Join John Helfen for an in-depth discussion in this video Adding placed holes, part of Inventor 2016 Essential Training.
- We're now ready to explore how we can place holes in our part files. As I mentioned earlier in the course, holes can fall into two different categories: they can either be placed features, or they can be sketched features. And we'll look at both over the next couple of movies. We're going to start by creating this through hole on this boss. In the following movies we will also create holes using sketches, and then we'll rotate around to the back and we'll create the threaded hole as well. To do this, I've created Holes.ipt that we can use to begin from. The hole command can be found in the 3D Model tab under the modified panel in the ribbon bar.
It can also be accessed by right-clicking in the graphics window and selecting Hole from the marking menu. When you do that, you see the hole dialog box is presented and there's quite a bit of information here. We have different placement types. We have different hole types. We have the overall diameter. We have termination types. We have different drill points, and even different fits for the holes. Once you understand all of these settings, you should be able to create any hole you need for just about any design you create. You'll notice that the placement type has defaulted to Linear. If you select this drop-down, you will notice that there's several other options as well.
There's From Sketch. After Linear, there's Concentric, and On Point as well. Now, if Inventor had seen an unconsumed visible sketch in the browser it would have defaulted to From Sketch. But you'll notice in the browser we have Sketch6, which is not visible, so Inventor ignored it. Now if we look back at these placement options, you'll see that the input options for a Linear placement are Face and several reference edges. When we switch to Concentric, which is the hole type we need for this exercise, you'll notice that these input values update.
To create a concentric hole, you need a plane to place the hole on, and you need a concentric reference so that you can center the hole. Let's go ahead and left-click on the top face of the boss to place our hole. You'll see that in the dialogue box that the plane option is now white, and we've automatically been moved to the Concentric Reference option. When you go to select your concentric reference, you should consider what you're selecting. For example, we need cylindrical face or edge and we have several on this model. We could select the face down here or it's edge, or the face up here and it's edge.
Now, if we were to select the face on the bottom, we would get the right result. The center of the hole would be placed at the center of the boss. However, if at a later time this boss was moved on this top platform, it would no longer be concentric to this face. So a better option would be to select either the face or the edge around this circle and, by left-clicking, you can see I've selected the edge and the hole is now concentric. The next thing we want to look at in the dialogue box are the different hole types. By default we have Drilled Holes, and that's what we'll use so we'll leave those, but we also have Counterbore Holes, Spotface Holes, and Countersunk Holes.
We also have the ability to change the overall diameter of the hole. We can do that here in the dialogue box, or in the Heads Up display, or we can left-click and drag on the orange ring to update it through the Heads Up display. Now that the hole is set up to 0.750 inch in diameter, we can look at some of the other options. Below the overall diameter we have the Termination type, which defaults to Through All. This is actually what we want for this hole so we can leave it, but there are several other options that we'll explore in the coming movies. Finally, at the bottom of the screen, you can see that we have a Simple Hole by default, and these are the different types of fits for the hole.
We also have Clearance Hole, we have Tapped Hole, and we have Tapped and Tapered Hole. We're gonna go ahead and select OK and the hole that we were defining is now created, and has been added to our model. If we rotate to the top view you can see that the hole does go all the way through the model, which is what we expected, and in the browser Hole3 has been created. What's important about the hole in the browser is that it is a placed hole. You can tell this because it doesn't have a + symbol next to it. Unlike the Extrusions above, which are sketched features, they have a sketch driving them.
In this case, we use the face on the model and the edge on the model to define the location for this hole. Therefore, this is a placed hole and we'll look at sketched holes in the next couple movies.
- Reviewing the Inventor workflow and file types
- Creating a project
- Sketching and working with origin geometry
- Creating and modifying sketch geometry
- Projecting and importing geometry
- Modeling parts
- Building parts with placed features
- Creating feature patterns and sculpted objects
- Adding parts to an assembly
- Using constraints to position parts
- Creating drawing views
- Adding annotations