###################################################################################################
#
# PySpice - A Spice Package for Python
# Copyright (C) 2014 Fabrice Salvaire
#
# This program is free software: you can redistribute it and/or modify
# it under the terms of the GNU General Public License as published by
# the Free Software Foundation, either version 3 of the License, or
# (at your option) any later version.
#
# This program is distributed in the hope that it will be useful,
# but WITHOUT ANY WARRANTY; without even the implied warranty of
# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the
# GNU General Public License for more details.
#
# You should have received a copy of the GNU General Public License
# along with this program. If not, see <http://www.gnu.org/licenses/>.
#
####################################################################################################
"""This modules provides classes to generate the simulation part of the Spice desk, i.e. the line
starting by a dot at the end of the desk.
.. warning:: Simulation features depend of the simulator.
"""
####################################################################################################
import logging
import os
####################################################################################################
from ..Tools.StringTools import join_list, join_dict, str_spice
from ..Unit import as_Degree, u_Degree
from .AnalysisParameters import (
ACAnalysisParameters,
AcSensitivityAnalysisParameters,
DCAnalysisParameters,
DcSensitivityAnalysisParameters,
DistortionAnalysisParameters,
MeasureParameters,
NoiseAnalysisParameters,
OperatingPointAnalysisParameters,
PoleZeroAnalysisParameters,
TransferFunctionAnalysisParameters,
TransientAnalysisParameters,
)
####################################################################################################
_module_logger = logging.getLogger(__name__)
####################################################################################################
[docs]class Simulation:
"""Define and generate the Spice instruction to perform a simulation.
Constructor Parameters
----------------------
Simulation temperatures are set by default to 27°C, you can change theses values using the
parameter `temperature` and `nominal_temperature`, respectively.
Analysis Method Parameters
--------------------------
For *ac* and *transient* analyses, the user must specify a list of nodes using the *probes* key
argument.
You can log the desk using the parameter `log_desk` set to `True`.
By default the analysis method runs the simulation and return the result, you can disable this
feature using the parameter `run` set to `False`.
.. warning:: In some cases NgSpice can perform several analyses one after the other. This case
is partially supported.
"""
_logger = _module_logger.getChild('Simulation')
DEFAULT_TEMPERATURE = u_Degree(27)
##############################################
def __init__(self, simulator, circuit, **kwargs):
self._simulator = simulator
self._circuit = circuit
self._options = {} # .options
self._measures = [] # .measure
self._initial_condition = {} # .ic
self._node_set = {} # .nodeset
self._saved_nodes = set()
self._analyses = {}
self.temperature = kwargs.get('temperature', self.DEFAULT_TEMPERATURE)
self.nominal_temperature = kwargs.get('nominal_temperature', self.DEFAULT_TEMPERATURE)
##############################################
def __getstate__(self):
# Pickle: get state
state = self.__dict__.copy()
# state['_simulator'] = self._simulator.__class__.__name__
state['_simulator'] = self._simulator._AS_SIMULATOR
# state['_circuit'] = ...
return state
##############################################
def __setstate__(self, state):
# Pickle: restore state
self.__dict__.update(state)
# Fixme: ok ??? duplicate simulator ???
from .Simulator import Simulator
self.__simulator = Simulator.factory(simulator=state['_simulator'])
##############################################
@property
def circuit(self):
return self._circuit
@property
def simulator(self):
return self._simulator
##############################################
[docs] def options(self, *args, **kwargs):
for item in args:
self._options[str(item)] = None
for key, value in kwargs.items():
self._options[str(key)] = str_spice(value)
##############################################
@property
def temperature(self):
return self._options['TEMP']
@temperature.setter
def temperature(self, value):
self._options['TEMP'] = as_Degree(value)
##############################################
@property
def nominal_temperature(self):
return self._options['TNOM']
@nominal_temperature.setter
def nominal_temperature(self, value):
self._options['TNOM'] = as_Degree(value)
##############################################
@staticmethod
def _make_initial_condition_dict(kwargs):
return {f"V({key})": str_spice(value) for key, value in kwargs.items()}
##############################################
[docs] def initial_condition(self, **kwargs):
"""Set initial condition for voltage nodes.
Usage::
simulator.initial_condition(node_name=value, ...)
General form::
.ic v(node_name)=value ...
The `.ic` line is for setting transient initial conditions. It has two different
interpretations, depending on whether the uic parameter is specified on the `.tran` control
line, or not. One should not confuse this line with the `.nodeset` line. The `.nodeset`
line is only to help DC convergence, and does not affect the final bias solution (except for
multi-stable circuits). The two indicated interpretations of this line are as follows:
1. When the uic parameter is specified on the `.tran` line, the node voltages specified on
the `.ic` control line are used to compute the capacitor, diode, BJT, JFET, and MOSFET
initial conditions. This is equivalent to specifying the `ic=...` parameter on each
device line, but is much more convenient. The `ic=...` parameter can still be specified
and takes precedence over the `.ic` values. Since no dc bias (initial transient)
solution is computed before the transient analysis, one should take care to specify all
dc source voltages on the `.ic` control line if they are to be used to compute device
initial conditions.
2. When the uic parameter is not specified on the `.tran` control line, the DC bias (initial
transient) solution is computed before the transient analysis. In this case, the node
voltages specified on the `.ic` control lines are forced to the desired initial values
during the bias solution. During transient analysis, the constraint on these node
voltages is removed. This is the preferred method since it allows Ngspice to compute a
consistent dc solution.
"""
d = self._make_initial_condition_dict(kwargs)
self._initial_condition.update(d)
##############################################
[docs] def node_set(self, **kwargs):
"""Specify initial node voltage guesses.
Usage::
simulator.node_set(node_name=value, ...)
General form::
.nodeset v(node_name)=value ...
.nodeset all=val
The `.nodeset` line helps the program find the DC or initial transient solution by making a
preliminary pass with the specified nodes held to the given voltages. The restrictions are
then released and the iteration continues to the true solution. The `.nodeset` line may be
necessary for convergence on bistable or astable circuits. `.nodeset all=val` sets all
starting node voltages (except for the ground node) to the same value. In general, the
`.nodeset` line should not be necessary.
"""
d = self._make_initial_condition_dict(kwargs)
self._node_set.update(d)
##############################################
[docs] def save(self, *args):
# Fixme: pass Node for voltage node, Element for source branch current, ...
"""Set the list of saved vectors.
If no *.save* line is given, then the default set of vectors is saved (node voltages and
voltage source branch currents). If *.save* lines are given, only those vectors specified
are saved.
Node voltages may be saved by giving the node_name or *v(node_name)*. Currents through an
independent voltage source (including inductor) are given by *i(source_name)* or
*source_name#branch*. Internal device data are accepted as *@dev[param]*.
If you want to save internal data in addition to the default vector set, add the parameter
*all* to the additional vectors to be saved.
"""
self._saved_nodes |= set(*args)
##############################################
[docs] def save_internal_parameters(self, *args):
"""This method is similar to`save` but assume *all*."""
# Fixme: ok ???
self.save(list(args) + ['all'])
##############################################
@property
def save_currents(self):
""" Save all currents. """
return self._options.get('SAVECURRENTS', False)
@save_currents.setter
def save_currents(self, value):
if value:
self._options['SAVECURRENTS'] = True
else:
del self._options['SAVECURRENTS']
##############################################
[docs] def reset_analysis(self):
self._analyses.clear()
##############################################
[docs] def analysis_iter(self):
# Fixme: -> analyses / item()
# used for ???
return self._analyses.values()
##############################################
def _add_analysis(self, analysis_parameters):
self._analyses[analysis_parameters.analysis_name] = analysis_parameters
##############################################
def _add_measure(self, measure_parameters):
self._measures.append(measure_parameters)
##############################################
def _impl_operating_point(self):
"""Compute the operating point of the circuit with capacitors open and inductors shorted."""
self._add_analysis(OperatingPointAnalysisParameters())
##############################################
def _impl_dc_sensitivity(self, output_variable):
"""Compute the sensitivity of the DC operating point of a node voltage or voltage-source
branch current to all non-zero device parameters.
Examples of usage::
analysis = simulator.dc_sensitivity('v(out)')
Spice syntax:
.. code:: spice
.sens outvar
Examples:
.. code:: spice
.sens V(1, OUT)
.sens I(VTEST)
"""
self._add_analysis(DcSensitivityAnalysisParameters(output_variable))
##############################################
def _impl_ac_sensitivity(self, output_variable, variation, number_of_points, start_frequency, stop_frequency):
"""Compute the sensitivity of the AC values of a node voltage or voltage-source branch
current to all non-zero device parameters.
Examples of usage::
analysis = simulator.ac_sensitivity(...)
Spice syntax:
.. code::
.sens outvar ac dec nd fstart fstop
.sens outvar ac oct no fstart fstop
.sens outvar ac lin np fstart fstop
Spice examples:
.. code::
.sens V(OUT) AC DEC 10 100 100 k
"""
self._add_analysis(
AcSensitivityAnalysisParameters(
output_variable,
variation, number_of_points, start_frequency, stop_frequency
))
##############################################
def _impl_dc(self, **kwargs):
"""Compute the DC transfer fonction of the circuit with capacitors open and inductors shorted.
Examples of usage::
analysis = simulator.dc(Vinput=slice(-2, 5, .01))
analysis = simulator.dc(Ibase=slice(0, 100e-6, 10e-6))
analysis = simulator.dc(Vcollector=slice(0, 5, .1), Ibase=slice(micro(10), micro(100), micro(10))) # broken ???
Spice syntax:
.. code:: spice
.dc src_name vstart vstop vincr [ src2 start2 stop2 incr2 ]
*src_name* is the name of an independent voltage or a current source, a resistor or the
circuit temperature.
*vstart*, *vstop*, and *vincr* are the starting, final, and incrementing values respectively.
A second source (*src2*) may optionally be specified with associated sweep parameters. In
this case, the first source is swept over its range for each value of the second source.
Spice examples:
.. code:: spice
.dc VIN 0 .2 5 5.0 0.25
.dc VDS 0 10 .5 VGS 0 5 1
.dc VCE 0 10 .2 5 IB 0 10U 1U
.dc RLoad 1k 2k 100
.dc TEMP -15 75 5
"""
self._add_analysis(DCAnalysisParameters(**kwargs))
##############################################
def _impl_ac(self, variation, number_of_points, start_frequency, stop_frequency):
# fixme: concise keyword ?
"""Perform a small-signal AC analysis of the circuit where all non-linear devices are linearized
around their actual DC operating point.
Examples of usage::
analysis = simulator.ac(start_frequency=10@u_kHz, stop_frequency=1@u_GHz, number_of_points=10, variation='dec')
Note that in order for this analysis to be meaningful, at least one independent source must
have been specified with an AC value. Typically it does not make much sense to specify more
than one AC source. If you do, the result will be a superposition of all sources, thus
difficult to interpret.
Spice examples:
.. code::
.ac dec nd fstart fstop
.ac oct no fstart fstop
.ac lin np fstart fstop
The parameter *variation* must be either `dec`, `oct` or `lin`.
"""
self._add_analysis(
ACAnalysisParameters(
variation, number_of_points, start_frequency, stop_frequency
))
##############################################
def _impl_measure(self, analysis_type, name, *args):
"""Add a measure in the circuit.
Examples of usage::
simulator.measure('TRAN', 'tdiff', 'TRIG AT=10m', 'TARG v(n1) VAL=75.0 CROSS=1')
simulator.measure('tran', 'tdiff', 'TRIG AT=0m', f"TARG par('v(n1)-v(derate)') VAL=0 CROSS=1")
Note: can be used with the .options AUTOSTOP to stop the simulation at Trigger.
Spice syntax:
.. code:: spice
.meas tran tdiff TRIG AT=0m TARG v(n1) VAL=75.0 CROSS=1
"""
self._add_measure(MeasureParameters(analysis_type, name, *args))
##############################################
def _impl_transient(self, step_time, end_time, start_time=0, max_time=None, use_initial_condition=False):
"""Perform a transient analysis of the circuit.
Examples of usage::
analysis = simulator.transient(step_time=1@u_us, end_time=500@u_us)
analysis = simulator.transient(step_time=source.period/200, end_time=source.period*2)
Spice syntax:
.. code:: spice
.tran tstep tstop <tstart <tmax>> <uic>
"""
self._add_analysis(
TransientAnalysisParameters(
step_time, end_time, start_time, max_time,
use_initial_condition
))
##############################################
def _impl_polezero(self, node1, node2, node3, node4, tf_type, pz_type):
"""Perform a Pole-Zero analysis of the circuit.
node1, node2 - Input node pair.
node3, node4 - Output node pair
tf_type - should be `cur` for current or `vol` for voltage
pz_type - should be `pol` for pole, `zer` for zero, or `pz` for combined pole zero analysis.
See section 15.3.6 of ngspice manual.
Spice syntax:
.. code:: spice
.tran tstep tstop <tstart <tmax>> <uic>
.pz node1 node2 node3 node4 cur pol
.pz node1 node2 node3 node4 cur zer
.pz node1 node2 node3 node4 cur pz
.pz node1 node2 node3 node4 vol pol
.pz node1 node2 NODE3 node4 vol zer
.pz node1 node2 node3 node4 vol pz
Examples:
.. code:: spice
.pz 1 0 3 0 cur pol
.pz 2 3 5 0 vol zer
.pz 4 1 4 1 cur pz
"""
# do some rudimentary parameter checking.
if tf_type not in ('cur', 'vol'):
raise NameError("polezero type must be 'cur' or 'vol'")
if pz_type not in ('pol', 'zer', 'pz'):
raise NameError("pz_type must be 'pol' or 'zer' or 'pz'")
self._add_analysis(
PoleZeroAnalysisParameters(node1, node2, node3, node4, tf_type, pz_type)
)
##############################################
def _impl_noise(self, output_node, ref_node, src, variation, points, start_frequency, stop_frequency, points_per_summary=None):
"""Perform a Pole-Zero analysis of the circuit.
output_node, ref_node - output node pair.
src - signal source, typically an ac voltage input.
variation - must be 'dec' or 'lin' or 'oct' for decade, linear, or octave.
points, start_frequency, stop_frequency - number of points, start and stop frequencies.
points_per_summary - if specified, the noise contributions of each noise generator is produced every points_per_summary frequency points.
See section 15.3.4 of ngspice manual.
Spice syntax:
General form:
.. code:: spice
.noise v(output <,ref >) src ( dec | lin | oct ) pts fstart fstop <pts_per_summary >
Examples:
.. code:: spice
.noise v(5) VIN dec 10 1kHz 100 MEG
.noise v(5 ,3) V1 oct 8 1.0 1.0 e6 1
"""
# do some rudimentary parameter checking.
# Fixme: mixin
if variation not in ('dec', 'lin', 'oct'):
raise NameError("variation must be 'dec' or 'lin' or 'oct'")
output = 'V({},{})'.format(output_node, ref_node)
self._add_analysis(
NoiseAnalysisParameters(output, src, variation, points, start_frequency, stop_frequency, points_per_summary)
)
##############################################
def _impl_transfer_function(self, outvar, insrc):
"""The python arguments to this function should be two strings, outvar and insrc.
ngspice documentation as follows:
General form:
.. code:: spice
.tf outvar insrc
Examples:
.. code:: spice
.tf v(5, 3) VIN
.tf i(VLOAD) VIN
The .tf line defines the small-signal output and input for the dc small-signal
analysis. outvar is the small signal output variable and insrc is the small-signal input
source. If this line is included, ngspice computes the dc small-signal value of the transfer
function (output/input), input resistance, and output resistance. For the first example,
ngspice would compute the ratio of V(5, 3) to VIN, the small-signal input resistance at VIN,
and the small signal output resistance measured across nodes 5 and 3
"""
self._add_analysis(
TransferFunctionAnalysisParameters(outvar, insrc)
)
##############################################
def _impl_distortion(self, variation, points, start_frequency, stop_frequency, f2overf1=None):
"""Perform a distortion analysis of the circuit.
variation, points, start_frequency, stop_frequency - typical ac range parameters.
if f2overf1 is specified, perform a spectral analysis, else perform a harmonic analysis.
See section 15.3.3 of ngspice manual.
- harmonic analysis,
The distof1 parameter of the AC input to the circuit must be specified.
Second harmonic magnitude and phase are calculated at each circuit node.
- Spectral analysis,
The distof2 parameter of the AC input to the circuit must be specified as well as distof1.
See the ngspice manual.
Spice syntax:
General form:
.. code:: spice
.disto dec nd fstart fstop <f2overf1 >
.disto oct no fstart fstop <f2overf1 >
.disto lin np fstart fstop <f2overf1 >
Examples:
.. code:: spice
.disto dec 10 1kHz 100 MEG
.disto dec 10 1kHz 100 MEG 0.9
"""
# do some rudimentary parameter checking.
if variation not in ('dec', 'lin', 'oct'):
raise NameError("variation must be 'dec' or 'lin' or 'oct'")
self._add_analysis(
DistortionAnalysisParameters(variation, points, start_frequency, stop_frequency, f2overf1)
)
##############################################
[docs] def str_options(self, unit=True):
# Fixme: use cls settings ???
if unit:
_str = str_spice
else:
_str = lambda x: str_spice(x, unit)
netlist = ''
if self.options:
for key, value in self._options.items():
if value is not None:
netlist += '.options {} = {}'.format(key, _str(value)) + os.linesep
else:
netlist += '.options {}'.format(key) + os.linesep
return netlist
##############################################
def __str__(self):
netlist = self._circuit.str(simulator=self.simulator.SIMULATOR)
netlist += self.str_options()
if self._initial_condition:
netlist += '.ic ' + join_dict(self._initial_condition) + os.linesep
if self._node_set:
netlist += '.nodeset ' + join_dict(self._node_set) + os.linesep
if self._saved_nodes:
# Place 'all' first
saved_nodes = self._saved_nodes
if 'all' in saved_nodes:
all_str = 'all '
saved_nodes.remove('all')
else:
all_str = ''
netlist += '.save ' + all_str + join_list(saved_nodes) + os.linesep
for measure_parameters in self._measures:
netlist += str(measure_parameters) + os.linesep
for analysis_parameters in self._analyses.values():
netlist += str(analysis_parameters) + os.linesep
netlist += '.end' + os.linesep
return netlist
##############################################
def _run(self, analysis_method, *args, **kwargs):
# Trick to execute code before/after the analysis implementation
log_desk = kwargs.pop('log_desk', None)
run = kwargs.pop('run', True)
if 'probes' in kwargs:
self.save(* kwargs.pop('probes'))
# Execute analysis implementation
analysis_method(self, *args, **kwargs)
# Set simulator's specific settings
self._simulator.customise(self)
# Log the desk ?
message = 'desk' + os.linesep + str(self)
if log_desk:
self._logger.info(message)
else:
self._logger.debug(message)
# Run simulation ?
if run:
return self._simulator.run(self)
##############################################
# Register analysis wrappers and shortcuts s in Simulation
def _make_wrapper(analysis_method):
def wrapper(self, *args, **kwargs):
return self._run(analysis_method, *args, **kwargs)
return wrapper
_ANALYSES_PREFIX = '_impl_'
_ANALYSES_METHOD = [
method
for method in Simulation.__dict__.values()
if callable(method) and method.__name__.startswith(_ANALYSES_PREFIX)
]
_SHORTCUTS = {
'transfer_function': 'tf',
}
for _analysis_method in _ANALYSES_METHOD:
_wrapper = _make_wrapper(_analysis_method)
_wrapper.__doc__ = _analysis_method.__doc__
_analysis = _analysis_method.__name__[len(_ANALYSES_PREFIX):]
setattr(Simulation, _analysis, _wrapper)
_shortcut = _SHORTCUTS.get(_analysis, None)
if _shortcut:
setattr(Simulation, _shortcut, _wrapper)