Problem using template projects, footprints duplicated after changing refdes


Hi, I am using 5.0.0 on a Mac. I am trying to use a template as a starting point for my project (specifically the raspberry pi hat template).

Everything initially works OK if I create from template, open eeschema, generate netlist, and then open pcbnew and read netlist. The problem starts if I change the refdes of some parts.

For example, the template initially has a 2x20 pin header named J3. If I change that redes to J1 in eeschema, and regenerate the PCB, I end up with J1 floating in space and J3 is still there!

I found out that it’s possible to “Lock” things on the PCB, and it appears that if something is “locked” the intent is to keep it from being changed (presumably even by refdes).

So, I started from the beginning, but before reading the netlist, I right-clicked on the J3 part and selected “unlock”, saved the PCB, and then read netlist again. But I STILL GET and “extra” header. BTW, when I read the netlist, I do select “Change” for Exchange Footprint and “Delete” for Extra Footprints.

At this point, I am totally lost. How can I use a template if I can’t even change the refdes without ending up with an extra part? How do I avoid this problem?

I would rather not start with an empty project, it is too much work to recreate what is in the template.


The create netslit -> import netlist workflow is outdated in v5. Use “update pcb from schematic” tool found in the tools menu of pcb_new.
Not sure if this will solve your problem but might be worth a try.


Thanks Rene, that solves most of the problem! What a relief!

If I unlock the part and then use “update PCB from schematic”, it no longer creates the duplicate part.

However, it does remove traces from that part and floats it. I have to reposition it.

This could be a problem on templates with many parts that need new refdes, but I can live with it for this particular project.


you could also try the old netlist import workflow with identify by timestamp instead of by reference. I am not sure if there is an equivalent option for the new update pcb from schematic workflow.

Ok i just checked it, there is a radio button in the update dialog that can switch you over to by timestamp.


OK, I see… I was wondering what it means to “identify by timestamp”.


I can now change the refdes of parts which are part of the template. Thank you!