Any tips for cutting acrylic? I am using a shapeoko five pro with the VFD spindle. I was trying to “drill” some 1/8" holes with a 1/8" bit. I made some test drill that worked fine. But for the actual project the plastic heated up, melted and then cooled, sticking to the endmill. When this happened the acrylic stuck to the endmill started cutting through the acrylic
Look at a “Mill-Drill” tool. made to end cut with higher speeds. Or use a O-flute, single flute cutter.
Slowest setting on the spindle, fast feedrate. And if you’re drilling use short pecks to keep clearing the chips.
I prefer to “Hole mill” whenever I can. Use an undersized mill, 1/2 - 3/4 the size of the hole, and a helical cutting pattern.
3 Likes
You need to use cast acrylic. Cast acrylic cuts pretty well with a single flute cutter.
Extruded acrylic will melt and gum up just like that.
Typically (and not guaranteed) extruded acrylic has a plastic protective sheet on it, and cast has a paper protective sheet on it.
2 Likes
some remarks:
- whenever possible use cast acrylic, the one with the paper protection layer, maybe there is a cast acrylic out there with transparent protection layer, but that should be rare. It just has another struture and therefore another melting temperature.
- Cast Acrylic: Softens at around 160°C (320°F) and melts at approximately 300°C (572°F).
- Extruded Acrylic: Softens at a slightly lower temperature, around 150°C (302°F), and melts at approximately 260-280°C (500-536°F).
Cast acrylic generally has better optical clarity, chemical resistance, and machining properties, whereas extruded acrylic is more cost-effective and easier to thermoform.
Yep, few degrees that make a difference.
- And we need to keep the temperature at the contact site of the tool and the acrylic as low as possible.
reduce heat at the cutting site by:
a) smallest contact surface possible: “O”-flute is the choice:
That small sharp tip has the smallest contact surface of all bits, and has just one flute.
b) keep the speed at the tip as low as possible, thus reducing the contact time of the tip with the plastic
c) get the heat producing site away from the acrylic as fast as you can: means fastest as possible feed speed.
Do some test cuts before the real deal, and never proceed if anything else is produced than dry chips.
Since the melting temperature is not so much a difference extruded acrylic may work as well, consider some tests with that too, but always remove the protection foil.
These tips work with any kinds of thermoplastics.
GL!
3 Likes
What were your drill settings?
Plunge rate.
Was it a pecking cycle? If so what was the depth per plunge?
RPM?
1 Like
There’s lot’s of good advice in this thread. Single flute endmills and pecking are the two biggest changes you can make to increase the possibility of success.
Now, get back on that horse and cut again!
2 Likes
RPM for 1/4 inch O-flute in acrylic 6000, for 1/8 inch 8000. Will not be responsible for broken bits though, all depends also on the depth of the cut.
So a Mill-Drill is a different type of bit?
By hole-mill, do you mean just cutting a hole instead of using the drill feature?
This was supposed to be cast, but it did have a plastic sheet instead of cast.
The cutter was doble flute, I think. It was the 1/8" endmill that came with the endmill starter pack.
So, slow RPM and fast feed rate? Is this the same for cutting and drilling?
I will look into one of those bits! Thanks.
Yes, I think so. Get away from the site of heat production as fast as possible: high feed rate, and low friction: slow RPM.
Using the #102 eighth inch end mill.
Plunge rate: 8 ipm
Feed Rate: 10 ipm
RPM: 10,000
depth per pass 0.5 inches
Peck distance: 0.0625 inches
I did six test cuts with those settings and the results were flawless.
Looking at the actual cuts, it was 18,000 RPM. I thought both were at the same speed. So I am thinking I have found the problem.
2 Likes
I will check that out! I need to get a diamond drag bit, so today may be a good day to do some shopping!
Ah, yeah, if the RPM is way higher, that will mean the plunge would have to be equally faster in order to keep the same chip load.
1 Like