PCB Design

Owned by Jack Christensen
Last updated: Jul 14, 2022 by Zachariah Henry Howden Mears
3 min read

Our PCB Design Specifications

  • Track Clearance: 8 mils (0.2032 mm)

  • Minimum Track Width: 8 mils (0.2032 mm)

  • Minimum Via Side: 30 mils (0.762 mm) / 15 mil drill (0.381 mm)

  • Copper Thickness: 1 oz

Note: Most of our manufacturers can handle smaller traces and spacing. If you want to use anything less than the above specs, please check with others and have justification.

  • If your PCBs are meant to be screwed onto something, put mounting holes on your layout, and if at all possible, use M3 screws. This is for standardization purposes. If you have a space restriction, smaller screws might be fine, but check with someone mechy first. 

  • If a pin is listed as NC (not connected) on a data sheet, don’t tie it to ground. Just leave it unconnected. Some manufacturers use NC pins for in production testing, and as such they aren’t actually high impedance pins, and shorting them elsewhere may destroy your IC.

  • Use plated holes for any through-hole components. This is default in most PCB design software. If a trace on the bottom and a trace on the top of the board meet at a component lead, the hole, not the lead, should be the conductor between them. Not using plated holes can cause continuity issues if the solder doesn’t wick completely through the hole during assembly.

  • Add debug LEDs to PCBs that use microcontrollers when possible. 

  • If it is reasonable, route traces so that if a solder joint on one component fails (e.g. if a pad rips off), it does not affect downstream components (see Figure 1 below). This applies especially to power connections for independent parts of the circuit. Don’t daisy-chain power lines through the leads or pads of components.

Power Trace Routing

  • Don’t print PCBs at the 3D Printing Center in E5. These are typically poor quality.

  • Make sure that solder-mask clearance is set such that there is solder-mask between component pads (pay attention to fine-pitched components) and that there is no mask on the pads themselves.

  • Thoroughly check the Gerber files for the board before you send them out for fabrication: 

    • Check the copper layers and ensure that there are no unintended connections. 

    • Make sure that all pours that should be connected are, especially if you manually stitched together different parts of the pour. 

    • Make sure that the solder-mask appears the way you expect it to (Note: the places where solder-mask is shown is actually where there isn’t solder-mask).

  • Use SMD pads that are longer than you need. KiCad has specific footprints whose names end in HandSoldering, which have extended pads for easier hand-soldering (e.g. use ”R 0805 HandSoldering” instead of ”R 0805”). 

  • BGA components can’t be hand-soldered. We have a reflow oven, but laying paste and inspection will be difficult to impossible. Avoid BGA packages if you plan to assemble by hand. QFN packages can be assembled by hand using the reflow oven, but it is very very difficult, avoid if possible.

  • Don’t batch assemble boards (if you are making multiple) when they arrive. You will be less inclined to change your design if you notice small bugs if you’ve already committed lots of components (which are worth far more than the cheap boards) to this design. Build one, test to death, then decide whether to make another revision or to assemble the rest.

See also: PCBs