Cutting Aluminum? --- Anyone???

Discussion about the CNC Shark Pro Plus HD

Moderators: al wolford, sbk, Bob, Kayvon

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Cutting Aluminum? --- Anyone???

Post by Rando »

cjablonski wrote:That is, hands down, the BEST informational post I have read in 4 years. It has quelled my concern about an upcoming project requiring machining with the shark. Even beyond that has me kinda pumped to get to it. Honestly, this SHOULD become a thread headed up by Rando to which I would absolutely follow. Awesome info Rando! Thank you!
Thanks, Man...one thing I forgot to mention, but is really important: use 2-flute bits, NOT 4-flute bits in Aluminum. Some people even go down to a 1-flute (aka O-flute). The reasons are a bit obscure, but let's just leave it at "our machines can't work as fast as those extra flutes require it to." I'll go back and add that to the other post.

Regards,

Thom "there's too many details" Randolph
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

User avatar
Kayvon
Posts: 552
Joined: Tue Oct 21, 2014 11:46 pm

Re: Cutting Aluminum? --- Anyone???

Post by Kayvon »

Thom, that's great information. I'm still nervous about trying aluminum, especially with a router. I know you have an awesome spindle setup on your Shark. Is cutting aluminum still viable with a router? Will the small aluminum chips get sucked into the router intake and short it out?

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Cutting Aluminum? --- Anyone???

Post by Rando »

Nah, Rest easy. You're in a good place.

Short answer: Heck yeah a router will work. I did all my early cutting with a DeWalt D618. The air comes out the bottom and does greatly help with chip removal. Chips tend to blow away, but they don't go far--they're quite a bit heavier than sawdust and wood chips. Chips that might get into the router would have to be pretty small, which means they'd also not short anything out. I mean, don't let it get encrusted, but I never saw any significant chip accumulation around the router intake vents.

The one thing I added that made a big difference when using the DeWalt was to get a non-contact tachometer. The dial indications on routers are notoriously unhelpful in setting an actual RPM, and with aluminum, it's helpful to be accurate to within ~100RPM. So when it says 15.6K, it doesn't mean 15.7K or 15.5K. That non-contact tachometer can fix that when using a router. The spindle's Variable Frequence Drive unit display the RPM it's driving at. This is the one I got:

https://www.amazon.com/AGPtek-Professio ... B004Q8L894

I also erected a simple clear-acrylic shield (0.020"...thin sheet stuff) about six inches up, around the perimeter of the bed (inside the gantry arms). The end that I view it from (the end where the spindle can be seen, not the back of the gantry plate) has a taller barrier of about 16". That shielding lets way under 1% of the chips out, so they all stay on the machine to be later vacuumed out (or scooped with a trowel). Still, I make sure I'm not getting chips into electronic things like computers.

Thom Writes Too Much answer ;-)

It certainly wasn't as good as the spindle I use now, but I started with a well-used DeWalt D618 router, and it wasn't until I was comfortable I was going to be successful did I make the investment in a spindle.

Besides rotational accuracy and just the loudness of the router, there are two primary areas you're going to see the difference:

* RPM range. The default settings for a spindle are about 1k to 24K RPM. I have mine set to go from 500RPM to 36K RPM. That default range restricts somewhat the bits you can use (ideally, nothing under 1/8"), since that ~1000-1200 SFM is inversely proportional to the diameter of the bit. So, an 1/8" bit "wants" around 32K, but I've run them at 24K as long as I'm careful. But, a 1/16" endmill? That thin wants, IIRC 38000 RPM...even I'm not willing to spin stuff that fast! But, that doesn't mean that normal-sized bits can't be used quite successfully. With aluminum, I've found that 3/16" bits actually work best on Sharks. 1/4" bits tend to work best cutting more metal than our flexy machines are good with, and 1/8" bits remove so much less metal that toolpaths run for hours. 3/16" bits, however, can be run at quiet speeds (14-18k RPM) and at feedrates that respect the machine's abilities, while still cutting quite productively.

* Downdraft. The routers almost always use air cooling, with the air coming out the bottom toward the spindle. This will actually help you, because it will tend to blow out nearly all the chips, without your needing to get that chip blower. A spindle, even an air-cooled one, does not break wind...err, produce airflow from the bottom, so the chips just sit there if there's no blower.

If you're worried, get some cheap aluminum stock and make some test cuts and just try them. Always ramp the bits into the material. Never ramp more than 2.5 degrees, and always give it at least 3*diameter as the minimum ramp length. If it can do more in the pocket being cut, longer is okay, but avoid allowing a bend in it.

One thing you can be afraid of, for sure, is the Vectric toolpaths are, um, "not the best" for aluminum. They'll work, but jamming the bit into the corners produces large torque spikes in the spindle as it goes from cutting just on one side, to nearly 270 degrees around the bit, right in that corner. If the speed going into the corner is too fast, that torque can snap the bit in an instant. That's part of the reason I moved to BobCAD: less stressful cutting paths. A lot of times the best way to overcome this is in the design. Make it so the inside corners of your design have a radius just slightly larger than the bit, so it produces a rounded corner. For an 1/8" bit, a radius of 0.080" will help prevent those spikes. All it takes is enough room for the cut chips to get out, and that corner will come out much better.

And, you have my cut catalog, something I didn't have when I started. Like I said, as long as you can get the bit safely into a pocket using ramping or other appropriate lead-in, those cut parameters should work well. Especially on a simple rectangular pocket like you were mentioning.

Other than that, fear not...do buy extra stock to practice on, and extra bits. Indeed, something like a 12" length of 1/4 x 2" bar would give you more than enough space to try creating toolpaths to see how they react. Keep in mind it's the learning period, and you can't learn what the boundaries of its capabilities are unless you get up close to those boundaries. And boundaries mean broken bits and ugly cuts until you learn to stay on the right side of the border, so to speak. The cut catalog can provide those points of guidance.

Oh right!...my ONE rule about bits: NEVER start a cut unless I have a spare, new bit of the same kind on hand in case something bad happens. And that's for toolpaths I'm confident in. For ones I think might have problems, I keep **at least** two spares of that type and size of bit on hand. Bits go dull, and dull bits tend to break, and create burrs, and other bad things. Sometimes the machine will freak out and break the bit "for me". It happens. But there's not much worse than getting up early on a Saturday morning for a weekend of fun aluminum machining, only to have that bit break and realize I have ZERO more....and can't get a new one until Monday. Same with the metal stock: I keep extra on hand just in case.

Regards,

Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

MDHunt
Posts: 31
Joined: Sun Dec 04, 2016 8:34 pm

Re: Cutting Aluminum? --- Anyone???

Post by MDHunt »

I joined the 'Aluminum cutting club' today as well.....when I didn't set the X,Y, zero properly from design to machine and went right into one of my clamps! :?
The bit was still ok though and I am really thankful that the clamp was aluminum and not something that would tear up my new bit! :D

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Cutting Aluminum? --- Anyone???

Post by Rando »

MDHunt wrote:I joined the 'Aluminum cutting club' today as well.....when I didn't set the X,Y, zero properly from design to machine and went right into one of my clamps! :?
The bit was still ok though and I am really thankful that the clamp was aluminum and not something that would tear up my new bit! :D
LOL...yeah, that's how most of us cut our first bit of the buttery silver stuff!
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Post Reply