Stats

  • Locked Locked
  • Replies 4
  • Subscribers 165
  • Views 15551
  • 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

Capture to PCB editor

JBmtk

Hello,

 I have a schematic finished in Capture, and I am able to produce a netlist. However, in PCB editor, I am unable to load in the parts:

 

#39  WARNING(SPMHNI-316): Property warning detected.

WARNING(SPMHNI-301): Problems with component 'C1'. Error with component property '' and value 'VOLTAGE': 'CMAX'

#13  WARNING(SPMHNI-192): Device/Symbol check warning detected.

WARNING(SPMHNI-194): Symbol 'VRES10' for device 'POT_VRES10_1K' not found in PSMPATH or must be "dbdoctor"ed.

 Also, is there an easier way of adding generic footprints? In Orcad Layout I remember being able to easily add in default footprints. In Capture I resort to simply putting in something like "dip2". 

  • steve

     

    The warning is saying that it cannot find a footprint part VRES10. Under setup - user preferences - paths - library define your padpath and psmpath to point to where your pcb footprints and pads are stored. Make sure you have a footprint (symbol) called vres10.dra and vres10.psm here.

    Store all your footprints in this defined directory. Unfortunately there is no Library Manager as there was in Layout.

  • HANUMAGOUDA
    hi, for first warning , choose the capacitor which is having polarity that is c/ANALOG_P instead of c/ANALOG
  • techworks

     Steve,

       Thanks for that response ...I think I am starting to see the links in the chain now ?  Are you saying that if I set my pcb footprint value in the property edits table (for a symbol on a CAPTURE schematic) to the name of a footprint symbol called  xxx.dra  and xxx.psm and also ...set the padpath and psmpath to where they are stored  , then PCB Editor will associate the schematic netlist with this footprint ??

    (ORCAD 10 and Layout was so much easier to understand )

  • redwire

     Pads are stored wherever you want; Symbols are stored wherever you want.  padpath points to pads only; psmpath points to symbols.

    The netlister looks for parts in psmpath.  When placing, Allegro caches the pad from padpath.

    Your netlist in Capture will refer to the psm filename only.  ".dra" are only used to create the ".psm" and do NOT have to be in the same paths.

    Watch your use of "VOLTAGE" for passives -- Allegro does not use this property for a rating.  Create a new property such as "VOLTAGE_RATING" instead.

    VOLTAGE is used on nets to assign a DC voltage level for further analysis only.

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.