Re-use Methods

Eric Albach

I just found a snippet design re-use method that is quite reasonable. Basically, append a question mark to the designators and create the snippets. Place the snippets in the new schamatic and PCB. Link the components between the schematic and PCB. Use Annotate Schematics Quietly. Update the PCB.

It's pretty easy. With this method it takes less than a minute to add a fully linked and annotated design. I used to spend a lot more time.

From the original schematic and PCB:
Update and Link the components between the schematic and PCB
Select the schematic section

Use SCH Inspector set to include only parts and use Smart Edit Formula on designators to append with a question mark.
        
Example formula : !+'?'

ends up with R12? (leaving the numbers keeps the components linkable and the question mark allows quiet annotation)

Update the PCB with the new designators
Create the schematic and PCB snippets

In the new schematic and PCB:
Place the snippets
Link the components using Project > Component Links > Add Pairs Matched by Designator
Use Annotate Schematics Quietly
Update the PCB

Source https://forum.live.altium.com/posts/221757/645999

Rich Betz

When you paste PCB snippets, be careful with existing 'ON' Planes. Your via's can and will connect to the first plane they contact, throwing your net connections all out of whack.

Either turn off all of your Plane Layers before you place the snippet, or place it outside the board outline until you get all of your component net connections linked up correctly.

When you get your Sch/Pcb component pin nets all linked up with All Layers On, select the whole snippet area.

Use PCB Filter (IsSelected and (IsVia or IsTrack))  to filter out the parts but hold on to all the connections.

Then CUT the connections with reference to Pin1 somewhere in the snippet,

Then Paste right back in the same place.  All tracks and via's will adopt NetName from component pin nets.

Then... you can turn your Planes back on and position the snippet where you want it.

Source: https://forum.live.altium.com/posts/221757/646088

Eric Albach 

Possibly the best method for the PCB side is to keep "snippets" in a PcbDoc then you can select, copy and paste special with Keep Net Name. That way you won't lose the polygon pour nets.

Source: https://forum.live.altium.com/posts/221757/646099