Panelization and Bridge Design – PCB DFM Part 3

In this post we will learn the part 3: Panelization and Bridge Design. If you have learnt this tutorial, you can order pcb directly from Seeed Studio Fusion by click pcb fabrication.

3.1 V-CUT Scoring

  • V-cut scoring can be used can be used on PCB panels to separate individual boards. They must run across the entire length of the panel, parallel to a flat edge and not interfere with any component placement.
  • For panels incorporating v-cut scoring in their design, the recommended board thickness is greater than 3.0mm.
  • For PCB panels that require machine automated depaneling, a clearance area of 1.0mm is required along both sides of the v-cut line (and on both top and bottom surfaces) to protect the components from damage.
V-CUT Scoring Figure 1: Clearance area requirements for PCB panels undergoing automated depaneling. At the same time, the structure of the blade of the v-cut scorer must be considered. As shown in figure 2, no components with a height of over 25mm are allowed within a 5mm distance from the v-cut line. v-cut line Figure 2: Demand of blade of automatic board cutter to device in the banned layout area of PCB edge When v-cut design is applied, these conditions must be met in order to protect components during the splitting process, and ensure that the boards will split freely. board thickness Figure 3: Board thickness requirements for v-cut scoring. A safe distance of ‘S,’ as shown in Figure 4, must be maintained between the v-cut line and any copper traces to avoid damaging the trace. S ≥ 0.3mm is usually satisfactory. V-CUT Scoring Figure 4: The safe distance (S) between v-cut grooves and copper traces.

3.2 Stamp Hole Design

  • The recommended width of milling grooves is 2mm. Milling grooves are often used in situations where a certain distance must be maintained between individual boards on a panel. It is generally used together with V-CUT scoring and stamp holes.
  • The distance between the origins of adjacent stamp holes should be 1.5mm. Recommended distance between the two groups of stamp hole is 5mm, as shown in picture 5.
Stamp Hole Design Figure 5: Stamp hole design parameters.

3.3 Panelization

There are three recommended modes of panelization: The same direction splice, central symmetric splice, mirror symmetry splice.
  • For PCB boards smaller than 80mm x 80mm, panelization is recommended.
  • The designer should consider the utilization rate of the design when choosing the PCB material. This is a key factor affecting the cost of the PCB.
Note: For some irregular shapes (such as an ‘L’ shaped board), applying the appropriate panelization mode can drastically improve the utilization ratio of a panel and reduce costs, as shown in picture 6. panel Figure 6: L type PCB layout on a single panel.
  • If the PCB is to be processed with reflow soldering and wave soldering techniques, and the cell board size less than 60.0 mm, then no more than two rows should be stacked in one panel (that is, the board should be no more than two boards in height.
Single Board Panelization Figure 7: Diagram of panelization width.
  • For smaller boards, the number of boards running across the longest side can be greater than 3, but the width should be no more than 150.0 mm, Margins or tooling bars should be added on the longest sides during production to prevent panel deformation.
  • Single Board Panelization
  • Regular shape board
Margins are not required for boards with v-cut grooves that satisfy the clearance area requirement stated in [4.1]. Single Board Panelization Figure 7: Example layout of step and repeat panelization
  • Irregularly shaped boards
A combination of v-cut lines and milling grooves can be used to shape irregularly shaped boards or boards where components hang over the edge. v-cut lines Figure 8: Panelization of irregularly shaped PCBs
  • Center Panelization
  • Center panelization can be applied to irregularly shaped PCBs. They are arranged in such a way that the outer shape is regular.
  • If the two boards do not fit together completely, milling can remove the excess and separate the boards.
  • For larger pieces of excess material, the panel can be designed such that the excess pieces may be broken off using stamp hole connections. See figure 9.
stamp hole Figure 9: Two irregular boards with the excess connected via stamp holes.
  • PCBs with gold finger connectors need to be positioned so that the fingers face outwards as shown in figure 10. This is necessary for the gold plating process.
gold finger Figure 10: Recommended layout of PCBs with gold fingers.
  • Symmetrical Panelization
If the SMD of cell board both sides meet the requirement of back reflow soldering, you can use the mirror symmetry splice board. Note: Mirror symmetry panelization requires that the design mirrors the original exactly, for example for a 4-layer board, if the second layer is the negative power / ground plane, then the third layer must also be negative. Otherwise mirror symmetry panelization cannot be used. Mirror symmetry panelization Figure 11: Mirror panelization Fiducial marks on the mirrored boards must match after flipping. For specific placement requirements, please refer to the Fiducial mark design section later in this document.

3.4 Panelization Methods for Irregularly Shaped PCBs

  • General principle
  • If the assembled PCB does not have a clearance area of 5mm along the edge of the board, margins/tooling bars should be added along its perimeter.
  • If the PCB is irregular in shape, for example, a corner is missing or a segment cuts into the board, block filler pieces should be used to make the outline more rectangular in shape to aid assembly.
corner Figure 12: Completing the PCB outline of irregularly shaped boards.
  • It is recommended that SMT and wave soldering techniques be used for irregular boards with filler pieces larger than 35mm x 35mm. For filler pieces greater than 50mm in length, two sets of stamp holes should be used, otherwise, one set is satisfactory.
SMT Figure 13: Stamp hole placement for filler pieces greater than 50mm in length. More Chapters: 1. Brief Introduction 2. Seeed Fusion PCB Specification 4. Component Layout Considerations 5. PCB Hole design 6. Solder Mask Design 7. Copper Trace Design 8. Silkscreen Design 9. PCB Lamination Structure 10. PCB Dimensions Specification 11. Fiducial Mark Design 12. Surface Treatment 13. Files for Manufacture Requirements 14. Appendix 

About Author


May 2017