Introduction to CNC Lathe Programming

Neo Structure
3 followers
7 Video Views·Oct 18, 2024
Whether you are just getting started with CNC lathe programming or need a refresher, this video covers all the basics. Join us as we attend a class at Meridian Community College. Brian Warren, division chair of industrial technology at Meridian Community College, allowed us to attend one of his classes at the Gene Haas Advanced Manufacturing Center. During this session about CNC lathe programming, Brian explained some of the main concepts, gave an overview of the most important G-codes and shows an example of how to program a single part.
All right, guys.
So, so far, we've done CNC milling,
and you've done some milling programming,
milling operation, that's by design.
Because good news is programming a CNC lathe
is much easier, to me it is, than programming a mill.
Bad news is, is once you shut that door
and the coolant kicks on, you can't see anything,
so it's a lot easier to crash.
So we're going to kind of take an intro
to CNC programming on the lathe,
and we're going to start out simple,
just doing some basic roughing and finishing,
just turning cycles.
All right, so we're going to do this on our Haas TL-1.
Now, the reason we're going to do this on a TL-1,
when you start the program,
there's a couple things is,
we got a regular scroll chuck on there.
On a turning center, you're going to have
the hydraulic chuck that only gives you
about a 16th of movement,
so your jaws will have to be bored
based on what size you're doing.
On the TL, you got a regular scroll chuck,
just like you got on a regular manual mill,
so manual lathe, I mean, you can put any size in there
that it'll open and close to,
and we can also reverse jaws.
That particular machine's got seven and a half horsepower,
so that's really underpowered
compared to a normal turning center.
You only have 2200 RPM,
but we're not going to even get close to that,
because look what you have in front of you
between that chuck and you.
It's just a thin little piece of sheet metal
with some plexiglass on it.
If you sling a part out, it's not going to be pretty,
so we're probably going to cap most of our programs.
When you're first getting started,
we're going to cap them around 1200 RPM,
and we're going to make sure nothing's going to come out.
We're going to be safe about it.
You got a 2.3 through bore,
so what that means on any lathe
is the bore inside the chuck,
you can get a piece of up to 2.3 inches inside that chuck,
which is always better.
Anything bigger than that,
you're only going to be holding on to by the chuck jaws.
Now, something to keep in mind on any lathe
is they have a little trap door in the back.
When you slide stock into the chuck,
into the headstock,
you don't exceed that little trap door.
You don't want a, on any CNC,
you don't want six feet
sticking out of the headstock of that chuck,
because the torque on it could bend that into an L,
and it could literally flip your lathe over.
So they got a little warning on there,
and a little slide,
and you do not go past that.
I think the TL,
you can get about 20 inches inside of it,
and that helps you a lot for grip,
but it also helps you when you're parting off.
You just slide it out.
You part it off,
slide it out to the next length,
start the program over.
You got to make multiple parts.
I think it's got 16 inches of swing.
I'm not sure on that one.
It's 16 to 20,
but we're not going to put anything over 16 on our setup.
You know, in a particular way,
we got a tool post.
You're going to be at limited at 16.
And a cool thing about it
is the tool comes in from the left,
from the front,
just like you're on a manual lathe.
But if you notice all the other CNC lathes,
they come in from the backside,
and your tools are flipped upside down because of that.
But on this,
you're going to put the tool in
just like a regular lathe,
but you don't have to change anything about your program.
And the computer on the machine is set up
so that it is what it is.
And you don't have to go around
and think about,
well, I'm coming from this direction,
but the only thing it's going to mess you up on
is on a lathe,
cutter comp is referred to a tool nose compensation.
So you're going to look,
well, I'm left of the tool path.
No, you're not.
You're right of the tool path.
So when you're turning,
you're going to be G42 on turning it.
Yeah, but you're going to look at it
and think you're left.
You need to do 41
and your part's going to come out way too small.
And that SA for the most part,
it's a really good machine.
It's a good machine to learn on
and it holds pretty good tolerance.
Does that machine have coolant on it?
That machine does have coolant
and it's going to spray all over the place.
Because you only have that little door,
it's going to make a mess.
It's going to get all over you.
And I'll tell you something else about them,
a little tip of the trade on it.
That coolant pump is very strong.
It's got a valve on it.
If you turn that valve all the way up,
it'll blow that plastic nozzle straight off of it
and rain coolant down on top of you.
So you kind of just crack it open just a little bit.
When that M8 hits and the coolant goes on,
it's going to come out.
But if you got it full pressure,
it's going to be enough to at least bend the plastic up
and point straight up.
And I've seen many people get coolant rained down on them
over the years with that machine.
Now, when you're saying, this is the previous slide,
I tried to catch it when you had it up there.
You referenced 16 inches, roughly a swing.
What was that referring directly to?
Swing on a lathe is how big of a diameter can you put in it?
Because, you know,
basically everything comes off the center line.
So if my lathe has 16 inches of swing
and I try to put a 20 inch piece in it,
I'm going to hit the rails of the lathe.
You know, I can't fit it in there.
So all your lathes are rated by swing
and distance from head to the tailstock.
I believe a TL1 has 30 inches of travel.
It's enough to do a baseball bat.
And we made the baseball bat on it.
So it's enough to do that.
Cool thing about this is your X zero
is always the center of the part.
Now, on a mill, you know,
your X zero could be anywhere on that table.
On a lathe, it's always the center
because that's the way a lathe works is, you know,
however big that diameter is doesn't matter
because zero is always in the same place.
It's on the center line of the tailstock,
center line of the headstock,
however you want to look at it.
So your machine knows where the part is
based on the coordinates you give it
because the machine knows where X zero is also.
So based on the coordinates you put in your program,
that's how it knows how big the part is.
Z zero is typically on the face of your part.
So that means everything you do past the face
is going to be a Z negative.
Now that's going to make it a little different
how you've been doing with mill programming
because you're going to have X positives
and all Z negatives in your program
when you actually start cutting
because everything past the face
is going to be a Z negative towards the chuck.
A real important one, a couple of the common is a G50.
That's spindle speed clamp.
You can think about that as pumping the brakes.
If momentum starts to take over,
that G50 is going to clamp it
and not let it exceed whatever RPM you set it to.
And I'm going to show you how to set that in your program.
Remember what I said with ours,
you know, we don't want to go over 1200.
So we're going to set our G50 to 1200
and it's going to be G50 S 1200 on there.
And most of the time, you're not going to get over that
with the cutting speed we're using on that TL
with low horsepower.
But think about when you're facing off,
you know, your diameter actually goes negative.
You know, you go past zero, a little negative into it.
So that calculation based on that surface footage we gave,
it can really ramp it up.
So that G50 is going to stop it.
G96 and G97.
G96 is constant surface speed on.
G97 is constant surface speed off.
So it's probably easier to explain to you
what G97 is first.
You can think about G97 like a manual lathe.
You put G97 S 400.
It turns that spindle on at 400 with an M3 command.
If you put S 800, it's going to turn your spindle on at 800.
G97 is going to run the RPM at exactly what you tell it to.
G96 is constant surface speed on.
That's going to take your formula that you use for RPM,
the 3.82 times your surface footage divided by diameter.
This is what gets you a lot better finish
on a CNC lathe compared to a manual,
is if I put S 400 in my G96,
every time it cuts, it's going to recalculate the RPM
based on what diameter it is now.
So if I started out with two and a half inch stock
and I cut it down to 2.4,
it's going to recalculate speed up.
The smaller it gets, the faster it's going to go,
but you're always running
at the perfect surface speed for it.
Your RPM is always there.
Now, where do you get the surface footage
for your tools from?
Where's the best place to get that information from?
From, like, with your tools?
Yeah, with your inserts and your turning tool holder.
From the manufacturer?
From the manufacturer.
Whoever you bought that tool from
can tell you what that insert is rated at,
and they generally just give you a range,
and that's not gospel.
You know, just because, well, prime example,
in our ST10, we have a tool in there.
The recommended surface footage is 1500.
So take 3.82 times 1500 and divide it by inch and a half.
You're running faster than you want to run,
faster than the machine can go.
But so I try not to buy any that's rated that high,
but, yeah, we do,
but you can always compensate it by,
I'm going to keep it in proportion,
so if I'm going to knock my RPM down,
I'm going to knock my feed down by this much, too,
and I'm going to kind of,
because of that G96, it's going to keep it in proportion.
Another thing to know about lathes that's not on here
is they're in inch per revolution
instead of inch per minute.
You've been used to programming inch per minute,
and now you're going to be in inch per revolution,
and that's going to make a big difference,
because on a lathe, if I tell you
you put your feed rate at 10,
I'm talking 10 thousandths, 0.010 per revolution.
If you put in 10 point,
you're running faster than rapid on that TL,
and we've had that happen.
I think it was Jody had one in at 10 point,
and it just took off that first pass,
and it never, it acted like it never went out of rapid,
and he said, hey, you know, I got a G01 right there,
but what he had was he had 10 inches per revolution,
and he was moving probably 1,000 RPM.
Yeah, you had a piece of aluminum on the plug.
I don't remember when that happened.
No.
So, G71 is a rough can cycle.
That's what you're going to rough your stock down with.
G70 is the finish turn, and it's backwards.
You know, I like to think that somebody
was sitting around when they come up with this,
and say, hey, let's mess with somebody,
and let's put the finishing number
lower than the roughing,
but you always rough first and finish.
G71's kind of a long cycle, a lot of parameters in it.
We're going to go over that.
G70 is short and quick to the point.
Now, here's a trick that you won't see in your books.
While you're programming your part,
and you're having issues with an alarm or whatever
with your G71, you can change that G71 to a G70,
and it will force it to run the geometry
no matter what you have on there.
Now, this is just for simulation purpose.
Don't actually do this.
You know, you hit cycle start and run it,
but for the simulation, if you're getting an alarm
and you can't figure out why,
more than likely you've got a movement
that's went the wrong direction
or not what you meant for it to do.
If you do G70, it will run it,
and it will show you, and sometimes you can see
what's wrong with your program and what part of it,
and go back and fix it and find your error.
It's in place of 71?
Yeah, in place.
So I can just flip them?
Yeah, just take out the G71, alter it to a G70,
and it will show you the geometry then,
because here's what G70 does.
It cuts it all at one time,
and G70 doesn't have the same kind of rules as G71 does.
So G70, you know, that's a bad idea
to forget to change it back
because it's going to cut it all at one time.
If you've got a four-inch piece of material in
and your smallest diameter is going down to one inch,
well, guess what?
It's gonna try to take three inches at one time off there.
And so I like to tell people that
because it helps them fix their program sometimes,
but I don't like telling you that
because I'm afraid you're going to forget
to change it back and run.
On a mill, you had G91 for incremental.
A lathe program does not have G91.
If you want incremental on here,
you're going to have to go with a U or a W.
U is incremental for X.
W is incremental for Z.
And G0, G1, G2, G3 are still the same.
Nothing about them has changed on a lathe.
The only thing, you got to think about
what motion am I moving in?
Yeah, so sometimes it's going to feel like your gut,
oh, that's a G2.
No, that's counterclockwise G3.
You got to think about where you're starting from
and which direction you're going back.
And it can flip between turning and boring,
but you just got to think about the direction of the arc
from where you started.
And there was something else I wanted to tell you.
Do I have any questions so far?
All right, does everybody feel pretty good about it?
All right, your two most common alarms,
you're going to have type one and type two roughing.
I got to work around for that one.
Type one roughing means everything has to go
in the same direction.
If you're turning, all your Xs are getting larger
as you go up and all your Zs are going further back.
Type two, which that's a lot of the little cool parts
you can make on CNC where your X may get small,
get big, you got a dip in it or something.
You need type two roughing for that.
There is no parameter on the control to set it to type two.
If your X changed direction,
you're just going to get an alarm that says
type one, type two roughing or non-monotonous.
So the way you can get around that
is put a Z move in your first numbered block.
So that first number line, you set your PQ for the G71,
which we'll talk about in a minute.
You have to put a Z in that line.
It has to have an X and a Z
to make it select type two in the first.
If all you have is an X, it's type one.
Now here's something you can do.
Say you need type two, but for whatever reason,
you don't need a Z in that block.
You don't need Z to move yet.
Put a W zero because W is Z and it's incremental zero.
So it's in there, gets it in type two,
but it doesn't move anything.
I've done that a lot to fix students' programs
over the years because I don't want to change
their geometry or their plan.
I want to see, yeah, I want them to better run their part
like they meant for it to run,
but I need it to go to type two to be able to run it.
So that's something you can do is going to go into a W zero
and non-monotonous, I can't even say the word,
so I pulled it up for you, monotonous.
If you get that alarm,
that means that you have left off a negative sign
on your Z where you meant Z negative
and you just put Z and say, hey, Z's changing direction.
Or you're in type one and one of your X's went smaller
than back up larger from when it was larger
because it wants you to think about like a step shaft.
It wants you to go plain, bigger, plain, bigger, plain,
just real simple, smooth cuts through there.
That's what it wants you to do.
All right, now here's an example of a program
from the Haas book.
We're going to shorten this up a little bit
and it's going to be a little simpler than that,
but what they've got in here is good information.
It's, you see the way they do it
and I wish everybody would do this actually
is to go in and list your tools at the beginning
because whatever you put in parentheses gets ignored.
So you can put all your tools in
and you'll notice they got the tool nose radius on there.
Most of your roughing tools is going to be a 31 radius.
Most of your finishing tools are going to be a 64th.
And you also have tip direction.
So when we actually start setting up the machines,
I'll have to show you how to store the tip direction,
but you're telling it what direction from home
is it approaching the work.
So even though, now you're going to get confused on the TL
because you're coming from this direction,
but we've got to program it
like it's coming from the backside of it.
And those tools of course will be upside down
because they're coming in from the backside,
but on a TL, we're going to keep them right side up.
But if you notice at the very front of it,
they take and they hone the machine out,
which they're doing it with G28,
and that's fine at the beginning.
You always want to start a lathe program from home.
You go in with T1-01.
Now what's different here, a lot different than a mill,
is I don't have to put a height number, you know,
with my tool at all.
I don't have to put an M6 really, it's going to go get it.
So, but that T1 means that's tool one and offset one.
So it's going to get tool one
and grab the offset stored for tool one.
So T10 would be T10-10, or T5 would be T05-05,
you know, whatever you got going.
And then they face off.
You know, they take their G50 and set it 2,500.
They turn the spindle on at 591.
And you'll see most everybody does that.
They'll go in G97, have the spindle turned on,
and just at RPM and running.
I mean, do you have any idea why we would want to do that?
I mean, because it's not actually cutting anything yet.
It's still at home.
But why go ahead and turn the spindle on,
running it at whatever number, 591?
Do you have any idea why?
It just looks better.
Because you think about, like, the machine.
How does the machine know how big your stock is
by the coordinates where you're at?
So if you're at home, that X is pushed out
as far as it can possibly go.
So it thinks you have the biggest piece of stock
in there possible.
So if you turn it on there with a G96,
it's going to run really slow
until it gets up closer to the work.
So it just looks better.
And it goes ahead and have your spindle,
you know, get warmed up, too, while it's running.
So you'll see most people are gonna go G50 first.
Then they're gonna put a G97, turn the spindle on.
Then they're going to approach to their starting point.
And think about this like a landing strip.
You see the Z is positive.
The X is 2.1.
So that's telling me they're using two-inch stock.
Because I don't want to come in already hitting a stock.
I'm in rapid.
So I got my tool a hundred thousandths in front of the part
and a hundred thousandths above the part
when I come in on the approach.
And that's very important.
If you got two and a half inch, make it 2.6.
If you got one inch, make it 1.1.
Always stay a little bit above it
when you're coming in on rapid.
And then from there, you're going to go in.
Yeah, you reference your steel G54 or whatever you're using.
Then we set our speed we want to run.
So we're going to go in at G96 S325, which is kind of slow.
Maybe that's steel or something they're doing in this program.
But that's going to take your program.
It's going to calculate your RPM, 3.82 times 325,
divided by the diameter.
At that point, it would be 2.1.
But, you know, if this was a very large machine
and they turned it on with no 97, just 96,
that spindle is just crawling until it gets to that point.
And you'll see there that they go into it.
They face theirs off.
And this is a cool way to do it.
When you do your Z face measure
and tell it where the front of the stock is,
you can go back in and subtract five thousandths
and have it face to zero or have it face plus five
and add five to it.
And it's just going to come in and face it.
Do you notice that it's going to X negative 63 for the face
and feeding it at 10 revolutions?
But why are they going to negative 63?
Because where's X zero?
In the center of it.
So you get to the center,
but you also have the nose of that tool.
So if you notice, that tool one had a radius of 31.
So they just doubled that.
And you always want to go two times the radius past center.
So that's whatever size radius you have in your tool,
two times that past zero in negative,
and it gets a clean face on it.
And then from there, they get ready to start turning.
I will show you kind of an example
of what we're going to do.
This is the neon certification part.
And I just took like a little snapshot of it.
And I'm not going to give you the coordinates
for the neon certification part,
but we're going to do something similar to it
and work our way to that.
And we'll see how close we're getting.
But on a lathe motion,
now this is another thing that I throw people off about lathe.
The X zero is there, right?
So if I need to go here, how far to,
what's my X coordinate?
You can't see the dimensions,
but let's say this is one inch.
And I'm X zero there.
So if I want to go to that point, what's my coordinate?
X one point.
But why, I mean, why is it X one point if that's X zero
and the whole thing is one inch?
That's what throws people off.
A lot of people want to say, okay, that's X zero,
then that's 0.5 if the whole thing is one inch.
But you program by the diameters.
So you don't think about where X zero is
because really when you're programming,
you're only programming half the part.
Yeah, you're not programming the whole thing,
but you program the whole diameter in.
So cutting a chamfer on the end, 45 degrees,
make it really easy.
All I have to do there is figure out where I am here,
subtract 60 from it, that's my first X.
And to cut that angle,
I just put my X and Z on the same block together.
And it's gonna make it move at the same time.
So I would put my X point in,
then I would put my X and negative Z back.
I know what my negative Z would be back 60.
My X would be that full diameter.
It cuts the angle.
Then my next block, X is already where it's at.
So I just move Z back negative to there.
And then the next block,
I just got to find out where X and Z are now
and move them at the same time.
And then here, when you get to a radius,
we'll have to do the math
because we've got a little bit of straight
before we get to the radius.
But that's what we're gonna work on and show you how to do.
And hopefully by the end of the night, you'll be able to do it.
So we got any questions so far?
All right, so I just made this drawing up on the fly.
It's probably not proportioned right,
but it'll give you an idea of,
you know, it'll serve its purpose
to come up with a part program
to generate that we can write by hand.
So we got two and a half inch total stock material.
So we'll just call that two and a half inches.
And we'll go from there,
like we're gonna use two and a half inch stock
because this is just to get you simulated
and run your first part on a TL,
get you used to how everything's gonna work.
And then I'll give you the actual print.
It's good, you're going to have to make the tolerance.
And we'll do a generous tolerance on your first one,
like maybe plus or minus three thousands.
So the way we're gonna start this out is,
you know, you're gonna be at the control.
So there's no need to put percent signs in.
We're gonna call our tool up.
Our roughing tool is tool one.
So we're gonna call it T-1-0-1.
That's gonna be tool one, I'll set one.
And then we're gonna go in,
we're gonna set our G50.
Now, what do we want to set our G50 to for the TL?
We're swinging two and a half inches.
We got at least three and a half inches sticking out,
which is not bad.
So it's pretty safe.
I think we can do, I think we can do 1200, no problem.
That's actually really slow,
but we're gonna go ahead and start it up there.
At that point, what do we want to do next?
Just like you're on a regular machine,
you know, regular manual mill,
what do you want to do next?
You want to turn your spindle on, get it going.
Do I want to use 97 or 96?
96.
No, 97.
I want to go with G97.
And why is that?
So it'll get, so it'll wrap it to the part.
Well, just so it'll spin at a normal rate,
go ahead and get it warmed up
while it's all the way at home.
Because, now the way I'm gonna have you do this
is you're gonna home the machine out
before you start the program at the control.
But what we could do, if you didn't do that,
you forget to do that a lot,
we'll put a G28 in there,
be in between that to home both of them out.
But you're gonna start this program
from the home position on that TL.
So there's no need to home out.
But because we're starting from home,
X is all the way at its extreme limit.
So we have to turn it on just to get it running.
And that way it's not just barely turning
until we get going.
So now we're gonna go ahead and bring it in to the start.
So I'm gonna go into rapid
and I'm gonna put G00, G54.
All right, so where should my X go?
My stock is two and a half inches in diameter.
Where should my first X go?
One inch?
No, not one inch.
I mean 2.6.
2.6, I wanna be about 100 above it.
So X, 2.6.
Z, I can go 0.1.
And then M8, I can go ahead and turn my coolant on then.
That's going to its first point.
Yeah, that's coming in from home,
not actually touching the metal yet.
That's I don't want it touching the stock yet.
I just wanna wrap it up, get close.
I don't wanna feed real slow all the way from home,
particularly on a TL lathe
that has a lot of travel in Z.
Yeah, it's gonna take forever to feed up there,
but I can wrap it up there fairly quick,
but I don't wanna actually touch anything
while I'm in rapid.
And then from that point,
I can go ahead and set my surface speed
that I'm gonna use.
Got a question?
Yeah, I do.
I'm trying to, so why did you start
with the widest part of the stock now?
All right, so think about it.
Your stock is spinning in the chuck
and your tool's gotta come in and get close to the stock.
So it's moving out, not in,
of how they moved in.
It's moving towards the center of the chuck.
So I don't wanna move past the outside edge
of that stock in rapid.
Yeah, this is basically,
I'm staying 100 in front of it
and I'm staying 100 above it.
So it's kind of like a safety line.
No, safety line's a startup line.
It's getting your tool close to ready to start to cut,
but not actually cutting anything yet.
All right, then from there,
I'm gonna go ahead and put in my surface footage
because I want it to recalculate my RPM every time it cuts.
So I'm gonna go in with G96.
We're using a ISCAR tool, a WNMG 332,
and it runs pretty good on that machine
at a surface footage of 400.
So I'm gonna go G96, S400.
My M3 is already active.
No need to put it again.
If you do put it again, doesn't hurt a thing.
I could put it there.
And now I can skip,
because we've already faced this off
when we did our Z-face measure.
We could put a face off in and we will do that later on.
There's a face and can cycle,
but the way we're setting up our TL with these tools,
we have no probe, you're touching it,
and we just go ahead and face it off right then
when we touch it.
So there's no need to face off.
Now I can go in and put my G71 cycle in.
And this is the part that you're gonna need to write down
and you have to practice and remember,
but the more you do it,
the better off you're gonna be.
Is G71, I have a P and a Q.
Think about those as pick up and quit.
So whatever number, and I can give it any number here,
but whatever number I give it,
I gotta be consistent and number that line, that number.
Now for the longest time, I always,
every time I showed a class, I'd say 101, 102.
And it got stuck in people's head
because I use 101 and 102 every time
that it had to be 101 and 102.
It does not have to be 101 and 102.
It can be one, two, it can be five, 10,
it can be three, four,
or you could go backwards with it and say 90, 70.
It doesn't matter, whatever you do,
just make sure those first two.
So what number do y'all wanna give this one?
Any number you want, 12?
12 and 15.
All right, so that's the first part,
and that's gonna take the control,
put the control in rough turning,
and it's gonna tell it to read blocks 12 through 15.
Now does that mean we can only have three blocks there?
No, it does not mean that.
That just means that whatever the first block is
needs to be 12, whatever the last block is needs to be 15.
And it doesn't matter if we got 100 between there.
That's all it's gonna pick up and read is those.
I gotta, if I'm doing roughing,
that means I'm on a finish,
so I gotta give it something to finish.
So U is for what?
And W is for what?
U is for X.
U is for X, W is for Z.
So I wanna tell it to leave 10 thousandths in X
for a finish cut,
and leave five thousandths for a shoulder.
A shoulder and a face.
I wanna leave those two.
I'm out by that.
So I got a G71, a PQ, a U, a W.
I need two more things in here to make this work.
I need a depth of cut, and I need a feed rate.
I need to tell it how much I want it to cut each time,
and how fast to feed it at.
So depth of cut is gonna be D,
and I'm gonna set my depth of cut at 50 thou,
and then my F is gonna be my feed rate,
and I'm going to make that,
generally on this lathe with a carbide insert,
you can feed anywhere between eight to 12,
depending on how aggressive you're moving.
I'm moving at a surface speed of 400.
That's not real aggressive.
I'm gonna go ahead, I'm just gonna do a happy medium,
and I'm gonna look at the chips.
So I'm gonna set it at 10,
so I'm gonna put my feed rate at 10,
and then I'm gonna look at the chips on it.
If my chips are breaking off, they're not stringy,
and everything's looking good,
the finish looks good, and it sounds good,
that's what I'm gonna stick with.
If it sounds kind of light, and it's stringing,
I'm gonna increase that.
I may bump it up to 12, or I may bump up my 400 to 425.
You can't just say one number is always the right number,
because it depends on the material, depends on the tool.
That's why the best machinists, operators, programmers,
they're gonna have sight and sound.
They're gonna be able to listen to it, look at it,
and see if it's cutting like it should.
I feel pretty confident with that aluminum on that machine,
with that tool at 400, you're gonna chip up,
chips are gonna come off,
it's gonna have a good finish on it.
This finish doesn't matter so much as our G70,
but we want it to look good, we don't want it rough
and building up a bunch of heat
while we're cutting and look back.
That just makes it harder to get a good finish out of it,
and the heat will make your metal do what?
Expand, so when it cools,
it may draw in half a thousandths or so,
and then that half a thousandths may make the difference
whether your part passes inspection or not.
So I wanna cut it right,
even though this is just roughing, and then that's it.
Yeah, that's a lot, but that's it for the G71.
Now think about it, what this is doing for you
is you're able to put the finished coordinates in
for the program for the toolpath.
You don't have to sit and program every single path of it.
Imagine taking 50 to the side at one time,
how many lines of code you would have.
It would go through and feed to there, then back off.
Imagine having to program every single pass it makes,
you know, X and Z, X and Z, X and Z.
That would be a lot of programming.
So that's what this is for.
You can put the coordinates of the finished path in
and you're good to go.
And G71 is gonna take it down 50 at a time,
so with this, we called it 12,
so my first thing I have to do here is the N12.
N?
N12.
What does the N do?
That's just a number block.
If you'll notice on software,
software will number every single line you have
if you have it turned on in your post.
You know, you notice this is not the 12th line,
but that doesn't matter.
You know, just whatever we want it to be,
that's what it is.
Now the only thing would be if I got two sides
to this operation,
where like I gotta turn this side,
then I gotta flip it around and drill
and bore something out,
I couldn't use that 12 and 15 again on the same part
because it would go back and read these coordinates
instead of the second set of coordinates.
So do keep that in mind.
If you got a flip where you're gonna do something
to the second side of the part,
you gotta pick a new set of numbers.
And some people would just say,
hey, I count by five, five, 10, 15, 20, 25, 30.
This is 35 and they're gonna put 35 right there.
And there's nothing wrong with that.
You could do that or you count by one.
So what's my first coordinate on here?
What's my first X?
So my first X is,
I'm plotting out the points.
I'm right here trying to get to there and then here.
So what's my first X set at?
0.950.
Because if it's 45, it means it's equal.
I'm dropping down 50 from one.
So my first X is 0.95.
That's my first block.
That's all I needed to do from there.
And then my second one,
where's my X going to move at the end of that angle?
What's it gonna move to?
X1.
Where's my Z at?
Z negative 0.50.
Yep.
Z's gonna go back 50 and it's got to be negative.
I put them on the same block.
It cuts, it goes.
Anytime, even on the mill,
if you put two numbers on the same block,
it's gonna get there the fastest way possible.
So naturally, the fastest way possible
is gonna be a linear path diagonally like that.
So it automatically works to your advantage.
You know, you don't have to figure out,
you don't have to figure a right triangle for this,
especially for a 45.
You know, because whatever one side is,
the other side has to be the same on the triangle.
Now, this was 30 or 60.
You'd have to do a little math on it to figure it out
if that's all they told you.
But for this, you're good to go.
All right, so we've moved to here.
Now, what do we need to do to get to there?
Go over Z minus 2.95.
Yeah, just bring Z back.
To this point, it's gonna be one inch.
And make sure you put your decimal points
because it's gonna be just like a mill.
If you leave off a decimal point,
it's gonna move it four places over.
So that gets me to there.
So what do I gotta do to get to right here?
Where's, what's my X and Z gonna be?
X is gonna be 2.5.
X will be 2, yep.
And I don't think I have this right in right,
but that's fine.
We'll still make an angle, but it's not gonna be 45.
But this is gonna be X2.
And then where is Z?
Z is at negative 2.5 to get to right there.
And that gets me to there.
Now, I'm gonna have to erase some of this
to have room to do it.
But, well, I'll tell you what,
we'll draw a line.
And you keep yours right below it,
but I gotta move over a little bit, but that's fine.
That's a little section line.
So we're gonna pick back up right here.
So to get to here, where is,
I don't need to move my X at all,
but I need to move my Z to what?
And as I tell you right now, that's wrong.
This is going to be 3.5.
This is going to be 4.5.
So my Z from end to end, I'm gonna go Z negative 3.5.
Right?
Everybody agree?
What?
Oh, I was wondering, why is that piece longer?
Like, why is that part longer than the other one?
That's just the way we drew it.
Yeah.
I was wondering.
See here, I tried to give you dimensions
from this two side, but I gave you from the front
all the way.
Remember, this is Z zero.
So everything's about, where does it get measured from?
This is all absolute.
So where are we measuring from?
Z goes back negative 3.5.
Then what do we do to get to here?
You gotta go up.
Change X.
Change X to what?
2.5.
X, 2.5.
And then I'm gonna bring Z back all the way
to 4.5 inches.
So Z negative 4.5.
And then I like to do this,
especially when we start using tool nose radius,
it's gonna be a good line for you to put it in.
I got to end these coordinates with a Q15.
So I'm gonna go ahead and bring it back
to where it started at 2.6.
So I'm gonna take this line, the very last one,
because actually my part is cut now.
I just need to bring it up.
So I'm gonna take N15,
take X to 2.6,
and then I'm ready to home out.
And the way I would home this tool out
is I would bring X out first
with a G00, G53,
X0.M9, turn my coolant off.
And then I would do the same thing,
G00, G53, Z0.
Bring that tool back to home position.
And at that point, I would do my tool change
to do the finishing cycle.
And we'll have to pick that one up next time
because we'll run this one first
and then we'll finish next time.
So like, on the wave, is the X going this way?
Yeah.
Yeah, X is in and out and Z is back and forth.
Z is always tailstock to spindle
and X is always cross.
So once you set up your cycle well,
you're giving it the end spindle coordinates?
Yeah, that's all you have to do, G71.
You got your finish coordinates.
That makes life a lot simpler
than having to program every tool path.
It is easier than that.
And so what could happen here, though,
with this is, which it doesn't have any radius,
so its likelihood is a lot smaller,
but say you forgot to
put a Z negative there or something.
So you get an alarm or it looks real funny
and it won't run right.
I could switch that to G70
and just see the actual shape of it
because G70, that's the difference between G70 and G71
is G70, if that was there, it needs that P and Q
and it needs the feed rate and that's it.
That's all G70 needs.
It would ignore your U, W, and your D.
So what happens there, that tool comes in
and tries to take it all at one time.
No finish, nothing.
And that's where you can really do some damage.
I've seen people absolutely destroy tools, tool holders,
seen chuck jaws broke off chucks,
chucks ripped off the machine,
turrets broke where you can walk up
and just spin the turret like Wheel of Fortune.
So you can do a lot of damage.
That's what I say, it's easier to learn
how to program a CNC lathe,
but it's more dangerous running it
because that mill, I got big giant doors,
nice clean glass.
I can see what's going on in that mill.
That lathe, I can't really see once I shut that door.
I gotta trust my setup, trust my program.
And in here, we'll say, all right,
we're gonna have a half inch cushion
coming off your chuck jaw.
So you're gonna watch your distance to go
and it's gonna stop and move back.
You get out in the real world,
you may work to 10 thousandths off the chuck jaw.
And it's like that because the closer you are
to the chuck jaw, the more rigidity you have.
So your tolerances are going,
especially if you're working in the tents.
Now you can't have, the more excess you have
hanging out of the chuck, the worse it's gonna be.
So that's, I say, don't let it scare you.
I'm not gonna lie to you, it's just going to be scary
when you watch it coming up that first one.
Yeah, that first pass.
And once you make it past that first pass with that tool,
you know that tool's good.
It's not gonna hit the chuck jaws.
But then what, yeah, guess what?
When you switch to tool two to do the finish,
now you gotta watch that first one again
because those offsets could be off.
But hopefully, you know, everybody set your offsets,
you're paying attention,
you're not talking to anybody while you're doing it.
And you don't, not let anybody distract you
and your part's gonna come out just like you want it to.
And always what we want is no crash.
Yeah, we never want a crash in it.
