I am developing a custom board using the LPEMCC2340 board as a reference. I am encountering an issue where I cannot add the ground pad of my PCB antenna with zone filling. I’ve attached an image of my PCB layout for reference. Could someone please help me understand why this might be happening and how to resolve it?
Your screenshot does look strange. Net name of the zone and the two GND pads of the antenna are the same, and yet, the zone preserves a clearance.
Implementation of Net-ties and of handling of graphics as part of a net has changed a few times during the history of KiCad. I assume the antenna design for an older KiCad version creates a conflict in a newer KiCad version. The easiest way verify and/or troubleshoot this is if you upload a simple (dummy) project that uses this antenna footprint and post it here. I’m still using KiCad V8 myself and can’t help in this way if you use V9, but others will probably have a look at such a dummy project.
Take a look at your Nets, do you have more than one Net called “GND” ?
Are all your GNDs on your schematic actually GND ?
Have you tried B to refill the zones ?
and . . .
Can you paste your version info here please, you can get it from KiCad > Help > About KiCad > Copy Version Info
There are ratsnest lines between the GND pads of the antenna and the GND via’s in the zone.
Light bulb moment:
Your antenna has two GND pads, but they still have a ratsnest line between them, so your antenna copper is not recognized as a valid copper connection. The reason behind that is guesswork from a screenshot.
Application: KiCad PCB Editor (32-bit)
Version: (6.0.11), release build
Libraries:
wxWidgets 3.2.1
libcurl/7.83.1-DEV Schannel zlib/1.2.13
Platform: Windows 10 (build 19045), 64-bit edition, 64 bit, Little endian, wxMSW
Build Info:
Date: Jan 26 2023 07:27:00
wxWidgets: 3.2.1 (wchar_t,wx containers)
Boost: 1.80.0
OCC: 7.6.2
Curl: 7.83.1-DEV
ngspice: 38
Compiler: Visual C++ 1934 without C++ ABI
Build settings:
KICAD_USE_OCC=ON
KICAD_SPICE=ON
1 Like
KiCad V6 is really old. Built in 2023 according to your build info.
I think back then, the hack was to add the key word “net tie” into the description field of the footprint, and without that, KiCad always keeps a clearance from graphic items (such as most of your antenna).
I designed this antenna in to footprint editor. is there is any problem for this method?
“any problem” is a wide blanket statement, but creating footprints in (I assume) KiCad’s own footprint editor is a common task. But as I wrote earlier, there are some quirks for using graphic items on a copper layer, and each KiCad version is a bit different in this regard.
And we can’t see how the individual parts of the footprint are combined from a screenshot. For a self designed footprint, you probably did not set the (quite well hidden) net tie keyword. Load the footprint in the footprint editor, then: Footprint Editor / File / Footprint Properties and add: Net tie, into the description field. This is a hack specific for KiCad V6 to fix issues with graphics in footprints.
KiCad V6 is a long time ago for me. I forgot whether the Description or the Keywords string was the essential hack. The screenshot above is from a default net tie footprint in KiCad V8.
I never even knew this existed, well remembered.
More info for the OP