cuting 1 inch plastic

[c_kling]

I was told that i can cut up to 1/2 inch at a time with a .25 bit can
anyone tell me the bit to use. shopbot told me one and osrude said that
would not work at .50 cut. I need to cut these parts quickly for there is
not alot in them can anyone help with the bit and speed thanks

[dana_swift]

It would depend on the plastic density.

The chip size is nearly a constant, so the amount of material removed with each turn of a cutting edge should be about 0.015 or so. The cut gets a little cleaner with lower chip loading. Feed rate is determined using the standard formulas without regard for pass depth.

With any given material the force required to part the chip from the stock is dependent on the depth of the cut. The sharper the bit the lower the forces, how fast the bit gets dull depends on the material too.

As the force increases so does the bit deflections, so accuracy suffers with increased pass depth. What is acceptable?

At some point the cutting forces exceed the horsepower available from the router/spindle. That is a hard limit for the pass depth in the material, and each material is different.

Another limiting factor is the strength of the bit, at some point the forces in the bit exceed the strength of the bit. When the pass depth is high and bit deflections are higher, the bit gets warmer from the heating of the bending on each revolution. The warmer carbide gets, the less strength it has. Bit life suffers with pass depth from heating effects.

With most of my HDPE cutting, 0.2 is a typical pass depth for my PC router. The router is "medium" loaded at that point from the sound it makes. 0.5 is probably possible, I don't think I have ever tried it.

And lastly the CEL "cutting edge length" of the cutter matters, a free 1/4 inch or so above the material edge is needed to clear chips. More is good, but longer CEL's weaken the bit. Another trade off that is learned with experience as to what works with any material.

With other plastics such as various foams, a half inch pass depth would be no problem.

Interesting question, whatever your material is, you will learn that 1/2" is too much or too little.

A good experiment is to design a test cut that starts at 0.1 and increases 0.1 each second cutting a straight line. When the router reaches max load you can hear it. Abort the cut, and note the cut depth you reached. It is possible to break the bit first of course.

If you find your bits breaking after a few minutes of cutting, then the heating and work-hardening of the bit have become the limiting factors.

Good luck-

D

[jerry_stanek]

You didn't say what kind of plastic. Is it acrylic cast or extruded? Plexiglass can be tough to cut because of the rewelding. Sintra is easy to cut but I still only cut it .25 a pass with a .01 offset and a cleanup pass. 1/4 inch bits flex a lot when trying to cut to deep.

[rcnewcomb]

Dana,

That was an excellent write-up. Thanks!

[dana_swift]

Thanks Randall.. whenever I write something like that, I wish later I had added 4 other relevant topics, and not mentioned one or two others.

Posting is like that I suppose..

D

[c_kling]

thanks dana what you said makes alot of sence .I ran in to alot of things you said .i am cutting acrylic cast.I have cut plexiglass but i cut .25 depth at one pass with a .25 bit
and was told somthing els. what you said matches what i know but the way you layed it out i can try to get as much as i can

[2talltary]

Best way if you are cutting plexiglass (acrylic) is to go slow and careful because it tends to be brittle. If you would need a substitute try polycarbonate. It is 25 times stronger than acrylic and machines better too.

[Xray]

I cut alot of .25 plexi, I usually use a 1/4 shank ball nose spiral which tapers down to 1/8.
16,000 rpm's, I've neve rhad any problems rewelding or breaking, and I have cut some fairly intricate shapes.
Offhand, I don't see what that wouldn't work with .50 ,,, And of course, the bit doesn't need to be tapered. Point is, I prefer ballnose to endmills for plexi cutting.

[dubliner]

Why ballnose? for a "soft" entry into the material? On first read I thought you were carving Plexi.

[Machinist-Mike]

Some of you have posted info and questions about machining of Plexi. First, Plexi or Plexiglass is just a brand name for Acrylic. Second, there are two major varieties of Acrylic, Cast and Extruded.
The Cast material is excellent for machining. The extruded becomes 'gummy' at a much lower temperature due to the additives used to extrude the resin.
Thickness tolerance on the Cast is much greater (+/-15%) and can vary widely in the same sheet. This is because the Cast is poured as a liquid between two sheets of glass and then cured. The extruded stuff has a great thickness tolerance and is very consistent within the same sheet. I use the extruded stuff for some fabrication I do that needs to be bent - lower temp than cast - so it forms quicker.
Both look the same. Ask for CAST if you want to machine without the gummy stuff. Sharp tools and greater relief angle helps.
I have bought from the places listed in this forum. Both Industrial Plastic and High Tech Plastic. The metals guys don't have a clue about the differences between plastic materials. You can probably get the Cast Acrylic from any good plastic supply house though. Good luck.
Hope this clears up some stuff for 'Plexi' machining.