very small holes (for me)

[littlerob]

I'm posting here because you guys drill small holes. I have 50 small holes to drill .75 mm/ .03". The hole is center line of the spindle in a lathe with 3000 max RPM. I have the tools (10 circuit board drills) and I dialed the tool holder within about .0002 of the spindle rotation. I haven't tried drilling yet (monday), but do you guys use the standard formula, drill diameter divided by 1/64 for a feed, that gives .0004 per rev. And what about peck amount? Another piece of info. the hole is about 15 X the diameter.

So my question is what feeds would you use for a drill this small?
And what peck amount?

Thank you Robert

[neilw20]

Small holes, but in what material?
Smallest drill I have is 0.25mm.
Peck depth for 0.75mm, I wouldn't use above 1mm normally, but it depends on the material.
Some material types clog the drill flutes.
Feed? 5-30mm/min is my guess.
I just start gently, and careful examination of the chips is what guides me. Stainless steel? Forget HSS. Use carbide.
3000 RPM means your feed will be slow.
As your hole is quite deep, a touch start with a center drill is a good idea, even in wood. Wood has hard spots and drills tend to wander.

[littlerob]

Originally Posted by neilw20 Small holes, but in what material? Smallest drill I have is 0.25mm. Peck depth for 0.75mm, I wouldn't use above 1mm normally, but it depends on the material. Some material types clog the drill flutes. Feed? 5-30mm/min is my guess. I just start gently, and careful examination of the chips is what guides me. Stainless steel? Forget HSS. Use carbide. 3000 RPM means your feed will be slow. As your hole is quite deep, a touch start with a center drill is a good idea, even in wood. Wood has hard spots and drills tend to wander.

Material is 7075 -T6

I am planning on spotting the hole, that peck depth seems a little aggressive, but okay with me.

But 5 mm/min seems really slow to me, it is a lathe so we feed in IPR and my table tells me 5 mm/min is about .00004" per revolution, is that right?

Robert

[neilw20]

5 was at the slow end before I knew the material.
For the AL, being T6 1-3 IPM, but that is only my guess. 3000RPM is slow
Some cutting compound, or kerosene in a spray bottle, will let you get more aggressive.
At that depth ratio I go chicken doing it dry.
PCB drills are usually carbide, with peck depth same as diameter, or a little less once it gets deeper.

(Z0 is touching the face - center drilling already done.)
(All inches - we are multilingual :)
M3 S3000
M8 (coolant)
G83 Z-0.2 R0.1 Q0.03 F3
Z-0.35 Q0.02 F2.5
Z-0.45 Q0.015 F2
G80
M5 M9
M30

[littlerob]

That seems a little more realistic, thanks Neil. If anyone else wants to chime in thats okay too. What I've got seems pretty straight forward, is the .0002 TIR going to sway the result of this?

[neilw20]

Runout will be OK on a 0.75 drill. My smaller drills needs centering checked with a magnifying glass so they don't break.

[littlerob]

First drill built 25 parts, still in the machine waiting for tomorrow to begin. It is really timid and slow, but not broken. Thanks Neil

[DCogswell]

5x dia 1st
3x dia until final depth for pecking

Being a Circuit Board Drill, I can't imagine you're going more than 15x dia deep.

maximum rpm (or as much as you are comfortable with)
f.0013 to f.003

Too slow and the material will clog your flutes. Spot before.

[Kutz]

How'd you make out?
I've drilled a Ø.0040" before RPM is your friend
To bad no live tooling you could counter rotate the drill against the spindle and really get the R's up there.
Misubishi makes a really good center drill with a minimal flat (about .0005) these work best for starting small drills.
Kyocera, in my eyes, leads the industry for circut board drills.
Get lots of oil and air down there if the drill starts to bind in the gummy aluminum it'll be over in a hurry.
Good luck

[littlerob]

Everything went fine, 1 drill 50+ parts. RPM is good and I was limited to 3000. Being attentive to chip load. Also I think making sure the holders and run out were/was reasonable helped.

Robert

[neilw20]

You just get better at it. Examine the drill tip with x10 magnification and make sure no dull spots.
You can resharpen if you really want.!!
What better use for worn drills, other to bust a few learning how.

How long on the grinding wheel?
Sense the temperature rise with your fingers 2mm away from the wheel.!!
http://www.cnczone.com/forums/453542-post181.html
http://www.cnczone.com/forums/453963-post183.html
Then use a diamond lap.
If the drill is just dull, a few rubs on the lap and it works again.