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
|
#!/usr/bin/env python
# -*- coding: utf-8 -*-
# Python GetFEM interface
#
# Copyright (C) 2015-2020 Yves Renard.
#
# 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.
#
############################################################################
#
# Contact of a deformable 'wheel' onto a plane deformable obstacle.
#
############################################################################
import numpy as np
import getfem as gf
gf.util('trace level', 1) # No trace for mesh generation nor for assembly
export_mesh = True;
Dirichlet_version = False; # Use a dirichlet condition instead of a global load
#
# Physical parameters
#
E = 21E6 # Young Modulus (N/cm^2)
nu = 0.3 # Poisson ratio
clambda = E*nu/((1+nu)*(1-2*nu)) # First Lame coefficient (N/cm^2)
cmu = E/(2*(1+nu)) # Second Lame coefficient (N/cm^2)
clambdastar = 2*clambda*cmu/(clambda+2*cmu) # Lame coefficient for Plane stress
applied_force = 1E7 # Force at the hole boundary (N)
#
# Numerical parameters
#
h = 1 # Approximate mesh size
elements_degree = 2 # Degree of the finite element methods
gamma0 = 1./E; # Augmentation parameter for the augmented Lagrangian
#
# Mesh generation. Meshes can also been imported from several formats.
#
mo1 = gf.MesherObject('ball', [0., 15.], 15.)
mo2 = gf.MesherObject('ball', [0., 15.], 8.)
mo3 = gf.MesherObject('set minus', mo1, mo2)
print('Meshes generation')
mesh1 = gf.Mesh('generate', mo3, h, 2)
mesh2 = gf.Mesh('import','structured','GT="GT_PK(2,1)";SIZES=[30,10];NOISED=0;NSUBDIV=[%d,%d];' % (int(30/h)+1, int(10/h)+1));
mesh2.translate([-15.,-10.])
if (export_mesh):
mesh1.export_to_vtk('mesh1.vtk')
mesh2.export_to_vtk('mesh2.vtk')
print('\nYou can view the meshes for instance with')
print('mayavi2 -d mesh1.vtk -f ExtractEdges -m Surface -d mesh2.vtk -f ExtractEdges -m Surface \n')
#
# Boundary selection
#
fb1 = mesh1.outer_faces_in_box([-8.1, 6.9], [8.1, 23.1]) # Boundary of the hole
fb2 = mesh1.outer_faces_with_direction([0., -1.], np.pi/4.5) # Contact boundary of the wheel
fb3 = mesh2.outer_faces_with_direction([0., -1.], 0.01) # Bottom boundary of the foundation
HOLE_BOUND=1; CONTACT_BOUND=2; BOTTOM_BOUND=3;
mesh1.set_region(HOLE_BOUND, fb1)
mesh1.set_region(CONTACT_BOUND, fb2)
mesh1.region_subtract(CONTACT_BOUND, HOLE_BOUND)
mesh2.set_region(BOTTOM_BOUND, fb3)
#
# Definition of finite elements methods and integration method
#
mfu1 = gf.MeshFem(mesh1, 2)
mfu1.set_classical_fem(elements_degree)
mflambda = gf.MeshFem(mesh1, 2)
mflambda.set_classical_fem(elements_degree-1)
mflambda_C = gf.MeshFem(mesh1, 1)
mflambda_C.set_classical_fem(elements_degree-1)
mfu2 = gf.MeshFem(mesh2, 2)
mfu2.set_classical_fem(elements_degree)
mfvm1 = gf.MeshFem(mesh1, 1)
mfvm1.set_classical_discontinuous_fem(elements_degree)
mfvm2 = gf.MeshFem(mesh2, 1)
mfvm2.set_classical_discontinuous_fem(elements_degree)
mim1 = gf.MeshIm(mesh1, 4)
mim1c = gf.MeshIm(mesh1, gf.Integ('IM_STRUCTURED_COMPOSITE(IM_TRIANGLE(4),2)'))
mim2 = gf.MeshIm(mesh2, 4)
#
# Model definition
#
md=gf.Model('real');
md.add_fem_variable('u1', mfu1) # Displacement of the structure 1
md.add_fem_variable('u2', mfu2) # Displacement of the structure 2
md.add_initialized_data('cmu', [cmu])
md.add_initialized_data('clambdastar', [clambdastar])
md.add_isotropic_linearized_elasticity_brick(mim1, 'u1', 'clambdastar', 'cmu')
md.add_isotropic_linearized_elasticity_brick(mim2, 'u2', 'clambdastar', 'cmu')
md.add_Dirichlet_condition_with_multipliers(mim2, 'u2', elements_degree-1, BOTTOM_BOUND)
# Contact condition (augmented Lagrangian)
md.add_initialized_data('gamma0', [gamma0])
md.add_interpolate_transformation_from_expression('Proj1', mesh1, mesh2, '[X(1);0]')
md.add_filtered_fem_variable('lambda1', mflambda_C, CONTACT_BOUND)
md.add_nonlinear_term(mim1c, 'lambda1*(Test_u1.[0;1])'
'-lambda1*(Interpolate(Test_u2,Proj1).[0;1])', CONTACT_BOUND)
md.add_nonlinear_term(mim1c, '-(gamma0*element_size)*(lambda1 + neg_part(lambda1+(1/(gamma0*element_size))*((u1-Interpolate(u2,Proj1)+X-Interpolate(X,Proj1)).[0;1])))*Test_lambda1', CONTACT_BOUND);
# Prescribed force in the hole
if (Dirichlet_version):
md.add_initialized_data('DData', [0., -1.0])
md.add_Dirichlet_condition_with_multipliers(mim1, 'u1', elements_degree-1, HOLE_BOUND, 'DData');
else:
md.add_filtered_fem_variable('lambda_D', mflambda, HOLE_BOUND)
md.add_initialized_data('F', [applied_force/(8*2*np.pi)])
md.add_variable('alpha_D', 1)
md.add_linear_term(mim1, '-lambda_D.Test_u1 + (alpha_D*[0;1] - u1).Test_lambda_D + (lambda_D.[0;1] + F)*Test_alpha_D + 1E-6*alpha_D*Test_alpha_D', HOLE_BOUND)
# The small penalization 1E-6*alpha_D*Test_alpha_D seems necessary to have
# a convergence in all cases. Why ?
#
# Model solve
#
print('Solve problem with ', md.nbdof(), ' dofs')
md.solve('max_res', 1E-9, 'max_iter', 40, 'noisy') # , 'lsearch', 'simplest', 'alpha min', 0.8)
if not(Dirichlet_version):
print('alpha_D = ', md.variable('alpha_D')[0])
# print('Contact multiplier ', md.variable('lambda1'))
#
# Solution export
#
U1 = md.variable('u1')
U2 = md.variable('u2')
VM1 = md.compute_isotropic_linearized_Von_Mises_or_Tresca('u1', 'clambdastar', 'cmu', mfvm1)
VM2 = md.compute_isotropic_linearized_Von_Mises_or_Tresca('u2', 'clambdastar', 'cmu', mfvm2)
mfvm1.export_to_vtk('displacement_with_von_mises1.vtk', mfvm1, VM1, 'Von Mises Stresses', mfu1, U1, 'Displacements')
mfvm2.export_to_vtk('displacement_with_von_mises2.vtk', mfvm2, VM2, 'Von Mises Stresses', mfu2, U2, 'Displacements')
print('You can view solutions with for instance:\nmayavi2 -d displacement_with_von_mises1.vtk -f WarpVector -m Surface -d displacement_with_von_mises2.vtk -f WarpVector -m Surface')
|
