Working on a stacked two board design. What’s the best/easiest way to convert the layout of my upper board to a footprint so I can place the connectors/mounting holes in the correct place on the lower board?
I would:
1). (Partially) design the first PCB.
2). Copy the PCB to the “other” project.
3). Delete everything, exept what you want to preserve (outline, holes, connectors, etc)
4). Make sure the Refernces of the connectors you want to keep coincide with the references on the schematic on the other design.
5). Update the PCB from the schematic [F8].
Alternatively, you can make a “mini” project that contains only the common parts between both PCB’s.
Then:
1). Start KiCad with one of the original projects.
2). Start Pcbnew from KiCad’s project manager.
3). Save the empty PCB file in Pcbnew.
4). COMPETELY EXIT KICAD.
5). START PCBNEW FROM THE COMMANDLINE.
(sorry for yelling, it was important.)
Pcbnew is now opened in “stand alone” mode (not from the project manager).
6). Pcbnew / File / Open … and open the empty PCB file you had made in steps 2 & 3.
7). Pcbnew / File / Append Board. And then select the “mini project” with the board template.
8). Save the project and EXIT Pcbnew.
9). Open Kicad’s project manager and continue from there.
10). [F8] etc, from within Eeschema to import netlist and components.
The “stand alone” mode of Pcbnew is different from the normal mode because it is disconnected from any schematic. Netlist and components import is (as far as I know) not possible in stand alone mode.
The “stand alone mode” of KiCad is meant for “appending boards” from diffferent projects, for example for making a panel from several unrelated boards. But it can also be used (abused?) for copying tracks or partial layouts between different, but similar boards.
Yet another way in which this can be done is to first design one of the boards, and generate gerber files. Then, with the gerber viewer from KiCad (called Gerbview) you can “export” a PCB back to a KiCad PCB file. This is not a perfect “back export” because a lot of info is simply not available in gerber files, but you can recover board outline, mounting holes, tracks, pad locations from any gerber file. This function can be a timesaver when reverse-engineeering a board of which only the Gerbers are available.
1 Like
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.