# linear_elasticity/elastodynamic.py¶

Description

The linear elastodynamics solution of an iron plate impact problem.

Find such that: where ## Usage Examples¶

Run with the default settings (the Newmark method, 3D problem, results stored in output/ed/):

sfepy-run sfepy/examples/linear_elasticity/elastodynamic.py


Solve using the Bathe method:

sfepy-run sfepy/examples/linear_elasticity/elastodynamic.py -O "ts='tsb'"


View the resulting displacements on the deforming mesh (1000x magnified), Cauchy strain and stress using:

sfepy-view output/ed/user_block.h5 -f u:wu:f1e3:p0 1:vw:p0 cauchy_strain:p1 cauchy_stress:p2


Solve in 2D using the explicit Velocity-Verlet method with adaptive time-stepping and save all time steps (see plot_times.py use below):

sfepy-run sfepy/examples/linear_elasticity/elastodynamic.py -d "dims=(5e-3, 5e-3), shape=(61, 61), tss_name='tsvv', adaptive=True, save_times='all'"


View the resulting velocities on the deforming mesh (1000x magnified) using:

sfepy-view output/ed/user_block.h5 -2 --grid-vector1=1.2,0,0 -f du:wu:f1e3:p0 1:vw:p0


Plot the adaptive time steps (available at times according to ‘save_times’ option!):

python3 sfepy/scripts/plot_times.py output/ed/user_block.h5 -l


Again, solve in 2D using the explicit Velocity-Verlet method with adaptive time-stepping and save all time steps. Now the used time step control is suitable for linear problems solved by a direct solver: it employs a heuristic that tries to keep the time step size constant for several consecutive steps, reducing so the need for a new matrix factorization. Run:

sfepy-run sfepy/examples/linear_elasticity/elastodynamic.py -d "dims=(5e-3, 5e-3), shape=(61, 61), tss_name='tsvv', tsc_name='tscedl', adaptive=True, save_times='all'"


The resulting velocities and adaptive time steps can again be plotted by the commands shown above. source code

r"""
The linear elastodynamics solution of an iron plate impact problem.

Find :math:\ul{u} such that:

.. math::
\int_{\Omega} \rho \ul{v} \pddiff{\ul{u}}{t}
+ \int_{\Omega} D_{ijkl}\ e_{ij}(\ul{v}) e_{kl}(\ul{u})
= 0

where

.. math::
D_{ijkl} = \mu (\delta_{ik} \delta_{jl}+\delta_{il} \delta_{jk}) +
\lambda \ \delta_{ij} \delta_{kl}
\;.

Notes
-----

The used elastodynamics solvers expect that the total vector of DOFs contains
three blocks in this order: the displacements, the velocities, and the
accelerations. This is achieved by defining three unknown variables 'u',
'du', 'ddu' and the corresponding test variables, see the variables
definition. Then the solver can automatically extract the mass, damping (zero
here), and stiffness matrices as diagonal blocks of the global matrix. Note
also the use of the 'dw_zero' (do-nothing) term that prevents the
velocity-related variables to be removed from the equations in the absence of a
damping term.

Usage Examples
--------------

Run with the default settings (the Newmark method, 3D problem, results stored
in output/ed/)::

sfepy-run sfepy/examples/linear_elasticity/elastodynamic.py

Solve using the Bathe method::

sfepy-run sfepy/examples/linear_elasticity/elastodynamic.py -O "ts='tsb'"

View the resulting displacements on the deforming mesh (1000x magnified),
Cauchy strain and stress using::

sfepy-view output/ed/user_block.h5 -f u:wu:f1e3:p0 1:vw:p0 cauchy_strain:p1 cauchy_stress:p2

Solve in 2D using the explicit Velocity-Verlet method with adaptive
time-stepping and save all time steps (see plot_times.py use below)::

sfepy-run sfepy/examples/linear_elasticity/elastodynamic.py -d "dims=(5e-3, 5e-3), shape=(61, 61), tss_name='tsvv', adaptive=True, save_times='all'"

View the resulting velocities on the deforming mesh (1000x magnified) using::

sfepy-view output/ed/user_block.h5 -2 --grid-vector1=1.2,0,0 -f du:wu:f1e3:p0 1:vw:p0

Plot the adaptive time steps (available at times according to 'save_times'
option!)::

python3 sfepy/scripts/plot_times.py output/ed/user_block.h5 -l

Again, solve in 2D using the explicit Velocity-Verlet method with adaptive
time-stepping and save all time steps. Now the used time step control is
suitable for linear problems solved by a direct solver: it employs a heuristic
that tries to keep the time step size constant for several consecutive steps,
reducing so the need for a new matrix factorization. Run::

sfepy-run sfepy/examples/linear_elasticity/elastodynamic.py -d "dims=(5e-3, 5e-3), shape=(61, 61), tss_name='tsvv', tsc_name='tscedl', adaptive=True, save_times='all'"

The resulting velocities and adaptive time steps can again be plotted by the
commands shown above.
"""
from __future__ import absolute_import

import numpy as nm

import sfepy.mechanics.matcoefs as mc
from sfepy.discrete.fem.meshio import UserMeshIO
from sfepy.mesh.mesh_generators import gen_block_mesh

def define(
E=200e9, nu=0.3, rho=7800,
plane='strain',
dims=(1e-2, 2.5e-3, 2.5e-3),
shape=(21, 6, 6),
v0=1.0,
ct1=1.5,
tss_name='tsn',
tsc_name='tscedb',
ls_name='lsd',
save_times=20,
):
"""
Parameters
----------
E, nu, rho: material parameters
plane: plane strain or stress hypothesis
dims: physical dimensions of the block (L, d, x)
shape: numbers of mesh vertices along each axis
v0: initial impact velocity
ct1: final time in L / "longitudinal wave speed" units
tss_name: time stepping solver name (see "solvers" section)
ls_name: linear system solver name (see "solvers" section)
save_times: number of solutions to save
"""
dim = len(dims)

lam, mu = mc.lame_from_youngpoisson(E, nu, plane=plane)
# Longitudinal and shear wave propagation speeds.
cl = nm.sqrt((lam + 2.0 * mu) / rho)
cs = nm.sqrt(mu / rho)

# Element size.
L, d = dims[:2]
H = L / (shape - 1)

# Time-stepping parameters.
# Note: the Courant number C0 =  dt * cl / H
dt = H / cl # C0 = 1

t1 = ct1 * L / cl

def mesh_hook(mesh, mode):
"""
Generate the block mesh.
"""
mesh = gen_block_mesh(dims, shape, 0.5 * nm.array(dims),
name='user_block', verbose=False)
return mesh

elif mode == 'write':
pass

def post_process(out, problem, state, extend=False):
"""
Calculate and output strain and stress for given displacements.
"""
from sfepy.base.base import Struct

ev = problem.evaluate
strain = ev('ev_cauchy_strain.i.Omega(u)', mode='el_avg', verbose=False)
stress = ev('ev_cauchy_stress.i.Omega(solid.D, u)', mode='el_avg',
copy_materials=False, verbose=False)

out['cauchy_strain'] = Struct(name='output_data', mode='cell',
data=strain)
out['cauchy_stress'] = Struct(name='output_data', mode='cell',
data=stress)

return out

filename_mesh = UserMeshIO(mesh_hook)

regions = {
'Omega' : 'all',
'Impact' : ('vertices in (x < 1e-12)', 'facet'),
}
if dim == 3:
regions.update({
'Symmetry-y' : ('vertices in (y < 1e-12)', 'facet'),
'Symmetry-z' : ('vertices in (z < 1e-12)', 'facet'),
})

# Iron.
materials = {
'solid' : ({
'D': mc.stiffness_from_youngpoisson(dim=dim, young=E, poisson=nu,
plane=plane),
'rho': rho,
},),
}

fields = {
'displacement': ('real', 'vector', 'Omega', 1),
}

integrals = {
'i' : 2,
}

variables = {
'u' : ('unknown field', 'displacement', 0),
'du' : ('unknown field', 'displacement', 1),
'ddu' : ('unknown field', 'displacement', 2),
'v' : ('test field', 'displacement', 'u'),
'dv' : ('test field', 'displacement', 'du'),
'ddv' : ('test field', 'displacement', 'ddu'),
}

ebcs = {
'Impact' : ('Impact', {'u.0' : 0.0, 'du.0' : 0.0, 'ddu.0' : 0.0}),
}
if dim == 3:
ebcs.update({
'Symmtery-y' : ('Symmetry-y',
{'u.1' : 0.0, 'du.1' : 0.0, 'ddu.1' : 0.0}),
'Symmetry-z' : ('Symmetry-z',
{'u.2' : 0.0, 'du.2' : 0.0, 'ddu.2' : 0.0}),
})

def get_ic(coor, ic, mode='u'):
val = nm.zeros_like(coor)
if mode == 'u':
val[:, 0] = 0.0

elif mode == 'du':
val[:, 0] = -1.0

return val

functions = {
'get_ic_u' : (get_ic,),
'get_ic_du' : (lambda coor, ic: get_ic(coor, None, mode='du'),),
}

ics = {
'ic' : ('Omega', {'u.all' : 'get_ic_u', 'du.all' : 'get_ic_du'}),
}

equations = {
'balance_of_forces' :
"""dw_dot.i.Omega(solid.rho, ddv, ddu)
+ dw_zero.i.Omega(dv, du)
+ dw_lin_elastic.i.Omega(solid.D, v, u) = 0""",
}

solvers = {
'lsd' : ('ls.auto_direct', {
# Reuse the factorized linear system from the first time step.
'use_presolve' : True,
# Speed up the above by omitting the matrix digest check used
# normally for verification that the current matrix corresponds to
# the factorized matrix stored in the solver instance. Use with
# care!
'use_mtx_digest' : False,
}),
'lsi' : ('ls.petsc', {
'method' : 'cg',
'precond' : 'icc',
'i_max' : 150,
'eps_a' : 1e-32,
'eps_r' : 1e-8,
'verbose' : 2,
}),
'newton' : ('nls.newton', {
'i_max'      : 1,
'eps_a'      : 1e-6,
'eps_r'      : 1e-6,
}),
'tsvv' : ('ts.velocity_verlet', {
# Excplicit method -> requires at least 10x smaller dt than the
# other time-stepping solvers, or an adaptive time step control.
't0' : 0.0,
't1' : t1,
'dt' : dt,
'n_step' : None,

'is_linear'  : True,

'verbose' : 1,
}),
'tscd' : ('ts.central_difference', {
# Excplicit method -> requires at least 10x smaller dt than the
# other time-stepping solvers, or an adaptive time step control.
't0' : 0.0,
't1' : t1,
'dt' : dt,
'n_step' : None,

'is_linear'  : True,

'verbose' : 1,
}),
'tsn' : ('ts.newmark', {
't0' : 0.0,
't1' : t1,
'dt' : dt,
'n_step' : None,

'is_linear'  : True,

'beta' : 0.25,
'gamma' : 0.5,

'verbose' : 1,
}),
'tsga' : ('ts.generalized_alpha', {
't0' : 0.0,
't1' : t1,
'dt' : dt,
'n_step' : None,

'is_linear'  : True,

'rho_inf' : 0.5,
'alpha_m' : None,
'alpha_f' : None,
'beta' : None,
'gamma' : None,

'verbose' : 1,
}),
'tsb' : ('ts.bathe', {
't0' : 0.0,
't1' : t1,
'dt' : dt,
'n_step' : None,

'is_linear'  : True,

'verbose' : 1,
}),
'tscedb' : ('tsc.ed_basic', {
'eps_r' : (1e-4, 1e-1),
'eps_a' : (1e-8, 5e-2),
'fmin' : 0.3,
'fmax' : 2.5,
'fsafety' : 0.85,
}),
'tscedl' : ('tsc.ed_linear', {
'eps_r' : (1e-4, 1e-1),
'eps_a' : (1e-8, 5e-2),
'fmin' : 0.3,
'fmax' : 2.5,
'fsafety' : 0.85,
'red_factor' : 0.9,
'inc_wait' : 10,
'min_inc_factor' : 1.5,
}),
}

options = {
'ts' : tss_name,
'tsc' : tsc_name if adaptive else None,
'nls' : 'newton',
'ls' : ls_name,

'save_times' : save_times,

'active_only' : False,

'output_format' : 'h5',
'output_dir' : 'output/ed',
'post_process_hook' : 'post_process',
}

return locals()