[metlshpr]

Could anyone please post a lathe tap cycle for a fanuc control? I don't think that I am getting the feed and speed right. I'm using a standard .375-24 tap.

[DocHod]

Hi , if you are looking for something for rigid tapping these blocks may help.

O0018(3/8-24 TAP)
T0606(TAP CYCLE)
G0X0.Z.1M08
M29 (CONTROLER MAY REQUIRE THIS M CODE SOME DO NOT)
G84Z-.975R0.F.0416 M03S600 (RIGID TAPPING CYCLE)
G0Z.1M09
G80
G28U0.M9
M5
M30

Or the good old fashion way with a spring loaded tap holder

O0018(3/8-24 TAP)
T0606(TAP CYCLE)
G0X0.Z.1M08
M03S600(R.P.M. DEPENDS ON THE REACTION OF YOUR MACHINE)
G32Z-.975F.0416 (TAPPING CYCLE)
M04
G32Z.1F.0416 (FEED BACK OUT MAY BE A LOWER FEED RATE)
G0Z1.M09
G80
G28U0.
M5
M30

[metlshpr]

Thanks.That helped alot. I like the oldfashioned way.

[DocHod]

Yeah whats nice about G32 on older machines is that if your feed rate override is set anywhere above or below 100% for operations other than the tap , the machine should still feed at the proper feed rate for the tap when the controller reads the G32 (it locks out the override). Just curious but how were you doing your tapping cycle prior to my last posting I know at one time long ago I had a cnc machine that did not have a tapping cycle and I just used a G01 and you had to be right on the money with the feed rate override dial , anybody remember the Southbend cnc lathe with the ultrapath programing ? or even further back , the old Herbert 3M automatic turret lathes with the pegboard I use to set up , or the old Clevomatic 2 1/2 A.B. with the cam action apparatus or even further back and I know some of those old beaters are still pumping out parts , man I think I've been in this profession too long ! Boy I look back at those days and appreciate what any of the machine builders do today.

[chakaloso]

Hi!

I am learning about tapping in a CNC lathe and I like to know if there is a ration between RPM and the feed rate. I know for milling there is a ration between TPI and feed rate.

Thanks !

[chakaloso]

Is there a ration between feed rate and spindle speed in tapping?

[g-codeguy]

Is there a ration between feed rate and spindle speed in tapping?

No ratio as a lathe is normally programmed in IPR so the spindle speed has no bearing on the feedrate.

[g-codeguy]

Thanks.That helped alot. I like the oldfashioned way.

You might want to consider using a smaller lead for the infeed, and then pull out at the correct lead.