Actions
Forum Thread Details
  • State Verified Answer
  • Locked Locked
  • Replies 8 replies
  • Answers 2 answers
  • Subscribers 91 subscribers
  • Views 1987 views
  • Users 0 members are here
Related
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Back Annotation Broken

r.gibson

I am trying to re-annotate the PCB and then push the re-annotated reference designators back to the schematic. Unfortunately, every time I try, Altium breaks all sorts of links and then asks me to try to match the unmatched nets without offering any ability to cross probe or zoom to the net location either on the schematic or on the PCB...horribly frustrating. I've had to manually revert to an older saved file several times now because it's so messed up. Has anyone else had luck with this? Maybe I'm just doing something wrong, but I don't think so...this should be a really easy process and it's NOT!

Parents
  • 0

    Hi Ryan, sorry to hear of the frustrations with back annotation. Before starting to rename components on the PCB did the designs match? Things to check are that the component instances align between PCB and schematic (PCB editor: Tools | Component Links) and the netlists match (Schematic editor: Home | Projects > Update PCB Document). Also be aware that back annotation does not work if using repeated design blocks. If you cannot get back annotation working then feel free to reach out to me (a private message or email software@element14.com) and if you can supply a copy of your design I will take a look.

  • 0 in reply to e14softwareuk

    I verified that the links and netlists match...that was the first thing I tried. I'm not using any repeated design blocks.

    I just sent my project package to your Farnell account...hopefully you can figure out why it's not working...

  • 0 in reply to r.gibson

    Maybe you are doing this already but....

     

    After doing the back-annotate operation the schematic symbols should have two designators, with the greyed out one being the old designator.

    It is important to recompile the project at that point before doing anything else.

     

    After the recompile your schematic net names will change (since auto net names are based upon component designators), so you must pull those net name changes into the PCB (Project > Import Changes)

  • 0 in reply to voltsandjolts

    That is a lot of steps for something that should be much simpler...however what you say does make sense. I will try your suggestions this evening and see if that is the problem. If that is the case, it would be nice if Altium could be a little smarter and handle the net renaming automatically...since one of the main advantages that Altium has over it's competitors is the integration between Schematic and PCB software tools.

  • 0 in reply to r.gibson

    Just to confirm Kevin's answer, a two step process is required after updating the designators on the PCB.

    1. PCB editor - run Home | Project > Update Schematics
      This updates the designators on the schematic sheets
    2. SCH editor - run Home | Project > Update PCB Document
      This updates net names and net classes back to the PCB
Reply
  • 0 in reply to r.gibson

    Just to confirm Kevin's answer, a two step process is required after updating the designators on the PCB.

    1. PCB editor - run Home | Project > Update Schematics
      This updates the designators on the schematic sheets
    2. SCH editor - run Home | Project > Update PCB Document
      This updates net names and net classes back to the PCB
Children