# 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 dolfinx
import numpy as np
from dolfinx import BoxMesh, DirichletBC, Function, VectorFunctionSpace, cpp
from dolfinx.cpp.mesh import CellType
from dolfinx.fem import (apply_lifting, assemble_matrix, assemble_vector,
locate_dofs_geometrical, set_bc)
from dolfinx.io import XDMFFile
from dolfinx.la import VectorSpaceBasis
from mpi4py import MPI
from petsc4py import PETSc
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, V.dofmap.index_map_bs) 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]

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

# Build translational null space basis
for i in range(3):
basis[i][dofs[i]] = 1.0

# Build rotational null space basis
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

# 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.shared_facet)

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

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))
```

## Assembly and solve¶

```# Assemble system, applying boundary conditions
A = assemble_matrix(a, [bc])
A.assemble()

b = assemble_vector(L)
apply_lifting(b, [a], [[bc]])
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)
```