[WATERJET71]

Ok I have everything that I been told but for some reason the tap is wiping off the threads after is finish the operation there is not threads looks like if I was using a bigger drill but I double check it and it is a 5/64 drill (.0781) here is the program can some one check it for me . I'm still learning so dot get mad at me please ha ha

G0 G90 G54 X.195 Y-.172 M3 S6000
M8
G43 H5 Z.5 T6
G83 G98 X.195 Y-.172 Z-.235 R.1 Q.0671 F5.
X1.395
Y-1.148 T5 M6 (.078 drill)

X.195
G80
M9
G0 G91 G28 Z0 M5
M1
N6 G0 G90 G80 G40
G91 G28 Z0 M05
T6 M6 (2-56 TAP)
G0 G90 G54 X.195 Y-.172 M3 S896
M8
G43 H6 Z.1 T4
G84 G98 X.195 Y-.172 Z-.188 R.1 F16.
X1.395
Y-1.148
X.195
G80
M9
G0 G91 G28 Z0 M5
T4 M6
G00 G90 X0
G53 Y0.
M30
%

[fizzissist]

As soon as I see G91 I stop reading code. I like to know absolutely where I am, and I think going back and forth is asking for trouble. I'm sure there's plenty of guys who'll disagree and are fine with it, but I don't like it.

[txcncman]

According to my drill-tap chart, 0.070" is the maximum drill size for #2-56 tap. The major maximum diameter for a #2-56 screw is 0.0854". If you are drilling to 0.078" You are leaving yourself about 0.0035" per side for threads.

[WATERJET71]

But .070 that's for cutting tap correct? I'm using roll tap.

[G0G90]

As soon as I see G91 I stop reading code. I like to know absolutely where I am, and I think going back and forth is asking for trouble. I'm sure there's plenty of guys who'll disagree and are fine with it, but I don't like it.

That's only used on the "HOME" routine. The entire program is actually in Absolute.

[fizzissist]

How are you holding the tap?

You know, at 896rpm, the F16. is correct.... but what is the actual rpm? You should probably lag the rpm ever so slightly to allow the tap to lead the spindle, not the other way around.

[G0G90]

Your calculations look correct for using a Roll tap however, your only in the 65% of thread.
If you want to get up to the 77% range, you'll need to be closer to .076".
Have you tried to measure the hole? Are you getting runout in the drill or is it cutting oversize? This would give you the same low thread %.

[Anders6612]

As soon as I see G91 I stop reading code. I like to know absolutely where I am, and I think going back and forth is asking for trouble. I'm sure there's plenty of guys who'll disagree and are fine with it, but I don't like it.

"G0 G91 G28 Z0" That is reference point in Z. You could not be more sure about where you are.

What chuck do you use? Maybe you need a chuck that
is floating, but if your machine can do rigid tapping, you need
a "M29" before the tapping cycle.

Like this:

M29
G84 G98 G95 X.195 Y-.172 Z-.188 R.1 F0.0178
.
.
.
.
G94 (tapping finish)

G95 is ipr, mutch better for tapping, because if you want to change rpm, the feed follows.

[txcncman]

But .070 that's for cutting tap correct? I'm using roll tap.

Your calculations look correct for using a Roll tap however, your only in the 65% of thread.
If you want to get up to the 77% range, you'll need to be closer to .076".
Have you tried to measure the hole? Are you getting runout in the drill or is it cutting oversize? This would give you the same low thread %.

Yes, that info was for a cutting tap. I looked back and never saw where you said you were using a roll form tap.

What is the minor diameter after tapping? Spec calls for 0.0667"/0.0737". That will be your biggest determining factor for a "good" thread in this case.

If the tap is actually pulling threads out of the hole, try putting a dwell, 1-2 seconds.

[Delw]

Ok I have everything that I been told but for some reason the tap is wiping off the threads after is finish the operation there is not threads looks like if I was using a bigger drill but I double check it and it is a 5/64 drill (.0781) here is the program can some one check it for me . I'm still learning so dot get mad at me please ha ha

G0 G90 G54 X.195 Y-.172 M3 S6000
M8
G43 H5 Z.5 T6
G83 G98 X.195 Y-.172 Z-.235 R.1 Q.0671 F5.
X1.395
Y-1.148 T5 M6 (.078 drill)

X.195
G80
M9
G0 G91 G28 Z0 M5
M1
N6 G0 G90 G80 G40
G91 G28 Z0 M05
T6 M6 (2-56 TAP)
G0 G90 G54 X.195 Y-.172 M3 S896
M8
G43 H6 Z.1 T4 that could be one problem change the z to z1.0 and you have a T4 in there whats up with that
G84 G98 X.195 Y-.172 Z-.188 R.1 F16.
X1.395
Y-1.148
X.195
G80
M9
G0 G91 G28 Z0 M5
T4 M6
G00 G90 X0
G53 Y0.
M30


are you using a cadcam program, not trying to ridicul but your code looks like crap its all over the place. you need to have some organization in it.

[Delw]

are you running this off your haas mini mill?
also are you using a center or spot drill before the drilled hole?

your tap program should look like this
YOUR R VALUE IS OFF ALSO MAKE THAT R1.0

YOU ALLOW FOR NO LEAD IN, IN THE MACHINE
dELW

[Delw]

T4 M6 ( SPOT DRILL) <<<<< must use center or spot drill
G0 G90 G54 X.195 Y-.172
T5 <<<<<< Position drill tool
S6000 M3
M8
G43 Z0.1 H4
G98 G82 Z-.052 R0.1 F15.0
X1.395
Y-1.148
X.195
G00Z1.0
M9
G91 G28 Z0 M5
M01

T5 M6 (.078 DRILL)
G0 G90 G54 X.195 Y-.172
T6 <<<<<<<< position tap tool
S6000 M3
M8
G43 Z0.1 H5
G98 G83 Z-.188 Q0.05 R0.1 F5.
X1.395
Y-1.148
X.195
G00Z1.0
M9
G91 G28 Z0 M5
M01
T6 M6 (2-56 TAP)
G0 G90 G54 X.195 Y-.172
T4 <<<< Position 1st tool
S896 M3
M8
G43 H6 Z1.0 <<<<<<< must have a lead in I allow 1" on fast feed rates and a min of .5 on slow feed rates
G98 G84 Z-.188 R1.0 F16. <<<<<<<< R should be same as z in above
X1.395
Y-1.148
X.195
G00Z1.0
M9
G91 G28 Z0 M5
G91 G28 Y0.0 (TAKES THE "Y" AXIS HOME)
M30

on a haas you dont need a g80 at the end of the cycles UNLESS your using the same tool for milling, IE using a spot drill for chamfering the edges of a part.
with an unbrella type tool changer DONT position a tool as you dont need to, with a side mount you can and helps on speed alot like the above code.
also things are easier done by using 1000 rpms in tapping cycle on alum.
to get the feed rate for the tap use 1/thread pitch*rpm or 1/56*1000