Sign in to watch this lesson

Hello, so in this video we're going to move on to external threading and then the drilling operations for this part. So first off, I'd like to take a look at where we're going to do the threading. We intend to thread this profile section here. If we go into the operations menu under lathe and then choose OD threading because we're doing an outer diameter thread.

You can see how it automatically defaults to covering the entire thing, so we'll go back to manipulating the individual handles to get it to just the area we want. To do so, we go into job assignment and then just move the handles across to where we need them to be. Now that we've got this, let's take a quick look at the rest of the settings for the threading. Under cycle parameters, we can see how the thread pitch is one millimeter, which gives us an M30 by one, a very fine thread pitch for this sort of thing, but it works for our needs.

The rest of these all appear to be okay to me, so I'm going to generate that toolpath now, and we have defined our first threaded part. We'll quickly simulate this, click run, and slow it down a little bit to ensure the path is coming in as we expect, and yes, that covers all of our parts there. If we turn on machining result visibility, we can see how we've got that threaded part worked out there. We'll have to turn off part visibility to see it clearly because the part visibility is the actual design as opposed to the finished part itself.

The finished part is the machining result, but for now, we can see that this perfectly fits our needs. We can now move on to checking out the drilling operations, and fortunately, because we've set this to a three-quarter view as defined down here, we can see into the part that we need to clear out these various sections. We need to ensure they're machined away according to what we want. So we'll go back into the machining environment, and under add operation, we can go back to lathe and then lathe hole machining.

The first thing we want to do is select the correct tool because at the moment, it thinks it's going for a 20mm drill, which is not ideal. We click on tool and then click on the select tool button, and in the new window that appears, we click on 10mm drill and select the tool for the operation. This is the perfectly sized drill to go all the way through that bore for us. We'll have a quick look at the strategy for this, and we don't want to leave it as simple drilling because that's just a straight plunge drill with no chip clearance strategies and no pecking or anything.

We'll click on the drop-down arrow here and choose chip removing. Okay, so that will not only break chips but will also pull them out by maintaining a pecking operation throughout. I'm going to click on generate toolpath now, and we can see here by how dense the red dashed lines are that there's a fair bit of forwards and backwards motion, but we'll simulate just to be certain. We'll slow this down a little bit, click on run, and we can see how the drill comes in and goes through, which is great, but it doesn't clear the bottom of the part quite as we want it to.

We'll go back into the machining environment now, go to job assignment, highlight this, and under properties, we'll turn on drill tip compensation and do it by drill tip. What that will do is automatically determine the extra length it needs to travel based on the angular geometry of this tip. Now we click on okay and regenerate that toolpath, and since we're machining, we don't really need to bother resetting this, so we'll just press run again and watch it go through. We should see it extend beyond this point, and there we go, that's now cut all the way through, which means that when we undertake the operation to move this part over to the other spindle, we'll be able to cut away a clean face there.

We'll have a proper hole bored all the way through. Back into the machining environment now, and we want to cut away this section, so I'm going to go with another lathe hole machining operation. However, this time the tool I'm going to select is actually not the 20mm drill again; it's the 20mm cylindrical mill. We select the tool for the operation because that gives us a flat base to work with.

We're going to move back to job assignments at this point, and I'd like to take a quick look at how far we're going to bring this down. I don't want this to go any further than 15mm down. I'm just going to move this around to ensure that we're definitely square onto it because at the moment, there appears to be something of a cant indicated. However, I'm going to roll this until it hits 15mm.

I'm going to generate the toolpath accordingly, and under properties, I'm going to ensure the drill tip compensation is turned off because this is a flat bottom tool. We don't want any of that to be implemented, even though there's nothing to implement given that it's a flat base tool; it's always best just to make sure. We click on OK again and generate the toolpath of the current operation, and we can see how that should be a nice clear plunge. However, under strategy, I'm not going to have that as a single plunge pass because I'm not a big fan of that; it's generally not very safe.

I'm going to go with chip removal again. It's not super necessary for an actual chip removal process per se since there's already a clean bore through there for chips to move into if needed, but for the sake of safety and diminishing tool load, I generally tend to default to using that. We're now going to simulate this, and we'll leave it at a fairly slow speed because it's not doing much of a cut, and we'll click on run now. There we go, and it still does it in a single pass.

We're going to go back to chip removing, and we are going to set the step because currently, that's down to 100% of the tool, which is 20mm in a 15mm bore. We're going to set that to 25% of the tool diameter, which means it should only go down by 5mm each time. We'll regenerate that now, simulate, reset, and then simulate up to the current operation, and then we'll run this. There we go, so we now have three clean passes there.

In the next video, we're going to cover the part changeover and machining the rear face of this to clean up the final parts of it. I shall see you then.