What are some good general settings for cutting polycarbonate on a CNC machine? What type of bit should we use? RPMs? Feed rate? I know some of this will depend on the router, but what are some general rules?
The parts our construction class makes for us usually come out with melted burs along the edges. They clean up fine, but we didn’t know if there was something we should adjust or not.
We use 1/8in and 6mm endmills from TTB and have worked perfectly for both aluminum and polycarbonate.
Because they are single flute endmills we use higher rpm’s around 12k or more. Also the for the feed rate we use something from 500-900 mm/m depending on the Endmill and have gotten pretty good results
You’d really need to be able to see it in action to know exactly what the issue is. But you could try upping the feed rate - go too slow, and it tends to melt. Also depending on exactly what you’re doing, you might want to add some air to help clear out the chips. When cutting out deep polycarb (we did some parts out of 1/2" today), the chips can easily get stuck in the path, meaning they get caught up in the next step, and the next one, etc, and can cause problems.
I’m not sure what our speeds and feeds are (we set them up in our tools library a couple of years ago, so we just pick the right tool), but I could get that at the meeting on Monday if I remember. From the linked instagram post, you can see that the parts come out pristine, although we do a fair amount of manual air to help clear the chips (we really need to spend some time getting air and misting set up on that thing…)
We use 4 mm single flute. 20-24 K rpm. 45 in/min feed. 3 mm DOC. Lots air to keep the chips blown out of the cut.
Others are more aggressive. Take some test cuts and do what works for you
Use the thrifty bot or west coast cutters
WCP-1517
I like the 1/8” cutters because it gets in tighter corners
Max RPM (mine does 24k) and usually around 50-100 IPM. You could go faster but you run into work holding limits.
We go .18” deep (our polycarbonate sheets are typically that thick). You could probably go over .25” thick
6 - 10 degree helix/ramp. Honestly you really don’t even need to ramp, but I like how it slowly reduces cut force before the part is fully cut so it doesn’t fling it
No coolant
Just to share another set of feeds and speeds for polycarbonate. We have a ShopBot and use bits from Onsrud. Here are the two that we use most often:
We use the 1/8” bits from TTB and 1800mm/min @ 18,000 RPM 1.5mm step down.
For CNCing Polycarbonate, we generally use these settings:
1/4" Single-Flute Endmill: 0.1"-0.14" Depth of Cut, 18,000 RPM, 100 inch/min
1/8" Single-Flute Endmill: 0.8"-0.1" Depth of Cut, 22,000 RPM, 75 inch/min
1/8-1/4" Drill (drilling operations only): 9000 RPM, 10 inch/min plunge
While it seems counterintuitive, it’s actually possible to cut polycarbonate too slow, which results in the piece heating up and melting. The trick is to find the right balance of RPM and feedrate for your machine.
Other general rules:
Note that using endmills with more flutes or running on a machine not capable of the RPMs I listed above will require you to reduce your feedrates and/or depth of cut accordingly.
This is probably from a too-low spindle speed. A higher RPM will give you a clean cut versus scooping away partly melted plastic. For my own setup I use 19000 but you can safely go higher than that.
With single flute Huhao 4mmx12mm bits, we typically run around 24krpm at 100ipm full depth of cut on our Omio, up to 1/4" polycarb. Bore angle 30 degrees or so. If you’re spinning fast you gotta feed fast. If your machine isn’t rigid enough to feed fast you gotta slow down the spindle speed.
Just to better explain the whole “up your feedrate” thing, with something like polycarb, the amount of effort it takes for the cutter to actually make the chip is much lower than with metal. Having a thicker chip (from running higher feedrates) actually makes the chip heavier, and the heavier chip is usually able to be evacuated away from the part much better than thinner ones, which tend to get stuck in the cut and gum up the cutting action.
This increase in chip evacuation is one of the main benefits of increasing your feedrate for polycarb cutting.
If you’re melting the edges, then the feed rate needs to be increased, and possibly decrease the speed of the spindle if it’s on the high end currently. This happens when the cutter is spinning, imparting heat into the part, but staying in the same place too long, and transmitting too much heat. You stop cutting and you start pushing through melted plastic instead. You can and should cut polycarb surprisingly fast, and if the feed rate is higher, it will move on before the material gets too much heat transfer.
I’m not a machinist at all, but we found feed rates similar to that much too slow. See: CNC Routers for FRC Robotics - #617 by Max_Morehead It’s interesting that you suggest it though, because, we got the 15000k spindle speed and 30in/min feed (used in the video in that thread) from a 1678 document posted in the thread, so I don’t know what is causing the discrepancy.
We used 4mm single flute cutters at 100 in/min and 15000k spindle speed last year with success (1/4" DOC).
Definitely on the slow side of things. Better to start there and work up. I have not had a problem with melting. But I am using an air jet with a goodly amount of air.
Hi we just got our first CNC but only ordered 4flute bits what would be the appropriate spindle speed and feed rate for 1/8in polycarb? I appreciate it.
Polycarb works really well with high feed rate and rpm. We run 24k rpm, 4mm bit single flute, .25 doc, 100 ipm
I recommend single flute for routers. 4 Flute will work but it’ll get clogged easier than a single flute
TTB and WCP have a bunch of single flute cutters
We use this 1678 CNC Tool Database - Google Sheets
One minor tip I can add is to make sure your work holding is really good. Especially for eighth inch poly or large sheets and if you are using an up-cut endmill. Early on we had material get pulled upwards by the bit resulting in either a rough edge or the part snapping off.
Otherwise I agree with a lot of what has already been said.
This probably isn’t the correct way to do it, but as a general rule for a given Feed rate you can divide the single-flute RPM by the number of flutes on your cutter and you’ll get something that roughly works (though you may need to adjust if you start melting poly).
So for instance if you take the speeds and feeds I posted above…
1/4" Single-Flute Endmill: 0.1"-0.14" Depth of Cut, 18,000 RPM, 100 inch/min
1/8" Single-Flute Endmill: 0.8"-0.1" Depth of Cut, 22,000 RPM, 75 inch/min
… and divide them by four flutes, you would get:
1/4" Single-Flute Endmill: 0.1"-0.14" Depth of Cut, 4,500 RPM, 100 inch/min
1/8" Single-Flute Endmill: 0.8"-0.1" Depth of Cut, 5,500 RPM, 75 inch/min
The issue of course with doing this is that most routers don’t go down this slow (or if they do they often have significantly lower power). As a result you may have to increase your feed rate to compensate for the slower speed (otherwise you’ll get a lot of heat build-up). What you’re targeting is a “Feed per Tooth” range (a number which is raised by lowering RPM and raising feedrate, or vice-versa).
That being said, you may also want to reduce your depth of cut to prevent excess chip loading on the endmill, and having air running on the cutter never hurts either. Long term I would still STRONGLY recommend getting some 1 or 2 flute endmills, I wouldn’t recommend using 4 flute even for aluminum (they’re really meant for harder materials like steel, generally).