Copper Zones that filled previously no longer fill

Hello smart people - I’m having a problem getting zones to fill. I draw the zone with CTRL-Shift-Z, assign the GND net to it, set it for one or more layers, hit B, the process looks like it is working, but in a 3" x 14" area I get 9.7534 sq mm of fill (which I can’t find). “Show Filled Areas of Zones” is selected, and the layers I’m working on are visible. There are many pads (including actual THT pads (not just vias) of the same net in the fill area. I’ve tried turning off remove islands, I’ve upgraded from 7.0.8 to the current stable release of 7.0.9. I’ve changed clearances and priorities, but haven’t found my problem yet.

I’m sure i did something to break the fill process, but haven’t been able to figure out what. A screen shot of my settings should be attached, as well as a screen shot showing part of the outline of this zones. I can’t really upload the project publicly as it’s a work project…
Screenshot 2023-12-05 163548

Here’s my version info - any suggestions or something that makes me smack my forehead and say “duh,” would be appreciated.

Application: KiCad PCB Editor x64 on x64

Version: 7.0.9, release build

Libraries:
wxWidgets 3.2.3
FreeType 2.12.1
HarfBuzz 8.2.1
FontConfig 2.14.2
libcurl/8.4.0-DEV Schannel zlib/1.3

Platform: Windows 11 (build 22621), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
Date: Nov 5 2023 19:26:40
wxWidgets: 3.2.3 (wchar_t,wx containers)
Boost: 1.83.0
OCC: 7.7.1
Curl: 8.4.0-DEV
ngspice: 41
Compiler: Visual C++ 1936 without C++ ABI

Build settings:
KICAD_SPICE=ON

Ahhh I found at least some of the fill that did occur - it’s highlighted in this screenshot:

I’m also surprised - what is going on.
Do your fill is still GND?
This small copper island is next to GND pads and not connected to them…

Unless i’m totally missing something - yes the fill is set to the GND net (selected from the list of nets)

At first glance I could not see a problem. If possible upload the kicad project (from kicad manager–>File–>archive project). This allows us to search more deeply in the board.

When I select the small copper pour area the properties show it as GND net…

CTRL-B removes it and B puts it right back, exactly the same. I also deleted the fill zone and it went away, so I believe it IS the same fill zone. No fill seems to occur on the other two layers selected for the fill - not even that little island.

I thought for sure I would find it if I deleted most everything from the board, but… no help. I dragged the shape of the zone back to what was left of the components and the amount of fill changed, but it’s still less than 1 sq mm. Here’s the archive - Mike
edp_part.zip (213.5 KB)

Your board outline is just one segment. Delete it from the group and move the big rectangle on the F.Fab layer to Edge.Cuts.
Why is this segment and a rectangle in a group even?

2 Likes

Blockquote

Dsa-t,

The grouping is a leftover from before I started reading the Kicad docs. RTFM… Hand slaps forehead…
Thank YOU! I think having the edgecuts on the fab layer was a brain-cell leftover from another EDA program.
I don’t understand why that broke a fill zone, but it seems to have been the culprit.

Thanks again for the assist!

Mike

1 Like

In KiCad, zones only fill inside the board outline. If the board outline is invalid, no zone can fill.

2 Likes

This small copper piece is surprising :slight_smile:

Maybe J9’s silk is actually on the Edge Cuts layer :wink:

The small copper piece is called an “island” in KiCad, and normally it wouldn’t be there, but this zone in particular is set to “Remove islands: Never”

When the board outline is missing, the “main part” of the zone (in other words, the part up to the zone border) will all be removed/unfilled, but any internal islands are controlled by this setting.

1 Like

I’d expect other islands - for example between +3.3V track and track from J9 pad 6 (the other over J9 pad 1). What happened with them? For me it is still surprising that only that one island left.

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