SLiCAPngspice.py

SLiCAP module for interfacing with NGspice.

class MOS(refDes, lib, dev, W, L, M)

MOS Transistor.

Parameters:

  • refDes (str) – Reference designator used in SLiCAP circuit file

  • lib (str) – path to library file, absolute or relative to python script.

  • dev (str) – Device name (as in library)

MOS attributes:

  • self.refDes = refDes

  • self.lib = lib

  • self.dev = dev

  • self.modelDef = Text string with SLiCAP model definition for this device

  • self.parDefs = Dictionary with SLiCAP parameter definitions for this device

  • self.params = Dictionary with names and values of parameters provided by ngspice

  • self.errors = Relative difference between forward and reverse parameter measurement

  • self.step = Step data for VG or ID, defaults to False

getOPid(ID, VD, VS, VB, f, step=None)

Returns operating point information of the device with the drain current as (swept) independent variable.

Parameters:

  • W (float) – Width of the device in [m]

  • L (float) – Length of the device in [m]

  • M (int) – Number of devices in parallel

  • ID (float) – Drain current [A]

  • VD (float) – Drain voltage with respect to ground in [V]

  • VS (float) – Source voltage with respect to ground in [V]

  • VB (float) – Bulk voltage with respect to ground in [V]

  • step – Step data for ID; list with start value, number of values and stop value. Defaults to None

getOPvg(VG, VD, VS, VB, f, step=None)

Returns operating point information of the device with the gate voltage as (swept) independent variable.

Parameters:

  • W (float) – Width of the device in [m]

  • L (float) – Length of the device in [m]

  • M (int) – Number of devices in parallel

  • VG (float) – Gate voltage with respect to ground in [V]

  • VD (float) – Drain voltage with respect to ground in [V]

  • VS (float) – Source voltage with respect to ground in [V]

  • VB (float) – Bulk voltage with respect to ground in [V]

  • step – Step data for VG; list with start value, number of values and stop value. Defaults to None

getSv_inoise(ID, VD, VS, VB, fmin, fmax, numDec)
ngspice2traces(cirFile, simCmd, namesDict, stepCmd=None, parList=None, traceType='magPhase', squaredNoise=False, postProc=None, saveLog=True, optDict=None)

Creates a dictionary with values or traces from an ngspice run.

Parameters:

  • cirFile (str) – Name of the circuit file withouit ‘.cir’ extension, located in the cir folder.

  • simCmd (str) –

    ngspice instruction,

    • ac dec 20 1 10meg

    • tran 1n 10u

    • dc Source Vstart Vstop Vincr [ Source2 Vstart2 Vstop2 Vincr2 ]

    • noise V(out) Vs dec 10 1 10meg 1

    • op

  • stepCmd (str, nonetype) –

    Step instruction or None if no parameter stepping is performed:

    Syntax: <parname> <stepmethod> <firstvalue> (<lastvalue> <numberofvalues | listwithvalues>)

    • parname (str): name of the parameter (not a RefDes)

    • stepmethod (str): lin, log or list

  • namesDict (dict) –

    Dictionary with key-value pairs:

    key: plot label (str)

    value: nodal voltage, branch current or device parameter in ngspice notation

  • traceType (str) –

    Type of traces for AC, noise, and FFT analysis:

    • realImag: real and imaginary parts

    • magPhase: magnitude and phse

    • dBmagPhase: dB(magnitude) and phase

    • onoise: output referred noise

    • inoise: input referred noise

  • parList (list) –

    List with parameter definitions, each item in the list must be a tuple with the name and the value of a parameter. The name must be a string, and the value a string, an integer, a float, or a SPICE expression (between curly brackets). The order of parameter definitions should be such that SPICE can evaluate a numeric value for each parameter in a non-recursive way.

    Example:

    >>> params = [('R', '1k'), ('C', '1n'), ('tau', '{1/(R*C)}')]

  • squaredNoise (Bool) –

    • True: output in V^2/Hz, A^2/Hz, V^2 or A^2

    • False: output in V/rt(Hz), A/rt(Hz), V or A

    Defaults to True

  • postProc (str, NoneType) –

    Post processing fuction for transient analysis:

    • None

      No post processing is performed

    • FFT <vector> (<vector> …)

      Returns the Fast Fourier Transform of one or more vectors obtained from a transient analysis. Curently only Hanning windowing has been implemented.

    • FOURIER <vector> (<vector> …)

      Lists the values of the first ten harmonics of one or more vectors obtained from a transient analysis in the simulation log file.

  • saveLog (Bool) – True | False, defaults to True. The log file is saved in the txt folder in the project directory. The name is the circuit file name with ‘.log’ file extension.

  • optDict (NoneType, dict) – None (default) or a dictionary with NGspice options, The keys are the NGspice option names and the values are ‘None’ if the option requires no value, or the option value.

Returns:

  • In case of an “OP” instruction without parameter stepping:

    A dictionary with key-value pairs:

    • key: str Name of the variable

    • value: float Value of the parameter, voltage or current

  • In all other cases: a tuple (dict, str1, str2)

    • dict

      • key: str Name of the variable

      • value: SLiCAP.SLiCAPplots.trace object or single value

    • str1: name of the x-variable

    • str2: units if the x-variable

Return type:

tuple: dict, (dict, str, str)

selectTraces(traceDict, namesList)

This function returns a dictionary selected traces from a dictionary with traces.

Parameters:

  • traceDict – A dictionary with key-value pairs: - key: name of the trace - value: a SLiCAP.SLiCAPplots.trace object holding trace (x, y) data and a trace label

  • namesList – A list with names of traces (== keys in traceDict) that needs to be returned

Returns:

a dictionary with selected traces (sub of traceDict)

Return type:

dict