Machining Polycarbonate

[jdwhittaker]

How fast should I be cutting polycarbonate? I've never cut it before, and don't want to start off out in left field.
I have a 5-axis CNC Router that's capable of feeding at 600ipm. It has a 24000RPM Spindle. I'll probably be using 1/4" - 1/2" tools. The material is 1/2" thick.
Any advice would be greatly appreciated.

Thanks,

Dave

[Geof]

Always use new cutters that have never touched metal. Polycarbonate needs a very sharp edge so use uncoated carbide, preferably the micrograin carbide with a highly polished finish that is used for the cutters used on aluminum.

24,000rpm is a bit high so if you can back it down to 15,000rpm that might be better. Read below, keeping the chipload high enough at high rpm means the feed has to be high which can affect accuracy for curves and sharp corners.

Keep the feed high, something like three times what would be used on aluminum which translate to around 8 to 10% of the cutter diameter per tooth for the chip load.

A 1/2" high helix cutter should be able to go full width and 1/2" deep because it tends to screw the chips up out of the cut, 1/4" it may be necessary to reduce the depth to around 0.2" for full width but for side facing with an engagement of up to 80% of the tool diameter full depth should be okay.

An air blast is a good idea to clear chips and provide some cooling. For deep slots where it is impossible to get good chip evacuation coolant may be needed. Polycarbonate is resistant to most water mix coolants or a soap and water mix can be used.

For drilling it is absolutely essential to use sharp drills and keep the speed moderate to avoid melting the chip in the hole. Moderate is about as slow as you would drill mild steel but with three or four times the feed.

Good clamping is essential; polycarbonate is flexible and slippery and it likes to climb up the helix on drillls and milling cutters.

[MadMax]

I find high quality HSS tools work better than carbide on PC. HSS has a finer grain structure than carbide and can be sharpened to a sharper edge than micrograin carbide.

Airblast is a good way to clear chips. Chip evacuation is very important to prevent the chips from sticking together and welding back onto your workpiece. If ventilation permits, I find a mist spray works very well for keeping cutter temp low without having to flood everything. Pick your coolant concentrate very carefully. PC is sensitive to some oils (which may include soluble oils) and can microcrack or craze. You may not see it immediately, but the long term longevity of your product may be reduced by an incompatible coolant selection.

I find you can go with a fairly aggressive feed with hole drilling. In fact it's sometimes necessary to give the chips less time to heat up and weld back onto the workpiece. Geoff is right on the money here: 4x the feed, same rpm as mild steel. Drill with too low a feed and the fine chips crumple up and wipe in the hole and start to melt. Higher feed rates give stronger chips which seem to shoot up the flutes and go away. Peck as necessary to get some coolant onto the drill with deep bores or the drill may heat up and melt chips in the flutes.

[jdwhittaker]

Thanks for the advice. I'll let you know how it goes. I should be cutting early next week.

Thanks again,

Dave

[sunworksco]

I have picked so many machinists' brains trying to find a solution for threading inside diameter 4" O.D. x 3.5" I.D. x 36" length polycarbonate pipe and have come up with a design that I think will work.I am using a 3.5" wooden mandrel with a 7/8" hollow shaft then mounting Acme standard thread flanges on each end.I will then insert into the hollow shaft mandrel an Acme screw shaft with a rotary cutting tool attached at the end of the pipe with a hand crank.The cutting tool can be adjusted for several shallow passes for a desired depth.The pipe will be sealed with threaded pvc end-plugs for a water tight container for scuba camera gear.This is a copy of a 2-1/8" diameter x 9" length scuba container.Image is attached.

[shearder]

I know this is an old thread but i have been doing some reading on this throughout the interweb... I actually worked some PC this weekend. 10mm and 12mm sheet. From what i had been reading it was basically a FAST feed and spin at max i.e. 24k rpm. Well i started off doing this but i found even running at a fast feedrate, which was scary as i was only using 1/8 or 3mm end mill HSS type - i was afraid it would break.

Anyhow: it was too fast and instead of chips i got melted bits of PC all over. Long story short i was bust milling small nano tank lid struts. So the BEST finish i got - smooth and slightly smokey - i ran at 12000 rpm @ 200mm/min. May be a bit slow for some BUT let me tell you it was spewing chips for 14 hours non stop. The finish was excellent and the end mill held out to the point that it is still sharp enough for more work.

If i was brave enough i would have maybe played around more - any end mill sponsors out there?? LOL