Tension Compression tapping help

I have a 770 Series 3 and a TC tapping head. I'm trying to tap 6-32 in 1/4" thick 6061 using high-speed mode at 800 RPM with a good HSS spiral flute tap. Yes, I calibrated speed. I'm using conversational in Path Pilot and set the dwell to 0.4s. All seems to go well and the program runs fine, but many threads are fouled when I try to run a screw through. It appears the entry threads get mangled when the TC head pops up slightly coming out of the hole. At least that's the only thing I can guess. I've messed with the dwell to try have no compression or tension when the tap leaves the hole, but I've noticed that the tension is not same on every hole, so I can't find one dwell that never "pops" on exit. Maybe my speed is varying too much because I'm trying to get away without changing the belt to low speed. Obviously, the point of the TC head is that it CAN compress or stretch a bit, so it seems this shouldn't wreck the threads. The other possibility I wonder about is maybe the TC spring is too stiff. It's seems stronger than necessary, but I don't know what normal is. If it were weaker, maybe it wouldn't rip the threads (if that is in fact what's happening). I have to chase all the threads with a hand drill after the job, which kind of negates the point of TC head. I could just as well tap them with the drill. I'm hoping someone has wisdom to impart. Thanks

Is the tap completely clearing the hole on retraction?

can you post your code so that people can look at it and advise you

I have the large TC tapping head and the springs are a bit too strong for aluminum and small taps in my opinion.
I have the same thread fouling problem however they arent fouled enough that I cant run a screw in the hole, its just a bit tight (6-32).
I would like to try some weaker springs to see if that helps but havent yet, I think they are fine for the larger taps and for tapping in steel, it does beat doing it by hand though.

Quote:

---

Originally Posted by rcs60

can you post your code so that people can look at it and advise you

---

Here it is. Generated by PP Conversational

(Mill - Pattern Tap G-code generated: Wed Jun 24 14:46:39 2020)
(PathPilot Version: 1.9.1)
(Description = alum clamp 12 hole)


(Units = G20 inches)
(Work Offset = G54)
(Tool Number = 51)
(Tool Description = 6-32 tap in TC head)
(Tool Diameter = 0.0000 inches)
(Spindle RPM = 800)


(Z Clear = 0.3000)
(Z End Location = -0.3750)
(Z Feed = 18.8 inches/minute)
(Hole Bottom Dwell = 0.40)
(Pitch = 0.0312)
(Threads per inch = 32.0000)




(----- Start of G-code -----)
(<cv1>)


G17 G90 (XY Plane, Absolute Distance Mode)
G64 P 0.0050 Q 0.0000 (Path Blending)
G20 (units in inches)
G54 (Set Work Offset)


G30 (Go to preset G30 location)
T51 M6 G43 H51


S 800 (RPM)
M8 (Coolant ON)


M3 (Spindle ON, Forward)
F 18.80 (Z Feed, inches/minute)


G0 X 0.5000 Y -0.6250 (Hole 1 of 12)
G0 Z 0.3000 (Z Clear)
G84 Z -0.3750 R 0.3000 P 0.40 (Canned Dwell Tap)
X 0.5000 Y -1.0000 (Hole 2)
X 0.5000 Y -1.3750 (Hole 3)
X 1.6000 Y -1.7500 (Hole 4)
X 2.2500 Y -1.7500 (Hole 5)
X 2.9000 Y -1.7500 (Hole 6)
X 4.0000 Y -1.3750 (Hole 7)
X 4.0000 Y -1.0000 (Hole 8)
X 4.0000 Y -0.6250 (Hole 9)
X 2.9000 Y -0.2500 (Hole 10)
X 2.2500 Y -0.2500 (Hole 11)
X 1.6000 Y -0.2500 (Hole 12)


G80 G0 Z 0.3000


M9 (Coolant OFF)
M5 (Spindle OFF)


G30 Z 0.3 (Go in Z only to preset G30 location)


G30 (Go to preset G30 location)


M30 (end program)

- - - Updated - - -

Quote:

---

Originally Posted by Tbkahuna

Is the tap completely clearing the hole on retraction?

---

Yes

I'm concerned about the slower feedrate of F18.8
my calcs.... 1/32 x 800 = F25.0
your slower feed would make the holder pull out as the tap is cutting
, the spring would try to pull the tap back ( possibly distorting the true pitch being cut )
a T&C holder allows any movement at the bottom of tapping for spindle stopping & reversal of the tap
the programmed feedrate should be between 95-105% of the actual pitch.

If your machine feed stops instantly, but the spindle is slow to stop & reverse.... then you need to realise that time to stop actually pulls the head a little more & you need to allow for this to not "bottom out" the tapping head.

Superman appears to have found at least one issue, unless you changed the feed rate manually. I see you're still using PPv1.9.1 but when I plug your values into PPv2.5.1 it calculates F25. I've found no evidence in the release notes that there was an issue back then, and I don't use TC heads myself, but if I were you I'd upgrade to at least PPv1.9.13 and preferably make the step up to the latest version.
Step

I've been using a TC head on my machine to do tapping and the reason I see to include a delay at the hole bottom is to allow the VFD to stop and change direction without tripping - and avoid the spindle withdrawing before the tap has started to back out.

My machine has a fairly large motor, so in low gear (needed for tapping), it is spinning at a decent rate and takes some time to slow down, even with the proper braking resistor. In practice it limits the max tapping speed I can use and the min delay I can set. The problem is worse for small taps where there is very little load on the spindle, whereas the larger taps help to slow down the spindle due to their larger load. At double the speed, there is four times the energy in the motor to dump, so that's the condition that limits the VFD decel parameter on my system (Yaskawa V1000).

...using High Gear range for tapping is better sometimes for quicker reversing and easier on VFD's.
My 2 cents,
DJ