On Thursday 17 November 2016 02:11:53 hubert wrote: > I have a step and Direction driven AC Servo spindle with encoder > output that is supposedly capable of rigid tapping. I want to tap > some 1/4 inch aluminum with M3x0.5 spiral flute HSS tap. Initially I > have the spindle speed set at 150 rpm. What type of tapping cycle > should I use, Continuous, or some type of peck cycle. Also what are > your > recommendations at some test trials to get the feel of the Machines > capabilities. I have on hand up to 8mm taps, should I try one of > those first. I hope not to break a tap in a part that already has > time invested in it. I know I could hand tap them, but that wouldn't > give me experience in rigid tapping. > > Thanks > > Hubert
Study up on the gcode G33.1. This is not normally a peck tap routine. however there is no problem wrapping it up in a routine that does a peck, increasing the z depth per peck by whatever amount you feel the tap is comfortable without clogging. Here is code I run, for a 3mmx0.5 metric tap, but itsnot near as capable a tap as your spiral flute tap, clogging in a deep hole, but this code has yet to break a straight flute 3mmx0.5 tap. You'll see a pause before it starts a new peck, giving you time to blow the tap clean and put a little bit more buttercutt on it. ========================================= % ( tap3mmhole.ngc ) ( center over hole to tap, z touched off with tap tip just above hole ) ( working in metric ) G21 ( measure in mm's ) #<_z_depth> = -18.00 ( peck decrement, a bit farther each time, adjust to suit) ( try at 4 to 6 for your tap if its a deep hole ) #<_z_dec> = [ #<_z_depth> / 12 ] (debug,8 z_dec=#<_z_dec>) #<_z_tmp> = 0.00000000 g1F50 z#<_z_tmp> ( here, the usable speed depends on how fast your spindle ) ( can reverse as there will be an overshoot! but z will track it ) ( which means the tap can bottom and break if too fast ) S400 M3 o100 WHILE [#<_z_tmp> ge #<_z_depth>] G33.1 Z#<_z_tmp> k0.500000 ( per turn for metric tap is as marked ) ( inch taps, then k is reciprical of tpi. In inches of course. ) #<_z_tmp> = [#<_z_tmp> + #<_z_dec>] G4 P3 (4 second pause to blow chips off tap & buttercutt the tap ) o100 ENDWHILE M5 (stop spindle) G20 (back to inches) M2 % =================================== I have some hal code that will give you the overshoot value expressed as encoder edges, which can be converted to distance by kcalc or similar. Because of the mass of the chuck on a lathe, it is much harder to reverse than a mill spindle so the overshoot distance can grow to unusable amounts very quickly. But 125-150 revs is usable on TLM, which has a 5" 4 jaw on it. I hope this helps, Hubert. It is not the only way, but this works for me. As always, cut air above the hole first. Touching z off about an inch high for the first run in case I missed something. And make sure your hole is deep enough, which with a 2.5mm drill, will require a peck drill else it may clog the flutes and break the drill off in the hole if not retracted and cleaned. Cheers, Gene Heskett -- "There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order." -Ed Howdershelt (Author) Genes Web page <http://geneslinuxbox.net:6309/gene> ------------------------------------------------------------------------------ _______________________________________________ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
