Mill Turn 2.0 with Autodesk HSM

LAURENS WIJNSCHENK: All right. So good morning. As the first class, we're going to start it off slow. So I'm going to do a lot of demos and try and keep the Powerpoints to a minimum so you can actually see what's going on. A little about me-- this is a picture taken at my wedding this year-- so officially, I'm married now, even at 25. I've been a self-taught machinist.

My brother started a company in 3D design, and he got the chance to buy some machines. And from there on, the company took off. And I joined them, and I didn't know anything about machining or a metal work at all. But now we're here.

So I was going to say, I'm from Europe just like HSM. [INAUDIBLE] HSM, sorry. But I'm from the Netherlands, and HSM was from Denmark. But that didn't sound as cool, so we're both from Europe.

I was in the first customer advisory group that we started for the HSM products. Actually, I didn't start it. But [INAUDIBLE] started it, and I was one of the first guys to actually that, mainly because I was an active forum member-- still am. And I tried to push the software beyond its limits so we can give the best feedback to the HSM guys to actually-- what to develop next and how to give us better software.

So this lesson is about mill-turn. Then the question first is, what do, at least, I mean with mill-turn? We're talking about late-turning machines that actually half milling capabilities as well. It should work for milling machines with turning capabilities, but they're not as common. I don't have one myself. So we'll focus on the lathes with live tooling.

What I'm going to show you here works for Fusion, Inventor, and HSMWorks. They all look a little different, but beneath the skin they're all the same product. Where they used to have different levels in the software and for military and stuff we needed a more expensive license, now it's included in all the versions. So there's only one version of Inventor HSM and HSMWorks and only one version for Fusion. So you can all actually just use this when you've got a license to one of these three softwares.

So we'll start with turning, because that's what the machines were originally designed to do. One of the main differences with creating a setup and turning and milling is that the coordinate system has always going to be on the rotary axis of your machine. We're going to use what we call spin profile, which we need for if the part isn't completely round.

My main thing about turning, which we all seem to forget, is that we've got templates. And these will help you work so much faster. Yes, usually they're underused by everyone. So that's why I've put it down four times.

It's currently in heavy development by one of the guys that just came in. Angelo is one of the guys that you should talk about if you want any changes in the turning bit of the software. We've seen really big changes in the last few months, weeks. So that's been good.

So we'll start with the first demo that we made for you guys. So this our very simple turning part. By default, the setup will be setup as a milling setup. But if you actually do mostly turn and/or mill-turn, you can actually save this as a default so it starts the setup always in mill-turn, which I've done for some computers we use at work, mainly to program mill-turn machines and others that we mainly use for milling machines-- our setup with milling.

So if we see this part right now, we do not need the spin profile, because it's just one revolved shape. But the great thing is that if we create from a template-- these are templates we actually use on a daily basis-- I can actually just click those and it generates a path for me. This path uses just a rough facing operation, then facing [INAUDIBLE] finishing, roughing it out, and then finishing the whole part.

We can actually do the same for internal turning operations. For that, I do need to set the hole floor for the drilling operation. You can choose how you set up your template, with the drill always going straight through the part. The only problem with that is that your tool might not be long enough. Or if you've got a really long drill, you might be drilling 40 millimeters too deep. So for this I tend to have it just set to model bottom. And then for each different part, I set it up.

So I need to setup the drill. But after that, I've got these two turning operations. [INAUDIBLE]. And these generate with the selected parameters that we used to create a template. So if you look at this now, within a couple of seconds, we actually programmed most of this part. We should still do a grooving operation. And if we do it like that, even the groove is programmed.

Now, the funny part is that if you do the same for the other side-- which, I tend to just duplicate the setup so I've got the same stock lengths, stuff like that-- I click here to flip the z-axis. The only thing you need to think about if your stock is not in the center but offset from front or back, and you see if you flip the z-axis, the stock will actually move. So if your first setup is like this, with the stock offset from front one millimeter, when you change the z-axis, you also have to change this offset from back, and you actually have the setup the same as on your first operation.

If we now generate these paths again, it will try and cut the outside again. But there's one really nice button we can click in the setup. It's continue machining from previous setup, which means that it will actually look at the stock that's been machined in the setup prior to this. So you'll see that the roughing operation only does this little chamfer. So with that, I could even just remove that one and we can just finish that with a finishing tool.

And do the same for the inside. We can remove the drill, because it's been drilled through. And you see that it actually stops where it has been machined from the other side. Because if you look at these two together, they machine the whole inside of the part. But from the second side, you do not have to machine anything you've already done.

So that actually is the easy way to program a turning part. With templates, you can be done in a couple of minutes. Once you've set up templates for different hole sizes-- because usually you have different drills and boring bars setup for different hole sizes and lengths. So we've got a different-- like, here for drill with 20 millimeters, which has the correct boring bar setup to actually machine within the 20 millimeter diameter for 30 and 40. These three are for steel, and then up top here, we've got even different ones for stainless and aluminum.

So that was the quick way to actually program a training part. Then we get to the milling, because turning seems fairly easy. Like I said, it's available to everyone. Which it wasn't before, but it is now.

I put the Haas machine in [INAUDIBLE] lathe just to kind of show what the capabilities are that you get with using this. I'll be using tool orientation. Tool orientation is your friend to actually get tool parts that are not aligned with the z-axis. It might feel weird to just use milling operations, but we actually see that, in the end, it actually turns out great.

There's just a few rules that we need to look at with what operations we can use for what kind of machine. If you've got a lathe with just live tools-- so that's just x and z-axis, and you can use the main spindle as your c-axis what we call axial is any tool path that has the drill or end mill aligned with your z-axis. And radial is when it's aligned with your x-axis.

So you see that for axial, we can use any type of 2D, 3D path, and drill for a machine with just live tools, a machine with a y-axis, or even multi-tasking machines with the b-axis, which we have. And I'll show you a video of that later. When you're looking at radial tool paths, just a machine with live tools has some limitations. So there, we're mainly looking at slotting operations, 2D contour if the slot doesn't work for that, and drilling operations.

The 2D contour, for example, could also be used for wrapping your 2D part around a circle. I don't have anything to show you with that, but that would be possible as well. And If you move to a machine with a y-axis, actually, you get all the options that you would get on a vertical machining center with a fourth axis. So we can use any 2D and 3D operation, even four-axis operations. There are not that many in the software right now, but you probably should bug Al about getting that done. And then what the next step would be for multitasking machines is actually having tilted planes-- so not having to an axial or a radial tool, but actually having the capability of doing any plane you like.

So this is the part that I programmed beforehand, because I wanted to know if everything worked. But this is the kind of part that we see a lot on our machines with live tooling. So we've got a slot on this side and some holes with counterbores on the other side. And it's even machine on the outside.

So if we setup the operation again, here we do need the spin profile. So what this actually does is take it apart and it imaginarily spins it around. So it sees the turning solid that you're actually machining, instead of having using the x-axis.

So I can actually show you what happens if you don't use it. And it's probably a big battle for anyone trying to do this the first time, and then the tool paths look wrong. So you see here that the turning actually stops at the top of this flat and not at the round part.

So if we simulate this, you'll see it cut too much. So when we change this to turn the spin profile on, we actually get the correct paths. And you see that it just machines the chamfer and doesn't cut away too much.

Now, we've done the training on this side, we actually want the machine to slot. And to do that, we would just use the 2D slot operation. I'm taking a guess that it's the six millimeter slot here.

By default, the tool will always be aligned with your z-axis. So to actually change the orientation, we used the tool orientation [INAUDIBLE]. But usually it's to set the bottom surface of your slot. Pick the slot-- come on. Now, if we just generate, it will probably generate from the top of the part, which is not what we want. So we change the top height-- and we created our slot.

This is actually all there is to it. But, as always, there is a little catch. If we now try to post this with, for example, the Haas ST-30 post, which is for a machine that has no y-axis but just live tooling, you'll see we got an error, which is that the conversation offset was out of range. But actually, you see this error, which says the y-axis motion is not possible without y-axis for his operation.

Now, the first thing I would say is I do not need the y-axis for his operation, because it's just an ordinary slot. But it's something you'll experience very often if you actually get models from your customer or that the slot is not completely aligned with your z-axis. So in this case, if we look at it-- which is this one, I guess--

AUDIENCE: [INAUDIBLE]

LAURENS WIJNSCHENK: I'm a SolidWorks guy, with that in mind. So I just tricked it here with putting in a very small number. So it actually is not aligned with the z-axis. But it's something you'll see with models that are not designed by yourself. And the first thing you tend to do is blame the software or blame the post. But in the end, it usually turns out to be the model that's actually screwed up.

So if we now-- it's not done yet-- post it again, once we've fixed that, we actually see that we just got the movements of x and z and actually machined this part. Now, if we go to the other site, which seems a little more tricky, actually it's not that much harder to actually program. So we just take a drill, select all these holes, [INAUDIBLE] the whole segments-- that drill seems a little too big. That's better. We can actually just drill these holes and use an adaptive operation. Because we said, we can use any 2D or 3D operation for any axial machining.

So I'll just take a 10-millimeter tool-- it's at the bottom, because you do not need to get it to go any further-- and make it generate. Since I've just got a Surface Book here, it might actually take a while.

While it does that, we can actually program a 2D contour just to finish the outside afterwards. We use the same tool, put the bottom a little below, and outside should be roughed and finished as well. If you look at the simulation now, it doesn't rotate the part around. Which it would do on the machine, because it will be machining this with the c-axis instead of a y-axis, because it doesn't have that. But because all the smarts of that is actually in the post, there is no need for you to tell the operation that for the operation you can actually program it the same as it would be your three-axis machine.

So we can actually post these out. And as you'll see, you see x and z values instead of x and y. We'll get to how that works in the post later on.

So this is something, an ordinary part for what you would do with a machine with live tools. If we then go to a part that's a little more tricky-- so this is a part where we would actually need a y-axis to machine these slots-- we kind of start the same. Create your template, that's the easiest way to go. Generate these. Do the same for the inside

[INAUDIBLE] drilled straight through. Generate the turning operations. So what it actually does right here for the inside is actually pre-machine the square that we'll actually mill out afterwards. So if we now simulate this-- [INAUDIBLE] show this [INAUDIBLE]-- we actually see that where the square will be is now a circle. Because it actually pretty machine this with the turning. It does as much as it can.

You can, of course, limit it by diameter or width setting and confinement from the front or the back of a part. But usually, the roughing of a part with a turning tool is pretty fast. So we tend to actually do the roughing but not due the finishing. So we're not getting any lines with tools not being fully aligned between turning and milling. So for the turning operation, we could probably most easy set the outside radius for the finishing one to there.

So now, I would actually want to rough out the pocket, which we again can use any 2D or 3D operation. But we're going to use a 3D operation, because then it can actually use the rest machining. So it can actually see what has been machined by the operations. So there's no need to redo that. We're setting the boundary to machine inside the square in this case. I didn't select the bottom.

So now, you see that for the roughing operation it actually takes notice of what has been machined by the turning operation and only roughs out the remaining stock. So these two actually see what the other has done. It goes the other way around as well. If you first machine it, mill it, and then afterwards turn it, it actually knows the stock has been removed, and it doesn't cut it again.

Now, we want to machine the outside of the square. We'll be using, just to show, the Haas ST-30Y, which has a y-axis of just over 100 millimeters. So this square would be too big to actually machine with the y-axis. So you got to have a vision on how the machine depart on a given machine. There's no way for the software to tell you yet that it's outside of the machine limits before you actually post it. And so that is something that probably will be improved upon in the future when you get a machine configuration, so it can actually tell you the machine only has 100 millimeter of y-axis travel.

So we cannot do this operation. But for now, you would get an error only during posting. So it's just a lot more convenient to think about what you're doing before you actually start he programming. So we could actually use the same adaptive but now give no boundary and set a bottom to below here to machine the outside. And we should probably finish it as well.

So now, all the axial tool paths that I would be planning on this part are done-- are still generating. But radially, we want to machine these slots. And since it's a y-axis machine, we can. These things just take a slot operation again. But I didn't set the tool orientation yet, so it still thinks that it's got a machine to slot axially.

So we've set the tool orientation. It shows us the correct slot. Set the top height. And now we created this one slot.

We can actually do this for all four sides, but it's a bit of a pain if it's getting to 20 or 50 different sides of the same part. Well, you're actually doing the same upward same operation, so it's easier to just use a pattern and duplicate it around this cylinder four times. This also has advantages later on if you want to play tricks on retracts in the post, then you can actually say, if it's patterned, we know it's the same tool, it's the same kind of operation, so we don't have to do a full retract, which I can actually show you in a minute as well.

But if you now post this with the y-axis post ST-30Y, you'll see you get four different slot programs. In theory, we could actually make a sub program, and then call that, and afterwards rotate the c-axis. But since most machines do not care about the amount of lines of code too much anymore, because their storage is big, most posts are set up to just output the code in one file. So you see here it starts at c0, uses the x and y movement to make the slot, and here it's at c minus 90. And so it does all the four slots.

So up until now, you're probably wondering to yourself, how can it actually be this easy, that I can actually just take any operation I could use on a milling machine and put it on a turning machine and get the right output for that type of machine? And if you ask [INAUDIBLE], which is the main post guy for HSM, he'll tell you that, as usually, all the smarts are in the post. And in this case it really is, because we can machine usually the same part, if you've got a y-axis machine, with using the y-axis movement or using c-axis rotation to mimic the y-axis.

And there's two versions of that using polar interpolation and just giving out very small line segments with what we call XZC mode. We've got generic posts for a lot of different machines now. So for Haas, you can probably find any model they make online. They fully set up. For Siemens, Okuma, and Doosan, I've probably been the one to help create those ones, because we've got machines with those controls. And Mazak is now being finalized, I know, as well.

But to have the post actually know what the capabilities of your machine are, we need to set it up. So we need to tell the post that if we've got a y-axis, for example, and what the limits of the y-axis and the x-axis are. About pulling interpolation, if you look at this picture that I took from the Okuma manual, the red lines, if we want to machine that's square, we can use x,y,z if your machine is capable, or actually use c values to move the part around so actually your tool can get to any side as well. I've got a video to show that.

You saw myself just standing there setting up the machine. Just facing off the part with the lower turret, because this is an Okuma Multus U3000. We've got a lower turn on it and a milling head. This is all programmed straight from Inventor HSM. I'll show you the part in a minute.

So now, we'll get to the milling of the same kind of square. So this is just with x, y, and z motion like you would do on any three-axis milling machine or five-axis as well, finishing this sidewall. So if you have a y-axis, this would usually be the way you want the machine to machine, because it's most accurate to do it this way.

Yeah, it's not always possible, for example, when the tool path would be outside of your y-axis range. So I'm changing the part right now-- waiting for the door to open so I can actually change the part. I forced the post to actually use polar interpolation here. So by default it uses the y-axis. We can force it as well.

So we're doing the seam facing operation. I turned down the rapids a little on the machine, because I just had the GoPro sitting on top of the milling head, and I was kind of scared that I would just fall off. So the machine can actually go faster. But now you see, we're not using any y-axis movement, but the c-axis is rotating.

I could actually show you the same movement for what we call XZC mode, because the movement on the machine would actually be the same. But there's a reason we've got both of them. We used polar interpolation here, which usually tells the machine-- it gives it x, y, and z-coordinates, and the machine actually converts that to c-axis motion.

We do this because with that you can actually use cutter compensation, which you would probably want on machining just a pocket or a [INAUDIBLE] like this. The setback of using pulling interpolation is that many machines do not support any drilling cycles or any other type of cycles with this kind of interpolation. So for any drilling cycles, we need the post at least to be able to give out x and z-values to actually rotate the part correctly to drill the holes.

Then you would probably say, why not use XZC always? Well, that's because you don't have the option to use cutter compensation anymore. It also depends on your machine if the post will choose one or the other. For example, Haas machines turn out to not like polar interpolation very near the center of rotation. So for that, they actually do XZC motion, again, if you will actually cross the rotary axis. So all that kind of smarts usually is built into generic posts, and you don't have to do anything about that.

AUDIENCE: [INAUDIBLE]

LAURENS WIJNSCHENK: Yeah, we didn't. But it might actually be a similar issue indeed. If you come very near to the rotary axis, it tends to have problems. Yeah, we already had the video.

So for the machine configuration, you see a part of the Haas post processor on the left side and a part of the Okuma mill-turn post processor on the right side. For the Haas, this at the very top of the post. So it says got y-axis, true. Because this is the ST-30Y, 30y has a y-axis minimum, a y-axis maximum, and an x-axis minimum. Those are the most important parts if you're just setting up your ordinary mill-turn0 machine-- or actually, not the Okuma, but the Doosan and post. So you can actually see that they put a define machine function in that post, so you can see in the post properties if it's a Puma machine or a Lynx. And it sets these values automatically for you.

But in the end, it's the same things we're looking for it to setup-- has it got a y-axis, what's the y-axis minimum and maximum, stuff like that. So if we actually go to a post like that, which is for a machine, got y-axis is usually the thing you'll find easiest. It also here has the actual minimum and maximums the y-axis needs. But also it needs to know the minimum of the x-axis. Because if you would use x and y and it would go too low, it would have to use the polar interpolation or XZC mode as well. So all these kinds of things are actually built into the post and make it work for you.

Now, if you actually want to force it, most of these post processors have the function built in that if you go through to manual and c action and say use polar mode, it will use the polar mode for the next operation in the tree only. This can happen that you want to do this if, for example, all the tools would be in the way if your using x, y, z. So the machine would actually be capable of doing it with the axial strokes of the axes. But other reasons cause you to not want to use the y-axis.

You can force it. So if we would just use this 3D contour, this would be the x, y, z motion. For some reason, no. Let's use the Okuma one. So you see, it's a very short program which just has G1s for x, y, and z to move around.

But then if we force the polar mode-- [INAUDIBLE] straight over, that's fine-- we see G137 C0, which actually turns on the polar interpolation. And we still see x and y values, but with a G100 for the Okuma post to actually know that it needs to make straight line segments while using the rotation of the c-axis, just like you saw in the video we just had. And then if you force x, y, z motion-- that's not [INAUDIBLE]-- you see you get a very large amount of very short line segments. Because in XZC mode, the machine cannot actually machine a straight line on the part, because it will rotate the c-axis and the x-axis to the given coordinates.

So if you just would program a straight line in your mind, it would actually cut into the part. So it gives a lot of tiny line segments. So it usually will actually make your machine run out of look-ahead and stutter if you want to do roughing operations with this.

We should have another demo. Yes.

Another thing I would want to show you is that by default-- I'll first show you the part we're making actually. This is this part, which is used as a fan to cool during an operation for a float hill. So they put this on the tool holder. So what we're doing here is milling out a part and drilling most of the material out so the end mill doesn't load up with aluminum and then finish the rest of this slot and the rest of it actually on the other side. So we only machine to half of it and machine rest on the other side.

But when you get your generic posts, by default it's made to be safe. So what it does is do a full retract between any kind of plane changes. This is the same for any ordinary live tooling machine. So it will do a full retract in x and z usually before rotating the c-axis to the next orientation.

So if you look at it like this, a lot of time is wasted. Because there is no need for the machine to move all the way back all the time. With the milling, I tend to think it's fairly OK. Because usually, the milling takes longer than drilling a couple of holes, for example, so it doesn't feel as bad. But now we're doing the drilling of the holes, and it really feels very bad to go all the way back, rotate the c-axis, and then drill the next hole.

So what I did by default in our post, is that if any operation is patterned around the c-axis, which we can just check for in the post, we'll always only do a retract in the x-axis. This is by default. So if I just program any part and pattern it, it will only do to retract in the x-axis, change the part, rotate the part, and come back in. It saves a lot of time already.

But as you can see, of course, it's not the optimum path that you would actually want. So for the drilling, for example, it already looks better. But the way the Okuma actually prepositions, it still moves in z a little, and it's still a lot of movement that would not be necessary.

So what I actually did is create another manual NC action, which I put in a template as well. And I've called it [DUTCH WORDS], which is just the Dutch version of "short retract." And with that, having putting that in front of the pattern, you'll actually get a tool path looking like this.

So while you cannot simulate or control this during the programming, you can actually do a lot of it in the post and get close to an optimum tool path without too many retracts actually machining your part. This is the milling. But especially for the drilling, you'll now see that it saves a lot of time.

So if you're able to edit your post a little-- it's not the most complicated stuff that I did here-- it can save you a lot of time when actually making apart. Stuff like this is just logic built into there. So I check for if the cycle is patterned, yes, and if I put in the short retract manual NC before this. And then the post knows that it's allowed to do this.

With that one, I actually said I want to be able to turn it on and off, because I might want to be able to do 20 operations with just a short retract. But the post, again, is smart enough to know if it needs to do a tool change, for example, that it actually does a full retract to the home position and then does the tool change. So there's no need for me to be scared that if I put in short retract between different tools that it will actually crash, because it doesn't go to home. It will actually go to home as well. So in the same time as the other ones would have drilled a couple of holes, we actually did the whole part now.

I can show you-- so this actually is the part that causes this. Before it sets the work plane for the b-Axis, it checks if the current section is patterned. And if I gave in short refract, in that case I just write the comment in the NC code. There is no retract, because I gave in the manual NC. So I can actually know, in the code, what's going on.

Otherwise, I check that if the current section is patterned and the b-axis will be on the same orientation for the next operation as it was for the previous one, then I can just do the x retract, because that should always be fine. If both of those cases are not valid, then it does a full retract in x and z to the home position of the machine.

So that was my short introduction to mill-turn with Autodesk HSM products. I hope you learned something. And if you've got any questions, please feel free. John.

AUDIENCE: On your polar interpolation video, it looked like you transitioned from an adaptive to a contour [INAUDIBLE]

LAURENS WIJNSCHENK: Yes.

AUDIENCE: How did you do that?

PRESENTER: So Laurens, just for the purpose of the recording, could you repeat the questions.

LAURENS WIJNSCHENK: Oh. So what you're asking is that there is no retract between the roughing part of the adaptive and the finishing of the 2D contour. Actually, there is a retract in z.

AUDIENCE: [INAUDIBLE]

LAURENS WIJNSCHENK: Yes, I can actually get it back. Otherwise, it would have cut straight through the part. But it was real quick. Yeah, you can see that with this part actually, the machine cut the corners a little. This is a problem that still needs to be fixed in our machine.

AUDIENCE: I was wondering about that.

LAURENS WIJNSCHENK: Yeah. I actually heard today that there should be a software option to fix this. I actually made some people angry complaining about it.

AUDIENCE: [INAUDIBLE]

LAURENS WIJNSCHENK: Yeah.

AUDIENCE: When you duplicated the operation [INAUDIBLE], you didn't define the sub-spindle turning [INAUDIBLE].

LAURENS WIJNSCHENK: So you're asking why I didn't put sub-spindle when I duplicated the setup for the other side. That is because, in theory, I didn't program anything to actually grab the part and moved it to the sub-spindle.

AUDIENCE: OK.

LAURENS WIJNSCHENK: So this would have been a manual change on the main spindle. But here, with this part, we actually machine it in one go with the sub-spindle. So there you see the secondary spindle check operation returning the sub-spindle. And then here, this setup, as you can see, actually is set to the secondary spindle.

AUDIENCE: Because that reverses all in the z-direction. And so the it does everything it needs to do. Or is that [INAUDIBLE]?

LAURENS WIJNSCHENK: So if you're asking if this button actually reversed the z-axis motion and stuff like that. In the software, the answers is no, because that's all done in the post. Because it also depends on the kind of machining control you have. For example, the Okuma machine, I just give in that it's sub-spindle work, and I can actually run the same program that I made for the main spindle on the sub-spindle with just changing one G code.

So the z-axis was reverted by the machine. Whereas, for example, by most FANUC machines and the Haas machine, you have to do this c-axis reverse and then actually do the smarts on if the y-axis need to be reversed as well and the c-axis, which we had a lot of problems with when we first started the Doosan mill-turn post. So this actually, the software always creates a positive z away from the part. But the post can actually change that to suit your machine, if needed.

AUDIENCE: So when do you decided to use [INAUDIBLE] axis, [INAUDIBLE] and how do you go about it?

LAURENS WIJNSCHENK: So you're asking if when we used to b-axis for turning and when we would use the lower turret? Or if you're asking, how do we program the b-axis turning?

AUDIENCE: Yeah. So if I were going to choose to use the [INAUDIBLE]

LAURENS WIJNSCHENK: To actually program anything with the b-axis at 45 degrees?

AUDIENCE: Yeah. For example, which a lot of tools are made to specifically do, we use something which I tend to call witchcraft to anyone. And to do that, we see that this tool, for example, we put 45 in the vendor, and the post actually looks at that and puts the tool at 45 degrees. And this is because the software just isn't capable of rotating the tool 45 degrees and keeping the compensation point at the correct point where you would want it.

So I'd love for this software to fully do this. And I tend to always say, we're this close, but we just need to finish up some small hiccups, then we should actually be able to use what's in the operation here. There's a tool orientation, which you could put at 45 degrees, It would actually rotate the tool 45 degrees. The only problem with doing this right now is that the compensation point of the tool would be at the wrong position. So we cannot use that yet.

But if we look at [INAUDIBLE] closely this week, we might actually be able to force him to fix that for us.

PRESENTER: [INAUDIBLE]

LAURENS WIJNSCHENK: So it shouldn't be hard. And it should help us a lot.

AUDIENCE: [INAUDIBLE] the post and the descriptors are [INAUDIBLE]

LAURENS WIJNSCHENK: About the Visual Studio-- it's something that was released, I believe, a couple months ago, which George Roberts made. So it actually looks for the function list, for example. And you could actually post straight from here given files that are in here, like CSV files that it can actually machine. So it was made to make it easier to edit posts.

But you can actually do what, by default, most people do, is if you click open config right here while doing your post, it opens in-- at least if you've got a vendor HSM or HSMWorks, you get the HSM edit software. And it opens in there.

PRESENTER: I'm going to do a video on that today. [INAUDIBLE] And I think maybe you had a more generic post questions, and there's no post classes. So to quickly explain, post and [INAUDIBLE] is written in JavaScript. And something you should be aware of is that it has access to every bit of data the CAM system was created.

So through the post engine, think of it as though the external API to get data, [INAUDIBLE] CAM system and put into an external source. So you have access to solids that were created for the stock and the body of access to request STLs of tools. You can get more than just motion data. So think of the post engine engine as your external API to access [INAUDIBLE]

AUDIENCE: [INAUDIBLE].

PRESENTER: Yeah. So we're [INAUDIBLE]--

LAURENS WIJNSCHENK: No, no, no. If you ask me, there's actually a difference in you would want some control of this back into the software. So as someone that speaks to the development quite often, we've discussed, would you want a box to select polar mode or x,y,z mode in an operation, stuff like that? But on the other hand, it's really convenient that all of these decisions that you should have made yourself in most other kind of systems, like select if I wanted to use one or the other, because otherwise it wouldn't work, are all done for you. So we need to find a middle ground between automating it still so it selects the correct version for you, like it does with the post now, and being able to overrule it and change to the one you would want.

PRESENTER: So I think there's two pieces to that questions too. One is, do you have to build your own post. And the answer is no. Laurens has done considerably more working with our post authors. But many of these posts are already built. [INAUDIBLE] on post works, [INAUDIBLE]. But you can just download those. You shouldn't have to do it.

Post logic allows us to make very specific machine decisions. Then the question is, how do you visualized this? That's more a questions of how we make the post made make it back into the simulation so you can see what happened. So the net result is you want to see the results of the post in the software. How we get there is maybe mechanically different than what you're thinking about. But we're very well aware of decisions made in the post need to be visualized in the software.

AUDIENCE: [INAUDIBLE]. Are you going to keep the post and [INAUDIBLE] or are you [INAUDIBLE]?

PRESENTER: We'll move as much logic as we can into the software to make the decision when the tool path is being created. And that's happening. Like, some of the kinematic decisions already get passed to the post, so it has the answer before it runs. But the other piece of the there's always stuff that's going to happen in the post, so that's a little bit more of taking some simulation data and feeding it back into the CAM system so you can visualize it.

It's a bit of a chicken and egg, where you want the flexibility to fully define what the machine does, but then you want to see the answer back in the software. We could talk all day about post though, so it might be better to--

AUDIENCE: [INAUDIBLE] Thank you. Do you know a way how to save automatically the current post configuration as a new version. Because when I [INAUDIBLE] the post processor [INAUDIBLE] times. And I'd like to version it automatically-- a way how to do it in Visual Studio code.

LAURENS WIJNSCHENK: I'm actually not aware of how to do that a Visual Studio code, to just make sure [INAUDIBLE] happens. But this is something you'd probably ask [INAUDIBLE], which I can just--

PRESENTER: [INAUDIBLE]

AUDIENCE: Thank you. [INAUDIBLE]

PRESENTER: I just want to remind to rate Laurens's class. He went first, so that should give him a couple bonus points. But it's always helpful for next year.

[APPLAUSE]