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:)

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.

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.

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

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

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

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

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.

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.

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.

So how did it cut with those feeds and speeds?

AC

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

Using sharp 1... 2 flute 2...6mm endmills will help. And Coolant! Last half of year I cut what ever with coolant ONLY, speed ca 30k RPM.
Herbert

I have a spritzer bottle....Would that work?

Not trying to be fresh, I just have a low budget right now

I have a spritzer bottle....Would that work?

Not trying to be fresh, I just have a low budget right now
You will be very tired to spitz water by handy. Small pump does not cost much - search eBay *mini water pump* or go to local scrap store and take it out from some car. Simpe PWM controller (or just variable power supply) few meters of silicone hose - thats all you need.
Herbert

Any little electric pump motor, even from a little desktop fountain or fish tank circulator or similar. Cheap little pump motors can be found new for only a two or three bucks. Almost anything will do in a pinch that will deliver more than a spray bottle, and do so a constant stream. Poke a small hole in the side of a plastic water bottle if you need to and direct the stream that way, its still less trouble to refill before every cut than pumping a manual spray bottle all day!

Or cut the bottom out of a large plastic bottle.

Put a cork in the top with a length of tube inserted in a hole through it.

Hang the thing upside down a few feet above the machine, fill with coolant and let gravity do the work.

Good ideas.

I tried 3/16" diameter bit at 50 IPM and .1" deep. Made some nice chips.

On the longer cuts vibrations started to get scary, but the part came out:)

I cut plastics all the time. MANY MANY MANY thousands acrylic windows for security cameras. The trick with acrylic is to GO FAST!!! In Any condition the heat needs to go out with the chips otherwise it melts. Keep air blowing all the chips out. What'll happen is the chips load up and you're cutting the melted chips along with clean acrylic. Though I use a machine at about 300 IPM at 20kRPM and a vacuum table. the best cutter I've ever used for acrylic is a 3/8 3 flute solid carbide endmilll from Onsrud. (sorry don't know the number off the top of my head.) I will take a single pass up to 3/8 thick and a full depth finish cut of about .01. Another thing to avoid is plunging right in to the material. If you can give yourself a good entry in the air. Acrylic is just tough to cut slow. It melts right behind itself. If I have to cut slow I'll use a straight single flute o-cut bit. It keeps the chips big to carry out the heat. Just remember in all your experimenting keep the chips out!

Hopefully this helps.

While I have not started cutting it yet. All of my research shows that the Onsrud O flute spirals are the best all around bit for this.

https://www.onsrud.com/xdoc/plastics

https://www.onsrud.com/oc/pdf/O_Flute_Plastics_Brochure.pdf