7
\$\begingroup\$

I am designing a board where I want to have the ability to separate the connection between two power net's by cutting a trace. Originally headers were meant to be used but due to size constrains I decided to go with this instead.

Googling terms like "PCB break trace footprint" and whatnot doesn't give much since it's mostly about how to fix those traces. So, what is the name of a footprint like this and where can I find more info on it? For example, recommended trace width, pad size, etc.

So far I have something like this where I can cut the two 6 mil traces, make a solder bridge if I need, and via's for if I need to solder wires with more rigidity than just relying on them being attached to the pads using solder. Example jumper thing

\$\endgroup\$
  • 1
    \$\begingroup\$ Why don't you use a zero ohm resitor as a link? \$\endgroup\$ – Jesus Castane Jan 13 '15 at 16:34
  • 2
    \$\begingroup\$ @JesúsCastañé Zero-Ohm resistor has a cost associated with it. A footprint with a trace between the pads doesn't add cost. \$\endgroup\$ – Nick Alexeev Jan 13 '15 at 18:03
  • \$\begingroup\$ Zero ohm resistors, like Nick Alexeev said, have a cost but also in my case I am worried about resistance since this is a somewhat high current connection across a power rail. Turns out zero ohm resistors can have up to 20 milliohms of resistance. \$\endgroup\$ – hak8or Jan 13 '15 at 19:43
7
\$\begingroup\$

Sometimes called a "Solder-Short" pattern. To create it you could use two half-moon shaped pads placed very close together, be sure to keep solder mask off the junction area. Usually the idea here is if you need the two signals shorted you then put down a solder blob covering both pad ends. With this method you start out with an open.

A way to create it and still keep the net connection would be to use an oval shaped pad with an oversized (non-plated) drill hole. You then run the two traces to the pad from opposite ends. The drilling of the over-sized hole physically cuts the pad in two. Re-solder the connection if needed later on.

\$\endgroup\$
  • \$\begingroup\$ Other then "oval" shape, you could also call it a "rounded rectangle". \$\endgroup\$ – Nedd Jan 13 '15 at 14:26
  • \$\begingroup\$ This is what I have done. I made a footprint that was about the size of a 0402, with the pads a bit closer together than they normally would be, and it worked great. \$\endgroup\$ – whatsisname Jan 14 '15 at 6:34
5
\$\begingroup\$

In Sparkfun-Passives Eagle library the part is called JUMPER-PAD, with several variants, like -NC (normally closed, i.e., paste layer present over the jumper), -NO, as well as one with a copper trace shorting two halves. Both 2 and 3 way, 3 way with paste or trace over 1,2 or 2,3.

\$\endgroup\$
3
\$\begingroup\$

Maybe you want to use a solder short and parallel it with a single-layer pad that can be drilled out. You'd probably want to make the drill-out pad and connections to it a net tie so the DRC deals appropriately with the shorted connections to the solder short. Here (from an earlier post of mine) is the solder short portion:

enter image description here

\$\endgroup\$
2
\$\begingroup\$

One of my coworkers just called it a scratch trace, but I haven't been able to find any evidence of this being a common term.

\$\endgroup\$

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.