Join John Helfen for an in-depth discussion in this video Adding threaded holes, part of Autodesk Inventor 2018 Essential Training.
- Now let's look at how we can create threaded holes. If we rotate around on the final model, we can see that we have a threaded hole on the back of this model. And, what's important here is that this hole is actually terminating at this hole that runs through the boss. If we rotate a little bit, you can see that it cuts through the model, but it doesn't cut all the way through the model. Once it hits this hole, it simply stops. Let's go ahead and create that threaded hole now. I've created "holes.ipt" as a starting point, and if we rotate to the backside of the model, you can see that this starting point doesn't have that hole.
Let's go ahead and create a sketch, and we can generate that threaded hole now. We'll right-click in the graphics screen, and select "New sketch"....... And then simply left-click on the face on the back of the model. To help us in locating this hole, let's go ahead and project some geometry. If we return to the create panel in the sketch tab, we can select "Project Geometry". And then, we can left-click on the face we just sketched on... That'll project all of the edges to the sketch so that we can use that in generating additional geometry. If we right-click and select "Line", we can simply connect these two lines by left-clicking, and then left-clicking again on the other end.
We'll right-click and select "OK", and you can see, Inventor went ahead and projected some of the information that we hovered over. We can right-click and select delete on that if we need to. And, we're now ready to continue. What we wanna do now is create a point in this sketch that Inventor will specifically see as a center to a hole. And the we can do that is return to the create panel, and select the point tool here on the ribbon bar. Now Inventor wants us to locate the point. And, we're gonna do that by hovering over this line.
Until we get to the midpoint, you'll know that you've hit the midpoint when you see the green dot. That indicates Inventor has found a midpoint, and is gonna create a coincident constraint. By left-clicking, and then right-clicking and selecting "OK" to get out of that, you can now see that we have a point here. And this is a very special point in the sense that Inventor will see this as a center of a hole. I'm gonna go ahead and finish the sketch. To create the hole, we're gonna right-click in the graphics window, select "Hole" from the marking menu, and you can see that a few things have happened.
Inventor has automatically selected the center of the hole, which was the sketch point, and, it's created a preview... Now, Inventor remembers the last settings that you used in the dialog box. So, you're gonna need to take some time to make sure that your settings are appropriate for the hole you're creating. In this case, we're gonna go ahead and leave this as a simple drilled hole. And, rather than setting the diameter, we're gonna change this to a threaded hole, or a tapped hole......... And we can do that down here at the bottom of the dialog box by selecting the threaded or "tapped hole" option.
When we do that, instead of seeing information about fasteners, in this case we're seeing information about threads. Now we wanna make sure we take some time and look at these options so that we are ensured that we're selecting the right type of hole. In this case, I do wanna essentially create a corner twenty threaded hole. If, for some reason, quarter-inch isn't selected, go ahead and select quarter-inch from the list, and you can see here the thread designation is defaulting to quarter twenty UNC, which is really the most common type of thread for a quarter-inch hole.
But, if needed, you can select this drop-down, and there's many different options, depending on your specific design needs. The other thing we'll notice is that, in the previous steps, we created a through-all hole. And you can see that the preview is cutting all the way through the model. And that's not what we want... So, let's go ahead and look at the different types of termination we have. If we select the drop-down menu, you can see that we have an option for distance, where we can manually set how deep we want this hole to be drilled. But in this case, we're gonna select the "Two" option.
This allows Inventor to define a specific face where we want the hole to stop at, or terminate at. If we left-click on the hole that we created in the first hole movie, you can see that the preview is updated and the hole now only runs into this drilled hole. If we select "OK", the hole is created, and we can zoom in and take a closer look. First thing you'll notice is that there is a cosmetic representation to the threads. What this means is that Inventor didn't actually carve threads out of the solid model.
Instead, it's using a piece of graphic information in order to let you know that this is a threaded hole. Now, in the background, what's happened is Inventor has taken all of the information that was in that dialog box and attached it to this hole. The reason that's important is because when you get to the drawings, and you use the hole note feature, Inventor will pre-populate that with all the information from that dialog box. It'll set the thread designation, the thread depth: any other information that's critical. The other thing we wanna look at is if we rotate this model a little bit, you can see that the hole cuts through to the hole that we created in the first movie, but it doesn't run all the way through the part.
And that's what we wanted..... Finally, let's look at the hole in the browser real quick. Hole five now is in the browser, and it's a skteched feature, because it was created using that sketch. If we expand that, or hover over it and pause for a moment, it'll automatically expand and you can see sketch seven has been consumed, indicating that this is a sketched feature.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers