Altium - Back-Annotation Error

Question

I have re-annotated PCBs and back-annotated the schematics countless times before and never saw this problem.

I first make sure that my PCB and my schematic are synchronized and up-to-date. In the PCB I go to Tools -> Re-Annotate. I select my direction, set my comparison threshold, etc and click "OK". The board re-annotates as expected. I save the board and the project. However, once I go back into my schematic and click Tools -> Annotation -> Back Annotate Schematics and select the .WAS file that was just generated, I get the following error:

There are only 294 components in the design. I cannot seem to track down the cause or solution to this problem. What might the issue be?

Once again, I am using the same process I always use and it has always worked in the past. I have even tried resetting all component designators in the schematic, annotating the PCB, and back-annotating to the schematic but that does not work either.

I am using Altium 17.1.5.

Answer 1

Go figure, I struggle with this for two hours and as soon as I finally post the question I manage to figure it out.

Apparently in one of Altium's latest updates either the functionality changed or a setting was changed. For some reason I am not able to update schematic designators unless their respective components are selected. In the case of the above problem only a few of the schematic designators were selected when I attempted the back-annotation, so to the annotation tool the number of components on the PCB that were re-annotated and the number of components selected in the schematic did not match. I had to select all of the components in the schematic in order to perform back-annotation.

Seems a bit ridiculous to me, so if anyone knows if there is a setting to change this, please let me know. Regardless, the solution mentioned above worked for me.

Answer 2

I always used back annotate and it seems that sometimes the .WAS file doesn't include all the changes, especially if you do multiple PCB re-annotations it seems to me that the .WAS file only include incremental changes which can cause problems later on.

anyway, here is a simple method which I wonder why haven't I been using it from the first time.

1. Ensure that there is no broken link between components in schematic and PCB by going to PCB->Project->Component Links, the unmatched component section should be empty
2. Re-annotate the PCB PCB->Design->Re-Annotate
3. Push the changes back to schematic PCB->Design->Update Schematics in project.PrjPcb
4. From the schematic do a compile and then do a Design->Update PCB Document to update and fix the net names and other changes and pushes them back to PCB