How can I design plated milling slots in my Gerber files?
For Seeed Studio Fusion, the way in which plated milling slots are communicated in the manufacturing files is similar to plated through holes (PTH). That is, there must be some sort of hole, copper plating and an opening to expose the copper. The following simple steps show you how to do this:
1. In your chosen design software, draw the slot outline in the Mechanical layer (GML or GKO), this will be the final size of the hole after plating. To preserve the exact dimensions, the outline should be drawn using a zero-width line, the same as the board outline (so it looks like a small cut-out). Only the area inside the shape will be cut out.
2. In both Copper layers (GTL, GBL and any other copper layers), draw the same slots but at least 0.1 mm (about 4 mil) larger than the slots in the mechanical layer. The amount of copper exposed is up to you. The copper layer is shown in blue below,
3. Finally, draw the slot openings in the Solder Mask layers (top and bottom), at least 0.16mm (about 6 mil) larger than the copper pads. The opening is shown in light blue in the example.
4. Remember to do this for the other copper and solder mask layers. And now you have designed a plated slot.
The only real difference between a plated slot and a plated through hole is the shape of the cut-out. For PTH, we usually illustrate this in the NC drill layer with a drill hit. For plated milling slots, we design this by drawing the opening as a cut-out. Some component libraries will generate plated milling slots in a separate milling NC layer, but we do not recommend this since it can be difficult to import NC milling layers Into CAM software correctly. They may also be designed as filled shapes – but our engineers may not follow the exact dimensions of the shape, which is why we recommend using a zero-width outline.
Please note that our smallest milling tool is 0.8mm in diameter, so if you require milling slots smaller than this, we suggest you design them as a row of overlapping drill holes and include them in the NC drill layer.
Extra Design Notes:
In Eagle, be careful when using milling with multi-layer PCBs (more than 2 layers). The milling may not correctly adjust the copper pour spacing in the inner layers, resulting in the pour being electrically connected to the slots and potentially causing short circuits. So to avoid this, draw an isolated trace beneath the slots in the inner layers as well, and be sure to check the isolation is preserved in the exported Gerber files.