Home > News > fpc-flexible-pcb-design-guide-8-key-points-you-must-know.html

FPC Flexible PCB Design Guide: 8 Key Points You Must Know

03 Jun 2025 15:48:06 GMTPCBASAIL
Table of Contents

FPC flexible board, namely Flexible Printed Circuit Board, is a type of printed circuit board made from flexible substrates, often referred to as soft circuit boards or flexible circuit boards. FPC flexible boards have now been widely used in modern electronic products, as they are thin, lightweight, and bendable, and can be processed into any shape and size, complementing FR-4 PCB rigid boards. However, due to differences from rigid PCB boards, there are special considerations in design. This article focuses on 8 key design points of FPC:


FPC Design Pitfall Avoidance Guide


Drilling, board frame, circuit, solder mask, and text design for flexible boards are similar to those for PCBs, except that stiffener layers need to be added on the back of components and at interface positions. However, there are also special considerations, introduced as follows:

1. Outline and Drilling Design


(1) The minimum distance from a through-hole to the board frame line is 0.5mm. If less than 0.5mm, it should be changed to a U-shaped hole (the hole is connected to the board frame).
(2) The distance from a via to the solder mask opening should be at least 0.2mm; otherwise, copper may be exposed at the hole edge.
(3) It is not recommended to design vias-in-pad for FPC. FPC cannot perform resin plugging, and vias-in-pad may cause solder leakage. Modified panel frame.jpg

2. Circuit Design


(1) Oxidation of large copper surfaces: Due to the design of large copper surfaces, air is difficult to evacuate during film lamination. Moisture in the air reacts with the copper surface under high temperature and pressure to cause oxidation, resulting in poor appearance (functionality is not affected). To avoid this, design grid copper cladding or add solder mask openings on large copper surfaces.
(2) Avoid independent solder pads: As shown in the figure, circuit solder pads that are independent and overlapping on both sides are prone to detachment (since the intermediate substrate of FPC is only 25μm). It is recommended to add copper cladding, connect the four corners of the pads to the copper cladding with connecting lines, and stagger the upper and lower pads to increase bonding strength.
Independent pad.jpg
(3) Pad detachment: Connector seat pads are relatively independent and prone to detachment; use pressed PAD design.
(4) Avoid large areas of exposed copper, as this may cause wrinkles.
(5) FPC uses coverlay as the solder mask layer. The coverlay needs pre-opening and bonding. There should be a 0.2mm spacing between the solder pad and the trace, and the solder mask bridge should be at least 0.5mm (i.e., the spacing between two solder pads should be at least 0.5mm). Otherwise, open a full window and accept exposed traces.
(6) Tearing at corners: Sparse cable traces make corners prone to tearing. Add anti-tear copper strips on the board edge or grid copper on the back. The sparse wiring of the flex cable makes it prone to tearing at the corners..jpg

(7) The circuit grid is preferably laid at a 45-degree angle for better signal transmission. The recommended line width and spacing are 0.2/0.2mm.

3. Edge Gold Finger Design


(1) For pluggable fingers: High-temperature carbonization at the board edge during laser cutting may cause micro-shorts between gold fingers. The gold fingers need to be recessed by 0.2mm (generally uniformly recessed; special requirements should be specified).
(2) For soldering fingers: Vias on the in-board solder pads should not be arranged in a single row to prevent stress concentration and breakage.
(3) The upper and lower coverlays of soldering fingers should be staggered by more than 0.3mm to prevent breakage.
(4) Soldering fingers are recommended to have a solder mask film pressing PAD effect (i.e., extend the solder pad so that the coverlay presses the pad by more than 0.3mm).
(5) Solder mask opening for gold fingers: The opening is recommended to press the pad by more than 0.3mm to prevent disconnection between the gold finger PAD and the connection.
(6) If hollow boards are not supported, reverse fingers need to add pads and vias to achieve layer change.
(7) Since FPC solder mask film cannot form solder mask bridges like green oil, IC-type pads should have no extra copper cladding (unreasonable design may cause soldering short circuits due to larger pads and reduced spacing).
(8) Gold finger pads should be independent; copper cladding or traces on finger pads will be exposed after solder mask opening.
(9) The default tolerance for gold finger outline is ±0.1mm; ±0.05mm requires confirmation when placing an order.

4. Solder Mask Design


(1) FPC connector seats are prone to detachment; use pressed PAD design.
(2) Bridging is required in the middle of the IC to retain the intermediate solder mask.
(3) Gold finger pads must have solder mask openings; otherwise, they cannot conduct with the connector.
(4) Soldermask is used as the default solder mask layer; ensure the correctness of the solder mask layer.
(5) To prevent via copper from breaking during bending, FPC vias are generally defaulted to be oil-covered; opening requires notation when placing an order.
(6) Test points designed as via attributes may not be transferred correctly; avoid via attributes or set separate openings.
(7) Large exposed copper gold surfaces on the edge of double-sided boards may cause edge blackening; add a circle of coverlay on the board edge.

5. Silk Screen Design


(1) If there are character silk screens on the stiffener, select "silk screen on stiffener" when placing an order to prevent process errors.
(2) Instruction text should not be designed inside the board to avoid issues in subsequent processes.

6. Panelization Design


(1) For boards with steel stiffeners: The minimum spacing between boards is recommended to be 3mm, the slot width is 0.5mm, and the connection point width is 1mm (one added every 15mm or so). Note when placing an order: Separate each piece with paper, and ship with cardboard clamping top and bottom.
(2) Panelization connection positions on gold fingers will cause uneven front ends of gold fingers.
(3) Too few connection points cause boards to fall off easily; each PCS should have at least 2 connection points (width 0.8mm), with more for larger boards.
(4) For small boards without SMT: Each PCS only needs 2 connection points of 0.3mm for easy hand-breaking.
(5) Low panelization utilization leads to high quotations; optimal panel widths are 119mm or 240/250mm; third-party panelization is recommended.
(6) Boards smaller than 20×20mm may be sucked away by laser dust suction; deliver panels or depanelize after production.

7. Stiffener Design


Stiffening of flexible circuit boards refers to adding rigid materials to local areas of FPC to facilitate assembly. PI stiffeners are suitable for gold finger pluggable products; FR4 for lower-end products; steel sheets (good flatness, no deformation) for chip mounting products. See details in the Stiffener Specification Diagram.

(1) Avoid steel sheets as stiffeners for component insertion holes (risk of short circuits), with Hall elements (weak magnetism), or for pluggable gold fingers.
(2) For pluggable gold fingers, note total thickness requirements (specified in connector specifications); PI stiffener thickness is not directly calculated by subtracting FPC board thickness from total thickness.
(3) Stiffener opening design: Avoid underlying component holes or pads (customer design is preferred; default avoids pads by 0.3mm). Stiffeners with remaining width <2mm after cutting are omitted.
(4) The height of the gold finger stiffener should be at least 1.0mm longer than the gold finger pads to prevent breakage.
(5) Electromagnetic film with conductive sides: Cancel design if the lower film is not a single network.
(6) For electromagnetic film grounding resistance requirements: Customer designs independent grounding solder mask openings (default adds >1.0mm windows randomly). Note: Ungrounded electromagnetic film may cause signal problems; prototyping and verification are necessary.
(7) Attaching steel sheets to solder pads causes short circuits.
(8) Stiffener width: FR4 stiffeners with width <5mm are prone to breakage and carbonization; change to PI or steel stiffeners. Adhesive backing minimum width >3mm.
(9) No stiffeners or adhesive backing around chip mounting pads (prevents solder paste printing); chip mounting should precede stiffener/adhesive backing attachment if necessary.

8. Board Thickness Specifications


The board thickness includes the coverlay, copper thickness, and substrate PI thickness. Boards with copper-free areas or no coverlay have correspondingly reduced thickness; pay special attention during design.