How does one make a cuttable trace (or trace fuse) footprint?

I have need for a 2 pin cuttable trace or trace fuse. This is a 2 pin schematic symbol which is easy but when it comes to making a 2 pad footprint that is shorted by copper, I am unable to route to/from the pin once the footprint is placed. It is like it knows that it is shorted and will not allow a connection when routing. Any suggestions appreciated. Thank you!


Create a custom 2-pad footprint and add the required trace in the footprint editor! First you’ll have to place the trace on a non-copper layer (e.g. silk), then edit said trace and change to required copper layer. The program will complain, just ignore.

Noteworthy: the DRC is 100% agnostic about the trace added in the footprint editor, so care must be taken that it doesn’t short out stuff.

You can use the same process for creating footprints for joining “identical” nets (e.g. logic-GND to PWR-GND).

1 Like

Why make one to cut when that damages the board? You can design pads for a solder bridge instead and you can connect/disconnect without damage to the board.

The double ended arrowhead >< is used when a made connection is the default (most common) usage. The double D (back to back) is used when the open connection is the most common usage. Much cheaper than dip switches or pin jumpers. This has been standard practice on circuit boards during my 43 years of electronic repair. Only a small score with a xacto knife is required to break the trace. It is usually a one time configuration setting.

When using madworms solution, make the connecting trace as narrow as possible keeping within the limitations of the board house.


Madworm! Thank you so so much. I figured it had to be simple but I just didn’t know about the moving layers in the footprint editor and that makes a lot of things possible that I didn’t know before. I hesitated to post a question like this but it was killing me. Did what you said and it routes fine. Thank you!