Results 1 to 15 of 15
Thread: small hole drilling
01-29-2009, 07:24 PM #1
small hole drilling
Need to drill about 200, .024 diameter holes through .094 thick 304 stainless steel.
Using a machining center with 10,000 rpm available, what would you recommend for speeds and feed (IPM), and pecking length. What I have available in house is just some HSS Jobber drills, black coated (basic drills).
Also, I can either flood it, or micro drop it (preferred). Which would you use?
01-29-2009, 07:33 PM #2
For cheap jobber HSS drills - 2300rpm, 1ipm.
I'd flood it myself, single peck at .06.
You can probably go up to about 6krpm on the and feed accordingly but they should be a decent start point without knowing whether the drills are decent or not.
01-29-2009, 07:43 PM #3
I'd run it at 40-50 feet per min @ 45'/min your at about 7163rpms, 2300 is way to slow. as far as feed goes I would start at .0005/rev, maybe even less. keep the drill as short as possible too.
01-29-2009, 09:25 PM #4
I would definitely try and get a straight flute carbide drill, if I had to do 200 of those holes. Don't know the speeds and feeds, but I can say it'll be way faster than an HSS drill, and it'll go the distance once you get everything dialed in.
01-29-2009, 09:34 PM #5
Carbide circuit board drill?
01-29-2009, 09:37 PM #6
dont know if you have cts... but mitsibushi has a micro with coolant holes that will work well (no peck)
01-29-2009, 10:27 PM #7
Tulon Circuit board drills are VERY good tools.
Chip load is a little shy of .0004" per flute. Find an rpm on your machine which runs smooooooth!
It really doesn't matter what the rpm is as long as the chip load is the same, or you exceed the cutting tool's ability to handle the heat.
The smaller the drill (tool) the more you need absolute concentricity. Think of a 1" drill running out .010" -- No big deal. Worry that down to a .024" drill and the runout gets a bit tight. Around .00024" TIR
The first peck is good for 3 to 3.5 diameters. After that .5 diameter per peck.
I've drilled .020" holes at 1000rpm and .6 ipm with this pecking idea just to show my help you don't need a million rpm to drill holes.
Put a 1" travel indicator on the "Z" axis and see how it reacts when peck drilling. Slow everything down to a walk so you can see what is going on. Look for it to snatch the drill out of the hole while it is still taking a cut. I don't think you will see any dwell before it retracts. If so, that fact is very hard on the drill's cutting edges.
I'd build a special routine bit by bit reversing the feed for a revolution before the rapid up.
You can get away with it in the softer materials but sst is mean.
These are what I've found to be good things.
01-29-2009, 10:36 PM #8
01-30-2009, 12:12 AM #9
I would run that hss drill in collet holder @ 5570 rpm, 3.3 ipm, .006 pecking.
When You get done with the drilling; Let' s know what combination used to do the job. Good luck to You.
01-30-2009, 04:18 PM #10
Stan, that was interesting about the reverse being hard on the drill. I never noticed that before. I'll check that out. Thanks.
01-30-2009, 05:13 PM #11
02-02-2009, 01:59 PM #12
VERY interesting stuff. Thanks again, Stan.
02-02-2009, 02:25 PM #13
If it's SST sheetmetal good luck, the skin on SST sheet is some of the nastiest stuff to drill that I've encountered.
02-02-2009, 02:39 PM #14
For what its worth, I used 4000 rpm and 2.0 ipm. Pecked it every .008 and used microdrop mister. This combo worked about the best.
The part was actually tubing, with 8 holes around the perimeter. It was .250 OD x .062 ID.
I changed bits often on the parts, just for insurance purposes. Time wasn't as much a matter as scrapping a high dollar part.
Thanks for all the suggestions, and for all the info provided!!
02-02-2009, 03:11 PM #15
Glad you've worked it out.
Thankfully I don't even have to spend a second worrying about holes under 1/8 into anything with a holepopper at my disposal.
Just for future reference, an EDM holpopper eats a job like this for breakfast.
Most start at .4mm up to 3mm in increments of .1mm, but some of the higher end ones can handle electrodes down to .0005".
They also drill very fast, your hole for example would have taken 20 seconds at most per hole and would have produced no burrs at all.