11.1.12.8. HighLevelElement¶

This module implements high level elements built on top of Spice elements.

class PySpice.Spice.HighLevelElement.AcLine(netlist, name, node_plus, node_minus, rms_voltage=230, frequency=50)[source]¶: Bases: PySpice.Spice.HighLevelElement.SinusoidalVoltageSource

class PySpice.Spice.HighLevelElement.AmplitudeModulatedCurrentSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.CurrentSource, PySpice.Spice.HighLevelElement.CurrentSourceMixinAbc, PySpice.Spice.HighLevelElement.AmplitudeModulatedMixin

This class implements a amplitude modulated waveform current source.

See AmplitudeModulatedMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.AmplitudeModulatedMixin(offset, amplitude, modulating_frequency, carrier_frequency, signal_delay)[source]¶

Bases: PySpice.Spice.HighLevelElement.SourceMixinAbc

This class implements a Amplitude Modulated source.

Name	Parameter	Default Value	Units

Vo	offset		V, A

Va	amplitude		V, A

Mf	modulating frequency		Hz

Fc	carrier frequency	1 / Tstop	Hz

Td	signal delay		s

Spice Syntax:

AM(VA VO MF FC TD)

The shape of the waveform is described by the following equation:

\[V(t) = V_a (V_o + \sin (2\pi M_f\,t)) \sin (2\pi F_c\,t)\]

format_spice_parameters()[source]¶

class PySpice.Spice.HighLevelElement.AmplitudeModulatedVoltageSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.VoltageSource, PySpice.Spice.HighLevelElement.VoltageSourceMixinAbc, PySpice.Spice.HighLevelElement.AmplitudeModulatedMixin

This class implements a amplitude modulated waveform voltage source.

See AmplitudeModulatedMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.CurrentSourceMixinAbc[source]¶

Bases: object

AS_UNIT(value, none=False)¶

class PySpice.Spice.HighLevelElement.ExponentialCurrentSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.CurrentSource, PySpice.Spice.HighLevelElement.CurrentSourceMixinAbc, PySpice.Spice.HighLevelElement.ExponentialMixin

This class implements a exponential waveform current source.

See ExponentialMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.ExponentialMixin(initial_value, pulsed_value, rise_delay_time=0.0, rise_time_constant=None, fall_delay_time=None, fall_time_constant=None)[source]¶

Bases: PySpice.Spice.HighLevelElement.SourceMixinAbc

This class implements a Exponential waveform.

Nomenclature:

Name	Parameter	Default Value	Units

V1	Initial value		V, A

V2	pulsed value		V, A

Td1	rise delay time	0.0	sec

tau1	rise time constant	Tstep	sec

Td2	fall delay time	Td1+Tstep	sec

tau2	fall time constant	Tstep	sec

Spice Syntax:

EXP ( V1 V2 TD1 TAU1 TD2 TAU2 )

The shape of the waveform is described by the following formula:

Let V21 = V2 - V1 and V12 = V1 - V2.

\[\begin{split}V(t) = \begin{cases} V_1 & \text{if}\ 0 \leq t < T_{d1}, \\ V_1 + V_{21} ( 1 − e^{-\frac{t-T_{d1}}{\tau_1}} ) & \text{if}\ T_{d1} \leq t < T_{d2}, \\ V_1 + V_{21} ( 1 − e^{-\frac{t-T_{d1}}{\tau_1}} ) + V_{12} ( 1 − e^{-\frac{t-T_{d2}}{\tau_2}} ) & \text{if}\ T_{d2} \leq t < T_{stop} \end{cases}\end{split}\]

format_spice_parameters()[source]¶

class PySpice.Spice.HighLevelElement.ExponentialVoltageSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.VoltageSource, PySpice.Spice.HighLevelElement.VoltageSourceMixinAbc, PySpice.Spice.HighLevelElement.ExponentialMixin

This class implements a exponential waveform voltage source.

See ExponentialMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.PieceWiseLinearCurrentSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.CurrentSource, PySpice.Spice.HighLevelElement.CurrentSourceMixinAbc, PySpice.Spice.HighLevelElement.PieceWiseLinearMixin

This class implements a piece wise linear waveform current source.

See PieceWiseLinearMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.PieceWiseLinearMixin(values, repeat_time=None, delay_time=None, dc=None)[source]¶

Bases: PySpice.Spice.HighLevelElement.SourceMixinAbc

This class implements a Piece-Wise Linear waveform.

Spice Syntax:

PWL( T1 V1 <T2 V2 T3 V3 T4 V4 ... > ) <r=value> <td=value>

Each pair of values (Ti , Vi) specifies that the value of the source is Vi (in Volts or Amps) at time = Ti . The value of the source at intermediate values of time is determined by using linear interpolation on the input values. The parameter r determines a repeat time point. If r is not given, the whole sequence of values (Ti , Vi ) is issued once, then the output stays at its final value. If r = 0, the whole sequence from time = 0 to time = Tn is repeated forever. If r = 10ns, the sequence between 10ns and 50ns is repeated forever. the r value has to be one of the time points T1 to Tn of the PWL sequence. If td is given, the whole PWL sequence is delayed by a delay time time = td. The current source still needs to be patched, td and r are not yet available.

values should be given as a list of (Time, Value)-tuples, e.g.:

PieceWiseLinearVoltageSource(
    circuit,
    'pwl1', '1', '0',
    values=[(0, 0), (10@u_ms, 0), (11@u_ms, 5@u_V), (20@u_ms, 5@u_V)],
)

format_spice_parameters()[source]¶

class PySpice.Spice.HighLevelElement.PieceWiseLinearVoltageSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.VoltageSource, PySpice.Spice.HighLevelElement.VoltageSourceMixinAbc, PySpice.Spice.HighLevelElement.PieceWiseLinearMixin

This class implements a piece wise linear waveform voltage source.

See PieceWiseLinearMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.PulseCurrentSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.CurrentSource, PySpice.Spice.HighLevelElement.CurrentSourceMixinAbc, PySpice.Spice.HighLevelElement.PulseMixin

This class implements a pulse waveform current source.

See PulseMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.PulseMixin(initial_value, pulsed_value, pulse_width, period, delay_time=0, rise_time=0, fall_time=0, phase=None, dc_offset=0)[source]¶

Bases: PySpice.Spice.HighLevelElement.SourceMixinAbc

This class implements a pulse waveform.

Nomenclature:

Name	Parameter	Default Value	Units

V1	initial value		V, A

V2	pulsed value		V, A

Td	delay time	0.0	sec

Tr	rise time	Tstep	sec

Tf	fall time	Tstep	sec

Pw	pulse width	Tstop	sec

Period	period	Tstop	sec

Phase	phase	0.0	sec

Phase is only possible when XSPICE is enabled

Spice Syntax:

PULSE ( V1 V2 Td Tr Tf Pw Period Phase )

A single pulse so specified is described by the following table:

Time	Value
0	V1
Td	V1
Td+Tr	V2
Td+Tr+Pw	V2
Td+Tr+Pw+Tf	V1
Tstop	V1

Note: default value in Spice for rise and fall time is the simulation transient step, pulse width and period is the simulation stop time.

Public Attributes:

delay_time

fall_time

initial_value

period

phase

pulse_width

pulsed_value

rise_time

format_spice_parameters()[source]¶

property frequency¶

class PySpice.Spice.HighLevelElement.PulseVoltageSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.VoltageSource, PySpice.Spice.HighLevelElement.VoltageSourceMixinAbc, PySpice.Spice.HighLevelElement.PulseMixin

This class implements a pulse waveform voltage source.

See PulseMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.RandomCurrentSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.CurrentSource, PySpice.Spice.HighLevelElement.CurrentSourceMixinAbc, PySpice.Spice.HighLevelElement.RandomMixin

This class implements a random waveform current source.

See RandomMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.RandomMixin(random_type, duration=0, time_delay=0, parameter1=1, parameter2=0)[source]¶

Bases: PySpice.Spice.HighLevelElement.SourceMixinAbc

This class implements a Random Voltage source.

The TRRANDOM option yields statistically distributed voltage values, derived from the ngspice random number generator. These values may be used in the transient simulation directly within a circuit, e.g. for generating a specific noise voltage, but especially they may be used in the control of behavioral sources (B, E, G sources, voltage controllable A sources, capacitors, inductors, or resistors) to simulate the circuit dependence on statistically varying device parameters. A Monte-Carlo simulation may thus be handled in a single simulation run.

Spice Syntax:

TRRANDOM( TYPE TS <TD <PARAM1 <PARAM2> > >)

TYPE determines the random variates generated: 1 is uniformly distributed, 2 Gaussian, 3 exponential, 4 Poisson. TS is the duration of an individual voltage value. TD is a time delay with 0 V output before the random voltage values start up. PARAM1 and PARAM2 depend on the type selected.

Type	Parameter 1	Default	Parameter 2	Default

uniform	range	1	offset	0

gaussian	standard dev.	1	mean	0

exponential	mean	1	offset	0

poisson	lambda	1	offset	0

format_spice_parameters()[source]¶

class PySpice.Spice.HighLevelElement.RandomVoltageSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.VoltageSource, PySpice.Spice.HighLevelElement.VoltageSourceMixinAbc, PySpice.Spice.HighLevelElement.RandomMixin

This class implements a random waveform voltage source.

See RandomMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.SingleFrequencyFMCurrentSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.CurrentSource, PySpice.Spice.HighLevelElement.CurrentSourceMixinAbc, PySpice.Spice.HighLevelElement.SingleFrequencyFMMixin

This class implements a single frequency FM waveform current source.

See SingleFrequencyFMMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.SingleFrequencyFMMixin(offset, amplitude, carrier_frequency, modulation_index, signal_frequency)[source]¶

Bases: PySpice.Spice.HighLevelElement.SourceMixinAbc

This class implements a Single-Frequency FM waveform.

Spice Syntax:

SFFM (VO VA FC MDI FS )

Name	Parameter	Default Value	Units

Vo	offset		V, A

Va	amplitude		V, A

Fc	carrier frequency	1 / Tstop	Hz

Mdi	modulation index

Fs	signal frequency	1 / Tstop	Hz

The shape of the waveform is described by the following equation:

\[V(t) = V_o + V_a \sin (2\pi F_c\, t + M_{di} \sin (2\pi F_s\,t))\]

format_spice_parameters()[source]¶

class PySpice.Spice.HighLevelElement.SingleFrequencyFMVoltageSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.VoltageSource, PySpice.Spice.HighLevelElement.VoltageSourceMixinAbc, PySpice.Spice.HighLevelElement.SingleFrequencyFMMixin

This class implements a single frequency FM waveform voltage source.

See SingleFrequencyFMMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.SinusoidalCurrentSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.CurrentSource, PySpice.Spice.HighLevelElement.CurrentSourceMixinAbc, PySpice.Spice.HighLevelElement.SinusoidalMixin

This class implements a sinusoidal waveform current source.

See SinusoidalMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.SinusoidalMixin(dc_offset=0, ac_magnitude=1, offset=0, amplitude=1, frequency=50, delay=0, damping_factor=0)[source]¶

Bases: PySpice.Spice.HighLevelElement.SourceMixinAbc

This class implements a sinusoidal waveform.

Name	Parameter	Default Value	Units

Vo	offset		V, A

Va	amplitude		V, A

f	frequency	1 / TStop	Hz

Td	delay	0.0	sec

Df	damping factor	0.01	1/sec

The shape of the waveform is described by the following formula:

\[\begin{split}V(t) = \begin{cases} V_o & \text{if}\ 0 \leq t < T_d, \\ V_o + V_a e^{-D_f(t-T_d)} \sin\left(2\pi f (t-T_d)\right) & \text{if}\ T_d \leq t < T_{stop}. \end{cases}\end{split}\]

Spice syntax:

SIN ( Voffset Vamplitude Freq Tdelay DampingFactor )

Public Attributes:

ac_magnitude

amplitude

damping_factor

dc_offset

delay

frequency

offset

format_spice_parameters()[source]¶

property period¶

property rms_voltage¶

class PySpice.Spice.HighLevelElement.SinusoidalVoltageSource(netlist, name, node_plus, node_minus, *args, **kwargs)[source]¶

Bases: PySpice.Spice.BasicElement.VoltageSource, PySpice.Spice.HighLevelElement.VoltageSourceMixinAbc, PySpice.Spice.HighLevelElement.SinusoidalMixin

This class implements a sinusoidal waveform voltage source.

See SinusoidalMixin for documentation.

format_spice_parameters()¶: Return the formatted list of parameters.

class PySpice.Spice.HighLevelElement.SourceMixinAbc[source]¶

Bases: object

AS_UNIT = None¶

class PySpice.Spice.HighLevelElement.VoltageSourceMixinAbc[source]¶

Bases: object

AS_UNIT(value, none=False)¶