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 --> 00:00:10,950 offer high quality educational resources for free to make a 5 00:00:10,950 --> 00:00:14,430 donation or view additional materials from hundreds of MIT 6 00:00:14,430 --> 00:00:17,872 courses, visit MIT OpenCourseWare at ocw.mit.edu. 7 00:00:21,296 --> 00:00:23,370 PROFESSOR: Ladies and gentlemen, welcome to this 8 00:00:23,370 --> 00:00:26,235 lecture on non-linear finite element analysis of solids and 9 00:00:26,235 --> 00:00:27,890 structures. 10 00:00:27,890 --> 00:00:30,770 In the previous lectures, we have considered quite a bit of 11 00:00:30,770 --> 00:00:33,510 theory related to non-linear finite element analysis in 12 00:00:33,510 --> 00:00:35,860 some example solutions. 13 00:00:35,860 --> 00:00:38,700 The objective in the next two lectures now, the last 14 00:00:38,700 --> 00:00:42,170 lectures of this video course, is to show how an actual 15 00:00:42,170 --> 00:00:46,030 finite element analysis is performed on the computer. 16 00:00:46,030 --> 00:00:49,760 We start with a linear solution in this lecture, and 17 00:00:49,760 --> 00:00:53,820 then consider a non-linear solution in the next lecture. 18 00:00:53,820 --> 00:00:58,930 We cannot discuss really, in this amount of time given, all 19 00:00:58,930 --> 00:01:02,520 the aspects of the analysis, but want to summarize and 20 00:01:02,520 --> 00:01:06,050 demonstrate on the computer the major steps of the 21 00:01:06,050 --> 00:01:09,840 analysis and concentrate on possible difficulties, 22 00:01:09,840 --> 00:01:15,200 possible pitfalls, and some general recommendations. 23 00:01:15,200 --> 00:01:18,460 As the example problem, we want to use the plate with a 24 00:01:18,460 --> 00:01:21,350 hole, that we already considered earlier. 25 00:01:21,350 --> 00:01:24,200 And we performed a linear analysis and then 26 00:01:24,200 --> 00:01:25,750 a non-linear analysis. 27 00:01:25,750 --> 00:01:28,530 Remember, I pointed out in the previous lectures that it is 28 00:01:28,530 --> 00:01:31,830 very important to always do linear analysis first before 29 00:01:31,830 --> 00:01:34,700 you go into a non-linear analysis. 30 00:01:34,700 --> 00:01:37,880 The elastic analysis is performed to obtain the stress 31 00:01:37,880 --> 00:01:41,440 concentration factor at the hole, then we do an 32 00:01:41,440 --> 00:01:46,020 elasto-plastic analysis to estimate the limit load, and 33 00:01:46,020 --> 00:01:49,820 an analysis also to investigate the effect of a 34 00:01:49,820 --> 00:01:51,440 shaft in the plate hole. 35 00:01:51,440 --> 00:01:55,070 These two analyses are being performed in the last lecture 36 00:01:55,070 --> 00:01:57,280 of the video course. 37 00:01:57,280 --> 00:02:01,430 The plate we are analyzing is shown on this view graph here. 38 00:02:01,430 --> 00:02:03,610 Notice it's a square plate. 39 00:02:03,610 --> 00:02:07,750 Here, we show the hole, the plate is loaded as shown up 40 00:02:07,750 --> 00:02:10,050 here, and down here. 41 00:02:10,050 --> 00:02:12,670 The material property for the elastic analysis are given 42 00:02:12,670 --> 00:02:17,130 here and the thickness of the plate is 0.01 meter. 43 00:02:17,130 --> 00:02:19,930 Because of symmetry conditions, we only need to 44 00:02:19,930 --> 00:02:22,710 consider this quarter here. 45 00:02:22,710 --> 00:02:25,370 Of course, using appropriate boundary conditions along 46 00:02:25,370 --> 00:02:29,880 these two lines. we will talk about that more later on. 47 00:02:29,880 --> 00:02:33,880 The first step for a finite element analysis is to select 48 00:02:33,880 --> 00:02:37,710 a computer program, and we, of course, use the ADINA system. 49 00:02:37,710 --> 00:02:42,430 ADINA-IN is the pre-processor to prepare, generate the 50 00:02:42,430 --> 00:02:43,810 finite element data. 51 00:02:43,810 --> 00:02:47,250 ADINA then solves the actual finite element model, and 52 00:02:47,250 --> 00:02:50,040 ADINA-PLOT is used to this display numerically or 53 00:02:50,040 --> 00:02:52,470 graphically the solution results. 54 00:02:52,470 --> 00:02:56,320 Schematically, we are sitting here at a terminal and we're 55 00:02:56,320 --> 00:02:59,170 inputting the data to ADINA-IN. 56 00:02:59,170 --> 00:03:03,220 We can also receive here, numerical output, and we can 57 00:03:03,220 --> 00:03:07,380 also plot on this terminal here, any of the information 58 00:03:07,380 --> 00:03:08,550 that we like to plot. 59 00:03:08,550 --> 00:03:10,200 This is a graphics terminal. 60 00:03:10,200 --> 00:03:13,190 Notice ADINA-IN, of course, communicates to a storage 61 00:03:13,190 --> 00:03:17,030 device and further on to ADINA, as we will 62 00:03:17,030 --> 00:03:19,650 discuss just now. 63 00:03:19,650 --> 00:03:22,630 The user inputs, in other words, or 64 00:03:22,630 --> 00:03:24,400 types into the terminal. 65 00:03:24,400 --> 00:03:27,690 ADINA-IN commands interactively or for batch 66 00:03:27,690 --> 00:03:31,670 processing and then the user checks also the input and the 67 00:03:31,670 --> 00:03:35,420 generated data on the graphics device, as I showed you on the 68 00:03:35,420 --> 00:03:38,020 previous view graph. 69 00:03:38,020 --> 00:03:43,750 ADINA-IN generates the input data for ADINA. 70 00:03:43,750 --> 00:03:46,965 The input data is checked internally in ADINA in for 71 00:03:46,965 --> 00:03:51,430 errors and inconsistency, and also is displayed as you are 72 00:03:51,430 --> 00:03:53,330 requesting it as a user. 73 00:03:53,330 --> 00:03:59,850 The degree of freedom numbers are generated and to obtain 74 00:03:59,850 --> 00:04:05,560 minimum bandwidth, we have a minimum bandwidth minimization 75 00:04:05,560 --> 00:04:09,020 algorithm in the program, as I will point out a bit 76 00:04:09,020 --> 00:04:12,480 stronger later on. 77 00:04:12,480 --> 00:04:18,459 ADINA data inputs then, is available to ADINA, and the 78 00:04:18,459 --> 00:04:24,350 user runs ADINA, and ADINA then stores the output data on 79 00:04:24,350 --> 00:04:29,600 a porthole file and on an output file. 80 00:04:29,600 --> 00:04:33,130 The output file, in other words, contains really the 81 00:04:33,130 --> 00:04:36,640 ADINA model data and the calculated results. 82 00:04:36,640 --> 00:04:41,740 We access ADINA porthole file using ADINA-PLOT. 83 00:04:41,740 --> 00:04:45,870 We can, of course, also look at the output file and see 84 00:04:45,870 --> 00:04:49,610 numerically the data that was calculated using ADINA. 85 00:04:52,610 --> 00:04:57,100 Here, we have the action displayed or schematically 86 00:04:57,100 --> 00:04:59,200 shown by the user. 87 00:04:59,200 --> 00:05:04,830 User uses ADINA-PLOT to fetch data from the ADINA porthole 88 00:05:04,830 --> 00:05:09,430 file and then ADINA-PLOT displays those data either 89 00:05:09,430 --> 00:05:12,220 numerically or graphically. 90 00:05:12,220 --> 00:05:17,480 Let's look very briefly at an overview of ADINA. 91 00:05:17,480 --> 00:05:20,610 The program can be used for static and dynamic solutions, 92 00:05:20,610 --> 00:05:24,250 for linear and non-linear analysis, for small and very 93 00:05:24,250 --> 00:05:28,030 large finite element models, and the formulations finite 94 00:05:28,030 --> 00:05:31,400 elements and numerical procedures used in the program 95 00:05:31,400 --> 00:05:35,640 have largely been discussed in this course. 96 00:05:35,640 --> 00:05:39,710 The displacement assumptions that can be employed for the 97 00:05:39,710 --> 00:05:43,340 finite element models are either infinitesimally small 98 00:05:43,340 --> 00:05:46,150 displacements, large displacements, large rotations 99 00:05:46,150 --> 00:05:50,480 but small strains, and large deformations, large strains. 100 00:05:50,480 --> 00:05:53,750 We discussed these assumptions, of course, also 101 00:05:53,750 --> 00:05:55,310 in the course. 102 00:05:55,310 --> 00:05:59,240 Material models that are available in isotropic linear 103 00:05:59,240 --> 00:06:02,110 elastic model, orthotropic linear elastic model, 104 00:06:02,110 --> 00:06:05,350 isotropic thermo-elastic model, a curve description 105 00:06:05,350 --> 00:06:08,300 model for analysis of geological materials, a 106 00:06:08,300 --> 00:06:14,000 concrete model, isothermal plasticity models, 107 00:06:14,000 --> 00:06:17,300 thermo-elastic-plastic and creep models, and non-linear 108 00:06:17,300 --> 00:06:22,430 elastic incompressible, and user-supplied models. 109 00:06:25,040 --> 00:06:29,540 The elements available in the program, is available number 110 00:06:29,540 --> 00:06:32,650 nodes tress element, an element that can have two 111 00:06:32,650 --> 00:06:35,780 nodes, three nodes, or four nodes. 112 00:06:35,780 --> 00:06:39,461 It can also be used as a ring element. 113 00:06:39,461 --> 00:06:42,990 A two-dimensional solid element that is used for plane 114 00:06:42,990 --> 00:06:46,840 stress axis symmetric and plane strain analysis. 115 00:06:46,840 --> 00:06:50,510 This also can have available number of nodes, from four 116 00:06:50,510 --> 00:06:54,300 nodes to nine nodes. 117 00:06:54,300 --> 00:06:56,800 Similarly, available number of nodes element for 118 00:06:56,800 --> 00:06:58,190 three-dimensional analysis. 119 00:07:01,980 --> 00:07:06,890 Then also a beam element, a 2-node beam element, Hermitian 120 00:07:06,890 --> 00:07:09,890 beam element. 121 00:07:09,890 --> 00:07:13,830 And the isoparametric beam element that we talked about 122 00:07:13,830 --> 00:07:14,920 in the course. 123 00:07:14,920 --> 00:07:20,020 This element can carry, or can be used with two nodes, or 124 00:07:20,020 --> 00:07:24,200 three nodes, or four nodes. 125 00:07:24,200 --> 00:07:28,260 A pipe element that we did not discuss in the course, but you 126 00:07:28,260 --> 00:07:31,950 might be interested in reading about that element is a curved 127 00:07:31,950 --> 00:07:36,390 beam element, of course, of pipe section. 128 00:07:36,390 --> 00:07:41,250 Which however, also includes the effects of ovalization So 129 00:07:41,250 --> 00:07:45,000 this element also carries, if desired ovalization degrees of 130 00:07:45,000 --> 00:07:47,740 freedoms at the nodes. 131 00:07:47,740 --> 00:07:52,140 And shell elements, we talked about the use of the 16-node 132 00:07:52,140 --> 00:07:57,420 element, and the MITC 4, the 4-node element. 133 00:07:57,420 --> 00:08:00,850 We also talked briefly about transition elements that I 134 00:08:00,850 --> 00:08:04,470 used to model shells, or thin structures 135 00:08:04,470 --> 00:08:08,330 that couple into solids. 136 00:08:08,330 --> 00:08:10,580 Let us summarize some important observations 137 00:08:10,580 --> 00:08:13,500 regarding finite element analysis. 138 00:08:13,500 --> 00:08:16,210 It's important to check the finite element data, of 139 00:08:16,210 --> 00:08:18,820 course, very carefully. 140 00:08:18,820 --> 00:08:20,310 The data must be checked prior to the 141 00:08:20,310 --> 00:08:21,730 actual response solution. 142 00:08:21,730 --> 00:08:25,410 This is done, of course, with the pre-processor, by plotting 143 00:08:25,410 --> 00:08:29,380 the data, looking at it very carefully, typically. 144 00:08:29,380 --> 00:08:33,330 And then after the response solution, you still want to 145 00:08:33,330 --> 00:08:39,200 check the input data once more by seeing whether the boundary 146 00:08:39,200 --> 00:08:42,350 conditions are properly satisfied, that you want to 147 00:08:42,350 --> 00:08:44,800 impose on to the model, whether the displacement and 148 00:08:44,800 --> 00:08:46,050 stress solution is a reasonable. 149 00:08:49,000 --> 00:08:51,970 Once the analysis has been performed, you want to very 150 00:08:51,970 --> 00:08:53,640 carefully evaluate and interpret 151 00:08:53,640 --> 00:08:55,390 the calculate response. 152 00:08:55,390 --> 00:08:58,130 You want to start in detail the calculated displacement 153 00:08:58,130 --> 00:09:00,360 and stresses along certain lines. 154 00:09:00,360 --> 00:09:02,960 In particular, look at stress jumps. 155 00:09:02,960 --> 00:09:06,120 We pointed that out already in an earlier lecture, and we 156 00:09:06,120 --> 00:09:10,200 will do so in our example solution again, just now. 157 00:09:10,200 --> 00:09:14,180 And here, I'd like to add that stress averaging, stress 158 00:09:14,180 --> 00:09:17,300 smoothing should only be done after the above careful 159 00:09:17,300 --> 00:09:18,230 evaluation. 160 00:09:18,230 --> 00:09:22,260 That's something important to keep in mind. 161 00:09:22,260 --> 00:09:25,790 I believe that you should first look at the stresses, 162 00:09:25,790 --> 00:09:29,310 the way they have been calculated by the program and 163 00:09:29,310 --> 00:09:32,020 then start thinking about stress smoothing. 164 00:09:32,020 --> 00:09:36,630 Only after you've gone through this phase here. 165 00:09:36,630 --> 00:09:42,410 The data for the construction of the finite element mesh, 166 00:09:42,410 --> 00:09:51,150 that we want to deal with in the example solution is input 167 00:09:51,150 --> 00:09:54,180 for this quarter of the plate, as I 168 00:09:54,180 --> 00:09:55,630 pointed out earlier already. 169 00:09:55,630 --> 00:10:00,180 We have these elastic material constants, we're looking at a 170 00:10:00,180 --> 00:10:01,590 plane stress analysis. 171 00:10:01,590 --> 00:10:03,510 This is the thickness of the plate. 172 00:10:03,510 --> 00:10:05,800 And once again, here is a loading. 173 00:10:05,800 --> 00:10:08,770 Notice, we are putting this boundary on rollers, and we 174 00:10:08,770 --> 00:10:12,720 want to put this boundary as well on rollers to model the 175 00:10:12,720 --> 00:10:16,640 symmetry conditions that we need to model in order to 176 00:10:16,640 --> 00:10:19,990 consider a whole plate, where we actually analyze here, only 177 00:10:19,990 --> 00:10:22,230 one quarter of that plate. 178 00:10:22,230 --> 00:10:24,770 The finite element mesh that we will be using is shown on 179 00:10:24,770 --> 00:10:25,550 this view graph. 180 00:10:25,550 --> 00:10:31,120 It consists of 64 8-node isoparametric elements. 181 00:10:31,120 --> 00:10:34,820 Well, we performed this analysis on the computer in my 182 00:10:34,820 --> 00:10:38,832 laboratory at MIT a few weeks ago, and we have brought in a 183 00:10:38,832 --> 00:10:42,060 video crew to record all the actions that we have been 184 00:10:42,060 --> 00:10:45,270 performing to actually complete the analysis. 185 00:10:45,270 --> 00:10:50,230 I like to now share with you what we have recorded and 186 00:10:50,230 --> 00:10:54,470 narrate to you as we go step by step through the analysis 187 00:10:54,470 --> 00:10:57,950 of this plate on the computer. 188 00:10:57,950 --> 00:11:02,060 Our first step is to look at how we are generating using 189 00:11:02,060 --> 00:11:06,400 ADINA-IN, how we are generating this mesh, and also 190 00:11:06,400 --> 00:11:11,210 the other data that are required for use of ADINA. 191 00:11:11,210 --> 00:11:15,000 So let's look at this first step now, after which I will 192 00:11:15,000 --> 00:11:20,140 then introduce you to the next step and narrate continuous 193 00:11:20,140 --> 00:11:23,660 narration of the analysis. 194 00:11:23,660 --> 00:11:25,780 Here we show briefly the hardware equipment we are 195 00:11:25,780 --> 00:11:28,490 using in my MIT laboratory. 196 00:11:28,490 --> 00:11:32,300 A MASSCOMP minicomputer with two megabytes of real memory, 197 00:11:32,300 --> 00:11:35,320 and 330 megabytes of disk storage. 198 00:11:35,320 --> 00:11:37,200 We also have a tape drive. 199 00:11:37,200 --> 00:11:39,600 The computer features virtual memory, and we use a 200 00:11:39,600 --> 00:11:41,045 Unix-based operating system. 201 00:11:44,560 --> 00:11:46,890 Roughly, for our purposes, the computer is 202 00:11:46,890 --> 00:11:50,670 equivalent to a VAX 750. 203 00:11:50,670 --> 00:11:51,940 We use two terminals. 204 00:11:51,940 --> 00:11:54,190 One terminal for alphanumerical and numerical 205 00:11:54,190 --> 00:11:57,410 input and output, and one terminal, the one to the 206 00:11:57,410 --> 00:11:58,660 right, for graphical output. 207 00:12:01,210 --> 00:12:02,210 We also have a plotter. 208 00:12:02,210 --> 00:12:05,110 We use this plotter to generate the figures of finite 209 00:12:05,110 --> 00:12:09,440 element meshes, and results for this course. 210 00:12:09,440 --> 00:12:11,640 Here comes my student, Ted [? Sossman, ?] 211 00:12:11,640 --> 00:12:13,660 who will sit at the terminal to input 212 00:12:13,660 --> 00:12:15,670 the data to the program. 213 00:12:15,670 --> 00:12:18,720 In what follows, we will see the data input prepared by Ted 214 00:12:18,720 --> 00:12:21,030 on the terminal at which he sits. 215 00:12:21,030 --> 00:12:23,730 Non-graphical output is displayed by that same 216 00:12:23,730 --> 00:12:26,990 terminal, whereas we will see graphical output displayed on 217 00:12:26,990 --> 00:12:29,540 the right terminal. 218 00:12:29,540 --> 00:12:31,200 Here, we see the start of input 219 00:12:31,200 --> 00:12:33,470 preparation for ADINA-IN. 220 00:12:33,470 --> 00:12:36,370 We have opened the data base, on which the data input and 221 00:12:36,370 --> 00:12:39,460 generated will be stored and have already input the title 222 00:12:39,460 --> 00:12:44,700 for the analysis, quarter plate with hole, 64 elements. 223 00:12:44,700 --> 00:12:47,420 We have also defined master degrees of freedom conditions 224 00:12:47,420 --> 00:12:50,820 by specifying the values of IDOF. 225 00:12:50,820 --> 00:12:54,330 1 means of a deleted degree of freedom, 0 means a free, 226 00:12:54,330 --> 00:12:56,360 existing degree of freedom. 227 00:12:56,360 --> 00:12:58,970 Here, all degrees of freedom have been deleted except for 228 00:12:58,970 --> 00:13:01,860 the yz displacements. 229 00:13:01,860 --> 00:13:03,920 Notice also that at our request, all 230 00:13:03,920 --> 00:13:05,840 text appears twice. 231 00:13:05,840 --> 00:13:08,900 After we have typed a line, the line is echoed back by the 232 00:13:08,900 --> 00:13:11,520 program merely for checking. 233 00:13:11,520 --> 00:13:14,020 In what follows, we now specify the coordinates of a 234 00:13:14,020 --> 00:13:17,110 few key points that defines the outline of the 235 00:13:17,110 --> 00:13:18,360 quarter of the plate. 236 00:13:22,660 --> 00:13:24,583 Note we define the y- and z-coordinates. 237 00:13:30,560 --> 00:13:39,100 First of node 1, then for nodes 2, 3, 4, 5, and 6. 238 00:13:46,670 --> 00:13:50,110 Note that these coordinates are input in free format. 239 00:13:50,110 --> 00:13:53,230 Here the node 6 input is not aligned with the other nodal 240 00:13:53,230 --> 00:13:54,480 point coordinate input. 241 00:13:56,970 --> 00:14:00,520 We now want to look at the plot of these nodal points. 242 00:14:00,520 --> 00:14:02,950 This is achieved by the frame and mesh commands. 243 00:14:10,880 --> 00:14:13,030 Here they are, the six points. 244 00:14:13,030 --> 00:14:17,670 Point 1 is the center of the hole, points 2 and 3 defines 245 00:14:17,670 --> 00:14:18,920 the boundary of the hole. 246 00:14:21,640 --> 00:14:24,850 Points 4, 5, 6 defines the remaining corners of the 247 00:14:24,850 --> 00:14:27,050 quarter plate. 248 00:14:27,050 --> 00:14:31,510 And here, you see the first set of generated nodes. 249 00:14:31,510 --> 00:14:34,210 Note that the nodal points have consecutive numbers along 250 00:14:34,210 --> 00:14:37,430 the vertical symmetry edge, except for the top and bottom 251 00:14:37,430 --> 00:14:41,700 nodes, numbers 3 and 4, similarly for the horizontal 252 00:14:41,700 --> 00:14:44,090 symmetry edge. 253 00:14:44,090 --> 00:14:46,540 This would mean a large bandwidth unless we use a 254 00:14:46,540 --> 00:14:48,410 bandwidth minimizer. 255 00:14:48,410 --> 00:14:51,150 And we will do so, hence we are not concerned with the 256 00:14:51,150 --> 00:14:54,800 nodal point numbering used at this stage. 257 00:14:54,800 --> 00:14:57,175 Next, we generate also the nodal points on the remaining 258 00:14:57,175 --> 00:14:59,630 edges of the quarter plate. 259 00:14:59,630 --> 00:15:02,810 And here they are. 260 00:15:02,810 --> 00:15:07,670 We now want to generate the elements of the plate. 261 00:15:07,670 --> 00:15:10,040 For this we define, first the material to be a elastic. 262 00:15:13,070 --> 00:15:18,120 Young's modulus E, Poisson's ratio NU. 263 00:15:25,900 --> 00:15:27,820 We want a plane stress element group. 264 00:15:36,110 --> 00:15:37,630 The Gauss integration order is 3x3. 265 00:15:40,570 --> 00:15:44,300 The material set has a number 1, this is the material set we 266 00:15:44,300 --> 00:15:45,550 just defined. 267 00:15:47,340 --> 00:15:51,320 The G-surface command next generates the 8-node elements 268 00:15:51,320 --> 00:15:54,070 in the domain defined by the corner points, so to 269 00:15:54,070 --> 00:15:55,450 say 6, 4, 3, 2. 270 00:15:59,260 --> 00:16:04,000 We now want to plot the generated element mesh, and 271 00:16:04,000 --> 00:16:05,250 here, you see it. 272 00:16:08,390 --> 00:16:12,500 Note once again, we use 8-note isoparametric elements, around 273 00:16:12,500 --> 00:16:14,010 the hole, they are curved elements. 274 00:16:16,850 --> 00:16:20,920 Finally, we also define in the ADINA-IN input the elements 275 00:16:20,920 --> 00:16:24,690 thicknesses to be 0.01 and the loads which correspond to the 276 00:16:24,690 --> 00:16:27,180 pulling on the plate. 277 00:16:27,180 --> 00:16:29,180 This [? end ?] completes the input preparation 278 00:16:29,180 --> 00:16:30,430 for ADINA-IN . 279 00:16:32,660 --> 00:16:35,330 ADINA-IN has now all the information to generate a 280 00:16:35,330 --> 00:16:38,380 complete input file ADINA. 281 00:16:38,380 --> 00:16:41,830 In addition, we also want to ask ADINA-IN to assign 282 00:16:41,830 --> 00:16:44,300 equation numbers that correspond to a minimum 283 00:16:44,300 --> 00:16:47,190 bandwidth for the solution of this problem. 284 00:16:47,190 --> 00:16:52,210 So our next step is to have ADINA-IN go through these 285 00:16:52,210 --> 00:16:56,670 actions, and turn back to our laboratory and see what is 286 00:16:56,670 --> 00:16:59,420 happening now. 287 00:16:59,420 --> 00:17:02,700 Here, we see the end of the ADINA-IN input file that we 288 00:17:02,700 --> 00:17:05,530 saw already before. 289 00:17:05,530 --> 00:17:10,109 The command ADINA now generates the ADINA file. 290 00:17:10,109 --> 00:17:12,569 At the same, also, the bandwidth of the stiffness 291 00:17:12,569 --> 00:17:15,430 matrix is minimized. 292 00:17:15,430 --> 00:17:18,619 We use the reverse Cuthill-Mckee algorithm. 293 00:17:18,619 --> 00:17:24,680 Notice that the bandwidth has been reduced from 399 to 93. 294 00:17:24,680 --> 00:17:28,400 The original bandwidth was, of course, artificially large 295 00:17:28,400 --> 00:17:30,740 because our nodal point generation did not take 296 00:17:30,740 --> 00:17:33,900 account of any bandwidth considerations, as I pointed 297 00:17:33,900 --> 00:17:36,570 out before. 298 00:17:36,570 --> 00:17:38,500 Let us briefly look at the ADINA file 299 00:17:38,500 --> 00:17:41,360 generated by the ADINA-IN. 300 00:17:41,360 --> 00:17:44,120 Here, we see common cards, automatically inserted by 301 00:17:44,120 --> 00:17:47,290 ADINA-IN to explain the input cards. 302 00:17:47,290 --> 00:17:50,760 We see the master control card, the load control card, 303 00:17:50,760 --> 00:17:55,580 the Eigenvalue solution control card, and so on. 304 00:17:55,580 --> 00:17:59,230 Let us look a bit closer at the element data cards. 305 00:17:59,230 --> 00:18:05,990 Element 1 has eight nodes and the first three are 6, 64, 74. 306 00:18:05,990 --> 00:18:10,325 Element 2 has 8 nodes and the first three are 64, 62, 76. 307 00:18:14,040 --> 00:18:16,800 Note a maximum of nine nodes is possible. 308 00:18:16,800 --> 00:18:20,370 The last 0 is the node card signifies that the ninth node 309 00:18:20,370 --> 00:18:21,620 is not used. 310 00:18:24,720 --> 00:18:28,070 With a complete ADINA input file now available, we can 311 00:18:28,070 --> 00:18:32,110 call ADINA to execute this file and this gives us our 312 00:18:32,110 --> 00:18:33,900 first solution results. 313 00:18:33,900 --> 00:18:36,590 We look at the solution results and, in particular, we 314 00:18:36,590 --> 00:18:41,390 plot the deformed mesh onto the original mesh, and this 315 00:18:41,390 --> 00:18:45,540 shows, in fact, that we have made an error in the input 316 00:18:45,540 --> 00:18:46,560 description. 317 00:18:46,560 --> 00:18:50,660 It will show us that we have fixed all these nodes down 318 00:18:50,660 --> 00:18:55,190 here, whereas they should have been on a roller. 319 00:18:55,190 --> 00:18:57,940 This is shown by plotting the deformed mesh on to the 320 00:18:57,940 --> 00:19:00,080 original mesh, and it's also shown by 321 00:19:00,080 --> 00:19:02,120 looking at the stresses. 322 00:19:02,120 --> 00:19:07,780 We do so by using an option in the ADINA system for the 323 00:19:07,780 --> 00:19:12,570 stress vector outputs, and this is schematically shown 324 00:19:12,570 --> 00:19:14,500 here, this option. 325 00:19:14,500 --> 00:19:17,510 We plot maximum principle stresses-- 326 00:19:17,510 --> 00:19:19,780 say tensile in this case here-- 327 00:19:19,780 --> 00:19:26,040 as a line with two arrows, and principles stress that's 328 00:19:26,040 --> 00:19:29,920 compressive as simply a line. 329 00:19:29,920 --> 00:19:34,820 So we can see, in other words, how the stress flows through 330 00:19:34,820 --> 00:19:38,280 the material, and we can see, of course, compressive and 331 00:19:38,280 --> 00:19:42,170 tensile stress situations, and notice that the lengths of 332 00:19:42,170 --> 00:19:46,490 these lines corresponds or is proportional to the magnitude 333 00:19:46,490 --> 00:19:48,680 of the stresses. 334 00:19:48,680 --> 00:19:54,030 We can plot this stress vector output for all the integration 335 00:19:54,030 --> 00:19:59,210 points stresses in the mesh, and that, as I said already, 336 00:19:59,210 --> 00:20:01,930 indicates clearly once again, that we have used the wrong 337 00:20:01,930 --> 00:20:04,280 boundary conditions down here. 338 00:20:04,280 --> 00:20:08,350 So we go and correct the boundary conditions down here, 339 00:20:08,350 --> 00:20:10,900 and re-run the analysis. 340 00:20:10,900 --> 00:20:15,520 In other words, call ADINA again and those results that 341 00:20:15,520 --> 00:20:19,610 we obtained then, once again, displacements, in other words, 342 00:20:19,610 --> 00:20:22,750 are plotted by plotting the deformed mesh onto the 343 00:20:22,750 --> 00:20:24,120 original mesh. 344 00:20:24,120 --> 00:20:26,350 We see that we now got much better, much more 345 00:20:26,350 --> 00:20:28,110 realistically-looking results. 346 00:20:28,110 --> 00:20:32,850 And we also will look at the stresses using the stress 347 00:20:32,850 --> 00:20:38,730 vector plots again, in the elements, that show us also 348 00:20:38,730 --> 00:20:42,340 that the results are now quite realistic and that our mesh, 349 00:20:42,340 --> 00:20:45,050 including the boundary conditions have been quite 350 00:20:45,050 --> 00:20:46,860 properly defined. 351 00:20:46,860 --> 00:20:52,080 So let us now look at this step of the analysis. 352 00:20:52,080 --> 00:20:54,420 The command runadina calls ADINA to 353 00:20:54,420 --> 00:20:57,450 execute the input data. 354 00:20:57,450 --> 00:20:59,770 The data input file is in ADINA-IN F02. 355 00:21:04,890 --> 00:21:07,680 And here, we see now the deformed plotted onto the 356 00:21:07,680 --> 00:21:08,890 original mesh. 357 00:21:08,890 --> 00:21:11,690 The original mesh is plotted in dash lines. 358 00:21:11,690 --> 00:21:13,395 Of course, the deformations are magnified. 359 00:21:16,190 --> 00:21:19,570 Note that as expected, the top face has uniformly moved up. 360 00:21:26,080 --> 00:21:28,630 However, note that the nodal points on the horizontal 361 00:21:28,630 --> 00:21:31,580 symmetry line have not displaced at all. 362 00:21:31,580 --> 00:21:34,420 This is quite unphysical and shows that the wrong boundary 363 00:21:34,420 --> 00:21:37,380 conditions have been used. 364 00:21:37,380 --> 00:21:40,220 If we look at the stress vector plot over the mesh, the 365 00:21:40,220 --> 00:21:42,200 same conclusion is reached. 366 00:21:42,200 --> 00:21:44,680 For clarity, on the video, we show here the stress vectors 367 00:21:44,680 --> 00:21:48,940 just on the elements closest to the hole. 368 00:21:48,940 --> 00:21:51,670 And we can see in the element adjoining the horizontal 369 00:21:51,670 --> 00:21:56,010 symmetry line, a stress that acts normal to the whole. 370 00:21:56,010 --> 00:21:59,160 This is, of course, unphysical. 371 00:21:59,160 --> 00:22:01,330 Next, we show the stress vectors in the outer most 372 00:22:01,330 --> 00:22:03,090 elements of the quarter plate. 373 00:22:03,090 --> 00:22:06,420 And you can see here, a stress acting perpendicular to the 374 00:22:06,420 --> 00:22:09,360 free edge of the plate, when we look near the horizontal 375 00:22:09,360 --> 00:22:11,530 symmetry line. 376 00:22:11,530 --> 00:22:14,610 This is also unphysical and is due to having specified the 377 00:22:14,610 --> 00:22:16,050 wrong boundary conditions on the wrong 378 00:22:16,050 --> 00:22:17,300 horizontal symmetry line. 379 00:22:20,910 --> 00:22:22,450 The specification of the boundary 380 00:22:22,450 --> 00:22:24,520 conditions is shown here. 381 00:22:24,520 --> 00:22:26,860 The character, C, denotes the boundary condition on the 382 00:22:26,860 --> 00:22:28,150 horizontal symmetry line. 383 00:22:32,930 --> 00:22:35,280 The character B denotes the boundary condition on the 384 00:22:35,280 --> 00:22:37,410 vertical symmetry line. 385 00:22:37,410 --> 00:22:40,780 Where B means only the z displacement is free and C 386 00:22:40,780 --> 00:22:43,810 means all displacements are fixed. 387 00:22:43,810 --> 00:22:45,610 For the six possible displacements and 388 00:22:45,610 --> 00:22:46,370 [? flotatations, ?] 389 00:22:46,370 --> 00:22:49,620 a 1 means the degree of freedom is fixed, and 0 means 390 00:22:49,620 --> 00:22:50,870 the degree of freedom is free. 391 00:22:54,610 --> 00:22:56,170 We now correct the boundary conditions. 392 00:22:59,320 --> 00:23:02,380 And B on the horizontal symmetry line means now the v 393 00:23:02,380 --> 00:23:05,620 displacement is free. 394 00:23:05,620 --> 00:23:08,520 C on the vertical symmetry line means now the w 395 00:23:08,520 --> 00:23:09,770 displacement is free. 396 00:23:13,810 --> 00:23:16,480 We run ADINA again, and here you see the deformed mesh 397 00:23:16,480 --> 00:23:19,270 plotted on the original mesh. 398 00:23:19,270 --> 00:23:22,820 The deformations look very reasonable. 399 00:23:22,820 --> 00:23:25,750 The plate has contracted horizontally, and 400 00:23:25,750 --> 00:23:27,990 correspondingly, the hole has shrunk horizontally. 401 00:23:33,260 --> 00:23:35,830 The deformations closest to the hole are shown here. 402 00:23:38,840 --> 00:23:40,350 And here, we see the stress vector 403 00:23:40,350 --> 00:23:42,310 plots for these elements. 404 00:23:42,310 --> 00:23:45,110 The stresses align nicely with the hole. 405 00:23:45,110 --> 00:23:47,680 Notice that there is no stress perpendicular to the free 406 00:23:47,680 --> 00:23:50,640 surface of the hole when we look at the integration point 407 00:23:50,640 --> 00:23:51,910 layer closest as a hole. 408 00:23:54,460 --> 00:23:56,790 The value of the maximum stress is given here. 409 00:23:56,790 --> 00:24:01,040 It is 301.9 megapascal. 410 00:24:01,040 --> 00:24:03,170 Here, we look at the element which carries the largest 411 00:24:03,170 --> 00:24:06,600 stress, element 57. 412 00:24:06,600 --> 00:24:08,870 Once again, we can see that the stresses align 413 00:24:08,870 --> 00:24:11,940 nicely with the hole. 414 00:24:11,940 --> 00:24:15,610 We now recall is that the objective of our analysis is 415 00:24:15,610 --> 00:24:18,920 really the calculation of the stress concentration factor. 416 00:24:18,920 --> 00:24:21,930 And if we look at the problem once more, here, we have the 417 00:24:21,930 --> 00:24:23,990 plate with the hole. 418 00:24:23,990 --> 00:24:28,050 The plate subjected to the tractions, as shown here. 419 00:24:28,050 --> 00:24:30,550 We now need to, of course, predict the stresses 420 00:24:30,550 --> 00:24:33,770 accurately around the hole, and in particular, at this 421 00:24:33,770 --> 00:24:35,290 point here. 422 00:24:35,290 --> 00:24:37,170 Here, we have our finite element 423 00:24:37,170 --> 00:24:39,690 method used in the analysis. 424 00:24:39,690 --> 00:24:42,370 And so far, the only calculated stresses at the 425 00:24:42,370 --> 00:24:45,720 integration points in the elements. 426 00:24:45,720 --> 00:24:49,040 Now this is here, by the way, element number 57. 427 00:24:49,040 --> 00:24:53,210 And for this element, we have calculated so far, only the 428 00:24:53,210 --> 00:24:56,150 stresses at these integration points. 429 00:24:56,150 --> 00:24:59,470 However, these integration points do not lie on the 430 00:24:59,470 --> 00:25:03,200 circumference of the hole, on the boundary of the hole. 431 00:25:03,200 --> 00:25:06,350 And that is where the maximum stresses occur. 432 00:25:06,350 --> 00:25:10,380 Of particular interest is, of course, also this point here, 433 00:25:10,380 --> 00:25:12,880 where we anticipate to obtain the maximum 434 00:25:12,880 --> 00:25:14,910 stress in the analysis. 435 00:25:14,910 --> 00:25:18,970 If you look at, schematically, how the stresses would vary, 436 00:25:18,970 --> 00:25:24,090 say, through the element, to the boundary of the hole, we 437 00:25:24,090 --> 00:25:27,470 would see a schematic plot as shown here. 438 00:25:27,470 --> 00:25:30,900 Here is an actual element, the other elements lie next to it, 439 00:25:30,900 --> 00:25:33,480 and here you can see schematically shown the stress 440 00:25:33,480 --> 00:25:36,960 computed at the closest integration point to the 441 00:25:36,960 --> 00:25:38,530 boundary of the hole. 442 00:25:38,530 --> 00:25:40,790 And here, we would have the stress computed 443 00:25:40,790 --> 00:25:42,140 at the nodal point. 444 00:25:42,140 --> 00:25:45,580 That is actually the stress that we are interested in. 445 00:25:45,580 --> 00:25:49,660 Well, we can ask ADINA to calculate the stresses at the 446 00:25:49,660 --> 00:25:55,260 nodal points, and then we can ask ADINA-PLOT to enter with 447 00:25:55,260 --> 00:25:59,640 these nodal point stresses into this formula here. 448 00:25:59,640 --> 00:26:04,940 Sigma yy, sigma zz, and sigma yz are the stresses at the 449 00:26:04,940 --> 00:26:06,900 nodal points. 450 00:26:06,900 --> 00:26:12,170 To calculate, ADINA-PLOT calculate this Sigma 1, which 451 00:26:12,170 --> 00:26:16,300 is the maximum principle of stress at that nodal point. 452 00:26:16,300 --> 00:26:19,770 We can ask ADINA-PLOT to calculate sigma 1 at all the 453 00:26:19,770 --> 00:26:26,160 nodal points in the mesh, and by doing so, we obtained these 454 00:26:26,160 --> 00:26:29,270 stresses and then they can ask ADINA-PLOT to search through 455 00:26:29,270 --> 00:26:32,490 those nodal points stresses, these sigma 1 stresses, to 456 00:26:32,490 --> 00:26:37,770 find us the location, the element and the nodal point, 457 00:26:37,770 --> 00:26:41,200 to have the physical location of the maximum stress 458 00:26:41,200 --> 00:26:42,525 occurring in the mesh. 459 00:26:42,525 --> 00:26:49,950 We will see that doing so, ADINA-PLOT comes up to tell us 460 00:26:49,950 --> 00:26:55,640 that this is the point, element number 57, point 461 00:26:55,640 --> 00:26:58,990 number 4, that is this physical point here, where the 462 00:26:58,990 --> 00:27:02,320 maximum stress occurs and will also give us that maximum 463 00:27:02,320 --> 00:27:04,720 stress, and that maximum stress, of course, gives us 464 00:27:04,720 --> 00:27:07,450 then the stress concentration factor. 465 00:27:07,450 --> 00:27:13,500 So let us now look at this phase of the analysis. 466 00:27:13,500 --> 00:27:15,830 Here, we have input some information regarding 467 00:27:15,830 --> 00:27:18,910 variables that need be defined in ADINA plot. 468 00:27:18,910 --> 00:27:25,220 TYY refers to tau yy, TZZ refers to tau zz, TYZ 469 00:27:25,220 --> 00:27:28,120 refers to tau yz. 470 00:27:28,120 --> 00:27:30,430 We define the result and variable to calculate the 471 00:27:30,430 --> 00:27:34,350 maximum principle stress. 472 00:27:34,350 --> 00:27:40,010 Hence, when TYY, TZZ, and TYZ are defined [? smax ?] 473 00:27:40,010 --> 00:27:41,880 gives the maximum principle stress. 474 00:27:46,640 --> 00:27:49,700 Here, we now enter the command to look for the maximum 475 00:27:49,700 --> 00:27:51,140 principal stress in the mesh. 476 00:27:57,280 --> 00:28:01,270 First we make a small input error, obtain a message, we 477 00:28:01,270 --> 00:28:13,350 correct the input, and here comes the result. 478 00:28:13,350 --> 00:28:17,510 We see that indeed element 57.4 carries a maximum 479 00:28:17,510 --> 00:28:25,260 principle stress and this value is 345.151 megapascal. 480 00:28:25,260 --> 00:28:27,840 We have now actually obtained an answer to the 481 00:28:27,840 --> 00:28:29,760 question that we asked. 482 00:28:29,760 --> 00:28:31,900 Originally, namely, we wanted to calculated the stress 483 00:28:31,900 --> 00:28:34,670 concentration factor around the hole. 484 00:28:34,670 --> 00:28:37,040 And we have obtained a number for that stress 485 00:28:37,040 --> 00:28:38,880 concentration factor. 486 00:28:38,880 --> 00:28:42,630 However, a valid question, certainly is to ask, how good 487 00:28:42,630 --> 00:28:43,480 is this number? 488 00:28:43,480 --> 00:28:47,710 After all, we used a finite element mesh to approximate 489 00:28:47,710 --> 00:28:50,910 the plate a particular finite element idealization was used, 490 00:28:50,910 --> 00:28:54,230 and we have only obtained an approximation 491 00:28:54,230 --> 00:28:57,310 to the exact result. 492 00:28:57,310 --> 00:29:01,070 Well, to evaluate that question, to obtain insight 493 00:29:01,070 --> 00:29:05,140 into that question, to evaluate how good our analysis 494 00:29:05,140 --> 00:29:10,970 results really are, we can plot stress jumps, the way we 495 00:29:10,970 --> 00:29:13,130 discussed it in an earlier lecture. 496 00:29:13,130 --> 00:29:17,370 And in particular, for the analysis that I'd like to show 497 00:29:17,370 --> 00:29:21,660 you in this final phase, we have plotted stress jumps 498 00:29:21,660 --> 00:29:25,390 along these two lines. 499 00:29:25,390 --> 00:29:28,570 Now, notice that, for example, at this node here, we have 500 00:29:28,570 --> 00:29:32,940 four elements coupling into this node, so at this node we 501 00:29:32,940 --> 00:29:36,760 get four different stress predictions 502 00:29:36,760 --> 00:29:39,450 for each stress component. 503 00:29:39,450 --> 00:29:43,760 At this node here, we would have only two stress 504 00:29:43,760 --> 00:29:46,900 predictions, for each stress component because only two 505 00:29:46,900 --> 00:29:49,960 elements couple into this node. 506 00:29:49,960 --> 00:29:55,430 That is one way to evaluate or to look at how accurate our 507 00:29:55,430 --> 00:29:56,680 results are. 508 00:29:58,890 --> 00:30:02,830 An alternative way is to plot pressure bands, and the 509 00:30:02,830 --> 00:30:05,270 pressure here is scalar. 510 00:30:05,270 --> 00:30:09,410 It's computed as shown here, and we can plot bands of 511 00:30:09,410 --> 00:30:12,150 constant pressure, the way we already have discussed it in 512 00:30:12,150 --> 00:30:13,240 an earlier lecture. 513 00:30:13,240 --> 00:30:17,880 Notice because this is a scalar, it can be used very 514 00:30:17,880 --> 00:30:21,910 nicely to plot these bands of constant pressure. 515 00:30:21,910 --> 00:30:24,170 Of course, we could also have used here, say, an effective 516 00:30:24,170 --> 00:30:29,810 stress, which is also a scalar, and we could plot 517 00:30:29,810 --> 00:30:33,440 bands of constant effective stresses. 518 00:30:33,440 --> 00:30:38,560 One example that you've seen already early, is this one 519 00:30:38,560 --> 00:30:42,960 here where we plotted pressure bands, with band magnitude of 520 00:30:42,960 --> 00:30:48,435 5 MPa, megapascal, and you can see here this white band, here 521 00:30:48,435 --> 00:30:52,580 a black band, in other words, we're going in steps 5 MPa 522 00:30:52,580 --> 00:30:55,390 from one band to the next. 523 00:30:55,390 --> 00:30:59,970 Notice that there's a pressure band discontinuity right here, 524 00:30:59,970 --> 00:31:03,710 which already indicates that we have a stress discontinuity 525 00:31:03,710 --> 00:31:06,800 here, and which indicates that the mesh that we used is 526 00:31:06,800 --> 00:31:10,180 really not a very fine mesh. 527 00:31:10,180 --> 00:31:13,450 And if we are interested in obtaining a very accurate 528 00:31:13,450 --> 00:31:18,250 result, then based on these pressure band plots, and also 529 00:31:18,250 --> 00:31:21,750 the stress jump plots that I will show you just now, we may 530 00:31:21,750 --> 00:31:23,980 actually decide to use a finer mesh. 531 00:31:23,980 --> 00:31:27,360 We discussed this issue already in an earlier lecture. 532 00:31:27,360 --> 00:31:32,400 So let us now then look at what happens, or what happened 533 00:31:32,400 --> 00:31:35,420 in this final phase of the analysis. 534 00:31:35,420 --> 00:31:38,140 Let's go back to the laboratory and share the 535 00:31:38,140 --> 00:31:40,175 experiences that we'll see there. 536 00:31:42,840 --> 00:31:44,490 Here, we see once more the mesh we're 537 00:31:44,490 --> 00:31:45,740 using in the analysis. 538 00:31:48,090 --> 00:31:51,230 We will plot the stresses, and hence, we can see the stress 539 00:31:51,230 --> 00:31:54,930 jumps along the horizontal symmetry line, and the 540 00:31:54,930 --> 00:31:56,350 diagonal line of the plate. 541 00:32:04,100 --> 00:32:06,670 Here, you see the stresses along the horizontal symmetry 542 00:32:06,670 --> 00:32:08,660 line, Tau zz is plotted. 543 00:32:12,760 --> 00:32:15,110 The horizontal axis measures distance along 544 00:32:15,110 --> 00:32:16,360 the symmetry line. 545 00:32:20,430 --> 00:32:22,955 And the vertical axis measures the stress values. 546 00:32:31,810 --> 00:32:34,200 Note that the stress predictions at the nodes, when 547 00:32:34,200 --> 00:32:38,590 calculated for the different elements are almost the same. 548 00:32:38,590 --> 00:32:42,000 Only at one node can we actually see a difference, and 549 00:32:42,000 --> 00:32:44,600 it is quite small. 550 00:32:44,600 --> 00:32:48,990 Note that two elements couple into this node. 551 00:32:48,990 --> 00:32:51,750 Hence, there are only small stress jumps along the 552 00:32:51,750 --> 00:32:54,010 horizontal symmetry axis of the plate. 553 00:32:56,790 --> 00:32:59,450 Next, we look at the stress plot along the diagonal line 554 00:32:59,450 --> 00:33:01,200 of the model. 555 00:33:01,200 --> 00:33:04,440 Here the maximum principle stress is plotted. 556 00:33:04,440 --> 00:33:07,850 Note that at one node into which four elements couple, we 557 00:33:07,850 --> 00:33:11,690 have four markedly different stress values. 558 00:33:11,690 --> 00:33:15,040 Indeed, we have significant stress jumps at that node, but 559 00:33:15,040 --> 00:33:16,530 otherwise the stress predictions do 560 00:33:16,530 --> 00:33:17,780 not show large jumps. 561 00:33:25,220 --> 00:33:29,240 Finally, we look at the pressure band plots. 562 00:33:29,240 --> 00:33:31,710 Here, they are drawn. 563 00:33:31,710 --> 00:33:34,550 To save time, we skipped some of the drawing process and 564 00:33:34,550 --> 00:33:36,430 jumped to a later picture here. 565 00:33:46,570 --> 00:33:51,260 We notice that the pressure bands are quite continuous, 566 00:33:51,260 --> 00:33:54,150 except between the first and second layer of elements 567 00:33:54,150 --> 00:33:55,370 around the hole. 568 00:33:55,370 --> 00:33:58,190 This corresponds to the stress discontinuity between these 569 00:33:58,190 --> 00:34:00,110 element layers that we saw earlier. 570 00:34:02,840 --> 00:34:05,480 We see now this is now completed, I'd like to look 571 00:34:05,480 --> 00:34:09,070 with you once more back on to two view graphs that we 572 00:34:09,070 --> 00:34:13,370 already have looked at earlier. 573 00:34:13,370 --> 00:34:15,800 On this you graph, we summarize some important 574 00:34:15,800 --> 00:34:16,840 observations. 575 00:34:16,840 --> 00:34:19,590 And we said that it is very important to check the finite 576 00:34:19,590 --> 00:34:23,540 element data input carefully prior to the actual response 577 00:34:23,540 --> 00:34:24,580 solution run. 578 00:34:24,580 --> 00:34:27,940 That, of course, means plotting the data. 579 00:34:27,940 --> 00:34:30,500 And we have done so, of course, in our analysis. 580 00:34:30,500 --> 00:34:33,960 And after the response solution has been obtained, by 581 00:34:33,960 --> 00:34:36,360 starting whether desired boundary conditions are 582 00:34:36,360 --> 00:34:39,110 satisfied, whether displacement and stress 583 00:34:39,110 --> 00:34:41,820 solution is reasonable. 584 00:34:41,820 --> 00:34:45,429 Remember, in our analysis, we did this, of course, as well 585 00:34:45,429 --> 00:34:50,900 and we found, by looking at the boundary conditions, the 586 00:34:50,900 --> 00:34:54,610 way they were represented in the actual solution, that we 587 00:34:54,610 --> 00:34:57,230 have actually made an error. 588 00:34:57,230 --> 00:35:00,570 In other words, we looked at the deformed mesh, and the 589 00:35:00,570 --> 00:35:03,060 boundary conditions on the deformed mesh in our first 590 00:35:03,060 --> 00:35:07,030 analysis showed that we had fixed the boundary at the 591 00:35:07,030 --> 00:35:10,190 bottom off the mesh, which was an error. 592 00:35:10,190 --> 00:35:14,720 So it is very important to go through this step, to look 593 00:35:14,720 --> 00:35:16,820 very closely whether the boundary conditions are 594 00:35:16,820 --> 00:35:21,550 actually satisfied on the mesh that you have been using, in 595 00:35:21,550 --> 00:35:22,640 the right way. 596 00:35:22,640 --> 00:35:27,930 Of course, the same holds for the stress and solution. 597 00:35:27,930 --> 00:35:31,230 Remember, that we looked at the stress plots for the mesh 598 00:35:31,230 --> 00:35:34,540 that was fixed at the bottom and we could directly see 599 00:35:34,540 --> 00:35:38,050 there were errors there, and, in other words, the error of 600 00:35:38,050 --> 00:35:42,860 having fixed the boundary at the bottom of the plate. 601 00:35:42,860 --> 00:35:46,080 So this step is most important, and we have seen an 602 00:35:46,080 --> 00:35:50,450 example in the analysis that we just completed. 603 00:35:50,450 --> 00:35:54,520 I also had this view graph already on, where we said that 604 00:35:54,520 --> 00:35:56,690 we want to carefully evaluate and interpret 605 00:35:56,690 --> 00:35:58,580 the calculated response. 606 00:35:58,580 --> 00:36:01,580 We want to study, in detail, the calculated displacement 607 00:36:01,580 --> 00:36:04,630 and stresses along certain lines, study stress jumps. 608 00:36:04,630 --> 00:36:08,660 Well, we saw an example of that in the analysis that we 609 00:36:08,660 --> 00:36:13,310 just completed, and we also pointed out that it is 610 00:36:13,310 --> 00:36:16,760 important to go through this step here first, prior to 611 00:36:16,760 --> 00:36:20,280 using a stress averaging because if you do average 612 00:36:20,280 --> 00:36:23,700 stresses, of course, you would never see stress jumps. 613 00:36:23,700 --> 00:36:27,210 And this can be an important step to gain confidence in the 614 00:36:27,210 --> 00:36:30,210 analysis results that you have obtained. 615 00:36:30,210 --> 00:36:32,970 This then completes what I wanted to share with you in 616 00:36:32,970 --> 00:36:33,710 this lecture. 617 00:36:33,710 --> 00:36:35,080 Thank you very much for your attention.