Hello,
I am designing the PCB NFC antenna in my project. The problem which I have faced is that on the schematic I place two pins 1 , 2 for antenna , but since this a traces on the layout it treat entire trace as single net so not allow me to connect second end to the right output see below. Could you advice me what trick I should you to overcame this limitation?
Schematic
Layout
Thanks a lot in advance
Jacek
There is a special component type called a Net Tie for situations like this, where you need to purposefully short two nets together.
Create a simple symbol(2 pins in this case), and set the type to Net Tie
Create a footprint with 2 pads, and short the pads together with copper inside the footprint. In a situation like this I would probably just place a couple surface mount pads of the proper size to match the trace width, the track to short them usually matches this width as well.
Link the footprint model to the symbol and use it in your project. Wire each net to the separate pins for the net tie symbol
When you ECO to the PCB, this new Net Tie footprint can be placed in the area where you want this controlled short to happen.
Route Net_1 to one side, and Net_2 to the other, the short happens internally to the footprint, so it is understood by DRC, and this is a Net Tie component so it will not appear in the BOM.
There is also a checkbox in the Design Rule Check dialog for Verify Shorting Copper. This particular check is specific to Net Ties, and checks any Net Tie components in your design to make sure they have internal shorting copper if they are set to Net Tie
