I'm making a 4 layer board, with ground on one of the inner layers, as usual. I would like to keep the digital and analog grounds logically separate, although they of course connect on the PCB, and the standard solution to this is a net tie component, which allows me to connect the nets exactly where I choose to.

My problem is that while the newer KiCad versions (I'm using 5.1.5) finally officially support net ties, there is no obvious way to place the tie on an inner layer. I wouldn't want to bring my ground to the front via vias (no pun intended [2]) and back again just to satisfy a DRC rule by tying them on an outer layer.

So the question: how can I place a net-tie in KiCad on an inner layer? "Official" solutions are preferred, but workarounds and hacks are also welcome. I would really like for the final solution to pass DRC though, and even better if the net tie itself is not DRC exempt [1].

[1] In earlier KiCad version, the net tie you could make yourself was based on the DRC not noticing graphic polygons, which would make the tie pass DRC. However, as a side effect if you happened to pass another track through the graphic polygon of the tie, that wouldn't get picked up by DRC either, so extra manual checking was needed.


    pun indented

Sadly version 5 (and earlier) rely on a workaround for making net ties. This workaround as you noticed relies on footprint pads plus graphic elements on copper. Sadly there is no way to get such a pad to an inner layer.

Version 6 (planned to be released within a year or two from now) will most likely have a direct net tie tool that will not be limited this way.

  • \$\begingroup\$ So there's no way to make an inner layer net tie? I was afraid that that would be the case... \$\endgroup\$ – Timo Dec 13 '19 at 18:05
  • \$\begingroup\$ Can you just bridge the planes where you want and tolerate the ERC error? \$\endgroup\$ – Chris Stratton Dec 13 '19 at 21:11
  • \$\begingroup\$ @chris Well, if there's no reasonable workaround, I'll probably just keep the planes separate while routing, and then connect them iin the schematic and board as the very last step. \$\endgroup\$ – Timo Dec 14 '19 at 12:13

I just finished a board with a footprint that used all 4-layers and this is the KiCad forum post that I've used as a reference: https://forum.kicad.info/t/footprints-pads-on-internal-layers/11214/16

I would suggest to create your net-tie on the top layer, edit the kicad_mod file in a text editor and swap F.Cu with In1.Cu (or In2.Cu) for all the pads (also delete F.Mask and F.Paste layers if present). The pads will disappear from the footprint viee (KiCad does not support inner layers for footprints yet) but they will be exported to your gerbers after you place the footprint on your board. I suggest you draw the net-tie outline on another "visible" layer to be able to place your net-tie exactly where you want it.

Hope this workaround helps, it did for me :)

  • \$\begingroup\$ Thanks for the suggestion, I actually tried something similar at some point. However, the errors that are also mentioned in the forum post you link are really annoying (as is the "net tie not moved" effect), so I think I'll prefer just connecting the planes directly without a net tie at the very end. \$\endgroup\$ – Timo Dec 16 '19 at 7:00
  • \$\begingroup\$ Yes these errors are annoying, however as long as the net tie footprint is not selected they shouldn't pop-up. I do prefer the idea of manually connecting the shapes at the end too, make sure to consider all return paths! Good luck ;) \$\endgroup\$ – Cisco25 Dec 16 '19 at 12:11

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.