Try this:  [https://easyeda.com/andyfierman/shorting-link](https://easyeda.com/andyfierman/shorting-link)  

I just trace out the dotted line ground planes separately for the digital and analogue side and join them with a single track.   Same net name but no joining where I don't expect them to.

@andyfierman Thanks Andy!

@andyfierman Just hoping that there would be a way to merge the points that were compatible with copper/ ground pours

The basic problem is that despite what you call them - unless they are galvanically isolated or separated by things like optional (fit/not fit) 0R links - a Digital Ground is exactly the same physical net as an Analogue Ground. The only thing that distinguishes them is how they are physically routed. Electrically there is DC continuity between them and so as far as the netlister is concerned, they are actually the same net.

I thought that is what was going on. Maybe a nifty solution would be to have an exception in the software that would not join the two nets into one for that specific part that you showcased.

So if you place an instance of that 2-pins-same-number symbol and the associated footprint when it is pulled into the pcb, then the software respects the different netnames either side of it and does not merge them? @support, would that be possible?

How about just place two netlabels at one wire? just like:  when convert to PCB, the editor will choose only one as PCB net

That works too. The function of the SHORTING_LINK symbol and footprint however is to provide a visual reminder, that is automatically passed from the Schematic into the PCB, that these nets must be tracked carefully. In fact the symbol (as text as part of the symbol) and the footprint (in the Document layer) could be modified to add a text note to describe what has to happen in PCB layout. :)

@support @andyfierman This is all fine but with a copper pour the PCB editor does not respect that there are in fact two nets. Schematically it doesn't make a difference but like said above the pcb editor treats as one net. In the PCB editor the nets may need to be kelvin connected where when they merge can be ground poured. Currently, say on a ground plane, when using a ground pour the two nets are merged everywhere instead of only at one point.

Been playing... I think this is a procedure that will accommodate any situation. * For Kelvin Connections in particular, the easiest way is to place a Board Cutout "No Solid" region around the tracks that you want to keep clear of copper flood. A refinement of this is to: 1. create the Kelvin connections as separate tracks and not as part of the whole net tracking (i.e. stop drawing the track when you get to the Kelvin connection section and then draw just that section);  2. copy the track segments forming Kelvin connections;  3. paste them in a blank area of PCB;  4. For each copied section;  5. select the whole copied section;  6. increase the track width by something like 2 to 5 times (may need to experiment);  7. right click off the selected section;  8. click **Convert to Board Cutout**;  9. re-select the whole copied section; 10. select **No Solid**;  11. set the **Copper Zone** canvas attribute **Invisible**;  12. reduce the canvas Snap Size to about 1mil for accurate placement;  13. select both **No Solid** areas;  14.  check and if necessary, set the desired layer for the newly formed No Solid regions;  15. move them to overlap the original Kelvin Connection track sections;  16. reset the **Copper Zone** canvas attribute V**isible**; 17. **Shift+B** to rebuild all copper areas;  18. Check the **Design Manager**. * This technique can be used to create separations such as those required for ground plane start points by drawing a track **in the Silkscreen layer** that defines the route of the desired gap between planes and then converting that to a **No Solid** region. This will automatically set to a **Top Layer** object that can then be set to the desired layer and placed to define the required gap once the layers are rebuilt.