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:

enter image description here

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.


2 Answers 2


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.


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

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.