The Inventor 7 Deadly Sins of 3D Part Modeling

PAUL MUNFORD: Good morning, everybody. So yeah, Elan just mentioned, if you do make any notes to this system it send you an email with all your notes on it. So you get those back. Thank you very much.

There are a few people waiting outside. They're not allowed until five past 8:00. So there might be a little bit of disruption.

But we're going to carry on. You get all the best bits and they're going to miss out. So that's well done for those that come in first.

It's great to see so many people wide awake and ready for class at this time of the morning on AU. I'm from the UK so I'm feeling a little bit jet lagged. So if I fall asleep just please all leave quietly.

[LAUGHTER]

I always put this slide up first, just to remind everybody what you signed up for. Make sure everybody knows what we going to be doing here today. If you've ever built something in Autodesk Inventor and it didn't behave, how many people have built something in Inventor that didn't behave? Everybody. We've all been there.

So I'm hoping this class will help you understand what's going on under the hood. And maybe you can either work differently or at least understand what went wrong, and maybe you can fix it. So we'll discover some bad modeling practices, how we can avoid them or overcome them. We can diagnose and fix some unexpected failures, create some more successful models. But key to this is learning how Inventor interprets your requests to build shapes. That's really the fundamental part of this class.

To just introduce myself, my name is Paul Munford. I'm an application engineer with Graitec. We're a reseller based in the UK. So my job is to help our customers get the best use out of their investment, the Autodesk software.

This class was originally written by a member of the Autodesk Shape Manager team, called Jake Fowler. It was a fantastic class. It was really fundamental to me and my understanding of Inventor.

So I was really pleased to be asked by the ASM team to help them update this course, and come do it again at Autodesk University to keep this information alive. You can watch the original version from back in 2012 via that link. And you'll also find Indee from the ASM team in London.

We presented this class at ASU London as a lab. And Wes did some hands-on exercises with people to test some stuff out in work. So if you want some data set you can play with, you can follow that second link there. And you can watch, again, his interpretation of the presentation, and try some of that stuff out.

And there is a very detailed handout that goes with this. It goes into way more detail than I can cover in the hour. So if you find this interesting, again, do download the handout. Take a look at it and work through some of that stuff.

PRESENTER: That's all posted on the AU app.

PAUL MUNFORD: It's posted on the AU app, so you can download it. This class is being recorded, so you better watch it back, take the handout, and follow it through.

Good. So we're going to start right here. Who knows what ASM is? Sir.

AUDIENCE: This is a Shape Manager.

PAUL MUNFORD: Yes. So ASM is the Autodesk Shape Manager. It's the bit of the program that calculates the 3D shape that you're requesting. So it's the bit that does the math. It's the bit that does the heavy lifting.

So it's the software component, known as a kernel. And it's the same kernel that's used in AutoCAD, Fusion, Inventor. And it's used a little bit in some of the other Autodesk programs. Not all of them. Some of them are acquisitions and work on different kernels. But certainly ASM is where they go for any additional functionality.

So ASM calculates 3D shapes using something called a boundary representation, or Brep. Does that sound familiar to anybody, Breps? So what actually is a Brep?

So Breps start with vertices. So a vertice is just the point in 3D space. And if we have at least two points we can create an edge. If we have at least three points we can create a face. And if we have enough faces we can enclose a volume.

So now we have a boundary, a boundary representation. There are a few more rules to this, and we'll cover some of those towards the end of the presentation. But this is the method, the mathematical method that the ASM uses to put shapes on screen.

So the first part this presentation is called Get Smart. And we're going to talk through some of the Inventor tools. And I'll talk through some of the lesser well-known features those tools, and the way the Autodesk team expects you to use them, and see if I can enlighten anybody as to the best way to use these tools.

So we're going to start here. We've got a few creation tools. I'm going to talk about Sweeps and Lofts, and a few modification tools. And also a Patch tool in the Surfacing environment.

Let's start here with the Sweeps. So who's used a Sweep in Inventor? Just about everybody. In fact, I know you've used a Sweep recently, as well. So the Sweep tool takes a single profile along a path.

Here we go. Here's a standard sweep. Create a shape. It looks something like that. But in fact, under the hood, all of these things are Sweeps

An Extrude is a Sweep, a Revolve is a Sweep, a Call is a Sweep. The same method of calculation is used, the same algorithm is used in the ASM Shape Manage kernel to calculate all of these shapes. And the thing that they have in common is a consistent cross-section.

So when we use the Inventor interface to create an Extrusion we are sweeping a profile along a path. But we don't have to give Inventor a path. The path is implied as being perpendicular to the sketch plane we're on.

If we're doing a Revolve, we don't have to give a path because the path is implied as being a circular shape around our axis. Calls are more complicated. But it's the same idea. It's taking a profile and it's sweeping along the path. It's only with a Sweep that we actually give a path.

So when should we use a Sweep? Well, whenever you need a consistent cross-section. When I talk about Sweep, I could be talking about any of these. I'm talking about something with a consistent cross-section the whole way along.

Now because we have a consistent cross-section, it means we can't warp the shape. We can't apply end conditions. We can't apply tangency or smooth end conditions. So it's usually a good idea for a Sweep, one of these, Sweep, a Loft, Extrude, Revolve.

It's always a good idea for one of those to be the first shapes you're building inside your model. So generally, we build these first. And then if we need something that has a smooth flow between features we can go into a Loft for that. Build Sweeps first.

Here's a question. This is a side point. Sometimes, people ask, well, can I have a Sweep but Sweep between two profiles? So we know now the answer is no because a Sweep has to have a consistent profile.

But what we could do is we could use a Loft. So how many people have used Loft with Centerline? Yeah. Cool. So the Loft with Centerline is actually using a very similar algorithm.

It is effectively sweeping this one shape along the centerline path in one direction. And it's sweeping the other shape back in the other direction. But it's also merging them at the same time. It's a combination of Sweep and Loft.

Here's another question I often get asked is Guide Rails, how do they work? With a Sweep, we know that we've got to have a consistent cross-section. That's the rule we have to work with. But we can rotate that cross-section on the path. And we can scale that cross-section on the path.

So we do have options now to better do that with the Taper option in Sweep, and the Revolve option in Sweep. But we've always had this option to do Guide Rails and Guide Surfaces. So the Guide Rail or Surface can twist the profile along a path.

And if I just illustrate that with a Guide Rail, if you could imagine some lines drawn between the Guide Rail and the Sweep path, those lines would be twisting the shape. So these lines would be perpendicular to the shape as it twists. So we can use a Guide Rail to provide twist.

A Guide Surface looks slightly differently. In this case, we're drawing lines that are normal to the surface. So who's familiar with the term "normal"? Most of you. A few of you.

So normal just means perpendicular. It's a mathematical term. So perpendicular to the surface.

How can we use this? Well, we can use this to be able to apply twist. I've put a little animation in here.

So we've got a curved, twisted surface, and we'd like a Sweep to follow it. So we can use the Guide Surface option to twist the shape as it goes along to make sure we've got something that is nice and uniform to the shape. So this is a really useful option when you have to build these slightly more complex models.

But a really cool tip for Sweeps is to remove twist. So in this case, I've deliberately built something that has twist in it because of the way I've built the profile. And that may not be what I want.

So I could in this case, use the Sweep with Guide Surface and provide actually a flat work plane. And that would then remove twist from the shape. So that's another way of thinking about these tools, another methods you might find useful. Fantastic.

So let's move on and talk about Loft. The Loft is not defined by its sections in the same way. We can interpolate between a number of sections of the Loft. So with this shape, I've got up in the screen here, a Loft will create a surface that goes directly between these two profiles.

Towards the front, we've got something that's roughly circular. And towards the back, we've got something that's roughly square. And in the middle, we've got an exact match between those two shapes.

So this is what the Loft tool does well. It creates a smooth transition between profiles, as smooth as it can get, which makes it the right tool for surfacing work because we can warp this surface. We can apply end conditions. We can have tangency and smoothness to get a good blend between surfaces.

Talking about Lofts, what is the difference between a Rail and a Centerline. So again, this is something I often get asked because they look pretty similar. So what are they doing?

So as an example here, I've got exactly the same geometry. But this time, I've picked this curved spline here as a Rail. And in my other example, I've picked it as a Centerline. So I think that illustration shows the difference already.

So with a Rail, the Loft is still trying to go directly from the input surface to the export surface. And the row is pulling it off to one side. But with the Centerline, it's following it like a Sweep. So the profiles we've picked are actually staying perpendicular to that centerline as they go along.

So for a Rail, it's like an additional constraint. So when we talk about constraints for a Loft, it's not sketch constraints. But we are giving Inventor in the ASM Shape Manager kernel, conditions it must meet. So these are constraints.

But with the Centerline, it guides the shape. And so that's why the Centerline tool is a really good tool to know about because it can give you a much smoother transition between profiles then you'll get by putting loads, and loads, and loads of profiles in for a Loft. And we'll see an example of that in a moment as well.

How to improve the quality of the Loft? Firstly, the fewer profiles the better. If we have lots and lots of profiles we are applying lots of constraints to our Loft. And it's going to find it hard to give us a nice, smooth transition and match all the profiles as we go along.

So in this case, this doesn't look too bad. But we'll see in a minute, there is some warping going on here. One of the key things is, did you notice I put a load of fillets in my sketches? And we always say don't put sketch fillets in, put them in afterwards.

The reason is, because we can't guarantee these are going to be precise. Because the Loft tool is warping from one profile to the other it may not be a consistent radius because it's allowed to warp. The Loft tool is allowed to warp this. It's not a consistent profile. So we could find these fillets here and not actually section through an arc, section through a circle at all.

So first thing is, take the fillets out of the sketches if you can. Build the Loft, and then do the fillets afterwards. And then we'll definitely get something that has the correct radius. So that's step one.

So what else can we do to improve precision? So if I turn on the zebra striping-- how many people use the zebra striping analysis? So in terms of zebra striping, I can see there's some weird wobbly transitions here.

For anybody who's not used to reading zebra striping, we're looking for a nice smooth flow. These black and white lines should be nice and smooth. But there's some weird wobbly stuff going on here. So we're pretty confident that's not a great surface.

And if we look at where those weird, wobbly zebra stripes are it's not a surprise to find out that they are where these sketches are. So the Loft is trying to do a direct Loft between these two profiles. But because we've got so many profiles, it's struggling to meet all the constraints we've given it.

What else can we do to improve the quality? Well, how about a Centerline Loft instead? So a Centerline Loft is always going to give us the smoothest transition between profiles. And if we give Inventor fewer profiles on a centerline, it's going to give us a smoother shape.

So in this case, we do our shape, we apply our fillets. Check it out. That's a much better surface. And if we took sections through each point, we'd probably finally hit the same sections. So if we want these conditions to be absolutely correct we can still achieve that. But we're going to create some things are better quality surface in the first place.

Does that sound useful? Cool. I see a few heads nodding. Excellent.

Let's have a look at some of these rarely used little options, or options that people often don't know what they do. Merged tangent faces. Anybody come across that one? Just one or two, three. Good.

So Merged tangent faces is really useful. The way that the ASM Shape Manager calculates Loft is it creates a four-sided surface. And it will fit it to our input geometry. And if we have tangencies in the input geometry it will calculate a number of four-sided faces to try and meet each of these inputs.

Now that's usually OK. But if we want something really smooth we can turn on Merged tangent faces. And whenever we have tangency it's just going to create one patch. So instead of creating one patch for each input it's created one complete patch that goes around everything.

So this will always be a four-sided patch. If you did a completely enclosed surface, you would find you still have a seam somewhere, where it's wrapping the patch around the input geometry. But you'll find you have something much smoother. So again, if we look at the zebra striping here, we can see there are some definite changes of direction on the left-hand side there. But on the right-hand side, you can see that it's all very nice and very smooth.

Now the key one for me, if you're not doing product design or industrial design, I think this is still a really useful option to know about. Because, well, who's built a thicken that didn't work? So if your thicken didn't work, maybe try turning on Merged tangent faces.

See if you can calculate a smoother surface. And then see if that will thicken. So try it out and see what you think. Give me some feedback and let me know that helps you.

So let's talk about patches. How many people have used the Patch tool? Used it for surfacing industrial design, or is it just to fill gaps? Both, also.

So the Patch tool works differently to a Loft. The Patch tool will always create a four-sided boundary, just like the loft does. That's the way the Shape Manager works. It's always going to be a four-sided shape.

But the Patch tool will trim it back to input surfaces. So rather than fitting to your input surfaces it will be trimmed. And the reason that's helpful is for anything that's not four-sided. So if we're creating a four-sided surface, the Loft tool is usually the right tool to use. But if we don't have four sides then it may be that a Patch tool does a better job.

So this is an illustration of that happening. The Patch tool is a four-sided shape. And it trims it back to the boundary condition we've given it.

So if we tried creating a Loft with the same geometry, we get something like this. So in this case, on the right-hand side of the screen here, I've done a Loft from the bottom edge to a point. And then I've included the sides in as Rails.

And it's created two patches, two four-sided patches, and just put them together. So we have a seam coming up the middle. I think in this condition, the Patch is probably the best tool to use because it gives us one seamless face, rather than using a Loft.

So what about faces with less than four sides? So here's a one-sided input. And the Patch tool will do that absolutely fine. Calculate a four-sided surface and trim it back to our circular boundary.

But the Loft tool, we're not even going to be able to create a Loft tool without-- we've only got one input. And that's not enough for Loft. It needs more than one input.

Three sides? So a three-sided shape. Again, the Patch tool will be absolutely fine with that. It will calculate this four-sided shape, automatically trim it back to the boundary for us.

A Loft, you can still do a Loft with three sides. Again, this is a Loft from the bottom edge. Loft to point, and then include the sides in as as Guide Rails.

But what we get here is we get something called a singularity. So has anybody ever created a shape like that and found they've got some-- thickened it and got some weird stuff going on? So what happens here is, the Loft tool will always create a four-sided surface. But then it will fit it to our boundary condition.

So in terms of a three-sided boundary condition, it's collapsing that fourth edge into a single point. And that single point, we've got all the math is happening by zero. And anybody who's ever divided anything by zero on a computer knows that doesn't work. That's really hard to calculate.

There's nothing wrong with this. There's nothing wrong with Loft to point. You're allowed to do it. And it's a good tool. If it's the last surface you're creating in your model you'll be fine.

But if it's one of the first surfaces, you'll find you probably can't do an extend surface on that because it just can't calculate it. And you'll find if you do a thicken, it's actually pretty good now. They fixed the algorithm a few years back.

But you'll find as you thicken it, you'll get a weird cone-shaped feature coming off it. So you might want to avoid that early on. If you really need to use Loft, then I suggest you Loft a four-sided shape and then trim it back to your boundary conditions, just like the Patch command would do. And that will allow you then to continue working with that Loft.

So when should we use a Loft? When should we definitely use a Loft? Well, if it's a four-sided input then we should definitely use a Loft. And what we'll find is that because our Loft goes directly from one profile to the next profile, a Loft is stiffer.

Can you make this out on the screen here? On the patch side, the patch side definitely dips between the two surfaces. I imagine this is like stretchy fabric. And as you stretch it between the profiles it bows in between because it's been influenced by these side rails as well.

Whereas, the Loft is more like a rolled surface going directly from one profile to the other. And because of that you'll get a much stiffer surface. So patches are pretty good when you've got relatively flat areas and relatively small areas. But if it's a bigger area you're trying to cover, then you should definitely try and use the Loft somehow.

So here's an interesting one. If we use the Patch tool on two profiles like this, and it works. And we get an awesome shape. Maybe not quite what we expected. But that's pretty cool.

So with a Loft, because we've got three inputs, ASM's calculated three patches, and we can see the seams here between the patches. But with the Patch tool, it's created something. Again, you see it stretching between the profiles. But remember, the Patch is still creating a four-sided surface and fitting it to our inputs.

So if we could see what was going on, we'd see it is actually something like this, which doesn't look quite so cool now. I might explain why if we tried to do anything else with that surface it might fail. If we tried to thicken this patch, it might fail. But not because the bit between our two inputs, which looks nice and smooth and really cool, but because the underlying four-sided shape it trimmed back is all over the place. So you may find that you have difficulty in those conditions with a patch. If we can do something with a loft that's definitely going to work better.

The next topic, tangency. Who's used those end conditions on Lofts to better set constraints? Just a few. OK.

So often, when we put a patch in, we can create something that looks a bit odd. So it's weirdly warped. And we fiddle with those conditions. And we think, why is this not better? I've applied a G2 smooth condition. Why have I not got a to better surface?

I've just put a little tip on the side here. And if I just step back one-- so this is a boundary patch, and we can see the conditions for the boundary patch. We can pick from Free condition, we can pick a Tangent condition or a Smooth condition.

And to illustrate what we mean there, I've just put the sketch constraints, like the 2D sketch constraints, next to the 3D constraint so you can associate those two together. So a Free condition just means that the two wedges have to touch. So they're sharing the same edge in space, which is a bit like a coincident constraint.

A tangent condition is a bit like a tangent constraint. They have to be tangent at the point where they touch. And the G2 Smooth constraint-- who's used G2 Smooth constraint in Sketches? I always show it.

But a lot of people, unless you're doing industrial design or product design, you might not need it. That's matching curvature, the points where they meet. So the curves have to have the same radius.

If it's a spline curve it may not be a consistent radius. But they have to have the same radius at the point where they meet. So if we looked here, if we applied a tangent or smooth condition at the bottom we're going to end up with a weird surface because it's trying to follow the surface at the bottom. And it's trying to create the surface coming down and make it tangent.

So it will create a weird S curve. So we're probably over constraining that if we applies a G1 or a G2 constraint at the bottom. Probably what we really want is to have a Free condition at the bottom edge and the side edge because these are definite changes of direction. So we just want to make sure the surfaces meet. But they can go in any direction that's appropriate.

But on the side there, we don't have any curvature, despite the fact it's curving down towards us. If we looked across it, we would see that it's pretty flat. So actually, a Free condition on the left there would probably work. But we can apply tangency. It's not going to hurt.

At the top, we definitely want our surface to be tangent and come off in a nice smooth direction. So tangency would be the correct condition to ask for up there. So typically, when we get weird shapes when we use these conditions it's because we're asking for the wrong condition, or the condition is not appropriate. And if we choose the right condition then we get a really good surface.

Fillets. How do we resolve fillet failures? Well firstly, how many people create fillets that have multiple radii? A few people. Again, it's not wrong. You're allowed to do that.

But I generally advice don't do it unless you're advanced and you know what you're doing. The reason being that if one of those fillet fails it's really hard to diagnose which one is causing the failure. And also, downstream, if you are passing information off to somebody who is maybe going to use your part for CNC programming, they might want to suppress some of those fillets. And it's much easier for them to suppress if they've got lots of individual fillets rather than one big fillet feature with everything in it. So it's not wrong. But I'd say, most of the time, I'd encourage you to use separate fillets anyway.

The first thing we do is break any complex fillets up into separate fillet features. And then a couple of rules of thumb that you might find helpful. I guess most if you look like you're pretty advanced. So you know this, right?

So do your big fillets first and then do your small fillets. That's going to give you a better result. And do your concave fillets before your convex fillets. That will also give you a better result. So there's a couple of rules of thumb that should hopefully stop fillet failures happening in the first place.

But the other one is, some of the options we've got in the Fillet dialogue. If you do have a fillet failure what can we do to diagnose where the problem is? So one of the things we can turn off is automatic edge chaining.

The Automatic Edge Training option will just find from the first edge you pick anything that's tangent to it. And it will try and do the fillet the whole way along. So if you pick an edge and it picks a whole bunch of edges and there's a failure somewhere, try turning this off. And then you can pick on one edge at a time and see where you get before the failure happens. And then you can maybe work backwards or work around that and work out what we need to do next.

You can fiddle with [INAUDIBLE] banks conditions. But the other one I really wanted to highlight is face fillets. Any people use a face fillet? Cool. Face fillet actually uses a slightly different algorithm. So if your edge fillet fails, try a face fillet and see if that succeeds.

I don't think you need to face fillets very often on prismatic shapes. But when you get into more complex and organic shapes it's a really useful tool to use. So I've got here a little illustration of this happening.

So I'm going to take all fillets here and we'll see if this works. I'll pick OK. Nah. Got a failure. One tip here. We'll just see this as I go through.

Who knows about these red hyperlinks? If you click on them, it highlights where the failure is. I've never seen that in any help documentation. I don't know how I found out about it. I guess it's just that for the developers.

So this time I picked my first one. That works. Pick my second one. See if that works. Nope, got a failure again.

So I'll pick on that red hyperlink. Where's the problem? I click on it. There's a little red spot. It's really hard to see on my screen. There's a little red spot appears telling me that's where the problem is.

So maybe if I turn off the edge condition I can work along that edge one at a time and see where the edge is. So they all work. And I click Apply. And then try for that difficult one again. And now it works just fine.

But I think I'll just include it in the end here. I've included a face fillet to just show you how that works. We just pick two faces. Inventor will calculate for us any tangencies. And it will just run along that edge for us anyway. So it's a pretty cool one to try out.

So next topic. What's the difference between a shell and a thicken? So when we do a shell the original shape is honored. So any side walls are built from the original shape.

But when we do a thicken, the side walls are built normal. So normal, again, means perpendicular. So it would be about 90 degrees as it can be to the shape. And the same thing with the offset. Although there's no side walls, it's the same algorithm under the hood that's calculating the offset surface.

So if you really want to control those side walls then probably Shell is going to be your best option. If you're doing something like sheet metal, and you're working with a more complicated surface, and at some point you want to try and unfold that, you definitely want to use Thicken. One of the rules of sheet metal is that the edges have to be perpendicular to the face, otherwise it won't unfold. So by using a Thicken tool, it can be one of the things you can do to help yourself out.

Automatic Blending in Thicken. Anyone noticed the Automatic Blending option? Have you tried playing with that? Nobody. Well, this is what it does.

With Automatic Blending turned off, Inventor will just thicken that face. So it's just going to do basically an offset and provide all the surfaces it needs to complete that boundary. So we'd end up with something that looks like this.

With Automatic Blending turned on, Inventor will look at the input surfaces. It will offset the face and will try and extend the input surfaces to create something that represents the original condition. So we'll end up with something like that.

So it's in there to help you. It's in there to make less work for you when you want that kind of option. But you might find if you're trying to thicken a complicated surface it doesn't help. So if you find that you try and thicken and it fails, try turning Automatic Blending off.

See if that helps. And the other way around. Why not? Let's see.

So with Thicken/Offset, failures, again, how do we solve those? I've put together a little illustration of this happening. But again, watch out for that red hyperlink.

So once again, when we click on the red hyperlink a little point appears on screen that says that's where I've got a problem. I'm not sure what happens if it's got more than one problem. I guess it's only going to highlight one.

So we hunt around and we see which faces will thicken and successfully. Not surprisingly, when we get near the one that doesn't work we get a failure again. What I need to do is I need to remove one of the faces around the area, and then we get a successful thicken.

So I guess for me, the tip there is not the hunting around. I guess we all do that. But press on that red link again and see where the issue is. It may help you to zone in and fix the error a little bit quicker.

There we go. That was the problem. Replace that face. That works.

Just take a minute. I've let you put a timer here for one minute. So I want you to stand up and stretch and wake up a little bit. Yawn. And remember that at Autodesk University the contacts you make are even more important than the knowledge you'll learn.

So if you don't know who you're sitting next to, grab a business card, give it to somebody. Say hello. There will be somebody in this room who's solved your problem.

I don't want anybody to get PowerPoint fatigue this week. So hopefully, that'll just help you to waken up for the second half of the presentation. So the next half of the presentation we're going to be looking at something we've called the seven deadly sins. These are seven things that you definitely want to avoid when you're building Inventor models. And hopefully, some of the information we've already given you will help you to avoid these problems.

So the first problem we're going to talk about is something we call high curvature. I did get my mic back on, didn't I? Yeah.

So out on the left here we've got something that's flat. So no curvature. Or if you want to be pedantic, infinite curvature. So it's not curved. Anyway.

In the middle here, we have low curvature. And on the right-hand side over here, we have, therefore, high curvature. So high curvature can cause issues. And I'll try and illustrate that.

So this is just looking at curvature in two dimensions. So again, we have zero curvature. This entity here is an arc. So we have the same curvature the whole way along.

[INAUDIBLE], I've turned on the curvature diagram for this. Who's used the curvature comb diagrams? So for those of you who haven't, these little lines here that are perpendicular to the curve give us an idea of how much curvature we've got. The longer they are the more curvature we've got. The shorter they are the least curvature we've got.

So this arc has consistent curvature the whole way along. The spline here in the middle has changing curvature. It's low curvature. The length of the spines are pretty flat. The way the curvature changes across from one into the other is called acceleration.

But I wanted to illustrate, over on the right-hand side, we do have high curvature, even though the spline looks relatively flat. By pulling the tangency handle and making it really tight we can see the length of the curvature combs here. It's telling us we've got a really high curvature spline there.

And the reason that could cause us problems-- well, here's an illustration. On the left-hand side here I've built a sweep with a profile on the path that are made of consistent arcs. And actually, the algorithm in ASM will calculate that pretty happily.

But on the right-hand side here I've used a spline. And we get a fail. And again, if I click down and show you the highlight, bink, we've got a fail because you've got self intersections.

So I don't know if you remember, but a few years back we couldn't do self intersections with a standard sweep. But they fixed that. They got that sorted out. So we can now do self intersections with standard geometry. We may not always get what we expect but we'll get a result.

But if we put a spline on there with a high curvature condition we get a failure, we would get a self-intersection. So I did ask the ASM team-- by the way, the ASM team are based in Cambridge in the UK. So I'm very proud of that. We make part of Inventor.

I asked them, OK, so why does it fail when it gets to a spline and self intersects? And I was expecting some really mathematical answer I wouldn't understand. And they just said, well, we just haven't got round to fixing it yet.

[LAUGHTER]

So if that's a problem to you please post your example on the forums. And we can get some enthusiasm around getting that fixed. Because it's not a mathematical problem, it's not like it can't be done. It's just it needs to get higher up on their list of things to do. And if we complain it will get higher.

So if I try and illustrate that further-- so in this case, we've got a face here with high curvature. And when we try and offset the face we've got self intersections. And when we have self intersections we get a failure.

So if you can avoid high curvature you may be able to avoid these problems. So the resolution here is to avoid high curvature if you can. If you can't, maybe we need to do a rebuild, see if we can fix it.

If we can't fix it maybe we can trim the bit away that we don't need. And then maybe patch that back in or approach in a different direction. But maybe that will give you an insight as to why that might fail.

So the next one is near tangency. So I'm just going to jump back into that little discussion we had earlier about end conditions. And I've illustrated this in 2D again.

So right at the top there we have two lines, and they have no continuity at all. They don't touch, they don't share any properties. So not continuous. We measure continuity with something called G. So this has no G, nothing.

When we have two curves and they meet at a point, they're sharing one property. And the property they're sharing is that we have two endpoints in the same position in space. And we call that a G0 condition. And as we add in more G, we're matching more properties.

So if we looked at G1, which is a tangent condition, these two curves have to be tangent at the point where they meet. So two properties, they touch and they're tangent. And we can tell by looking at these curvature combs. Because the curvature comb always goes perpendicular to the curve, and both curvature combs are pointing in the same direction, we know we have a G0 condition. So we can see that quite clearly.

Below that, we have G2, which is a curvature condition. Now we're matching the same curvature at the point where they meet. So we're matching three properties, position, tangency, curvature. And in this case, when we turn the curvature combs on, the curvature combs at the end of each curve are all the same length. So we know we have a G2 condition. We can see that quite clearly.

At the bottom, I've illustrated a G3 condition. Now Inventor doesn't have any G3 constraints. We don't have anything that'll do that for us. But we can manually massage something that looks G3.

When we're talking about G3, we're matching acceleration. We're matching that change of curvature over the length. So we're looking for the same change of curvature.

And the illustration for that is, that not only are the curvature combs pointing in the same direction and they're all the same length, but the comb that goes across the top there, illustrating the change in acceleration, is also tangent. So if we messed around with-- in this case, it's a CV spline-- if we mess around the endpoints and get a really nice looking change in acceleration across the whole curve, we know we've got something that's as close to G3 as we're going to get.

So why is near tangency a problem? The problem is that Inventor uses different algorithms to offset surfaces that are tangent and surfaces that are non-tangent. And if we have near tangency, if we have surfaces that are tangent but not quite, it can pick the wrong algorithm. It depends on the tolerance. And if it uses the wrong algorithm, we either are going to get an unexpected result or we'll get a failure.

So to illustrate that I've created a shell here. And on the left-hand side, we've got a condition that is definitely non-tangent. It's like a 45-degree shape. And we can see that the end walls-- remember we said, shells, end wall is always the existing wall. It's built from the existing face.

So we can see that we've picked the right surface. That we get what we expect. If we have something that is tangent, in this case, it was flat along the top, a different algorithm is used. So instead of trying to offset all these faces it's built a nice 90-degree edge there.

But if we get something that's near tangent, in this case, it's picked the wrong algorithm. It hasn't done what I expected. It's tried to do a non-tangent offset instead of a tangent offset. So sometimes you get these weird conditions, not what you're expecting. Maybe that's the reason why?

So how do we diagnose that? Well, one way we can diagnose it is by using curvature combs. So in this case, instead of a two-dimensional curvature comb it's a 3D curvature comb.

Who's used that analysis type? Just Chris. Maybe I need to come back and do a lesson in that.

So these three-dimensional curvature combs, you can analyze a face and you can look across the entire face to see whether we've got any continuity problems. So on the left-hand side here, you can see the curvature combs are giving us a nice, smooth G3 looking condition. In the middle, they're definitely a characteristic V shape. They're pointing in different directions. So we know they're definitely not tangent.

But over on the right-hand here, it's so close to being tangent that you probably can't see unless you zoomed in really close to see that's not a tangent surface. So that's certainly one way we can diagnose. The other way that's maybe slightly easier is just see if we can do a fillet on it.

And if we can do a fill it on an edge then it must be an edge there. It can't be tangent already. If we can't fillet that edge it's because it's tangent.

So if your model's not too complicated you could start the Fillet command, tick All Fillets. And if edges try and get filleted that you didn't think should be then maybe that's where your issue is. If it's a more complicated model you don't run that in case it locks everything up.

The other way you can do is just select on it. And if you select on an edge, and it offers you the opportunity to fillet it, you know that edge is sharp, it's not tangent. Inventor will always give you an option if it's got one.

So the next thing. Near coincidence. So coincidence is where we have things next to each other. On the left-hand side here, we have something that is definitely not coincident. These shapes are definitely overlapping each other. So that's not an issue.