FPC Design Rules: 13 Safety Distances You Can’t Ignore
6 min
- 1. Solder Mask Design
- Outline Design
- Via Design
- Spacing Design
- Stiffener Design
In FPC （Flexible Printed Circuit Board） design, neglecting safety distances can lead to issues such as pad detachment or circuit short circuits. For example, insufficient solder mask bridge distance (less than 0.5mm) can cause it to break, pads placed too close to the edge (less than 0.2mm) may result in carbonization and short circuits, and improper via placement can lead to fractures. Precisely controlling these details is key to ensuring design reliability.
Some people believe that safety distances in FPC design don't need to be strictly followed, and approximate measurements are good enough. Others think that as long as the circuits work, the design is fine. But did you know? In FPC design, many seemingly insignificant safety distances, if overlooked, can lead to serious problems! Today, let’s take a closer look at those easily ignored safety distances in FPC design—how many do you know?
1. Solder Mask Design
Insufficient Solder Mask Bridge Distance
A solder mask bridge refers to the solder mask film between two pads. The distance between the pads should be at least 0.5mm to ensure the solder mask bridge doesn’t break. If the distance is too small, the solder mask bridge is prone to breaking.
Before After
Solder Mask Window to Copper Distance
The distance between the solder mask window and the copper should be greater than 0. solder mask window and the copper should be greater than 0.15mm. If the distance is too small, the solder mask may shift, causing copper exposure, which increases the risk of a short circuit.
Wrong Right
Solder Mask Window Length
The length of the solder mask window should generally not exceed 20mm, and large-area windows should be avoided. If the window is too large, the solder mask may deform during application, leading to poor fit or misalignment.
Wrong Right
Outline Design
Pad to Outline Distance
The pad must be at least 0.2mm away from the outline. Otherwise, during laser cutting, the pad may carbonize, causing a short circuit.
Via Design
1. Via to Edge Distance
The distance from the via edge to the center of the board outline should be at least 0.5mm, to prevent laser damage to the via during cutting, which may cause pad detachment. Additionally, vias should not be arranged in a straight line but should be staggered either horizontally or vertically.
2. Via to Window Distance
Vias should not be designed at the edge of a window and should maintain at least a 0.3mm distance from the solder mask’s edge. This area is where welding fingers are applied, and during welding, bending could concentrate stress at the junction of the uncovered and covered areas, which may cause copper at the hole to break.
Not recommend Recommend
Spacing Design
1. BGA Pad Diameter
The BGA pad diameter must be greater than or equal to 0.25mm. If it's smaller, the pad may be too small or may detach.
BGA pad diameter less than 0.25mm
2. Edge Pad Width
The width of edge pads should be at least 0.5mm. When placing orders, be sure to specify that pads should not be shaved. If not specified, JLCPCB will default to shaving 0.2mm off the pad’s edge, which could cause the pad to detach or lead to a cold solder joint.
Wrong Right
3. Trace or Copper Pour to Edge Distance
To prevent copper damage during the formation process, traces or copper pours should be at least 0.2mm away from the board edge. If the copper pour is flush with the edge of the board, it could lead to an open circuit during CAM processing.
4. Pad to Trace Distance
When the pad spacing is less than 0.5mm, avoid routing traces between pads. The minimum distance between a pad and a trace should be 0.20mm. It is recommended to route the traces from the back side or accept exposed traces.
The distance between IC pad and trace is only 0.1mm
Stiffener Design
1. Stiffener to Pad Distance
The stiffener area should be at least 1.0mm larger than the pad. If the distance is insufficient, bending can lead to fractures at the junction between the pad and the trace, causing an open circuit.
Wrong Right
2. Minimum Width of Stiffener
If the stiffener is too narrow, it may cause difficulty in fitting and could easily fracture.
FR4 stiffener is too narrow and more prone to breaking.
The minimum width for stiffener materials is as follows:
FR4 Stiffener: Minimum width 3mm;
PI Stiffener: Minimum width 2mm;
Stainless Steel Stiffener: Minimum width 3mm (1mm is possible with 2.5mm length).
3. EM Shielding Film to Pad Distance
EM Shielding Film are conductors, so the distance between the electromagnetic film and the pad window must be at least 0.8mm to avoid interference.
The safety distance data above is derived from JLCPCB’s experience in the FPC production process. Mastering these design details can effectively avoid common issues in the design and ensure the reliability and stability of FPCs.
Popular Articles
• The Ultimate Guide to Flexible PCB: Types, Design, and Applications
• 45 Must-Know Flex PCB Design Tips You Can't Afford to Miss!
• Choosing the Right Bend Radius for Durable Flexible PCBs
• FPC Design Rules: 13 Safety Distances You Can’t Ignore
• Mastering PCB Stiffeners: A Comprehensive Guide to Types, Applications, and Design Best Practices for Flexible Circuits
Keep Learning
Medical Flex Circuits: Manufacturing, Applications, Materials, and Design Guide
Medical flex circuits made to fit inside a 1.0 mm disposable endoscope, wrap around a hearing aid shell, and sit on a patient's arm for ten straight days. When one fails, it is not a warranty return but a device history file and a regulatory conversation. In this guide, you will learn: What separates a medical flex circuit from a consumer one How they are built, tested, and released Polyimide, copper, coverlay, and stiffener choices Fine line, bend radius, and layer count limits What to check before c......
FPC Thickness Guide: How to Choose Flexible PCB Thickness
Flexible PCB can bend, but how much? And here is why thickness becomes a crucial factor in flex PCB design. If we made the mistake, it would either become too thin and jiggle around inside a ZIF connector, or too thick, fatigue the outer copper and crack traces within a few thousand bend cycles. It is also the number most designers quietly leave to the fab. But today in this guide, we will cover: What an FPC thickness includes The range you can go up to and order How the stackup adds thickness layer b......
FPC Electronics: What Is It, How It Works, Applications, and Benefits
FPC electronics is the reason your phone camera still works after a hundred open-and-close cycles. Peel apart almost any modern device, and you will find a thin amber ribbon carrying signals around corners no rigid board could turn. In this guide, you will learn: What does FPC stand for, and what are the differences between FFC and FPC? A flexible circuit that conducts a signal as it flexes The materials include one polyimide, copper, coverlay, and stiffener FPC manufacturing process (etching to elect......
Fast Turn Flex PCB: Rapid Prototyping & Lead Time Guide
Fast turn flex PCB service is what stands between a validated concept and a product that ships this quarter. Most flex delays are not caused by the factory. They come from a coverlay opening drawn 0.05 mm too tight or a missing stiffener drawing, and each one parks your job while an engineer emails. In this guide, you will learn: What separates fast-turn flex PCB from standard FPC production Which design choices add days to the flex PCB lead time Panel, fiducial, and carrier rules for flex SMT assembl......
Custom Etched Flex Circuits: Guide to Materials & Manufacturing
Custom-etched flex circuits are the reason a folding phone hinge and a hearing aid can route wiring through spaces where no cable would fit. The hard work is custom. Everyone is cut to your outline, bend zones, and stiffener map, so one wrong dimension turns a finished part into scrap. In this guide, you will learn: How custom etched flex circuits differ from catalog flex cables How the subtractive etch and lamination process actually runs Polyimide, copper, coverlay, and stiffener material choices Tr......
The Ultimate Guide to Flexible PCB: Types, Design, and Applications
Key Takeaways JLCPCB 1–4 Layer Flex PCB: Supports 1 to 4-layer FPCs with polyimide (PI) substrates and trace/space down to 3/3 mil. Stiffener Selection: Use PI (0.1–0.25mm) for ZIF connectors, FR4 (0.1–1.6mm) for SMT support, and Stainless Steel (0.1–0.3mm) for high rigidity. Layout Optimization: Use cross-hatched copper ground planes and stagger 2-layer traces to eliminate the "I-Beam effect." Surface & Protection: Combine Immersion Gold (ENIG 1u"/2u") for SMT planarity with flex coverlay to protect ......