# User manual | 7. Analogue simulation in Alecsis # 7. Analogue simulation in Alecsis

In time-domain analogue simulation, system of equations that describes the analogue circuit (system) is composed and solved in many time instants. If the circuit is nonlinear, the linearized system is created and solved in many iterations in every time instants, until the convergence occurs. Therefore, there are two loops - time-domain

(outer) loop and iterative (inner) loop. The control of time-step size and convergence control are described in

Chapter 5. In this chapter, built-in models and model description in AleC++ will be described.

As other circuit simulators, Alecsis is forming system of equations component by component, not equation by equation. That means, contribution of each component is determined as a "stamp", that is added to the system of equations. Therefore, discretization of differential equations, and linearization of nonlinear equations, is performed when the stamp is defined. To model the component, means actually to determine the stamp. Of course, AleC++ hides many formal aspects of such model description from the user, so the user has to describe the model equations, rather than the stamp itself.

One can conclude easily that the stamps of linear time-independent components are constant throughout the simulation. Therefore, these calculations should be performed out of both simulation loops. Time-dependent linear components would have stamps that change in every time instant, so these calculations should be pulled out of the iteative loop. Finaly, nonlinear components have stamps that has to be recalculated in every iteration. For that reason, model designer can use process synchronization, as described in Chapter 5.

There are no many language constructs that are specific for analogue simulation. Chapter 5, giving general overview, applies in full. Analogue circuits can be described structurally, combined with a functional description, or using purely functional description (command eqn ).

### 104

Alecsis 2.3 - User’s manual

### 7.1. Built-in analogue models

Alecsis has a set of built-in SPICE-like models. Alecsis should not be used as a replacement of SPICE, but rather for simulation using new models, that are not available in SPICE. However, it was useful to have a set of built-in models, that can be used for SPICE-like simulation, and also as a basis for structural and combined structural-functional modelling.

### 7.1.1. Resistor, capacitor, inductor, and ideal sources

Basic components are resistor, capacitor, inductor, ideal current and ideal voltage source. All such components have two terminal nodes (in AleC++ terminology, two terminal links of type node ). In Alecsis, they have only one parameter, named value , representing resistance, capacitance, inductance, current or voltage, respectively. That means, they are defined without the model card.

These elements allow shorthand notation. resistor r1, r2; capacitor cload, c2; cgen i1; vgen vdd; inductor l1; r1 (n1, 0) value = 3.4k; // 3400 ohms r2 (n1, n2) 2.7k; // short of value = 2.7k c2 (n2, 0) { value = 2.7k; } // long, but legal i1 (0, n2) 1mA; // current has direction from 0 to n2 vdd (0, n3) 5v; // 0 is 'positive' terminal, voltage of n3 is -5V l1 (n1, n5) 5uH;

In the description given above, you can see that such parameters allow shorthand notation, where the keyword value is omitted. Nodes n1 , n2 , etc., represent unknown quantities in the system of equations.

0 (number zero) is reserved for ground node.

Note: For ideal voltage source modelling and the inductor modelling, the branch current, i.e. current through the element is necessary. Therefore, every time when we connect such an element, a new link of type current is created. Such current carries the name of the element ( vdd and l1 are two currents in the example above). Creation of such new link, that is also an unknown quantity in the system of equations, is hidden from the user. However, one might need that current somewhere else -- as a result in command plot , or as a controlling variable in some other model. It can be accessed as any other link, using its name. This is the same as in SPICE.

We wanted to have user-defined models that have same characteristics as built-in components. It is already mentioned in Chapter 5, that the

module

can return link under its name. This is obviously intended for modelling of different voltage generators, where the current flowing through the branch can be returned to the hierarchically higher level. That current carries the name of the module .

In the example above, declarations can be omitted if we use implicit declarations given in standard header file alec.h

. Without the declarations, the above code is very similar in structure to SPICE input file.

From the components given above, resistor, ideal current and ideal voltage source are linear timeindependent models. Capacitor and inductor are linear, but time-dependent models, as time derivatives appear in

7. Analogue simulation in Alecsis

### 105

model equations. Time derivatives are discretized using formulae given in Chapter 5, where the time-step size is changing during the simulation run.

### 7.1.2. Built-in signal generators

Alecsis does not have many built-in signal generators. This is not a drawback since the user can define new signal generators easily. Some models already exist in model library. For such description, one can use ideal voltage and current source as a structural basis, and can add signal function easily in the functional part of the model - an example of combined structural-functional modelling. Such models are used the same as built-in models.

For example, pulse generator is not an built-in component, although an unavoidable element of time simulation. It is described as a module whose declaration is stored in a standard library "alec.h", and the body in the appropriate library (alec.ao). You can find more details about this model in the appendix on standard libraries of

AleC++.

Actually, built-in signal generators are here for historical reasons, as they were needed before language

AleC++ was completed.

### 7.1.2.3. Piecewise linear signal generators

Piecewise linear (PWL) sources are built-in components in Alecsis. There are voltage and current piecewise linear generators, declared as

vpwl

and

cwpl

.

It is defined time-value pairs, as in this example: vpwl vin; vin (n1, 0) { 2, 3; 4, -4; 6s, -4V; 8.0s, 1; }

The waveform of this voltage generator is given in Fig. 7.1.

Figure 7.1. Waveform of piecewise-linear voltage generator, given by 4 time/voltage pairs.

### 106

Alecsis 2.3 - User’s manual

The waveform is given by time/voltage pairs. The pairs have to be enclosed in parentheses, regardless of the number of points.

If the time instant of the first pair is greater than 0, the voltage value assumes the constant value between t=0 and the first pair, as in the example above. If the last time/value pair is before the tstop , the voltage keeps the constant value until tstop . Therefore, if there is only one pair, such voltage generator behaves as ideal voltage source of constant value. Similar rules apply for the current generator of type cpwl .

As any other voltage generator, vin in the example above generates link of type current . The current carries the same name, vin .

The number of parameters of such generator is not fixed. However, it need not to be a built-in element.

AleC++ allows realization of a module where the action block has variable number of parameters (see

Chapter 5 for details): module new_vpwl(node i,j) action(double time0, double value0, ...);

You need to use alternative syntax of determining of actual parameters (similar to function calls) and to define some terminator (e.g., time moment -1 ), which will mark the end of the list. The call of such a component would be:

#define EOL -1.0 new_vpwl vin; vin(n1, 0) action(0ns, 1v, 10ns, 2v, 100ns, 2v, 110ns, 2.5v, EOL);

Keep in mind that compiler cannot check the type of parameters in the place of symbol '...'. That is, all parameters, except the first two, have to meet expected types ( double in this case). See Chapter 5 for details on implementation of such action blocks.

### 7.1.2.4. Sinusoidal signal generators

Alecsis has built-in voltage and current source of sinusoidal signal

vsin

and

csin

. The parameters are

amp

(amplitude in V or A),

freq

(frequency in Hz),

phase

(initial phase shift in rad), and

dc_offset

(DC component in V or A): vsin vs; vs (n2, 0) { amp=2V; freq=1kHz; phase=30rad; dc_offset=0.5V; }

As any other voltage generator, vs in the example above generates link of type current . The current carries the same name, vs .

### 7.1.3. Controlled sources

Controlled sources are implemented as built-in elements, too. The controlling quantity at the input is either current or voltage, and the output quantity can be also either current or voltage. Therefore, there are four combinations:

vcvs

- voltage-controlled voltage source (takes parameter

gain

)

ccvs

- current-controlled voltage source (takes parameter

mi

)

7. Analogue simulation in Alecsis

### 107

vccs

- voltage-controlled current source (takes parameter

gm

)

cccs

- current-controlled current source (takes parameter

beta

) vcvs vg1; ccvs vg2; vccs cg3; cccs cg4; vg1 (n1, 0, n3, n4) gain = 2; vg2 (n5, 0, vg1) mi = 1.2; cg3 (0, n2, n3, n4) gm = 1e-4; cg4 (0, n2, vg2) beta = 50;

The first two actual links in all examples above are of type node . Voltage source vg1 has n1 as positive terminal, and vg2 has n5 as positive terminal. Currents of both current sources cg3 and cg4 assume direction from 0 to n2 as positive.

Current-controlled sources vg2 and cg4 have one more actual link of type current , which is the controlling variable. Voltage-controlled sources have two actual links of type node for control. Both sources vg2 and cg3 are controlled by the difference of voltages at nodes n3 and n4 .

The example shows that voltage sources of type vcvs and ccvs generate new currents. They are here used for control of generators of type ccvs or cccs .

### 7.1.4. SPICE-compatible nonlinear components

Circuit simulator SPICE has become a standard for circuit simulation. The biggest quality of this simulator are the models of nonlinear electronic components. For that reason, we have implemented the same models (as built-in models) in Alecsis.

For these models, Alecsis accept unmodified SPICE model cards. The keyword spice is used for that. For instance, if file mosfet.mod

, located in the working directory, contains models of MOS transistor given in

SPICE syntax, it can be included in your description using: spice {

# include "mosfet.mod"

}

### 7.1.4.1. Diode

Declaration of semiconductor diode utilizes the key word

diode

. A diode has two nodes -- anode and cathode, given in that order, and a model card of class

d

. The list of model card parameters, together with their default values, is given in Appendix. diode d1, d2; d1 (n1, 0) model = _1n914; d2 (n2, n1) model = by238;

### 108

Alecsis 2.3 - User’s manual

Declaration of metal-oxide-semiconductor field effect transistor (MOSFET) utilizes the key word

mosfet

.

MOS transistor has four terminal nodes -- drain, gate, source, and bulk, given in hat order, which is adopted from

SPICE. It also accepts a model card of class

nmos

/

pmos

(the same model parameters, but for n and p type of transistor channel).

Alecsis supports 4 types of MOS transistor models. There are three SPICE2 models (model parameter

LEVEL is 1-3), and also a BSIM model (Berkeley short-channel IGFET model) for transistors with submicron dimensions. According to HSPICE classification, BSIM model cards have the LEVEL parameter set to 13.

Regardless of the level, MOS transistors have geometric parameters for length (

l

), width of the channel (

w

), area (

,

as

) and circumference of drain and source (

pd

,

ps

). Channel length and width must be given, while other parameter have default value of 0. mosfet m1, m2; m1(n1,n2,0,0) { model=nes2mos; l=2u; w=6u; ad=as=10p; pd=ps=40u; } m2(n3,n4,n2,0) { model=pes2mos; l=w=3u; }//other parameters are 0

Note: MOS transistor models LEVEL 1, 2, and 3 have parasitic capacitances implemented as nonlinear capacitors, whose capacitances are calculated for given terminal voltages. This is so-called Meyer model, which exhibit charge nonconservation. Only BSIM ( LEVEL =13) model has correct parasitic capacitance model, where charge conservation is guaranteed. In this model, terminal charges are calculated rather than capacitances, and parasitic currents are derivatives of these charges. Terminal charges can (optionally) appear as independent variables in the circuit system of equations (see section on options in Chapter 5).

Any SPICE manual will offer additional information on the names of parameters in cards, their typical values, and the appropriate equations for different levels. We give the list of model parameters and their default values in the Appendix.

### 7.1.4.3. Bipolar junction transistors

For declaration of bipolar junction transistor, keyword

bjt

is used. There are four terminal nodes -- collector, base, emitter, and substrate, given in that order. The last node, substrate, can be omitted. It accepts standard SPICE model card of class

npn

/

pnp

. Beside the model card, there is an optional parameter,

area

(area of the transistor). bjt q1; q1 (c, b, e) model = bc1107a;

The list of model card parameters, together with their default values, is given in Appendix.

### 7.1.4.4. JFET

For declaration of junction field effect transistor (JFET), keyword

jfet

is used. It has three terminal nodes

-- drain, gate and source, given in that order. It accepts standard SPICE model card of

njf

/

pjf

type. Parameter

area

(area of the transistor) is optional.

7. Analogue simulation in Alecsis

njf j1; j1 (d, g, s) model = J2N2068;

The list of model card parameters, together with their default values, is given in Appendix.

### 7.1.5. Ideal switch

Switch is implemented in Alecsis as ideal component, whose resistance is zero when the switch is closed (on state) and infinite when it is open (off state). In Alecsis, switch is a voltage-controlled component. Unlike other ideal switches this does not pose any limits in circuit topology. Even loops and cutsets of switches are allowed, providing that the switching is regular. It can be used in both linear and nonlinear circuits. Switch is itself modelled as nonlinear.

Note: SPICE switch model has finite Ron and Roff resistances. Therefore, our switch model is not compatible with SPICE. You can easily define your own SPICE-like model of non-ideal switch, as a resistor whose resistance value is changed inside action block (see Section on combined structural-functional modelling on how to do that).

Switch is declared using keyword switch . switch sw; sw (n1, 0, n2, 0) { hyst=1; val_on = 3.5v; val_off = 1.5v; }

Switch has four terminal nodes. The first two are contact nodes, connected by the switch ( n1 and 0 in the example above). The last two are controlling nodes - voltage between two nodes is the controlling voltage Vc. In the example above, switch is controlled by the voltage at node n2 , as 0 represents the ground node.

The switch has four parameters -

val_on

,

val_off

,

hyst

and

paststate

. The first two are the thresholds, which are compared to the controlling voltage Vc. In most of the applications, these two thresholds are equal, val_on = val_off . If Vc> val_on , the switch is closed. If Vc< val_off , the switch is open.

If val_on = val_off , parameter

hyst

plays no role. In the example above, you can see that val_on can be different than val_off . When Vc is between these thresholds, the behaviour of the switch is determined by the parameter hyst . This parametercan take values 0 and 1 . If hyst is 1 , the switch has hysteresis. The switch state if Vc is between val_on and val_off depends on the switch history. It is allowed both that val_on > val_off , and val_on < val_off in that case. If hyst =1, and val_on > val_off, the controlling of the switch is the following:

• when Vc is growing, when it passes the threshold val_on , the switch is turned on (closed);

• when Vc is decreased, when it passes the threshold val_off , the switch is turned off (closed).

If hyst=1, and val_on > val_off , the control is somewhat different:

♦ when Vc is growing, when it passes the threshold (whatever comes first, val_on or val_off ) the switch is turned on (closed);

♦ when Vc is decreased, when it passes the threshold (whatever comes first, val_off or val_on ), the switch is turned off (closed).

If parameter hyst is 0 (which is the default value), the switch has no hysteresis. In this case, val_on must be equal or greater than val_off . Between val_on and val_off , the switch has continuous change of resistance. It should be noted that this is a continuous change between 0 (for

val_on ) and

(for

val_off

).

### 110

Alecsis 2.3 - User’s manual

hyst is optional, its default value is 0 (no hystersis).

Swtich also has parameter

paststate

. This is also an optional parameter. This parameter is actually not used to pass information to the model. It is intended to be used in another direction -- it returns information about the switch state in the previous (last solved) iteration.

In Alecsis, the switch is implemented as internally controlled, i.e. it is controlled by some circuit voltage. As that voltage can change from iteration to iteration, it is clear that the final state of the switch can be determined only when convergence occurs. In some cases, we want to know that switch state in the new iteration, and the parameter paststate can be used for that. For instance, if we model the diode D as the ideal switch, the model can be described as:

D

closed

open

if if p p

,

p

i

### ⎨

v if if

D is closed

, (7.1)

D is open

where i is the current through the diode (switch), and v is voltage on the diode (switch). The diode can be controlled by voltage or current, depending on the diode state. To model it correctly using ideal switch, we have to know the previous state of the switch. module switch_diode (node a; node k) {

vgen vcaux;

switch sd;

vcaux (aux,0);

sd (a,k,aux,0) { val_on=val_off=0.5; }

action () {

process per_iteration {

if ( !sd->paststate ) { /* switch was on (closed) */

if((current) sd>0) vcaux->value=1;

else vcaux->value=0;

} else { /* switch was off (open) */

if((node)a<(node)k) vcaux->value = 0;

else vcaux->value = 1;

}

}

}

}

This is an example of combined structural-functional modelling that will be explained later in more details.

The structural part of the model introduces the switch sd , and the ideal voltage source vcaux , which is used for switch control. (For diode model, we need switch controlled by the current. Switch is, however, implemented as voltage-controlled element, so we need some auxiliary voltage (node aux ) that will reflect changes of current). In the structural part, generator vcaux is left without voltage value. This value is given in the functional part

( action block), as an implementation of formula (7.1). Parameter paststate is used to return state of the switch in the previous iteration.

Note: The current through the switch is introduced as a new quantity in the system of equations (as was the case with ideal voltage generators). In the above example, current sd was used in the action block.

We have tried to diminish differences between built-in component models and user-defined models

(modules). We have explained in Chapter 5, that the action parameters can be used bidirectionaly. As you can see from this example, this is also the case with parameters of built-in components. Indirection operator -> was used to access both the action parameters and the built-in component parameters.

The switch model was implemented as built-in, as it has some influence to time-step control. In some classes of circuits, it was very important to simulate the switch just before the switch transition, and just after the switch

7. Analogue simulation in Alecsis

### 111

transition. It is important to simulate it just before the transition to obtain exact capacitor charges and inductor fluxes in the moment of transition, as these quantities are of importance for the circuit after the transition. After the transition, the time-step is reset, since the circuit has new topology. As the switches in Alecsis are internally controlled, the exact switching instant is not known in advance. An iterative process is implemented to find the switching instant with desired accuracy. See section on options in Chapter 5, where options SC_vtol ,

SL_itol and SDDT_tol are described.

Note: We have already stated that ideal switch model can be used in any circuit topology, even when there are loops of switches and ideal voltage generators exist, or cutsets of switches and ideal current generators.

The condition is that the switching is regular. If it is not the case, the solver cannot converge, which should be information for the user that there is problem with switching consistency (e.g. the part of the circuit is floating).

However, you should be aware that options for difficult convergence, dump and dcon , can sometimes force convergence even in such cases. Therefore, they should be used with care.

### 7.2. Structural modelling

Many models can be described as connections of some other models, e.g. resistors, controlled sources, etc. If we have a module , that has only declarative and structural part, and no functional part (no action block), we consider that as a structural modelling. Both built-in components and user-defined modules can appear as parts of such model. module real_voltage_source (node 1, 2) {

resistor r1;

vgen vg;

vg(1,3) 5;

r1(3,2) 1k;

}

Node 3 is implicitly declared in this example.

Purely structural model is actually describing subcircuit, defining circuit hierarchy in that way.

### 7.3. Combined structural-functional modelling

In fully functional modelling, the user can write model equations freely in the action block. However, this lack of restrictions can cause errors in the modelling process. Combined structural-functional modelling should be the preferred way of modelling, as it is more restrictive, and therefore not so error-prone.

In the combined approach, the user gives the structural description of the model (like in the structural modelling) but omit some or all of the parameters. These parameters are calculated and assigned to the components later, in the functional part ( action block). Such modelling technique is often used in electronics. An example is modelling of a nonlinear component, for instance diode, by linearizing it. Linearized diode model consists of a resistor and ideal current source (Figure 7.1.). Parameters of these components R

d m

and i

ds m

are recalculated in every iteration m using expressions (7.2) and (7.3)

### 112

Alecsis 2.3 - User’s manual

Figure 7.2. Diode and its linearized model.

R m d

i d

v d

### 1

v d

=

v m d

(7.2)

i m ds

=

i m d

v d m

R m d

(7.3)

Therefore, combined structural functional model of diode would consists of a resistor and ideal voltage source connected in parallel, and an action block, where parameters of these components are calculated in every iteration.

There is another reason to use combined approach instead of purely functional modelling whenever possible:

Alecsis can check circuit irregularities, such as loops of ideal voltage sources and inductors, or cutsets of ideal current sources and capacitor, and inform the user about them. Such checking is possible when we use combined modelling, since notion of these electronic components is still there. However, if we use equations, Alecsis cannot recognize components in them.

In combined modelling, you need to reference elements inside a process to access them. The name of an element in expressions is a pointer to the structure of element parameters. Some elements (resistor, capacitor, etc.) have only one element in the structure -- value , while the others have more (named) parameters. For instance, parameter value of resistor r1 is accessed as r1->value . All built-in element parameters are of double type, and the parameters of user defined components (submodules) are given in their declaration.

The problem can arise with component that return current (or some other link), like voltage sources and inductors are, since the names of element represent the current at the same time. Confusion is avoided as we can get the current (or other link) using cast operation (for source v1 the current is (current)v1 ). Without cast, the name represents the pointer to parameters.

### 7.3.1. Time-dependent linear models

We have already said that Alecsis has only ideal voltage and current source, and a pair of ideal signal generators as built-in components. Using combined modelling approach with ideal source as a basis, any signal generator can be easily described. To describe their behaviour, you often need only one process, and one line. For modelling of linear generators process with per_moment synchronization is used. The process is executed once in the given time instant.

#define twopi 6.282 module singen (node i, j) {

7. Analogue simulation in Alecsis

### 113

vgen gen;

gen (i, j);

action per_moment (double amp=1.0v, double freq=1kHz,

double phase=0.0rad, double offset = 0v) {

gen->value= offset + amp * sin( twopi*freq*now + phase );

}

} root test () {

singen g1, g2;

g1 (node1,node2) { amp=0.2V; freq=50Hz; phase=0; offset=0.5V; }

g2 (node3,node4) action (0.2V, 50Hz, 0, 0.5V); // another way

...

}

This example shows the simplicity of modelling of sinusoidal generator with adjustable amplitude, offset, frequency, and phase (all these parameters have default values, as well). As there is only one process , the keyword process synchronization

is not used, since the compiler takes the body of action with per_moment

Name of voltage source gen is used as pointer to structure containing parameters. There is only one parameter in the structure. That parameter can be reached using operator of indirection ( -> ), i.e. as gen-

>value . In such case, when there is only one parameter in the structure, one can use indirection by dereferencing

(operator * ), too:

*gen = offset + amp * sin ( twopi * freq * now + phase );

Built-in elements have their signals for synchronization. This is why linear and time-independent elements behave as if they have processes sensitive to signal initial , in other words the contributions to the system of equations are calculated only once. If we change values of parameters of such an element in the

process per_moment , like we do with the voltage source gen in the example above, we change their synchronization to per_moment

. In the same way, we can change synchronization of linear time-independent and linear time-dependent models to per_iteration, if we change values of their parameters in a process per_iteration . Nonlinear elements (transistors, diodes, etc.) cannot change their synchronization , as they already have the most frequent refreshing, per_iteration .

Note: You may have noticed operator

now

inside the function sin . It simply returns the current time moment of the simulation, which amounts to 0 for structural , post_structural and initial processes. You can call it from any C/C++ -like function, but if the function has not been called during the simulation the value of the operator will be 0.

Note: In the structural description, parameter values need not to be omitted. If parameter value is assigned in functional description ( action block), the value given in structural part is overwritten. The value assigned in the structural part is valid before the first execution of appropriate functional description. If no value is assigned, 0 is assumed until the first execution of functional description. It is useful to assign nonzero values in the case when zero values lead to singular matrix, which would abort the program in the phase of matrix renumeration

(only processes with synchronization structural are executed before the renumeration).

### 7.3.2. Nonlinear models

All built-in nonlinear components are modelled in Alecsis using Newton-Raphson method of linearization.

We can use Newton-Raphson method to linearize nonlinear models before composing equations, rather than to

### 114

Alecsis 2.3 - User’s manual

linearize nonlinear equations. You need to create a linearized scheme representing nonlinear component, where linear components in that scheme change values of parameters in every iteration. Iterations are repeated until convergence is reached.

We have already described such method in this section, using diode model as an example (Fig. 7.2.). The parameter values of linear components are obtained by differentiating nonlinear functions. Therefore, model of any nonlinear component can be described by declaring and connecting components of the linearized circuit, followed by calculations of differentials in every iteration. Differentiation has to be performed with respect to all controlling quantities, i.e. quantities that appear in the original nonlinear expressions. Often, all terminal quantities of that nonlinear component are the controlling quantities.

We shall give here example of a MOS transistor. This is the simplest version of MOS transistor model,

SPICE level 1 (Shichman-Hodges) model, without parasitic capacitances. Model is given as dependence of drain current I

D

on all terminal voltages. This nonlinear model has to be linearized with respect to all controlling quantities. If we consider source S as referent voltage, there are three controlling voltages - V

GS

, V

DS

, V

BS

. Linearized model is given as a parallel connection of three voltage-controlled current sources, and one independent current source (Figure 7.3.). Their parameters are recalculated in every iteration m using expressions (7.4.-7.7.).

Figure 7.3. MOS transistor and its linearized model.

g m m

I

D

V

GS

V

GS

=

V m

GS

,

V

DS

=

V m

DS

,

V

BS

=

V m

BS

(7.4)

g m ds

I

D

V

DS

V

GS

=

V m

GS

,

V

DS

=

V m

DS

,

V

BS

=

V m

BS

(7.5)

g m mbs

I

D

V

BS

V

GS

=

V m

GS

,

V

DS

=

V m

DS

,

V

BS

=

V m

BS

(7.6)

I m

S

I m

D

g m m

V m

GS

g m ds

V m

DS

### −

g m mbs

V m

BS

(7.7)

MOS model has a number of technological parameters. Those parameters should be grouped in model card.

A class containing these parameters is defined firstly. Model code is then described using functions that are methods of model class. These functions have access to parameters. Processes become shorter when bulk of the calculations is performed in methods.

The following example gives a functional description of MOS transistor:

#define Ntype 1.0

#define Ptype -1.0

7. Analogue simulation in Alecsis

### 115

class simple_mos { // new class of model cards

double type, gamma, phi;

double uo, vto, lambda;

public:

simple_mos ();

>simple_mos ();

~simple_mos ();

friend module smos;

}; simple_mos::simple_mos () { // constructor sets the initial values

type = 0.0 ; gamma = 0.7 ; phi = 0.5 ;

uo = 0.06; vto = 1.0 ; lambda = 0.0 ;

}

#define max(x,y) ((x)>(y)?(x):(y)) module simple_mos::smos (drain, gate, source, bulk) {

vccs e_gm, e_gmbs, e_gds;

cgen e_iaux;

/* linear voltage-controlled sources */

e_gm (drain, source, gate, source) gm=0.0;

e_gds (drain, source, drain, source) gm=0.0;

e_gmbs (drain, source, bulk, source) gm=0.0;

/* ideal current source */

e_iaux (drain, source);

action per_iteration ( double w, double l ) {

double vto_mod, vd, vg, vs, vb, vds, vbs, vgs;

double sarg,von,vgst,arg,beta,betap;

double gm, gds, gmbs, ids;

vd = drain; vg = gate; vs = source; vb = bulk;

vds = type * (vd - vs); vbs = type * (vb - vs);

vgs = type * (vg - vs); vto_mod = type * vto;

beta =w/l*uo;

if (vbs<=0.0) sarg=sqrt(phi-vbs);

else {

sarg=sqrt(phi); sarg -= vbs/(sarg+sarg);

sarg=max(0.0,sarg);

}

von=vto_mod+gamma*(sarg -sqrt(phi)); vgst=vgs-von;

if (sarg<=0.0) arg=0.0;

else arg=gamma/(sarg+sarg);

if (vgst<=0.0) {

/* cutoff region */

ids = gm = gds = gmbs = 0.0;

}

else {

betap=beta*(1.0+lambda*vds);

if (vgst<=vds) {

/* saturation region */

double vgst2;

### 116

Alecsis 2.3 - User’s manual

vgst2= 0.5*vgst*vgst; ids = betap*vgst2;

gm = betap*vgst; gds = lambda*vgst2;

gmbs = gm*arg;

}

else {

/* linear region */

double betap_vds,vdsh, arga;

betap_vds=betap*vds;

vdsh = 0.5*vds;

arga = vds *(vgst-vdsh);

ids = (gm=betap_vds)*(vgst-vdsh);

gds = betap*(vgst-vds)+lambda*beta*arga;

gmbs = gm*arg;

}

}

/* update element values */

e_gm->gm = gm; e_gds->gm = gds; e_gmbs->gm = gmbs;

*e_iaux = type *(ids - gm*vgs - gds*vds - vbs*gmbs);

}

} model simple_mos :: simnmos { type=Ntype;

vto = 0.82; gamma=0.59; phi=0.686; uo=0.051; lambda=0.051;

} model simple_mos :: simpmos { type=Ptype;

vto = -0.84; gamma=0.933; phi=0.733; uo=0.021; lambda=0.05; } root module test () {

smos m1, m2;

m1 (n_out, n_in, 0, 0) { W=5u; l=3u; model=simnmos; }

m2 (n_out, n_in, n_Vdd, n_Vdd) { W=5u; l=3u; model=simpmos; }

...

}

Note: In the structural description, parameter values need not to be omitted. If parameter value is assigned in functional description ( action block), the value given in structural part is overwritten. This is the case with values for gm given in the structural part to sources e_gm , e_gds and e_gmbs in the example above.

The value assigned in the structural part is valid before the first execution of appropriate functional description. If no value is assigned, 0 is assumed until the first execution of functional description. It is useful to assign nonzero values in the case when zero values lead to singular matrix, which would abort the program in the phase of matrix renumeration (only processes with synchronization structural are executed before the renumeration).

### 7.3.3. General nonlinear sources (automated linearization)

The linearization performed on MOS transistor model in the previous example means that we use Newton-

Raphson method. The drawback is that the user is responsible to define both the structure of the linearized circuit, and to define partial derivatives with respect to all controlling variables.

To make description of nonlinear models less error-prone and more user-friendly, we have developed special nonlinear controlled generators, where the process of linearization is performed automatically. These are:

7. Analogue simulation in Alecsis

### 117

♦ nlcgen - general nonlinear current generator; nlvgen - general nonlinear current generator; nlgen - general nonlinear equation.

In these nonlinear controlled generators, the user supplies only the nonlinear dependence, and Alecsis estimates partial derivatives, replacing them with appropriate finite differences. Alecsis is able to calculate these finite differences automatically. That means that the secant method is used for solving nonlinear problems in that case. Newton-Raphson method has quadratic convergence (error in the next iteration is equal to the square root of the error in the previous iteration). Secant method has lower order of convergence -- 1.62, instead of 2. Therefore, order of convergence is decreased.

Note: If we have a nonlinear circuit, usually only some of the models are described using nonlinear generators nlcgen , nlvgen , and nlgen . Other, for instance, built-in models use Newton-Raphson linearization. Therefore, the actual decrease of the convergence rate is low, and depends on the problem.

Since Alecsis estimates partial derivatives numerically, the nonlinear dependence can be even non-

differentiable (it is, however, understandable that non-differentiable functions with very strong nonlinearities would lead to convergence problems).

In all three types of nonlinear generators, there can be any number of controlling links (the only constraint is that there should be at lest one controlling link). Besides, type of controlling links is not constrained, too -- they can be of any analogue type ( node , current , charge , and flow ).

We shall now describe syntax of each type of nonlinear generators in more details.

### 7.3.3.1. Nonlinear current generator -- nlcgen

Nonlinear current generator has two nodes for connection, denoting where the generator current is flowing, and at least one controlling link (of any analogue type). The connection nodes are given first. The order of connection nodes is important, since it gives direction for current, as in any other current generator. The order of controlling links is arbitrary. If the connection nodes are also controlling (i.e. if the value of the current depends on connection nodes), they has to be stated again as controlling nodes).

In the structural part of the model, nonlinear generator is given without any parameters - only its connection is defined. The nonlinear dependance of the current is given in the functional description, i.e. in the action block. A process synchronized per_iteration has to be used, as dependence is nonlinear.

The example of MOS transistor model using nlcgen. module simple_mos::smos (drain, gate, source, bulk) {

nlcgen mos_current;

mos_current (drain, source, drain, gate, source, bulk);

/* current flows between drain and source, and is controlled

by node voltages drain, gate, source and bulk */

action per_iteration ( double w, double l ) {

...

... // calculates ids without derivatives - skipped here

nlcgen mos_current = type * ids;

}

}

### 118

Alecsis 2.3 - User’s manual

The current flows between nodes drain and source , and the voltages of all for connections control it.

As drain and source are controlling voltages, too, they are repeated in the set of controlling links. In the structural part of the module , no parameter is assigned to the nonlinear generator. The current value is calculated in the process synhronized per_iteration . In the same process, value is assigned to the generator using its name. In our example this was: nlcgen mos_current = type*ids;

In simpler cases, the whole calculation can be performed on this assignment, so that the process contains only one line of the code.

Note: Assignment operand ( = ) must not be understood literally here. The current is not actually assigned a value, partial derivatives are calculated and the contributions are added to the system of equations (so-called model stamp).

There can be any number of nonlinear generators declared inside one module . However, in the action block of the module, each nonlinear generator value is calculated inside separate process . In every iteration,

Alecsis executes that process code more than once, to estimate partial derivatives. Therefore, each nonlinear generator needs its own process , and all calculations regarding this generator should be in that process .

Therefore, there has to be one, and only one process per nonlinear generator:

module two_generators (node n1, n2, n3; current c3; flow f4) {

nlcgen gen1, gen2;

gen1(n1, n2, c3, f4);

gen2(n1, n3, n2, c3, n4);

action () {

process per_iteration {

nlcgen gen1 = c3*f4;

}

process per_iteration {

nlcgen gen2 = 5.*n2 - 6.*c3*n4;

}

}

}

Keyword nlcgen and component name ( gen1 or gen2 ) give information to Alecsis which process to connect with particular nonlinear generator.

Some special cases of controlled sources behave as basic components. So, nlcgen controlled by its own voltage behaves as a resistor: module new_resistor (node n1, n2) {

nlcgen r1;

r1(n1, n2, n1, n2);

action (double value) {

process initial {

if (value == 0.) warning ("zero resistance", 0);:

}

process per_iteration {

nlcgen r1 = (n1-n2)/value;

}

}

}

7. Analogue simulation in Alecsis

### 119

You can also model easily current-controlled and voltage-controlled current source ( cccs and vccs ).

However, in all these examples, synchronization per_iteration is used for otherwise linear and constant models, which makes such description inefficient.

Nonlinear generator frees the user from determining structure of the linearized model and from calculating partial derivatives. Nevertheless, you can use nonlinear generators in a different way, with user-defined partial derivatives. In this way, only the structure of the linearized model is determined automatically. The user has to define partial derivatives, and the Newton-Rahpson method is used, with quadratic convergence. The following example demonstrates modelling of a diode: module new_diode (node an, ch) {

nlcgen Id;

Id (an, ch, an, ch);

/* current flows from an to ch, controlled by

node voltages an and ch */

action (double is=1e-14) {

process per_iteration {

double vt = 25.8mV;

double gd, id;

id = is*(exp((ah-ch)/vt) - 1);

gd = (id + is)/vt;

nlcgen Id = id { @an = gd; @ch = -gd; }

}

}

}

With this description, simulator knows that source Id has the value id , and partial derivatives with respect to controlling links an and ch in every iteration. Operator @ is used with controlling link name to denote partial derivatives of a nonlinear function with respect to a particular link. If you omit the block containing partial derivatives, the secant method is used:

... nlcgen Id = id;

When partial derivatives are explicitely stated, the restriction about the number of nonlinear defined sources in a single process does not apply (the process is now executed only once in every iteration).

### 120

Alecsis 2.3 - User’s manual

### 7.3.3.2. Nonlinear voltage generator -- nlvgen

Nonlinear voltage generator has two nodes for connection, and at least one controlling link (of any analogue type). The order of connection nodes is important, since it gives orientation of the generator (positive node first).

All other rules and restrictions are the same as for nonlinear current generator ( nlcgen ). root module an_example_for_nlvgen () {

nlvgen nonlinear_vgen;

vgen v1, v2;

resistor r;

v1(n1, 0) 2;

v2(n2, 0) 3;

nonlinear_vgen(a,0, n1, n2);

r(a,0) 1.k;

timing { a_step = 1.; tstop = 100.; }

// current through nlvgen is available under its name

plot { node a; current nonlinear_vgen; }

action {

process per_iteration {

nlvgen nonlinear_vgen = n2*n3;

}

}

}

This is a very simple example with nlvgen , which here multiplies two voltages (2 and 3 volts), giving result of 6. As for any other voltage source, current through

nlvgen is introduced as new analogue link in

the system of equations. Here, current nonlinear_vgen is plotted out, and its value is 6mA.

Nonlinear voltage generator can be also used with user-defined partial derivatives, using the same syntax as for nlcgen .

### 7.3.3.3. Nonlinear equation -- nlgen

Nonlinear equation ( nlgen ) has somewhat different usage than nlcgen and nlvgen , although it follows the same syntax rules. It has no connection nodes, but has an arbitrary number of control links. It creates a new analogue link of type flow , which carries the same name as the generator. All contributions to the system matrix are in the same row, which corresponds to this new flow . For that reason, we can say that nlgen creates new (linearized) equation in the system matrix.

# include <math.h> // includes declaration for sqrt function module nlgen_test (flow f1, f2) {

nlgen gen;

gen(f1, f2); // f1 and f2 are controlling flows

action per_iteration {

nlgen gen = sqrt(n1*n2); // new equation

}

}

7. Analogue simulation in Alecsis

### 121

In this example, equation gen =( n1*n2 )

1/2

is created, and is added (in linearized form) to the system of equations. Obviously, unlike nlvgen and nlcgen , generator nlgen does not correspond to any electrical element. As it creates new quantity of type flow (in our case, flow gen ), it is to be used for modelling of nonelectrical problems.

Other rules and restrictions are the same as for nlcgen and nlvgen . Generator nlgen can be used with defined partial derivatives, too.

Note: As automatic linerization is very convenient for users, we would create other forms of automated linearization in the following versions of Alecsis. This wouls be automated linearization in purely functional modelling (command eqn ).

### 7.3.4. Virtual synchronization of processes

It is already explained that combined structural-functional modelling is based on connecting some built-in, or previously modelled components, and than changing their parameters in the functional part of the description

( action block).

All built-in components have their internal synchronization -- resistors are filled into the system matrix as processes initial , capacitors as processes synchronized per_moment , etc. When such built-in components are used in the structural part of model, their synchronization can be changed in the functional part. For instance, if linear and time-independent built-in component is used as part of the linearized model, their parameters are updated in every iteration when they are referenced in process per_iteration . Naturally, re-synchronization is possible only from less frequent to more frequent synchronization level (e.g. if nonlienar components are referenced in process initial , they would be still updated in every iteration).

On the other hand, user defined models have processes with fixed syncronization. For instance, we can have model described using fully functional modelling (explained later in this Chapter) with process initial : module constant_component (node n1, node n2) {

...

action (double value) {

process initial {

...

}

}

}

When describing some other model using combined approach, we can use a component of type contant_component as submodel. However, the problem can arise, since synhronization is here fixed, and no re-synchronization is possible. We want user-defined models to behave in the same manner as built-in components, and to be used equally. To enable that, we can add word

virtual

before the word process : module constant_component (node n1, node n2) {

...

action (double value) {

virtual process initial {

...

}

}

}

Such process will behave as ordinary process initial , if you set the component parameter value when connecting the component, and do not change it afterwards. However, if the parameter value is

### 122

Alecsis 2.3 - User’s manual

changed in a higher-order process ( per_moment , per_iteration ), the virtual process will be re-synchronized to that more frequent synchronization level.

If parent component is digital (processes are sensitive to changes on signals), such child virtual process initial would be re-synchronized to per_moment . The parameter value would be then updated when the parent process activates (when there is change on signal the parent process is sensitive to). However, the child process would be executed in every time-instant ( per_moment synchronization), in order to fill the analogue system matrix.

Processes sensitive to signals cannot have virtual synchronization.

### 7.4. Functional modelling -- eqn statement

In fully functional modelling, user can freely write the equations that contribute to the system of equations.

Therefore, there are no restrictions in what is to be described as a model.

Note: Lack of restrictions makes functional approach very powerful, but also error-prone. Alecsis, for instance, check if there are any loops of ideal voltage generators and inductors, or cutsets of ideal current sources and capacitors, etc. However, in fully functional modelling, there is no information about the model structure, so such checking is not possible. Therefore, one can make an error in eqn statement and create singular system of equations.

Equations are written using command eqn . They are written in the processes of the action block.

Therefore, structural part of the model can be completely omitted. There are three basic forms of this command:

simple eqn statement;

through eqn statement;

across eqn statement.

Simple eqn statement defines a single equation. All contributions to the matrix are in the same row.

Through eqn statement defines the current flowing through the branch between two specified nodes. It has contributions in two rows, corresponding to these two nodes, and can be replaced by two simple eqn statements.

Across eqn statement defines the voltage across the branch, between two specified nodes. It has contributions in three rows, corresponding to these two nodes and to the current flowing between them. Therefore, an across eqn statement can be replaced by three simple eqn statements.

Electrical current is therefore a through quantity, while the voltage is an across quantity. Such approach can be used in other physical problems, since we can define through and across quantities in them. Few examples are given in Table 7.1.

7. Analogue simulation in Alecsis

### 123

Table 7.1. Across and through quantities in different physical domains. generalized quantities electrical mechanical translational mechanical - rotational hydraulic across quantity through quantity power

P=V I P=v F

angular velocity

ω torque

τ

P=

ω τ pressure p ... flow Q ...

P=p Q etc.

...

For across quantity, an equation equivalent to Kirchhoff Voltage Law is satisfied, while through quentities must satisfy an equivalent of Kirchhoff Current Law. If the designer of electrical or nonelectrical models uses such paradigm of modelling, consistent system of equations will be built by Alecsis. Through and across

εθν

statements are more restrictive than simple eqn

statement, but they lead to better models.

Note: Using eqn

statements, linear differential equations can be described. Nonlinear equations cannot be described directly. Linearization of the model, according to Newton-Raphson method, has to be performed by the user. Such linearization and eqn

statement have to be in process

synchronized per_iteration

. In the following versions of Alecsis, we plan to introduce nonlinear eqn

statement, that uses the mechanisms developed for nonlinear generators ( nlgen

).

### 7.4.1. Simple eqn statement

An example of simple eqn statement is the following: eqn i: g*{i}-(2*v-8.)*{j}-4*{k}+5.-g*j=67.;

In this equation, contributions to the system matrix are defined. They are all in the row specified directly after keyword eqn , i.e. in the i -th row. The column where the contribution appears is given by the index in parentheses '{', '}', which multiplies the contribution. Expression g*{i} means that there is contribution g in the i -th column. So we have contribution

( -2*v+8.

) in the column j , and -4 in the column k . All indices representing row and column, must be declared as analogue links ( node , current , charge , or flow ), so that a row and a column in a matrix corresponds to each of them.

Contributions that do not multiply any index in parentheses, are contributions to the right-hand side of the system of equations. So, in our example we have contribution to the right hand side of the row i , which is ( 67-

5+g*j) . Note that j is here given without parentheses, which means that this is not a position in the matrix, but the number of type double , which represent the current value (last solution) of the analogue link j .

Note: The contributions to the columns must be before the symbol ' = ', while the contributions to the righthand side vector can appear both before and after the symbol ' = '.

If the above equation is the only one that contributes to the row i , then the equation appear as such in the system of equations. Nevertheless, other eqn statement in the same or some other module, or any other built-in or user-defined model, can contribute to the same row. All these contributions are added to the row i , following the concept of "stamps" common in electronic simulation.

We can form a stamp for any model using eqn statement. Here is an example of resistor: module new_resistor (node i, j) {

### 124

Alecsis 2.3 - User’s manual

action (double value=0.0) {

process structural {

if (!value) warning("zero valued resistor", 1);

}

virtual process initial {

double g = 1/value;

eqn i: g*{i}-g*{j}=0;

eqn j: -g*{i}+g*{j}=0;

}

}

}

The first eqn statement contributes to the row i , and defines the current flowing through the resistor branch from node i to node j . The same applies to the second eqn statement, but this defines current flowing from j to i .

Expression g*{i}-g*{j} is the current that is flowing out of node i . If eqn i would be the only one that contributes to matrix row i , we would have that this current is 0, which is senseless. But other components connected to the node i contribute to that eqn , and the complete equation is stating that the sum of all currents flowing out of node i is zero (Kirchhoff Current Law). For such case, when we are modelling currents or

voltages, it is much more readable, and less error-prone, to use through eqn statement or across eqn statement, described in the following sections. Simple eqn statement should be used only when we are not using Kirchhoff Laws or its equivalents described in Table 7.1., and that should be avoided if possible.

Equation eqn i: g*{i}-g{j}=0; can be also written as: eqn i: g*{i,j}=0; which makes equations shorter.

If i and j are links of type node , this can be also written as: eqn i: g*{i,j}.v=0;

Extension ' .v

' denotes voltage. In this case, Alec++ would check the type of i and j , and would exit and give an error message if they are not of type node . It can be also written as: eqn i: g*{i}.v-g{j}.v=0;

If i

and j

are declared as links of type flow

(rather than node

), you can use extension .a. So, the appropriate equation would be: eqn i: g*{i,j}.a=0; or: eqn i: g*{i}.a-g{j}.a=0;

Extension '.a' denotes nonelectrical variable of across type. Alecsis checks if i and j are declared as links of type flow.

7. Analogue simulation in Alecsis

### 125

Note: Alecsis differs between electrical across quantity -- voltage ( node ) and electrical through quantity -- current ; but with nonelectrical quantities, there is no such differentiation (in this version of Alecsis). All of them are of type flow , which can be used both as an across and as a through quantity.

As you can conclude from examples above, extensions ' .v

' and ' .a

' are optional, but are recommended, as they reinforce type checking. If extensions are not used, Alecsis checks only if both links in the pair {m,n} are links of the same type.

Note: Analogue links in eqn statement -- for instance, nodes i and j in statement: eqn i: g*{i,j}.v=0; must be scalars, as they are representing rows and columns in the system of equations. This applies for through and

across eqn statement, too.

### Analogue links in eqn statement can be scalars that are member of composite signals. Therefore, it is legal to define:

eqn w: 5*w-6*w=32;

w

w[]

### . However, it is not legal to write:

eqn w[m]: 5*w[m]-6*w[n]=32;

### This problem can be avoided with one additional hierarchical level in description. For instance, if you want to define:

process structural { for (m=1; m<=k; m++) for(n=1; n<=k; n++) eqn w[m]: 5*w[m]-6*w[n]=32;

}

### you have to define an additional module for equation:

module Equation (node w1, w2) { action initial () { eqn w[m]: 5*w[m]-6*w[n]=32;

}

}

clone

### Chapter:

module Equation Eqn;

... process structural { for (m=1; m<=k; m++) for(n=1; n<=k; n++)

}

eqn

### 7.4.2. Numerical integration in eqn statement (ddt, d2dt2, idt)

Up to now, we have explained how to describe linear algebraic equations, that directly contribute to the system of equations. However, many physical problems need differential equations to be modelled. Simple eqn ,

### 126

Alecsis 2.3 - User’s manual

across

eqn , and through eqn statements can be all modelled as differential equations. For example, c apacitor modell ed using equation:

i

=

C dv dt

(7.8) where i is the current through the capacitor, and v is the voltage accross its nodes, can be described as: module new_capacitor (node i, j) {

action (double value) {

process per_moment {

eqn i: value * ddt{i} - value * ddt{j} = 0;

eqn j: -value * ddt{i} + value * ddt{j} = 0;

}

}

}

Equation (7.1) is a typical through equation, so it is better to use through eqn statemen t. This will be explain ed in the next section.

Operator ddt

stands for time derivative. It performs numerical integration (discretization). The numerical integra tion method is chosen in the options block, which is explained in Chapter 5. The way of filling the matrix depends on t he method, but this is hidden from the user when operator ddt is used.

When operator ddt is used, cont ributions to the matrix is not constant - it depends on the time step, and on the syst em history (sol utions in the previous time instants). For that reason, in the above example, eqn command is used in the process synchronized per_moment .

Shorter written is allowed here, too: eqn i: value * ddt{i,j} = 0; as well as extension ' .v

' or ' .a' : eqn i: value * ddt{i,j }.v = 0;

The previous example of a capacitor can be mod ified, so that the current through the capacitor appears as unknown in the system of equations. The stamp is 'expanded' for one row and one column, and these carry the name of the current, which is here the sam e as the name of the component: module current new_icap (node i, j) { // returns current on name

action (double value) {

process per_moment {

eqn i: {new_icap} = 0;

eqn j: {new_icap} = 0;

eqn new_icap: value*ddt{i,j}.v -{new_icap} = 0;

}

}

}

node i

new_icap

node j

-new_icap

### Capacitor model given by eqn. (7.8) can be rewritten as:

7. Analogue simulation in Alecsis

v

=

1

C

idt

idt

### , which stands for integration with respect to time:

module newer_icap (node i, j) {

actio n (double value) {

pr ocess per_moment {

}

}

}

idt

ddt

### is normally used for all SPICE-like modelling and simulation problems.

For appli cation i n modelling of electronic components, operator ddt (time derivative) is enough, as there are only first or der differential equations. However, for modelling of mechanical systems, second time derivat ive is often necessary . One could avoid usage of second-order time derivative by introducing additional equation.

Nevertheless, for the sake of model readability and to reduce size of the system o f equations, we have introduced

second-order time derivative d2dt2

: process per_moment {

eqn x: m*d2dt2{x} + ro*ddt{x} + c*{x} - {F} = 0;

}

In this example of mechanical equilibrium m denotes the mass, ro is the friction resistance, and c is the spring constant.

Operators ddt , d2dt2 , and id t are connected to time-step control. Time-step control parameters are given i n Section 5.6.3.1. in Chapter 5.

Operators ddt , d2dt2 , and idt cannot appear in arithm etic expressions outside of comma nd eqn .

### 7.4.3. Through eqn statement

If we want to describe behaviour of a quantity that has through character (Table 7.1.), the simplest way to is to use through eqn statement. For example, resistor model from section 7.4.1. can be described as: module new_resistor (node i, j ) {

action (double value=0.0) {

process structural {

if (!value) warning("zero valued resistor", 1);

}

virtual process initial {

double g = 1/value;

### 128

Alecsis 2.3 - User’s manual

eqn {i,j}.i = g*{i,j}.v;

}

}

}

Ex tension ' .i

' on the left-hand side of the equation denotes the current. The equation above means that the current flowing between node i and node j equals g times the voltage between node i and node j .

Expres sion {i,j}.

i r einforces type checking, as i and j must be links of type node (current can flow only betwee n nodes.

The through eqn statement above is fully equivalent to two simple eqn statements used for resistor model in sect ion 7.4.1. This equation can be also written as: and to: eqn {i,j}.i = g*{i}.v-{j}.v; eqn {i,j}.i = g*{i,j}; which means that extensions on the right-hand side of the equation can be omitted. (They cannot be omitted on the left-hand side of through equation.) The above equation can be also given with two through eqn statements. eqn {i}.i = g*{i,j}.v; eqn {j}.i = g*{j,i}.v; where expression {i}.i

on the left-hand side denotes the current flowing out of node i .

Many electrical models can be naturally described by through equation. For instance, statement: eqn {i,j}.i = I; describes current source of value I . It is equivalent to two simple eqn statement: eqn i: 0 = I; eqn j: 0 = -I;

It is clear that the through equation is much more readable, whenever the model represents the current through the component as some function of controlling quantities.

An equivalent expressio n for nonelectrical quantities would be: eqn {m,n}.t = g*{m,n}.a; where extension ' .t

' denotes through quantity. The ab ove equations means: through quantity flowing from flow m to flow n equals g times the difference of across quantities m and n . Extension ' .t

' reinforces type checking, so m a nd n have to be links of type flow (of across nature -- howe ver, Alecsis does not differentiate between across flows and through flows).

All variations of through equation, which are given above for currents and voltages, are valid for flows, too.

On the right-hand side, both nonelectrical and electrical variables can appear: eqn {m,n}.t = g1* {m,n}.a + g2{i,j}.v;

This equations states that the through quantity flowing between flow m and flow n is the function of across quantity between flow m and flow n , and of voltage between node i and node j .

7. Analogue simulation in Alecsis

### 129

Note: Extension on the left-hand side of the through eqn statement (' .i

' or ' .t

') cannot be omitted.

Only nodes or flows can appear on the left-hand side (it does not make sense to define the current flowing between quantit ies of type current ). On the right-hand side, extensions (' .v

' and ' .a

') can be omitted, but are recommended to reinforce type checking.

.i

' or ' .t

' can appear only on the left-hand side of through eqn statement. It does not make sense to put expression {i,j}.i

on the right-hand side of the equation, since current flowing between nodes i and j is not available as the solution of the system of equations. If link k is of type current (for instance, current through the voltage source named k ), it can appear on the right-hand side of the equation, but without any extension (extension ' .i

' would be confusing, since {k}.i

denotes current flowing out of node k ). For the reason s explained in this Note, extensions ' .i

' and ' .t

' cannot be used in simple eqn statement at all).

Through eqn statement can describe differential equation, since operators

ddt

,

d2dt2

and

idt

can be used, too. Here is an example of capacitor model: module new_capacitor (node i, j) {

action (double value) {

process per_moment {

eqn {i,j}.i = v alue * ddt{i,j}.v;

}

}

}

The model given above is fully equivalent to the first example from section 7.4.2. You can note that through eqn sta tement given in th is model clearly describe model given by eqn. (7.8).

### 7.4.4. Across eqn statement

As we are using nodal approach for solving the system of equations, we describe most of the models as throug h equations (current as function of voltages). H owever some of the models cannot be described in this way.

For in stance, all kinds of ideal voltage generators ( independent and controlled) have to be described as voltage dependence on other quantities. For that reason, we need modified nodal approach, where current through the branch is added as an additional unknown in the system of equation, and branch voltage equation is added as additio nal equation. This can be easily described using across eqn equation.

An ideal voltage source can be described in this way: module current new_vgen (i, j) {

action (double value) {

virtual process initial {

eqn new_vgen, {i,j}.v = v alue;

}

}

}

Expression {i,j}.v = value gives the dependence of vol tage between node i and node j (in this ca se, this is a co nstant voltage). In through equation, current through t he branch has also to be specified, since this is the row i n the system matrix where this equation is added. The name of the current is given after keyword eqn , before the equation itself is given. In our example, the name of he current is new_vgen , and this is also the name of the module , declared as the current (this returning the current

on the

module name will be declare d later in this Chapter). It is important that this variable, representing the current through the branch, is declared as current before the functional description ( action block).

Across eqn statement

### 130

Alecsis 2.3 - User’s manual

eqn new_vgen, {i,j}.v = value; from the example above has the same contribution to the system of equations as three simple eqn statements: eqn i: 1*{new_vgen} = 0; eqn j: -1*{ new_vgen} = 0; eqn new_vgen: 1*{i} -1*{j} = value;

These two descriptions define the same model stamp.

Across equation: eqn k, {i}.v = r*{k}; has the same effect as: eqn k, {i,0}.v = r*{k}; since 0 is always representing ground node.

Across equation can be described for nonelectrical quantities (flows), too. An example is: eqn k, {m,n}.a = r*k;

The quantity that represents difference of flow m and flow n equals r times quantity k . Links m and n have to be of type flow , and of across nature, according to Table 7.1. (However, there is no d ifference between across and through flows on declaration in this version of Alecsis). Link k has to be of type flow (of through nature) .

Note: Extension on the left-hand side of the across eqn statement (' .v

' or ' .a

') cannot be omitted.

Only nodes or flows can appear on the left-hand side. On the right-hand side, extensions (' .v

' and ' .a

') can be omitted, but are recommended to reinforce type checking.

.i

' or ' .t

' cannot appear on the right-h and side of across eqn statement. If link k is of type current (for instance, current through the voltage source named k ), it can appear on the right-hand side of the equation, but without any extension.

Across eqn statement can be differential, i.e. operators

ddt

,

d2dt2

and

idt

can be used. We have already defined model of a capacitor, with the current through the capacitor is added as unknown to the system of equations, in section 7.4.2. ( module newer_icap ). This can be easily described using across eqn statement: module newer_icap (node i, j) {

action (double value) {

process per_moment {

}

}

}

This ac ross eqn statement clearly describes model given by eqn. (7.9).

For the c apacitor model, we do not need current through the capacitor as new unknown in the system of equatio n, so it is more natural to use through equation. However, to model inductance, we need that current, since voltage is dependent on the current:

v

=

L di dt

(7.10)

7. Analogue simulation in Alecsis

The inductor model using across eqn statement is: module current new_l (i,j) {

action (double value) {

process per_moment {

eqn new_l, {i,j}.v = value*ddt{new_l};

}

}

}

### 7.5. Appointed simulation in a time-instant -- b reakpoint

Alecsis works with variable time-step. Time step is changed to meet demands on numerical integration error.

For that reason, we cannot know in advance which time-instants would be chosen for simulation. However, in some particular cases, we want to force Alecsis to perform simulation in some particular time-instants. Function

set_bpoint

is used for that. It sets a breakpoint for a given time-instant (i.e. appoints simulation for that timeinstant ).

For instance: set_bpoint(now+Period); appoints simulation for time instant that happens Period after current time (keyword

now

returns current simulation time). Simulation proceeds with normal time-step control until it approaches the breakpoint, and then the time step would be shortened to meet the breakpoint. That means, it will not be allowed to jump over the breakpoi nt.

Function set_bpoint() can be used inside a process of action block.

An application example can be found in definition of module pulse (in file alec.hi

in subdirectory sys that is normally installed with Alecsis.). This is definition of voltage generator of trapezoidal waveform. If time-step is large, corners of trapezoidal waveform can be missed. The simulation results are still correct, but the waveforms that are plotted out are not always nice -- corners of trapezoidal waveform can be cut out. Function set_bpoi nt is used here to force simulation in corners of trapezoidal waveform.

Note: As simulation time is variable of type double in floating-point a rithmetic, the appointed breakp oints cannot be met exactly, due to some rounding errors.

### 7.6. Returning the link using name of a module

We have already mentioned that some built-in elements have to be modelled using branch voltage equations.

For these elements, current through the branch has to appear as new unknown in the system of equations. That current can be plotted out, or used as controlling current for other models, using the name of the built-in component.

This is the same as in SPICE.

Our concept was that user defined modules can be used equally as built-in c omponent models. For that reason, AleC++ allows that the module name return the current (similarly as functions return variables - but here, it is not t he value of the current that is returned, but the actual position in the matrix).

We have already given such examples in the previous section, for instance, ideal voltage source model:

### 132

Alecsis 2.3 - User’s manual

module current new_vgen (i,j) { // new_vgen is name of the current

action (double value) {

virtual process initial {

eqn new_vgen, {i,j}.v = value;

}

}

}

Here, current new_vgen is not declared separately, but when the module name is defined, as: module current new_vgen used to declare component s of type module new_vgen , each component of that type returns the current on its name:

Current new_vgen can be used inside that module like any othe r current. However, when this module is module Y (node i,j,p,q) {

module new_vgen X; // THIS DECLARES X AS CURRENT

ccvs Z; // a current-controlled voltage source

X(i,j) action( 5);

Z(p,q,X) mi=1; // current X is used for controlling

}

If we model the above voltage generator in the following way: module newer_vgen (i,j) {

current k; // separate declaration for current

action (double value) {

virtual process i nitial {

eqn k, {i,j}.v = value;

}

}

} then no associ ation between name of the module and name of the current is established. Voltage source model is correct, but it does not return any current under its name, and cannot be used in our module Y .

This explains how to return current using the name o f the module when the current is declared locally, inside the giv en module. But what to do when this current is pas sed by another module? For instance, when current returne d by our mo dule new_vgen has to be returned by our module Y , too. An association can be established in such case: module current Y (node i,j,p,q){ // Y is also an current,

module new_vgen Y; // and it is returned by new_vgen

ccvs Z;

return Y(i,j) action( 5); // keyword 'return' is necessary

Z(p,q,Y) mi=1;

}

In this example, m odule Y also returns current under its name. It is the current returned by module new_ vgen , and for that reason, component of type new_vgen also carries the name Y . When the com ponent Y is con nected, keyword return has to be used before the name Y , to point out the association of the names.

(Witho ut keyword retur n , Alecsis would consider this as name redeclaration, which is an error.)

This works in the same manner if we use built-in component (e.g. vgen ), instead of user defined module new_ vgen .

The compiler will not allow association of more than one component with the name of a module.

7. Analogue simulation in Alecsis

### 133

If you consider this too complex, you can return the current using list of formal parameters: module Y (node i,j,p,q; current X){ // formal param. X is current

module new_vgen X; // and it is returned by new_vgen

ccvs Z;

X(i,j) action( 5);

Z( p,q,Y) mi=1;

}

Here, module Y does not return any current on its name, but it returns current usi ng list of formal parame ters. As we have already explained, formal parameters of a module can be used f or bi-directional communi cation, unlike parameters of C-like function. They are passed by reference, not by value, as they are represe nting position in the system of equations. Keyword

return is here not used for association.

More than one com ponent cannot associate with the same formal parameter, because that would be a name redefin ition in the same structural visibili ty area (every component has its own current -- for example, every inducto r has a current flowing through it.)

It is not legal to associate with a formal parameter that is not a scalar

.

Note: Links of type charge and flow can be returned using name of the module , too. All what is here explained for links of type current , is also valid for charge and flow . However, this feature is introduced for links of type current , to make Alecsis compatible with SPICE.

### 7.7. Variable number of action parameters

The nu mb er of parameters in the header of the action block of the module can be variable. This is described in the Chapter 5, as it is the same for digital and analogue modules.

### 7.8. Modules with variable structure -- clone and allocate

Some complex models cannot be easily described using standard Alecsis syntax. Sometimes we want that model card parameters or action parameters determine not only the behaviour, but also the structure of the model. There are two cases when this can be necessary:

• When some subcomponents appear in the module structure conditionally, depending on the model card parameters of action parameters. This can be, for instance, the case with resistances connected in series on com po nent terminals, that are usually optional; or with whole optional subcircuits, e.g. som e compensation subcircuits for opamps, etc.

• To define regular subcomponent arrays of variable size. Some electronic circuits exhibit clear regularity.

Therefore, one can describe an array of variable size, where the size is an user-defined parameter.

Command

clone

is used to describe such mode ls. It defines cloning of the previously described or built-in component. Cloning can be executed only in processes synchronized as structural

, since execution of com mand clone

defines the structure of the circuit. As this command is used inside a process

( stru ctural

), it can be executed conditionally, or in a loop, depending on the user-defined parameters.

Note: Models defined using command clone

cannot be classified as either structural or combined

(structural-functional), since here execution of process structural

determines structure of the model.

### 134

Alecsis 2.3 - User’s manual

The syntax of command clone follows all rules for component coupling:

clone_command:

### clone body_of_command_clone

body_of_command_clone: component ;

{ component_list } component_list: component ; compone nt_list component ;

Whe n we use command clone to create arrays of variable size, it is clear that the number of links (e.g. size. T hat dynamical allocation of link arr ays is enabled using command

allocate

.

We can se e application of both cl one and allocate on the following example of ring oscillator: module invert er(node vout, vin, vdd, vss) { mosf et mup, mdo wn;

mup (vout, vin, vdd, vd d) { model=Mpmos; l=3u; w=8u; }

mdown (vout, vin, vss, vss) { model=Mnmos; l=w=3u; }

} module ring_oscillator (vout, vdd, vss) {

inverter inv;

node joint[auto]; // array of nodes (size not defined)

action (int size = 3) {

process structura l {

allocate joint [size-1]; // dynamical allocation

int i;

if (size < 3 || size % 2 == 0)

warning("wrong number of inverters in ring", 1);

for (i=0; i<size; i++) {

if (i==0)

clo ne inv (joint, vout, vdd, vss);

else if (i==size-1)

clone inv[i] (vout, joint[i-1], vdd, vss);

else

clone inv[i] (joint[i], joint[i-1], vdd, vss);

}

}

}

}

In this example, an MOS inverter i s defined structurally, and that module inverter is used as compo nent to be cloned into an array. In module ring_oscillator we have compone nt inv of type inve rter declared. We also have declaration of an array of nodes with the name joint . Command: node joint[auto]; is declaration of one-dimensional array of nodes. Length of that array is not yet defined, it will be done using comma nd allocat e .

7. Analogue simulation in Alecsis

### 135

We can note that module ring_ocillator has no structural part, i.e. declared component inv of type inverter is not connected in the structural part.

Inside the functional part ( action block) a process structural is defined. In that process, array of nodes joint is allocated as: allocate joint [size-1];

Array joint has length size-1 , and zero-offset is used (from 0 to size -2). Parameter size is passed as an action parameter (default value is 3 ).

Note: Array of links can be have more dimensions, can have lower limit defined, etc. (all rules for Alecsis link ar ray apply). Example: allocate joint[1:size]; // array with offset 1;

node a[auto][j];

### but you cannot declare:

node a[auto][auto];

### If you need to dynamically allocate array of links with more than one dimension, you can either reorganize it as one-dimensional array (which is always possible); or you can use array with static allocation, and recompile the model when you change dimensions:

# define FIRST_DIM 150

# define SECOND_DIM 200

... a[FIRST_DIM][SECOND_DIM];

In our examp le of ring oscillator, parameter size is checked firstly (it cannot be an even number, if we fter that, a for loop is defined, where size instances of component inv are cloned. A i-th instance of compone nt inv is connected between nodes joint[i] and joint[i-1] using command: clone int [i] (joint[i], joint[i-1], vdd, vss);

In dex [i] a fter co mponent name int can be omitted. H owever, it is useful, as it enables us to approach the par ticular component int[i] later -- in c ommand plot , for instance.

T his ring of inverters is a regular structure, but it has exceptions at the beginning, and at the end of the array

(connections to output node vout ). This is handled using if / else commands.

From this example one can conclude that both the component to be cloned, and the array of links of variable size, have to be declared in the declarative part of the module . The actual size of the link array, and cloning of components, are in the action block, process structural .

### 136

Alecsis 2.3 - User’s manual

Note: Action parameters of cloned components can be different. However, if the component that is cloned has a model card, parameter model must be known in the compilation time (the model card name cannot be passed as a variable).

In command: clone int[i] (joint[i], joint[i-1], vdd, vss); index [i] after component name int can be omitted. However, it is useful, as it enables us to approach the particular component int[i] later -- in command plot , for instance. Index becomes a part of the component name, and in c om mand plot , it must be used inside quotation marks, without any blanks inside the quotations: plot { nod e s1/s2/"comp"/n1; current "lserial"; }

In the above c ommands, we use cloned component name to define absolute path (to local link node n1 in the component "comp" ); or to get the values of current returned under module name

( "lse rial" ).

Note: Commands clone and allocate apply to analogue, digital, and hybrid circuits in the same way, since nowhere in the syntax does the command demand a particular link type or component type. It is especially useful in digital simulation, for instance to describe registers of different lengths.