Drilling 80 000 3/16 hole in 4x10x3/8 of Brass(C280)

Hello,excuse my english i am not a native speaker

like the title says i have 80000 holes to drill per sheet (10 sheet of brass 4x10x3/8), im currently using short 3/16 HSS drill, with coolant.
Im running at 6800RPM/20IPM and im struggling with my chip evacuation,

any tips for the perfect feed and speed, and i dont want to have to change my tool too often.

Thanks

4 by 10 feet is 13.8 holes per square inch. Makes 38% of material removed

You may need a drillbit specifically sharpened for brass.

what tip angle should i use?

I recall drilling 1/8 holes in 3/16 brass with a standard HSS drill. I was limited to 3500 rpm but think we were doing 40ipm even at that relatively low sfm. Try bumping up your feed and the chips may fly off the drill without any problem.

Sounds like the kind of project a drill bit manufacturer could be tapped for advice. How many lines in that program?

Surely such a job would justify the cost of a solid carbide drill! The tip angle is irrelevant, the rake angle should be zero, which you can do by using a diamond hone inside the flute to flatten the cutting lip for a distance equal to the feed in inches/revolution. Feed rate should be boosted enough to get a good chip ejection. I don't know that coolant would be a requirement, maybe a bit of an air blast would keep the area clear of the gunk.

i dont have the number of line on my software, but its about 16hours of machining, and i cannot heat the sheet or its going to warp, my machine can go up to 24000 rpm, should i up the rpm and ipm?

Gabriel Lemelin said:

i dont have the number of line on my software, but its about 16hours of machining, and i cannot heat the sheet or its going to warp, my machine can go up to 24000 rpm, should i up the rpm and ipm?

Click to expand...

Think of the feed rate required to form any kind of chip except dust at 24k rpm.

No, high speeds like that won't buy you performance.

ive uped my ipm to 30 and its seems to help, chip is about 0.01-0.013 thickness and isnt too long.

A parabolic flute drill or a carbide drill for brass would definitely help but it looks like the issue is your feed rate. I'd recommend running the 3/16" Drill at .004"-.005" IPR in long chipping brass and it looks like you are currently at .0029" IPR which could be keeping you from breaking the chip. I'd try it at the higher feed rate and see if it does a better job of breaking the chips and getting them to evacuate (your RPM looks a little high but as long as drills aren't burning up quick on you then you can keep it there).

Here is an option for the Cobalt Parabolic Flute Drill that would help chip evacuation:
YG- DN51412 -Shop ToolHIT

If you are looking to cut cycle time then a carbide drill for Brass would be the best way to go, here is info on it:
M275-476AU: Mapal 3/16" Diameter 5XD Solid Carbide ALU Drill - ToolHIT
Speeds/Feeds for Above Drill in Brass:
SFM: 197-722 (Start at 550 SFM)
IPR: .0028-.0071" (start at .0055")
IPM: 61

Hopefully this helps!

Mike