[Crawler374]

So whats the secret to cutting plastic? i'm trying to drill and mill ABS 1/8" plastic and i cant get a clean cut to save my life. I have a 1/8" router bit which chips upwards. I've tried running the machine as fast as it will go, and as slow as it goes and i get virtually the same results, melted plastic. I bought a .062" plastic bit but all it does is melt and jams the bit which ruins my project. I have a router with a 1/4" shank, and i need a 1/8" milling bit ford drilling and side cutting. Any tips?

[ger21]

How fast can you cut, and do you have variable speed? With small tools, you have to get the chips out of the cut, or they'll melt on the next pass. A blast of compressed air on the cut will help.

[RomanLini]

ABS is elastic and if you cut too deep it squeezes around the bit and generates too much heat, and like ger21 said you have to get the chips out of the bit.

Try making much shallower cuts, and maybe try a 2 flute bit instead of 4 flute. And use a sharp bit, not one that has been used on metals or other materials.

[Jay C]

I had good luck with a 2-flute bit on some .25" ABS sheet. But I recently bought a purposed bit for plastic. It's an Onsrud single O-flute and it works as advertised. Like Ger and Roman pointed out, it's all about the heat you generate when cutting. I was running my spindle way too fast and cutting way too slow.

Using the chip load calculations I've learned that slower RPM and faster feeds are required for the optimum chip load. If your machine is feed limited, then you can reduce the number of flutes and slow the RPM. I'm not an expert and am only sharing my experience. The plastic is UHMW.

Chip load = Feed rate / (RPM * # of Cutting Edges)
Feed rate = RPM * Cutting Edges * Chip load
RPM = Feed rate / (# of cutting edges * Chip load)

Example:
Onsrud gave a chip load of .002
I had my feed at 26ipm
Thus my RPM should be 13K RPM

You can see the results of the new end mill following the guidelines. It's perfect right off the machine. You can see the 2-flute try right. The plastic was "smearing" instead of cutting. That was at 20K RPM and with 2 flutes.

Bad example:
Chip load = 26/(20,000 * 2) = .00065 or 67.5% too small
At 20K RPM I would have had to use a feed of 80ipm to get the recommended chip load

FWIW,
Jay

[Jay C]

http://www.plasticrouting.com/facts.asp

[accroul]

You need to keep the tool and the work as cool as possable, try air from a vaccumn cleaner or compressed air .
Run the cutter as slow as possable with a fast feed rate.

[Jason Marsha]

Personally I cut with 1/8" (.125") or larger upcut spirals 20 to 25K rpm and never had a problem with melting at about 40 inches/min. My bits are always very sharp.

Jason