machining plexiglass

[Harry Kroyer]

I don't have experience cutting plastics and need to machine a piece of .5" plexi in fabricating a dust collection intake for my ShopBot.

Kindly share some info regarding spindle and travel speeds for a .5" or .25" end mill to cut holes and to cut-out the shape.

Thanks,

Harry

[Perry]

Hello Harry,
I would suggest that you stay away from cutting Plexi with the Shopbot and instead locate some cast acrylic. Plexi has a low melting point and can be tricky to cut. Cast acrylic much more forgiving, will hold a thread tap and more durable (IMO).

[lockeyone]

Here is a copy of my Dinosaur file. I used a 1/4" bit, tried up spiral, O-Flute and even a down spiral. Also tried some WD40 and a few others. Nothing seemed to make a whole lot of difference. I did break one bit and what I think it was that the plastic would load up on the bit. I would stop and clean it off once in awhile and this one part of the run I got side tracked and forgot till I heard the bit go.

As far as the Plexiglas, my guess You/he is calling it that as a generic term. Truthfully, I'm not sure what I cut, it was part of a scrap package the guy I bought my machine from gave to me. So the price was right.

Here is the thread I posted on this.
http://vectric.com/forum/viewtopic.php?t=854&highlight=

[Paco]

The key is O-flute tooling. With O-flute, you'll be cutting many kind of plastics including extruded acrylic. Such large tool diameter as you intend to use are very forgiving.

With such thick material, I'd go with spiral up cut single O-flute. As always, try to use the shortest cutting tool. Keep the RPM low to mid (10 000-14 000); the higher for either fast feed or small diameter tooling (1/8" CED and smaller).

For cut out from 1/2" acrylic with a 1/4" diameter (CED) tool with no more than 3/4" cutting length (CEL), I'd set the RPM to 13 000-14 000 and feed at 2-4"/sec. (120-240"/min.). The lower feed for small and curvy parts and faster for straighter cut. Ramp in the cut (no straight plunge) and no more than the cutter diameter for step down (100% CED). That is a maximum of 0.25" step down for a 1/4" CED cutter. Less for longer tool and for less flex/stress. I'd use 0.15" stepdown and make a final ~0.02" allowance clean up pass.

Make sure you have a good hold down as vibration is enemy number 2 for cutter. Heat being number one. I've had some fellow Botter using HSS tooling with plastics with success and saving on the cost... Just don't use HSS with wood products.

I just happen to make some tests today; 3/16" acrylic (extruded sheet stock) with 1/16" CED, 1/4" CEL spiral O-flute. 0.04" step down, 12 000 RPM, 0.72"/sec. (about 45"/min.) and very gentle ramps on the corners. The cut out is about 2" tall letter with the base.

I hope that get you confident to cut your dust shoe.

[James E]

Agree with Paco, those are about my speeds, although I tend to feed a bit slower, and i take similar shallow cuts. If you start off shallower, you can always get deeper as you become more experienced.

Better than getting cheesed off with breaking a bit.

Heat is enemy no 1, as Paco says,and a solution I found on here, to the problem of reweld, was to cool the bit with air. A tiny jet right at the bit, for best effect.

My best bit is a 3 flute upcut spiral, tapers down to 1/64 in dia.

Good luck
Jim

[James E]

Agree with Paco, those are about my speeds, although I tend to feed a bit slower, and i take similar shallow cuts. If you start off shallower, you can always get deeper as you become more experienced.

Better than getting cheesed off with breaking a bit.

Heat is enemy no 1, as Paco says,and a solution I found on here, to the problem of reweld, was to cool the bit with air. A tiny jet right at the bit, for best effect.

My best bit is a 3 flute upcut spiral, tapers down to 1/64 in dia.

Good luck
Jim

[West Coast Sign Guy]

I've never seen 1/2" come as extruded most of the time it's already cast. Plexiglas is an actual brand, MC is Extruded and MG is Cast.

I usually use a single upspiral bit, 15,oooPRM's at 2.5" IPS

[brockadeau]

Hi-- I have a magnetic based coolant delivery system I put on my machine when cutting plexiglas or aluminum. The main difference I find with the coolant is the beauty of the the edge when I'm done. The edges look polished, the material does not melt onto the bit, and the coolant helps to keep the plastic chips from flying all over the place (I have to take my dust collector off to use the mister). I purchased mine on ebay for $75.00 and I have saved many bits while cutting aluminum instead of MELTING the substrate. I bolted a metal plate onto the spindle bracket so I can quickly place the unit in place with the magnetic base--There is a flexible and adjustable tube to the nozzle making it very easy to set up the coolant spraying directly on the bit and it is worth every penny in my estimation-- Jack

[Harry Kroyer]

Thanks for all the input.

With your help, I have gotten the cutting done satisfactorily with reasonably smooth edges and without melt. I used a 1/4" up spiral @ 12000 & 3 ips with air on the bit/surface.

Harry
Magdalena WOOD(not plastics)shop

[maxmachine]

I don't have experience cutting plastics and need to machine a piece of .5" plexi in fabricating a dust collection intake for my ShopBot.

Kindly share some info regarding spindle and travel speeds for a .5" or .25" end mill to cut holes and to cut-out the shape.

Thanks,

Harry

May I suggest polycarbonate instead of plexiglass? It is a lot stronger, and has about the same cutting characteristics.

Mark

[knighttoolworks]

here is mine for my shopbot. I started with the dc in back with brushes all around. worked better then the original till you cut at the back of the table then it was useless. but it is a very tight fit.
this mod moved the hose to the front and improved things quite a bit. but you can't sue a 4" hose. atleast for last years shopbot as there is not enough room.

[AAASIGNCOM]

I HAVE found that a .25 single flute upcut aluminum cutting bit works on almost everything but wood. i use it on aluminum, all types of plex, polycarbonate, pvc, di-bond, hard rubber as used on big machines. i use air and light mist on aluminum and engraving acrylic. also i get 50 sheets plus from this bit. remember the basics, it all about chip size and heat removal on all materials. if you are not THROWING large chips your killing your material and bit. your other 2 indicators are bit sound and the vibration you feel on the table. check your bit often with your fingernail. will it still easily shave the end of your fingernail with light pressure?