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Already up and running? This course is the next step in building your Autodesk Inventor skillset. Author John Helfen takes you through the interface and key processes of this parametric design system, including sketching, part modeling, assemblies, and drawings. Each process works in conjunction with the rest, allowing you to create parts and assemblies and document them in a way that they can be manufactured. Learn how to set up your project file; create and modify geometry; create extrusions, sweeps, and lofts; build parts with placed features and patterns of features; and create iParts and iFeatures. John also covers assembly visualization techniques, drawing views, and balloons and parts lists.
The course was created and produced by John Helfen. We're honored to host this training in our library.
Now that we've learned how to create iParts and place iParts, it's time to learn how to create and place iFeatures. iFeatures and iParts are very similar. But they do have differences, and we'll see that here. iFeatures are actually quite a bit easier to create. On the screen what you can see is a standard part I've developed from scratch. I created a new part. I drew a rectangle to create this base extrusion and then, I created a new sketch and I placed a couple of holes in that sketch and that you can see here.
And, the holes are the ones I'm going to use to create the iFeatures. But in order to do that, similar to preparation work you'd have to do on an iPart, there's a little preparation work that we need to do on this part as well. I'm going to go ahead and expand hole one and double-click on sketch two to edit it, because really, what I want to do is use this iFeature to automate the process of creating the sketch, placing these two hole centers, connecting it with a construction line, and adding this dimension.
While it might not seem like a lot of work, once you do it over and over and over again, or you have more features than just a couple of holes, it can became tedious. And this is a great way to speed the design process. But in order to do that there's some cleanup work we want to do. I don't know that this hole is always going to be positioned in this manner. I don't know that it's going to use this vertical line, I don't know that it's going to use this horizontal line to locate the distance. So what I want to do is start cleaning up by windowing these dimensions, and clicking delete on the keyboard to remove them.
Next, I want to strip out these projected edges. I'm going to highlight those through a window mode, and then delete it. And I'm going to select this by left clicking on it and delete it as well. And the reason for that is just for simplicity sake and clarity. I know I don't need any of that stuff so I don't want to risk clicking on something by mistake and adding it to any iFeature when I don't need it because it can just add a little bit of complexity and simply slow the design process down. So, I now have these two-hole points in a construction line along with a dimension.
And if I left-click and drag, you can see I can move it anywhere I want. And that's what I want in this case to set this up. I'm going to go ahead and finish this sketch by left-clicking on finished sketch. And you'll see that the holes move a little bit because I made some modifications. But what I've done is prepare that feature for exporting as an iFeature. So let's go ahead and look at how to do that. If you click the Manage tab, you can go back to the author panel, just like we did with iPart, but this time we're going to use the extract iFeature button in the upper right.
I'm going to left click on that to bring up the extract iFeature dialogue box. And what you'll find is we have a couple of different types of iFeatures that we can extract, standard features or sheet metal features. Both work in a very similar fashion, just in different environments. And sheet metal is beyond this course, so we'll skip that for now. What we'll do is we'll begin by simply selecting the features we want to export. Now I'm going to hover over the graphics window and select the hole. And by doing so, since we created two holes in that single hole feature, both holes are selected, and you can see what Inventor has done is split out some of the information it's going to need to place this or locate it when you put it into a new part file.
The first section is the size parameters. When I created that hole, we had a hole diameter dimension and we had a length between those two holes. And we'll be able to change those when we place those features. So, there are, are prompts that you can adjust based on your needs. You can, I'm going to leave it as the default of inner length or inner hole diameter, but you could change that based on your specific features that you're exporting. And then finally it needs something to position this. And that, right now, is just this sketch plane.
And it's going to ask you to pick a sketch plane by default. Again, the prompt can be changed very easily, just by left clicking here and replacing that text but at this point, that's all we needed to do. By clicking save, we can then go to our exercise file folder. And I'm going to save that here as iFeature one. Because it's the first one I've created. But you can name it according to whatever's going to make it easiest for you to identify that iFeature by the name.
It could be two-hole pattern. It could be a specific part number for the iPart you're going to attach to it. It could be a bunch of different things. It is up to you as the designer to pick what is most appropriate for your environment. I'm going to go ahead and save it as iFeature one and we now have that feature saved off in a folder. Here you can see that we have iFeature one along with the plate that we started with and we'll use that in the next movie to place that onto a new part.
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