Still trying to master acrylic. Still not happy and need help!

[ColdBlooded]

I have been experimenting with different bits cutting .177 and .22 clear and black acrylics. Trying to get a cut that will not require edge prep before gluing. So far I have not been happy. I will list the bits I have used and a 1 - 10 rating on the edge finish. 10 being the best. Does anyone have any other suggestion in my quest for a perfect 10? I have tried many different speed/feed with these bits and have not had much of a difference in edge quality. I am using vacume hold down, pressure foot and just to make sure my stock is not moving at all spray adhesive.

Harvey Tool

Plastic Single "O" Flute Up Cut 1/8" # 51508 my rating 6
Plastic Single "O" Flute Up Cut 3/16" # 51212 my rating 5
Plastic End Mill Up Cut Spiral 2 Flute 3/16" # 48712 my rating 3
Plastic End Mill Strait 2 Flute 3/16" # 14612 my rating 7 (best bit overall, so far)

Amana Tool

Plastic Single "O" Flute Up Cut 1/8" # 51410 my rating 6
Plastic Single "O" Flute Up Cut 3/16" # 51412 my rating 6

Onsrud

Acrylic Single "O" Flute Up Cut 1/8" # 63515 my rating 6
Acrylic Single "O" Flute Up Cut 3/16" # 63520 my rating 5

If you have another bit recommendation please list model # and the speed/feed you are using to get the best edge finish.

2nd problem

I am also using a Amana Tool In-Groove CNC Insert Engraving Tool with 90° V-Tip Engraving Insert Knife / 0.04" tip width. Does anyone have any tips for speed/feed to get a clean cut .02" deep engraving in acrylic without the white tool marks.

Thanks for the help.


Thanks,

Brendan

[jerry_stanek]

I watched this video and learned some about cutting different materials. Speed and feed with what cutters.

http://www.youtube.com/watch?v=_b5I3H2Hp6M

[steve_g]

Brendan:

I have success with just about anybody's "O" flute. Cast and extruded Acrylic cut entirely different, and clear cuts different than black. you just have to play with speeds to see what works with this manufacture or that one. That said, I still have to use a medium bodied solvent cement.

Good luck!

Steve

[ColdBlooded]

Thanks for the video. All of the acrylic being cut in the video was then followed up by a Mono-Crystaline Daimond Pollisher. Guess I am getting the best cut I can, just never thought of using a 2nd tool to clean up the edge. Looks like I will be ordering some new tooling today. Again thanks for the video. Have you used a polishing tool yourself? Do you use the same tool path or a finishing path after your cut?@

[ColdBlooded]

I take that back, at $1800 for 1 bit I will keep looking for a better cutting tool. WOW! Is there anyother finishing tool options out there?

[jerry_stanek]

I should have mentioned that I checked on the price about a year age and it was about $1500.

[Brady Watson]

Give an Onsrud 3-flute finisher a try. It is an upcut spiral O flute with 3 cutting edges. Works lovely in soft PVC to acrylics. Go 3/8" on the diameter unless you really need to go smaller. Make sure your machine is clean & tight and that you have an excellent hold down on the material.

-B

[jerry_stanek]

At work we use a 1/2 vortex bit

[Rick W]

Hey Brendon,

Try your #7 bit
Plastic End Mill Strait 2 Flute 3/16" # 14612 my rating 7 (best bit overall, so far)

Cut the piece out two times (the first time don't go all the way through or use tabs whatever to hold the piece in place). On your second cut take off a hair
(make sure you cut in the right direction on your second cut). Basically what you will be doing is creating space so your bit isn't cutting on both sides creating friction. I've cut a 3" letter A out of 1/8" plexi (extruded) using a cheap cobalt two flute 1/8" down spirol (one pass 2 depths) MS .75,.5 depth.0625 per pass.
Hope this helps and is explained properly.

[ColdBlooded]

Hey Brady, thanks for the suggestion. Do you have a series # or model # for your recommended finisher? Harvey Tool has what looks like Onsruds Diamond Finisher ($1800) for only $180. Have you ever worked with these tools? The video shows it finishing a very nice edge. If they really work that good it may be worth the $1800. Just don't want to gamble.

[Brady Watson]

Brendan,
No doubt Harvey makes some really good stuff. The diamond tools are nice because they polish the edge some on the cut because of the micro 'grit' of the diamond. I would not spend 1800 beans on ANY tool & I really don't think that you need even a diamond coated bit, but it would not hurt for doing your own R&D for the type of work that you do. I'm sure that I've spent well over $7500 in diamond tooling in the past couple of years, and none of it was for acrylic.

I like the Onsrud 52-650 and 60-249 (2 and 3 flute spiral O upcut) for acrylic. The trick is to hog out material with allowance, leaving maybe .02 on the profile and bottom of the part. Then come back and shave that .02 off in a single step down to eliminate waterline marks. Don't go less than .02 because the tool will not be able to really pull a chip off and it will have more of a tendency to melt. I forget where I read it, but I saw something that backed up my own research pursuant to leaving enough meat on the part on the final pass.

These things are absolutely essential when cutting plastics:

1) A well tuned, tight machine with relatively fresh pinions.
2) A powerful vacuum hold down setup.
3) The correct tooling run at the correct range in MS & RPM
4) Adequate chip extraction, which aids in cooling.
5) Thoughtful CAM programming and execution.

What issues, exactly, are you having with cut quality?

-B

[kaaboom_99]

HI Brendan.
I don't normally chime in because my PRT is orphaned in another province and I'm out of touch.
But I will offer my CDN $0.02 for what it is worth.
I spent 4 hours one afternoon with a "Plastics" man in his fab shop.
He primarily used cast acrylic for his line of work, cleaned and polished edges with a hydrogen torch (it has the cleanest flame). All his stuff looked like polished glass.
Straight cuts were done on his table saw. Nothing special. A quick pass with the hydrogen torch and all saw marks were gone.

Good luck!

[Rick W]

Hey Perry,
Just for the record, it is not advisable to glue acrylic after it has been flame polished, it could craze or crack. You could glue the saw cut acrylic though.

[MogulTx]

Brady,

Another question in the same vein:
I am doing some acrylic stuff (fairly simple, edge lighted sign).

I am usign a Whiteside 1/4" x 90 degree V Bit (works pretty good for V carving letters) and an Onsrud 52-190 ( 1/4" down spiral)... works "fair"...

If I were to switch to something in the same geometry style as the bits you are using, but with smaller diameters- I am assuming that that is what you would recommend for smaller cuts, correct? I need to do a little better on the detail quality and not get any chip outs when I do a clearing cut on a larger area ( which I am having a small amount of with the 52-190.) Do you use a similar V bit? Any other recommendations?

The 52-190 does show the machining paths in the cleared area, but I think that is just a "necessary evil" as far as I can tell... Other than leaving white, hard (heated then cooled) acrylic behind ( speed and feed adjustments) I have been fairly pleased with the performance, but the idea of clearing and then finishing with a modest path seems very logical.

Thanks for your input here on the forum.

MGM

[Brady Watson]

You NEVER want to use a downcut bit on any type of plastic. It doesn't pull the chips out & can cause the bottom edge to shatter. You also NEVER want to use a downcut bit for doing pocketing/area clears since it will give you a poor finish. Straight or upcut spiral is the way to go. I don't know the number off the top of my head, but Onsrud makes a spiral-O specifically for getting a clean bottom finish when pocketing. Sniff around and see if you can find it.

Yes - you can certainly use smaller bits to get the detail, but the rule of thumb with acrylics is to use the largest diameter bit you can to get the chips out and to reduce cutter deflection and vibration. 3/8 is a nice size for general cutting. I've gotten good results with a regular 2-flute carbide end mill as well, but the O-flutes do give a better result. If you can't get an O-flute in the dia you need, just use a fresh sharp end mill - no HSS - carbide only.

Now...if you want to do a little R&D on your end, rig up a cooling setup in one of two ways: 1) Get a 'football inflator needle' (Husky blowgun kit @ Depot) and cobble together some 90 deg elbows, a close nipple and long nupple and fasten it to your spindle/router so that it blows right on the bit. You won't be able to run dust collection. Set PSI @ 20-30 psi and tape off the safety hole on the inflator. This should eliminate any white marks provided you don't use a downcut bit. OR...2) Put some denatured alky in a spray bottle and spritz the area to be machined. Do a test first. If it deglosses the plastic, then it is a no-go; switch to rubbing alky. (I doubt you'll have trouble with the denatured) - Evaporation is a cooling process, so as it evaporates, the plastic will cool. Just use caution as it is flammable and you wouldn't want to run dust collection on that setup either. Either will produce better results...although with the right bit, the DC should cool things enough to get a clean edge.

Don't underestimate the importance of fresh lubricated pinions and a well adjusted machined. This includes your VR settings in SB3. You want to minimize shock loads @ direction changes, but at the same time, you don't want the tool to dwell in the corners either. A default Slow Corner Speed value of 65 can be pulled down to 45 to cushion the corners a little and reduce bit deflection - which means better edge & bottom pocket quality.

-B