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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 finished exploring sketched features in Inventor, we're ready to begin looking at placed features. And we're going to start with one of the more unique place features, and that's a hole. As I mentioned in one of the introductions to part modeling, the hole feature can actually be created as a place feature or as a sketched feature. I'm going to look at a few different ways to create holes within this example file. To create a hole you can go to the Modify panel in the 3-D Model tab and select hole. Or, you can right-click and select Hole from the Marking menu.
When you do that, you're going to get a few different options in this dialog box. Actually more than a few, because there are so many different types of holes you can creat here, you should be able to create anything you need from this specific dialogue box. We'll begin by looking at the different type of placement for holes. By default it starts with a linear option and the reason for that is that there is no unconsumed visible sketches in the browser. The one sketch that we have that's unconsumed is not visible and therefore ignores it. We'll circle back to this one in a little bit.
To start, we're going to look at the concentric option. By selecting Concentric, you'll notice that the options for placement have changed. If I switch back to Linear you can see here we have Face and two reference lines. But on a Concentric option, we have a Plane and a Concentric reference. The Plane is simply the face you want to create the hole on. In this case I'm going to select the top of this cylinder. You can see a preview and currently it's off center. But what you'll notice is the dialog box is changed. The plain option now how a white arrow indicating inventor has what it needs to move forward and it's automatically placed us on the concentric reference option which is indicated by red.
This means we still have to select a concentric reference so that we can align this hole. And what Inventor is looking for is any circular edge or face that it can align with. You'll notice as I hover over the fave, there's a little x that previews where the center is going to be located. It doesn't matter which one you select, but you want to consider. The fact that this cylinder might move and not end up being concentric to the box below it but I'm always going to want this whole to be centered in this location. So I'm going to select the concentric references this top cylinder.
By doing that I'm going to move the whole to the center and we're ready to look at the more detailed components of creating this whole. We have a few different ways we can create holes. We can create them as drilled holes, counter board holes, spot face holes and counter sunk holes. We're going to go ahead and leave this one as a drilled hole. Some of the other options we have available are the type of fit that the hole is going to have. Is it going to be a simple hole? Isn't going to be a clearance fit hole, a threaded hole or, a tapered hole? For right now, we're going to go ahead and leave it as a simple hole and, we're going to leave it drilled.
And, we're going to set the termination type to Through All, which it is by default. The next thing we're going to do is change the diameter of this hole. We can either change it in this dialog box. Or we can use the Heads-Up display if we want to. Or finally, we could click and drag on the circle to manually change the diameter. In this case, I'm going to go ahead and enter 0.75 in the dialog box. Because I want a three quarter inch hole to cut all the way through this part. By clicking OK, you'll see we now have a hole in the browser and it's different from the excursions that we had.
The excursions that are above this are actually sketched features indicated by the plus symbol, which will expose the sketch that's driving that shape or that feature. Our hole is actually a placed feature. It uses a model rather than a sketch to located itself. There are a few other options for hole though. I'm going to go ahead and rotate to the back side of the part and we're going to sketch on this back face. We can left-click on the face and use the heads up display to create a new sketch. I'll right click in the graphics window and select Create Line. We can then locate this line by selecting the intersection of those two lines, and the intersection of the lines directly across from them.
Now that I've created the line, I'm going to right-click on it and convert it to construction. And to finish this sketch, I'm going to go to the Draw panel in the Sketch tab and select Point, and the reason for this is, I want a very specific location for my hole. I'm going to select the mid-point of this line, and create a point. What that does is locks that point to the mid-point of this line. And, Inventor sees that point as a special type of point. When I finish the sketch, I can go to my Home view and I can right-click in the Graphics window and select Hole.
Now, you'll notice it defaults to using the last settings I entered when I created this sketch, with one exception. Because we had sketch seven in the browser unconsumed invisible, Inventor automatically went to the From Sketch option as a placement type. And because there was a point that we created specifically for a hole, Inventor automatically selected that point for us, so we didn't have to manually select our center points. But you'll also see that it also left the termination type to through all. It's left the diameter to 0.75 which is okay.
But we're going to need to change it for this hole. In this case, we're actually going to create a threaded hole or a tapped hole so I'm going to select that option. And you'll notice that that display changed, because we're no longer going to change. The size of the hole based on our diameter. Instead we're going to select the type of screw we're going to place in this hole. Down below in the thread section that opened up when we selected the threaded hole we have all the information we need from the engineering handbook. We can select that we want a quarter inch hole from the list.
And, by selecting that, we have the thread designation change automatically to a quarter 20. We also have a bunch of different thread options, but I find that quarter 20 is the most used. I'm going to leave the default. And you'll notice that we have one last thing we need to change for this hole, and that's the fact that the termination is currently through all, and I don't want it to go through the entire part. Instead, I want it to go through to a specific location. And Inventor changes the inputs, and allows me to select a specific location I want that to terminate at.
In this case, I want it to stop at this hole. If I select OK on the dialog box and rotate to the back side of the part, you'll see that we have a hole that, when we rotate the model of it, cuts through to the other hole but doesn't poke through the entire part. The other thing I wanted to call out is because we created a threaded hole, there's a cosmetic representation of that thread here. This isn't the actual model being cut as threads, it's simply a cosmetic representation.
But it's more than that. What Inventor is doing it's simply giving you an indication visibly that this is a threaded hole, but in the background, in the inventor engine behind the modeling system. It's actually captured all the intelligent information from that hole, so that when we go create a drawing of this model, and we use the hole note functionality, Inventor will automatically pull all the information it needs from this hole. It'll know the thread designation, it'll know the depth, it'll know all the information that you would typically need to put onto a drawing to describe a hole.
So by defining the proper type of hole in the modeling environment, you'll end up saving yourself a lot of time when you're in the drawing environment. The other item I wanted to call on about this hole, is compared to hole three, it's slightly different. You'll notice that hole four has a plus symbol next to it that shows sketch seven. And you can see the difference between these holes is the hole three is a place feature, and hole four is a sketched feature meaning it's driven by that sketch. The final type of hole I want to show you is a hole that allows you to create multiple holes from a single sketch.
In the last hole, we only created a single hole on a specific point. In this case, I'm going to go to the browser, right click on sketch 6 and turn it's visibility on by selecting it. This is a sketch I created just so we can save a little time and we can use it place multiple holes. When I go to the Hole command, I'm going to have to select a few different options. I know that I'm going to select the centers. Because I didn't create individual points here, Inventor is asking me to select the centers I wish to use. I'm going to select the end points of these lines and you can start to see some of the previews pop up.
And the reason for that is I've selected the clearance hole. So that I can define the type of screw that I'm going to put in this hole. The fastener type I'm going to use is not hex bolt. Instead I'm going to use a socket head cap screw. And instead of a quarter inch screw I'm going to drop that down to a size 10 screw. And you'll notice that it automatically updates all the previews to show the changes. And, because I'm selecting a specific type of bolt or screw, Inventor is automatically updating the information in the dialogue box to represent the proper dimensions for that type of screw.
By selecting OK, you'll see now that hole five actually represents four different holes. They're all the same size but, I do have the ability to share this sketch at additional points and even drive multiple sized holes off the same sketch. It's not something you'll do all the time but if you're creating a large hole pattern, that will come in quite handy.
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