Using a 1/16th" O flute Amana Spektra (51441-K) to cut 1/8" acrylic. Running at suggested feeds and speeds of 60 in/min at 18K RPM with a 1/16th" depth of cut. I get like 2min of runtime before the bit is coated in melted plastic and starts destroying my workpiece. Is there something I’m missing?
The chips aren’t fully getting cleared. I can see stringers sticking to the bit, and it just keeps accumulating. Maybe I should be using high pressure air assist? If so, any suggestions? Target CFMs etc?
Ugh. I never thought acrylic would wind up being the most difficult material for me to cut.
General advice. Feed faster.
I run at 3200mm/min with an 1/8" single flute. I’d probably start at least 2500mm/min (100in/min) with that endmill, but I’m sure it’ll handle faster.
Reduce the DOC with the 1/16".
Interesting. I’ll take a look at these. Thanks! Fairly sure it’s extruded (for one, it doesn’t say). Didn’t know to look for that, guess it’s like the mistake I made buying undefined brass alloys my CNC can’t cut well.
Cool! I’ll try that. This is the first non-cheap bit I’ve used, so I was a bit afraid of snapping it feeding too fast. Amana suggested 35-70 IPM @18K RPM for acrylic for this bit and a 1x diameter for DOC, but it def. feels like I could do a much faster feed.
If I reduce the DOC, that’s going to be more doable. I could cut the DOC in half, then split the cuts into two passes, so I cut to half the desired depth in the first pass for the entire piece, then finish with a follow up pass that cuts all the way thru. These are small 1x1cm cutouts, so maybe not good to spend too much time in one area cutting for too long? Or maybe I’m overthinking it.
If I blow thru $30 worth of acrylic figuring it out, it’s worth it. Thanks for the suggestions!
Generally… Cast acrylic has a paper cover and extruded has a thin plastic cover. Cast acrylic is much better for cutting on a CNC. I cut cast acrylic at 120 IPM with a slower rpm using a .125 0 flute bit. On a .125 thick sheet I do two passes. I cut it every week with no melting. These are some room numbers cut out of white and black cast acrylic.
Nice! Those looks great! Yeah, no paper cover, just the normal plastic stuff (which I removed from the top layer to avoid gumming up the bit). I didn’t have regular dish soap, but I did have some viscous cutting fluid I use for AL, so I tried that. Totally helped, so thanks for that!
I also ran it at 100 IPM @18K and slashed the DOC to 1/32". I still had stringers that would collect, but they were fewer and far between. It also gave me time to pause the machine, turn the spindle off, clean the bit, apply cutting fluid to it, then resume. When I ran the outer cutout, I did it one pass, and I didn’t have to stop the machine once, so I’m guessing the longer the time between the point the initial cut is made and when the bit passes it again, the better.
The pic doesn’t do justice to how nice the cut is (wood from the spoil board, reflections, etc. on clear acrylic), but it turned out perfect! Still not something I can just run and walk away from, but it’s a very nice cut on par with the AL I normally do.
