Essential FPC Design Guidelines for Engineers – Part 1: Mastering the Basics of Flexible PCB Design

Master FPC design with these essential guidelines! Learn best practices for outline, drilling, circuit, and solder mask design to create reliable and high-quality Flexible PCBs.

Discover the essential Flexible PCB (FPC) design guidelines in Part 1 of our series. Learn the basics every engineer needs to create reliable, space-saving, and cost-effective FPCs

Outline and Drilling Design

1. The minimum distance between through-holes and the board frame should be 0.5mm. If less than 0.5mm, change to a U-shaped hole (connecting the hole to the board frame).  

2. The distance between vias and the solder mask opening must be at least 0.2mm; otherwise, copper may be exposed around the hole.  

3. FPC should not have via-in-pad design because FPC cannot perform resin plugging, which may cause solder leakage.  

Circuit Design  

1. Large copper areas may oxidize: Air trapped during pressing may cause oxidation under high temperature and pressure, leading to poor appearance but no functional impact. To avoid this, use a copper grid pattern or add solder mask openings on large copper areas.  

2. Avoid isolated pads: If pads are isolated and overlapping on both sides, the 25um core material in the FPC makes them prone to peeling. It is recommended to add copper fill and connect pads at four corners for better adhesion. Upper and lower pads should be offset to improve bonding strength.  

3. Connector pads are prone to peeling. Use a pressure PAD design.  

4. Avoid designing large exposed copper areas, as they may wrinkle.  

5. FPC uses coverlay as the solder mask layer. Coverlay must be pre-cut before lamination. The distance between pads and traces should be at least 0.2mm. Solder mask bridges should be at least 0.5mm wide. If pad spacing is below 0.5mm, JLC will default to exposing traces.  

6. Sparse traces in flexible cables are prone to tearing at corners. Add tear-stop copper strips at board edges or network copper on the back.  

7. Prefer a 45-degree copper grid for better signal transmission. Recommended trace width/spacing: 0.2/0.2mm.  

Edge Gold Finger Design  

1. Plug-in fingers: Laser cutting may cause carbonization, leading to micro shorts between gold fingers. Offset gold fingers inward by 0.2mm (JLC will adjust by default; specify if different).  

2. Soldering fingers: Do not place vias in a straight row along the pads, as stress concentration may cause breakage.  

3. Offset coverlay openings for soldered gold fingers by at least 0.3mm to prevent breakage.  

4. Extend soldered fingers so that the solder mask covers the pads by at least 0.3mm for a pressed PAD effect.  

5. Gold finger solder mask openings: Extend at least 0.3mm beyond pads to prevent separation from the connecting traces.  

6. JLCPCB does not support hollowed-out boards. Reverse fingers require additional pads and vias for layer switching.

7. Since FPC uses coverlay instead of green solder mask, solder mask bridges cannot be formed the same way. Do not add unnecessary copper fill on IC pads; otherwise, pad size will increase, reducing spacing and causing short circuits during soldering.  

8. Gold finger pads should be independent. If pads are connected to copper fills or traces, exposed copper or traces may appear when opening solder mask.  

9. Gold finger dimensional tolerance is ±0.1mm by default. If ±0.05mm is required, specify when placing the order.  

Solder Mask Design  

1. Connector seats in FPC are prone to detaching. Use a pressure PAD design.  

2. IC center areas must have solder mask bridges to retain inner solder mask.  

3. Gold finger pads must have solder mask openings; otherwise, they cannot connect with the connector.  

4. The default solder mask layer is "soldermask." Ensure the correct solder mask layer is used.  

5. To prevent via copper from breaking when bending, FPC vias are tented by default. If via openings are required, specify clearly when placing the order.  

6. If test points are defined as vias, they may not be correctly generated. Test points should not be set as vias or should have separate solder mask openings.  

7. Large exposed copper edges on double-sided boards may cause blackening. Add a ring of coverlay around the board edges.  

Silkscreen Design

Avoid placing text inside the board outline, as it may be removed during manufacturing.

Following these FPC design guidelines will help you create reliable, high-quality Flexible PCBs for a wide range of applications. From outline and drilling to solder mask and silkscreen design, every detail matters.