.. raw:: html

This work is licensed under a Creative Commons Attribution-ShareAlike 4.0 International License

.. _vonMisesPlasticity:
==================================================
Elasto-plastic analysis of a 2D von Mises material
==================================================
-------------
Introduction
-------------
This example is concerned with the incremental analysis of an elasto-plastic
von Mises material. The structure response is computed using an iterative
predictor-corrector return mapping algorithm embedded in a Newton-Raphson global
loop for restoring equilibrium. Due to the simple expression of the von Mises criterion,
the return mapping procedure is completely analytical (with linear isotropic
hardening). The corresponding sources can be obtained from :download:`vonMises_plasticity.zip`.
Another implementation of von Mises plasticity can also be found at
https://bitbucket.org/fenics-apps/fenics-solid-mechanics as well as in
the numerical tour :ref:`PlasticityMFront`.
We point out that the 2D nature of the problem will impose keeping
track of the out-of-plane :math:`\varepsilon_{zz}^p` plastic strain and dealing with
representations of stress/strain states including the :math:`zz` component. Note
also that are not concerned with the issue of volumetric locking induced by
incompressible plastic deformations since quadratic triangles in 2D is enough
to mitigate the locking phenomenon.
The plastic strain evolution during the cylinder expansion will look like this:
.. image:: plastic_strain.gif
:scale: 80%
-----------------
Problem position
-----------------
In FEniCS 2017.2, the FEniCS Form Compiler ``ffc`` now uses ``uflacs`` as a default
representation instead of the old ``quadrature`` representation. However, using
``Quadrature`` elements generates some bugs in this representation and we therefore
need to revert to the old representation. Deprecation warning messages are also disabled.
See `this post `_
and the corresponding `issue `_
for more information.::
from dolfin import *
import numpy as np
parameters["form_compiler"]["representation"] = 'quadrature'
import warnings
from ffc.quadrature.deprecation import QuadratureRepresentationDeprecationWarning
warnings.simplefilter("once", QuadratureRepresentationDeprecationWarning)
The material is represented by an isotropic elasto-plastic von Mises yield condition
of uniaxial strength :math:`\sigma_0` and with isotropic hardening of modulus :math:`H`.
The yield condition is thus given by:
.. math::
f(\boldsymbol{\sigma}) = \sqrt{\frac{3}{2}\boldsymbol{s}:\boldsymbol{s}} - \sigma_0 -Hp \leq 0
where :math:`p` is the cumulated equivalent plastic strain. The hardening modulus
can also be related to a tangent elastic modulus :math:`E_t = \dfrac{EH}{E+H}`.
The considered problem is that of a plane strain hollow cylinder of internal (resp. external)
radius :math:`R_i` (resp. :math:`R_e`) under internal uniform pressure :math:`q`.
Only a quarter of cylinder is generated using ``Gmsh`` and converted to ``.xml`` format. ::
# elastic parameters
E = Constant(70e3)
nu = Constant(0.3)
lmbda = E*nu/(1+nu)/(1-2*nu)
mu = E/2./(1+nu)
sig0 = Constant(250.) # yield strength
Et = E/100. # tangent modulus
H = E*Et/(E-Et) # hardening modulus
Re, Ri = 1.3, 1. # external/internal radius
mesh = Mesh("thick_cylinder.xml")
facets = MeshFunction("size_t", mesh, "thick_cylinder_facet_region.xml")
ds = Measure('ds')[facets]
Function spaces will involve a standard CG space for the displacement whereas internal
state variables such as plastic strains will be represented using a **Quadrature** element.
This choice will make it possible to express the complex non-linear material constitutive
equation at the Gauss points only, without involving any interpolation of non-linear
expressions throughout the element. It will ensure an optimal convergence rate
for the Newton-Raphson method. See Chapter 26 of the `FEniCS book `_.
We will need Quadrature elements for 4-dimensional vectors and scalars, the number
of Gauss points will be determined by the required degree of the Quadrature element
(e.g. ``degree=1`` yields only 1 Gauss point, ``degree=2`` yields 3 Gauss points and
``degree=3`` yields 6 Gauss points (note that this is suboptimal))::
deg_u = 2
deg_stress = 2
V = VectorFunctionSpace(mesh, "CG", deg_u)
We = VectorElement("Quadrature", mesh.ufl_cell(), degree=deg_stress, dim=4, quad_scheme='default')
W = FunctionSpace(mesh, We)
W0e = FiniteElement("Quadrature", mesh.ufl_cell(), degree=deg_stress, quad_scheme='default')
W0 = FunctionSpace(mesh, W0e)
.. note::
In older versions, it was possible to define Quadrature function spaces directly
using ``FunctionSpace(mesh, "Quadrature", 1)``. This is no longer the case since
FEniCS 2016.1 (see `this issue `_). Instead, Quadrature elements must first be defined
by specifying the associated degree and quadrature scheme before defining the
associated FunctionSpace.
Various functions are defined to keep track of the current internal state and
currently computed increments::
sig = Function(W)
sig_old = Function(W)
n_elas = Function(W)
beta = Function(W0)
p = Function(W0, name="Cumulative plastic strain")
u = Function(V, name="Total displacement")
du = Function(V, name="Iteration correction")
Du = Function(V, name="Current increment")
v = TrialFunction(V)
u_ = TestFunction(V)
Boundary conditions correspond to symmetry conditions on the bottom and left
parts (resp. numbered 1 and 3). Loading consists of a uniform pressure on the
internal boundary (numbered 4). It will be progressively increased from 0 to
:math:`q_{lim}=\dfrac{2}{\sqrt{3}}\sigma_0\log\left(\dfrac{R_e}{R_i}\right)`
which is the analytical collapse load for a perfectly-plastic material (no hardening)::
bc = [DirichletBC(V.sub(1), 0, facets, 1), DirichletBC(V.sub(0), 0, facets, 3)]
n = FacetNormal(mesh)
q_lim = float(2/sqrt(3)*ln(Re/Ri)*sig0)
loading = Expression("-q*t", q=q_lim, t=0, degree=2)
def F_ext(v):
return loading*dot(n, v)*ds(4)
-----------------------------
Constitutive relation update
-----------------------------
Before writing the variational form, we now define some useful functions which
will enable performing the constitutive relation update using a return mapping
procedure. This step is quite classical in FEM plasticity for a von Mises criterion
with isotropic hardening and follow notations from [BON2014]_. First, the strain
tensor will be represented in a 3D fashion by appending zeros on the out-of-plane
components since, even if the problem is 2D, the plastic constitutive relation will
involve out-of-plane plastic strains. The elastic consitutive relation is also defined
and a function ``as_3D_tensor`` will enable to represent a 4 dimensional vector
containing respectively :math:`xx, yy, zz` and :math:`xy` components as a 3D tensor::
def eps(v):
e = sym(grad(v))
return as_tensor([[e[0, 0], e[0, 1], 0],
[e[0, 1], e[1, 1], 0],
[0, 0, 0]])
def sigma(eps_el):
return lmbda*tr(eps_el)*Identity(3) + 2*mu*eps_el
def as_3D_tensor(X):
return as_tensor([[X[0], X[3], 0],
[X[3], X[1], 0],
[0, 0, X[2]]])
The return mapping procedure consists in finding a new stress :math:`\boldsymbol{\sigma}_{n+1}`
and internal variable :math:`p_{n+1}` state verifying the current plasticity condition
from a previous stress :math:`\boldsymbol{\sigma}_{n}` and internal variable :math:`p_n` state and
an increment of total deformation :math:`\Delta \boldsymbol{\varepsilon}`. An elastic
trial stress :math:`\boldsymbol{\sigma}_{\text{elas}} = \boldsymbol{\sigma}_{n} + \mathbf{C}\Delta \boldsymbol{\varepsilon}`
is first computed. The plasticity criterion is then evaluated with the previous plastic strain
:math:`f_{\text{elas}} = \sigma^{eq}_{\text{elas}} - \sigma_0 - H p_n` where
:math:`\sigma^{eq}_{\text{elas}} = \sqrt{\frac{3}{2}\boldsymbol{s}:\boldsymbol{s}}`
with the deviatoric elastic stress :math:`\boldsymbol{s} = \operatorname{dev}\boldsymbol{\sigma}_{\text{elas}}`.
If :math:`f_{\text{elas}} < 0`, no plasticity occurs during this time increment and
:math:`\Delta p,\Delta \boldsymbol{\varepsilon}^p =0`.
Otherwise, plasticity
occurs and the increment of plastic strain is given by :math:`\Delta p = \dfrac{f_{\text{elas}}}{3\mu+H}`.
Hence, both elastic and plastic evolution can be accounted for by defining the
plastic strain increment as follows:
.. math::
\Delta p = \dfrac{\langle f_{\text{elas}}\rangle_+}{3\mu+H}
where :math:`\langle \star \rangle_+` represents the positive part of :math:`\star`
and is obtained by function ``ppos``. Plastic evolution also requires the computation
of the normal vector to the final yield surface given by
:math:`\boldsymbol{n}_{\text{elas}} = \boldsymbol{s}/\sigma_{\text{elas}}^{eq}`. In the following,
this vector must be zero in case of elastic evolution. Hence, we multiply it by
:math:`\dfrac{\langle f_{\text{elas}}\rangle_+}{ f_{\text{elas}}}` to tackle
both cases in a single expression. The final stress state is corrected by the
plastic strain as follows :math:`\boldsymbol{\sigma}_{n+1} = \boldsymbol{\sigma}_{\text{elas}} -
\beta \boldsymbol{s}` with :math:`\beta = \dfrac{3\mu}{\sigma_{\text{elas}}^{eq}}\Delta p`.
It can be observed that the last term vanishes in case of elastic evolution so
that the final stress is indeed the elastic predictor. ::
ppos = lambda x: (x+abs(x))/2.
def proj_sig(deps, old_sig, old_p):
sig_n = as_3D_tensor(old_sig)
sig_elas = sig_n + sigma(deps)
s = dev(sig_elas)
sig_eq = sqrt(3/2.*inner(s, s))
f_elas = sig_eq - sig0 - H*old_p
dp = ppos(f_elas)/(3*mu+H)
n_elas = s/sig_eq*ppos(f_elas)/f_elas
beta = 3*mu*dp/sig_eq
new_sig = sig_elas-beta*s
return as_vector([new_sig[0, 0], new_sig[1, 1], new_sig[2, 2], new_sig[0, 1]]), \
as_vector([n_elas[0, 0], n_elas[1, 1], n_elas[2, 2], n_elas[0, 1]]), \
beta, dp
.. note::
We could have used conditionals to write more explicitly the difference
between elastic and plastic evolution.
In order to use a Newton-Raphson procedure to resolve global equilibrium, we also
need to derive the algorithmic consistent tangent matrix given by:
.. math::
\mathbf{C}_{\text{tang}}^{\text{alg}} = \mathbf{C} - 3\mu\left(\dfrac{3\mu}{3\mu+H}-\beta\right)
\boldsymbol{n}_{\text{elas}} \otimes \boldsymbol{n}_{\text{elas}} - 2\mu\beta\mathbf{DEV}
where :math:`\mathbf{DEV}` is the 4th-order tensor associated with the deviatoric
operator (note that :math:`\mathbf{C}_{\text{tang}}^{\text{alg}}=\mathbf{C}` for
elastic evolution). Contrary to what is done in the FEniCS book, we do not store it as the components
of a 4th-order tensor but it will suffice keeping track of the normal vector and
the :math:`\beta` parameter related to the plastic strains. We instead define a function
computing the tangent stress :math:`\boldsymbol{\sigma}_\text{tang} = \mathbf{C}_{\text{tang}}^{\text{alg}}
\boldsymbol{\varepsilon}` as follows::
def sigma_tang(e):
N_elas = as_3D_tensor(n_elas)
return sigma(e) - 3*mu*(3*mu/(3*mu+H)-beta)*inner(N_elas, e)*N_elas-2*mu*beta*dev(e)
--------------------------------------------
Global problem and Newton-Raphson procedure
--------------------------------------------
We are now in position to derive the global problem with its associated
Newton-Raphson procedure. Each iteration will require establishing equilibrium
by driving to zero the residual between the internal forces associated with the current
stress state ``sig`` and the external force vector. Because we use Quadrature
elements a custom integration measure must be defined to match the quadrature
degree and scheme used by the Quadrature elements::
metadata = {"quadrature_degree": deg_stress, "quadrature_scheme": "default"}
dxm = dx(metadata=metadata)
a_Newton = inner(eps(v), sigma_tang(eps(u_)))*dxm
res = -inner(eps(u_), as_3D_tensor(sig))*dxm + F_ext(u_)
The consitutive update defined earlier will perform nonlinear operations on
the stress and strain tensors. These nonlinear expressions must then be projected
back onto the associated Quadrature spaces. Since these fields are defined locally
in each cell (in fact only at their associated Gauss point), this projection can
be performed locally. For this reason, we define a ``local_project`` function
that use the ``LocalSolver`` to gain in efficiency (see also :ref:`TipsTricksProjection`)
for more details::
def local_project(v, V, u=None):
dv = TrialFunction(V)
v_ = TestFunction(V)
a_proj = inner(dv, v_)*dxm
b_proj = inner(v, v_)*dxm
solver = LocalSolver(a_proj, b_proj)
solver.factorize()
if u is None:
u = Function(V)
solver.solve_local_rhs(u)
return u
else:
solver.solve_local_rhs(u)
return
.. note::
We could have used the standard ``project`` if we are not interested in optimizing
the code. However, the use of Quadrature elements would have required telling
``project`` to use an appropriate integration measure to solve the global :math:`L^2`
projection that occurs under the hood. This would have needed either redefining
explicitly the projection associated forms (as we just did) or specifiying the
appropriate quadrature degree to the form compiler as follows
:code:`project(sig_, W, form_compiler_parameters={"quadrature_degree":deg_stress})`
Before defining the Newton-Raphson loop, we set up the output file and appropriate
FunctionSpace (here piecewise constant) and Function for output of the equivalent
plastic strain since XDMF output does not handle Quadrature elements::
file_results = XDMFFile("plasticity_results.xdmf")
file_results.parameters["flush_output"] = True
file_results.parameters["functions_share_mesh"] = True
P0 = FunctionSpace(mesh, "DG", 0)
p_avg = Function(P0, name="Plastic strain")
We now define the global Newton-Raphson loop. We will discretize the applied
loading using ``Nincr`` increments from 0 up to 1.1 (we exclude zero from
the list of load steps). A nonlinear discretization is adopted to refine the
load steps during the plastic evolution phase. At each time increment, the
system is assembled and the residual norm is computed. The incremental displacement
``Du`` is initialized to zero and the inner iteration loop performing the constitutive
update is initiated. Inside this loop, corrections ``du`` to the displacement
increment are computed by solving the Newton system and the return mapping
update is performed using the current total strain increment ``deps``. The resulting
quantities are then projected onto their appropriate FunctionSpaces. The Newton
system and residuals are reassembled and this procedure continues until the residual
norm falls below a given tolerance. After convergence of the iteration loop,
the total displacement, stress and plastic strain states are updated ::
Nitermax, tol = 200, 1e-8 # parameters of the Newton-Raphson procedure
Nincr = 20
load_steps = np.linspace(0, 1.1, Nincr+1)[1:]**0.5
results = np.zeros((Nincr+1, 2))
for (i, t) in enumerate(load_steps):
loading.t = t
A, Res = assemble_system(a_Newton, res, bc)
nRes0 = Res.norm("l2")
nRes = nRes0
Du.interpolate(Constant((0, 0)))
print("Increment:", str(i+1))
niter = 0
while nRes/nRes0 > tol and niter < Nitermax:
solve(A, du.vector(), Res, "mumps")
Du.assign(Du+du)
deps = eps(Du)
sig_, n_elas_, beta_, dp_ = proj_sig(deps, sig_old, p)
local_project(sig_, W, sig)
local_project(n_elas_, W, n_elas)
local_project(beta_, W0, beta)
A, Res = assemble_system(a_Newton, res, bc)
nRes = Res.norm("l2")
print(" Residual:", nRes)
niter += 1
u.assign(u+Du)
sig_old.assign(sig)
p.assign(p+local_project(dp_, W0))
----------------
Post-processing
----------------
Inside the incremental loop, the displacement and plastic strains are exported
at each time increment, the plastic strain must first be projected onto the
previously defined DG FunctionSpace. We also monitor the value of the cylinder
displacement on the inner boundary. The load-displacement curve is then plotted::
file_results.write(u, t)
p_avg.assign(project(p, P0))
file_results.write(p_avg, t)
results[i+1, :] = (u(Ri, 0)[0], t)
import matplotlib.pyplot as plt
plt.plot(results[:, 0], results[:, 1], "-o")
plt.xlabel("Displacement of inner boundary")
plt.ylabel(r"Applied pressure $q/q_{lim}$")
plt.show()
The load-displacement curve looks as follows:
.. image:: cylinder_expansion_load_displ.png
:scale: 20%
It can also be checked that the analytical limit load is also well reproduced
when considering a zero hardening modulus.
-----------
References
-----------
.. [BON2014] Marc Bonnet, Attilio Frangi, Christian Rey.
*The finite element method in solid mechanics.* McGraw Hill Education, pp.365, 2014