Issue link: https://resources.pcb.cadence.com/i/1541046
15. Confirming Board Edge Clearances for Copper, Vias, and Components How To Implement 1. Obtain the fab and safety requirements: f Confirm the minimum copper-to-edge, via-to-edge, and component-to-edge clearances with your PCB fabricator's capabilities and your regulatory safety requirements (UL, IEC, IPC-2221). f For most fab processes, a minimum copper-to-edge clearance of 10-20 mil (0.25-0.5 mm) is typical; for high voltage or safety-rated boards, clearance may need to be 2 mm or more. 2. Set up mechanical layers and keepouts: f Draw the finished board outline using the mechanical or outline layer. f Add keepout zones inside the board edge for copper, vias, and components per your fab's guidelines. 3. Position all components and traces inside keepout zones: f During placement, ensure all components (including their courtyard and silkscreen) are inside the edge keepout. f Do not route traces or place copper pours within the restricted zone. f For edge-mount connectors or antennas, consult datasheets and fab guidance for special exceptions. 4. Manage vias and test points: f Do not place vias, test pads, or through-hole pins within the edge clearance area unless specifically intended for edge plating (castel- lations). f For high-speed or RF, ensure that stitching vias used for edge fencing are set back from the edge by at least the minimum clearance. 5. Check for slot, cutout, and panelization effects: f For boards with internal slots or cutouts, maintain the same clearances from their edge as from the board perimeter. f Consider panelization V-scores and breakaway tabs; increase clearance for fragile or critical areas. 6. Run DRC and visually review before release: f Use your EDA tool's DRC to catch any copper, via, or part encroaching on the edge keepout. f Review in the 3D viewer or print overlays to verify physical fit. Common Pitfalls, Their Impact, and How to Avoid Them Common Pitfall How to Avoid it Assuming fab defaults cover your use case Can end up with impedance mismatches, wrong clearances, and reliability issues – Always check the specific capability for your stackup and board thickness. Placing small passives, vias, or traces close to edge These can become exposed, break off, or short during handling or assembly – Define and ensure your design maintains minimum copper-to-board edge clearance. Ignoring cutouts or slot edges Copper inside internal slots can be just as problematic as at the outer edge – Define all board outlines and internal cutouts as well as set clearance rules. Not accounting for scoring and breakaway These processes can chip or remove copper if not enough setback is provided – Consult with your manufacturer on panelization method and add extra copper setback near v-score and breakaway tabs.