[SomeWhatLost]

ok, so I got the tension/compression tapping head kit thingy when I got my mill, figured it was about time to start playing with them a bit...
so I figured I would try to hand code it... mostly from a learning point of view, sometimes doing things by hand helps the learning process I think... of course I could be wrong on that? who knows... still seemed like a fun thing to do...
ok, so this is what I have so far (fwiw it is a #8-32 tap, and a 0.136" hole)

( TAP )
( T0 : tap )
M998
T0 M6
G43 H0
S250 M3
G0 X-0.0007 Y0.0006
G98
G84 X-0.0007 Y0.0006 Z-0.27 R0.1 F80
{more to come later}
M5
M30

just wanted some professional feedback, does what I have so far have any chance at all of working?

[GJeff]

Can we also get some feedback from people using the compression tapping doohickeys concerning which one they recommend? Tormach has a lot of them available on their site, some auto reversing, some just compression and even among the compression ones the price varies greatly.

[kevinro]

ok, so I got the tension/compression tapping head kit thingy when I got my mill, figured it was about time to start playing with them a bit...
so I figured I would try to hand code it... mostly from a learning point of view, sometimes doing things by hand helps the learning process I think... of course I could be wrong on that? who knows... still seemed like a fun thing to do...
ok, so this is what I have so far (fwiw it is a #8-32 tap, and a 0.136" hole)

( TAP )
( T0 : tap )
M998
T0 M6
G43 H0
S250 M3
G0 X-0.0007 Y0.0006
G98
G84 X-0.0007 Y0.0006 Z-0.27 R0.1 F80
{more to come later}
M5
M30

just wanted some professional feedback, does what I have so far have any chance at all of working?

Well, honestly, no! First thing to do is to think about how the tap is going to go through the hole. As the spindle turns, you need to advance the bit at 'just the right' speed. The head you are using helps out a lot here, but you do have to do some math.

Specifically, the feed rate needs to be mathmatically related to the spindle speed. You have set your speed to 250 RPM. Nothing wrong with that. That means there will be 250 turns in a minute. The tap has 32 threads per inch. Therefore, 32 revolutions of the spindle should happen at the same time as 1 inch of travel.

When I set one of these up, I usually try to pick a feed that gives me a nice round number. So I would go with 320 RPM on the spindle. To go with that, I would be looking to travel 10 inches per minute ( 320 RPM / 32 TPI = in IPM feed). You program has the feed rate of 80 ipm (unless you are doing an 8-32 using metric numbers?)

Some people, Tormach included, suggest introducing a small error into the math. Many of the Tormach instructions say that you should do 10%. Here is a program with for tapping a 1/4-20

(.25x20 Tap)
N190 S300 M3
N200 G0 X1.25 Y-0.875 Z0.2
N220 M8
N230 G98
N240 S300 M3    (clockwise)
N250 G1 Z-0.6 F13.5 (feed 15ipm * .90)
N260 M4 (reverse spindle)
N270 G4 P0.3 (pause for 300ms)
N280 G1 Z0.2 F16.5 (retract feed = 15ipm * 1.10)

Does that help?

[Wog]

You might want to pick up a photo tachometer before braking too many taps. I'm not sure how accurate the Series III's spindle speed is, but my older Tormachs were off.

You can get them from Tormach
http://www.tormach.com/store/index.p...show&ref=30527
or most any tool supply catalog. I think even Horrible Freight has them.

Especially important at the lower RPM's.

The nice thing is you just need to apply a little piece of reflective tape on all your equipment's spindles. I have one reader for 5 mills and 4 lathes.

[SomeWhatLost]

first I would just like to say thanks for all the feedback...
and 2nd I would like to say that the F80 was a typo/the effect of a DpMD (Decimal point of Mass Destruction) I actually meant F7.8125, not sure why I rounded up to 80 really...

I really like the idea of spindle = 320, that makes the math so much nicer...

also, I was going to ask if I should just toss the G84/canned cycle and do each step separately, as I have seen lots of recommendations for the -(some)% slow going in, and +(some)% faster coming out and I could not figure out how to do that with G84... but I am not going to ask that question anymore, because it was preemptively answered by kevinro already...:cheers:

so thanks, this does help a lot.

edit: just one more question... how fast can you go? can you go with like S3200 F100? is the Tormach rigid enough for that? do the Tension/Compression doohickies hold up?/react fast enough?

[shred]

It might be just my machine, but I did find the Tormach spindle reverse to be somewhat slower than advertised, so do some test-taps before relying on quick stopping and reversing.

[SomeWhatLost]

no issues with reversing or anything like that, threads cut just fine...
the one issue I did run across is that apparently you really should wait for the tap to completely clear the hole before moving on to the next hole... who knew?

[BAMCNC.COM]

no issues with reversing or anything like that, threads cut just fine...
the one issue I did run across is that apparently you really should wait for the tap to completely clear the hole before moving on to the next hole... who knew?

Fun isn't it.

[MichaelHenry]

FWIW, I've used both the basic and deluxe T-C heads from Tormach and both worked well for me in taps ranging from 4-40 to 1/2-13, aluminum only so far. I tend to use the deluxe one in practice because of the ease in changing taps.

I've used a Procunier 1E in my manual mill and that also worked well. The T-C head seems easier to use in the Tormach though, especially with a PDB so I've only used teh T-C heads on the Tormach.

Mike

[SomeWhatLost]

Fun isn't it.

fun,
but somewhat expensive...

still fun though... can wait for my replacement taps to come in Thursday... ordered 4... hopefully that will be enough to do 12 holes

[BAMCNC.COM]

Look for Tap LOTS on eBay, there are good deals at times, then it won't feel so bad breaking them.

[takewhatyoulike]

FWIW, I've used both the basic and deluxe T-C heads from Tormach and both worked well for me in taps ranging from 4-40 to 1/2-13, aluminum only so far. I tend to use the deluxe one in practice because of the ease in changing taps.

I've used a Procunier 1E in my manual mill and that also worked well. The T-C head seems easier to use in the Tormach though, especially with a PDB so I've only used teh T-C heads on the Tormach.

Mike

I have had very good luck for many years in using a TTS modified Procunier 1E reversing tap head on my Tormach using a Balax forming tap in tapping tens of thousands of 4-40 blind holes in aluminum. Rarely ever break a tap unless there was some untested change to the programming. Also changing taps is quick and easy with the Procunier Pro-Quik quick change system http://www.rockford-ettco.com/Portal...ro-QuikTap.pdf . The Procunier also works extremely well extremely well with my PDB. For holes greater than 1/4" I use thread milling.
Here is a video of how easy it is to change the TTS Procunier with the PDB. http://s72.photobucket.com/user/milt..._3879.mp4.html

A video of how easy it is to change a tap using the Pro-Quik system:
http://s72.photobucket.com/user/milt...hange.mp4.html

Also a few pictures of the TTS Procunier:






Don Clement

[takewhatyoulike]

x

[takewhatyoulike]

x

[takewhatyoulike]

x

[SomeWhatLost]

just a quick update...successfully tapped all 12 holes...
and successfully broke 2 taps...
overall, not too bad...
now some of you may think "successfully broke 2 taps" may be the wrong way to phrase the breaking of two taps, but hey, they are (were?) my taps, and I choose to follow a "Don't worry, Be happy" general philosophy... so I chose a happy way to phrase that...
also, that is two taps total, just the one from earlier in this thread (ie taps don't like rapiding off to the next hole, while still in the first), and the second one broke because I forgot to use some tap magic, and the 6061 got all gooey or something and jammed up the tap on the 4th hole...
but still, 3rd time was a charm...