Glossary of Generic Analog & Mixed-Mode Devices & Sources

From Emagtech Wiki
Jump to: navigation, search

Contents

4-Bit ADC Bridge

GK44.png

This 8-pin device is simply a bundle of 4 1-bit ADC bridges. Each analog input pin has a corresponding digital output pin.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
in_low maximum 0-valued analog input V 0.1 required
in_high minimum 1-valued analog input V 0.9 required

4-Bit DAC Bridge

GK45.png

This 8-pin device is simply a bundle of 4 1-bit DAC bridges. Each digital input pin has a corresponding analog output pin.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
out_low analog output for 0 digital input V 0 required
out_high analog output for 1 digital input V 1 required

AC/RF Current Source

GL11.png

This is a simplified version of the standard Current Source, in which the AC "Use" box has been checked by default. Therefore, it is ready to be used for AC frequency sweep. Note that for AC frequency sweep, you do not need to specify the frequency.


Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
VA peak current amplitude A 1 required
Freq frequency Hz 1 required
Phase phase deg 0
offset DC offset for small-signal current A 0

AC/RF Voltage Source

GL10.png

This is a simplified version of the standard Voltage Source, in which the AC "Use" box has been checked by default. Therefore, it is ready to be used for AC frequency sweep. Note that for AC frequency sweep, you do not need to specify the frequency.


Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
VA peak voltage amplitude V 1 required
Freq frequency Hz 1 required
Phase phase deg 0
offset DC offset for small-signal voltage V 0

Alternate Ferrite Core Transformer

GK96.png

The alternate ferrite core transformer is a four-pin two-port device, which has the same behavior as the Ferrite Core Transformer, except for the reversed polarity of its secondary port.

Alternate Ideal Transformer

XFMR2.png

The alternate ideal transformer is a four-pin two-port device, which has the same behavior as the Ideal Transformer, except for the reversed polarity of its secondary port.

AM Modulated Source

GL23.png

This is a voltage source with a single-tone amplitude modulated waveform. The AM modulation index MDI is defined as the ratio of maximum amplitude deviation to maximum signal amplitude.


Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
V0 offset V 0
VA amplitude V 1
FC carrier frequency Hz 1 required
MDI modulation index - 0 required
FS signal frequency Hz 1 required

Analog Clock

GL30.png

This is a periodic pulse generator with a default 0V low output level and a default 5V high output level.


Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
delay delay time sec 0
rise rise time sec 0.1n
fall fall time sec 0.1n
pulse_wid clock pulse width sec 1u required
period clock period - 2u required
out_low low output voltage level V 0
out_high high output voltage level V 5

Analog-to-Digital Converter (ADC) Bridge

GK42.png

The ADC Bridge takes an analog value from an analog node and may be in the form of a voltage or current. If the input is less than or equal to "in_low", then a digital "0" is generated. If the input is greater than or equal to "in_high", a digital "1" is generated. Otherwise, a digital "UNKNOWN" is the output value. Unlike the DAC Bridge, ramping or delay is not applicable. Rather, the continuous ramping of the input provides for any associated delays in the digitized signal.

This model also posts an input load value based on the parameter input_load.

Model Identifier: adc_bridge

Netlist Format:

A<device_name> [<in_pin> {<in2_pin>> ...}] [<out_pin> {<out2_pin> ...}] <model_name>

.model <model_name> adc_bridge {<param1 = value> < param2 = value> ...}

Example:

A [1] [2] adc_bridge

.model adc_bridge adc_bridge in_low = .1 fall_delay = 1n

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
in_low maximum 0-valued analog input V 0.1 required
in_high minimum 1-valued analog input V 0.9 required
rise_delay L-to-H delay time sec 1n
fall_delay H-to-L delay time sec 1n

Arbitrary Temporal Waveform Generator

GL17.png

This is a voltage source with an arbitrary waveform defined by a mathematical expression. You have to open the subcircuit model dialog by clicking the View Subcircuit button and edit its text. Enter any mathematical expression in the variable "v(t)" standing for time.

Examples:

  • v(t) is equivalent to f(t) = t.
  • 0.1*(v(t))^2 is equivalent to f(t) = 0.1t^2.
  • sin(2*pi*v(t)) is equivalent to f(t) = sin(2πt).

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
Tmax maximum signal duration sec 1e6 required

Auto-Transformer

GK102.png

This 3-pin device models an auto-transformer with mutual coupling effect.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
Lp primary inductance H 1m
Ls secondary inductance H 1m
k coefficient of coupling - 1.0

Bipolar Junction Transistor (BJT)

G11.png

The BJT is an active device which has up to 4 pins. The three standard pins are base, emitter, and collector. These are given in the default symbol. The substrate, which is grounded by default, is the fourth pin. To use the BJT with the substrate, create a new 4-pin BJT using the Device Editor and Symbol Editor.

The standard device parameters are AREA, OFF, IC, and T. They are described below:

AREA area factor (optional) (If not specified, the default value is 1.0.)
OFF initial condition for the DC analysis (optional)
IC initial condition (optional) (Used when a transient analysis is desired, which starts from other than the quiescent operating point.)
T operating temperature of the device (optional)

Area factor scales the model parameters RE and RC. IC VBE is the initial voltage from base emitter. IC VCE is the initial voltage from collector to emitter. TEMP is the overriding temperature. These parameters are based on the Gummel and Poon integral-charge model. If these parameters are not specified, then it will reduce to the simpler Ebers-Moll model.

The process model is mandatory for the BJT. Descriptions of the process model parameters are given in the following table:

NAME PARAMETER UNITS DEFAULT EXAMPLE
IS transport saturation current A 1.0e-16 1.0e-15
BF ideal maximum forward beta 100 100
NF forward current emission coefficient 1.0 1
VAF forward Early voltage V infinite 200
IKF corner forward beta high current roll-off A infinite 0.01
ISE B-E leakage saturation current A 0 1.0e-13
NE B-E leakage emission coefficient 1.5 2
BR ideal maximum reverse beta 1 0.1
NR reverse current emission coefficient 1 1
VAR reverse Early voltage V infinite 200
IKR corner reverse beta high current roll-off A infinite 0.01
ISC B-C leakage saturation current A 0 1.0e-13
NC B-C leakage emission coefficient 2 1.5
RB zero bias base resistance ohms 0 100
IRB current where base resistance falls halfway to minimum value A infinite 0.1
RBM minimum base resistance at high currents ohms RB 10
RE emitter resistance ohms 0 1
RC collector resistance ohms 0 10
CJE B-E zero bias depletion capacitance F 0 2pF
VJE B-E built-in potential V 0.75 0.6
MJE B-E junction exponential factor 0.33 0.33
TF ideal forward transit time sec 0 0.1ns
XTF coefficient for bias dependence of TF 0
VTF voltage describing VBC dependence of TF V infinite
ITF high-current parameter for effect on TF A 0
PTF excess phase at freq=1.0/(TF*2PI)Hz degree 0
CJC B-C zero bias depletion capacitance F 0 2pF
VJC B-C built-in potential V 0.75 0.5
MJC B-C junction exponential factor 0.33 0.5
XCJC fraction of B-C depletion capacitance connected to internal base node 1
TR ideal reverse transit time sec 0 10ns
CJS zero bias collector-substrate capacitance F 0 2pF
VJS substrate junction built-in potential V 0.75
MJS substrate junction exponential factor 0 0.5
XTB forward and reverse beta temp. exponent 0
EG energy gap for temperature effect on IS eV 1.11
XTI temperature exponent for effect on IS 3
KF flicker-noise coefficient 0
AF flicker-noise exponent 1
FC coefficient for forward bias depletion capacitance formula 0.5
TNOM parameter measurement temperature deg. C 27 50

Capacitance Meter

G37.png

The Capacitance Meter measures the total capacitance between a circuit node and the ground. The input pin of the device is connected to the measurement node. The output voltage of the device is then a scaled value equal to the total capacitance seen on its input multiplied by the gain parameter. This model is primarily intended as a building block for other models which must sense a capacitance value and alter their behavior based upon it.


Model Identifier: cmeter

Netlist Format:

A<device_name> <in_pin> <out_pin> <model_name>

.model <model_name> cmeter {<gain = value>}

Example:

A1 1 2 cap_meter

.model cap_meter cmeter gain = 1

Parameters:

The only parameter is the gain with a default value of 1.0.

Capacitor

GK120.png

Capacitors are used to store electrical energy. They can filter or remove AC signals or block DC current without disrupting AC signals. A capacitor's ability to store energy is termed capacitance and is measured in Farads, with values from pF to mF. The only time current flows through a capacitor is when the charge is collected on, or is removed from, its parallel plates. This means that the voltage across the capacitor is changing, which doesn't conform to DC analysis. In a physical circuit, there is a transition stage during which capacitors charge up to their final values. The result is the same as if these capacitors did not exist and the connections to them were left dangling. In other words, in a (steady-state) DC analysis, a capacitor behaves like an open circuit. Therefore, it is important that no section of the circuit is isolated from the capacitors. Every circuit node needs some path for DC current to the ground.

A capacitor's transient behavior is described by the equation:

i(t) = C * (dv(t)/dt)

Its initial voltage is only important when the simulator performs a transient analysis, and the "Use Initial Conditions" checkbox is checked.

An capacitor's AC behavior is described by the equation:

i = j ω * C * v

All capacitor names must begin with C.

Netlist Format:

C<device_name> <N+> <N-> <value>

Example:

C1 1 2 10p

RF.Spice A/D provides three types of capacitors: simple, user-defined (or real) and semiconductor. The standard capacitor parameters are N+, N-, VALUE, and IC. In a simple capacitor, VALUE must be specified for the capacitance in Farads. IC is the (optional) initial condition for the capacitor voltage.

Center-Tapped Ferrite Core Transformer

GK97.png

This five-pin three-port device models a center-tapped physical transformer with a magnetic ferrite core. Its model is based on XSPICE's magnetic core and inductive coupling models. For this device you need to specify physical parameters like cross sectional area, core length and number of primary and secondary turns. The physical model of the magnetic device is defined by two vectors: magnetic field intensity H in A/m and magnetic flux density B (also known as magnetic induction) in Tesla. The default array values are:

H_array = [-250 -100 -50 -37.5 -25 -12.5 0 12.5 25 37.5 50 100 250]

B_array = [-0.375 -0.36 -0.32 -0.29 -0.24 -0.15 0 0.15 0.24 0.29 0.32 0.36 0.375]

To change the value of H/B arrays, open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
n_prim number of primary inductor coupling turns - 100 required
n_sec number of full-winding secondary inductor coupling turns - 100 required
area cross-sectional area m2 1e-5
length core length m 0.01

Controlled Sine Wave Oscillator

G24.png

This is a four-terminal function generator with a sinusoidal wave output, whose frequency is controlled by an input voltage. The functional dependency of the output frequency on the input voltage is piecewise linear and is defined as a two-dimensional table similar to a piecewise linear (PWL) controlled source. In the "frequency vs. voltage" curve, the array "cntl_array" defines voltage values in Volts and the array "freq_array" defines the corresponding frequencies in Hz. This function has parameterizable values of low and high peak output voltage.

Model Identifier: sine

Netlist Form:

A<device_name> %vd(<cntl_in_pin> <cntl_in_ref_pin>) %vd(<out_pin> <out_ref_pin>) <model_name>

.model <model_name> sine cntl_array = [<value1> <value2>] freq_array = [<value1> <value2>] {<param1 = value> < param2 = value> ...}

Example:

A1 %vd(1 3)  %vd(2 4) sine

.model sine sine cntl_array = [0 1] freq_array = [1 1000]

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
Cntl_array control array V [0 1] required
Freq_array frequency array Hz [1 1000] required
Out_low output peak low value V -1.0
Out_high output peak high value V 1.0


Controlled Sources

Circuits can contain linear dependent sources characterized by one of the following equations (where g, e, f, and h are constants representing transconductance, voltage gain, current gain, and transresistance, respectively):

iout = g vin      vout = e vin      iout = f iin      vout = h iin

For further information, refer to:

Linear Current Controlled Current Source (CCCS)

Linear Voltage Controlled Current Source (VCCS)

Linear Current Controlled Voltage Source (CCVS)

Linear Voltage Controlled Voltage Source (VCVS)


Controlled Square Wave Oscillator

G25.png

This is a four-terminal function generator with a square wave output, whose frequency is controlled by an input voltage. The functional dependency of the output frequency on the input voltage is piecewise linear and is defined as a two-dimensional table similar to a piecewise linear (PWL) controlled source. In the "frequency vs. voltage" curve, the array "cntl_array" defines voltage values in Volts and the array "freq_array" defines the corresponding frequencies in Hz.

Model Identifier: square

Netlist Format:

A<device_name> %vd(<cntl_in_pin> <cntl_in_ref_pin>) %vd(<out_pin> <out_ref_pin>) <model_name>

.model <model_name> square cntl_array = [<value1> <value2>] freq_array = [<value1> <value2>] {<param1 = value> < param2 = value> ...}

Example:

A1 %vd(1 3)  %vd(2 4) square

.model square square cntl_array = [0 1] freq_array = [1 1000]

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
Cntl_array control array V [0 1] required
Freq_array frequency array Hz [0 1000] required
Out_low output peak low value V -1.0
Out_high output peak high value V 1.0
Duty_cycle Duty cycle - 0.5
Rise_time Output rise time sec 1.0e-9
Fall_time Output fall time sec 1.0e-9

Controlled Triangle Wave Oscillator

G26.png

This is a four-terminal function generator with a triangle wave output, whose frequency is controlled by an input voltage. The functional dependency of the output frequency on the input voltage is piecewise linear and is defined as a two-dimensional table similar to a piecewise linear (PWL) controlled source. In the "frequency vs. voltage" curve, the array "cntl_array" defined voltage values in Volts and the array "freq_array" defines the corresponding frequencies in Hz.

Model Identifier: triangle

Netlist Format:

A<device_name> %vd(<cntl_in_pin> <cntl_in_ref_pin>) %vd(<out_pin> <out_ref_pin>) <model_name>

.model <model_name> tirangle cntl_array = [<value1> <value2>] freq_array = [<value1> <value2>]{<param1 = value> < param2 = value> ...}

Example:

A1 %vd(1 4)  %vd(2 3) triangle

.model triangle triangle cntl_array = [0 1] freq_array = [1 1000]

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
Cntl_array control array V [0 1] required
Freq_array frequency array Hz [0 1000] required
Out_low output peak low value V -1.0
Out_high output peak high value V 1.0
Rise_duty Rise time duty cycle 0.5

Crystal

GK78.png

This is a 2-pin parameterized crystal device.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
CM motional capacitance F 10f
C0 shunt capacitance F 1p
RM motional resistance Ohms 100
LM motional inductance H 100m

Current Noise Source

GL16.png

This is a current noise generator characterized by a spectral density and corner frequency. You have to click the Edit Model... button to access the parameters of this device.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
En noise current A/√Hz 1p required
freq noise corner frequency Hz 100 required

Current Source

G17B.png

Current source has a DC value, a transient behavior, an AC behavior, and distortion parameters. The transient type, AC parameters, and distortion parameters are defined on the first tab of the source's property dialog. The transient expression can be a pulse, sinusoid, exponential, or piecewise linear. The DC value of a current source is its initial transient value. For a source with a sinusoidal transient behavior, for example, the DC value will be equal to its transient offset current. The AC parameters are magnitude and phase. These are used during the AC Frequency Sweep analysis. The distortion parameters, two sets of magnitude and phase, are used during the distortion analysis. The AC and distortion parameters are defined on the second tab of the source's property dialog.

Current-Controlled Switch

G20.png

Switches are devices that exhibit high resistance when open (OFF state) and low resistance when closed (ON state). The switch model allows an almost ideal switch to be specified. With careful selection of the on and off resistances, they can effectively represent zero and infinite resistances in comparison to other circuit elements, while sustaining the model condition of a positive, finite value.

There are two versions of Current-Controlled Switch: two-terminal and four-terminal. For the two-terminal device, you must specify the name of the controlling Ammeter or voltage source, as well as the turn-on and turn-off currents in Amperes and on and off resistance values in Ohms. The four-terminal device already provides nodes for a controlling ammeter, and you just specify the rest of parameters. When the current through the switch or controlling device is greater or equal to the turn-on current, the switch closes. When the current through the switch or controlling device is less than or equal to the turn off current, the switch opens.

NAME PARAMETER UNITS DEFAULT NOTES
I_ON turn-on current A 0.0
I_OFF turn-off current A 0.0
RON closed resistance Ohms 1.0
ROFF open resistance Ohms 1/GMIN

Darlington Pair

GK108.png

A Darlington pair is a three-pin device that consists of two interconnected BJT transistors of the same type. The collectors of two transistors are connected together to provide the "Collector" pin of the pair. The base of the first BJT acts the "Base" pin of the pair. The emitter of the first BJT is internally connected to the base of the second BJT. The emitter of the second BJT acts as the "Emitter" pin of the pair. There are two types of Darlington pair: NPN and PNP. The parameterized generic Darlington pair also contains a diode connected between the collector and emitter pin as well as two base-emitter resistors, one across each BJT.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
is_bjt bjt saturation current A 1.0e-12
bf_bjt bjt forward beta - 150
nf_bjt bjt forward emission coefficient - 1
ise_bjt B-E leakage saturation current A 0
ne_bjt B-E leakage emission coefficient - 1
br_bjt ideal maximum reverse beta - 1
nr_bjt reverse current emission coefficient - 1
isc_bjt B-C leakage saturation current A 0
nc_bjt B-C leakage emission coefficient - 1
rb_bjt zero bias base resistance Ohms 0
irb_bjt current where base resistance falls halfway to minimum value A inf
rbm_bjt minimum base resistance at high currents ohms 0
re_bjt emitter resistance Ohms 0
rc_bjt collector resistance Ohms 0
cje_bjt B-E zero bias depletion capacitance F 0
vje_bjt B-E built-in potential V 0.75
mje_bjt B-E junction grading coefficient - 0.33
cjc_bjt B-C zero bias depletion capacitance F 0
vjc_bjt B-C built-in potential V 0.75
mjc_bjt B-C junction exponential factor - 0.33
tf_bjt ideal forward transit time sec 0
tr_bjt ideal reverse transit time sec 0
is_d diode saturation current A 1.0e-12
rs_d diode resistance Ohms 0
n_d diode emission coefficient - 1
cjo_d diode junction capacitance F 0
vj_d diode junction potential V 1
m_d diode grading coefficient 0.5
tnom parameter measurement temperature deg C 27
r1 first base-emitter resistance Ohms 1k
r2 second base-emitter resistance Ohms 1k

DC Bias Sources Vcc, Vee, Vdd, Vss

GL12.png

These are simple 1-pin DC voltage sources. Vcc and Vdd provide a positive voltage, while Vee and Vss provide a negative voltage

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
vcc bias voltage V +15 required
vee bias voltage V -15 required
vdd bias voltage V +15 required
vss bias voltage V -15 required

Digital-to-Analog Converter (DAC) Bridge

GK43.png

The DAC Bridge takes a digital value from a digital node and can only be eiter "0", "1", or "U". It then outputs the value "out_low", "out_high" or "out_udndef", or ramps linearly toward one of these "final" values from its curent analog output level. This ramping speed depends on the values of "t_rise" and "t_fall".

Model Identifier: dac_bridge

Netlist Format:

A<device_name> [<in_pin> {<in2_pin>> ...}] [<out_pin> {<out2_pin> ...}] <model_name>

.model <model_name> dac_bridge {<param1 = value> < param2 = value> ...}

Example:

A [1] [2] dac_bridge

.model dac_bridge dac_bridge out_low = 0 fall_delay = 1n

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
out_low analog output for 0 digital input V 0 required
out_high analog output for 1 digital input V 1 required
out_undef analog output for undefined digital input V 0.5 required
input_load capacitive input load F 1p
t_rise L-to-H delay time sec 1n
t_fall H-to-L delay time sec 1n

Diode

G9.png

Diodes allow current flow only in one direction, following their symbol's arrow, and thus can be used as simple solid state switches in AC circuits.

The standard device parameters are AREA, OFF, IC, and T. They are described below:

AREA area factor (optional) (If not specified, the default value is 1.0.)
OFF initial condition for the DC analysis (optional)
IC initial condition (optional) (Used when a transient analysis is desired, which starts from other than the quiescent operating point.)
T operating temperature of the device (optional)

The process models can be either junction diodes or Schottky barrier diodes. Area factor scales the model parameters IS, RS, CJO, and IBV. VD is the initial voltage, and TEMP is the overriding temperature. Descriptions of the process model parameters are given in the following table:

NAME PARAMETER UNITS DEFAULT NOTES
IS saturation current A 1e-14
TNOM parameter measurement temperature deg C 27
RS ohmic resistance Ohms 0
N emission coefficient - 1
TT transit-time sec 0
CJO zero-bias junction capacitance F 0
VJ junction potential V 1
M grading coefficient - 0.5
EG activation energy eV 1.11
XTI saturation current temp. exp. - 3.0
KF flicker noise coefficient - 0
AF flicker noise exponent - 1
FC forward bias junction fit parameter - 0.5
BV reverse breakdown voltage V inf
IBV current at breakdown voltage A 1e-3

Diode Bridge

GK107.png

This four-pin device is a bridge configuration of four generic diodes.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
IS saturation current A 1e-14
RS ohmic resistance Ohms 0
N emission coefficient - 1
TT transit-time sec 0
CJO zero-bias junction capacitance F 10p
VJ junction potential V 1
M grading coefficient - 0.5
BV reverse breakdown voltage V 1000
IBV current at breakdown voltage A 1e-3
TNOM parameter measurement temperature deg C 27

Doubly Center-Tapped Ferrite Core Transformer

GK98.png

This six-pin four-port device models a doubly center-tapped physical transformer with a magnetic ferrite core. Its model is based on XSPICE's magnetic core and inductive coupling models. For this device you need to specify physical parameters like cross sectional area, core length and number of primary and secondary turns. The physical model of the magnetic device is defined by two vectors: magnetic field intensity H in A/m and magnetic flux density B (also known as magnetic induction) in Tesla. The default array values are:

H_array = [-250 -100 -50 -37.5 -25 -12.5 0 12.5 25 37.5 50 100 250]

B_array = [-0.375 -0.36 -0.32 -0.29 -0.24 -0.15 0 0.15 0.24 0.29 0.32 0.36 0.375]

To change the value of H/B arrays, open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
n_prim number of full-winding primary inductor coupling turns - 100 required
n_sec number of full-winding secondary inductor coupling turns - 100 required
area cross-sectional area m2 1e-5
length core length m 0.01

DPDT Switch

GK74.png

This is an 8-pin device that models a double-pole double-throw switch. It has two input signals and four output pins. When the control voltage is at the high state, the first and second input voltages are transferred to the first and third output pins, respectively. When the control voltage is at the low state, the first and second input voltages are transferred to the second and fourth output pins, respectively.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
von turn-on voltage V 3.3
voff turn-off voltage V 0.3
vt threshold voltage V 1.0
ron on resistance Ohms 1.0
roff off resistance Ohms 1Gig

DPST Switch

GK73.png

This is a 6-pin device that models a double-pole single-throw switch. It has two input signals and two output signals. When the switch on, the first and second input voltages are transferred to the first and second output pins, respectively. When the switch is off, the output pin do not receive any input signals.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
von turn-on voltage V 3.3
voff turn-off voltage V 0.3
vt threshold voltage V 1.0
ron on resistance Ohms 1.0
roff off resistance Ohms 1Gig

Ferrite Core Transformer

GK95.png

This four-pin two-port device models a physical transformer with a magnetic ferrite core. Its model is based on XSPICE's magnetic core and inductive coupling models. For this device you need to specify physical parameters like cross sectional area, core length and number of primary and secondary turns. The physical model of the magnetic device is defined by two vectors: magnetic field intensity H in A/m and magnetic flux density B (also known as magnetic induction) in Tesla. The default array values are:

H_array = [-250 -100 -50 -37.5 -25 -12.5 0 12.5 25 37.5 50 100 250]

B_array = [-0.375 -0.36 -0.32 -0.29 -0.24 -0.15 0 0.15 0.24 0.29 0.32 0.36 0.375]

To change the value of H/B arrays, open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
n_prim number of primary turns - 100 required
n_sec number of secondary turns - 100 required
area cross-sectional area m2 1e-5
length core length m 0.01

FM Modulated Source

GL24.png

This is a voltage source with a single-tone frequency modulated waveform. The FM modulation index MDI is defined as the ratio of maximum frequency deviation to maximum signal amplitude.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
V0 offset V 0
VA amplitude V 1
FC carrier frequency Hz 1 required
MDI modulation index - 0 required
FS signal frequency Hz 1 required

Frequency Meter

G114.png

The Frequency Meter is a four-pin shunt device that is connected in parallel with an AC source just like a voltmeter and measures the operating frequency of the AC circuit. The input pins are connected across the AC source. The voltage across the output pins is equal to the frequency of the source in Hertz within a scale factor SF. Note that the Frequency Meter is designed to work with a single-tone AC source of unit amplitude. If the amplitude of the source is not one, multiply the SF parameter by the non-unit source amplitude value. The output voltage of the Frequency Meter can be used in conjunction with linear or nonlinear dependent sources to model frequency-dependent quantities.


Model Identifier: fmeter


Parameters:

The only parameter is the scale factor SF with a default value of 1.0. Set SF = 1e-6 to read out the frequency in MHz. Set SF = 1e-9 to read out the frequency in GHz. Set SF = 6.283185 (2*pi) to read out the angular frequency ω in radian/s.

Fuse

GK76.png

This is a 2-pin interactive current-controlled switch. If the current passing through the fuse is less than a specified threshold current, the switch is closed. If the current exceeds the threshold level, the fuse breaks and remains open thereafter. The device's symbol changes to display its state.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
r resistance when intact Ohms 1.0
i_thresh threshold current A 1.0

Ground

G15.png

Ground has a voltage of zero (0) and is used as a reference to compute electrical values in the circuit. All circuits must be grounded to be properly simulated. There is no limit on the number of grounds you may use in a circuit. All components connected to ground are referenced to a common point and treated as linked through ground.

Hysteresis Block (XSPICE)

G37.png

The Hysteresis block is a simple buffer stage that provides hysteresis of the output with respect to the input. The in_low and in_high parameter values. The output values are limited to out_lower_limit and out_upper_limit. The value of \93hyst\94 is added to the in_low and in_high points in order to specify the points at which the slope of the hysteresis function would normally change abruptly as the input transitions from a low to a high value. Likewise, the value of \93hyst\94 is subtracted from the in_high and in_low values in order to specify the points at which the slope of the hysteresis function would normally change abruptly as the input transitions from a high to a low value. In fact, the slope of the hysteresis function is never allowed to change abruptly but is smoothly varied whenever the input_dowmain smoothing parameter is set greater than zero.

Model Identifier: hyst

Netlist Format:

A<device_name> <in_pin> <out_pin> <model_name>

.model <model_name> hyst {<param1 = value> < param2 = value> ...}

Example:

A1 1 2 hysteresis_block

.model hysteresis_block hyst in_low = 0.0 in_high = 1.0

Parameters:

Name Description Default
In_low input low value 0.0
in_high input high value 1.0
hyst hysteresis 0.1
out_lower_limit output lower limit 0.0
out_upper_limit output upper limit 1.0
input_domain input smoothing domain 0.01
fraction smoothing fraction/absolute value switch true

Ideal Center-Tapped Transformer with Push-Pull Input

XFMR4.png

The ideal center-tapped transformer with push-pull input is a five-pin three-port device with two primary input ports and one secondary output port. Its model is based on the Ideal Transformer, and the relationship between its primary and secondary voltages is given by:

[math] \frac{v_P1}{v_S} = \frac{v_P2}{v_S} = n [/math]

where vS is the secondary voltage, vP1 is measured between the top primary pin P1 and the center tap pin, and vP2 is measured between the center tap pin and the bottom primary pin P2. The red dots show the polarity of the windings on each side. This model has one parameter: ratio = n = NP1/NS = NP2/NS, which represents the primary-to-secondary (half-winding) turns ratio.

Ideal Center-Tapped Transformer with Push-Pull Output

XFMR3.png

The ideal center-tapped transformer with push-pull output is a five-pin three-port device with one primary input port and two secondary output ports. Its model is based on the Ideal Transformer, and the relationship between its primary and secondary voltages is given by:

[math] \frac{v_P}{v_{S1}} = \frac{v_P}{v_{S2}} = n [/math]

where vP is the primary voltage, vS1 is measured between the top secondary pin S1 and the center tap pin, and vS2 is measured between the center tap pin and the bottom secondary pin S2. The red dots show the polarity of the windings on each side. This model has one parameter: ratio = n = NP/NS1 = NP/NS2, which represents the primary-to-secondary (half-winding) turns ratio.

Ideal Diode

GK106.png

This 2-pin device is a very basic and primitive model of a diode as a rectifier or switch. When the voltage across the device's terminals is positive, it acts as a short circuit. When the voltage across the device's terminals is negative, it acts as an open circuit.

Parameters:

None

Ideal Operational Amplifier (Op-Amp)

GK105.png

This is a very basic and primitive model of an operational amplifier. It has only one parameter, open loop gain with a default value of 50,000, which is adequate for most cases. The ideal Op-Amp device doesn't require any DC bias voltages.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
A open loop gain - 50,000

Ideal Transformer

XFMR1.png

The ideal transformer is a four-pin two-port device with the following relationship between the voltages and currents at its primary and secondary ports:

[math] \frac{v_P}{v_S} = - \frac{i_S}{i_P} = \frac{N_P}{N_S} = n [/math]

where vP, iP, NP are the primary voltage, current and number of turns, respectively, and vS, iS, NS are the secondary voltage, current and number of turns, respectively. The red dots show the polarity of the windings on each side. This model has one parameter: ratio = n = NP/NS, which represents the primary-to-secondary turns ratio. Note that the ideal transformer model is defined based on controlled sources and does not involve any magnetic physical parameters as opposed to mutual inductors or ferrite core transformer.

Inductance Meter

G37.png

The Inductance Meter measures the total inductance between a circuit node and the ground. The input pin of the device is connected to the measurement node. The output voltage of the device is then a scaled value equal to the total inductance seen on its input multiplied by the gain parameter. This model is primarily intended as a building block for other models which must sense an inductance value and alter their behavior based upon it. Care must be exercised when connecting an Inductance Meter to the inductors of a circuit. This is due to the fact that inductors are treated by SPICE as current sources. This can cause a problem when an inductor is connected in series with a current source, or in series with a voltmeter, or in series with another inductor.

Model Identifier: lmeter

Netlist Format:

A<device_name> <in_pin> <out_pin> <model_name>

.model <model_name> imeter {<gain = value>}

Example:

A1 1 2 inductance_meter

.model inductance_meter lmeter gain = 1

Parameters:

The only parameter is the gain with a default value of 1.0.

Inductive Coupler Block

GK99.png

The Inductive Coupler Block couples any two existing inductors. This block doesn't have any pins because it doesn't actually represent inductors, only the coupling between them. This is useful if you want to couple two inductors that are in different parts of the circuit, or if you want to couple more than two inductors together. In the latter case, use more than one of these, with each one coupling a pair of inductors.

The standard parameters are Inductor1, Inductor2, and k. Inductor1 is the name of first inductor, Inductor2 is the name of the second inductor, and k is the coefficient of coupling, 0 < k ≤ 1.

Inductive Coupling (XSPICE)

G41.png

This function is a conceptual model which is used as a building block to create a wide variety of inductive and magnetic circuit models. This function is normally used in conjunction with the “core” model, but it can also be used with resistors, hysteresis blocks, etc. to build up systems which mock the behavior of linear and nonlinear components. The lcouple takes as an input (on the “l” port) a current. This current value is multiplied by the num_turns value, N, to produce an output value (a voltage value which appears on the mmf_out port). The mmf_out acts similar to a magnetomotive force in a magnetic circuit; when the lcouple is connected to the “core” model, or to some other resistive device, a current will flow. This current value (which is modulated by whatever the lcouple is connected to) is then used by the lcouple to calculate a voltage “seen” at the “l” port. The voltage is a function of the derivative with respect to time of the current value seen at mmf_out.

The most common use for lcouple will be as a building block in the construction of transformer models. To create a transformer with a single input and a single output, you would require two lcouple models plus one “core” model.

Example:

A1 (1 0) (2 3) lcouple1

.model lcouple1 lcouple ( num_turns = 10 )

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
num_turns number of turns - 1 required

Inductor

GK121.png

Inductors are used to store magnetic energy. An inductor's ability to counteract current changes passing through it is called its inductance (L), which is measured in Henrys. In a (steady-state) DC analysis, the inductor acts like a short circuit. It is indeed treated as a current source, which can be problematic if an inductor is connected in series with a current source, or in series with a voltmeter, or in series with another inductor. The resistor may be of negligible value or one that accounts for the coil resistance of the inductor. In AC and transient analyses, the inductor develops a voltage across it in response to the changing magnetic flux within its coil.

An inductor's transient behavior is described by the equation:

v(t) = L*(di(t)/dt)

The inductor's initial condition is optional. It is the initial value of the inductor current in Amperes that flows from node N+ through the inductor to node N-. The only time that the initial current matters is when the simulator performs a transient analysis, and the "Use Initial Conditions" checkbox is checked.

An inductor's AC behavior is described by the equation:

v = j ω * L * i

All inductor names must begin with L.

Netlist Format:

L<device_name> <N+> <N-> <value>

Example:

L1 1 2 10u

Inductor with Ferrite Core

GK94.png

This 2-pin device models a physical inductor with a magnetic ferrite core. Its model is based on XSPICE's magnetic core and inductive coupling models. Unlike the standard inductor device, you do not specify an inductance value for the inductor with ferrite core. Rather, you specify physical parameters like cross sectional area, core length and number of turns. The physical model of the magnetic device is defined by two vectors: magnetic field intensity H in A/m and magnetic flux density B (also known as magnetic induction) in Tesla. The default array values are:

H_array = [-250 -100 -50 -37.5 -25 -12.5 0 12.5 25 37.5 50 100 250]

B_array = [-0.375 -0.36 -0.32 -0.29 -0.24 -0.15 0 0.15 0.24 0.29 0.32 0.36 0.375]

To change the value of H/B arrays, open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
n_turns number of turns - 100 required
area cross-sectional area m2 1e-5
length core length m 0.01

Insulated Gate Bipolar Transistor (IGBT)

GK111.png

This is a 3-pin parameterized Insulated Gate Bipolar Transistor (IGBT) device with three pins: Collector(C), Gate (G), and Emitter (E). It is primarily used as a fast electronic switch. The IGBT combines the simple gate-drive characteristics of MOSFETs with the high-current and low-saturation-voltage capability of bipolar transistors. The device's model consists of an isolated gate FET for the control input, and a PNP bipolar power transistor as a switch. To further modify the internal device models, open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
cap parasitic capacitance F 1n
rg gate resistance Ohms 5
re emitter resistance Ohms 0.05
bf pnp transistor forward beta - 1
vto MOSFET threshold voltage V 5
kt MOSFET transconductance - 2.99
cgso MOSFET voltage gate-source overlap capacitance F 5u
nd diode emission coefficient - 50
cjo diode junction capacitance F 1n

Interactive Switch

GK75.png

This device is an interactive switch that can be closed or opened either directly from the Schematic Editor by clicking on its symbol or from the Instrument Panel.

Junction Field Effect Transistor (JFET)

G12.png

The JFET is the simplest transistor device and has three pins: gate, drain and source. The JFET defaults are based on the Shichman and Hodges FET model. This is a square-law device because of the expression relating the drain current to the gate-to-source voltage: Idrain=*(VGS-Vthreshold)2. In real JFETs, near the saturation point, the drain currents vary with the drain voltages. This can be modeled by the following formula: Idrain=*(VGS-VTO)2*(1+*VDS), which yields an increasing drain current for increasing values of VDS.

The gate-to-source and gate-to-drain junctions each have a nonlinear capacitor. The zero-bias capacitance value is selected for each junction.

The standard device parameters are AREA, OFF, IC, and T. They are described below:

AREA area factor (optional) (If not specified, the default value is 1.0.)
OFF initial condition for the DC analysis (optional)
IC initial condition (optional) (Used when a transient analysis is desired, which starts from other than the quiescent operating point.)
T operating temperature of the device (optional)

The process model parameters are listed in the following table:

NAME PARAMETER UNITS DEFAULT EXAMPLE
VTO threshold voltage V -2 -2
BETA transconductance parameter A/V2 1.0e-4 1.0e-3
LAMBDA channel-length modulation parameter 1/V 0 1.0e-4
RD drain ohmic resistance ohms 0 100
RS source ohmic resistance ohms 0 100
CGS zero-bias G-S junction capacitance F 0 5pF
CGD zero-bias G-D junction capacitance F 0 1pF
PB gate junction potential V 1 0.6
IS gate junction saturation current A 1.0e-14 1.0e-14
B doping tail parameter 1 1.1
KF flicker-noise coefficient 0
AF flicker-noise exponent 1
FC coefficient for forward-bias depletion capacitance formula 0.5
TNOM parameter measurement temperature deg. C 27 50

Light Emitting Diode (LED)

GK114.png

This is a two-pin parameterized diode device that emits light of a certain wavelength when it is forward-biased.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
rs ohmic resistance Ohms 10
vj junction potential V 0.6
cjo zero bias junction capacitance F 10p
tt transit time sec 0.1n

Linear Current-Controlled Current Source (CCCS)

G2.png

The CCCS is a current source whose current is directly proportional to the current across a controlling Ammeter or a voltage source. There are two versions: two-terminal and four-terminal. For the two-terminal device, you must specify the name of the controlling Ammeter or voltage source, as well as the current gain, which has a default value of one. The four-terminal device already provides nodes for a controlling ammeter, and you just specify the current gain.

Model Identifier: cccs

Netlist Format:

F<device_name> <N+> <N-> <controlling_device_name> <value>

Example:

F1 1 0 V1 1.0

Linear Current-Controlled Voltage Source (CCVS)

G4.png

The CCVS is a voltage source whose voltage is directly proportional to the current through a controlling ammeter or a voltage source. There are two versions: two-terminal and four-terminal. For the two-terminal device, you must specify the name of the controlling Ammeter or voltage source, as well as the trans-resistance gain, which has a default value of one. The four-terminal device already provides nodes for a controlling ammeter, and you just specify the trans-resistance gain.

Model Identifier: ccvs

Netlist Format:

H<device_name> <N+> <N-> <controlling_device_name> <value>

Example:

H1 1 0 V1 1.0

Linear Voltage-Controlled Current Source (VCCS)

G3.png

The VCCS is a current source whose current is directly proportional to the voltage across a controlling voltmeter or the voltage between two circuit nodes. There are two versions: two-terminal and four-terminal. For the two-terminal device, you must specify the name of the controlling voltmeter or the two controlling nodes, as well as the trans-conductance gain, which has a default value of one. The four-terminal device already provides nodes for a controlling voltmeter, and you just specify the trans-conductance gain.

Model Identifier: vccs

Netlist Format:

G<device_name> <N+> <N-> <NC+> <NC-> <value>

Example:

G1 1 0 2 0 1.0

Linear Voltage-Controlled Voltage Source (VCVS)

G1.png

The VCVS is a voltage source whose voltage is directly proportional to the voltage across a controlling voltmeter of the voltage between two circuit nodes. There are two versions: two-terminal and four-terminal. For the two-terminal device, you must specify the name of the controlling voltmeter or the two controlling nodes, as well as the voltage gain, which has a default value of one. The four-terminal device already provides nodes for a controlling voltmeter, and you just specify the voltage gain.

Model Identifier: vcvs

Netlist Format:

E<device_name> <N+> <N-> <NC+> <NC-> <value>

Example:

E1 1 0 2 0 1.0

Lossless Transmission Line

G21.png

The lossless transmission line is a four-pin two-port device that models only one propagating mode of an ideal transmission line. When using this SPICE model, should all four nodes of the actual circuit be distinct, two modes may be activated, and this device would be insufficient for that purpose. To circumvent this potential problem, two transmission line devices would be required. Due to the implementation details, you may produce more accurate simulation results with a lossy transmission line device with zero loss.

Optional initial condition parameters are the voltage and current at each of the transmission line ports.

The standard device parameters are Z0, TD, F, NL, IC, described below:

Z0 characteristic impedance
TD transmission delay
F frequency
NL normalized electrical length of the transmission line with respect to the wavelength in the line at frequency F. (If F is specified, but NL is not, the default is 0.25.)
IC initial condition (Specifies the voltage and current at each of the transmission line ports.)

Lossy Transmission Line

G22.png

The lossy transmission line is a four-pin two-port convolution model for uniform constant-parameter distributed lines. MNAME is the process model name, which includes a set of pre-specified options as described below.

The device model parameters are listed in the following table:

NAME PARAMETER UNITS DEFAULT EXAMPLE
R resistance /length Ohm /m 0.0 0.2
L inductance/length henrys/m 0.0 9.13e-9
C capacitance/length farads/m 0.0 3.65e-12
LEN length of line m none 1.0
LININTERP use linear interpolation flag not set set
QUADINTERP use quadratic interpolation flag not set set
MIXEDINTERP use linear when quadratic seems bad flag not set set
COMPACTREL special reltol for straight line checking flag RETOL 1.0e-3
COMPACTABS special abstol for straight line checking flag ABSTOL 1.0e-9
NOCONTROL don't do complex time control flag not set set
STEPLIMIT always limit timestep to 0.8*(delay of line)
NOSTEPLIMIT don't always limit timestep to 0.8*(delay of line) flag not set set
TRUNCNR use Newton-Raphson method for timestep calculation in LTRAtrunc flag not set set
TRUNCDONTCUT don't limit timestep to keep impulse-response errors low flag not set set

The RLC (uniform transmission line with series loss only), RC (uniform RC line), LC (lossless transmission line), and RG (distributed series resistance and parallel conductance only) lines have been implemented. The length (LEN) must be given. COMPACTREL and COMPACTABS control the compaction of past history values used in convolution. Larger values for these lower accuracy but improve speed. These are used with the TRYTOCOMPACT option.

Magnetic Core (XSPICE)

G42.png

This device is used as a building block to create a wide variety of inductive and magnetic circuit models. It is almost always to be used in conjunction with the "lcouple" model to build up systems which simulate the behavior of linear and nonlinear magnetic components. There are two fundamental modes of operation for the core model. These are the "PWL" mode (which is the default and most likely to be of use to you) and the "Hysteresis" mode.

PWL Mode (mode = 1)

In the PWL mode, the model takes a voltage as input which it treats as a magnetomotive force (mmf) value. This value is divided by the total effective length of the core to produce a value for the Magnetic Field Intensity, H, which is then used to find the corresponding Flux Density, B, using the piecewise linear relationship described by you in the H_array / B_array coordinate pairs. B is then multiplied by the cross-sectional area of the core to find the Flux value, which is output as a current. The pertinent mathematical equations are:

H = mmf / L, where L = Length (in apmere-turns/meter)

B = f(H)

Φ = B * A, where A = Area

The B value is derived from a piecewise linear transfer function described to the model by the H_array and B_array coordinate pairs. This transfer function does not include hysteretic effects; for that, you would need to substitute a HYST model for the core. The magnetic flux value Φ in turn is used by the "lcouple" code model to obtain a value for the voltage reflected back across its terminals to the driving electrical circuit.

Hysteresis Mode (mode = 2)

In the Hysteresis mode, the model takes a voltage as input which it treats as a magnetomotive force (mmf) value. This value is used as input to the equivalent of a hysteresis code model block. The parameters defining the input low and high values, the output low and high values, and the amount of hysteresis are as in that model. The output from this mode, as in PWL mode, is a current value which is seen across the magnetic core port.

One final note to be made about the two core models is that certain parameters are specific to one or the other. In particular, the in_low, in_high, out_lower_limit, out_upper_limit, and hysteresis parameters are not available in PWL mode. Likewise, the H_array, B_array, area, ad length values are unavailable in Hysteresis mode. The input_domain and fraction parameters are common to both modes (though their behavior is somewhat different; for explanation of the input_domain and fraction values for the Hysteresis mode, please refer to the Hysteresis Block discussion.

Model Identifier: core

Netlist Format:

A<device_name> <mc1 _pin> <mc2_pin> <model_name>

.model <model_name> core area = <value> length = <value> H_array = [<value1> <value2>] B_array = [<value1> <value2>] {<param1 = value> < param2 = value> ...}

Example:

A1 1 2 core

.model core core area = 1 length = 1 H_array = [0 1] B_array = [0 1]

Parameters:

Name Description Default Notes
H_array magnetic field array [0 1] required
B_array flux density array [0 1] required
Area cross-sectional area 1 required
Length core length 1 required
Input_domain input smoothing domain 0.01
Fraction smoothing fraction/abs switch True
Mode mode switch (1=pwl, 2=hyst) 1
In_low input low value 0.0
In_high input high value 1.0
Hyst hysteresis 0.1
Out_lower_limit output lower limit 0.0
Out_upper_limit output upper limit 1.0

Marker

G16.png

The marker serves several purposes:

  • It can appear as a default plot in simulations if the "Voltage Probe" box is checked.
  • It can be used to set the initial voltage or voltage guess at the node it is connected to.
  • It can be used as a port for a subcircuit when you choose the checkbox labeled "Use as Subcircuit Port" is checked.
  • It can be used to explicitly set a node number in place of the arbitrarily assigned node number by the program. In this case, make sure the "Set Node Index" box is checked. Otherwise, it will act as just a voltage probe.
  • It can be used to connect different parts of a circuit in place of wires. To use markers as virtual connectors, place them at points where wires would otherwise connect. Then set the Part Title of the two (or more) markers to the same name, and they will act as a single circuit node.

MESFET

G14.png

The MESFET is a Schottky-barrier gate FET with six times greater electron mobility than silicon. MESFETs are important devices for creating high frequency circuits. They function by creating a potential barrier between the gate and the channel when the metal gate contacts the gallium-arsenide substrate. Electron velocity saturates for fields approximately ten times lower than with silicon. The Curtice model includes linear and saturated operation.

The standard parameters are AREA, OFF, IC, and T. They are described below:

AREA area factor (optional) (If not specified, the default value is 1.0.)
OFF initial condition for the DC analysis (optional)
IC initial condition (optional) (Used when a transient analysis is desired, which starts from other than the quiescent operating point.)
T operating temperature of the device (optional)

All the MESFET process model parameters are described in the following table:

NAME PARAMETER UNITS DEFAULT EXAMPLE
VTO pinch-off voltage V -2 -2
BETA transconductance parameter A/V2 1.0e-4 1.0e-3
B doping tail extending parameter 1/V 0.3 0.3
ALPHA saturation voltage parameter 1/V 2 2
LAMBDA channel-length modulation parameter 1/V 0 1.0e-4
RD drain ohmic resistance Ohm 0 100
RS source ohmic resistance Ohm 0 100
CGS zero-bias G-S junction capacitance F 0 5pF
CGD zero-bias G-D junction capacitance F 0 1pF
PB gate junction potential V 1 0.6
KF flicker noise coefficient - 0
AF flicker noise exponent - 1
FC coefficient for forward-bias depletion capacitance formula - 0.5

MOSFET

G13.png

The MOSFET is an active device that has up to 4 pins. The three standard pins are gate, drain, and source. These are given in the default symbol. The bulk node, which is grounded by default, is the fourth pin. The MOSFET with the bulk is named mos_n_lvl1_4 (the lvl1 is for level 1, the n for nmos, and the 4 for 4 pins.)

The standard parameters are L, W, AD, AS, PD, PS, NRD, NRS, OFF, IC, and T. They are described below:

L channel length, in meters
W channel width, in meters
AD,AS areas of the drain and source diffusions, in meters2
PD,PS perimeters of drain and source junctions, in meters(They default to 0.0.)
NRD,NRS equivalent number of squares of the drain and source diffusions (These values multiply the sheet resistance for an accurate representation of parasitic series drain and source resistance of each transistor. The default value is 1.0.)
OFF initial condition for the DC analysis (optional)
IC initial condition (optional) (Used when a transient analysis is desired, which starts from other than the quiescent operating point.)
T operating temperature of the device (optional)

There are five different default models: square-law I-V characteristic, analytical, semi-empirical, and BSIM and BSIM2 (Berkeley Short-channel IGFET Model), which include second-order effects such as channel-length modulation, subthreshold conduction, scattering-limited velocity saturation, small-size effects, and charge-controlled capacitance. The process parameter LEVEL specifies which of the models is chosen as indicated below:

LEVEL 1 Schichman-Hodges
LEVEL 2 MOS2
LEVEL 3 MOS3
LEVEL 4 BSIM
LEVEL 5 BSIM2
LEVEL 6 MOS6

The process model parameters for levels 1,2,3, and 6 are listed in the following table:

NAME PARAMETER UNITS DEFAULT EXAMPLE
LEVEL model index 1
VTO zero-bias threshold voltage V 0.0 1.0
KP transconductance parameter A/V2 2e-5 3.1e-5
GAMMA bulk threshold parameter V1/2 0.0 0.37
PHI surface potential V 0.6 0.65
LAMBDA channel-length modulation (level 1 & 2 only) 1/V 0.0 0.02
RD drain ohmic resistance ohms 0.0 1.0
RS source ohmic resistance ohms 0.0 1.0
CBD zero-bias B-D junction capacitance F 0.0 20fF
CBS zero-bias B-S junction capacitance F 0.0 20fF
IS bulk junction saturation current A 1.0e-14 1.0e-15
PB bulk junction potential V 0.8 0.87
CGSO gate-source overlap capacitance per meter channel width F/m 0.0 4.0e-11
CGDO gate-drain overlap capacitance per meter channel width F/m 0.0 4.0e-11
CGBO gate-bulk overlap capacitance per meter channel length F/m 0.0 2e-10
RSH drain & source diffusion sheet resistance ohm/area 0.0 10.0
CJ zero-bias bulk junction bottom capacitance per meter2 junction area F/m2 0.0 2e-4
MJ bulk junction bottom grading coefficient 0.5 0.5
CJSW zero-bias bulk junction sidewall capacitance per meter junction perimeter F/m 0.0 1.0e-9
MJSW bulk junction sidewall grading coefficient 0.5, 0.33 (level1), (level2,3)
JS bulk junction saturation current per meter2 of junction area A/m2 1.0e-8
TOX oxide thickness meter 1.0e-7 1.0e-7
NSUB substrate doping 1/cm3 0.0 4.0e15
NSS surface state density 1/cm2 0.0 1.0e10
NFS fast surface state density 1/cm2 0.0 1.0e10
TPG type gate material(+1 if opp. substrate, 0 if A1 gate, -1 if same as substrate) 1.0
XJ metallurgical junction depth meter 0.0 1
LD lateral diffusion meter 0.0 0.8
UO surface mobility cm2/Vs 600 700
UCRIT critical field for mobility degradation (level2 only) V/cm 1.0e4 1.0e4
UEXP critical field exponent in mobility degradation (level2 only) 0.0 0.1
UTRA transverse field coefficient (deleted for level2) 0.0 0.3
VMAX maximum drift velocity of carriers m/s 0.0 5.0e4
NEFF total channel-charge (fixed and mobile) coefficient (level2 only) 1.0 5.0
KF flicker noise coefficient 0.0 1.0e-26
AF flicker noise exponent 1.0 1.2
FC coefficient for forward bias depletion capacitance formula 0.5
DELTA width effect on threshold voltage (level2,3) 0.0 1.0
THETA mobility modulation (level3 only) 1/V 0.0 0.1
ETA static feedback (level3 only) 0.0 1.0
KAPPA saturation field factor (level3 only) 0.2 0.5
TNOM parameter measurement temperature deg. C 27 50

The BSIM model has no default parameters, and leaving one out is considered an error. The additional process model parameters for level 4 and 5 models are listed in the following table:

NAME PARAMETER UNITS
VFB flat-band voltage V
PHI surface inversion potential V
K1 body effect coefficient V1/2
K2 drain/source depletion charge-sharing coefficient
ETA zero-bias drain-induced barrier-lowering coefficient
MUZ zero-bias mobility cm2/V-s
DL shortening of channel m
DW narrowing of channel m
U0 zero-bias transverse-field mobility degradation coefficient V-1
U1 zero-bias velocity saturation coefficient m/V
X2MZ sens. of mobility to substrate bias at Vds=0 cm2/V2-s
X2E sens. of drain-induced barrier lowering effect to substrate bias V-1
X3E sens. of drain-induced barrier lowering effect to drain bias at Vds= Vdd V-1
X2U0 sens. of transverse field mobility degradation to substrate bias V-2
X2U1 sens. of velocity saturation effect to substrate bias mV-2
MUS mobility at zero substrate bias and at Vds= Vdd cm2/V2-s
X2MS sens. of mobility to substrate bias at Vds= Vdd cm2/V2-s
X3MS sens. of mobility to drain bias at Vds= Vdd cm2/V2-s
X3U1 sens. of velocity saturation effect on drain bias at Vds= Vdd mV-2
TOX gate oxide thickness m
TEMP temperature at which parameters were measured deg. C
VDD measurement bias range V
CGDO gate-drain overlap capacitance per meter channel width F/m
CGSO gate-source overlap capacitance per meter channel width F/m
CGBO gate-bulk overlap capacitance per meter channel length F/m
XPART gate-oxide capacitance-charge model flag
N0 zero-bias subthreshold slope coefficient
NB sens. of subthreshold slope to substrate bias
ND sens. of subthreshold slope to drain bias
RSH drain and source diffusion sheet resistance ohms/area
JS source drain junction current density A/m2
PB built-in potential of source drain junction V
MJ grading coefficient of source drain junction
PBSW built-in potential of source drain junction sidewall V
MJSW grading coefficient of source drain junction sidewall
CJ source drain junction capacitance per unit area F/ m2
CJSW source drain junction sidewall capacitance per unit length F/m
WDF source drain junction default width m
DELL source drain junction length reduction m

XPART=0 selects a 40/60 drain/source charge partition; XPART=1 selects a 0/100 partition.

Mutual Inductors

GK100.png

The mutual inductors device is a pair of inductors that are coupled to each other. L1 and L2 are the names of two inductors. You have to specify the inductance of inductor L1, the inductance of inductor L2, the initial current through each, and the coupling coefficient k, 0 ≤ k ≤ 1. The mutual inductance M expressed in units of H can be calculated using the following definition:

[math] k = \frac{M}{\sqrt{L_1 L_2}} [/math]

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
inductance1 inductance of inductor 1 H 1
inductance2 inductance of inductor 2 H 1
ic1 initial current through inductor 1 A 0
ic2 initial current through inductor 2 A 0
k coefficient of coupling - 1.0

Non-Ideal Current Transformer

GK104.png

This 8-pin device models a non-ideal lossy current transformer. Its model consists of an ideal transformer with more secondary turns than primary turns along with a number of parasitic elements. The interior pins with red wires give you direct access to the primary and secondary pins of the internal ideal transformer. on each side of the internal ideal transformer, there is a series leakage inductance LLk, followed by a shunt winding capacitance CWk and a series winding resistance RWk, which connects to the exterior positive pin on that side. The inter-winding resistance R12 is connected across the negative pins of the primary and secondary of the ideal transformer model. In a more complete model, an external inductor LM can be connected between the positive and negative interior pins of either the primary or secondary to account for the effects of the magnetization inductance.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
ratio secondary-to-primary turns ratio - 2 required
rw1 primary winding resistance Ohms 0.1
rw2 secondary winding resistance Ohms 0.1
ll1 primary leakage inductance H 1m
ll2 secondary leakage inductance H 1m
cw1 primary winding capacitance F 1p
cw2 secondary winding capacitance F 1p
r12 inter-winding resistance Ohms 10Meg

Non-Ideal Diode

G9.png

This 2-pin device is a basic simplified model of a diode as a rectifier or switch. When forward-biased, it acts as a low-valued voltage source. When reverse-biased, it acts as an open circuit until the reverse voltage exceeds the specified breakdown voltage. Then it acts as a high-valued voltage source of the reverse polarity.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
vf forward drop voltage V 0.5 required
vr reverse breakdown voltage V 100 required

Non-Ideal Voltage Transformer

GK103.png

This 8-pin device models a non-ideal lossy voltage transformer. Its model consists of an ideal transformer with more primary turns than secondary turns along with a number of parasitic elements. The interior pins with red wires give you direct access to the primary and secondary pins of the internal ideal transformer. There are series combinations of a winding resistance RWk and a leakage inductance LLk on the primary and secondary sides. These are connected between the positive interior and exterior pins on each side. There are also two shunt branches at the inputs of the primary and secondary sides (connected between the positive and negative exterior pins), each consisting of a distributed turn-to-turn winding resistance RDCk in series with a distributed turn-to-turn winding capacitance CWk. The inter-winding capacitance CWW12 is connected across the positive pins of the primary and secondary of the ideal transformer model. In a more complete model, an external inductor LM can be connected between the positive and negative interior pins of either the primary or secondary to account for the effects of the magnetization inductance.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
ratio primary-to-secondary turns ratio - 2 required
rw1 primary winding resistance Ohms 0.1
rw2 secondary winding resistance Ohms 0.1
ll1 primary winding leakage inductance H 1m
ll2 secondary winding leakage inductance H 1m
rdc1 primary distributed turn-to-turn winding resistance Ohms 1u
cw1 primary distributed turn-to-turn winding capacitance F 1p
rdc2 secondary distributed turn-to-turn winding resistance Ohms 1u
cw2 secondary distributed turn-to-turn winding capacitance F 1p
cww12 inter-winding capacitance F 1p

Nonlinear Capacitor

GK89.png

The nonlinear capacitor model allows the capacitor to be described by an arbitrary relationship between the capacitor's charge Q and the voltage V across the capacitor. In other words, Q = f(V). The nonlinear capacitance is then defined as C(V) = dQ/dV. You need to define the charge Q by a mathematical expression in the voltage V. You have to open the subcircuit model dialog by clicking the View Subcircuit button and edit its text. Enter any mathematical expression in the variable "v(pos,neg)" standing for the terminal voltage. The default expression is:

{ C_DEF } * v(pos,neg)

which implies a linear capacitor, where Q = CDEF V. Therefore, C = C(V) = dQ/dV = CDEF.

Another example is 1e-4*(v(pos,neg))^2.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
C_DEF default capacitance F 1

Nonlinear Conductor

GK88.png

The nonlinear conductor model allows the conductor to be described by an arbitrary relationship between the conductor's current I and the voltage V across the conductor. In other words, I = f(V). The nonlinear conductance is then defined as G(V) = dI/dV. You need to define the current I by a mathematical expression in the voltage V. You have to open the subcircuit model dialog by clicking the View Subcircuit button and edit its text. Enter any mathematical expression in the variable "v(pos,neg)" standing for the terminal voltage. The default expression is:

{ G_DEF } * v(pos,neg)

which implies a linear conductor, where I = GDEF V. Therefore, G = G(V) = dI/dV = GDEF.

Another example is 1e-4*(v(pos,neg))^2.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
G_DEF default capacitance S 1

Nonlinear Dependent Sources

G18.png

Nonlinear dependent (arbitrary) sources use an equation or mathematical expression to describe their behavior. One and only one of the two forms: V=<expr> or I=<expr> must be given.

Netlist Format:

B<device_name> v = <expression>

B<device_name> i = <expression>

Examples:

v = I(v1) + 3* I(v2)

I = v(i1) + 3* v(2) + 5 * v(3) ^2

The first example is a current-controlled voltage source. The v on the left side of the equation indicates that it is a voltage source. I(v1) and I(v2) are the currents through voltage sources named v1 and v2, respectively.

The second example is a voltage-controlled current source. v(2) and v(3) represents the voltages at nodes 2 and 3, respectively, and v(i1) represents the voltage across a current source named i1.

The following mathematical functions defined for real variables can be used in the expressions:

abs, acos, acosh, asin, asinh, atan, atanh, cos, cosh, exp, ln, log, sin, sinh, sqrt, tan.

The function "u" is the unit step and "uramp" is the integral of the unit step. The unit step is one if its argument is greater than zero and zero if its argument is less than zero. The ramp function (uramp) is 0 for argument values less than zero and equal to the argument for argument values greater than zero.

The following operators are permissible: +, -, *, /, ^, and unary-.

To get time into an expression, integrate the current from a constant current source with a capacitor and use the voltage across the capacitor.

Nonlinear Inductor

GK90.png

The nonlinear inductor model allows the inductor to be described by an arbitrary relationship between the inductor's magnetic flux Φ and the current I flowing through the inductor . In other words, Φ = f(I). The nonlinear inductance is then defined as L(I) = dΦ/dI. You need to define the flux Φ by a mathematical expression in the current I. You have to open the subcircuit model dialog by clicking the View Subcircuit button and edit its text. Enter any mathematical expression in the variable "i(vx)" standing for the device current. The default expression is:

{ L_DEF } * i(vx)

which implies a linear inductor, where Φ = LDEF I. Therefore, L = L(I) = dΦ/dI = LDEF.

Another example is 1e-4*(i(vx))^2.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
L_DEF default inductance H 1

Nonlinear Resistor

GK87.png

The nonlinear resistor model allows the resistor to be described by an arbitrary relationship between the voltage V across the resistor and its current I. In other words, V = f(I). The nonlinear resistance is then defined as R(I) = dV/dI. You need to define the voltage V by a mathematical expression in the current I. You have to open the subcircuit model dialog by clicking the View Subcircuit button and edit its text. Enter any mathematical expression in the variable "i(vx)" standing for the device current. The default expression is:

{ R_DEF } * i(vx)

which implies a linear resistor, where V = RDEF I. Therefore, R = R(I) = dV/dI = RDEF.

Another example is 10*(i(vx))^2.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
R_DEF default resistance Ω 1

Operational Amplifier (Op-Amp)

GK105.png

This three-pin device models a parameterized operational amplifier with a very high voltage gain, a very high input impedance and a very low output impedance. The behavioral model of the parameterized Op-Amp device is based on the algorithm found in the book Macromodeling with Spice, authored by Connelly & Choi, published by Prentice Hall. The default parameters are those of the 741 Op-Amp. This device doesn't require external DC bias voltage sources. Its positive and negative DC bias voltages are specified as its parameters. Sometimes the simulation doesn't converge if there is no DC path from the output of the Op-Amp to the ground.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
r_in_dm differential mode input resistance Ohms 2Meg
r_in_cm common mode input resistance Ohms 2G
Avd0 differential mode DC gain dB 106
CMRR common mode rejection ratio dB 90
r_out output resistance Ohms 75
c_in input capacitance F 1.4p
ios input offset current A 20n
ib input bias current A 80n
vio input offset voltage V 1m
slew_pos positive slew rate V/s 0.5e6
slew_neg negative slew rate V/s 0.5e6
curr_src_max maximum output source current A 25m
curr_sink_ maximum output sink current A25m
fp1 dominant pole frequency Hz 5
fp2 second pole frequency Hz 2Meg
fp3 third pole frequency Hz 20Meg
fp4 fourth pole frequency Hz 100Meg
fz first zero frequency Hz 5Meg
vcc_pos positive dc voltage source V 12
vcc_neg negative dc voltage source V 12

Optocoupler

GK115.png

This is a five-pin parameterized optocoupler device. Its model consists of an ideal diode device in series with an Ohmic resistance connected between the Anode (A) and Cathode (K) pins together with a bipolar junction transistor device with three accessible pins, Collector (C), Base (B) and Emitter (E). A current-controlled current source is connected between base and collector of the BJT, whose current is controlled by the current passing through the diode. The proportionality constant is twice the specified value of the current transfer ratio (ctr) parameter.

You can change or enhance the models of the diode and BJT by adding more parameters. To do so, you have to open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
ctr current transfer ratio - 0.5
rd diode ohmic resistance Ohms 0.1

Overtone Crystal

GK79.png

This is a 2-pin parameterized overtone crystal device.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
LM fundamental motional inductance H 250m
CM1 fundamental motional capacitance F 10f
RM1 fundamental motional resistance Ohms 20
RM3 3rd overtone motional resistance Ohms 50
RM5 5th overtone motional resistance Ohms 100
RM7 7th overtone motional resistance Ohms 150
C0 shunt capacitance F 3p

Photodiode

GK113.png

This is a 4-pin parameterized photodiode device. A pair of pins, Anode (A) and Cathode (K), represent the physical terminals of the photodiode. The photodiode model connected between the anode and cathode pins consists of the parallel connection of an ideal diode, a dark current source, a noise current source, a current-controlled current source, a diode capacitance, a shunt resistance altogether with a series resistance.

Another pair of pins IS+ and IS- act as an ammeter that must be inserted in a control circuit. The current passing through this ammeter controls the current of the photodiode. The default proportionality constant is unity. The controlling current is typically a function of light intensity incident on the surface of the photodiode.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
id dark current A 1n
ir noise current A 1p
cd diode capacitance F 10p
rs series resistance Ohms 1m
rp parallel resistance Ohms 1Meg

Piecewise Linear (PWL) Controlled Source

GL49.png

The Piecewise Linear (PWL) Controlled Source is a single-input and single-output function generator whose output is not necessarily linear for all input values. Instead, it follows an I/O relationship that is specified by the x_array and y_array coordinates. The x_array and y_array values represent vectors of coordinate points on the x and y axes, respectively. The x_array values are progressively increasing input coordinate points, and the associated y_array values represent the outputs at those points. There may be as few as two pairs specified, or as many as memory and simulation speed allow.

In order to fully specify outputs for values of Vin outside of the bounds of the PWL function, the PWL controlled source model extends the slope found between the lowest two coordinate pairs and the highest two coordinate pairs. This has the effect of making the transfer function completely linear for Vin less than x_array[0] and Vin greater than x_array[n]. It also has the potentially subtle effect of unrealistically causing an output to reach a very large or small value for large inputs. You should thus keep in mind that the PWL Source does not inherently provide a limiting capability.

In order to diminish the potential for divergence of simulations when using the PWL block, a form of smoothing around the x_array and y_array coordinate points is necessary. This is due to the iterative nature of the simulator and its reliance on smooth first derivatives of transfer functions in order to arrive at a matrix solution. Consequently, the two parameters "input_domain" and "fraction" are included to allow you some control over the amount and nature o the smoothing performed.

Fraction is a switch that is either TRUE or FALSE. When TRUE (the default setting), the simulator assumes that the specified input_domain value is to be interpreted as a fractional figure. Otherwise, it is interpreted as an absolute value. Thus, if fraction = TRUE and input_domain = 0.10, the simulator assumes that the smoothing radius about each coordinate point is to be set equal to 10% of the length of either the x_array segment above each coordinate point, or the x_array segment below each coordinate point. The specific segment length chosen will be the smallest of these two for each coordinate point.

If fraction = FALSE and input_domain = 0.10, then the simulator will begin smoothing the transfer function at 0.10 volts (or amperes) below each x_array coordinate and will continue the smoothing process for another 0.10 volts (or amperes) above each x_array coordinate point.

Model Identifier: pwl

Netlist Format:

A<device_name> %vd(<in_pin> <in_ref_pin>) %vd(<out_pin> <out_ref_pin>) <model_name>

.model <model_name> pwl x_array = [<value1> <value2> ...] y_array = [<value1> <value2> ...] {<param1 = value> < param2 = value> ...}

Example:

A1 %vd(2 3)  %vd(1 4) pwl .model pwl pwl x_array = [0 1] y_array = [0 1]

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
x_array x-element array V [0 1] required
y_array y-element array V [0 1] required
input_domain input smoothing domain - 0.01
fraction smoothing %/abs switch - True

PM Modulated Source

GL25.png

This is a voltage source with a single-tone phase modulated waveform. The PM modulation index MDI is defined as the ratio of maximum phase deviation to maximum signal amplitude.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
V0 offset V 0
VA amplitude V 1
FC carrier frequency Hz 1 required
MDI modulation index - 0 required
FS signal frequency Hz 1 required

Potentiometer

GK77.png

This is a 3-pin device that models a potentiometer with options for either linear or logarithmic resistance. position = 0 corresponds to the wiper being at the extreme left and position = 1 corresponds to the wiper being at the extreme right. With the default position = 0.5 corresponding to the midpoint, this device functions as a one-half voltage divider.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
position position of wiper connection - 0.5 Must be between 0.0 and 1.0.
log log-linear switch - False Select False for linear and True for logarithmic.
r total resistance Ohms 0.1u
log_multiplier multiplier constant for log resistance - 1.0

Programmable Unijunction Transistor (PUT)

GK112.png

This is a 3-pin parameterized Programmable Unijunction Transistor (PUT) device with three pins: Base 1 (B1), Base 2 (B2) and Emitter (E). It is biased with a positive voltage between the two bases. This device has a unique characteristic that when it is triggered, its emitter current increases regeneratively until it is restricted by emitter power supply. It exhibits a negative resistance characteristic and so it can be employed as an oscillator. The device's model involves an NPN BJT and a PNP BJT. The forward beta parameters of the two transistors are set equal to 100 and 1, respectively. To change these values, open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
eta - - 0.6
rbb total base-to-base resistance Ohms 40k
rf forward resistance Ohms 1Meg
rr reverse resistance Ohms 1Meg
rgk gate-to-cathode resistance Ohms 100
bvf breakdown voltage of forward diode V 100
bvr breakdown voltage of reverse diode V 100
bvgk breakdown voltage of gate-to-cathode diode V 5

Random Resistor

GK93.png

The random resistor device models a resistor whose resistance is a random number between 0 and a maximum specified value.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
max_val maximum resistance value Ω 1k

Real Capacitor

GK117.png

This is primarily a non-ideal, temperature-dependent capacitor model. You can access it from the Parts Menu as User-Defined Capacitor. It has two temperature coefficients: first-order TC1 temperature and second-order TC2. The value of the temperature-dependent capacitance is computed using the quadratic equation:

C(T) = C(T0) * [ 1 + TC1 * (T - T0) + TC2 * (T-T0)^2 ]

The device's model includes a series resistance and a series inductance together with the capacitor, all in parallel with a shunt resistance.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
Resr series resistance Ω 10
Ls inductance H 1p
C capacitance F 1n
Rp parallel resistance Ω 1G
ic voltage initial condition V 0
temp operating temperature deg C 27
tc1 first-order temperature coefficient F/°C 0.1
tc2 second-order temperature coefficient F/°C2 0.01

Real Inductor

GK118.png

This is primarily a non-ideal inductor model. You can access it from the Parts Menu as User-Defined Inductor. Its series resistor has two temperature coefficients: first-order TC1 temperature and second-order TC2. The value of the temperature-dependent resistance is computed using the quadratic equation:

R(T) = R(T0) * [ 1 + TC1 * (T - T0) + TC2 * (T-T0)^2 ]

The device's model includes a series resistance together with the inductor, and the combination in parallel with a shunt capacitance.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
Rdc series resistance Ω 10
L inductance H 1
Cp capacitance F 1p
ic current initial condition A 0
temp operating temperature deg C 27
tc1 first-order temperature coefficient Ω/°C 0.1
tc2 second-order temperature coefficient Ω/°C2 0.01

Real Resistor

GK116.png

This is primarily a non-ideal, temperature-dependent resistor model. You can access it from the Parts Menu as User-Defined Resistor. It has two temperature coefficients: first-order TC1 temperature and second-order TC2. The value of the temperature-dependent resistance is computed using the quadratic equation:

R(T) = R(T0) * [ 1 + TC1 * (T - T0) + TC2 * (T-T0)^2 ]

The device's model includes a series inductance together with the resistor.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
R resistance Ω 1k
Ls inductance H 1n
temp operating temperature deg C 27
tc1 first-order temperature coefficient Ω/°C 0.1
tc2 second-order temperature coefficient Ω/°C2 0.01

Resistor

GK119.png

Resistors are passive devices that dissipate power. Their resistance value varies depending on how much power they can dissipate and is measured in Ohms. The transient, DC and AC behaviors of a resistor are all described by the same equation:

v = R * i

where v is the voltage across the resistor, i is the current passing through the resistor, and R is the resistance. The value of R must be nonzero.

All resistor names must begin with R.

Netlist Format:

R<device_name> <N+> <N-> <value>

Example:

R1 1 2 1k

RF.Spice A/D provides three types of resistor: Simple, User-Defined (Real Resistor) and Semiconductor. The resistance of the simple resistor is a single value expressed in Ohms. You can also set the Monte Carlo tolerance for this resistor.

Schottky Diode

GK80.png

The Schottky diode has the same model as the generic diode with a nonzero transit time (tt), a nonzero junction capacitance (cjo) and a typically larger saturation current (is), a lower junction potential (vj) and a smaller grading coefficient (m).

Semiconducting Capacitor

GK83.png

This is the more general form of the Capacitor model and allows for the calculation of the actual capacitance value from strictly geometric information and the specifications of the process.

General Form:

CXXXXXXX N1 N2 <VALUE> <MNAME> <L=LENGTH> <W=WIDTH> <IC=VAL>

If VALUE is specified, it defines the capacitance. If MNAME is specified, then the capacitance is calculated from the process information in the model MNAME and the given LENGTH and WIDTH. If VALUE is not specified, then MNAME and LENGTH must be specified. If WIDTH is not specified, then it is taken from the default width given in the model. Either VALUE or MNAME, LENGTH, and WIDTH may be specified, but not both sets. The optional initial condition "IC" is the initial voltage across the capacitor for transient simulations.

The capacitance is computed as:

CAP = CJ * (LENGTH - NARROW) * (WIDTH - NARROW)+ 2 * CJSW * (LENGTH + WIDTH - 2NARROW) * CAP

To modify the model parameters, first double click on the capacitor to edit its top-level model parameters. Then choose the button labeled Edit from Table in the process model section. This will open a window in which you can edit CJ, CJSW, NARROW, DEFW, and CAP.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
CJ junction bottom capacitance F/m2 -
CJSW junction sidewall capacitance F/m -
DEFW default device width m 1u
NARROW narrowing due to side etching m 0
CAP nominal capacitance for Monte Carlo simulation F 1

Semiconductor Resistor

GK82.png

This is the more general form of the resistor model and allows for the modeling of temperature effects and for the calculation of the actual resistance value from strictly geometric information and the specifications of the process.

General Form:

RXXXXXXX N1 N2 <VALUE> <MNAME> <L=LENGTH> <W=WIDTH> <TEMP=T>

If VALUE is specified, it overrides the geometric information and defines the resistance. If MNAME is specified, then the resistance may be calculated from the process information in the model MNAME and the given LENGTH and WIDTH. If VALUE is not specified, then MNAME and LENGTH must be specified. If WIDTH is not specified, then it is taken from the default width given in the model. The (optional) TEMP value is the temperature at which this device is to operate, and overrides the temperature specification in the SPICE Options Dialog.

The resistance is computed as:

R(T0) = (RSH) * [(L - NARROW) / (W - NARROW)] * RES

R(T) = R(T0) * [ 1 + TC1 * (T - T0) + TC2 * (T-T0)^2 ]

To modify the model parameters, first double click on the resistor to edit its top-level model parameters. Then choose the button labeled Edit from Table in the process model section. This will open a window in which you can edit TC1, TC2, RSH, RES, etc.

NAME PARAMETER UNITS DEFAULT NOTES
TC1 first order temperature coefficient Ω/°C -
TC2 second order temperature coefficient Ω/°C2 -
RSH sheet resistance Ω/sq -
DEFW default device width m 1u
NARROW narrowing due to side etching m 0
TNOM the parameter measurement temperature deg C 27
RES resistance multiplier for Monte Carlo simulation Ohms 1

Silicon-Controlled Rectifier (SCR)

GK109.png

This is a 3-pin parameterized Silicon-Controlled Rectifier (SCR) device with three pins: Anode (A), Cathode (K) and Gate (G). It is a unidirectional device which can conduct current only in one direction. The SCR can be triggered only by a positive current going into its gate. The device's model involves an NPN BJT and a PNP BJT. The forward beta parameters of the two transistors are set equal to 100 and 1, respectively. To changes these values, open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
rf forward resistance Ohms 1Meg
rr reverse resistance Ohms 1Meg
rgk gate-to-cathode resistance Ohms 100
bvf breakdown voltage of forward diode V 100
bvr breakdown voltage of reverse diode V 100
bvgk breakdown voltage of gate-to-cathode diode V 5

SPDT Switch

GK72.png

This is a 5-pin device that models a single-pole double-throw switch. The input voltage is transferred to the first output pin if the control voltage is at a high state. Otherwise, its is transferred to the second output pin.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
von turn-on voltage V 3.3
voff turn-off voltage V 0.3
vt threshold voltage V 1.0
ron on resistance Ohms 1.0
roff off resistance Ohms 1Gig

SPST Switch

GK71.png

This is a 4-pin device that models a single-pole single-throw switch. It is virtually equivalent of the standard voltage-controlled switch.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
von turn-on voltage V 3.3
voff turn-off voltage V 0.3
vt threshold voltage V 1.0
ron on resistance Ohms 1.0
roff off resistance Ohms 1Gig

Tabulated Conductor

GK92.png

The tabulated conductor model allows the conductance to be described by a table relating the device's current i(t) to its terminal voltage v(t). In effect, the conductance is defined as G = di(t)/dv(t). The model provides two interpolation options: cubic spline and piecewise linear. You can enter the (v,i) data pairs in the text box provided in the property dialog. Or you can import the data from a text file.

Tabulated Resistor

GK91.png

The tabulated resistor model allows the resistance to be described by a table relating the device's terminal voltage v(t) to its current i(t). In effect, the resistance is defined as R = dv(t)/di(t). The model provides two interpolation options: cubic spline and piecewise linear. You can enter the (i,v) data pairs in the text box provided in the property dialog. Or you can import the data from a text file.

Tapped Inductor

GK101.png

This 3-pin device models a tapped inductor with mutual coupling effect.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
Lt total inductance H 1m
ratio ratio of number of turns between positive terminal and tap to total number of turns - 0.5
k coefficient of coupling - 1.0

Temperature-Dependent Current Source

GL14.png

This is a current source whose current is an arbitrary function of the circuit temperature. You have to open the subcircuit model dialog by clicking the Edit Model... button and edit its text. Enter any mathematical expression in the variable "v(T)" standing for temperature. Note that the circuit temperature is set and controlled by the parameter "temp" in the Miscellaneous tab of the SPICE Simulation Options dialog.

Examples:

  • v(T) is equivalent to f(T) = T.
  • 1 + 0.1*(v(t))^2 is equivalent to f(T) = 1 + 0.1T.

Parameters:

None

Temperature-Dependent Voltage Source

GL13.png

This is a voltage source whose voltage is an arbitrary function of the circuit temperature. You have to open the subcircuit model dialog by clicking the Edit Model... button and edit its text. Enter any mathematical expression in the variable "v(T)" standing for temperature. Note that the circuit temperature is set and controlled by the parameter "temp" in the Miscellaneous tab of the SPICE Simulation Options dialog.

Examples:

  • v(T) is equivalent to f(T) = T.
  • 1 + 0.1*(v(t))^2 is equivalent to f(T) = 1 + 0.1T.

Parameters:

None

Thermometer

G115.png

The Thermometer is a two-pin device that measures the operating temperature of a circuit. The voltage across the device pins is equal to SPICE's operating temperature in degrees centigrade. The output voltage of the Thermometer can be used in conjunction with linear or nonlinear dependent sources to model temperature-dependent quantities.


Model Identifier: thermo


Parameters:

This device has no parameters.

Triac Thyristor

GK110.png

This is a 3-pin bidirectional thyristor device that conducts current in either direction when triggered. A thyristor is analogous to a relay in that a small voltage and current can control a much larger voltage and current. The triac has two anode pins termed Main Terminal 1 (MT1) and Main Terminal 2 (MT2) and a Gate (G) pin. In order to create a triggering current for a triac, either a positive or negative voltage can be applied to the gate. Once triggered, the thyristor continues to conduct, even if the gate current ceases, until the main current drops below a certain level called the holding current. The device's model involves two NPN BJT transistors and two PNP BJT transistors. The forward beta parameters of the NPN and PNP transistors are set equal to 20 and 5, respectively. To changes these values, open the subcircuit model dialog by clicking the View Subcircuit button and edit its text.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
rf forward resistance Ohms 1Meg
bvf breakdown voltage of forward diodes V 100
rh resistance controlling reverse holding current Ohms 100
rgp resistance controlling forward holding current and trigger current Ohms 50

Uniform RC Transmission Line

G23.png

The standard parameters are L, and N. They are described below:

Two of the nodes are the element nodes connected by the RC line. The third is the node to which the capacitances are connected. L is the length of the RC line in meters. N is the number of lumped segments to use in modeling the RC line.

This device is derived from a model proposed by Gertzberrg. It expands the URC line into a network of lumped RC segments with internally generated nodes. These segments increase toward the middle of the URC line in a geometric progression with K as the proportionality constant.

The URC line is made up entirely of resistor and capacitor segments, unless the ISPERL parameter has a non-zero value. In this case, capacitors are replaced by reverse biased diodes with an equivalent zero-bias junction capacitance, a saturation current of ISPERL amps per meter of transmission line, and optional series resistance of RSPERL ohms per meter.

Parameters:

NAME PARAMETER UNITS DEFAULT EXAMPLE
K propagation constant - 2 1.2
FMAX maximum frequency of interest Hz 1.0G 6.5Meg
RPERL resistance per unit length Ohm /m 1000 10
CPERL capacitance per unit length F/m 1.0e-15 1pF
ISPERL saturation current per unit length A/m 0 -
RSPERL diode resistance per unit length Ohm/m 0 -

Varactor Diode

GK81.png

A varactor diode is a combination of the generic diode with additional package inductance, package capacitance and a series resistance. This diode device has a typically large value of junction capacitance (cjo).

Parameters (in addition to standard diode parameters):


NAME PARAMETER UNITS DEFAULT NOTES
q quality factor - 5000
f0 frequency of Q-factor specification Hz 50Meg
ls package inductance H 0.5n
cp package capacitance F 0.05p

Voltage-Controlled Capacitor

GK85.png

This 3-pin device models a voltage-controlled two-terminal capacitor whose capacitance is linearly proportional to a control voltage that is applied to a third (CTRL) pin. The proportionality constant is a conversion factor which you need to specify in F/V.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
K_C conversion factor F/V 1.0

Voltage-Controlled Inductor

GK86.png

This 3-pin device models a voltage-controlled two-terminal inductor whose inductance is linearly proportional to a control voltage that is applied to a third (CTRL) pin. The proportionality constant is a conversion factor which you need to specify in H/V.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
K_L conversion factor H/V 1.0

Voltage-Controlled Resistor

GK84.png

This 3-pin device models a voltage-controlled two-terminal resistor whose resistance is linearly proportional to a control voltage that is applied to a third (CTRL) pin. The proportionality constant is a conversion factor which you need to specify in Ω/V.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
K_r conversion factor Ω/V 1.0

Voltage-Controlled Switch

G19.png

Switches are devices that exhibit high resistance when open (OFF state) and low resistance when closed (ON state). The switch model allows an almost ideal switch to be specified. With careful selection of the on and off resistances, they can effectively represent zero and infinite resistances in comparison to other circuit elements, while sustaining the model condition of a positive, finite value.

There are two versions of Voltage-Controlled Switch: two-terminal and four-terminal. For the two-terminal device, you must specify the name of the controlling Voltmeter or controlling voltage nodes, as well as the turn-on and turn-off voltages in Volts and on and off resistance values in Ohms. The four-terminal device already provides nodes for a controlling voltmeter, and you just specify the rest of parameters. When the voltage across the switch or controlling device is greater or equal to the turn-on current, the switch closes. When the voltage across the switch or controlling device is less than or equal to the turn off current, the switch opens.

Parameters:

NAME PARAMETER UNITS DEFAULT NOTES
V_ON turn-on voltage V 0.5
V_OFF turn-off voltage V 0.0
RON on resistance Ohms 1.0
ROFF off resistance Ohms 1G

Voltage Noise Source

GL15.png

This is a voltage noise generator characterized by a spectral density and corner frequency. You have to click the Edit Model... button to access the parameters of this device.

Parameters:

NAME PARAMETER UNIT DEFAULT NOTES
En noise voltage V/√Hz 1n required
freq noise corner frequency Hz 100 required

Voltage Source

G17A.png

A voltage source has a DC value, a transient behavior, an AC behavior, and distortion parameters. The transient type, AC parameters, and distortion parameters are defined on the first tab of the source's property dialog. The transient expression can be a pulse, sinusoid, exponential, or piecewise linear. The DC value of a voltage source is its initial transient value. For a source with a sinusoidal transient behavior, for example, the DC value will be equal to its transient offset voltage. The AC parameters are magnitude and phase. These are used during the AC Frequency Sweep analysis. The distortion parameters, two sets of magnitude and phase, are used during the distortion analysis. The AC and distortion parameters are defined on the second tab of the source's property dialog.

XSpice Devices and their models

XSpice devices have the following form:

A<device_name> <node1> <node2> ... <model_name>

e.g., A2 1 2 transfer_function Note that XSpice devices must start with the "A" designation, much as a resistor starts with an "R". Some devices will have grouped (or vector) pins and are designated by being placed inside square brackets. In the example shown below, the 1 and 2 pins are grouped. Pin 3 is not.

A1 [1 2] 3 summer

Some models will have voltage differential pairs of pins and will be denoted by a %vd( ). In the following example pins 1 and 4 are differential pairs, as well as pins 2 and 3. Differential pairs must go between parentheses ().

A1 %vd(1 4)  %vd(2 3) triangle

Refer to individual devices for more information.

Each XSpice device will also have a model associated with it. Each model will have the following form:

.model <model_name> <model_identifier> {<pname1 = pval1>} {<pname2 = pval2>} ...

e.g., .model transfer_function s_xfer in_offset = 0.0 gain = 1.0

Model_name refers to the name given in the device line. Model_identifier is an internal designation and must be of an existing designation Refer to each device's example for the correct designation.

Parameter values are optional. If they aren't specified, then the default will be used. Some devices have parameters that require a value and must be specified. Refer to individual devices for any required parameters.

Zener Diode

G10.png

The Zener Diode models the DC characteristics of most zeners. Since most data sheets for zener diodes do not give detailed characteristics in the forward region, only a single point defines the forward characteristicThe saturation current refers to the relatively constant reverse current that is produced when the voltage across the zener is negative, but breakdown has not been reached. The reverse leakage current determines the slight increase in reverse current as the voltage across the zener becomes more negative. It is modeled as a resistance parallel to the zener with value v_breakdown / i_rev.

Note that the limt_switch parameter engages an internal limiting function for the zener. This can, in some cases, prevent the simulator from converging to an unrealistic solution if the voltage across or current into the device is excessive. If use of this feature fails to yield acceptable results, the convlimit option should be tried (add the following statement to the SPICE input deck: .options convlimit)

Model Identifier: zener

Netlist Format:

A<device_name> <z_pin> <z_out_pin> <model_name>

.model <model_name> zener v_breakdown = 1 {<param1 = value> < param2 = value> ...}

Example:

A1 1 2 zener

.model zener zener v_breakdown = 1

Parameters:

Name Description Default Notes
v_breakdown breakdown voltage 1 required
i_breakdown breakdown current 2.0e-2
i_sat saturation current 1.0e-12
N_forward forward emission coefficient 1.0
limit_switch switch for on-board limiting (convergence aid) False

 

Back icon.png Back to RF.Spice A/D Wiki Gateway