Nets name conflict

[grimmjaw]

Hi,

First off, I am no expert in alitum so bear with me.
As you can see in the attached pic, I have a shunt resistor that I need to measure.
I'm using a multiple sheets design(power is set to global), and use port to connect the
different sheets.

My problem is am using differential measurement to measure the resistor and is connected to analog GND, and now i have a conflicting nets name, one is Vsense low and the other is Vssa. I would like to separate this two , to avoid any ground loop.

Anyone has any suggestion?

[poorchava]

I'd separate them on schematic and then use some sort of sopper fill to connect them on PCB. DRC error can be removed by setting a rule to allow short circuit between two nets.

This is kind of a workaround, but it works.

You can also use a dummy component consisting of two pads connected by a piece of copper, but you're gonna get short-circuit DRC error too.

[T3sl4co1l]

Two options:
1. Delete the port.  The netlist doesn't give a damn how you intend to wire it: ground is ground.  Route it differentially in the PCB by hand.
2. Split the ground net (and possibly the other one, too) and use a net bridge or zero-ohm resistor to join them.

A net bridge footprint can easily be made (or there might be libraries for them) by making a component with two SMT pads (specified with negative solder mask expansion so they remain as covered copper), shorting them with a trace or fill.  The part needs to be specified as a net bridge somewhere (I forget what property does this).  When placing this component, the shorting copper is ignored by DRC checks, and won't be assigned a net (or if it is, it doesn't matter) by Netlist from Physical Connection.

This also works for other planar components like RF stripline and filters, "gimmick" capacitors, planar transformers and so on.

Tim

[grimmjaw]

I think I prefer zero-ohm resistance.
Thanks for the tip