Routing aluminum sheeting and dibond (max metal)

PhilSwatch

New Member
We're still ironing out (no pun intended) our milling of aluminum, up to 0.80" and dibond materials. Trying different settings and different bits. Having to do with bits, any good recommendations on brands? We use Esko Kongsberg bits, X-Edge, and thinking of trying out Helical. Has anyone used these brands before and what are your experiences with them? We're looking for a consistent clean edge that requires little or no cleaning up, other than just dust. Thanks much and happy cutting!!
 

JBurton

Signtologist
Belin LMT is what I use on all my aluminum and acm. Anything beyond .040" will need coolant mist, other than acm. I use 33317a on aluminum and acm, and 13317a on acrylic and polycarb.
 

Raum Divarco

General Manager CUTWORX USA / Amcad & Graphics
What machine do you have?
What RPMs are you using.

What direction (clockwise or counterclockwise) are you using.
 

jfiscus

Rap Master
We made a dry erase board for our router bits and settings. This way as we improve our cuts and try new/better bits we have a "best" setting/bit to use for each material.
 

Attachments

  • 288194430_558319699099004_4095650019349314834_n.jpg
    288194430_558319699099004_4095650019349314834_n.jpg
    275.1 KB · Views: 61

Raum Divarco

General Manager CUTWORX USA / Amcad & Graphics
If you have a typical flatbed cutter you will likely have a 6mm collet.
There are some good options for coated tooling in that diameter.
I would recommend to use 8mm-10mm diameter tooling.
These larger diameters will increase edge quality but will reduce intricate details.
I typically use tooling from a variety of vendors including VTX Tools, Crowne Norge, Toolstoday and Superior Carbide.
Coating on a tool is nice.
ACM like dibond can be cleanly cut with a variety of bits for a variety of edge quality finishes.

You are going to find some variances in aluminum depending on where you get it.
Alloy type/composition is key when looking at tooling.
Online stores for example have a wide selection of more or less wholesale options.
The problem with similar eshops is that soft premium alloy types cut very clean, and that may not be what you are getting.
Cheaper alloys have different compositions, are harder and provide some challenges.

For a comparative example.
Find a comparable thickness panel from Chromaluxe and two other same size sheets from 2 other vendors.
Its likely that the luxe panel will route smoothly, quieter, smoother and the bit will last longer.
One if not both of the sheets from someone else might have a louder shriek to the cutting or the chips fuse with the tip of the bit.
You can still get some good edges but you will also probably have decreased tool life.
This will cause a rough tear like cut or heavy burrs.
Fusing of metal to the tip of the bit is reduced with coated tools as well as misting systems.
Misting systems are great depending on the application and misting solution used.
This can be messy and depending on your process and graphics, this might not be the best choice.

The closer to .125" (1/8") you get with all metal, the less effective routers can be especially with the HF (high Frequency) router types.
Spindles that can reach 55k to 100k RPMS have a high frequency but low torque.
Spindles typically from 18k to 24k RPMs are high torque options.
Just because your 1KW, 1.8KW, 3KW, 3.6KW router spindles are powerful, it doesn't mean its the most efficient for all material types.
Compounding this is the standard 6mm collets that are commonly used.
At slightly under 1/4" you may have a 2.5" OAL bit where close to 1.25" of it is sticking out of the chuck.
On this .08 example, you are exerting a good amount of force just on the tip.
A variety of factors can reduce edge quality, tool life and sound during operation.
Having a good carbide tip on your bit may give you a good "bite" when enters the material and cutting.
This can also be problematic if you nest shapes too closely as this may lead to parts lifting or shifting.
Material movement while cutting will put added stress on your tooling and in many cases cause it to break or damage you cuts.
larger diameter tooling on HF spindles does lessen the gap between high and low torque spindle options.
The larger tool will experience less deflection by the reduction of force on the tip and absorb more vibration.
 

JBurton

Signtologist
We made a dry erase board for our router bits and settings. This way as we improve our cuts and try new/better bits we have a "best" setting/bit to use for each material.
I like how polycarb is blank, it's such a b*tch to cut compared to any other substrate due to the lack of rigidity. Best results I get are running it 90% of the thickness on the first pass, and running all shapes on a sheet at that depth (.15" on a sheet of .177) before cutting any of them out. We typically nest channel letter faces really tight on these sheets, and it keeps the later parts from shifting as the vacuum drops off when parts get cut out from the sheet..
 

nastewart0521

New Member
We're still ironing out (no pun intended) our milling of aluminum, up to 0.80" and dibond materials. Trying different settings and different bits. Having to do with bits, any good recommendations on brands? We use Esko Kongsberg bits, X-Edge, and thinking of trying out Helical. Has anyone used these brands before and what are your experiences with them? We're looking for a consistent clean edge that requires little or no cleaning up, other than just dust. Thanks much and happy cutting!!
For Dibond I'd recommend a belin 22317 downcut bit at 24,000 rpm and 175in/min feed rate in the climb direction. I get very consistent results with these settings. I've never tried this on raw aluminum but I have used the belin 33635 on raw aluminum and it did great.
 

JBurton

Signtologist
belin 33635 on raw aluminum and it did great.
That's a good 1/4" bit for sure, though it increases the radius you have to put on something like a push through letter. Plus it's loud af on .090" aluminum! I keep a couple whenever I get fed up with broken 1/8" bits.
belin 22317 downcut bit at 24,000 rpm and 175in/min
I've had more trouble with the edge on acm when using a downcut bit vs upcut. I haven't had the rpm's that high though, may try this. What sort of bed does your router have? I've been running the 33317a at 200ipm, 20k RPM for acm.
 

nastewart0521

New Member
That's a good 1/4" bit for sure, though it increases the radius you have to put on something like a push through letter. Plus it's loud af on .090" aluminum! I keep a couple whenever I get fed up with broken 1/8" bits.

I've had more trouble with the edge on acm when using a downcut bit vs upcut. I haven't had the rpm's that high though, may try this. What sort of bed does your router have? I've been running the 33317a at 200ipm, 20k RPM for acm.
I got a 5x10 AXYZ with a 10hp spindle
 

Evan Gillette

New Member
I don't do a lot of volume but have had good results with pretty much any good quality single O flute upcut bit for acp (usually maxmetal or bebond prem.) I mostly use Amana (from toolstoday) and LMT Onsrud (63-xxx series iirc). Sometimes you can catch sales on amazon for 50% off on onsrud bits. Got about $500 of bits half off last year around this time, makes a good chance to try different diameters and styles. I haven't done much aluminum but pretty much the same bits playing around with speeds and diameter to thickness seems to make a big difference in noise and I would assume that less noise is a decent indicator that your bits are experiencing less chatter and should get better life.
 
Top