The two pins are next to each other and they must be connect together.

How should I do that?

enter image description here

Just connect them together with a simple trace?

enter image description here

Or pour them together?

enter image description here

  • 2
    Does this really matter? – Andy aka Mar 23 '16 at 8:29
  • I would use the first option, but enable teardropping to remove the nasty right-angle copper lines. If teardropping is not viable, just draw on some extra track instead. – CharlieHanson Mar 23 '16 at 8:47
  • Can you place a zero ohm resistor between the 2? This way it could be removed it needed. – Eric Johnson Mar 23 '16 at 18:51
up vote 26 down vote accepted

A large pour would allow more current (just like a wider trace), and would result in a larger solder blob. You probably need neither.

A simple trace between the middles of the pads might look like an accidental solder bridge if you don't know the circuit. To avoid such a misunderstanding, it might be a better idea to route the trace outside, if you can afford the space:

two pads connected with loop

  • 6
    I always use this idea if at all possible. Using this technique makes it easy to cut the trace in the case that the design has to change for some reason. On a recent design I had four I2C chips with their address pins connected like this to GND or VCC. It was necessary to replace one of the chips with a much larger capacity memory device and it necessitated changing the address range of one of the other I2C parts. I was able to re-work the design very simply by cutting one of the loops and then adding a neat short loop of wire. – Michael Karas Mar 23 '16 at 10:13
  • This is a very nice answer. I used to do as in this answer, but I haven't lately, because I forgot the reason for it. – pipe Mar 23 '16 at 10:45
  • 2
    If the space is a concern, it can also be tucked under the chip. Not ideal but better than having a blob of solder over two pins. – Sebi Mar 23 '16 at 15:23

In general it's best not to pour over pads (without thermal reliefs). It makes them harder to solder and desolder. The exception is high current stuff or stuff where you are using the tracks as heatsinks.

Going directly between pads with a track can lead people to think there is a manufacturing fault, especially if the soldermask on the track flakes off. Still it may be the best option on a very cramped board.

Usually a U shaped track coming out from the chip as CL suggests is the way to go.

I have been known to put a U shaped track under the chip, the downside of that approach is you have no way of cutting the track if you discover a design flaw.

Your Answer

 

By clicking "Post Your Answer", you acknowledge that you have read our updated terms of service, privacy policy and cookie policy, and that your continued use of the website is subject to these policies.

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