Seven DFM checks that prevent a PCB re-spin

A re-spin costs more than a new set of boards: it costs engineering time, a new prototype cycle and sometimes a customer commitment. These seven checks catch most of the issues that cause one.

1. Annular ring

If the copper ring around a via or component hole is too thin, the drill can break out of the pad. Keep at least 0.15 mm annular ring, and 0.20 mm on high-reliability designs. Check the pad size against the finished hole size, not the drill size before plating.

2. Solder mask between fine-pitch pads

A mask dam narrower than 0.1 mm may lift or flake, exposing copper and causing bridging. For fine-pitch parts, use a mask-defined pad strategy or remove the dam intentionally and adjust the stencil.

3. Via-in-pad without fill

An open via inside a BGA or QFN pad wicks paste away during reflow, leaving voids or an open joint. Either move the via out of the pad or specify epoxy/copper fill and planarization.

4. Copper too close to the board edge

Routing and V-scoring can expose or damage copper within 0.3 mm of the edge. Keep 0.5 mm where possible, and check the panel rail and break-away features at the same time.

5. Drill aspect ratio

A 0.2 mm hole in a 3.2 mm board is a 16:1 aspect ratio, which is outside standard plating capability. Reduce board thickness, increase the hole size or expect a process review and a higher price.

6. Silkscreen on pads

Legend printed over a pad can prevent solder wetting. Check the mask expansion and move the reference designator clear of the pad. This is especially common on 0402 and 0201 passives.

7. Missing or inconsistent fab notes

If the Gerber says one thickness and the drawing says another, the build stops until someone confirms. Put the stack-up, finish, mask colour, impedance and tolerance class in one drawing and reference the revision in the file name.