Overlapping Planes

Can someone tell me why this overlap of planes occurred? The VCC plane is underneath a processor, and then the GND plane was dropped over the entire board. That is the only violation that came up for those planes, but why did this even happen?

Is there a trick to plane rules that I should be aware of?

Edit the plane and add a priority number. The higher the number the higher the priority.


Ok, so this stops KiCad from connecting two distinct power planes?

It’s good that the DRC caught it, but how does it happen in the first place? In no way should two seperate power planes be drawing over each other - that’s a pretty serious bug!

Kicad has no idea what you are thinking, hence priorities. Just up the priority of the VCC and hit the b key to refill.

I get that it doesn’t know what I am thinking. And pour priority is a good tool for making sure that planes pour in the correct sequence.

But indicating two separate net names (and power net names), regardless of pour priority should not touch or overlap. This shouldn’t be controversial, so I’ll log this as a bug.

I’ve never seen that occur - have you checked for other items that may be bridging things accidentally ?
If you display in outline mode, what does it show ?

What version are you running, there have been bug fixes in pours.
Planes of different priorities can overlap as it is clear what the outcome should be.
Planes of the same priority should not overlap and an attempt to do so is flagged by DRC

I was on a 5.1.0 build (on this windows machine vs my ubuntu box) but have now updated to 5.1.4, and it generated the planes correctly. Glad to see that fixed! Thanks everyone!

KiCad allows overlapping zones to make it easier to have two (or more) zones on the same layer while kicad handles which one gets to fill which area. To do that kicad needs to know which zone should get exclusive right in which area. This is done with priorities (you can have a zone over the full area with low priority and then place smaller zones inside it with high priority. Kicad will then allow you to have these high priority zones with the proper clearances.)

Without you giving priorities kicad has two options:

  • fill anyways (current option, gets DRC to complain as it should)
  • do not fill (similar result as DRC will complain about unconnected, probably harder to see by users and us as there are other reasons why a zone might not fill.)

I think it is in accordance with KiCad zone conception. Try to put GND zone at top (where you have elements) then fill zone and then move any component to the place filled by GND. You can do it. You can add different net traces going through zone like it was not there. Zone (even filled) don’t disturb you doing your work. The consequences of it is that two different net zones can be one on another (like other elements).
If filled zone would not allow for any move of components it would much more disturb your work then a need to refill zones. To protect you against forgetting doing it there are some moments when it is done automatically. I don’t know KiCad very well yet, but I noticed that even in Plot dialog box you have “Check zone fills before plotting” check box (I think checked by default).
Thanks to possibility to work on filled zone I can hide GND net connections while positioning elements. Even if I plan to have GND at bottom I place GND zone at top just to not see GND connection lines (it helps me positioning as I need not to do GND connections as I have everywhere GND one via from me).

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.