WEBVTT 00:00:00.040 --> 00:00:02.470 The following content is provided under a Creative 00:00:02.470 --> 00:00:03.880 Commons license. 00:00:03.880 --> 00:00:06.920 Your support will help MIT OpenCourseWare continue to 00:00:06.920 --> 00:00:10.950 offer high quality educational resources for free to make a 00:00:10.950 --> 00:00:14.430 donation or view additional materials from hundreds of MIT 00:00:14.430 --> 00:00:17.872 courses, visit MIT OpenCourseWare at ocw.mit.edu. 00:00:21.296 --> 00:00:23.370 PROFESSOR: Ladies and gentlemen, welcome to this 00:00:23.370 --> 00:00:26.235 lecture on non-linear finite element analysis of solids and 00:00:26.235 --> 00:00:27.890 structures. 00:00:27.890 --> 00:00:30.770 In the previous lectures, we have considered quite a bit of 00:00:30.770 --> 00:00:33.510 theory related to non-linear finite element analysis in 00:00:33.510 --> 00:00:35.860 some example solutions. 00:00:35.860 --> 00:00:38.700 The objective in the next two lectures now, the last 00:00:38.700 --> 00:00:42.170 lectures of this video course, is to show how an actual 00:00:42.170 --> 00:00:46.030 finite element analysis is performed on the computer. 00:00:46.030 --> 00:00:49.760 We start with a linear solution in this lecture, and 00:00:49.760 --> 00:00:53.820 then consider a non-linear solution in the next lecture. 00:00:53.820 --> 00:00:58.930 We cannot discuss really, in this amount of time given, all 00:00:58.930 --> 00:01:02.520 the aspects of the analysis, but want to summarize and 00:01:02.520 --> 00:01:06.050 demonstrate on the computer the major steps of the 00:01:06.050 --> 00:01:09.840 analysis and concentrate on possible difficulties, 00:01:09.840 --> 00:01:15.200 possible pitfalls, and some general recommendations. 00:01:15.200 --> 00:01:18.460 As the example problem, we want to use the plate with a 00:01:18.460 --> 00:01:21.350 hole, that we already considered earlier. 00:01:21.350 --> 00:01:24.200 And we performed a linear analysis and then 00:01:24.200 --> 00:01:25.750 a non-linear analysis. 00:01:25.750 --> 00:01:28.530 Remember, I pointed out in the previous lectures that it is 00:01:28.530 --> 00:01:31.830 very important to always do linear analysis first before 00:01:31.830 --> 00:01:34.700 you go into a non-linear analysis. 00:01:34.700 --> 00:01:37.880 The elastic analysis is performed to obtain the stress 00:01:37.880 --> 00:01:41.440 concentration factor at the hole, then we do an 00:01:41.440 --> 00:01:46.020 elasto-plastic analysis to estimate the limit load, and 00:01:46.020 --> 00:01:49.820 an analysis also to investigate the effect of a 00:01:49.820 --> 00:01:51.440 shaft in the plate hole. 00:01:51.440 --> 00:01:55.070 These two analyses are being performed in the last lecture 00:01:55.070 --> 00:01:57.280 of the video course. 00:01:57.280 --> 00:02:01.430 The plate we are analyzing is shown on this view graph here. 00:02:01.430 --> 00:02:03.610 Notice it's a square plate. 00:02:03.610 --> 00:02:07.750 Here, we show the hole, the plate is loaded as shown up 00:02:07.750 --> 00:02:10.050 here, and down here. 00:02:10.050 --> 00:02:12.670 The material property for the elastic analysis are given 00:02:12.670 --> 00:02:17.130 here and the thickness of the plate is 0.01 meter. 00:02:17.130 --> 00:02:19.930 Because of symmetry conditions, we only need to 00:02:19.930 --> 00:02:22.710 consider this quarter here. 00:02:22.710 --> 00:02:25.370 Of course, using appropriate boundary conditions along 00:02:25.370 --> 00:02:29.880 these two lines. we will talk about that more later on. 00:02:29.880 --> 00:02:33.880 The first step for a finite element analysis is to select 00:02:33.880 --> 00:02:37.710 a computer program, and we, of course, use the ADINA system. 00:02:37.710 --> 00:02:42.430 ADINA-IN is the pre-processor to prepare, generate the 00:02:42.430 --> 00:02:43.810 finite element data. 00:02:43.810 --> 00:02:47.250 ADINA then solves the actual finite element model, and 00:02:47.250 --> 00:02:50.040 ADINA-PLOT is used to this display numerically or 00:02:50.040 --> 00:02:52.470 graphically the solution results. 00:02:52.470 --> 00:02:56.320 Schematically, we are sitting here at a terminal and we're 00:02:56.320 --> 00:02:59.170 inputting the data to ADINA-IN. 00:02:59.170 --> 00:03:03.220 We can also receive here, numerical output, and we can 00:03:03.220 --> 00:03:07.380 also plot on this terminal here, any of the information 00:03:07.380 --> 00:03:08.550 that we like to plot. 00:03:08.550 --> 00:03:10.200 This is a graphics terminal. 00:03:10.200 --> 00:03:13.190 Notice ADINA-IN, of course, communicates to a storage 00:03:13.190 --> 00:03:17.030 device and further on to ADINA, as we will 00:03:17.030 --> 00:03:19.650 discuss just now. 00:03:19.650 --> 00:03:22.630 The user inputs, in other words, or 00:03:22.630 --> 00:03:24.400 types into the terminal. 00:03:24.400 --> 00:03:27.690 ADINA-IN commands interactively or for batch 00:03:27.690 --> 00:03:31.670 processing and then the user checks also the input and the 00:03:31.670 --> 00:03:35.420 generated data on the graphics device, as I showed you on the 00:03:35.420 --> 00:03:38.020 previous view graph. 00:03:38.020 --> 00:03:43.750 ADINA-IN generates the input data for ADINA. 00:03:43.750 --> 00:03:46.965 The input data is checked internally in ADINA in for 00:03:46.965 --> 00:03:51.430 errors and inconsistency, and also is displayed as you are 00:03:51.430 --> 00:03:53.330 requesting it as a user. 00:03:53.330 --> 00:03:59.850 The degree of freedom numbers are generated and to obtain 00:03:59.850 --> 00:04:05.560 minimum bandwidth, we have a minimum bandwidth minimization 00:04:05.560 --> 00:04:09.020 algorithm in the program, as I will point out a bit 00:04:09.020 --> 00:04:12.480 stronger later on. 00:04:12.480 --> 00:04:18.459 ADINA data inputs then, is available to ADINA, and the 00:04:18.459 --> 00:04:24.350 user runs ADINA, and ADINA then stores the output data on 00:04:24.350 --> 00:04:29.600 a porthole file and on an output file. 00:04:29.600 --> 00:04:33.130 The output file, in other words, contains really the 00:04:33.130 --> 00:04:36.640 ADINA model data and the calculated results. 00:04:36.640 --> 00:04:41.740 We access ADINA porthole file using ADINA-PLOT. 00:04:41.740 --> 00:04:45.870 We can, of course, also look at the output file and see 00:04:45.870 --> 00:04:49.610 numerically the data that was calculated using ADINA. 00:04:52.610 --> 00:04:57.100 Here, we have the action displayed or schematically 00:04:57.100 --> 00:04:59.200 shown by the user. 00:04:59.200 --> 00:05:04.830 User uses ADINA-PLOT to fetch data from the ADINA porthole 00:05:04.830 --> 00:05:09.430 file and then ADINA-PLOT displays those data either 00:05:09.430 --> 00:05:12.220 numerically or graphically. 00:05:12.220 --> 00:05:17.480 Let's look very briefly at an overview of ADINA. 00:05:17.480 --> 00:05:20.610 The program can be used for static and dynamic solutions, 00:05:20.610 --> 00:05:24.250 for linear and non-linear analysis, for small and very 00:05:24.250 --> 00:05:28.030 large finite element models, and the formulations finite 00:05:28.030 --> 00:05:31.400 elements and numerical procedures used in the program 00:05:31.400 --> 00:05:35.640 have largely been discussed in this course. 00:05:35.640 --> 00:05:39.710 The displacement assumptions that can be employed for the 00:05:39.710 --> 00:05:43.340 finite element models are either infinitesimally small 00:05:43.340 --> 00:05:46.150 displacements, large displacements, large rotations 00:05:46.150 --> 00:05:50.480 but small strains, and large deformations, large strains. 00:05:50.480 --> 00:05:53.750 We discussed these assumptions, of course, also 00:05:53.750 --> 00:05:55.310 in the course. 00:05:55.310 --> 00:05:59.240 Material models that are available in isotropic linear 00:05:59.240 --> 00:06:02.110 elastic model, orthotropic linear elastic model, 00:06:02.110 --> 00:06:05.350 isotropic thermo-elastic model, a curve description 00:06:05.350 --> 00:06:08.300 model for analysis of geological materials, a 00:06:08.300 --> 00:06:14.000 concrete model, isothermal plasticity models, 00:06:14.000 --> 00:06:17.300 thermo-elastic-plastic and creep models, and non-linear 00:06:17.300 --> 00:06:22.430 elastic incompressible, and user-supplied models. 00:06:25.040 --> 00:06:29.540 The elements available in the program, is available number 00:06:29.540 --> 00:06:32.650 nodes tress element, an element that can have two 00:06:32.650 --> 00:06:35.780 nodes, three nodes, or four nodes. 00:06:35.780 --> 00:06:39.461 It can also be used as a ring element. 00:06:39.461 --> 00:06:42.990 A two-dimensional solid element that is used for plane 00:06:42.990 --> 00:06:46.840 stress axis symmetric and plane strain analysis. 00:06:46.840 --> 00:06:50.510 This also can have available number of nodes, from four 00:06:50.510 --> 00:06:54.300 nodes to nine nodes. 00:06:54.300 --> 00:06:56.800 Similarly, available number of nodes element for 00:06:56.800 --> 00:06:58.190 three-dimensional analysis. 00:07:01.980 --> 00:07:06.890 Then also a beam element, a 2-node beam element, Hermitian 00:07:06.890 --> 00:07:09.890 beam element. 00:07:09.890 --> 00:07:13.830 And the isoparametric beam element that we talked about 00:07:13.830 --> 00:07:14.920 in the course. 00:07:14.920 --> 00:07:20.020 This element can carry, or can be used with two nodes, or 00:07:20.020 --> 00:07:24.200 three nodes, or four nodes. 00:07:24.200 --> 00:07:28.260 A pipe element that we did not discuss in the course, but you 00:07:28.260 --> 00:07:31.950 might be interested in reading about that element is a curved 00:07:31.950 --> 00:07:36.390 beam element, of course, of pipe section. 00:07:36.390 --> 00:07:41.250 Which however, also includes the effects of ovalization So 00:07:41.250 --> 00:07:45.000 this element also carries, if desired ovalization degrees of 00:07:45.000 --> 00:07:47.740 freedoms at the nodes. 00:07:47.740 --> 00:07:52.140 And shell elements, we talked about the use of the 16-node 00:07:52.140 --> 00:07:57.420 element, and the MITC 4, the 4-node element. 00:07:57.420 --> 00:08:00.850 We also talked briefly about transition elements that I 00:08:00.850 --> 00:08:04.470 used to model shells, or thin structures 00:08:04.470 --> 00:08:08.330 that couple into solids. 00:08:08.330 --> 00:08:10.580 Let us summarize some important observations 00:08:10.580 --> 00:08:13.500 regarding finite element analysis. 00:08:13.500 --> 00:08:16.210 It's important to check the finite element data, of 00:08:16.210 --> 00:08:18.820 course, very carefully. 00:08:18.820 --> 00:08:20.310 The data must be checked prior to the 00:08:20.310 --> 00:08:21.730 actual response solution. 00:08:21.730 --> 00:08:25.410 This is done, of course, with the pre-processor, by plotting 00:08:25.410 --> 00:08:29.380 the data, looking at it very carefully, typically. 00:08:29.380 --> 00:08:33.330 And then after the response solution, you still want to 00:08:33.330 --> 00:08:39.200 check the input data once more by seeing whether the boundary 00:08:39.200 --> 00:08:42.350 conditions are properly satisfied, that you want to 00:08:42.350 --> 00:08:44.800 impose on to the model, whether the displacement and 00:08:44.800 --> 00:08:46.050 stress solution is a reasonable. 00:08:49.000 --> 00:08:51.970 Once the analysis has been performed, you want to very 00:08:51.970 --> 00:08:53.640 carefully evaluate and interpret 00:08:53.640 --> 00:08:55.390 the calculate response. 00:08:55.390 --> 00:08:58.130 You want to start in detail the calculated displacement 00:08:58.130 --> 00:09:00.360 and stresses along certain lines. 00:09:00.360 --> 00:09:02.960 In particular, look at stress jumps. 00:09:02.960 --> 00:09:06.120 We pointed that out already in an earlier lecture, and we 00:09:06.120 --> 00:09:10.200 will do so in our example solution again, just now. 00:09:10.200 --> 00:09:14.180 And here, I'd like to add that stress averaging, stress 00:09:14.180 --> 00:09:17.300 smoothing should only be done after the above careful 00:09:17.300 --> 00:09:18.230 evaluation. 00:09:18.230 --> 00:09:22.260 That's something important to keep in mind. 00:09:22.260 --> 00:09:25.790 I believe that you should first look at the stresses, 00:09:25.790 --> 00:09:29.310 the way they have been calculated by the program and 00:09:29.310 --> 00:09:32.020 then start thinking about stress smoothing. 00:09:32.020 --> 00:09:36.630 Only after you've gone through this phase here. 00:09:36.630 --> 00:09:42.410 The data for the construction of the finite element mesh, 00:09:42.410 --> 00:09:51.150 that we want to deal with in the example solution is input 00:09:51.150 --> 00:09:54.180 for this quarter of the plate, as I 00:09:54.180 --> 00:09:55.630 pointed out earlier already. 00:09:55.630 --> 00:10:00.180 We have these elastic material constants, we're looking at a 00:10:00.180 --> 00:10:01.590 plane stress analysis. 00:10:01.590 --> 00:10:03.510 This is the thickness of the plate. 00:10:03.510 --> 00:10:05.800 And once again, here is a loading. 00:10:05.800 --> 00:10:08.770 Notice, we are putting this boundary on rollers, and we 00:10:08.770 --> 00:10:12.720 want to put this boundary as well on rollers to model the 00:10:12.720 --> 00:10:16.640 symmetry conditions that we need to model in order to 00:10:16.640 --> 00:10:19.990 consider a whole plate, where we actually analyze here, only 00:10:19.990 --> 00:10:22.230 one quarter of that plate. 00:10:22.230 --> 00:10:24.770 The finite element mesh that we will be using is shown on 00:10:24.770 --> 00:10:25.550 this view graph. 00:10:25.550 --> 00:10:31.120 It consists of 64 8-node isoparametric elements. 00:10:31.120 --> 00:10:34.820 Well, we performed this analysis on the computer in my 00:10:34.820 --> 00:10:38.832 laboratory at MIT a few weeks ago, and we have brought in a 00:10:38.832 --> 00:10:42.060 video crew to record all the actions that we have been 00:10:42.060 --> 00:10:45.270 performing to actually complete the analysis. 00:10:45.270 --> 00:10:50.230 I like to now share with you what we have recorded and 00:10:50.230 --> 00:10:54.470 narrate to you as we go step by step through the analysis 00:10:54.470 --> 00:10:57.950 of this plate on the computer. 00:10:57.950 --> 00:11:02.060 Our first step is to look at how we are generating using 00:11:02.060 --> 00:11:06.400 ADINA-IN, how we are generating this mesh, and also 00:11:06.400 --> 00:11:11.210 the other data that are required for use of ADINA. 00:11:11.210 --> 00:11:15.000 So let's look at this first step now, after which I will 00:11:15.000 --> 00:11:20.140 then introduce you to the next step and narrate continuous 00:11:20.140 --> 00:11:23.660 narration of the analysis. 00:11:23.660 --> 00:11:25.780 Here we show briefly the hardware equipment we are 00:11:25.780 --> 00:11:28.490 using in my MIT laboratory. 00:11:28.490 --> 00:11:32.300 A MASSCOMP minicomputer with two megabytes of real memory, 00:11:32.300 --> 00:11:35.320 and 330 megabytes of disk storage. 00:11:35.320 --> 00:11:37.200 We also have a tape drive. 00:11:37.200 --> 00:11:39.600 The computer features virtual memory, and we use a 00:11:39.600 --> 00:11:41.045 Unix-based operating system. 00:11:44.560 --> 00:11:46.890 Roughly, for our purposes, the computer is 00:11:46.890 --> 00:11:50.670 equivalent to a VAX 750. 00:11:50.670 --> 00:11:51.940 We use two terminals. 00:11:51.940 --> 00:11:54.190 One terminal for alphanumerical and numerical 00:11:54.190 --> 00:11:57.410 input and output, and one terminal, the one to the 00:11:57.410 --> 00:11:58.660 right, for graphical output. 00:12:01.210 --> 00:12:02.210 We also have a plotter. 00:12:02.210 --> 00:12:05.110 We use this plotter to generate the figures of finite 00:12:05.110 --> 00:12:09.440 element meshes, and results for this course. 00:12:09.440 --> 00:12:11.640 Here comes my student, Ted [? Sossman, ?] 00:12:11.640 --> 00:12:13.660 who will sit at the terminal to input 00:12:13.660 --> 00:12:15.670 the data to the program. 00:12:15.670 --> 00:12:18.720 In what follows, we will see the data input prepared by Ted 00:12:18.720 --> 00:12:21.030 on the terminal at which he sits. 00:12:21.030 --> 00:12:23.730 Non-graphical output is displayed by that same 00:12:23.730 --> 00:12:26.990 terminal, whereas we will see graphical output displayed on 00:12:26.990 --> 00:12:29.540 the right terminal. 00:12:29.540 --> 00:12:31.200 Here, we see the start of input 00:12:31.200 --> 00:12:33.470 preparation for ADINA-IN. 00:12:33.470 --> 00:12:36.370 We have opened the data base, on which the data input and 00:12:36.370 --> 00:12:39.460 generated will be stored and have already input the title 00:12:39.460 --> 00:12:44.700 for the analysis, quarter plate with hole, 64 elements. 00:12:44.700 --> 00:12:47.420 We have also defined master degrees of freedom conditions 00:12:47.420 --> 00:12:50.820 by specifying the values of IDOF. 00:12:50.820 --> 00:12:54.330 1 means of a deleted degree of freedom, 0 means a free, 00:12:54.330 --> 00:12:56.360 existing degree of freedom. 00:12:56.360 --> 00:12:58.970 Here, all degrees of freedom have been deleted except for 00:12:58.970 --> 00:13:01.860 the yz displacements. 00:13:01.860 --> 00:13:03.920 Notice also that at our request, all 00:13:03.920 --> 00:13:05.840 text appears twice. 00:13:05.840 --> 00:13:08.900 After we have typed a line, the line is echoed back by the 00:13:08.900 --> 00:13:11.520 program merely for checking. 00:13:11.520 --> 00:13:14.020 In what follows, we now specify the coordinates of a 00:13:14.020 --> 00:13:17.110 few key points that defines the outline of the 00:13:17.110 --> 00:13:18.360 quarter of the plate. 00:13:22.660 --> 00:13:24.583 Note we define the y- and z-coordinates. 00:13:30.560 --> 00:13:39.100 First of node 1, then for nodes 2, 3, 4, 5, and 6. 00:13:46.670 --> 00:13:50.110 Note that these coordinates are input in free format. 00:13:50.110 --> 00:13:53.230 Here the node 6 input is not aligned with the other nodal 00:13:53.230 --> 00:13:54.480 point coordinate input. 00:13:56.970 --> 00:14:00.520 We now want to look at the plot of these nodal points. 00:14:00.520 --> 00:14:02.950 This is achieved by the frame and mesh commands. 00:14:10.880 --> 00:14:13.030 Here they are, the six points. 00:14:13.030 --> 00:14:17.670 Point 1 is the center of the hole, points 2 and 3 defines 00:14:17.670 --> 00:14:18.920 the boundary of the hole. 00:14:21.640 --> 00:14:24.850 Points 4, 5, 6 defines the remaining corners of the 00:14:24.850 --> 00:14:27.050 quarter plate. 00:14:27.050 --> 00:14:31.510 And here, you see the first set of generated nodes. 00:14:31.510 --> 00:14:34.210 Note that the nodal points have consecutive numbers along 00:14:34.210 --> 00:14:37.430 the vertical symmetry edge, except for the top and bottom 00:14:37.430 --> 00:14:41.700 nodes, numbers 3 and 4, similarly for the horizontal 00:14:41.700 --> 00:14:44.090 symmetry edge. 00:14:44.090 --> 00:14:46.540 This would mean a large bandwidth unless we use a 00:14:46.540 --> 00:14:48.410 bandwidth minimizer. 00:14:48.410 --> 00:14:51.150 And we will do so, hence we are not concerned with the 00:14:51.150 --> 00:14:54.800 nodal point numbering used at this stage. 00:14:54.800 --> 00:14:57.175 Next, we generate also the nodal points on the remaining 00:14:57.175 --> 00:14:59.630 edges of the quarter plate. 00:14:59.630 --> 00:15:02.810 And here they are. 00:15:02.810 --> 00:15:07.670 We now want to generate the elements of the plate. 00:15:07.670 --> 00:15:10.040 For this we define, first the material to be a elastic. 00:15:13.070 --> 00:15:18.120 Young's modulus E, Poisson's ratio NU. 00:15:25.900 --> 00:15:27.820 We want a plane stress element group. 00:15:36.110 --> 00:15:37.630 The Gauss integration order is 3x3. 00:15:40.570 --> 00:15:44.300 The material set has a number 1, this is the material set we 00:15:44.300 --> 00:15:45.550 just defined. 00:15:47.340 --> 00:15:51.320 The G-surface command next generates the 8-node elements 00:15:51.320 --> 00:15:54.070 in the domain defined by the corner points, so to 00:15:54.070 --> 00:15:55.450 say 6, 4, 3, 2. 00:15:59.260 --> 00:16:04.000 We now want to plot the generated element mesh, and 00:16:04.000 --> 00:16:05.250 here, you see it. 00:16:08.390 --> 00:16:12.500 Note once again, we use 8-note isoparametric elements, around 00:16:12.500 --> 00:16:14.010 the hole, they are curved elements. 00:16:16.850 --> 00:16:20.920 Finally, we also define in the ADINA-IN input the elements 00:16:20.920 --> 00:16:24.690 thicknesses to be 0.01 and the loads which correspond to the 00:16:24.690 --> 00:16:27.180 pulling on the plate. 00:16:27.180 --> 00:16:29.180 This [? end ?] completes the input preparation 00:16:29.180 --> 00:16:30.430 for ADINA-IN . 00:16:32.660 --> 00:16:35.330 ADINA-IN has now all the information to generate a 00:16:35.330 --> 00:16:38.380 complete input file ADINA. 00:16:38.380 --> 00:16:41.830 In addition, we also want to ask ADINA-IN to assign 00:16:41.830 --> 00:16:44.300 equation numbers that correspond to a minimum 00:16:44.300 --> 00:16:47.190 bandwidth for the solution of this problem. 00:16:47.190 --> 00:16:52.210 So our next step is to have ADINA-IN go through these 00:16:52.210 --> 00:16:56.670 actions, and turn back to our laboratory and see what is 00:16:56.670 --> 00:16:59.420 happening now. 00:16:59.420 --> 00:17:02.700 Here, we see the end of the ADINA-IN input file that we 00:17:02.700 --> 00:17:05.530 saw already before. 00:17:05.530 --> 00:17:10.109 The command ADINA now generates the ADINA file. 00:17:10.109 --> 00:17:12.569 At the same, also, the bandwidth of the stiffness 00:17:12.569 --> 00:17:15.430 matrix is minimized. 00:17:15.430 --> 00:17:18.619 We use the reverse Cuthill-Mckee algorithm. 00:17:18.619 --> 00:17:24.680 Notice that the bandwidth has been reduced from 399 to 93. 00:17:24.680 --> 00:17:28.400 The original bandwidth was, of course, artificially large 00:17:28.400 --> 00:17:30.740 because our nodal point generation did not take 00:17:30.740 --> 00:17:33.900 account of any bandwidth considerations, as I pointed 00:17:33.900 --> 00:17:36.570 out before. 00:17:36.570 --> 00:17:38.500 Let us briefly look at the ADINA file 00:17:38.500 --> 00:17:41.360 generated by the ADINA-IN. 00:17:41.360 --> 00:17:44.120 Here, we see common cards, automatically inserted by 00:17:44.120 --> 00:17:47.290 ADINA-IN to explain the input cards. 00:17:47.290 --> 00:17:50.760 We see the master control card, the load control card, 00:17:50.760 --> 00:17:55.580 the Eigenvalue solution control card, and so on. 00:17:55.580 --> 00:17:59.230 Let us look a bit closer at the element data cards. 00:17:59.230 --> 00:18:05.990 Element 1 has eight nodes and the first three are 6, 64, 74. 00:18:05.990 --> 00:18:10.325 Element 2 has 8 nodes and the first three are 64, 62, 76. 00:18:14.040 --> 00:18:16.800 Note a maximum of nine nodes is possible. 00:18:16.800 --> 00:18:20.370 The last 0 is the node card signifies that the ninth node 00:18:20.370 --> 00:18:21.620 is not used. 00:18:24.720 --> 00:18:28.070 With a complete ADINA input file now available, we can 00:18:28.070 --> 00:18:32.110 call ADINA to execute this file and this gives us our 00:18:32.110 --> 00:18:33.900 first solution results. 00:18:33.900 --> 00:18:36.590 We look at the solution results and, in particular, we 00:18:36.590 --> 00:18:41.390 plot the deformed mesh onto the original mesh, and this 00:18:41.390 --> 00:18:45.540 shows, in fact, that we have made an error in the input 00:18:45.540 --> 00:18:46.560 description. 00:18:46.560 --> 00:18:50.660 It will show us that we have fixed all these nodes down 00:18:50.660 --> 00:18:55.190 here, whereas they should have been on a roller. 00:18:55.190 --> 00:18:57.940 This is shown by plotting the deformed mesh on to the 00:18:57.940 --> 00:19:00.080 original mesh, and it's also shown by 00:19:00.080 --> 00:19:02.120 looking at the stresses. 00:19:02.120 --> 00:19:07.780 We do so by using an option in the ADINA system for the 00:19:07.780 --> 00:19:12.570 stress vector outputs, and this is schematically shown 00:19:12.570 --> 00:19:14.500 here, this option. 00:19:14.500 --> 00:19:17.510 We plot maximum principle stresses-- 00:19:17.510 --> 00:19:19.780 say tensile in this case here-- 00:19:19.780 --> 00:19:26.040 as a line with two arrows, and principles stress that's 00:19:26.040 --> 00:19:29.920 compressive as simply a line. 00:19:29.920 --> 00:19:34.820 So we can see, in other words, how the stress flows through 00:19:34.820 --> 00:19:38.280 the material, and we can see, of course, compressive and 00:19:38.280 --> 00:19:42.170 tensile stress situations, and notice that the lengths of 00:19:42.170 --> 00:19:46.490 these lines corresponds or is proportional to the magnitude 00:19:46.490 --> 00:19:48.680 of the stresses. 00:19:48.680 --> 00:19:54.030 We can plot this stress vector output for all the integration 00:19:54.030 --> 00:19:59.210 points stresses in the mesh, and that, as I said already, 00:19:59.210 --> 00:20:01.930 indicates clearly once again, that we have used the wrong 00:20:01.930 --> 00:20:04.280 boundary conditions down here. 00:20:04.280 --> 00:20:08.350 So we go and correct the boundary conditions down here, 00:20:08.350 --> 00:20:10.900 and re-run the analysis. 00:20:10.900 --> 00:20:15.520 In other words, call ADINA again and those results that 00:20:15.520 --> 00:20:19.610 we obtained then, once again, displacements, in other words, 00:20:19.610 --> 00:20:22.750 are plotted by plotting the deformed mesh onto the 00:20:22.750 --> 00:20:24.120 original mesh. 00:20:24.120 --> 00:20:26.350 We see that we now got much better, much more 00:20:26.350 --> 00:20:28.110 realistically-looking results. 00:20:28.110 --> 00:20:32.850 And we also will look at the stresses using the stress 00:20:32.850 --> 00:20:38.730 vector plots again, in the elements, that show us also 00:20:38.730 --> 00:20:42.340 that the results are now quite realistic and that our mesh, 00:20:42.340 --> 00:20:45.050 including the boundary conditions have been quite 00:20:45.050 --> 00:20:46.860 properly defined. 00:20:46.860 --> 00:20:52.080 So let us now look at this step of the analysis. 00:20:52.080 --> 00:20:54.420 The command runadina calls ADINA to 00:20:54.420 --> 00:20:57.450 execute the input data. 00:20:57.450 --> 00:20:59.770 The data input file is in ADINA-IN F02. 00:21:04.890 --> 00:21:07.680 And here, we see now the deformed plotted onto the 00:21:07.680 --> 00:21:08.890 original mesh. 00:21:08.890 --> 00:21:11.690 The original mesh is plotted in dash lines. 00:21:11.690 --> 00:21:13.395 Of course, the deformations are magnified. 00:21:16.190 --> 00:21:19.570 Note that as expected, the top face has uniformly moved up. 00:21:26.080 --> 00:21:28.630 However, note that the nodal points on the horizontal 00:21:28.630 --> 00:21:31.580 symmetry line have not displaced at all. 00:21:31.580 --> 00:21:34.420 This is quite unphysical and shows that the wrong boundary 00:21:34.420 --> 00:21:37.380 conditions have been used. 00:21:37.380 --> 00:21:40.220 If we look at the stress vector plot over the mesh, the 00:21:40.220 --> 00:21:42.200 same conclusion is reached. 00:21:42.200 --> 00:21:44.680 For clarity, on the video, we show here the stress vectors 00:21:44.680 --> 00:21:48.940 just on the elements closest to the hole. 00:21:48.940 --> 00:21:51.670 And we can see in the element adjoining the horizontal 00:21:51.670 --> 00:21:56.010 symmetry line, a stress that acts normal to the whole. 00:21:56.010 --> 00:21:59.160 This is, of course, unphysical. 00:21:59.160 --> 00:22:01.330 Next, we show the stress vectors in the outer most 00:22:01.330 --> 00:22:03.090 elements of the quarter plate. 00:22:03.090 --> 00:22:06.420 And you can see here, a stress acting perpendicular to the 00:22:06.420 --> 00:22:09.360 free edge of the plate, when we look near the horizontal 00:22:09.360 --> 00:22:11.530 symmetry line. 00:22:11.530 --> 00:22:14.610 This is also unphysical and is due to having specified the 00:22:14.610 --> 00:22:16.050 wrong boundary conditions on the wrong 00:22:16.050 --> 00:22:17.300 horizontal symmetry line. 00:22:20.910 --> 00:22:22.450 The specification of the boundary 00:22:22.450 --> 00:22:24.520 conditions is shown here. 00:22:24.520 --> 00:22:26.860 The character, C, denotes the boundary condition on the 00:22:26.860 --> 00:22:28.150 horizontal symmetry line. 00:22:32.930 --> 00:22:35.280 The character B denotes the boundary condition on the 00:22:35.280 --> 00:22:37.410 vertical symmetry line. 00:22:37.410 --> 00:22:40.780 Where B means only the z displacement is free and C 00:22:40.780 --> 00:22:43.810 means all displacements are fixed. 00:22:43.810 --> 00:22:45.610 For the six possible displacements and 00:22:45.610 --> 00:22:46.370 [? flotatations, ?] 00:22:46.370 --> 00:22:49.620 a 1 means the degree of freedom is fixed, and 0 means 00:22:49.620 --> 00:22:50.870 the degree of freedom is free. 00:22:54.610 --> 00:22:56.170 We now correct the boundary conditions. 00:22:59.320 --> 00:23:02.380 And B on the horizontal symmetry line means now the v 00:23:02.380 --> 00:23:05.620 displacement is free. 00:23:05.620 --> 00:23:08.520 C on the vertical symmetry line means now the w 00:23:08.520 --> 00:23:09.770 displacement is free. 00:23:13.810 --> 00:23:16.480 We run ADINA again, and here you see the deformed mesh 00:23:16.480 --> 00:23:19.270 plotted on the original mesh. 00:23:19.270 --> 00:23:22.820 The deformations look very reasonable. 00:23:22.820 --> 00:23:25.750 The plate has contracted horizontally, and 00:23:25.750 --> 00:23:27.990 correspondingly, the hole has shrunk horizontally. 00:23:33.260 --> 00:23:35.830 The deformations closest to the hole are shown here. 00:23:38.840 --> 00:23:40.350 And here, we see the stress vector 00:23:40.350 --> 00:23:42.310 plots for these elements. 00:23:42.310 --> 00:23:45.110 The stresses align nicely with the hole. 00:23:45.110 --> 00:23:47.680 Notice that there is no stress perpendicular to the free 00:23:47.680 --> 00:23:50.640 surface of the hole when we look at the integration point 00:23:50.640 --> 00:23:51.910 layer closest as a hole. 00:23:54.460 --> 00:23:56.790 The value of the maximum stress is given here. 00:23:56.790 --> 00:24:01.040 It is 301.9 megapascal. 00:24:01.040 --> 00:24:03.170 Here, we look at the element which carries the largest 00:24:03.170 --> 00:24:06.600 stress, element 57. 00:24:06.600 --> 00:24:08.870 Once again, we can see that the stresses align 00:24:08.870 --> 00:24:11.940 nicely with the hole. 00:24:11.940 --> 00:24:15.610 We now recall is that the objective of our analysis is 00:24:15.610 --> 00:24:18.920 really the calculation of the stress concentration factor. 00:24:18.920 --> 00:24:21.930 And if we look at the problem once more, here, we have the 00:24:21.930 --> 00:24:23.990 plate with the hole. 00:24:23.990 --> 00:24:28.050 The plate subjected to the tractions, as shown here. 00:24:28.050 --> 00:24:30.550 We now need to, of course, predict the stresses 00:24:30.550 --> 00:24:33.770 accurately around the hole, and in particular, at this 00:24:33.770 --> 00:24:35.290 point here. 00:24:35.290 --> 00:24:37.170 Here, we have our finite element 00:24:37.170 --> 00:24:39.690 method used in the analysis. 00:24:39.690 --> 00:24:42.370 And so far, the only calculated stresses at the 00:24:42.370 --> 00:24:45.720 integration points in the elements. 00:24:45.720 --> 00:24:49.040 Now this is here, by the way, element number 57. 00:24:49.040 --> 00:24:53.210 And for this element, we have calculated so far, only the 00:24:53.210 --> 00:24:56.150 stresses at these integration points. 00:24:56.150 --> 00:24:59.470 However, these integration points do not lie on the 00:24:59.470 --> 00:25:03.200 circumference of the hole, on the boundary of the hole. 00:25:03.200 --> 00:25:06.350 And that is where the maximum stresses occur. 00:25:06.350 --> 00:25:10.380 Of particular interest is, of course, also this point here, 00:25:10.380 --> 00:25:12.880 where we anticipate to obtain the maximum 00:25:12.880 --> 00:25:14.910 stress in the analysis. 00:25:14.910 --> 00:25:18.970 If you look at, schematically, how the stresses would vary, 00:25:18.970 --> 00:25:24.090 say, through the element, to the boundary of the hole, we 00:25:24.090 --> 00:25:27.470 would see a schematic plot as shown here. 00:25:27.470 --> 00:25:30.900 Here is an actual element, the other elements lie next to it, 00:25:30.900 --> 00:25:33.480 and here you can see schematically shown the stress 00:25:33.480 --> 00:25:36.960 computed at the closest integration point to the 00:25:36.960 --> 00:25:38.530 boundary of the hole. 00:25:38.530 --> 00:25:40.790 And here, we would have the stress computed 00:25:40.790 --> 00:25:42.140 at the nodal point. 00:25:42.140 --> 00:25:45.580 That is actually the stress that we are interested in. 00:25:45.580 --> 00:25:49.660 Well, we can ask ADINA to calculate the stresses at the 00:25:49.660 --> 00:25:55.260 nodal points, and then we can ask ADINA-PLOT to enter with 00:25:55.260 --> 00:25:59.640 these nodal point stresses into this formula here. 00:25:59.640 --> 00:26:04.940 Sigma yy, sigma zz, and sigma yz are the stresses at the 00:26:04.940 --> 00:26:06.900 nodal points. 00:26:06.900 --> 00:26:12.170 To calculate, ADINA-PLOT calculate this Sigma 1, which 00:26:12.170 --> 00:26:16.300 is the maximum principle of stress at that nodal point. 00:26:16.300 --> 00:26:19.770 We can ask ADINA-PLOT to calculate sigma 1 at all the 00:26:19.770 --> 00:26:26.160 nodal points in the mesh, and by doing so, we obtained these 00:26:26.160 --> 00:26:29.270 stresses and then they can ask ADINA-PLOT to search through 00:26:29.270 --> 00:26:32.490 those nodal points stresses, these sigma 1 stresses, to 00:26:32.490 --> 00:26:37.770 find us the location, the element and the nodal point, 00:26:37.770 --> 00:26:41.200 to have the physical location of the maximum stress 00:26:41.200 --> 00:26:42.525 occurring in the mesh. 00:26:42.525 --> 00:26:49.950 We will see that doing so, ADINA-PLOT comes up to tell us 00:26:49.950 --> 00:26:55.640 that this is the point, element number 57, point 00:26:55.640 --> 00:26:58.990 number 4, that is this physical point here, where the 00:26:58.990 --> 00:27:02.320 maximum stress occurs and will also give us that maximum 00:27:02.320 --> 00:27:04.720 stress, and that maximum stress, of course, gives us 00:27:04.720 --> 00:27:07.450 then the stress concentration factor. 00:27:07.450 --> 00:27:13.500 So let us now look at this phase of the analysis. 00:27:13.500 --> 00:27:15.830 Here, we have input some information regarding 00:27:15.830 --> 00:27:18.910 variables that need be defined in ADINA plot. 00:27:18.910 --> 00:27:25.220 TYY refers to tau yy, TZZ refers to tau zz, TYZ 00:27:25.220 --> 00:27:28.120 refers to tau yz. 00:27:28.120 --> 00:27:30.430 We define the result and variable to calculate the 00:27:30.430 --> 00:27:34.350 maximum principle stress. 00:27:34.350 --> 00:27:40.010 Hence, when TYY, TZZ, and TYZ are defined [? smax ?] 00:27:40.010 --> 00:27:41.880 gives the maximum principle stress. 00:27:46.640 --> 00:27:49.700 Here, we now enter the command to look for the maximum 00:27:49.700 --> 00:27:51.140 principal stress in the mesh. 00:27:57.280 --> 00:28:01.270 First we make a small input error, obtain a message, we 00:28:01.270 --> 00:28:13.350 correct the input, and here comes the result. 00:28:13.350 --> 00:28:17.510 We see that indeed element 57.4 carries a maximum 00:28:17.510 --> 00:28:25.260 principle stress and this value is 345.151 megapascal. 00:28:25.260 --> 00:28:27.840 We have now actually obtained an answer to the 00:28:27.840 --> 00:28:29.760 question that we asked. 00:28:29.760 --> 00:28:31.900 Originally, namely, we wanted to calculated the stress 00:28:31.900 --> 00:28:34.670 concentration factor around the hole. 00:28:34.670 --> 00:28:37.040 And we have obtained a number for that stress 00:28:37.040 --> 00:28:38.880 concentration factor. 00:28:38.880 --> 00:28:42.630 However, a valid question, certainly is to ask, how good 00:28:42.630 --> 00:28:43.480 is this number? 00:28:43.480 --> 00:28:47.710 After all, we used a finite element mesh to approximate 00:28:47.710 --> 00:28:50.910 the plate a particular finite element idealization was used, 00:28:50.910 --> 00:28:54.230 and we have only obtained an approximation 00:28:54.230 --> 00:28:57.310 to the exact result. 00:28:57.310 --> 00:29:01.070 Well, to evaluate that question, to obtain insight 00:29:01.070 --> 00:29:05.140 into that question, to evaluate how good our analysis 00:29:05.140 --> 00:29:10.970 results really are, we can plot stress jumps, the way we 00:29:10.970 --> 00:29:13.130 discussed it in an earlier lecture. 00:29:13.130 --> 00:29:17.370 And in particular, for the analysis that I'd like to show 00:29:17.370 --> 00:29:21.660 you in this final phase, we have plotted stress jumps 00:29:21.660 --> 00:29:25.390 along these two lines. 00:29:25.390 --> 00:29:28.570 Now, notice that, for example, at this node here, we have 00:29:28.570 --> 00:29:32.940 four elements coupling into this node, so at this node we 00:29:32.940 --> 00:29:36.760 get four different stress predictions 00:29:36.760 --> 00:29:39.450 for each stress component. 00:29:39.450 --> 00:29:43.760 At this node here, we would have only two stress 00:29:43.760 --> 00:29:46.900 predictions, for each stress component because only two 00:29:46.900 --> 00:29:49.960 elements couple into this node. 00:29:49.960 --> 00:29:55.430 That is one way to evaluate or to look at how accurate our 00:29:55.430 --> 00:29:56.680 results are. 00:29:58.890 --> 00:30:02.830 An alternative way is to plot pressure bands, and the 00:30:02.830 --> 00:30:05.270 pressure here is scalar. 00:30:05.270 --> 00:30:09.410 It's computed as shown here, and we can plot bands of 00:30:09.410 --> 00:30:12.150 constant pressure, the way we already have discussed it in 00:30:12.150 --> 00:30:13.240 an earlier lecture. 00:30:13.240 --> 00:30:17.880 Notice because this is a scalar, it can be used very 00:30:17.880 --> 00:30:21.910 nicely to plot these bands of constant pressure. 00:30:21.910 --> 00:30:24.170 Of course, we could also have used here, say, an effective 00:30:24.170 --> 00:30:29.810 stress, which is also a scalar, and we could plot 00:30:29.810 --> 00:30:33.440 bands of constant effective stresses. 00:30:33.440 --> 00:30:38.560 One example that you've seen already early, is this one 00:30:38.560 --> 00:30:42.960 here where we plotted pressure bands, with band magnitude of 00:30:42.960 --> 00:30:48.435 5 MPa, megapascal, and you can see here this white band, here 00:30:48.435 --> 00:30:52.580 a black band, in other words, we're going in steps 5 MPa 00:30:52.580 --> 00:30:55.390 from one band to the next. 00:30:55.390 --> 00:30:59.970 Notice that there's a pressure band discontinuity right here, 00:30:59.970 --> 00:31:03.710 which already indicates that we have a stress discontinuity 00:31:03.710 --> 00:31:06.800 here, and which indicates that the mesh that we used is 00:31:06.800 --> 00:31:10.180 really not a very fine mesh. 00:31:10.180 --> 00:31:13.450 And if we are interested in obtaining a very accurate 00:31:13.450 --> 00:31:18.250 result, then based on these pressure band plots, and also 00:31:18.250 --> 00:31:21.750 the stress jump plots that I will show you just now, we may 00:31:21.750 --> 00:31:23.980 actually decide to use a finer mesh. 00:31:23.980 --> 00:31:27.360 We discussed this issue already in an earlier lecture. 00:31:27.360 --> 00:31:32.400 So let us now then look at what happens, or what happened 00:31:32.400 --> 00:31:35.420 in this final phase of the analysis. 00:31:35.420 --> 00:31:38.140 Let's go back to the laboratory and share the 00:31:38.140 --> 00:31:40.175 experiences that we'll see there. 00:31:42.840 --> 00:31:44.490 Here, we see once more the mesh we're 00:31:44.490 --> 00:31:45.740 using in the analysis. 00:31:48.090 --> 00:31:51.230 We will plot the stresses, and hence, we can see the stress 00:31:51.230 --> 00:31:54.930 jumps along the horizontal symmetry line, and the 00:31:54.930 --> 00:31:56.350 diagonal line of the plate. 00:32:04.100 --> 00:32:06.670 Here, you see the stresses along the horizontal symmetry 00:32:06.670 --> 00:32:08.660 line, Tau zz is plotted. 00:32:12.760 --> 00:32:15.110 The horizontal axis measures distance along 00:32:15.110 --> 00:32:16.360 the symmetry line. 00:32:20.430 --> 00:32:22.955 And the vertical axis measures the stress values. 00:32:31.810 --> 00:32:34.200 Note that the stress predictions at the nodes, when 00:32:34.200 --> 00:32:38.590 calculated for the different elements are almost the same. 00:32:38.590 --> 00:32:42.000 Only at one node can we actually see a difference, and 00:32:42.000 --> 00:32:44.600 it is quite small. 00:32:44.600 --> 00:32:48.990 Note that two elements couple into this node. 00:32:48.990 --> 00:32:51.750 Hence, there are only small stress jumps along the 00:32:51.750 --> 00:32:54.010 horizontal symmetry axis of the plate. 00:32:56.790 --> 00:32:59.450 Next, we look at the stress plot along the diagonal line 00:32:59.450 --> 00:33:01.200 of the model. 00:33:01.200 --> 00:33:04.440 Here the maximum principle stress is plotted. 00:33:04.440 --> 00:33:07.850 Note that at one node into which four elements couple, we 00:33:07.850 --> 00:33:11.690 have four markedly different stress values. 00:33:11.690 --> 00:33:15.040 Indeed, we have significant stress jumps at that node, but 00:33:15.040 --> 00:33:16.530 otherwise the stress predictions do 00:33:16.530 --> 00:33:17.780 not show large jumps. 00:33:25.220 --> 00:33:29.240 Finally, we look at the pressure band plots. 00:33:29.240 --> 00:33:31.710 Here, they are drawn. 00:33:31.710 --> 00:33:34.550 To save time, we skipped some of the drawing process and 00:33:34.550 --> 00:33:36.430 jumped to a later picture here. 00:33:46.570 --> 00:33:51.260 We notice that the pressure bands are quite continuous, 00:33:51.260 --> 00:33:54.150 except between the first and second layer of elements 00:33:54.150 --> 00:33:55.370 around the hole. 00:33:55.370 --> 00:33:58.190 This corresponds to the stress discontinuity between these 00:33:58.190 --> 00:34:00.110 element layers that we saw earlier. 00:34:02.840 --> 00:34:05.480 We see now this is now completed, I'd like to look 00:34:05.480 --> 00:34:09.070 with you once more back on to two view graphs that we 00:34:09.070 --> 00:34:13.370 already have looked at earlier. 00:34:13.370 --> 00:34:15.800 On this you graph, we summarize some important 00:34:15.800 --> 00:34:16.840 observations. 00:34:16.840 --> 00:34:19.590 And we said that it is very important to check the finite 00:34:19.590 --> 00:34:23.540 element data input carefully prior to the actual response 00:34:23.540 --> 00:34:24.580 solution run. 00:34:24.580 --> 00:34:27.940 That, of course, means plotting the data. 00:34:27.940 --> 00:34:30.500 And we have done so, of course, in our analysis. 00:34:30.500 --> 00:34:33.960 And after the response solution has been obtained, by 00:34:33.960 --> 00:34:36.360 starting whether desired boundary conditions are 00:34:36.360 --> 00:34:39.110 satisfied, whether displacement and stress 00:34:39.110 --> 00:34:41.820 solution is reasonable. 00:34:41.820 --> 00:34:45.429 Remember, in our analysis, we did this, of course, as well 00:34:45.429 --> 00:34:50.900 and we found, by looking at the boundary conditions, the 00:34:50.900 --> 00:34:54.610 way they were represented in the actual solution, that we 00:34:54.610 --> 00:34:57.230 have actually made an error. 00:34:57.230 --> 00:35:00.570 In other words, we looked at the deformed mesh, and the 00:35:00.570 --> 00:35:03.060 boundary conditions on the deformed mesh in our first 00:35:03.060 --> 00:35:07.030 analysis showed that we had fixed the boundary at the 00:35:07.030 --> 00:35:10.190 bottom off the mesh, which was an error. 00:35:10.190 --> 00:35:14.720 So it is very important to go through this step, to look 00:35:14.720 --> 00:35:16.820 very closely whether the boundary conditions are 00:35:16.820 --> 00:35:21.550 actually satisfied on the mesh that you have been using, in 00:35:21.550 --> 00:35:22.640 the right way. 00:35:22.640 --> 00:35:27.930 Of course, the same holds for the stress and solution. 00:35:27.930 --> 00:35:31.230 Remember, that we looked at the stress plots for the mesh 00:35:31.230 --> 00:35:34.540 that was fixed at the bottom and we could directly see 00:35:34.540 --> 00:35:38.050 there were errors there, and, in other words, the error of 00:35:38.050 --> 00:35:42.860 having fixed the boundary at the bottom of the plate. 00:35:42.860 --> 00:35:46.080 So this step is most important, and we have seen an 00:35:46.080 --> 00:35:50.450 example in the analysis that we just completed. 00:35:50.450 --> 00:35:54.520 I also had this view graph already on, where we said that 00:35:54.520 --> 00:35:56.690 we want to carefully evaluate and interpret 00:35:56.690 --> 00:35:58.580 the calculated response. 00:35:58.580 --> 00:36:01.580 We want to study, in detail, the calculated displacement 00:36:01.580 --> 00:36:04.630 and stresses along certain lines, study stress jumps. 00:36:04.630 --> 00:36:08.660 Well, we saw an example of that in the analysis that we 00:36:08.660 --> 00:36:13.310 just completed, and we also pointed out that it is 00:36:13.310 --> 00:36:16.760 important to go through this step here first, prior to 00:36:16.760 --> 00:36:20.280 using a stress averaging because if you do average 00:36:20.280 --> 00:36:23.700 stresses, of course, you would never see stress jumps. 00:36:23.700 --> 00:36:27.210 And this can be an important step to gain confidence in the 00:36:27.210 --> 00:36:30.210 analysis results that you have obtained. 00:36:30.210 --> 00:36:32.970 This then completes what I wanted to share with you in 00:36:32.970 --> 00:36:33.710 this lecture. 00:36:33.710 --> 00:36:35.080 Thank you very much for your attention.