["mg_levels_esteig_ksp_type"] = "cg"
opts["mg_levels_ksp_chebyshev_esteig_steps"] = 20

# Create PETSc Krylov solver and turn convergence monitoring on
solver = PETSc.KSP().create(msh.comm)

# Set matrix operator

Create a solution Function, uh, and solve:

uh = Function(V)

# Set a monitor, solve linear system, and display the solver
# configuration
solver.setMonitor(lambda _, its, rnorm: print(f"Iteration: {its}, rel. residual: {rnorm}"))
solver.solve(b, uh.vector)

# Scatter forward the solution vector to update ghost values


The computed solution is now post-processed.

Expressions for the deviatoric and Von Mises stress are defined:

sigma_dev = σ(uh) - (1 / 3) * ufl.tr(σ(uh)) * ufl.Identity(len(uh))
sigma_vm = ufl.sqrt((3 / 2) * inner(sigma_dev, sigma_dev))

Next, the Von Mises stress is interpolated in a piecewise-constant space by creating an Expression that is interpolated into the Function sigma_vm_h.

W = FunctionSpace(msh, ("Discontinuous Lagrange", 0))
sigma_vm_expr = Expression(sigma_vm, W.element.interpolation_points())
sigma_vm_h = Function(W)

Save displacement field uh and the Von Mises stress sigma_vm_h in XDMF format files.

with XDMFFile(msh.comm, "out_elasticity/displacements.xdmf", "w") as file:

# Save solution to XDMF format
with XDMFFile(msh.comm, "out_elasticity/von_mises_stress.xdmf", "w") as file:

Finally, we compute the \(L^2\) norm of the displacement solution vector. This is a collective operation (i.e., the method norm must be called from all MPI ranks), but we print the norm only on rank 0.

unorm = uh.x.norm()
if msh.comm.rank == 0:
    print("Solution vector norm:", unorm)

The solution vector norm can be a useful check that the solver is computing the same result when running in serial and in parallel.