FEDEVEL
Platform forum

frangz , 04-02-2020, 05:58 AM

Hello.

I have many boards already designed and tested independently, part of the bigger final system, that will need to be integrated. Some of them will form a single PCB. Ideally, I would want to combine them on a single PCB, adding all the schematics and importing all the layouts into a single .PcbDoc somehow.

Is it any clever way to do this? Or should I forget about it and start designing my "integration board" the regular way?

willyduke , 04-04-2020, 12:26 AM

I think you should try snippets, so define snippets for every board you have and then in your final board you can integrate them

frangz , 04-05-2020, 08:36 AM

Thank you very much willyduke, I've never used snippets and while researching about them I found this post that describes the solution I was searching for:

https://altiumpcbdesigner.blogspot.c...e-methods.html

robertferanec , 04-06-2020, 01:36 AM

I am not 100% sure what situations you are in, but there are usually two situations:

- Multiple completely independent PCBs placed on 1 PCB: I would manufacture the independent PCBs as independent PCBs. Sometimes we do place multiple independent PCBs on one board, but some PCB manufacturers will still charge you for one PCB with multiple PCBs as multiple independent PCBs (even if you place them on 1 board).

- Multiple independent PCBs merge into one PCB: If you need to place multiple sub-circuits on 1 PCB, there may be more ways how to do it. We normally simply CTRL+C and CTRL+V the circuits and we re-do PCB layout on the one board.

PS:
When merging multiple circuits into one PCB, the biggest problem may be conflict between designators. So:

- Maybe I would have a look at hierarchical structure and maybe channels and there may be a way how to place multiple different circuits into schematic the way the component designators will not be in conflict and that PCB can be simply re-use.

OR, what I would probably do:

- I would maybe re-annotate the schematics and PCBs with prefix (to get unique reference designators between different circuits) and then copy and paste everything into one project

frangz , 04-06-2020, 02:48 AM

This is the situation. A colleague of mine took exactly this approach when faced with this situation back in the day, copy and re-do layout, but now I wanted to do a quicker prototype and I find that all the single developed PCBs are highly reusable for this integration. They are different power stages that just need to be mounte on the same final PCB, so in practice I only need power rails connecting them and changes in connectors for the moment.

Also with the way we do things here (individual stage development and testing and latter integration with the never ending physical and mounting demands by the client) I wanted to know a methodology for reusing and integrating layouts faster.

This is exactly the problem I was looking for how to deal with.

Yes. This is what I did based on the link I found. What I did is (starting with same layer stack individual PCBs):

• I started re-using one individual project for integration. This project has already Schematics and a PCBdoc which will be my final integration PCB.
• In the other independent project of next board to be integrated: add "?" as a suffix after all designators on the Schematic. Just select all components (Sch filter with IsPart) and write !+? into Designator field in Properties.
• Then Design Update the independent PCB with this ? after all designators.
• Next add the whole schematic to the integration project and copy and paste special with Keep Net Name from the independent PCB into the integrated PCB. This way it keeps all nets and polygons.
• Link the components using Project > Component Links > Add Pairs Matched by Designator on the integrated PCBdoc. I did this as recommended, but I don't know yet if it's really necessary.
• Then Annotate Schematics Quietly
• And finally Design > Update. Everything keeps linked with regular Designators.

I ended not using Snippets, because the amount of information re-used is bigger than what I would call a snippet (a whole project basically), and if I use a snippet of the PCB instead of copy and paste special with Keep Net Name, I lose netlist information (also might be doing something wrong here).