Speeds and Feeds: Tooling and Cutting Strategies to Improve Parts and Profitability

JOHN SAUNDERS: Welcome to my talk on speeds and feeds. I'm actually pretty excited about this. As I've gone through my journey of machining and manufacturing, I've come to learn and appreciate a lot of things. I think speeds and feeds are a really fascinating topic, and I think they're-- it's not to say that they're underappreciated, but I think there's probably a lot to be gained or a lot that people are leaving on the table.

The goals of the class, let's talk about what speeds and feeds actually are. Let's really dive into some terminology. My hope is to raise the level of knowledge and awareness so that we establish some common baseline. Obviously, a 60-minute class, let alone a week-long class, wouldn't be able to give you all of the answers.

But every time I hear a buzzword or a terminology or a term, I want to help you guys learn what you can do after this class to do something better, or to learn, or go research that issue-- so dive into some best practices and troubleshooting-type of stuff, and then again, resources going forward beyond just what we're getting into today.

My name is John Saunders. I run a shop called Saunders Machine Works. I'm a self-taught machinist. I got into this because I was trying to bring a product to market. And if you go watch some of my earliest YouTube videos on my tag, I couldn't get a face mill to work or a fly cutter to work. It was a high-speed steel insert bar. And I thought maybe if I turn it at 6,000 RPMs, it'll give me the recipe I'm looking for. So we all start somewhere.

I'm proud to say now I realize how dumb that was. But seriously, it's not obvious why things happen the way they happen. It ends up that that tool was not doing well because I had it mounted in there incorrectly. It wasn't just the RPM issue.

But I enjoy doing what I'm doing. I run a YouTube channel called NYC CNC where we put out videos on how to make stuff generally around the machining world, but also a topic that I very much like, which is manufacturing entrepreneurship. So it's not just the process of CAD or CAM or Fusion or machining, but rather the context of making this my life or making it your life-- hobbyist, weekend warrior, entrepreneur, working at a big company, anything of the sorts.

It's called NYC CNC because I started this when I was in New York City. I'm now back in Zanesville, Ohio, with my wife and two kids. And again, very much enjoy that I get to do what I do.

So if somebody were to ask you what are feeds and speeds, it would not be incorrect to say, OK, well, we've got a probably-- it looks like a half-inch four-flute tool. And I'm going to tell you, fun fact, feeds and speeds. So I'm going to tell you, ah, 0.002 of an inch and 300 surface feet per minute. So that's not an incorrect answer.

But what I want to do today is look at speeds and feeds more from a contextual standpoint of why are we doing this. So the number one reason, certainly for folks that are new to machining, new to a machine tool, new to a material, is going to be, I just don't want to break the tool, or some version of success. Like, I want to make the part. I want to make the part with some decently good outcome. I don't want to snap it off. I don't want to have chatter. But it's kind of an avoiding really bad outcomes.

The second reason is starting to do more of a, let's optimize something. So I put ROI up here. I don't think anybody is doing an actual financial return-of-investment calculation on a tool. But I will tell you, when you move into production, you will start doing more of an analysis of what is that cost of that tool, what's the life of it.

But really what I mean here is, is a tool being pushed hard enough? Is it the right tool for the process? Should I switch things up? Is it giving me the right outcome for the whole scenario or environment? So trying to optimize things and make more money, make something safer. Yeah, go ahead.

AUDIENCE: Or should I spend twice as much or half as much on a different tool?

JOHN SAUNDERS: Exactly. Yeah, so that's actually the fourth one. But the third one-- thank you. I appreciate you-- is finish or some equivalent. We've probably all seen on the Instamachinist post insanely good mirror finishes. Or maybe it's something more technical where you actually need a specific Ra as a bearing surface.

Or it's a pre-ream bore, so you care about that. Or there's some really cool tools called burnishing tools that will actually take the peaks and valleys left from a boring bar or a turning tool, and that actually cold flow-that material out. Well, in those situations, you very much care about the finish, but not from an aesthetic standpoint, from a tolerancing or some other standpoint.

And then lastly, the Buy tag here is a backward look at speeds and feeds and tooling, which is not, if I open up my tool box, what is the best tool to grab for the job at hand? But rather, what is out there in the world? Like John said, I would be willing to spend a huge amount of money if I knew it were the right tool. So how do you go figure that out?

When it's a hobby-- and I can vividly remember buying my first $8 end mill and thinking, oh, my god, this needs to last a really, really long time. Now we probably literally spend hundreds of dollars a week, sometimes a day, on tooling. But nevertheless, I care, as an entrepreneur, as a shop owner, as the guy that writes the checks. I'll buy the $800 Sandvik face mill if it can do what I think it can. So how do you get to that point to make that investment?

So speeds and feeds aren't just speeds and feeds. They are the material you're cutting. And this may seem obvious. You may be saying, well, of course it is. And when you think about something like an end mill, most machine shops intuitively or unintuitively say, oh, that's our quarter-inch end mill for aluminum, or that's the tool we use in steel.

And I agree. That's very normal. But who here actually keeps a set of high-speed steel twist drills separated by material? I would argue nobody or very few folks. So you have a lot of mixed materials or cutting tools where you share the cutting tool across different materials.

What machine tool are you running it in? Again, probably an obvious point, but nevertheless, it's not always the first thing that people mention. And when you pull up a manufacturer's speeds and feeds PDF, there is no mention of the machine tool. That's actually a really important part of it.

And then lastly, something that I think is not just neglected but more relevant than people realize is the holder itself. How are you holding onto that tool? ER collets are very common, and they're great, and we use them. But collets can compress under load.

And I think Rob Lockwood did a good job in his presentation of clarifying that he is not an expert or an engineer. I am not an expert, but I've become pretty fascinated with it. So I share this much as a layman in practice and not as somebody who is, by any means, formally qualified. But the tool holder matters. How are you holding onto that tool? And then the gauge length, the overall length of the tool, the stickout, et cetera.

But it's not just that. So that's what takes speeds and feeds to the next level. This is my quick-ish summary of many other factors that will play a role in speeds and feeds-- work holding. How hard are you holding onto that work piece? Is it moving? How hard do you want to go at it?

Fun fact, I love superglue. It might change how you machine that part-- not just because of the work-holding capabilities of superglue, but because superglue and, in our situation, the tape that we use for it, are more affected by heat than other things in this stack of cutting recipe stuff.

The coolant that you're using-- we'll come back to many of these-- chip evacuation. Coolant plays three roles. It actually lubricates the cut. It will provide an actual transfer of heat away from the tool or the part. But most importantly, at least for most of us, most importantly, the role that coolant performs is getting the chips out of there. We'll come back to this again.

Stickout or gauge length, toolpath style that you're using-- we probably take it for granted the value that adaptive toolpaths bring to us, but it's not to be taken for granted. It massively changes the types of tooling that we can use and the capabilities that we can get out of lighter-duty machine tools.

The hardness of the material, whether it has a hardened scale on the outside, is it flexing in the cut, the effects of chip thinning. I don't throw these up to antagonize you, but rather to hopefully introduce the fact that there are so many more complexities to what will result in a successful cutting recipe.

So I think it's awesome that we live at this point in history and in mankind. There are more-- I have no data to back this up. There are more people using more types of machine tools than ever before in the history of mankind. And conversation to AU include folks who are using machines like [? KUMA ?] at one point at a time in their day, and then they're using a machine like a ShapeOko hours later.

Our story has been tied a lot around the Tormach machines, and we're moving upward into the vertical machining centers. And you may have a 3/16 end mill, and that end mill may be a great tool for all three of these machines, but with very different cutting recipes.

So again, what are speeds and feeds? 300 surface feet per minute, 2 and 1/2 THOU per tooth-- I tried to be kind to the non-imperial folks here to throw in the metric equivalents. So that, again, is the basics.

What is cutting speed? The textbook definition is the speed difference or relative velocity between the cutting tool and the surface of the work piece it's operating on. I don't really enjoy that definition of it.

The real question is, why do we use surface feet per minute instead of RPM? Wouldn't RPM work? And so the example is the two millennials are going down the sidewalk on a bicycle and a skateboard. They are traveling at the same rate of speed so that they can have a conversation. The bicycle tire and the skateboard wheel, are they traveling at the same speed or the different speed?

AUDIENCE: Different.

JOHN SAUNDERS: Huh?

AUDIENCE: Different.

AUDIENCE: Same speed.

AUDIENCE: Different.

AUDIENCE: Different relative to the surface.

JOHN SAUNDERS: Yeah, so it depends. They're potentially traveling at the same surface footage, but at different RPM. So surface feet per minute is simply a-- or surface speed is simply a term that lets us give you the number you need regardless of the diameter.

Now, here's the thing. Who here remembers carpet burns? Carpet burns-- hopefully as a kid. If you're still doing it as an adult, god bless you. Carpet burns are the relationship between your skin and carpet, and they don't really occur when you're going at a certain speed. But when you go too fast, it's not very much fun.

So surface feet per minute is important because tools, a carbide cutting tool or a high-speed steel cutting tool, or the coating on that tool, may have a surface feet per minute or a surface speed that it wants to operate at, as does the material that you're cutting.

And so the other example would be on a lathe-- not a big fan. But if you are using a lathe, when you're turning on the outside of a part, you are constantly changing the RPM requirements to maintain the surface speed as you come into the center line of the part.

What is feed? Feed per tooth. Feed rate is a relative velocity at which the cutter is advanced along the work piece. So the diagram in the top right, courtesy of Sandvik, the tool is moving that way. And we can see here, the tooth of the tool is actually engaged with the material. It is taking a chip load per tooth.

We don't use inches per minute because inches per minute don't tell me important information. How many flutes are you using in this case?

Feed is more important than speed. This is a generalization that has some risks for sure. But as a general rule, for free machining materials-- many plastics, many aluminum and basic steels-- surface speed, it's not that it isn't important. It's that the feed per tooth is always more important. And we'll come back to this in the example of if you use something like a 3/64 or a 2-millimeter end mill, most of us aren't going to have machines to even come close to getting to the surface feet per minute that you would like to get to.

Feed always matters, and it matters because the way cutting tools interact with the material. And it's kind of easy to just not think about this and you just assume that cutters work because they work. But if you think about my hand as the cutting tool, and if I go push into something, I can't go through this right now, right? But if I had a knife on me or a scalpel-- unlike Kevin, I don't fly with knives.

[LAUGHTER]

And I were to take that knife and push into it, I think it's pretty reasonable that the Venetian would be upset with me, right? You can actually get into that. So if you had a scalpel, it would cut material. And I tell this. Sometimes, I will actually take a knife, my Norseman, and I will literally cut into material. You can sometimes see what's happening.

The reason we don't use scalpel-like edges for cutting tools is they wouldn't last. They wouldn't last at all, which both means they have a very short life. But equally important and a little bit different, they wouldn't have a consistent performance throughout the life. In other words, it's not binary. It doesn't just work, work, work, work, work, and then fail. It's going to change.

So what cutting tool manufacturers do is they have some amount of bluntness to the edge of the cutting tool, and that's a good thing because it makes it a lot stronger and makes it last longer. But we have to overcome that bluntness with power.

And the key here, to tie it back into why feed rates are so important, is if you look at the picture, if you think about instead of a sharp edge, it having some amount of bluntness to it, if we don't move over enough before we cut, then we're not going to be actually shearing off a chip. And I'm not an engineer. I don't know the correct terms when it comes to things like fracturing the material or shearing the material. But that is what we are doing.

We are actually using a sharp edge, pushing against that material. And as we push against it, we're ultimately causing it to yield or crack or fracture, and then we're sweeping through it. So we need to have our feed rate over enough so that we're actually forming a chip.

This is really important. If you guys leave understanding one thing, especially if you're new to this, it's the role that that plays. We want to form a chip because we don't want to burnish. So if you burnish, you're not feeding over enough to form a real chip.

The scary thing is you're going to think you're the best machinist in the world for about five minutes because the cuts are going to look great. But you're generating massive amounts of heat because you're rubbing. You're not forming a real chip. The tool will fail very, very, very quickly.

And again, heat is the enemy. You're rubbing. You're creating a lot of heat, and you're not forming a natural chip, which normally serves a role of carrying the heat away from the part.

So some end mill anatomy basics, I thought it would be better to include in this deck, which you can download, some links to folks that, frankly, have done a really good job. This example is a company called-- this is Harvey. Harvey and Helical are the same parent company.

Most of this stuff is relatively basic. On an end mill, in this case, we have the section that is the flute. We have the section that is the shank. I doubt I'm teaching anybody much here. But we can have, on an anvil, a square shoulder. We can have a slight radius, or we can have a full ball.

Things that do matter that start to change a little are things like the overall length of the cutting tool, the length of the reach. So in this example, we have a reduced neck-- that may serve a role of letting us cut deeper but maintain a stiffer core-- the overall length, the length of the cut.

And the last section on this page which I want to point out is we've got an example of the helix angle and the pitch. So this is important because I suspect many folks have seen the terms "variable pitch" and "variable helix." And so what that means here, on the variable helix, is each helix isn't just a patterned instance of itself around the tool. They vary slightly. And this has to do with interrupting the harmonics or resonance of the tool.

Same thing with variable pitch. It just means that the four cutting flutes, in this example, aren't 90 degrees offset from each other. They vary ever so slightly to give a slightly better performance or avoid resonance bands.

OK, rake angle, something you guys need to know what it is, at least the basics of it-- it's a little bit more common, or certainly visually easier to understand, in the context of turning or a lathe. If we had a wood lathe in here turning a baseball bat, and I handed everybody a-- what is it called, a-- what's the woodworker tool called?

AUDIENCE: [INAUDIBLE].

JOHN SAUNDERS: What is it?

AUDIENCE: [INAUDIBLE].

JOHN SAUNDERS: Gravel? Am I making that up? What is it? Chisel?

AUDIENCE: Gouge would be one that--

AUDIENCE: A gouge.

AUDIENCE: A gouge.

JOHN SAUNDERS: OK, the tool. I would suspect most of you would probably naturally hold it in what's called a positive rake angle. It's just kind of the way you would think about the tool interacting with the material to form that shearing action. And that's totally fine. There's neutral tooling, and then there's negative tooling.

So the reason that we have negative tooling is twofold. Number one, positive rake tooling has a weakness, which is that the cutting tip ends up being unsupported. It's just not as strong. So you can't run it quite as hard.

The second issue is-- and there's some quirky exceptions to this. But positive rake tooling cannot be flipped over. So on a negative rake tooling, if you have two cutting edges on one side of the insert, usually, you can flip it over, and just get two more for free. So on production, relative to tooling cost, that's a really big deal. You just got 50% more for free.

Because negative rate tooling has this intrinsic support underneath it, you also, again, can run the tool harder. It does require more rigid, more capable machine. It has more tool pressure. So if you're cutting something really thin, negative rake tooling might just push it away, where positive rake tooling can help actually engage it and shear it away.

You see it in face mills as well, though. There's a fellow named [INAUDIBLE] who I think was maybe one of the first guys to really show off the Mitsubishi ASX face mills. Nothing new there. Sandvik has the 245 that's basically this version.

And you can see here, that is a positive rake as it's going around and cutting that material. The opposite would be the guy over here on the right, which is a negative rake tooling. It's a little bit tricky to see, but these inserts are actually tipped backward. It's a very awkward thing to look at.

These actually have a little bit of positive geometry snuck into the insert, so it's a little bit of an exception. But the cool thing about that insert is you can flip it around. So it holds true to that negative rake tooling that gets you twice as many cutting edges. And those Sandvik inserts are very expensive, but it's very helpful.

AUDIENCE: But also, doesn't the rake affect how the chip's being evacuated?

JOHN SAUNDERS: Does the rake affect how the chip is being evacuated? I'm not sure I--

AUDIENCE: [INAUDIBLE].

JOHN SAUNDERS: Yeah, it's certainly-- I'm not sure I can answer that question, at least on the spot. In insert tooling, there's chip breakers which will affect how the chip is rolled over and formed. I'm not sure rake itself would-- anybody want to take a stab at answering that, or--

AUDIENCE: [INAUDIBLE], but obviously, [? you have ?] chip-breaking features to overcome that.

JOHN SAUNDERS: Yeah, so it's a good point, for sure. And chip evacuation-- we'll come back to it-- is huge. So one of the things I want to do in this presentation is both talk philosophically about resources and the whats and the whys and the hows, but also leave you guys with some actionable stuff, especially if you're new to this.

This is an Excel file that we make available. If you go to nyccnc.com, we have this Speeds & Feeds page. If you click on the first guy there, The Basics, there's a 15-minute video or so that talks a lot about the same sort of things I'm talking about here.

But then we have this Excel file that we've put together, and we use this on a daily basis. And the first column here is by surface footage. The next one is by RPM. Again, most the time, if you pull up a PDF, it's going to give you surface speed. But sometimes, I've got a 2-millimeter ball end mill, and I know I've got a 10k spindle. So I really care what the surface speed is.

I just want to know, hey, if I've got a-- tool diameter equals 3. You divide it by 64. And I'm going to run it at, say, 8/10 of an inch feed per tooth, and it's two flutes, and I've got 10,000 RPMs. I now know that-- did I do all that right? Yeah, it looks right. 16 inches per minute is certainly what I could start at or generally gives me the right ballpark. Everybody with me so far on that?

So feel free to download this worksheet. The first tab of it is some starting recipes. So again, trying to stay away from the theoretical and rather just spoon-feeding you, this is an actual link to a tool, some specific width of cut, depth of cut, inch per tooth, and some cutting condition tips for aluminum and steel, again with the idea that if you have access to a machine and a makerspace or you're new, you're certainly not going to break this tool, and you're probably going to get a pretty good result.

Drilling, some similar sort of information of starting recipe stuff. Most drills tend to be high-speed steel. If you grab a drawer or a drill somewhere at a shop, it's probably high-speed steel. 150 surface feet per minute, 0.003 to 0.007-inch per revolution-- it's one of the big differences. Most cutting tools are inch per tooth. Most drilling recipes are inch per revolution. For things like stainless or the super alloys, there isn't any way to give you a equivalent starting recipe or go-to. So you've got to handle those on a case-by-case basis.

So let's talk about speeds and feeds sheets. Any tooling manufacturer is going to make these available. I'm going to pick on Helical a little bit here, and I'm comfortable picking on them because they probably do a better job than just about anybody else of putting out really, really, really good information.

So when you look at one of these PDFs, this is the whole PDF. There's a lot of numbers here and a lot of information. In this case, we've got the tool number of 03345. It's a 3/8-inch-- I think it's a three-flute end mill. And we've got to figure out how do we use this tool.

So if we're cutting aluminum, you're somehow supposed to know [? bit ?] wrought and cast. Most machinists don't necessarily know that there's a wrought and cast. They give you a little tip point here in the series. And most of the aluminums you're going to see, the 6061s and 7075s, happen to be wrought.

Then there's this HBS. Anybody know what HBS is? Nobody?

AUDIENCE: Hardness on the Brinell scale.

JOHN SAUNDERS: Thank you, hardness on the Brinell scale. It's actually a great thing to say, I don't know. They did give me this information down here, but even I took a minute to go figure out, making sure that's what they were referring to because you also hear Rockwell as a hardness scale.

Surface feet per minute, 2,200. That's a really high surface speed, but modern carbide tooling can handle that in aluminum. 3/8 of an inch. They give us slot, roughing, and finishing. I blew this up over here. So basically, what we get is a 1.8 THOU to 3.5 THOU range depending on whether you're slotting, roughing, or finishing.

They give us some axial and radial depth of cut information. And so this is good. This is what's very common. But it's also, in very many ways, inadequate. Remember this slide I showed you earlier with the machine tool and the coolant and the toolpath strategy? None of that is addressed here.

So one of the ironies is Helical also makes software called Machining Advisor Pro. It's actually pretty good. It's generally limited to their own tool library. I can't blame them for that.

But you punch in the EDP number. We pick aluminum. We pick that we're doing a high-efficiency milling, fancy word for what we would generally call adaptive. You're actually required to say that when you're at an Autodesk event.

[LAUGHTER]

ER collet, maximum RPMS, the width of cut, the depth of cut-- it generally populates this stuff. And the output is, frankly, pretty different than the same tooling manufacturer's PDF that they just gave us. In this case, the surface speed is only 1,473. So why is the surface speed here 1,473, but the PDF was 2,200?

AUDIENCE: Because it requires spindle speed.

JOHN SAUNDERS: Yeah, max spindle speed. In this case, I put in as 15,000. So we know, immediately, we can't even come close with a 3/8-inch tool, which is a pretty big tool. On a 15k spindle-- it's a decently fast spindle-- we can't even come within 75% of their originally requested surface speed per minute.

Surface speed matters, but not as much as feed per tooth. Feed per tooth is 5.1 thousandths of an inch. That's a third higher than the highest number they gave us on the PDF. Again, I'm not faulting them. I'm saying there's so many different outcomes.

The reason we can run this feed per tooth so high is because, in this case, we've really been able to tell it the rigidity of this machine and the fact that we're running a trochoidal toolpath. It still, though, doesn't speak to all the cutting conditions, and I would be willing to bet you could run the tool even quite a bit harder than this.

Coatings, everybody has seen and heard of coatings. There's many different types. To be honest, I struggled with how to address them in this presentation. You can't not address them when you're talking about tooling.

But the role that they play-- so they can help make the cutting action-- they can add a level of lubricity. They can make the cutting action have a lower element of friction. They can increase the performance when they are run at temperature. Most coatings are temperature-specific. In other words, they need to be activated at speed. They can definitely help with dry machining, and they can add hardness and toughness to the actual cutting edge in the tool. So they are a good thing.

However, it's very difficult to give a brief summary of what they are and what they can be used for. And I would generally say don't worry too much about it in most general use cases. I would also mention, many of us would see the tool on your right and say, oh, that's the gold color that you always use for aluminum. And you may see the tool here on your left and say, that's the one that we use for steel.

That's usually true, but there are enough exceptions to where I would recommend being really careful with that. We had an IMCO-- I-M-C-O-- tool in where their aluminum coating looked quite a bit like this. And that can really throw you. So don't just assume that the colors of the coating tell you what you need to know.

And it's a great time to mention that if you're using coating, it may be application-specific. And in those situations, there is no better person than having a relationship with a tooling vendor or the tooling manufacturer. There's no shortcoming. These people live this daily and can really help guide you on those sort of solutions.

High-speed steel, you are no longer allowed to use it for end mills.

[LAUGHTER]

Seriously. If someone wants to challenge me on that, go ahead. But the lack of rigidity, the lack of ability to hold a long-term edge, and the availability and low price of good carbide tooling-- carbide tooling is so much stiffer.

And again, if there's another thing I want you guys to take away from this presentation, of all the things that you can do to improve your machining, it is rigidity. Stickout of the tool, size of the core of the tool, gauge length of your work holding, overall rigidity is such a key role in machining. And carbide just absolutely smokes high-speed steel.

You are still going to see high-speed steel in things like cut-off saws, woodruff cutters, drills, form tools, taps. So it's OK. I'm not saying we're banishing it forever. But even if you're getting started and you're bootstrapping, I would really encourage you not to crack open that drawer of Chinese high-speed steel end mills. Go buy yourself a carbide tool for $15, $20, and take care. Use the speeds and feeds here. You're not going to break it.

OK, so first section, summary-- build awareness around basic variables. Make sure you guys have the resources to try something new and not break it. And then some best practices stuff and references are what we're going to come to.

But again, think about speeds and feeds in the context of what you are trying to do. That slide I had with the four blocks across it, are you just trying to get this part made? John Grimsmo was making your cooling platens, right?

And so you don't normally cut big chunks of aluminum. You don't normally slot. So how do you get the resources to just figure something that's outside of your wheelhouse? I normally don't cut tool steel. But if you do it, you want to be able to figure out how to get that done.

What's your goal, though, for other situations of maximizing the tool life, maximizing process reliability, unattended machining, things like that? Make sure you are aware of what is driving the requirement.

Best practices, tips, troubleshooting. So we want to climb cut as a general rule. And going back to how we form a chip, climb cutting causes us, graphics courtesy of Sandvik and Harvey here, to create a thick-to-thin chip. So if we rotate that tool over and start cutting, we've moved it over. We've started cutting a large chip at the beginning. So that's really good because we're not rubbing. We're giving it something to start with.

And then we're thinning it out as we revolve through the cut. What that means is when you're done exiting that cut, you're not tearing off a big chunk, which would be what happens when you down-mill cut or inversion of this. So creating a thick-to-thin chip is a cleaner shear plane; less wear on the tool; less work-hardening, which is really saying less heat; and a larger starting chip.

So because we're starting with the bigger chip and curling it down, it means there's more time spent with a larger chip to transfer the heat into it. Also, to your point, in this case, it exits the chip behind the cut. So if you've seen that rooster tail when guys are doing high-feed machining and you see those chips just whaling off, that's a benefit of climb cutting and a better surface finish.

Thick-to-thin chip, I wanted to watch this little video. I think it's worth it. [INAUDIBLE].

[VIDEO PLAYBACK]

[MUSIC PLAYING]

- How you approach the part is very important. The first thing that we need to consider is how the chips are being formed. In this episode, we'll discuss the golden rule in milling, thick to thin.

If we reference the illustration, there are many things wrong in respect to good milling practice. We're climb milling on one side and conventional milling on the other. We're driving straight down the center of the part. The diameter of the cutter isn't being optimized. And as a result, we're generating thick chips on exit, which lead to edge failure and poor tool life.

The cutter position forms the chip. We want a thick chip as you enter and a thin chip as you exit. In this animation, we're milling straight down the center of the work piece and generating a thin-to-thick-to-thin chip, not a good situation.

When entering, the cutter's rubbing rather than shearing the material. This causes heat and vibration. To ensure proper cutting action, we simply reposition the cutter so that approximately 70% of the diameter is engaged. This ensures immediate cutting action or climb milling. And we're generating a thick-to-thin chip, resulting in less stress on the insert.

There is a wrong way to position the cutter. Notice the areas illustrated with the red explosions. We're now exiting with a thick chip, so the insert is under heavy load. And all of this leads to premature wear and possible insert breakage.

In summary, remember the golden rule, thick to thin. The process should ensure the smallest chip thickness possible when exiting a cut. Proper--

[END PLAYBACK]

JOHN SAUNDERS: So again, I just want to emphasize, some of the things about speeds and feeds that are so important are not necessarily the things that you can visually see but, rather, understanding the science behind it. And when you see it explained like that, you kind of realize, wait, if I'm leaving and exiting with a thick chip, you've got this chunk breaking off, which can cause material finish problems, and it can cause chipping on the inserts.

AUDIENCE: For the nerdy [INAUDIBLE] in the room, that's a little bit different concept when you're a manual machine, though.

JOHN SAUNDERS: Sorry, what is a manual machine?

[LAUGHTER]

Next slide. No, I'm kidding.

[LAUGHTER]

So you don't want-- well, do you want to continue? Or do you want me to--

AUDIENCE: No, go ahead.

JOHN SAUNDERS: So the idea is you're not supposed to climb on a Bridgeport, because climb milling is walking along the part. So you've got intrinsic slop usually between the nut and the screw. And as you start that cut, it's going to lurch forward. There's actually some ways you can take that out by preloading before you come into it. To be honest, I don't use manual machines anymore, ever. And I think most people don't. So it's not something I-- I consciously chose not to focus on it, but it is a good point.

What is adaptive? This came up again this week at a dinner, and I think it's really worth bringing up what a game-changer the strategy is. It didn't exist before. And by maintaining a constant engagement, you really are able to change how you program your machine tools and the toolpaths, and use your tooling.

So if you aren't familiar with adaptive, I've got the same pocket here with an adaptive strategy and a non-adaptive. The adaptive has this kind of look of these swirl lines of the toolpaths, and those aren't by accident. And when we compare it against a non-adaptive here where we're just pushing out the toolpath at even increments, that's OK as you're moving along a face.

But as you enter a corner-- you can see I tried to blow up this simulation here-- what's called the tool engagement angle. Basically, you're going to massively change how you engage that cutter as you come into a corner. And the way you solved this before adaptive was you solved for the worst-case scenario. So you would back down your feeds or your speeds because tools deflect. Tools have horsepower requirements. They have rigidity requirements.

And so if you think it's going to give you a problem in a corner or somewhere else, you just say, I've got to run the whole thing a little slower. So adaptive generally takes care of that. There's a bunch of other names that it's called by.

What is absolutely amazing that I want to stress is you can take recipes and tooling that used to be better designed for very, very heavy, rigid machines-- 50 taper or [? lathes. ?] And you're now able to take lighter duty machines, whether that is a drill mill-type machine or even a garage-sized machine, and you're able to cut materials at really good feed rates using thinner cuts. And that's what's awesome.

Remember that picture of that tool that we showed on the Harvey website? And everyone knows what an end mill looks like. The area in between the flutes is called the gullet. It's the negative space.

When you cut, the chip has to go somewhere. By using an adaptive strategy, we're forming a thinner chip. Generally, it's taller because we're using more of the tool. And that chip naturally forms inside that gullet. That's a good thing. It also tends to evacuate really well. That's a good thing.

The other benefit is we can have more flute counts. More flute counts means we can go faster. The other benefit is the more flutes that you have, the smaller the gullet. That's OK because we're forming a chip that naturally fits in that gullet.

Where you get the benefit is a thicker core. And having a thicker core means you've got a stiffer tool. And that is not a negligible fact. Going between the exact same tool in a two-flute and a four-flute version, the four-flute will be stiffer.

Tyson Lamb, if you follow him on Instagram, is now cutting his putters on a Haas machine-- a great machine, not a 50-taper Makino though-- stainless steel with a seven-flute end mill at something like 300 inches per minute, reliably, with pretty high material removal rate using adaptive strategies. They are absolutely awesome. I know it's become kind of a household word and just the go-to [? roughing ?] strategy in Fusion, but don't take them for granted as it relates to speeds and feeds.

Part tolerances, what does that have to do with speeds and feeds? Cutting tools deflect. And that's not a if scenario. It's an always scenario. They are always deflecting. Even if you take a relatively stiff tool and you cut with a good recipe on a free machining material, I challenge you. Go home. Put a Sharpie line on that, or [INAUDIBLE], and go recut it. That line will be gone, and you'll be forming yet again another chip.

What that means, if you're creating chips on a spring pass, is that the first pass didn't necessarily create it to dimension. So how does that play a role in this? Depending on the tolerances you're trying to achieve, you either need to account for that deflection, or you need to take spring passes.

I'm not against spring passes in every situation. But remember what we've talked about about chip formation. Spring passes are likely going to involve some amount of heat generation or rubbing. I do it a lot. I know [INAUDIBLE], who I talk to the most about machining, does it a lot on his knives. So I'm not saying you shouldn't do it. But it's not always a good answer.

And we also do a lot of-- it's not really cutter comp in the sense of a machine tool cutter comp, but we will program our toolpath strategies to know how that's going to deflect. So we kind of overcut based on what we know that spring pass is going to be-- or the deflection, excuse me.

AUDIENCE: John?

JOHN SAUNDERS: Yes?

AUDIENCE: So this whole process in Fusion, though, of roughing and multiple finishing passes, the idea is to make your last cut small, but not a burnished cut.

JOHN SAUNDERS: Not a burnished cut, and there's a few different ways to do that. That's a really good strategy-- again, it depends on whether you're production or whether the stakes are high. But it can be really good to separate your roughing and finishing tools even if they're the identical tool.

Let your finisher be your finisher. And over time, it could become the rougher. But you're going to keep that tool in better condition, and you're going to keep it sharper. And you're going to get better tolerances because it's going to do a better job of doing its job, which is a relatively small amount of time in the cut compared to the rougher.

And you can also start mixing in some axial strategies. So you can use something like a boring operation, or walking down where you're putting some of the deflection or the tool pressure axially, not radially, which can actually help increase your tolerances. Now, the consequence of that or the price you pay is you're going to be cutting more with the leading edge of the tool. So you're going to be putting more work on that, which can cause more wear, if that makes sense.

I'm not really going to talk about these, but you can print this out from the handouts, or you can just go google it and download it. But lots of the more industry big players-- so the Sandviks and Secos and so forth-- are going to use a lot of these words or terminology. And to be honest, I don't know a lot of them by heart. I don't use them in my daily machinist talk at the shop. So I have a little printout version of this at my desk so that I don't look like an idiot when I'm trying to figure out what the heck the insert box says when you're trying to figure something out.

So the zigzag method-- so how do you figure out a recipe? We've talked about feed. We talked about speed. In that Excel sheet that you should download, there's some discussions about your depth of cut and your width of cut. Again, when we're doing high-speed machining strategies like adaptive or finishing, the great thing is we can use more of the tool that we bought. If our quarter-inch end mill has a 1-inch length of cut, I can now use all 1 inches of that or 950 of it to do my adaptive strategies around-- so I've got more axial depth of cut, less radial depth of cut.