[FuriousGeorge]

I'm about to do some milling of "easy to machine" ABS plastic (McMaster-Carr) on my Tormach. I'll be doing some roughing with a 1/2" 2 flute HSS Cutter and contouring with a 1/2", 1/4" and 1/8" Ball mill (All HSS, 2 flute) and a 2 flute 1/8" EM (prolly HSS, but carbide is an option). Any advice for feeds and speeds? What kind of WOC and DOC can I take before I start to crack the stuff? Any general advice for milling ABS? I'm mostly a metal guy.

Thanks!

[SCzEngrgGroup]

You can treat ABS largely like 6061, at a minimum. I typically run max RPM (6000 in my case), then double, or even triple, the 6061 feedrate. Just start with 6061 settings, and increase feed in steps and see how far you can go. It will come down to the exact configuration of the material, and how good your work holding is. HSM toolpaths help to get good MRR without ripping the piece out and tossing it across the room.

Regards,
Ray L.

[SCzEngrgGroup]

BTW - Carbide router bits also work well with plastics, and eliminate "fuzz" on the top/bottom of the part.

Regards,
Ray L.

[FuriousGeorge]

Thanks for the advice! Are there any problems with taking very light cuts (my cam doesn't do HSM toolpaths). My first operation should be fine, but my second op is a bit sketchy. I'm putting some #2 press fit threaded inserts into the enclosure and using four #2 screws to attach it to a negative of the cavity (machined AL). I'm definitely scared about thing flying off so I was gonna take lots of light passes (say, 0.05 DOC/LOC).

[SCzEngrgGroup]

You'll find very "thin" cuts just rub, and don't cut. With plastics, I generally try to do no less than 0.010" width, preferably more. 0.05" is fine, though you can do a LOT more when roughing if securely held. Keep feedrate up so you still get a decent chipload on thin cuts.

You can "fake" HSM toolpaths, depending on your CAM. For example using a contour toolpath with small stepover, and high feed. On pockets, you may have to first do a helical or slotting cut to provide room to get started, and you'll be limited by the speed through inside corners. Outside profiles generally don't require anything special unless there are "inside" corners.

Regards,
Ray L.

[cordvision]

For a 1/2", 2 flute endmill: You should easily be able to use a DOC of 1/2" with a 25-30% step-over at 30"/min (with proper work holding). ABS cuts like butter.

[AUSTINMACHINING]

You can go shallow, but keep your chip load up to keep down the heat. Once you start melting and clogging flutes, it's all over. If my my work holding is questionable, I'll go about .1" deep and 60/70 IPM at 6000 rpm's and go up from there when slotting,

[Steve Seebold]

Quinco makes some cutters that are right hand cut, left hand sprairal that will actually push your part down while it's being machined.

I think the smallest cutter they mahe that style is 1/4 inch.

I have done lots of ABS and delrin machining with these cutters and had great success.