I'm trying to decide on the best layout for caps on a DC/DC converter. Which of the following options (or another, unlisted option) is the best choice?

  1. GND Out plane with 5V Out going the opposite direction of the caps.
  2. GND Out plane with 5V Out going the same direction of the caps.
  3. GND Out and 5V Out both going the opposite direction of the caps.
  4. GND Out and 5V Out going the same direction of the caps.

Or does this even matter?

enter image description here

Other details:

  • There are less than 5 components on the output side so a ground plane may be overkill?

  • Caps are 1uF

  • \$\begingroup\$ Why do you have so many caps so close together? \$\endgroup\$ – Ignacio Vazquez-Abrams Sep 20 '14 at 17:16
  • \$\begingroup\$ Anyways, bulk caps in-line, decoupling caps out. \$\endgroup\$ – Ignacio Vazquez-Abrams Sep 20 '14 at 17:17
  • \$\begingroup\$ Number 2 is the most correct of the set. I matters because the goal is to get output with minimum ripple voltage. For example in the first case, capacitor tries to maintain constant voltage, but the output pin is jumping up and down due to inductance between the output and the capacitor. \$\endgroup\$ – venny Sep 20 '14 at 17:28
  • \$\begingroup\$ What are you trying to achieve - we know nothing about your circuit and maybe also what does the data sheet inform you? \$\endgroup\$ – Andy aka Sep 20 '14 at 19:39
  • \$\begingroup\$ Is the converter designed to be galvanically isolated? If not, why not tie the ground planes together - they are almost certainly connected internally inside the chip. \$\endgroup\$ – Damien Mar 21 '15 at 22:59

Option 2 is the most suitable given the choices presented.

Why: Ground planes are always better for re-circulating currents than tracks. (eliminating options 3 and 4). The capacitors are likely to serve dual purposes: first for recirculating currents, second bulk capacitance of the output rail. Given the later that eliminates option 1. Hence option 2 is the most suitable given the choices.

However, you need to consider input ripple current and how to filter that, so ideally your should have a series inductor followed by your bulk capacitance with low esr before the input supply. This will keep input ripple localised.

Next splitting ground planes is never a good thing. You are better off having an isolated ground copper shape around your DC/DC converter with all of your filter components (input inductor and capacitor and output capacitors) attached to the ground shape and then connect it to your overall PCB ground plane. Ideally you should have a ground plane on an internal layer and isolate it from your through hole component with a ground shape around the DC/DC with filter components, and then stitch your local ground shape to the plan around the edge or in one location.

this will achieve two things: one you have a continuous ground plane across your whole board, two your recirculating currents are kept on the local ground shape.


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.