/
demo_elasticity.py
275 lines (217 loc) · 7.85 KB
/
demo_elasticity.py
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
112
113
114
115
116
117
118
119
120
121
122
123
124
125
126
127
128
129
130
131
132
133
134
135
136
137
138
139
140
141
142
143
144
145
146
147
148
149
150
151
152
153
154
155
156
157
158
159
160
161
162
163
164
165
166
167
168
169
170
171
172
173
174
175
176
177
178
179
180
181
182
183
184
185
186
187
188
189
190
191
192
193
194
195
196
197
198
199
200
201
202
203
204
205
206
207
208
209
210
211
212
213
214
215
216
217
218
219
220
221
222
223
224
225
226
227
228
229
230
231
232
233
234
235
236
237
238
239
240
241
242
243
244
245
246
247
248
249
250
251
252
253
254
255
256
257
258
259
260
261
262
263
264
265
266
267
268
269
270
271
272
273
274
275
# ---
# jupyter:
# jupytext:
# text_representation:
# extension: .py
# format_name: light
# format_version: '1.5'
# jupytext_version: 1.13.6
# ---
# # Elasticity using algebraic multigrid
#
# Copyright © 2020-2022 Garth N. Wells and Michal Habera
#
# This demo ({download}`demo_elasticity.py`) solves the equations of
# static linear elasticity using a smoothed aggregation algebraic
# multigrid solver. It illustrates how to:
#
# - Use a smoothed aggregation algebraic multigrid solver
# - Use {py:class}`Expression <dolfinx.fem.Expression>` to compute
# derived quantities of a solution
#
# The required modules are first imported:
from mpi4py import MPI
from petsc4py import PETSc
# +
import numpy as np
import dolfinx
import ufl
from dolfinx import la
from dolfinx.fem import (
Expression,
Function,
FunctionSpace,
dirichletbc,
form,
functionspace,
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
dtype = PETSc.ScalarType # type: ignore
# -
# ## Create the operator near-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 a 3D elasticity problem. The nullspace is
# spanned by six vectors -- three translation modes and three rotation
# modes.
def build_nullspace(V: FunctionSpace):
"""Build PETSc nullspace for 3D elasticity"""
# Create vectors that will span the nullspace
bs = V.dofmap.index_map_bs
length0 = V.dofmap.index_map.size_local
basis = [la.vector(V.dofmap.index_map, bs=bs, dtype=dtype) for i in range(6)]
b = [b.array for b in basis]
# Get dof indices for each subspace (x, y and z dofs)
dofs = [V.sub(i).dofmap.list.flatten() for i in range(3)]
# Set the three translational rigid body modes
for i in range(3):
b[i][dofs[i]] = 1.0
# Set the three rotational rigid body modes
x = V.tabulate_dof_coordinates()
dofs_block = V.dofmap.list.flatten()
x0, x1, x2 = x[dofs_block, 0], x[dofs_block, 1], x[dofs_block, 2]
b[3][dofs[0]] = -x1
b[3][dofs[1]] = x0
b[4][dofs[0]] = x2
b[4][dofs[2]] = -x0
b[5][dofs[2]] = x1
b[5][dofs[1]] = -x2
_basis = [x._cpp_object for x in basis]
dolfinx.cpp.la.orthonormalize(_basis)
assert dolfinx.cpp.la.is_orthonormal(_basis)
basis_petsc = [
PETSc.Vec().createWithArray(x[: bs * length0], bsize=3, comm=V.mesh.comm) # type: ignore
for x in b
]
return PETSc.NullSpace().create(vectors=basis_petsc) # type: ignore
# ## Problem definition
# 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,
ghost_mode=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))
# Define the elasticity parameters and create a function that computes
# an 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 = functionspace(msh, ("Lagrange", 1, (msh.geometry.dim,)))
u, v = ufl.TrialFunction(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 facets on these boundaries, 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 call
# `A.assemble()` completes any parallel communication required to
# compute the matrix.
# +
A = assemble_matrix(a, bcs=[bc])
A.assemble()
# -
# The linear form `L` is assembled into a vector `b`, and then modified
# by {py:func}`apply_lifting <dolfinx.fem.petsc.apply_lifting>` to
# account for the Dirichlet boundary conditions. After calling
# {py:func}`apply_lifting <dolfinx.fem.petsc.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) # type: ignore
set_bc(b, [bc])
# -
# Create the near-nullspace and attach it to the PETSc matrix:
ns = build_nullspace(V)
A.setNearNullSpace(ns)
A.setOption(PETSc.Mat.Option.SPD, True) # type: ignore
# Set PETSc solver options, create a PETSc Krylov solver, and attach the
# matrix `A` to the solver:
# +
# Set solver options
opts = PETSc.Options() # type: ignore
opts["ksp_type"] = "cg"
opts["ksp_rtol"] = 1.0e-8
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_ksp_chebyshev_esteig_steps"] = 10
# Create PETSc Krylov solver and turn convergence monitoring on
solver = PETSc.KSP().create(msh.comm) # type: ignore
solver.setFromOptions()
# Set matrix operator
solver.setOperators(A)
# -
# Create a solution {py:class}`Function<dolfinx.fem.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 {py:class}`Expression<dolfinx.fem.Expression>`
# that is interpolated into the
# {py:class}`Function<dolfinx.fem.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 = la.norm(uh.x)
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.