I have designed part of a jig that has to be thick transparent cast acrylic. (.708 x 12” x 24”) Thickness is the closest availability to 3/4”, so that’s what I have to live with.
I have zero experience when it comes to machining this material. I know I have to use specialized 1-fluted router bits.
I need to know how to handle machining these specific features:
Countersink holes for Phillips flat head screws. Do I just cut a thru hole and then use a counterbore tool with a hand-drill or drill press? Or will a V-Bit be sufficient if I can match the screw head angle?
Profile routing outline of part. I presume it would be the standard 1-flute bit to do this?
Dovetail groove? Yikes! Can this even be achieved in acrylic? If so, I would have to hog out a channel to complete depth and width of shank prior to using a dovetail bit. Will it crack?
I did a simple contour cut on cast acrylic all of one time. I didn’t order a special bit but used a 2-flute 0.25” downcut bit at 70 ipm with 0.0625” step-downs plus a full-height finishing pass. The important thing for contours, IIRC, is to ramp in and ramp between step-downs. My ramp angle was 3 deg. No idea if these values are good ones, but they worked. I sanded the edge after. I didn’t try flame polishing. Sorry I can’t offer any info for the drilling and dovetailing.
I did one acrylic project too, and I’ll add my tiny advice: you want the bit to be moving fast and cutting shallow so the plastic has no time to heat up, and so the bit is definitely cutting a chip and not just rubbing. I kept an air hose aimed at the bit the whole time to avoid chip packing. My bit was a 1/8” single flute O-bit.
With any plastic, the #1 thing is to keep it cool. Use an air nozzle on it if you have one, and do NOT use downcut bits (I have made some horrific messes with those), you gotta get the chips out quick.
Use sharp bits and keep it moving. I’ve used regular two flute upcut bits, and good Vbits (I use the Amana ones) work well for counter sinks and chamfers.
I have not done dovetail bits, but I suspect that would be a hot guey mess.
Makes sense. I didn’t have good workholding and would have had chattering with an upcut. The test cut turned out fine, so I went ahead with it. I did use compressed air to clear chips. Probably if I had increased the feed rate or step-downs, I would have had issues with clearing chips, and on the other side I would have had issues with heat. My feeds & speeds probably weren’t great for bit longevity, but mine was just a single cut.
I think it would depend on the dimensions. A wider groove would give you room to take lateral steps with the dovetail bit. If the groove is tight to the dovetail bit, then I agree with Jim, you’ll probably have issues. For one, cutting both sides means one side would be a conventional cut, pushing chips into the bit’s path. Even a little extra width would help with that. Either way, you could try removing material with a second dovetail bit that’s either narrower or has a steeper angle before moving to your final bit.
It sounds like a catch-22 scenario. Damned if you do, damned if you don’t. Hope for the best, expect the worse. I hope I get this right because the material cost a little over $100!
Good information! As long as I stick with the same 14 degree dovetail bit, this might work. Wait!
It JUST occurred to me a method which might work. My final dovetail groove would be for a 1/2 x 14 degree and 3/8” deep. (This is for the MicroJig dovetail clamps). Therefore, if I channel out a groove with an upcut bit to a dimension that is identical or a little wider than the intersecting diameter (where the angle meets the top surface) of the 1/2 x 14 dovetail, then I could use a 3/8 x 14 degree dovetail bit and cut only ONE SIDE AT A TIME, with incremental jogs to carefully nip away. And then repeat for the other side. I’m going to do a physical cross section layout and see if I can detect any problems before attempting this. And it would help with knowing how to create the toolpaths in Vcarve as well.
What do you think about this method? Think it would work?
I may have to buy extra material to test this out.
***If this does not work, I could probably pocket a groove much wider and deeper and then epoxy a wooden piece that has the final size for the clamp? Last resort though.
I do a fair amount of cast acrylic and HDPE. For cast acrylic use an o flute bit. I cut at 12,000-14,000, 120 in/min 1/4” doc with a 1/4” bit. If you need a fine finish use a 3 flute high helix bit and taking about .015” up to 3/8 doc on a profile cut on these I run 18,000 rpm. I also run my vac to keep the chips out.
Perfect timing! I’ll be starting this project sometime this week. I’ll take your information into great consideration and will adjust my tool database and toolpaths accordingly. Thank you!
When I used to run a lot of HDPE I did similar feeds and speeds. On my setup I was doing 300 IPM at 20k RPM, which if you scale up your 120@14k roughly matches.
I did a lot of acrylic too, but it was thinner sheets with vacuum hold down. I was always limited by hold down and not the max feed and speed I could go…
Hope for the best, expect the worse. I hope I get this right because the material cost a little over $100! 