In this Tip of the Day, Mark shows you everything you need to know to drill on a Haas lathe. Whether you have a standard 2-axis lathe, a dual-spindle lathe, or even a live-tool lathe, Mark simplifies the process, and explains all the G and M codes you’ll ever need. We’ve even included a downloadable cheat sheet that you can keep on your machine or in your toolbox for easy reference. This is a must-see video for every Haas lathe operator, whether beginner or advanced.
This video provides a comprehensive guide on drilling essentials for Haas live tool lathes. It explains the fundamental differences between standard and live tool drilling, introduces a four-question framework for programming, and details the specific G and M codes required for main, secondary, axial, and radial drilling configurations.
Hello and welcome to this Haas tip of the day. This is a shiny new Haas live tool lathe. Now if
you've just gotten one or are trying to figure out why you might need one, we want to help you
get up and going quickly making parts. So today's tip is all about covering the essentials of
drilling on your new live tool lathe. We're going to show you how to drill from all different
directions with all kinds of different spindle configurations that your parts might require.
This is what I'd want to know on day one. Haas lathes come in a few different configurations,
but programming them is consistent across all models. Now on our standard two-axis lathes,
you've got a main spindle, an x-axis, and a z-axis. When you want to drill a hole on this lathe,
it's going to be the part that turns, that rotates, while the tool stays still. It stays static. On
live tool lathes, you're going to mount the driven tool or the live tool into the turret.
When drilling holes with that setup, it's the live tool that spins while the part stays still.
Now this is helpful because it allows us to drill holes off center, off the center line
of the main spindle. Now our live tools can be mounted either axially or radially. If we mount
them axially, our tool is going to be facing either to the left or to the right on a DS
dual spindle lathe along the z-axis. If the tool is mounted radially, it's going to be
mounted up and down. It's going to be drilling from the x-positive direction down onto our parts.
To drill or tap on your Haas live tool lathe, we need to answer a few questions.
Four questions. One, two, three, and four. One, which axis? Are we going to be drilling along the
x-axis or the z-axis? Number two, what is spinning? Are we going to spin up our main spindle or the
secondary spindle or maybe one of our live tools? Number three, which direction is it spinning?
Are we going to go clockwise, forward, or counterclockwise, reverse? And fourth,
what RPM is it spinning at? We might be using a P code or an S code to command this,
but you don't have to write all this down. We've actually made a cheat sheet for you.
And if you go to the end of the YouTube version of this video, you can click on the bonus content
and download this little spreadsheet here, this little table. It's going to give you all the
relevant GNM codes you need to drill and tap anything, okay? You can print this out on your
own and stick it to your toolbox or your refrigerator. So we're going to go through
these right now one by one and cover the main spindle, secondary spindle, the axial, and the
radial live tooling. And this will become really obvious, really simple for you. Let's go to the
machine and take a look. So here's our first part. And I know right away that I want to drill a hole
along the center of this part. Now, I'm going to go and load this into my main spindle.
And then we got to go back to those four questions, right? Starting with number one,
which axis? Which axis do we want to drill along? We're going to be drilling along the Z axis. So
I'm going to use a G83 peck drilling cycle. Now, the G83 not only tells our Haas control that we
want to peck drill, but it tells us which axis we want to drill along, the Z axis. If we wanted to
drill along the X axis, we would use an entirely different G code. On all Haas lathes that leave
the factory today, the G83 is only used to peck drill along the Z axis. Okay, questions two and
three. What is spinning and which way does it spin? Now, because we want to drill a hole with
our main spindle, we're going to use an M03. But that one code not only tells the control
to turn the main spindle, but it tells it to turn clockwise. Again, the M03 is answering
two questions. What is spinning and which way does it spin? Okay, we're turning this spindle
clockwise. But clockwise from whose perspective? From the operator's perspective or from the
machine's perspective? Well, imagine this. Imagine that your spindle has eyes. As a rule of thumb,
the clockwise, counterclockwise perspective is always from the spindle. When we say M03 clockwise,
it's from the perspective of the spindle. When we say M04 counterclockwise, that's also from
perspective of the spindle, not the operator. Now, this is a little bit corny, but it's going
to come in handy when we start talking about secondary spindles. So number four, what RPM
is my spindle turning at? So I want to drill at 2600 RPMs. So I'm going to command an S2600
from within my program with no decimal point. So that's pretty much it. We know how to drill using
our main spindle. Well, I'm up here in our demo room because we've got a DS dual spindle lathe up
here, and we want to show you how to drill on that secondary spindle. Now, we already showed you how
to drill on the main spindle. So programming for this secondary spindle is super easy, really
simple. In fact, it doesn't matter if you're drilling, tapping, turning. We're going to program that
secondary spindle in the same way. You program it for the main spindle just like normal, and then
you preface all that G code with a G14, and it runs just fine. It takes care of everything for
you. It swaps all that code to run on the secondary spindle. Let me repeat that. You program for the
main spindle just like normal, preface with a G14, the control does the rest. It runs it on
the secondary spindle. When you're all done, you call up a G15 to turn that off. Well, we're back
to our one, two, three, four. One, which axis? Well, we're going to be drilling along our Z axis,
so we're going to go ahead and use that same G83. Number two, what is spinning? In this case,
our secondary spindle is turning, and the machine knows this because sometime earlier,
we commanded that G14. So the G14 is modal. Everything that happens after a G14 is going
to happen on the secondary spindle, not the main spindle until we turn it off with a G15.
Number three, which way, which direction is it spinning? Well, we want to go clockwise because
we're using a right-hand drill. Remember, imagine that your spindle has eyes. That M03 or M04 is
always from the perspective of the spindle, even when we're talking about this spindle swap mode.
Number four, what RPM is it spinning at? And this is going to be easy. It's the same as
our main spindle. We use an S code to control the RPM for both our main spindle and the secondary
spindle. Well, we're ready to walk through our one, two, three, four for our axial live tooling.
We'll go ahead and populate that table for you now, and you can follow along. Number one,
which axis? Well, we're still drilling along our Z axis, so we're going to use that same
G83 G code. Pretty straightforward. Now, here's where things get different. Number two and three,
what is spinning? Our live tooling has a dedicated spindle motor for it,
so we've got separate M codes for that. We're going to use either an M133 or an M134. That's
spinning in which direction? If we use an M133, that's going to tell the control that we're using
the live tooling spindle. It's also going to tell the control to go clockwise. M134 would have gone
counterclockwise. Now we're on to number four. How fast is it spinning? How many RPMs,
revolutions per minute, are we going to turn that live tooling? Here's where most people make
mistakes when using live tooling. While on the main spindle, we use an S code to command our RPM,
and on the secondary spindle, we use that same S code with a G14 spindle swap command. On our live
tooling, for milling and drilling, we use a P code to command how many RPMs we'd like to go.
There might be a scenario someday on your machine where you want to run the main spindle and the
live tooling at the same time, so we've given them separate codes. Main spindle, secondary spindle,
S codes for drilling and milling, turning, and for our live tooling, we use a P code for drilling.
So if I want to drill at 2600 RPMs, I'm going to command a P2600 with no decimal point to control
that RPM. Well, this is it, our final drilled hole of the video. We're looking right now at radial
live tool drilling, and we go back to our 1, 2, 3, 4. Number one, which axis? We're going to be
drilling along our x-axis on our lathe. So for this, we're going to use a G243. You'll see it right there
on your table. The G243, by definition, drills along the x-axis. Now, remember, this is a lathe,
so all of our x values are in diameter. So two and three, what is spinning, and which way does
it spin? Well, what is spinning? It's going to be that live tool motor, and we're going to command
that with an M133 spindle forward or an M134 spindle reverse command. Which way does it spin?
Well, this is where things get tricky. Now, I love rule books.
Here at Tip of the Day, we love rule books. I wish I could tell you right now to always use
an M133 to go forward or to always use an M134 to go reverse, but in this case, you've got to
throw away the rule book. We really have no idea which way your particular geared head is going to
turn. Lots of right-angled heads have gear reversal in them. When you command an M133 to go clockwise,
the tool might actually be going counterclockwise. You can only trust these. You need to visually
verify every live tool that you use to make sure that it's spinning the way you intended.
Well, we're here at the end of our live tool drilling video, but there's one thing that
we haven't mentioned yet. We never talked about plane selection, G17, G18, and G19,
and there's a reason for this, because on all Haas lathes that are leaving the factory today
are drilling and tapping can cycles ignore your plane selection entirely.
So if you've got a lathe built since right around June of 2012 with a software version 1106 or
newer, it's going to behave exactly like we described today. If you have an older lathe,
something built before 2012, then check out the lathe manual that shipped with your machine or
talk to your dealer and get some pointers on how to program that piece of equipment exactly.
Or you can just click on the bonus content at the end of the YouTube version of this video
and download our document. We've got a little spreadsheet there that tells you all the
different codes to use. We'll even give you proof programs for every Haas lathe made,
whether it was made before or after 2012. Just look at the document. Well, that's about it.
Be sure to subscribe to this channel. You don't want to miss what's coming up next.
We've got some more videos on live tool tapping coming up. And like if you're on Facebook,
you know, share, comment. We want to hear what you have to say.
Well, thanks for letting us be a part of your success and for watching this Haas tip of the day.