Cutting Acryclic

[FirstLook37]

I am trying to route a logo into .220 Clear Acrylic.  I am using an .125" End Mill bit and i'm only plunging .09375" into the material. Can anyone give me advice on what my feed rate, spindle speed, etc..etc.. should be in order for me to get a smooth cut? Ive been toying with it but it seems everything i try still comes out poor. The acrylic is basically melting and re hardening where i'm cutting. The edges are coming out not as smooth as I'd like. Acrylic isn't cheap- so I'd like to stop this shoddy work! Please help acrylic masters!

Thanks- Brian

[gadget47]

Greetings,
  I have been playing w/acrylic for a few months and here is my standard parameters- 8-10ipm feedrate,.035- .045 depth of cut on 1/8 or 1/4 2flute endmill (up spiral) or ball nose- & LOW rpm (1-2000). These settings have eliminated (for me) almost all re-welding and tool clogging (I know the rpm is correct when the chips look good). One thing i discovered w/acrylic is the feed rate and the rpm have to be adjusted (minor) for every different  pice of plastic i cut. The mfg state its the slight variations in the formula that causes this.
   I also just started to use an "O" flute bit designed for acrylic (amana tools), i'll have to get back to you after this week-ends projects.
  I don't use a lube or cooler to cut and i know they would help for more agressive cuts (light soapy water and/or cool air injection work good from what i hear)
hope this helps

gadget
arrzeecustom.com

[FirstLook37]

Thanks Gadget47...looking forward to hearing about the Amana Tools bits....I was looking into them as well. please let me know how they work out for you!

[gadget47]

HI Brian,
   My first "O" flute trials went well, i got a smooth clean cut on the plexi- both the bottom (tip) and side left a really smooth finish , before and after the finish cut. As with my other tips i went slow 8-10 ipm feedrate, and .030-.045 at about 2000 (as far as i can hear the rpm-speed control is set low but motor doesnt stall). I ran a project that took 2 hours to cut this way and had no problem at all.
  I also purchased the "in groove" tool holder ans a 60' bit- these work very well (so far). I'm going to buy a few different replacement bits for this tool and a 1/4 O flute bit -im happy with the results

Gadget
arrzeecustom.com

[BruceJ]

HI, what worked well for me for years were very sharp tools, good chip evacuation ( 2 or 3 flute endmills), slower spindle speeds, higher feeds, pre-drill for endmill plunge, and coolant if you can use it.

[tazzydean]

i've been cutting acrylic for years and highly recomed an o flute bit i run  at speeds of between 100 and 140 IPM and an RPM of around 18,000 RPM to key to cutting acrylic is to climb mill  the cut as compaired to conventional cutting, if your gettin  melting  or remelting behind the cut your cuttin gto slow of a feed and over heatingthe acrylic and the cutter. Hope this helps you should be able to do a single pass with a 1/4 inch cutter into at least 3/8 thick and stil get a good cut

[Fastest1]

Water alone works great when machining acrylic. BTW plastic stuck to the endmill is damned hard to get off!

[CoreDeep]

I would like to note it makes a HUGE difference if you're cutting CAST or EXTRUDED acrylic!  Cast cost more, but it chips more nicely, doesn't gum um or stick to the bit and can generally be cut faster.  I'm presently working on a deep sea camera housing and originally began with extruded.  After many moons, I am now using cast and WOW what a difference.  So if you're getting acrylic stuck to your bit ... you're ... well ... obviously melting the acrylic ... a VERY not so desired trait.  This will have to do with the quality of your bit (should be using carbide, not carbide coated) and the quality of your material.  (*scratches head*) Now I have to go look for an answer to MY question ...

Ms. Sterling

[Tweakie.CNC]

Just one more point to note is that you actually have acrylic and not polycarbonate. 

Tweakie.