PDA

View Full Version : Machining Polycarbonate



jdwhittaker
11-03-2009, 01:14 PM
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
11-03-2009, 02:25 PM
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
11-04-2009, 01:45 AM
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
11-04-2009, 04:29 PM
Thanks for the advice. I'll let you know how it goes. I should be cutting early next week.

Thanks again,

Dave

sunworksco
11-11-2009, 02:22 AM
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.:confused:

shearder
03-15-2013, 05:25 AM
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

cgallery
09-17-2014, 11:46 AM
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

I machined my first piece of polycarbonate this morning using a new 1/4" Onsrud bit intended for PC. I was trying 15-RPM and 15-IPM, and was getting a lot of chattering and shaking on my little CNC router. I'm not sure if the PC will work for me in the long run, but it will be interesting to try slowing my feed rate further and seeing if I get better results. I suspect I would, but was afraid of chips melting to my cutter.

cgallery
09-18-2014, 12:12 PM
Well just a follow-up, I tried reducing my speed to 7.5 ipm (.125" depth) and it was still grabby and didn't cut so great. After some experimentation, I discovered that as long as I kept my passes to .05" or less, I could cut at 14k at up to 60-IPM, which is really the limit for my machine anyhow.

cgallery
09-19-2014, 08:48 PM
Well another follow-up to my follow-up. I tried .04" per pass and found out also that normal milling (as opposed to climb milling) isn't a great option, the bit wants to grab into the material too much and I get chatter and gouges into my walls. Climb milling works a ton better. So I was running .04" per pass and about 50-IPM but I think the 50-IPM was too fast, too, as the polycarbonate is very grabby and I got a couple of more gouges in my walls at 50-IPM. So I slowed down to a crawl, 15-IPM, climb cut, .04" per pass, and got real nice results. No melting plastic as my reading would have caused me to believe.

Oh, and I would normally do a .01" clean-up pass at full depth, but even with a climb cut, I got some chatter and found that I didn't really need a clean-up pass anyhow, I had no ridges in my walls or anything from my dozen passes at .04".

Just thought I'd provide the update. In a nutshell, climb cut, slow down (15-IPM feed and plunge), no clean-up pass.

My router is a table-top CNC router from K2, and my spindle is a Bosch Colt running at the lowest speed (about 15k). I was using a new Onsrud spiral upcut double flute intended for hard and soft plastics.

rdlohr
11-02-2014, 08:47 AM
Has anyone tried a cold gun to avoid the melting? I cut a lot of small parts out of 3/16" PC with a 1/16" 2 flute spiral end mill at 23,000 RPM and 8 IPM with no cleanup pass. I've had pretty good luck with mostly straight lines but the set of parts I am working on now has all curves and I am getting build up on the blade that turns into big melted blob that ruins the cut. ( The bits are 130007 1/16” 2 Flute End Mill bits from American-carbide.com )

Sounds like I should slow down to 15000 RPM and possibly go back to multiple passes. Also maybe try climb cut.

LeeWay
11-02-2014, 09:27 AM
I would say climb cut for sure.
I cut a lot of PC and the best bits I have found are the Onsrud 2 straight flute solid carbide type. They are designed for soft plastics and have no spiral, so no lifting or pushing properties.

I get clean dado's, holes etc and no melting with a standard PC router.

shearder
11-02-2014, 10:00 AM
If you are running @ 8 ipm you can slow the spindle to 8000-10000rpm or speed up more on your feed. You can add a air blast to keep things cool but I never do. But try 8000rpm first. AH but just remembered you can only drop to 15k. Maybe speed up to 12ipm multiple passes


Has anyone tried a cold gun to avoid the melting? I cut a lot of small parts out of 3/16" PC with a 1/16" 2 flute spiral end mill at 23,000 RPM and 8 IPM with no cleanup pass. I've had pretty good luck with mostly straight lines but the set of parts I am working on now has all curves and I am getting build up on the blade that turns into big melted blob that ruins the cut. ( The bits are 130007 1/16” 2 Flute End Mill bits from American-carbide.com )

Sounds like I should slow down to 15000 RPM and possibly go back to multiple passes. Also maybe try climb cut.

LeeWay
11-02-2014, 10:12 AM
Speed way up on the feed.
I probably cut at 40 to 80 IPM depending on the type of cut. Sometimes as much as 150 IPM.

shearder
11-02-2014, 10:30 AM
I would speed up little by little. A 1/16 end mill is not that strong. You may need a few to find that sweet spot.

LeeWay
11-02-2014, 10:34 AM
Good suggestion. I use 1/8", 3/16" and 1/4" bits. Feed rate does vary depending on which is chucked up and the type of cut.

shearder
11-02-2014, 10:47 AM
Yeah I typically use 1/8" when machining acrylic or PC

rdlohr
11-02-2014, 11:33 AM
Thanks. All good suggestions. I use a 1/16" bit because I do some intricate cuts. I'm currently cutting through in one pass so I think I will try multiple passes then a finish pass full depth.

shearder
11-02-2014, 12:14 PM
What depth are your cuts currently?

Thanks. All good suggestions. I use a 1/16" bit because I do some intricate cuts. I'm currently cutting through in one pass so I think I will try multiple passes then a finish pass full depth.

rdlohr
11-02-2014, 02:01 PM
What depth are your cuts currently?

Its 3/16" Lexan and I was cutting it with one cut. I'm doing 2 cuts and a final finish pass now at 15 IPM and 23000 RPM and its working well even with a bit that I have quite a few cuts on.
Climb out vs. traditional didn't matter much.
Lower speed (10,000) produced a rough finish. I didn't try any intermediate speeds.
Not sure I even need the Cold Gun now.

shearder
11-02-2014, 02:33 PM
That's great news :) like I said I don't use any air though I have it. If it is moving fast enough it doesn't get tine to heat the material. You should be ok now 👍

Its 3/16" Lexan and I was cutting it with one cut. I'm doing 2 cuts and a final finish pass now at 15 IPM and 23000 RPM and its working well even with a bit that I have quite a few cuts on.
Climb out vs. traditional did matter much.
Lower speed (10,000) produced a rough finish. I didn't try any intermediate speeds.
Now sure I even need the Cold Gun now.

rdlohr
11-02-2014, 03:41 PM
Thanks for the help all!
Rick

shearder
11-02-2014, 09:47 PM
Most welcome. It's why we're ALL here :) for help

Thanks for the help all!
Rick

rdlohr
11-02-2014, 10:32 PM
:cheers:

rdlohr
11-14-2014, 05:04 PM
Just an update. The multi pass approach is working well. I read somewhere that the depth of each pass should not be more than the width of the bit as a rule of thumb. I've been sticking to that and all is well.

I did some climbout tests, and for my application, climbout left shreds hanging on the part I was cutting rather than on the surrounding Lexan so I am sticking with regular milling.

Using a speed of 15 ipm did not leave the part quite as smooth as 10 so I am using 15 ipm for the initial depth passes then I do a final pass at 10 ipm and cut the entire thickness but just the last .01 inch. That removes any artifacts from the multi pass and leaves a nice finish.