If your cuts are like a tuna can, I suspect there is something amiss with your machine. Not getting your settings right or using a dull bit can do that. You might even have excessive machine flex, or even machine slop due to wear of parts. I just had to replace some gear rack on one of mine last Thursday. Think about it, if you have a lot of wear somewhere, that will translate into sloppy movement, that will translate directly to your cut. Check out all your components and see if there is any slop due to wear.
-
I want to thank all the members that have upgraded your accounts. I truly appreciate your support of the site monetarily. Supporting the site keeps this site up and running as a lot of work daily goes on behind the scenes. Click to Support Signs101 ...
Clean edges on cnc routed dibond
- Thread starter jhd
- Start date
We cut alot of brushed acm at my shop.
I typically run a 3/16" Belin bit. On 3mm acm I'll run 2 passes. 1st pass at 150-220 ipm cutting .111 depth. 2nd pass at 220 ipm .125" depth with a .015" width. This is at 16000 RPM. With a smooth and flat sheet of MDF spoil board for a proper vaccum.
The clean pass takes off .015" off the side and finishes the cutout of the finish piece.
With ACM, alot of time if the cut isn't clean it's because your feedrate is too slow. The material is very soft and easy to cut for a sharp bit. Don't be afraid to ramp the speed up. Also, it's important to use an accurate caliper. We use a calibrated Mitutoyo. Had trouble getting accurate readings with cheap alternatives.
Hope this helps, I've had to spend lots of time sanding down edges before I figured it out. Now they come out clean everytime.
I typically run a 3/16" Belin bit. On 3mm acm I'll run 2 passes. 1st pass at 150-220 ipm cutting .111 depth. 2nd pass at 220 ipm .125" depth with a .015" width. This is at 16000 RPM. With a smooth and flat sheet of MDF spoil board for a proper vaccum.
The clean pass takes off .015" off the side and finishes the cutout of the finish piece.
With ACM, alot of time if the cut isn't clean it's because your feedrate is too slow. The material is very soft and easy to cut for a sharp bit. Don't be afraid to ramp the speed up. Also, it's important to use an accurate caliper. We use a calibrated Mitutoyo. Had trouble getting accurate readings with cheap alternatives.
Hope this helps, I've had to spend lots of time sanding down edges before I figured it out. Now they come out clean everytime.
jdwilliams1
New Member
Superior Adam, you are cutting 3mm ACM at 8 inches a second with the smaller router head? Also what type of life are you getting out of the Zund 154 bit?. Are you pre printing and then cutting with registration?
Superior_Adam
New Member
I am sure I pulled those settings right off the machine. I get a long life out of router bits on ACM as it is a pretty soft material.
MikePro
New Member
Belin is still my favorite brand. 33317(.125")/33475(.188")/33635(.25").
huge fan of multiple passes for clean edges, or at least a singlular roughpass halfway through the material at a ~.03"+ offset so the metal chips have an easier path to flow-out when doing your final part cuts.
huge fan of multiple passes for clean edges, or at least a singlular roughpass halfway through the material at a ~.03"+ offset so the metal chips have an easier path to flow-out when doing your final part cuts.
fixtureman
New Member
I just cut a bunch of circles in Komalu with a 1/8 straight cut bit they came out without having to do anything. I ran the machine at 9000 rpm and 200 inch per min here is the bit I used
JBurton
Signtologist
Gotta love Belin's, they never seem to dull, except for on acrylics. Though for ACM, you ought to use the 33317A, it has a 5/16" CEL, shorter OAL, and more/narrower groves on the sides, so it's just a little stiffer. I never seem to get the same mileage on a 33317A when I have to use one on ACM/Aluminum. We use it on aluminum up to .25" thick all the time. I've probably clocked a couple of miles on an aluminum bit more than a few times. More often than not they get broken when someone set up a program wrong, didn't see an inside piece get ejected, or when the depth is set wrong.
Andrew Heiner
New Member
Single flute bits tend to be best for aluminium and plastic - something with a nice Polish will just fly through.
Alot also depends on speeds and feeds. The issues are often that you are not going fast enough. Imagine you have a 1hp plus router.. Its not going to struggle with cutting sign material, then you look at the rpm - use that to see how much the bit is cutting per inch/mm, etc. The bits usually tell you the preferred cutting rate. Then do the math that suits your situation.. Usually it's just rpm / movement speed.
But in most cases.. Go faster and use sharp bits.. You're slicing - not grinding. You don't want to be recutting the swarf you've already cut.
Alot also depends on speeds and feeds. The issues are often that you are not going fast enough. Imagine you have a 1hp plus router.. Its not going to struggle with cutting sign material, then you look at the rpm - use that to see how much the bit is cutting per inch/mm, etc. The bits usually tell you the preferred cutting rate. Then do the math that suits your situation.. Usually it's just rpm / movement speed.
But in most cases.. Go faster and use sharp bits.. You're slicing - not grinding. You don't want to be recutting the swarf you've already cut.