The links are broken between schematic and pcb. this can happen if you kludged in parts in the pcb that were not originally in the schematic and added symbols later and then fudged with designator renumbering.
Not a problem. easy fix
But first : here is why this happens.
When you place a component on the schematic and give it a name ,like R33 and then update the PCB altium does not store the part in its internal database system ( the design is essentially a massive database containing objects. when you open a schematic view it pulls the parts it needs. when you open the pcb it pulls the parts it needs. ( even though the documents are the in physically different files there is cross-correlation by various parts of the program .
so, storing by reference deisngator woudl not be a good idea. what if you have two the same designators ? ( multichannel design , or a stupid mistake ? ) or you renumber all of them , how will you find what is what ?
so altium uses an index key ( if you double click a schematic part you will see this key it is an 8 digit alphanumerical string like K4F53TZ3 (an example )
Anything that is done , whetehr in schematic or PCB or any other part of the program is done using this key. The key is created when a new part is placed ( can be in pcb or schematc , doesn;t matter )
any subsequent operation refer to that key.
If you fudge around with the system deleting a footprint , placing a different one and then manually changing the designator you break this tracking system.
if you doubleclick an existing part and select a different one there you do NOT break this system
Anyway, long story short , it is possible for the indexing system to go wonky.
How is it solved ?
Very easily :
in the PCB : Project - Component Links
a window will open. with two colums. you can throw stuff from left to right.
between the columns are buttons with arrow. click the the double arrow left <<
this removes everything from the right column.
Now at the bottom of this windo is a button : Group by reference designator. Click Execute.
This will cross reference , reset all the unique ID's and bind them together . PCB will go to schematic and copy the ID's from there.
Close this window.
Now , if you have managed to break the links , your netlist will be messed up most likely too.
Design - Netlist - Clear all nets
this destroys the existing netlist in the PCb and all the history in the ECO's
Go to your schematic and do D-U ( Design-Update PCB )
this will restore the netlist
and you are good to go now.