Stats

  • Replies 4
  • Subscribers 160
  • Views 11637
  • Members are here 0
More Content

How to correctly perform new annotation between revisions

thomasli

Hi

I have inherited a schematic where Revision A has already been produced. The schematic is in less than ideal shape, e.g.  RefDes control was only partly enabled. So some pages have correctly assigned designators for parts, others don't. Also, I'll need to add another schematic page somewhere in the middle.

Now when I enable RefDes control and perform an unconditional annotation, OrCAD will remind me that the netlist has already been generated and the physical design might get out of sync. Since approx. 90% of the PCB stays the same I want to keep the changes for the PCB Designes as little as possible.

If I perform this annotation, will this bring over the changes to designators or will they have to be re-assigned in the PCB as well?

First tests showed the following behaviour:

* Performing an additional annotation for the added parts went ok. Very few changes to the PCB, probably about those that were expected.

* Re-Annotating the whole design shifted many parts all around, e.g. U400 is now where U500 was but is a different footprint. 

  • Alright, Ithink I can answer this on my own after a few hours of trying.

    Do a re-annotation with designators which do not already exist, eg. U10000+, create a netlist, import the netlist, do another re-annotation with the designators you actually want (e.g. U100), create a netlist, import the netlist, done.

    No need for back-annotation or similar. It's important to no re-use any designators during any of both re-annotations

  • If your schematic and board are in-sync when you start, then all new parts you add will skip over any existing reference designators.

    Let's say you want to clean up the order of the parts of just the new parts in Allegro and back annotate to OrCAD.  Easy.

    1)  Add parts to schematic, annotate, and import to Allegro

    2) Edit->Properties->Components (in Allegro). Select "Temp Group".  Select the pages in OrCAD which will grab the parts in Allegro.  Once all the new pages have been selected, choose "Done".  This will close the temp group.

    3) Add property "Auto_Rename" which will default to "TRUE". OK the Edit Property window

    4) Choose "done" then go to Logic->Auto Rename Ref Des", choose "Setup" and set up what you want to do (Right to Left, Top to Bot for example).  Then OK, then choose "Rename".  Allegro will resequence only the parts to which you added the "Auto_Rename" property".   It will start with the next available refdes or if you use "set fst_ref_des xxx" where "xxx" is the value you want it will start with that.

    5) Save board.  Back annotate in OrCAD.

    You might want to practice this a couple of times as this is the old-school method but it works flawlessly.  First-timers might not follow all the instructions and get tripped up.  Hope it works.

  • in reply to redwire

    Hi

    If I understand you correctly, this is how to perform a re-annotation on PCB Level and then transfer that back to Schematic Capture. My question was pointed to do it the other way round (Full re-annotation in OrCAD, then transfer that to PCB without having to re-do the whole layout).

    In any case, thanks for the response, this might come in handy another time :-)

  • in reply to thomasli

    Yes, you are right.  The typical flow is via backannotion since it risks tear-up in the forward mode.  Glad you came up with a way that works for you.

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.