Is there a way of swapping parts in a schematic? say you have a resistor and realise you need to change the value or a zener diode. The symbols are identical they will just carry different part numbers.
Is there a way of swapping parts in a schematic? say you have a resistor and realise you need to change the value or a zener diode. The symbols are identical they will just carry different part numbers.
As in AD, each symbol has a unique ID. On the schematic this can be found by the component properties (2X click the part).
On the PCB you will find the comparable parts unique ID in a similar manner; it is in the lower right side as Schematic Reference Information and it gets a prefix \ character.
That is what binds the two. So if you replace a part on the schematic, say one resistor for another, you could note the unique ID on the schematic and then make the new schematic part have the same unique ID.
It gets more complicated if you replace a schematic part with another that has a different footprint. When you update the PCB to synchronize to the schematic, it should attempt to match the two using designators. It would probably delete the original footprint and then place a new footprint in a default location and not where the other one was deleted from.
You should be able to learn more by searching for Altium and Unique ID.
Thomas, great explanation of unique IDs.
Just to clarify, if you delete a schematic symbol and add a new symbol with the same ref des you will see the following dialog when attempting to update the PCB:
Say YES, the PCB will be updated and the footprint will be updated as necessary to match that specified by the schematic. The component will remain in the same place on the PCB.
To get rid of the rather annoying dialog each time you update, in the PCB editor use Tools > Component Links. Any parts where the unique IDs don't match will be listed in the first two columns (matched by ref des). Use the right arrow button to add to the Match Components list and then click Perform Updates.
