+ Post New Thread
Results 1 to 16 of 16
  1. #1
    Member level 1
    Points: 1,629, Level: 9

    Join Date
    Sep 2006
    Posts
    36
    Helped
    1 / 1
    Points
    1,629
    Level
    9

    NetList Generation for OrCAD PCB editor

    I am using OrCAD 16.0 and new to OrCAD PCB Editor. I draw the schematic
    in Captur CIS .and copy foot print from OrCAD Laout Library manager and
    past it into the foot print(cell) in edit prorerties of Schematic. i got
    the error. inter-tool request denied in library manager. then i select
    creat netlist for PCB Editor. Check the option as

    * create PCB editor netlist
    * create or PCB update PCB editor board
    * Place Change Componenet
    * Board Lunch Option Open in OrCAd PCB editor

    during the netlist generation i get the error

    netrev failed please refer to session log

    thwer i get the error

    ************************************************** **********************\
    **********

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


    #1 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'MC33171/ON_DIP.100B/8/W.300/L.4'. JEDEC_TYPE property
    'DIP.100B/8/W.300/L.450' is illegal: 'Package name has invalid
    characters or is too long.'.

    ERROR(SPMHNI-170): Device 'MC33171/ON_DIP.100B/8/W.300/L.4' has library
    errors. Unable to transfer to Allegro.

    #2 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'R_RAD/.300X.100/LS.200/.031_1K'. JEDEC_TYPE property
    'RAD/.300X.100/LS.200/.031' is illegal: 'Package name has invalid
    characters or is too long.'.

    ERROR(SPMHNI-170): Device 'R_RAD/.300X.100/LS.200/.031_1K' has library
    errors. Unable to transfer to Allegro.

    #3 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'CON6_BLKCON.100/VH/TM1SQ/W.100/'. JEDEC_TYPE property
    'BLKCON.100/VH/TM1SQ/W.100/6' is illegal: 'Package name has invalid
    characters or is too long.'.

    ERROR(SPMHNI-170): Device 'CON6_BLKCON.100/VH/TM1SQ/W.100/' has library
    errors. Unable to transfer to Allegro.

    #4 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'C_RAD/.300X.100/LS.200/.031_0.1'. JEDEC_TYPE property
    'RAD/.300X.100/LS.200/.031' is illegal: 'Package name has invalid
    characters or is too long.'.

    ERROR(SPMHNI-170): Device 'C_RAD/.300X.100/LS.200/.031_0.1' has library
    errors. Unable to transfer to Allegro.

    #5 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'C_ELECT_CYL/D.225/LS.125/.031_1'. JEDEC_TYPE property
    'CYL/D.225/LS.125/.031' is illegal: 'Package name has invalid characters
    or is too long.'.

    ERROR(SPMHNI-170): Device 'C_ELECT_CYL/D.225/LS.125/.031_1' has library
    errors. Unable to transfer to Allegro.

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


    ************************************************** ****************

    can any bdy help me solving the problem

    thanks

  2. #2
    Advanced Member level 4
    Points: 8,133, Level: 21

    Join Date
    Feb 2010
    Location
    UNITED KINGDOM
    Posts
    1,239
    Helped
    406 / 406
    Points
    8,133
    Level
    21

    Re: NetList Generation for OrCAD PCB editor

    try removing "/" from names.


    1 members found this post helpful.

  3. #3
    Junior Member level 3
    Points: 1,036, Level: 7
    mashak's Avatar
    Join Date
    Dec 2007
    Posts
    28
    Helped
    6 / 6
    Points
    1,036
    Level
    7

    Re: NetList Generation for OrCAD PCB editor

    Quote Originally Posted by zia.roghani View Post
    I am using OrCAD 16.0 and new to OrCAD PCB Editor. I draw the schematic
    in Captur CIS .and copy foot print from OrCAD Laout Library manager and
    past it into the foot print(cell) in edit prorerties of Schematic. i got
    the error. inter-tool request denied in library manager. then i select
    creat netlist for PCB Editor. Check the option as

    * create PCB editor netlist
    * create or PCB update PCB editor board
    * Place Change Componenet
    * Board Lunch Option Open in OrCAd PCB editor

    during the netlist generation i get the error

    netrev failed please refer to session log

    thwer i get the error

    ************************************************** **********************\
    **********

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


    #1 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'MC33171/ON_DIP.100B/8/W.300/L.4'. JEDEC_TYPE property
    'DIP.100B/8/W.300/L.450' is illegal: 'Package name has invalid
    characters or is too long.'.

    ERROR(SPMHNI-170): Device 'MC33171/ON_DIP.100B/8/W.300/L.4' has library
    errors. Unable to transfer to Allegro.

    #2 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'R_RAD/.300X.100/LS.200/.031_1K'. JEDEC_TYPE property
    'RAD/.300X.100/LS.200/.031' is illegal: 'Package name has invalid
    characters or is too long.'.

    ERROR(SPMHNI-170): Device 'R_RAD/.300X.100/LS.200/.031_1K' has library
    errors. Unable to transfer to Allegro.

    #3 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'CON6_BLKCON.100/VH/TM1SQ/W.100/'. JEDEC_TYPE property
    'BLKCON.100/VH/TM1SQ/W.100/6' is illegal: 'Package name has invalid
    characters or is too long.'.

    ERROR(SPMHNI-170): Device 'CON6_BLKCON.100/VH/TM1SQ/W.100/' has library
    errors. Unable to transfer to Allegro.

    #4 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'C_RAD/.300X.100/LS.200/.031_0.1'. JEDEC_TYPE property
    'RAD/.300X.100/LS.200/.031' is illegal: 'Package name has invalid
    characters or is too long.'.

    ERROR(SPMHNI-170): Device 'C_RAD/.300X.100/LS.200/.031_0.1' has library
    errors. Unable to transfer to Allegro.

    #5 ERROR(SPMHNI-176): Device library error detected.

    ERROR(SPMHNI-164): Problems with device
    'C_ELECT_CYL/D.225/LS.125/.031_1'. JEDEC_TYPE property
    'CYL/D.225/LS.125/.031' is illegal: 'Package name has invalid characters
    or is too long.'.

    ERROR(SPMHNI-170): Device 'C_ELECT_CYL/D.225/LS.125/.031_1' has library
    errors. Unable to transfer to Allegro.

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


    ************************************************** ****************

    can any bdy help me solving the problem

    thanks
    Hi,

    No special characters are allowed in the JEDEC Name, you can use Underscore but no other special characters.
    Mashak
    IPC CID



    •   Alt14th February 2011, 13:17

      advertising

        
       

  4. #4
    Member level 3
    Points: 1,382, Level: 8

    Join Date
    Jul 2008
    Location
    ITALY
    Posts
    58
    Helped
    4 / 4
    Points
    1,382
    Level
    8

    Re: NetList Generation for OrCAD PCB editor

    You have to use the footprint name (file naming convention af PDB Editor).
    Than You MUST set the path of the PCB Editor such us device, padstack and so on.



  5. #5
    Newbie level 6
    Points: 538, Level: 4

    Join Date
    Mar 2010
    Location
    Bangalore
    Posts
    12
    Helped
    0 / 0
    Points
    538
    Level
    4

    Re: NetList Generation for OrCAD PCB editor

    If you do not have the footprint name, give it as "dummy" at the Footprint name string. this will solve the problem



    •   Alt1st December 2011, 09:38

      advertising

        
       

  6. #6
    Advanced Member level 4
    Points: 8,133, Level: 21

    Join Date
    Feb 2010
    Location
    UNITED KINGDOM
    Posts
    1,239
    Helped
    406 / 406
    Points
    8,133
    Level
    21

    Re: NetList Generation for OrCAD PCB editor

    I think the hint was in the error description 'Package name has invalid characters or is too long' as allegro stores the footprints as seperate *.dra files in the library folder only certain non printable characters are allowed, "/" is not one of them.



  7. #7
    Member level 3
    Points: 1,382, Level: 8

    Join Date
    Jul 2008
    Location
    ITALY
    Posts
    58
    Helped
    4 / 4
    Points
    1,382
    Level
    8

    Re: NetList Generation for OrCAD PCB editor

    short name without path.
    the path of your library is used in the PCBEditor path configuration.
    No special characteres.
    For the Pad name....you have to use a very short name 7/8 characteres.
    You can use this symbol _



    •   Alt2nd December 2011, 16:08

      advertising

        
       

  8. #8
    Newbie level 3
    Points: 192, Level: 2

    Join Date
    Dec 2011
    Location
    east coast USA
    Posts
    3
    Helped
    0 / 0
    Points
    192
    Level
    2

    Re: NetList Generation for OrCAD PCB editor

    hi there. sorry to dig up an old post, but i am having the same problem. my footprint libraries are named in the same manner, with the "/" between various parameters. these are default with Cadence 16.0 and there are 1000s of them with this naming convention (default install directory for these is OrCad_16.0\tools\layout_eng_ed\library).

    example:
    Code:
    #2   ERROR(SPMHNI-176): Device library error detected.
    
    ERROR(SPMHNI-164): Problems with device 'R_BUSS_100_SIL8_BLKCON.100/VH/T'. JEDEC_TYPE property 'BLKCON.100/VH/TM1SQS/W.100/8' is illegal: 'Package name has invalid characters or is too long.'.
    
    ERROR(SPMHNI-170): Device 'R_BUSS_100_SIL8_BLKCON.100/VH/T' has library errors. Unable to transfer to Allegro.
    i really believe i have generated a netlist in the past using these footprints. but if that was impossible, is there an easy way to convert these 10000 files to an expectable format (i guess with no slashed or dots)



  9. #9
    Member level 3
    Points: 1,382, Level: 8

    Join Date
    Jul 2008
    Location
    ITALY
    Posts
    58
    Helped
    4 / 4
    Points
    1,382
    Level
    8

    Re: NetList Generation for OrCAD PCB editor

    the name of the footprint BLKCON.100/VH/TM1SQS/W.100/8 is invalid. The "/" is a special character. You can't use it in the footprint name (ora JEDEC_TYPE Propriety). Other special Character that you can't use is ".".
    BLKCON.100/VH/TM1SQS/W.100/8 is the name of the footprint without path? If yes, than change the name of the footprint: delete the special character and reduce the lenght of the name.
    if no, than you have to store the full path where you are stored the footprint in the Allegro Options and than you change the footprint name with a short name.
    For example:
    the path C:\footprint\passive => Allegro->Setup->User Preferences->Path->Config->...
    The footprint name IR0402X65 how name of the footprint stored in the previous path and how JEDEC_TYPE propriety in the Concept HDL Library of R Symbol or in the part file table.


    1 members found this post helpful.

  10. #10
    Newbie level 3
    Points: 192, Level: 2

    Join Date
    Dec 2011
    Location
    east coast USA
    Posts
    3
    Helped
    0 / 0
    Points
    192
    Level
    2

    Re: NetList Generation for OrCAD PCB editor

    hi again. valeriogiampa thank you for the reply
    BLKCON.100/VH/TM1SQS/W.100/8 is the name of the footprint without path?
    the footprint libraries i am using are stored in the path: "C:\OrCAD\OrCad_16.0\tools\layout_eng_ed\libra ry"
    the library i am using is: "bcon100t.llb"
    the footprint in that library is called "BLKCON.100/VH/TM1SQS/W.100/8"

    Does this sound normal?

    again, these are the stock libraries that came with Cadence Allegro 16.0, with stock footprint names. they all use this naming scheme and there are 1000s of them. i dont know why they would name them this if i had to rename each one every time i wanted to use it?




    sorry if this sounds juvenile but i'm really lost. also i appreciate your time for tying to help me out thank you



  11. #11
    Advanced Member level 4
    Points: 8,133, Level: 21

    Join Date
    Feb 2010
    Location
    UNITED KINGDOM
    Posts
    1,239
    Helped
    406 / 406
    Points
    8,133
    Level
    21

    Re: NetList Generation for OrCAD PCB editor

    When Prcad schematics was used with Orcad Layout, these component footprint names were legal, now when Orcad Schematics is used with Orcad PCB Editor (a cut down version of Allegro), these footprint names are illegal, as the footprints are stored as seperate *.dra files and thus the \ is not allowed.
    Somewhere withing the Orcad software is a way of converting the libraries, that was provided when Orcad Layout became defunct in 2008.



  12. #12
    Newbie level 3
    Points: 192, Level: 2

    Join Date
    Dec 2011
    Location
    east coast USA
    Posts
    3
    Helped
    0 / 0
    Points
    192
    Level
    2

    Re: NetList Generation for OrCAD PCB editor

    ah good too hear (well, at least what the problem is). thank you marce i will look into this this evening when i get home and provide you with an update



  13. #13
    Member level 3
    Points: 1,382, Level: 8

    Join Date
    Jul 2008
    Location
    ITALY
    Posts
    58
    Helped
    4 / 4
    Points
    1,382
    Level
    8

    Re: NetList Generation for OrCAD PCB editor

    the name BLKCON.100/VH/TM1SQS/W.100/8 is assignet at the file .dra and .psm?
    If Yes,..this is abnormal becouse you have used a name with special characters and don't short.
    You have to change the name BLKCON.100/VH/TM1SQS/W.100/8. You can use BLKCON100VHTM1SQSW1008 or BLKCON100_VH_TM1SQS_W100_8.
    Test it and send me a feedback.



  14. #14
    Advanced Member level 1
    Points: 3,287, Level: 13

    Join Date
    Dec 2009
    Location
    INDIA
    Posts
    442
    Helped
    86 / 86
    Points
    3,287
    Level
    13
    Blog Entries
    1

    Re: NetList Generation for OrCAD PCB editor

    OrCAD layout & OrCAD PCB Editor both are different tool. if you have existing board created using Layout yu can convert these into PCB Editor. User layout to Allegro translator for that. You can find this tool's short cut in PCB Accessories

    Capture-PCB editor netslist would not support special char like / . in names, while these were supported in OrCAD layout.
    Also please note what ever footprint name you assign in schematic, you need to have footprint with same name available for PCB editor. Thus by merely assigning layout footprint name for in PCB Editor netlist would not serve any purpose.

    Hope this gives some insight.
    The road of life twists and turns and no two directions are ever the same. Yet our lessons come from the journey, not the destination. ~ Don Williams, Jr.



  15. #15
    Advanced Member level 4
    Points: 8,133, Level: 21

    Join Date
    Feb 2010
    Location
    UNITED KINGDOM
    Posts
    1,239
    Helped
    406 / 406
    Points
    8,133
    Level
    21

    Re: NetList Generation for OrCAD PCB editor

    There is a way of converting the footprint library as well, I had a document from Cadence that covered the change from Orcad Layout to Orcad PCB Editor (Allegro cut down). I am trying to find it, when I do I will post it.



  16. #16
    Member level 3
    Points: 1,382, Level: 8

    Join Date
    Jul 2008
    Location
    ITALY
    Posts
    58
    Helped
    4 / 4
    Points
    1,382
    Level
    8

    Re: NetList Generation for OrCAD PCB editor

    yes, you can use Orcad Layout translator to convert .mx file. I think that this utility is windows only.



+ Post New Thread
Please login