Cutting Plexiglass

[jay_mack1@hotmail.com]

I'm looking at a shopbot to cut 1/2" plexiglass? What is the best bit to use, bit speed and bot speeds?

Will I spiral downcut, 1/4" do fine?

[elcruisr]

I've found a 3/8 or 1/2 to be best in anything over 5/16. Get a bit designed to cut acrylic and go with an uspiral to clear chips unless there is a hold down issue. Probably two passes with a 3/8 upspiral o-flute finisher (slow spiral) at 2.3"/sec at 12,000 rpm would be a good start. Also see if the manufacturer recommends climb or conventional cutting. Several manufacturers make good plastics bits. Onsrud and Cormat come to mind first off. Onsrud has an excellent guide for feeds and speeds at their website.

Eric

[jay_mack1@hotmail.com]

Eric,

Do you have a bit number from onsrud?

[elcruisr]

We use a 60-243 for something like that. 3/8 dia wth 5/8 cutting length. A 60-245 woul give you 1 1/8 cutting length. These bits are best ramped in if possible although you could straight plunge for two 1/4" passes. They are also a good wood bit, we've even done a good job cutting some pressure treated pine with them! It was a what-the-heck situation and it actually worked!

If edge finish isn't as important you could use a 1/4" 63-725 and two pass the cut as well. The problem with a 1/4 tool is there will be alot of flex and this is a single edge tool as well, just cheaper. The first tool I mentioned is a three flute tool with a smoother cut.

Eric

[rgbrown@itexas.net]

Cast acrylic will break at a later date along cut induced fracture lines. Spiral bits can cause this fracture.

Acrylic cuts well with a straight flute bit, bit speed slow and cuttting speed high. If you can, cool the bit. I do not like cutting more than 1.5 diameter in one pass in acrylic and would rather have a 1 or less ratio of material thickness to bit diameter.

Ron

[elcruisr]

Hmmm, it's my understanding that the "slow" spirals are designed to prevent this. These are designed specifically for acryllic. There is barely any twist to these, just enough to aid chip clearance. We've been able to give a little finish sand and then flame polish so the cut is pretty smooth.

Ron, if you've got some technical info I don't I'd love to have it as we do this for several customers.

Eric

[rgbrown@itexas.net]

Eric,

The slow spirials will probably be fine. A "conventional" 1/4" spiral upcut WILL pull chunks fron the top edge, by experience I know this. Bits FOR acrylic have little or negative hook or rake (depending on how you learned the term) and scrape the material off. You will note the drill bits have different angles and a metal or wood bit will "break-out" the backside of the material.

The only literature I know of is a pamplet from: http://www.craftics.com. One of my friends was a plastic fabricator for about 20 years. When I have a question, I ask him.

If you are getting a smooth finish and have stress relieved the edges, I doubt you will have problems.

There is little like going back to a job where the material was special order, $374 a sheet and having the pleasure of replacing it at your cost. Impalement and crusifiction are close to the experience. BTW put another $200 or so in for freight on those sheets that broke due to raw edges....

But, do it as you see fit....

Ron

[rgbrown@itexas.net]

Eric,

I am told the sharp edges of cut acrylic, and the edges of drilled holes, have a stress thst needs to be relieved by sanding, scraping or beveling. As all of the work I have been doing lately has been large and not having polished edges, I'm not familiar with the problems created by the process.

In drilling. one can actually see the deformity caused when the object is drilled and see the material move when the hole is beveled. Remember too, that I am talking about pieces in the 30 square foot size and some larger attached to structures. A smaller piece sitting on a desk will not have the same problems.

Ron

[gerald_d]

Ron, I believe that you are talking about "stress raisers (http://www.google.com/search?hl=en&lr=&ie=UTF-8&oe=UTF-8&q=stress%2Braiser%2Bcrack%2Bconcentration&btnG=G oogle%2BSearch)" as opposed to stresses. A "stress raiser" is a mark/notch/scratch (with a tiny inner radius) that causes a stress concentration at that point when a load is applied. Cracks normally start at a stress raiser point where the stress get concentrated. (Same as tearing open a crisp packet from a tiny notch)

If you get rid of all the marks/notches/scratches then there is no obvious place for a crack to start developing. The item will be able to withstand higher loads and stresses if the stress raisers are polished out.

The actual "stresses" inside a material, before and after machining, are very low, and are not changed much by the cutting process.

[prosigns]

I've had good luck with 1/4'' spiral up carbide bits. Only because they are redily avaiable at the hardware store. I ajust the bit speed until I get nice shavings off the bit that are (Not melting into clumps) and it makes a cut smooth enough to glue the edges together with acrylic glue without sanding. Iv'e cut acrylic letters from 3/4'' material with no problems. I would like to try the acrylic bits. Maybe they will cut faster? My 2¢.

[stickman]

I'm working on a project - I bought a falloff piece of 1/2" polycarbonate sheeting. I'm cutting letters out of it.. 6" - 8" for a backlit sign. The customer and I am protyping it at the moment. I'm machining along vectors with a V-bit 60 degree... the profile with 1/4 on the outer edge to create a tab for mounting. these letters will project through the face of the sign.. to be dibond or 1/2 mdo laminated with an aluminum face. I'm using my v-carve bit to cut through the face to give the letters good seat through the material.

I was running my v-carve bit at 13,000 rpm and the feed rate at .60. When I tried to slow the bit to 10,000 the lettering had a rough chatter to it, it ran better at 13,000. I'd like to get this a little smoother... Any suggestions?

Thanks, Jay

[elcruisr]

Vee bits in polycarbonate are a headache. I did a job similar to what you are doing. The problem is the vee bit just has a marginal geometry for plastics. O flutes are the way to go but I've yet to see an o flute vee bit. We ended up doing shallow passes at a fairly fast feed to keep the heat problems down and then sanding the job with fine sandpaper before having them flame polished.

Eric

[stickman]

Eric,

I haven't had too much of a heat problem.. but I would guess that running shallow passes would give me a better finish, by not putting a load on the bit. I need to cut the face board again for the sample.. messed up the tool path, wasn't figuring my offset correctly... stood on my head to get the proper offset... I might try the shallow passes... we'll see what the client think of the inital product... Do you charge for sample work? This is a sign up on the exterior of a building, so I would see where the chatter would be seen... but that is only my though...

Jay

[elcruisr]

You might try a faster feed rate with the shallow passes. If I remember right it did help us a little. The explanation I got from one tooling wizard was that the polycarbonate material "pulls" a little during the cut and can make the chatter worse in heavy cuts. Don't know if it's true or not but lighter, faster cuts helped us. Be nice if there was a little scrap to try it on.

Sample work is tricky. If it's a pain in the @## job and I'm not so sure we'll land it anyway then I like to charge. If it's one of my regular customers who brings me lot's of good work I'm usually inclined to do it free, as long as it dosn't use up too much table time!

Eric

[stickman]

4757

[stickman]

4758

[stickman]

4759

[stickman]

4760

This is the project that I am working on currently. I errored on my letter offset for the face board, what the letter project through and I'll need to fillet any of the inside corners to match the radius of the v-carve bit. I've also cut little pieces for the interior of the letters. I'd like to cut the face board out of dibond material. But we'll see what the client wants to do.

Jay