PDA

View Full Version : Anyone routing polycarbonate/acrylic?



kong
07-22-2003, 06:01 PM
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
07-22-2003, 07:02 PM
I have cut it before, What is it you are trying to find out Sir?

kong
07-23-2003, 04:07 AM
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
07-23-2003, 10:17 AM
You cah use regular endmills, as for coolant a waterbase type is fine or cold air.

Jennifer
07-23-2003, 10:36 AM
Here's a good source:

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

gloomyandy
07-24-2003, 12:51 PM
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
07-24-2003, 01:24 PM
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
07-24-2003, 02:24 PM
But like gloomy just said, the speed is rated as in/m

Jennifer
07-24-2003, 02:32 PM
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
07-24-2003, 02:48 PM
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
07-24-2003, 04:26 PM
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
07-27-2003, 01:09 PM
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 (http://www.onsrud.com/) site - especially the FAQs and their sister site Plastic Routing (http:///www.plasticrouting.com/) where you will find the Van Niser Articles (http://www.plasticrouting.com/Van.asp) an excellent primer on plastics machining.

Hope this will be of some help

gloomyandy
07-27-2003, 01:33 PM
Hi Scrit,
Where in the UK are you? I'm based just outside of Leeds. You don't by any chance have any recommendations for UK based suppliers of cutting tools do you (in small quantaties for hobby use)?

Thanks

Andy

Scrit
07-27-2003, 02:40 PM
Hi Andy

I'm about 25 or so miles from you going towards Manchester. If you want off the shelf router cutters for wood/plastics I'd try (Carbide UK (http://www.carbideuk.com) in Hull on 01482 227234 - they are a trade outfit (the make their own spirals) but they will do credit card and their prices make Trend look sick. Another way of doing it is to find a Freud dealer in Leeds (you could always ring Freud UK on 0113-245 3737 for your nearest dealer) and try to get a discount - Freud is a bit pricy at list (almost as bad as Trend) but I generally manage to squeeze a reasonable discount out of them - some of the builder's merchants like Travis-Perkins sell their stuff at quite good prices, too. The final "choice" is to try the local Trend dealers (almost every power tool shop you'll ever come across). All three makes have solid carbide spirals in their range. Another option is to talk to ATA Engineering Processes in Hemel Hempstead on 01442-264411 - they are the Onsrud agents in the Uk and seem to carry stock of most things. Finally, you could always contact Clico Tooling in Sheffield on 0114-243 3007 - Clico don't yet do solid carbide, but they do make high quality spirals is HSS (suitable for UHMW, polycarbonate, etc) and they will do mail order.

Beware! Solid carbide spirals are not cheap!