Stats

  • Locked Locked
  • Replies 9
  • Subscribers 166
  • Views 18624
  • 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

Help with how to transfer a user defined property in orcad capture to PCB editor

JasonW

I have test points in capture where I want to display a specific name on the board.  For example, lets say for TP1, I want a silkscreen name called MasterSupply to show up on the board instead of TP1.  At first I thought I'd just rename the refdes from TP1 to MasterSupply in capture.  Unfortunately when I annotate it changes it to MasterSupply1.  I couldn't figure out how to stop it from annotating that particular part easily so I thought I'd create a user property called SSNAME (silk screen name) and import that property into PCB editor.

 I've read through some of the documentation on how to bring in user defined properties, such as opening up the contraint manager and adding a new column called SSNAME in the component properties with a string property.  Now I thought that's all I needed, but when I netlist the board into PCB editor, the SSNAME value does not transfer.

 What am I missing?

 

Thanks,

Jason

  • BillZ

    Hi,

    You could use one of the default lables for this. For example add a place Holder in the Testpoint footprint for Value on Silkscreen top. Then put your Mastersupply as the value in Capture. It should netlist over and all you have to is enable this layer in your silk screen.

    Don't add a placeholder for the testpoint on ref des silkscreen top.

    Give it a try. You could use partnumber or device the same way.

    Regards,

    BillZ

    EMA Design Automation 

  • redwire

     Hi,
    I recently posted the same question and got the answer needed here: http://www.cadence.com/community/forums/T/10494.aspx

    It appears you have good working knowledge of how to pass the value across to Allegro but don't know how to make it show up.

    If in the schematic, you attach "SSNAME" of "MasterSupply" and have SSNAME=yes in the allegro.cfg under components, then it will attach to component in Allegro but it won't display.  Do "display->property" and map it to some layer on the symbol.


    HTH,
    Bill (not Z) :)

  • John Davies
    Is it possible to use this technique to display the name of a pin as well as its number? For example, ebc as well as 123 for a bipolar transistor? (Useful for students.) The name of each pin is in the pstchip.dat netlist created by Capture but I can't find it listed as a property in PCB Editor.
  • tltoth

    Hi John,

    Yes it is.  First, we should check the "Allow user defined property" in, in the check box of Create Netlist to transfer our data through netlist. Second, in the "Setup"  within Create netlist we should edit the "allegro,cfg" file and add the following line below [ComponentDefinitionProps]
    SSNAME=YES.

    Obviously all this is done when we already have our SSNAME property set in Capture.

    In the PCB Editor we can use Display>Property.  To find our newly created property just click on Find and look for "user defined"

    Regards, Lajos

  • redwire

     John,

    One way to do that is to have each transistor pin order as a unique component and display the EBC, BCE, CEB, etc... based on which variant is selected.  If you are using CIS you can eliminate a lot of guesswork and make it very user friendly.

     

    Bill 

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.