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
241
242
243
244
245
246
247
248
249
250
251
252 | # -*- coding: utf-8 -*-
"""
Created on Mon Apr 22 15:12:06 2019
@author: pchi893
"""
# Converted to openseespy by: Pavan Chigullapally
# University of Auckland
# Email: pchi893@aucklanduni.ac.nz
# Example 2c. 2D cantilever column, dynamic eq ground motion
# EQ ground motion with gravity- uniform excitation of structure
#In this example, the Uniaxial Section of Example 2b is replaced by a fiber section. Inelastic uniaxial materials are used in this example,
#which are assigned to each fiber, or patch of fibers, in the section.
#In this example the axial and flexural behavior are coupled, a characteristic of the fiber section.
#The nonlinear/inelastic behavior of a fiber section is defined by the stress-strain response of the uniaxial materials used to define it.
#To run EQ ground-motion analysis (BM68elc.acc needs to be downloaded into the same directory)
#the problem description can be found here: http://opensees.berkeley.edu/wiki/index.php/Examples_Manual(example: 2c)
# --------------------------------------------------------------------------------------------------
# OpenSees (Tcl) code by: Silvia Mazzoni & Frank McKenna, 2006
#
# ^Y
# |
# 2 __
# | |
# | |
# | |
# (1) LCol
# | |
# | |
# | |
# =1= _|_ -------->X
#
# SET UP ----------------------------------------------------------------------------
import openseespy.opensees as op
#import the os module
import os
import math
op.wipe()
#########################################################################################################################################################################
#to create a directory at specified path with name "Data"
os.chdir('C:\\Opensees Python\\OpenseesPy examples')
#this will create the directory with name 'Data' and will update it when we rerun the analysis, otherwise we have to keep deleting the old 'Data' Folder
dir = "C:\\Opensees Python\\OpenseesPy examples\\Data-2c"
if not os.path.exists(dir):
os.makedirs(dir)
#this will create just 'Data' folder
#os.mkdir("Data")
#detect the current working directory
#path1 = os.getcwd()
#print(path1)
#########################################################################################################################################################################
#########################################################################################################################################################################
op.model('basic', '-ndm', 2, '-ndf', 3)
LCol = 432.0 # column length
Weight = 2000.0 # superstructure weight
# define section geometry
HCol = 60.0 # Column Depth
BCol = 60.0 # Column Width
PCol =Weight # nodal dead-load weight per column
g = 386.4
Mass = PCol/g
ACol = HCol*BCol*1000 # cross-sectional area, make stiff
IzCol = (BCol*math.pow(HCol,3))/12 # Column moment of inertia
op.node(1, 0.0, 0.0)
op.node(2, 0.0, LCol)
op.fix(1, 1, 1, 1)
op.mass(2, Mass, 1e-9, 0.0)
ColSecTag = 1 # assign a tag number to the column section
coverCol = 5.0 # Column cover to reinforcing steel NA.
numBarsCol = 16 # number of longitudinal-reinforcement bars in column. (symmetric top & bot)
barAreaCol = 2.25 # area of longitudinal-reinforcement bars
# MATERIAL parameters
IDconcU = 1 # material ID tag -- unconfined cover concrete (here used for complete section)
IDreinf = 2 # material ID tag -- reinforcement
# nominal concrete compressive strength
fc = -4.0 # CONCRETE Compressive Strength (+Tension, -Compression)
Ec = 57*math.sqrt(-fc*1000) # Concrete Elastic Modulus (the term in sqr root needs to be in psi
# unconfined concrete
fc1U = fc # UNCONFINED concrete (todeschini parabolic model), maximum stress
eps1U = -0.003 # strain at maximum strength of unconfined concrete
fc2U = 0.2*fc1U # ultimate stress
eps2U = -0.01 # strain at ultimate stress
Lambda = 0.1 # ratio between unloading slope at $eps2 and initial slope $Ec
# tensile-strength properties
ftU = -0.14* fc1U # tensile strength +tension
Ets = ftU/0.002 # tension softening stiffness
Fy = 66.8 # STEEL yield stress
Es = 29000.0 # modulus of steel
Bs = 0.01 # strain-hardening ratio
R0 = 18.0 # control the transition from elastic to plastic branches
cR1 = 0.925 # control the transition from elastic to plastic branches
cR2 = 0.15 # control the transition from elastic to plastic branches
op.uniaxialMaterial('Concrete02', IDconcU, fc1U, eps1U, fc2U, eps2U, Lambda, ftU, Ets) # build cover concrete (unconfined)
op.uniaxialMaterial('Steel02', IDreinf, Fy, Es, Bs, R0,cR1,cR2) # build reinforcement material
# FIBER SECTION properties -------------------------------------------------------------
# symmetric section
# y
# ^
# |
# --------------------- -- --
# | o o o | | -- cover
# | | |
# | | |
# z <--- | + | H
# | | |
# | | |
# | o o o | | -- cover
# --------------------- -- --
# |-------- B --------|
#
# RC section:
coverY = HCol/2.0 # The distance from the section z-axis to the edge of the cover concrete -- outer edge of cover concrete
coverZ = BCol/2.0 # The distance from the section y-axis to the edge of the cover concrete -- outer edge of cover concrete
coreY = coverY-coverCol
coreZ = coverZ-coverCol
nfY = 16 # number of fibers for concrete in y-direction
nfZ = 4 # number of fibers for concrete in z-direction
op.section('Fiber', ColSecTag)
op.patch('quad', IDconcU, nfZ, nfY, -coverY,coverZ, -coverY,-coverZ, coverY,-coverZ, coverY,coverZ) # Define the concrete patch
op.layer('straight', IDreinf, numBarsCol, barAreaCol, -coreY,coreZ,-coreY,-coreZ)
op.layer('straight', IDreinf, numBarsCol, barAreaCol, coreY,coreZ, coreY,-coreZ)
ColTransfTag = 1
op.geomTransf('Linear', ColTransfTag)
numIntgrPts = 5
eleTag = 1
#import InelasticFiberSection
op.element('nonlinearBeamColumn', eleTag, 1, 2, numIntgrPts, ColSecTag, ColTransfTag)
op.recorder('Node', '-file', 'Data-2c/DFree.out','-time', '-node', 2, '-dof', 1,2,3, 'disp')
op.recorder('Node', '-file', 'Data-2c/DBase.out','-time', '-node', 1, '-dof', 1,2,3, 'disp')
op.recorder('Node', '-file', 'Data-2c/RBase.out','-time', '-node', 1, '-dof', 1,2,3, 'reaction')
#op.recorder('Drift', '-file', 'Data-2c/Drift.out','-time', '-node', 1, '-dof', 1,2,3, 'disp')
op.recorder('Element', '-file', 'Data-2c/FCol.out','-time', '-ele', 1, 'globalForce')
op.recorder('Element', '-file', 'Data-2c/ForceColSec1.out','-time', '-ele', 1, 'section', 1, 'force')
#op.recorder('Element', '-file', 'Data-2c/DCol.out','-time', '-ele', 1, 'deformations')
#defining gravity loads
op.timeSeries('Linear', 1)
op.pattern('Plain', 1, 1)
op.load(2, 0.0, -PCol, 0.0)
Tol = 1e-8 # convergence tolerance for test
NstepGravity = 10
DGravity = 1/NstepGravity
op.integrator('LoadControl', DGravity) # determine the next time step for an analysis
op.numberer('Plain') # renumber dof's to minimize band-width (optimization), if you want to
op.system('BandGeneral') # how to store and solve the system of equations in the analysis
op.constraints('Plain') # how it handles boundary conditions
op.test('NormDispIncr', Tol, 6) # determine if convergence has been achieved at the end of an iteration step
op.algorithm('Newton') # use Newton's solution algorithm: updates tangent stiffness at every iteration
op.analysis('Static') # define type of analysis static or transient
op.analyze(NstepGravity) # apply gravity
op.loadConst('-time', 0.0) #maintain constant gravity loads and reset time to zero
#applying Dynamic Ground motion analysis
GMdirection = 1
GMfile = 'BM68elc.acc'
GMfact = 1.0
Lambda = op.eigen('-fullGenLapack', 1) # eigenvalue mode 1
import math
Omega = math.pow(Lambda, 0.5)
betaKcomm = 2 * (0.02/Omega)
xDamp = 0.02 # 2% damping ratio
alphaM = 0.0 # M-prop. damping; D = alphaM*M
betaKcurr = 0.0 # K-proportional damping; +beatKcurr*KCurrent
betaKinit = 0.0 # initial-stiffness proportional damping +beatKinit*Kini
op.rayleigh(alphaM,betaKcurr, betaKinit, betaKcomm) # RAYLEIGH damping
# Uniform EXCITATION: acceleration input
IDloadTag = 400 # load tag
dt = 0.01 # time step for input ground motion
GMfatt = 1.0 # data in input file is in g Unifts -- ACCELERATION TH
maxNumIter = 10
op.timeSeries('Path', 2, '-dt', dt, '-filePath', GMfile, '-factor', GMfact)
op.pattern('UniformExcitation', IDloadTag, GMdirection, '-accel', 2)
op.wipeAnalysis()
op.constraints('Transformation')
op.numberer('Plain')
op.system('BandGeneral')
op.test('EnergyIncr', Tol, maxNumIter)
op.algorithm('ModifiedNewton')
NewmarkGamma = 0.5
NewmarkBeta = 0.25
op.integrator('Newmark', NewmarkGamma, NewmarkBeta)
op.analysis('Transient')
DtAnalysis = 0.01
TmaxAnalysis = 10.0
Nsteps = int(TmaxAnalysis/ DtAnalysis)
ok = op.analyze(Nsteps, DtAnalysis)
tCurrent = op.getTime()
# for gravity analysis, load control is fine, 0.1 is the load factor increment (http://opensees.berkeley.edu/wiki/index.php/Load_Control)
test = {1:'NormDispIncr', 2: 'RelativeEnergyIncr', 4: 'RelativeNormUnbalance',5: 'RelativeNormDispIncr', 6: 'NormUnbalance'}
algorithm = {1:'KrylovNewton', 2: 'SecantNewton' , 4: 'RaphsonNewton',5: 'PeriodicNewton', 6: 'BFGS', 7: 'Broyden', 8: 'NewtonLineSearch'}
for i in test:
for j in algorithm:
if ok != 0:
if j < 4:
op.algorithm(algorithm[j], '-initial')
else:
op.algorithm(algorithm[j])
op.test(test[i], Tol, 1000)
ok = op.analyze(Nsteps, DtAnalysis)
print(test[i], algorithm[j], ok)
if ok == 0:
break
else:
continue
u2 = op.nodeDisp(2, 1)
print("u2 = ", u2)
op.wipe()
|