In this lesson, we'll focus on toolpaths for drilling and tapping. After completing this lesson, you'll be able to create a drilling toolpath and create a tapping toolpath. Let's carry on with the file from our previous example and let's take care of drilling and tapping that mounting bus hole. At this point, we're going to select drilling. We're going to navigate to our tools, into our cloud library and we want to select the number 7 drill, tool number 3. In the geometry section, we need to select the location of the hole. Now I'm going to do this a little bit differently and I'm actually going to start the upper portion. So we're going to start all the way from here. And what this does is it actually selects the top section, as well as the bottom section of the hole. So it already factors in the height of that geometry. Now remember, this is a counterbore and this is something that we've already cut. So if we delete this and we select the actual hole, you can see that it is calculating it there as well. So, the tool is starting the feed where this green line is, and it's moving all the way down to the bottom of the part. We need to be mindful of the fact that the geometry in this file actually has a drill point in the bottom of it. So we need to make sure that we are drilling down far enough. So what we want to do is we want to just use this selection and move on to our heights. Notice that here we have this drill tip through bottom option. So if the hole went all the way down to, for example, the bottom of the part. We might want to use this drill tip through bottom option to add a small amount. And if we need to add a breakthrough depth, this is going to be based on the diameter of the tool. So, the diameter of the tool in this case is 0.201, we're not going to add any additional clearance, because this drill tip through bottom will automatically enable it. So we'll come back and we'll check this setting after the toolpath has been created to make sure we don't need to have any adjustments. For cycle, we're going to change it from drilling rapid out, and we're going to be using either the deep drilling or chip breaking options. You'll notice we're drilling if you hover the cursor over any of these options, we get a nice tooltip that tells us all about each of these cycles. Chip breaking is going to be a pack drilling cycle and the deep drilling option is going to be very similar to chip breaking or pack but it retracts all the way out of the hole. We're not drilling very deep so we're going to use the chip breaking option. We're going to leave the packing depth based on the diameter of the tool. There's a depth reduction that we could do. So, as we're going down, we could reduce the amount that we're packing. And then we could add a dwell to forward track, but we're going to say okay to all of these defaults settings that are based on the tool itself. Now what we want to make sure is that we're getting the tool all the way down to the bottom of that hole. And when we navigate to a side view, one thing that we can see is the location of that green line and the location of the bottom of the hole of the geometry. So everything looks pretty good in terms of the location of that hole. Before I move on to simulating this like I normally do, I'm going to go ahead and just create the tapping operation as well. We're going to again use a drilling operation, but this time for the tool, we want to make sure we select our tap. By selecting a tap, this is going to change some of the parameters. We're no longer going to have a lot of control over various parameters that we would if we were just doing a drilling operation. You'll notice that this first page changes, and the feeds and speeds are based on the parameters in our tool. And keep in mind that when we're using this rigid tapping methodology, that it is going to be important that the speed is going to be gear driven inside of the machine. It's going to have to stop the tab at the bottom and reverse it coming out. So, that speed needs to be linked to the feed rate of the z axis as well as the speed of the spindle. In the geometry section, the whole mode is going to be based on selection. But we could also select a point or use a diameter range. If we use a diameter range, it'll grab all five of the holes. So we're going to use the selected reference. We also have the option to select the same diameter and if we do that again, it will grab all the other holes on the part but this can help simplify our selection. Inside of this cycle, you'll notice that it automatically grabs tapping, so we can simply say okay, and now we've created that tapping operation. Let's select set up one, go into simulate, jump all the way to the end, then go back to operations. So we're going to play through and notice that we've drilled it, and then the tap comes in and it taps the whole. If we take a look at the preview on the screen, you'll notice that we're seeing gray here. And this is because the hole was created infusion using an appearance of a tap tool which means the actual diameter is going to be that 0.201. And it's not going to actually be a quarter inch which would be the major diameter or root diameter depending on if we're talking about a internal or external thread of that quarter 20 threat. So everything looks pretty good here and again, if we turn off the model, you can see that we've cut all the geometry. We've cut the boss down to size. We've done the counterbore, we've drilled and tapped it. We've cut all the pockets, and we've done our chamfer operations. Also remember that we were assuming that when we started this part, the four holes were drilled and tapped from the bottom. The bottom was already faced and bolted down to a fixture. This allowed us to create all the rest of the operations from the top without having to worry about holding the part or having any tabs on the outside that needed to be cleaned off. So everything at this point is done and cleaned up, so we can go ahead and navigate back to a home view and we can save our file before moving on to the next step.
