We use cookies to personalize content, interact with our analytics companies, advertising networks and cooperatives, and demographic companies, provide social media features, and to analyze our traffic. Our social media, advertising and analytics partners may combine it with other information that you’ve provided to them or that they’ve collected from your use of their services. Learn more.
Acrylic is hard to cut! I’ve mainly been working on clear acrylic.
So far, I’ve had the best results using the straight 2 flute bit (the one sold here on Inventables and included in my End Mill Starter set) at a feed rate of 40in/min, 0.02" deep passes.
This works great up until about 3/16" deep, when there begins to be a lot of material against the bit that isn’t being cut…just rubbing and generating heat. Then things start to get a bit melty. Small gobs of molten acrylic travel up the bit, fouling the nicely cut surfaces in the upper layers, before being flung across the room in every direction.
Any tips to get good cuts in 1/4" acrylic? I don’t know if I should be focusing on the bit, feed rate, depth, or technique.
@SpencerShepard other than @Zach_Kaplan’s advice you may want to look at a better way of chip clearance. A vacuum and vigilance, or better yet tool paths that only cut on one side with the width of the chanel being cut and leaving room for the clearing of chips…
Here is something similar to what I was trying to describe. He’s talking about aluminum, but I think it could apply to acrylic as well.
@TaitLeswing talks about it as well in this thread:
The trick in the tool path here would be to find a way to have a side of the bit that is clear of the material that you are cutting so as to have a cooling effect and at the same time have space to throw the chips away from the bit.
In the end though, I could be wrong and am just a beginner when it comes to learning about CAM, so if I need correcting… please speak up, because I am here to learn as well as help.
I cut acrylic all the time. I have access to a lot of lasers and will use them if there is any engraving involved or the part needs a decorative edge.
If I want something purely mechanical with tight tolerances and sharp edges (most of my stuff), I prefer a CNC router. The trick to acrylic is dealing with the chips. The cuts must stay clear. If you are re-cutting chips your edge quality will suffer and you will might break bits due to the sudden changes in load. Sometimes the chips will even re-weld in the grooves.
I like to use spiral upcut bits. The fishtail bits work great for me. I like the 1/16th. It is fragile, but it produces less chips. Try to blow out the chips immediately. If they are getting hot they will still be soft. Get them out fast before they harden into a tangled clump. Experiment with some depths of cut.
Thicker acrylic tends to show a line on the edge for each pass even on a rigid machine. Try cutting almost all the way through with a little offset from the edge and then doing a full depth finish pass right on the edge.
I agree with Bart regarding the up-cut spiral bit to get the chips out, but using the proper grade of plastic is key. It doesn’t matter what bit you use or the spindle or travel speed. If you are using “Extruded” plastic it will have melting problems. Most home centers sell the least expensive extruded acrylic sheet. Try going to a plastic supplier like A&C or Laird plastic. Also a good source is sign supply wholesalers. Ask for Cast acrylic sheets. Another good one is “SG” grade, it has a higher impact or breaking point while still giving good cut quality without melting behind the bit.
First, I used Zach’s suggestion of 100in/min and 0.010" passes with the 2 flute straight bit, while clearing the chips with a shopvac. This was a failure, as the bit would choke on the tiniest amount of chips and the molten ball would begin.
Then I tried the single flute spiral upcut. It left more chips behind, but it doesn’t seem bothered by them nearly as much as the straight flute bit. It just tosses them out of the way and continues on.
So here’s my results with single flute spiral upcut, 100in/min 0.010" passes:
Spencer, I used to sell and install CNC machines into the sign industry. They cut a lot of plastic for backlit channel letters. I can tell you without a doubt that if you try cutting some cast acrylic plastic your cutting issues will be eliminated. You won’t find it at the home centers but at a wholesale plastic supplier. They usually have a scrap bin area that sells small sheets and scraps perfect for small projects.
Hi Mike, I made note of that from your previous post. I bought the acrylic from a plastics fabricator, so it could be either cast or extruded. I will call them up after the weekend and find out what I have. Whatever it is cut pretty well with the setup I posted above.
Hi @SpencerShepard we sell cast. What size and color do you need? I’ll send you a complimentary piece to test since my suggestion screwed up your last one.
@AndrewBishop, good question. Did you ever get answers on this? I’m interested in the answer to this myself. I’ve got cast 1/8" cast acrylic, but really don’t have a firm grasp on bits yet. I’m using 24" x 24" sheets of 1/8". Even with clamping the edges, i’m finding the 2-flute upcut that I have makes relatively small chips, but it tries to lift the sheet in the middle due to the vast expanse of the sheet. Downcut would seem to help in that department, but it won’t clear the chips well. I need to order up a 2-flute straight bit and give that a shot.
@SpencerShepard Played around using your and @Zach_Kaplan settings as a starting point this weekend and had great results. I was cutting roughly 1/8" thick acrylic, using the 1/16" spiral upcut bit supplied with the kit. The settings were 75/min @ .01 depth and worked amazingly.
Wanted to say thanks to the contributions in this thread! I had a 6.5 hour cut yesterday on some .5" thick clear acrylic sheet (the cast kind from Inventables) and the settings above with the single flute spiral upcut bit worked wonderfully!
