Ground Plane Copper Pour Suddenly "Broken"

Because my PCB outline is quite odd shaped, my plane layers are just arbitrarily drawn polygons which extend beyond the boundaries of the PCB (as defined in the Edge Cuts layer. Until today, this has always worked. The copper pour always stopped at the edge of the PCB.

The other power plane, 5V / 3.3V split, still behaves properly. Only the ground plane acts weird. Is there something I could have done that caused only one copper pour to suddenly ignore the PCB boundary?


  • picture/screenshot?
  • project files?
  • kicad version + OS you’re using?
  • any steps that you remember between “all dandy” and “hell broke loose” we should know about?
1 Like

Okay, noted. I was suspecting cockpit error rather than program bug. But here are the particulars.

- picture/screenshot

I’ve posted a couple of pics on my project’s blog, here.

- project files

I’ll post the project files as soon as I can, in their current state.

any steps that you remember between “all dandy” and “hell broke loose” we should know about?

I love that description! Well, I was doing final cleanup of the layout. This included the following:

  • Edit -> Cleanup Tracks and Vias. This didn’t seem to cause any ground plane problems, although I selected the option to “delete unconnected traces”, which had an unwanted side effect (deleted traces which appeared to be connected but weren’t really). I would’ve preferred to find these by the DRC rules, rather than completely re-rounting them.

  • Running and fixing DRC and Unconnected Nets reports. Mostly this involved tweaking the split power plane boundaries and/or bumping some vias slightly one direction or another, especially in a region where a 3.3V and 5V via were very close to each other. No problems observed with the ground plane during these steps.

  • Added stiching vias at the main connection points to the plane layers at the power supply I tried a variety of methods, the one I ended up using was one recommended on these forums by another user. I made my own via “footprint” with solid plane connection, added them in the schematic and placed them on the board. Despite all my previous tries which had various side issues, I’m certain that this final approach (a) works, and (b) did NOT cause the ground plane to jump the board boundary. I know this because I was frequently re-pouring all the planes, ground included, as I tried these various solutions.

  • Added five mounting holes, originally floating, and finally connected them to ground

- kicad version + OS you’re using

  • OS X El Capitan Version 10.11.5
    MacBook Pro, Retina, 13-inch, Mid 2014
    2.6GHz Intel Core i5, 8GB 1600 MHz DDR3
    Intel Iris 1536 MB

  • KiCAD version 4.0.2-stable, release build
    wxWidgets 3.0.2 Unicode and Boost 1.57.0
    Mac OS X (Darwin 15.5.0 x86_64) 64 bit


I found the problem. Updated that blog post above to show the answer and a screenshot.

Short version, grounding the mounting hole, which was located astride a slot, caused KiCAD to think I wanted the area outside the board filled, too. I temporarily solved this by adjusting the board outline to fall just beyond the perimeter of these two mounting holes’ pads. After talking to the PCB shop, I may do something different, or even just not ground these two pads.

1 Like

Yup, makes sense.
I think in the strictest mathematical sense, KiCad actually floods both inside and outside PCB outline, but then removes the outside planes as ‘not connected’ to a NET.

1 Like

If you want/need really round copper pour outlines on those circular board edges have a look at my circular zone fill script. The max KiCAD will give you at the moment are 64 segments per full circle…
I used it myself with success on a round pcb.

As for your problem with the pour flooding the outside, have you tried to place a ‘no copper zone fill’ area where you placed that arc?
A test I just did prevents filling past that zone.
I’m just mentioning it, as the 3D viewer will have a field day with that unconnected outline arc…

1 Like

Indeed it does! I changed the arc to a keep out as suggested, and it now pours properly (as expected) and the 3D viewer works. Thanks.

Any reason why the 3D viewer renders the inside curves (concave) of my PCB board outline just fine, but the outside curves (convex) are just straight lines?

simplification by the graphics package. I think it’s something around 12 or so segments per full circle. It’s not adaptive but will only affect the visuals. The outline arc will come smooth in the gerbers.

On the other hand, the copper pour segmentation for circles will affect your final board.

1 Like