• Skip to main content
  • Skip to search
  • Skip to footer
Cadence Home
  • This search text may be transcribed, used, stored, or accessed by our third-party service providers per our Cookie Policy and Privacy Policy.

  1. Community Forums
  2. PCB Design
  3. Gnd picking up another name gnd_324535 on different pages...

Stats

  • Locked Locked
  • Replies 3
  • Subscribers 165
  • Views 16780
  • 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

Gnd picking up another name gnd_324535 on different pages.

TamiWright
TamiWright over 13 years ago
Gnd symbols picking up another name (gnd_324535) on different pages they are sapose to be the same name. Why!
  • Cancel
  • redwire
    redwire over 13 years ago

     Let me ask you a question and see if you can figure this out.  What if the net were called "ABC" instead of "GND".   Does it matter?

    Read on for the answer....

     

     

     

     

     

     

     

     

    OrCAD does not "know" what "GND" means.  If you mean to have a power/gnd net then use the appropriate Power/Ground symbol and name the net "GND".  This will give the net a global definition.  Then OrCAD will connect it everywhere.  If you wire a signal net up and name it "GND" then OrCAD will differentiate this from the global net and call it "GND_xxxxxx".  The same thing happens if you have a signal net that is local between two parts and you do not use an off-page connector.

     

    So in your case, use a global power/ground symbol or use an off-page connector to make sure OrCAD connects the "GND" net correctly.

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • TH Designs
    TH Designs over 13 years ago

    I have seen this before. Eventhough you use the same ground symbol on each sheet, Orcad is interpreting this as you want two different grounds and appends the "_12345" to the net name to differentiate them from one another.

    If you want the grounds tied together, use an off page connector. Call it GND and tie it directly to the local sheet GND symbol. I do this on all of my multisheet schematics, not only with GND, but power connections also.

     I have also seen this happen when combining sections of different schematics together to generate a new schematic. I have had the same gnd symbol called GND and GND_POWER. Eventhough they look the same they are different nets and won't connect until you verify that all of the symbols have the correct net name associated with them. Easy to do using the spreadsheet.

    One of the many reasons I always check the net names and verify that I only have the power and gnd nets I expect to have.

    Tom

    Tom

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • steve
    steve over 13 years ago

    One comment - If you just use the Global power signals and don't connect them to an offpage connector or a hierarchical port then the signals will remain global. If you connect them to hierarhical ports then you take responsibilty of where it connects and then you get GND_12345 etc.

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
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.

© 2025 Cadence Design Systems, Inc. All Rights Reserved.

  • Terms of Use
  • Privacy
  • Cookie Policy
  • US Trademarks
  • Do Not Sell or Share My Personal Information