Stats

  • Locked Locked
  • Replies 10
  • Subscribers 166
  • Views 20597
  • 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

Duplicate the RefDes

PurdueMark
Board layout is finshed, just adding final touches to silkscreen, would like to to make a second copy of the refdes.  Example: 1st RefDes for an IC (DIP package) is dead center in the middle of the componant package (under the body of the IC) but a second RefDes is placed such that you can see it after the componant has been installed.  I used to do this all the time with Orcad Layout.  I can simply add text but this would not be associated with any symbol and therfore would not follow the componant if I moved it later in the design.  Is there a way to add a copy of the RefDes to nearly complete layout?    
  • Ron Scott
    Thanks for the replies. I'll get on this tomorrow morning.
  • Ron Scott
    What I have found in trying out both methods of duplicating text is Scott's method seems to be a universal change which might handy in some situations. Mike's method worked well with individual cases. The one common aspect is I was able to change text as I wanted but if I moved the part, it would immediately snap back to the original text. Does this occur in your experience and might there be a script out there to perform this function?
  • ScottCad

    Ron my idea is a universal one. Now I verified what you mentioned about moving a part and I see what you mean about the text block snapping back to it's original size. To change this default try the following.

    In the auto silkscreen dialog box check the following "Lock auto silk text for incremental updates" Believe that should get you where you need to be.

    Thanks Scott.

  • Ron Scott
    Scott, Took your latest suggestion and it works great! Thanks for your help. Now if I could get Mike to chime in and see if there is a similar fix to his method. Thanx, Ron
  • mcatramb91

    Sorry for the slow response.  I used my method across the board in 100s of locations so I wouldn't consider it a solution for individual cases only.  To get the properties values loaded quickly I generate an incremental 3rd Party Netlist to add the properties to all the components all at once.  I created a user defined property (Setup > Property Definitions...) so it doesn't get mixed up with other properties that may already have values assigned.

    Here is what the 3rd Party Netlist would look like:

    $PACKAGES
    $A_PROPERTIES
    TOP_SILK   "DC_IN"     ;  TP31
    BOT_SILK  "DC_OUT"  ;  TP900
    $END

    Use File > Import > Logic then select the Other tab to load the netlist above. (make sure that Supersede all logical data" is unchecked)

    You could also add this property to the schematic and pass it forward to the layout. (remember you would need to setup the tool to pass the user defined property forward)

    As far as moving a part which had the property value text changed reverting back to the original text, I don't see the text change in my method.  The only issue that I have is the text is not dynamic so if you change the property value it will not automatically update the text on the board so you have to go thru the property display process again or just rename the text.

    Hope this helps,
    Mike Catrambone
    Plexus Engineering Solutions

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.