Most people use it to mill PCBs but that's boring
The Othermill creates very dimensionally accurate parts, but may be slower and more complex than other prototyping processes. If your part significantly depends on being diemnsionally accurate (for example, low backlash gears), then the othermill may be a good choice. Laser cutters produce a noticeable and uneven kerf, and 3D printing (FDM) cannot produce very fine details well.
The smallest commonly available Othermill bit that can be used to mill out parts is the 1/32" bit. This bit can cut up to materials that are 0.125" thick. Be aware that machining speed can be significantly slowed down the smaller the bit size is. Refer to online resources on Computer-Aided Machining (CAM) best practices on what bit to choose.
In order of machinability, here are the materials the authors have used successfully on the Othermill:
Delrin (acetyl homopolymer resin)
Lexan (polycarbonate)
Aluminum
The Othermill should not be used to cut steel.
Download the Jacobs Hall tool library from the Jacobs Hall bcourses training for the Othermill. Do not download the tool library directly from Bantam Tools, as it contains some inaccuracies.
Measure the stock and CAD the part to be no greater than the thickness of the stock. If the part is mostly flat, have its thickness match the thickness of the stock unless facing is needed.
Set up the Work Coordinate System as follows. Other tutorials may recommend you set the origin at the top of the stock, but this can cause poor results and collisions with the spoilboard. While these toolpaths will be offset in the Z direction when we import them into the Bantam Tools software, we will correct this at a later time.
Input the accurate dimensions of your stock in the Stock tab. Then, adjust the position of your part relative to the edges of the stock. Items in red boxes should generally be changed for each part or stock piece, while the rest should match the image.
The term "feeds and speeds" refers to how quickly the tool rotates and how quickly it moves along the x, y, and z axis. Smaller tools should generally be used with slower feeds and speeds.
Aluminum is significantly tougher than plastics. most important is the stepdown on operations with multiple depths; use a stepdown of at most 0.004". For drilling, use a very conservative chip clearing toolpath, pecking in 0.001" increments at a speed of 0.5 in/min. Milling aluminum with the Othermill is somewhat of an acquired skill, so don't worry if you break a bit or two at first. Do not attempt to mill aluminum with anything smaller than a 1/16" endmill.
Climb milling will result in a better finish and longer tool life.
Check the "keep tool down" checkbox or cuts with multiple depths will lift the tool each time.
Always keep the Ramp checkbox checked and generally use a ramp angle of 3-5 degrees depending on the material (larger angle ok on softer materials).
Facing
Bore
2D Contour
Always simulate your toolpaths in Fusion before exporting them for use on the machine. This is the primary way to prevent damage to the machine, the tooling, and the part
Open the simulation settings and check the "Stock" box. You can change from the default green color by changing the material options, but this is not important. Watch the entire simulation; if it is long, speed it up as little as necessary to ensure you catch any unintended behavior.
Right click on each operation on the left dropdown and select "Post Process". Select the settings for the Othermill and give your toolpath a descriptive name and number: e.g. 1_facing, 2_bore, etc. Numbering will help you keep track of the order in which to run each operation.
This step will produce .gcode files; these are text files containing a list of instructions that will be fed to the Othermill during operation. Make sure you save the gcode files in an accessible location on your filesystem.
Turn on the Othermill using the power switch at the back left corner.
Ensure that the emergency stop (big red button) is not engaged.
Connect the machine to a computer that has Bantam Tools installed.
Open Bantam Tools, and home the machine.
If using the fixturing bracket, locate the bracket by pressing "locate".
Insert a 1/8" endmill upside down (with the cutting flute inside the collet).
Load the material (tbd)
Load the toolpaths. Click the "Open Files" button and select your .gcode files.
Offset the toolpaths. If you do not perform this step, nothing will be milled. For each toolpath, open the "Placement" dropdown and enter -[stock thickness] under the z-offset. For exampele, if I have a sheet of nominally 1/8" Delrin that I have measured to be 0.135" thick, I would put "-0.130 in". You may also add x and y offsets, but be sure to repeat the process for each individual operation / toolpath.
Load a tool by clicking "Change...". Mount the desired bit and select it from the drop down menu. Click "Locate" and ensure that the mill has moved the bit above a clear section of the spoilboard (metal bed). If not, manually adjust. Confirm the position, and the machine will begin to move the bit down to touch the bed. While this is happening, make sure you are ready to stop the machine (press "ESC" or the emergency stop to stop). Once the bit has made contact with the bed, the machine should immediately stop trying to move the bit down. If you head any sound of resistance STOP THE MILL and try again.
A way to selectively remove material from a piece of stock
Contrary to popular belief, a mill is not a drill press. This is a manual mill:
A mill has a spindle which holds an end mill. End mills are similar in appearance to drill bits, but are not the same!
The spindle spins the end mill rapidly while the material (or the spindle) is moved in the x, y, or z directions. More advanced, usually computer numerical control (CNC) machines can also sometimes rotate, giving up to 4 or 5 "axes" to move in. With CNC milling, a computer, rather than a human machinist, handles the motion of the stock and spindle. Here is an example of a CNC mill in action:
Both manual mills and CNC mills generally share some basics in terms of how they operate. Here is a video that covers the basics of mills:
Just like drill presses, mills can make holes in materials. You can either use an end mill, or simply put a standard drill bit in the mill using a removable chuck. Mills are particularly useful if you would like a set of very precisely spaced holes, as they possess an x-y coordinate system (drill presses generally do not).
In the image above, notice that the center hole is not bored all the way through. This is generally possible to do fairly accurately even on a manual mill, with the use of a stop. However, dimensional accuracy may vary. Always check with your machinist first.
When it comes to sizing holes, make sure that there is actually a drill bit or end mill with the correct diameter for your hole. Perform a google search for a drill bit sizing chart or see the table here: https://en.wikipedia.org/wiki/Drill_bit_sizes#Drill_bit_conversion_table for a conversion between letter and number drill bits to decimal inches.
In the US, drills come in number sizes (smallest useful size being #50-#60 and going all the way up to #1, which is roughly 0.228 in) as well as letter sizes, which start at A (0.234 in) up to Z (0.413). Beyond and interspersed with the letter and number drills are standard fractional inch size, ranging commonly from as small as 3/64 in up to 1 1/2 in. Check with your machinist to see what sizes are available first.
A mill can remove material from a face or create a flat surface at any depth. Furthermore, sharp corners are possible if the tool is allowed to travel off the end of the part (see Pockets section for examples of when this is not the case). It is best if these cuts are at right angles to each other; more complex geometry will require the use of CNC.
For an example video of a CNC machine cutting a more complex profile, see below:
When a flat surface with some type of wall on the sides is desired, we have a pocket. Mills are able to do pockets, but keep a few things in mind:
End mills (the tool) have finite radii. For example, if an 1/8" diameter end mill is used to make a pocket, the interior corners will have a minimum 1/16" radius. Use a fillet in CAD to reflect this.
Conventional (manual) mills may not easily be able to make, for example, a rectangular pocket with precise corner coordinates, especially if the pocket is deep and requires multiple passes. This type of geometry is better suited for a function mill or a CNC mill. When in doubt, check what can and cannot be done with the person who will be making the part!
This type of geometry will generally only be possible with a CNC mill. Please be aware that CNC parts can have long lead times if coming from the machine shop. Furthermore, there are still limitations on what a CNC machine can do; as with manual mills, there are limits based on available tooling (curved surfaces generally require ball end mills) and the material.
That being said, there are some parts that are great candidates for CNC and it can certainly be a useful technology. Small parts especially will be easier to make (see: Othermill) and can make design significantly easier.
Try to limit the number of different tools needed to make your part. Tool changes can cost significant time and effort. For example, try making all holes a standard diameter, or choose just a few. If a pocket is large, use large-radius fillets on the corners to allow the machinist to use a single large tool to make the feature in one pass, rather than switching to a smaller tool just for the corners.
As a general rule, simple geometry is better. Things like right angles and low requirements for accuracy and precision (see: Tolerancing) make everyone's lives easier.
When in doubt, ask. Other club members or the machine shop staff are happy to help!
