4

I am designing a PCB which has +5V input from a USB jack and I want this power trace to be as large as possible to reduce input resistance. While doing my large traces on my PCB tool, one of the stock design rules is giving me an error that my neck down is too large.

Neck-down error

design rule

I don't see how this can cause a problem. Is there a reason why this type of design rule exists?

Alex C
  • 347
  • 2
  • 12
  • I don't see that being a problem, _provided that_ it is a DC power-supply line _only_. If there is an AC component to the flow on the trace, the neck-down that your software is complaining about could potentially cause reflected signals due to 'impedance mismatch'. Also, if it's actually complaining about _too little_ neck-down between pads & trace, that could be a 'parasitic capacitance' concern...also only applicable to ac/pulsed signal traces. – Robherc KV5ROB Feb 20 '16 at 17:44
  • Alex C, In my opinion, You can delete this rule or You can make %100. – O.Blue Feb 20 '16 at 18:21

1 Answers1

12

This rule aims to solve a manufacturing problem known as tombstone. During reflow, a too large connection to an SMD pad acts like a heatsink, creating a situation where one side of the component has a slightly lower temperature. Because of this, one side of the component can lift up from the PCB. This is especially true for small (0402 and smaller) components.

Lior Bilia
  • 7,282
  • 1
  • 20
  • 30
  • +1 You can join the SMD part with a reasonable width trace- like a thermal to a polygon pour- and then expand it out. The short thin trace will prevent the error (and the potential manufacturing issue), and won't add much resistance. – Spehro Pefhany Feb 21 '16 at 06:31