CAM Settings and Your Haas Machine - AutoDesk visits Haas Automation.

Recently, we invited CJ Abraham from Autodesk here to the factory to discuss the relationship between your Haas machine and your cam system. Now, a high-performance machine tool like this VF2YT with features like high-speed machining, G187, can easily underperform if your program was output with the improper cam settings. Now, before we get to the meat of this video, we thought it would be helpful to break down some of the key terms that CJ and I discussed in our conversation. That way, if this is the first time you're hearing some of these terms, this will make it a lot easier to follow along with the video. Let's get started with G187. You'll hear CJ and I talk a lot about G187 in this video. G187 is a feature that is standard on all Haas mills. Adding a G187 P1 to your program will increase accelerations, which means you'll decrease cycle times, but the tool may slightly overshoot or undershoot corners. This is most useful when roughing, when you want to remove as much material as quickly as possible. A G187 P3 would typically be used for a finishing pass. Now, P3 will slow accelerations, which means an increased cycle time, but a more accurate part. Tolerance refers to settings within the cam system that determine how accurately the program toolpath matches your desired shape. A tighter tolerance, or smaller number, means more line segments. Now, you might assume that this will make for a more accurate part, and it might, but there's a big trade-off. Too many line segments in your program may have so many lines of code that the machine can't process them all efficiently. This can result in not only a slower cycle time, but in some cases your machine will slow down or stop as it tries to process thousands of lines of code. To complicate matters, you should often employ a different strategy when roughing than when finishing. When we are roughing, it's all about speed, removing material as fast as possible, and you don't worry too much about accuracy or surface finish. But when it's time for that finishing pass, we'll often want to slow things down and end up with an accurate part and a nice surface finish. Now, let's dive into the topic now with CJ. Hey everybody, I'm Brian O'Falun from Haas Automation. I'm here today with CJ Abraham from Autodesk, and the topic today is going to be cam settings and how they relate to the Haas machine. So CJ, you've been here about half the day already doing some demos, and you're going to show us how some of these settings affect not just surface finish, but cycle time. Yep, so we're going to use G187, okay, and high-speed machining, all right, and also we're going to look at the tolerance settings for the toolpath so we can see accuracy versus machining time. Okay, so the cool thing that you showed me was a really loose tolerance, and we're going to cut a part here and show it, and it's really an awful surface finish. Yep. And so my first instinct would be, oh man, I got to tighten that tolerance up to some crazy tight number. And you did that, and you showed me what the part looked like, and the surface finish looked better, although it wasn't perfect, but all of a sudden the cycle time was just killed. Right, the machine had a hard time keeping up with all the points that we were feeding it. Okay, so what we've done where we had the loose tolerance, we had very few points, and that's why we had the bad surface finish, but now we went in the complete other direction, right? Yep. Okay, so really where you need to be is somewhere in between, I would imagine. Yep, and we can do that through arc filtering and some other toolpath settings, but basically we would like to take all the points that we had along a spline, and instead of feeding thousands of lines, we could just feed it a couple of arcs. So this is the part that you've cut, raw material obviously. Looks like a pretty simple part. Can you explain what you're doing? Yep, so this is just a simple spline, and it's just a worst-case scenario. There are no arcs in the spline, so we have to generate lots and lots of G1 linear moves. Okay, so the first thing you're going to do today on the machine is show us that worst-case scenario. So can you show me the tolerances that you've got, and how many points? Yep, so right in the passes tab, we have the tolerance setting at the top. Okay, we've got ten thousands, and how many points? You said that resulted in about 90 points. Yep, got it. Now, you need to know that this machine is set up with high-speed machining, which you will see is a distinct advantage, but when our cam settings are applied incorrectly, high-speed machining has no effect at all. So let's go machine apart. All right. Yeah, so I noticed when you put in the vise, you had no stops, but you don't care because you've got a probe. Right. Now, you're machining this part with high-speed machining, right? Yep. And we're gonna, we'll show a little bit later what it looks like without high-speed machining. Right, this is a combination of high-speed machining and G187P1. Okay. Okay, so our part's roughed out now. Okay. And this first tool path is going to be our loose tolerance tool path, so the 10,000. Okay, this is the 10,000 with the 90, roughly 90 points. Right. Okay, let's see how it looks. Commanded feed rate is 80 inches per minute. Okay. So we're at the full feed rate, but you can clearly see we got some faceting. Oh, I can see it already. Yeah. It looks terrible already. Yeah, so the machine motion was quite good. It was, but I can see I'm standing four feet away that it looks awful. Yep. I can see the faceting. I could probably go through and count all those points, all those 90 points right now. Right. Okay, so first reaction would be, let's tighten that all up. Yep. Right, so we're going to take the 10,000 tolerance, and I'm actually going to make it a 10,000,000 tolerance. Okay. Tiny. That's what I would do, right? If I didn't know better, I'd say that looks terrible. I can see those 90 points. I want 90,000 points. Right. So it takes that faceting out. Okay, let's see what it looks like. So this is about 2,000 points or 2,500 points. It's crawling. Yeah. So much better surface finish. Yep. But the machine's coming down to a crawl. And we're still, feed rate's still at 80, but it was very obviously not going as fast. Yep. It was slowing down, and you know what's funny? Even from this distance again, I can still, that's not a great surface finish. Yep. We're still working with lots of lines, and so we're going to have micro faceting on the part. Okay, so the problem that we solved to an extent was the surface finish. By adding more points, obviously we don't have those big facets in there. Right. But we choked the machine down with so many points, but I can still see those lines, and that's because the machine's doing exactly what we asked it to do, right? Yep. Instead of big faceting, we just have really tiny faceting. Okay. Now what you're going to show next is the best of both worlds. Yep. We're going to have good surface finish, but we're not going to have the faceting anymore, right? Correct. We're taking all those points that we generated, and we're filtering them into arcs. Okay. And that's something that the software does. Yes. Okay. Let's see it. So now we're both up to the full feed rate and have an excellent surface finish. And the machine is, yep, the machine didn't hesitate at all. Nice and smooth, and I can already see it looks like a beautiful part. All right, let's check them out. Okay, so now that we've got all three on the desk, we can really take a look at them. So this is the first one we cut with the really obvious faceting and a tolerance of 10,000s. And again, you can see it, you can feel it, it looks terrible. Yep. And we did what I would do, not being an experienced programmer, say, well, that looks terrible. I changed it to 10 millionths, and we came up with this. So it looks better when you look from a distance, but when you really look up close, you can still see all the lines. Right. It's the same effect that we have here, just with much smaller lines. Okay. And the program ran a lot slower. Correct. So we choked the machine down with so many lines. Yep. Yeah, even the high-speed machining option didn't pull us out of that. Okay. So I was going to ask you about that because I know we have the high-speed machining option on this machine, but it sure wasn't evident when you cut this part. Right. So even though we have the increased look ahead and the better interpolation, we still are feeding it too many points. Okay. So high-speed machining, whether we did G187, P1, P2, P3, all those things we talked about earlier, none of that would have mattered because of our cam settings. Right. Okay. And then finally, the good part. Yep. So within our toolpath settings, we turned on the arc filtering. Okay. So we specify a slightly different tolerance that will take all the lines and fit them into arcs where applicable. Okay. Right. So instead of lots of G1s, we had 2,500 G1s here. Yep. Now we're down to about 50 G2 and G3 arcs on this part. Okay. So same geometry, just a different number of points. Now, how as a programmer do I go from this to this? Can you show me how to do that? Within the toolpath. Okay. So you're going to edit your toolpath. Yep. If I look at the passes tab in Fusion 360, we have the tolerance setting. Okay. So this is the number that's controlling the three results that we got. Got it. It's these numbers here. Yep. And to do the arc filtering, all I need to do is turn on our smoothing option and this will filter those points into arcs. So literally you check that box? Yep. I check that box and I give it a tolerance of my choice. Okay. Right. And whenever the lines fits within those bounds, it will turn it into an arc. Easy as can be. Yep. So literally with one filter and one checkbox, you took it from this to this. Yes. Nice. Okay. So now we just went over cam settings. Yep. That was really fascinating, especially to me, to learn how just a tolerance like that can make such a huge difference in your part. But now let's take some of that knowledge and apply it to a real world setting. Right. So what are we going to do here? So we took the worst case scenario where we had our tolerance settings. Okay. And we're going to apply it to our high speed roughing strategy. Okay. So in Fusion 360, we call it adaptive clearing. And adaptive clearing generates a lot of points. Okay. Right. So we've chosen a tolerance that is appropriate. We've arc filtered it. Okay. Right. And now we're going to see how G187 can change the cycle time. Okay. Now I referenced G187 or maybe you did earlier. Explain what G187 is. We've got P1, P2, and P3. Three different settings. Yep. Explain the difference. So G187 P1 is the loosest setting. Okay. Okay. You'll have a great cycle time. Right. Okay. But it's going to round corners really quickly. Right. It has the fast acceleration. So it's fast, but not necessarily accurate. Correct. Okay. And then P3 is the opposite. It's the most accurate, but it's going to be a bit slower. So if you're strictly roughing, all you want to do is remove a bunch of material. You want to set, you want to program in a G187 P1. Correct. And you're not, you don't care about accuracy. You just want to get the material gone as quickly as possible. Yep. And that's what we're See how it really slows you down on those corners? Yeah. I was just going to say when you were feeding in a straight line, I thought, oh, what's the big deal? But then it comes to the corner and you can really see it noticeably slow down. Right. And that's because the machine is trying to take the most accurate path around the part. So whatever that radius is, the machine's trying to reproduce that as closely as possible. Right. This is really good for like 3D finishing, or if you're trying to finish certain features, because you'll have a very accurate feature. Okay. Just won't be a good cycle time. Got it. Yeah. I was just going to say, I can already tell the cycle time is going to suffer because it's slowing down every time it comes to a corner. It's even more noticeable now. Yeah. So we're already at a minute and 30 seconds. Okay. See, now I know we're going to do better on the next one, but I'd be willing to bet that most people look at that and they have no baseline. They have nothing to compare it to. And they'd say, well, that's just the way it is. Right. So I've hit option stop on here. Okay. We're at a minute 39. Okay. Okay. So let's put in a new one. Okay. So we've got a new piece of material and I'm going to change the G187P3. I'm going to change that to a P1. Okay. Okay. And that's the only thing you've changed? Yep. That's only thing I've changed. And this is the loosest setting for G187. Okay. By the way, before you get started here, if you don't program in a G187 at all, what do you get? You get a G187P2. That's the default. And P2 is default. Yeah. Okay. So we've got a P1 and this should go faster. Let's try it. Time to beat is 139. Okay. All right. Let's see. Oh, that thing didn't even slow down. See, but if you were trying to do that accurately, it would round that corner off, right? But we don't care because we're just moving with that. Great. All we want to do is get rid of all that material right now. It's really dramatic there. You can really see the difference. What cycle time? Down to 116. Wow. That's a huge difference. So 26 seconds, 23 seconds, if I knew how to do math, you can tell my engineering skills have fallen off. So from 139 to 116. And again, we don't care. This is just a roughing operation. If we were to come in here and do a finish pass, then we'd worry about it. But that's a dramatic difference. So now we've seen the difference between pure cam settings and pure machine settings, and it takes a mixture of both to really get good machine performance. Right. So the analogy we always use is it's like a recipe, right? If you're cooking something, you've got to have all the ingredients in order for the finished product to come out right. And machining is no different. You've got to have your machine settings and your cam settings. Okay. So that was an eye-opener, something that most people probably don't even think about, or maybe even know about G187, big cycle time savings. Okay. So we've learned a lot from you today. If I want to use G187, and I know I would with this kind of cycle time savings, do I program at the machine or is that something we do in the cam system? You can do it on both. Okay. Right. But in the cam software, all we need to do is select the operation to post. Okay. And then the post processor properties, I look for the checkbox that says use G187, and I just turn it on. That's it. Simple as that. Okay. So in this pocket example, I've got two toolpaths. Okay. The first one is adaptive clearing. It's going to rough out the pocket. That's your roughing. Yep. Okay. And I'd like to loosen up the tolerance a bit. So I'm going to go to the passes tab. Okay. Yep. Look for the tolerance setting, and I'm going to change this to four thousands. Okay. Okay. So that's nice and loose. That'll trigger a G187 P1. Okay. And that's, again, the cam system being smart enough to recognize the toolpath and the tolerance and applying that P1. Yep. That is correct. Okay. And now for the pocket, I'm going to right-click and edit the pocket. This is your finish pass. Yep. And we've already got a tight tolerance on there, but this is a spline. So we're going to get lots of lines again. So I'm going to turn on the arc filtering. Okay. And that's what we talked about here. That's the arc filter example we did at the beginning. Yep. So all you need to do is turn on the smoothing checkbox. Okay. Okay. And it has a tolerance associated with it. Okay. But I'm going to leave that tolerance alone for now. And then I click okay. And that's it. That's it. Yeah. Okay. So talk about what we're going to do here. So we're just going to mill a pocket. Okay. And the first operation will be a roughing operation, and that's going to use G187 P1. Okay. And then the second operation will be a finishing pass, and that'll switch over to G187 P3. Okay. Let's see it. We're going to probe it first, of course. Now, what is your tolerance setting for this part? For the adaptive clearing toolpath, I'm using 4,000. Okay. Right. So it's a wide tolerance, but we don't need too many points, right? We're roughing it out. We're leaving a lot of stock on there. Okay. And for the finishing pass, again, I'm using 10 millionths just to demonstrate. Okay. And then we've done arc filtering on that as well. Okay. Okay. So we're ramping in. What's your feed rate? Feed rate is 350 for the cutting feed rate. Okay. And you can really see the machine accelerating quickly between the passes. Yep. And that's from the G187 P1. And we already saw from before if we were running P3, it'd be significantly slower. Correct. And with the high-speed machining option enabled, it's really flying through the points right now. We've got a nice balance. Now, how fast would this go if we had through spindle coolant? Oh, we could push the tool way more. Right now, it's got a 100,000 step over. Okay. With coolant and all those things, we could go 350 on the feed rate, but do a step over 300,000, so more than half the tool. Now our finished pass. Yep. So this is using G187 P3. Okay. And the points have been arc filtered. So the wall is a spline. And I can already see the surface finish looks great. Look at that. Yeah, that looks awesome. Yep. Beautiful. It's pretty amazing how using the correct G187 setting made such a big difference in the roughing. I can't believe how quickly it removed all that material. Yeah. So we tied everything together by making this part. We number of points. We got some great visuals on that. Arc filtering, G187, like I just mentioned, high-speed machining, and then we tied it all together with this part. And if viewers want to see more content, we have a Fusion 360 YouTube channel. Okay. And we have a great video on adaptive clearing. Great. So they can learn more about adaptive clearing and how that works. Users can also reach out to me on Instagram. I'm very active. And we have a really healthy Instamachinist community. Great. Thanks again for coming out. We'll do more of these, and we'll see you next time.