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?
I don't care for flood because you might be drilling for twenty minutes and find the drill broke on the first hole. *s
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.
Best regards,
Stan-