Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: FirstLook37 on April 15, 2009, 11:08:41 AM
-
I am trying to route a logo into .220 Clear Acrylic. I am using an .125" End Mill bit and i'm only plunging .09375" into the material. Can anyone give me advice on what my feed rate, spindle speed, etc..etc.. should be in order for me to get a smooth cut? Ive been toying with it but it seems everything i try still comes out poor. The acrylic is basically melting and re hardening where i'm cutting. The edges are coming out not as smooth as I'd like. Acrylic isn't cheap- so I'd like to stop this shoddy work! Please help acrylic masters!
Thanks- Brian
-
I have done acrylic quite a few times and its always come out well but it was on the Bridgeport with flood coolant. If you dont have coolant maybe spraying some WD40 would help.
Hood
-
I'm running a spindle without coolant- so spindle speed and feed rate don't matter much?
-
With flood coolant it wouldnt really matter too much as long as you were not going too slow for the feed. Sorry I cant be much more help as I have never tried without the flood.
Hood
-
I am trying to route a logo into .220 Clear Acrylic. I am using an .125" End Mill bit and i'm only plunging .09375" into the material. Can anyone give me advice on what my feed rate, spindle speed, etc..etc.. should be in order for me to get a smooth cut? Ive been toying with it but it seems everything i try still comes out poor. The acrylic is basically melting and re hardening where i'm cutting. The edges are coming out not as smooth as I'd like. Acrylic isn't cheap- so I'd like to stop this shoddy work! Please help acrylic masters!
Thanks- Brian
If it's melting, then you need to reduce RPM, and/or increase feed. But, to get the best finish, you want higher RPM and lower feed, so best results do really require coolant. Just air might suffice. It might also help to use a very high helix cutter. You should be able to find tooling made for plastics.
If you're looking for a really smooth finish, do the best you can with the router, the flame polish to remove the machining marks, which will leave the cut surfaces clear and glossy, just like the unmachined surfaces. You can do this with a cheap propane torch set on a pretty high flame. Hit it *just* long enough for the surface to gloss over, then move on, before it catches fire. Takes a little practice, but leaves a really ncie finish when done right.
Regards,
Ray L.
-
Hi, From your description"I am trying to rout" i assume you are using a router which is probably 10k rpm or more.
I cut acrylic on my router using an onsrud or micro 100 1 flute (The Onsrud is super- o flute) I have cut through 1/4" in one pass. at 30"/min 10K rpm. The Edge or bottom finish, if not a through cut are great.
What I would suggest is, increase the feedrate A LOT, use compressed air to blow the chips out. the problem with an endmill on acrylic is the chips don't come out fast enough and stick to the cutter or the work piece.
You need the chips to come off and carry the heat with them, not the chips to heat the cutter.
Hood's solution of flood cooling works if you have that option too, But my MDF table is not conducive to Flood! :)
hope that helps,
Cutmore
-
I am operating with a 6hp spindle. If that makes a difference.
-
It also makes a big difference what type of acrylic you are using. Cast acrylic is best for machining, extruded has a much lower melting point. There is also tooling specifically designed for routing/milling plastics as well.
-
Just general stuff:
Definately test any coolants on the acrylic before use. Some oils can cause permanent discoloration, clouding or even micro stress cracking in certain plastics . . . including arcylic.
Constant stream of high velocity compressed air, single flute cutter (two flute at most)
Consider using polycarbonate instead of acrylic.
-
What is the best router bit for this application? I've been told single and or double flute - O Flute? Any suggestions?
-
If by 0 flute, you mean a burr type cutter (for fiberglass/carbon fiber. etc) definately not.
I would suggest for acrylic that you use high speed steel straight single flute.
You can use a two flute spiral cutter if your stock is thick enough to not try and climb up the cutter. It will be really tricky if you have a high speed spindle. When I have to cut plastic, I use the fastest feed that does not check up the edge and the fastest spindle speed that won't melt the plastic . . which is usually still pretty slow.
I much prefer Polycarbonate as it is harder, stronger, and cuts fine with two flut end mills. Best again to use high speed steel made for aluminum which are high helix and poilshed.
Avoid carbide insert or brazed carbide cutters for soft plastics like acrylic unless you have some method of putting a razor edge on the carbide.
No matter what cutter, the best thing I have found for success is LOTS of very high velocity compressed air to keep the tool and the plastic cooled down and keep the chips from recutting or sticking to the tool. I've never used fluid on plastic so other than the caveat I mentioned previously, I can't comment on it's effectivness compared to air.
-
Apparently, Canola cooking oil when used with a misting system has good results as a coolant / lubricant when cutting acrylic and alluminium. I have used a dilute mix of Methelated Spirits and water, sprayed on with a hand spray bottle, as a coolant also with some success. (keep it wet) ( be careful of spark swhen handling the metho!). I agree with he other comments, you need to keep the chip loads high to allow the chips to take the heat away from the cutting tip.
Bruce
-
Lots of info here,
http://www.plasticrouting.com/Van.asp
Greg
-
I'm new here and just a hobbyist with this, but I spent weeks on this as 95% of what I'm currently working with is Acrylics. I found as someone else said, you need CAST Acrylic and be careful, even some vendors or their employees don't realize the difference or it's not real clear what they are selling. TAP sells only cast, a little pricey, but it will be cast. I'm using 2 flute carbide bits I purchased from Precise Bits and I'm generally using bits 3mm and under. For example, I run a .1181 2 flute end mill at around 8-12 ipm with the router speed around 25k with .04 passes and I get gorgeous chips with a nice clean edge. I'm using no lubrication and having zero issues, sorry I can't help with extruded, I gave up on it as I couldn't come up with the right combination and using cast is so much easier.
-
We are cutting acrylic successfully with O-cut (single flute) cutters. Keep the plunge moves slow to prevent the acrylic broken only. Speed is around 18000 rev/min . Spindle concentricity is very important to get smooth finish.Othervise you will see rough surface. With 5 mm cutter you can go 25mm/sec. Last thing do not use climb milling. Conventional milling gives better result.
-
Like it has been said here, you have to use razor sharp cutters for plastics. High helix cutters designed for aluminum work well. The feedrate should be very fast - about 3 times faster than for aluminum with a given cutter diameter and spindle speed. For example, I am limited on my mill to 2000RPM, and I found that a feedrate of 600mm/min with a 6mm cutter gives a nice finish.
Daniel