I recently finished a 3 axis gantry router for work that is designed to cut complex notches in aluminum curtainwall (window) extrusions. While programming the machine I had trouble getting things to work correctly and I couldn't understand why. I was using info I found on this site, as well as in the Machinery's Handbook to set my feed and speed and still the machine just was not working as intended.

Finally it dawned on me one day that I was not "Milling" aluminum, I was "Routing" aluminum. I took everything I had been told about milling and threw it out the window. With a stopwatch in hand I headed down to the shop and grabbed a porter cable router (just like the one on the gantry) and found a piece of scrap to experiment on.

What I found is that the Router has a "natural" feed rate at which it will cut through aluminum, and that natural feed rate is much slower than "the book" says.

Based on my own testing here is the data that I've been using to set my speed and feed rates.

Tool: 3/8" 2 Flute End Mill
Speed: 21,000 RPM (Max)
Coolant: KoolMist (Pressurized Air & Mist Coolant)
Material: 6063-T5 Aluminum Extrusion 1/8" Wall Thickness

Depth of Cut: .125" (Full)
Width of Cut: .375" (Full)
Feed Rate: 5 - 10 in/min (Depends on Machine Rigidity)

Depth of Cut: .050"
Width of Cut: .375" (Full)
Feed Rate: 15 - 18 in/min

Depth of Cut: .125 (Full)
Width of Cut: .1875 (Half)
Feed Rate: 22 - 25 in/min

Depth of Cut: 1.0" (Face Finishing Pass)
Width of Cut: 0.02"
Feed Rate: 25 - 30 in/min

Keep in mind that these feed rates will shorten tool life if you're using a regular HSS end mill. However that has to be balanced against the cost of replacing the router due to overloading it. Even with a "shorter" tool life I've still been getting well over 40 hours of cutting time out of each end mill.

I would also like to note that I have been having better luck keeping tolerances by programming the router to cut in a "Climb Cutting" configuration instead of "Up Cutting".

These are just my observations, but I figured someone else might find them useful.

This is a great post - thanks for taking the time to lay it out.

In my opinion, you are wasting your money if you are buying HSS tools for spindle speeds above 3,000. Solid carbide is the way to go for sure and I am sure you agree - 40 hours of cutting from one tool - nice.

Thanks again, musicmkr. I am sure a lot of people will get good use of this information.

Scott

Hi,

Thank you for information. As I am not an English mother language speaker I would like to understand what is the difference between milling and routing, and what you defined as a cut width.

Thank you.

Zoltan

Cut width - in this case, he is machining a trough or valley into the aluminum the full width of the cutter. Instead of cutting a step or a shoulder on the edge of the part, he is using the cutter almost like a saw to cut the material in two - plowing right down the middle, so to speak.

The difference between milling and routing is terminology. You are removing material if you are routing or if you are milling but milling usually means higher removal rates at slower speeds with more rigidity and accuracy of cut. Routing usually means higher spindle speeds, faster cutting, but less material removed with each pass and the machine is typically not as heavy-duty. Routers are light-duty compared to milling machines.

Scott

I see. Thank you for help.

Zoltan

I'd like to third the thanks....

THANKS


It's posts like this that make this site special.

Carlo

40 hours in aluminum with HSS is great you could increase the load and reduce the cutter life in my mind. but I use carbide stuff most of the time.

good info. keep it coming.

In my opinion, you are wasting your money if you are buying HSS tools for spindle speeds above 3,000. Solid carbide is the way to go for sure and I am sure you agree - 40 hours of cutting from one tool - nice.
Scott

I tried a few carbide bits but I put them back on the shelf above the Bridgeport when one snapped and almost took my head off.

The Router I built is entirely constructed out of 3/4" thick aluminum bar stock so I imagine that the frame isn't rigid enough to keep the carbide tool "happy".

One trick I have learned to expand tool life is to use the full length of the tool. For example to make a straight cut through the wall of an aluminum extrusion I program the tool to move not only in the X direction, but also in the Z direction. So over the length of my cut the tool will use the entire length of the flutes. This makes it wear more evenly, and helps keep the tool cooler.