This feature was already accepted for development because I sponsored it, but I'm creating this Gitlab entry so other users know it's coming and can provide comments, ideas, criticism etc. I decided to sponsor it after lengthy discussion in #22270 and my [subsequent forum thread](https://forum.kicad.info/t/moving-symbols-between-schematic-sheets-how-to-prevent-breaking-of-pcb-layout-upon-next-update/65503/8). The idea is that PCB layout will stay unbroken upon next F8 update, no matter how many symbols you move between schematic sheets, even after reannotating them. It will "just work", without needing to think about it (and without having to manually enable the "Re-link footprints" checkbox during the F8 update). It should also resolve other issues mentioned in the forum thread. It will be an optional feature enabled on a per-user basis in the preferences. It's slated to appear in v11 release (I decided too late for v10). The UUID linkage mechanism will have some limitations, but they should affect only minority of workflows and projects. In essence, it will work as long as you use only cut+paste to move stuff around schematic and keep both editors open at the same time. Below is more detailed explanation by @sethhillbrand which I compiled from our e-mail communication. --- Initial feature outline: > We could implement a best-effort "synchronize schematic/PCB" communications channel. This could effectively update the symbol UUID link in PCB editor when moving symbols between sheets in the schematic. We say best effort because this would still break when running schematic editor in stand-alone mode and when a schematic sheet is shared between multiple projects. It would also break when using non-standard workflows like Copy -\> Paste -\> Delete instead of Cut -\> Paste. Using the F8 Update would still be required for all other synchronization tasks. This would only work SCH-\>PCB because you are not able to adjust the Schematic UUID in the PCB Editor. Editor windows behavior: > Both SCH and PCB editors have to be opened at the same time. Closing KiCad will prompt the user to save both schematic and PCB. If they save both, re-open and performed an F8 update, the update would work as expected. If, however, they only saved one and not the other, the update using reference designator would still be required to re-synchronize the components. > > As long as KiCad is launched from the main KiCad window, the application will ensure that schematic and PCB editors are properly opened as needed. This is similar to how we check for schematic/PCB synchronization during DRC. Only cut+paste will preserve UUID linkage: > If users cut and paste to move their elements around, the board will be updated with the new UUID path and re-annotating will maintain their symbol-footprint links. If, however, they copy elements and paste them into a new sheet and then go back to delete the original symbols, the UUID path will not be updated. Then, if they re-annotate without first updating the board, all links between board and schematic will be lost. This happens because when elements are duplicated, they no longer have matches on the board. Only cut/paste maintains this. Projects with shared sheets: > In KiCad, a schematic sheet can be shared between multiple projects. The UUID update linkage will work only in the currently opened project. If some changes were done to a shared sheet, then PCB layout in the other projects will become broken. In other words, changing a shared sheet will require manually updating all other boards other than the one currently open. One \*.kicad_sch file linked as multiple sheets in the same project: > This would be handled in the same way as moving any set of symbols. There you will have multiple symbols with different reference designators moved to have a new UUID path. Each corresponding footprint would be updated on the board. Compatibility with Multichannel feature: > Multichannel will not impact this feature and this feature will not impact multichannel. Compatibility with scripts: > Scripts that modify the PCB file should have no effect except that if they change the symbol UUID information, we will lose sync. Editing this is not supported by the KiCad scripting system, so a script would need to directly edit a file while KiCad is closed to break this. --- Since keeping both editor windows open is crucial for correct operation, I also asked about some frills to make it more foolproof. Among them was (Eagle-like) forced auto-saving of SCH and PCB files at the same time, or (Eagle-like) warning popup when one editor is inadvertently closed. They would kick in only when the base feature was enabled. But mr. Hillbrand felt the existing KiCad functions explained above will be enough. I might yet sponsor their development later, based on user experience and popularity of the base feature. # KiCad Version <!--Copy version information (from main menu Help->About KiCad ->Copy Version Info) and paste it between the triple backticks below to preserve the formatting.--> ``` ``` ``` Application: KiCad x64 on x64 Version: 9.99.0-4097-g97dc4fa4bd, release build Libraries: wxWidgets 3.3 FreeType 2.13.3 HarfBuzz 12.2.0 FontConfig 2.15.0 Platform: Windows 10 (build 19045), 64-bit edition, 64 bit, Little endian, wxMSW wxWidgets: 3.3.0 (wchar_t,STL containers) Boost: 1.89.0 OCC: 7.9.2 Curl: 8.17.0-DEV ngspice: 45.2 Compiler: Visual C++ 1944 without C++ ABI KICAD_IPC_API=ON KICAD_USE_PCH=OFF Locale: Lang: en_GB Enc: UTF-8 Num: 1,234.5 Encoded кΩ丈: D0BACEA9E4B888 (sys), D0BACEA9E4B888 (utf8) ```