[Beezle]

In 6061, 0.75" blind holes, drilled with a No 21 (0.159) bit, cleared out, full of aluminum specific tapping fluid.

10-32 HSS spiral flute tap bought from McMaster: McMaster-Carr

Program using M871, spindle speed of 1000, tapping head settings to Procunier and TPI of 32 for 871. Tap to 0.6 into the hole.

First try, snap on withdrawal. This also happened the last time I tried to do this in brass. Brass? I've tapped many holes before with no problem.

Am I missing something? I did order some of the taps Tormach sells to try. I'd go manual if these little taps had a dimple for a tap guide.


PS, any tips on removing the @#$%ing tap appreciated. I assume the $60 worth of 1" 6061 plate is headed to the recycle bin.

[SCzEngrgGroup]

For machine tapping, especially when going that deep, you need to use a lower thread percentage, which means a larger drilled hole. For 10-32, use #18 instead of #21. Or, if you need a 75% thread, only machine tap to 0.5" depth, then do the last 1/4" by hand, or using a drill-driver. Also, PLENTY of oil, or aluminum tapping fluid, not coolant.

If you want to preserve the hole, take the plate to a machine shop with an EDM machine, and have the broken tap removed. You can also drill out using a carbide endmill, though it will trash the endmill. After drilling it out, you can clean up the hole, and turn a plug with a heavy press fit (0.003" or so), then press the plug in, surface it flush, and re-drill and tap the hole.

Regards,
Ray L.

[Beezle]

Thanks. I think I will try the machine/hand approach. I was thinking about that.

Fussed over my spindle calibration and got it within 1% for the speed used for tapping.

[Philbobb]

For tap removal, check out:

Tip to Remove broken Tap, Drill, Reamer

[waltpermenter]

Seriously, get yourself a set of tap extractors, they work very well and no damage to your part from trying to mill them out or the expense of edm.
Tap Extractors for Machine Screw, Hand, Pipe & STI Taps | Walton
walt

[MichaelHenry]

Just guessing here but you might also try drilling deeper, tapping more shallow, and dropping the spindle speed to 500 rpm or so. I've been tapping a lot of 8-32 blind holes lately with a spiral point tap and notice the tap might run a couple of threads deeper when the program depth is reached before the spindle fully reverses. Drilling 0.75" deep for a nominal 0.50" deep tapped hole and tapping at 500 rpm has worked flawlessly for me in aluminum.

I've only tried spiral flute taps but have had more trouble with them snapping than with the spiral point taps, maybe because of the depth I was tapping. I've started using form taps and am growing to prefer them, at least for smaller holes.

Mike

[popspipes]

I drilled a 10 24 out of an aluminum part with a carbide spotting drill. I lined it up in the old Bridgeport, locked the xy down and slowly advanced the spindle, drilled it out and didnt damage the spotting drill either maybe a stroke of luck??

edit: I am relatively new to this machine tapping, but on my 5mm .8 (close to 10 32) holes I use 320 rpm 10 ipm, drill for a 75% thread.5 second delay at the bottom of the hole, seems to work fine.

[Beezle]

Seriously, get yourself a set of tap extractors, they work very well and no damage to your part from trying to mill them out or the expense of edm.
Tap Extractors for Machine Screw, Hand, Pipe & STI Taps | Walton
walt

I have other extractors but had no idea those existed. Seems they may be less effective with spiral flute taps as there is little room for the fingers, but I'll get a set anyway as I do use form taps too.

Thanks for all the suggestions everyone.

[Beezle]

I noticed that both of these taps snapped at the same spot - just at the top of the spiral flutes. Maybe that's a weak spot on these taps?

What brand taps do you all use and where do you get them? 10-32 most of the time, with the Procunier head.

[Superman]

I noticed that both of these taps snapped at the same spot - just at the top of the spiral flutes. Maybe that's a weak spot on these taps?

What brand taps do you all use and where do you get them? 10-32 most of the time, with the Procunier head.

Curious..... are you using a rigid tap cycle with a T/C holder ? or a sold collet type holder ?
---- some machines say they have "rigid tapping" ....but .... they don't lock the spindle rotation with the tapping axis.....spindle stopping & reversing when feed dead stopped, is NOT rigid tapping

Suggest using a T/C holder, even if you do have rigid, just to take some of the shock off the tap when reversing the spindle.

[BAMCNC.COM]

https://www.youtube.com/watch?v=b2M6ta7QtIg

[SCzEngrgGroup]

Curious..... are you using a rigid tap cycle with a T/C holder ? or a sold collet type holder ?.

As the thread titles says, he's using a Procunier tapping head.

Regards,
Ray L.

[velocityxlrg]

I have a similar setup with a Procunier and a Series 3. I was snapping taps until I got a tachometer and calibrated the spindle speed. That got things pretty close, but I got things even closer by picking a certain speed (lets say 1000 rpm) and then just before tapping that day, recording the actual speed with 1000 rpm selected (lets say 1012 rpm). I then tweak the spindle speed up or down until I get my desired 1000 rpm (or as close as possible). The other thing I did was to set my Z travel to lets say 31.25 inches per minute (1000 rpm divided by 32 threads per inch). I then lifted the head as high as possible and timed it with a stopwatch as it went down for a certain distance. For example G01 Z-15.0 F31.25 I timed the head travel for 10 of those 15 inches (to let the machine accelerate and decelerate to the proper speed). It should take 28.8 seconds to do 10 inches. It doesn't. So I figured out a speed that will give the required rate. I did this for all the regular tap sizes, RPM and speeds and wrote it down. Now I just look it up, and I don't break taps anymore.

[SCzEngrgGroup]

Spindle speed should not be at all critical, as the distance travelled with the tap engaged in the workpiece is so short. Just for added safety, you should under-feed slightly (5-10% is typical), to ensure you don't push the tap. The tapping head will dis-engage and re-engage automatically if you're going too slow

If your measured travel times are not VERY close to what they should be then something is VERY wrong somewhere. Acceleration time should insignificant unless you have it set ridiculously low.

Regards,
Ray L.

[BAMCNC.COM]

Velocity - anyway I can get that info from you - I'm sure it's closer than my setup now - but you did watch my video right?

Ray - Good info on downfeed, I think there is "pull" left in the tap head - but at the same time there is still some slop in push. Not sure if it matters or not with the slow speed of a Tormach

[SCzEngrgGroup]

Velocity - anyway I can get that info from you - I'm sure it's closer than my setup now - but you did watch my video right?

Ray - Good info on downfeed, I think there is "pull" left in the tap head - but at the same time there is still some slop in push. Not sure if it matters or not with the slow speed of a Tormach

Tapping heads are different - the cheap Chinese ones are knock-offs of the Tapmatics, while the Procunier is another, far better, animal entirely. The Tapmatic have a pretty wide range of compliance on both directions - you'd have to over or under feed by a considerable margin to have any problems. I've accidentally run up to 30% over-feed with no problems. The Procunier is, I think, not as forgiving about over-feed, as I don't believe they will compress further from the fully engaged position the way the Tapmatics will. So it is wise to under-feed by 5-10%. Both heads, when under-fed, will simply dis-engage and re-engage as needed to stay in an acceptable range of travel. The major advantage of the Procunier is it uses conical friction clutches, rather than dog clutches. This makes the engagement very smooth, where the Tapmatics and Chinese head engage with a Bang!, which is stressful on the tap.

I got a deal on a Procunier head a couple of weeks ago - $100 for a 1E in perfect condition. I haven't tried it yet, as I'm going to convert it to use quick-change tap holders before I start using it.

Regards,
Ray L.

[Beezle]

Velocity - anyway I can get that info from you - I'm sure it's closer than my setup now - but you did watch my video right?

Ray - Good info on downfeed, I think there is "pull" left in the tap head - but at the same time there is still some slop in push. Not sure if it matters or not with the slow speed of a Tormach

I watched your video the other day when I was pondering this issue.

I am curious what led you to use a drill cycle vs. plain code or the 87x macros?

[BAMCNC.COM]

Ray, I'll slow the down feed by 5% from now on.

Beezle - HSMWorks uses only "cycles" for drilling, so I had no choice but to try it. However with a post edit I can now have it do long hand g-code and it works with the numbers I enter for feeds now. I'll probably never use a cycle again - but it works.

[velocityxlrg]

I am not making any claims that these numbers are at all appropriate, only that I am using them on my Series 3 with a Procunier with some success in a non-production, limited run, environment.

Aluminum

6-32 S950 (corrects to 1000 rpm) F33.6 (corrects to 31.25 ipm)
8-32 S950 (corrects to 1000 rpm) F33.6 (corrects to 31.25 ipm)
10-32 S488 (corrects to 500 rpm) F16.8 (corrects to 15.625 ipm)
1/4-28 S488 (corrects to 500 rpm) F19.2 (corrects to 17.86 ipm)

Mild steel

6-32 S721 (corrects to 750 rpm) F25.2 (corrects to 23.44 ipm)
8-32 S721 (corrects to 750 rpm) F25.2 (corrects to 23.44 ipm)
10-32 S721 (corrects to 750 rpm) F25.2 (corrects to 23.44 ipm)
1/4-28 S327 (corrects to 333 rpm) F12.78 (corrects to 11.89 ipm)

I use spiral flute bottom taps and leave 0.15" at the bottom of blind holes.

[CDGentile]

Not to derail the thread, but I had a similar issue this weekend - 0.75" through holes in 6061, drilled 0.1590", tapping 10-32 with spiral point tap and Procunier head.

I used the recommended M871 cycles with a P of 1.0 (from a 0.2 clearance height), but broke the tap on the 2nd hole when I was tapping full depth. After that I switched to a manual 'peck cycle', 0.3 at a time, and got good results on the other 150+ holes (making a tooling plate).

Is there a better/faster solution? Does anyone else use peck tapping with the Procunier?

Thanks-