Punches, Embosses, and Patterns, Oh My! Creative iFeatures and Punches.

PETE STRYCHARSKE: Hey, everybody. My name is Pete, and I want to welcome you to my class, Punches, Embosses, and Patterns, Oh My-- some of the creative iFeatures and punches that I've created with customers over the years. So before we get into it, at the outset, I just want to say a couple of quick things.

Number one, I'm making an assumption that you all know what an iFeature is and that you know some of the basics of iFeatures-- how to select the features, how to control the parameters, things like that. If you don't understand those things, there is going to be a Q&A session. We can bring it up then.

Also, because of time constraints, I'm going to go relatively quickly through a bunch of the material. So please refer back to the handout and specifically Appendix A, which has a lot of video links to the YouTube videos I've created to walk through more specifics in more detail.

Before we get into the meat and potatoes of the presentation, I figured I should let you know a little bit about who you're dealing with. So again, my name is Pete. I'm an implementation consultant with D3 Technologies. And we're an Autodesk Platinum Partner.

And most of my responsibilities fall into the following areas-- I teach a lot of classes, usually with Inventor and Factory Design. I provide technical support on the Autodesk software. So if you press the Enter key and the software closes, that's the kind of thing that we deal with there.

Within the last year or so, I've taken over the YouTube channel, particularly the Inventor side of our YouTube channel, and try to produce one to two videos a week. My wife has jokingly started telling people I'm a CAD influencer. And I tell her, babe, nobody is saying that. But it's kind of fun. I like it. And I finally consult on a lot of design questions that our customers have around the workflows, data transfer, and sometimes even helping them develop the content myself.

When I'm not doing CAD stuff, I love to interact with God. I love working with kids and serving my church. I'm a huge Star Wars nerd. And in Minnesota a little bit tricky, but I try to get to the beach as much as I can. And as often as my knees allow me to, I try to play some basketball.

So why are we here? Why did you come to take this class? My personal feeling is that iFeatures are a pretty underutilized part of Inventor. And I think that comes from a couple different reasons. They're tricky to make, sometimes, exactly the way you want. They can be a bit intimidating. And getting them just right for the end user to place them properly can be challenging as well.

So my goal is sharing these examples that you see on my slide. I want to try and demystify some of the items around iFeature generation and expand the possibilities for you to use iFeatures at your company.

I'm going to accomplish that a few different ways. First of all, I want to talk about some of the important considerations, really, for any iFeature. And then we're going to break it down into three specific categories. We're going to talk about compound iFeatures-- this means that the operations go in more than one direction-- embossed sheet metal punches-- when I say embossed, that means that there's a forming element to them-- they're not just cuts-- and an internal iFeature. This is a little bit unique because the use case has kind of so far, at least in my experience, been limited to woodworking companies. But you can actually embed feature patterns within that overall iFeature.

So we're going to get started with important considerations, really, for any iFeature. So the first one I like to talk about is the base features themselves. These are the models that are used to generate each iFeature. And I strongly recommend that you store those somewhere. The reason why I think that's helpful is you may have other users who need to use that base model in the future to either tweak an iFeature or make a one-off. So it's helpful if you can go back and access those models.

For some of my more complex iFeature models, it's actually faster, sometimes, to go back to the base model, and make the changes there, and simply republish it versus trying to edit the already-published iFeature. And as I mentioned before, one-offs-- if you've got the base model, it's really easy to do a Save and then create the next version that you wish to generate.

For example, if you look on the slide, you can see at the left-- this is a compound iFeature. I'm going to lovingly call this the IKEA feature. You'll see why later. And the one on the left is very flexible, meaning I can place it lots of different areas, utilize the angles, et cetera. But the image on the right is a very specific location for that IKEA feature from the upper left corner of a board. So that's an example of a one-off type scenario.

Using parameters effectively is actually a core parametric function within Inventor and any other software. You really want to take the time to set up a consistent and well-named set of user parameters. Part of the reason why this is important is it helps us think through the design. If we've taken the time to create all of these parameters, it's less likely that something is going to be overlooked or slip through the cracks.

It also helps us establish consistency, especially if we start to take these features, and we build that library, as I showed in the previous slide, or create templates of the IPTs. It also improves the user experience because when they go to place the iFeature, if everything is very well-organized, named effectively, it just makes that process much better for them. And then lastly, if we're consistent, as we get into more advanced iFeatures, we actually may want to link the iFeature parameter to the model parameter. And that's just much easier if they're named consistently.

We also want to try to minimize the reference geometry. So as much as possible, we want to tie all of the features, all of the sketches, to a single geometric reference. So that could be a work point, it could be a sketch point, et cetera, et cetera.

We want to try to utilize a single design sketch as often as we can. And in cases where we can't do that, then we may have to create additional work planes, some additional sketches. We want to base each one of those work planes or sketches solely off of that initial reference or that initial design sketch.

So for example, if you look on the slide, the upper portion, you can see there's that IKEA feature. The bore and the hole are being driven by a single sketch. If you look down below, there's this embossed feature. And that's being driven by a design sketch, which is the cut. But then we had to make an additional plane and sketch. So that work plane you can see at the bottom right is derived solely from the design sketch.

And lastly, we want to simplify the placement as much as we can to improve the end user experience. So in any way that we can, as much as possible, we want to minimize the number of selections required when placing the iFeature. So in the case of the threaded stud, which you'll see in a bit more detail in a second, it's a singular work point.

Also, we want to rename the positional geometry, if that's useful, so that we can clarify exactly where the iFeature should be placed. So you can see an example at the bottom of the slide, where I'm identifying the plane where the bore is going to be drilled and the center point to locate said bore. So those are some important considerations in any iFeature that you're going to generate.

And now I want to take a look at an example-- that threaded stud again-- where we'll take a little bit more of an in-depth look at this one. I am going to take a quick peek at publishing the iFeature. And I'm not going to do that for all the other examples, just in the interest of time. But let's dive over to Inventor. And we can see that threaded feature here.

So again it's a super simple feature. There's not a lot to it. It's an extruded cylinder. It's got some threading applied to it to make it a quarter 20. So the feature itself is very straightforward. What I want to take a look at, though, is the idea of how to control the placement.

So I'm going to highlight the sketch. And you can see in the sketch, there is the origin point. Here is the center of my box. And one quick note-- there is a little bit of debate about whether or not you should use origin geometry inside of an iFeature. Some people have said that they've run into scenarios where, if they use the origin point, when they place the iFeature later, it tends to get tied to that origin point. Personally, I've never had that happen.

So I would say this-- you can feel free to use the origin point. Or, like in the scenario I'm showing here, don't use it. Just be consistent, and make sure that you test out your iFeature before you pass it along to an unsuspecting colleague.

So again, in this case, I created an off-centered square. I then create a work point, which-- let me just show you that quickly. The work point is right in the middle of that face using the Center Point of a Loop of Edges option. And then I built the extrusion and the threaded feature.

So to publish this-- it's very straightforward. I'm not going to take a ton of time. You, of course, know how to do a lot of this stuff. But what I want to highlight here is that the placement is very traditional, meaning it's going to give me an option to place a sketch. I can kind of freewheel, move it wherever I want. Or I could edit the sketch when placing it and then, more specifically, locate it.

But what if I want to make this act more like a sheet metal punch? Well, by choosing an additional piece of work geometry, I can now grab that work point. And you can see it's going to add a second selection. So it's still going to be a face where I want to locate the feature. But it's also going to give me a location point.

And so really quickly-- again, I'm not going to go through this for the other features-- but I can write in information that I deem relevant. That could be renaming it. I could also say, pick point where stud is centered-- if you can spell better than I can.

And we can also rename the iFeature. So again, as it makes sense, you can rename the features, the position geometry, even the parameters. If they're not clear, we could clear those up. We don't have any in this case, but the same approach applies.

Really quickly, if you go to my handout, in Appendix C, it does give us some information on what you have to watch out for if you're going to rename the feature, like you can't have spaces. It's similar to a parameter name. So we'll save this guy.

The last thing I'm going to talk about with the publishing is it automatically pushes you to the catalog. But another tip I would share is that, in your workspace, create a folder for your published iFeatures. You don't have to do this, but it makes it easier for people to find. It's all in that central project file location. So if somebody remapped their application options, or they just lose the catalog location, they can always find it within the project file. I've already published this one. So I'm going to save the time to finish it. And let's take a look at applying it.

So here we've got a simple board. And I'm going to insert the iFeature. Going to find my threaded stud, place it on the plane. There's my stud attachment surface. There's my location point. And there's nothing to change, so I just finish it. And there you see your threaded stud.

As a bonus, if I hit the Sketch Driven Pattern, I can pick my feature, I can choose my sketch, and now I can have that pattern out the other two studs. And then that would work as a feature pattern inside the Inventor assembly if you wanted to apply washers, nuts, et cetera.

So moving on-- let's talk about compound iFeatures. So if we take a look at the compound iFeatures, you might ask yourself, well, what the heck does Pete mean by that? Well, it simply means operations in multiple directions.

So if you take a look at the image at the right-- some of you may be very familiar with this, especially if you've put together IKEA furniture as much as I have. You'll see-- very familiar-- you thread this fastener into one board. It passes through the other board that's perpendicular to it. And you lock it down with the cam nut. I lovingly call this the IKEA feature simply because it's on almost every piece of IKEA furniture I've ever built.

So that's what we're going to talk about when we look at a compound iFeature. So some things to keep in mind-- you want to utilize parameters well, and you want to utilize a single design sketch so that you can generate all kinds of features from that single sketch.

So just a quick example-- in real life, this is what one would look like. And I'm not going to go through the authoring process. A couple things to note here-- if you look at the upper left, notice that I've included the work point. So again, by including the work point, now we can have the bore center point, penetration plane, et cetera, et cetera. So things like that-- very, very helpful.

All right. So let's jump over and take a look at this IKEA feature. So again, the geometry is not super complex, but there is a lot going on here. So again, I created it off center. You can see by the sketch. There's the origin point. And then I apply a work point at the center of a loop of edges again.

So the first trick with a feature like this is, if I want to use a single design sketch, I want to be able to drive the bore and this perpendicular hole all at once. Well, to do that, I created a work plane. So I'm going to turn on the visibility here quickly. And that work plane is embedded into the shape a certain distance-- a parameter value called the hole edge distance-- that allows me to then create the sketch, which drives both features.

So again, think through the design. I have the bore information-- bore depth will come in handy in a second-- the hole edge distance-- that's defining the depth of that plane-- and then some other hole criteria, including the angle, which we'll talk about in a second. So that's the first trick. I have to embed or get a little creative sometimes to get things to work out the way I want.

So if I take a look at the sketch-- I'll just highlight it here. It's pretty straightforward. If we look at the bore, it's just centered on that projected work point. I created a three-point rectangle that allows me to control it at any angle. And of course, the 90 degree is my angle parameter. And then I convert the left-hand edge to a centerline format so that I can apply a linear diameter. So it's really straightforward as far as a sketch goes.

The last trick is this extrude. So if we look at the extrusion, it's a little bit complex. So because I'm starting at some central plane, from the penetration surface, there's a bore depth. But I'm already partway through it, so how do we figure that out?

So from the plane, I'm going to do an asymmetric extrude. The one distance is, of course, just hole edge distance. That gets me back to that outside. And then to get the overall depth, I say bore depth minus that hole edge distance. That gives me that little bit right there. So again, by using just a little bit of math and Inventor techniques, we can quickly generate more complex types of features. And of course, the circle is just a revolve cut.

So really quickly, I do want to touch on extracting this one because there is one catch to it. So if we grab the extrusion and the revolution, you'll see it still just has the one thing. But if we pick on the plane, now it's going to have the reference point and the plane.

So we can rearrange these if we want and, of course, rename them. So now it picks the surface. That'll determine the work plane. And then the reference point, again, is that center point. So experiment with different features in your roster, and sometimes that will give you different positional geometry to work with.

So I'm going to jump over to the iFeature placement. We're going to orbit this really quickly. And let's insert that iFeature.

So if we go to the IKEA Flexible-- I'm going to open that up. Here's my penetration plane. Here's my point. And then just for the sake of time, boom, there it is.

But if I place it a second time, pick my penetration plane, pick my point, I can edit some of the values. So in this case, if I say 0 for the angle-- I finish that, and you can see that now I've shot the hole out the side of the part. So it does give us a lot of flexibility if we think through and utilize those parameters effectively.

So we're going to move away from standard iFeatures, at least for a little bit. And let's talk about these embossed sheet metal features. So what do I mean by embossed? So I'm going to use the traditional Inventor definition.

So if you've ever placed some of those standard, out-of-the-box punches-- you'll see there's the square embossed, there's the circular embossed. All that that means is that there's some kind of forming. It could be pure forming, like you see at the left, which would be a dimple or a blister, depending on how people term that. Or if you look to the right, that's where I'm actually doing some cutting as well as forming. So either of those options-- that would include some embossing.

So when we build up embossed features, a lot of the same stuff applies, right? Use the parameters well. Try to operate from a single design sketch as much as you can.

One quick thing that is a requirement for a sheet metal punch is your design sketch must contain a sketched center point. That's how it gets located in the sheet metal environment. So that's absolutely necessary. And as a reminder-- the bottom bullet point-- if you have a need to generate a secondary plane or a secondary sketch, it must reference the main design sketch only-- only.

So let's take a look at some examples of this. The first example we're going to take a look at is this traditional formed emboss. See behind, it's just like a blister? We're going to use the revolve feature for this one.

And the extraction properties that I want to highlight here is, of course, that the top-- it's a sheet metal punch. So that gives us an opportunity down at the bottom to give it a punch ID, and if you need to, a simplified sketch representation. So if we ever get to the flat pattern, that's what they would see.

So let's take a look at this in Inventor, jump over here to our sheet metal revolved emboss. So again, extremely straightforward example-- it's simply on a face. There's a sketch that locates the feature. You can see the center point. And it's just a profile with a centerline in the middle to denote where it's going to get revolved. So the sketch is very straightforward.

If we look at the first revolution, the first revolve is the solid part, OK? The second revolve is the cut inside of it. And that's what forms this feature.

Really quickly, before we move on, I want to highlight that I'm not adding any fillets here to these edges. I'm not saying you can't. You can add fillets. But what happens is it adds additional placement geometry the users have to select. And is it worth it? Inventor can't flatten this shape anyway. So if I add fillets here, I really am not gaining a whole lot. So it seems like it's a waste of time for the end user. And it doesn't really give me the result that I'm looking for.

You can use the Unwrap tool in Inventor to flatten things like this. But yeah, it doesn't really impact the flat pattern in the sheet metal environment. So I usually don't bother.

So we would go ahead and publish this, just like you saw on the slide. And then let's take a look at how this works in the punch environment. So we go ahead and find the Punch tool. We'll navigate to our published punches. And here's that Tapered Embossed Slot. I hit open. I pick the point. I could adjust the geometry if I wanted to, but I'm not going to bother. I'll just hit Finish. And there it is.

So you can build your own embosses. This could have been an extruded emboss. I used the revolve example. Critical things to note is that it generally works best if it's all generated from the same design sketch.

Another example would be open-sided emboss. So this is where the material isn't connected to the base plate everywhere. So it could be open-sided, open-ended. If you look at this example on the slide, these tabs to lock things in place-- yeah, those are definitely open-ended.

So this one is, again, pretty straightforward from a punch standpoint. The trick here is that we can't do it all with a single design sketch. So we're going to have to get a little bit creative with the work plane.

So taking a look at this one, again, the geometry is not super complex. It's simply a cut with the sketch. So I'm going to move up here, turn on the visibility of the sketch. And if you're curious, it does have dimensions. It's just the parameters, right?

So what we're going to do is we'll just create this sketch. And that's great for the cut, but it's really difficult to create the extrusion from that same sketch. It's possible, but it's a lot of trigonometry.

So what I ended up doing was creating a work plane. And this work plane is defined using one of these edges and then this point. And that's how we define the work plane. It's the center-- it's a normal to the axis through that center point. So when we create that, now we can do the cut. And that work plane allows us to create this secondary sketch, which is the actual shape of the profile.

And a couple things to note-- when I created this profile, I made sure that I projected this point and this point purely from the sketch edges, not the geometry. Additionally, when I extrude this shape, I use the parameter Emboss_Width, not a from-to. And the reason why I'm careful with these projections and I'm not using from-to is I want to minimize the number of selections when this feature gets published.

So pretty straightforward stuff. That's your feature. We would go through the publishing process. And then when we go to the punch placement, we'll grab this Punch tool, again, navigate to our shape, and then there's our open-sided emboss. Again, I pick my point. I could play with the sizing. I'm going to do that in the next feature. So I'll just go ahead and hit finish. And there is your example of that open-sided emboss.

So you can create a fully-closed embossed. With a little bit more creativity, you could create an open-sided or open-ended emboss. You've got some options.

So the last example that I want to look at for the forming and the sheet metal is these teeth. So this is kind of wild because the customer approached me years ago and said, I wanted to take these teeth, and I actually want to flatten them out. I need to generate a very accurate 2D flat pattern so that we can laser cut the sheet. So in this example, I had to do a bit more math and, again, some creativity to be able to generate the shape.

So when we look at what was required for extracting it, a lot of the stuff is relatively straightforward. The trick, though-- if you look at the positional geometry, you'll see that I have identified a Bend_Radius_Fillet_Face. So in order for this thing to actually flatten, it has to be a valid sheet metal feature so that we can flatten it in the 2D flat pattern. So I have to give the end user an additional selection to make. There's no way around it. So make sure that we rename this one really clearly so they understand what they're trying to do.

This is crazy complex, so I'm going to breeze through this. Definitely take a look at the handout for this one because there's lots and lots of math. So taking a look at the feature-- I'm just going to talk you through it for a minute or so. It's these formed teeth. They're opposing, chamfered teeth. They could be used as a locator. It could be used to hold down material, maybe a sheet material of some type or fabric.

And what they wanted to do is generate this accurate flat pattern. So what needed to be done was we needed to take this shape, flatten it in such a way where this length right here is the actual length of the cut. And then because these aren't flat, they would terminate here in the middle. But because they're longer, they extend a little bit.

So what we had to do is we have to take some material away, which ends up being the tab width because it's all 45-degree angles, right? And then there's this little bit of a gap this direction, and the cut width is directly here. So again, using trigonometry, Pythagorean theorem-- A squared plus B squared equals C squared-- I can compute this distance.

So by taking into account the unfold criteria-- K-factors, bend allowances, et cetera-- I can compute this accurate length of the tab. And then taking into account the reductions because of the 45-degree angle, and the tab width, and this little distance here, we can in fact generate an accurate flat pattern.

So let's take a quick look at the parameters before we dive into the feature. So again, we're defining some critical things like cut width. And in order for this feature to work properly, I'm internalizing the K-factor and the bend radius. We'll take a look at that later. There's a tab height-- that's the desired height from the bottom. And then we've got the desired width of that tab.

Putting all this together, we can now make some pretty wild math. So because my design sketch is at the top of the part, I need to include the thickness to get the actual tab height. And then we're calculating the bend allowance. So this isn't a sheet metal theory.

We've got that bend radius we're using. And then we've got the K-factor multiplied by the thickness to actually get that neutral surface somewhere between the interior and exterior of the sheet metal. And then, since it's a 90-degree bend, there's my pi over 2. That's my bend allowance.

So what we can do then is we take the square root of our chamfered gap. And we'll-- again, it's just that cut size in both the A and the B direction. So it's 2 times that squared and then the square root-- that gives me that little gap between them.

Phew. Put all that together into this wild formula, and you actually get the length. So it's the tab height plus that bend allowance times 2, right, two tabs. And then we have to take away that tab width and then that little gap between them, and we get this overall length. It's crazy. Please see the video. It's awesome.

All right. And then when we build the feature-- again, stepping through it quickly. It's an extrusion-- solid extrude-- of the profile of the tooth, not to the bend radius. Then I cut it. That gives me the leftover shape. Then there's fillets on the outside, the fillet for the bend radius. And then we chamfer it.

So the last thing is I created the sketch. That can serve as the 2D flat pattern as well. You can either form it, or you can have this representative sketch, which is all based on the geometry projections. It's a lot-- a very cool feature, but it's a lot.

So when we take a look at this in the placement-- we'll grab this Punch tool, work features, find our published iFeature. Let's see. Yep, here it is, Formed_Teeth_Tabs. Hit Open.

And so because it's the only sketch remaining, now you get the preview that you're probably used to seeing. But when we slide over to the geometry area, it's actually asking for an additional selection. So because that design sketch was on the top of the part, we actually have to go to the underneath side of the part. That's going to be where the bend radius is applied. So I orbit, select this face. Now it's satisfied. We could play with the sizing. We're going to dive back in here in a second. So I'm just going to finish. And here is your formed teeth.

Before we can move on, we did internalize a couple of parameters-- the K-factor and that bend radius. So somehow, we have to tie those internal iFeature parameters to this overall host part. So to do that, we're going to go up to the Parameters.

And the bend radius-- it just exists. It's a part of that sheet metal rule. And if we look down below, I've already created a K-factor. And the K-factor-- I can type in a number. So the trick is the K-factor is not inherently tied to the sheet metal rule. I have to extract it somehow.

So this is where iLogic comes into play. And if I edit this rule-- it's a very simple rule. I've got this as Appendix B in the handout. But I'm going to grab the active sheet metal rule K-factor, assign it to the K_Factor parameter I just created. And that's how we link the two.

Cool. So to look at that in the final edit of the feature, I can come over here, edit the feature, and I can tie these values back. So here's your K-factor. Here's your bend radius. And I can simply click on K-factor and say, I want to tie that by listing parameters to my K-factor of the part. Same thing with the bend radius-- list my parameters and then grab the bend radius from the component.

Not only that-- this is how we could make changes too. So since I'm already here, if I say, oh, you know what, we want that to be 1 inches wide, we can do that and hit Finish. And you'll see that the characteristics-- the bend got a little bit bigger because it's a bigger bend radius, and the slot got wider.

So to see the final result, I hit the flat pattern. And there it is. There are your formed teeth. If you wanted to see this as a 2D representation, we would just edit that flat pattern definition, and we could see what it looks like as 2D with the center mark.

And there you have it. So you can represent it either way, but it is an accurate flat pattern of that particular feature. So if you keep your band radii very consistent, if you make the right selections when placing it, you can have fully formable features.

All right. So the last feature that we're going to look at in this class is what I'm calling internal pattern iFeatures. What this means is that every single one of the features exists as a pattern within the entire-- or the overall context of the iFeature. So all the stuff that we've talked about-- using parameters and equations well, working with the single design sketch-- all those things are still applicable. The bottom two bullet points, though, are a little bit unique if you're going to generate a pattern.

So when you set the direction, as much as you can, you should only use the internal sketch geometry to drive that direction because it will eliminate a potentially confusing selection during the placement. And then, when you're working with these types of features in particular, you'll end up with a lot of equations-- calculating the spacing or whatever-- and you have to remove those.

Number one, the iFeatures typically won't publish well. They won't place well. They'll fail if they've got equations inside of it. And then number two, you've taken the time to write the equation. You don't want the users to go back and eliminate that. Maybe they type in the number 4, and your elaborate equation is wiped out. So again, do not include any type of equation parameters. It's just not a good idea.

The last warning I'm going to share is, when you use an internalized pattern iFeature, the Inventor assembly will not recognize that as a feature pattern. So be very careful about that. Again, this use case is more specifically for woodworking. In fact, if you look at the example picture I have here, pocket hole drilling-- they're not going to populate that with parts, typically, but they are going to drill that so they know exactly where to locate those features on the CNC equipment.

So a couple of quick things to note here-- basically the same as the other extractions we looked at when publishing. If you look at the size parameter, note that there's no hole spacing. So I'll talk about why that is in a moment. But that has an equation built into it. It is not appropriate to export as a size parameter.

And then, especially with tricky features like this one, make sure that you take the time to rename that position geometry well. So you can see I've added the edge location point, and talking about, where is that going to be located?

So let's take a look at this last feature in Inventor. We've got this internal hole pattern. Again, it is not difficult. The geometry is not hard. But we want to be careful in how we model it.

So first thing I'm going to talk about actually, in this case, are the parameters. So you'll see there's an overall length. We'll see that when we link it up. Then there's an end distance. So I'm assuming in this particular design I'm going to have two holes spaced the same distance from each end of the board. And then utilizing a whole quantity, which I'm letting the users define, there's your equation for calculating the spacing in between the holes at the ends. So pretty straightforward type of a pattern.

When we go to execute it, the first thing I did was I defined a work point. So this is your locator point. So by putting it at the midpoint, what I'm saying is I want this to be centered along this edge surface.

Then we define the sketch-- again, pretty straightforward. I project the work point. I draw the line, again, using that end distance. And I either add or convert the endpoint to a center format so I can drill the hole. The line is important because, as you'll see in a second, it also serves as the direction for the pattern. Drill the hole. Create the pattern. So hole quantity, hole spacing-- simple parameters that define that spacing pattern.

The tricky bit here is, for the direction, I'm using that sketch line itself. That internalizes that selection, meaning when I get to the iFeature placement, I just have to pick a surface and a reference point. It does all the work from there.

So let's take a look at this last example. We'll go back to our iFeature, and we'll take this open side here. And let's insert that pattern. So it's the Hole_Pattern iFeature. Pick on this plane here. Pick on this point. And then, if you want to see what that looks like, go ahead and hit Refresh.

Don't sweat it if you hit Refresh and it doesn't preview it. I've run into some features where maybe the preview is too complex to generate well. It doesn't work, but when you hit Finish, it actually does produce the iFeature correctly. So hit Refresh. Don't worry about it if it doesn't finish. Click on that button to get out of the iFeature. And if it doesn't work then, now we've got to go figure out what's going on.

But in this case, the Refresh was fine. And we see that it doesn't quite look right on this back side. And this is where we can come over here, just like we saw in the previous example, but we can do it as we're constructing the iFeature. We can add that OA_Length, refresh it again if we want, hit Finish. Now it's tied to this particular design scenario.

One additional tip-- if I hit f sub x and I get up into my parameter table, we can create additional parameters. And we can tie them back to the iFeature even in the parameter table. So if I give users the opportunity to create their hole quantity, make that unitless.

And let's say there are seven holes now. I can copy-paste that new user parameter into the equation field of my iFeature. And now you'll see there are seven holes instead of four. So you have a lot of freedom to take these pattern iFeature and tailor them to very specific placement scenarios.

That was the last example. And that concludes the class. So my goal was to give you several different examples of iFeatures that we've worked on-- and again, reference Appendix A of the handout-- there's lots of video links there-- and to try and help you see where you could use iFeatures. So I really want to thank you for taking the time and watching my presentation.

But I also don't work in a vacuum. So I want to take some opportunities to thank people that have helped me. First and foremost, I want to thank God for this great opportunity to teach at AU again. It is a privilege, and I'm thankful for everything that he's given to me.

I also want to thank my boss, Rick, and my former bosses, too, because they give me the time and the space to explore all kinds of things that are personally interesting and to take time with customers and really try to drive in and get the best results. So I appreciate that freedom.

And finally I do want to thank the customers because every example that you saw in this presentation was generated either with a class, or I was doing consulting with the customer. And you all just ask really good questions. You take the software above just creating boxes. And I enjoy that. And I love working with that. And you actually provide a lot of motivation to find these solutions.

I hope to see you at the Q&A. Please feel free to ask questions. You can also reach out to me. I'm on the web. You can see our YouTube channel. Looking forward to it. And I hope you have a blessed day and an awesome rest of your AU.