i built a full size 4x8 lowrider 4. I am trying to cut some small 1/8th thick 6061 plates for my ftc robotics team and i keep breaking bits. ive tried watching various youtube videos etc but i’m really struggling with feeds and speeds the last one i had going was 4.4mm/s 0.5mm doc this did a couple small plates before failing. the bit was a 20$ bit from amazon 1/8 single flute upcut. it seemed to be cutting nice then a sudden chatter and snap. i do not have air blast or mist, but i was vaccuming the slots manually to try and keep clear. I’m not sure if i just have the settings wrong or if its the bits? any advice at all would be amazing we have a competition in a week and i really need to get these parts made for the kids.
My starting parameters were:
- 18,000 RPM
- 600 mm/min feed rate
- 0.4 mm depth per pass
- 120 mm/min plunge rate
- Ramp or helical entry instead of plunging straight down
- Constant compressed air
- A small amount of WD-40 or cutting fluid to help prevent aluminum from sticking to the bit
- Around 0.6 mm stepover for side milling
I also tested a slightly more aggressive range before, around 16,000–18,000 RPM, 900–1,200 mm/min feed, 0.5 mm depth per pass, and about 200 mm/min plunge.
I’d start with the more conservative settings and then increase the feed gradually while watching the chips, temperature, and how the machine behaves.
You can try reading through this:
It’s not the fastest, or maybe even the most optimal, but it’s a good starting point that I think has worked for everyone who tried.
It’s a good place to start, then tune from there for reduced time if it matters
The “cutting nice, then sudden chatter and snap” pattern usually means the flute is packing with aluminum, and your feed is probably part of the cause. 4.4 mm/s is about 264 mm/min. At something like 18k RPM on a single flute, that’s roughly 0.015 mm per tooth. That’s too thin to make a real chip, so the edge rubs and heats up, aluminum welds onto it, and eventually the slot jams and the bit lets go.
Daniel’s settings are a good place to start. 600 mm/min at 18k is more than double the chip thickness. Ramp in rather than plunging, and put a drop of WD-40 on the cut every pass since you don’t have air.
A few other things that help a lot on 1/8" plate:
- Keep the bit stickout as short as the depth allows.
- Clamp or screw the plate down hard near the cut. Thin plate that lifts or vibrates breaks bits fast.
- If your CAM allows it, make the slot a bit wider than the bit, or use an adaptive path, so the cutter isn’t buried full width.
Cheap bits aren’t always the problem, but a proper aluminum single flute (polished, sharp) is a lot more forgiving when you’re up against a deadline.