Acrylic cutting results

[esolberg]

I've been getting some advice here on cutting acrylic and I've run a test run on a handful of end mills on half inch acrylic (.472). I thought I'd come back and share my results in case they are helpful to others, and perhaps folks here can comment if it looks like I should be getting better results than I am.

I'm building a prototype for a project I'm working on, so I can afford to play around with different end mills to see which will work best. The part I'm cutting out forms a "dome window" on my project and is important to the cosmetic appearance of the project. I had tried laser cutting these first, but the 60W laser I have access to does a terrible job on 1/2" acrylic. But I did use it to rough cut blanks to then finish on the shopbot. This was a little easier than cutting all of these out of a flat sheet. I focused on Onsrud since they seem to be what everyone is using for plastic and the company has lots of data/experience on plastic. I also had a couple of YG1 end mills that I got for aluminum, and I threw those into the test as well. One of them performed better than the Onsrud bits.

Here's the endmills, feeds & speeds I used. More below on the results, but these are listed in order of the best to worst cut (subjective eyeball/finger analysis). In each case (except as noted below) I cut the full edge of the plastic with 2 passes removing 0.125" with each pass.

The top 2 end mills could easily be swapped between 1st & 2nd best. The YG1 looks a little shinier but you can feel deeper ridges. The Onsrud has a smoother feel but you can see & feel 2 annoying tool marks down the full length of the cut. That should polish out I'm guessing.

YG1 21593 1/2" 2 flute 42 degree helix 4711 RPM 28.17 IPM
Onsrud 63-535 3/8" 1 'O' Flute 5968 RPM 17.09 IPM
(The 63-535 is designed specifically for acrylic)
Onsrud 61-121 3/8" 1 straight flute 6122 RPM 26.99 IPM
Onsrud 61-081 1/4" 1 straight flute 6122 RPM 26.99 IPM
(The 61-081 has a 3/8" cutting length so I cut in 2 passes)
Onsrud 56-650 1/2" 2 'O' flute 4711 RPM 27.24 IPM
YG1 32593 2 flute 4711 RPM 28.17 IPM
Onsrud 60-249 1/2" 3 Flute Low Helix Finisher 5149 RPM 27.02 IPM

Feeds & Speeds - you might be wondering where I came up with numbers like 26.99 IPM. I'm using a feed & speed calculator called "GWizard" and I'm still not sure how much to trust it. Especially for smaller bits it comes up with some extreme recommendations. It uses the bit diameter, cut depth, bit length (for deflection calculations) and manufacturers recommended chip loads (and some other parameters) to calculate recommended feeds and speeds for you and lets you calibrate from conservative (improved finish) to aggressive (higher removal rates) and will optimize tool deflection for rough vs. finish cuts. Supposedly! (any one else using it?) But since I don't have a background in machining I don't have the experience to draw on so I need some kind of calculator to get me started.

Here's the photo of my results, and a few more comments after about the cuts and about what this tells me about the shopbot.

https://dl.dropboxusercontent.com/u/10530820/Acrylic%20Test%20Cuts.jpg

First thing you'll notice is the parts are wildy different sizes. They are actually the same part and should have been identical. There are 2 reasons:
Two of them seem to be off by exactly 0.125". Although I can't believe I did it, apparently I forgot to make the 2nd pass on those.

The rest of the differences must be related to something I posted on another thread. The Onsrud bits all measure under size, so I used the measured diameter. But judging from these results that seems to be incorrect. It must be that these 1 flute cutters are not exactly symmetrical so I can't just measure across the widest diameter. That's the only explanation I've got at the moment but it would explain why every one of these bits measured under size. I plan to cut out some slots and measure the slots to be sure.

Another thing is that the worst cut - the 60-249 - almost looks like the best cut in the picture. For sure this is going to make me take a closer look at it- maybe some of what I judged it on was coloration which would buff out. But I did look at it and the bottom half of the cut (not in the picture) does have significantly more tool marks than the top half of the cut. But still, worth a closer look.

Another thing you don't see in the picture: these cuts are forming a gently rounded edge with about a 32" radius. Out of the picture there is a straight edge as well. In every single case the straight edge came out much cleaner than the rounded edge.

I also don't show the back of the piece here. This is an inside cut made with a 1/8" cutter because I have some smaller features. I didn't show this because all of these cuts are horrible. Its the inside of my part so that isn't as critical. I haven't played too much with this but I'm not really confident in the speeds/feeds for this I'm getting from the calculator and for sure the cuts are not acceptable. I'll play with this later, its lower priority.

So here are my takeaways from this test:

First - the Shopbot (Buddy in this case, but I got same results on an Alpha) seems to like 3/8" 1-flute cutters for thick acrylic. the reason I say this is that the bigger cutters need higher chip feeds and you quickly get out of the horse power rating of the SB with the aggressive cuts these want to make. And as I noted above I'm just getting wacky speeds/feeds with 1/8 cutters if I try to minimize tool deflection.

Second- judging from those results I'm wondering if the Shopbot is the best tool for making these curved cuts on acrylic. Its doing nicer/smoother cuts on straight surfaces. I wonder if the marks I'm seeing here reflect the stepping geometry as the motors digitize the arc?

Well this is very long, but I wanted to share the results in case its useful. If anyone has any suggestions on what I should do different, that would be appreciated. My plan next is to play with speeds/feeds on the 63-535 and YG21593 to see if I can improve these cuts even more, then I'll test out some sanding, and then compare wheel and flame polishing.

Cheers,
Eric

[Brady Watson]

At the RPMs listed, you are milling these parts and not routing them. You want to be in the 16,000-18,000 RPM range for the tools listed and moving between 1 and 2 IPS XY speed. Your machine should be clean (rails) and tight (properly set pinion gears and lubed racks) before running these types of tests.

You will get best results with a 2-step approach. Cut the parts with a .02-.04" Allowance (cut them large), stepping down 1/8" per pass and leave say, .04" on the bottom. This is called 'onion skinning'. Then come back, change the pass depth to go full depth (.48") in one go, and shave off all those step down marks. You want nice, clean, smooth movement - so alter VR and MS settings accordingly to minimize actions that would cause shock loads or abrupt movements that will telegraph into your edge finish.

You are correct, you want a 3/8" cutter as it will yield much better results than a 1/4" one (stiffer, better harmonics) and a 2-flute spiral-O is the way to go. Vacuum hold down is a must, since a lot of quality can be lost with slip-shod hold down techniques like screws.

-B

[esolberg]

Hi Brady,

Thanks for the tips. I did a couple tests (not as thorough) using speeds & cutting approach like that initially, and got similar results. But perhaps it makes sense to try again. These shopbots are shared by a lot of people so very likely all the adjustments are suboptimal. The main thing I've run into with some of them- at least based on this feed calculator- is I start to run into the horsepower limits of the shopbot. According to the calculator a 3/8" 1 flute cutter cutting at 1/8" depth & 1/8" width at 16000 RPM at about 2 IPS will require .28 HP. According to the specs the shopbot can do about .27 HP. Now I could be completely off base on that, lord knows I'm overthinking all of this.

Dumb question - when you make the finishing cut, do you recalc the feed/speed for that cut? Because that thin cut is going to have a thin chipload. Does that matter for the finishing cut?

Regarding the vacuum hold, I don't think I can do it on this part, so I am actually using screws. My part is cut from a blank about 3" x 6" and is a bit smaller than that when cut out. What I did is use the laser to cut screw holes, and the shopbot to drill corresponding screw pilot holes in the underboard. I've got the screw holes fitted very tight- the screws squeak a lot going in. An example is shown below. The outer edge is the blank, the inner edges are the part profile/cutting paths. The top & bottom holes are M1.6 screw holes (which I drill on the shopbot) and the other little dots are lasered in to help with setting x&y (which don't need to be that accurate theres plenty of wiggle room in the blank).

https://dl.dropboxusercontent.com/u/10530820/dome-cutting-paths.jpg

[Brady Watson]

If this is a shared space, plan on cuts being less than 100% optimal, unless the machine is routinely maintained, cleaned, lubricated, adjusted and treated properly.

You are going to have less than optimal cut quality if using screws or any other hold down strategy that does not hold down the sheet uniformly, such as vacuum.

I don't mean to sound harsh, but take those chipload and horsepower calculations and throw them in the trash. They may be applicable to a machine running production, but they don't apply on a ShopBot Standard machine with no vacuum system that will most certainly need to run at a much lighter chipload.

Try running a 2-flute spiral-O at 18,000 RPM and a move speed of 1.2 to 1.7 IPS, using first allowance and stepping down .125 per pass with .04" or so left on bottom. Come back and shave off AT LEAST .02 to get part to spec size. You NEED more than .015" on certain plastics so that the tool will properly bite in.

Run dust collection as it will aid in cooling & get those chips out.

Go play with these values & report back. Routing is VERY different from milling...that being said, see if your scrap looks better than the finished cut. If it does, reverse direction to climb or conventional - no sense in throwing away your best edge.

-B

[esolberg]

Hey Brady,

Thanks again for the tips. Definitely don't mind the blunt advice - I don't really trust the calculator either I just didn't have anything else to work from. Its funny if you google advice for routing acrylic you will get people swearing that slower is better and others swearing higher is better.

I don't have a 3/8" 2-flute bit but I did try it with my 3/8 single O flute that is made for acrylic. This time I used 18,000 rpm and the chip feed / rate calculation given by Onsrud. Their recommendation for this is actually works out to 1.8ips. So I ran it at 1.8, 1.7, 1.6 and 1.5 using the onion skin approach with both climb and conventional cut for the finish cut. They actually came out exactly like before, with the climb cuts being slightly better. I think this equipment is just too abused, this is probably the best I'll get. I'm doing this at a place called TechShop, and there are actually 3 in my area - each with a Shopbot Buddy, Alpha and desktop. I suppose I could try all of the other machines!