I was working with a customer recently who had two PCBs that were related. He wanted to work from a single schematic package, yet have a subset of the schematics populate two different boards. It’s a common enough scenario, and it’s reasonably simple to achieve in Altium Designer. Here’s how.
Altium Designer currently supports only one PCB per PCB Project. In other words, each PCB project targets only a single board. So in order to have related schematics populate different PCBs, we first need to have multiple PCB Projects (PrjPCB), one for each board we are targeting. The secret to amalgamating the schematics is to have a third project for the overall design that doesn’t target a board, but acts as the design project for the multi-board system.
Consider the Design Workspace in the figure below. Here we have three PCB projects. The first - PCB_Project1.PrjPCB - contains the complete set of the schematics for the two PCBs. It is in this project that all schematic design, electrical rule checking, etc. takes place. This is in fact the master design project for all boards to made from the design. Since all of the schematics are in the same project, their net connectivity will be extant throughout the design.
The remaining two projects - PCB_Project2.PrjPCB and PCB_Project3.PrjPCB - contain a subset of the schematics in the first project, as well as the PCBs which will be updated by the defined schematic subsets. PCB_Project2.PrjPCB and PCB_Project3.PrjPCB simply have the appropriate schematics added to them by right clicking on the PrjPCB file and using the "Add Existing to Project" command to add the relevant schematics.
At this point any changes made to the schematics in PCB_Project1.PrjPCB will be reflected in the schematics of the other two projects, as the schematics you’ve added to these are in fact the same files contained in the master project.
When the PCBs are updated in PCB_Project2.PrjPCB and PCB_Project3.PrjPCB, only those schematics contained within each PCB Project will be reflected in the updates.
While the demo design used in this blog targets just two PCBs, this technique can be used for any number of PCBs and provides a simple way to consolidate the front-end schematic design of complex multi-board projects.