I’m sure this has been asled before, but I don’t know the correct terms to search for. Sorry
In the schematic, I have moved components from one sheet to another. Now I am getting duplicate components when importing to the pcb layout. Though only one component exists in the schematic.
Is there a simple way to resolve this please. 
Are you sure they are not duplicated in other sheets?
Otherwise just delete from all from PCB layout and F8 to sync them again from the schematic. If duplicates came back them they must be duplicated in the schematic.
Hey, thanks gmc.
I will try what you suggest
No, that didn’t work
I cut and pasted from one sub schematic, to another, and deleted the redundant sub schematic.
Can you post the project here
I can certainly try.
Which component is duplicated? I don’t see any duplications
Actually I see a issue with J3/J2. The footprint on the PCB is wrong. Delete it on the PCB, press F8 and then the correct footprint appears.
The main connector is trying to import again, when it is already there.
Perhaps it’s my settings. What should I try?
The issue is with the footprint being ouf on sync between the PCB and schematic.
On PCB:
On schematic:
Connector_PinSocket_2.54mm:PinSocket_2x02_P2.54mm_Vertical
Delete and F8 to bring the the correct one back.
Thank you @gmc 
Sorted, once I actually read what you wrote, and let go of my thoughts on it. 
Now to sort out the bigger issue, of why the MCU is getting hot. Something fixable I hope
Internally KiCad uses an UUID for both the schematic symbol and the PCB footprint, and KiCad only recognizes the connection if both of them have the same UUID. With a normal copy and paste operation, KiCad changes he UUID from the schematic symbol, as two symbols with the same UUID is simply not allowed.
If your intention is to move a part from the schematic to another sheet without loosing the connection with footprints, then you have to apply a two step process. The first step is to use Paste Special (Either from the main menu or from the popup menu under the right mouse button) and use it with the option: Keep existing reference designators, even if they are duplicated.
(This assumes that Reference Designators have already been assigned, otherwise KiCad won’t even allow putting the footprints on the PCB in the first place).
In the second step, you have to use: Re-link footprints to schematic symbols based on their reference designators during the Schematic Editor / Tools / Update PCB from Schematic [F8], because KiCad always assigns new UUID’s when pasting. This “Match by RefDes” can also be used for repairing the links whenever the UUID’s got out of sync.
Thank you, both of you. Great explanations.
I should have known better, but have a lot of issues with the board now it’'s arrived, and wasn’t really concentrating on what was in front of me.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
