Replacing parts in a schematic

I set my parts up first so that I will come out with a manufacturing BOM at the end of my design so swapping parameters will presumably just alter the part, i could of course copy the same properties from another part ? or if I say delete a resistor and replace it giving it the same reference number like "R10" will that still link to the placed footprint on the PCB ?

I set my parts up first so that I will come out with a manufacturing BOM at the end of my design so swapping parameters will presumably just alter the part, i could of course copy the same properties from another part ? or if I say delete a resistor and replace it giving it the same reference number like "R10" will that still link to the placed footprint on the PCB ?

If you have the full manufacturing / BOM data attached to the library part then you would need to delete the part and add the correct one from your library otherwise the BOM would be wrong, just changing the Value parameter of the resistor from say 1K to 22K would not work as the other part information would not be updated. Instead you would presumably have a 22K resistor in your library to pull in. If you have set your library to have a components for every possible resistor value you are using then you would have to already have set up exactly one footprint on the part that matches the part you will be purchasing. This way the schematic user doesn't need to be concerned because the correct footprint would be part of the symbol. If allowing a choice of footprint from the library (e.g. a 22K resistor in 0805 and 1206 variants) then you can have two footprints attached but your BOM generation / purchasing department would need to be able to use the footprint column to differentiate between otherwise identical parts. The same would apply if you chose to have one generic resistor, the purchasing department would have to use the Value and Footprint column to determine the actual part to buy.

With regards to PCB linking, if you delete a resistor, add in a replacement one and give it the same reference designator then it will link to the PCB part by virtual of identical ref des. You would need to use the Update PCB function to pass across the new data because it is possible the footprint will have changed.

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.

You say Altium designer, does it apply to CS ?

Yes, both AD and CS should have the same underlying mechanism to synchronize the schematic and PCB. 

Hi Thomas

Could the same be achieved using Component Links from PCB editor -> Tools ribbon?

I have found this function very useful recently.

Thanks for reminding me about that.  When I used Altium Designer I used to confirm that all schematic and PCB parts were fully matched as part of final cleanup.  I hadn't yet done this in CS.