Fixing PCBnew fails to properly import netlist after changing annotation with copper pours

Software
1

I discovered this bug while working on an issue with RenumKiCadPCB.

Sometimes after changing reference designations on PCB and eeSchema if you then generate a netlist and re-import it into PCB there are netlist errors and DRC errors.

This is likely a bug in PCBnew since I can recreate it without using my software. I have filed a bug report with the developers.

The fix is easy. Type ‘B’ and the pours will regenerate except where there are errors. Note the rats nest netlist name in the error zone. Edit the zone (hit ‘E’ near a zone edge) and change the net to the rats net netlist name. (the rats nest name is usually near the top of the selection window). Type ‘B’ again, and the pour will fill. Run DRC and the errors are gone.

3 Likes
2

This will likely be tagged an enhancement request, as it is more a NET coverage issue than a bug.
( Other EDA tools do not drill this deep)

To clarify, there are special cases where this happens.

  • The NET with Fill must use an Auto-Generated Name, not a user-Name.
  • The SCH re-annotate or other editing, must change the Auto-Name

If the above are true, then NET import may give mesages like

Warning: Copper zone (net name 'Net-(C67-Pad1)'): net has no pads connected.
Warning: Copper zone (net name 'Net-(C62-Pad2)'): net has no pads connected.
Warning: Copper zone (net name 'Net-(D10-PadK)'): net has no pads connected.

Those cases need to be manually re-named.

1 Like
3

KiCad has confirmed [Bug 1609401] Re: PCBnew fails to properly import netlist after changing annotation with pours

** Changed in: kicad
Status: New => Confirmed

** Changed in: kicad
Importance: Undecided => Low

see: https://bugs.launchpad.net/kicad/+bug/1609401

3 Likes