KB: Multiple/different designators in schematic

Solution Details

When the Board Level Annotation command is invoked in a schematic document, a special file with the project name and an .Annotation extension is created in the project directory. This file affects how designators are displayed and managed. There is no automated method to remove this file. This article explains how to manually remove it from your project.

Altium Designer uses dynamic compilation to create and manage a unified data model of the project's components and their connectivity. This data model can then be used to propagate design changes between the design domains – for example, synchronizing to resolve differences between documents in the Schematic and PCB domains.

When a project is compiled, each schematic page will have at least two tabs at the bottom:

• The first tab is the Editor tab. This has the logical designators of the components.
• The second tab is the Compiled tab, which contains the physical designators of the components.
  

Normally, the designator values in both tabs are identical unless multi-channel annotation is applied or the component’s physical designator has been modified directly in the compiled document view using Graphical Designator Editing.

If an .Annotation file has been added to the project, any values assigned through the Board Level Annotation dialog or by using Graphical Designator Editing will override the designator values in the Editor tab, and the compiled designators will be transferred to the PCB document.

If you did not intend to use Board Level Annotation, the .Annotation file must be manually deleted. Follow these steps to remove the annotation file from your project:

1. Open the Project Directory
   In Altium Designer, right-click the PrjPcb file (the top-level project file) and select Explore. This will open the project folder in Windows Explorer.
2. Close the Project
   In Altium Designer, close the project (or close Altium Designer entirely).
3. Delete the Annotation File
   Switch back to Windows Explorer and locate the file with the same name as your project and the .Annotation extension. Delete this file.
4. Reopen the Project
   Return to Altium Designer and reopen the project. You will receive an error the the fille could not be found and that is has been marked as missing
5. Remove the missing file from the project. For detailed instructions, see Managing Missing Documents
6. Save the Project
   Save the project to finalize the changes.

At this point, the Editor and Compiled tabs should display identical annotation values, and the .Annotation file will no longer be referenced.

For more information on Board Level Annotation, please refer to our online documentation:

• Board Level Annotation