Stats

  • Locked Locked
  • Replies 8
  • Subscribers 166
  • Views 25139
  • 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ROOT PROBLEM: the dra, psm, and pad were out of date and downreved on the dra and psm on 16.6 and the pad was 15.x.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REQUEST TO CADENCE: if there was a check to give an out of date or try db docoring (dra,psm,pad...)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.

Parents
  • 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.

  • steve
    in reply to RCG Jon

    You can use wildcards in dbdoctor so try browsing for a padstack (filename.pad) then edit it to say <pathtopads>\*.pad which will do this as a batch on all padstacks. Repeat for *.dra. That should seed things up.

  • RCG Jon
    in reply to steve

    I did the update on Friday and over the weekend it looks like it did fix some things in the library. I now get a new error message. I checked the DRA

    E- (SPMHGE-626): Symbol RES0805_002_0180X0140_0050_1 is not valid on any layer. Check symbol and layer embedding requirements to ensure they match.

    I opened up the RES0805_002_0180X0140_0050_1.DRA and I didn't see any issue it had a top and bottom, I will start checking each layer.

    Is there any other tool for an automated fixer?

  • RCG Jon
    in reply to RCG Jon

    I did the update to the pad stacks too and I am able to place everything in the library. thank you all for all your help.

Reply
  • RCG Jon
    in reply to RCG Jon

    I did the update to the pad stacks too and I am able to place everything in the library. thank you all for all your help.

Children
No Data
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.