[party o one]

HI All
Be easy on me I'm a virgin here, this is my 1st post.

We just picked up an IKEGAI-AX15Z lathe with an upgraded Fanuc 6T-B control(this machine is older than dirt) . I have never used anything older then Fanuc 0-M. We did get a programing book, but the funnest thing there is no G-code listing for tapping cycle (G-84) is there a different cycle I'm suposed to use for tapping?(from the days before sand). It took me some time to figure out you use what they call a face groving cycle for peck drilling.
Oh and I'm a milling man not a lathe man , so take your shots and have your fun. Just get me where I can put a 3/8-16 tap into the end of a round, spinning piece of steel, how hard can it be?

[party o one]

This is just a bump. I hope this gets me back to the top. Anyone got an answer good or bad?

[Dan Fritz]

The 6T-B has several types of single-point threading cycles, but not a "Tapping" cycle per se. If you have user macro capability, you can write any kind of tapping cycle you want as a macro.

We used to use a spring-loaded tap holder, and we would program a Z move to engage the tap with feedrate slightly slower than the thread pitch would call for. As the tap ran into the hole, the spring loaded holder would extend a bit, then, when the spindle reversed and the Z retracted, the tap holder would compress a bit. No dramas. Just a Z minus move with a feedrate, then an M04 and a Z plus move in the next block.

You can tell if you have user macros on the 6T-B by pressing the OFFSET button twice. If a "MACRO VAL" page shows up, you've got the macro option. With the macro option, you can make any G-code into a tapping cycle, using variables for spindle speed, depth, tap pitch, etc.

[party o one]

Thank you Dan
I do have a spring loaded tap holder I can use and I'll check out the macros opp. My Fanuc 0M has it (G-65 or something) I haven't had to use that for 10 or more years, we setup a DNC straight to a PC and we could run as big a program as we wanted. I changed jobs on the machine today so I'll post when I go back to that job to let you know how it went. I knew it would be something simple.

DRRRR DAAAA DRRRRR

Let me see if I understand you right.

3/8-16 TAP

N10 M3
N20 G01 Z-1. F.06
N30 M4
N40 G01 Z .05 F.06

Once again Thanks Dan

Party O One

[Dan Fritz]

Your program should work, but beware that your spindle speed may not be exactly what you program with your S-code. DC Spindle drives are somewhat adjustable for speed, so when you calculate your feedrate, it may not extend or compress your tap holder exactly as you expect. You may have to adjust the spindle speed or the feedrate to make it so the tap holder does not overextend or overcompress.

Also, the spindle drive has an adjustment for accelleration and decelleration, so the M04 may take a bit longer than expected to completely reverse the spindle. This is especially true with lathes that have large chucks or long bars inside barfeeders. If your spindle drive takes a long time to stop & reverse, you should put the M04 in a separate block. That would make sure that the spindle is "up-to-speed" in reverse before the Z axis starts backing out. In your example, the M04 is in a separate block. If the spindle reverses FASTER than that, just put the M04 in the same block as the Z minus move, like so:

N10 M3
N20 G01 Z-1. F.06
N30 M4 Z .05 F.06

That way, the Z will reverse direction without a delay for the spindle to reverse.

In any case, you'll have to play with this a bit and watch the spring loaded tap holder. Once you get it right, It should repeat the thread depth very well, and you can just modify the Z move to adjust the depth.

[party o one]

Worked like a champ. Almost no spring movement.

One minor note for those reading. You need a M5 between the M3 and M4, at less on my machine.

M3
G1 Z-1. F.06
M5
G1 Z.5 M4 F.06

Thanks Dan :cheers:


Party