What's new
What's new

Rigid Tapping - Breaking Taps on Tormach

nyjiki

Plastic
Joined
Jan 20, 2020
Hi Guys,

New machine owner, need some help. I keep breaking taps on my Tormach. It has rigid tapping and i'm using an ER20 tap collet, standard ER collet.

M2.5 X 0.45 Tap size.
6061 Aluminum
Fusion 360
Tormach

Do I need a dedicated tool? I thought I could just use a standard ER Collet holder if I had rigid tapping.
 
Last edited:
Post your code and maybe someone can help you. What taps are you using? What size is your hole before tapping? Bottom hole or thru hole. We need more details.
 
Thanks VTM,

Through hole tap, my drill size is a #45 drill / 0.820" / using a YMW spiral bottoming tap. I can't even hit bottom of the part before the tap breaks. I'm using a ER tap collet with just an ER holder. My machine has rigid tapping.

Here's my code:

G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
G20 (Inch)
G30

N10(M2.5x.45 tap)
T25 G43 H25 M6
S250 M3 M8
G54
G0 X1.8 Y0.6705
G0 Z0.38
G0 Z0.28
S250
G98 G84 X1.8 Y0.6705 Z-0.65 R0.28 F4.4
X1.998 Y0.4295
X2.802
X3. Y0.6705
X3.198 Y0.4295
X4.002
X4.2 Y0.6705
X4.398 Y0.4295
X5.202
X5.4 Y0.6705
X5.598 Y0.4295
G80
G0 Z0.38
M5 M9
 
Thanks VTM,

Through hole tap, my drill size is a #45 drill / 0.820" / using a YMW spiral bottoming tap. I can't even hit bottom of the part before the tap breaks. I'm using a ER tap collet with just an ER holder. My machine has rigid tapping.

Here's my code:

G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
G20 (Inch)
G30

N10(M2.5x.45 tap)
T25 G43 H25 M6
S250 M3 M8
G54
G0 X1.8 Y0.6705
G0 Z0.38
G0 Z0.28
S250
G98 G84 X1.8 Y0.6705 Z-0.65 R0.28 F4.4
X1.998 Y0.4295
X2.802
X3. Y0.6705
X3.198 Y0.4295
X4.002
X4.2 Y0.6705
X4.398 Y0.4295
X5.202
X5.4 Y0.6705
X5.598 Y0.4295
G80
G0 Z0.38
M5 M9


Your original post said 4-40 tap but your program says 2.5 X .45, which is it? But, to your point, if it is 4-40, you are using a way undersize drill if you are using a .082" drill. My tap chart calls for .089 (#43) drill. 4-40's are hard enough, don't make it any harder.
 
In addition to using the wrong drill, your feed is wrong. If you are going to use 250RPM, then your feed should be F6.25. 250RPM X .025 pitch=6.25 feedrate.

Is the program you posted the actual program you are using? Because it is programmed for a 2.5MM X .45.

Paul
 
Haven't looked at your code but why are you using a bottoming tap on a through hole? Spiral point gun tap will reduce cutting forces. Also might want to consider form tapping it.

Teryk

Sent from my XT1710-02 using Tapatalk
 
I was thinking roll forming it as well. The bottoming tap was what we had, didn't think about the cutting forces. Thanks for the input
 
I don't know on your Tormach, but most of the time when you are rigid tapping your federate is the pitch, not the pitch times rpm.
 
Are you using Path Pilot? If you are and it still follows Linuxcnc then G33.1 is for rigid tapping.

G33.1K(pitch)Z(depth)

Ed.
 
On my VMC's I always use IPM. On the lathe, it's IPR.

Either one is fine, you just better know which one you are using...

@OP- get your speeds and feeds better- for 250rpm you should feed at 4.43 rather than 4.4. You can round away the third decimal place, but not the second. 250 is way too slow anyway,

I'd run that tap no less than 1500 rpm, which would work out to 26.574 IPM feed.

It's a small tap, and spiral flute taps are more fragile than SP/Plugs. If you machine has peck tapping, take it in 2 or 3 pecks.
 
I'd be shocked if your tap even had .65" of flutes. The deepest M2.5 tap on McMaster only goes 1/2" and Balax doesn't have anything deeper in that size either. If you run out of flute, you snap immediately, even if everything else is perfect.
 
Used a reduced neck tap, I can clear the depth but I think I took too much depth for an ER Collet holder. Thanks
 
I can't peck, i've been looking for someone using a "Q" value in their G84 for their path pilot and I can't find it.
 
Yes! Only issue is that I can't find a "Q" value for a standard G84 code that would help me take this depth. I think i'm breaking taps because i'm taking a single pass the tap
 
Used a reduced neck tap, I can clear the depth but I think I took too much depth for an ER Collet holder. Thanks


Which is great, but a spiral flute tap pulls the chips up behind the cut, so once you run out of flutes, they pack up and snap.

Or keep faffing about looking at your collets. Your choice.
 








 
Back
Top