Anyone routing polycarbonate/acrylic?

[kong]

I'm just thinking of new materials for making fan grills (already using aliuminium and carbon fibre), and polycarbonate seems like a good choice. I'd be interested if anyone has any experience in machining it.

[cadcam]

I have cut it before, What is it you are trying to find out Sir?

[kong]

Well I've not routed plastics before, so general tips would be nice. Not sure on the cutters, I know you can get special single flute designs for acrylic, so I guess I will need these for polycarbonate, I have some real small two flute high-helix (0.8 - 1.3mm) cutters that I will try first, but I'm a bit worried about heat welding the plastic so what's a decent coolant to use? Erm, I'm sure I'll have more questions when the stuff arrives and I get cutting!

[Bill]

You cah use regular endmills, as for coolant a waterbase type is fine or cold air.

[Jennifer]

Here's a good source:

http://www.alhyde.com/pdfs/alh07695.pdf

[gloomyandy]

Folks,
I'm probably a bit dumb on this stuff. The document above talks about Speed and Feed rates to use. Both are in in./min. I assume that feed is the rate at which the cutter is moved around the toolpath, so is speed in this case the rate at which the tool is rotated? If this is the case how do you turn the in./min speed into revs? Is it simply rpm*d*pi where rpm is the revs per min of the cutter d is the diameter of the cutter and pi is 3.142, or is it more complex than this..... or do I have all of this wrong.... In which case can someone point me at a good page that explains all!

Thanks

Andy

[balsaman]

Feed is the rate the tool moves, speed is spindle rpm, as far as I know there are no calculations to do, unless you want to figure out chip loading, which is the amout of material the tool removes per turn.

Eric

[kong]

But like gloomy just said, the speed is rated as in/m

[Jennifer]

I tried calling the number from that website to find out...they didn't seem to know if a calculation needed to be done or if it was a misprint and should be rpms...sorry.

Jen

[CAMmando]

Speed is usually Feet Per Minute. For milling (routing) RPM would be calculated based on tool diameter. For turning RPM is calculated based on work diameter (or constant surface speed is commanded).

I use a simple formula (with no Pi) for easy calculation on the fly.

RPM = 4 X SFM / DIA (cutter)

This formula is simple because you figure for a 4 in cutter RPM = SFM.

For a 2 in. Cutter RPM = 2XSFM

For a 1 in cutter RPM = SFM X 4 etc.

I suspect the value given in the tech data cited is 12 times the SFM which would give IPM so divide by 12

So RPM = Surface Speed (ipm) / (Cutter Dia x Pi)

[gloomyandy]

Hi Folks,
Well maybe I'm not so dumb after all! Thanks for the help a special thanks to Jennifer for:
a) Posting the link in the first place
b) Trying to call these guys to get an answer to my question....

All the best

Andy

PS Eric - love the new machine!

[Scrit]

The biggest problems you are going to have are melt- or weld-back and polymer memory. Melt-/weld-back is where the chips weld themselves back onto the stock material because they are so hot. Polymer memory is where the material flexes under pressure and springs back after the cutter has passed. Polymer memory is much more of a problem with softer materials such as polycarbonate than with harder stuff such as acrylic and the cure is simple - machine the stock (preferably a roughing pass allowing 0.3mm or so oversize all round) then do a second pass at maximum depth and final path to clean up the cut.

I wouldn't use conventional engineering end mills for the job simply because in general they don't have a sufficiently high chip load. Plastics cutters are much like those used in the woodworking industry - spiral up- or down-cut with a high chip load capacity. Those for softer plastics such as polycarbonate, UHMW, etc. are generally designed for lower revolutions and high feed rates. I typically mill UHMW plastics (which have similar machining characteristics to polycarbonate) at 12,000 rpm at 12 to 14 metres/min (480 to 550 in/min) feed rate with a depth per pass of 4 to 6mm on 1/2in diameter 2-flute solid-carbide upcut spirals. I try to avoid using smaller diameter cutters as they heat up to much and suffer from more problems of weld back than larger diameter cutters IMHO. We have rigged an air blower onto one of our spindles to assist cooling and the router has just going through a refit of the dust extraction to handle the chip waste - you must clear this to get a clean job. BTW, many plastics seem to respond well to climb cutting and woodworking spirals work almost as well as the proper plastics ones - just remember if you don't feed them fast enough they will break!

If you want a good site for reference go take a look at the Onsrud Cutter site - especially the FAQs and their sister site Plastic Routing where you will find the Van Niser Articles an excellent primer on plastics machining.

Hope this will be of some help