Cutting Acrylic? some help?

Talk about all things CNC
Post Reply
awesomename
Posts: 40
Joined: Tue Mar 04, 2014 11:49 pm

Cutting Acrylic? some help?

Post by awesomename » Mon Apr 21, 2014 5:30 am

I'm going to be cutting some pieces out of 1/4in thick Cast Clear acrylic sheet. I plan on using a 3 or 4 flute 1/8in straight endmill.

I have the DNP611 spindle I can spin anywhere from 16k to 26k RPM. Can you guys suggest some feeds and rpm speeds? As wel as the depth of cut per pass?

Thanks fellas. :D

WillAdams
Posts: 8489
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Cutting Acrylic? some help?

Post by WillAdams » Mon Apr 21, 2014 10:09 am

Here's what we have so far: http://www.shapeoko.com/wiki/index.php/ ... ls#Acrylic

and I did a quick search and added some additional references / notes.
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

TDA
Posts: 31
Joined: Wed Dec 18, 2013 11:14 pm

Re: Cutting Acrylic? some help?

Post by TDA » Mon Apr 21, 2014 4:34 pm

When cutting plastics you really need to keep your chipload up. This is due to the cut material being what keeps the tool cool. Too little chipload and you will melt the plastics. For this reason you typically don't want to use more than 2 flutes for cutting soft plastics. There are exceptions where very high feed or low RPM can be used.

Also, if you haven't got your acrylic yet try to get cast material and not extruded. An easy way to tell (most of the time) is that cast will have a paper protective film and extruded will have plastic. Cast material is MUCH easier to cut.

I would start at your lowest RPM and for a starting feed go at least 1IPM per RPM per flute (e.g. 16K RPM, 2 flute 32IPM). This would be the bare minimum but still watch for melting. Typically your best feed/speed will be much higher but this depends on the tool geometry. One thing to look for is you should have decent sized chips coming out of the cut. If you are getting really fine hair like swarf or melting increase you feed or reduce your RPM.

Let me know if I can be of help.
John Torrez
Think & Tinker / PreciseBits

danimal
Posts: 332
Joined: Wed Mar 13, 2013 5:53 pm
Location: Colorado

Re: Cutting Acrylic? some help?

Post by danimal » Mon Apr 21, 2014 6:36 pm

From my experience, running the variable speed routers at their slowest speed is hard on them for anything other than short duration jobs. They are fan cooled and get a little too hot running that slow under load.

Feed speed(in/min) = RPM x Chip Load(in/rev/flute) x Number of flutes

Chip load is determined by the mill manufacturer based on the geometry of the end mill and the material being milled. Most manufactures have very little information for plastics because the end mills are designed for metal. The best that you can do estimate using aluminum chip load information. Also as you can see by the equation above the number of flutes that you have literally doubles or triples your optimal feed speed. You will get the best results using at most a double flute, but better yet a single flute. Most 1/8" end mills list .001 to .003 for chip load values so at 16K RPM you are looking at a feed speed of 48 IPM (best case 3 flutes) to 192 IPM (worst case at 16K RPM 4 flutes). Most 1/8" end mills are only rated for a maximum of 80 to 100 IPM per their manufacturer documentation, but even heavily modified Shapeokos will not drive a spindle any where near that fast without missing steps.
Shapeoko # 1458

RT0701C Spindle || dual y motor || x axis nema23 with custom carriage 1000mm length || z axis nema23 linear rail upgrade with 1/2-10 ACME

Post Reply