Stats

  • Locked Locked
  • Replies 5
  • Subscribers 165
  • Views 14940
  • Members are here 0
More Content
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

Problem Updating Component in PCB Editor

ace5582

 I'm using Orcad PCB Editor v16.2. I started a PCB design, imported a netlist from Capture CIS, and placed all of my components. I then changed one of the components (modified it's DFA and Place boundaries). I assumed it would be easy to update my design with this change...

 1) I deleted the old component and placed it as a "components by refdes" component again. The component didn't update.

 2 )I then went to the Advanced Settings tab in the Placement window, enabled the "Library" option under the "List construction" setting. I tried to place the component under the "Package Symbol" dropdown menu. Still no change...

 3) In the main menu bar I went to Place > Update Symbols. I clicked on "Package Symbols". I then clicked on the component I wanted to update. I enabled the "Update symbol padstacks",  "Reset symbol text locations", "ignore FIXED property" options and clicked on "refresh". The log showed the component updated.

 4) Looking back at the design the component didn't update. I tried steps 1 & 2 and still no update.

 5) I can create a new board design and place the component. and it is an updated version.

 6) One other thought: the refdes text block size for that component doesn't match the one it's supposed to have either...

 

Any thoughts on what I'm doing wrong or why it's not working?

 

Thanks in advance!

 

 

 

  •  Have you tried dbdoctor  (Tools >Database Check) on the design and then execute Update Symbols?

  •  I just tried your suggestion and no fix.

  •  Hi ace--the procedure is simple.  Deleting and replacing doesn't fix it as you found out.

    Only during place-update symbols does it work. But, where does it get its symbols?  First occurrence found in your psm path.

    Sounds like you have rogue copies floating around in other directories.


    Do a symbol library path report and see where it's getting the current symbol from.

  •  Thanks redwire, your suggestion fixed the problem. For some reason Orcad was using the symbol from the same directory the PCB design is in, but that directory is not in the psm path. I deleted that symbol and re-ran symbol update and problem solved.

     

    Thanks again.

  •  I wonder if "." is hiding in the PSMPATH from you as it's typically part of the default install.

    One way you can see your real path is type in "set" at the Allegro command line.

    Scroll down and look for psmpath and see if "." is in the definition.  If you don't want it there (most installs have it) then you need to modify with  Setup->User Preferences and be sure to look at the expanded view

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.