Breaking Small Diameter Acrylic Cutting Bits

I am using the Shapeoko Pro XXL while trying to use a 1/16" O flute 1/4" shank bit to make pocket cuts of different fonts into acrylic without much luck. Even after using an 1/8" O flute for clearing cuts and using recommended speeds and feedrates the bits keep breaking.

For instances I have been using the Astra Coated* Bits&Bits 1/16" ‘O’ Flute Up-Cut Spiral Bit – 1/4" Shank (425-UP062) at 18000 RPM with a plunge rate of 30 and feed rate of 60 IPM with a cutting depth of .0625 (these are recommended on Bits and Bits website) and I have broken 3 bits even tho I have tried adjusting the plunge and feed rates.

Additionally, I have also broken 3 Amana Tool 51441-K Spektra Coated SC Spiral O Single Flute, Plastic Cutting 1/16 D x 1/4 CH x 1/4 SHK x 2 Inch Long Up-Cut CNC Router Bit while using it’s recommended plunge, RPM and feed rates from the Toolstoday website.

Obviously, something is wrong. Either I am completely in the dark when it comes to cutting acrylic as far as setting the correct speeds and feeds, the bits themselves are defective or perhaps I am not using Carbide Create incorrectly while setting toolpaths. For example, does Carbide Create have the ability to adjust ramp plunge rates?

I need help (yes, my wife has been telling me that for years!) - ANY SUGGESTIONS OR HELP would be greatly appreciated. (BTW and in case you couldn’t tell, I am a novice when it comes to using a CNC and it’s associated software.)

There’s a bit on calculating feeds and speeds at:

and @wmoy has some videos on single flute tooling and acrylic at:

A few general comments:

  • Before the endmills break, are you getting nice little chips, or a stringy mess ? If you don’t get chips, you are probably not feeding fast enough. If you do get chips, you may be feeding a tad too fast and taking a too large chipload. 60ipm at 18000RPM is .0033" chipload, which is a great value for 1/4" single flute, but may be a bit too much for a 1/8"and more so for a 1/16" in acrylic. A 0.0015" chipload should work, have you tried halving the feedrate ?
  • the depth per pass of 0.0625" is 100% of the endmill diameter, which I know is a common recommendation on tool manufacturers sites but…50% or less is known to be a safer working zone for us casual users, or at least a better starting point. Breaking endmills happens when too much lateral force is put on the tool, either because the flutes get clogged by melted material or from packed chips, or because of excessive deflection when there is a lot of axial engagement of the tool in the material. Reducing the depth per pass is a sure way to minimize both risks.
  • have you checked runout of your router ? It’s not easy if you don’t have a test indicator on hand, but it’s one of those things that don’t matter much on large tools, but become critical for micro-machining, and 1/16th is borderline micromachining.
  • if the tool break immediately upon entering the material, you may not been plunging fast enough. This is quite counter-intuitive since we are told that endmills make for poor drills and should plunge very slowly, well plastics are the exception: if you don’t plunge fast enough, while entering the stock melting can happen, which is likely to leave a small amount of melted plastic in the flute, and then bad things happen. 50% of the feedrate is my go to rule for plunging in plastics.

Great information! I have had endmill break as soon as enterering the material, but for the most part I have noticed that bit creates a stringy mess and material is melted on the bit itself before the bits breaks. With the information you provided, I have a much better understanding of what is going on - A BIG THANK YOU!

1 Like

Thank you for the information and link. I guess there is more to know about using a CNC and bits then just putting a bit in and starting the milling process. The realization that I have to put more work into researching and understanding this whole process is beginning to sink in.

1 Like

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.