Cut jumper link footprint

I would like to create a cut-jumper footprint, normally closed, meaning that on my schematics it would look like:

And the footprint like this (actually this one is a cut-jumper/solder-jumper combo):

But even if I’m unable to create such part in the footprint editor, in pcbnew, clearance prevent me from joining 2 pads with different net within a footprint.

How can I create such part, without placing a 0ohm resistor or solder strap?

  1. Create a new footprint, place all the pads you need.
  2. Draw the link on a non-copper layer
  3. Edit the piece of line and switch it to F.Cu layer & ignore the warning
1 Like

Good question, I have tried a few ways. The simple way is just to create an extra pad which bridges the two pads. That will create DRC errors (pad near pad), but otherwise works.

To avoid DRC errors, create a graphic segment, then edit it to be on the copper layer. That avoids the DRC error, but now the copper bridge will be under the silk screen. Additionally, with the FreeRoute autorouter it will route tracks between the pads, it does not “see” the bridge. I got round that by putting an additional small pad on top of the graphic line, to deter the autorouter.

If you want the graphic line exposed, maybe there is a way to add a solder mask at that point.

Heh, madworm ninja’d me, but it’s the same method.

1 Like

Looks like it’s THE solution:

Yes, adding an extra graphic identical line on the F.Mask, keeps the copper exposed.
Thanks a lot for your fast responses.

That’s bad for production.
Just soldering a jumper closed is faster and does not damage the pcb.

Well, we use a 5V/100A to burn off whiskers between wires.

Sure, never said it was for production: it’s for prototyping: it allows me to change option, resistor switch, path, etc.