Plastic machining on a CNC router.

[Chris Flint Two Ft Pty Ltd]

Hi All,

I got a bit of an interesting job today, ( first time) to machine a large sign out of 5mm FOAMALUX produced by Brett Martin company.

I followed the feeds and speeds on their website to the letter and after a few tools had broken and I had melted the cut material back into the groove, slowed down the feed.VIS: 3/16 upcut 2 flute solid carbide, 18000 rpm feed reduced to 1000mm per minute, and used compressed air to blow on the tool the whole time, eventually got the job done.

Here are the questions:

1. What tools should I have used.

2. Do I need air for cooling or was this just an incorrect tool choice.

3. I have an opportunity to do a lot of this including machining ABS what should I be doing to get, a) a faster cut, the above took ages, and a clean finish.

thanks in advance.

chris f

[Jacob]

What kind of router do you use? I work with KOMO.

Actually, for contour cut I usually use 6mm 1 flute solid carbide strait cutter at 18000 rpm and 2000 mm/min. About cooling: of course, use air! Also use depth cuts, it may be good

Jacob,

Router programmer

[email protected] - private

[email protected] - work

[Mike@Dive Lab Inc.]

there is a company called Onsrud that makes tools for that kind of application. I have never used them, check MSC page 525

[crazy^millman]

ABS will cut alot different than that stuff. I have cut abs at 24000 rpms and 600 ipm with no problem using regular endmills for alum and air blast. Depth of cut is your friend and your enemy. To deep chip has no where to go but back into the cut if it does that then you got rubbing then you got melting. Go high on your chip load per tooth the smaller the more problems. If the machine does not have the feed capability then back down the spindle to meet .007" to .02" per tooth feed when roughing on plastics if they are not too brittle but if you keep the depth of cut right most time does not matter. All plastics cut different so what work on one may completly suck on another so experiment, keep mental note or a note book so when you come across it again you dont go know what the hell did I do last time.

 

HTH

[TyK]

I program and machine a fair bit of acrylic and plastic. We sourced tooling specifically for this. We came across a bit from Onsrud called an o-flute. Its a single flute upcut, carbide, and it does an excellent job. We also found that it needs to have a fairly high feed rate, like 8-11 m/min @18000rpm based on depth of cut.