Stats

  • Locked Locked
  • Replies 3
  • Subscribers 125
  • Views 22077
  • 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

import a Spice Model in a schematic

Friedrich

Hello,

I would like to import a model which is written in Spice. In the end, I want a simple symbol which contains this model and which i could place in my other schematics.

The model I want to include in my schematic is the following:
www.diodes.com/.../DMT6016LPS


I tried the following steps:
    
    I tried to open a new cellview and chose the Type "Spice". Then I copied the model text in the new created spiceText file and saved it. I created a "Cellview from Cellview" and got a symbol which doesn't contain any information or netlist I think. That means it is like a open circuit.

    Then I tried to use the "Spice In" import. I chose my netlist file and the Spice option as netlist language. I named the "Top Cell" and for the Reference Library List I chose "basic" and "analogLib".  As Output view information, I chose netlist. In the tab "Device Map", I mapped some models the following way:
    capacitor to cap
    DLIM to diode
    DSUB to diode
    DCGD to diode
    resistor to res

I got the output log file and the end of my post.

After that I wrote a config file which contains the imported file as a netlist...
But the symbol doesn't contain any information as it seems.


Could you clarify which way is the correct to include a spice netlist or a spice subckt?
Could you give me a step by step guide on how I can import my Subckt file to generate a valid symbol?

Thank you!

===================
Spice In Log File
===================
Parameter file: /tmp/spiceInPvh1632
Import Parameters:
    Netlist file name: ...
    Output library name: dmtimport
    Output View Type: netlist
    Netlist view name: netlist
    Reference Library List: basic analogLib dmtimport
    Top cell: dmt6016lps
    Device-mapping file name: ...
    Master Cell for Ground: gnd
    Cells to be Overwritten: <all>
    Schematic Generation parameter file: /tmp/schOpts_spiceInPvh1632
    Simulator: spectre
    Output Simulator: spectre
    paramCaseValue: default
    Language: SPICE
Total number of files: 1.

Netlist File: ...
Total number of Subckts: 1.
    Master Cellview Found in dmtimport::DMT6016LPS::netlist
    Cellview already exist in output library and overwrite flag is set, hence re-importing

********
Created dmtimport.DMT6016LPS:netlist
    Created net 10.
    Created term 10.
    Created net 20.
    Created term 20.
    Created net 30.
    Created term 30.

    Total number of Insts: 15.

    Inst: M1
        Created net '1'.
        Created net '2'.
        Created net '3'.
        Found net '3'.

        Master Cell: 'nmos'.
        Did not find 'basic.nmos:symbol'.
        Master Cellview: 'analogLib.nmos:symbol' found.
        Created instance 'M1'.
        Created connection between net '1' and term 'D'.
        Created connection between net '2' and term 'G'.
        Created connection between net '3' and term 'S'.
        Created netSet prop 'bulk_n' between net '3' and term 'B'.
        Created propName='model'; propType='string'; propVal='nmos'.
        Created propName='l'; propType='string'; propVal='1e-06'.
        Created propName='w'; propType='string'; propVal='1e-06'.

    Inst: RD
        Found net '10'.
        Found net '1'.

        Master Cell 'resistor' mapped to 'res'.
        Did not find 'basic.res:symbol'.
        Master Cellview: 'analogLib.res:symbol' found.
        Created instance 'RD'.
        Created connection between net '10' and term 'PLUS'.
        Created connection between net '1' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='resistor'.
        Created propName='r'; propType='string'; propVal='0.006728'.

    Inst: RS
        Found net '30'.
        Found net '3'.

        Master Cell 'resistor' mapped to 'res'.
        Master Cellview: 'analogLib.res:symbol' found.
        Created instance 'RS'.
        Created connection between net '30' and term 'PLUS'.
        Created connection between net '3' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='resistor'.
        Created propName='r'; propType='string'; propVal='0.001'.

    Inst: RG
        Found net '20'.
        Found net '2'.

        Master Cell 'resistor' mapped to 'res'.
        Master Cellview: 'analogLib.res:symbol' found.
        Created instance 'RG'.
        Created connection between net '20' and term 'PLUS'.
        Created connection between net '2' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='resistor'.
        Created propName='r'; propType='string'; propVal='1.35'.

    Inst: CGS
        Found net '2'.
        Found net '3'.

        Master Cell 'capacitor' mapped to 'cap'.
        Did not find 'basic.cap:symbol'.
        Master Cellview: 'analogLib.cap:symbol' found.
        Created instance 'CGS'.
        Created connection between net '2' and term 'PLUS'.
        Created connection between net '3' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='capacitor'.
        Created propName='c'; propType='string'; propVal='8.475e-10'.

    Inst: EGD
        Created net '12'.
        Master Cellview: 'basic.gnd:symbol' found.
        Created net 'gnd!'.
        Found net '2'.
        Found net '1'.

        Master Cell: 'vcvs'.
        Master cell CDF data not found for 'basic.vcvs'
        Master Cellview: 'analogLib.vcvs:symbol' found.
        Created instance 'EGD'.
        Created connection between net '12' and term 'PLUS'.
        Created connection between net 'gnd!' and term 'MINUS'.
        Created connection between net '2' and term 'NC+'.
        Created connection between net '1' and term 'NC-'.
        Created propName='model'; propType='string'; propVal='vcvs'.
        Created propName='egain'; propType='string'; propVal='1'.

    Inst: VFB
        Created net '14'.
        Master Cellview: 'basic.gnd:symbol' found.
        Found net 'gnd!'.

        Master Cell: 'vsource'.
        Did not find 'basic.vsource:symbol'.
        Master Cellview: 'analogLib.vsource:symbol' found.
        Warning! termOrder of this master has more entries than required. Ignoring the extra entries
        Created instance 'VFB'.
        Created connection between net '14' and term 'PLUS'.
        Created connection between net 'gnd!' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='vsource'.
        Created propName='vdc'; propType='string'; propVal='0'.

    Inst: FFB
        Found net '2'.
        Found net '1'.

        Master Cell: 'cccs'.
        Did not find 'basic.cccs:symbol'.
        Master Cellview: 'analogLib.cccs:symbol' found.
        Created instance 'FFB'.
        Created connection between net '2' and term 'PLUS'.
        Created connection between net '1' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='cccs'.
        Created propName='vref'; propType='string'; propVal='VFB'.
        Created propName='fgain'; propType='string'; propVal='1'.

    Inst: CGD
        Created net '13'.
        Found net '14'.

        Master Cell 'capacitor' mapped to 'cap'.
        Master Cellview: 'analogLib.cap:symbol' found.
        Created instance 'CGD'.
        Created connection between net '13' and term 'PLUS'.
        Created connection between net '14' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='capacitor'.
        Created propName='c'; propType='string'; propVal='6e-10'.

    Inst: R1
        Found net '13'.
        Master Cellview: 'basic.gnd:symbol' found.
        Found net 'gnd!'.

        Master Cell 'resistor' mapped to 'res'.
        Master Cellview: 'analogLib.res:symbol' found.
        Created instance 'R1'.
        Created connection between net '13' and term 'PLUS'.
        Created connection between net 'gnd!' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='resistor'.
        Created propName='r'; propType='string'; propVal='1'.

    Inst: D1
        Found net '12'.
        Found net '13'.

        Master Cell 'DLIM' mapped to 'diode'.
        Did not find 'basic.diode:symbol'.
        Master Cellview: 'analogLib.diode:symbol' found.
        Created instance 'D1'.
        Created connection between net '12' and term 'PLUS'.
        Created connection between net '13' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='DLIM'.

    Inst: DDG
        Created net '15'.
        Found net '14'.

        Master Cell 'DCGD' mapped to 'diode'.
        Did not find 'basic.diode:symbol'.
        Master Cellview: 'analogLib.diode:symbol' found.
        Created instance 'DDG'.
        Created connection between net '15' and term 'PLUS'.
        Created connection between net '14' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='DCGD'.

    Inst: R2
        Found net '12'.
        Found net '15'.

        Master Cell 'resistor' mapped to 'res'.
        Master Cellview: 'analogLib.res:symbol' found.
        Created instance 'R2'.
        Created connection between net '12' and term 'PLUS'.
        Created connection between net '15' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='resistor'.
        Created propName='r'; propType='string'; propVal='1'.

    Inst: D2
        Found net '15'.
        Master Cellview: 'basic.gnd:symbol' found.
        Found net 'gnd!'.

        Master Cell 'DLIM' mapped to 'diode'.
        Master Cellview: 'analogLib.diode:symbol' found.
        Created instance 'D2'.
        Created connection between net '15' and term 'PLUS'.
        Created connection between net 'gnd!' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='DLIM'.

    Inst: DSD
        Found net '3'.
        Found net '10'.

        Master Cell 'DSUB' mapped to 'diode'.
        Did not find 'basic.diode:symbol'.
        Master Cellview: 'analogLib.diode:symbol' found.
        Created instance 'DSD'.
        Created connection between net '3' and term 'PLUS'.
        Created connection between net '10' and term 'MINUS'.
        Created propName='model'; propType='string'; propVal='DSUB'.

Saved and closed 'dmtimport.DMT6016LPS:netlist'.
INFO (SPICEIN-54): Spice In successfully imported the netlist file ....

Parents

  • FYI, this post went into moderation because of the repeated text in the post; that's often a sign of spam (it isn't in this case though). So I've allowed it through, and moved it into the Custom IC Design forum which is more appropriate since it's not really mixed-signal related.

    Using File->Import->SPICE is not really the right method here because the subckt contains .MODEL statements; Import SPICE is more appropriate for structural SPICE netlists, not for models.

    The right mechanism is to do what you did first - create a view of type "Spice" (or possibly "pspice" might be a better choice as I suspect this is more likely to have been provided as a model for PSPICE; I got fewer warnings when simulating with it if I used "pspice").

    Anyway, having imported the text and created a symbol, you can place the symbol in your schematic. In ADE you either need to use a config, or on Setup->Environment add "spiceText" or "pspice" (or whatever you have called the view name when you created the model view) to the Switch View List. This means that during netlisting, it will know to pick the textual model representation, and that will get included into the netlist and hence the simulator will be able to use the model.

    Regards,

    Andrew

Reply

  • FYI, this post went into moderation because of the repeated text in the post; that's often a sign of spam (it isn't in this case though). So I've allowed it through, and moved it into the Custom IC Design forum which is more appropriate since it's not really mixed-signal related.

    Using File->Import->SPICE is not really the right method here because the subckt contains .MODEL statements; Import SPICE is more appropriate for structural SPICE netlists, not for models.

    The right mechanism is to do what you did first - create a view of type "Spice" (or possibly "pspice" might be a better choice as I suspect this is more likely to have been provided as a model for PSPICE; I got fewer warnings when simulating with it if I used "pspice").

    Anyway, having imported the text and created a symbol, you can place the symbol in your schematic. In ADE you either need to use a config, or on Setup->Environment add "spiceText" or "pspice" (or whatever you have called the view name when you created the model view) to the Switch View List. This means that during netlisting, it will know to pick the textual model representation, and that will get included into the netlist and hence the simulator will be able to use the model.

    Regards,

    Andrew

Children

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.