Melting Lexan like the pros

Well, I just melted a big glob of polycarbonate onto one of my .0625" flat end mills. I used Carbide Auto Toolpath for Plastic - Polycarbonate in MeshCAM on a piece that required milling some stock away.

Here’s what my endmill looks like:

A couple of questions:

  1. Is there a good way to salvage this end mill?

  2. Could this have been avoided? One thing that has confused me so far is that the spindle speed seems to be associated with the tool definition in MeshCAM, and not the material. I would think you would want different spindle speeds based on material, feedrate, chipload etc.



i think PC hates alcohol so soak it and see what happens.

Take a pair of nippers and start chomping away at the plastic. Usually it’ll fracture off after a couple attempts. That’s always worked for me. Failing that, I’d try light application of a heat gun and then twisting the blob in the direction of rotation of the flutes.

I’ve had decent luck with 2 or “O”/single flute end mills and shallow passes with PC.

Thanks guys. Once I split the melted part with side cutters, it just broke away from the tool. What was left were a bunch of stringy lexan chips which had wrapped themselves around the flutes. Cleaned those off and it’s as good as new.

Glad you got the PC off without difficulty—as a general rule most plastics prefer to stick to themselves more than the metal of a tool, especially once the tool is cool. Therefore once you get them started they’ll come off pretty cleanly. Also, almost all thermoplastics will expand/contract a good bit more than the metal of the tool will, and as an added bonus most are much more brittle when cold, so you may also want to try chilling the tool before trying to knock the welded plastic off.

I’m in agreement with you that feed-rates and chip-loads need to be factored in on a per-material basis in addition to being calculated per tool, and this has cropped up elsewhere in the forum as a suggestion—so I’m considering your experience here as an “up-vote” for that.

Regarding how to avoid this in the future—compared to materials like wood or renshape (a thermoset plastic), thermoplastics like Acrylic,Nylon and PC need a higher chip-removal rate to help pull the heat of cutting away from the tool in order to prevent the plastic from melting and welding itself to the tool, which then prevents future cutting, which then leads to even more plastic welding… which leads to what you have shown us here!

Here’s a resource that may help: the basic values in the HSMworks documentation.

And also, here’s an online calculator from Monster Tool for feeds and speeds :wink:

For the 1/8" tools cutting in Polycarbonate, you’ll want to have a chip-load of 0.002-0.005", or 0.002–0.003" for the 1/16" tool, so using the chip-load formula that means you’d have a feed-rate of 40-80ipm at 10krpm, or at 5krpm you’d have a feed-rate of 20-40ipm, which should depend on if you’re roughing or finishing, and if you’re more concerned about fracturing the plastic or melting it.

I haven’t cut polycarbonate on my Nomad yet, but once I do, I’ll be sure to post my “fine-tuning” and I’d invite others to do so as well!

Thanks @UnionNine – I really appreciate you taking the time to share your experience on this forum. I’ve learned a lot from reading your comments!

Glad to help :relaxed:

I learned what I know from stuff others posted before me (which I reference all over the place) so now it’s your turn to continue the virtuous sharing of tips! :wink:


Your info in this thread regarding cutting acrylic was very helpful.

I am wondering if you Have had a chance to cut some Acrylic and do a little ‘fine tuning’ as noted above. If so what feeds and speeds did you find worked well for the standard Carbide3d cutters?

Sure have, sorry for not getting back to this sooner—for the .063" tools you want to run them with a fairly aggressive chip-load.

Looking back at what I ran the truck-panel job at, it was:

.063" flat end mill:
Spindle: 8krpm
Feedrate: 650mm/min
chipload per tooth: ~0.040mm
Lead-in feed: 250mm/min
Lead-out feed: 250mm/min
Ramp feed: 200mm/min
Plunge: 101.6mm/min

Also, for a 0.5mm flat endmill:
Spindle: 9krpm
Feedrate: 144mm/min
chipload per tooth: 0.008mm
Lead-in feed: 120mm/min
Lead-out feed: 120mm/min
Ramp feed: 100mm/min
Plunge: 40mm/min

I’m not 100% that this was the final files used, so it may have adjusted slightly from there, so be sure to watch the job a bit to make sure you’re happy with it.


What was the depth of cut, how much did you take off in each pass?

Good questions, should have included that previously. I generally stick to a 1:1 depth by diameter ratio, so in this case maximum roughing step-downs were .063" and finishing-step downs were .0325", on the .63" flat end mill, and the 0.5mm flat end mill I was a bit gentler on with 0.3mm step-downs and 0.1mm finish step-downs.

I have been cutting polycarb for 30 years and have tried a lot of different cutters and cutting speeds and feeds for the different cutters. Some of the most expensive cutters suposedly made for cutting polycarbonate or recomended by the tool manufacturers for polycarb did the worst job. about 2 years ago I came across a cutter that I would highly recomend. To my surprise it isn’t an expensive one at all. It is a 3 flute endmill with a ZrN coating. The first one I bought was an Accupro from MSC. Since I have found that promax and Rushmore also make them with the ZrN coating. The Promax and Rushmore work well but not as well as the Acupro when it comes to the finish. the grind on the Acupro is a little more pollished. I run them at 900-1200sfm with a chip load of .002" per tooth and a finish pass of .010" 1200sfm .001"per minute 1/2" cutter. The finish I get is see through and the best I hve ever gotten with any other cutter