To save cost on a board I'm designing, I'm considering replacing an 8x2 male pin header intended for jumpers (which previously replaced an 8-position DIP switch) with 8 pairs of rectangular solder bridge pads.

My question is: How much of a gap should I leave between the pads in each pair?

Also, if I want some of them to be closed by default, where you scratch away the trace to open them (and can rebridge them with solder later), how thick should I make the scratch trace?

  • 2
    \$\begingroup\$ Personally, I prefer using 0 ohm resistors for this. Costs almost nothing, and then it is easy to set it up during PCB assembly all with machines. If we are talking about saving cost I assume it's fairly high volume production, so making solder bridges or cutting by hand is not very cheap. \$\endgroup\$
    – Klas-Kenny
    Nov 26, 2021 at 21:27

2 Answers 2


There's no definitive answer to your question, because it depends:

  • How often do you expect to need to bridge or un-bridge these?
  • What is the accessibility of the area like? Are other components nearby making it difficult to work on the bridges?
  • Who are these jumpers intended for? End users? Hobbyists? Engineers?
  • Are you space-constrained? The bridges could be 0201 component size and require magnification to work on.
  • I expect this to not apply, but what is the voltage? Higher voltages would require a larger gap.

Have you hand-soldered 0402 components? The gap between pads of an 0402 is about 0.5 mm. On the larger end, 2.54 mm (0.1 inch) is the same distance as typical perfboard (proto board) and those are relatively easy to bridge with enough solder (of course the copper-to-copper pad spacing is probably closer to 1 mm). As long as you keep the gap wide enough for the fabricator tolerances (e.g. 0.15 mm or 6 mil is sometimes a minimum), and voltage is not a concern, select a gap that meets your criteria, similar to the ideas I listed.

As for track width for closed-by-default jumpers, that depends primarily on current and how much effort you want to go through to cut the track later. If these are just short tracks for logic voltages, consider using an 0402 component with a 0.2-0.3 mm wide track connecting them. That's what I do for prototypes and it works well. Mind you, cutting tracks with a knife later is a bit messy. I prefer to use 0-ohm 0402 jumpers instead of tracks meant for cutting.

  • 3
    \$\begingroup\$ Also you may be interested in an article by Altium about this. \$\endgroup\$
    – JYelton
    Nov 26, 2021 at 21:19
  • 2
    \$\begingroup\$ 0805 (2012 metric) work well for perf board (as do 0603/1608 but they're a bit small). 1206 (3216) work particularly well but they span 3 pads so to avoid shorts the middle pad needs to be removed with a scalpel. \$\endgroup\$ Nov 26, 2021 at 21:47

Simply add 0 Ohm resistors to the schematics, using standard footprints. Do not include the ones that should be open to BOM and position files when you send them out to manufacturer. The cost of a few jumper resistors is negligible.

For a few $ buy a bunch of these resistors for yourself in case you need to reconnect pads in the future.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.