Up and Running with Inventor Nastran: Tops Tips and Workflows

WASIM YOUNIS: OK, welcome to the "Up and Running with Inventor Nastran, Top Tips and Workflow Session." We're going to go through four different examples to demonstrate Inventor Nastran's best practices with some top tips and workflows.

The first example is going to be based on linear analysis using a spreader beam example. The second example it will be based on the automated impact analysis using a drop test as an application. The third one will be a nonlinear transient response, or NLTR, using a blast load as an application. And the final example will be using explicit analysis using again a drop test.

So let's have a look at the first example around linear analysis. So the example I have chosen is a spreader beam. And we want to simulate the lifting scenario. And as you can see here, the spreader beam comprises of box sections and four sort of pad eyes, or lifting eyes, or in some places they call them air monkeys.

So the first tip on this example is that if you have components that are welded together, I suggest you combine them using derived parts or substitutes. This will help to reduce the number of contacts created. And then it will also help to make the run times faster.

The second tip is any component with a ratio of 1 to 50 thickness to length ratio should be idealized with shell elements. In this case, we will use the box sections. And we will use rigid bodies to simulate pin connections when components are meshed using solid elements.

Solid elements have no rotational degrees of freedom. So you can see here we have a shaft. And by applying rigid bodies at either end of the shafts, we can see the color contour that it is behaving like a simply supported beam. This is one way to simulate a simply supported beam shaft or any components you want using rigid bodies.

The fourth tip is to always use offset bonded contacts when using shell elements, as they have 6 degrees of freedom restrictions. If you were to use a bonder contact, then your rotational degrees of freedom will not be fixed. They will be free to move. So you may have more like a hinge connection. So I suggest every time you use a shell element, always use offset bonded contacts, instead of bonder contacts.

The fifth one, if you have failure in your Nastran software, the most typical one is the E5000 warnings, then I suggest you can either use grounded spring elements to stabilize rigid body motion. Another phrase used in the other FEA world is weak springs. And this will hopefully stabilize your model without any errors.

Then also, the example I'm going to demonstrate in the next couple of minutes is that we want to be able to simulate slings. By four slings being lifting the spreader beams, what we want to allow pin connections on either side as if it's free to rotate and move. And the way we're going to do that is to use rod elements, as they have pin connections at either ends, which will allow rotations.

So this is the example. As you can see, the result what happens when you try to lift a spreader beam using chains, ropes, or any other mechanisms, you can see how it deforms. So this is what we're going to go through. And as I go through the workflow, I will give you some ideas indications of best practices.

So let's just go straight into Inventor. So as you can see here, we have the spreader beam. And one of the things you can see here if I zoom in, one of these components you can see here has already been simplified into a single component because these washers on either sides are welded. So we have a substitute. So this is the primary-- you can see it-- as an assembly, separate components, but we'll go back and use the substitute.

So that has already been simplified. So all the pad eyes are essentially a single component. So let's go into Nastran.

OK, so once we are in Nastran, we are basically going to idealize these components. The first one I'm going to do here is I'm going to use-- I've already got the idealization defined. So we're going to copy it from the model tree.

Now, when I click on Solid 1-- OK, let's just edit that-- you can see, it's already defined. OK, it's going on to a different screen. There we go. You can see it is already defined the pad eyes. We've got four selected. So that's solid elements.

Now, we're going to define these box sections with shell elements. So we're going to go and define a new idealization. And down here, we're going to pick shell elements.

And we know the thickness is going to be-- well, 6.3, I'll cancel that for a moment. I don't need to cancel it. We can go in here, and you can see 6.3. So let's define 6.3 mm.

I'm going to move this to one side here. I'm going to now define the shell elements. And you're going to go and pick the box frames.

Now, when I pick one of these surfaces, it only picks one surface. So I'm going to delete that. And I'm going to create a face chain.

So we're going to pick that one. OK, that didn't work. So let's delete that again because I picked the wrong one. Here's the face chain we want. So let's try again, second time, 1, 2, 3, and 4.

So basically, what you see there is basically picked all the tangent surfaces. So we're going to define shell elements. Because I only pick the surfaces, it will only pick the surfaces, not the whole thickness as well.

So we're going to press OK. And the next thing we'll do here is I'm going to generate the mesh to see what it's done basically. So let's have a look. So we'll use the default mesh size. OK, I know the mesh is pretty coarse. We're not so much concerned about the mesh yet.

So one of the things I want to show you here-- if I get the view right-- there is a way to check the shell thickness of what is going to represent as an FEA model. So if I go and display the cross-section, you can see what happens.

You can just barely see it. The white line basically is inside. It's basically given a thickness. So the surface was used at the mid surface. But I don't want it to used at the mid surface. That is the external surface. I want the thickness to go inwards, not both ways as it's done here.

So how do we do that? We basically go back into the Shell command, or the Properties, and click on Edit. You click on the Advanced Options. And you can see here that's going both ways.

If you put a negative value, the thickness will go into the geometry. If you specify another value, it'll go the other way. So I'll put minus there, and plus sign will go outwards. So minus 3.5, which is half.

And then we press OK again. And let's see what happens. And you can see now the white line is on the border, which means the thickness is going inwards.

Now, we can get a better idea. Now, the reason why did not refine the mesh is because when you have a very fine mesh and you display the cross-sections, it can take a little longer to populate it. So now we're going to Mesh settings.

And let's just try something like 50 here. And then just generate the mesh and see what it looks like. There. OK, so what's happening here, we're populating it.

Now, you can see here, it's still not following this curvature here. So we're going to go into the Settings button. And we're going to activate Project Midside Nodes. So we're going to press that.

And this will follow-- the mesh will follow the curvature of the geometry. Now, so if we say Generate Mesh, and you'll see that the curvature-- there you go. OK, you can see it is following the curvature now.

So I'm happy with the mesh. Obviously, we can refine it further. But I'm doing this live. So I just want to make this run a little bit quicker.

OK, so that's that. So now we have the mesh defined, the materials already defined. And now let's apply the load.

So the loading has already been defined. So I'm just going to copy it from my model tree. So we're just going to pick this load here. And I'm going to drop it onto this load here.

So we're copying it. So let's see what the load is. So if I right-hand click on here-- and obviously, nothing's been selected here. So I'm going to use the other one. So let's cancel that one because that was blank.

So we'll pick load 3 instead. Where's it gone? There we go. Let's copy that one.

And we'll try a second time round. And let's see, OK, this has got four faces pre-selected. We have total force of 20,000 newtons. And you can see them. There they are, one here. So that's all the load being simulated.

Now, what I'm going to show you here, first of all, I'm going to-- obviously, it's been held by 4 chains. I'm going to just do four pin constraints, which allow rotation. So let's pick one, this one, pin 1.

And we'll say, click on the New one. So that'll create one pin constraint. And then we'll pick Pin again. And I'm going to go all the way around and pick four pin constraints so that it allows the rotation.

And then we'll do this one again. So click on New again. Just be careful that you pick the Pin constraint again. Otherwise, by default, it will be structural, which is not what we want.

And then we'll go again and pick New again. And this is the last one. And now we have four pin constraints.

OK, so I think we have the loading. Now, the one thing left here to do is the contacts because the white lines, you can see there, the thick white lines represent that the geometry is not connected. Now, typically what would happen is we would always use automatic contacts.

Now, automatic contacts usually works if you are using solids. The other option is use manual. But then again, this can be pretty tedious because you've got to go and pick all four sides.

The best way of doing it is we can use the Solver Contact. This is a very common option when we are doing shell models. So I'm going to go in there, pick Offset Bonded, not Bond, Offset Bonded. And we'll press OK.

Now, you're not going to see contact pairs like you would normally see when you create automatic. So it will create contact between the pad eyes and the box sections once I press Run. So what we're going to do here is we're just going to press Run. This shouldn't take too long.

OK. And what you'll notice is the deformation obviously is not a true representation. So I'm going to go and click on the Options here. And we're going to go to Deform Options. And I'm going to say, let's represent it as true representation, actual. So we don't have it--

And then we're going to say Displacement values here and press-- now, I'm going to press OK here. You can see the value here. It's very, very small. So basically, what's happened here is that all the loading-- no load has been transferred across the box sections.

It's because a pin constraint is held in position. It's not moving in or out as you would expect in the real world, as when you pull it up with springs-- not springs, cables, chains-- then you expect the spread of beam to tilt inwards. Now, obviously, there's no single way of doing this. What we have to do here is we got to do a little bit of more work to make it behave like the real situation.

So if I go back and press Return, the first thing I'm going to do here is I'm going to delete the constraints we had created, first of all, because they are going to be irrelevant. So we can remove them. Now, because solid elements don't have any rotational degrees of freedom what we have to do here is because we're going to create a beam element, a rod element to be precise, from that point to that point.

Now, once we have a point in space here, that point then needs to be connected to the pad eye. So how do we do that? One of the ways to do it is we basically go in and specify a rigid body. Rigid body, first of all, you select the dependent entities. And then we can simply pick Point at Center. Then it creates a point in the middle. And that point once connected to the beam element will then be connected to the pad eye and then always will have rotation degrees of freedoms from the rod.

So now, we're going to repeat this four times. So I'm going to click on Next here. And then we go to the next pad eye. I could have these prepared, but I think it's a lot easier. You can see how simple it is and how quick it is.

So that's done. So we'll go to next. You don't need to create four separate connectors. You can have one connector, and you can have four of them defined in the same dialog box. It just makes it clean.

So if I go into here, you see that the point of center is already predefined. So it's pretty easy how it does that. Then we go to the next.

And we're going to go in here. And then that's it. So you don't need to specify Next. We go straight in and press OK. Now, I have four rigid bodies connected.

Now, the final task is to now connect all four pad eyes at the top here, representing for slings. So now, we're go into Connectors. And we're going to use rods. And the only value we need to specify is this area.

So I'm going to go in there, specify an area. And then the same way we did the rigid bodies, we pick that point there. Zoom into here. And then there's your first sling, or first rod.

You go Next again. Pick the top. Zoom into here. That's the second one. And we'll repeat that one for the third and fourth, and finally, the last one.

The only thing left now here is we're going to hold it at the top. So we're going to fix it. OK, so I think everything's predefined. We've got the four slings. And I think we are now ready to run this.

So I'm just going to press Run. And let's see what happens. Again, it shouldn't take too long.

Ah, it's come with some red text, which is not good. It's failed. And if we look at the E5000 connection, it's going to bring this green back here. It basically is one of the most common errors within Nastran.

And it refers to that it's not stable. It needs fixing, whether there are more constraints or any other parameter. But the trouble is we don't-- this is how it behaves in real world. I can't restrain.

Now, one of the things we can do here to make the model stable so that it runs successfully is we can create so-called weak springs. It's a bit like having a guy leaning against this spreader beam as it's being lifted so that it doesn't swing all over the place. We're going to create grounded springs, because the quickest way to create springs.

And then if you pick the Advanced Options, now K1 is in the direction of x. K2 is in the direction of y. And K3 is in direction of z. So we're going to pick on stiffness. We can specify small value in the x and the z. But no value's defined in the z direction.

And what we can now do here is we're going to go around the four corners. Pick one point here. Click Next. And then down here, I'm just going to repeat this and click Next. And the last one we're going to do here is-- there we go.

And now, we have attached four weak springs in the four corners to stop it swinging. And now, we can try it one more time. And what I'm trying to establish here is the behavior of the spreader beam represents reality.

So we're looking for a smiley face of the box section in essence. Let's see what happens. . Excellent there we go. We have a smiley face.

So what we can do here is I'm going to hide the CAD body, the connectors, for example. So there's the slings. Now, if you think the slings are having too much deflections, you can increase the area of the rods to stiffen up the slings.

But we're only interested in the values in the actual spreader beam itself. So I'm going to just go here. Let's just create a view like this to see what-- I think the one-- this is probably a better view. You can see how it's coming inwards. And now, what we can do here is-- the deflection is not true scale, it just showing us how it is going to deform, in which direction.

And now, it's going to start the animation. You can see how it works. So you can see the pad eyes are actually pointing inwards. And it sort of deforms. And now the results are a lot more realistic compared to our first model, which didn't have any displacement in the actual spreader beams.

So hopefully-- this was the first example. We can go through stresses. It's the same thing. But the most important one I want to demonstrate here is the smiley face of how it deforms.

So now, let's have a look at the second example. Let's stop the animation for a moment. OK. Not this one. OK, let's go to the PowerPoint. There we go. OK.

Right, so let's have a look at the second example. This one here is more to do with the drop test. And we're going to use a special type of analysis inside Inventor Nastran. It used to be called Automated Impact Wizard. But now it's called Impact Analysis because that's what it's designed for.

And you can see here we have a ball dropping onto a very thin channel. And to speed up the analysis for the demonstration purposes, I have modeled the channel as a surface model because it's a lot quicker to run. And also, to help us with the runtimes, I have moved the ball from a height closer to the target of the channel. And then we can then define the initial velocity using the formula on the screen.

One of the things we have to define in the Automated Impact Wizard is a sketch connecting the projectile to the target body using a sketch, as you can see as down here. And that sketch needs to be connected to the mesh on both sides. And we can achieve that using the Point mesh control, which is probably very rarely used in a mesh control. But this is one of the benefits, one of the applications I've seen where I've used it is to basically get the sketch to connect to the mesh on both sides. Use the Point mesh control, which we'll demonstrate in a moment.

Also, when you have multiple surfaces, as you see here, I recommend that you use a Continuous Meshing button. This allows you to connect the meshes on each adjacent surface of your component. And this basically means that we do not need to create manual contacts or automatic contacts. Again, having contacts basically will increase your run times.

The 10th tip is to always specify a contact tolerance value for models with high levels of curvature, anything which is round. For example, in this case here, we have the ball. If we don't have it set to Automatic, then it may not have contact with the channel. So recommend to put a value in there.

OK, so now let's go straight into Inventor. OK, and we'll have a look at the Impact wizard. OK, so you can see here we have created a sketch in the Assembly mode, just basically connecting the two parts. Make sure you don't have any gaps between the ball and the channel in this case.

So we're going to Nastran. OK, so the first thing I'm going to do here is we're simply going to change the analysis type. So let's go into Edit. And we're going to look at-- there you go-- Impact Analysis.

Basically, Impact Analysis is the automatic version of nonlinear transient response. So it is nonlinear transient response, but obviously it does all the automation in the background. And it is designed for anything to do with-- if you are doing an impact analysis, then this is the way forward.

OK, so the first thing we're going to do here is let's just idealize this. So I'm going to pick the ball first here, right-hand click, and see what it's doing. Obviously, you can see here it's only selected the ball here. You can see it here.

And then, rather than me creating a new shell idealization, I'm going to drag it from here and take it to the top. And then we can have a look at what it's doing. So if I then right-hand click on Shell and click on Edit, you can see here it's basically already predefined with a thickness of 3 millimeters for the actual channel itself.

We're not going to be so much concerned about which way it's going in this example. We'll assume that the surface is representing the middle of the component.

OK, so we go down to a Mesh settings. And here, what we can do basically is let's pick a value of, let's say, 9. And we're going to press OK. I'll just show the mesh for a moment. You'll see what I'm talking about here.

Now, can you see the thick white lines appearing between the adjacent surfaces here? They are not connected. They may seem like connected by looking at the elements. But if I then click on Continuous Meshing here and then click on Generate Mesh, you'll notice the thick white line disappear. That indicates that you have basically got connected surfaces. So I'm happy with that.

The next thing we need to do here is, if I Zoom in here, you can see straight away that line is not connecting my mesh. And this applies at both ends. So how do we do that?

So based on the presentation slide I have shown two minutes ago, we're going to go into Mesh Control. And we're going to give it a value of, let's say, 2. But the most important part here is the two points.

Now, this feature is a new feature within Inventor 2024. Because if I now click on that, you had to press OK. Then you have to go and click on Generate Mesh.

I'm going to click Generate Mesh here. And you'll notice something what will happens. You see there is connected there, and it's connected there.

But what I'm going to do here is I'm going to go back to the Mesh Control 1 or 2. One thing you may not realize is that if you want to have now define another mesh control, you don't have to go and define a new dialog box or a new mesh control. I'm going to go in here. This is referring to the points.

And now, I'm going to pick that surface, which has been split, and that surface there. And I'm going to put 2 there. Now you see there, I have basically got two different mesh controls in the same dialog box.

If I then go and click on Generate Mesh, and you can see that is connected. That is connected. And I think we're almost there.

So the next thing we're going to do here is we're going to need to fix that channel. So I'm going to go and again, I'm going to pick one of the constraints, Fixed Constraint, and then drag that up here. And then I'm going to see what it is. And you can see, it's a fixed constraint on that piece there.

Now, we go with the final setting, which is the Impact Setup. So I'm going to go in here. OK, the first thing is asking for is that you want to be able to specify the projectile, which is this one.

Then you got to pick the sketch connecting the projectile with the channel. So you highlight in here. And then you want to see the direction of the projectile. And if you zoom in there, it's in the right direction.

Because I've moved it a certain distance closer to the target, that will generate initial velocity. In this case here, we can specify 10,000. No need to specify negative or positive because it's going to follow the sketch.

But one final thing, because it's a round object, Predict Curvature, you see that automatic. I will recommend you specify a value. And once you've pressed that and then press OK, then you can press Run.

Now, this will probably take a couple of minutes to run because it does create a lot, a lot of iterations. So what I'm going to do here I have one already completed. So if I'm going to activate that. Now, in Nastran once you open a file again, you need to load the results. OK, here we go.

And what I want to show you here is how the ball drops. Now, what you can do here-- and let's just probably go into Results and click on Edit. And I'm going to probably pick-- you see how many increments, how many results it creates by default. This takes about a couple of minutes to run.

I'm going to go and pick the last one for a moment. I'm not looking at the stress values. I want to see the displacement. I want to see how it deforms.

And then I'm going to go to Deform Options. And I'm going to pick Actual. When I'm doing this and you're flicking between the different increments, it's always best not to have the display active because if you are moving between the increments and changing the result, it takes a little while for it to update.

So now I want to press Display. And let's see how it behaves. There you see the red dashed line there. So you can see it slightly to one side.

And what we can do here-- you can see it now. And one thing I like about this process is that it's nice to see an animation. The animation will only animate this current time step.

So I'm going to cancel this. And I want to see as the ball drops onto the channel going through each time step, like as it would happen in real world. So the way to do that is go into Results, right-hand click. Click on Multiset Animation Settings. OK.

And what we're going to do here is it goes from step 1 to step 105. I want to see displacements. I want to see actual. And I think this is it.

So then what we can do here is press Animate. And this will take less than a minute to generate. So we'll click on Animate.

You can create a video as well. So I'm simply going to make it look like this. And then let's press Animate and see what happens.

So it is actually going through a lot of data. And it gives me some time to take a break from talking. Oh, that was a bit quick. Spoke too soon, I guess.

See what's happening? It's hitting it. And what the Impact Analysis does it actually will determine when it's going to hit it and then also the rebound, when the ball-- it won't go all the way back. If you want to simulate the ball going all the way back from the rebound, then you would probably run it as a nonlinear transient response.

Or if you want to do something different here, because this is a full spline circle, if I go to Animation Options here, let's do Half. Because it'll hit it, then it'll go back, and then do it again. Let's just try that once more.

I should have actually picked that before I hit the first one. But let's just see what happens. You can slow down also the recording as well by changing the value from 200 to a higher value.

OK, let's see what happens now. There we go. So hitting it. What I'm hoping for it to do is that when it goes to the end of its iterations I want it'll go back to 0 again and then drop it again. If you watch it very carefully, the ball will try to go back slightly. And then there, just about there-- there, then it'll go back to there. You see? It repeats there.

So what it does, the Impact Analysis will work out the point of impact and then the rebound. And it's a pretty powerful analysis. And this was linear materials, the first two analyses. You can define nonlinear materials so that you can actually then predict the perma deformation.

But the next two examples, we'll talk about nonlinear materials as well. So let's just stop the animation. Go back to the slide. And let's have a look at our third example.

So the next example is NLTR, or Nonlinear Transient Response, which is the manual version of the one you saw before, which was the Impact Analysis. And the example, or the application I'm going to demonstrate is a blast load. You'll notice that my examples are very, very simple because I thought it's probably worth showing you a simple example. It runs pretty quick. And then it gets you a better idea of how simple, how difficult it is set up.

So this one is simulating a door being struck by a blast load. And the typical blast load would be a missile rocket or some sort of explosion, external. So in this case, it's a missile. It has no consequence on the workflow as the workflow will be the same.

Now, when we do a Nonlinear Transient Response Analysis, there is a lot more settings we have to go through unlike the Impact Analysis. So the first one, the most common one I get asked a lot of questions on is what is the dominant frequency value we need to specify? Because if you don't specify damping, the whole thing will just oscillate. Excuse me.

So the Dominant Frequency basically is the first mode of your modal analysis. So do that first. The second one, which is a value, which you need to specify is a damping value. The damping value you can obtain from an engineering handbook. It could be a value ranging from 3% to 5% for steels. But the engineering handbook will have a value you can specify. If you don't know, just specify anything between 3 and 5, or run multiple analysis and see if it has any impact on your damping.

OK, now there's a dialog box in there, called the Nonlinear Setup. If you open it, by any chance because you're curious, you will get this dialog box. And you can see in there, there are so many things you can change.

Now, as engineers, we are curious. I would suggest don't change anything. You only need to go in there if things are not working, and which I would suggest that you liaise with the forums, the Autodesk forums for help, or one of the experts from Autodesk. But there is no need to change any values in here. Just leave it.

OK, now, one of my favorite parameters is the NPROCESSORS. So you can change that to the maximum number of processors your machine will allow so it will run faster. So changing the value in here in the parameters will only be saved in your file.

So if you open a new part or a new file, then you would have to do it again. There is a way to change it for everything. But that's not covered here. If you have any questions, we can discuss that after the presentation.

OK, so this is the example we're going to go through. You can see here, when we're doing blast load, or nonlinear type examples, we are looking at two values. One is the permanent deformation. As you can see here, when the load has gone back to 0, it's still deformed to 59 millimeters. That's the permanent deformation.

And on the left-hand side image, you see the strain. And the strain there is 1.97%, not a lot. But it can put a lot of burden on your machines. It's a simple example. And we'll run it live, and you can see what and how it responds. So let's go back into Inventor. And again, we have a simplified version of a door, represented by a very thin surface.

OK, so what we have here is we have a material. There's the door thickness. We have mild steel. And we're using quadrilateral elements. So it's already been defined. OK? And it's restrained on the three edges. You can see by the symbols.

And the blast load, we need to define. So we have a value of a blast load, which is not constant. Now, I can go and define a new table. Or I can be more efficient-- didn't say lazy. I have one here, and I'm going to drag that table and put it on top of my blast load copy.

So when I go back to my blast load copy, you'll see that I have a table defined. So basically, we have a 3 millisecond blast load. If I do my Show my xy plot here, you can see here it goes for 3 milliseconds. Then it goes down, and then it stays off.

And then we want to find out what is happening to the model once the blast load has come off. This is where damping comes into effect. You will get oscillations. And eventually, it become stable. So dumping will have an effect after the blast load has gone. OK, so we've got the blast load defined.

So the next thing we got to do here is we're going to go into Damping. Now, before I do damping, I'm going to show you-- I've got Normal modes here. I'm going to go in there and activate that.

Same example, it's already been set up. I'm just going to update the mesh as it's-- I don't know why it's got an exclamation mark there. And then what we're going to do here, I can either upload the results if they're loaded. No, let's run it. It's pretty quick.

And when you run Modal Analysis, I have requested only one mode. Normally, it's the first mode, which you need. And the first mode, you can see there it's 59.66. Or you can get it from here. If I click on Edit here, and there, 59.66. So that's what value I'm going to specify.

And then I'm going to show you one more thing before I go back to my analysis. See there? I only requested the first mode. That's the only mode you need to define.

So let's go to Analysis2. Click on Activate. OK. So what we're going to do here is I'm going to go to Damping. You see when did the Impact Analysis, I did not have to define these. The more values you got to define, I guess there's more risk of you might make a mistake, or you might be uncomfortable.

So I'm going to go to Structured Damping. That's going to be 5%. That was 55.69, I think. That's the first one.

And then, let me click on that once for-- now you see a lot of values in there. I've been using this for a long, long time. I've never ever needed to go in here. The only time I've been in here is when I want it to run faster.

So by default, it uses all these three results to converge. You can basically use Work and Displacement and put values in there to make it go faster. But we're not going to do that. OK?

The other one is Dynamic Setup. Now this can be a little bit-- first, let's first define the time step. It's a 1 millisecond. OK.

And then how many time steps do I want? Let's see, if I say 100, you can see there, that's running for 10 milliseconds. So basically, we're running for 3 seconds. But I don't want to run it for that long. I'm going to say let's run it for 5 milliseconds. So after the blast, we have 2 milliseconds to see what it does.

Now, the more time steps you request, the longer it's going to take to run. So let's just try 50 for a moment. As long as it covers the blast-- I want to see what happens. I'm going to press OK.

And then one last thing I want to show you here before we press Run, if I click on Edit here, there is a lot a lot of parameters you can actually customize and change. But the one I'm going to change here is Pro. It's already been changed by me. So 16 is OK. By default, it's 4. And I think I've got everything set up.

One more thing I want to show you here, which I forgot to mention, is that I have defined the elastic plastic by linear material behavior. So that one, the stress goes beyond yield, it will start to deform. So we can find out how much deformation actually happens.

So I'm going to press Run. And we'll see how long this takes. So typically when you're running a nonlinear transient response, or like a blast load or an impact, sometimes what happens is when you look at the results, you probably still get vibration, which means that you still got to run it for a lot longer until the vibration settles. So you'll see that very clearly.

I'm just trying to find where the dialog box disappeared onto my fourth screen. So I'm just going to go and bring it back. Oopsie daisies, there we go.

And then hopefully, you see there? I'm looking at the time. It should be 5 milliseconds. Then it'll stop. And we're almost done. OK. There we go.

And the best way to look at, when you're doing these type of examples, is look at the xy plot, maximum displacement versus time. And if I click on that, you can see here how it's deforming. And you can see that it's probably going to start settling after a while.

So what I'm going to do here is I have got one completed already, which has run over a longer period of time. So I'm going to go in here, activate the one which has already been done over a longer duration. I'm going to click at Results and load the results. And then, I'm going to look at my xy plot to show you that-- there you go. You can see how it sort of smooths out. And eventually, the permanent deformation is around 59 millimeters.

Let's have a look at that. So now, when we look at deformation, we know that it's going to be true deformation. It's not a rebound effect, or it's not oscillating. So how do we do that?

I'm going to pick the last time step. And you can see there again, it's doing a lot of time steps, several hundred. Pick the last one.

And if I pick displacement here, 59.7 is permanent deformation. And then make sure it's by default. When you're doing nonlinear, it will actually pick the actual.

Now, if I press Display, you can see here that is actual deformation of the model. I'm not going to animate this. But you can see you got an idea how it works. It's basically-- that's a permanent deformation.

Another value when you do nonlinear, which is very useful, is the strain value. I'm going to go in here. Not that, one this one here. And we can look at strain.

And the strain value, typically it gives you an alphanumeric number. You simply times it by 100. That's basically 1.9%, which is pretty low.

Now, this leads to our next example. When you expect strains, let's say-- this is my opinion-- less than 10%, then doing it like this, you can do that with nonlinear transient response. But when you get a lot of strain, over 10%, then we will have a look at the next example. And we will recommend using explicit dynamics.

So let's go back into our last example. So this is again a drop test, but the mechanism, whether it's a blast load or a drop test, this scenario is still the same. So this example, we're going to drop a concrete block onto an aluminum floor. Now, as I've mentioned before, if you are expecting large strains, large deformation, as you can see here on the screen-- in this case, 28% strain-- then you should use Explicit Dynamics, not the NLTR, or Nonlinear Transient Response, analysis.

Also, in this case here, we will need to refine the mesh at the contact region. So rather than refine the mesh on the whole face, it's very common practice to split surfaces or component faces, where you can define a region to specify a local mesh control, as you will see here. And this one makes a huge difference when we do a nonlinear analysis.

If you had the default parabolic elements and run that, it will take a lot longer to finish. Linear elements are a far more efficient way to do a nonlinear analysis. It shouldn't have a huge impact on your results.

Again, we are not interested in the concrete block hitting the aluminum floor. So we can define it as a rigid body. It basically means that when it does a calculations, it won't work out the stress and strain energies of the concrete block, which means it'll be faster runtimes.

OK, now, in this example, we need to define the time steps. And then what we can-- and the way to find the time of impact in this example here is the distance between the flow and the block divided by 10,000, in this case here, will give you the time of impact. And that then becomes a value you can use to work out your time steps, like you see on the left-hand side. So this is how you work out the impact.