Stats

  • Locked Locked
  • Replies 8
  • Subscribers 165
  • Views 26263
  • 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

Unable to import psm path

RCG Jon

Problem Statement:

I am not able to re-import all of my libraries I used in the 16.6 in the 17.2. I pointed to the original files and they didn't import then I pulled all the pad, psm, and dra files to a common directory. I added those locations to the paths, but the export and pcb library can't find these. I can pull other manually created symbols and components by placing them in the schematic and being pulled to the same board, but I couldn't pull the old 16.6 symbols.

I want to know how to incorporate the 16.6 into my 17.2 library and designs or libraries into my new design.

Here is the error:

W- (SPMHUT-127): Could not find padstack R_01910X01020R100_1.
E- Cannot load symbol 'CONNSMT_010_25530X02840_07540_1'
E- because WARNING(SPMHUT-127): Could not find padstack R_01910X01020R100_1.
due to ERROR(SPMHDB-273): Unable to load shape symbol R_01910X01020R100_1 (Check PSMPATH setting for this symbol).
With Padstack: WARNING(SPMHUT-48): Scaled value has been rounded off.
ERROR(SPMHDB-273): Unable to load shape symbol R_01910X01020R100_1 (Check PSMPATH setting for this symbol).
last pick: -282.66 3883.79

Here are my dra, psm and pad paths:

J:\cad_resources\dra

J:\cad_resources\psm

J:\cad_resources\pad

ROOT PROBLEM: the dra, psm, and pad were out of date and downreved on the dra and psm on 16.6 and the pad was 15.x.

SOLUTION THAT WORKED:The solution was using "DB Doctor" tool to update everything in my library it is an application that is installed with cadence and using *.psm *.dra and *.pad updated all of my options, I then reexported my schematic and was finally able to place my components.

REQUEST TO CADENCE: if there was a check to give an out of date or try db docoring (dra,psm,pad...) these I would have saved a couple days.

  • steve

    So the padstack has a shape symbol as part of it and PCB Editor cannot see that file. Make sure that any filename.dra and filename.ssm are available in your psmpath. Personally I tend to keep dra and associated ?sm (psm, bsm, ssm, fsm, osm) in the same folder. There's a guide to setup psmpath and padpath orcad.co.uk/.../Defining_padpath_psmpath.pdf

  • RCG Jon
    in reply to steve

    Thanks Steve I tried putting the dra, psm, and pad into the same folder perfectly flat, but after exporting it still puts an error and when placing the symbol in Allegro 17.2. Is there a file other than psm in a psm path, pad in a pad path?

  • steve
    in reply to RCG Jon

    As above "Personally I tend to keep dra and associated ?sm (psm, bsm, ssm, fsm, osm) in the same folder." check the spelling of the filenames carefully. This is usually the culprit. You may also want to try deleting the psmpath entries then re-adding them but only after you have enabled the Expand button. This can sometimes cause issues so only add paths after you have checked the Expand button.

  • mcatramb91

    A little late to the conversation here.  Reviewing the error messages, it looks like you are missing the Shape Symbol "R_01910X01020R100_1.SSM" that is being referenced in Padstack "R_01910X01020R100_1.PAD"

    Shape Symbol "R_01910X01020R100_1.SSM" should be available in folder specified in your PSMPATH.

    Hope this helps,
    Mike Catrambone

  • RCG Jon

    Sorry for the late responce I tried putting everything flat and it wasn't successful. I tried placing some resistors too and it was showing errors with it and this time the error was 

    E- because WARNING(SPMHUT-127): Could not find padstack S_00508X00508R05_1.
    With Padstack: ERROR(SPMHDB-181): Design revision 15.x is too old. Must run the batch dbdoctor to uprev.

    So I checked the pad stack I was pointing to and ran DBDoctor

    "You have to go to the Start>Programs>cadence SPB 16.2> PCB Editor Utilities>DB Doctor select the board or library files and run update."mashak from post https://www.edaboard.com/showthread.php?127597-Allegro-PCB-Editor-and-OrCAD-PCB-Editor

    I will update it. It looks like it might take a few days.

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.