Home > Community > Forums > PCB Design > Change a symbol, Orcad PCB Editor

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Change a symbol, Orcad PCB Editor 

Last post Mon, Apr 7 2008 3:31 PM by archive. 6 replies.
Started by archive 07 Apr 2008 03:31 PM. Topic has 6 replies and 3725 views
Page 1 of 1 (7 items)
Sort Posts:
  • Mon, Apr 7 2008 3:31 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    Change a symbol, Orcad PCB Editor Reply

    As a former Layout user, who has attended the Orcad PCB Editor class, I'm baffled why it's so hard to change a symbol within an existing design; for example, you decide that a 603 passive ought to be a 1206.

    I did update the symbol by deleting the part in Capture, netlisting, importing logic into Pcb Editor, puting back the same part with the different symbol into Capture, netlisting, and finally importing into Pcb Editor, but this seems like an overly complex thing to have to do.

    What is the preferred method?

    Thanks,
    Mike


    Originally posted in cdnusers.org by mmagargee
    • Post Points: 0
  • Wed, Apr 9 2008 1:07 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Change a symbol, Orcad PCB Editor Reply

    HI Mike, you might want to try exporting the netlist w properties, in here it contains the $PACKAGES in here you can just sub out the footprint name for the new one, then save and do an import Logic (other) this saves time on the schematic, however I think its best practice to use the schematic. and I would in most cases advise that.

    Stephen Grant-Davies (QuantumCad)
    www.quantumcad.co.uk


    Originally posted in cdnusers.org by stephen@quantumcad.co.uk
    • Post Points: 0
  • Wed, Apr 9 2008 2:58 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Change a symbol, Orcad PCB Editor Reply

    >I did update the symbol by deleting the part in Capture, netlisting, importing logic into Pcb Editor, puting back the same part with the different symbol into Capture, netlisting, and finally importing into Pcb Editor, but this seems like an overly complex thing to have to do.

    That seems a bit more than needed- maybe try, in Capture, right click the part, edit properties, change PCB Footprint, build netlist, switch to PCB Editor, import logic, place part. It's pretty quick?

    If you need to change, for example, all the 0603's to 1206's, then it's easier to open the .upd file, edit>replace the footprint name in the text editor, then in capture tools>update properties, build netlist... -Phil


    Originally posted in cdnusers.org by DEKTRON
    • Post Points: 0
  • Thu, Apr 10 2008 7:27 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Change a symbol, Orcad PCB Editor Reply

    Hi Mike u can try following. Use "Alternate Symbol" property in Capture. Give different package 0603,1206 for exapmple seperated by comma(or semicolon, just check it). When placing a component in PCB editor use pop up menu and select "Alt Symbol" which will give u your defined alternatives. Regards Ishant


    Originally posted in cdnusers.org by ishantdave
    • Post Points: 0
  • Thu, Apr 10 2008 1:36 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Change a symbol, Orcad PCB Editor Reply

    Hit the Select Component Tool, then click on the component. Right click, select Properties, then Footprint.  This brings up a dialog where you can graphicaly browse the footprints.

    Randy


    Originally posted in cdnusers.org by rdawson
    • Post Points: 0
  • Thu, Apr 10 2008 3:05 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Change a symbol, Orcad PCB Editor Reply

    Thank you for all of the replys. I believe that some of the problem was related to the location of my symbol directory. Placing these at the root (rather than C:\Profiles\My Documents and so on) made the search path work better when the padstack was matched up with the symbol. It then worked as I intended: loading a new footprint into an existing placed part without having to rip up that part.


    Originally posted in cdnusers.org by mmagargee
    • Post Points: 0
  • Mon, Apr 14 2008 11:13 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Change a symbol, Orcad PCB Editor Reply

    "My Documents" folder is not a great idea: allegro does not like space in file names, despite they try to handle it in new release.
    And pecial caracters (such ç ô à) are not welcome in directory name.


    Originally posted in cdnusers.org by jch teyssier
    • Post Points: 0
Page 1 of 1 (7 items)
Sort Posts:
Started by archive at 07 Apr 2008 03:31 PM. Topic has 6 replies.