Renumber hole schematic sheets without losing component links

[electricar]

Hello folks

what is the easiest way to renumber the designators in hole schematic sheets in Altium without losing the component links?
My layout is finished and I want to reduce the sheets and renumber the designators as mine are numbered like this:
Sheet 1: R100, R101…
Sheet 2: R200, R201…
…
Now some parts from sheet 2 were moved to sheet 1 and have to be renumbered to R1xx and so on...
I did the reset and re-annotation in Altium but I loose the component links.

Thank you very much in advance!
Kind regards

[ajb]

Did you restore component links after moving the parts but before reannotating?  Moving the parts from one sheet to another is likely what's breaking the links, so if you restore the links immediately after, before you change the designators, you should then be able to reannotate without issue. 

There may be additional complications if you have repeated sheets or something depending on annotation settings, but then you probably wouldn't be moving parts into those sheets.

[electricar]

Did you restore component links after moving the parts but before reannotating?  Moving the parts from one sheet to another is likely what's breaking the links, so if you restore the links immediately after, before you change the designators, you should then be able to reannotate without issue. 

There may be additional complications if you have repeated sheets or something depending on annotation settings, but then you probably wouldn't be moving parts into those sheets.

Hi ajb,

I found the solution in the official Altium forum:
https://forum.live.altium.com/posts/198084

It has to do with the cut and paste of the parts to the new sheet, what resets the unique IDs, which make the link between the schematic and the PCB. Selelcting the components, right click and  "Refactor > Move Selected Subcircuit to Different Sheet" keeps the unique IDs.
If you move the components like that, you can renumber them to your wishes without having to make the links again.

I'll just paste the post here, as it is quicker than to login into the Altium forum to view the post:

Chris, This is probably as a result of you using cut-and-paste to move a component.

When you paste, a different Unique ID will be assigned to the component. Altium links components between the schematic and the PCB by their Unique ID, so when you "Design > Update PCB Document" from the Schematic editor, it will be seen as a different component, even though the designator is the same. In this case, if you examine the "Engineering Change Order", you will see that the existing component on the PCB will be marked as "Remove", and another line will "Add" the new part from the schematic. (If the Unique IDs are the same, then the action will be "Modify".)

If you want to move a component on a schematic sheet, then the best way to do that is to drag it to its new position. If you want to move one or more components to a different sheet, then select the components you wish to move, right-click on one of the selected components, and go "Refactor > Move Selected Subcircuit to Different Sheet", then select the target sheet. Both these methods will retain the original Unique ID of the components.

If you suspect that your component links have got out of sync (by observing the "Remove"/"Add" in the ECO instead of a "Modify"), then use the PCB editor function "Project > Component Links" to manually correct them by matching the reference designators together. You can move things around manually, or you can simply press the "Add Pairs Matched by" button to move all the parts with matching designators (and optionally matching comments and footprints) to the right hand side.