I am trying to achieve the connection of two PCB boards using solder pads, like in the picture below. For each trio of the pads is a footprint that I created. Tthe problem is that I am not able to route tracks to these pads. What I want to achieve is that each pad (1, 2, 3) will be a "portal" to the "brother" pad. Also I need to be able to separate these trios, like in the second picture because for fabrication it will be placed differently.

The final PCB board will be wide so it will be expensive to make it in one piece so I came up with an idea to separate it into pieces and then solder them together.

Does anyone know how to achieve this?

enter image description here

enter image description here

  • \$\begingroup\$ how did you make these pads? I'd assume that if you make a footprint with these \$\endgroup\$ Apr 6, 2023 at 10:43
  • \$\begingroup\$ @MarcusMüller I created footprint and there I put three normal pads and edited size \$\endgroup\$
    – Matej
    Apr 6, 2023 at 10:47
  • \$\begingroup\$ but this looks as if you didn't add a symbol that uses that footprint (for example, you could add a 3-pin pin header symbol) to your schematic and connect it \$\endgroup\$ Apr 6, 2023 at 11:39
  • \$\begingroup\$ @MarcusMüller Yes, I wanted to do it without schematic so this is just footprint, no symbol \$\endgroup\$
    – Matej
    Apr 6, 2023 at 11:42
  • \$\begingroup\$ ha, then that's the problem :) \$\endgroup\$ Apr 6, 2023 at 11:43

2 Answers 2


I presume you're using kiCad by the looks of things.
You'll be best of just separating the nets and the pads into two separate parts like so. basic schematic drawing

Anything else and Kicad will expect the nets to be connected and complain. If you don't mind the error you could do another schematic and just not actually connect them.

  • \$\begingroup\$ Is there any way to do it without involving Schematics into it? Something like "via" but using separated pads \$\endgroup\$
    – Matej
    Apr 6, 2023 at 10:54
  • 1
    \$\begingroup\$ @Matej No way to do it without schematics. But! You can put this bridge on a separate page. No need to change net names. Add a dummy copper layer to the layout. Connect those pads on that layer. Doesn’t need to be the pads - as long as you have any connection between two halves of the net you’ve split, it’ll pass DRC. So you don’t need to add vias next to the pads. Perhaps there are vias or other through hole pads for those nets elsewhere. Just connect them on the dummy layer that won’t be sent to manufacturing. It’s an old trick, also usable for incremental routing with passing DRC. \$\endgroup\$ Apr 6, 2023 at 14:07
  • \$\begingroup\$ @Kubahasn'tforgottenMonica I wonder what exactly would happen if you set the pads to through-hole and "only connected layers", with a hole size of zero. Would the gerbers come out okay, or would your drill file end up with some zero-size drills? \$\endgroup\$
    – Hearth
    Apr 6, 2023 at 14:14
  • \$\begingroup\$ If you refuse to draw a schematic, you may be able to turn off DRC (Design Rule Check) in the PCB layout program to permit your desired connections. DRC will prevent you from making connections between different nets. \$\endgroup\$ Apr 6, 2023 at 15:30
  • \$\begingroup\$ I'm sure you could do it, even if it meant writing some scripts, but it would be easier for you to learn how to use schematics than it would be to figure out how to do it without. \$\endgroup\$
    – LordTeddy
    Apr 6, 2023 at 20:30

Tracks and pads belongs to different signals. This is the reason you can't connect them together. Create library component with schematic symbol and footprint, then place components on schematic and connect them via wires. You can also name the wires via add net label. Switch to the PCB and click Update PCB witch changes made to schematic (F8) button. Now you can easily connect your footprints via traces.


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.