Trouble milling acrylic

So I’m trying to cut and etch some cast acrylic, I did a test piece and it worked great, now when I try to do my good piece it seems to be melting and the acrylic is getting stuck to the bit. Don’t know what I’m doing wrong, running the same settings as the test piece. My cut settings are 25in/min, depth is 0.02in per pass, and the speed on the Dewalt 611 is on 2.

Thanks guys

I’m cutting HDPE, which is harder than Acrylic, with the Dewalt 611 set to 1, a feedrate of 3200mm/min, and a DOC of 0.05mm. For the lazy, 3200mm/min is about 126in/min. I think you could easily bump your feed rate way up and keep your router at 1. Honestly, it seems to be an opinion of growing consensus that the 611 can be run with just about any wood or plastic without ever bumping the speed above absolute minimum, which is around 16,000RPM. 3200mm/min is a value I’ve worked up to and I’ve just about gotten rid of any melting. Though, keep in mind your ideal feed rate for Acrylic will likely be different, this should at least go to show you much faster you could reasonably go.

Have you done any stiffening mods?

1 Like

Hi @BobNevalainen looks like you are going to slow on the feed rate and it is melting. Is that a 1 flute bit?

If so try 54inches per minute.

Feed Rate = Spindle speed x chip load x flutes

The Dewalt speeds are: 16,000-27,000rpm

1 Like

Ok I was running it at the recommended speed and feed for cast acrylic. Maybe my bit is dull as well, not sure

A little googling is turning up recommended chiploads of 0.003" - 0.006" on average for soft plastic and 0.002" - 0.004" for hard plastic. So, let’s pick a nice middle ground of 0.004" chipload. Chipload, by the way if you didn’t already know, means the amount of material cut with each “cut” of your bits tooth. So it’s essentially the chip size. Like Zach said, the equation dictates that the Feed Rate = Spindle Speed x Chip Load x Flutes. If you’re using a 1 flute, it simplifies the math. It’s good practice to keep your router set to 1 for a few reasons, the biggest being, in my opinion, that it reduces runout or inaccuracy to have it spinning as slow as possible. So, solving for feed rate then gives us 16,000 * 0.004 = 64ipm. Because I don’t know exactly how hard the plastic you’re machining is, 54ipm is probably a very good first bet with the router set to 1. After that, if you get some melting, don’t be afraid to crank it up even higher.

Bob- I run a shop-vac in blow mode ( hose attached to the exhaust outlet) with a crevice tool attachment blowing directly at the bit as it carves. This keeps the chips clear and cuts down on the melting .

Another tip is to make sure you use an up-cut bit . A downcut bit does not pull the chips away and increases the chances of the molten glob .

I run ~ 60-70 IPM on most cuts.

Full disclosure - My " shop- vac" is actually a craftsman .

+1 @jeffschultz Shallow cuts, fast feedrate, low rpms. I also spritz my bit with wd40. blowing the chips away is a big help.