I need to create this package on EAGLE but I've problems with this elongated plated holes on sides. How I can do that?

enter image description here

  • \$\begingroup\$ I believe you'd had to add that to the "Milling" layer. You'd also have to check with your pcb fab house if they can do plating after milling. \$\endgroup\$
    – Wesley Lee
    Nov 2, 2015 at 13:43

2 Answers 2


They are called plated slots. Whether or not you can make them however depends on your PCB fab. Some companies refuse to make plated slots, others allow it. Best to contact them directly to ask if they can do it and how they want it specified.

Some Methods:

  1. If you add multiple overlapping holes on your design you can emulated plated slots, but these are generally not liked by manufacturers because they an cause issues with the small drill bits.

  2. Add either 'long' style through-holes (or SMD pads on the top and bottom) and a line on the milling or dimension layers inside the pads. This will likely cause DRC errors, and you have to make sure the manufacturer knows that these are supposed to be plated slots.

  3. The third option, and which doesn't require plated slots is to make round holes which are large enough to encompass the whole slot. So for example in the left and right holes in your recommended layout, you could use a 1.2mm plated hole placed on the centre of where the slot would otherwise be. This would provide enough space for the tabs on the component to go through the hole without needing a slot.


Create a pad (green circle) with the correct outer dimensions (oval that is) ignoring the hole in the center. Then create the outline of your hole on top of the pad using the dimension layer and a wire of zero width.

Some people add the outline to the milling layer but often that layer is ignored or overlooked when generating gerbers. I like the dimension layer because it is difficult to overlook.

I've had about a dozen of these boards manufactured with slots. enter image description here


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.