Connect with:

What you didn’t know about EAGLE: Slotted Holes

eagleblog

slotted holes

At first glance, it may appear that there is no way to create slotted holes in EAGLE! Currently, there is no built-in mechanism to handle slotted holes directly, however our customers make boards with slotted holes all the time! “How,” do you ask?

Slotted holes are becoming quite common as components have to manipulate ever increasing amounts of current. A wide pin is also useful for giving a component additional mechanical integrity. For these reasons and more, many modern components have wide pins which make slotted holes on the PCB layout necessary.

So let’s create the slotted holes. We’ll use the DC-10 power jack from Cliff Electronic Components (Fig 1). The key is to use a normal through hole pad, with a diameter that fits the slot you need. Oblong pads are usually the best choice for this operation (Fig 2).


Figure 1 DC-10 Power Jack from Cliff Electronic Components

 


Figure 2 oblong pads placed

 

Drawing the Slots

Draw your slotted openings by simply drawing the slot outlines on layer 46 Milling (Fig 3). Now there is a different way to do this, sometimes in the wild, you’ll find people who recommend using the Dimension layer for this purpose. While it does work, the problem with this approach is that the autorouter won’t be able to reach the inside of the pad and you’ll get some Copper/Dimension errors in the DRC.

A couple of things to note:  1. Set the drill size of the pad to be able to fit within the slot outline, this will avoid confusion later and guarantees a nicer result; 2. The width of these lines is 0, they are just an outline. The board manufacturer will make sure that the area within these lines is milled from the board.


Figure 3. Oblong pads with features on the milling layer

 

Getting Milling Data to Board Manufacturer

How do you get the milling data to them? After using a part in a design, make sure to export a Gerber file for layer 46 Milling(Fig 4). Include a note to the manufacturer with your Gerber files specifying that the contents of that specific Gerber file are to be milled from the board.

We hope this procedure come in useful next time you need to create slotted holes in EAGLE!

Thanks for Following Us!

EAGLE Support Team

Please share your thoughts and questions!
Comment or Email:  support@cadsoftusa.com

Subscribe for Updates

Stay up to date with the latest news, knowledge and tutorials for Autodesk EAGLE and electronics design.

12 Trackbacks

SIGN UP FOR UPDATES

The Nest

Stay connected with the latest news, knowledge and tutorials for Autodesk EAGLE and electronics design.