Anyone milling plastic?

[oxford]

I just tried my first cut today and smashed the bit with too high a feedrate.

I am milling acrylic with a 1/8" end mill.

I used a less than scientific approach and reasoned 1/4 depth cuts would not be too much.

Now I am thinking 1/64"

or is that too conservative?

Thanks

[Stepper Monkey]

What was the rpm and feedrate? More importantly, how many flutes did the bit have and was coolant used? You can actually get pretty aggressive if you experiment with it a bit and can manage to clear all the chip you are creating. Feedrate isn't usually the issue, either loading or remelt is what usually breaks the most bits.

[Rustybolt]

What stepper said and to add cutters should be razor sharp. People run into problems when the cutting is dull and the material is melted rather than cut.

[oxford]

I have a router that does 30,000rpm

20"/min

2-flutes, new end mill 1/8"

My coolant system right now is a spray bottle:P

[Alex_Cole]

I would think at those speeds you are most likley melting the material. I think you would want to keep your chipload at about .0025 to start testing at. I don't know what the diameter of your tool is and this also will have an effect on feeds and speeds but here is a generic approach.

So we take .0025 Feed per tooth. times number of flutes = .005 X 30000 rpm give you a feed rate of 150 Inches per min.

If your machine cannot go that fast you may be able to get away with lighter cuts but with that high spindle speed it will be hard not to melt it.

Hope this helps
AC

[oxford]

Thanks.

The equation helps.

I can hit about 65in/min before I start skipping steps.

Looks like I will have to burn off the plastic a little at a time:P

[teamtexas]

You could try a different type of plastic. ABS machines much cleaner. I use it all the time and cut with a .250 end mill @ about 30 ipm to a cut depth of .260.

Dan

[Stepper Monkey]

Sounds like a first solution is to go from a two-flute to a single flute bit - the IPM needed is then obviously cut in half, which starts to put it very near the range of what you are looking at your machine being able to do.

Also, unless a 1/8" bit is the max size you can use due to slotting or whatever, if you can also get away with slightly bigger bit like a 3/16" or 1/4" it would be better. This changes the SFM, therefore allowing you to also use a slower IPM. In doing so you are then decreasing the demand on your overworked steppers, bringing them back from near their maximum, and trading it for increased demand on your router motor which is likely nowhere near its maximum load.

Don't know if you've seen them, but single flute mills look rather like the mutant offspring of a corkscrew and a traditional end mill. It not only decreases the the IPM needed, it also increases the tools capacity for rapid chip clearing, a big win both ways when required to move a lot of material fast as you need to with plastic and MDF.
I don't know who has the best deals or selection on plastic cutting mills, I don't use single flutes often enough to have shopped around much. Onsrud.com is one place for serious quality and selection, but Ebay dealers have basic crappy Chinese ones to practice with if you want until you learn to stop breaking tools! The router forum guys should have a pretty good handle on more sources for single flutes, so you might want to do a search on here and see if it's been covered.

[LeeWay]

I cut polycarbonate all the time on my router with no coolant. It does have a higher melt temp than acrylic. I use 2 flute 3/16" carbide cutters and mill from 80 IPM to 150 IPM depending on the profile. Slower around tight curves and slots at 80 and highest in straights and larger curves. My depth of cut is usually .065", but on slots, it's .1". This is using a PC 690 router @ full speed.

I agree that the feed is likely too slow. I would try 50 IPM and as shallow a cut as possible and then increase depth until you get something that looks like what you want. Running it that slow and turning the bit that fast is likely the trouble you are having. It is simply heating up way too much.
You might also try an inexpensive router speed controller and get the speed down to about half of what you are running. Careful that you don't go so slow as to loose torque, but if you are taking shallow cuts like you are, you won't need much of that anyway.

[oxford]

Made my first significant cut today.

Decided to go with 3/16 of an inch diameter bit.

Ran it at 50 IPM 30000RPM

.005" depth cuts

Got 4/5ths done with the piece and then the computer crashed.

LOL

I spent an hour trying to recover four hours of work. Didn't work. Food, a workout, and the idea of doing it again with deeper cuts at .05" have calmed me down.

[Alex_Cole]

So how did it cut with those feeds and speeds?

AC

[oxford]

The cut made little chips that looked like small curled pieces of thread up to a 1/4" long.