Issue link: https://resources.pcb.cadence.com/i/1541046
38. Specifying and Checking Solder Mask and Paste Mask Clearances How To Implement 1. Set solder mask expansion values per fab guidelines: f Typical expansion is +2 to +4 mil (0.05-0.10 mm) per side of the pad, but check your manufacturer's minimum and recommended values. f For very fine-pitch or closely spaced pads (QFN, BGA, 0.5 mm pitch or below), request "solder mask defined" (SMD) pads if required. 2. Check for mask slivers and potential bridging: f In dense areas, verify that solder mask dams (the mask strip between adjacent pads) are at least the fab's minimum (typically 3-4 mil, 0.08-0.10 mm). f Avoid mask "slivers" (thin strips) that can peel or lift off during assembly. 3. Review paste mask (stencil) reductions for large pads: f For large thermal pads (QFN, PowerPAK, D2PAK), reduce the paste mask opening by 30-50% and use "windowpane" or segmented stencil apertures for even solder spread and optimal thermal contact. f Apply smaller paste openings or "paste reductions" to fine-pitch pads to avoid solder bridging. 4. Perform layer-by-layer checks in CAD: f Visually review all mask layers against pad geometry for coverage, clearance, and alignment. f Run the EDA tool's mask/paste DRC to catch unintentional openings or coverage errors. 5. Request solder mask and stencil files from the manufacturer for review: f Many fabs and assemblers generate their own masks from your Gerbers, IPC-2581, or ODB++ - always review their proposed layers before approving for production. 6. Document special requirements in the fab notes: f Call out areas needing "no mask" (bare copper), custom mask clearance, or special stencil reduction in your fabrication drawings and assembly notes. Common Pitfalls, Their Impact, and How to Avoid Them Common Pitfall How to Avoid it Using default mask settings without review Can cause opens, shorts, or tombstoning, especially in fine-pitch areas – Define and enforce mask-specific DRCs. Too small mask dams or slivers Prone to mask lifting, bridging, and assembly failures – Set minimum mask width rules. Not specifying paste mask reduction for thermal pads Causes excessive solder, voiding, or part float – Include paste mask notes in fabrication documentation. Missing or misaligned mask coverage on critical parts Risk of corrosion, shorts, or unreliable solder joints – Add a DFM/CAM step to inspect soldermask and paste overlays.