Stats

  • State Not Answered
  • Replies 7
  • Subscribers 48
  • Views 25270
  • Members are here 0
More Content

Preferred Method to Indicate Non-Populated Components

David Yackman

What is the preferred method for indicating components that aren't populated in OrCAD Capture 16.6?  Do I just simply add text next to the schematic symbol that says "Do Not Populate", or is there something in the property editor that I can add or change so that the component shows that it shouldn't be populated when I generate the BOM? 

 I can manually make the changes to the bill of materials as well as the schematic, I was just wondering if there was some feature of OrCAD that could handle this for me.

  • 0

    I usually just put OPEN in the part value. When you run the BOM you will have all of the unpopulated part references listed under OPEN.

    I have another customer that likes to have a dashed box put around the part with DNI insode the box. This maintains the part value on the schematic, but you can't tell it is a "Do Not Install" when you run the BOM.

    Tom

  • 0

    Ah.  OK, thanks, Tom.  Well, I made a few copies of the DSN file, labeled the components that aren't populated with DNP (Do Not Populate), and then made copies of the BOM and made the changes to the individual BOMs.

    I was thinking that there might have been a more streamlined way to do this in OrCAD. If anybody has any more suggestions or methods for doing this, let me know.

  • 0
    The "streamlined" approach is to use the CIS Option, it supports BOM Variants, you have a "core design" of "everything" and the BOM Variants where parts are the same as the core design, not fitted, or fitted with a different value from the core design - the CIS reporting supports the generation of BOM reports for the variants.
  • 0

    I use a slighty more cumbersome system but it supports certain MIL requirements I have had to comply with in the past.

    I add a delta note (or flag note or whatever you want to call it) that states: INDICATED COMPONENTS NOT INSTALLED.   I then place the delta note call-out next to each component not to be installed.  I work with some engineers who want this flexibility in their designs and this seems to satisfy both the engineering and manufacturing sides of the various companies I have worked for.  The down side is that you do have to manually remove the components from the BOM to start with.  The up side is that it is just simple editing of the note text on the schematic and updating the BOM via am ECN.

  • 0

    My KISS method:

    Add a feild called note

    In the "Note" feild place the text DNP.

    Display the value only of the note feild

    Add this feild to the BOM output.

     

    Results:

    Move part, the DNP follows the part.  In a Hierachical drawing, you can populate or blank this feild out per occerance....

     

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.