Depanelization Tab Routing

Board assemblies can be de-tabbed using perforated breakaway tabs, v-grooves breakaway tabs, or hand-cutting with a de-tabbing tool. For Tab and V-Score (i.e. PCBs that must be sheared along an edge):

1. Traces and via should be a minimum distance of 0.050"(1.27 mm) from the routed/scored edge.
2. Components should be a minimum of 0.100"(2.54 mm) away from routed/scored edge.

The rules are set to prevent components or board damage during the depanelization process and prevent flooding during the wave soldering process.

For 0.062" (1.6 mm thickness) Printed Circuit Boards:

1. Perforation holes should be typically spaced at 1 mm intervals.
2. Tab routed with a 1 mm radius.
3. Routed slot should be 2 mm minimum, for single image panels. Use 3 mm routed slots when two or more boards are in a panel. This allows for more accurate edge dimensions.
4. 75 mm typical distance between tabs, not to exceed 100 mm.
5. Place tabs approximately 25 mm from corners to reduce sagging during reflow or wave soldering.
6. Desirable to have at least one tab per side.
7. A slight inset of perforation is preferred; it provides an edge that requires little or no additional labor to clean up.

NOTE: Two parallel edges are required for a PCB to be processed in the SMT line. This is to prevent skewing through the conveyor system. All odd-shaped PCBs MUST have edge rails incorporated to meet this requirement. Custom reflow fixtures will be made if this requirement is not met.

Design for manufacturing or DFM

Design for Manufacturability rules and guidelines are a collection of PCB design best practices to help our design be as easily manufacturable as possible. The easier it is to manufacture a PCB, the more likely it will be to reduce both manufacturing errors and costs. DFM rules have been developed by PCB manufacturing experts and the rules will vary depending on the board design, and the manufacturer's capabilities.

It is highly recommended to check with the PCB manufacturer for their precision and limit on the width of the solder mask Dam. Solder mask dam between surface mount pads will prevent solder bridging during assembly. Below is one of the PCB suppliers' capabilities.

In summary, the width of the solder mask dam depends on the copper thickness and solder mask color. Generally, 3 mils of solder mask dam can be achieved using 1oz of copper but that will be 6 mils for 2 oz of copper. Similarly, the minimum solder mask dam for the Green solder mask is 3 mil and others will be 5 mil.

To get a solder mask dam between pads (if individual relief is required) spacing between copper should be 8 mils or more. Otherwise, the finished PCB will get block relief without a solder mask dam.

PCB under microscope with and without solder mask dam can be seen in the photo below.