Thin Aluminum Sheet, Tooling Issues

[jacobcarlgrant]

I am using a Multicam APEX3R CNC Router to machine slots in thin aluminum sheets (20ga, 0.028" thick). I was able to get the sheets to stay down to the spoilboard by using down-cut tooling. However, I am having issues preventing the aluminum from sticking and gumming up to the tool.

The machine is equipped with mist coolant. I've had the best luck with a 2-flute HSS 3/16" down-cut end mill, 16700 RPM and 150 IPM (820 SFM, 0.0045 IPT). The material does not stick to the end mill and the cut looks great with minimal burrs, but the first tool broke after less than an hour of cutting time.

I tried a similar end mill, except made of uncoated carbide instead of HSS. I used the same feeds/speeds on the same material, but the end mill gums up almost instantly and produces a horrible cut.

Why does the HSS tool resist sticking, while the carbide tool gums up so easily? Do I need to increase the SFM?

HSS tool link:
Amana Tool HSS1651 HSS Spiral Aluminum Cutting Double Flute Down-Cut 3/16 D x 5/8 CH x 1/4 SHK 2-7/8 Inch Long Router Bit

Carbide tool link:
57-060

Thank you in advance for the help.

 

[ducesrwld]

haven't cut AL on our routers in several years but the last job we had to cut 1/4" sheets we retrofitted and rigged up a "mister" with a steady spray of wd40 to give the tool some lubrication. as you found out downcut geometry is the preferred tooling for routers n vacuum. if i remember correct we were using the same 57 series from Onsrud you mention above but we were cutting with a 1/4" tool. Your #'s look ok if it is gumming up you need to make sure you are spraying a decent amount on the tool and i'd try lowering your rpm down you are creating too much heat. to help further look at Onsrud single flute "O" tools that will help create even a larger chip which is necessary to pull more heat away from the tool and eliminate the gumming.

after a 2nd look the feed n speed you mention seems high for HSS you are def prob running her hot. Those feed n speeds look ok for a starting point for the carbide tool. we don't use any hss end mills on our routers only cheap hss for basic drilling in non metals. Onsrud has pretty good charts for starting chiploads on all their tools look em up.

 

[MaxPrairie]

The helix on those two tools is quite different. If you can get the chips away from the cutter you will have less packing in the flutes.

 

[Scruffy887]

Have you tried the ZrN coated bits for aluminum? Zirconium Nitride? I tried some on my router cutting with mineral spirits. Huge waste of time because I was cutting a max crappy grade 1/8" sheet. Took forever with multiple passes. But for sure it was not a good test because that grade of aluminum is like cutting bubble gum.
That was before I got my laser. Fiber laser does not care what grade it is.

 

[Omega]

It's probably 5052 H32 sheet which is formulated to bend easily, you will want to decrease rpm and lots of water/oil in the mist stream. Carbide will work fine just keep it cool.

 

[jacobcarlgrant]

I tried it again today with a tool we had lying around, which is the 1/4" version of the HSS 2-flute down cut that I listed earlier from Amana Tool. I ran 12,500 RPM and 150 IPM, which keeps the SFM the same but increased the chip load some. I completed about an hour total of cut time and saw pretty good results, with no chips gumming up. I know I am at/beyond the limit of recommended SFM and IPM, but the machine and parts seem happy so far.

Is it worth trying the same cuts but with carbide tooling? My concern is that I cannot find a tool with the exact same geometry in carbide. As MaxPrairie mentioned earlier, the helixes are very different between the Amana and the Onsrud tools that I previously tried.