PCB Panel Design

PCB panel design, also known as paneling or panelization, is an important step in the high-volume PCB manufacturing process. To improve the efficiency of PCB production and surface-mount assembly lines, small individual PCBs are often arranged together in a larger manufacturing panel.

This group of repeated or combined PCB designs is called a panel or multiblock. Depending on the production process and the PCB design, the individual boards are separated from the panel after manufacturing, SMT assembly, THT assembly or in-circuit testing. This separation process is called depaneling.

Several methods can be used to determine how the individual PCBs will be separated from the panel. However, before selecting the depaneling method and designing the panel, the physical characteristics of the PCB design must be reviewed carefully.

For example, sensitive components placed close to the board edge, connectors extending beyond the PCB outline or mechanically critical areas can directly affect the panel design method.

Starting a PCB Panel Design

Before starting a PCB panel design, the first step is to obtain the minimum and maximum panel size information from the manufacturer. These limits may vary depending on the number of different PCB designs placed on the panel, the PCB thickness and the production capabilities of the manufacturer.

For example, if two different PCB designs with a thickness of 1.6 mm will be placed in the same panel, the manufacturer may define limits such as a minimum short edge of 50 mm and a maximum long edge of 300 mm.

After the panel size is determined, the edge rail areas required on at least two parallel sides of the panel should be subtracted from the total panel area. The remaining area gives the usable panel area for PCB placement.

If at least 70% of the usable panel area can be filled without creating manufacturing risks during production, assembly and depaneling, the result can generally be considered an efficient panel design.

PCB Panel Design Methods

In PCB design, several physical details may limit the panel design method. These include sensitive components located near the board edge, connectors or other components extending beyond the board outline and the mechanical strength required during production.

After these details are evaluated, the most suitable edges of the PCB are selected for panel connection. Then one or more panel design methods can be applied according to the edge structure and manufacturing requirements.

In some cases, a single method may seem sufficient. However, to prevent problems during production and to increase panel strength, multiple methods may be used together. If needed, additional bridges can be placed between boards by sacrificing some usable panel area.

For efficient panel design, two common depaneling methods are often used: V-scoring and stamp holes.

1. V-Scoring Method

V-scoring, also known as V-cut or V-groove, is a depaneling method in which a circular cutting blade creates aligned grooves on the top and bottom surfaces of the panel. In general, the cutting blade has an angle of 30–45 degrees, and approximately one-third of the board thickness is removed from each side.

The remaining material creates a controlled breaking line between the PCBs. Although the board thickness is reduced along this line, separating the PCBs from the panel still requires care.

As shown in Figure 1, components should not be placed too close to the V-scoring line. A safe clearance should be maintained between the cutting line and nearby components to reduce the risk of mechanical stress during depaneling.

Figure 2 shows the typical V-groove structure and the remaining board thickness after cutting. Since only part of the PCB thickness remains in the scored area, the panel becomes easier to separate, but also mechanically weaker along this line.

Trying to separate V-scored boards manually can cause the PCB to bend. If the board has already gone through component assembly and testing, it is better to use a proper depaneling machine to reduce mechanical stress and minimize risk. Figure 3 illustrates the depaneling blade approach and the clearance required around taller components near the V-cut line.

V-scoring requires several design considerations:

• V-scoring lines should continue across the entire panel and remain parallel to a straight panel edge. They should not intersect with any component along the cutting path.

• Components with a height below 7 mm should be placed at least 1 mm away from the V-scoring line. However, a distance of at least 3 mm is often preferred to reduce the risk of stress or vibration damage during separation.

• Considering the cutting blade geometry, no component higher than 25 mm should be placed within 5 mm of the cutting line.

• PCB traces should generally be placed at least 0.3 mm away from the V-scoring line to prevent damage during cutting.

• After V-scoring, the mechanical strength of the panel decreases. If the panel will go through a wave soldering process, additional strength measures may be needed even if this reduces the usable panel area.

2. Stamp Holes Method

The stamp holes method is based on connecting individual PCB designs to each other or to the edge rails with small bridge areas. Holes are then placed on these bridges to define controlled breaking points.

This method is especially useful when the PCB outline is not suitable for straight V-scoring lines or when the board geometry requires more flexible panel connections.

A single row of holes placed directly along the center of a bridge should be avoided, as shown in Figure 4. This type of structure can leave unwanted protrusions on the PCB edge after separation and may create an irregular break.

A more suitable stamp hole structure is shown in Figure 5. In this structure, the holes are positioned to create a controlled break line while reducing the amount of remaining material on the PCB edge.

Important points for stamp hole design include:

• PCB traces and components should be placed at least 3 mm away from the holes where the break will occur. For mechanically sensitive components such as MLCCs, a distance of 5–6 mm may be preferred.

• A single row of holes placed directly along the center of a bridge should be avoided, as this can leave unwanted protrusions on the PCB edge after separation.

• A commonly used stamp hole structure may include the following dimensions:

  • Hole diameter: 1 mm

  • Number of holes: 5

  • Hole center-to-center distance: 1.5 mm

  • Bridge length: 5 mm

  • Bridge width: 2 mm

If there is not enough space for traces and components, or if deformation is acceptable in areas such as edge rails, the number of holes may be reduced to 3. In this case, the bridge width and hole spacing should also be reduced accordingly.

Bridges should be placed according to the required mechanical strength. For 5-hole bridge structures, a spacing of approximately 5–7.5 cm can be used. For 3-hole bridge structures, a spacing of approximately 3–5 cm can be preferred.

Bridges should not be placed under components that extend beyond the PCB edge. As shown in Figure 6, breakout tabs should be positioned away from overhanging components. The preferred approach is to place the bridge so that the component body does not interfere with the breaking area.

Bridges should also be placed as close as possible to the ends of the panel to reduce surface bending. Otherwise, if the panel enters a wave soldering process, unsupported PCB sections may bend and cause soldering defects. Figure 7 shows how unsupported areas may be pulled down during wave soldering, which can lead to topside solder flooding or similar assembly issues.

Before depaneling, the breaking axes should be reviewed carefully. There should be no geometry or mechanical feature on the breaking line that can resist the break or change the direction of the applied force. As shown in Figure 8, extending the break axis to the edge helps prevent upward force on the adjacent PCB edge and results in a cleaner separation.

Conclusion

PCB panel design directly affects production efficiency, assembly quality and the reliability of the depaneling process. A good panel design should consider not only how many boards can fit into a panel, but also how the panel will behave during manufacturing, assembly, testing and separation.

By selecting the right panel size, edge rail structure, depaneling method and bridge geometry, PCB production can become more efficient and less risky.