Up and Running with Inventor Nastran

WASIM YOUNIS: Morning, everyone. We've got a slight hiccup. Just bear with us for a couple of minutes.

AUDIENCE: [INAUDIBLE] better. If they say something else--

WASIM YOUNIS: [INAUDIBLE]

AUDIENCE: Stand at the bottom like [INAUDIBLE].

WASIM YOUNIS: At the back, so when this-- huh? And Tom is there. We're ready to start?

Morning, everyone. Thank you very much for coming to this first session. Just to give you a little bit of a heads up, I'm not feeling great. I think I've got the Las Vegas flu. So I might be taking a bit of a [INAUDIBLE]. But you can hear me, OK, everyone, yes? Can you hear me, everyone? OK. So let's get cracking.

Just before I begin, hands up if you've used Nastran before, less than six months [INAUDIBLE]. Now, this is brilliant. And who's been using it for a while? Oh, OK. You might learn something, I think. OK.

OK. So ideal class-- we're all absolute beginners, starting life in simulation. So this is the class to be. And I always get some experts who know more than me, allegedly. So I hope they will learn something from me, as well. That's the idea. But this is all very hands on. So I'm going to-- I'm not a PowerPoint person, but just to give you a gist of what's happening-- OK.

This is a big one. The class basically is to give you confidence in designing, to help you make better products so you don't end up overdesigning. That's what tends to happen. A lot of customers I've spoken to all over the world tend to over-engineer just because they can, and it's safer. That's the idea. So we're going to try to avoid that.

So the example we're going to go through is basically a lever, which is part of an assembly. This is part of a security door locking mechanism. Now, we then have to make a decision. Do we include the whole assembly, or do we just work on the single lever? That's the big confusion.

And what's this confusion? It's a dilemma. Because we, as CAD engineers, have every single detail inside Inventor, and it's easy for us to just click it, go into Nastran, and then press the Mesh button and hope it meshes. And then, you wait hours trying to get the results. And then, once you get the results, then you sit there and try to make sense of it. So this is what happens. As a CAD person, we then have to strip out everything and make it as simple as possible, and then work from that. If you're not happy with that, then start building detail. Work from bottom up, not from top down.

OK. So what we've got here, guys, is a bit of pros. So as a single part, it's a lot easier to set up. We have much less elements, and we don't have to worry about contacts. I don't like contacts. Contact gives a lot of headache for me, personally. And if you've been using Nastran, it is something we have to be very careful about, because as soon as you change the contact types, you get different results, and you start scratching your head. By the end of this collab, you won't be scratching heads. You will be experts just as good as me, I believe. No one's convinced yet, but we'll ask you that question again afterwards.

The only problem is, if you do the single part, because it's attached to other parts, we have to restrain it, which means you're going to over-constrain it. So the stress you will get there will be lot higher than what-- let me rephrase that. It will be higher than if you were doing it as an assembly. So what I tell everybody is to do it single parts. Once you're happy with everything, which-- we are going to go through the process-- then do it as an assembly to finish it off.

And what we're going to show you today is we will start from a single part, get an idea, get the results. Then, we're going to compare it as a assembly. And you will see there isn't much difference. So why bother with assemblies? That's me. You can carry on in assemblies. With assemblies, it will take longer to run. You have to take in contacts, and basically it just takes a lot longer to run. By the way, you have these as PDFs, anyway. So you don't [INAUDIBLE].

OK. Now, this is the $6 million question. When I get one set of results, do I believe it? How many people have just relied on one mesh result? There's no stupid questions. There's no right or wrong here, guys. Don't be shy. But basically, you have to run the mesh three or four times to see not the displacement, but the stress result changes. It's a bummer, but that's what has to go through the process.

Now, over time when you become familiar with the software, you may not do it three or four times. You may only do it twice, just to get an idea. You go from one extreme to the other extreme, and there is some benchmark value, which we are looking at just to make sure the stress value is something we can believe in. Now, inside Inventor, that's the only thing you can do. Compare the results inside Nastran-- there are other avenues we can compare. And that's what I'll go through with you guys, as well. OK.

OK. So this is the first example we're going to go through. So what we need to do is I've set projects on your machines with the help of my colleagues. So I've got some clever chaps at the back. So I'm going to carry on. If you are lagging behind, just stick your hand up, and then my esteemed colleagues will give you a hand. OK?

OK. Right. Is everybody at this stage of it? Excellent. So the first thing we're going to do here is-- well, you should all see that. Has everyone got that? And we're going to open the Exercise 1 file. So we click inside here, Exercise 1, Lever, and click Open. Now, just bear with-- oh, that was very quick. When I did it the first time, there was a bit of delay. So I'll give you a couple of minutes.

Has it appeared on anyone's screen? Still waiting? That was-- I've done it already once, so it's in the cache. Yes. Got it? Super duper. Are we all there, Chris, now? I don't want to leave anyone behind. It doesn't usually take this long. It's just because of the way it's been set up through FRAME system. But hopefully, your other files will come up pretty quick. Are we almost everyone? OK.

Right. So this is a very simple part, obviously. There's two reasons for that. I don't want to have long run times. Everything we're going to do this morning is live. I've not got any backup files, because it's very easy to set it all up. So if it crashes, which-- Inventor never crashes. But if it does, stick your hand up, guys, and then we can repeat. I was going to have saved files, but it's simple just to run it again, and very, very quickly.

Now, this example doesn't require any simplifications. It's simply going to go straight into Inventor and Nastran. Now, if you're using 2019, it's called Nastran In-CAD. If you're using 2020, it's called Inventor Nastran. Next year, it might be called something different. OK. Right. So we're basically going to run it as a single part analysis. We are going to apply the boundary conditions-- that's the terminology. We're going to apply the load and constrains to make it behave as if it's going to be a part of an assembly.

OK. So the first thing we're going to do here is I made a intentional mistake. No, I forgot to do it. Right. Let's go back into-- hang on. Now, nobody's gone into Nastran. So go back in 3D Model. Everybody there? I'm going to specify the material, OK? The materials are basically the same materials you use inside Inventor-- the Inventor materials library or the [INAUDIBLE] materials library. If I had carried on doing it inside Nastran, it picks up the same library. But it's better to actually specify the materials first. And we can modify them.

So I'm going to basically have mild steel. And we're going to change the values. So you can see right at the top there, it's generic. So I'm going to go in here, first of all, and make sure we pick-- let's just pick mild steel. But I'm not going to use those values. I'm going to change them.

Now, you have two choices. You can change them here, or you can change them in Nastran. It's probably easier in Nastran, but let's just do it here. At least you can know to find and click on that little icon there when it comes up. There we go. OK. And mild steel's bolded, so click on the little tip against that one to modify it. Let's move this dollar box to one side. Change the name, first of all. Let's call it Steel DP1.

And because I'm from the UK, I'm going to use metrics. So I do apologize for using metrics. Now, to change it to metrics from the imperial system-- where the heck is it? Is it before this? It's there. OK. Right. Just bear with me, guys. You want to press OK first. There it is. Set display units-- and metric. I should have done that first. Is everybody there, more or less? OK. If I didn't do that, when I changed the materials, they'd all be imperial. OK. So now, we'll click on the modification for steel. Go to Physical.

Now, there is a lot of information there. You've got thermal information in there. You've got physical properties there. We don't need to change the thermal properties. OK? We're just going to change the mechanical properties here. OK. Well, that's interesting. Do you all get 0 in yours? OK. So that's not what I wanted.

OK. Just bear with me a minute. Let's get rid of all that. Change it back to the original state. Let's just pick-- is mild steel anywhere again? Just go back, guys, and we'll do it in Nastran. It's a lot easier. Have you all specified mild steel? OK. I'll just give everybody a couple of minutes. OK. Once you've got it back to mild steel, go to Nastran. You'll get a-- press OK, guys. Everybody there?

OK. So now, what we're going to do here-- we're going to change it here, because it's a lot easier. So I'm going to -click where it says mild steel. That's better. So I'm going to change some values, because we can. So the e value-- the [INAUDIBLE] is the most important value-- if that's different, you'll get different results. That's the big one. So we're going to change the value from 2.2e to the 5 to 2 e to the 5.

And then, the portions ratio-- 0.29. And the yield material here-- I'll explain that one afterwards-- and that's it, guys. We don't need to change the names. Leave it. OK. Are we all there? OK. Right. For the e value, it's 2 e to the 5. The portions ratio is 0.29. And the SY is 200. These values will have an impact on the results. And I don't know what you think, but I think it's a lot easier to change values here rather than what I was trying to do. OK. I think we're ready to-- right.

OK. Right. So next thing we're going to do here-- so what you notice here, guys, is you have an analysis tree. That's the most important thing. And underneath, unlike Inventor, you have a model tree. The model tree basically is a copy of what happens in the analysis tree. If I wanted to run the analysis with different load cases, I have three or four load cases on the model tree. I can drag and drop, and have different subcases and different analyses. It's a backup. It's a bit like our Inventor's templates, but the difference here is this is local. You can't use that model tree outside the part file. It's just inside there.

OK. Guys, remember-- if you are running behind, just make sure you stick your hands up. OK. So what we're going to do here-- you can see straight away-- just before I begin, how many people are here familiar with Inventor [INAUDIBLE]? OK. So the first thing we're going to do here is if I look at it square on, we have a pin here in the assembly file. But I don't have a pin here now.

So what we're going to do here-- we are going to create a special pin constraint similarly as if there's a pin inside it. So we're not going to fix it. We simply are going to say that circular hole can actually rotate around a pin, which you can't see. It's called a pin constraint. So in 2020, you can click on the arrow there and pick Pin.

And what we'll do then, here, is if I spin it around and move down our box to one side-- and if you look at the screen now, everyone, under Coordinate Systems, I only see part 1. It's dragged into Coordinate Systems from my Inventor part file. As soon as I pick that circular face, it's going to create a local coordinate system on that circular face. So we go up in that circular face there. And when we do a pin constraint, we actually restrain the radial direction, and also the actual direction.

And I would suggest you change the name to something meaningful. Let's see-- pin constraint or something. I have a bad habit of not naming it. But when I have lots of constraints, I'm back to clicking on it just to make sure which one it is. So we have one constraint now. Actually, the only thing I can see there is a symbol.

Now, if you want to change the number of symbols on there, what you can do here is if you want to double-click on the pin constraint-- and then, down here, you can see you can change the density. Click here, and click on the spectacles down there. You can make the size bigger. There you go. You can see how the tip of the arrow is pointing towards the circular face that's normal to it. OK.

All right. So the next one we're going to do here-- now, because we don't have the full assembly, I'm basically going to restrain it on this side. And when we do FEA, we're looking at the worst case scenario. So we're going to actually put the constraint on the far side of the slot. So we'll do the same thing again-- pin constraint, and pick this circular face here. And you see there, you've got Coordinate System 2, which has its own origin. And we'll pick fix axial, fix radial. Again, you can have change the density. You can even change the color. So this is a different constraint, and I'm going to rename it to Slot Constraint.

So the next thing we're going to do here-- we have a pin pushing against this slot here. So I'm not going to put another constraint. I'm going to put a bearing load to simulate the effect of a pin pushing against it. OK? So in the loads command, which is next to the setup, next to the pin-- and let's move to one side-- and the type from force to a bearing load. Now, a bearing load is like a force. But basically, it's more accurate trying to simulate a pin pushing against a slot. So every time you want to specify a force inside a hole, always pick a bearing load. OK.

And now, what we need to do here-- first of all, let's pick the face. Now, as soon as I pick the face, we're going to change a couple of things here. The first thing we need to do here-- and it will help if you put the value in there first. Now, the value is going to be in the minus x direction. And we're going to put a value of minus 30 newtons.

And if you take the spectacles, you see what's happened to the arrows? They're all normal to the circular face. I didn't want that. I want it to go in the x direction. And I'm going to change components. Now, once you've got that, you can press OK. Now, we've done all the tedious bit. Now, it's the fun bit. Everybody there? OK.

So the next thing we do here-- I can run this analysis. As best practice, it's always a good idea to look at the mesh size-- which size you want to start off from. So if you click on where it says Mesh Settings, it always comes with a five or six digit number. It never comes with a nice, one significant figure. Let's change the value to two.

And then, if you want to have a feel for what the mesh looks like, you can click on Generate Mesh. If you want-- in this case here, I'm going to press OK. Then, it will come with [INAUDIBLE]-- OK. Now, if you want to change the color of the mesh color, you can click on that little blue box. And then, do you get the same thing I'm getting? Thank you very much.

And there we go. There's the mesh. Now, is it a good mesh? I'm not really bothered. You shouldn't be bothered, as well. We're going to go through three different settings. And then, you'll get an idea. What we were trying to do here was trying to get an idea of whether the mesh has any impact on our results. So once you've got that, go ahead and press Run. This will probably take half an hour.

And then, you get lots of text appearing on the left-hand side, and you get lots of warnings. Ignore them, honestly. I can switch them off as well, if you don't want to see them. They're not there-- they're just there to scare you. I've got 18 warnings. Now, if you've been doing this for a long time, you may have hundreds of warnings. You may have thousands of warnings, depending on how big it is. Don't let that put you off, honestly. And if you want to see me after the class, I'll show you how to switch it off. Just like Inventor, it's a black box. Everything's correct. OK.

Right. So we are going to get a set of results. The first thing you need to check is where it's going to be. Now, as an engineer or a designer, if it's your parts or your components, you'll have an idea of where the stress is going to be. The big problem is if that stress is in a different location to what you had expected. So somebody is not right. Normally, it's the software's fault. OK.

So we get a stress value of 8.693. It's a very small stress value, because this thing runs for years and years. And we're going to do a bit of fatigue if we have time towards the end of the class, anyway.

OK. So what we are looking for here-- I'm not so much concerned about the mesh. I want to see that when I'm applying my boundary conditions, and my constraints, and my loading--

AUDIENCE: [INAUDIBLE]

WASIM YOUNIS: Ah, OK. Right. Just a minute, then. OK. So this is a load dialog box. And it's minus 30 newtons minus 30. And I think what you need to do here is-- this is the value you need to change. That needs to be components. Not normal to face-- these components.

Anyone not got the load? No? Are you OK? OK. Right. Once you've got that, click on the rear. Run the analysis, just to make sure if the people have not run it. And for everybody else, you can just simply click on [INAUDIBLE] here. And we're going to do the fun bit. OK. It's always hard. Try to keep up. Are you [INAUDIBLE] far behind?

AUDIENCE: No, I think we're fine.

WASIM YOUNIS: Oh, OK. Nobody's-- so the big two eat the five. 0.29 for unit portions ratio, and 200. I wouldn't worry too much about this, because it'd be nice if we could compare it. But everybody got a result of some form?

So if you click on a button called Animation when my results come up-- can you see here? Click on Animate. Now, it doesn't deform by that much, what you see on the screen. That is scaled by 10%. It's always nice to look at results. So if you just click on Animate, guys, this then gives me an idea if the loading seems to be in the correct direction.

OK. Now, if I had it deformed as actual, it won't look as nice as that. It's like flashing then. Are we all are keeping up? Is anyone not at this stage? With hands-- that's a good sign. OK. OK. So just unselect Animate again.

Now, we're going to go through the laborious task to change the mesh at least three times to check whether the stress in the high area is going to change. The magic number we are trying to compare is 10%. In the real world, it's never going to be 10%. It's probably going to be 5%, 3%, 2%. If you get a value close to 9%, then maybe you might want to change the mesh the fourth time, just as a sanity check. OK?

So how can we do this? The easy way to do this is to write and click on Analysis 1. And you have a button called Duplicate. It'll copy everything. It'll copy your constraints. It'll copy your loads. And if you do it at least five times, you'll have a massive tree. So it's not ideal, from that point of view. So I'm going to show you another method afterwards, which is as good. OK.

So the only thing we're going to do here is we're going to click on Mesh Settings, and we're going to change the value to 1. And just click OK. Now, this is going to change the mesh everywhere. It's called global meshing. That's the terminology used in the [INAUDIBLE] world. [INAUDIBLE]. 1-- I'll bring it back up again for-- so when you copy it, it's copies of the 2 millimeters. I've changed that to 1 millimeter.

Now, once you've got that, click OK, and it'll take a little bit longer to run. And I've still got 17 warnings. OK. Distress value has slightly increased. And I've worked it out. I think it's about 7% or something-- still less than 10%.

So what we're going to do here is I'm going to run it again once more, but I'm not going to change the mesh everywhere by 0.5, because if you think about it, the stress is only in one area, and that's what we're comparing. So we're going to do it slightly differently this time. I'm going to click on New. OK. Analysis 3-- and then, I'm going to press OK.

And what'll happen is it's a brand new analysis. It's not created any copies. I'm simply going to drag and drop items from a model tree. This is my preferred method. If you were to do different load cases and different [INAUDIBLE] cases, this is what I would suggest you do. OK? So you've got to be careful here. Ignore the copy ones.

So if I-- watch me here. I'm going to pick a solid one here under the model tree. Keep your left mouse button pressed, and drag that side one onto Idealizations, and it copies it. Then, drag the constraints onto the constraints. And then, I'm not copying. I'm not using the copied ones. And then, one load, which is down here-- constraints on the constraints nodes under Loads, and idealizations on the Idealizations. So what you should all have is basically [INAUDIBLE] idealizations, the same load, and two constraints.

AUDIENCE: Did you take both the [INAUDIBLE] and the [INAUDIBLE]?

WASIM YOUNIS: Sorry?

AUDIENCE: Did you copy both the [INAUDIBLE] and the [INAUDIBLE]?

WASIM YOUNIS: Yeah-- have I? Yes. And if you're confident, just run it. Oh, whoa, whoa, whoa. We've got to change something-- the mesh. Who's run it. You should never believe what I say. That wasn't intentional. I just forgot. So I'll click on Mesh Settings. And now, because I didn't copy it-- I'll wait for one or two guys. Let me know when it's completed.

For everybody else, change their value to 1, because I'm not going to change everything to 1. Or below it-- sorry. So pick one. And that is exactly the same as my Analysis 2. So what I'm going to change now is something called Mesh Control. OK. So that's the same as my number 2 analysis. And can you see something called Mesh Control? Click on that. And this is what we call raw code mesh control. I can pick a point. I can pick an edge. I can pick a face.

And if it was an assembly, I can have different parts with different mesh sizes. Because a single part here, I don't have the option. This is where the part option appears down here.

So I'm going to click in this face selection box here. I'm going to move this to one side. I'm going to pick the fillet here. OK. And now I'm going to change the 1 to-- let's make it 1/2.

Now nothing happened. Like Mesh settings, when you click on the dialog box, press OK, it generates the mesh. With mesh control, it doesn't generate the mesh. So if you run it, it hasn't done anything. I can't see the mesh change anywhere. So always as best practice, click on Direct Mesh every single time before you run it.

Is everybody at this stage? Anyone-- you [INAUDIBLE]? So you can see the mesh change slightly. Now the one thing which hasn't changed is from the transition is very coarse, from a fine mesh to a coarse mesh. So what we're going do here is we have something called Mesh settings. And in the Advanced Settings dialog box, this dialog box, guys, is very similar to the Inventor dialog box.

And the thing I'm going to change here is the Max Element Growth Rate. What that basically means is how fast it changes from a fine mesh to a course mesh. It grows at 50% rate. We're going to change that at 10% rate. So we're going to change the value to 1.1. Never put 1 in there because the mesh will be horrendous. So 1.1 is pretty fine.

And there are other dialog boxes and other options-- just ignore them for a minute. Once you press-- once you changed it to 1.1, because I was in the Mesh Settings dialog box when I pressed OK, it updates the mesh, and you'll see some changes. It will be more smoother transition. OK, there we go.

Now once you've got that, click on Run. And again, we're checking whether the value has changed. If you get different values to [INAUDIBLE], just put your hands up. We should all get the same values.

OK. So let's see what we get now. You get 9.726. It's a small change. That's a 5% change.

We'll just do one more change. Has everybody got a result? Who hasn't? This one-- is still running?

AUDIENCE: [INAUDIBLE]

PRESENTER: Chris. So I'm not going to copy it again. I'm simply going to-- watch me on the screen here-- I'm simply going to change the mesh control 1 value, double click on that value there, and make it 0.25. You notice something? I'm dropping it by 1/2 and 1/2. That's the best way of doing it.

Remember to generate the mesh. And you'll see a lot of refined mesh around the fillet.

OK. Everybody got a very fine mesh? Once you've got that, just click on Run. And I'm not expecting a big change, maybe 1%.

Now you notice something. As we make the mesh finer and finer, it just takes a little bit longer. Now imagine how long it'll take if you had an assembly.

AUDIENCE: [INAUDIBLE]

PRESENTER: Yes. Yeah, but you don't want to see all the warnings though, do you?

AUDIENCE: No.

PRESENTER: No.

AUDIENCE: [INAUDIBLE]

PRESENTER: Just ignore the warnings. [BLOWS NOSE] Sound effects. OK.

Have we lost anyone yet? Is everybody in a similar--

Now so we've got 9.7 to 6-- there, we've got 9.9. I'm not going to go any further. That is basically less than 1%. And that is a value I would choose. So it was wiser to pick the higher value.

OK. Anybody got anything different to that? If you have, then the only thing which will create that is Young's modulus. It should be 2e to the 5.

OK, so once you've got that, let me show you-- how many people are interested in safety factor? Would you take that value and divide it by 200, and that is what you will-- or do you want to see a plot? Want to see a plot? OK.

Right, so let's see what happens if you got that safety factor here, if I click on that, it goes all red. So what we're going to do here-- let's make it a little bit better to look at-- it's giving me a minimum safety factor of 21.07. Now if anybody had a calculator, and divide 200 by my latest value, it's not going to match that. It would be slightly out. There's a reason for that. It's not wrong, but Nastran calculates it slightly differently. And I'll show you how.

Because I remember five years ago, it was my first support call, and the guy rang and said it's giving me wrong results. And I said I was going curious. It's not.

But first of all, let's make a slight change. If you double click on safety factor, you get a dialog box. And that dialog box basically gives you the-- did I double click on it, or click on Edit then. There you go. That dialog box gives me ample opportunity to change how to display it.

But the thing I'm going to change here in safety factor, click on where it says Specify Min and Max. And where it is data max, I'm going to specify 100. What you do not-- don't click on OK. Click on Display. And it should be a little bit better to the-- there we go. I don't see a lot of red now, so that's good.

So how would that 21.107, so how does it work? So let me show you something. Now I might lose you here. If I do, apologies for that. If I go to [INAUDIBLE] here-- now just to confuse you guys further-- there are two different results we can look at in Nastran.

OK, that's 9.903. Click on Edit. And then where it says Data Type, it says Corner by Default. OK, change that to the other option called Centroidal. And there will be a slight difference in the value. Both values are correct. It's entirely up to you which you want to choose.

Now if you take that value and divide it by 200, then your results will match. So if you're interested in looking at [INAUDIBLE] safety factor values, use centroidal results. It's up to you guys. There's a lot of options in Nastran. You pick and choose what you want.

Any questions before I proceed?

AUDIENCE: [INAUDIBLE]

PRESENTER: It'll give you a stress value, and then if that stress value is above your yield, then you can assume it's going to fail. We would need to run it as non-linear and explicit, which is above-- beyond this class.

AUDIENCE: [INAUDIBLE]

PRESENTER: Well, it's failed. I know it.

AUDIENCE: [INAUDIBLE]

PRESENTER: It'll give you the same plot. The results will be the-- the color plot will be the same. But if you click on safety factor, it will be less than 1. That's human error, I think. OK. Right, save the file, guys.

OK, let's skip through this. So this is basically going through Nastran calculation 21.07 like previously. My hand calculation, if I did it, would be the same value. It's 23, so a slight discrepancy. The reason why they're different is Nastran calculates the average value per element-- centroidal. So use that centroidal value. You have this on the PDF handouts anyway, so I don't want to go explain all that.

So basically, that's it. Use centroidal stretch results, so then you will get exactly the same stress values and safety factor values.

OK, and there you go. You can check the values. They are very, very similar. Right. When we change the mesh, we don't really care about displacement. If someone here wants to look at displacement results, provided you start from a reasonable mesh size, that's enough. The displacement results will never change. It's just-- I don't want to go through the mathematics. Just assume they never change. But everybody is more or less concerned with stress values.

And where do you stop? So if you start from a very fine mesh in your first iteration, then by the time you go to the fourth one, there'll be very little difference. So I always suggest that you pick a reasonable mesh size. Make it pretty coarse, the first one. If you make it too coarse, then the differences will be a lot bigger. So basically here, it's entirely up to you how you want to do this.

I always compare the last three with the first, and the third or second and the fourth. I never compare the second and third. That's my own personal preference. I'm a bit paranoid. But you're happy to do that second and third. So this is just to give you an idea how differences in the stress results. It's very little, guys. By the time you go to the third and fourth, the fourth one-- 1.8%-- that's pretty good.

AUDIENCE: [INAUDIBLE]

PRESENTER: Yeah. So as an example, if I had a very coarse mesh there in the first one, the difference would be huge. Second one-- if you start from a finer mesh in the one, by the time you go to the third one, the difference being the first and third will be very small. But usually, it's asked that-- you might find it tedious, but this is what everybody does. As time goes by, you become an expert. You'll probably do two or three. You could probably get by with two measures. OK? Any more questions? OK.

All right.

This is the more exciting one now. So what we're going to do here, we're going to treat it as an assembly. We're going to put the pins in there and root it as an assembly analysis. This is by far the most popular method, and it gives-- there's a little bit more work involved.

OK. Right. So if you save the other file you've got-- because if we have time, I'm going to ask you to do some optimization. We save the file and close the first file you did.

OK. So open Exercise 2. It's a small assembly file. Just leave it [? assembly.im. ?] And we're not going to go through all the mesh changes here. We're simply going to dump it with the final mesh settings, and apply the contacts, and let's see if we get any difference in the results. That's what we're checking for. If you didn't want to do a single part analysis, you would have to take the assembly and change the mesh three or four times-- which is no big deal. It just takes a bit longer to run. You'd have to do four different changes.

Has everybody got this file opened? No? Who's no? Yes? [INAUDIBLE]. Have you opened it? You got it?

AUDIENCE: [INAUDIBLE]

PRESENTER: OK. Now this one has got the material saved. OK, it's the same materials. We'll check them in Nastram because it's a lot easier to do that. So let's go into Nastram. And just to make it a little more exciting, the pins are made out of alloy. Now the first thing you'll notice is I've got three parts in there. And I've only got two idealizations-- solid one and solid two. What's done there is based on the materials. If I had 50 parts, three different materials, then I'm going to have three idealizations, not 50 of them. It's basically dictated by the materials.

So let's just click on one of them. Let's try a solid two. And have you noticed that that is on the pins? And you can see there's a tick box against a sort of geometry, and this is signed over to the pins. OK.

So what we're going to do here is we're not going to specify the-- we're going to do a little bit of a-- I'm going to treat this example as a half a model because we can. OK? So if you did Nastran like I am, I'm going to finish Nastran and go back into Inventor. And you can see extrusion one in your browser. I'm going to drag it to the end of features-- I've already done this for you. So if I click on extrusion, just drag the end of features. Come on. There you go. Right there. [INAUDIBLE].

Wow. Done it. Everybody got that? OK, once you've actually got the half a model, let's go back into-- what's the benefit? The benefit is it's simpler, it'll be quicker. Now I want to show you a little technique, how to display the whole model as results. Stress analysis gone. [INAUDIBLE] I've found a method to do it. So if you have a large assembly and you can chop it in half or a quarter, that's what you should do-- unless you've got a beast of a machine.

Right. So what we'll do here is click on the load command. And because I've got half a model, half the material we're going to specify half the load, or minus 15 newtons. So we'll go in there and click on that circular face. And [? fx ?] is going to be minus 15. And click on the tick box in your spectacles.

I've done something wrong. No one told me I'm doing something wrong.

[LAUGHTER]

AUDIENCE: [INAUDIBLE]

PRESENTER: What's that?

AUDIENCE: [INAUDIBLE]

PRESENTER: It's the bearing load. Bearing, bearing, bearing, bearing. Otherwise-- there we go. Oh, and it does all this. Now change the normal surface direction to Components. I'll leave that on the screen for a little bit. OK. Now everyone there? OK. Right, let's press OK.

So now we're not going to go through four or five different mesh controls. I'm going to specify what we finish off with. That's what we're going to do. So first of all, let's specify the mesh control. If I zoom in here--

AUDIENCE: [INAUDIBLE]

PRESENTER: Where am I-- you're jumping the gun. I will come to that in a minute.

AUDIENCE: Oh, sorry.

PRESENTER: No, don't sorry me, it's fine. OK. I mean, there's no hard and fast rule. You can do it-- [INAUDIBLE] constraints, then lowers the mesh, whichever method you prefer. OK, so what [INAUDIBLE]. Yes, so I'm going to specify and [INAUDIBLE] that face, I'm going to 0.25%. OK. Now we're going to specify the mesh on everything else. If I go to Mesh Settings, change that to 1. And we're going to change one more thing. Settings, like we did in the earlier example, K I'll move it down a box to this side here. This controls how smooth it transitions from a small value to a big value, 1.1. Anyone not there? OK, OK.

Then go ahead and press OK.

I'm going to change the color of the mesh. Just click on the little boxes. It would be nice if it goes to black always. But don't run it yet, because we've got to now apply the constraints and something else. Has everybody got a mesh? So in this example here, because we've got the pins-- I'm going to turn it around, not on the face, where I cut it in half-- let's Zoom out a little bit. I'm going to pick this side of the pins and I'm going to apply a fixed constraint. So the pins can't go anywhere. So the pins are anchored to the geometry or to the background.

So click on the Constraints databox here. I'm going to pick that face and that face. OK. Make sure you're on this side. Make sure you're not on the other side. Yes. If you want to determine the reaction forces, then I would suggest you create two separate constraints. But here I'm not doing that. Just put your two pins together.

The two pins are going to just stay there. They're not going anywhere. But the lever is going to move around it. OK.

Let's click. Don't slide the pins on this side, the cut face. Pick it on the other side, this one and that one.

AUDIENCE: [INAUDIBLE]

PRESENTER: Got it? OK.

Now we're going to do something special. Because we have got a half a model, we are going to define symmetry conditions. Or in simpler terms, we're going to specify a frictionless constraint. OK, if we didn't do that, then Nastran or any [INAUDIBLE] software will treat it as a half a model. So we go in the Constraints box here, click Frictionless, and you go and click on the three faces which are generated as a result of the cut-- so the two pins and the side.

Make sure you're on the cut side.

Yes? Everyone here? OK, what we got left? What we got left, anyone?

AUDIENCE: [INAUDIBLE]

PRESENTER: The slot test. OK, because we [? didn't get ?] assemblies, we got specify contacts. Now the easy way to do this is you click on the Automatic button here in the Contacts panel. And it'll go and create contacts between touching faces. It's very similar to Inventor [INAUDIBLE]. Now once you've done that, in your browser, under the surface Contacts, I have got four contacts. I was only hoping for two, but it's given me four.

Now I could run this. The more contacts you have, the more [INAUDIBLE] you're going to get, and the longer it's probably going to take. So I'm going to suppress two contacts. Why? Let me show you what I mean by this. If you look at your pin around the slot area-- I'm just going to zoom in here. If I look at contact one, that's between the circular surface of my pin and the flat. It's basically because [INAUDIBLE] is at the edge. You don't need that. So we're going to suppress that. You can't delete automatic contact. We can suppress them.

Now if you were to retain these and run it, the results would be the same. They're just going to be a little bit longer than the other ones. OK, so just suppress them. Keep it simple. So now I'm assuming your contact one is the same as mine. OK, so right hand click and suppress, and the other one is contact four, and suppress. OK.

Now the default contact, when it's generated, it creates it as a bonded contact, a bit like glued. Now in the real world, it's not glued. In the real world, it allows it to sort of rotate about it. So we're going to change the contact type. And we are going to go and pick the two items, shift key press to multiselect, right on Click, and eventually, Edit.

And everybody should have this dialog box. Yes? OK.

You have lots of different type of contacts in there. Now just to give you a warning here-- separation contacts they can take a lot longer than sliding no separation. So as a first port of call, use sliding or separation. It's basically you can slide along the pin, but it can't separate it. This one allows to separate, and we'll see the differences. So use that one, and I'm hoping it'll take a couple of minutes. So once you've done that, nothing else will change. You know what? You can specify friction if you want. But we'll leave it for the time being.