Our engineering team reviews thousands of PCB Gerber files every year. While every design is different, certain mistakes appear repeatedly — and many of them cause delays, additional cost, or in the worst case, boards that don’t work. Here are the five most common DFM (Design for Manufacturability) issues we encounter, and how to avoid them.
1. Insufficient Annular Ring on Drilled Holes
An annular ring is the copper pad surrounding a drilled hole. If the annular ring is too small, drill registration tolerances can cause the drill to break through the edge of the pad — creating a “breakout” that severs the electrical connection.
The IPC-A-600 standard requires a minimum annular ring of 0.05 mm for Class 2 boards and 0.075 mm for Class 3. In practice, we recommend designing to 0.125 mm (5 mil) or greater to provide comfortable manufacturing tolerance. Check your DRC settings in your EDA tool — most tools have an annular ring check built in.
2. Copper Too Close to the Board Edge
Copper placed within 0.3 mm of the board edge is a common cause of shorts and exposed conductors. During routing (cutting the board from the panel), the router bit can cause copper to lift or the board to delaminate at the edge if copper is too close.
The standard minimum copper-to-edge clearance is 0.3 mm (12 mil). For designs with board-edge castellations (half-holes), the rules are different — discuss your requirements with your fabricator before finalising the design.
3. Missing or Incorrect Solder Mask Clearances
Solder mask clearance defines how much copper is exposed around each pad. Too tight, and solder bridges form between adjacent pads during assembly. Too large, and pads on neighbouring nets get accidentally exposed.
Standard solder mask expansion (clearance beyond the copper pad) is 0.05–0.1 mm per side. For BGAs and fine-pitch QFN packages, discuss NSMD (Non-Solder Mask Defined) vs SMD (Solder Mask Defined) pad design with your assembly partner before generating Gerbers.
4. Via-in-Pad Without Filling and Capping
Placing a via directly in a component pad (via-in-pad) can cause solder wicking — molten solder flows into the via barrel during reflow, starving the joint and causing a cold or open connection. This is particularly problematic under BGA packages where joint inspection is difficult.
If via-in-pad is necessary for high-density designs, vias must be filled with epoxy and plated over (capped) before assembly. This adds cost but eliminates wicking. If via-in-pad is not essential, moving vias outside the pad and connecting with a short trace is the simpler and less expensive option.
5. Fabrication Notes That Contradict the Gerber Data
A surprisingly common issue: the fabrication drawing or fab notes specify a board thickness of 1.0 mm, but the impedance-controlled trace widths in the Gerbers are calculated for a 1.6 mm stackup. Or the notes say “4 layers” but only 2 copper layers are present in the file package.
Before submitting files, always cross-check that your fabrication notes, drill drawings, and Gerber layer count are consistent. At EazyPCB, our DFM process catches most of these discrepancies — but finding them after production starts costs time and money.
Running Your Own DFM Check
Before submitting files to any fabricator, run a DFM check in your EDA tool (KiCad, Altium, Eagle all have built-in DRC). Pay particular attention to:
- Minimum trace width and spacing
- Minimum annular ring and drill size
- Copper-to-edge clearances
- Solder mask apertures vs pad sizes
- Layer count and stack-up consistency
EazyPCB runs a free DFM review on every order. We will flag any of the above issues before production starts — but catching them yourself first saves time for both of us.
