Join John Helfen for an in-depth discussion in this video Creating and editing components in an assembly, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] Now that you know how to place components into an Assembly file, we can look at how we can create and edit parts within the context of this assembly. What we're going to do is we're going to create a handle that'll go on the end of this arm. We can either go to the Assemble tab under the Component panel and select Create or we can right-click and select Create Component from the Marking menu. That's what I'm going to do. Once you select that, the Create In-Place Component dialogue box is presented, and we can enter all the information we need to create this component in the context of this assembly.
First, we need a name. In this case, I'm going to name it Handle, and just to the right of that, we have a Template that we can select. It defaults to Standard.ipt, and that's going to work in most cases, but if needed, you can change that. For example, we could create a blank assembly file or we could create a Sheet Metal part or a Weldment assembly. We didn't cover these in this course, they're a little more advanced, but I know Lynda.com has a Sheet Metal course for Inventor you may want to check out. Below that, we have the New File Location.
There's a default value that you could change if you want or if you want to, you can browse to a different location on your hard drive, but I'm going to leave the default. And now, we can look at the Default BOM Structure information. What this does is allows you to define the type of component this is going to be in respect to the bill of materials. If you select the drop-down, you can see we can create Normal, which is what we'll use in most cases, or we can define this as Inseparable, Purchased, Phantom, or Reference. The check box to the right allows you to create a Virtual Component.
What this means is the part will show up in the browser and it'll be reflected in the bill of materials, but it's not something that's actually modeled. For example, it might be paint, it might be glue or a lubricant of some sort, something you wouldn't model, but you want represented in the bill of materials. Finally, we have the ability to constrain this sketch plane to the face we select when we create the component. I'm going to leave this selected, and I'll show you the results of that in just a second. I'm going to select OK. Now we need to select a face where we can begin creating this model.
I'm going to select the end of this arm, and what you'll see is the entire assembly is now grayed out. And in the browser, you can see the same is true. All the parts at the top are grayed out and down at the bottom, you see a white area, and you can see Handle that we just created. The unique thing here is you see the End of Part icon. This is telling us that we are in the part modeling environment. Not only do we see End of Part, but the ribbon bar now reflects all our part modeling tools. And we can begin creating a part just like we would in any other case.
For example, I'm going to right-click, select New Sketch from the Right-click menu, and Inventor brings up the Origin planes. We want to select the plane that is parallel to the end of this arm. In this case, it's XY, we'll left-click, and we rotate normal to that view, and we can begin sketching. We're going to start by right-clicking and selecting Center Point Circle. We'll left-click on the center point of the sketch and enter .25 as the diameter for that circle. That's the diameter of the arm, so this will essentially be pressed onto that arm.
While we're in the Circle command, we'll left-click again on the center point and this time, enter .5 as a diameter. We now have the geometry we need for our handle, and we can select Finish Sketch. We can right-click and select Extrude from the Marking menu, and select the ring we just created. Inventor applies all the default settings, it extrudes to direction one, it enters a value of one, and now we can go ahead and make some minor modifications. And this comes in very handy that we're in the context of an assembly. Let me go ahead and hit the Home button on the View cube, and rotate to the front view.
You can see here that we're extruding in the wrong direction. I want this to be extruded towards the model, so I'm going to go to the Heads-Up display and change to direction two. You can see here if we zoom in a little further that this extrusion at one inch runs all the way down to the other end of this arm, and that's not what we want. So we're going to left-click and drag on the Heads-Up display. We're going to move this back to 1/2 inch. Now you can see it doesn't interfere with the end of this arm, instead it leaves a small gap so the parts won't rub together.
We can go ahead and select the green check mark, and apply that, and hit the Home button. To finish this up, let's go ahead and select the circular edge on the end, and select the Chamfer tool from the Heads-Up display. While we're in the command, select the other edge as well, and now you can see we've got both ends chamfered at 1/8 of an inch, and that's fine. Select the green check mark and the chamfers are applied. We're generally finished with our part now, so what we can do is we can return to the ribbon bar on the far right and select Return.
What that's going to do is move us up a level and essentially return us to the assembly modeling world. We still have Handle down here, you can see it in the browser, but we also have this Flush constraint. That's the constraint that was created when we first created this part. There was a check box in the dialogue box that told us that that was going to happen. Let me show you what that does. If we zoom in, and we left-click and drag on this part, you can see that it moves off of the arm, and that's expected. Let me show you what I mean.
If we look at it from the front view, even though we can move this part, if we left-click and drag on it and try to move it in any direction, you'll find that it maintains that Flush constraint. These two surfaces are flushed to each other based on this constraint. Now, you don't need to understand that, we'll cover constraints in a little bit, but let's finish this up by adding one additional constraint. We can right-click, select Constraint in the Marking menu, and then we can zoom in, and hover over the center of the handle, and hover over the center of the arm.
By selecting each of those, the axes through both of them are aligned, and we can select OK. Now when we left-click and drag on this part, you can see that the entire model moves, and that's what we really want. Now before we finish up, I also mentioned we can edit these parts within the assembly as well. If we right-click on the part in the Graphics window, there's an option in the Marking menu to Edit or because the browser is just the same as the Graphics window, we can right-click here as well, here's Edit at the top.
However, the way I prefer to do it is to simply double-click on the part in the Graphics window to do the same thing. By double-clicking on it, all the parts are grayed out, we're back to the 3D Model tab, and you can see all our features here in the browser. Let's go ahead and make a minor edit. Let's select this edge that was created by the Chamfer and use a Fillet on it, leave it at 1/8 of an inch, and we'll select the other edge as well. We can click the green check mark to apply that change, and now we can return to the assembly level by clicking Return on the ribbon bar.
Here you can see a fillet has been applied, we now have an additional Mate constraint, and if we left-click and drag, we still have the parts moving the way we would expect.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers