How to Un-Manage a Managed Project? - Altium Discussion Forums
Thank you Ted !
For a schematic document:
1. Create a new blank schematic library and blank PCB library (File»New»Library»Schematic Library/PCB Library).2. Open an existing schematic in your project and create a new schematic library from the placed parts. (Design»Make Schematic Library).
3. In the temporary library just created in the previous step, open the library panel and copy all symbols into your library created in step 2(This will remove the vault link). http://techdocs.altium.com/display/ADOH/Creating+Library+Components+Tutorial#CreatingLibraryComponentsTutorial-CopyingComponentsfromOtherLibraries
4. Save the Schematic Library.
5. In the PCB document, create a new PCB Library. (Design»Make PCB Library)
6. Copy the footprint from the temporary project library(using the PCB library panel) into your library.
7. Save your PCB library.
8. In one of your schematic documents, open the SCH List.
9. Set filter to Edit, All Objects, from Open Documents of the Same Project, and to include only Parts.
10. Select all Part entries, and change the Library column to the name of your newly saved Schematic library.
11. Execute Tools -> Update From Libraries.
12. Set proper settings in the configuration window, then click Finish.
13. Execute ECO.
For a PCB document:
The following requires the attached script to be used.
1. Unzip the attached file
2. Open the script Project (*.PrjScr) file in Altium Designer
3. Open the PCB (*.PcbDoc) that needs to be updated
4. Select the components that need to be updated, or Ctrl + A for all
5. From the menu, select: DXP » Run Script...
6. Select the replace_library_paths_ckbox script, click OK
7. In the script dialog, check boxes for the fields to overwrite
8. Type in the text to place in those fields. The PCB Library field should be set to the name of the new PCB Library (*.PcbLib) file
9. Click the button: Update Comps
10. Close the dialog. The path and information have now been updated
This will unlink the components in both schematic and PCB documents from the above procedure.
My 2 Cents
All the above reminds me that it might be a good idea to have an Escape Plan.
That's it !
