KB: Different Schematic Designators After Board Level Annotation

Solution Details

Identify Logical and Compiled Designator Differences

When a project is compiled, a schematic document provides an Editor view containing the logical component designators and a Compiled view containing the physical designators of the compiled components.

Normally, these designators can be identical. However, different logical and physical designators are not necessarily an error. They can occur when Board Level Annotation or multi-channel annotation is used, or when a physical designator has been changed through Graphical Designator Editing.

Understand Why Physical Designators Can Differ

Board Level Annotation operates on the compiled, physical component view of the design. It is particularly useful for multi-channel designs and designs that contain Device Sheets because compiled components can be assigned appropriate physical designators without changing the original logical components on the source schematic sheets.

In a multi-channel design, the logical source remains unchanged while compilation expands repeated circuitry into the physical component instances used by the design. This allows logical and compiled component designators to differ intentionally.

When Board Level Annotation is used, its annotation changes are stored in a project-specific *.Annotation text file. Values assigned through the Board Level Annotate dialog or Graphical Designator Editing can therefore differ from the logical designators shown in the Editor view. The compiled physical designators are the values transferred to the PCB.

This differs from Schematic Level Annotation, which operates on the logical view of the design. As a result, changing or reviewing only the logical schematic designators might not resolve a mismatch caused by Board Level Annotation.

Determine Whether Annotation Should Be Removed

Before removing the .Annotation file, determine whether the different physical designators are intentional. Board Level Annotation can be used deliberately to manage compiled component naming, including resolving duplicate designators in designs that use repeated channels or Device Sheets.

If Board Level Annotation was applied accidentally or is no longer wanted, remove the project's .Annotation file. The file must be deleted from disk, and its missing document reference must then be removed from the project because the Projects panel represents the project's logical document structure rather than simply mirroring files stored on disk.

Remove the Unwanted Annotation File Manually

1. Open the project directory. In Altium Designer, right-click the top-level .PrjPcb project file and select Explore. This opens the project folder in Windows Explorer.
2. Close the project. Close the project in Altium Designer, or close Altium Designer entirely.
3. Delete the annotation file. In Windows Explorer, locate the file that has the same name as the project and the .Annotation extension, then delete it.
4. Reopen the project. Return to Altium Designer and reopen the project. Altium Designer reports that the deleted file cannot be found and marks it as missing.
5. Remove the missing document. Remove the missing .Annotation document reference from the project. Refer to the Managing Project Documents documentation for instructions on managing missing documents.
6. Save the project. Save the project to finalize the changes.

Additional Notes

After removing unwanted Board Level Annotation, the Editor and Compiled views should display identical annotation values when no other feature, such as multi-channel annotation, intentionally produces different logical and physical designators. The deleted .Annotation file should also no longer be referenced by the project.

References

• Board Level Annotation
• Graphical Parameter Editing
• Managing Missing Documents
• Annotating the Components in a Design
• Creating a Multi-channel Design