Elasticity equation¶
Copyright (C) 2020 Garth N. Wells and Michal Habera
This demo solves the equations of static linear elasticity. The solver uses smoothed aggregation algebraic multigrid.
from contextlib import ExitStack
import os
import numpy as np
from mpi4py import MPI
from petsc4py import PETSc
import dolfinx
from dolfinx import BoxMesh, DirichletBC, Function, VectorFunctionSpace, cpp
from dolfinx.cpp.mesh import CellType
from dolfinx.fem import (Form, apply_lifting, assemble_matrix, assemble_vector,
locate_dofs_geometrical, set_bc)
from dolfinx.io import XDMFFile
from dolfinx.la import VectorSpaceBasis
from ufl import (Identity, SpatialCoordinate, TestFunction, TrialFunction,
as_vector, dx, grad, inner, sym, tr)
Nullspace and problem setup¶
Prepare a helper which builds PETSc’ NullSpace. Nullspace (or near nullspace) is needed to improve the performance of algebraic multigrid.
In the case of small deformation linear elasticity the nullspace contains rigid body modes.
def build_nullspace(V):
"""Function to build null space for 3D elasticity"""
# Create list of vectors for null space
index_map = V.dofmap.index_map
nullspace_basis = [cpp.la.create_vector(index_map) for i in range(6)]
with ExitStack() as stack:
vec_local = [stack.enter_context(x.localForm()) for x in nullspace_basis]
basis = [np.asarray(x) for x in vec_local]
# Build translational null space basis
for i in range(3):
basis[i][V.sub(i).dofmap.list.array] = 1.0
# Build rotational null space basis
x = V.tabulate_dof_coordinates()
dofs = [V.sub(i).dofmap.list.array for i in range(3)]
basis[3][dofs[0]] = -x[dofs[0], 1]
basis[3][dofs[1]] = x[dofs[1], 0]
basis[4][dofs[0]] = x[dofs[0], 2]
basis[4][dofs[2]] = -x[dofs[2], 0]
basis[5][dofs[2]] = x[dofs[2], 1]
basis[5][dofs[1]] = -x[dofs[1], 2]
# Create vector space basis and orthogonalize
basis = VectorSpaceBasis(nullspace_basis)
basis.orthonormalize()
_x = [basis[i] for i in range(6)]
nsp = PETSc.NullSpace().create(vectors=_x)
return nsp
mesh = BoxMesh(
MPI.COMM_WORLD, [np.array([0.0, 0.0, 0.0]),
np.array([2.0, 1.0, 1.0])], [12, 12, 12],
CellType.tetrahedron, dolfinx.cpp.mesh.GhostMode.none)
def boundary(x):
return np.logical_or(np.isclose(x[0], 0.0),
np.isclose(x[1], 1.0))
# Rotation rate and mass density
omega = 300.0
rho = 10.0
# Loading due to centripetal acceleration (rho*omega^2*x_i)
x = SpatialCoordinate(mesh)
f = as_vector((rho * omega**2 * x[0], rho * omega**2 * x[1], 0.0))
# Elasticity parameters
E = 1.0e9
nu = 0.0
mu = E / (2.0 * (1.0 + nu))
lmbda = E * nu / ((1.0 + nu) * (1.0 - 2.0 * nu))
def sigma(v):
return 2.0 * mu * sym(grad(v)) + lmbda * tr(sym(grad(v))) * Identity(
len(v))
# Create function space
V = VectorFunctionSpace(mesh, ("Lagrange", 1))
# Define variational problem
u = TrialFunction(V)
v = TestFunction(V)
a = inner(sigma(u), grad(v)) * dx
L = inner(f, v) * dx
u0 = Function(V)
with u0.vector.localForm() as bc_local:
bc_local.set(0.0)
# Set up boundary condition on inner surface
bc = DirichletBC(u0, locate_dofs_geometrical(V, boundary))
Controlling compilation parameters¶
Parameters which control FFCX and JIT compilation could be set
directly with the interface of Form
or
via environmental variables.
This demo shows a mixed approach, where C compilation
flags are set with environmental variables.
Some parameters which control FFCX compilation are passed directly to the Form
.
os.environ["DOLFINX_JIT_CFLAGS"] = "-Ofast -march=native"
os.environ["FFCX_VERBOSITY"] = "20"
form = Form(a, form_compiler_parameters={"quadrature_degree": 1})
The use of such aggresive compiler flags (e.g. -Ofast
violates IEEE floating point standard)
often results in a faster assembly code, but slower JIT compilation.
FFCX verbosity levels follow Python std logging library levels, https://docs.python.org/3/library/logging.html.
To see all available form compiler parameters run ffcx --help
in the commandline.
Warning
Environmental variables override any other parameters passed to the Form
, or directly stated
in the metadata of an integral. Please make sure there are no environmental variables set
with side-effects.
Assembly and solve¶
# Assemble system, applying boundary conditions and preserving symmetry
A = assemble_matrix(form, [bc])
A.assemble()
b = assemble_vector(L)
apply_lifting(b, [a], [[bc]])
b.ghostUpdate(addv=PETSc.InsertMode.ADD, mode=PETSc.ScatterMode.REVERSE)
set_bc(b, [bc])
# Create solution function
u = Function(V)
# Create near null space basis (required for smoothed aggregation AMG).
null_space = build_nullspace(V)
# Attach near nullspace to matrix
A.setNearNullSpace(null_space)
# Set solver options
opts = PETSc.Options()
opts["ksp_type"] = "cg"
opts["ksp_rtol"] = 1.0e-12
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 CG Krylov solver and turn convergence monitoring on
solver = PETSc.KSP().create(MPI.COMM_WORLD)
solver.setFromOptions()
# Set matrix operator
solver.setOperators(A)
# Compute solution
solver.setMonitor(lambda ksp, its, rnorm: print("Iteration: {}, rel. residual: {}".format(its, rnorm)))
solver.solve(b, u.vector)
solver.view()
# Save solution to XDMF format
with XDMFFile(MPI.COMM_WORLD, "elasticity.xdmf", "w") as file:
file.write_mesh(mesh)
file.write_function(u)
unorm = u.vector.norm()
if mesh.mpi_comm().rank == 0:
print("Solution vector norm:", unorm)