[Mori]

HI ALL,
I HAVE OLD MORI MH-40 CONTROL MF-M5. I BELIEVE IT DOESN'T HAVE RIDGID TAPING SO I BOUGHT A TAPPING ADAPTER AND IT STILL DOESN'T WORK. WHAT IS THE RECOMMENDATION? WHAT IS THE TAPING CYCLE?

THANKS ALOT!
MORI

[dcoupar]

Most people use G84 for tapping. What kind of tapping adapter? What do you mean when you say "It still doesn't work"? What happens when you try to tap a hole? What does your program look like?

This should be roughly what you need to program.

N10 T10 M6 (1/2-13 TAP)
G54 X0. Y0. S260 M03
G43 Z0.2 H10 M08
G84 Z-1.0 R0.2 F20.
X1.0
X2.0
G80 M09
G91 G28 Z0
G91 G28 Y0
M30

[Superman]

Also remember that milling machines tend to be programmed in feed / min.
**change the RPM and the feedrate also has to be altered****
If you program in feed / rev
*** changing RPM has no effect on pitch***

If you want to program in feed / rev ( pitch ) a g-code must be stated on or before the tapping cycle.

If using a tapping head that allows extension and compression, use approx 95% feedrate factor,


ie 1/2 UNC tap
G95
G84 G99 X--- Y--- Z-1.5 R.2 F0.0769 (100%)
G84 G99 X--- Y--- Z-1.5 R.2 F0.0730 (95%)
X--- Y---
G80
G94

[Rich Kay]

Your controller might also need to read an "M29" code to initiate rigid tap mode?

( TAP 5/8"-11-4 HOLES ON 5.5" B.C 1" DEEP.)

G00G40G80G90
G80T16M06
G00 G54 X1.9446Y-1.9446 S0130 M03
G43 Z4 H16
M29 S0130
G98 G84 X1.9446 Y-1.9446 Z-1 R.4 F11.82
X-1.9446
Y1.9446
X1.9446

[Boots]

Some Moris' need or accept an G84.2 for rigid tapping and you can use a solid holder like a drill chuck.

[xEstrnDrgnx]

Here's a program that might help......

T8 M06;
G90 G54 G00 X0 Y0 S754 M42;
G43 H08 Z.5 M8;
G84 G99 Z-1. R.5 F58.;
G80 G00 Z1. M9;
G28 G91 Z0 Y0 M5;
M30;

HERES SIMPLE FORMULA TO FOR CALCULATING THREADS PER INCH,

1 DIVIDED BY 13(this number is the thread pitch) = ???

Take ??? X RPM(ei. S754) = F58. (is the feed )

Suggestion; Might want to make sure you drill the hole with the drill which call for the tap size. Use the right kind of tap (I prefer EXO tap spirral flute
black oxide, a little expensive but u can really tap at pretty high speed with this and this tap pulls out the chip instead of being clogged inside the hole which in most cases can break taps, with this sample pro gram ucan use
standard tap holder, try not to use holder with collet for tap cuz the tap can
spin in the holder that cross thread and also break.)

[dpuch]

Something I always like to do when tapping is to pick speeds and feeds that do not have any rounding (or decimal smaller than X.1).

IE 13 tpi I would use a RPM that can be divided evenly by 13
13 RPM = 13 threads = 1 inch per minute. So:
130 RPM = 10 IPM feed ect. Just pick you speed and feed range and find the closest speed that results in even numbers.

A decimal for a feed is fine as long as you are sure your control uses all the digits and there is not any rounding when you calculated it.

[KQHung]

Dear Friends,

do you know if the mill OKK MCV-500, manufactured 1988, fanuc OM-B can do rigid tapping? If yes how I can activate it?

Thank you very much for your quick help as now I am using foating tap holder but it still frequent breaks the taps.

Best regards,

Hung

[cncurmudgeon]

Wrong feed vs. speed? Lack of tapping fluid? Packing chips in a blind hole? Wrong tap drill size? Too many questions here and not enough information provided to tell why you're breaking taps. You haven't posted your code either, so no one can check to see if the program is in error.

[toolmaker7]

For feed rate it is 1/ pitch x rpm Example: (1/2-13) with and rpm of 450. so 450 x .0769 =34.605.
and don't power tap four fluted taps they always brake.

[Daniel1313]

Most people use G84 for tapping. What kind of tapping adapter? What do you mean when you say "It still doesn't work"? What happens when you try to tap a hole? What does your program look like?

This should be roughly what you need to program.

N10 T10 M6 (1/2-13 TAP)
G54 X0. Y0. S260 M03
G43 Z0.2 H10 M08
G84 Z-1.0 R0.2 F20.
X1.0
X2.0
G80 M09
G91 G28 Z0
G91 G28 Y0
M30

Im running fanuc oi-tc and am trying to run a G 84 tapping cycle and when it is completed on my next tool I get an al-15 spindle command and time over alarm and can no longer use the spindle what do I do

[dpuch]

General advice, make sure you have a G80 after the G84 lines.
Beyond that, read the manuals for your machine to make sure your not missing something specific to your machine/control.