- 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 metric values in this video but I have made another
video for those of you that are running inches. A few key concepts, a formula and we'll reach the
RPM that our program needs. Another quick calculation
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 kilometer per hour, that's roughly 17 meters per minute, which tire is moving faster? Our small front tire or
our larger rear tire? Everything for me begins
with my setup sheet. So check this out I've
got a block loaded... Now if you tightening up
those tools by hand... 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. 17 surface meters per minute. See both tires travel the same distance, where it matters along the tires 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 with some kind of ratio between a tires 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 circles diameter and its circumference is pi. So no matter what 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 at 100 millimeter diameter has a circumference of 314 millimeters. 100 times pi is 314. Now this tire has a diameter of one meter. And a circumference of 3.14 meters. One times pi equals 3.14. Okay back it up get out of here. If we were to run our tires too fast, too many surface meters 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 and quickly wears out. In machinist talk, if
we're talking about speeds, like speeds and feeds, we could be talking about
one of two different things. We're either talking about cutting speed or spindle speeds. Our cutting speed Vc is our
surface meters per minute. 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. We'll get our tools cutting
speed in meters per minute right from our tool catalogs. But the control the Haas
machine, it needs an RPM value. A spindle speed that's our S code. To get from here to here,
we're gonna use a formula. And that formula is gonna make use of pi and our tool's diameter to convert our meters per minute into an RPM value, a spindle speed. 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
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 1000, all divided by our diameter times pi. n is our RPM, revolutions per minute. That's the S code in our program, what we're trying to solve for. Vc is our cutting speed, our
surface meters per minute. D or sometimes Dc or D1
depending on the catalog, is our tool diameter in millimeters. The 1000 in this formula
is there to convert our meters per minute into
millimeters per minute. This formula works fantastic, but we're gonna simplify
it a bit using algebra. We're gonna divide the 1000 by pi. 1000 divided by pi is about 318. We're gonna go ahead and
use this simplified formula for the rest of the video. 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 our tool catalog. We can download the manual
for 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 super alloys,
materials like titanium. And H is for hard cast
irons or hardened steels. I am working with a 4140 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 42CR 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 ISO material class. Now the number that follows
are color coded ISO letter changes between manufacturers. So be careful here. Kennamental calls this material a P4. Niagara and Seco may call it a P5. Sandvik classifies it as a P 2.1, 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. (crowd cheering) Yeah that's what I thought. From the section of the
manual for our exact tool under the row that lists our
material group, P5 in our case. We're gonna find our
cutting speed, our Vc, our meters per minute. If your catalog gives you
a range of values there then you'll make your choice based on the length of your tool, how strong your setup is and
how aggressive we tend to cut. In general the more we do the setup the faster we can go
with our cutting speeds. But remember tools tend to last longer, have better tool life
at lower cutting speeds. For my tool and material we're gonna use a cutting speed of 100. That's 100 meters per minute. I'm using a 20 millimeter end mill so we'll drop in 20 there. And after a little bit
of math we come up with an RPM value of 1592. So our s code back in our
program is gonna be S1592. We now have a cutting speed
and 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 of feed rate. The feed rate is how
far the tool will travel in one minute in millimeters
along the tool's center line. Here is our feed rate formula for n mils. We've got our 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, three teeth. This tool's got six teeth
and this one's got four. We want our tool to take
a very specific size bite with each tooth. This is our feed per tooth in millimeters. Just like our cutting
speed the book or PDF will give us that feed per tooth value. The catalog says that for my tool, material and type of tool
0.08 millimeters per tooth is a good starting range. 0.08, our feed per tooth, times four, our number of teeth, times 1592, our RPM, will give us our millimeters
per minute feed rate. F509.44. Again this is how far the center
line of our tool will move along its programmed path in millimeters each and every minute. 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 side milling. Our ae is our width of
cut, that's our step over. That's our radial depth of cut. And our ap is our axial depth of cut. How deep the tool is moving in the Z-axis. Most times if you're slotting, your "byte" is gonna be about 25% less than if you're just side milling. With the popularity of
optimized tool paths like dynamic adaptive,
volume mill type high speed machining 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 kinds of different tool paths. You'll choose one and then
match your speed and feed to the path that you're using. Now if you are dealing with
drills and not end mills our feed rate might be
listed in our catalogs as a feed per revolution,
and not a feed per tooth. We just multiply the millimeters
per revolution chip load from the book times our RPM, to get our feed rate in
millimeters per minute. Now watch out for and know the difference between millimeters per tooth Fz, which we typically use for milling tools, and millimeters per revolution Fn, which we often use for drills. Here is that completed legder, and the formulas we
typically use for calculating our speeds and feeds. We've got our cutting speed
formulas, spindle speeds. We've got our feed rate formulas for both n mills and drills. And we've got all of the notations, all the 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 finally you don't have
to do any math at all. (crowd 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 tapping feed rates. We will 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. (gentle music)
