I have two nets (GND and GNDA) which I want to bridge at a defined point, so in the schematic they are separate and there is a closed solder bridge which connects them. However pcbnew doesn’t want to connect them. I can put a zero ohm resistor without issues, but not a closed or open solder bridge, those pads won’t get connected to the GND or GNDA planes.
Is that intended behaviour, am I doing something illegal here or why am I forced to put a zero ohm component there instead of my solder bridge?
This is the right behaviour. GND and GNDA are two different nets, just as GND and +5V.
Look for a net tie in the Device library.
1 Like
I have never used net ties, I don’t know how they are connected to a zone.
This is an unintended consequence of the net-tie footprints using the new custom pad feature. Custom pads won’t auto generate thermal connections to zones. You can solve your issue one of two ways:
- Manually draw a short trace stub from the pad of the net-ties into the zone area. I haven’t tested this myself so it might not work. Also, if you use the auto clean stubs tool you will loose the connection to the zone. So maybe it would be better to draw a trace from the custom pad in the net-tie to the nearest normal pad in another component.
- Modify the pad properties of the net-tie footprint to solid connection to copper fills. (I don’t have Pcbnew open right now so I don’t remember the exact wording.) You can change it at the board level, but if you update those footprints from libraries you will loose your change. You can change it at the library level, but it would be best to copy the net-tie to a personal library, make the changes there, then point the schematic symbol(s) to your modified footprint in your personal library.
5 Likes
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.