Peck Drilling on a Fanuc 0i Mate TB....

[Darc]

Hi Guys, I'm currently using the attached sheet for peck drilling (G74) and I notice that when it retracts, it only retracts the peck distance you specify in an incremental movement, so basically if it's a 100mm deep hole and it's in 80mm with a specified peck distance of 5mm, it will only pull the tool out 5mm (75mm in Absolute) then rapid back to 80mm and resume drilling, any other machine I've ever worked pulls the tool out the the start value (normal Z1.0) then rapids back to where it was, thus resuming drilling. (this cleans all the swarf out of the drill flutes)
Is there a different G code so as I can do this?
I can't find one in the book.

[Dan Fritz]

I'm not sure if your 0T Mate is the same as the 0T, but check your manual for parameter 031, bit #4 (the 5th bit from the right). According to my manual, if this parameter is a "1", the peck drilling retract amount is to the initial start point in Z. If the parameter is a "0", then the "high speed" peck motion with a fixed retract amount is used.

[Dan Fritz]

I just noticed that you said you had a 0i Mate (different animal from the 0T). Check your parameter manual for 5101 bit #2 (the third bit from the right). The function is the same as for the 0T. A setting of "1" should make your Z axis retract all the way.

[Darc]

Hi Dan, Thanks for the replies, I changed the parameter 5101 bit #2 to "1" and it didn't seem to change anything, so I thought I'll restart the machine.
Unfortunately now when the machine starts up, the computer only stays on for about 5 seconds then shuts down, I can't restart the machine unless I turn it off at the isolator switch, any ideas?

[Dan Fritz]

I can't imagine why changing that parameter would cause the problem you described. It's a pretty ordinary parameter for setting the retract value of the peck drilling cycle.

Here's a page from the 0i parameter manual.

[Darc]

Hi Dan,
Sorry false alarm, it had blown one of the 3 phase fuses, I didn't think of the fuse because the machine still fired up but shut down after 5 seconds.
Sorry to scare you.
Darc

[shawnc74361]

The G74 drill cycle you are using is a high speed peck cycle. It eliminates some time over a standered G83 peck cycle.

G74 M99 Z-1.0 Q.1 R.1 F10.
Will rapid up and down only .1 in per peck.

G83 M99 Z-1.0 Q.1 R.1 F10
Will rapid up to the absoult retact postion of .1 above the part surface then back to the last point stoped.

On the machine I run it drills 40 holes in one cycle the G74 saved almost 15 min over the G83

[Darc]

I tried to use the G83, and it kept telling me improper G code, does this mean the machine doesn't support it.
I just noticed that the machine is actually a Fanuc 21-T, but the book is for a 21-TB, any ideas if they are different in any way?

[CNCRim]

Darc,

G80-G87 is to for Milling and you working on the Lathe, the only pecking cycle for 2axis lathe is G74, the option you have are limit. What you can do is program manual the retract and rapid to the point you want.... or you can use marco programming.

[shawnc74361]

Yea the g83 is a mill g code. The g74 is a high speed peck drill cycle on my machine. It is a Daewoo DVC 320/40 VMC with a 18T fanuc control. It might be a daewoo thing. I was not realizing it was a lathe question sorry my mistake.