Drill diagnostics

Eric U · Feb 2, 2021

I typically machine aluminum. Figuring out wear issues when machining steel is new to me. This is a .250” Garr AlTiN drill in 4140PH. Machine is a Doosan Lynx. I made it about 500 holes .380” deep. Should I expect more or could speeds/feeds be adjusted for better life? I’m running 2500rpm at .002”/rev.

Thanks!

Milland · Feb 2, 2021

Are you pecking? How is the tool held? Is it short, or jobber length? Any air blast or coolant?

FWIW, if that's .001"/rev per edge, I think you're feeding too slow.

Mtndew · Feb 2, 2021

Are you spotting? If so what angle is the spot drill?
If I were using that drill in 4140PHT, I'd run it at 350SFPM .0046" ipt all day long.
5348rpm 23.4IPM.
Basically double what you're running it at now.

Eric U · Feb 2, 2021

Milland said:
Are you pecking? How is the tool held? Is it short, or jobber length? Any air blast or coolant?

FWIW, if that's .001"/rev per edge, I think you're feeding too slow.

Answers:
Pecking .200”, ER16 collet, short drill, external coolant.

FYI, this is for a family of parts. The speed is from the largest size drill (.3438”) and the feed is from the smallest (.2188”). This is the drill I’ve run the most parts with so has actually made it to failure. I’d like to prevent premature wear with all of them of possible.

Milland · Feb 2, 2021

If the drill is stable on entry (so no spotting), then just drill to depth, no peck. I'll bet that's where at least some of your damage comes from. You could also at a couple revolution dwell at the bottom of the hole to finish shearing the chip before retraction.

When was the last time you checked centering? If the drill isn't straight on axis it's hard on the carbide.

And like 'Dew says, up the feed. May have to mod the code to suit the drills, but it's worth it.

Eric U · Feb 2, 2021

Mtndew said:
Are you spotting? If so what angle is the spot drill?
If I were using that drill in 4140PHT, I'd run it at 350SFPM .0046" ipt all day long.
5348rpm 23.4IPM.
Basically double what you're running it at now.

No spotting. I’ll mod the code to use drill diameter to calculate speeds and feeds. I’ll also remove the peck.

Thanks guys!

Mtndew · Feb 3, 2021

Eric U said:
Answers:
Pecking .200”, ER16 collet, short drill, external coolant.

FYI, this is for a family of parts. The speed is from the largest size drill (.3438”) and the feed is from the smallest (.2188”). This is the drill I’ve run the most parts with so has actually made it to failure. I’d like to prevent premature wear with all of them of possible.

If you were cutting plastic or aluminum that would most likely be ok, but since you're cutting steel you really don't want 1 program with static speeds and feeds for different drill sizes.

michiganbuck · Feb 3, 2021

And watch the drill wear land to see perhaps .02 rounded cutting edge, perhaps that would happen at 400 holes. Have perhaps 6 or 12 drills and know a shop that can sharpen them like new. Perhaps even have the sharpener make all the same length if that would help tool change.

Breaking or causing such a large cut off needed is a waste of money.

thesidetalker · Feb 3, 2021

Looks like what you get when you try to spot (to countersink dia) with a 90° spot drill. I had a guy who liked to do that. had.

Not saying you're doing that, and you mentioned no spot, it just makes me think of it. Tool life was horrendous. Brand-new looking drills with the tips blown out, everywhere. Drove me nuts.

BT Fabrication · Feb 3, 2021

pecking will kill the tips just like that. its the retract that loads it up and rips the edge off.

Milland · Feb 3, 2021

BT Fabrication said:
pecking will kill the tips just like that. its the retract that loads it up and rips the edge off.

That's why I suggested adding a dwell after a straight-shot to clear the chips before retract.

Eric U · Feb 3, 2021

Milland said:
That's why I suggested adding a dwell after a straight-shot to clear the chips before retract.

I missed the dwell yesterday. I’ll add one.

Thanks all!

Eric U · May 6, 2021

Just circling back around to tie a bow on this thread: after incorporating the following suggestions: drill straight to depth, slight dwell at bottom, and rpm calculated from drill diameter, I'm still going strong on all my drills, having only had to replace that worn out 1/4" one. I've drilled a total of maybe 7000 holes so far and the suggestions kept a lot of money in my pocket. Thanks!

Milland · May 6, 2021

Sounds like you're doing it right, good to hear!

Search

Largest Manufacturing Technology Community on the Web

Search

Drill diagnostics

Eric U

Hot Rolled

Milland

Diamond

Mtndew

Diamond

Eric U

Hot Rolled

Milland

Diamond

Eric U

Hot Rolled

Mtndew

Diamond

michiganbuck

Diamond

thesidetalker

Stainless

BT Fabrication

Titanium

Milland

Diamond

Eric U

Hot Rolled

Eric U

Hot Rolled

Milland

Diamond

Similar threads