17
\$\begingroup\$

I don't do my own CAD work. I have a mental checklist of what to look for when the PCB is placed, critical routed and routed. But is there a good checklist you have or can point me to? I'm not looking for schematic items, that is covered here.

\$\endgroup\$
7
\$\begingroup\$

From the previous question, this link also contains Atlantic Quality Design's PCB checklist. A one you can check off is here

Edit Jan 6 2011: Electronic Product Design has one with some unique items.

An archive of one from Avanthon has a good list.

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

Preliminary

  • Check the footprints, especially for connectors, parts that are available in multiple packages, and those new footprints. Print 1:1 plots and place the parts on them.
  • Have PCB fab check your controlled impedance calculations.

Placement

  • Check that the decoupling caps are where you wish. Since they go from power to ground, it isn't obvious where they were intended to go without looking at the schematic.
  • Check connector placement, board size, etc. Don't forget mounting holes.

Critical Route

  • Inspect every critical route, including before and after and resistors used for termination.

Full Route

  • Report on all net lengths. Check for ones that are too long.

Other

  • Fiducials, both global and for BGAs.
\$\endgroup\$
7
\$\begingroup\$

This is my list for boards I lay out in Ultiboard.

  • Are there any antennas? Edit -> Copper Delete -> Open Trace Ends
  • Are there any unused vias? Design -> Remove Unused Vias
  • Are there any design rule errors you can't explain?
  • Are there any connectivity errors at all?
  • Does it look wrong? Look at the board for obvious stupidity like parts that have been eaten or moved.
  • Are there bypass caps directly on the power rails of EVERY chip? Even the ones that don't look like ICs, like regulators?
  • Are there filters directly on EVERY transistor gate/base? Even the ones in processors? Half an inch is probably too far away.
  • Are there filters directly on A/D converter pins?
  • Are the traces wide enough? Especially power traces? Make the traces as large as reasonable, unless you have specific reason not to.
  • Use power planes where possible, especially under processors
  • Are the thermal reliefs as you intended? High-current components get no thermal relief, but also no solder mask! Otherwise it will be very difficult to solder. Make sure there's plenty of exposed copper on both sides of the board for those components. Everything else gets standard thermal reliefs, 10 mil or so is probably fine spoke width.
  • Are all test points labeled?
  • Is the board name (or part number) printed on the silkscreen? Correct revision?
  • Is there sufficient distributed cap on the power rails? One big cap in the corner isn't as good as four smaller caps spread around the board.
  • Are all isolation barriers wide enough?
  • Are all high voltage clearances in place? Look particularly for traces under heat sinks tied to high voltage through a transistor tab. Also look for clearances to any mounting holes.
  • Check all the layers. Sometimes I've left the solder mask layer turned off, only to find that there was some odd shape on it that I'd placed by accident.
  • Are all footprints and pinouts correct? Collector-emitter reversal has happened to me on more than one occasion.
  • Is the silkscreen correct, showing reference designators, not values? Check the actual exported gerber.
  • Are all user terminals marked with function, + -, other relevant information?
  • Are all op-amp power rails connected? Ultiboard likes to randomly eat them.
  • Don't trust the auto-router. It's tempting, but ultimately not worth the effort. Only use it if there's a question if something is at all routable.
\$\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.