Understanding Lathe/Mill Cutter Comp Startup Moves

[Nerdlinger]

Hi Everyone!

I have a few questions about cutter comp I am hoping y'all could help with (especially #3):

1) It is my understanding that when invoking cutter comp on a mill, the G41/G42 line must include either a G00 or G01 move of at least the radius of the tool in either, X, Y, or X AND Y. Is that correct?

2) It is my understanding that whilst in G41/G42 on a mill you either 2.1) can not or 2.2) should not make Z moves. Are either of those correct?

3) How the heckarooney do you properly invoke cutter comp on a lathe for a standard turning op? I have been successfully getting away with it but don't actually know what I am doing! I have read the FANUC section on it and I THINK it sounds like you are supposed to make an X move on the G41/G42 line at a Z location somewhere "upstream" of where you will be cutting and from there it will move such that 2) the tool nose center will be lined up in Z to the programmed location of the very next block...the block right after the startup block. If that is correct then going to Z0. on the block right after the startup block would gouge into the face by the radius of the insert...is my understanding correct? Any insight on this topic would be appreciated!

Thank you!

 

[DeadStiff]

#1 Yes, it can do funky things or alarm out if you don't.
#2 As long as your in G17(XY plane) it shouldn't matter unless you're using some form of 3D cutter comp. I would just consider it bad form.
#3 I'm not a lathe guy so I'll leave that to others.

 

[Houdini]

I'm gonna be lazy, maybe the answer is here, and elaborated on.

 

[sinha]

#2: Z movement is allowed. In fact, in profile cutting into a plate, on a mill, you may invoke radius compensation in air, and thereafter, dig into the plate. The only restriction is that there should be no two consecutive non-movement commands in the XY plane, while in the compensation mode; otherwise, the next block will not incorporate compensation correctly. It will not alarm out, though.
For example,
G01 Z-1 F_
M08
as consecutive blocks, cannot be used.

#3: There is no specific/different requirements for lead-in/lead-out moves on a lathe, compared to these on a mill. Of course, the nose number must be correct, which we do not have to bother about on a mill.

You are on the right track. All basic doubts must be got clarified.

 

[EmGo]

Any insight on this topic would be appreciated!

Nerd - on a lathe, skip the worthless, stupid, pointless tnr. It's shit. It just fucks up perfectly good programs for no return at all.

Back when we didn't have easy cheap cad and everything had to be trigged out it was useful. But nowadays there are so many cheap effective 2d cad programs for pulling the points, tnr is stupid shit. Just program to tool centerline. Your programs will run better, your life will be better, it will be like banging the tambourine in the celestial choir. Tnr and part surface programming and diameter programming, all that shit is kind of like crack cocaine, people get addicted but in the end, nothing good comes of it.

 

[Donkey Hotey]

Nerd - on a lathe, skip the worthless, stupid, pointless tnr. It's shit. It just fucks up perfectly good programs for no return at all.

What are you going on about? It's absolutely necessary on the lathe. Heck, it's probably more necessary than on the mill. You can't cut a 0.010" chamfer or radius (or any radius really) if the tool has 0.032" TNR. If there's a taper, it will be in the wrong place and size. If there's a precisely sized radius, it won't be round, etc, etc.

And while night shift is here arguing about truncating the dodecahedron, where has @empower been?

 

[EmGo]

What are you going on about? It's absolutely necessary on the lathe. Heck, it's probably more necessary than on the mill. You can't cut a 0.010" chamfer or radius (or any radius really) if the tool has 0.032" TNR. If there's a taper, it will be in the wrong place and size. If there's a precisely sized radius, it won't be round, etc, etc.

This is a joke, right ? And I'm just too dumb to pick it up ?

 

[Donkey Hotey]

This is a joke, right ? And I'm just too dumb to pick it up ?

No, not a joke. For square shoulders, everything is fine without cutter comp. The second you introduce angles and radii, it all goes to hell. The parts turn out wayyyy better with small chamfers, etc.

If you're saying to do that in the CAM software, that's a different story. I program lathe stuff at the control. Plus: I can fine tune the features with the TNR value at the control if I've properly used it.

 

[sinha]

I am of the opinion that using a CAM software on a lathe in an overkill, unless there is an application like parabolic turning.

 

[rjwalker1973]

I am of the opinion that using a CAM software on a lathe in an overkill, unless there is an application like parabolic turning.

For most lathe operations I agree, but we have some live tooling stuff on ours that is much easier with CAM

 

[sinha]

Live-tool programming does need some expertise.
But, can be done.

 

[Mtndew]

No, not a joke. For square shoulders, everything is fine without cutter comp. The second you introduce angles and radii, it all goes to hell. The parts turn out wayyyy better with small chamfers, etc.

If you're saying to do that in the CAM software, that's a different story. I program lathe stuff at the control. Plus: I can fine tune the features with the TNR value at the control if I've properly used it.

It can easily be done on the lathe, if you know trig. I did it for years at the control because it was the stone age and we didn't have a computer or cad until the mid-90's.
My chamfers and radii were perfect, so were my tapers without comp. I made thousands of poly-v sheaves of all different sizes in incremental sub programs.
It's a wonder my hair isn't grey and I'm not bald.


OP,
My best advice for the lathe is just make a move toward the part in X and Z that is larger than the insert radius value set in the control for that tool.
Same with turning off comp... make a move larger than the TNR away from the part.

 

[rjwalker1973]

Live-tool programming does need some expertise.
But, can be done.

Oh yea but when it is faster to just CAM it I do.

 

[maguilera]

Just program to tool centerline. Your programs will run better, your life will be better, it will be like banging the tambourine in the celestial choir.

Honest question. What are the benefits of using centerline programming? Because it feels kind of counter intuitive to me. For instance, if I want to take an external parallel pass at Ø40mm using an insert with a 0.8mm TNR, the program would need to read X41.6, which, as I said before, feels counter intuitive to me.

Cheers.

 

[gmc1724]

Nice to see someone wanting to learn g-code instead of relying on what the cam software spews out. In my opinion I wouldn't let anyone near a CNC unless they can read c-code but the amount of people posting cam programs on this site and asking why it isn't doing what they thought it should is shocking.

 

[sinha]

Oh yea but when it is faster to just CAM it I do.

CAM may not be faster if manual programming is possible.

 

[rjwalker1973]

CAM may not be faster if manual programming is possible.

Thats where experience comes into play. Having the experience to look at a part and know what needs to be done to make it and the best practice to get there in the most efficient way to make a quality part. You know this buddy.

 

[EmGo]

For most lathe operations I agree, but we have some live tooling stuff on ours that is much easier with CAM

But that's really 4th-axis milling

Honest question. What are the benefits of using centerline programming? Because it feels kind of counter intuitive to me. For instance, if I want to take an external parallel pass at Ø40mm using an insert with a 0.8mm TNR, the program would need to read X41.6, which, as I said before, feels counter intuitive to me.

To be brutally honest, it depends on whether you give a shit or not. And I can understand not caring. It's just a job, the parts come out fine, who gives a crap ?

But the why, for me :

A turning tool is round. Yes, once every three thousand years you will have to deal with a sharp corner but in almost all cases, your tool has a nose radius. In 2d it is a circle.

If all you ever did was turn along a surface - either a face or a diameter - then nothing would matter. Pick whatever number you like, no difference. But if you intend to turn faces and diameters and radiuses and chamfers, then the fact that the nose is round matters. This "imaginary sharp tool nose" actually does infuriate me. There is no fucking sharp nose on that tool ! So why do people come up with this stupid crap when the truth is easy and clear and simple ? You are, in effect, rolling a 1/32" circle along a set of lines and arcs. The center of that circle is the tool path. Simple, easy, clear.

When you use cutter comp, all you are doing is telling the control to do the math. So in fact, what you tell the machine is NOT what to do, but where to end up after it does all the work. The centerline is what it calculates from the data you give it. Then that is the actual tool path. You've just added an extra step, for nothing.

On easy stuff that works fine but when things get complicated and it fails, that's when people come here and ask all these cutter comp (and canned cycles, but that's another subject) questions. If they knew what the machine was doing and how to tell it what to do directly, then they wouldn't have these questions.

I do know people who know how it works, and they still use cutter comp. That's because they don't really care. If they have a problem, they also know what's really going on so they know how to fix it. I wouldn't say they are lazy, they just care about other things but I have ocd about turning. I don't like sloppy programs very much.

But if you're like Donkey here and you don't even know ... well, at the very least you should know how it really works, so you don't get trapped when things go wrong.

Since you brought it up, I was thinking ... it's probably only people like me who grew up driving a lathe or mill, then got into nc, who care. I want the tool to go where I tell it, and no hopping around like a fucking bunny rabbit.

People who started out on Mastercam or whatever are different. They grew up with a program that had a set of choices, so they think this is machining. To me, it's not. It's driving a program that does metal-cutting but what they are doing is choosing from a set of menus that do z-level roughing or hole drilling or pocket removal, spiral or back and forth, whatever. They are not telling the machine what to do. Whether they think of it this way or not, they are not machining. They are choosing between predetermined options on a computer.

For mill work I guess the ends justifies the means. But for lathe work, it's just as easy to do it correctly and then the machine does exactly what you ask it to, not what some dork in an office thought looked cool onscreen.

Went through this with Sandy Livingstone years and years ago. Lathe cam has not improved. For regular ol 2 axis lathe, a hand-written program will flat kick ass over anything out of any cam program, including all those cool fanuc features. I can't count the number of times I've read a question here and just scream in my head "just write the fucking tool path ! you don't need all that retarded shit !" but people don't want to hear that. They want to use fanuc feature 173.4-a subsec p, or change the parameters, or whatever.

Lucky for me I don't work in their shop

btw, in your example, it should be x 20.8 With a 40 mm diameter profile, from center is 20 then the radius is .8 so x=20.8

Just draw up the profile in 2D ....

 

[DouglasJRizzo]

Hi Everyone!

I have a few questions about cutter comp I am hoping y'all could help with (especially #3):

1) It is my understanding that when invoking cutter comp on a mill, the G41/G42 line must include either a G00 or G01 move of at least the radius of the tool in either, X, Y, or X AND Y. Is that correct?

2) It is my understanding that whilst in G41/G42 on a mill you either 2.1) can not or 2.2) should not make Z moves. Are either of those correct?

3) How the heckarooney do you properly invoke cutter comp on a lathe for a standard turning op? I have been successfully getting away with it but don't actually know what I am doing! I have read the FANUC section on it and I THINK it sounds like you are supposed to make an X move on the G41/G42 line at a Z location somewhere "upstream" of where you will be cutting and from there it will move such that 2) the tool nose center will be lined up in Z to the programmed location of the very next block...the block right after the startup block. If that is correct then going to Z0. on the block right after the startup block would gouge into the face by the radius of the insert...is my understanding correct? Any insight on this topic would be appreciated!

Thank you!

1) Most controls require a G01 mode either before or during Cutter Comp engagement. There has to be at least one axis movement - in the plane the machine is programmed.

2) Z axis moves are allowable, and sometimes needed for clearance, but usually not done.

3) In turning centers, cutter comp is invoked similarly to mills - a G01 line perpendicular to the surface. It is disengaged the same way, a single G01 line off of the part.
So, I usually program an OD like this:

G0 G99 T0404
X8. Z8. M8
G96 S800 M3
X.75 Z.12
G1 G42 Z0
X1.25 R-.032
Z-.5
X1.75 R-.032
Z-1.
G40 X1.875 M9
G0 X8. Z8. M5
M30
%

 

[e30ryan]

1) It is my understanding that when invoking cutter comp on a mill, the G41/G42 line must include either a G00 or G01 move of at least the radius of the tool in either, X, Y, or X AND Y. Is that correct?

Just a slight revision to this. The length of the compensation move you want/need depends on how your tool path is created, not necessarily on the size of the cutter. Center compensation (none), CAM compensation, Control compensation, etc. If the toolpath is offset from the edge (CAM compensation), then the length of the move only needs to be larger than any wear adjustments you want to make. The control has no idea (and doesn't care) how large of a cutter you are using.

For example, I can use a 1/2" cutter with an offset path (CAM compensated), and using a 0.010" compensation move is fine (as long as I don't try to put more than 0.010" of wear compensation in).