Stats

  • Locked Locked
  • Replies 7
  • Subscribers 50
  • Views 7773
  • Members are here 0
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

Generate spectre netlist from command line/script

coco009
Hi, I would like to find a method of generating spectre netlists using a script, preferably an Ocean script. At present, I have a pile of schematics, which do not have netlists. I can create netlists by running up the ADE GUI (which automatically creates a netlist), but ideally I want to avoid running up ADE at all and do all my work from the command line, i.e. within Ocean Does anybody know if this is possible and if so, how? Thanks very much in advance! Regards coco009
  • (Sorry, just re-posting as I appeared to lose all "\n" s) 
    Hi,
    I would like to find a method of generating spectre netlists using a script, preferably an Ocean script.
    At present, I have a pile of schematics, which do not have netlists. I can create netlists by running up the ADE GUI (which automatically creates a netlist on startup), but ideally I want to avoid running up ADE at all and do all my work from the command line, i.e. within Ocean
    Does anybody know if this is possible and if so, how?
    Thanks very much in advance!
    Regards coco009

  •  You'll probably have better luck getting this answered in the 'Custom IC' section of the forums, but the quick answer is to use the 'design( lib cell view )' form of the command in OCEAN.

     See OCEAN Reference.

     Andrew.

  • Hi Andrew,

     

    Thanks for your prompt reply. I did have a try using the design() command, e.g, design( "myLib" "mydesign" "schematic" ), but I kept getting an error stating that "currently you cannot specificy a lib-cell-view with the design() command in ocean". This obviously contradicts the information provided in the Ocean reference document. This is exactly what I would like to be able to do though, just define the cell in the library rather than the netlist itself.

     

    If you have any further thoughts, I would be very grateful. In the meantime, I will re-post this question in the Custom IC section as you suggest.

     

    Thanks again!

     

    coco009

  • I'm guessing you've already solved your issue by now. For anyone else looking through these threads and are hung up on this issue maybe this can shed some light on the subject.

    make a simple script to run the non graphical icfb then give it lines of commands followed by "exit" and it will spit out a spectre netlist ".scs" file.

     icfb -nograph < filewithcommands

     

     heres what the "filewithcommands" looks like inside:

     

    simulator( 'spectre )

    design( "libname" "cellname" "viewname")

    createNetlist( ?recreateAll t)

    exit

  • I had no idea i want your idea. thank you
  • here is my guess:

    modelPath = "/home/models.scs"
    modelPath_list = list( modelPath "nom")

    ; Start of an Analog Design Environment session
    sessionId = sevStartSession( ?lib libName ?cell cellName ?view viewName)

    ; Get databaseIDs
    o_sessionId = sevEnvironment( sessionId )
    o_formatterId = asiCreateFormatter( o_sessionId )
    o_netlisterId = nlGetNetlister( o_formatterId )
    netlistPath = nlGetNetlistDir( o_netlisterId )

    println( netlistPath )

    asiNetlist( o_sessionId )
    nlNetlist( o_netlisterId )

    ; Creation of input.scs
    simulator( 'spectre )
    design( strcat( netlistPath "/netlist" ) )
    modelFile( modelPath_list )
    saveOption()
    save( 'alli )
    saveOption( 'subcktprobelvl 6 'save "all" 'currents "all" )
    option( 'maxwarns 500 )
    saveOption()
    analysis( 'tran ?start 0 ?stop 40n )
    input_scsPath = createNetlist()

    printf("\n input.scs createed \n")
    printf("\n input_scsPath : %s \n" input_scsPath)

    greetins,

  •  Hi,

    I have a similar issue. I have an extracted .dspf file how can I simulate it from command line?

    If I have netlist of a circuit, is there any way I can generate/attach a cell symbol for this netlist?

     Thanks

    Sarik 

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.