1
00:00:00,040 --> 00:00:02,470
The following content is
provided under a Creative

2
00:00:02,470 --> 00:00:03,880
Commons license.

3
00:00:03,880 --> 00:00:06,920
Your support will help MIT
OpenCourseWare continue to

4
00:00:06,920 --> 00:00:10,570
offer high quality educational
resources for free.

5
00:00:10,570 --> 00:00:13,470
To make a donation or view
additional materials from

6
00:00:13,470 --> 00:00:17,872
hundreds of MIT courses, visit
MIT OpenCourseWare at

7
00:00:17,872 --> 00:00:19,122
ocw.mit.edu.

8
00:00:22,130 --> 00:00:23,870
PROFESSOR: Ladies and gentlemen,
welcome to this

9
00:00:23,870 --> 00:00:26,570
lecture on nonlinear finite
element analysis of solids and

10
00:00:26,570 --> 00:00:28,010
structures.

11
00:00:28,010 --> 00:00:30,840
In this lecture, I would like
to continue to consider the

12
00:00:30,840 --> 00:00:33,650
plate with a hole that we
already considered in the

13
00:00:33,650 --> 00:00:34,830
previous lecture.

14
00:00:34,830 --> 00:00:36,550
But I now would like to
turn our attention

15
00:00:36,550 --> 00:00:38,910
to a nonlinear solution.

16
00:00:38,910 --> 00:00:41,920
As we mentioned in previous
lectures, a nonlinear analysis

17
00:00:41,920 --> 00:00:45,500
should only be performed only
once a linear solution has

18
00:00:45,500 --> 00:00:46,790
been obtained.

19
00:00:46,790 --> 00:00:49,680
The linear solution checks the
finite element model and

20
00:00:49,680 --> 00:00:52,260
yields valuable insight
into what

21
00:00:52,260 --> 00:00:54,390
nonlinearities are important.

22
00:00:54,390 --> 00:00:57,630
And once again, we considered
the linear solution of this

23
00:00:57,630 --> 00:00:59,585
plate in the previous lecture.

24
00:00:59,585 --> 00:01:03,110
We now want to go on with
the nonlinear solution.

25
00:01:03,110 --> 00:01:06,280
Here we have the plate with
the hole once again.

26
00:01:09,340 --> 00:01:13,630
It's a square plate subjected
to the loading shown.

27
00:01:13,630 --> 00:01:15,940
Here is the whole.

28
00:01:15,940 --> 00:01:17,730
These were the material
data that we used

29
00:01:17,730 --> 00:01:19,240
in the linear analysis.

30
00:01:19,240 --> 00:01:21,960
The thickness of the plate
is given here.

31
00:01:21,960 --> 00:01:26,170
We consider only one quarter
of the plate because of

32
00:01:26,170 --> 00:01:31,240
symmetry conditions, we can
considering that one quarter,

33
00:01:31,240 --> 00:01:34,220
analyze the whole plate,
as we have discussed in

34
00:01:34,220 --> 00:01:36,090
the previous lecture.

35
00:01:36,090 --> 00:01:39,610
In the previous lecture, we
also showed how we use

36
00:01:39,610 --> 00:01:44,540
ADINA-IN to generate the
data for this mesh.

37
00:01:44,540 --> 00:01:49,640
And this input data then is
used in ADINA to actually

38
00:01:49,640 --> 00:01:52,040
perform the analysis.

39
00:01:52,040 --> 00:01:54,560
We did the analysis for
linear conditions in

40
00:01:54,560 --> 00:01:56,300
the previous lecture.

41
00:01:56,300 --> 00:01:59,660
Some important considerations
for the nonlinear analysis are

42
00:01:59,660 --> 00:02:04,000
now what material model to
select, what displacement

43
00:02:04,000 --> 00:02:07,780
strain assumptions to make,
what sequence of load

44
00:02:07,780 --> 00:02:11,890
application to choose, and
what nonlinear equation

45
00:02:11,890 --> 00:02:13,070
solution strategy and

46
00:02:13,070 --> 00:02:15,220
convergence criteria to select.

47
00:02:15,220 --> 00:02:20,090
We will address these issues
in this lecture.

48
00:02:20,090 --> 00:02:23,770
We use, once again,
the ADINA system.

49
00:02:23,770 --> 00:02:24,740
Now, of course, for the

50
00:02:24,740 --> 00:02:27,990
elasto-plastic static response.

51
00:02:27,990 --> 00:02:31,880
We will also investigate the
effect on the response when a

52
00:02:31,880 --> 00:02:36,410
shaft is placed into
the plate hole.

53
00:02:36,410 --> 00:02:40,440
Some important observations
regarding the nonlinear

54
00:02:40,440 --> 00:02:44,190
analysis are given on
this viewgraph.

55
00:02:44,190 --> 00:02:47,630
First of all, we notice that
the recommendations that we

56
00:02:47,630 --> 00:02:51,820
discussed regarding the linear
analysis that we discussed in

57
00:02:51,820 --> 00:02:56,030
the previous lecture are also
very valid here of course.

58
00:02:56,030 --> 00:02:59,140
But for the nonlinear analysis,
we need also to

59
00:02:59,140 --> 00:03:03,600
consider and be careful with the
sequence and incremental

60
00:03:03,600 --> 00:03:07,510
magnitudes of load application
and the choice of convergence

61
00:03:07,510 --> 00:03:09,030
tolerances.

62
00:03:09,030 --> 00:03:12,780
We ill address, of course,
these issues just now.

63
00:03:12,780 --> 00:03:16,720
The first analysis that I'd like
to discuss with you is a

64
00:03:16,720 --> 00:03:19,740
limit load calculation
of the plate.

65
00:03:19,740 --> 00:03:25,130
Here we show the plate and the
load, p, will increase

66
00:03:25,130 --> 00:03:32,830
continuously up to a maximum
value and then decrease to 0.

67
00:03:32,830 --> 00:03:37,270
The plate is modelled as an
elasto-plastic material.

68
00:03:37,270 --> 00:03:40,830
And the material assumption
is summarized on

69
00:03:40,830 --> 00:03:42,540
this viewgraph here.

70
00:03:42,540 --> 00:03:44,150
Here are the material
properties.

71
00:03:44,150 --> 00:03:47,590
We assume basically
it is a steel.

72
00:03:47,590 --> 00:03:52,310
Notice the stress strain
law is shown here.

73
00:03:52,310 --> 00:03:55,330
We assume isotropic hardening
in the analysis.

74
00:03:55,330 --> 00:03:59,690
We discussed what this means
in an earlier lecture.

75
00:03:59,690 --> 00:04:03,400
The initial Young's modulus is
the one that we use for the

76
00:04:03,400 --> 00:04:04,940
linear analysis.

77
00:04:04,940 --> 00:04:07,070
Nu is equal to 0.3.

78
00:04:07,070 --> 00:04:10,350
And the strain hardening
modulus is given here.

79
00:04:12,890 --> 00:04:17,839
This idealization is probably
only applicable to small

80
00:04:17,839 --> 00:04:20,870
strain conditions,
strains that are

81
00:04:20,870 --> 00:04:23,940
smaller than 2% roughly.

82
00:04:23,940 --> 00:04:28,680
The maximum that you would want
to allow is probably 4%.

83
00:04:28,680 --> 00:04:33,000
And we will actually perform
the analysis first using a

84
00:04:33,000 --> 00:04:36,550
materially nonlinear
only formulation.

85
00:04:36,550 --> 00:04:40,990
This means, as we discussed in
the early lectures, that we

86
00:04:40,990 --> 00:04:44,080
neglect all kinematic
nonlinearities, that we only

87
00:04:44,080 --> 00:04:46,240
include the material
nonlinearities in the

88
00:04:46,240 --> 00:04:48,180
analysis, these material
nonlinearities.

89
00:04:50,880 --> 00:04:55,050
Later on, we however want to
also perform in this lecture

90
00:04:55,050 --> 00:04:59,200
an analysis that includes the
displacement large quotations

91
00:04:59,200 --> 00:05:01,620
and in fact even large
strain conditions.

92
00:05:01,620 --> 00:05:05,530
And we will study those analysis
results in comparison

93
00:05:05,530 --> 00:05:08,650
to the material nonlinear
only analysis results.

94
00:05:08,650 --> 00:05:11,090
The load history used
for the analysis is

95
00:05:11,090 --> 00:05:13,050
shown on this viewgraph.

96
00:05:13,050 --> 00:05:16,660
You can see that we are
increasingly linearly the load

97
00:05:16,660 --> 00:05:21,880
up to a maximum value of 650
MPa, megapascals, and then

98
00:05:21,880 --> 00:05:25,380
suddenly decrease
the load to 0.

99
00:05:25,380 --> 00:05:31,100
Notice we are using altogether
14 steps, 13 to increase the

100
00:05:31,100 --> 00:05:34,000
load and just one step
to decrease the load.

101
00:05:34,000 --> 00:05:37,060
Of course, we are having
here a time axis.

102
00:05:37,060 --> 00:05:40,930
But the load step or time
step that we used was

103
00:05:40,930 --> 00:05:44,100
delta t equal to 1.

104
00:05:44,100 --> 00:05:48,070
Well we performed this analysis
a few weeks ago in my

105
00:05:48,070 --> 00:05:50,150
laboratory at MIT.

106
00:05:50,150 --> 00:05:55,220
And we brought in a video crew
to video record our actions.

107
00:05:55,220 --> 00:05:59,690
I'd like to now share with you
what we have recorded and also

108
00:05:59,690 --> 00:06:05,820
narrate to you what actually is
happening in the computer

109
00:06:05,820 --> 00:06:09,510
run as we prepare the computer
run, as we run it, and also

110
00:06:09,510 --> 00:06:11,790
interprets the resides.

111
00:06:11,790 --> 00:06:16,680
Our first step is to modify
the input data that we

112
00:06:16,680 --> 00:06:19,210
prepared in the previous
lecture for the linear

113
00:06:19,210 --> 00:06:20,540
analysis of the plate.

114
00:06:20,540 --> 00:06:24,910
We now have to, of course,
modify this input data.

115
00:06:24,910 --> 00:06:29,130
First of all, to introduce the
load curve, this load history

116
00:06:29,130 --> 00:06:32,880
curve that we just discussed.

117
00:06:32,880 --> 00:06:38,490
And then we also have to modify
the material data to

118
00:06:38,490 --> 00:06:41,260
correspond to the elasto-plastic
material data

119
00:06:41,260 --> 00:06:43,740
that we now want to associate
with a plate.

120
00:06:43,740 --> 00:06:49,240
So let us look now at the video
record of what we did

121
00:06:49,240 --> 00:06:53,430
some weeks ago in my laboratory
at MIT regarding

122
00:06:53,430 --> 00:06:57,750
the change of these
input data.

123
00:06:57,750 --> 00:06:59,820
Here we see once more the
mesh that we're using

124
00:06:59,820 --> 00:07:01,760
to analyze the plate.

125
00:07:01,760 --> 00:07:04,950
And now we prepare input
data for ADINA-IN.

126
00:07:04,950 --> 00:07:07,250
Here we input the time function
that we employ.

127
00:07:10,220 --> 00:07:16,200
You recognize the function
points for time 0, 13, and 14

128
00:07:16,200 --> 00:07:32,100
with the values 0, 6.5, 0.

129
00:07:32,100 --> 00:07:35,430
We also input that 14 steps are
used in the analysis, that

130
00:07:35,430 --> 00:07:38,340
time step delta t is 1.

131
00:07:38,340 --> 00:07:40,630
Next we input the material
definition.

132
00:07:40,630 --> 00:07:43,700
And note that there is a
typographical error.

133
00:07:43,700 --> 00:07:48,100
We typed plestic instead
of plastic.

134
00:07:48,100 --> 00:07:51,880
We try to do the typing fast and
did not notice the error.

135
00:07:51,880 --> 00:07:54,790
Notice the Young's module E,
Poisson's ratio nu, the strain

136
00:07:54,790 --> 00:07:57,950
hardening modulus ET, and the
yield stress [? sigma ?]

137
00:07:57,950 --> 00:07:59,200
yield are defined.

138
00:08:01,590 --> 00:08:04,220
Because of the typographical
error, the program prints out

139
00:08:04,220 --> 00:08:07,300
an error message, namely the
plestic material is not found

140
00:08:07,300 --> 00:08:09,430
in the library.

141
00:08:09,430 --> 00:08:11,410
Here we see the library
of material models

142
00:08:11,410 --> 00:08:12,680
available in ADINA.

143
00:08:12,680 --> 00:08:16,830
The library consists of the
material models elastic,

144
00:08:16,830 --> 00:08:22,830
orthotropic, thermo-elastic,
and so on and so on.

145
00:08:22,830 --> 00:08:24,780
We know retype the material
data definition.

146
00:08:44,140 --> 00:08:46,660
We also do not want to use
equilibrium iterations.

147
00:08:49,400 --> 00:08:54,060
The default in ADINA is to use
equilibrium iterations.

148
00:08:54,060 --> 00:08:57,680
Actually, the BFGS method we
discussed earlier because

149
00:08:57,680 --> 00:08:59,860
large errors of solution
can accumulate when

150
00:08:59,860 --> 00:09:01,860
iterations are not used.

151
00:09:01,860 --> 00:09:03,930
We discussed all of
this earlier.

152
00:09:03,930 --> 00:09:06,710
Let's see what happens when we
do not iterate in the solution

153
00:09:06,710 --> 00:09:09,450
of this problem, just
as a point of study.

154
00:09:09,450 --> 00:09:12,150
We now finally by the command
ADINA generate

155
00:09:12,150 --> 00:09:14,190
the ADINA data input.

156
00:09:14,190 --> 00:09:16,880
Note that in this input
preparation we only change the

157
00:09:16,880 --> 00:09:19,500
data from the linear analysis
data used in the previous

158
00:09:19,500 --> 00:09:22,200
lecture to the data for the
nonlinear analysis we want to

159
00:09:22,200 --> 00:09:23,450
perform now.

160
00:09:26,030 --> 00:09:30,420
Having set up the proper input
data for ADINA-IN and having

161
00:09:30,420 --> 00:09:34,490
used ADINA-IN to generate the
input data for ADINA, we can

162
00:09:34,490 --> 00:09:38,440
now execute that input data with
ADINA obtain our first

163
00:09:38,440 --> 00:09:40,580
analysis results.

164
00:09:40,580 --> 00:09:45,490
We evaluate these analysis
results by plotting the force

165
00:09:45,490 --> 00:09:49,850
applied here as a function
of the displacements

166
00:09:49,850 --> 00:09:53,360
corresponding to this
motion as well.

167
00:09:53,360 --> 00:09:58,470
And we will see that the force
displacement curve looks

168
00:09:58,470 --> 00:09:59,850
rather unphysical.

169
00:09:59,850 --> 00:10:02,020
In other words, the
results don't make

170
00:10:02,020 --> 00:10:04,420
much physical sense.

171
00:10:04,420 --> 00:10:06,780
So we search for
an explanation.

172
00:10:06,780 --> 00:10:08,750
Why is that so?

173
00:10:08,750 --> 00:10:12,720
And we will find that the reason
is that we did not use

174
00:10:12,720 --> 00:10:15,300
equilibrium iterations
in the analysis.

175
00:10:15,300 --> 00:10:20,120
In fact, if you go back, you
will see that we deliberately

176
00:10:20,120 --> 00:10:22,750
did not want to use equilibrium
iterations in this

177
00:10:22,750 --> 00:10:27,280
first analysis, although in
ADINA the default is to use

178
00:10:27,280 --> 00:10:29,660
equipment directions.

179
00:10:29,660 --> 00:10:34,720
But I wanted to once show you
what kind of results you must

180
00:10:34,720 --> 00:10:37,780
expect if you don't use
equilibrium iterations.

181
00:10:37,780 --> 00:10:40,020
So we realized that we should
really use equilibrium

182
00:10:40,020 --> 00:10:42,800
iterations and that we will, of
course, have to change our

183
00:10:42,800 --> 00:10:47,840
input a little bit through
ADINA-IN in order to perform

184
00:10:47,840 --> 00:10:49,520
equilibrium iterations.

185
00:10:49,520 --> 00:10:54,230
The load history that we will
still be using is the same.

186
00:10:54,230 --> 00:10:55,790
Here it is shown once again.

187
00:10:55,790 --> 00:11:00,020
But now we will use the default
method of equilibrium

188
00:11:00,020 --> 00:11:03,570
iterations, the BFGS method.

189
00:11:03,570 --> 00:11:06,540
And this one will be applied,
this method of equilibrium

190
00:11:06,540 --> 00:11:09,690
iteration will be used
for each load step.

191
00:11:09,690 --> 00:11:13,730
Once again, 13 load steps up
and one load step down.

192
00:11:13,730 --> 00:11:17,490
The convergence criteria that
we using in the analysis are

193
00:11:17,490 --> 00:11:21,150
show here, the convergence
criteria on energy.

194
00:11:21,150 --> 00:11:23,920
And we talked about this one
quite extensively in a

195
00:11:23,920 --> 00:11:25,010
previous lecture.

196
00:11:25,010 --> 00:11:28,830
And the convergence criteria on
the force, again, I'd like

197
00:11:28,830 --> 00:11:32,120
to refer you to our
previous lecture.

198
00:11:32,120 --> 00:11:35,860
When we apply equilibrium
iterations in each step, we

199
00:11:35,860 --> 00:11:38,820
will see that our results
look good.

200
00:11:38,820 --> 00:11:40,520
They make physical sense.

201
00:11:40,520 --> 00:11:43,420
In fact, they look
quite appealing.

202
00:11:43,420 --> 00:11:46,460
So let us look now at these
solution results.

203
00:11:46,460 --> 00:11:49,780
Let us go, in other words, to
what has happened in the

204
00:11:49,780 --> 00:11:52,120
laboratory the way we
have been video

205
00:11:52,120 --> 00:11:55,270
recording it earlier.

206
00:11:55,270 --> 00:11:58,310
Here we see the solution
results, the load applied as a

207
00:11:58,310 --> 00:12:00,620
function of the displacement,
the extension

208
00:12:00,620 --> 00:12:03,220
of the quarter plate.

209
00:12:03,220 --> 00:12:05,270
On the horizontal axis, we
measure the displacement.

210
00:12:11,050 --> 00:12:13,790
On the vertical axis, we
measures of value of the load,

211
00:12:13,790 --> 00:12:15,080
actually the pressure applied.

212
00:12:21,670 --> 00:12:23,440
So far the curve looks OK.

213
00:12:23,440 --> 00:12:26,340
But we show here only the
responsible for the first 13

214
00:12:26,340 --> 00:12:30,280
steps for which the load has
increased monotonically.

215
00:12:30,280 --> 00:12:31,860
here we see now the
load displacement

216
00:12:31,860 --> 00:12:35,160
response for all 14 steps.

217
00:12:35,160 --> 00:12:38,290
Notice that the scale on the
horizontal axis measuring

218
00:12:38,290 --> 00:12:40,560
displacement is different from
what we used before.

219
00:12:45,530 --> 00:12:49,090
Note that the 13 first steps
bring us to the maximum load

220
00:12:49,090 --> 00:12:52,090
and maximum positive
displacement and that the

221
00:12:52,090 --> 00:12:55,330
predicted unloading response
in step 14 is quite

222
00:12:55,330 --> 00:12:56,580
unrealistic.

223
00:12:59,890 --> 00:13:02,770
We obtain a large negative
displacement.

224
00:13:02,770 --> 00:13:05,840
As we will see, this is due to
not having used equilibrium

225
00:13:05,840 --> 00:13:08,200
iterations.

226
00:13:08,200 --> 00:13:11,120
Next, we look at the mesh and
study the plastic zones as

227
00:13:11,120 --> 00:13:12,690
they develop with
increasing load.

228
00:13:15,520 --> 00:13:17,620
A time code is given
about the mesh.

229
00:13:17,620 --> 00:13:20,482
This time code gives
the step number.

230
00:13:20,482 --> 00:13:24,870
It increases until time
is equal to 14.

231
00:13:24,870 --> 00:13:26,960
The plastic zones are
shown by shading the

232
00:13:26,960 --> 00:13:28,940
area that is plastic.

233
00:13:28,940 --> 00:13:30,810
For the first steps, there's
no plasticity.

234
00:13:44,810 --> 00:13:47,370
Then the plastic zone is small,
it develops around the

235
00:13:47,370 --> 00:14:00,050
hole and it grows rapidly
as the larger

236
00:14:00,050 --> 00:14:01,300
load levels are reached.

237
00:14:04,850 --> 00:14:08,305
Note also how the plastic zone
spreads through the elements.

238
00:14:08,305 --> 00:14:12,080
We used 3 by 3 Gauss numerical
integration and test whether

239
00:14:12,080 --> 00:14:15,130
an integration point
has gone plastic.

240
00:14:15,130 --> 00:14:17,460
If so, we shade the contributory
area of the

241
00:14:17,460 --> 00:14:18,960
integration point.

242
00:14:18,960 --> 00:14:21,120
As an average for each
integration point, the

243
00:14:21,120 --> 00:14:25,470
contributory area is 1/9 ninth
of the element area.

244
00:14:25,470 --> 00:14:29,200
Here at step 12, you can very
nicely see how the plastic

245
00:14:29,200 --> 00:14:32,052
zones have progressed through
the elements.

246
00:14:32,052 --> 00:14:34,270
The elastic plastic
interface boundary

247
00:14:34,270 --> 00:14:37,790
goes through the elements.

248
00:14:37,790 --> 00:14:40,960
Note that at step 14, after
unloading much off the plate

249
00:14:40,960 --> 00:14:41,980
is still plastic.

250
00:14:41,980 --> 00:14:43,230
This is quite unphysical.

251
00:14:46,340 --> 00:14:49,280
We now rerun the analysis with
equilibrium iterations and

252
00:14:49,280 --> 00:14:53,130
here is the load displacement
response we now obtain.

253
00:14:53,130 --> 00:14:55,470
First we look at the
scales on the axes.

254
00:15:15,140 --> 00:15:17,900
We note that the loading
response is similar to what we

255
00:15:17,900 --> 00:15:19,550
had before.

256
00:15:19,550 --> 00:15:21,270
Although a much larger
displacement is

257
00:15:21,270 --> 00:15:23,770
reached in steps 13.

258
00:15:23,770 --> 00:15:27,280
The unloading response in step
14 is now quite realistic,

259
00:15:27,280 --> 00:15:31,210
with a permanent positive
displacement at zero load.

260
00:15:31,210 --> 00:15:36,900
Finally, we show the plastic
zones for this analysis.

261
00:15:36,900 --> 00:15:39,880
Note that we show the initial
mesh time 0 and then

262
00:15:39,880 --> 00:15:43,750
immediately the time
equals 6 results.

263
00:15:43,750 --> 00:15:46,500
Initially, the plasticity
progresses as much as in the

264
00:15:46,500 --> 00:15:49,400
analysis without equilibrium
iterations, but the final

265
00:15:49,400 --> 00:15:52,720
spread of plasticity reached
in step 13 is larger.

266
00:15:52,720 --> 00:15:55,200
And after unloading of the
load at the end of the

267
00:15:55,200 --> 00:15:59,150
analysis, the complete
plate is elastic.

268
00:15:59,150 --> 00:16:02,110
However, clearly permanent
deformations have occurred as

269
00:16:02,110 --> 00:16:05,190
can be seen by looking at the
default mesh at time 14.

270
00:16:09,070 --> 00:16:12,000
As we discussed already, our
analysis results now look

271
00:16:12,000 --> 00:16:12,690
quite good.

272
00:16:12,690 --> 00:16:14,780
They look quite reasonable.

273
00:16:14,780 --> 00:16:18,390
But one additional way to
evaluate the analysis results

274
00:16:18,390 --> 00:16:20,500
is to plot stress vectors.

275
00:16:20,500 --> 00:16:24,230
We did so in the linear analysis
of the previous

276
00:16:24,230 --> 00:16:28,020
lecture when we also looked at
the analysis results obtained

277
00:16:28,020 --> 00:16:31,530
from this mesh, but of course,
in linear analysis.

278
00:16:31,530 --> 00:16:35,010
We want to do now the same for
the nonlinear analysis results

279
00:16:35,010 --> 00:16:36,430
that we obtained.

280
00:16:36,430 --> 00:16:40,750
And let us just quickly look
at what we're doing in the

281
00:16:40,750 --> 00:16:42,990
stress vector output.

282
00:16:42,990 --> 00:16:50,450
We plot at each integration
point two lines as shown here.

283
00:16:50,450 --> 00:16:56,120
If they are carrying an arrow,
then it is tensile stress.

284
00:16:56,120 --> 00:16:59,760
No arrow means compressive
stress.

285
00:16:59,760 --> 00:17:02,410
And notice these two
lines correspond to

286
00:17:02,410 --> 00:17:06,550
the principal stresses.

287
00:17:06,550 --> 00:17:11,460
Notice that the lengths of these
lines are proportional

288
00:17:11,460 --> 00:17:13,890
to the magnitudes
of the stresses.

289
00:17:13,890 --> 00:17:19,920
So let's now do a stress vector
plot for the mesh at

290
00:17:19,920 --> 00:17:24,020
time 13 and at time 14, in other
words, at maximum load

291
00:17:24,020 --> 00:17:28,170
application and after removal
of the total load, four the

292
00:17:28,170 --> 00:17:29,995
results that we just
have obtained.

293
00:17:32,890 --> 00:17:35,590
Here we see the stress vectors
plotted onto the total mesh

294
00:17:35,590 --> 00:17:40,150
for the stress state at time
13, that is at total load.

295
00:17:40,150 --> 00:17:42,500
We note of course, that there
is very much information,

296
00:17:42,500 --> 00:17:44,750
there are many stress vectors.

297
00:17:44,750 --> 00:17:47,570
To see any detail we have to
focus our attention onto

298
00:17:47,570 --> 00:17:48,820
certain elements.

299
00:17:51,150 --> 00:17:53,890
Here we now look closer at the
elements adjacent to the

300
00:17:53,890 --> 00:17:56,770
horizontal symmetry line.

301
00:17:56,770 --> 00:17:58,980
We note that the stress vectors
correspond to vertical

302
00:17:58,980 --> 00:18:00,715
tensile stresses as expected.

303
00:18:04,730 --> 00:18:08,040
At a top edge of the plate we
see tensile vertical stresses

304
00:18:08,040 --> 00:18:10,820
and tensile horizontal
stresses.

305
00:18:10,820 --> 00:18:13,660
The maximum stress at any
integration point is 1100

306
00:18:13,660 --> 00:18:17,610
megapascals and occurs
near the hole.

307
00:18:17,610 --> 00:18:20,940
Here we now see the stress
vector plot at time 14, that

308
00:18:20,940 --> 00:18:24,300
is after load removal.

309
00:18:24,300 --> 00:18:26,030
It is most interesting
to study the

310
00:18:26,030 --> 00:18:28,050
stress flow in the mesh.

311
00:18:28,050 --> 00:18:32,240
Note that the stresses flow
along and parallel to the free

312
00:18:32,240 --> 00:18:34,690
surface of the plate.

313
00:18:34,690 --> 00:18:38,170
This must be so because there
are no externally applied

314
00:18:38,170 --> 00:18:40,100
tractions anymore.

315
00:18:40,100 --> 00:18:42,060
Here we see the detail of
the stress flow in the

316
00:18:42,060 --> 00:18:43,390
corner of the plate.

317
00:18:43,390 --> 00:18:47,940
The stress vectors are parallel
to the free surface.

318
00:18:47,940 --> 00:18:51,080
And here is the stress flow in
the elements around the hole.

319
00:18:51,080 --> 00:18:52,660
The same observations apply.

320
00:18:56,110 --> 00:19:01,150
The maximum stress is
880.3 megapascals.

321
00:19:01,150 --> 00:19:03,705
This completes what I wanted to
show you in this phase of

322
00:19:03,705 --> 00:19:06,620
the analysis.

323
00:19:06,620 --> 00:19:08,620
This completes our materially
nonlinear only

324
00:19:08,620 --> 00:19:10,330
analysis of the plate.

325
00:19:10,330 --> 00:19:12,770
However, if we look at the
solution results once more

326
00:19:12,770 --> 00:19:17,770
closely, we find that in this
element here the magnitude of

327
00:19:17,770 --> 00:19:23,620
the strains is about 2% at the
end of load step 11, 4% at the

328
00:19:23,620 --> 00:19:28,060
end of load step 12, and
14% to 15% at the end

329
00:19:28,060 --> 00:19:29,340
of load step 13.

330
00:19:29,340 --> 00:19:32,240
In other words, at maximum
load application, we have

331
00:19:32,240 --> 00:19:34,430
certainly here large strains.

332
00:19:34,430 --> 00:19:38,270
And one might very well ask,
what is the effect of this

333
00:19:38,270 --> 00:19:40,760
large strain on the
analysis results?

334
00:19:40,760 --> 00:19:43,330
Of course, in the materially
nonlinear only solution, we

335
00:19:43,330 --> 00:19:47,500
did not include any kinematic
nonlinearities.

336
00:19:47,500 --> 00:19:51,670
So our next objective is then to
perform analysis that said

337
00:19:51,670 --> 00:19:54,350
include kinematic
nonlinearities.

338
00:19:54,350 --> 00:19:57,830
And we want to now proceed
with a total Lagrangian

339
00:19:57,830 --> 00:20:02,110
formulation analysis, which
includes large displacements,

340
00:20:02,110 --> 00:20:05,750
large rotations, but
only small strains.

341
00:20:05,750 --> 00:20:09,030
And I also want to share with
you some solution results that

342
00:20:09,030 --> 00:20:13,310
we obtained using an updated
Lagrangian formulation.

343
00:20:13,310 --> 00:20:15,740
We did not talk about
this formulation

344
00:20:15,740 --> 00:20:16,930
in the earlier lectures.

345
00:20:16,930 --> 00:20:20,090
We did talk about this
formulation, but not about

346
00:20:20,090 --> 00:20:21,610
that formulation.

347
00:20:21,610 --> 00:20:24,210
This formulation really
is best covered

348
00:20:24,210 --> 00:20:26,290
in a separate lecture.

349
00:20:26,290 --> 00:20:30,000
However, it's still very
interesting to look at the

350
00:20:30,000 --> 00:20:32,270
solution results that we obtain
we this formulation.

351
00:20:32,270 --> 00:20:36,190
If you want to read up on this
formulation, please refer to

352
00:20:36,190 --> 00:20:39,440
the study guide in which
a reference given.

353
00:20:39,440 --> 00:20:42,160
A paper is referred
to in which this

354
00:20:42,160 --> 00:20:43,630
formulation is described.

355
00:20:43,630 --> 00:20:48,610
So let us now look at the
solution results obtained from

356
00:20:48,610 --> 00:20:52,010
these three formulations.

357
00:20:52,010 --> 00:20:55,110
And the solution results that
we want to look at are once

358
00:20:55,110 --> 00:20:58,650
again the force displacement
curve for each of these

359
00:20:58,650 --> 00:21:00,720
formulations.

360
00:21:00,720 --> 00:21:04,830
In other words, force applies
here, displacement seen here,

361
00:21:04,830 --> 00:21:07,540
for these three formulations.

362
00:21:07,540 --> 00:21:11,345
Let's turn back to the
laboratory and see what are

363
00:21:11,345 --> 00:21:14,110
the results.

364
00:21:14,110 --> 00:21:17,390
Here we see the analysis results
for the MNO, that is

365
00:21:17,390 --> 00:21:21,100
the materially nonlinear only,
the TL, that is the total

366
00:21:21,100 --> 00:21:24,140
Lagrangian, and to UL, that
is the updated Lagrangian

367
00:21:24,140 --> 00:21:26,930
formulations.

368
00:21:26,930 --> 00:21:29,670
We look first at the horizontal
axis scale giving

369
00:21:29,670 --> 00:21:30,920
the displacement.

370
00:21:34,480 --> 00:21:37,540
And then at the vertical axis
scale giving the load that is

371
00:21:37,540 --> 00:21:40,830
the pressure applied.

372
00:21:40,830 --> 00:21:43,490
Notice that there are three, in
fact we will we later four

373
00:21:43,490 --> 00:21:44,910
distinct curves.

374
00:21:44,910 --> 00:21:47,840
However, under this much
plasticity, the curves are

375
00:21:47,840 --> 00:21:50,210
almost the same.

376
00:21:50,210 --> 00:21:52,840
The TL analysis results
corresponds to the smallest

377
00:21:52,840 --> 00:21:54,100
displacements.

378
00:21:54,100 --> 00:21:57,160
The MNO solution gives
larger displacements.

379
00:21:57,160 --> 00:21:59,535
And the UL solution gives the
largest displacements.

380
00:22:02,870 --> 00:22:05,890
For the UL solution, we actually
see two curves when

381
00:22:05,890 --> 00:22:07,310
looking closely.

382
00:22:07,310 --> 00:22:11,460
These correspond to using once
14 steps as for the TL and MNO

383
00:22:11,460 --> 00:22:14,030
analyses and then using
once twice the

384
00:22:14,030 --> 00:22:15,620
number of load steps.

385
00:22:15,620 --> 00:22:18,400
Note that the unloading response
in all solutions is

386
00:22:18,400 --> 00:22:20,690
quite the same.

387
00:22:20,690 --> 00:22:23,270
However, of course, the
permanent displacements at 0

388
00:22:23,270 --> 00:22:25,990
applied load are quite different
because the maximum

389
00:22:25,990 --> 00:22:30,070
displacements corresponding to
peak load were different.

390
00:22:30,070 --> 00:22:32,640
These analysis results underline
the importance of

391
00:22:32,640 --> 00:22:34,100
choosing the appropriate
kinematic

392
00:22:34,100 --> 00:22:36,310
formation for the analysis.

393
00:22:36,310 --> 00:22:38,980
Here, large strain effects are
quite significant at the very

394
00:22:38,980 --> 00:22:40,230
high load levels.

395
00:22:43,230 --> 00:22:47,230
In the next analysis we now
consider the effect of a shaft

396
00:22:47,230 --> 00:22:48,890
in the hole.

397
00:22:48,890 --> 00:22:52,830
Notice, we look at the same
plate as before except that we

398
00:22:52,830 --> 00:22:56,880
know first consider elastic
condition only.

399
00:22:56,880 --> 00:22:59,190
And the shaft is shown here.

400
00:22:59,190 --> 00:23:02,310
The shaft has this Young's
modulus and Poisson ratio,

401
00:23:02,310 --> 00:23:04,310
same as the plate.

402
00:23:04,310 --> 00:23:08,230
But it is 5 times thicker than
the plate and for the shaft we

403
00:23:08,230 --> 00:23:11,760
also consider plane strength
conditions.

404
00:23:11,760 --> 00:23:16,530
What we want to do is place a
shaft in there, the shaft

405
00:23:16,530 --> 00:23:20,200
being initially flush with the
hole, assuming no friction

406
00:23:20,200 --> 00:23:22,160
between the shaft
and the hole.

407
00:23:22,160 --> 00:23:27,240
And then we pull on the plate
and want to investigate what

408
00:23:27,240 --> 00:23:30,320
is the effect of having
that shaft there.

409
00:23:30,320 --> 00:23:35,720
The analysis input data have to
now be modified because we

410
00:23:35,720 --> 00:23:40,760
have to put the shaft in there
using finite elements as shown

411
00:23:40,760 --> 00:23:41,930
here in red.

412
00:23:41,930 --> 00:23:43,620
We used collapsed 8-node
elements to

413
00:23:43,620 --> 00:23:45,190
represent the shaft.

414
00:23:45,190 --> 00:23:47,730
In other words, these collapsed
8-node isoparametric

415
00:23:47,730 --> 00:23:49,580
elements become, of
course, triangular

416
00:23:49,580 --> 00:23:51,760
elements as shown here.

417
00:23:51,760 --> 00:23:55,330
Notice we now have a contact
surface here.

418
00:23:55,330 --> 00:23:58,530
And that contact surface is
modeled using a contact

419
00:23:58,530 --> 00:24:01,150
algorithm, which we did
not talk about in

420
00:24:01,150 --> 00:24:03,570
this series of lectures.

421
00:24:03,570 --> 00:24:08,560
This again, would be best
covered in another lecture.

422
00:24:08,560 --> 00:24:12,990
I'd like to refer you here to
another paper, the reference

423
00:24:12,990 --> 00:24:15,800
of which is also given in the
study guide, if you're

424
00:24:15,800 --> 00:24:18,590
interested in reading about
the contact algorithm.

425
00:24:18,590 --> 00:24:21,050
The contact algorithm can take
into account friction

426
00:24:21,050 --> 00:24:24,570
conditions as well, but in this
particular analysis, we

427
00:24:24,570 --> 00:24:29,820
assume 0 friction along
the contact surface.

428
00:24:29,820 --> 00:24:33,570
The solution procedure that we
are using is it the full

429
00:24:33,570 --> 00:24:36,480
Newton method without
line searches.

430
00:24:36,480 --> 00:24:38,830
And the convergence criteria
that we are

431
00:24:38,830 --> 00:24:40,480
using are listed here.

432
00:24:40,480 --> 00:24:43,480
These we have been talking
about earlier already.

433
00:24:43,480 --> 00:24:46,260
Here we now because of the
contact conditions have to

434
00:24:46,260 --> 00:24:50,370
introduce also this convergence
criterion, which

435
00:24:50,370 --> 00:24:52,860
is really a convergence
criterion on the incremental

436
00:24:52,860 --> 00:24:55,440
contact force.

437
00:24:55,440 --> 00:24:58,200
So let us now proceed
with this analysis.

438
00:24:58,200 --> 00:25:02,730
And once again, we perform the
analysis and of course, we're

439
00:25:02,730 --> 00:25:05,470
looking at solution results.

440
00:25:05,470 --> 00:25:08,170
Here we see the mesh of the
plate once more, the mesh we

441
00:25:08,170 --> 00:25:10,120
used in the previous analyses.

442
00:25:10,120 --> 00:25:13,310
We now need to change the input
data for the analysis to

443
00:25:13,310 --> 00:25:15,890
also define the shaft.

444
00:25:15,890 --> 00:25:18,500
This is done using ADINA-IN.

445
00:25:18,500 --> 00:25:21,390
We need to define the addition
nodal points and elements for

446
00:25:21,390 --> 00:25:24,380
the shaft in the same way as
we input earlier the nodal

447
00:25:24,380 --> 00:25:27,110
points and elements
of the plate.

448
00:25:27,110 --> 00:25:29,570
Let's look at the information
that defines the content

449
00:25:29,570 --> 00:25:31,760
condition between the
plate and the shaft.

450
00:25:31,760 --> 00:25:35,990
And here we see the input
for ADINA-IN.

451
00:25:35,990 --> 00:25:37,550
There are two contact
surfaces.

452
00:25:37,550 --> 00:25:40,250
The one is the plate hole
surface and the other is the

453
00:25:40,250 --> 00:25:41,960
shaft surface.

454
00:25:41,960 --> 00:25:45,280
We denote these two to be
a contact surface pair.

455
00:25:45,280 --> 00:25:48,200
Here you now see the mesh of
the shaft and the plate.

456
00:25:48,200 --> 00:25:50,225
The shaft is defined by
triangular elements.

457
00:25:53,730 --> 00:25:56,430
Here we see the default
mesh at maximum load.

458
00:25:56,430 --> 00:25:59,170
Note that the plate has been
extended vertically and has

459
00:25:59,170 --> 00:26:01,850
shrunk horizontally.

460
00:26:01,850 --> 00:26:04,250
The shaft has prevented the
hole to shrink much

461
00:26:04,250 --> 00:26:05,400
horizontally.

462
00:26:05,400 --> 00:26:07,970
And on top off the shaft,
a gap has opened.

463
00:26:07,970 --> 00:26:12,130
All of these deformations
are quite realistic.

464
00:26:12,130 --> 00:26:14,760
Here, we see just the shaft and
the ring of elements of

465
00:26:14,760 --> 00:26:16,300
the plate around it.

466
00:26:16,300 --> 00:26:19,840
Once again, the calculated
deformations make sense.

467
00:26:19,840 --> 00:26:22,610
If you look closely at the shaft
by itself, you observe

468
00:26:22,610 --> 00:26:26,990
that it has been compressed
horizontally by the plate.

469
00:26:26,990 --> 00:26:29,790
Let's look next at some
stress vector plots.

470
00:26:29,790 --> 00:26:32,270
These also show that a
physically realistic solution

471
00:26:32,270 --> 00:26:34,680
has been obtained.

472
00:26:34,680 --> 00:26:37,180
Here we see the stress vectors
in the element layer of the

473
00:26:37,180 --> 00:26:39,030
plate around the shaft.

474
00:26:39,030 --> 00:26:41,070
Note that the stress vectors
are plotted onto

475
00:26:41,070 --> 00:26:43,050
the original mesh.

476
00:26:43,050 --> 00:26:46,030
For the element adjacent to the
horizontal symmetry axis

477
00:26:46,030 --> 00:26:49,750
off the plate, we see a vertical
tensile stress and a

478
00:26:49,750 --> 00:26:52,170
horizontal compressive stress.

479
00:26:52,170 --> 00:26:54,700
Such stresses are
to be expected.

480
00:26:54,700 --> 00:26:57,240
The horizontal compressive
stress is, of course, due to

481
00:26:57,240 --> 00:26:58,600
the contact with the shaft.

482
00:27:02,250 --> 00:27:04,830
Note that going around the
shaft, the stresses in the

483
00:27:04,830 --> 00:27:08,310
plate align to be parallel to
the free surface of the hole,

484
00:27:08,310 --> 00:27:11,070
since there is only contact near
the horizontal symmetry

485
00:27:11,070 --> 00:27:13,060
axis of the plate.

486
00:27:13,060 --> 00:27:15,510
This completes what I wanted to
discuss with you for this

487
00:27:15,510 --> 00:27:18,540
phase of the analysis.

488
00:27:18,540 --> 00:27:21,390
Finally, I would like to look
with you at the analysis

489
00:27:21,390 --> 00:27:26,070
results we obtained when we
apply to this plate with the

490
00:27:26,070 --> 00:27:30,000
shaft 100 MPa up there
and down here.

491
00:27:30,000 --> 00:27:32,910
We assume that they plate
is made of an

492
00:27:32,910 --> 00:27:34,380
elasto-plastic material.

493
00:27:34,380 --> 00:27:37,540
In fact, we model that
material as shown

494
00:27:37,540 --> 00:27:39,850
in our early analysis.

495
00:27:39,850 --> 00:27:44,130
And in addition to this loading
here shown, also the

496
00:27:44,130 --> 00:27:45,930
shaft expands.

497
00:27:45,930 --> 00:27:48,680
It expands uniformly.

498
00:27:48,680 --> 00:27:53,490
And in fact, it expands 0.05%
based on the initial

499
00:27:53,490 --> 00:27:58,570
dimensions of the shaft during
each load step and we apply 10

500
00:27:58,570 --> 00:27:59,950
load steps.

501
00:27:59,950 --> 00:28:03,870
So the loading then all together
is in the first load

502
00:28:03,870 --> 00:28:06,770
step, 100 MPa applied here.

503
00:28:06,770 --> 00:28:12,610
And from the second to 11th load
step, we expand the shaft

504
00:28:12,610 --> 00:28:18,570
by 0.05% in diameter, so to
say, based on the initial

505
00:28:18,570 --> 00:28:20,550
dimensions.

506
00:28:20,550 --> 00:28:23,850
We use the updated Lagrangian
formulation to model the

507
00:28:23,850 --> 00:28:25,520
response of the plate.

508
00:28:25,520 --> 00:28:29,850
Let's look now at these
analysis results.

509
00:28:29,850 --> 00:28:31,780
Here we see just as a
reminder once more

510
00:28:31,780 --> 00:28:33,350
the mesh we are using.

511
00:28:33,350 --> 00:28:35,542
Also, here is once more
the detail of the

512
00:28:35,542 --> 00:28:37,880
mesh around the shaft.

513
00:28:37,880 --> 00:28:41,410
This is the default
mesh at step 1.

514
00:28:41,410 --> 00:28:44,070
The deformations are due to the
tensile load of the 100

515
00:28:44,070 --> 00:28:47,140
megapascals on the plate.

516
00:28:47,140 --> 00:28:51,140
Next we plot the plastic zones
in the plate as they develop

517
00:28:51,140 --> 00:28:53,330
when the shaft expands.

518
00:28:53,330 --> 00:28:56,500
Notice again the time code above
the mesh giving the step

519
00:28:56,500 --> 00:29:00,010
number since delta t equals 1.

520
00:29:00,010 --> 00:29:01,750
There are all together
11 steps.

521
00:29:01,750 --> 00:29:06,320
The shaft expands from step
2 step to step 11.

522
00:29:06,320 --> 00:29:09,500
We see the time code running and
at time 7 we see the first

523
00:29:09,500 --> 00:29:10,750
plasticity.

524
00:29:12,950 --> 00:29:16,270
This plasticity spreads as the
shaft further expands.

525
00:29:16,270 --> 00:29:19,210
The maximum plastic zone is,
of course, reached at the

526
00:29:19,210 --> 00:29:24,560
maximum expansion of the shaft,
that is at time 11.

527
00:29:24,560 --> 00:29:28,000
This completes what I wanted
to say about this analysis.

528
00:29:28,000 --> 00:29:30,480
Note that after each analysis
step we looked at the

529
00:29:30,480 --> 00:29:32,880
calculated deformations and
stresses is to identify

530
00:29:32,880 --> 00:29:34,420
whether these make sense.

531
00:29:37,000 --> 00:29:39,540
This brings us to the end of
this lecture and to the end of

532
00:29:39,540 --> 00:29:40,500
this course.

533
00:29:40,500 --> 00:29:43,500
I'd like to now just take a few
minutes for some closing

534
00:29:43,500 --> 00:29:45,840
remarks regarding the course.

535
00:29:45,840 --> 00:29:48,400
I mentioned already in the first
lecture that nonlinear

536
00:29:48,400 --> 00:29:50,880
finite element analysis
is a very large field.

537
00:29:50,880 --> 00:29:54,110
There are continuum mechanics
principles, numerical

538
00:29:54,110 --> 00:29:57,460
algorithms, and software
considerations.

539
00:29:57,460 --> 00:30:02,140
We could not cover in detail
many aspects of all of these

540
00:30:02,140 --> 00:30:04,850
fields in these 22 lectures.

541
00:30:04,850 --> 00:30:08,630
However, I do believe that the
22 lectures provide a good

542
00:30:08,630 --> 00:30:12,200
introduction and a good
foundation for further study.

543
00:30:12,200 --> 00:30:14,890
I would hope that you would
listen to these lectures with

544
00:30:14,890 --> 00:30:18,670
your colleagues, that these
lectures would initiate

545
00:30:18,670 --> 00:30:22,280
discussions, stimulations for
your work in nonlinear

546
00:30:22,280 --> 00:30:25,860
analysis and, of course,
also questions.

547
00:30:25,860 --> 00:30:28,500
We at MIT continue to
work in nonlinear

548
00:30:28,500 --> 00:30:30,160
finite element analysis.

549
00:30:30,160 --> 00:30:33,520
And we also offer from time
to time weekly courses.

550
00:30:33,520 --> 00:30:36,330
I would be glad to see some
off you at these weekly

551
00:30:36,330 --> 00:30:40,130
courses to share some of the
experiences that you have had

552
00:30:40,130 --> 00:30:44,930
listening to these video
lectures and also regarding

553
00:30:44,930 --> 00:30:47,460
your work in practice.

554
00:30:47,460 --> 00:30:51,040
Finally, I'd like to mention
that a video course of this

555
00:30:51,040 --> 00:30:54,750
nature can only be produced
through the concerted effort

556
00:30:54,750 --> 00:30:57,420
of a number of very
devoted people.

557
00:30:57,420 --> 00:31:00,660
I'd like to thank for their
collaboration and support Dick

558
00:31:00,660 --> 00:31:03,820
Norris, Elizabeth DeRienzo,
Pat [? Regan ?]

559
00:31:03,820 --> 00:31:07,420
of the Center of Advanced
Engineering Study at MIT, and

560
00:31:07,420 --> 00:31:09,650
Ted Sussman, my student.

561
00:31:09,650 --> 00:31:14,630
And very finally, thanks also
for the crew around here.

562
00:31:14,630 --> 00:31:15,880
Thank you for your attention.