Two fold post, Wasino LJ63M m12 ?? and hex milling on it.

DMSentra · Nov 17, 2020

Going through old programs that were in the control trying to learn it's milling and I see an M12 right after the start.
N2(3/4 END MILL T0202)
G0M41G99G97G80G40
M12
M4S2000T0202
G0M8X0Z.1F300.
The manual for this live tooling lathe doesn't list M12, just M10/11(chuck clamping) and next in line is M19. Anyone familiar with that M12 critter?

Also, can anyone supply a small sample of a milling program for a hex or square on the end of a shaft using an old live tooling lathe like this. Once I get my head wrapped around how cutting from a square or hex point and somehow making code go closer to X0 and back out to the next point while the C axis is rotating I can start understanding the rest. Just cutting that simple feature has me stumped.

wmpy · Nov 18, 2020

We have some newer live tool Wasinos, but none of them have any description in the book for M12. Is that sample code you posted for using the live tooling? If so, it may be a C-axis engage or spindle clamp or live tooling engage code. Have you tried that code in MDI? What does the M41 in the 2nd line do?

What control is on the machine? Are you sure that it has full C-axis? I think this is a pretty old machine and am a little doubtful that it has full C-axis capabilities- in which case, you couldn't do any cutting with the C-axis turning.

DMSentra · Nov 18, 2020

wmpy said:
We have some newer live tool Wasinos, but none of them have any description in the book for M12. Is that sample code you posted for using the live tooling? If so, it may be a C-axis engage or spindle clamp or live tooling engage code. Have you tried that code in MDI? What does the M41 in the 2nd line do?

What control is on the machine? Are you sure that it has full C-axis? I think this is a pretty old machine and am a little doubtful that it has full C-axis capabilities- in which case, you couldn't do any cutting with the C-axis turning.

That is the code from the control I assume there were running. All those you mentioned (C axis, spindle locking, C axis gear on) are all accounted for in the manual. I haven't tried it in mdi yet, need to do that. M41 is high gear main spindle. This is a Fanuc 10T control. Whether it's full C or not is part of what I'm trying to figure out.

DMSentra · Nov 18, 2020

This is part of another program with M54(C axis gear on) and M12.1(idk what that is as it's not listed either).
N3(3/4 END MILL T0909)
G0G40G80G97G98G18M41
M54
G28H-30.
G50C0.
T0909
M4S400
G1X1.0Z.5F300.
M8
G12.1
G1G98G41X1.5708F30.
G1Z-.365F10.
X.7854C-.6802F2.0
X-.7854
X-1.5708C0
X-.7854C.6802
X.7854
X1.5708C0

wmpy · Nov 18, 2020

It looks like your machine does indeed have a full C-axis. That code you just posted is to mill a hex on the end of a part. G12.1 is polar interpolation. Do a search on that to learn more.

I don't know what M12 is. It could be something like parts counter. Maybe?

DMSentra · Nov 19, 2020

Ran across a video showing C milling 12.1, the poster mentioned swapping whatever Y value you would have for a feature for a comparable C value. Drawing it on CAD it looks to work.

TeachMePlease · Nov 19, 2020

DMSentra said:
Ran across a video showing C milling 12.1, the poster mentioned swapping whatever Y value you would have for a feature for a comparable C value. Drawing it on CAD it looks to work.

That is exactly how polar works.

On some controls, you actually program with an X and Y coordinate even. This is polar interpolation. You turn it on, program in X/Y (or X/C) for the feature you want, and the control does the math to make C and X work to create a Y axis.

DMSentra · Dec 7, 2020

So far it runs the sample program without issue, but I think tool touchoff for the endmill may be wrong. I'm setting that the same I do a turning tool but it's nowhere close to the dimensions programmed. I've got job coming that I need this hex to work to get the job. I'll try to post my program tonight if someone doesn't post a clue to my failure by then.

G1Z-.2F5.
X.463C.801
X-.463C.801
X-.925C0
X-.463C-.801
X.463C.801
X.925C0
X.463C.801
G0Z.5

Seems simple enough but cuts a slim diamond instead of a hex.

DMSentra · Dec 14, 2020

TeachMePlease said:
That is exactly how polar works

On some controls, you actually program with an X and Y coordinate even. This is polar interpolation. You turn it on, program in X/Y (or X/C) for the feature you want, and the control does the math to make C and X work to create a Y axis.

You have any idea why I'm getting a diamond shape instead of a hex? I've tried with and without re-stating the C values with no C movement. I've read yesterday I may need to double the C values and of course that only changed that movement. 3/4" end mill with spindle centerline set for it's offset value. The diamond is roughly 1" long and .2" wide. Tried G42 also.

wmpy · Dec 15, 2020

What size hex are you trying to make? The X and C values in the code you posted don't look right.

wmpy · Dec 15, 2020

OK, I just did some math, and you need to double your X numbers. Even with polar interpolation, you still need to program the X as if you're giving diameters. So, when the X point is 0.925" away from center, you need to tell it X1.85 .

DMSentra · Dec 15, 2020

The point values of the hex are X.925Y (C)0, X.463Y(C).801, and continued around using the appropriate + and - where needed.

DMSentra · Dec 15, 2020

I started with these values and doubled the C values per some posts when the originals wouldn't work. The weird thing is the diamond shape it cuts instead of a hex.

DMSentra · Dec 15, 2020

Ohhhh, so my modified C are right now but going radius values for X are not. I'll try that next then. Gracias.

DMSentra · Dec 17, 2020

I have it cutting a hex finally. And the distance across the flats is correct. But, the flats are slightly convex, enough to make the distance across the points 1.797 instead of the correct 1.85. Seen this issue before?
X1.85,C0/ X.926,C.801/ X-.926C.801/ X-1.85C0/ X-.926,C-.801/ X.926,C-.801/ X1.85,C0.

wmpy · Dec 17, 2020

Maybe you're feeding too fast? Try slowing the feed down and see if you get the same results.

Are you using G41/G42 cutter compensation? If so, what value do you have for R on the offset page?

DMSentra · Dec 17, 2020

wmpy said:
Maybe you're feeding too fast? Try slowing the feed down and see if you get the same results.

Are you using G41/G42 cutter compensation? If so, what value do you have for R on the offset page?

Feed is slow enough it's hard to believe that's a problem. G41, and I forgot to even look at the R so that's next after the dinner break. Thanks.

DMSentra · Dec 17, 2020

All comp and T and R values were 0 so I tried several different things, only change was adding diameter to the part when changing the X comp.

wmpy · Dec 18, 2020

Some of the things you posted aren't quite adding up to me... You said, "3/4" end mill with spindle centerline set for it's offset value". That's good. The end mill should have an offset value in X such that when the center of the end mill is in line with the center of the spindle, it should be at zero.

You said that the R value is at 0. Great. That's what I do. I only use it for compensation once the tool wears.

But then, you said that you're expecting to measure the points at 1.85" as programmed. Here's where you're losing me. Since your R value is 0 in the offset, you need to compensate for the radius of the end mill in the program. I thought you were trying to make a 0.852" hex. That would be (0.801-0.375)*2. The 0.801 is the C position from the program. The 0.375 is the radius of the end mill. What size hex are you trying to make? If you're trying to make a 1.602" hex, then you need to re-figure your hex points as if it were a (1.602 + 0.750) hex.

My guess is that you're looking for a 1.602" hex, didn't compensate for the end mill in the program, and got the machine to kind of cut to size by moving the X offset up so that the center of the tool is no longer zeroed at the center of the spindle. That would give some funky geometry like you're getting.

I hope this helps. I suppose I could be way off base. If I am, and your program is good, then I would start looking for mechanical issues with the machine like loose belts on the spindle.

DMSentra · Dec 18, 2020

Let me say now this is my first go with C axis and so far it's a totally foreign critter. So I'm starting from scratch on this and what I'm doing may make little sense as I'm trying whatever might seem to be a solution.
The size of the hex I'm working for is 1.85 ptp, 1.62 flat to flat. 2 points are on C0(Y0) for hex orientation, which is also something I may be doing wrong as I am starting from a program left in the control when I purchased the machine. No idea if the C orientation is right to cut the widest points on the X plane or I need to change that in the program too.
I've since found out the X1.85 is not right, and am now on to X.926(2x the X vector of .463 to that point. I'm now at X.926C.801 for the point at 60deg, and cutting points to the left as I go. I just this second realized it's cutting CW with my programming going CCW around the hex.
I am using g41 But no idea if the system is picking it up yet.
Does that clear some of my mud?

Two fold post, Wasino LJ63M m12 ?? and hex milling on it.

Cast Iron

Hot Rolled

Cast Iron

Cast Iron

Hot Rolled

Cast Iron

Diamond

Cast Iron

Cast Iron

Hot Rolled

Hot Rolled

Cast Iron

Cast Iron

Cast Iron

Cast Iron

Hot Rolled

Cast Iron

Cast Iron

Hot Rolled

Cast Iron

Similar threads