[travisn]

After seemingly figuring out m3x1.5 rigid tapping (just needed to put a drop of oil in each hole before) I'm somewhat struggling with drilling the 0.098" holes 0.5" deep in 6061. I broke two bits today, 6 holes apart, after doing about 60 on one bit. I've been running ~9700 rpm, 250 sfm, 0.0019 ipr with a ~0.030" spot drill. Both are 118*. I think my problems today were because the chamfer after the spot was too large (per the customer), so I lowered it from 0.040 deep. The bit is breaking in the hole, but I've been unable to retrieve the broken bit to see how far it is getting. The spot depth was all I changed recently.

Using F360 and a 99 Fadal 4020

I've been pecking with the following:
0.1" peck depth
0.05" min peck depth
0.25" accumulated peck depth
0.004" Chip Break Distance
and a 0.25" dwell

I ordered some carbide drills because why not. Based on my research I'll be getting rid of the pre drill, keeping the SFM at 250 (due to the rpm limits of my machine), increasing the IPR to 0.003, and maybe pecking halfway to clear chips and get coolant back in? That would give a feedrate of almost 29.

I'm not worried about cycle time, I just need to get through 2500 drilled and tapped holes with minimal tool breakage.

Any help/guidance for (small?) HSS or Carbide drills would be much appreciated. I have a few HSS bits left that I'd like to continue making parts until the carbide bits arrive.

[machinehop5]

...1/2" deep x .100 dia Alum6061T6 ...4000Rpms with flood oil/coolant at 20ipm and peck once..1st pass about 3/8 deep>>>Retract to Z0 to cool the drill tip then. finish the 1/2" deep. Screw machine type drill work best HSS and cheaper and tougher to break.
https://www.mcmaster.com/screw-machine-drill-bits/
If, you are brave try one pass...lol



Is good start point..old school may be slower...but, less broken burned up stuff in the long run. 10cent drill broken off in 1000 dollar part cost...you do the math.

[travisn]

I was looking at those short length bits, McMaster doesn't have them small enough though.

Strictly looking at the math, those speeds don'e make sense. that's about 103 SFM and 5 thou IPR, pretty aggressive feed even for carbide at those sizes. Unless you meant 8k rpm?

[travisn]

I just tried 15 ipm at 9700 rpm with 0.25" peck, it snapped on the second hole.

Fun times.

Gonna try .05 peck

[CNCMAN172]

Use solid carbide drill bits they cut aluminum like butter, especially at that higher rpm

[machinehop5]

make sense. that's about 103 SFM and 5 thou IPR, pretty aggressive feed even for carbide at those sizes.

..chipload ipr

[travisn]

working ok at 4800RPM (125 SFM), 9.6 IPM (0.002 IPR) with a HSS bit.

[machinehop5]

...17-4 stainless steel ...work hardens if, not drilled with the corroct chipload. Alum is easy.. keep failing til you keep failing ...then backoff 10 percent
the mission

[CL_MotoTech]

The carbide might be trickier yet. When carbide wanders at all it tends to break. That said, carbide is sharp and when all is good it flies through aluminum.

For deep holes do full retract, usually chip binding is what breaks the bit. I usually just turn the feed down to like 10% and get through the first hole, then bump to like 20% on the second, and keep increasing until I break a bit again. Then I back off 15% from the feed that broke the bit and leave it there. You will probably want some sort of schedule on replacing bits too. I recently did a bunch of M4 holes and found I could only get like 20 .9" deep holes on a single bit. The bit would get squeaky and I knew it was going to break pretty soon.