Sign in to watch this lesson

Hi there, so in this video we're going to cover the first of the roughing operations for our workpiece and we're also going to look at how we import tool tables. So first off I'm going to import the tool table as initially stated. So we're going to do so by hovering over this tool icon up here in the machining tab and we're going to click on import tools to the project and you can see here on my desktop I've got the milling tutorial tools. tom file.

Both this and the geometry file you're going to be working with will be available for download alongside this, so don't worry about that. And we can see here that we've got four tools defined in here, a 20mm cylindrical drill mill, sorry, a 6mm cylindrical mill, an 8mm drill and a 10mm conical mill. So for this particular operation we're going to start out with the 20mm milling bit but it will auto select that for what we're doing. So the first thing that we're going to do is we're going to take a look at doing a facing operation to take off that 2mm extra that I specified at the beginning of last video.

So we're going to go to add operation and there are a couple of different ways of doing this. We've got a drop down menu option which is for when you know where the operation that you want to work with is or we can also click where it says add operation and it opens up a window with a complete breakdown of everything that we've got as well as little example images of what the toolpath generally abides by and a few other settings as well. For the moment though we're going to be looking at 3D entry and we're going to be looking at face milling. So we're going to create this operation and we are going to check the tool to make sure it's using the correct one which it should be.

As you can see it's the 20mm cylindrical mill which is tool number 1 so that's perfect for our needs and we are going to click on strategy and we want to check the top level and the final level. So the top level is 0mm the final level is minus 2. That's predicated off the G54 that we defined. I know that previously when we set the G54 it said it was in positive 2 but obviously that's now defined as the local 0.

Beyond that we've got the spiral strategy, we've got a 75% step over. Everything there looks pretty much as anticipated. So we are going to generate the toolpath from this and we're going to take a look at how it machines. So we click on the generate toolpath button up here and we give it a second to think about it and we can see that it's already come up with a pretty logical looking toolpath that does exactly what we'd expect it to.

It's a spiral that runs from outside to inside, yeah that's pretty unambiguous. So we're now going to click on the simulation tab button so we can take a look at what it's going to look like when machining. Now of course something to note is with a milling machine obviously the table moves around so it's best to try and keep the viewpoint aligned with the centre of the spindle just for the sake of preserving your own sanity when viewing it. So I'm going to slow this down a little bit and I'm going to click on run just so we can see what the motions are likely to look like.

And so far there's nothing unexpected happening, it comes down to that zero point just outside the block and then it starts to move in. So I'm going to speed this up because otherwise we could be here for a while and there you go we have a perfectly formed spiral toolpath that clears off the entire top of the block without any cause for concern, I'd say that's a good start. So we're going to go back to the machining space now and we are going to clear up the rest of this area as well with another roughing pass, a slightly more complicated one this time though. So we're going to go back to add operation and we're going to go back into 3D entry again and we are going to grab the roughing waterline option and we're going to create that as a toolpath.

So first things first, we want to decide what it is we do and we don't want to do with this and I've already decided I don't want this to do anything about that central bore right now, I want that to be a completely separate operation that we approach later on. So to achieve this we're going to go to the job assignment tab here and we're going to select a restriction zone. So to do this it's best to grab a piece of very obvious geometry from the particular subset of the part that you wish to conceal from the calculation. So making sure that you've got edge selection available I am going to grab this bottom edge of that central bore and I'm going to click on restrict zone now and you can see it's blocked out that entire region using a red plug for lack of a better term.

That now means that when it's starting to put together the calculations to generate a toolpath for this operation it completely ignores that area, doesn't go near it, refuses to touch it, which is ideal. So now I'm going to move into the strategy tab and I'd like to take a look at the top level and bottom level again because obviously we need to make sure it doesn't go too far down because obviously it's going to try and take off these corners all the way down which it can't do because if it wants to go around the edge it's going to end up hitting the vice jaws and that gets a bit messy. So we ideally want it to come down to this face. Now the best way of being able to see for definite what the height of that face is, is if we click on the front or left view so we've got a perfect alignment there and we zoom in.

Now if we highlight the bottom level we can see that this green plane has been generated and it is a plane. Sorry I'll just snap back to the view there. And we can actually drag this plane. Because we don't know what that current numerical value is we can drag it to roughly whereabouts we want it to be.

It says minus 16 there, looks about right. And yes if we remember correctly it's at that 16 value that we were working with before. So that aligns pretty much perfectly. The last thing we want to take a look at is the depth step because obviously it's going to try and take off that entire thickness in one go.

Which yeah sure it's a 20mm end mill but that still feels a little unkindly aggressive. So I am going to set the depth step to, let's go with 50% of the diameter so that's 10mm. So we'll click on 50 there. And we are now going to generate the toolpath of the current operation.

So there you go you can see how it's now been divided up into a couple of different heights there. So we are going to move around so we've got a clearer view of everything that's going on. And we've got a pretty sensible looking set of toolpaths there. So the best thing we can do at this point is we can simulate to see exactly what it is that's about to happen.

So we'll click on the simulation tab again and we'll slow it down a little bit just so we've got a clear view of things and we'll click run. Now as we can see it's coming in from clearing up the corners initially which is pretty much what one would expect of a waterline style toolpath. And overall it's not doing anything particularly outlandish or brash. So I am going to speed this up so we can get through the toolpath generally.

You will have any errors reported here. This particular node colour will come up red if it has any problems or any concerns about what's done. As you can see the previous one came up perfectly green so that's all good. But so far there isn't any cause for concern being demonstrated.

And as we can see we've got a nice clean rendition of the toolpath that we wanted. So for the moment I think it's safe to say that we've got our roughing operations sorted and good to go. So in the next video we're going to take a look at dealing with that central bore and also dealing with the castellations on this section as well. So I shall see you then.