[GTOGuy]

I am using the Tormach Tension/Compression tapping head on a Series 3 PCNC and noticed when tapping my first holes in 1/4" thick steel with a 5/16-18 tap that when the spindle retracts , it is extending the tapping head further in tension that I expected (looks like maybe 3/8" of an inch. The RPM is 500 (and I calibrated the mill at 500) with a G84 tapping cycle (27.8 ipm calculated) and a P(dwell) of 0. Maybe I need to add a dwell? Can someone explain what the dwell actually does? for example, does it dwell after the spindle reverses (which would produce less tension extension on the tapping head I presume).

[vmax549]

Yes the dwell is to let the spindle start to spin up before Z starts the upfeed. On teh downfeed and at teh end of stroke the X stops and the spindle winds down to a stop this extends teh shaft on teh tap head. So a dwell is needed on the upfeed to allow the spindle to start before Z moves and that retracts the tap head shaft back to neutral. IF the shaft is extended to far on the upfeed at teh top of teh stroke the spring pressure can rip out the first tthread or 2.

(;-) TP

[GTOGuy]

Yes the dwell is to let the spindle start to spin up before Z starts the upfeed. On teh downfeed and at teh end of stroke the X stops and the spindle winds down to a stop this extends teh shaft on teh tap head. So a dwell is needed on the upfeed to allow the spindle to start before Z moves and that retracts the tap head shaft back to neutral. IF the shaft is extended to far on the upfeed at teh top of teh stroke the spring pressure can rip out the first tthread or 2.

(;-) TP

Thank you. That was exactly the explanation I was looking for to better understand the dwell. I noticed that the default in Fusion 360 is a zero value for the dwell. I also read that PathPilot will use a default in the conversational programming if a dwell value is not entered which I presume is the same value it will use if there is no P value in the G84 line from F360. Do you know what that value is or can you recommend a good value to use for a series 3 PCNC? I prefer to explicitly enter a value rather than depending on a blind default value

[TurboStep]

...Do you know what that value is or can you recommend a good value to use for a series 3 PCNC?

Tormach specify their value to be "half of a second per 1000 RPM". This would give 0.25s for your 500 RPM.
https://tormach.com/tapping-cycle-g84
I don't use a T/C tapping but from memory this value would appear to be about normal for a series 2/3. It's certainly a good starting point.
Step

[Tigster]

Sounds like you got the answer you were looking for...awesome. If I could ask you a question, on those Tormach tapping heads, how much movement in out do they have. I love my tapping head for the manual mill, so I am very interested for the CNC. ON m manual head, I have about 5/8" of movement and tend to preload the spring (in the pulling motion) then hit reverse. That first time using the Tormach tapping head would be terrifying and I know there would be some old habits to ditch and new ones to pick up.

[popspipes]

Maybe tap a block of wood first?? That would be easier on the tap if things arent quite right.

The dwell is the time in Sprutcam that it stays at the bottom before retracting. I use about .5 second, the purpose is to let the spindle come to a stop before the Z or spindle starts up in reverse.
most of my tapping is done at 320 rpm and .5 second is good for that, as the rpm increases you will need more dwell time. I always tap slowly, just an old habit I guess...

My tap cycles when set at 10 ipm, the down stroke will be at 9 ipm and the up stroke will be at 11 ipm.

I think the reason for that is to make sure the tap clears the hole before moving to the next one possibly..

movement on mine is 1/4" compressed and 1/2" extended approximately.

I have the one that goes up to 1/2" and its hard on the first thread of the small tapped holes in aluminum, my opinion is the springs are a bit too stiff for the small holes.

[GTOGuy]

Tormach advertises 3/4" in. of travel for the tapping head with the modular tap holders.

I am trying to figure out now what the tension adjustment on the holder actually does. It seems that it would control the amount of torque that the holder will resist from the tap before slipping but in playing with it so far, the tap will not rotate easily even when I loosen the adjustment nut. I probably don't fully understand its function. I am also trying to figure what actually locks the tap into the older. Guess I'll take it apart completely.

[popspipes]

Tormach advertises 3/4" in. of travel for the tapping head with the modular tap holders.

I am trying to figure out now what the tension adjustment on the holder actually does. It seems that it would control the amount of torque that the holder will resist from the tap before slipping but in playing with it so far, the tap will not rotate easily even when I loosen the adjustment nut. I probably don't fully understand its function. I am also trying to figure what actually locks the tap into the older. Guess I'll take it apart completely.

When you figure out how to get it apart, I for one would like to know!! I had a 6mm tap that wouldnt hold in the holder, finally would up grinding new flats on the tap just a bit shallower to get it to work, I couldnt figure out how to get it apart??
The clutch in the holder I tried to adjust had to be set almost at minimum travel to get it to release with a 10/32 tap.

[GTOGuy]

I see what you mean, I don't see an obvious joint to disassemble it.

[vmax549]

I learned a LONG time ago if it is not broke don't try to fix it.

(;-) TP

[popspipes]

I learned a LONG time ago if it is not broke don't try to fix it.

(;-) TP

I agree, shallower flats on the 6 mm tap fixed my problem, I suppose there is a holder made for that tap but I didnt have one.

[GTOGuy]

I learned a LONG time ago if it is not broke don't try to fix it.

(;-) TP

Generally speaking ....good advice. But how else will I get my thrills if not by watching something fly apart before I could see how it was put together in the 1st place!

[vmax549]

Well I guess it depends on if you like working WITH the machine or working ON the machine.

(;-) TP

[mountaindew]

Generally speaking ....good advice. But how else will I get my thrills if not by watching something fly apart before I could see how it was put together in the 1st place!

When you no longer crash your mill enough to get good thrills. Add a cnc lathe to your shop, For such a simple machine tool they are surprisingly easy to crash.

Thread topic.
I use long hand code in cam software to drive tc tap operations between 500-1000 rpm and adjust feed to match (1/pitch x rpms) imperial or (pitch x rpms/25.4) metric. or did cam software does some of this now.
I also use a 0.3 dwell at bottom. Note :I have never used these numbers with a tap cycle only long hand code!
and I dont tap much over 0.25" . Anything larger I like to use thread mills. They are slow but you get drama free results

[vmax549]

The real trick to tapping large holes or harder material with low HP spindles is to use a peck tapping cycle which PP does not have yet. On other controllers that do have peck tapping it is the cats meow for tapping larger holes or harder materials. Drama free. You don't even have to stand there with your finger on the estop button. You can even go make a cup of coffee while the machine does all the work. I guess one could remap the G84 to include peck tapping.

(;-) TP

[mountaindew]

The real trick to tapping large holes or harder material with low HP spindles is to use a peck tapping cycle which PP does not have yet. On other controllers that do have peck tapping it is the cats meow for tapping larger holes or harder materials. Drama free. You don't even have to stand there with your finger on the estop button. You can even go make a cup of coffee while the machine does all the work. I guess one could remap the G84 to include peck tapping.

(;-) TP

The new MX mills have encoder and rigid tap ability.
My cam software has no less then a dozen setting and cycles for tapping including peck.
sadly my old s3 mill has no spindle encoder so no go on rigid tap cycles. But New 8l lathe has rigid tapping and I will be testing this soon.
Waiting on a center bore finder tool to accurately locate the mt2 radial tool holder to spindle center. Slow deliveries these days .

Quick question
I only have mt taper drill chucks to hold taps. Will a keyless chuck hold a tap?

Cant find a mt2 to er20 collet holder that is not on backorder.

[kstrauss]

https://www.amazon.com/Collet-Holder.../dp/B08CRM1PK8 promises delivery on Sunday.

I'm curious: what is a "center bore finder"? Link?

[jwatte]

[quote]Will a keyless chuck hold a tap?
[/quote[

Will it stay in there? Probably.
Will it be sufficiently centered? No.
Will it be sufficiently rigid along the Z axis so it doesn't get pushed in or pulled out a bit? No.

I really would not recommend a drlll chuck for anything other than jobber drills. I've taken to using stub length drills and ER20 tool holders when I can. At this point, I think drill chucks are mainly for wood, but that's probably taking it a bit too far on the dogmatic side :-D

[mountaindew]

https://www.amazon.com/Collet-Holder.../dp/B08CRM1PK8 promises delivery on Sunday.

I'm curious: what is a "center bore finder"? Link?

Accusize Industrial Tools 0-0.15 inch by .0005'' Graduations, Co-Ax Indicator, Coaxial Centering, Yellow Dialing Face, Jd21-0003

links didnt work
Sorry I made the name up!
I used one to find centers of motorcycle cylinder bores when I was a kid.

[mountaindew]

[QUOTE=jwatte;2440270]

Will a keyless chuck hold a tap?
[/quote[

Will it stay in there? Probably.
Will it be sufficiently centered? No.
Will it be sufficiently rigid along the Z axis so it doesn't get pushed in or pulled out a bit? No.

I really would not recommend a drlll chuck for anything other than jobber drills. I've taken to using stub length drills and ER20 tool holders when I can. At this point, I think drill chucks are mainly for wood, but that's probably taking it a bit too far on the dogmatic side :-D

I would agree on every point! I used to centers to align the tool holder to spindle as is.
Good for drilling a hole not much more. and I didn't think it would be accurate to run a tap into. So I ordered a coaxial indicator

Reason for asking is I see people do it on knee bridge port type mills all the time.