Sign in to watch this lesson

Hi there, so in this follow-up video we're going to be doing something slightly different. We are using a part that's already been machined in the majority and we're going to go through the rest of the processes on this. Again this is purely exemplar stuff for dealing with the various hole machining options that are available to us. So first things first, I'm going to add a new hole machining operation and I would like to drill through this central bore at the moment.

So the 10mm drill, absolutely fine for that by default, that's not a problem at all. We are going to select the bore that we're working on, so I'm going to click on centre for there and due to the fact that there is a conical tip on a drill, I want it to drill through a little bit further. So I'm going to double click and I am going to set the height to 45mm, just to make sure it definitely goes through, so as we can see that kind of exceeds by about 3mm. It doesn't have to be particularly precise but given that we're going to be going through this with a cylindrical mill to take it out to almost final depth, afterwards we ideally want a breakthrough so there's no extra chip loading applied to the cylindrical mill.

So I'm quite happy with that, I'm going to generate the toolpath based on this. At the moment it's a simple drilling operation, so I am going to go with chip removal just because it's habit at this point and I prefer to. So again, I'm quite happy with how that works out. So for the next operation, we're going to go back to hole machining again and I am going to go with hole pocketing and we're going to change the tool to an end mill, so let's have a quick look and we'll grab a 16mm cylindrical mill, select the tool for the operation, that should be okay.

Oh, we have a slight clash there, so what I'll do instead is I'll just select that same cylindrical mill and we can see that that's gone now. So in case that was a little bit fast for you, what I'd done is I'd gone and grabbed the cylindrical mill and because it's part of the standard tool assignation table, what it did was it tried to generate a tool 10. 1 to differentiate it from the previous milling tool. We don't want that.

So when I selected the tool again, if we open this window up, what you can always do is you can just select from the project tools instead of from the toolkits and if you select from the project tool and you're reusing the same tool again, it will just grab the one that's already been defined. Anyway, so we've got that, we want to apply that and I am going to define the bore that we're going to be working with again, which is this one. I'm going to click on center, but what I want to do is I want to cut this slightly undersized for reasons that will become apparent a little bit later on. So again, double click on there and I am going to set the diameter to 26 and I'm going to click on OK and that should do the job.

So we'll generate that toolpath now and we can see a nice tight little spiral there forming. So that should give us a nice clean bored out central bore. Now the next ones that I want to do, I would very much like to do these blind holes here and these countersunk holes here. So we shall add another hole machining operation.

This time we are going to, hmm, let's start with a smaller drill just to start the holes off. OK, we'll go with a, let's go with a five millimeter drill. So we'll select that tool and we will let it go down all the way to depth on each of these. So yeah, that'll bore through cleanly.

OK, so first things first, we want to set our job assignment. So I'm going to select all of these bores and I'm also going to select these, but I won't select the base one because there's no point in pre-drilling those and I'm going to click on center and I am going to click on generate toolpath. Now as we noted before, it won't break through to the very, very end. It doesn't do automatic tip compensation.

So we'll just go down to the base with the tip, which leaves us a little bit of material to cut away when we're using an end mill to clean out the bore, but again, that's not a problem. So that's defined now. I'm going to add one more operation since the trouble is with doing these multi-stage hole machining jobs, there is invariably a lot of hole machining to do. So let's grab each of these again.

And center, and we are now going to grab an end mill. I think a six millimeter end mill should do the job nicely. So actually, no, we can push that up to an eight millimeter. I'm going to select the tool for the operation.

Now, as we can see, this end mill is a bit on the short side. So I'm just going to bump that up. Obviously, for the sake of argument in an actual machining job, you'll have an end mill of appropriate length for this sort of thing. But since we're dealing purely in hypotheticals here, it shouldn't really matter.

So I'm going to set that to 60 mil and I am going to set the shoulder length to like 20 just so we can see what's going on there and click on apply changes. And then we are going to change this from simple drilling to hole pocketing. And we're going to generate the toolpath. Now, as we can see here, we've got a nice tight little spiral working all the way down, which is exactly what we're after.

And it occurs to me that with the five millimeter drilling operation, we didn't set that for any kind of retraction or chip breaking or chip removal at all. So let's go back and fix that quickly. So we can see here, we've got it at a simple drilling operation. So let's go with chip removal and we'll click regenerate and we'll do the same for this.

Now, the penultimate job that we need to do is we want to go through this secondary bore here. Now, those are six millimeter holes. So we should just be able to do a clean drill all the way through. There's not a lot of material to account for.

So I'm not worried about chip breakage or chip removal. So if we add a very, very quick drilling operation there using a six millimeter drill. Let's have a look in the project tools. There's nothing there that fits.

So that's fine. We will now choose a six millimeter drill and select the tool for the operation. Okay, we'll now quickly select the bores. Let's hide the machine for the second to just do this easily.

Okay, I'm going to click on center. So that should be a little bit better now. Turn the machine back on so we can see where we are relative to everything. And as I've said, we're going to leave this as simple drilling because there's not really any great point in doing anything other.

And we'll click on generate toolpath. So now we've got those three bores. That's fine. I think it probably would be a good idea if we pushed and broke through a little bit further.

So let's very quickly do that. So we can select all four of the bores and adjust the properties. So the height is, shall we say, 10 millimeters instead of six. Now, bearing in mind that the height is actually based with the functional zero point being the top of the bore that is drilling.

So if we are to type in 10 now, we'll see that it extends down further through the base, which is exactly what we want. So we'll click on okay, and that bore should cut clean through. So now that that's regenerated, we're going to do something a bit fancy. Okay.

I would like to generate a multi-start thread going through this bore here. Okay. Obviously, this is just showing how to do multi-start threads. I'm not particularly worried about making sure I've got the correct geometry on the tool or anything.

You know, for the sake of argument, we can say it's trapezoidal thread or monogamy screw, depending upon whether or not you're working to ANSI or ISO standards. But it's very, very simple to do this in ANSI. So once again, we add an operation, we go for hole machining, and we define the bore that we want to work with. And we change the drilling type to by spiral, which is thread milling.

And you can see we've got a bunch of options here. So first things first, I'm actually going to change the tool profile. Just so we've got something to work with. So new tool.

And I don't think we've got any thread mills in the tool catalog by default. So I'm going to very quickly define a very, very basic one. It's probably not going to be the most accurate thing in the world, but it will do the job for this. So I'm going to go to tool type, and I'm going to go to thread mill.

And the diameter, let's pump that up to about 16. Put the stem diameter up to 10. That working length can probably come down a bit as well, because that's quite long. And I'm going to set the pitch count to one.

So it's only got one cutting tooth. And that should do the job for the moment. That is a very long tool. Let's say that's like 80 or something.

Not that it matters in real terms, but it looks a bit goofy. So let's apply the changes now, and we're going to create a new tool. So as you can see, that's defined its own tool number there, just to stop there from being any clashes or anything. Obviously, you can set all of those tool figures and everything according to what you've got in your machine carousel.

That's not an issue. So now the last bit that we're going to do is we're going to define the features of this thread. So we go back to setup, to strategy, my apologies. And the start count is where we can define how many threads are involved in this.

So say I want to go with four for now. And we want to change the thread depth. So instead of being based on a percentage of the tool, we want it to be a fixed depth. So in this instance, I'm going to go with two and a half millimeters.

Again, kind of pulling numbers out of thin air, but does the job. So that's fine. The initial angular setting is basically rotating it around the Z-axis as to where you want the thread to start, which obviously is important when you're defining something that has to make a specific fit. But again, that's down to your individual part.

In the case of this, we'll just go with zero because it works. You can obviously define whether or not it's a clockwise or counterclockwise thread. The compensation is where stuff gets a little bit weird. So basically, we've got a few different compensation modes.

We can do computer definition. We can do reverse wear or wear-based definition. Or you can just leave it entirely to your CNC controller's tool table compensation overrides, which again, those last three settings are largely predicated on the information that you have in your CNC machine's tool table. So our help texts are quite comprehensive about that.

We'll go into it in a fair bit more detail than I can in the space of this video because we're already at 13 minutes and I want to keep it under 15 if I can. Anyway, so I'm going to leave that on computer for the moment and I am going to set a count of three rough passes and one finish pass just to be safe. Last circle pass allows you to define a baseline ring almost at the bottom of it. So you've basically got thread relief down at the very bottom.

Stop any kind of vacuum lock, that sort of thing. But again, that's not relevant to this particular thread. So I'm not too fussed about it. The one thing I will say is that calculating this can take a couple of minutes.

So when I click on generate tool path, I will be pausing the video for a second. So don't think there's any silliness going on there, okay? I'll catch you in a second. All right, so we're back now and as we can see here, it's generated the requisite tool paths.

You can see the four different starting points here along with three roughing passes and a singular finishing pass. So what I'm going to do now is I am going to run through the simulation of what we've just done. Should hopefully be nice and quick. So I am going to bring us to this point and I'm going to simulate the current operation up to this stage because doing all the 5D stuff can take a couple of minutes, which is unnecessary.

And I'm going to click on run. So once it's worked out, it's a solid work piece. So we bypassed the initial whole machining and it's now going through that one, which is fine. And as we can see, it's coming in slightly undersized as requested.

So once that's machined right through to the bottom, we should start seeing the drilling processes come up. There we go. So as we can see, it's done the blind drilling. It's brought us down to the appropriate depth for that.

And again, each of these bores are going to be machined out of the cylindrical manner in a spiral manner, which will take a minute or so to render. So we can speed through that a little bit. The bit that I'm most interested in showing you is the multi-star threading. So that's the bit that I'm going to jump back on in a second.

And once this has come through, there's our four-point drilling. And we can see that we've got a very, very nice thread milling process and operation going through there. That's our first pass on it. So there'll be another two passes.

So the third pass and the finish pass on this one. And it will go through the same process again through all four planes, which is very, very quick and easy to set up. As you've seen with a minimum amount of fuss and is generally not a painful thing to do. So we have got an alert coming up here, which I'm guessing is going to be a gouge complaint or something.

Yep, gouge of the part. So this is a fairly common thing when doing threading processes like this in ENCY. If you haven't actually defined the thread in the initial CAD, sometimes it will come up like this. But remember, these warnings are purely advisory.

They're not show stopping. So for the sake of this particular part, we can always turn off gouge detections. That's just so we've got green across the board. But for the moment, I'm very, very happy with what I'm seeing here.

And I'm just going to very, very quickly accelerate through this so we can get to the finalized point of the job and see how it looks when it's done. And as we can see here, we've got all four lobes of the thread start forming there very neatly. Looks like a nicely defined thread. I'd call that good.

Anyway, I hope this has been informative for you. It's been a basic introduction into single point thread milling, as well as managing the various different forms of drilling again. But specifically, it was the thread milling that I was most interested in bringing to your attention. I'll catch you in the next video.

Take care.