Up and Running with Inventor Nastran Nonlinear Analysis—Real-World Examples

WASIM YOUNIS: Welcome, everyone, to the Up and Running with Inventor Nastran Nonlinear Analysis-- Real World Examples, and my name is Wasim. Before we begin, I just want to give you a little bit about me.

I've been passionate about simulation. I've been involved with the auto simulation software from the very beginning, and over the past 10, 12 years, I have written numerous books on Inventor Professional and Inventor Nastan. And I have a background in mechanical engineering and computer aided engineering.

Today, I'm going to give you an overview of nonlinear analysis. Going to demonstrate workflows and guidance using real world cases from customers like yourselves. Towards the end, we will summarize my favorite top 10 tips.

There's a feeling and perception that nonlinear is complex and used by engineers and designers with high level academic qualifications, typically with masters and PhDs. The goal of this session is to demystify nonlinear analysis by showing you simple, straightforward workflows and tips on setting up and analyzing nonlinear studies using various analyses types available within Inventor Nastran.

But before we begin, I thought we'd probably go through what types of nonlinear analysis behaviors are out there, which can help you pick the right analysis type. So first of all, let's come across geometric nonlinearity examples, which can include stress stiffening, snapthrough, buckling, and large deformations. In this example here, let's take a fishing rod, for example.

If we take a fishing rod of approximately two meters length and analyze that in Inventor Nastran linear analysis will get a deflection of around, I guess, 810 millimeters. And if we take the same example in a nonlinear analysis and set it up, we get a result which is completely different of 604 millimeters. The difference is that nonlinear analysis takes large deformation into account, and linear analysis assumes only small deformations.

Now, considering the rod is about two meters long, deflection is almost 50%, which is considered to be large deformations. If that's what you expect, then it is vital that you run it as a nonlinear analysis. The second phenomena is material nonlinearity. To keep it simple, any stress above yield inside the linear analysis would be incorrect. Material nonlinearity simply suggests that the high stress that will yield in some sort of localized yielding, or in other words, you'll have permanent deformation as you can see in this little hoop example.

And finally, the third type of phenomena which you'll come across is contacts, and these are typical in examples like these, when you have two components coming together. And the other example would be a drop test. So these are the three core examples of nonlinear analysis phenomena, and before we go into the real life cases, I thought we may want to have a look at the nonlinear analysis studies that you can do inside Inventor Nastran.

The first one is nonlinear static based on the implicit solver, and the example we're going to use, the first one, is to simulate elastic plastic behavior and to see the stresses beyond yield and see if there's any sort of permanent deformation. The second example we're going to go and look at is based on the nonlinear transient response analysis, which is again an implicit solver, and the example we're going to use in real life example is a drop test.

And in the third example is going to be a blast analysis of a door using the explicit dynamic solver. So these are the three examples I'm going to demonstrate using Nastran, but there are three more examples, which [INAUDIBLE] Nastran nonlinear analysis is capable of doing, and they are nonlinear buckling, explicit quasi static, and implicit [INAUDIBLE] analysis, which are not covered in this session.

Now, the first example is based on Simatek, a company based in Denmark, which designs and manufactures some sort of ventilation ducting type equipment. You can see the object highlighted by the red outline. That is called an inlet, and the goal here is to determine the maximum permanent deformation at a critical load, or if there is some sort of blockage, what happens. Can the inlet contain all the content inside?

Now for us to be able to perform any type of nonlinear analysis, we need some key information, and the two key information here are based on the nonlinear material behavior of carbon steel, which this component is made of, and obviously the critical load. The design limit, in this case, is that we don't want the permanent deformation to be exceeding 10%.

Now, in the real world, the performance test, we have to simulate some sort of blockage and leakage, which means it's very time consuming, and more importantly, that's not sustainable, especially if it fails. Then you've got to go through the whole process again.

Now, when we are performing nonlinear analysis, there is a very important workflow we need to consider, and that is the simplification of the geometry. And the simplification is typically two components. One is simply taking out non-structural components. The other one is non-structural features.

Now, depending on the complexity of the geometry, there may be an element of remodeling, and remodeling could be that we simplify the whole assembly as a solid model, we simplify the whole assembly into a single solid component, or if the structure is thin, we can make it out of a surface model. In this example, the customer decided to use the latter option, the simplified service model.

Now, when we perform a nonlinear analysis, the critical information is around elastic plastic. Now, inside Inventor Nastran, you have two types of options. You can select to apply the nonlinear material behavior, and that is called either bilinear approximation, which is the plastic part is based on 10% of [INAUDIBLE] modulus, or you can define a plastic curve or a multilinear curve, as sometimes referred to, but for that, we will need to obtain the stress and strain data.

In this example, we are going to use a plastic option because the client has got data to define the stress and strain curves. Once you perform a Nastran nonlinear static analysis, the type of results you can obtain in addition to stress are strain, and also you have the ability to look at permanent deformation.

Now, what we'll do here is we now will have a look at the workflow, what the customers go through, to perform a nonlinear study. So you can see here, we have the example all modeled in a single composite surface. Now, when I move my mouse over it, you can see that we have the ability to pick surfaces individually, so let's go into Nastran.

So in this first example here, I'm going to go through the whole process of setting it up, running it, and have a look at the results. And as we go through the different examples, we'll probably predefine certain criterias just to save time. Plus, this example is pretty simple to do.

So the first thing we're going to do here is that you can see that the first time you bring in a product or a design into Inventor Nastran, it will basically assume that you want to perform a linear study. Now, I'm going to change that. We're going to pick the first one, the nonlinear static, and while we pick this, is probably the most simplistic out of all the six options I suggested to you to perform. So let's pick that.

Now, obviously, the first thing I'm going to do here is we're going to define the idealizations and tell the software how thick these surfaces need to be for the analysis. So we'll go into Idealizations, and you can see here, we can have solid elements, shell elements. In this case, because it's a surface model, we're going to use shell elements.

So the first one is shell, and we're going to define the thickness of the main body, which is three millimeters. We have the carbon steel selected, and then because I'm going to assign this thickness to certain surfaces, I have to then pick them by selecting or enabling associated geometry.

Because there are lots of adjacent surfaces, and rather than me picking them individually, we can basically speed up the process by selecting-- excuse me-- phase chain. And now, we'll pick this surface here. You can see that [INAUDIBLE] all the adjoining tangent surfaces.

We're going to pick three more, this one, top, and bottom. That's the body. So once I have defined all these, we can click on the New button to start defining the other materials thicknesses.

So now, we pick shell elements. You can see it's created a body there, and this one's going to be support plate. So we'll just to tap in the name called SP, and we can make that one out of eight mil thickness.

Again, it can change the color, if you want, of the mesh, so these four support plates. Let's zoom in a little bit, [INAUDIBLE] one, two, three, and finally, four. So I'm happy with that one, so we press New again.

And the last one is going to be coflanges. For this one, we're going to simply define a value of four millimeters. Now, I can go and pick the flanges, one, two, and three, but one thing we can do cleverly in Inventor Nastran is that, if I press this button-- let's change the color to black, first of all. What it will do, it will assign the flanges and [INAUDIBLE] to all the surfaces which have been unassigned.

In this case here, it will be one, two, and three, and it's pretty clever how it does that. So if we want to press OK, just see and check if it's done all of them correctly. Let's change the color green because green on green won't look-- [INAUDIBLE] that color to, let's say, blue.

So when I finally say generate mesh, we'll know it's done it. You can see the body is pink, the support plates are blue-- light blue, you can barely see it. And then the other ones are more or less black one, two, and three.

So now, we have defined the mesh. Now, one more thing you'll notice here is, as you can see here-- the screen is probably easy if I go to the top here. This support plate is not connected to this surface here because the mesh is not linked. So we have two options here.

We can either use contacts-- now, having contacts in here, and running a nonlinear analysis, can be time consuming. So the alternative is, if you go to Mesh settings, you can click on this Continuous Meshing button. So if I click on that button there and then press Generate Mesh, you'll notice that the elements will now be coinciding with the plate, which means-- and also, there's no thick line appearing at the interface of the surfaces, which means it's connected.

Now, one of the tips is, when we're doing nonlinear analysis, is that we tend to use linear elements because it will converge quicker, and the results between linear and parabolic may not be that significantly different. Now, in the real world, a customer will probably use a finer mesh, but because I want to run this live, I'm going to use a mesh size of 100.

So I need to bring back the Inventor. So now, we have created the mesh. We've created the [INAUDIBLE]. The next thing here is we need to define the load and the constraints.

Now, before we do that, I'm simply going to go and have a look at the material properties. If you double click on here, that's the material we're using, and you can see here, I have already activated nonlinear properties on because, in this example here, I have used the plastic options, and to make it-- to save time, I have predefined the values strain and stress.

If I click on Show X, Y Plot, we have a true stress and strain curve now. So this is the ideal curve, so if you have data, then use this. So I'm going to close the box now.

So the material has been assigned elastic plastic, and now, we can go and create the-- let's do the constraint first. Let's rename it Fixed Flange. And then I'm going to zoom in here, and I want to fix that flange here. We can change the density and size and press OK there. Now, the bottom flange is fixed.

Now, we can specify the blast or the critical load. It's a pressure, and we're going to put in 0.082. And again, because we have multiple surfaces we need to pick, let's activate phase chain like we did in the idealization creation. And if I pick that phase there, or surface, this one, this one, and this one, the same surfaces which we used to create our body idealization.

And I want to see which way the pressure is going to be applied before I press OK, and to do that, we're going to click on the Preview button here. And I could change the color of this to black. Let's have a look.

That's not very clear, so we can change the density. I can see, straightaway, the pressure is being exerted from the outside, so we can change that by simply putting a negative value in there. I'm going to make the size a little bit smaller.

So now, I think we're almost ready. So we have the loading applied, and the constraints. Now, I can see the results pretty clearly. I'm simply going to hide the loads and the constraints. And then what I'm going to do here is I'm going to run this and see what happens assuming that everything here has been defined, so let's press Run.

Now, you can see here that's pretty quick. I have enabled Inventor Nastran to use all cores on my machine, which I have 16 cores. Before you run analysis, you need to change the process parameters and change it. I'll show you that one [INAUDIBLE].

Now, we have it finished. That's fine. Now, this gives me a stress, which is fine, but I'm interested in having a look at the displacement.

Now, you see that it's giving me 25 millimeter deformation on here, but that's fine. If I then look at this strain value, now, this gives me a pretty small strain value, which is pretty small. Now, I need to understand if that small strain value has resulted in permanent deformation in my model.

Now, one of the ways to find out how to do permanent deformation is that we can create multiple subcases inside the nonlinear analysis. Each subcase is dependent on the one before it, so subcase two will start at the end of subcase one. So subcase one could be loaded, and subclass two could be unloaded, for example.

So that's what we're going to do here, and before I want to do that, you can see it took 20 seconds. And if I go all the way up to here, you can see it's using 16 colors. Now, how did I do that? Well, if I go into Parameters and right hand click and click Edit and type in Pro, you see there? The default is four. You can change that to your maximum number of colors before your press run and you can tell that it's been defined because it's green. And if you want to reset it, it'll go back to four, so that's fine.

And now, I'm going to create two subcases. [INAUDIBLE] subcases, right hand click, press New, and we'll pick, for the second subcase, I'm not going to use load one, which was a pressure load. But I need the constraint.

Now, for us to run the second subcase, which is number three here, we need a load. So typically if there's no load existing, we can put in gravity, and the gravity will go in the direction of y minus 0.9810. And we select both subcases, so the gravity will be assigned to both subcases. And I want to give it a name. Call it gravity.

And you can see, in the browser, we have gravity in my subcase three, and gravity and the load in subcase one. Let's rename the subcase, so that it makes it more meaningful. So subcase one, rename it, and we call it Loader. And subcase three, we'll load that one and say Unloader. What this will give me basically is that, when I look at the Unloader subcase results, I should be able to see the deformation indicating permanent deformation.

Now one more thing you might be interested in. If you're interested in looking at 10% of loading displacement and what happens at 50% of the loading and the displacement, we can change the intermittent output from off to on.

So the way Nastran-- the way nonlinear analysis works is that it simply increases the load from 0% to 4% over a series of, typically, eight increments. They're not necessarily equal increments, but it may go from 10%, 30%, 51% to 80%, and 100%. If you want them equally, then you can specify 10 increments, but typically, as good practice, leave it blank.

So we have the ability now to see intermediate results, and then on Unloader, I'm only interested in when it's fully at the end. So I don't care about intermediate outputs. I'm happy with that, and that's it. So now, we go ahead and press Run.

You can see here, it's going through increment one, two, three, four. When I say the subincrement, it basically cannot converge, so it breaks the time step into smaller number and then goes back again. And now, we've got increment eight, so you can see here that it run the first subcase, and eight increment, and the last sub case, the Unloader one, goes through it pretty quickly. And we're almost there. [INAUDIBLE]

What you see on the screen is the load two unloader. So if I spin this one around, let's have a look at displacements. Now, what it's telling me here that I have maximum permanent definition of 9.9 millimeters because the results are on the load two.

If I click on load one, which is basically increment 8 from my last increment I've loaded, that will be the same as my first analysis 25. So it fully deforms 25, but when you take the load off, it does not come back fully to zero. And this is how you can quickly check [INAUDIBLE] definition in a nonlinear static analysis, and then at the same time, you can look at how much strain that is on that loader.

Let's have a look. The criteria was less than 10%, and this one is less than 1%. It's very small, so it basically fits the criteria. And this is a very quick way for the client to check under a critical load when they have blockages rather than actually testing it in real life scenarios because that is not economical and sustainable.

So let's go back and go through our second case. So the second case is based on a client. Dellner is a global company, but the company-- or the example I'm using is based in the UK and Nordics. And the criteria here is that they're designing these gangways between the [INAUDIBLE].

And what they want to be able to do here is to be able to drop a rock from a height of five meters, something that maybe some kids or teenagers might drop something from a bridge, and they if anybody was standing inside it, how much it would deform, and if there's any clearance between the person's head, I guess, and how much it deforms by.

Now, the key information required for this type of analysis is that we need to have a look at the aluminum nonlinear material behavior. Now, obviously, to make the analysis simple, we probably will bring the block from a five meter height and have it close to the frame or the object, which means we need to define the impact velocity which would have been generated if it was to drop from five meters. And then also, we need to find the time of impact between the small gap because that will help us to create time steps and also material damping.

Now, you can see here, straightaway, that this is going to be a nonlinear transient response analysis, and it requires a lot more information than the first one, which was based on nonlinear static. Again, the usual stuff-- now, obviously, for the client to do this, they need to do it in a workshop and drop something. Obviously, if it doesn't work, then they got to do it all over again.

They've got to make the components and a lot of wastage, so hence, again, it's not economically feasible and more important, it's not sustainable. So hence, the client is relying on a lot of it on virtual testing and maybe the final design could be physically tested before they start building it.

And again, the process is to simplify the geometry by, first of all, removing non-structural components and features if possible. Again, if it's too complex, then it may be easy to create a simplified solid assembly half, in this case, or a simplified surface assembly half because it's symmetrical. And doing it as a half or a quarter and defining symmetry conditions is absolutely brilliant from a nonlinear analysis because it makes it more stable. In this case, we have a simplified solid assembly.

Now, in the first example, we use the plastic curve where we have several points. Define the stress and strain, and as an example here, we're going to use the bilinear approximation, which is pretty easy. The plastic part of the curve is a 10% gradient, or 10% of the [INAUDIBLE] modulus. So you can change that to whatever value.

You can make it flat almost, and have it set to 689 or 68.9. In this case, by default, it's 10%. Now, obviously, it's an approximation. So if you want to make it more realistic, then obviously, I would suggest you use a plastic curve if you can obtain the data.

Now, as I suggested before, rather than having the orange concrete block here at five meter height and running it, that can be very time consuming, we bring it closer to the red hook. That's a 10 millimeter gap, and we can then define the initial condition by the impact velocity by using this formula, 2 times gravity times the distance, which is 5 meters. And we have a impact velocity of almost 9,900 millimeter per second. That's the first value we need to specify.

Because we are running it as a nonlinear transient response analysis, then we have to specify some sort of damping in an ideal world. And the dominant frequency, W3, is pretty easy. We can run the same component as a modal analysis, and the first mode will be our dominant frequency, which you can specify. Damping value is not so straightforward, and that information needs to be obtained from a good textbook or engineering handbook.

And then we have another setup we have to go through and consider, which is the dynamic setup data. Now, basically, this can be broken down into two subcases, not that we are creating a [INAUDIBLE]. It's because the subcases are used to define a smaller timestamp and a larger timestamp. So when the first one finishes, the second one starts with a bigger timestamp, and this basically helps speed up the analysis. And it doesn't take a long time to run.

Now, to get an indication of what timestamp we require, we can use a little formula here. T is equal to distance between the two components and by the velocity. In this case here, we have a suggested timestamp of one milliseconds, so in this case here, for my initial subcase, we will specify 0.5 milliseconds. So after two timestamps we will hit-- we will get impact.

So these are the considerations, and what you see here on the screen now is showing you that we need to keep the durations long enough for it to obtain equilibrium, as you can see by the flat line and the permanent deformation of 108 on the left hand side. On the right hand side, you can see the component completely deformed.

So the key thing for a Nastran nonlinear transient response analysis is that you have to have a sufficiently long timestamp. Hence, the reason why we create two subcases. The first one is a small time step for the impact and rebound, and the next one here is for the rebound and to obtain equilibrium. So let's go back into the Nastran, and we can have a look at the gangway example.

So this is the gangway. We can see two examples. One is the hoop, and the other one, the orange one, is a concrete block brought very close to the hoop to speed up the analysis. And the other thing I've done here is, you can probably see it almost, I have created a split face on the hoop.

Now, the reason for that is that we're going to put a defined mesh at the contact regions. Now, if I did not have a split, then if I picked that face, it will go along the whole length of the hoop, which means you'll end up with having more elements. So it's always good practice to always split faces in the contact regions to minimize the number of contacts the software creates, and also the mesh.

So we're going to Nastran, and the first thing we'll notice here, it has created two analyzations. So if I expand these, one is aluminum and the concrete. The aluminum one I'm interested in because that is the red hoop, and this is the one which we will know has permanently deformed.

So I'm going to go and, first of all, let's change the analysis type. Now, this is time based because we want to see, over the duration of period, what happens. So we're going to pick the nonlinear transient response, and now this is probably one of the most difficult ones because it requires a lot of data.

So once we have that, we will check the material behavior of aluminum. The nonlinear has not been activated in this example. I simply go in there and switch on elastic plastic or the bilinear, and that's it, as simple as that.

Now, it's activated, and now, what we can do here, because it's half a model, we need to go and define some symmetry conditions. And how we do that is we go to Constraints. I'm going to select Frictionless as the easiest way to define symmetry, and then just to give it a name, the y arrow is normal to this face here, so I'm going to go and call it YSim.

And then I'm going to pick that, and you'll see there is [INAUDIBLE] fixed, and then we're going to fix that one. And then we're going to put the bottom face down here somewhere. There we go. There's three faces selected. I'm happy with that.

And then we're going to do the next restraint-- or the next constraint. And I'm going to call it Restraint, and we're going to stop the hoop going sideways. So we're going to pick the side faces, one, two, and we got here three, and then the concrete block side face. I'm happy with that one.

And then finally, we're going to go and fix the hoop so it doesn't go and fall into space. And we call it fixed, and we're going to here and specify these two thin, flat faces. And we're going to go on and press OK. So now, I have the constraints defined, I'm going to hide the symbols now.

Now, because we brought the block closer to my hoop, I am going to define the impact velocity, which would have been generated as if it would have been from five meters height. So in here, we have something called initial conditions. We're going to change that to velocity, and which direction is it going down in z? Type in 9904 negative.

So that is initial conditions. Once it hits z, then that's it, and then we click on-- we need gravity on as well. So click on New.

That's my mistake. It hasn't selected the entity, so I have to-- when I click on it, it only picks the face. But when you define initial conditions, you need to be able to pick the whole solid. Now, we'll do it again. Click New. Hang on, let's call it Name Impact. [INAUDIBLE] v, click new. There we go.

Now, we're going to specify gravity. Give it a name, G, and the gravity is again in the minus 9,810. And I can see here it's got a transient table. You can define a table and specify that it's always on, for example, which it is. If you leave it blank, or you do not define a table, then the software will assume it's active always, which is what we're going to do here.

Let's hide the loads again. So now, we have defined the constraints, loads, and the materials. The next task, we're going to do here is-- let's do some meshing. So I'll pick Mesh Control.

I'm going to put the face option here. We're going to pick-- specify five millimeters of the contact face. You can see here, when I pick that face and that face, you can see it is not picking the whole length of the hoop because I split it. And this basically helps you to reduce significantly the number of contact elements it generates in addition to mesh size. So that's five.

Then we go to mesh settings, everywhere else it would be 15. But at the same time, I want the transition from the fine mesh to the coarse mesh to go smoothly, and we'll change it to 1.1. And the final thing here, use linear elements, and that's it. And then when I press OK, we should have a mesh which is reasonably defined, so let's go back.

So we have the mesh, and we have the boundary conditions, and now we need to define contacts. So if you go to contacts [INAUDIBLE] here, I'm going to just [INAUDIBLE] contact, and I'm going to specify the regions in contact so that it helps us to reduce the number of contact-- rather than actually using it in overall size. Pick the first there, that one, and that one.

And then we can specify that, within 10 millimeters between the components, create the contact. Anything outside it, it won't create it. So this helps to also reduce the number of contacts.

So this is what we're going to do here. So that's more or less done. Now, we have to do something special in nonlinear transient response analysis, and that is, first of all, damping. So per my original suggestion, we'll use 5% here.

We would had to run a modal analysis on this assembly to determine what the first mode is, which is a dominant frequency. So we'll put 15 here. So that bit has been done, and then we-- now, if I was to click on nonlinear setup, now, you'll see here, we have a vast number of parameters you can pick and choose.

Now, typically, this dialog box used stay well away from it. This is sometimes used by experienced users, maybe [INAUDIBLE] through support, if something is not converging. But as a first rule of thumb, do not touch anything. If the software converges, then you don't need to modify anything. So even though it's there, most of the time, you'll never need to do anything with it.

Now, if we go dynamic setup one, now, what happens here is we need to specify a time step. Now, we worked out the time step, which was 0.0001, but this time, we're going to create a timestamp which is half of that, so make it 0.005. So that after 2 times that, it hits [INAUDIBLE] creates impact, and we want 20 of these.

Now, obviously, we'd need to run this for a longer duration, so that we get the equilibrium. So what I'm going to do here is I'm going to press OK. I'm going to create a new sub case, and we're going to not include the impact v. We'll include g, and this gives me the ability-- or you the ability to go in here and specify a smaller time step like that and 20.

So when the first subcase finishes with the impact and rebound, it will carry on to second subcase. Now, obviously, this takes a significant amount of time to run, up to 10 minutes or longer, depending on the number of elements it creates, so I'm going to go and show you the-- which I've done one already with results, as you can see here.

And typically, you want to see two things here. The first one we want to see here has the equilibrium has been achieved from the impact. So the way to do this is, you right hand click on x, y plot. Click on New, and what we can do here is we zoom into here.

We pick a point, which is about there, and step one, step 71 displacement, look in the tz direction like that and show x, y plot. So that's [INAUDIBLE], and you can see that it deforms, and it achieves equilibrium around this point here, 108. That's it, so 108. That's perfect.

And then what we can then do here is close the dialog box down. Right-hand click on Results here. Click on Edit. And then go and pick the last time step, which is this one here, 71. Let's have a look at displacement first. And the form options is always actual. So we look at displacement deform options. Press display.

You can see here that it is my permanent deformation, which has been achieved here. And then at the same time, I can change the results to Strain. And you can see here, we have 3.5% strain in the model. So that's less than 10%. And then finally, what we can do here is I have a video, but I won't show you here. If I cancel this.

And this is pretty cool. What you can do here is you right-hand click on Results, and you have Multiset Animation Settings. And you set the time 1 from the beginning, and you go all the way to the bottom time step. You look up animation options-- user half. So what happens is it lowers it, and then it starts all over again.

Now, this can take-- you could create an AVI. I have done that, but I can show you that in a moment. But let's have a look what happens if you want to animate it. Now, this one can take up to 30 seconds to get the animation ready. But the animation inside a non-linear analysis is true. It's not virtual. It basically shows you exactly what is happening to the model.

You can see the bottom of my screen. That green needs to go all the way to the right before we can see it. So we'll just give it a moment. Why not take a sip of water? Ah, there we go. You see the impact is sufficiently high and causing the concrete block to continue hitting the hoop. And now you can see here, after the rebound, it carries on going back up again.

And that is showing me my permanent definition. There you go. Impact velocity causes it to go down, and then you can see it. So it's pretty powerful on what you can achieve from inside Inventor. And doing this in real life, you're probably going to damage their hoops. And if it doesn't work, you'll have to do it all over again, and it's not pretty safe.

So if I'm going to press OK here. And then I'm going to stop the animation by right-hand clicking here, Stop the Animation. Let's go back to my PowerPoint. And as I said before, the next slide here, this is when I hit the AVI button. And this is type of AVI you can create and embed it in your PowerPoint report to show you what is happening. This is showing me displacement results. OK.

Right, now, this takes us to our final example. And that is based on Euro EMC Products based in the United Kingdom. And they are involved in the business of supplying high-security blast doors to the defense military, the government, anybody who wants to have valuables protected from the outside world. A typical example would be like a missile, a rocket, hitting into the door, and they want to make sure that the rocket doesn't go through it and everything inside the room in this case is safe.

Now, imagine doing that in the real world is not sustainable. And where would you get the rockets from? It's noisy. Again, hence the reliance on virtual testing. Again, the key behavior, or the key information required, are two things. One is the nonlinear material behavior. And secondly, of course, is a blast load and its duration.

And again, we have to go through the same simplification process and remodeling. And in this case here, the client suggested or decided to go down the a simplified solid model. So we've gone through three different scenarios. We've gone through a simplified service model in the first example. We've gone through a simplified solid assembly in the second example. And the final example, we're going to take a simple solid for the door.

And again, we have done the elastic/plastic. We have done the plastic also based on design data. If you don't have design data, and it's difficult to get hold of, then you can simulate the worst-case scenario by having 100% plastic. And this is the case what we have done here. So this may not happen in the real world. It may not be as bad as this, but this is a worst case. If it passes here, it will pass in the real world. So that's what we're going to do here.

And also, then we have the ability to apply a dynamic load, like an impulse. So here is a three-millisecond impulse. And then after 3 milliseconds, it goes back to 0 again, which means the load has come off. And that's what we're going to define. And also, we have the ability to define how many output sets we want to have, 10, 20, or 30.

But the key information is this. You need to have a duration long enough to achieve maximum deformation. And you can see by that by the curve. If it's still rising, it means it's still increasing the deformation. So we need to create the curve and see if the maximum definition has been achieved. And that can only be achieved by having this duration long enough.

This is absolutely brilliant because inside in Nastran, we can have objects, which almost have very, very high strains. That's almost 86% strain and permanent definition 709. And that is very difficult to do in the two examples I showed you earlier. So hence the reason why I want to show you how simple and how easy it is to set up explicit dynamic studies. So let's have a look at the example inside Inventor.

OK, so let's go to the blast door. OK, so you can see here it's a simple component. We have a split faces where it's restrained. I'm going to apply the load onto the side here. So let's just do that. OK. Right. So like the previous examples, we're going to go and change the analysis type to explicit dynamics-- this one here. I'm going to press OK. And then before we do anything else, let's do the material 355, the glass what we're using.

And because we can't get hold of data, for example, we're going to simply assign a "make it worst case" scenario. So we're going to go into there. Type in 0.5 or 0.1-- anything higher than that one will carry on going. So if we have an 80% strain in this case, it will carry on at 355. So we've got a flat curve like that. So now that's been defined.

The next thing we can do here is we can simply go and put the constraint and pick that fixed. And then on the other side, we're going to apply a blast load, which could be from a rocket missile or any other foreign object. And here, we need to define the load, which is going to be 2 e to the 8. Go into here. Define new table.

And we're going to specify the impulse duration. So time 0 second is going to be full load. It's a 3-millisecond duration, so we go and type in 0.003. And then we will drop it down to 0 after. And then we're going to specify 0.005 milliseconds. And there you go. So if it's going to take longer than 5 milliseconds-- 10, 20, 30-- it'll carry on at 0. So that's been defined. OK.

And the next thing we're going to do here is we have something called here, well, mesh settings. Let's just put a default mesh. Let's make it diagonal. 150. Linear. And press OK. So we created a mesh. Remember, if the mesh is smaller, it will take a lot longer to run in the explicit dynamics. The other thing which we need to be aware of, if it's a small duration, it run quicker. If it's a long duration, it will take a lot longer to run. That is where we specify the dynamic setup.

So we want to specify how many output results do I want to see? Let's say 30. And what is the duration? Well, the impulse load is 3 milliseconds. We can have it to 30 milliseconds. OK, so what we'll do here. And then we press OK. So the longer the duration, the longer it takes. The more the mesh, the longer it will take. If I press OK.

And the one thing I like about explicit dynamics, you can actually do a data check. And this data check gives us the ability to check how long it may take to run this type of analysis. So OK, so that's fine. So what we can do now is we can go into here. And that is-- let me expand it further. Estimated Wall Clock Time-- 2, almost 3 seconds-- sorry, 3 minutes. That's how long it'll take.

If I now go back in here, and I go and refine the mesh and make it, let's say, 50, which may be required, we'll keep the durations the same. But now if I do a data check, before it was 2 minutes, 40 seconds. Let's see how long this will take.

OK. Before I press OK, you can see down there, it's going to take 60 minutes and 28 seconds. So as I said before, just be aware of the mesh sizes and the durations. So press OK. Now, obviously, I'm not going to run this for 16 minutes. What we're going to do here is I'm going to show you results from the one we've done before. OK, then here it is. And right-hand click Results. Click on Edit. And we look and look at the last one.