tapping metric thread on fanuc

[WJ MARK]

Im tapping 3 holes M3x.5 in 304 ss on a fanuc robodrill

to get my feedrate do I do .5 x .03937 x 150 rpms??? to get my feedrate??

I never do anything in metric so not sure if my calculations are correct.


Also a g82 spot drilling cycle axample would be helpful.


Thanks!

[stevo1]

Because you are in metric mode you do not need to multiply by .03937. You just take your .5*150=75.

I assume this thread is in reference to the “robodrill” one you posted in the fanuc forum??

Stevo

[WJ MARK]

Originally Posted by stevo1 Because you are in metric mode you do not need to multiply by .03937. You just take your .5*150=75. I assume this thread is in reference to the “robodrill” one you posted in the fanuc forum?? Stevo

Thanks again for the replie Stevo!

[Superman]

Simple formula

Feed per minute = Pitch x RPM

If you alter the RPM at any time, the feed would also need re-calculating.

Another common solution when tapping, is to use feed per rev ( G95 ), so the feedrate you dial in is the pitch of the tap, you can alter the RPM but the feed is still locked to the tap pitch and will not require adjusting.

The only problem is that you must change back to G94 immediately after using the tap, to avoid the next tool having 10" per rev feeds, for example
.


ie.(tapping)(imperial)
G95
G99 G84 Z-.75 R.12 F.0394 (M6x1.0mm tap)
Xx.x Yy.y
G80
G94

ie.(tapping)(metric)
G95
G99 G84 Z-19.05 R3. F1. (M6x1.0mm tap)
Xx.x Yy.y
G80
G94


ie.(spotting)(G81 and G82 do the same thing-one CAM software outputs G82 if you put a dwell in the cycle)
G99 G81 Z-.1 R.2 F.01 (90° spotdrill)
Xx.x Yy.y
G80
G94

[b.locke]

You can also add a Q to the G84 line. This would define a peck tap, which is handy in deep holes.

G99 G84 Z-19.05 R3. Q.05 F1.

Brian

[diamondyarn]

Hi There , I am new to The CNC Zone , and if any one could help, I want to do Metric Tapping on Fanuc 21M Control, its a Blind hole and need to Tap 5mm Tap , what could be the Feed Rate (.8pitch x300rpm=240 F ) is it correct or i should use any other M code Prior to this g84 line ?
Please guide me

[christinandavid]

On our Fanuc 31i we need to put an additional M29 before G84 to put the machine into Rigid Tapping Mode.

DP