Aluminum

Store-Material-Aluminum-0.125in-Bar

What is aluminum?

Aluminum is a lightweight, durable, and corrosion-resistant metal that is electrically conductive. It comes in a vast number of different alloys, each with different physical and thermal properties. Some of these alloys are easily cast, wrought, machined, or extruded. Other alloys are extremely strong, ductile, or resistant to stress cracking. The most commonly used, general-purpose alloy is 6061 aluminum, and it’s our favorite alloy for milling because it’s a great blend of strength and machinability. It’s strong enough to be used for many applications but soft enough to mill.

What is aluminum used for?

Aluminum is used for everything from engine parts to MacBooks to jewelry to soda cans to airplanes. The Othermill machining bed, spoilboard, and z-carriage are all made of aluminum. It’s popular because it’s a great blend of price, strength, and machinability, and it can be anodized to give a premium surface finish.

Is aluminum safe?

Yes. Just make sure you don’t get aluminum dust/chips in your eyes or lungs. We recommend vacuuming them after each milling job.

Where can I get aluminum?

We sell pre-cut pieces of 6061 aluminum in our store! They’re the perfect size for many Othermill projects, and they fit nicely on the Othermill bed. You can also get aluminum from metal suppliers, scrap yards, and even soda cans. Just make sure you know what alloy it is, lest you risk encountering one that is difficult to mill.

What’s the best way to fixture aluminum to the bed of my Othermill?

Aluminum is one of the harder materials in the Othermill’s repertoire, so more force is required to push the tool through the material. This means that proper fixturing is more important than with softer materials like wax or FR-1. If the fixturing isn’t strong enough to resist the higher cutting forces, the material can be knocked loose during milling, which can damage itself, the tool, and even the machine.

For thin, flexible aluminum sheets, it’s important to make sure the material is as flat as possible. If it’s not flat, parts of it may stick up and cause a small tool to cut too deeply. This can break tools or damage the part. We recommend removing all burrs and covering the bottom of the material with double-sided tape to attach it to the bed. To prevent the material from bending when you remove it from the bed, you can optionally use a sacrificial layer like FR-1 circuit board and stick the aluminum to it. Then put tape on the underside of the board and stick the whole thing to the Othermill bed. Offset your material origin by the thickness of the board.

aluminum1 Aluminum sheet with burrs on the edge that need to be removed.

aluminum2 Aluminum sheet with double-sided tape applied.

aluminum3 Aluminum sheet secured to scrap FR-1, ready to be milled.

For thicker aluminum bar stock, fixturing is even more important because the center of gravity is higher. A heavy-duty tape like Nitto Permacel P-02 does a great job of keeping the stock from moving. Hot glue can do the job reasonably well, but make sure to apply the around the edges of the stock, not underneath, or else your material height will be affected. We also like to use the alignment bracket because it constrains the movement of the material on two sides, which adds to the effect of other fixturing methods. If you’re feeling ambitious, you can remove the spoilboard, drill holes in the material that align with the slots in the T-slot bed, and then bolt it to the bed with M5 bolts. This provides extremely strong fixturing.

aluminum4 Aluminum bar stock with Nitto tape applied.

aluminum5 Aluminum bar stock secured to the bed with Nitto tape.

aluminum6 Aluminum bar stock secured to the bed with hot glue around the edges.

What end mills should I use when milling aluminum?

Use the biggest tool you possibly can to allow for the fastest material removal and least chance of tool breakage. The easiest tools to use are 1/8" and 1/16" flat or ball end mills. Aluminum is one of the less forgiving materials, and it’s easy to break small tools with too high of a feed rate or inadequate fixturing. The 1/8" and 1/16" tools are very strong, and they can cut away a lot of material at once. That being said, any tool can be used to mill aluminum as long as the settings are correct. The default feeds and speeds in Otherplan do a good job of making sure bits don’t break.

What are some example projects?

Lighting Gobos Lighting-gobo

Anodized Aluminum Voronoi Pattern Earrings voronoi-earrings

Custom Aluminum and Brass Rings rings-1

Note: The feeds and speeds below are optimized for the V2 Othermill. If you are using an Othermill Pro or Kickstarter Othermill, you may need to experiment to find optimal settings.

Recommended Feeds and Speeds

Note: These feeds and speeds are used by default in Otherplan and are provided here as a reference.

Tool: 1/8" flat end mill
Feed rate: 7.087 in/min (180 mm/min)
Plunge rate: 0.591 (15 mm/min)
Spindle speed: 12,000 RPM
Max pass depth: 0.002" (0.05 mm)

Tool: 1/16" flat end mill
Feed rate: 7.087 in/min (180 mm/min)
Plunge rate: 0.591 (15 mm/min)
Spindle speed: 12,000 RPM
Max pass depth: 0.003" (0.08 mm)

Tool: 1/32" flat end mill
Feed rate: 7.087 in/min (180 mm/min)
Plunge rate: 0.591 (15 mm/min)
Spindle speed: 12,000 RPM
Max pass depth: 0.003" (0.08 mm)

Tool: 1/64" flat end mill
Feed rate: 1.417 in/min (36 mm/min)
Plunge rate: 0.157 in/min (4 mm/min)
Spindle speed: 12,000 RPM
Max pass depth: 0.001" (0.02 mm)

Tool: 1/100" flat end mill
Feed rate: 1.417 in/min (36 mm/min)
Plunge rate: 0.157 in/min (4 mm/min)
Spindle speed: 12,000 RPM
Max pass depth: 0.001" (0.02 mm)

Advanced Feeds and Speeds

Warning: These settings are for advanced users. Before using any of the information provided here, you must read the section above on fixturing your material, and you must have a way of precisely measuring your material thickness (we recommend digital calipers). The feeds and speeds specified here are more aggressive (and thus faster), and improperly fixtured material can be knocked loose and damage itself and your machine. Additionally, the material surface needs to be completely flat, or else 1/32", 1/64", and 1/100" end mills will break when they encounter part of the material that is sticking up. BitBreaker Mode must be enabled in order to change your feeds and speeds.

Lastly, if you’re using tools smaller than 1/16", you must make sure that the tool is removing the correct amount of material on the first pass, or else your tool may cut too deep and break. All subsequent passes will be correct, but the first pass can be affected by anomalies like tape thickness, burrs on the material edges, and material warping, all of which can increase the height of the material surface, causing the tool to cut too deep. To make sure you’ve got it all dialed in, you’ll need to do two things. First, if you’re using tape, measure its thickness and offset the material’s z origin. Second, face your material with a 1/8" flat end mill before milling:

  1. Turn on BitBreaker Mode (Otherplan menu > Preferences > check the box for BitBreaker Mode)
  2. From the BitBreaker menu, choose Add Material Facing Job. It will come with a 1/8" flat end mill automatically selected.
  3. Set your facing depth to between 0.001" and 0.008", depending on how uneven the material surface looks.
  4. In Advanced settings for the facing plan, change your feeds and speeds to those specified below for a 1/8" tool.
  5. If you’re using the alignment bracket and you get a collision warning, check to make sure your material height is taller than the bracket screws. If it is, you can ignore the warning. Otherwise, you’ll have to remove the bracket or move your material away from it.
  6. Start cutting!

aluminum7

Once facing is done, your material thickness will be automatically reduced to compensate for the material that was removed. Now you can enjoy the benefits of milling at high feed rates, while being confident that your material is flat and will not cause any little end mills to break. Yay!

Tool: 1/8" flat end mill
Feed rate: 59 in/min (1500 mm/min)
Plunge rate: 5 in/min (127 mm/min)
Spindle speed: 16,400 RPM
Max pass depth: 0.002" (0.05 mm)

Tool: 1/16" flat end mill
Feed rate: 59 in/min (1500 mm/min)
Plunge rate: 5 in/min (127 mm/min)
Spindle speed: 16,400 RPM
Max pass depth: 0.002" (0.05 mm)

Tool: 1/32" flat end mill
Feed rate: 59 in/min (1500 mm/min)
Plunge rate: 5 in/min (127 mm/min)
Spindle speed: 16,400 RPM
Max pass depth: 0.002" (0.05 mm)

Tool: 1/64" flat end mill
Feed rate: 15 in/min (381 mm/min)
Plunge rate: 1 in/min (25.4 mm/min)
Spindle speed: 16,400 RPM
Max pass depth: 0.001" (0.02 mm)

Tool: 1/100" flat end mill
Feed rate: 15 in/min (381 mm/min)
Plunge rate: 1 in/min (25.4 mm/min)
Spindle speed: 16,400 RPM
Max pass depth: 0.001" (0.02 mm)