kicad-developers team mailing list archive
Mailing list archive
Re: What does /path do in PCBNew files?
So the approach to duplicating a section would be
1) Copy the design in eeschema
2) in eeSchema push to PCBNew
3) Layout a single section.
4) Copy and paste that section
5) Re-annotate the PCB section (this works now!) without pushing to
schematic so the references correspond to the schematic
6) in eeSchema push to PCBNew associating by reference
On 2020-02-15 6:47 p.m., Jeff Young wrote:
Pasting creates new timestamps. So copy/paste works fine, there’s
just no way to do a unified copy/paste between eeschema *and* pcbnew.
The timestamps are moving to UUIDs as we speak.
The links are reset/updated when you do an Update PCB from Schematic
and chose the “re-associate by reference” option. (The
timestamps/UUIDs encode said “association”.)
On 15 Feb 2020, at 23:40, Brian Piccioni <brian@xxxxxxxxxxxxxxxxxxxxx
I guess I'd wonder then why provide Copy and Paste/Duplicate if the
result is not usable?
It seems like a sort of honey pot.
On 2020-02-15 6:34 p.m., Eeli Kaikkonen wrote:
On Sun, Feb 16, 2020 at 1:20 AM Brian Piccioni
I think optionally removing the path might be a good idea - or,
simply removing it from duplicated/pasted footprints. Of course
I am probably missing something.
You can't backannotate something which doesn't have the "path". But
those footprints can of course be re-annotated.
I don't think it's possible to cleanly copypaste groups of
footprints to create "duplicated design elements" as you say. Either
they point to one group of symbols while they should point to
hierarchical sheet instances (each of which have different path), or
they don't have corresponding symbols at all.
If you have two footprints with identical "paths" you can reannotate
from eeshcema (with a warning IIRC) and both footprints will have
the same refdes. But it doesn't make sense to have two footprints
with different refdes to point to one symbol because the symbol has
only one refdes.
Having identical paths in more than one footprints is problematic
anyways. I have used it but I don't recommend it.
Mailing list: https://launchpad.net/~kicad-developers
Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
Unsubscribe : https://launchpad.net/~kicad-developers
More help : https://help.launchpad.net/ListHelp