SuperPID-help cutting aluminum?


I’m getting close to pulling the trigger on a Shapeoko. I have a project in mind that involves aluminum, if it works out I would probably be cutting aluminum often. I’ve looked at the carbide speeds and feeds guide and it recommends speed 1.5 on dewalt dial i.e. +/- 17k for cutting aluminum. SuperPID seems to enable speeds as low as 5-6k rpm. Is carbide3d recommending that speed b/c it’s best case scenario for included hardware? Would slower speeds help with cutting aluminum?

thx in advance


The Makita RT0701 Router option has a lower base RPM of 10k - which would be a better option for 6061.

Lots of info on the Makita and Aluminum here:


You don’t need the PID, and both the Makita and DeWalt work great at cutting Aluminum. The slower speed of the Makita helps when cutting steel. Check out my InstaGram for some of my projects. I cut metal about 90%

IG: JPL_Richard

1 Like

Okay, here’s a question for @ApolloCrowe and @RichCournoyer :

If we work up the chip load and Material Removal Rates for the Dewalt feeds and speeds as was done for the Nomad at: would it then be helpful to go from those chip loads to work up an optimized feed and speed chart for the Makita where at suitably lower speeds, we calculate a feed rate which achieves the same chip load.

Is that the purpose / intent of chip load and is that a valid procedure / set of calculations?

If I’m understanding this, there would be some sort of torque rating for the motors involved which would show what torque it can achieve at a given RPM, and that one then needs to match that torque and speed to the expected cutting forces, and so not exceed the torque which is part of what causes problems when cutting.

As an experienced maker and an engineer and not the Manufacture (Apollo), let me tell you my findings:

I am going to talk about horsepower rather then torque just to simplify things. The Makita is rated at 1.25hp but consumes 700 watts and that means 1hp (100% available) with a little bit of reserve (1.25 total available for perhaps 10-25% duty cycle), and since the router has speed detection, it does in fact maintain the 10k speed at just about anything that I can throw at it (I am referring to the Router NOT the machine).

My Shapeoko (Spindle: Makita 0700 and an Shapeoko 3 (9mm belts), with a metal table)

During heavy machining, the Z Axis plate will flex considerably when taking a 1 1/4 hp cut (Example: 1/4 End Mill, 0.25 DOC (Axial), 0.22 DOC (Radial) with a 25 Inch/Min Feed rate) when cutting in the Y direction (Note 2 drive motors, which will produce about 36 pounds of pulling force). It will also stall (skip) the X Axis Stepper motor (Stalls at 18 pounds) when cutting in the X direction. (I won’t even go into the noise factor)

What does all these numbers and math mean: The Shapeoko cannot take advantage of the available horsepower that these (Makita and DeWalt) Spindles can provide. My recommendations for speeds and feeds are based upon the machine’s STRENGTH and are pretty much spot on with that is published in the recommended published document.


Are you referring to the C3D feeds and speeds chart for the SO3, or a different one?

Yup, that one.

BUT It also depends on several other factors:

Rigidity of your machine
Squareness of your machine

Quality (sharpness) of the end mill
Coated or non-coated cutter
Height of the Z (Higher (Z+) is weaker then Lower (Z-)
Length of the cutter
Amount that the cutter sticking out of the collet

Work Holding/Material:
How rigid is the material (sheet vs. flat bar)
How are you holding it to the table
Where on the table

I generally teach the 10/10, 20/20, 30/30 rule.

Start off with 10 IPM, and 0.010" DOC, if that sounds snd looks good, work your way up the Feed and DOC latter until you max out at 30IPM and 0.030 DOC (at about 80% Rad of the cutter.

That’s the max I would recommend for a S3 (for general roughing (material removal)

Finish cuts? Full width of the material (up to 1/2" thick material)) at 0.005 DOC


Thanks for the replies.

To clarify

@ApolloCrowe you stated the makita’s lower base rpm of 10k would be better for 6061. Carbide speeds and feeds list higher speeds for dewalt and makita, is that for simplicity? If I plan to cut aluminum what would be primary benefits of using the lower speed, tool life, finish quality etc.? Is 10k speed enough of a reduction to use a 4 flute with aluminum? A part I’m looking to make has an undercut and there are a lot more options for spherical end mills in 4 flute vs 2. Appreciate all the info, thx.

1 Like

Lower speed equals lower temp.
More flutes, more temperature.

Check out Richards Shapeoko videos, he has covered squaring the machine and coolant and proper fixturing for metal work.


Isn’t 1hp = 745.7 Watts? Isn’t the router’s output power further reduced from that 700W electrical consumption by the efficiency of it’s motor and drive electronics (likely 80 - 85%)? Isn’t the force on the machine (and workpiece) proportional the torque on the cutter and inversely proportional to it’s speed? So, why not maximize router speed rather than minimize it?

Because both the DeWalt and Makita have Hall-Effort systems that maintain the speed. Meaning that the hp is not speed dependent, so you do not need maximum speed to achieve the full 1.25 hp.

1 Like

Also, you want to adjust the speed of the trim router to match the feed rate which you can reasonably achieve so as to get a chip load which is suitable to the material you’re cutting — this often wants a lower speed, rather than a higher. See Tutorial on feeds and speeds (which needs to be expanded upon or finished)


Here’s some links that seem relevant.



Assuming router motor horsepower is determined by output (mechanical) rather than input (electrical) power, a router with a 700 Watt input would provide about 700 * 0.85 / 745.7 = 0.8 hp of mechanical power.

Rotational mechanical power (hp) = Torque (ft lbf) * Speed (RPM) / 5252. Cutter (and workpiece) force (lbf) = Cutter Torque (ft lbf) / Cutter radius (ft). Since the required cutter hp is proportional to material removal rate, increasing cutter speed reduces forces.

Motor output power is proportional to speed and torque. Torque is proportional to motor (winding) current, which = voltage across the windings / winding resistances. Voltage across the windings = supply voltage - motor back EMF (which is proportional to motor speed). Those are the factors that ultimately limit motor performance, not the type of speed/torque controller used with it.

I believe that most/all motors power ratings are at the maximum design motor speed. Higher speed means less winding current and less heat generation for the same power output.

The context of that is increasing milling spindles to speeds approaching that of the trim routers used in CNC routers.

That was my point. Higher spindle speeds enable higher material removal rates (MRRs) and reduce forces on the cutter, spindle, machine and workpiece (all good things)! They also reduce spindle heating for a given MRR.

Yes, but they also require a more rigid machine and faster feed rates — the machine can only accelerate so quickly, and for the most part isn’t able to take advantage of the faster spindle speeds.

See: for a testing methodology and for a discussion of the tradeoffs.

As shown above, more spindle speed = less rigidity required, and faster feed rates are not required - certainly not for wood and apparently not for aluminum (based on the previously posted links). Also see It’s unlikely that a hand held router would exceed the feed and acceleration capabilities of the Shapeoko 3.

Regarding your CNCCookbook link, you should take a closer look at that. In particular, consider that softwood hardness “family” “alloy” Janka hardnesses vary by an order of magnitude, yet G-Wizard uses a single undefined hardness value for the entire “family’s” calculations (the same is true of other “families”). There are numerous other problems with G-Wizard.

actually GW has about 126 different “soft woods” listed in the calculator. 135 under “hard wood”

1 Like

Yes, but what’s the point of that if the their hardness’ aren’t used in the calculations?