Cutting Sheet Aluminum on a CNC Router

Aluminum plate can be machined on CNC equipment designed for wood. Here, pros discuss the considerations involved (and the alternatives). March 21, 2006

Is it practical to cut aluminum 6061-t6 on any type of router? Sheet size would be 4' x 10' with a thickness of 1/4-1/2". We are a metal fabricator, however our parent company uses plastic and wood laminates. I feel it would be a better investment for the company to buy a machine that could do multiple things as opposed to a water jet which will only cut steel and aluminum.

Forum Responses
(CNC Forum)
From contributor K:
I know a local shop in our area that has a water jet. They cut a lot of different materials on it, such as steel, aluminum, plywood, solid wood, plastics, stone and glass. The finish is very good and does not require any grinding or sanding, like a laser cutting machine requires. The thickness of the material that can be cut on a water jet is far greater than laser. Actually, water jet cutting originated in the solid lumber industry in the 1900's.

From contributor D:
You can cut aluminum with a router. The router needs to be set up with lubricant spray and the vacuum pump cannot be one with graphite vanes - if the lubricant sucks through the vacuum to the pump and gets on the vanes, they are toast. Routers are not really made for cutting metals, however, the key word above is "can." For working metal, it is better to get a mill, as they are engineered for metal work in terms of feed rates, rotation speeds, adequate lubricant flow, recycling lubricant, etc. Hold downs are usually mechanical using t-channel (rather than vacuum, as is typical on CNC routers). Routers' rotation/hp ratio are typically best at higher rotational speeds (like 18,000 to 21,000 RPM), which are way higher than those normally used for metals. I have been doing aluminum on my CNC router and it's not as much fun as my machine shop owning friends running things on their CNC mills. It's way more "copey." It works, but I am currently looking for a used CNC mill so that I have a professional setup to do this sort of work - or will farm it out. That's my take.

From contributor C:
Yes, routers cut all sorts of non-ferrous metals and also engrave stainless. With the correct tooling and techniques, you can cut 6061 all day like the better sign shops. The guys making push-through channel letters use 6061, 5052, and softer (softer is harder to cut because it is gummy and loads the tool) aluminum at speeds anywhere from 50-200ipm. You do not want to flood the tool because you are not trying to lubricate it just to keep it cool. We have customers who run eight hours a day who go through about a gallon of lubricant every couple months. They use a micro mister and have very good tool life. The big advantage of a router over a mill is that you can work with a full sheet and nest the parts like a cabinet shop. You vacuum fixture the parts and machine faster. 18,000 rpm is not uncommon with a "o" flute single edge upspiral cutter with feed speeds up to 200 in 1/8" material.

Keep in mind the small CNC machines have made a great living successfully selling to the sign industry and job shop. Of course, I'm a salesman, so I probably can't be trusted.

From contributor T:
You can cut aluminum quite well on the router. The key is tooling design. If the tool is designed to pull the chips away from the sheet quickly, it keeps the contact area much cooler and therefore reduces the need for coolant. The mister noted above is also a good idea.

In regard to your comment about the waterjet, I think you will find that you can cut a very large diversity of materials, much more so than the router. In addition to the obvious choices of steel, aluminum and wood, you can also cut glass, rubber gaskets and much more. Many food producers use waterjets to cut frozen products out of sheets.

The downside with the waterjet is the economics and environmental concerns involved with disposing of the abrasives after cutting.

From contributor G:
As mentioned above, a single flute can be used on this material. We have a lot of customers who use A CP-AZ tool. Others prefer a Fast Helix for better chip removal and faster feed speeds. The fast Helix does not require a misting system.

From contributor C:
For those looking for clarification, I stated that we look to cool the tool not lubricate. Aluminum can be cut dry, or flood. Machinists flood the tool all the time to reduce gauling. When running a MDF suck through spoil board, this is a bad idea, as you will suck the material through the system. You will also make your vacuum much less efficient, as the board will become sealed from the oil. Anyone looking to avoid this can use my comment. Solid carbide tooling design has allowed us to use far less lubricant/coolant than in the past. I stick to my suggestion that single sheet, nested style vacuum fixtured cutting can and is run with little to no lubrication, just coolant. My customers successfully run an alcohol based misting fluid at a very light setting and cut aluminum for a living.

From contributor F:
The router can do 3D. The laser/water jet is only a 2D machine.

From contributor G:
I need to cut a custom mounting plate for the spindle on our CNC so we can mount a liquid dispensing unit alongside our router. The current mounting plate appears to be made from 1/2" aluminum. What type/hardness of aluminum should we make this part from? We purchased a 1/4 bit from that is supposed to be designed for cutting metal, but we have never cut metal before and we are not 100% sure if we have the right bit for this particular job. We have a new HSD 5hp spindle and a mister attachment. Is this a strong enough router for cutting metal? What RPM speed, feed rates and depth should we try to cut aluminum?

From contributor S:
For 6061 or 6063, use a 3/8" diameter high helix 2 flute hi speed steel bit good up to 18k rpm. I used to cut plate aluminum all day long at 80IPM at 10000RPM. Make sure the mister is on. Cut no more than about .125" per pass for a nice cut. I always used a .015" offset from the true part. Then went back on the true part line and did a full thickness pass at 110IPM at 11000RPM. Made a very nice edge. Machine was a Komo Innova Mach 1. Don't know if a 5 horse is strong enough.