Join John Helfen for an in-depth discussion in this video Placing fasteners from the content center, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] There's one final way we can add new parts to this assembly. And that's through our Content Center. By default, Inventor ships with an enormous array of standard components, such as nuts, bolts, washers, and other types of fasteners. On the screen you can see a Content Center.iam file that I created so that I can show you this. If you rotate the model just a little bit, so that we can see the top a little bit better, I'll explain what we have here. I've gone ahead and created a base plate that has four threaded 1/4-20 screw holes in it.
Above that, there's another plate that has corresponding holes that are counter board and set to be clearance fit for a 1/4-20 screw. Rather than manually creating every single screw, the Content Center lets you select from and generate a huge number of fasteners from a library. To do that, we're going to go the component panel and we're going to select the dropdown below Place. From the list, we're going to select Place from Content Center. And we're presented with a library of all the things we have available by default. Right now you're seeing that we have cable and harness selected.
And below that, you can see things such as fasteners, molds, sheet metal parts, shaft parts. We're not going to go through all of these. We're going to focus on the fasteners. But I do recommend that you take a moment to kind of glance through this, and get a feel for all the things that are available. It'll help when you get to that point in your design to know that it's available for you so that you can easily select it. To begin, we're going to select the Fasteners. We can either hit the plus symbol on the left, to expand the entire tree, or we can press on Fasteners, and we can see the categories on the right.
That's the method I prefer, it's just a little bit easier. You can see that in the Fasteners category we have Bolts, Nuts, Pins, Rivets, and Washers. We're focused on bolts, so we'll double click on that. And now we see the different types of bolts that we have within that category. We have Countersunk, Hex Head, eye bolts, but what we're really looking for are Socket Head bolts. So we're going to double click on that category. And here you can see if we scroll through this list, there's a large number of socket head-type screws. As a matter of fact, there's so many it might be a little difficult to find the one you're specifically looking for.
And there's an easy way to fix that. On the toolbar, there's a Filter button. And just to the right of that, there's an arrow that when you press it, it displays all the standards that are installed in Inventor. I'm looking for an ANSI bolt, so I'm going to select that standard. And the list is automatically filtered down to just those that fall into that standard. That makes it a lot easier to find this specific socket head cap screw in inch format. Once you find it, go ahead and double click on it. And you'll see that Inventor places us into the place component standard interface.
We have a part, in this case it's a fastener, and it follows our cursor around. Now, this is a little different than the standard part insert. Because it has much more intelligence. If I were to hover over the edge of the top of the counter board, Inventor's going to evaluate the overall diameter of that and it's going to find a fastener that would fit it. That's not what we want to do, I'm going to show that in just a second, but what we really want to do is select the edge where the bottom of the screwhead is going to touch, and it's the hole that the bolt is actually going to go through.
Because what Inventor will do is it will find the fastener that fits that, and generate it for you. And then you'll be given options to make additional changes. Let me show that. I'm going to hover over the top edge, it's the one we don't want, and you'll see Inventor increase the size of the bolt, and you can see it's a 7/16 bolt. That's much bigger than what we want. What we really want is the bottom of that counter board and the edge on the inside. That's going to shrink it to a 1/4-20 screw, and that's what we want. So I'm going to go ahead and do that one more time.
I'm going to hover over that edge, and I'm going to left-click, and you'll see that something happens. A dialog box is presented, and all the other edges that are that size are selected on this part. You can see on the far left, there's an Insert multiple option. And this is a toggle. If we click on it, it will simply remove the red highlights from the other holes. And it would only place a single fastener. In this case, we do want to create all four, so we can toggle that back on. And in this case, Inventor's going to create all four of these fasteners at once and place them into their hole.
To the right of that, we have an option for Bolted Connection. We're not going to cover that in this course, but what it does is say, for example, both these plates have clearance fit holes through them. We could create a bolted connection that would include the fastener, a washer underneath the fastener, a fastener that went all the way through both plates, and then there was a washer on the back, and a nut on that fastener as well. It allows you to create an entire bolted connection, or a bolted stack, in a single action. In this case, the next one is to apply this and continue adding additional fasteners.
That's not what we want. We want to go ahead and place these and be finished. But before we do that, let's go ahead and rotate one more time to the front view and have a look at our bolt. The reason I'm doing this is because if we zoom in a bit, you can see that this bolt doesn't go all the way into the plate. It touches it a little bit, but this is a threaded hole, and we want a little more engagement. So we can use the arrow here to left-click and drag this. And as we do that, you're going to see that Inventor snaps to standard sizes. Here we have 1/4-20 at 5/16.
Here we have it at 3/8. The next one is 7/16. The next one is 1/2 inch. What this is doing is selecting standard sizes. That way you don't, by mistake, create a bolt, or insert a bolt, that doesn't come in a standard size. We wouldn't want you to have to modify a standard bolt. So Inventor helps make sure that you're only creating things that you can either have in stock, or purchase off the shelf. That's going to save you a lot of time and money. If I select the Home view again, we can finally finish this by left-clicking on the button on the far right.
We'll see a table. We have a final opportunity to confirm that this is the bolt that we want, and we can select OK. And Inventor will generate that fastener and place it in each of those holes. If we rotate to the bottom, you'll be able to see that those run all the way flush to the bottom of that plate. And that's what we wanted. And if at any time your design changes, and you need to make a modification, you can always find the hex bolts in the browser. You could right-click on it, and you could change its size. This will bring up a new dialogue box that allows you to change this fastener out.
You could change its size, you could change its length or its thread type. Once you do that, you can either replace that individual bolt, or you could replace them all with this checkbox. I'm going to go ahead and Cancel. I like what we have on the screen. But that shows you how you can create fasteners very quickly from the library, rather than having to manually create them over and over again.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers