Spice simulator interface classess

Spice

Analog simulation interface package for TheSyDeKick.

Provides utilities to import spice-like modules to Python environment and generate testbenches for the various simulation cases.

Initially written by Okko Järvinen, 2019

Notes for developers

There are now two ways to provide simulator dependent structures that are (most of the time) followed:

1. Simulator dependent properties are defined in packages <simulator>/<simulator>.py that are used as spice_simulator instance in this spice class inside spice_simulator property. Properties and attributed of instance of this class (i.e. all TheSyDeKick Entitites) are made visible to spice_simulators through passing the self as parent argument in instance creation. Properties defined inside spice_simulator are accessed and set through corresponding properties of this class.

2. This is an interface package, generic spice simulation related methods should be provided in spice_methods module.

class spice.spice

connect_spice_inputs()

Automatically called function to connect iofiles (inputs) to top entity IOS Bundle items.

connect_spice_outputs()

Automatically called function to connect iofiles (outputs) to top entity IOS Bundle items.

property dcsource_bundle

A thesdk.Bundle containing spice_dcsource objects. The spice_dcsource objects are automatically added to this Bundle, nothing should be manually added.

This is to automate biasing and operation conditions of the circuit.

Type:

Bundle

delete_spicesimpath()

Method to clean up files from spicesimpath.

property distributed_run

If True, distributes applicable simulations (currently DC sweep supported) into the LSF cluster. The number of subprocesses launched is set by self.num_processes.

(Default False)

Type:

bool

property dspf

List containing filenames for DSPF-files to be included for post-layout simulations. The names given in this list are matched to dspf-files in ‘./spice/’ -directory. A postfix ‘.pex.dspf’ is automatically appended to the given names (this will probably change later).

Example

self.dspf = ['adc_top_level']

would include files ‘./spice/adc_top_level.pex.dspf’ as a top level dspf-file in the testbench. If the dspf-file contains definition matching the original design name of the top-level netlist, it gets also renamed to match the module name (dspf-file for top-level instance is possible).

Type:

[str]

property errpreset

Global accuracy parameter for Spectre simulations. Options include ‘liberal’, ‘moderate’ and ‘conservative’, in order of rising accuracy.

Example

self.spice_simulator.errpreset='conservative'

Type:

str

execute_spice_sim()

Automatically called function to execute spice simulation.

extract_powers()

Automatically called function to extract transient power and current consumptions. The consumptions are extracted for spice_dcsource objects with the attribute extract=True.

The extracted consumptions are accessible on the top-level after simulation as:

# Dictionary with averaged power of each supply + total
self.extracts.Members['powers']
# Dictionary with averaged current of each supply + total
self.extracts.Members['currents']
# Dictionary with transient current of each supply
self.extracts.Members['curr_tran']

The keys in the aforementioned dictionaries match the name-fields of the respective spice_dcsource objects.

property extracts

A thesdk.Bundle containing extracted quantities.

Type:

Bundle

property interactive_spice

Launch simulator in interactive mode. A waveform viewer (ezwave by default) is opened during the simulation for debugging. See plotprogram for selecting waveform viewer program.

( Default : False )

Type:

bool

property iofile_eventdict

Dictionary to store event type output from the simulations. This should speed up reading the results.

NOTE: Eldo seems to force output names to uppercase, let’s uppercase everything here to avoid key mismatches. (This should be changed).

Type:

dict

property load_output_file

Whether to load the outputs from simulator output file. This only works if the file exists in the state directory, i.e. the simulator was run with save_output_file=True. WARNING: This will read the IOS from the output file, and REWRITE THE ENTITY STATE on disk.

( Default : False )

Type:

bool

property load_state

Feature for loading results of previous simulation. The Spice simulation is not re-executed, but the outputs will be read from existing files. The string value should be the runname of the desired simulation.

( Default ‘’ )

Example

Loading the most recent result automatically:

self.load_state = 'last'
# or
self.load_state = 'latest'

Loading a specific past result using the runname:

self.load_state = '20201002103638_tmpdbw11nr4'

List available results by providing any non-existent runname:

self.load_state = 'this_does_not_exist'

Type:

str

property name

Name of the module.

Type:

str

property nproc

Requested maximum number of threads for multithreaded simulations.

Eldo : maps to command line parameter ‘-nproc’

Spectre : maps to command line parameter ‘+mt’.

Ngspice : maps to ‘set num_threads=’ line in testbench.

Type:

int

property num_processes

Maximum number of spawned child processes for distributed runs.

Type:

int

property plflag

Postlayout simulation accuracy/RC reduction flag.

Type:

str

property plotlist

List of net names to be saved in the waveform database.

Note

Obsolete! Moved to spice_simcmd as a keyword argument.

Type:

[ str ]

property plotprogcmd

Command to be run for interactive simulations.

Type:

str

property plotprogram

Sets the program to be used for visualizing waveform databases. Options are ezwave (default) or viva.

Type:

str

property postlayout

Enables post-layout optimizations in the simulator command options. (Default : False )

Type:

bool

property postlayout_subckts

List containing filenames for subcircuit DSPF-files to be included for post-layout simulations. The names given in this list are matched to dspf-files in ‘./spice/’ -directory. A postfix ‘.pex.dspf’ is automatically appended to the given names (this will probably change later).

Example

self.postlayout_subckts = ['inv_v2','switch_v3']

would include files ‘./spice/inv_v2.pex.dspf’ and ‘./spice/switch_v3.pex.dspf’ as postlayout_subckts-files in the testbench. If top level dspf (self.dspf) is given these are omitted. Otherwise simulator will replace subcircuits with corresponding name with the postlayout netlist defined in the dspf file.

Type:

[str]

property preserve_spicefiles

If True, do not delete generated Spice files (testbench, subcircuit, etc.) after simulations. Useful for debugging.

(Default : False )

Type:

bool

read_oppts()

Internally called function to read the DC operating points of the circuit TODO: Implement for Eldo as well.

read_spice_outputs()

Automatically called function to call read() functions of each iofile with direction ‘output’.

run_plotprogram()

Starting a parallel process for waveform viewer program.

The plotting program command can be set with ‘plotprogram’. Tested for spectre and eldo.

run_spice()

Externally called function to execute spice simulation.

property save_database

Whether to save the waveform database (.wdb-file for eldo, raw-database for spectre), when save_state=True.

( Default : False)

Type:

bool

property save_output_file

If True and save_state is True, copy the output file of simulator to entity statedir. Useful for scavenging results if simulator exited but state was not written to disk for some reason.

( Default : False)

Type:

bool

property si_prefix_mult

Dictionary mapping SI-prefixes to multipliers.

Type:

dict

property simcmd_bundle

A thesdk.Bundle containing spice_simcmd objects. The spice_simcmd objects are automatically added to this Bundle, nothing should be manually added.

Type:

Bundle

property spice_simulator

The simulator specific operation is defined with an instance of simulator specific class. Properties and methods return values from that class.

Type:

ngspice

Type:

eldo

Type:

spectre

property spice_submission

Defines spice submission prefix from thesdk.GLOBALS[‘LSFSUBMISSION’] and thesdk.GLOBALS[‘LSFINTERACTIVE’] for LSF submissions.

Usually something like ‘bsub -K’ or ‘bsub -I’.

Type:

str

property spice_tb

Testbench instance. You can set the attributes of the testbench and dut below it before you execute run_spice. if

Example

::

self.spice_tb.dut.custom_subckt_name=’custom_inverter’ self.run_spice()

Type:

spice_module

property spicecmd

Simulation command string to be executed on the command line. Automatically generated.

Type:

str

property spicecorner

Feature for specifying the ‘section’ of the model library file and simulation temperature. The path to model libraries should be set in TheSDK.config as either ELDOLIBFILE, SPECTRELIBFILE or NGSPICELIBFILE variable.

Example

self.spicecorner = {
        'temp': 27,
        'corner': 'top_tt'
        }

Type:

dict

property spicedbpath

Path to output waveform database. (<spicesimpath>/tb_<entityname>.<resultfile_ext>) (For now only for spectre. HOW? should work for Eldo too)

Type:

str

property spicemisc

List of manual commands to be pasted to the testbench. The strings are pasted to their own lines (no linebreaks needed), and the syntax is unchanged.

Example

Setting initial voltages from testbench (Eldo):

for i in range(nodes):

    self.spicemisc.append('.ic NODE<%d> 0' % i)

The same example for Spectre:

self.spicemisc.append('simulator lang=spice')
for i in range(nodes):
    self.spicemisc.append('.ic NODE<%d> 0' % i)
self.spicemisc.append('simulator lang=spectre')

Type:

[str]

property spiceoptions

Feature for specifying options for spice simulation. The key is the name of the option (as in simulator manual specifies), and the value is the value given to said option. Valid key-value pairs can be found from the manual of the simulator (Eldo, Spectre or Ngspice).

Example

self.spiceoptions = {
           'save': 'lvlpub',
           'nestlvl': '1',
           'pwr': 'subckts',
           'digits': '12'
       }

Type:

dict

property spiceparameters

Feature for specifying simulation parameters for spice simulation. The key is the name of the parameter , and the value is the value given to said parameter.

Example

self.spiceparameters = {
           'nf_pmos': 8,
           'nf_nmos': 4,
           'ibias': 100e-6
       }

Type:

dict

property spicesimpath

Path to the directory where the simulation results are stored.

( Default : self.simpath )

Type:

str

property spicesrc

Path to the source netlist. Can be set manually to desired location.

( Default: ‘spice/entityname.scs’ )

N.B!:

Netlist has to contain the top-level design as a subcircuit definition!

Type:

str

property spicesrcpath

Path to the spice source of the entity. Can be set manually to desired location. This variable provides the dspf-parasitic netlist filepath.

( Default: <entity path>/spice )

Type:

str

property spicesubcktsrc

Path to the parsed subcircuit file. (‘<spicesimpath>/subckt_entityname.<suffix>’). This shouldn’t be set manually.

Type:

str

property spicetbsrc

Path to the spice testbench (‘<spicesimpath>/tb_entityname.<suffix>’). This shouldn’t be set manually.

Type:

str

property syntaxdict

Internally used dictionary for common syntax conversions between Spectre, Eldo, and Ngspice.

Type:

dict

write_spice_inputs()

Automatically called function to call write() functions of each iofile with direction ‘input’.

Spice Common

Mix-in class of ommon properties and methods for spice simulator classes

class spice.spice_common.spice_common

Common properties and methods for spice simulator tool classes. Most of these are overloaded in __init__.py

property extracts

Bundle

A thesdk.Bundle containing extracted quantities.

property is_strobed

Check if simulation was strobed or not

property strobe_indices

Internally set list of indices corresponding to time,amplitude pairs whose time value of is a multiple of the strobeperiod (see spice_simcmd).

Spice Testbench

Testbench generation class for spice simulations.

class spice.testbench.testbench(parent=None, **kwargs)

This class generates all testbench contents. This class is utilized by the main spice class.

Executes init of testbench_common, thus having the same attributes and parameters.

Parameters:

**kwargs – See module testbench_common

property DEBUG

This fixes DEBUG prints in spice_iofile, by propagating the DEBUG flag of the parent entity.

copy_dspf()

property dcsourcestr

DC source definitions parsed from spice_dcsource objects instantiated in the parent entity.

Type:

str

property dspfincludecmd

String

DSPF-file inclusion string pointing to files corresponding to self.dspf in the parent entity.

property dut

Design under test

Type:

spice_module

export(**kwargs)

Internally called function to write the testbench to a file.

Parameters:

force (Bool, False) –

generate_contents()

Internally called function to generate testbench contents.

property includecmd

String

Subcircuit inclusion string pointing to generated subckt_* -file.

property inputsignals

Input signal definitions parsed from spice_iofile objects instantiated in the parent entity.

Type:

str

property libcmd

Library inclusion string. Parsed from self.spicecorner -dictionary in the parent entity, as well as ‘ELDOLIBFILE’ or ‘SPECTRELIBFILE’ global variables in TheSDK.config.

Type:

str

property misccmd

String

Miscellaneous command string corresponding to self.spicemisc -list in the parent entity.

property parameters

String

Spice parameters string parsed from self.spiceparameters -dictionary in the parent entity.

property plotcmd

All output IOs are mapped to plot or print statements in the testbench. Also manual plot commands through spice_simcmd.plotlist are handled here.

Type:

str

property simcmdstr

Simulation command definition parsed from spice_simcmd object instantiated in the parent entity.

Type:

str

property testbench_simulator

The simulator specific operation is defined with an instance of simulator specific class. Properties and methods return values from that class.

Type:

ngspice_testbench

Type:

eldo_testbench

Type:

spectre_testbench

Spice Testbench

Testbench generation class for spice simulations.

class spice.testbench_common.testbench_common(parent=None, **kwargs)

This class generates all testbench contents. This class is utilized by the main spice class.

property dcsources

bundle of DC sources inherited from parent

Type:

bundle

esc_bus(name, esc_colon=True)

Helper function to escape bus characters for Spectre simulations:

self.esc_bus('bus<3:0>')
# Returns 'bus\<3\:0\>'

property header

The header of the testbench

property iofiles

bundle of iofiles inherited from parent

Type:

bundle

property options

Spice options string parsed from self.spiceoptions -dictionary in the parent entity.

Type:

str

property simcmds

bundle of simulation commands inherited from parent

Type:

bundle

Spice IO-file

Provides spice file IO related attributes and methods for TheSDK spice.

Initially written by Okko Järvinen, 2020

class spice.spice_iofile.spice_iofile(parent=None, **kwargs)

Class to provide file IO for spice simulations. When created, adds a spice_iofile object to the parents iofile_bundle property. Accessible as iofile_bundle.Members[‘name’].

parent

The parent object initializing the spice_iofile instance. Default None

Type:

object

name

Name of the IO.

Type:

str

dir

Direction of the IO.

Type:

‘in’ or ‘out’

iotype

Type of the IO signal. Event type signals are time-value pairs (analog signal), whereas sample type signals are sampled by a clock signal (digital bus). Sample type signals can be used for discrete time & continuous amplitude outputs (sampled voltage for example), by setting iotype=’sample’ and ioformat=’volt’. Time type signals return a vector of timestamps corresponding to threshold crossings.

Type:

‘event’, ‘sample’ or ‘time’

ioformat

Formatting of the sampled signals. Digital output buses are formatted to unsigned integers when ioformat = ‘dec’. For ‘bin’, the digital output bus is returned as a string containing ones and zeros. When ioformat = ‘volt’, the output signal is sampled at the clock and the floating point value is returned. Voltage sampling is only supported for non-bus signals.

Type:

‘dec’, ‘bin’ or ‘volt’

sourcetype

Type of the source associated to a file. Default ‘V’.

Type:

‘V’, ‘I’ or ‘ISUB’

datatype

Inherited from the parent. If complex, the ioname is handled as a complex signal. Currently implemented only for writing the ouputs in testbenches and reading them in.

Type:

str

trigger

Name of the clock signal node in the Spice netlist. If a single string is given, the same clock signal is used for all bits/buses. If a list is given, and the length matches ionames list length, each ioname will be assigned its own clock. Applies only to sample type outputs.

Type:

str or list(str)

vth

Threshold voltage of the trigger signal and the bit rounding. Applies only to sample type outputs.

Type:

float

edgetype

Type of triggering edge. When time type signal is used, the edgetype values can define the extraction type as ‘risetime’ or ‘falltime’ additionally. Default ‘rising’.

Type:

‘rising’, ‘falling’ or ‘both’

after

Initial delay added to the input signal (sample) or time extraction (time). Useful for ignoring inital settling, for example. Applies only to sample and time outputs. Default 0.

Type:

float

big_endian

Flag to read the extracted bus as big-endian. Applies only to sample type outputs. Default False.

Type:

bool

rs

Sample rate of the sample type input. Default None.

Type:

float

vhi

High bit value of sample type input. Default 1.0.

Type:

float

vlo

Low bit value of sample type input. Default 0.

Type:

float

tfall

Falltime of sample type input. Default 5e-12.

Type:

float

trise

Risetime of sample type input. Default 5e-12.

Type:

float

strobe

True if the event type IO uses only the strobe filtered values. False if the IO contains all of the values simulated values (not consistently strobed). Default False.

Type:

bool

Examples

Initiated in parent as:

_=spice_iofile(self,name='foobar')

Defining analog input voltage signals from python to spice:

_=spice_iofile(self,name='inp',dir='in',iotype='event',sourcetype='V',ionames='INP')
_=spice_iofile(self,name='inn',dir='in',iotype='event',sourcetype='V',ionames='INN')

Defining time-domain output signal containing rising edge threshold crossing timestamps of an analog clock signal:

_=spice_iofile(self,name='clk_rise',dir='out',iotype='time',sourcetype='V',
               ionames='CLK',edgetype='rising',vth=self.vdd/2)

Defining digital output signal triggered with a falling edge of the analog clock:

_=spice_iofile(self,name='dout',dir='out',iotype='sample',sourcetype='V',
               ioformat='bin',ionames='DOUT<7:0>',edgetype='falling',
               vth=self.vdd/2,trigger='CLK')

Defining a discrete time & continuous amplitude output signal triggered with a rising edge of the analog clock. The iofile returns a 2D-vector similar to ‘event’ type signals:

_=spice_iofile(self,name='sampled_input',dir='out',iotype='sample',sourcetype='V',
               ioformat='volt',ionames='INP',edgetype='rising',
               vth=self.vdd/2,trigger='CLK')

Defining digital input signal with decimal format. The input vector is a list of integers, which get converted to binary bus of 4-bits (inferred from ‘CTRL<3:0>’). The values are changed at 1 MHz interval in this example.:

_=spice_iofile(self,name='ctrl',dir='in',iotype='sample',ionames='CTRL<3:0>',rs=1e6,
               vhi=self.vdd,trise=5e-12,tfall=5e-12,ioformat='dec')

Parameters:

• parent (object, None) – The parent object initializing the iofile instance. Default None

• **kwargs –

  name: str

  Name of the file. Appended with random string during the simulation.

  param: str, -g g_file

  The string defining the testbench parameter to be be passed to the simulator at command line.

property DEBUG

This fixes DEBUG prints in spice_iofile, by propagating the DEBUG flag of the parent entity.

append_to_data(arr=None, bits=False, buswidth=None)

Helper method to append array to self.Data.

The array(s) are padded with np.nan when bits=False, and ‘UUUU’ when bits=True. This is called automatically for time and sample type IOs.

property file

List<str>

List containing filepaths to files associated with this spice_iofile. For digital buses or arrays of signals, the list contains multiple files which are automatically handled together. These filepaths are set automatically.

interp_crossings(data, vth, nint, edgetype)

Helper method called for ‘time’ and ‘sample’ type outputs.

Interpolates the requested threshold crossings (rising or falling) from the ‘event’ type input signal. Returns the time-stamps of the crossing instants in a 1D-vector.

Parameters:

• data (ndarray) – Input data array. Expected an ‘event’ type 2D-vector where first column is time and second is voltage.

• vth (float) – Threshold voltage.

• nint (int) – Interpolation factor. The two closest points on each side of a threshold crossing are used for linear interpolation endpoints, where nint points are added to find as close x-value of the threshold crossing as possible.

• edgetype (str) – Direction of the crossing: ‘rising’, ‘falling’ or ‘both’.

Returns:

1D-vector with time-stamps of interpolated threshold crossings.

Return type:

ndarray

property ionames

List<str>

Set by argument ‘ionames’. This property casts the given argument to a list if needed.

parse_io_from_file(filepath, start, stop, dtype, labels, queue)

Parse specific lines from a spectre print file.

This is wrapped to a function to allow parallelism.

read(**kwargs)

Function to read files associated with this spice_iofile.

remove()

Remove the files

sample_signal(signal, trigger, nint=1)

Helper method called for ‘sample’ type outputs.

Finds the signal y-values at time instants defined by the clock signal (trigger).

Parameters:

• data (ndarray) – Input data array. Expected an ‘event’ type 2D-vector where first column is time and second is voltage.

• vth (float) – Threshold voltage.

• nint (int) – Interpolation factor. The two closest points on each side of a threshold crossing are used for linear interpolation endpoints, where nint points are added to find as close x-value of the threshold crossing as possible.

• edgetype (str) – Direction of the crossing: ‘rising’, ‘falling’ or ‘both’.

Returns:

1D-vector with time-stamps of interpolated threshold crossings.

Return type:

ndarray

write(**kwargs)

Function to write files associated with this spice_iofile.

Spice Simulation Command

Class for spice simulation commands.

Initially written by Okko Järvinen, 9.1.2020

class spice.spice_simcmd.spice_simcmd(parent, **kwargs)

Class to provide simulation command parameters to spice testbench. When instantiated in the parent class, this class automatically attaches spice_simcmd objects to simcmd_bundle -bundle in testbench.

parent

The parent object initializing the spice_simcmd instance. Default None.

Type:

object

sim

Simulation type.

Type:

‘tran’ or ‘dc’

plotlist

List of node names or operating points to be plotted. Node names follow simulator syntax. For Eldo, the voltage/current specifier is expected:

self.plotlist = ['v(OUT)','v(CLK)']

For Spectre, the node name is enough:

self.plotlist = ['OUT','CLK']

Note

Below applies only for Spectre!

When capturing operating point information with Spectre, adding the instance name to plotlist saves all operating points for the device, e.g:

self.plotlist = [XTB_NAME.XSUBCKT/M0]

saves all operating points defined by the model for the device M0 in subckt XSUBCKT.

Wildcards are supported, but should be used with caution as the output file can quickly become excessively large. For example to capture the gm of all transistor use:

self.plotlist = [*:gm]

It is highly recommended to exclude the devices that are not needed from the output to reduce file size. Examples of such devices are RC-parasitics (include option savefilter=’rc’ in self.spiceoptions to exclude them) and dummy transistors. See excludelist below.

Type:

list(str)

excludelist

Applies for Spectre only! List of device names NOT to be included in the output report. Wildcards are supported. Exclude list is especially useful for DC simulations when specifiying outputs with wildcards.

For example, when capturing gm for all transistors, use exclude list to exclude all dummy transistors with:

self.excludelist = [XTB_NAME*DUMMY_ID*],

where DUMMY_ID is extraction tool / runset specific dummy identifier.

Type:

list(str)

sweep

DC & Spectre models only. Name of parameter to be swept in DC analysis. If given as a list, performs a nested sweep of the parameters defined by the list (first element will be the outermost sweep). For example:

_spice_simcmd(sim=’dc’,sweep=’temp’,swpstart=27,swpstop=87)

sweeps the top-level parameter temp (temperature) from 27 to 87 in 10 degree increments.

Type:

List[str]

subcktname

If given, sweeps the parameter defined by property sweep from the subcircuit given by this property. For example:

_=spice_simcmd(sim='dc',sweep='Vb',subcktname='XSUBCKT',
               swpstart=0.1,swpstop=1.5,step=0.05)

sweeps the Vb parameter from subcircuit XSUBCKT from 0.1 volts to 1.5 volts with 0.05 volt increments.

Type:

List[str]

devname

If given, sweeps the parameter defined by property sweep from the device given by this property. For example:

_=spice_simcmd(sim='dc', sweep='w', deviceswp='XSUBCKT.XNMOS',
               swpstart='10u', swpstop='14u', step='0.1u')

sweeps the width of transistor XNMOS of subckt XSUBCKT from 10u to 14u in 0.1u increments.

Type:

List[str]

swpstart

Starting point of DC sweep. Default 0.

Type:

int, float or str

swpstop

Stop point of DC sweep. Default 0.

Type:

int, float or str

swpstep

Step size of the sweep simulation. Default 10.

Type:

int, float or str

tprint

Print interval. Default 1e-12 (same as ‘1p’).

Type:

float or str

tstop

Transient simulation duration. When not defined, the simulation time is the duration of the longest input signal.

Type:

float or str

uic

Use initial conditions flag. Default False.

Type:

bool

noise

Noise transient flag. Default False.

Type:

bool

fmin

Minimum noise frequency. Default 1 (Hz).

Type:

float or str

fmax

Maximum noise frequency. Default 5e9.

Type:

float or str

fscale

Logarithmic or linear scale for frequency. Default ‘log’.

Type:

‘log’ or ‘lin’

fpoints

Number of points for frequency analysis. Default 0.

Type:

int

fstepsize

Step size for AC analysis, if scale if ‘lin’. If fscale is ‘log’, this parameter gives number of points per decade. Default 0.

Type:

int

seed

Random generator seed for noise transient. Default None (random).

Type:

int

method

Transient integration method. Default None (Spectre takes method from errpreset).

Type:

str

cmin

Spectre cmin parameter: this much cap from each node to ground. Might speed up simulation. Default None (not used).

Type:

float

mc

Enable Monte Carlo simulation. This flag will enable Monte Carlo modeling for a single simulation. It will NOT execute multiple runs or do any statistical analysis. Intended use case is to generate a group of entities in the testbench with each having mc=True, simulating them in parallel (see run_parallel() of thesdk-class), post-processing results in Python.

Type:

bool

mc_seed

Random seed for the Monte Carlo instance. Default None (random seed).

Type:

int

model_info

For Spectre only! If true, print model parameters to raw-file.

Type:

bool

maxstep

Maximum time step Spectre simulator will use during transient analysis

Type:

float

step

According to Spectre: minimum time step used by the simulator solely to maintain the aesthetics of the computed waveforms.

Type:

float

strobeperiod

For Spectre only! Forces simulator to write output data to file at interval defined by this parameter. Note that the simulator still outputs points between the sampling points.

Type:

float

skipstart

For Spectre only! Delay between start of transient simulation and first strobed output, if strobedelay is None.

Type:

float

strobedelay

For Spectre only! Delay between skipstart and the first strobe point.

Type:

float

Examples

Initiated in parent as:

_=spice_simcmd(self,sim='tran',tprint=1e-12,tstop='10n',
               uic=True,noise=True,fmin=1,fmax=5e9)

For a simple transient with inferred simulation duration:

_=spice_simcmd(self,sim='tran')

Spice Module

Class for Spice netlist parsing.

class spice.spice_module.spice_module(**kwargs)

This class parses source netlist for subcircuits and handles the generation of a separate pruned subckt_* -file. This class is internally utilized by the spice_testbench module.

property custom_subckt_name

Custom name of the subcircuit to look from from the netlist file during parsing for ‘subckt’ property. Enables using compatible (in term sof IOs paremeters) netlists defined for designs of different name.

Type:

str

Example

Most common use case of module is a dut in a testbench. There you can set this parameter before execution as:

self.spice_tb.dut.custom_subckt_name = 'some_name'
self.run_spice()

export_subckts(**kwargs)

Internally called function to write the parsed subcircuit definitions to a file.

Parameters:

• file (str) – Path to file where to write.

• force (Bool, False) – Force writing

property file

Filepath to the entity’s spice netlist source file (i.e. ‘./spice/entityname.scs’).

Type:

str

property instance

The subcircuit instance to be placed in the testbench. Parsed from the subckt property

Type:

str

property name

Entity name

Type:

str

property subckt

The contents of the subcircuit definition file of the entity. Extract the definitions form the source netlist. The source netlist when accessed. Can be written to the subckt_file with export_subckt method.

Type:

str

Ngspice

Simulator specific definitions for Ngspice

Initially written by Marko Kosunen, 2021

class spice.ngspice.ngspice.ngspice(parent=None, **kwargs)

This class is used as instance in simulatormodule property of spice class. Contains language dependent definitions.

Parameters:

• parent (object, None (mandatory to define). TheSyDeKick parent entity object for this simulator class.) –

• **kwargs – None

property cmdfile_ext

Extension of the command file

Type:

str

property commentchar

Comment character of the simulator

Type:

str

property commentline

Comment line for the simulator

Type:

str

property csvskip

int

Type:

Needs documentation. Lines skipped in result file

property dcsource_declaration

DC source declaration

Type:

str

property dspfinclude

Netlist dspf-file include string

Type:

str

property eventoutdelim

Delimiter for the events

Type:

str

property include

Netlist include string

Type:

str

property lastline

Last line of the simulator command file

Type:

str

property nprocflag

String for defining multithread execution

Type:

str

property option

Netlist option definition string

Type:

str

property parameter

Netlist parameter definition string

Type:

str

property plflag

Postlayout simulation accuracy/RC reduction flag.

property plotprogcmd

Command to be run for interactive simulations.

Type:

str

property plotprogram

String

Sets the program to be used for visualizing waveform databases.

read_oppts()

Internally called function to read the DC operating points of the circuit TODO: Implement for Eldo as well.

property resultfile_ext

Extension of the result file

Type:

str

run_plotprogram()

Starting a parallel process for waveform viewer program.

The plotting program command can be set with ‘plotprogram’. Tested for spectre and eldo.

property simulatorcmd

Simulator execution command (Default: ‘ngspice’)

Type:

str

property spicecmd

Simulation command string to be executed on the command line. Automatically generated.

Type:

str

property subckt

Subcircuit include string

Type:

str

property syntaxdict

Dictionary

Internally used dictionary for syntax conversions

Eldo

Eldo simulation interface package for TheSyDeKick.

Initially written by Okko Järvinen, 2019

class spice.eldo.eldo.eldo(parent=None, **kwargs)

This class is used as instance in spice_simulatormodule property of spice class. Contains simulator dependent definitions.

Parameters:

• parent (object, None (mandatory to define). TheSyDeKick parent entity object for this simulator class.) –

• **kwargs – None

property cmdfile_ext

str

Type:

Extension of the command file

property commentchar

str

Type:

Comment character of the simulator

property commentline

str

Type:

Comment line for the simulator

property csvskip

int

Type:

Needs documentation. Lines skipped in result file

property dcsource_declaration

str

Type:

DC source declaration

property dspfinclude

str

Type:

Netlist dspf-file include string

property eventoutdelim

str

Type:

Delimiter for the events

property include

str

Type:

Netlist include string

property lastline

str

Type:

Last line of the simulator command file

property nprocflag

str

Type:

String for defining multithread execution

property option

str

Type:

Netlist option definition string

property parameter

str

Type:

Netlist parameter definition string

property plflag

Postlayout simulation accuracy/RC reduction flag.

property plotprogcmd

Command to be run for interactive simulations.

Type:

str

property plotprogram

String

Sets the program to be used for visualizing waveform databases. Options are ezwave (default) or viva.

read_oppts()

Internally called function to read the DC operating points of the circuit TODO: Implement for Eldo as well.

property resultfile_ext

str

Type:

Extension of the result file

run_plotprogram()

Starting a parallel process for waveform viewer program.

The plotting program command can be set with ‘plotprogram’. Tested for spectre and eldo.

property simulatorcmd

str

Type:

Simulator execution command

property spicecmd

String

Simulation command string to be executed on the command line. Automatically generated.

property subckt

str

Type:

Subcircuit include string

property syntaxdict

Spectre

Spectre simulation interface package for Spectre for TheSyDeKick.

Initially written by Okko Järvinen, 2019

class spice.spectre.spectre.spectre(parent=None, **kwargs)

This class is used as instance in spice_simulatormodule property of spice class. Contains simulator dependent definitions.

Parameters:

• parent (object, None (mandatory to define). TheSyDeKick parent entity object for this simulator class.) –

• **kwargs – None

property cmdfile_ext

str

Type:

Extension of the command file

property commentchar

str

Type:

Comment character of the simulator

property commentline

str

Type:

Comment line for the simulator

property csvskip

int

Type:

Needs documentation. Lines skipped in result file

property dcsource_declaration

str

Type:

DC source declaration

property dspfinclude

str

Type:

Netlist dspf-file include string

property errpreset

String

Global accuracy parameter for Spectre simulations. Options include ‘liberal’, ‘moderate’ and ‘conservative’, in order of rising accuracy. You can set this by accesssing spice langmodule

Example

self.spice_langmodule.errpreset=’conservative’

property eventoutdelim

str

Type:

Delimiter for the events

property include

str

Type:

Netlist include string

property lastline

str

Type:

Last line of the simulator command file

property nprocflag

str

Type:

String for defining multithread execution

property option

str

Type:

Netlist option definition string

property parameter

str

Type:

Netlist parameter definition string

property plflag

Postlayout simulation accuracy/RC reduction flag. See: https://community.cadence.com/cadence_blogs_8/b/cic/posts/spectre-optimizing-spectre-aps-performance

property plflag_simcmd_prefix

Simulator specific prefix for enabling postlayout optimization Postfix comes from self.plflag (user defined)

property plotprogcmd

Command to be run for interactive simulations.

Type:

str

property plotprogram

String

Sets the program to be used for visualizing waveform databases. Options are ezwave (default) or viva.

read_oppts()

Internally called function to read the DC operating points of the circuit TODO: Implement for Eldo as well.

property resultfile_ext

str

Type:

Extension of the result file

run_plotprogram()

Starting a parallel process for waveform viewer program.

The plotting program command can be set with ‘plotprogram’ property.

property simulatorcmd

str

Type:

Simulator execution command

property spicecmd

String

Simulation command string to be executed on the command line. Automatically generated.

property subckt

str

Type:

Subcircuit include string

property syntaxdict

Ngspice Testbench

Simulators sepecific testbench generation class for Ngspice.

class spice.ngspice.ngspice_testbench.ngspice_testbench(parent=None, **kwargs)

Executes init of testbench_common, thus having the same attributes and parameters.

Parameters:

**kwargs – See module testbench_common

property dcsourcestr

DC source definitions parsed from spice_dcsource objects instantiated in the parent entity.

Type:

str

property inputsignals

Input signal definitions parsed from spice_iofile objects instantiated in the parent entity.

Type:

str

property libcmd

Library inclusion string. Parsed from self.spicecorner -dictionary in the parent entity, as well as ‘ELDOLIBFILE’ or ‘SPECTRELIBFILE’ global variables in TheSDK.config.

Type:

str

property options

String

Spice options string parsed from self.spiceoptions -dictionary in the parent entity.

property plotcmd

All output IOs are mapped to plot or print statements in the testbench. Also manual plot commands through spice_simcmd.plotlist are handled here.

Type:

str

property simcmdstr

String

Simulation command definition parsed from spice_simcmd object instantiated in the parent entity.

Eldo Testbench

Simulators sepecific testbench generation class for Ngspice.

class spice.eldo.eldo_testbench.eldo_testbench(parent=None, **kwargs)

Executes init of testbench_common, thus having the same attributes and parameters.

Parameters:

**kwargs – See module testbench_common

property dcsourcestr

String

DC source definitions parsed from spice_dcsource objects instantiated in the parent entity.

property inputsignals

Input signal definitions parsed from spice_iofile objects instantiated in the parent entity.

Type:

str

property libcmd

Library inclusion string. Parsed from self.spicecorner -dictionary in the parent entity, as well as ‘ELDOLIBFILE’ or ‘SPECTRELIBFILE’ global variables in TheSDK.config.

Type:

str

property options

String

Spice options string parsed from self.spiceoptions -dictionary in the parent entity.

property plotcmd

All output IOs are mapped to plot or print statements in the testbench. Also manual plot commands through spice_simcmd.plotlist are handled here.

Type:

str

property simcmdstr

Simulation command definition parsed from spice_simcmd object instantiated in the parent entity.

Type:

str

Spectre Testbench

Simulators sepecific testbench generation class for Spectre.

class spice.spectre.spectre_testbench.spectre_testbench(parent=None, **kwargs)

Executes init of testbench_common, thus having the same attributes and parameters.

Parameters:

**kwargs – See module testbench_common

property dcsourcestr

DC source definitions parsed from spice_dcsource objects instantiated in the parent entity.

Type:

str

property inputsignals

Input signal definitions parsed from spice_iofile objects instantiated in the parent entity.

Type:

str

property libcmd

Library inclusion string. Parsed from self.spicecorner -dictionary in the parent entity, as well as ‘ELDOLIBFILE’ or ‘SPECTRELIBFILE’ global variables in TheSDK.config.

Type:

str

property num_cols

Number of columns in the output file, when using Spectre. Each signal takes 1 column (unless it is complex, then two). Each column is 15 bit wide, hence number of columns is multiplied by 15.

property options

String

Spice options string parsed from self.spiceoptions -dictionary in the parent entity.

property plotcmd

All output IOs are mapped to plot or print statements in the testbench. Also manual plot commands through spice_simcmd.plotlist are handled here.

Type:

str

property simcmdstr

Simulation command definition parsed from spice_simcmd object instantiated in the parent entity.

Type:

str

Spice DC Source

Class for generating DC voltage/current sources in the Spectre or Eldo testbench.

Initially written by Okko Järvinen, 9.1.2020

class spice.spice_dcsource.spice_dcsource(parent, **kwargs)

Class to provide DC source definitions to spice testbench. When instantiated in the parent class, this class automatically attaches spice_dcsource objects to dcsource_bundle -bundle in testbench.

parent

The parent object initializing the spice_dcsource instance. Default None.

Type:

object

name

Name of the source.

Type:

str

value

Value of the source.

Type:

float

paramname

To parameterize the DC source, provide this value during instantiation. The parameter will be automatically added to spiceparameters with the default value of self.value.

Type:

str

sourcetype

Type of the DC source. Either ‘V’ for voltage or ‘I’ for current.

Type:

‘V’ or ‘I’

pos

Name of the positive net in the netlist.

Type:

str

neg

Name of the negative net in the netlist.

Type:

str

extract

Flag the source for transient current and power consumption extraction. Extracted currents and powers are accessible through dictionaries self.currents and self.powers in the parent object. Default False.

Type:

bool

ext_start

Time to start extracting average transient power consumption. Default is 0.

Type:

float

ext_stop

Time to stop extracting average transient power consumption. Default is simulation end time.

Type:

float

noise

Enable the noise contribution of this source (only when transient noise is enabled). Default is True.

Type:

bool

ramp

Ramp up the source from 0 to value in ramp seconds. Default is 0 (no ramping).

Type:

float

Examples

A voltage source connected between circuit nodes ‘VDD’ and ‘VSS’, for which power and current consumptions are extracted in transient simulation. Initiated in parent as:

_=spice_dcsource(self,name='supply',value=1.0,extract=True,pos='VDD',neg='VSS')
_=spice_dcsource(self,name='ground',value=0,pos='VSS',neg='0') # Ground 'source'

A bias current flowing from ‘VDD’ to node ‘IBIAS’:

_=spice_dcsource(self,name='bias',sourcetype='I',value=25e-6,pos='VDD',neg='IBIAS')

property ext_file

String

Optional filepath for extracted transient current when self.extract=True.