Cutting plexiglas (PMMA)

How To
1

After several trials I’ve not found the right parameters to cut Plexiglas, I’ve reduce the feedrate up to 500 mm/min (aprox. 20 inch/min) -trying feedrates from 500 to 700 mm/min-, and reduced the step down up to 0.1 mm. But every single time I get the same result, the material got melted and it stuck to the mill. At this point I had to stop the milling and remove the material bonded to mill.

I’ve been googling and maybe the solution could be speed up the mill -in order to refrigerate the mill?-, till now I have set this mill (2mm diameter) on 3750 rpm on “select tool” display window.

I want to make a new trial on a speed of 12000 rpm. and 700mm/min of feedrate. But I’m not going to be able to test it till tomorrow.

Any of you have experience with plastics getting melted during the milling?

2

We have a bit on the Shapeoko wiki: http://www.shapeoko.com/wiki/index.php/Materials#Plexiglass

Big concerns:

  • cast or extruded
  • single flute endmill
3

Badly probably according with the link it is extruded, it has plastic protecting both sides. Using a 2 flute endmill.

What is maximun speed on The Nomad?

4

Hi David,

I wouldn’t recommend running over 10krpm just for the longevity of the spindle.

This is about optimizing chip-load and thermal transport away from the tool, so that you don’t get heat build-up in the tool or remaining plastic (leading to gluing you’re experiencing). I’ve posted a bit about this on this thread and given further details there, but the important part for you here:

The equation for chip-loading:

Chip Load = feed rate ( ipm ) ÷ ( cutting rpm x number of cutting edges )

that works out like this to solve for feed rate instead:

chip load x rpm x cutting edges = feed rate

According to PDS Spindle’s feeds/speeds chart here, the recommended chip-load for acrylic for a 1/8" tool, which would be 3.175mm, is 0.003-0.005" per-tooth which on a two-flute tool at 5krpm would be 30-50 inches per minute, or 762-1270mm/min.

Therefore yes, even though your tool is a 2mm tool, it’s likely that you’re running the tool too fast against the material relative to the feed-rate, so it’s rubbing the plastic more than cutting it.

Onsrud makes a series of plastic-oriented tools that you might be interested in: the 63-700 series here in their catalog which has an “O-flute” design to improve chip clearing to prevent the bonding you’re getting. They also have a bunch of different feeds & speeds tables available, but you’ll want the hard-plastics chip-loading chart. That specifies a chip-load of 0.002-0.004" with a 1/16" diameter cutter, which is a bit smaller than your 2mm cutter (it’s ~1.6mm), so ~770mm/min is probably a good “middle ground” feed-rate to try at 5krpm, and see how that goes at up to 1x diameter depth cuts.

Or, if we’re concerned that might still be too much heat or lateral load on things, you could go down to 3krpm, and then try a feed-rate of 18ipm, or ~460mm/min.

1 Like
5

One small addition, although we will not throw an error if you give a larger RPM, it will not turn faster than 10,000 RPM

-Rob

6

@robgrz

Rob, Are their reliability, or other, issues with running the cutter other than 5,000rpm? That seems to be the default speed, so I have just continued to use it and adjusted the other parameters based on the chip load formula.

Could you post screen shots of the ToolPath Parameters page that you used in the different projects that are shown in the carbide3D videos?

.

7

Historically, it was at 5k because it’s the middle ground that most machines can get to. 10k is fine though- it’s won’t harm anything

I’ll have Apollo share settings in the future.

8

is Plexiglas the same thing as acrylic? If so, there are presets already available in meshcam. I have used them a few times for acrylic and they seem to work just fine. goodly chips, no melting.

9

Yep, Plexiglas is a brand name for Acrylic (PMMA), but Acrylic does come in two major variants with extruded and cast behaving a bit differently.

We’re talking fine-tuning stuff here, to minimize chipping risk and optimize finish.

10

Thanks a lot to all of you, I’m going to learn a lot here.

According with the formula you have provide to me UnionNine and the links I will make some more tests today, I will start with these parameters as you recommend to me:

  • Spìndle speed: 5000rpm
  • Feed rate: 700mm/min
  • Step down: 0.5mm

If not success I will reduce feed rate first up to 400 mm/min on steps of 100 mm/min. If not success I will reduce spindle speed on steps of 500rpm at low feed rate up to 3500rpm.

In the mean time I’m going to order this tool:

Specific for plastics with just 1 flute.

Do you know which grip can grab the ER11 collet coming with the Nomad? the shank of this mill is 3mm diameter and the nomad is coming with 1/8" collet, this is 3.125mm. I guess I don’t need to buy a new collet for this, do you agree?

Silly question: Is the Nomad spinning right handed? I think so, but I’ve found the same mill on the same provider left handed and now I have the doubt.

-David

11

Hi David,

  1. The ER11 collet is fitted into a matching ER11 taper, and it’s the collet-nut that clamps the whole thing together to hold the tool. You can get different collet diameters if you want to hold more varieties of tools, but a 3mm shaft is within the clamping range of the 1/8" collet that comes with the machine. One of the advantages of the ER collet design is that it accommodates a fairly broad clamping range for each given size.

  2. I haven’t dug too much into the “handed-ness” of tools, to make sure the terms are truly equivalent, but the Nomad spins clockwise, so for this tool that helix (if it’s as drawn) is an upcut tool, whereas if the helix were reversed it would be a downcutting tool. It’s a matter of both spindle-rotation direction, which determines which way the cutting edge is facing on the tool, and the helix rotation direction, which tells you which way the chips are going to be pushed by default.

That should be a great bit to have, but just remember to cut your feed-rates in half for a given spindle speed since it’s got only one cutting flute instead of two.

Lastly, the key thing to remember with thermoplastics is that you want to clear the material without heating it up such that it melts and adheres to the tool. If it catches and is sticking to the tool still, then you should increase your feed-rate relative to your spindle speed to increase chip-loading and material clearing to try to resolve it.

12

I’ve been more or less success with 850mm/min feedrate and 5000 rpm on a 3mm cutting mill. I’m now focusing on the curve problem.

I will try it tomorrow with the new mill and thanks for your tip, I will half the feed rate tomorrow. I will keep you all on the loop updated.

-DAvid.

1 Like
13

HI David, I am going to mill some cast acrylic as well. I was wondering how did that new cutter work for you. What feed rate and settings worked for you.

Thanks,
Jay

1 Like
14

Sorry. So busy last weeks.

I’m getting good results with a 1 flute mill. Really good results. With feedrate 400 (mm). 3500 / 4000 rpm. Stepdown 1/3 - 1/4 of diameter. If you need something more specific I will check tomorrow. I’m at bed right now.

1 Like
15

Thanks David, that’s sounds like a good cutter. I can’t seem to buy that brand here in US. Do you know similar cutter that I can purchase here in US?

Thanks again :smile:

16

I’m not David (nor do I play him on television…) but 2linc here in the US sells a variety of 1-flute cutters (flat and ball-end!)

https://www.2linc.com/endmills_plastic_1fl_std.htm

and Precisebits also sell 1-flute cutters.

http://www.precisebits.com/products/carbidebits/micr-O_1F.asp?tsPT=!!!1Flute_micrO-flute_FishTail!!!1/8_shank!!!#Tabs

17

Harvey tools is also a U.S. supplier of 1 flute mills.

http://www.harveytool.com/prod/Browse-Our-Products/Application-Specific-Designs/Plastics---Composites_191/Plastic-Cutting-End-Mills---Square-Upcut-Single-Flute_113.aspx

When I start to look for this link was on the first links where I found it. Now I’m buying to an UK supplier cheaper than the previous one.

Good luck with your projects.

18

Thanks Randy for chiming in! I like you sense of humor, that makes this community even better :smile:

David, thanks for sharing your results of the new cutter and settings.

Please bear with me as I am a total newbie and here is what I am after:

I need to cut 20mm deep pocket (12mmx5mm) in clear cast acrylic piece(25mm stock height). I want to be able to cut many of them in a matrix pattern. What size of cutter should be best for me? I am little overwhelmed with so many choices of cutters to choose from. Can you guys please recommend a specific cutter that would fit my needs? I am not sure what diameter/length of cutter should I pick. And of course cheaper is better. However, if the cheap tool is going to wear out too soon, it might be better to invest in a better quality and little pricey tool. I would be doing lot of these cuts and may need to buy couple of cutters.

Thanks again folks!
-Jay

19

2Linc.com has some endmills with longer flute lengths; for example, the PWE1-250-1 is a single flute mill for acrylic that has a 1/4" shank (so will fit ER11 if you have a 1/4" collet), and has a 3/4" flute length - but that is unfortunately only 19mm, and you mention you need 20mm.

Lakeshore has much longer flute-length endmills with 1/4" shanks also, in a 2 flute:
http://www.lakeshorecarbide.com/14carbidelonglengthendmill10flutelength-1.aspx

20

Thanks Warba, I will order PWE1-250-1 bit as 1mm less deep is not a big deal. Since I am going to order this bit, I am thinking or ordering one more for aluminum. I used Carbide 3D’s #111 #102 on aluminum and they both broke. I played with slower feed rates and plunge speed extra. What bit should I order from aluminum, pretty much same material and cut requirements as acrylic part? Thanks again.