[Gujustud]

I'm starting to do more acrylic work at the shop, and was wondering whats the best way to cut acrylic? Mainly sheets, anywhere from 1/4" to 1".

I'll be doing this on either a Haas VF2, or VF7. Btw, I should be more clear when I say cutting, but milling parts out of the sheets.

Thanks in advance!

btw I wasn't sure where to post this, so please move the appropriate section if needed.

[Rekd]

I moved your thread here from the announcements section.

Cutting acrylic is not too bad. Use sharp cutters, avoid excessive heat, (melted plastic built up in flutes makes for nasty burrs! ), and try to cut into the material to avoid chipping as the end mill breaks out.

HTH

'Rekd

[KingPANO]

Make sure that your acrylic/plexiglas is a cast plastic not extruded. Extruded is noted for the melting and wrapping around your endmills. I cut cast acrylic with a 1/16 bit 30-40ipm rough with 15 ipm smooth pass. I get great results.

Bill

[marvinstov]

I don't know much about acrylic. How do you tell if it is cast or extruded?

Marv

[KingPANO]

Originally posted by marvinstov
I don't know much about acrylic. How do you tell if it is cast or extruded?

Marv

75%-90% of the time if the paper on the acrylic has writing on it is extruded...ie. the cheaper version of acrylic. I've ruined more bits by using extruded plastic. Cast is the more expensive but worth the .50-.75 extra per square foot. I have a good relationship with my local plastic fabricator and he gave me the tip.

Most of the plastic places will have a scrap bin that they will let you rummage through for a dollar a pound.

Bill

[Gujustud]

Originally posted by KingPANO
Make sure that your acrylic/plexiglas is a cast plastic not extruded. Extruded is noted for the melting and wrapping around your endmills. I cut cast acrylic with a 1/16 bit 30-40ipm rough with 15 ipm smooth pass. I get great results.

Bill

Good call (on cast vs. ext).

1/16 at 30-40ipm? How deep?

[KingPANO]

I cut about 0.1 each pass. The smooth pass takes off 0.02...with great results.

I've never cut wood or aluminum on my machine...only acrylic and HDPE. I'm entertaining an idea of making a collet out of aluminum for a larger router than my rotozip.

Bill

[Laff Riot]

May want to take a page from new hermes book and use a large laminate router with a 3" wheel on the end - they transfer the rotation using a rubber belt to the small spindle head increasing the rotation at the spindle by 2x the router speed.

I like this system as the bits are the only thing that get sacrificed when you bite into something. If the bit gets lodged the rubber band will break or spin freely without damaging the router.

If you need pics of this lemme know soon - I am getting the NH machine out of my shop in exchange for a laser. Will only have it for another cpl weeks I hope.

Like Rekd said cut into the material - commonly this is done by reversing your curve in your generation program or selecing climb cutting if you have the option. This leaves all the melted chips on the side of the waste substrate not your cutout piece, you will still have some flecks that need to be knifed off but the final edge can be cleared again using an oxygen torch and light passes.

[boxwood]

Hey guys what material for lithopanes, I had read acrylic so bought some on ebay called called plexiglass acrylic (clear) but when I cut the picture doesnt look anything like a lithopane! shoulf it be colored? what color, also read corian is good but isnt that stuff solid color so no light gets through and its thick from what I saw at HD any in put would be greatly appreciated

[DareBee]

I have not milled acrylic but am familiar with polycarbonate, I find it works best with coolant. Considering you are doing this in a VMC maybe you could give it a try and then it won't matter if it is cast or extruded.

[ger21]

Corian is translucent, the thinner you cut it the more light will show through. It would need to be backlit, though.

[miljnor]

I like this system as the bits are the only thing that get sacrificed when you bite into something. If the bit gets lodged the rubber band will break or spin freely without damaging the router.

For this to work right don't you have to have some mechanism to stop the forward Feed of the machine.. I don't think most machine tools care if the cutter is there or not (Ba$tards ). An overload sensor or something?

[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