Multiple boards/schematics - Page 1
Forum section: electronics / general

author: Poe
author_rank: Frequent Contributor
timestamp: January 30, 2014, 04:42:25 pm
content: How do you easily handle multiple-board projects in Altium? I have a project with several boards stacked on top of each other and I'm having a hell of a hard time.In the past, I would combine the PCBs into the same PCB file and just call out in the fab notes how to separate. Then I started to create an entirely unique project for each board. Unfortunately using this method I couldn't easily make schematic changes and verify connections.Today I tried to use a single PCB project and just create one schematic and one PCB file for each board. ...it's not working so well. Altium treats all the schematics as one (which is fine because my part designators and netlabels are all unique), and it wants both PCB files to be duplicates of each other. For example, when I make a small change to one schematic and try to update one PCB file, it tries to pull in the hundreds of parts and connections from the other schematics.Is there a way to 'link' one schematic with one PCB? If no, how are multiple PCB files used?

author: David_AVD
author_rank: Super Contributor
timestamp: January 30, 2014, 08:40:07 pm
content: So the boards all have their own parts and connectors and are part of a system?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 30, 2014, 11:04:32 pm
content: Somewhere in the docs, it says you can only use one PCB file per PCB Project.Best approach, make individual projects (now designators and net names don't have to be unique), ensure the connector pinouts are consistent between them, and maintain up-to-date STEP models of each board, so that each project has current models of the others with it (assuming you need to view mechanical fit and all that).If you need a simulation over all boards... best off making yet another project with all that in it (just schematics, no PCB). Might be able to get away with off-page connectors, or something to do with harnesses or subsheets, to 'mate' connectors' nets together so that you can at least use the same schematic files (of course, names have to be unique again, except for nets bridged across connectors, which must necessarily match).So you can generate simulations, schematics and BOM (over all PCBs, anyway) from the master project, but have to go into the sub-projects to generate fab files for each PCB. (I know OutJob files allow you to select a PCB File to output from, but... if you're only ever intended to have one PCB in the project, what use is that!? Might be worth asking Altium themselves about that, see if they have any ideas... or if it's just a remnant that is as useless as it seems.)Tim

author: Poe
author_rank: Frequent Contributor
timestamp: January 31, 2014, 01:57:29 am
content: Quote from: David_AVD on January 30, 2014, 08:40:07 pmYep. It's a new test fixture that has to fit in the small space of the previous test fixture, so the boards are stacked.Quote from: T3sl4co1l on January 30, 2014, 11:04:32 pmIt's kind of odd that you can add multiple PCB files to each project, yet it only wants one.I've never done a master project with sub-projects before. I'll have to try that out.

author: Richard Head
author_rank: Frequent Contributor
timestamp: March 24, 2014, 10:24:33 am
content: I'm not sure if it's like Protel 99SE but with Protel you have to create a Master schematic which links the two schematic pages together by labels. The Master schematic consists of only a table that links net names of the one schematic to the other. The master schematic is on a higher level than the linked schematics.It's a bit tricky to explain and I really only know when I'm sitting in front of the PC.I suspect Altiun is similar.

author: SL4P
author_rank: Super Contributor
timestamp: March 24, 2014, 11:03:59 am
content: Exactly.In the WORKSPACE object create a NEW PCB project - which will create another project branch in the workspace - at the same level as your first/existing PCB project.Put your new board SCHdocs and PCBdocs in that newly added PCB project.They will compile separately, and the SCH-PCB links are local to each PCBproj.Also as mentioned - create an interconnect SCH in each of the projects (basically identical) so that intrconnecting headers are identified correctly between the two or more schematics and PCBs.

author: mengfei
author_rank: Regular Contributor
timestamp: June 22, 2018, 08:22:41 am
content: With the new Altium 18 is this now possible? I can see Multiple Board assembly can be done but what about having multiple PCB's in one project?

author: Philfreeze
author_rank: Regular Contributor
timestamp: July 27, 2018, 07:49:37 am
content: As far as I know each PCB-project still only wants one PCB but you can add multiple PCB-project to one multiboard assembly