1/4" Aluminum Shapeoko End Plates

[Will Winder]

I've finally got a project that needs a wider X-Axis, so I needed to cut out some of the redesigned end plates. Honestly I'm surprised more people haven't been cutting these out! I actually purchased two sheets of 6"x12" 1/4" aluminum a year ago this month, but didn't need to finish the upgrade until now.

My machine has dual Y-Axis motors and a DW660 and had no trouble cutting these.

Cutting done 0.2mm per pass at 500mm/min.

I didn't want to waste any material, so I couldn't clamp on two sides of the bracket, this led to odd clamp configurations.


The first bracket came out perfect, I cut this one at 0.1mm per pass which didn't seem to stress the machine at all. It took about 90 minutes. The remaining 3 were cut at 0.2mm per pass which took about 50 minutes.


Finished products. I got a little greedy on the last clamp and accidently had it positioned wrong so its about 2mm narrow on the one side.


Edge finish, the top two are after 20 seconds of filing to remove the holding tabs, the bottom two are what the surface looked with no finishing.


I made a little time lapse video of cutting the last bracket (the one that was positioned wrong and came out 2mm narrow).

[zerblatt007]

Really nice!
What bit did you use?

[Will Winder]

Really nice!
What bit did you use?

I use some cheap 1/8" 2 flute carbide endmill's I bought off ebay, something like these.

[Improbable Construct]

Those are actually some of the nicest endmills I have used.
They are sharp, straight, last a long time, and are cheap enough to toss after a couple of jobs.
I have gone through 50+ of those things.

[chambrot]

Did you run the DW660 at full speed? Looking to do something like this soon.

[Will Winder]

Did you run the DW660 at full speed? Looking to do something like this soon.

Yes, I don't have any special speed control setup.

[samc99us]

Nice cuts!

Were these parts cut dry? Another question, were you running vacuum or air to help with chip evacuation? One thing I'll say is I will never, ever cut aluminum again without shields up around the v-wheels and without the dust collection hooked up. I spent easily an hour cleaning aluminum chips out of my delrin v-wheels, and I was running a vacuum the entire time (just no dust shoe on so I could squirt the bit with WD-40).

That's my biggest question and issue milling aluminum-what feed rate do you run at for a router? According to my feeds and speeds calculator, a 2 flute end mill turning at 15,000 RPM requires a feed rate of 120 inches per minute, or 3000 mm/min!! That is clearly waaay too fast for our little machines. 20 inches per minute seems much more reasonable at those step down distances (0.007"). I actually cut aluminum the other day at 0.05" step down depths, 35 inches per minute running a single flute end mill on the lowest setting my Dewalt 611 can go, using WD-40 as a coolant. It worked out, didn't break the tool but I would prefer to mill dry. I'm curious to know what this spindle speed this is IC (since you have a superPID), and what speeds and feeds you use when cutting aluminum?

LouisV is cutting aluminum at 20 IPM, 0.025" step down, with a 800 watt spindle on VFD control, not sure what spindle speed.

[DanMc]

I cut at about that speed as well, 500 mm/min with much lower depth/pass - .1mm. That's at 12k rpm.
I might be able to push a little more but I only have 300 watts available

[Will Winder]

All these were cut dry. I tried adding oil at one point, but it caused the aluminum chips to turn into a sludge that had to be pushed away by the router on every pass. In the past I've cut as much as 0.6mm per pass at 300mm/min, which worked alright but cuts weren't nearly as clean and really stressed the (single) X-Axis.

0.1mm per pass cut like butter, I couldn't hear the cutting over the router (through earmuffs).
0.2mm and I could hear the cutting clearly but the machine held steady with minor X-Axis wobbling (see the gouge in my edge picture above, those happened when plunging for the holding tabs).
0.6mm and I could clearly see the X-Axis wobbling in the Y direction on plunches.

[PsyKo]

When milling aluminium, you have to know which alloy you're milling.
Aluminium is like wood : milling oak, pine or plywood is not the same.
For instance in aluminium you have series (from 1000 to 7000 if I remember correctly). They all have different mechanical properties.
- AU4G (2017) is really good at machining : you can take deep passes (~0.3 to 0.5mm) at something around 500 to 800mm/min (20 to 23 ipm). This aluminium will resist to the heat and won't melt.
- 6060 is really different. It's much softer and melt faster and stick on the endmill, making it worse. You have to take smaller passes (0.2mm) at high feedrate (around 1000 to 1200 mm/min, or 40 or 47ipm). Using a 1 flute endmill usually give better results.
- 7075 alos give good results when milling.

Of course in the above example, I'm talking about my own experience with my Shapeoko. They are not the same as the best suited feed and speed in industry.
Knowing the alloy really helps...