Home > Community > Forums > PCB Design > Orcad to PCB Editor error during Create Netlist

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Orcad to PCB Editor error during Create Netlist 

Last post Sat, Jun 4 2011 9:39 AM by redwire. 7 replies.
Started by archive 15 Nov 2006 07:50 PM. Topic has 7 replies and 5315 views
Page 1 of 1 (8 items)
Sort Posts:
  • Wed, Nov 15 2006 7:50 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    Orcad to PCB Editor error during Create Netlist Reply

    I obtain the following session log error when i tried to create netlist from Orcad Capture to be used by PCB Editor for layout. Kindly help. It seem to be due to naming conflict of component.

    Is there a way to prevent the default naming component of Orcad to cascade during netlist creation?

    many thanks

    ********************************************************************************
    *
    * Netlisting the design
    *
    ********************************************************************************
    Design Name:
    Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\attocycler.dsn
    Netlist Directory:
    Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro
    Configuration File:
    C:\OrCAD\OrCAD_15.7\tools\capture\allegro.cfg

    Spawning... "C:\OrCAD\OrCAD_15.7\tools\capture\pstswp.exe" -pst -d "Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\attocycler.dsn" -n "Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro" -c "C:\OrCAD\OrCAD_15.7\tools\capture\allegro.cfg" -v 3 -j "PCB Footprint"
    Scanning netlist files ...
    Loading... Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro/pstchip.dat
    Loading... Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro/pstchip.dat
    Loading... Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro/pstxprt.dat
    Loading... Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro/pstxnet.dat
    packaging the design view...

    Exiting... "C:\OrCAD\OrCAD_15.7\tools\capture\pstswp.exe" -pst -d "Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\attocycler.dsn" -n "Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro" -c "C:\OrCAD\OrCAD_15.7\tools\capture\allegro.cfg" -v 3 -j "PCB Footprint"


    *** Done ***

    ********************************************************************************
    *
    * Updating Allegro PCB Editor Board
    *
    ********************************************************************************
    Netlist Directory:
    Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro
    Input Allegro Board:
    Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd
    Output Allegro Board:
    Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd

    Spawning... netrev.exe -5     -y 1 -n   -i "Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro" "Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd" "Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd"
    Reading File : Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstchip.dat
    (00:00:00.01)
    Reading File : Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstxprt.dat
    (00:00:00.00)
    Reading File : Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstxnet.dat
    (00:00:00.01)
    Starting to process component instances

    netrev run on Nov 16 11:20:54 2006
       DESIGN NAME : 'ATTOCYCLER'
       PACKAGING ON May 28 2006 22:05:31


      8 errors detected
     No oversight detected
     No warning detected

    cpu time      0:00:18
    elapsed time  0:00:00


    Exiting... netrev.exe -5     -y 1 -n   -i "Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro" "Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd" "Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd"
    Cadence Design Systems, Inc. netrev 15.7 Thu Nov 16 11:20:54 2006
    (C) Copyright 2002 Cadence Design Systems, Inc.

    ------ Directives ------

    RIPUP_ETCH FALSE;
    RIPUP_SYMBOLS ALWAYS;
    MISSING SYMBOL AS ERROR FALSE;
    SCHEMATIC_DIRECTORY 'Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro';
    BOARD_DIRECTORY 'Z:/Attogenix/Projects/Attocycler v2.0/Hardware/PCB/Cadence/Orcad/allegro';
    OLD_BOARD_NAME 'Z:/Attogenix/Projects/Attocycler v2.0/Hardware/PCB/Cadence/Orcad/allegro/attocycler.brd';
    NEW_BOARD_NAME 'Z:/Attogenix/Projects/Attocycler v2.0/Hardware/PCB/Cadence/Orcad/allegro/attocycler.brd';

    CmdLine: netrev.exe -5 -y 1 -n -i Z:\ATTOGENIX\PROJECTS\ATTOCYCLER V2.0\HARDWARE\PCB\CADENCE\ORCAD\allegro Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd

    ------ Preparing to read pst files ------

    Starting to read Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstchip.dat
       Finished reading Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstchip.dat (00:00:00.01)
    Starting to read Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstxprt.dat
       Finished reading Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstxprt.dat (00:00:00.00)
    Starting to read Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstxnet.dat
       Finished reading Z:/ATTOGENIX/PROJECTS/ATTOCYCLER V2.0/HARDWARE/PCB/CADENCE/ORCAD/allegro/pstxnet.dat (00:00:00.01)

    ------ Oversights/Warnings/Errors ------


    #1   ERROR(302) Device library error detected.

    Problems with device 'R_AX/RC05_15K'. JEDEC_TYPE property 'AX/RC05' is illegal: 'Package name has invalid characters or is too long.'.

    Device 'R_AX/RC05_15K' has library errors. Unable to transfer to Allegro.

    #2   ERROR(302) Device library error detected.

    Problems with device 'R_AX/RC05_45K'. JEDEC_TYPE property 'AX/RC05' is illegal: 'Package name has invalid characters or is too long.'.

    Device 'R_AX/RC05_45K' has library errors. Unable to transfer to Allegro.

    #3   ERROR(302) Device library error detected.

    Problems with device 'R_AX/RC05_22K'. JEDEC_TYPE property 'AX/RC05' is illegal: 'Package name has invalid characters or is too long.'.

    Device 'R_AX/RC05_22K' has library errors. Unable to transfer to Allegro.

    #4   ERROR(302) Device library error detected.

    Problems with device 'R_AX/RC05_10K'. JEDEC_TYPE property 'AX/RC05' is illegal: 'Package name has invalid characters or is too long.'.

    Device 'R_AX/RC05_10K' has library errors. Unable to transfer to Allegro.

    #5   ERROR(302) Device library error detected.

    Problems with device 'C_RAD/CK05_470N'. JEDEC_TYPE property 'RAD/CK05' is illegal: 'Package name has invalid characters or is too long.'.

    Device 'C_RAD/CK05_470N' has library errors. Unable to transfer to Allegro.

    #6   ERROR(302) Device library error detected.

    Problems with device 'C_RAD/CK05_100N'. JEDEC_TYPE property 'RAD/CK05' is illegal: 'Package name has invalid characters or is too long.'.

    Device 'C_RAD/CK05_100N' has library errors. Unable to transfer to Allegro.

    #7   ERROR(302) Device library error detected.

    Problems with device 'C_RAD/CK05_150N'. JEDEC_TYPE property 'RAD/CK05' is illegal: 'Package name has invalid characters or is too long.'.

    Device 'C_RAD/CK05_150N' has library errors. Unable to transfer to Allegro.

    ------ Summary Statistics ------


    #8   ERROR(102) Run stopped because errors were detected

    netrev run on Nov 16 11:20:54 2006
       DESIGN NAME : 'ATTOCYCLER'
       PACKAGING ON May 28 2006 22:05:31

       COMPILE 'logic'
       CHECK_PIN_NAMES OFF
       CROSS_REFERENCE OFF
       FEEDBACK OFF
       INCREMENTAL OFF
       INTERFACE_TYPE PHYSICAL
       MAX_ERRORS 500
       MERGE_MINIMUM 5
       NET_NAME_CHARS '#%&()*+-./:=>?@[]^_`|'
       NET_NAME_LENGTH 24
       OVERSIGHTS ON
       REPLACE_CHECK OFF
       SINGLE_NODE_NETS ON
       SPLIT_MINIMUM 0
       SUPPRESS   20
       WARNINGS ON

      8 errors detected
     No oversight detected
     No warning detected

    cpu time      0:@Ú
    00:18
    elapsed time  0:00:00



    *** Done ***

    ********************************************************************************
    *
    * Spawing Allegro PCB Editor
    *
    ********************************************************************************
    Spawing "C:\OrCAD\OrCAD_15.7\tools\pcb\bin\allegro.exe" -mpssession Administrator "Z:\Attogenix\Projects\Attocycler v2.0\Hardware\PCB\Cadence\Orcad\allegro\attocycler.brd"


    *** Done ***


    Originally posted in cdnusers.org by garylim
    • Post Points: 0
  • Wed, Nov 15 2006 8:02 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Orcad to PCB Editor error during Create Netlist Reply

    Gary,

    I am not sure if the the character '/' is giving you error. May be you can replace the value in schematic with underscore '_' and give a try.

    Try setting the system environmental variable ALLEGRO_LONG_PACKAGE and value as TRUE, this will allow to read in the netlist with long package names into allegro.

    Just a quick guess :-)

    Good Luck!!
    Raj.


    Originally posted in cdnusers.org by rajpcb
    • Post Points: 20
  • Wed, Nov 15 2006 8:10 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Orcad to PCB Editor error during Create Netlist Reply

    hi raj,

    Thanks for the fast response. Yes, we also suspect that was the issue. But it will be a integration nightmare to manual convert every component naming to fit Allegro requirement. Shouldn't cadence has design built in to rectify such integration problem?

    thanks for the ALLEGRO_LONG_PACKAGE tips.

    cheers
    gary


    Originally posted in cdnusers.org by garylim
    • Post Points: 0
  • Wed, Nov 15 2006 11:58 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Orcad to PCB Editor error during Create Netlist Reply

    garylim,

    i am so sorry to tell you that, maybe you have to modify the "pcb footprint" property of every component that caused error,

    some concept:

    property transition : Orcad Pcb footprint -> Allegro JEDEC

    there are no charactor available in "jedec" but english char like "a, b x..", numeric char like " 2 , 5 " and the underlin"_";

    and what's more, the design path of brds,symbles and pads do not permmit "space char" insede:)

    hope this helps


    Originally posted in cdnusers.org by tfsummer
    • Post Points: 0
  • Thu, Nov 16 2006 12:02 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Orcad to PCB Editor error during Create Netlist Reply

    and a number , 18 , is the longest char length of legal symbole and pad name:)


    Originally posted in cdnusers.org by tfsummer
    • Post Points: 20
  • Tue, Dec 4 2007 1:05 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Orcad to PCB Editor error during Create Netlist Reply

    I'm having a similair issue at the moment, I tried the underscore but it did not seem to work. I did this on a single part, I will try agian and see if this works. Its going to be a nightmare for me as well if I have to go and fix all the parts.


    Originally posted in cdnusers.org by Gun_metal
    • Post Points: 0
  • Sat, Jun 4 2011 12:33 AM

    • alokt
    • Top 25 Contributor
    • Joined on Fri, Aug 22 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: RE: Orcad to PCB Editor error during Create Netlist Reply

    You can have upto 255 char long names. Recommended is 31. If you need to increase this limit you can do so via Setup button in PCB Editor Netlist TAB.

     

    • Post Points: 5
  • Sat, Jun 4 2011 9:39 AM

    • redwire
    • Top 10 Contributor
    • Joined on Thu, Jul 17 2008
    • Allen, TX
    • Posts 876
    • Points 13,485
    Re: RE: Orcad to PCB Editor error during Create Netlist Reply

    archive:

    Gary,

    I am not sure if the the character '/' is giving you error. May be you can replace the value in schematic with underscore '_' and give a try.

    That's most likely it.  "/" has historically been used for the file system and can't be part of the package name as well.  I would do what rajpcb suggests.

    • Post Points: 5
Page 1 of 1 (8 items)
Sort Posts:
Started by archive at 15 Nov 2006 07:50 PM. Topic has 7 replies.