I think I know what I did wrong, but after ruining two bits, I just want to double check
I got a piece of .21" thick clear acrylic from Home Depot. I am trying to make a light guide for a sign. So, basically 1000 little dots (like etching) AND one profile cut to just cut out the shape.
Dots are fine, that was just a .005 cut depth to simulate etching.
The profile cut, as it got deeper, the acrylic started to cake up on bit, where it went from 1/16th to the wider 1/4th shank. Which then started spinning against the top of the acrylic itself mucking it up. When the cut was done, it had fused back together in parts. And while trying to clean off the bit, it broke it
Things I think I did wrong:
The Acrylic was extruded not cast. A few other smaller projects I have done with acrylic have all been cast, albeit much thinner, and have cut like butter just fine. I am hopeful it being extruded was a good portion of my problem.
The small size of my bit, 1/16th, didn’t leave enough room for chip evacuation, and the dust boot wasn’t effective enough to suck it out, and the chips just melted an fused together.
I may have also been going to slow in the IPM category. I did try speeding it up mid way after the problem started, but at that point it was a mess.
I am reading a lot of people using shallower Depth of Cut, I was just using the recommended from Amana for the cutter, which is equal do the cutter width, so .0625. I have seen folks say .002.
Thinking of chip load, the recommended was 35 IPM, .0625 Doc, 18k RPM was supposed to give a chip load of .002.
Part of me wonders if I just paused the machine and cleaned out the profile cut I could have avoided the mess.
Any feedback?
PS - How does one effectively clean off melted Acrylic from a bit?
Welcome to the community, and happy to see you have clearly done your homework!
True (about the difference), but you should still be able to cut both with the right cutting params.
more likely it was a combination of going a bit too slow (see next point) and slotting too deep, which aggravated the issue due to limited chip clearing indeed.
Possibly, but a 0.002" chipload on a 1/16" endmill in acrylic is not unreasonable in my book. I think the DOC might have been a bit too much to minimize risks of chip recutting. When in doubt, in acrylic I try to go shallower AND feed faster, and that usually works out for the best.
The manufacturers recommendation tend to not apply as is to a Shapeoko, and specifically about depth of cut. 100% of the tool diameter is a bit much as far as I am concerned, I usually tend to stay under 50%D (as a starting point at least)
Possibly, but you would just have postponed the problem to a later (unpredictable) time
I have read your guide and a bunch of your posts! I feel special you responded, thank you!
Thank you for the advice. One thing I haven’t fully grasped yet is the relation to Chipload and Depth of Cut. My head says they would be directly related. So, your advice to go shallower in DOC but Faster IPM, is to maintain the .002" shipload correct?
Is it just that the manufacture gives a Chipload rating based on their default DOC? If they are related, then it is just simple math to change either RPM or IPM to maintain the ideal Chipload correct?
Lastly, is the ideal Chipload, just derived from trial and error mainly? I am thinking of the soft plastics, soft wood/hard plastics, hard wood chart that had Chipload ranges from your guide.
That’s probably because there is no direct link between the two. Conveniently I commented on this earlier today here, let me know if that clears things up a bit?
Chipload = feedrate / (RPM x nb of flutes)
and that’s about it. DOC you set almost independently
Chipload guidelines are like religions, there are many and you can pick one, or none.
The chipload guideline I mentioned in the ebook is derived from this loooooooong thread, it is crowdsourced if you will, and then I tried to back it with my own experimentation.
So, basically Chipload is essentially chip “thickness”? Depth of Cut impacts the chip “length”. I feel like these things could have been named more clearly lol. (Specifically Chipload = Chip thickness)
For DOC, if my setup has enough power/rigidity/strength, I could have more aggressive DOC without adjusting other settings (in theory). But for my particular issue with Acrylic, being partly chip evacuation, shorter chips form shallower cuts would be easier to evacuate out of the channel.
Essentially yes. If we are being pedantic, “chipload” is the chip thickness at 50% stepover or more, while “chip thickness” is the actual max thickness of the chip after taking chip thinning into account (confused yet ? )
Yes, but no one hardly ever speaks about chip “length” because it’s mostly irrelevant to the quality of the cut.
Exactly.
That would be my guess about what happened, possibly combined with a feedrate that was a tad too slow. I went back and checked some of my settings back when I was doing tests cuts in acrylic using a 1/8" O-flute:
At that time I ended up using 16k RPM, 54ipm. But that was a stiffer 1/8" than your 1/16" endmill.
Maybe 40-45ipm @18K would improve the cut in your case (but don’t go breakings bits just to prove me wrong
)