Plated and Non-Plated Slots and Cutouts

About this tutorial

This tutorial shows you the capabilities and what you need to do to achieve elongated holes, plated and non-plated slots and cutouts.


  • For Plated Slots a maximum length of 15.0mm and diameter of 0.7mm to 2.8mm
  • For Inner Millings (i.e. cutouts), use at least 1.8 mm diameter and always confirm with our Board Viewer
  • Non-Plated Slots must be realized as inner millings (min. diameter of 1.8 mm (0,063 in))

Plated Slots

We support plated slots with a length of up to 15.0mm and a width of 0.7mm to 2.8mm (0.11 in).

              (Typical use case of plated slots)

Typical use case of plated slots.

As we give a guarantee on our renderings, you should always use the Board Viewer to check if plated slots are detected properly. Use the “Highlight Drills” Button for this.

Screen Shot 2019-07-26 at 11.48.53

        (Highlight drills function)

Enable drill highlight

Screen Shot 2019-07-26 at 11.50.48

                       (Plated Slots in the Drawing)

This plated slot will be manufactured properly, shown by the orange color.

Eagle Users should always check if a slot was detected as plated or non-plated slot.

Cutouts and Non-Plated Slots

Cutouts and Non-Plated Slots will always be milled and may have any shape you like. Please note that our smallest milling tool diameter is 1.8mm and ensure, that all Cutouts or Non-Plated Slots have at least this size.

Screen Shot 2019-07-26 at 12.19.11

      (Cutout with milling path highlighted)

Cutout with milling path highlighted.
Screenshot from 2021-03-30 11-05-42

      (Non-Plated Slots with milling path highlighted)

My PCB has plated slots for USB connectors, 0,7mm wide. The slots are not shown by the board inspector. Which layer should I use in Eagle so that Aisler detect these slots? Now I use milling layer 46, but that doesn’t work. I have tried the drill layer 44 and dimension layer 20.

1 Like

There are some ways to do those slots in EAGLE. :sweat_smile:

In the picture I have done it with the Milling layer. Note, that you have to do a closed line and not one line, see the following picture:


For the Pad itsef, you combine many parts, as seen the following pictures:


One note: In this picture the polygon on BStop is missing, it is the same for the bottom layer as on TStop (top layer).

The ‘SMD’ will define the outer size, the golden area you see here:

The inner part is defined by the Milling Layer.

Have you uploaded the EAGLE file or Gerbers? This makes the following difference: If you upload the EAGLE .brd file everything is done automatically. For the Gerbers, you have to select the Milling at export.

I hope this helps :smiley: