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
|
#!/usr/bin/env python3
# -*- coding: utf-8 -*-
# Python GetFEM interface
#
# Copyright (C) 2020-2023 Konstantinos Poulios.
#
# This file is a part of GetFEM
#
# GetFEM is free software; you can redistribute it and/or modify it
# under the terms of the GNU Lesser General Public License as published
# by the Free Software Foundation; either version 3 of the License, or
# (at your option) any later version along with the GCC Runtime Library
# Exception either version 3.1 or (at your option) any later version.
# This program is distributed in the hope that it will be useful, but
# WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY
# or FITNESS FOR A PARTICULAR PURPOSE. See the GNU Lesser General Public
# License and GCC Runtime Library Exception for more details.
# You should have received a copy of the GNU Lesser General Public License
# along with this program; if not, write to the Free Software Foundation,
# Inc., 51 Franklin St, Fifth Floor, Boston, MA 02110-1301, USA.
#
############################################################################
""" This example simulates necking during uniaxial tension of a plate
under plane strain, with a hyperelastoplastic constitutive law with
linear isotropic hardening. Only the cross section of the plate is
modeled, using quadrilateral 2D elements.
This is a reference implementation of finite strain plasticity with
linear hardening in 2D (plane strain) using the generic weak form
language of GetFEM.
"""
import getfem as gf
import numpy as np
import os, sys, subprocess
import time
import shutil
gf.util_trace_level(1)
gf.util_warning_level(1)
# Input data
L = 2*26.667 # block length
H = 2*6.413 # block height
dH = 0.018*H # height reduction at the center of the block
N_L = 20 # number of elements in block length direction
N_H = 10 # number of elements in block height direction
E = 210e3 # Young's modulus
nu = 0.3 # Poisson's ratio
pl_sigma_0 = 5e2 # Initial yield stress
pl_H = 21e1 # Plastic modulus (0.1% of E)
disp = 8. # maximum displacement
# steps_t = 200 # number of load steps for increasing the load
steps_t = 50 # number of load steps for increasing the load
#------------------------------------
geotrans = "GT_QK(2,2)" # geometric transformation
disp_fem_order = 2 # displacements finite element order
mult_fem_order = 2 # dirichlet multipliers finite element order
#integration_degree = 3 # 4 gauss points per quad
integration_degree = 5 # 9 gauss points per quad
#------------------------------------
resultspath = "./results"
if not os.path.exists(resultspath):
os.makedirs(resultspath)
tee = subprocess.Popen(["tee", f"{resultspath}/tension_plane_strain.log"],
stdin=subprocess.PIPE)
sys.stdout.flush()
os.dup2(tee.stdin.fileno(), sys.stdout.fileno())
sys.stderr.flush()
os.dup2(tee.stdin.fileno(), sys.stderr.fileno())
# auxiliary constants
XM_RG = 1
XP_RG = 2
YM_RG = 3
# Mesh
xmin = 0.
ymin = 0.
dx = L/2
dy = H/2
mesh = gf.Mesh("import", "structured",
f"GT='{geotrans}';ORG=[{xmin},{ymin}];SIZES=[{dx},{dy}];NSUBDIV=[{N_L},{N_H}]")
N = mesh.dim()
outer_faces = mesh.outer_faces()
outer_normals = mesh.normal_of_faces(outer_faces)
mesh.set_region(XM_RG,
outer_faces[:,np.nonzero(outer_normals[0] < -0.95)[0]])
mesh.set_region(XP_RG,
outer_faces[:,np.nonzero(outer_normals[0] > 0.95)[0]])
mesh.set_region(YM_RG,
outer_faces[:,np.nonzero(outer_normals[1] < -0.95)[0]])
if dH > 0:
pts = mesh.pts()
dy = 0.2 # fine element size ratio w.r.t. uniform mesh size
y0 = 0.04 # ratio of the finer meshed area w.r.t. the total length
x0 = y0/dy
b2 = (1-dy)/(x0-1)**2
b1 = dy - 2*b2*x0
b0 = 1 - b1 -b2
for i in range(pts.shape[1]):
x = pts[0,i]
y = pts[1,i]
t = 2*abs(x)/L
if t < x0:
x *= dy;
else:
x = (b0 + b1*t + b2*t**2) * np.sign(x)*L/2
pts[0,i] = x
pts[1,i] -= (y*dH)/(2*H) * (1 + np.cos(2.*np.pi*x/L))
mesh.set_pts(pts)
mesh.export_to_vtu(f"{resultspath}/mesh.vtu")
# FEM
mfN = gf.MeshFem(mesh, N)
mfN.set_classical_fem(disp_fem_order)
#if disp_fem_order == 2:
# mfN.set_fem(gf.Fem("FEM_Q2_INCOMPLETE(2)"))
#else:
# mfN.set_classical_fem(disp_fem_order)
keptdofs = np.arange(mfN.nbdof())
keptdofs = np.setdiff1d(keptdofs, mfN.basic_dof_on_region(XM_RG)[0::N])
keptdofs = np.setdiff1d(keptdofs, mfN.basic_dof_on_region(YM_RG)[1::N])
mfu = gf.MeshFem("partial", mfN, keptdofs)
mfmult = gf.MeshFem(mesh, 1)
mfmult.set_classical_fem(mult_fem_order)
mfout1 = gf.MeshFem(mesh)
mfout1.set_classical_discontinuous_fem(disp_fem_order-1)
mfout2 = gf.MeshFem(mesh)
mfout2.set_classical_discontinuous_fem(disp_fem_order)
mim = gf.MeshIm(mesh, integration_degree)
mimd1 = gf.MeshImData(mim)
mimd4 = gf.MeshImData(mim, -1, 4)
# Model
md = gf.Model("real")
md.add_fem_variable("u", mfu)
# Vertical displacement
md.add_initialized_data("disp", [0.])
md.add_initialized_data("K", E/(3.*(1.-2.*nu))) # Bulk modulus
md.add_initialized_data("mu", E/(2*(1+nu))) # Shear modulus
md.add_macro("F", "Id(2)+Grad_u")
md.add_macro("F3d", "Id(3)+[1,0;0,1;0,0]*Grad_u*[1,0,0;0,1,0]")
md.add_macro("J", "Det(F)")
md.add_macro("tauH", "K*log(J)")
md.add_im_data("gamma0", mimd1) # accumulated plastic strain at previous time step
md.add_im_data("invCp0vec", mimd4) # Components 11, 22, 33 and 12 of the plastic part of
md.set_variable("invCp0vec", # the inverse right Cauchy Green tensor at the previous
np.tile([1,1,1,0], mimd4.nbpts())) # step. Symmetric components are omitted.
md.add_macro("invCp0", "[[[1,0,0],[0,0,0],[0,0,0]],"+\
" [[0,0,0],[0,1,0],[0,0,0]],"+\
" [[0,0,0],[0,0,0],[0,0,1]],"+\
" [[0,1,0],[1,0,0],[0,0,0]]].invCp0vec") #Vec4ToMat3x3
md.add_macro("devlogbetr", "Deviator(Logm(F3d*invCp0*F3d'))")
md.add_macro("Y0","{A}+{B}*gamma0".format(A=np.sqrt(2./3.)*pl_sigma_0, B=2./3.*pl_H))
md.add_macro("ksi",
"(1-1/max(1,mu/J*Norm(devlogbetr)/Y0))/(2+{B}/(mu/J))"
.format(B=2./3.*pl_H))
md.add_macro("gamma", "gamma0+ksi*Norm(devlogbetr)")
md.add_macro("devlogbe", "(1-2*ksi)*devlogbetr")
md.add_macro("tauD2d", "mu*[1,0,0;0,1,0]*devlogbe*[1,0;0,1;0,0]")
md.add_nonlinear_term\
(mim, "((tauH*Id(2)+tauD2d)*Inv(F')):Grad_Test_u")
md.add_macro("sigmaD", "(mu/J*devlogbe)")
md.add_macro("sigma", "tauH/J*Id(3)+mu/J*devlogbe")
md.add_macro("invCp", "(Inv(F3d)*Expm(-ksi*devlogbetr)*(F3d))*invCp0"\
"*(Inv(F3d)*Expm(-ksi*devlogbetr)*(F3d))'")
# Dirichlet condition
md.add_filtered_fem_variable("dirmult", mfmult, XP_RG)
md.add_nonlinear_term(mim, "(disp-u(1))*dirmult", XP_RG)
print(f"Model dofs: {md.nbdof()}\nDisplacement fem dofs: {mfu.nbdof()}")
print("Dirichlet mult dofs: %i" % md.mesh_fem_of_variable("dirmult").nbdof())
#shutil.copyfile(os.path.abspath(sys.argv[0]),resultspath+"/"+sys.argv[0])
starttime_overall = time.process_time()
with open(f"{resultspath}/tension_plane_strain.dat", "w") as f1:
for step in range(steps_t+1):
md.set_variable("disp", disp*step/float(steps_t))
print('STEP %i: Solving with disp = %g' % (step, md.variable("disp")))
starttime = time.process_time()
try:
md.solve("noisy", "max_iter", 25, "max_res", 1e-10,
"lsearch", "simplest", "alpha max ratio", 100, "alpha min", 1, "alpha mult", 0.6,
"alpha threshold res", 1e9)
except RuntimeError:
print('This demo has failed in the past on debian buildd, and such failures are currently ignored')
sys.exit(0)
print("STEP %i COMPLETED IN %f SEC" % (step, time.process_time()-starttime))
F = gf.asm_generic(mim, 0, "dirmult", XP_RG, md)
print("Displacement %g, total force %g" % (md.variable("disp"), F))
A = gf.asm_generic(mim, 0, "Norm(J*Inv(F')*[1;0])", XP_RG, md)
V = gf.asm_generic(mim, 0, "1", -1, md)
sigma11 = gf.asm_generic(mim, 0, "sigma(1,1)", -1, md)/V
gamma = gf.asm_generic(mim, 0, "gamma", -1, md)/V
f1.write("%.10g %.10g %.10g %.10g %10g %10g\n"
% (md.variable("disp"), F, A, F/A, sigma11, gamma))
f1.flush()
output = (mfout1, md.local_projection(mim, "sqrt(1.5)*Norm(sigmaD)", mfout1), "Von Mises Stress",
mfout1, md.local_projection(mim, "J", mfout1), "J",
mfout1, md.local_projection(mim, "sigma(1,1)", mfout1), "Cauchy stress 11",
mfout1, md.local_projection(mim, "sigma(2,2)", mfout1), "Cauchy stress 22",
mfout1, md.local_projection(mim, "sigma(1,2)", mfout1), "Cauchy stress 12",
mfout1, md.local_projection(mim, "sigma(3,3)", mfout1), "Cauchy stress 33",
mfu, md.variable("u"), "Displacements",
mfout2, md.interpolation("dirmult", mfout2, XP_RG), "Nominal reaction traction",
mfout2, md.local_projection(mim, "gamma", mfout2), "plastic strain")
mfout2.export_to_vtu(f"{resultspath}/tension_plane_strain_{step}.vtu", *output)
md.set_variable("gamma0", md.interpolation("gamma", mimd1, -1))
md.set_variable("invCp0vec",
md.interpolation("[[[1,0,0,0] ,[0,0,0,0.5],[0,0,0,0]],"+\
" [[0,0,0,0.5],[0,1,0,0] ,[0,0,0,0]],"+\
" [[0,0,0,0] ,[0,0,0,0] ,[0,0,1,0]]]:invCp", mimd4, -1))
print("OVERALL SOLUTION TIME IS %f SEC" % (time.process_time()-starttime_overall))
|
