Brother tapping help

cmiddl01 · Jan 25, 2018

I have 2 brothers speedio RX650x1series High torque BT30 big plus built in 2017
we are roll form tapping extruded 1018 steel. I was trying to use Brothers G77 tapping cycle which is synchronized tapping. this is the tapping call out that I tried.

T2(TAP)M6
G0G90X-11.25Y-7.29S600M3
G43H2Z1.8386
M494
G77G98X-11.25Y-7.29Z-.1197R1.4386J16.921S600L1200
X-8.05
and so on.

this basically sends the tap in at 600rpm but doubles the exit.

When I run this without any Parts in the machine it runs just fine.

as soon as i introduce a part it is fine on the entry but on the return I get a z+ overload alarm. any Idea's of what could be going on. I get the same alarm if I change the L to 600. I am currently using a G84 tap cycle and it works fine. I would love to double or triple the exit to shave seconds of the run time.

thanks in Advance

Finegrain · Jan 25, 2018

I'm assuming this is NOT an M6 tap as the comment implies, otherwise J16.921 is going to be a big problem

. So it's probably M10, right?

Maybe the machine is having a hard time reversing to 1200 with an M10 tap stuck in steel?

Here's a rigid tap cycle that runs on my Speedio S700X1, FWIW:
(M3X0.5 TAPRH FB )
(TOOL - 12 D- 12 H- 12)
( DIA- .11811)
G0G90G17G40G64G69G80
G55G100T12L4X.9429Y-.4683
N12G43H12Z.375M8
G98G77Z-.2949R.2957J50.8S2000
X.3976Y-.6947
etc.

Regards.

Mike

BROTHERFRANK · Jan 25, 2018

First off, use I instead of J for the G77 pitch. J is for TPI. I is metric pitch. So M6 x 1 thread is I1.0, M10 x 1.5 is I1.5. That High Torque should handle that with ease. Make sure you have good lubricity in your coolant and make sure your tap cannot slip in the holder! Yes use the L to increase exit speed on G77.

Finegrain · Jan 25, 2018

Hole size is good? Maybe the hole is a bit small and the tap is getting wedged in the hole? I would expect it to break before stalling the spindle.

Regards.

Mike

AARONT · Jan 25, 2018

Finegrain said:
I'm assuming this is NOT an M6 tap as the comment implies...

M6 would be for the tool change...

eaglemike · Jan 25, 2018

As Frank notes, I should be used for metric pitch I6.0 would be for M6 pitch thread. J would be used instead of the I, for inch threads, and would be the number of threads per inch.Ex: J20 would be 20 threads per inch. It's really that easy. The G77 synchronizes the spindle better the spindle better than G84, according to what I've heard and observed. You might try to update your code using the correct I and J parameters. Also make sure your hole size is correct. When you go to return at a faster RPM, this will be more important, also proper tap geometry and coating, and coolant/lubricant. Good luck!

Nerdlinger · Jan 25, 2018

What kind of holder are you using? I was breaking taps on my Brother S2Dn and the sales guy said I shouldn’t use the quick change tap collet but rather an ER tap collet with the square receiver because they reverse so fast the little wiggle you get with the quick change ones allowed the tap to shift and then kind of get out of sync as the spindle goes up and the tap continues to go down for a billionth if a second. Maybe if I was using a larger tap like M10 it would’ve stalled instead of break.

Pete Deal · Jan 26, 2018

I am using J for both metric and inch pitches since my CAM system is single minded- it either works in inch (which is what I do) or metric across the board so for 0.5mm pitch it spits out J50.8 and seems to work fine.

BROTHERFRANK · Jan 26, 2018

In the OP's sample code, what thread is J16.921? That doesn't match anything metric or UN. They bought those excellent R650 machines to help them machine their parts more efficiently. They need to use them properly. Using J for everything doesn't always work. You will end up having to round off sometimes to get close. M10 x 1.5 is one example. Those machines should not be run like that.

brian.pallas · Jan 26, 2018

If J is TPI (1/16.921)*25.4=1.501

eaglemike · Jan 26, 2018

brian.pallas said:
If J is TPI (1/16.921)*25.4=1.501

Agree with that, but when one is reversing out at 1200 with a form tap in steel, it should be perfect. Along with the tool holder, tap coating, coolant, etc.

These machines are dead nuts accurate in tapping. I know a post can be set up in OneCNC and in BobCad to get the correct I and J.

Before I had my post working (which I need to set up again due to new version) I went back in and hand jobbed the code.

BROTHERFRANK · Jan 26, 2018

brian.pallas said:
If J is TPI (1/16.921)*25.4=1.501

More like 1.5011. Like I said you have to round off. Running a new R650 like that, or any machine that you are trying to maximize quality and production efficiency on, does not make any sense to me.

cmiddl01 · Jan 30, 2018

this is a m12x1.5 roll form tap. exact tap is. OSG EXO 1615012151 I figured pitch and threads per inch
1.5/25.4=.0591 then took 1/.0591=16.9205 so threads per inch is 16.9205. I program in inch so that is the reason for conversion.

Pete Deal · Jan 30, 2018

cmiddl01 said:
this is a m12x1.5 roll form tap. exact tap is. OSG EXO 1615012151 I figured pitch and threads per inch
1.5/25.4=.0591 then took 1/.0591=16.9205 so threads per inch is 16.9205. I program in inch so that is the reason for conversion.

I get that 25.4/1.5=16.93333. Maybe it is the extra rounding by doing it in two steps as you did?

BROTHERFRANK · Jan 30, 2018

cmiddl01 said:
this is a m12x1.5 roll form tap. exact tap is. OSG EXO 1615012151 I figured pitch and threads per inch
1.5/25.4=.0591 then took 1/.0591=16.9205 so threads per inch is 16.9205. I program in inch so that is the reason for conversion.

Your program can be all inch. If your tapping metric use the I instead of J. Use I1.5 for M12 x 1.5 for best results. The rest of the program can be in inch including Z depth, R amount, etc.... Best regards

cmiddl01 · Feb 3, 2018

BROTHERFRANK said:
Your program can be all inch. If your tapping metric use the I instead of J. Use I1.5 for M12 x 1.5 for best results. The rest of the program can be in inch including Z depth, R amount, etc.... Best regards

This worked like a charm! thank you so much. Being a self taught machinist some times can be rough. thanks for not beating me up to much!

BROTHERFRANK · Feb 3, 2018

cmiddl01 said:
This worked like a charm! thank you so much. Being a self taught machinist some times can be rough. thanks for not beating me up to much!

Glad it's working out for you and thanks for the update. Learning from experience is great, especially other people's experiences along with your own. You don't have enough time to experience everything yourself. Keep bringing your questions when you're stuck or curious. Don't forget Yamazen or Turnkey Solutions, depending on where in Michigan you are, has tech support for the equipment they install. Those brother R650 machines are really nice tools.

Houndogforever · Feb 14, 2018

BROTHERFRANK said:
First off, use I instead of J for the G77 pitch. J is for TPI. I is metric pitch. So M6 x 1 thread is I1.0, M10 x 1.5 is I1.5. That High Torque should handle that with ease. Make sure you have good lubricity in your coolant and make sure your tap cannot slip in the holder! Yes use the L to increase exit speed on G77.

The L? What does the L word do? This machine is still so much smarter than I am. Hell, I'm just now modiying my tap cycle to use G77.

Nerdlinger · Feb 14, 2018

L is the retract RPM... so you could use, say, S300L600 to save a half a second. If you leave it out I think it just retracts at the same RPM you went in at.

Houndogforever · Feb 14, 2018

oh, Damn books, I was thinking it was a percentage number or something complicated. That is simple. Yay, I'm off to tap some nylon.

Brother tapping help

Plastic

Diamond

Stainless

Diamond

Stainless

Stainless

Stainless

Titanium

Stainless

Hot Rolled

Stainless

Stainless

Plastic

Titanium

Stainless

Plastic

Stainless

Hot Rolled

Stainless

Hot Rolled

Similar threads