The Othermill is an excellent tool for making and prototyping circuit boards. However, there are some important things to consider when designing your board. This page is intended for people who already have some knowledge of PCB design. If you’re brand new, we recommend Sparkfun’s PCB Basics. We’ll start with the design rule list, and then go into detail about each design consideration.
Design Rule List
- Minimum trace width: 6 mil for Othermill Pro, 10 mil for Othermill
- Minimum trace spacing: 6 mil for Othermill Pro, 10 mil for Othermill
- Minimum via/pad annular ring thickness: 6 mil for Othermill Pro, 10 mil for Othermill
- Minimum drill size: 16 mil (or smaller with non-standard bits)
- Minimum SMD pad size: 6 mil for Othermill Pro, 10 mil for Othermill
- Polygon isolation value: 1 mil larger than the largest tool you want to use
- Route traces to through-hole pins on the bottom side only (holes are not plated)
- Slotted/oval holes are not supported
Spacing Between Traces and Components
When designing circuit boards to mill on the Othermill or Othermill Pro, it’s important to consider the distance between each element of your board because the spacing between elements dictates the size of the tool you’ll need to mill them.
For example, if you’d like to use a 1/32" end mill, your traces, pads, vias, etc. need to be greater than 0.03125" apart. You can use smaller tools, like a 1/64" or 1/100" end mill, which will allow you to place objects closer together. However, the trade-off is that smaller tools take longer.
The same holds true for vias and through holes — the inner diameter of each hole needs to be larger than the tool you’re planning to use to drill it. If you’re unsure as to whether some elements are too close together, you can test it by importing your files into Otherplan and seeing how it looks.
Spacing and hole size are too small for the chosen end mill.
Spacing and hole size are correct for the chosen end mill.
If you’ll be using surface-mount (SMD) components, the pads need to have enough space between them for the tool to fit. Check the SMD package compatibility list to make sure. If your package isn’t listed, you can test if it will work by exporting your EAGLE .brd file or Gerber files, importing them into Otherplan, selecting a tool, and looking to see if there are cut lines between the pads.
If your board has vias (electrical connections between the front and back of the board), you’ll need to create a connection between them by hand when you solder the board. For this reason, we recommend minimizing the number of vias and through-hole connections you use in your board.
The simplest way to connect a via is to put a short piece of wire through the via hole and solder both ends, but you can also use via eyelets (aka rivets), which sit neatly in the holes as you solder them. Just make sure your eyelets fit your holes. A third option, which is often the fastest, is to take a long piece of tinned wire and thread it through all the vias in your board. Then solder all the vias and snip off the excess wire.
PCB software autorouters will often use through-hole pins as vias. This presents a problem when you use components that can’t be soldered easily on both sides of the board, such as pin headers. To avoid this issue, draw polygons in the Restrict layers over the areas you want the autorouter to avoid. In EAGLE, for example, these are the tRestrict (41), bRestrict (42), and vRestrict (43) layers.
If your file is designed with a ground or power plane, check to make sure that your polygon isolation value is set to at least the width of the smallest tool you’re going to use on the Othermill. If the isolation is set to zero, which is often the default in PCB design software, the tool will not fit between the ground/power plane and the traces. If your design allows for it, setting the polygon isolation to the width of your largest tool will greatly speed up the milling process. For example, if your design has a few tiny features that need to be milled with a 1/100" tool, but most of the other features can be milled with a 1/32" tool, setting your polygon isolation to 0.032" instead of 0.011" will allow you to use a 1/32" tool for most of the board, which is much faster than using a 1/100" for the whole board.
Trace Width > 6 mil for Othermill Pro, 10 mil for Othermill
The minimum trace width we suggest is 6 mils (0.006") for Othermill Pro, 10 mils (0.010") for Othermill because thinner traces are more likely to delaminate from the board. We suggest using the widest traces your design can support.
Likewise, annular rings for through holes and vias should be at least 6 mils for Othermill Pro, 10 mils for Othermill (outer diameter minus inner diameter).
Slotted/Oval Holes Not Supported
Otherplan doesn’t support the G85 command which is used to make slotted/oval holes. If you need a slot, make a row of overlapping holes that are a few thousandths of an inch larger than the tool and overlap by about half their diameter (i.e. for a 1/32" (0.031") tool, make a row of 0.033" holes, with centers spaced 0.016" apart).
Ways to Increase Milling Speed
Larger end mills mill faster than smaller ones, so you can increase milling speed by spacing out your components, traces, and holes such that they can all be milled or drilled by a 1/32" or larger end mill.
Minimize the use of 1/64" and 1/100" end mills by using rounded corners instead of angles. Otherplan takes time to mill the innermost angle, where a 1/32" can’t reach, which is helpful in some situations but not here. The corner radius needs to be larger than 0.03125" for this to work with a 1/32” end mill.
DRC (Design Rule Check) Files
If you’ve never used DRC files, they help you find layout-related problems with your board, such as components or traces that are too close together.
We currently have DRC files for EAGLE, which you can download from the EAGLE page.
If you’ve made DRC files for your favorite software, please email them to us at firstname.lastname@example.org and we’ll post them here!