Acrylic Troubleshooting

I have been cutting acrylic today, trying to get a nice clean cut. So far I’m still getting a bit of a “bumpy” edge. Below are the settings that turned out the best. I used carpet tape to hold the material down, being careful to keep the tape away from the cut line.

My feed rate was set to 2000mm per minute and my spindle was set to approximately 18000RPM. I was cutting 2.2mm in a single pass.

I used a 1/8" single flute upcut bit:

Any ideas of how I can improve my cut? I appreciate any help!


I have not cut any acrylic, but I would lower your feedrate, 33mm/s is too fast. In doing that you can either cut deeper per pass or slow your spindle.

I do almost all my cuts at 12-18mm/s and adjust everything to work with that parameter.

That is just me, I think I do everything slower than most, even printing.

Okay thanks!

I tried to halve my settings so I could get into the 12-18 mm/s range.

This time I tried 1,000 mm/min and approximately 9,000-10,000RPM. My edge was a bit worse, but I’m not sure if I should be increasing RPM or feed rate. I can’t decrease RPM, since I’m at the lowest RPM my router can accomplish.

here’s a picture of my results at these settings (I’m also cutting about 2.5mm now because I ran out of scrap 2.2mm material, so that does change things a bit):

For those who are interested, I found a document from Onsrud that I think will be helpful for solving my issues. It’s called the CNC Production Routing Guide. Check out the attachment.

I plan to reduce my feedrate to 12mm/s, leaving my spindle RPMs alone, to see if it results in an improved edge.

LMT-Onsrud-CNC-Prod-Routing-Guide.pdf (1.06 MB)

How big is your build? Looks like the its not tracking straight. Might need to slow down further.

At that spindle speed you’re going to need trochodial milling. Otherwise it’s going to just refuze behind the cutter.

The single flute mill I got for acrylic was somewhat different looking:

Which I think is the same as the one Ryan sells in his store. I haven’t cut Acrylic (and Lexan) since last May so can’t remember the details off the top of my head. But I can try to look them up tonight from home. I was just using my old dremel with worn out brushes back then and it was dying so RPM’s were somewhat unknown and hard to estimate. I did keep the feed down under 15mm/s I remember but just how low escapes me at the moment.

I didn’t get a perfect cut - there were a few slight issues along the edges. But given the issues my dremel was having I was very happy.

I actually need to dig out the settings anyway because I need to replace the lexan plates after a particularly nasty crash.

Jason - when you say it’s not tracking straight, is that your diagnosis based on the bumpy/wavy edge? Or do you see some other issue? My tubes are 35.25" for X and Y. I set it up for 4 inches of Z travel and I used the calculator. I can’t recall how long the Z rails are exactly, but I think it’s like 11" or so.

Barry - when I tried trochoidal milling I got what I’d describe as a shark tooth edge. I don’t really know which trochoidal parameters do what. Any idea of a starting point for the trochoidal milling settings in Estlcam? I’m guessing I need to go with a slower spindle speed, right? I will be getting a PID controller soon.

Other Jason - I wonder if the difference is mostly due to the cutting length of the two end mills being different? Mine is supposed to have .87" cutting length, while the one in the link you shared is .4". Just a guess. I appreciate the ideas for the settings!

I’m traveling for work today, but I will try tweaking the settings some more tomorrow or on Thursday. Thanks!

Shark teeth is too much of a step length. Try 15 to 20mm/s 30% stepover, 20% step length, 50% width, .05mm oscillation. You should be able to set it full depth of cut. Test on a scrap first, if it’s still making teeth, lower the step length percentage.

There will always be some sawtooth to the edge, if you require perfectly flat edges, create another standard cut after the first cut to clean up the edge. When I did my dust collector window I didn’t bother, it was smooth enough for the purpose.
Google Photos

Cutting plastic
Google Photos
Cutting aluminum

Awesome, thank you so much for that. I will give it a shot. Hopefully I’m back home early tomorrow afternoon - fingers crossed that my meeting in the morning is short!

This site has quite a cache of information about the milling we do with the MPCNC.

Specifically, here’s a tutorial that covers cutting lexan/acrylic.

I have found the entire site valuable.

Great! Thanks Tom, I will definitely spend some on that website.

Alright, so I used Barry’s trochoidal settings. I think it is still possible to improve from here, but it is a huge improvement already. The chips are looking pretty good, not stringy and not dust, but somewhere in between.

Here is a picture of the results:

Here is a video:

And here is a screencap of Estlcam settings - you’ll have to click on the picture after clicking the link, the columns are all visible in the picture (I used a Makita RT0701C on speed setting #1):

Question about this fancy method of milling “trochoidal”… Would it be beneficial and make better cuts in wood too? Could the depth of cut per pass be deeper with this method?

Yep. You’ll need to do a final finish pass most likely.

I experimented with spindle speeds and adjusting the trochoidal parameters, but being at the absolute slowest spindle RPM I can accomplish limits my options. I also tried running a straight finishing pass, but it didn’t do much for me. I’m assuming that I would have to take more material off for the finishing pass to help.

With my setup, I think I’ve reached the point of diminishing returns and I found that a quick once over with fine grit wet/dry paper gave me a really nice edge. For this small 1-inch square, it took about 10 quick back and forth strokes per side, which is probably faster and less effort than any improvement I could eek out of my MPCNC setup until I get my Super PID.

Here’s a picture of what it looks like after sanding:

Not too shabby, if you ask me!

That’s much better!?

Thanks Barry!

I’m going to start testing HDPE next. Should I start with the same settings?

Yea, it’s pretty safe to start there.

Need some help/guidance here… I got some scrap plexi at Ace Hardware today in order to test cutting before trying out the 1/4" acrylic I got for some parts…

see the pictures for my results… seems the combination I have does not work and the material gets too hot and gums to the bit.

I am using these bits -

I am using this spindle - - at full speed so that is 12k rpms.

Looking at the other screen print I set up the trochoidal settings that someone mentioned here in this thread.