13 Critical Spacing Rules You Should Never Ignore in Flex PCB Design

Flexible PCB boards are the foundation of modern compact electronics. They enable lightweight, flexible connections in devices such as smartphones, medical equipment, and automotive sensors.However, improper spacing design is one of the most common causes of flex PCB defects — including solder bridging, copper cracking, and delamination during bending.

This article outlines 13 critical flexible PCB design spacing rules that every engineer should follow to ensure high yield, mechanical reliability, and electrical safety.

1. Coverlay Bridge Spacing

A coverlay (flexible PCB solder mask) bridge is the narrow section of coverlay between two adjacent pads. To maintain stability, the distance between pads must be at least 0.5 mm.If the gap is smaller, the coverlay bridge can easily break during lamination or reflow, leading to solder bridging or short circuits.

2. Coverlay Opening to Copper Spacing

The gap between a coverlay opening and nearby copper should be no less than 0.15 mm. When this clearance is too small, even slight misalignment during the coverlay process can expose copper, causing solder wicking or shorts during component mounting.

3. Maximum Coverlay Opening Length

Large openings in the coverlay are prone to deformation or stretching during the lamination process. The opening length should not exceed 20 mm, as oversized windows can cause misalignment, wrinkles, or adhesion issues when applying the coverlay film.

4. Pad to Board Outline Spacing

Pads must be placed at least 0.2 mm away from the board outline. During laser cutting, edge carbonization may lead to short circuits if the pad is too close to the outline. Sufficient spacing ensures clean edges and protects pad integrity.

5. Edge Pad Width

Pads located at the board edge must be at least 0.5 mm wide.When submitting your design, note explicitly that pads should not be trimmed. Some manufacturers automatically reduce 0.2 mm from the edge for safety, which could lead to pad lifting or cold solder joints.

6. Trace or Copper to Board Edge Spacing

To avoid copper damage during profiling, maintain at least 0.2 mm clearance between traces (or copper areas) and the board outline. If the copper is flush with the edge, the CAM engineer will typically retract it 0.2 mm inward, potentially breaking the electrical connection.

7. Trace to Pad Spacing

When pad spacing is less than 0.5 mm, avoid routing traces between them. Keep at least 0.2 mm between any trace and adjacent pad. If you must route through tight spaces, consider using a double-sided flex PCB to maintain solder mask alignment.

8. Stiffener to Pad Spacing

The stiffener region should extend at least 1.0 mm beyond the pad area. Insufficient spacing may cause cracks where the pad and trace meet during bending, resulting in open circuits.

9. Minimum Stiffener Width

The stiffener must have enough width for adhesion strength and cutting stability. Recommended minimum widths are:

FR4 stiffener: ≥ 3 mm

PI stiffener: ≥ 2 mm

Steel stiffener: ≥ 1 mm

Narrower stiffeners can cause lamination difficulty and are prone to carbonization during laser cutting.

10. EMI Shield to Pad Spacing

The EMI shielding film is conductive, so it must be kept at a certain distance from the pads. The opening of the EMI shielding film should be at least 0.8 mm away from the adjacent pads. This can prevent short circuits and maintain signal integrity during operation.

11. Via to Board Edge Spacing

Maintain a clearance of 0.5 mm or more from the via edge to the board outline. If vias are placed too close, laser cutting may damage the hole, leading to pad cracks or disconnections. Vias should also be staggered instead of aligned in a straight row to minimize stress concentration during bending.

12. Via to Coverlay Opening Spacing

Vias should never be positioned at the junction between covered and uncovered areas. Keep a minimum of 0.3 mm clearance between the via and coverlay window edge. The transition area experiences significant mechanical stress, and vias placed too close may develop copper fractures over time.

13. BGA Pad Diameter

The minimum pad diameter for BGA components should be 0.25 mm or greater. Smaller pads can result in insufficient plating, weak solder joints, or even pad detachment during reflow.

Additional Design Clearances in Flex PCB Layout

Beyond these 13 rules, designers should also observe several general clearances critical to flexible PCB reliability:

Trace-to-trace spacing: ≥ 0.05 mm (standard); ≥ 0.035 mm for HDI flexible circuits

Copper-to-outline spacing: ≥ 0.3 mm

Coverlay opening-to-copper spacing: ≥ 0.1 mm

Ground-to-signal spacing: ≥ 0.2 mm to reduce crosstalk and impedance drift

Trace-to-bend edge spacing: ≥ 0.5 mm in dynamic flex zones

Adhering to these parameters ensures that your design meets IPC-2223 flexible circuit standards and aligns with most manufacturers’ DFM (Design for Manufacturability) capabilities.

Why Flex PCB Spacing Rules Matters ?

Every spacing rule contributes to one or more of the following design goals:

Electrical safety – preventing shorts and leakage

Mechanical strength – reducing stress concentration in bending areas

Assembly yield – avoiding solder bridges and pad lift

Process reliability – ensuring coverlay, lamination, and laser cutting precision

Ignoring even a single clearance rule can lead to performance degradation, assembly failure, or high scrap rates.

Conclusion

Correct spacing design helps a flex PCB perform better, last longer, and maintain stable production quality. These spacing rules are closely tied to the fabrication tolerances of flexible PCBs. Understanding the manufacturing process will help you make more reliable designs — explore our FPC fabrication page to learn more.