[Don Clement]

Once you learn how to use form taps in aluminum, you'll never go back to cutting taps.

The max size limit on using form taps with the Procunier 1E in aluminum is #6, M3.5 http://www.rockford-ettco.com/Downlo...1000-23000.pdf With my Procunier 1E on blind holes in aluminum I use form taps for sizes less than #6 and spiral flute cutting taps in sizes #8 to 1/4. BTW with my Procunier in the Tormach I use 100% feed, no dwell, 200% feed retracting and don't break taps unless making a mistake like forgetting to reset the feedoveride. Also remember to use a larger size drill for the "H" value of the tap. Each "H" value means the tap is oversize by 0.0005". For example an H5 tap is oversize by 0.0025" and the drill size must be larger accordingly. On through holes #8-1/4" in aluminum I use a spiral pointed gun tap with the Procunier 1E.

Don Clement

[shred]

Last night I ran 350 #8-32 holes form-tapped in Aluminum with an ER-20 tension-compression head. Worked great (likewise I found that dwell wasn't needed). It didn't seem to require a lot of HP so any ideas why Procunier doesn't recommend anything bigger than #6?

[BAMCNC.COM]

I'd assume it could slip on the friction clutch?

[SCzEngrgGroup]

Last night I ran 350 #8-32 holes form-tapped in Aluminum with an ER-20 tension-compression head. Worked great (likewise I found that dwell wasn't needed). It didn't seem to require a lot of HP so any ideas why Procunier doesn't recommend anything bigger than #6?

The Procunier uses a conical friction clutch. The 1E is rated for cutting taps up to 1/4". Form taps require a bit more torque than the same size cutting tap, so it has to be a friction limit in the clutch. There are larger Procunier heads that will handle larger sizes.

Regards,
Ray L.

[Don Clement]

Last night I ran 350 #8-32 holes form-tapped in Aluminum with an ER-20 tension-compression head. Worked great (likewise I found that dwell wasn't needed). It didn't seem to require a lot of HP so any ideas why Procunier doesn't recommend anything bigger than #6?

Were they blind holes?

Don C.

[Don Clement]

The main differences between the Procunier reversing tapping head and the tension-compression tapping head are that the Procunier has a double-cone cushioned clutch that stops within 1/3 revolution and that the Procunier reverses the spindle at twice the tormach spindle speed when the Z-axis feed is going up which means no Tormach spindle reversing is needed. This means that the Procunier is perfect for quickly tapping blind holes. IMO for tapping through holes there may be no advantages of using the Procunier over the tension-compression head but no comparison when tapping blind holes in the Tormach. Programming is also easier with the Procunier only three line needed: spindle speed, 100% downfeed, ( no dwell), 200% upfeed.

Don C.

[shred]

Were they blind holes?

Don C.

Not in this case, although the form tap was bottoming because it's the only style I happened to have.

Without the dwell, it's just one G84 line per hole, although Tormach discourages that.

Close tolerance blind holes take a lot of tweaking with the T/C head-- I do very little of that.

[rowbare]

Last night I ran 350 #8-32 holes form-tapped in Aluminum with an ER-20 tension-compression head. Worked great (likewise I found that dwell wasn't needed). It didn't seem to require a lot of HP so any ideas why Procunier doesn't recommend anything bigger than #6?

The 1E is quite small, about the size of a large apple. It would start to slip because of the required torque. They have 4 different sizes, the largest one will drive a 1" tap into steel.

bob

[Beezle]

The main differences between the Procunier reversing tapping head and the tension-compression tapping head are that the Procunier has a double-cone cushioned clutch that stops within 1/3 revolution and that the Procunier reverses the spindle at twice the tormach spindle speed when the Z-axis feed is going up which means no Tormach spindle reversing is needed. This means that the Procunier is perfect for quickly tapping blind holes. IMO for tapping through holes there may be no advantages of using the Procunier over the tension-compression head but no comparison when tapping blind holes in the Tormach. Programming is also easier with the Procunier only three line needed: spindle speed, 100% downfeed, ( no dwell), 200% upfeed.

Don C.

Except for when it snaps taps, as it has been doing for me.

I spent the money on it with the hope that tapping would be reasonably reliable. Right now, I can't say that is the case.

I did calibrate the spindle speed a bit and tested with some through holes and it seems fine, but I won't be risking a part doing blind holes again anytime soon. Might do a test though.

I did change the spindle steps a fair bit calibrating so maybe that was it, but I won't know until I try again.

[SCzEngrgGroup]

Except for when it snaps taps, as it has been doing for me.

If you're snapping taps, then you're using it wrong. You must KNOW the actual spindle speed to use it safely. Then you simply feed down to depth at 5-10% less than (RPM / Pitch), and back out at twice that feedrate. On blind holes, allow PLENTY of extra depth, especially if using spiral point taps. If the tap bottoms out, it WILL break. Never use hand taps. Don't try to go too deep - the practical limit for smaller taps is 1/2" or less for really small ones, unless you pre-drill the hole over-size. As with most everything in CNC, take the time to understand how and why a tool works, then use it properly, and it will work perfectly pretty much every time.

Regards,
Ray L.

[Don Clement]

If you're snapping taps, then you're using it wrong. You must KNOW the actual spindle speed to use it safely. Then you simply feed down to depth at 5-10% less than (RPM / Pitch), and back out at twice that feedrate. On blind holes, allow PLENTY of extra depth, especially if using spiral point taps. If the tap bottoms out, it WILL break. Never use hand taps. Don't try to go too deep - the practical limit for smaller taps is 1/2" or less for really small ones, unless you pre-drill the hole over-size. As with most everything in CNC, take the time to understand how and why a tool works, then use it properly, and it will work perfectly pretty much every time.

Regards,
Ray L.

I have tapped 10s of thousands of blind 4-40 holes in 6061-T6 with a Balax form tap using the Procunier in my Tormach. I tap at the Procunier recommended 100% feed see: CNC Self-Reversing Tapping Attachments From Rockford-Ettco Procunier . I don't break taps unless doing something wrong like leave the feed override on. I also regularly tap 10-32 through holes using the Procunier and spiral pointed gun tap in 6061-T6 with no issues.

Don Clement

[waltpermenter]

I have tapped 10s of thousands of blind 4-40 holes in 6061-T6 with a Balax form tap using the Procunier in my Tormach. I tap at the Procunier recommended 100% feed see: CNC Self-Reversing Tapping Attachments From Rockford-Ettco Procunier . I don't break taps unless doing something wrong like leave the feed override on. I also regularly tap 10-32 through holes using the Procunier and spiral pointed gun tap in 6061-T6 with no issues.

Don Clement

he's never used a procunier yet so of course he knows more than you.

[Hirudin]

Except for when it snaps taps, as it has been doing for me.

I spent the money on it with the hope that tapping would be reasonably reliable. Right now, I can't say that is the case.

I did calibrate the spindle speed a bit and tested with some through holes and it seems fine, but I won't be risking a part doing blind holes again anytime soon. Might do a test though.

I did change the spindle steps a fair bit calibrating so maybe that was it, but I won't know until I try again.

So it's working in through holes but not blind holes? To me, that strongly suggest the problem is with something other than the tapping head. After-all, it doesn't know what kind of hole you're tapping. If I didn't know you had so much clearance I'd say that this single fact (through holes while blind do not) points squarely at a discrepancy between your hole depth (it's too shallow) and/or your tap depth (it's too deep).

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.

With 0.150in clearance I'd hope the problem isn't with the depths. Since you're using spiral flute taps I would imagine the hole isn't packing full of chips. Also, I'd imagine the flutes would let the cutting fluid out, so I doubt the holes being full of cutting fluid would be a problem (though, it might be worthwhile to try a couple holes without fluid). Beyond these points I'm at a loss.

Hmmm, here's an idea: maybe your through holes are actually larger in diameter because of the method you're using to drill them. Like, if you're peck drilling the through holes, perhaps each peck is widening the hole slightly because of runout or something.

It could be a coincidence. What kind of sample size are you working with? I gather that you've broken at least two taps. How many successfully tapped through holes have you done?

Another point that should be scrutinized is the failure point. I see that it's breaking during the withdrawal. Is it right at the start of the retract, or does it complete a couple turns and then snap?

In my video (which I've posed far too many times) of my Procunier tapping head doing 105 blind M5 holes, I drilled to a depth of ~10mm and tapped to a depth of 8.5mm I only had 1.5mm of clearance (~0.060in). Only 40% of what you have.
If you can post a video of your next attempt I'm sure it would be helpful in diagnosing the cause of this issue.

[Don Clement]

Why would spindle accurate speed/feed be a factor in breaking taps with the Procunier? Before using my Procunier 1E on the Tormach I used the Procunier to tap thousands of blind and through holes in my manual Rockwell mill feeding by hand. Rarely broke a tap, even in deep hole of 3/4" using the Procunier on my manual mill. So why say is necessary to calibrate the spindle so accurately? Also the Procunier has the same type of axial forgiveness as the tension-compression type head. BTW I tap blind holes with spiral flute taps (1/4-20 and M6) with the Procunier on the Tormach all the time in 6061-T6 without issues. I do use a #8 drill for both M6 and 1/4-20. I also use Relton A9 cutting fluid. I do not breaking taps with the Procunier in my Tormach unless the part is not rigidly held or some gross problem like leaving the feed override at 200%. Something my be wrong with YOUR Procunier. My Procunier has been very forgiving tapping in either my manual Rockwell mill or in the Tormach.

Don Clement

[Steve Seebold]

It could be a simple solution. WHAT ARE YOU USING FOR LUBRICANT? I tap 10-32 holes on my machine all the time, but I always use form taps. Drill your holes with a #16 drill and use a form tap. Not only are the form taps stronger, but a form tap will make a stronger thread.

[Don Clement]

It could be a simple solution. WHAT ARE YOU USING FOR LUBRICANT? I tap 10-32 holes on my machine all the time, but I always use form taps. Drill your holes with a #16 drill and use a form tap. Not only are the form taps stronger, but a form tap will make a stronger thread.

Steve,

I also tap #10-32 in aluminum with a form tap using a Tapmatic 50X. I use Relton A9 cutting fluid. I really don't like the tapmatic compared to the Procunier though having to futz with wrenches and those pesky rubberflex collets. However this thread is about using the Procunier in the Tormach.

Don C.

[Beezle]

So it's working in through holes but not blind holes? To me, that strongly suggest the problem is with something other than the tapping head. After-all, it doesn't know what kind of hole you're tapping. If I didn't know you had so much clearance I'd say that this single fact (through holes while blind do not) points squarely at a discrepancy between your hole depth (it's too shallow) and/or your tap depth (it's too deep).

With 0.150in clearance I'd hope the problem isn't with the depths. Since you're using spiral flute taps I would imagine the hole isn't packing full of chips. Also, I'd imagine the flutes would let the cutting fluid out, so I doubt the holes being full of cutting fluid would be a problem (though, it might be worthwhile to try a couple holes without fluid). Beyond these points I'm at a loss.

Hmmm, here's an idea: maybe your through holes are actually larger in diameter because of the method you're using to drill them. Like, if you're peck drilling the through holes, perhaps each peck is widening the hole slightly because of runout or something.

It could be a coincidence. What kind of sample size are you working with? I gather that you've broken at least two taps. How many successfully tapped through holes have you done?

Another point that should be scrutinized is the failure point. I see that it's breaking during the withdrawal. Is it right at the start of the retract, or does it complete a couple turns and then snap?

In my video (which I've posed far too many times) of my Procunier tapping head doing 105 blind M5 holes, I drilled to a depth of ~10mm and tapped to a depth of 8.5mm I only had 1.5mm of clearance (~0.060in). Only 40% of what you have.
If you can post a video of your next attempt I'm sure it would be helpful in diagnosing the cause of this issue.

Thanks for the thoughts. I appreciate the help.

I will make another attempt this week and make a video while doing so. Trying:

1. same drills size (no. 21, 0.159) and spiral flute tap, but shallower tapping depth. 0.25? Something like that.
2. just trying again after tweaking spindle calibration. Given I use the M871 macro, if the spindle speed was inaccurate it could have made poor calculations.
3. try just long hand code. Use the tach to know exact spindle speed, etc.
4. try a slightly larger hole - no. 19.

And so on.

[Beezle]

It could be a simple solution. WHAT ARE YOU USING FOR LUBRICANT? I tap 10-32 holes on my machine all the time, but I always use form taps. Drill your holes with a #16 drill and use a form tap. Not only are the form taps stronger, but a form tap will make a stronger thread.

Which form taps do you use? Source, etc? I will order some up. I have only hand taps, a spiral point and several spiral flute. The latter from McMaster and Tormach. The Tormach taps look interesting. Made in Korea.

I also ordered up some #19 drills so I could try a slightly larger hole.

I regularly drill holes that are them pre reamed and reamed for tight fitting with pins, so i would guess my drilling is pretty accurate. I buy drills in dozens and only use them when they are quite sharp.

Oh, and for lubricant I use Tap Magic for aluminum and lots of it.

[Beezle]

Why would spindle accurate speed/feed be a factor in breaking taps with the Procunier? Before using my Procunier 1E on the Tormach I used the Procunier to tap thousands of blind and through holes in my manual Rockwell mill feeding by hand. Rarely broke a tap, even in deep hole of 3/4" using the Procunier on my manual mill. So why say is necessary to calibrate the spindle so accurately? Also the Procunier has the same type of axial forgiveness as the tension-compression type head. BTW I tap blind holes with spiral flute taps (1/4-20 and M6) with the Procunier on the Tormach all the time in 6061-T6 without issues. I do use a #8 drill for both M6 and 1/4-20. I also use Relton A9 cutting fluid. I do not breaking taps with the Procunier in my Tormach unless the part is not rigidly held or some gross problem like leaving the feed override at 200%. Something my be wrong with YOUR Procunier. My Procunier has been very forgiving tapping in either my manual Rockwell mill or in the Tormach.

Don Clement

I don't really know. I figured because of the calculation for feeds. So they divide the spindle speed by the TPI of the tap. If the spindle speed is for example faster than the S word asks for, which is what I had before I fussed over the calibration, the retraction speed isn't fast enough.

I would imagine what I really have here is just a particular tap getting stuck and the application of torque to try to remove it is enough to break it. You know, the simplest explanation is usually the correct one.

[Beezle]

Was just working on a program for the part that got the broken tap and realized what my error was.

The surface of the hole was at -.127 and the hole was .75 deep from 0. So the hole was actually .623 deep.

And I sent the Procunier to .6 into that hole.

Sigh. At least it was me! I can fix that pretty easily.