KB: Short two different Nets to create a Net Tie

[Why] Need to create a footprint where two pads are ohmically shorted together for such components as planer inductor and other printed RF filters and antennas [What] Create and register its footprint and symbol as a 'Net Tie' component [How] In Properties panel, select 'Net Tie' from the the pulldown for Type attribute of both footprint and symbol. In the footprint, the two pads are to be shorted by placing a Region primitive in-between, just touching these two pads. The two pads need to be maximized in size with little to no overlap with the connecting region which need to be sized minimally in return, as the copper region belongs to a different net in view of DRC affecting track terminating to a pad or polygon pouring.

Starting in Version: 18.0
Up to Version: Current

Solution Details

In order to short two different Nets in the design, you will need to create a Net Tie.

• Place two pads in a footprint (PCB library)
• Short them with a Copper Region in between.
• Make sure that the copper Region just extends to the sides of the pad but not to the snap point in the middle of the pad itself. Otherwise, connecting tracks and polygons won't connect to the snap point of the pads later in the design.

Use Tools ► Footprint Properties to give it a Name and to set the Footprint Type to one of the Net Tie options.

You will also need to create a Schematic Symbol in a Schematic Library and use the Properties panel to set the symbol Type to one of the Net Tie options.

​​
​​​​​(Don't forget to add the footprint to the schematic library symbol.)
https://www.altium.com/documentation/altium-designer/a-look-at-creating-library-components-ad

If you see the error message:
Net Tie failed verification: [...] has isolated copper, then the shorting copper in between the Net Tie is too small, and is not connecting the Pads.

In a slightly different context where you do not want to introduce/place a net tie component, another technique/hack to short two different nets would be to make use of signal harness, which becomes particularly handy, for example, when connecting nets across many repeated multi-channel block in daisy-chain:
https://www.altium.com/documentation/altium-designer/buses-signal-harnesses#!signal_harness

For further information and reading, review the following resources:

https://resources.altium.com/p/using-net-ties-to-meet-pcb-design-requirements

https://www.altium.com/documentation/altium-designer/creating-connectivity-ad#intentionally-connecting-two-nets
 
https://www.altium.com/documentation/altium-designer/interactive-routing-ad#!connecting-two-nets-with-a-net-tie-component

Here's an older document, but it may have useful information:
https://resources.altium.com/sites/default/files/uberflip_docs/file_1176.pdf

You might also want to do a little research on Zero-Ohm Resistors.

Planer inductor:

Planer inductor, coil, spiral antenna pattern can be constructed by placing and connecting 180deg arc primitives of incrementally changing radius.  The end result is a long contiguous copper piece where its two ends are terminated by pads to be registered as Net Tie component type.

Below illustrate a visual example of how multiple arcs are placed together to form a spiral pattern.