for reverse engineering a schematic from pcb layout i use this workflow:
create a schematic sheet and place all components on it
PCB: identify pads that are connected, and select them
go to schematics an draw a wire (connection) between the pads that are highlighted
Update layout from schematics F8
PCB: A trace between 2 pads can only be drawn, when the pads have the same net name. This is the reason why you have to go to schematics and draw a wire between the associated components.
Question:
Is there a way to (automatically) name 2 (or more) pads on PCB?
Or, is there a way to switch off the check for net names when drawing a trace between two pads?
With predefinded names (e.g. GND) it can be done with property manager.
What about the others?
I am detecting some half story here.
What do you begin with?
First, KiCad can create a PCB from a set of Gerber files, see:
If you have photographs instead of Gerbers (if you have the real thing, then make photographs ) then you can use PCB Editor / Place / Add Image to add images to some of your PCB layers, and this is a great help with reverse engineering.
But I guess that what you are asking for is to disable DRC in: PCB Editor / Route / Interactive Router Settings. Set the Mode to Highlight Collisions and in the Options area, turn on the checkbox before Allow DRC violations.
It is also possible to create net names with PCB Editor / Inspect / Net Inspector, or in the Nets tab in the Appearance manager on the right side of the window. Then click on the Plus sign in the lower left corner and enter a new net name.
Once you have net names, you can select a pad, press e to edit it, and select one of the created net names from the list:
There is also a “Wire it” plugin for the PCB Editor that may be interesting for you.
However, I’m not sure if it’s actually useful to manually create the netlist in the PCB editor. It may be easier to just start creating wires from schematic symbols, label them, and then regularly push the netlist to the PCB editor as you go.
your detailed answer is very inspiring.
I agree the easier way is to realize it with schematics editor. All other methods need same/more effort.
I hoped for a macro to automatically name connections and reduce manually work…
It would be nice if it was possible to first just draw tracks in the PCB Editor, then port the netlist to the Schematic Editor, and then use ratsnest lines to sort out the schematic symbols and draw the wires. Maybe it will come… in a few years time.
Have you tried the Wire It plugin yet? I experimented a bit with it a few years ago, I think it’s related, but I’m not sure anymore.
) then you can use PCB Editor / Place / Add Image to add images to some of your PCB layers, and this is a great help with reverse engineering.
