# Elasticity

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,
locate_dofs_topological)
from dolfinx.fem.petsc import (apply_lifting, assemble_matrix, assemble_vector,
set_bc)
from dolfinx.io import XDMFFile
from dolfinx.mesh import (CellType, GhostMode, create_box,
locate_entities_boundary)
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[dofs] = -x1
basis[dofs] = x0
basis[dofs] = x2
basis[dofs] = -x0
basis[dofs] = x1
basis[dofs] = -x2

# Orthonormalise the six vectors
la.orthonormalize(ns)
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, ρ * ω**2 * x, 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),
np.isclose(x, 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])
A.assemble()


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]])
set_bc(b, [bc])


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

null_space = build_nullspace(V)
A.setNearNullSpace(null_space)


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)
solver.setFromOptions()

# Set matrix operator
solver.setOperators(A)


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)
solver.view()

# Scatter forward the solution vector to update ghost values
uh.x.scatter_forward()


## Post-processing

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)
sigma_vm_h.interpolate(sigma_vm_expr)


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:
file.write_mesh(msh)
file.write_function(uh)

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


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.