Hi Everyone,
I am using KiCad (5.1.5)-3, Platform: Windows 8(build 9200), 64 bit edition, 64.
I am doing a PCB layout and have completed nearly 60% of placement and routing manually. Now I have discovered that I need to include two additional pull-up resistors in the circuit for safe operation.
My question: After changing the circuit in the schematic entry, which is the better option:
Load or reload netlist (in my case)?
OR
Update PCB from schematic?
The background of my question is that if possible I don’t want to loose the manual placement and routing of components in PCB layout I have already completed.
Comments suggestions from your side would be most welcome.
Thanks and best regards
Starter99
SAVE the project. Use “Update PCB” and see what happens. If you don’t like the result, don’t save it, just close, reopen and try load the Netlist.
I have not successfully determined what causes the loss of traces. It is linked to the amount of changes in the schematic. Never renumber the refs.
It’s likely MUCH more free advice will be arriving shortly. (
good luck!
In the meanwhile I have tried out myself using a small test circuit. After PCB layout, I made changes in the circuit and then used the option “Update PCB from schamatic”. It worked all right. The circuit changes were implemnted in the PCB layout and the rest of the PCB layout I had already made before was intakt.
So, it seems the answer is to use the option: “Update PCB from Schematic”.
Actually, we can close the thread.
Thanks and best regards
Number 2 is the recommended way in all cases nowadays. Netlist is needed for external programs.
Updating doesn’t touch tracks or anything like that. (If it does it’s a bug.) Only the footprints. (EDIT: see the exception below.) If every footprint has a corresponding symbol in the schematic you won’t loose anything.
Updating adds newly added footprints (from the corresponding symbols).
If you have changed nets or connections you may have to remove old traces manually before rerouting.
You can change the annotations but never do that while you do other changes in the schematic. Keep reannotation an isolated task and update the board after that choosing the latter of the Match Methods.
(EDIT: exception to “tracks aren’t touched”: rewiring connections in the schematic may lead to situations where the old tracks create wrong connections. The tracks are always kept but the nets may be changed because of changed pad nets. After an update an old can can have different net than one of the pads it’s connected to. KiCad just can’t logically correct it for the user. In that case Edit->Cleanup Tracks and Vias -> Delete…different nets may be useful before rerouting.)
