Cutting Acrylic

[ImanCarrot]

I get a perfet optical finish on acrylic, polycarb, CR39 and MR7 plastics (I make aspheric lenses for various applications). I use Single Point Diamond tools, available from Countour Fine Tooling and Apex (Countour is in the States too). Feedrates etc are below:

Spindle speed: 2K-4K rpm
Tool radius: 0.020"- 0.040"
Top rake: 0- 5 deg
Front clearance: 15 deg
Depth of cut: 0.0004" to 0.040"
Feedrate finish cut: 0.2" to 1" per min

Clairsol 310 is a good coolant, but only comes in big drums so I use WD40 beleive it or not. This can be cleaned later using methanol and tissue.

[PEU]

ImanCarrot, your post triggered my curiosity

My other hobby is making flashlights, so I'm super interested in how you cut policarbonate/acrilic for optics making. Do you have pictures of your work? (you can see my flashlights here: www.neoca.com.ar)

Thanks


Pablo

[ImanCarrot]

Peu: Nice torches, I liked the photos of the setup stuff too- nice to know that Machine Shops are the same the world over

I have left my digital camera at home, so will post some piccies tomorrow, but basicaly these lenses are used in military and commercial applications- they are mostly aspherics meaning one lens replaces many lenses that would be otherwise needed (cuts costs and assembly time, decreases light loss).

Anyway will post some tomorrow.

[ImanCarrot]

Here you go... some lenses I'm making at the moment. We can pretty much make any lens (aspheres, spheres, concs, elipses etc etc).

[PEU]

Waaay cool. Thanks for sharing!!!

[MauserBob]

About 90% of everything my company makes is either acyric or polycarbonate. What we make is out of sheet stock, not blocks or bars, etc...we laminate 5 or 6 3/4" 40x20" sheets of acrylic together using resins and then bolt the whole thing to the machine table. Next we run our part program, cutting into our new laminate tabletop. This produces a pattern upon which our work will be done. Due to the fact that our parts rarely ever exceed .250" thick and are usually bigger than 6" x 6" in size, we cannot hold the workpiece in the traditional manner, so we use tape instead. Yep, I said tape. A brand called "polyken" which is somewhat like duct-tape, having the same sticky properties, but also possesing better accuracy in average thickness. We tape the perimeter of our pattern (the o.d.) and then we can place our raw cut (oversized) parts down upon the tape and apply pressure to seat it tightly. For this reason we cannot use coolant, so we run dry, and we never haev any finish problems to speak of, nor melting for that matter. We usually run 1/2" 2flem carbide strtflute tools @ 12,000 RPM and 70-100 IPM, with no problems at all. Tool wear and spindle load are virtually non-existent (it's like machining butter) and as long as we take a diamond stone and radius our tools ever so gently (about .010" radius per tooth) we get excellent finish on our poly and acrylic parts. Someone mentioned SHARP tools, and this is a must...acrylic generally wants and NEEDS a more acute cutting angle AND as much flute depth as possible, otherwise it'll chip-out. And when goiong around corners acrylic will chip-out so we always conventional-mill all our acrylic. We regrind and resharp our tools in-house...saves on tooling costs. Due to the aforementioned relative thinness of our parts (@ .100-.200" thick) we usually only use the first .300" to .500" of flute length, so instead of chucking the tool when it's dull we cut the used-up portion off with a diamond cutoff wheel and then regrind the toolface. Using a traditional 2" flute length on our 1/2" carbems, we can do this 5-or-6 times before the tool has no life left in it. Really saves on tooling costs. I wish I could tell you what angle we grind our tools at for acrylic, but our tooling grinder scale doesn't read angles in the usual manner, so our numbers won't mean much to you, but think about it like this...polycarbonate likes an AXE, but acrylic needs a SCALPEL.




Rob.

[the_paco]

How about the right tool?!... O-flute (that's single flute), spiral up if you use a vacuum setup; that may help with 1/8" CED and smaller... and use the shortess CEL possible to avoid any chatter (and breakage).

[XLR84x4]

I'm just re-reading through this old thread to get some ideas of where we are going wrong.

Firstly we wish to machine 1mm ploycarbonate approx size of part is 150 x 360mm. We have made a jig to hold down this part however today we machined the jig to incorpoarte a vaccum hold down.

The vaccum table is working great pulling -100kpa on the materal however using our 4mm two flute spiral end mill with spindle speed of 10000rpm and F2500 the moment it starts to cut it pulls the material up from the job. We are doing the cut in one pass and it is chatter that is also breaking the vaccum

What we are thinking is that a straight flute cutter of similar size may stop the poly carb climbing the tool.

I would like to hear of other peoples sucesses with tools/speeds and feeds

Jason

[Jaime128]

I just bought a scrap of cast acrylic sheet, but I was wondering what you guys recommend to cut this? Table saw, band saw, etc? I don't have either, but I'm thinking of getting something, if table saw, what type of blade do you use? I already bought an 80 tooth blade for the 10 miter saw, but that would still cut wide, hence the reason for the question on here. I know I need something with a small table to make a clean cut, but I've never cut any of this stuff until now. I want to make a filter for my lcd because even with the low settings this thing is still pretty bright. I love my old one, but that was on a crt.

Unfortunately the sheet is thick, 4.5mm is what the label says. It's light smoke and I checked to make sure I could see through it so that works. They didn't have anything thinner on the scrap not to mention the see through light smoke. I don't even know how well I will be able to bend it with the heat gun, but I need to make a filter for my lcd, it's just too bright and well, they don't sell anything cheap like this, so I'm making one. Any thoughts are appreciated. Thanks.