Cutting plexiglass problem

[TomGB]

I'm doing a cutout of a piece of .223 plexiglass with a 1/8" upcut endmill. Depth of cut is .033" per pass, speed is 40"/min, RPM around 12,000. I keep getting a buildup of the waste plexiglass on the bit on the 2nd or third pass that burns the edge of the plexiglass. Any suggestions?

[jeffhcarter]

I am experiencing the same problem with Engraving. Hoping someone has an answer for us

[TomGB]

I saw your post on what bit for engraving, I'm a novice, but used a 2 flute 1/4" dia. 60 degree Vee set .001 depth of cut and it worked great.

[martin54]

OK couple of things, firstly acrylic is less forgiving than wood so speed, feed & DOC settings need to be more accurate. A bit designed for cutting plastics is best something like an onsrund O flute. I use bits supplied by a UK company single flute, not cheap but great for the job. Chip extraction is essential to stop recutting & heat build up. If your dust extraction isn't the best (like mine) then an airline blowing in the cutting tip of the tool not only removes the chips & keeps the area clear but it also helps to cool the tool tip, doesn't need to be much just enough to remove cut chips.

[TomGB]

Thanks Martin, I will try putting the air on it

[martin54]

I would also look at increasing your feedrate or decreasing your spindle speed, best to experiment a bit really to get settings right for your machine but I cut with a faster feed rate than that with a single flute bit

[Xxray]

High feed *, slow RPM's, shallow passes [.125] + good sharp bit [the last 2 being most critical], you should have no problems. I have routinely cut up to 1.5" plexi smooth as butter [although some edge polishing is almost always necessary no matter what you do], when I notice the plexi starting to gum up at all or change pitch [which indicates a struggling tool], time to toss the bit and use a new one. Air/coolant could help, have personally never found them necessary.

Plexi will screech like nothing else if you are not in the sweet spot for cutting, if it is wailing like a banshee stop and change your strategy.
* "High feed" is subjective depending on the bit used, quality of the bit, sharpness of the bit, rigidity of the mount/machine and material thickness/depth of cut. High speed is always desirable in theory, insofar as higher feed rates minimize the friction heat buildup which causes gumming in acrylic, but going too fast can also over stress the bit and cause it to snap, can even warp/damage a cheaper machine [somethings got to give and it will either be the bit, material or machine]. In that case, you obviously have to go slower regardless of friction.

In other words, guys in a production shop using a $100K machine with $100 bits can get away with maxing out speed, me and you in a garage likely won't have that luxury. So a certain amount of trial and error [and broken bits] is usually required to find your particular sweet spot for cutting.

[dwilli9013]

Just my opinion to start.
The sweet spot for me with acrylic was an Amana tool 0 flute bit designed for acrylic and plastics. That coupled with tons of advice from this very forum and lots of gotchas I have managed to turn out some pretty fair pieces. My feedrate and spindle speed dialed in when I found my chips to be about the size of a babies fingernail. Once I hit that sweet spot my plastic cutting took off.
Your individual feeds and speeds will vary as it does with all of us. I cannot cut at near the speed Doug does due to my machines capabilities as well as I am not a production run shop. I rather enjoy watching the cut happen which gives me a bonus as I am right there should my pitch change or something else goes wrong. I have also found that edge finishing is dependent on the application. I do use various techniques and methods many of which I have learned here. at the moment my favorite method for edge finishing is using a card scraper. With a light hand and patience one can achieve a nearly clear edge finish.
As Martin mentioned a light spray of air on the tool can help as it will cool the tool and eliminate the chips from the cut for the next pass.
One thing I have found out the hard way is With an 0 flute upcut bit feed rate and depth of cut can become critical quickly. As your feeds and speeds increase so does the desire of the tool to pull up on the work piece. I have had instances where my material was securely clamped in place but the bit was still trying to pull the material up.
All I can really add is experiment, experiment and experiment. Continue following the advice of these great folks on this forum and above all enjoy yourself. Nothing sweeter than that first piece you pull off the table and realize you knocked it outta the park.

[GEdward]

One other point is whether your plexiglass is extruded or cast will make a difference as well. It seems that cast is preferred as it is less gummy when being machined. For my machine I have found that keeping the rpm down is more important than the feed rate. I have not found any bit in my arsenal that worked well over 9600 rpm but I am still fairly new to this.

[Rcnewcomb]

GEdward,
My grandparent's farm was just outside of Andover, SD -- about as far east of Aberdeen as you are west of it.

[GEdward]

GEdward,
My grandparent's farm was just outside of Andover, SD -- about as far east of Aberdeen as you are west of it.

I know a few people in the Andover area. I sometimes accompany my Dad to the annual threshing and steam engine show they have over there.