FEDEVEL
Platform forum

usernamezzz , 02-23-2022, 05:04 AM

I am trying to merge two independent altium projects, schematic and pcb designs, into one project with one PCB combining these two designs.

I can view both designs in altium in 3D, Schematic and PCB

I can add the project#1 schematic to project#2 , then re-annotate to avoid numbering conflicts. All components have a standardized foot print specified.

I can copy and paste project#1 pcb design into project#2 pcb design, and all looks good

But when I "import changes" to the project#2 combined pcb file, all the project#1 components disappear

What is the proper procedure for merging these two projects and libraries without manually copying each component one at a time into the Project#2 library.

qdrives , 02-23-2022, 02:23 PM

Renumber all components in project #1 first starting at 1000 (or something big that does not exist with project #2) - so R1000, R1001, R1002, etc. Synchronize schematic and PCB, and make sure there is no problem (with both projects!).
Make sure that the reset part designator on paste preference is UNchecked (unlike the screenshot below)
Then you can copy schematic and layout from one project to the other.
Validate project.
Synchronise PCB and schematic (from PCB -> Project / Component links) on designator.

usernamezzz , 02-23-2022, 05:08 PM

Thanks qdrives, working now, very much appreciated.

usernamezzz , 02-24-2022, 05:08 PM

I discovered that it is also necessary to have all files inside the target project folder, and that the altium project schematics and pcb files reference this folder, not the folder with the design to be added. This includes libraries if you generate an integrated library from the design to be added.

This required some juggling of files, deleting all files from project and then re-adding existing to the same project using the files copied to the project folder, before Altium used correct files all from the project folder.

This may be standard practice, but its easy to miss this level of detail since the project files do not indicate where they are being read from, and even if you manually save them all to the correct folder, they still get read and written to/from original folder, which could be anywhere depending on where you copied the additional design from.

Does anyone know a better way to manage project files or is this just a feature we have to manage with Altium.

Lakshamana Balakrishnan , 02-25-2022, 12:17 AM

Hi @usernamezzz ,

as @qdrives method is very good one. I have different solution also please try if you need.

You may use to Place--Embedded Board Array/Panelise to add another PCB into current PCB. For that your stackup should be same for both PCB. You can call whatever PCB's you want and also be able to duplicate it.

Remember: Its only for useful layout usage, For schematic you may have seperate files to keep. If You want everything in single project folder then copy & paste and component linking is correct option. and using snippets also help you.

qdrives , 02-25-2022, 03:02 PM

Design in one project to begin with

And depending on what you want / need the latest Altium live showed a system where design re-use was now including the layout.

@Lakshamana Balakrishnan I think that the merge was needed as two people created to parts of a project. Not placing two boards onto a single (production) panel.