FPC Design Rules: 13 Safety Distances You Can’t Ignore

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.