What's new
What's new

Peck drill cycle while drilling by carbide

M Code

Aluminum
Joined
Apr 4, 2021
I am using a carbide drill on 4130 material with high feed and speed, everything is ok and the chips are flying away, but with that we still use a peck drill cycle

1- I am wondering does the peck has any benefits while drilling by carbide?
2- Will the peck cycle hurt the tip of the drill?
3- As long as there is no chips problem while using carbide we will not need peck cycle?

we are from HSS school.
 
2- Will the peck cycle hurt the tip of the drill?
Eventually, yes... and the sides of the flutes as well, potentially.

Typically you don't want to peck with carbide unless you absolutely have to.
Thru spindle coolant makes it so we don't need to peck.
What size drill are you using?
How deep are you going?
Speeds and feeds?
Peck amount?
 
Agree with 'dew above. If you HAVE to peck, you might want to longhand code that gives you a very short dwell before each retraction, so you don't "pull" the chisel edge of the drill with the partially attached chip. A dwell of at least one revolution cuts away that chip, lowering risk to the drill edge.
 
If I have to peck rather than dwell i retract at a little higher than the drilling feedrate about 1.5x the drilling feed per rev to break the chip, thrn continue drilling. This doesn't seem to affect drill life.
 
Peck drilling with carbide can be risky as the intermittent load could cause failure.
Generally, I advise to drill straight thru (G01 or G81) and use as much coolant as possible.
 
I also peck. I do not do production but one-offs for injection molds. So tool life seems to be fine. I only have like 300 psi. on my TSC. I am scared of the published feeds and speeds so i baby the drills.
 
I am scared of the published feeds and speeds so i baby the drills.
What brand of drills? I've used Guhring, Sandvik, Kennametal,OSG, etc... their speed charts are pretty dialed in.
The main thing some people miss is the feed per revolution. Some people use that as feed per tooth and end up doubling the feedrate. :willy_nilly:
 
Agree with 'dew above. If you HAVE to peck, you might want to longhand code that gives you a very short dwell before each retraction, so you don't "pull" the chisel edge of the drill with the partially attached chip. A dwell of at least one revolution cuts away that chip, lowering risk to the drill edge.
I program lathes. So far I've only had to use a dwell at the bottom on one series of lathes. Daewoo MS200s. 9/16 inch carbide drills kept chipping on one job. I was aware that these lathes didn't reach programmed position before starting to move on the next block. I use a modified version of Hardinge's 9136 Deep Drill cycle (pecking). I added a dwell at the bottom, and no more chipped drills.
 
What brand of drills? I've used Guhring, Sandvik, Kennametal,OSG, etc... their speed charts are pretty dialed in.
The main thing some people miss is the feed per revolution. Some people use that as feed per tooth and end up doubling the feedrate. :willy_nilly:
I heard of this one guy that tried that. Ran the MA Ford series 229 drills, 3 flute, at three times the proper feed rate.

All said, I still got thru 3 holes before everything exploded. I mean, this one guy said so. Not me, I'm a professional.
 
I peck carbide drills all the time. Not so much deep drilling but in long chipping materials to predictably control chips. Not full out but just chipbreaking. I use macros, not canned peck cycles. Don't dwell but feed in reverse until chip breaks and then continue to drill. No discernible tool life reduction and much much better lights out security. Using both solid and indexable drills with high pressure through coolant. Same thing works with parting tools. No more birdnesting in stuff that is tough to break.
 








 
Back
Top