Hi, I want to design the PCB antenna. I used the RF_Antenna:Texas_SWRA117D_2.4GHz_Right footprint but it is showing the said errors.
It looks to me like a bug in the footprint definition… could it be that a KLC component doesn’t pass pcbnew’s DRC?
I was able to duplicate your problem; then I edited the footprint and prepended “net tie” to the footprint’s “Keywords” field… DRC then passed.
3 Likes
Hi, Thank you so much for the help. It did remove all the errors. What was the issue? I did not understand
1 Like
It’s an old footprint, made several KiCad versions ago.
It was made from a combination of pads and graphic lines (lines on a copper layer are not the same as a copper track in KiCad). Graphic items do not have netlist information for example.
When KiCad improved over the generations more checks were added and at some time KiCad became able to checkclearance violations beteween copper tracks and graphic items, and since then constructs such as this antenna got flagged by DRC.
There used to be (and still is) a trick in KiCad for a “net tie”.
The current implemenentation of a net tie, is two pads (so it can be connected to two nets) and a graphical line on a copper layer to connect those pads. When KiCad became able to flag graphic items as DRC violations, the “net tie” keyword in the description was added to suppress the DRC warning. This is a “hack” and in the future some better implementation will be implemented.
6 Likes
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.