# Small holes in Al, feed

I need to drill a bunch of small holes in Aluminum.
I need to drill about 32 0.029 (#69) holes in a 1/2" Aluminum plate.
My mill will only go to 4500 RPM.
What feed and peck depth would you use for this small of hole?
I also have to do 0.52 (#55) and 0.070 (#50) holes.
But I figure if I can get the #69 right the others will be easy.
Paul
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
snipped-for-privacy@Rasdoc.com wrote:

Paul:
Ask 10 different machinists, you'll probably get 12 different answers. But here's what I'd try (preferably in a piece of scrap first).
.029 Carbide Circuit Board Drill. 4,500 RPM (your machine max), a peck of half the drill dia., a feed in inches per revolution of around 2% of drill dia. or about .0006 IPR (around 2.7 inches per minute - RPM X inches per revolution). If you don't have any Circuit Board Drills you could use stub length 135 degree split point drills, at the same speed and feed.
I'd use similar feeds (2% of drill dia.) and half dia. pecks for the other small drills as well. If you have thousands of these holes to drill, I'd experiment with greater feeds. If you had 10's of thousands of holes to drill I'd consider an electric or air driven drilling attachment for the spindle, since these small drills could probably be spun at 30-60k.
--
BottleBob
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
At 3000 rpm you can use the drill's decimal equivalent, times 100 for the feed rate in inches / min. 1/8th drill = .125 @ 3000 rpm the feed will be (moving the decimal 2 places to the right) 12.5 inches per min.
at 300 rpm 1.2 inches per min... and @ 4500 it would be 18 inches per min. 1.5 times what it was @ 3000rpm.
Drill the first peck 3- 3.5 diameters deep and .5 diameters deep after the first peck.
Circuit board drills are wonderful.
This works for 90% of the materials, even 316 sst. ofhc copper isn't strong enough to support the cut so divide the feed by about 3. Makes less burr.
Best regards,
Stan-

<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Stan Dornfeld wrote:

Stan:
You know, I was thinking about you when I was writing my response to Paul. I haven't seen a post by you for some time. I hope things are going well with you and yours.
--
BottleBob
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Thank you Bob. *smile Everything is very crazy here.. house remodel, sold my main shop, trying to get my vise manufactured... All's very smooth.. LOL! Cya

<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>

Stan, Interesting concept. I was wondering where you got that from. The only drilling formulas I can think of right now are the ones that recommend .001 ipr for 1/8 dia. and under, .003 for 1/8 - 1/4 and so on. Numbers might not be exact but close as I don't have a chart in front of me. I'm going to have to give your formula a try. Thanks, Duffy
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>

Hi Duffy..
I developed it when I needed to drill .013" holes in alum 6061. 2400 per table full. Lasted well into the night. :- )
I stopped breaking tools with the formula..
The only material it fell out of bed on was Carpenter 49.. (much nickel) Whew!
It works out to about 1.6% of the diameter per flute on two flute drills. 3.2% of the diameter for the drill size as a whole (both flutes)
The geometry is basicly the same on twist drills. So the percentage is directly proportional as the size goes up and the RPM goes up. Of course as the diameter goes up, generally the rpmr goes down so the feed may stay the same.
I have used this approach from .010"- 1.00" diameter. I also used it drilling a .013 diameter in 316 SST 12 diameters deep! I was afraid to drill the second hole. *Grin
Best regards,
Stan-
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>

Stan, There's nothing like learning from someone else's experience. Sure beats breaking a bunch of drill bits to try and find the perfect speed and feed. I've used a few of those circuit board drills and they do work nice. I haven't done a whole lot of very small holes although I've done a few. Usually with one of those spring loaded 2 finger sensitive feed drill chucks. I wouldn't want to do too many holes like that but it's alright for a few. I'm going to bring your formula to work with me and try it out. I'm doing a recurring job now which requires a .062 +.001 -.000 dia. hole down the center of a 1/4 in. 303 ss shaft. crosswise, central within .002 and +-.001 from the end of the shaft. After quite a bit of trial and error I do them with a 1/16 solid carbide spade drill. I mill a slot in a soft jaw to hold the pin. Once over the location I peck drill it @ 3000 rpm, .01 per peck full retract @ .5 ipm. It's not the fastest operation in town but it cuts right to size and doesn't drift from location and I only get between 10 and 20 pieces at a time when they come around. The metal removed actually resembles a chip. I've been planning on trying a circuit board drill one of these days but it's hard to change after something works. Thanks again Duffy
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Hi again Duffy..
Here is how it works...
If you double the size of a drill diameter, you increase the cross sectional area of the drill body by four times. (A= Pi * radius^2) With four times the body area, you can twist it with four times the torque because you have that much more steel in the drill.
Since the cutting edges of the drill go across the diameter they increase in length as the diameter increases. this means a drill twice as large only uses two times the torque. That leaves two times the torque not being used.
So you can use it by doubling the chip load.
Therefore.. the chip load is directly proportional to the drill diameter.
I hope this makes sense.
Best regards,
Stan-