PDA

View Full Version : Need help reducing chatter lines in acrylic



eklug
01-22-2007, 01:08 PM
4777
I have been cutting out templates for grinding moulder cutters. They are cut out of .18" acrylic using a .05 straight bit. The machine is running as slow as it will go (10000 rpm and .05 ips). We need the template to be as smooth as glass. Currently our tooler files these edges down with a diamond file. It would be much more efficient if we could get a smoother cut from the get-go. Any suggestions?

wcsg
01-22-2007, 01:19 PM
Are you using CASt acrylic? I would use a Spiral O bit by Belin. What is your hold down method?

You can do two two tool paths. Kind of lie to the machine and tell it you have a .28 bit (If your using a .25 CED) then do your second profile as a true .25

A 3/8" or 1/2" bit can be a better edge quality if your part will allow it.

Also their are specialty bits to do a final pass on to help smooth over. But other factors can be mechanical or even software. Too many nodes in your file or improper seating of your bearings on x,y & z axis, etc etc the list can go on.

elcruisr
01-22-2007, 02:13 PM
A .05 tool, is that correct? That tool would be flexing like mad while cutting. Use a polished O-Flute spiral designed for acrylic in the largest possible diameter you can then make sure that the machine is tight mechanically. That would make a big difference. Some hand finishing might still be required but not as much.

richards
01-22-2007, 02:28 PM
Emily,
Are you using an Alpha? The chatter in your photo looks exactly like the chatter that I always got with my Alpha before installing 3:1 gear boxes on the motors. Even now, with acrylic, I still get some chatter, but now that much.

I'm assuming that the .05 inch bit was a typo, and that you're really using an 0.500 inch cutter. Both Eriks gave good ideas. Personally, I use an O-Flute spiral like Eric Lamoray suggests. I also do my first cut as a climb cut and then repeat the cut as a conventional cut. The cutter seems to flex about 0.020" away from the true path when in climb mode. Following it up with another cut in the conventional mode cleans off that 0.020".

paco
01-22-2007, 02:35 PM
I agree with all the above and mostly with the "your photo looks exactly like the chatter that I always got with my Alpha". That's pretty much what you can get with the 1:1 ratio and 3.4.X SB3 control... unfortunately...
A final very slow finishing pass (slow RPM too) might help some more.

eklug
01-22-2007, 02:55 PM
No that bit size is correct. A .05 bit. We have to do very tight corners on the templates in order to match the dimensions and profiles for the finished mouldings. we can't use a larger size for 95% of the templates we need. Even a .125 would be much too large. I would slow it down more but i cant go any slower. I do have the PRT alpha and we also have another shopbot with a colombo spindle but that one has horrible scallop marks when cutting diagonal and just as much chatter as the router. (I have to have maintenance look at the pinions on the spindle cnc to see if we can get rid of that scalloping). I cut the entire piece as a climb cut in order to get the cleanest cut on the finished piece and the bad edge on the waste. I screw the piece down to the spoil board. Several screws on the waste and one or two in the center of the template. The acrylic shavings pack the cutout very tightly so the piece is very stable. I think what we will finally end up doing is outsourcing our templates again. We used to go through somebody that had a laser cutter. They only cost $35 each and honestly we are probably spending more doing it ourselves. We have problems sending them our CAD files intact and usable for them (we use turbocad).

wcsg
01-22-2007, 03:43 PM
I would have to agree to have this work lasered, way you ge a polished edge too. But you should only be getting charged $100-150.00per hour

benchmark
01-22-2007, 04:10 PM
Hi Emily

We have produced cutter templates on the Shopbot. The method we use is a 45D V bit and an engraving strategy using VCarve Pro, this will give you sharp internal corners for the grinder to follow.


Paul

edcoleman
01-22-2007, 04:24 PM
Emily:

I agree with Erik - a laser would make quick work of this. Estimating the size of the piece based upon your picture, it would probably take less than 2 minutes on the laser table. If you're supplying a laser ready CAD file (which turbocad certainly is), then the $35 is a bit high. I'd be glad to cut them for you (the only problem would be shipping, I'm in NJ - it might make sense only if you are doing a bunch to spread the shipping cost). Drop me an email (ed_at_colemanwoodworking<dot>com) if you're interested.

-Ed

mklafehn
01-22-2007, 08:16 PM
Emily,

I have a laser machine that could do those pieces for you. I am located in Chicago, so shipping would be minimal. I agree with Ed, that $35 is a little high if everything is set up.

I'm not looking to compete with Ed, but if it saves you money on shipping then maybe I can be some help.
my email is images@digicomimaging.com

Send me a sample file and I will cut you a sample at N/C to see if this is what you are looking for.

GlenP
01-22-2007, 10:10 PM
Emily, I have used a propane torch to smooth or barnish an edge of acrylic before. If you do quick passes and not too close it will smooth out the cut perfectly. Just don't heat too much that you melt it and distort your piece. If you have more than one piece, stack them up and tape together and barnish them all at once.
gp

eklug
01-23-2007, 08:31 AM
Thanks Glen for your advice. We have tried that and the results were not so good. We did several quick passes but the radiuses and other critical dimensions began to melt and disort before all the ridges had disapeered.

Thank you Ed and Mike I will discuss those options with my boss.

Brady Watson
01-23-2007, 09:54 AM
There are a few things that I have found work well with acrylic:

1) Your artwork/drawing. Make sure the vectors are clean, with the least number of nodes possible. Drawings created in PW or ArtCAM are generally cleaner than those done in AutoCAD, since ACAD DXFs only used straight lines.

2) Be sure to use the arcs_inch post when saving a toolpath file. Curved cuts are generally smoother using the arcs post than the straight inch post.

3) I typically cut acrylic @ 13,000 RPM, 2 IPS with a .0625" stepdown using a 2 flute spiral O cutter from Onsrud. The reduced stepdown keeps the part very accurate & edges are very smooth with no visible stepdown marks. Use the largest cutter you can to reduce deflection.

4) Material hold down is paramount. Screws and/or clamps are NOT adequate. You must use either an adhesive tape (carpet tape) or vacuum to effectively hold the parts down to prevent vibration trasferring to the cut.

While you will still get some minor marks around some curves, you won't have to make excuses for your work. At least this is what I have found using the formula above.

-B

stevem
01-23-2007, 07:20 PM
Your spindle speed is too low for that size bit. The speed should be around 25,000 rpm with a feed speed of 15 ipm. Stepdown should be no more than 50% of bit diameter for the rough pass. Leave .005” of stock on the rough pass. You should be able to do a full depth, climb, finish pass to final dimensions.

Flame polishing will not remove any ridges. The surface must already be very smooth for flame polishing to work.

You may want to try using a bit with a larger diameter where the design permits, while using the smaller bit only for the tight spots.

Forum Admin
02-16-2007, 08:07 PM
Several messages have been removed. Let's get back to suggestions on how to reduce the chatter lins. Personal attacks are not allowed here.

rhfurniture
02-17-2007, 09:15 AM
"ACAD DXFs only used straight lines."
There are certain types of geometry that Autocad does convert to straight lines before exporting as DXF. However I have just tested polylines, arcs and splines, by exporting as R12, into partwizard, and out as part files and they all produced paths using the CG command (ie arcs).
I am posting this so that people who use autocad to produce their geometry (as I do) do not form the impression that they have to buy other software in order to get accurate results (which is the goal of us all).

R.

bob_healey
02-26-2007, 02:44 PM
Emily:

Erik was right on the money in your first reply. Belin spiral O's are made with a proprietary micro-polish process, and are specifically designed to solve this problem. I have many clients that can attest to this.

Bob Healey