SPICELib.src

Source code of SPICELib

Information

Library Designer Documentation

1. ARCHITECTURE

1.1 CONTROLLER LEVEL: ANALYSIS MODELS

1.2 CONTROLLED LEVEL: DEVICE MODELS

1.3 INITIALISATION FILE

1.4 GLOBAL PARAMETERS

2. DEVICE MODELS

2.1 LINEAR RESISTOR

2.2 CAPACITOR

2.3 INDUCTOR

2.4 PN-JUNCTION DIODE

2.4.1 Voltage-dependent capacitor

2.4.2 Voltage-controlled current source

2.5 LEVEL1 N-CHANNEL MOSFET

2.5.1 I_DS current source

2.5.2 Gate capacitances

2.6 LEVEL1 P-CHANNEL MOSFET

2.6.1 I_DS current source

2.6.2 Gate capacitances

2.7 INDEPENDENT SOURCES

2.7.1 DC analysis

2.7.2 Transient analysis

2.7.3 AC small-signal analysis

2.7.4 Model of the disabled formulations

2.7.5 Total power dissipation

3. ANALYSES

3.1 BIAS POINT CALCULATION

3.1.1 Static model iteration

3.1.2 Static model ramping

3.1.3 GMIN stepping

3.1.4 Dynamic model ramping

3.2 BIAS POINT ANALYSIS

3.3 AC SWEEP ANALYSIS

3.4 TRANSIENT ANALYSIS

1. ARCHITECTURE

A two-level architecture is proposed (see Figure 1):

Upper (controller) level is composed of the analysis models.
Lower (controlled) level is composed of the device models.
Unidirectional control signals (arrow in Fig. 1) and global variables transmit the information from analysis models to device models. In addition, global parameters set properties common to both analysis and device models.

The list of files and subpackages of package SPICELib.src is shown in Table 1.

Figure 1. Two-level architecture of SPICELib.

Table 1. Complete list of files and packages of SPICELib.src.

File	Package (SPICELib.src.)
analyses.mo	ANALYSES
breakout.mo	BREAKOUT
functions.mo
init.mo	INIT
interface.mo	INTERFACE
source.mo	WAVEFORMS SOURCE
special.mo	SPECIAL

1.1 CONTROLLER LEVEL: ANALYSIS MODELS

An important feature of SPICELib device models is their variable structure nature. A different device model is formulated for each analysis mode: static model (DC analysis), AC small-signal model (AC analysis), and large-signal model (transient analysis). The transitions among these three device formulations are carried out in simulation time.

A DC analysis

can be performed prior to a transient analysis to determine the transient initial condition, and
it is automatically performed prior to an AC small-signal analysis to determine the linearized, small-signal models for the nonlinear devices.

In addition, some bias point calculation algorithms require the combined use of the three device formulations. See Figure 2, where S.M.I., S.M.R., GMIN and D.M.R. stand for the four bias point calculation algorithms supported by SPICELib.

Figure 2. Some analysis require the combined use of several device formulations.

ANALYSES package contains the OP, TRAN and AC models. Bias point calculation is a part of OP and AC analyses and it is an option of TRAN analysis. Therefore, the four bias point calculation algorithms are programmed in a separate partial model, called BiasPointCalculation, inherited by the analysis models (see Fig. 1). Device models have a variable structure and signals are defined to control the model structure transitions. Each analysis model consist on an ordered sequence of elementary operations implying changes in the device model structure. Analysis models set the control signals in order to accomplish the required device-model structure changes. Control signals and global variables, evaluated in the analysis models, are shown in Figure 3.

Figure 3. Control signals, global variables and global parameters.

1.2 CONTROLLED LEVEL: DEVICE MODELS

Device models are grouped in three packages:

BREAKOUT,
SOURCE, and
SPECIAL.

The models of BREAKOUT and SOURCE packages allow the composition of user-defined circuits, while the SPECIAL's provide one way to specify the initial conditions. In addition, a fourth package containing the device model interfaces has been defined: INTERFACE.

1.3 INITIALISATION FILE

The initialisation file, init.mo, contains the INIT package. The control signals, the global variables and the global parameters (see Fig. 3) are defined in the INIT package. It contains two partial models:

Analysis, inherited by the analysis models.
Part, inherited by the device models.

The same set of control signals, variables and parameters are defined in both partial models: Analysis model variables are inner ones, while Part variables are outer ones.

1.4 GLOBAL PARAMETERS

Two global parameters have been defined (see Fig. 3). TimeScale parameter is used for setting the length of the source ramping processes of some bias point calculation algorithms. In addition, it is used for establishing the time elapsed between consecutive control signal transitions (conceptually similar to the system clock period). To this end, the integer constant TIME_SLOT constant is defined in the analysis models. It represents a porcentage (1 to 100). The time between consecutive events, CLOCK, is defined as shown in Fig. 3.

2. DEVICE MODELS

2.1 LINEAR RESISTOR

Resistor model is shown in Figure 4. The purpose of the static-model IC1-like circuits (switches, R_EPS resistors and voltage sources) is clamping the DC-formulation voltage at the resistor pins. The bias point claculation algorithm "dynamic model ramping" requires the following operation: clamping the DC formulation voltage to the instantaneous value of the large-signal formulation. The ctrl_RBREAK_Tran2DC signal controls this information transfer between formulations. When ctrl_ RBREAK_Tran2DC becomes true:

The source voltages (vDCclampP and vDCclampN; see Fig. 4) are set to the instantaneous value of the transient voltage at the correspondent pin. Then source voltages are held constant.
The switches are closed (see Fig. 4). They remain closed only while the signal is true.

Figure 4. Resistor model.

2.2 CAPACITOR

Linear and voltage-dependent capacitors have to be modelled. The partial model Capacitor (BREAKOUT package) describes all the capacitor behavior except its large-signal and AC small-signal capacitance. The Capacitor1 model (linear capacitor) and semiconductor-device capacitors models extend the Capacitor model. CBREAK is a linear capacitor without high index problems. It consists of Capacitor1 in series with a resistor.

Capacitor static formulation is shown in Figure 5. The implementation of the IC property requires the IC2-like circuit (switch, R_EPS resistor and vClampDC source).

Large-signal model is shown in Figure 5. IC2-like circuit is also included because the "dynamic model ramping" algorithm uses the large-signal formulation during the bias point calculation. The Boolean signals

ctrl_IC_clampDC, and
ctrl_IC_clampTran.

controls the static and large-signal model switches respectively.

The capacitor parameter IC_ENABLED enables or disables the IC property. It allows distinguishing between the cases when IC is intentionally set to zero and those cases when the IC property is not enabled.

The signal ctrl_IC_mode controls vClampDC and vClampTran voltages. Some bias point calculation algorithms need the independent source ramping from zero up to their nominal initial values. When implementing these algorithms, the voltage clamping sources of the IC symbols and the capacitor IC property need also be ramped from zero to their respective IC values. Two cases are distinguished:

ctrl_IC_mode=0, the clamping voltage (vClampDC or vClampTran) is constant and equal to the IC value.
ctrl_IC_mode=1, the clamping voltage is ramped from zero up to its IC value.

Figure 5. Capacitor model.

The model of the capacitor IC property depends on whether the bias point is calculated or the calculation is skipped (see Fig. 6):

During the bias point calculation, the capacitor IC property is implemented using an IC2 symbol in parallel with the capacitor. The capacitor model contains this voltage-clamp circuit (see Fig. 5).
When the initial transient solution is skipped, the capacitor voltage is initialised to its IC value using a when clause (see Fig. 5).

Figure 6. Implementation of the initial conditions.

2.3 INDUCTOR

Linear inductors have to be modelled. The partial model Inductor (BREAKOUT package) describes all the inductor behavior except its large-signal and AC small-signal inductance. The Lbreak model (linear inductor) model extends the Inductor model. Inductor static formulation is shown in Figure 7. The implementation of the IC property requires the circuit shown in figure 7 (switch, R_BIG resistor and iClampDC source).

Large-signal model is shown in Figure 7. The switch, R_BIG resistor and iClampDC source are also included because the "dynamic model ramping" algorithm uses the large-signal formulation during the bias point calculation. The Boolean signals

ctrl_IC_clampDC, and
ctrl_IC_clampTran.

controls the static and large-signal model switches respectively.

The inductor parameter IC_ENABLED enables or disables the IC property. It allows distinguishing between the cases when IC is intentionally set to zero and those cases when the IC property is not enabled.

The signal ctrl_IC_mode controls iClampDC and iClampTran voltages. Some bias point calculation algorithms need the independent source ramping from zero up to their nominal initial values. When implementing these algorithms, the voltage clamping sources of the IC symbols and the inductor and capacitor IC property need also be ramped from zero up to their respective IC values. Two cases are distinguished:

ctrl_IC_mode=0, the clamping current (iClampDC or iClampTran) is constant and equal to the IC value.
ctrl_IC_mode=1, the clamping current is ramped from zero up to its IC value.

Figure 7. Inductor model.

The model of the inductor IC property depends on whether the bias point is calculated or the calculation is skipped (see Fig. 7):

During the bias point calculation, the inductor IC property is implemented using the circuit dual to the IC2 symbol in parallel with the inductor. The inductor model contains this current-clamp circuit (see Fig. 7).
When the initial transient solution is skipped, the indutor current is initialised to its IC value using a when clause (see Fig. 7).

2.4 PN-JUNCTION DIODE

The PN-junction diode model is the PSpice model (see Massobrio, G. and Antognetti P.: Semiconductor Device Modeling with SPICE. McGraw-Hill 2 edition, 1998).
SPICELib diode model, PSPICE_diode, is composed of a linear resistor (of Rbreak class), a voltage dependent capacitor and a voltage controlled non linear current source (see Fig. 8).

Figure 8. Diode model.

2.4.1 Voltage-dependent capacitor

It extends the partial model Capacitor, defining the large-signal and the AC small-signal capacitance. The mathematical relationship between the large-signal capacitance of the diode, C, and the large signal voltage drop across the capacitor, v, is a two-branches function, that can be conveniently described using the modelica expresion if then else:

C_d(v) is a continuous, highly non-linear function of v (sum of several exponentila terms). In order to illustrate the shape of the C-V characteristic of the C-V characteristic, the C-V curve of D1N4002 diode is represented in Fig. 9.

Figure 9. C-V characteristic of D1N4002.

2.4.2 Voltage-controlled current source

The static and large-signal constitutive relation of the source are:

In Figure 10 the I-V characteristic of diode D1N4002 is shown.

Figure 10. I-V characteristic of D1N4002.

2.5 LEVEL1 N-CHANNEL MOSFET

SPICELib N-MOS model, SPICE2_MOS1, is composed of linear resistors (of Rbreak class), voltage dependent capacitors and voltage controlled non linear current sources (see Fig. 11).

Figure 11. N-MOS model.

The drain-to-source current (I_ds) and the gate capacitances (C_GB, C_GS and C_GD) are function of the variables V_DS, V_GS and V_BS. However, V_GS and V_BS cannot be calculated form the terminal variables of the I_DS) source model (i. e., the voltage and current at their pins). Gate capacitors modeling presents a similar problem. This situation is solved in SPICELib defining the variables V_DS, V_GS and V_BS as inner variables of the transistor model, and as outer variables of its components: the I_DS current source and the gate capacitors.
The variables are defined as follows:
V_DS=noEvent(abs(C_GS.v-C_GD.v))
V_GS=max(C_GS.v, C_GD.v)
V_BS=max(C_BS.v, C_BD.v)
C.v represents the voltage drop across the capacitor C. As all terms C.v are state-variables of the large signal MOSFET model, these definitions tear the computational-casuality loops of the MOSFET large-signal description.

2.5.1 I_DS current source

Drain-to source current is described by Eq. (1) when the transistor is in the linear region and by Eq. (2) when it is in the saturation region. Equations (1) y (2) are valid for V_DS>0 (normal mode). For V_DS lower than 0 (inverted mode), SPICELib switches the source and drain in equations (1) and (2).

2.5.2 Gate capacitances

The three gate capacitances (i.e. C_GB, C_GS and C_GD) are nonlinear, continuous functions of V_GS. In addition, C_GS and C_GD are functions of V_DS when the transistor operates in the linear region.
For V_DS<0 (inverted mode), SPICELib switches the source and drain in the capacitance calculation. The transition between C_GS and C_GD at V_DS=0 is discontinuous in the SPICE2 model. In SPICELib a continuous link between C_GS and C_GD in the vicinity of V_DS=0 has been introduced.

2.6 LEVEL1 P-CHANNEL MOSFET

SPICELib P-MOS model, SPICE2_MOS1P, is composed of linear resistors (of Rbreak class), voltage dependent capacitors and voltage controlled non linear current sources (see Fig. 11).

Figure 12. P-MOS model.

The drain-to-source current (I_ds) and the gate capacitances (C_BG, C_SG and C_DG) are function of the variables V_SD, V_SG and V_SB. However, V_SG and V_SB cannot be calculated form the terminal variables of the I_SD) source model (i. e., the voltage and current at their pins). Gate capacitors modeling presents a similar problem. This situation is solved in SPICELib defining the variables V_SD, V_SG and V_SB as inner variables of the transistor model, and as outer variables of its components: the I_SD current source and the gate capacitors.
The variables are defined as follows:
V_SS=noEvent(abs(C_SG.v-C_DG.v))
V_SG=max(C_SG.v, C_DG.v)
V_SB=max(C_SB.v, C_DB.v)
C.v represents the voltage drop across the capacitor C. As all terms C.v are state-variables of the large signal MOSFET model, these definitions tear the computational-casuality loops of the MOSFET large-signal description.

2.6.1 I_SD current source

Source-to-drain current is described by Eq. (3) when the transistor is in the linear region and by Eq. (4) when it is in the saturation region. Equations (3) y (4) are valid for V_SD>0 (normal mode). For V_SD lower than 0 (inverted mode), SPICELib switches drain and source in equations (3) and (4).

2.6.2 Gate capacitances

The three gate capacitances (i.e. C_BG, C_SG and C_DG) are nonlinear, continuous functions of V_SG. In addition, C_SG and C_DG are functions of V_SD when the transistor operates in the linear region.
For V_SD<0 (inverted mode), SPICELib switches the drain and source in the capacitance calculation. The transition between C_SG and C_DG at V_SD=0 is discontinuous in the SPICE2 model. In SPICELib a continuous link between C_SG and C_DG in the vicinity of V_SD=0 has been introduced.

2.7 INDEPENDENT SOURCES

There are a lot of similarities between the models of the voltage and the current independent sources:

the interface,
the DC and transient analysis signals (i.e., the stimulus),
etc.

The characteristics in common are defined in the partial model Stimulus (SOURCE package), and the source models (i.e., VSource and ISource) inherit it.

Source model parameters allow defining the DC and AC characteristics of the source: DC_VALUE, AC_MAG and AC_PHASE. Time-dependent waveforms used in the transient analyses are defined in the WAVEFORM package: EXP, PULSE, PWL, CONST and SIN. The Stimulus model inherits the waveform model as a replaceable model. Therefore, the waveform model can be redeclared when instantiating the source model (no waveform is selected by default). Some examples are provided in Table 2.

Table 2. Examples of source instantiations.

DC and AC specifications	SOURCE.VSource V1( DC_VALUE=3, AC_MAG=10, AC_PHASE=45 );
EXP waveform	SOURCE.VSource V1( DC_VALUE=3, AC_MAG=10, AC_PHASE=45, redeclare model TransientSpecification = WAVEFORMS.EXP( S1=1,S2=2,TD1=1,TC1=1, TD2=3,TC2=1 ));
PULSE waveform	SOURCE.VSource V1( DC_VALUE=3, AC_MAG=10, redeclare model TransientSpecification = WAVEFORMS.PULSE( S1=1,S2=2, TD=1,TR=1, PW=3,TF=1, PER=8 ));
PWL waveform	SOURCE.VSource V1( DC_VALUE=3, AC_MAG=10, AC_PHASE=30, redeclare model TransientSpecification = WAVEFORMS.PWL( signalCorners = { 1, 2, 4, 8, 16 }, timeCorners = { 0, 1, 2, 3, 4 } ));

2.7.1 DC analysis

The control signal ctrl_DC enables or disables the DC model (see Fig. 6):

While ctrl_DC==false, the DC value of all the independent sources of the circuit is zero.
While ctrl_DC==true, the DC value of the sources is determined by the integer parameters:
- ctrl_OP_mode, and
- ctrl_OP_value.

Figure 8. Independent sources. Static model.

In order to set the source value when calculating the initial transient condition, a parameter is associated to each waveform model: TRANS_INITIAL. This parameter coincides with the waveform initial value.

The parameter ctrl_OP_value determines the source value during the static model solution:

ctrl_OP_value==0: source value is DC_VALUE.
ctrl_OP_value==1: value is TRANS_INITIAL.

The parameter ctrl_OP_mode determines the mode of reaching the previous value:

ctrl_OP_mode==0: the source is hold constant to the value.
ctrl_OP_mode==1: the source value is increased linearly from zero with a slope equal to the value divided by TimeScale.

The "dynamic model ramping" algorithm requires the cancellation of the independent sources. The control signal ctrl_IS_inhibit allows this operation (see Fig. 7). While it is true:

voltage independent sources are substituted by opens (current=0), and
current independent sources by shorts (voltage=0).

Figure 8. Independent sources. Device models.

2.7.2 Transient analysis

The control signal ctrl_Tran determines (see Fig. 8):

whether the transient analysis is enabled, and the source signal is calculated of its associated waveform (ctrl_Tran==true),
or the static bias point calculation is enabled (ctrl_Tran==false). The algorithm "dynamic model ramping" requires the circuit large-signal model simulation in order to calculate a "good" initial value for static model iteration.

While ctrl_Tran==false, the source value is determined by the parameter ctrl_IS_TranOP:

While ctrl_IS_TranOP==false, the value is zero.
While ctrl_IS_TranOP==true, the value depends on the parameters ctrl_OP_mode, and ctrl_OP_value. The response associated to these parameters is the same than the previously discussed for the static formulation.

Figure 9. Independent sources. Large-signal model.

2.7.3 AC small-signal analysis

While the control signal ctrl_AC is true, the AC small-signal value of the source is set according to the source parameters AC_MAG and AC_PHASE. Otherwise, the value is zero.

2.7.4 Model of the disabled formulations

It is important to notice that while a model formulation is not enabled, the correspondent values of the independent sources are zero. In this situation, the circuit node voltages are trivially calculated and the simulation computational effort is not unnecessarily increased. The control signals that enable each of the three formulations are:

ctrl_DC,
ctrl_Tran, and
ctrl_AC.

2.7.5 Total power dissipation

The bias point calculation includes the evaluation of the total power dissipation. It is calculated adding the contribution of all the independent voltage sources. The calculation is implemented thanks to the Modelica capability of describing "physical fields". The PowerDisipation connector is defined. The model of the voltage source contains:

an instantiation of this connector,
the declaration of an outer connector of this type,
the connection between them.

The "environment" (inner) connector is defined in the BiasPointCalculation model.

3. ANALYSES

3.1 BIAS POINT CALCULATION

SPICELib provides four alternative algorithms for solving the circuit static model:

static model iteration,
static model ramping,
GMIN stepping, and
dynamic model ramping.

The SOLVE_STATIC parameter determines which of the four algorithms to use.

Two control signals, internal to the analysis models, are defined to synchronize the bias point calculation with other analysis operations:

biasPoint. Its transition from false to true indicates that the static-model solution must start.
biasPointCalculated. When the static-model solution is just finished, it becomes true.

The BiasPointCalculation model reads the value of biasPoint signal and writes biasPointCalculated.

Next, the four algorithms are briefly discussed. The control signal transitions required for algorithm completion are shown, but for the sake of clarity, their cause-effect relationships are omitted. Two additional comments:

ctrl_OP_value signal is not written by the bias point calculation algorithms.
Control signals evaluated at bias point calculation and hold to false during the whole algorithm, are omitted.

3.1.1 Static model iteration (SOLVE_STATIC:=0)

The solution of the static problem is left in hands of the modelling environment. SPICELib has two symbols to provide an initial guess for Newton-Raphson algorithm: NODESET1 and NODESET2. The implementation of the algorithm is shown in Fig. 9.

Figure 10. Static model iteration algorithm.

3.1.2 Static model ramping (SOLVE_STATIC:=1)

This algorithm consists in ramping the static-formulation value of the independent sources from zero up to their target values. The clamping voltages of the IC symbols and the capacitor IC property are also adequately ramped. The value of the parameter TimeScale determines the length of the ramping. The algorithm is implemented by means of the signal transitions shown in Fig. 10.

Figure 11. Static model ramping algorithm.

3.1.3 GMIN stepping (SOLVE_STATIC:=2)

GMIN stepping attempts to find a solution for the static model (with power supplies at 100%) by starting with a large value of GMIN, initially 1.0e10 times the nominal value. If a solution is found at this setting, SPICELib reduces GMIN by a factor of 10 and tries again. This continues until either GMIN is back to the nominal value, or a repeating cycle fails to converge. This algorithm makes heavy use of equation continuity with respect to GMIN model parameters. The implementation of this algorithm is shown in Fig. 11.

Figure 12. GMIN stepping algorithm.

3.1.4 Dynamic model ramping (SOLVE_STATIC:=3)

The initial condition to iterate the static model is obtained by simulating the large-signal model. A transient analysis is performed: all sources are ramped up from zero to the desired initial value for the simulation and this value is held for some time to allow the circuit to stabilise. Then the large-signal formulation voltages are transferred to the static model (using ctrl_RBREAK_Tran2DC and ctrl_IS_inhibit). This static-circuit setting is held for a clock cycle. Then, the power supplies are connected to the circuit, the resistor voltage-clamping circuits are disconnected, and the static model is solved. The implementation of the algorithm is shown in Fig. 12.

Figure 13. Dynamic model ramping algorithm.

3.2 BIAS POINT ANALYSIS

The OP analysis (see Fig. 13):

forces the biasPoint signal to become true,
sets ctrl_OP_value signal to zero, and
finish the simulation one clock cycle after the biasPointCalculated signal becomes true.

Figure 14. OP analysis signals.

3.3 AC SWEEP ANALYSIS

The TYPE_AC_SWEEP parameter defines the frequency sweep type:

TYPE_AC_SWEEP==0: frequency linear sweep.
TYPE_AC_SWEEP==1: the frequency is swept logarithmically by decades.

AC small-signal analysis (see Fig. 14):

forces the biasPoint signal to become true, and
sets ctrl_OP_value signal to zero.

When biasPointCalculated becomes true, the AC analysis:

forces ctrl_AC to become true, enabling the AC model.
Starts the frequency sweep. The frequency variation in time depends on the sweep type. In both cases, the required log frequencies are spaced at regular time-intervals of length 2*CLOCK. Therefore, the ctrl_log_AC signal is a pulse train of period 2*CLOCK.

The simulation is finished one clock cycle after the frequency reaches END_FREQUENCY.

Figure 15. AC analysis signals.

3.4 TRANSIENT ANALYSIS

When the transient simulation is started, the value of the time variable is different of zero. For this reason, a variable is defined to measure the transient simulation time: TIME. The length of the transient simulation is set by the TSTOP parameter.

The transient analysis depends on the SKIP_INITIAL_TRAN_SOLUTION parameter (see Table 3).

Table 3. Transient analysis with and w/o initial calculation.

SKIP_INITIAL_TRAN_SOLUTION:=false	When biasPointCalculated becomes true, the circuit static model contains the transient initial solution. Then (see Fig. 15): ctrl_CBREAK_Tran2DC becomes true. The large-signal circuit state is initialised to the static-circuit voltage values. ctrl_Tran becomes true. The large-signal device models are enabled. The simulation terminates when timeTran reaches the value TRAN_STOP_TIME.
SKIP_INITIAL_TRAN_SOLUTION:=true	At initial time (see Fig. 16): ctrl_CBREAK_Tran2IC becomes true. The large-signal circuit state is initialised to the IC-property correspondent values. ctrl_Tran becomes true. The large-signal device models are enabled.

Figure 16. Transient analysis with initial calculation.

Figure 17. Transient analysis without initial calculation.

Name Description

ANALYSES

BREAKOUT

Rect2Polar

Decibels

Rad2Deg

Deg2Rad

INIT

INTERFACE

SOURCE

SPECIAL

WAVEFORMS

Name	Description
ANALYSES
BREAKOUT
Rect2Polar
Decibels
Rad2Deg
Deg2Rad
INIT
INTERFACE
SOURCE
SPECIAL
WAVEFORMS

SPICELib.src.Rect2Polar

Modelica definition

function Rect2Polar 
  input Real rect[2];
  output Real module;
  output nonSI.Angle_deg angle;
protected 
  SI.Angle angFirst;
  constant Real pi=3.14159265358979;
algorithm 
  module := sqrt(rect*rect);
  angFirst := if not module > 0 then 0 else arcsin(abs(rect[2])/module);
  angle := if rect[1] < 0 then pi - angFirst else angFirst;
  angle := if rect[2] < 0 then -angle else angle;
  angle := 180*angle/pi;
end Rect2Polar;

SPICELib.src.Decibels

Modelica definition

function Decibels 
  input Real x;
  output Real x_dB;
algorithm 
  x_dB := if x > 0 then 20*ln(x)/ln(10) else -1e-100;
end Decibels;

SPICELib.src.Rad2Deg

Modelica definition

function Rad2Deg 
  input SI.Angle angle_rad;
  output nonSI.Angle_deg angle_deg;
protected 
  constant Real pi=3.14159265358979;
algorithm 
  angle_deg := 180*angle_rad/pi;
end Rad2Deg;

SPICELib.src.Deg2Rad

Modelica definition

function Deg2Rad 
  input nonSI.Angle_deg angle_deg;
  output SI.Angle angle_rad;
protected 
  constant Real pi=3.14159265358979;
algorithm 
  angle_rad := pi*angle_deg/180;
end Deg2Rad;

HTML-documentation generated by Dymola Tue Oct 14 18:26:24 2003 .

SPICELib.src

Information

Library Designer Documentation

1. ARCHITECTURE

1.1 CONTROLLER LEVEL: ANALYSIS MODELS

1.2 CONTROLLED LEVEL: DEVICE MODELS

1.3 INITIALISATION FILE

1.4 GLOBAL PARAMETERS

2. DEVICE MODELS

2.1 LINEAR RESISTOR

2.2 CAPACITOR

2.3 INDUCTOR

2.4 PN-JUNCTION DIODE

2.4.1 Voltage-dependent capacitor

2.4.2 Voltage-controlled current source

2.5 LEVEL1 N-CHANNEL MOSFET

2.5.1 IDS current source

2.5.2 Gate capacitances

2.6 LEVEL1 P-CHANNEL MOSFET

2.6.1 IDS current source

2.6.2 Gate capacitances

2.7 INDEPENDENT SOURCES

3. ANALYSES

3.1 BIAS POINT CALCULATION

3.2 BIAS POINT ANALYSIS

3.3 AC SWEEP ANALYSIS

3.4 TRANSIENT ANALYSIS

1. ARCHITECTURE

1.1 CONTROLLER LEVEL: ANALYSIS MODELS

1.2 CONTROLLED LEVEL: DEVICE MODELS

1.3 INITIALISATION FILE

1.4 GLOBAL PARAMETERS

2. DEVICE MODELS

2.1 LINEAR RESISTOR

2.2 CAPACITOR

2.3 INDUCTOR

2.4 PN-JUNCTION DIODE

2.4.1 Voltage-dependent capacitor

2.4.2 Voltage-controlled current source

2.5 LEVEL1 N-CHANNEL MOSFET

2.5.1 IDS current source

2.5.2 Gate capacitances

2.6 LEVEL1 P-CHANNEL MOSFET

2.6.1 ISD current source

2.6.2 Gate capacitances

2.7 INDEPENDENT SOURCES

3. ANALYSES

3.1 BIAS POINT CALCULATION

3.2 BIAS POINT ANALYSIS

3.3 AC SWEEP ANALYSIS

3.4 TRANSIENT ANALYSIS

SPICELib.src.Rect2Polar

Modelica definition

SPICELib.src.Decibels

Modelica definition

SPICELib.src.Rad2Deg

Modelica definition

SPICELib.src.Deg2Rad

Modelica definition

2.5.1 I_DS current source

2.6.1 I_DS current source

2.5.1 I_DS current source

2.6.1 I_SD current source