milling aluminum

Talk about all things CNC
nytro2413
Posts: 5
Joined: Fri Mar 27, 2015 3:13 am

Re: milling aluminum

Post by nytro2413 » Wed May 27, 2015 12:19 pm

I built a custom pool table. Ill post some pics later. The part is upside down as shown. They will be custom corners for the table. i only have to make 4 like that and the side pockets will be slightly different. I don't need a perfect finish. i can clean them up with files and sand paper, i just need them close as for the sides i can square them on the table saw so i'm not to concerned with that. Just wanted an idea from the pros about bits. I was thinking a ball mill for the curve and any lines i can clean by hand. Once i figure out a way to hold the piece down and flatten one side its not critical that the alignment is perfect.

JeromyReno
Posts: 225
Joined: Mon May 04, 2015 11:28 pm

Re: milling aluminum

Post by JeromyReno » Wed May 27, 2015 2:54 pm

Hans wrote:
Gadgetman! wrote:I think you'll be hard pressed to find a 1/8" bit that's long enough for the job at hand.
Good point, but it looks like OP isn't doing the sides. I don't know what cutting force to aim for with the new machine (JeromyReno's example only gives .02 lbs cutting force if those step numbers are in mm, I'm expecting capability around 2 lbs), but I think the smaller diameter endmill will give better MRR at the same force. For the conical feature, you're definitely right that at least a 1/4" shank will be needed to get the required reach. To avoid tool changes, I do 3D surfaces with an up-and-down ramping toolpath instead of a ball-nose. Any remaining scalloping can be cleaned out with a half-round file.
I was using inches, i was trying to push the machine as hard as i could. i wanted to see what would start to fail first.

Hans
Posts: 290
Joined: Tue Dec 25, 2012 5:19 am
Location: Connecticut, USA

Re: milling aluminum

Post by Hans » Wed May 27, 2015 3:27 pm

Do you mean .4 as in 40%, then? .40" cut width isn't possible with a .25" diameter endmill. 40% cut width and 10% cut depth would be about 1.3 lbs cutting force, .10" cut width and .40" cut depth would be about 20 lbs cutting force. If you're having success with a 20-lb cut, then sign me up for a Shapeoko 3!
Shapeoko #1,123

JeromyReno
Posts: 225
Joined: Mon May 04, 2015 11:28 pm

Re: milling aluminum

Post by JeromyReno » Wed May 27, 2015 8:08 pm

Hans wrote:Do you mean .4 as in 40%, then? .40" cut width isn't possible with a .25" diameter endmill. 40% cut width and 10% cut depth would be about 1.3 lbs cutting force, .10" cut width and .40" cut depth would be about 20 lbs cutting force. If you're having success with a 20-lb cut, then sign me up for a Shapeoko 3!
yes 40% .1" depth of cut

TomDChi
Posts: 184
Joined: Wed Mar 18, 2015 2:36 pm

Re: milling aluminum

Post by TomDChi » Thu May 28, 2015 2:41 pm

Hans wrote: A typical vise will add too much height to fit in the work envelope, especially a vise with a 7"+ opening.
As a noob, I just had one of those "duh"/lightbulb realizations: for the combination of long mills and thick workpieces, the Z travel needed is double the additional thickness. A 1" thick workpiece and a 1" (plus a little) mill sticking out of the spindle needs a bit more than 2" of Z travel, but to do the same thing with a 1.5" thick workpiece, you need a bit more than 3"... If I understand correctly, there's slightly more than 3" of clearance between the top of the wasteboard and the underside of the Z carriage, but I have no idea how much Z travel the S3 is capable of (and the wiki entry: http://www.shapeoko.com/wiki/index.php/Shapeoko_3 doesn't call it out specifically.) The rails and belt make it look like substantially more than 3" of travel, though 6"+ would be nice with the 3" of working space.

With the pem nuts in the frame (IIRC), it would be possible to mount a wasteboard on the bottom of the steel frame to gain a bit more clearance for something like a big/thick mill vise (after taking off stuff like a swivel base, of course) but... you'd have to shim the base of the vise with the thickness of the rails... and fitting in the handle to tighten it could be difficult... maybe...

WillAdams
Posts: 8488
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: milling aluminum

Post by WillAdams » Thu May 28, 2015 2:52 pm

Vise handle isn't a big deal --- just use the sort from a drill press (which is what I mounted to my SO1):

http://www.homedepot.com/p/BESSEY-4-in- ... vZc97yZdep
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

TomDChi
Posts: 184
Joined: Wed Mar 18, 2015 2:36 pm

Re: milling aluminum

Post by TomDChi » Thu May 28, 2015 2:55 pm

Hans wrote:Flycutters aren't used in industry anymore (they've been replaced by indexable face mills) but they're a cheap, re-sharpenable option for the hobbyist. I'm interested to see the results achievable with a flycutter in the S3, but one would need to run down around 5k rpm to get good results on a 1.5" diameter cutter in aluminum.
I keep eyeing my Bosch 1617 (3.5" diameter versus the 2.5" diameter of the DW611 and weighing about 1kg more) specifically because it's low end is 8000 RPM. Dropping from a 1.5" diameter fly cutter at 5k rpm to 1" diameter means a 7.5k rpm (if I did the math correctly) which is pretty close to 8k. (That's about 2000 SFM right?) I see that smaller fly cutters with 1/2" shanks are available...

This all seems fairly absurd, but maybe the S3 would be up for it?

Jimf
Posts: 233
Joined: Wed Feb 11, 2015 8:58 pm

Re: milling aluminum

Post by Jimf » Thu May 28, 2015 4:49 pm

Not to say that it can't be done but operating a fly cutter at 5000-8000 rpm is asking for trouble. The cutter must be very well balanced to run at those speeds and I don't think anyone would recommend it being done. I run my fly cutter on a mill under 1000rpm and I think that is still scary.

edwardrford
Posts: 1250
Joined: Mon Apr 09, 2012 5:40 pm
Location: Dixon, IL
Contact:

Re: milling aluminum

Post by edwardrford » Fri May 29, 2015 5:55 am

Of course, I'm really biased, but I think S3 does a great job cutting aluminum.

Here's a quick video I took last night on my Shapeoko 3. Sorry for the shakycam and the out of focus. Also - turn your speakers down, the camera was about 8 inches from the router.

Job Specs:
- Material: 1/8" Thick, 6061 Aluminum
- Feedrate: 60ipm
- Depth pass: 0.0625" (1/16")
- 45% overlap
- Plunge Rate: 20ipm
- Bit: 3 Flute, 1/4" Square end Mill, HSS
- CAD: Autodesk Inventor 2014 Professional
- CAM: MeshCAM v6 Pro
- Router: Dewalt DW611 (Speed set to 4)

Shapeoko 1 #0 - a couple of upgrades.
Shapeoko 2 #0 - a couple of upgrades.
Shapeoko 3 #2 - Stock

Hans
Posts: 290
Joined: Tue Dec 25, 2012 5:19 am
Location: Connecticut, USA

Re: milling aluminum

Post by Hans » Fri May 29, 2015 12:21 pm

Thanks for the detailed demo, Edward. For reference, FSWizard gives almost 4 lbs cut force with those parameters. And the machine's delivering good surface finish, too. Compared to my old Shapeoko 1, that's darn good.

EDIT: It looks like there's some slotting going on, and if that's at the same depth but full width then the cutting force is quite a bit higher. Lookin' good.
Shapeoko #1,123

Post Reply