In this lesson, we'll identify thin and small features. After completing this lesson, you'll be able to; analyze a part for machining, identify critical areas, and evaluate dimensions. To get started on this next lesson, we want to make sure that we upload the supplied file, obstacle pickup finishing, and navigate to the manufacturer workspace. What we want to do is we want to learn how to identify features on a part that might need a different approach to machining. So there are a couple of different ways that we can start the process of creating a cam program. You could be the designer, in which you have a knowledge of the features that were created in their critical nature. You could be given a part and potentially some instructions or even a detailed drawing that'll call out things like parallelism, where the datums are located, and specific features. You could also be given that part as a fusion files so you can navigate back through the timeline and hopefully get an idea of the features and specifics about them. For example, if there's a threaded hole, depending on what fit class it is or specific information about the whole depth, anything like that could be captured inside of the fusion file. With a detailed drawing, you could also be required to model the part based on that drawing, but again the drawing should contain all the critical information needed. Lastly, you could be given a part with relatively no instructions. Someone could just say, make this part, that could not have material applied, it might not have any specifics about features, and you'll have to really be an investigator, figure out what the intent was and maybe where we need to make some judgment calls. So this specific part, we don't have a detailed drawing, we don't have an idea of the features. In reality, the material that's applied, in this case steel is the default material that part come in with. So it doesn't even have the correct material for how we're going to be machining it. So what we need to do is we need to identify some different areas on this part and try to understand the process of which we might take to machine it. So to get started, the first thing that I want to notice on this part is the thin wall on the upper edge. We're going to use inspect and measure, and we're going to take a look at the thickness of the section. It tells me that it's 0.063, so likely it's 0.0625, which means that we have a thin wall section at the top. When I'm looking at this part, this tells me that I want to machine the entire outside of the part, do a roughing and finishing pass on it, then I want to come back, I want to machine out the inside, do all the pocketing operations, remove all the material from the inside, then I'm going to come back with a couple small cuts, and finish off this outside thinner lip. This allows me to machine the outside contour with the thickest wall possible to get it close to the final size, shape, and required feature. Now, in this case again, we don't have that requirement, but as we look at parts, they generally are going to be seen on the outside, and the inside is not usually as critical, in most cases. The whole locations will be critical, but likely the pocket sizes are generally able to be a little bit larger, a little bit smaller, or potentially have some surface finish issues. So that's not always the case, but again if we don't have that information, I always like to strive for making the outside have as tightest tolerance as possible and look as good as possible, which means that I'm going to approach doing the external contour first. The next thing that I notice on this part is going to be these small chamfers. Now, in reality, the chamfers aren't that hard to cut, but when I see here is the fact that they're relatively close to other features, which means that it might be difficult to get a tool down in here and actually cut that. So we're going to have to be very careful with our tool selection as well as how the tool enters and exits cutting that geometry. So this is going to be an area where we might have to be careful when we're simulating, and just make sure that we're not having any contact issues. Another area that I see is this internal section, which is cylindrical, but there is a piece missing, which means that when we start to cut this, we're not going to be able to select an edge, for example, a 2D contour. We'll likely explore some other 2D options such as a bore operation, which allows us to select a center point, but we have to keep certain things like this in mind and be careful when we're thinking about the tool paths we want to use. Lastly, I noticed several holes that actually do have a cosmetic thread appearance on them, but they don't actually have threads cut, which is okay and it's actually a better situation for us. So we can come in, and we can inspect, and we can measure those. Now, these holes are coming in at 0.202, which is a number 7, which is the drill size for tapping a quarter 20 hole in aluminum. So by identifying the diameter of these holes, I know that we're looking at a quarter 20 hole. Again, we can do the same thing over here, however, this hole is blind. So as we're identifying this, we need to figure out exactly how deep the hole is going to go, and you can take a look at this and see that there's actually a drill point at the bottom. So I'm going to measure from this top face down to the bottom edge before the drill point, and notice that it's 0.385, is the straight-line distance. But if we look at the measure dialog box over here, we can see that the distance is 0.385, but we want to focus on it in X, Y, and Z. We don't really need the straight-line distance, we need to figure out the depth of it. So in order to do that, let's take a look at some of our options. We have face, edge, vertex, we have body, and we have component. We want to deselect this upper face when we clear the selection, and we want to go from this edge down to this edge. This will give us an X, Y, Z distance. So now we can see that the diameter of the top hole is 0.375, and we can see the X, Y, Z position, and we can see the distance. The distance is 0.375 from that upper face to the bottom. So this tells me when I drill this hole with a 0.201, I can go down 0.375 from that top face, and I can extend it down the distance of the drill point because that's where I need to tap to. So without this information on a detailed drawing, these are the kinds of things that we need to do to investigate a part before we start programming in. We're going to get into programming some features on this part. We're not going to do a full program on it per se, but we are going to identify a few different methodologies in a few different areas that we can focus on. So make sure after you explore this that use the measure tool, you identify a few things such as the size of the chamfer, the depth of holes, and the diameter of holes. Once you've played around with that, let's go ahead and move on to the next step.
