- Hello and welcome to
this Haas tip of the day. In today's video, we're gonna talk all about speeds and feeds. We'll show you the path that we take to reach starting speed and feed values that we can trust, that will work with any tool and material combination. We'll be using inches in this video, but we've made an entire other video for those of you that are
using the metic system. A few key concepts, a formula, and we'll reach the RPM
that our program needs. Another quick calculation (bell chime) and we'll establish our feed rate. And have you home in time for supper. As we jump into one of
the coolest concepts in CNC programming, Speeds and Feeds, I've got a question
for you, are you ready? If our tractor is moving
along at an amazing one mile per hour, that's
88 feet per minute, which tire is moving faster? Our small front tire,
or our larger rear tire? (folk string music and engine purring) Everything for me begins
with my set-up sheet-- So, check this out, I've
got a block loaded up-- You're tidying up those tools by hand-- (marker scratching) That's it, pencils down, answers? I know, it's kind of a trick question. It depends on what I mean by faster. If what I am asking is how fast the tires are moving across the surface of the ground, where the rubber meets the road, then both tires are traveling
at the exact same speed, 88 surface feet per minute (cow mooing) See, both tires travel the same distance, where it matters, along the tire's edge. Now, if we're talking about
revolutions per minute, RPMs, then that's a different story. While both tires cover
the same amount of ground, the smaller tire had to
make more revolutions per minute to get there. If we want to calculate how much ground a tire will cover with each revolution, then we'll need to come
up some kind of ratio between a tire's diameter
and its circumference. Well, it turns out, someone
has already figured this out for us, and they've even
given this ratio a name. Pi. The ratio between a circle's diameter and its circumference is pi, no matter what our diameter our tire is, the distance around the
outside of that tire, where the rubber meets the road, is always 3.14 times greater. This tire has a diameter of 3.82 inches. 3.82 times pi is 12. Now this tire, come on. This tire has a diameter of 40 inches. 40 times pi, about 126
inches circumference. Okay, that's great, get out
of here (backing up beeping) If we were to run out tires too fast, too many surface feet per minute, they would overheat, blister and fail. Our end mills work in the same way. There's a limit, a maximum cutting speed, that a specific tool can
go on a specific material. Any faster, and it begins to
overheat quickly wears out. In machinist talk, if
we're talking about speeds, like speeds and feeds,
we can be talking about one of two different things. We're either talking about
cutting speed or spindle speed. Our cutting speed, our Vc, our
surface footage per minute, is the speed our tool is turning at where the rubber meets the road, where the tool meets the part. And our spindle speed is
simply our revolutions per minute, our RPM. Now we get our cutting speed,
SFM, right from our catalogs. But the control, the Haas machine, needs to know the RPM
value, our spindle speed. That's our S code. To get from here to here,
we're gonna use a formula. And that formula's gonna make use of pi, and our tool's diameter,
to convert our SFM that we got from our catalog into a spindle speed, an RPM value. Now once we've got that RPM value, we can calculate our feed
rates: speeds and feeds. Here is our formula to calculate our RPM. Now, I'm gonna start using some symbols, some notation, because
those are the symbols being used by all of
the tool suppliers now. And you'll need to recognize them. RPM equals cutting speed times 12, all divided by our diameter times pi. N is our RPM, our spindle speed,
the S code in our programs. This is what we're trying to solve for. V-C is our cutting speed, that is, our surface feet per minute. D, also sometimes listed as D1
or DC, is our tool diameter. This is the long version of the formula. The 12 in this formula is there to convert feet to inches,
there are 12 inches per foot. We already know what pi is. Now we're gonna simplify this formula. by dividing 12 by pi, that gives us 3.82. This new simple formula is
the one we're gonna use today. Before we open up our catalog,
and get our cutting speed, before the tractor even leaves the barn, we need to know exactly what
cutting tool we're gonna use. And we need to know exactly what material we are gonna be cutting. Now in the good old days,
all we really needed to know was whether our end mill
was high speed steel, carbide, PCD, or CBN. Those days are gone. Today's tools have coatings on them that might double their
allowable cutting speeds. So we really need to know
what tool we are working with. Otherwise we'll have to
use really generic values which are pretty wimpy. With our exact tool number in hand, we can go to our tool catalog. We can download the manual from any tool manufacturer in PDF form. Once that catalog is opened up, we're gonna search for the
material group section. That's gonna tell us what material group our exact material falls into. Our materials are color-coded P is for steels, M is
for stainless steels, K is for cast irons, N
is for non-ferrous metals without iron in them, like
aluminum or magnesium. S is for our superalloys,
materials like titanium, and H is for hard cast
irons, or hardened steels. I am working a 41 40 steel. At least that's what we call
it here in the United States. If you're in Europe and you're using EN names and numbers, this
might be called 42 CR MO4. If you're in Japan, you'll
call it something different. But no matter where you are in the world, this material is gonna find itself in the P isomaterial class. Now the number that follows
are color-coded isoletter, changes between manufacturers,
so be careful here. Kennametal calls this material a P4. Niagara and Seco, may call it a P5. Sabic classifies it as a P2.1 while Iscar and Widia
might call it a P6 or a P7. Same material, different tool vendor. Now, it's important
that we get this right. If you don't choose the
right material group, you are gonna burn up your tools Titanium has a different
machine ability than mild steel. If you try running a drill
or an end mill in titanium, at cutting speeds meant for mild steel, you are gonna melt that tool. It will overheat and
fail, so if you can't find what material group
your stock should be in, then give your tooling
representative a call. They would love to hear from you. How many tooling reps out there would love to hear from one of our
viewers and talk tools? (cheering) Yeah, that's what I thought. From the section of the
manual for our tool, under the row for our material type, we're gonna find out
cutting speed, Vc, our SFM. Now if your manual gives you a range like 2 to 300, then base your choice on your tool length and your set up. The more rigid the set
up, the faster we can go. But remember that tools
tend to live longer, they have a longer tool life, when cutting speeds are slower. For my tool and material,
our cutting speed is 300 SFM and I'm using a
three-quarter inch diameter tool, so we'll use .75 in our formula. We'll do the math and come
out with an RPM value of 1528. That's an S code of 1528. We now have a cutting speed, an RPM value that we can use, without
our tool (explosion) Exactly. We now know how fast to
spin our tool, our speed. The control now needs our table feed, our F code, a feed rate. The feed rate is how
far the tool will travel in one minute along
the tool's center line. That inch per minute feed rate is how far the tool will travel
along the machine's axes. Here is our feed rate
formula for end mills. We've got out table feed
equals our feed per tooth, times the number of teeth, times our RPM. So, what's a tooth? This is a tooth! It's just a cutting edge
along the outside of a tool. An insert is also a tooth. For most tools, the
number of teeth matches the number of flutes. This tool has three
flutes and three teeth. This tool's got six teeth,
and this one's got four. We want our tool to take
a very specific sized bite with each tooth. This our feed per tooth, in inches. Just like our cutting
speed, the books, or PDF, will give us that feed per tooth value. The catalog says that
for my tool, material and type of tool path,
three thousandths of an inch per tooth is a good starting range. 0.003, our feed per tooth, times four, our number of teeth, times 1528, our RPM, will give us our inch per
minute feed rate, F18.336. Some manuals will just
give out a single feed rate for all cutting conditions. But most will give us at
least two possibilities. One for slotting and
one for slide milling. Our A-E is our width of
cut, that's our step over, that's our radial depth of cut. And our A-P is our axial depth of cut. How deep the tool's moving in the z-axis. Most times, if you're slotting, your bite is gonna be about 25% less than
if you're just sidemilling. With the popularity of
optimized tool paths like dynamic, adaptive, volume-mill type high speed machine-y tool paths, the tool manufacturers are
getting more and more specific with their speed and feed recommendations. So you'll often see charts like
the one we'll show you here listing all different kinds of tool paths. You'll choose one, and then
match your speed and feed to the path that you're using. Now, if you're dealing with
drills and not endmills (laughs) our feed rate might be
listed in our catalogs as a feed per revolution,
and not a feed per tooth. We just multiply the inch
per revolution chip load, from the book, times our
RPM, to get our feed rate in inches per minute. Now watch out for, and
know the difference, between inches per tooth, F-Z, which we typically use for milling tools, and inches per revolution, F-N, which we often use for drills. Here is that completed legend, and the formulas we typically use for calculating our speeds and feeds. We've got our cutting speed
formulas, spindle speeds, we've our feed rate formulas, for both end mills and drills, and we've got all of the notations, all these symbols, that you're
gonna see over and over again in your tool catalogs. With all of that said,
there's a big shift happening with tooling catalogs in general. A lot of these tooling catalogs are just giving us our
feed rate and RPM values. No formulas needed. You may open up your manual and find that you don't have to do any math at all. (cheering) In the past, we used to have to rely on slide rules to calculate
our RPM and feed rate. I still like these, I think they're great. But today, we're more likely to use an app on our phone, or a piece of software on our computer or the
speeds and feeds calculator right on the Haas control. On machines with next-gen controls, you can reach the milling calculator by pressing current
commands and navigating to the milling tab. We've made some videos that help you calculate those tabbing feed rates. We'll link to those in the description. Well, that's it, let's go home. You can call your tooling
rep in the morning. Well, thanks for letting us be a part of your success, and for watching
this Haas tip of the day. (piano riff)
