Ocs package

OCS : Octave Circuit Simulator

Problem Formulation

The circuit description in OCS is based on (a variant of) modified nodal analysis (MNA) model for lumped-element networks. It is easy to verify that the common charge/flux-based MNA model is a special case of the model presented below.

We consider a circuit with M elements and N nodes, the core of the MNA model is a set of N equations of the form $\sum _{{m}=1}^{M}F_{mn}=0\qquad n=1,\,\ldots \,,N$

where $F_{mn}$ denotes the current from the node n due to element m.

The equations above are the Kirchhoff current law (KCL) for each of the electrical nodes of the network.

The currents can be expressed in terms of the node voltages $e$ and the internal variables $r_{m}\;(m=1\ldots M)$

$F_{mn}=A_{mn}{\dot {r}}_{m}+J_{mn}\left({e},{r}_{m}\right)\qquad {\begin{array}{l}n=1,\,\ldots \,,N\\m=1,\,\ldots \,,M\end{array}}$

Notice that the variables ${r}_{m}$ only appear in the equations defining the fluxes relative to the m-th element, for this reason they are sometimes referred to as internal variables of the m-th element.

The full MNA model is finally obtained by substituting the current definitions in the KCL and complementing it with a suitable number $I_{m}$ of constitutive relations for the internal variables of each element Failed to parse (SVG with PNG fallback (MathML can be enabled via browser plugin): Invalid response ("Math extension cannot connect to Restbase.") from server "https://wikimedia.org/api/rest_v1/":): {\displaystyle \sum_{{m}=1}^{M} \left[ \ A_{mn} \dot{{r}}_{m} + J_{mn} \left( {e}, {r}_{m} \right) \right] = 0 \qquad {n} = 1, \, \ldots \, ,N \\ B_{mi} \dot{{r}}_{m} + Q_{mi}\ \left( {e}, \{r}_{m} \right) = 0. \qquad \begin{array}{l} {i} = 1, \, \ldots \, ,{I}_m \\ {m} = 1, \, \ldots \, ,M \end{array} } Notice that the assumption that only time derivatives of internal variables appear above and that terms involving such derivatives are linear does not impose restrictions on the applicability of the model.

Data Structure

A circuit is represented in OCS by a struct variable with the fields listed below

Code: CIR file format

cir_struct = { LCR: struct  % the fields of LCR are shown below NLC: struct  % NLC has the same fields as LCR namesn: matrix  % numbers of vars that are assigned a name in and.nms namess: cell  % the names corresponding to the vars above totextvar: scalar % the total number of external variables totintvar: scalar % the total number of internal variables } outstruct.LCR = { 1x2 struct array containing the fields: % array has one element per block func  % name of the sbn file corresponding to each block section  % string parameter to be passed to the sbn files nextvar  % number of external variables for each element of the block vnmatrix % numbers of the external variables of each element nintvar  % number of internal variables for each element of the block osintvar % number of the first internal variable npar  % number of parameters nparnames% number of parameter names nrows  % number of rows in the block parnames % list of parameter names pvmatrix % list of parameter values for each element }

File Formats

There are several ways of setting up the data structure for an OCS simulation. The first approach is to just assign the fields of the data structure via Octave commands, otherwise one can parse an ascii file written in (a subste of) SPICE netlist language or in OCS's own netlist specification language called IFF (Interchange File Format)

IFF netlists

The name IFF stands for "Intermediate File Format" or "Interchange File Format" it represents an ASCII file format for describing coupled electrical circuits, devices and systems. The IFF syntx described here is version 0.1b1.

A circuit description is comprised of a set of files of three different types:

• 1 CIR (Circuit) file: an ASCII text file with filename <circuitname>.cir
• 1 NMS (Names) file: an ASCII text file with filename <circuitname>.nms
• N >= 1 SBN (Subnet) files: a set of M-functions or DLD-functions following the template described below.

SBN files are not necessarily specific to one circuit and can be grouped in libraries as long as the directory containing the library is added to the path when the IFF parser is run.

CIR file

The CIR file is divided into two sections describing the linear time–independent (LCR = linear circuit) and the non–linear and/or time–dependent (NLC = non–linear circuit) partitions of the circuit respectively. The syntax for the LCR and NLC section is identical. NLC can also contain linear elements, in fact the whole circuit could be described only by the NLC section but this could result in the evaluator unnecessarily recomputing local matrices for linear time–independent elements The content of CIR files is organized as follows:

Code: CIR file format

cir  := header nlc separator lcr separator ; header := '%' version_id '$\nl$' comment* ; comment:= '%' text '$\nl$' ; nlc  := block* ; block  := blockcomment? blockheader pv_matrix vnum_matrix  ; block_comment := '%' text '$\nl$' ; block_header  := func section n_extvar n_par '$\nl$' n_rows n_parnames '$\nl$' par_name*; section  := string ; n_extvar  := number ; n_par  := number ; n_rows  := number ; n_parnames  := number ; par_name  := string ; pv_matrix  := matrix ; vnum_matrix  := matrix ; matrix  := number+ ; separator := 'END $\nl$' ; lcr  := block* ;

where

• "version_id" is a string identifying the version on IFF in which the file is encoded
• "\n" is the new-line character string that represents anything that the Octave command "s=fscanf(file,%s)" would parse as a string i.e. any sequence of chars without white-space
• "text" is any sequence of chars without a \n, this differs from string because it can contain white–space number represents anything that the Octave command "s=fscanf(file,%g)" would parse as a number
• "func" is the name of a function to evaluate the elements described in the block
• "n_extvar" Is the number of external variables for the elements of a block
• "n_par" Is the number of parameters for the elements of a block
• "n_rows" Is the number of elements in a block
• n_parnames" Is the number of parameter names for the elements of a block, it corresponds to the number of par name entries. If "n_parnames" is 0 the line with the "par_names" is missing.
• "pv_matrix" Is a list of n_rows x n_par numbers separated by any character the Octave command "s=fscanf(file,%g)" would consider whitespace (including "\n"). Every row (a set of n par contiguous entries) in "pv_matrix" refers to an element of the circuit. The "n_par" numbers in a row represent the values of the parameters to be passed to the function that evaluates that element.
• "vnum_matrix" Is a list of "n_rows" x "n_extvar" numbers separated by any character the Octave command "s=fscanf(file,%g)" would consider white-space (including \n). Every row (a set of "n_extvar" contiguous entries) in "vnum_matrix" refers to an element of the circuit. The "n_extvar" numbers in the row represent the global numbering of the element external variables.

NMS files

NMS files are meant to contain the names of the circuit variables, the format of NMS is just a list of variable names one on each row preceded by the variable number:

Code: CIR file format

nms := version id ’\n’ comment∗ line∗ ; line := var number var name ; var number := number ; var name := string ;

the variable are ordered as follows:

• first all external variables of all elements in the order given by the global numbering of external variables as explicitly written in the CIR files
• then the internal variables of the elements in the same order as the corresponding elements appear in the CIR file ( internal variables of non-linear elements first, then those of linear elements)

Notice that the number of internal variables of each element is not included in the IFF files. This is because elements with a number of internal variables that is huge, that depends on the value of some parameter, or even that changes in time (for example distributed elements treated with a FEM with adaptive meshing, a large linear sub- circuit that is reduce via MOR...) and therefore it is more convenient to compute the number of internal variables when initializing the system.

SBN files

SBN files are Octave functions, implemented as M-scripts or as DLD functions, with the following signature

Code: Model evaluator file for simple MOSFET models

function [a, b, c] =... func (string , m(i ,:) , extvar , intvar , t)

i.e. it should get as inputs:

• the string entry of the "block_header"
• one row of the "pv_matrix" entry of the "block"
• the current values of all internal and external variables
• the current time

and it should produce as outputs three matrices:

• $a,b\in \mathbb {R} ^{({n_{extvar}}+{n_{intvar}})\times ({n_{extvar}}+{n_{intvar})}}$
• $c\in \mathbb {R} ^{({n_{extvar}}+{n_{intvar}})}$

where "n_intvar" is the number of internal variables that can be assembled in the complete system matrices.

SPICE netlists

SPICE .spc netlists are parsed via the function "prs_spice", which currently supports the set of "Element Cards" shown below with their instantiating syntax.

Code: Model evaluator file for simple MOSFET models

- Capacitors: Cname n+ n- cvalue - Diodes: Cname anode knode modelname <parameters> - MOS: Mname gnode dnode snode bnode modelname <parameters> N.B.: one instance of a MOS element MUST be preceeded (everywhere in the file) by the declaration of the related model. For instance: .MODEL mynmos NMOS( k=1e-4 Vth=0.1 rd=1e6) M2 Vgate 0 Vdrain 0 mynmos - Resistors: Rname n+ n- rvalue - Voltage sources: Vname n+ n- <dcvalue> <transvalue> Transvalue specifies a transient voltage source SIN(VO VA FREQ TD THETA) where: * VO (offset) * VA (amplitude) * FREQ (frequency) * TD (delay) * THETA (damping factor) * 0 to TD: V0 * TD to TSTOP: VO + VA*exp(-(time-TD)*THETA)*sine(twopi*FREQ*(time+TD)) Currently the damping factor has no effect. Pulse PULSE(V1 V2 TD TR TF PW PER) parameters meaning * V1 (initial value) * V2 (pulsed value) * TD (delay time) * TR (rise time) * TF (fall time) * PW (pulse width) * PER (period) Currently rise and fall time are not implemented yet. - .MODEL cards Defines a model for semiconductor devices .MODEL MNAME TYPE(PNAME1=PVAL1 PNAME2=PVAL2 ... ) TYPE can be: * NMOS N-channel MOSFET model * PMOS P-channel MOSFET model * D diode model The parameter "LEVEL" is currently assigned to the field "section" in the call of the element functions by the solver. Currently supported values for the parameter LEVEL for NMOS and PMOS are: * simple * lincap (see documentation of function Mdiode). Currently supported values for the parameter LEVEL for D are: * simple (see documentation of functions Mnmosfet and Mpmosfet).

Tutorials

A CMOS AND GATE

Schematic for a CMOS AND gate

Here we show how to set up the simulation of the CMOS AND gate in the figure. The circuit has

• 9 Elements
  • 6 MOSFETs (3 n-type + 3 p-type)
  • 3 Voltage sources

For the n-type MOSFETs we use a very simple algebraic model defined by the following code

Code: Model evaluator file for simple MOSFET models

function [a,b,c] = Mnmosfet (string, parameters, parameternames, extvar, intvar, t) switch string case 'simple', rd = 1e6; for ii=1:length(parameternames) eval([parameternames{ii} "=",... num2str(parameters(ii)) " ;"]) endfor vg = extvar(1); vs = extvar(2); vd = extvar(3); vb = extvar(4); vgs = vg-vs; vds = vd-vs; if (vgs < Vth) gm = 0; gd = 1/rd; id = vds*gd; elseif ((vgs-Vth)>=(vds))&(vds>=0) id = k*((vgs-Vth)*vds-(vds^2)/2)+vds/rd; gm = k*vds; gd = k*(vgs-Vth-vds)+1/rd; elseif ((vgs-Vth)>=(vds))&(vds<0) gm = 0; gd = 1/rd; id = vds*gd; else # (i.e. if 0 <= vgs-vth <= vds) id = k*(vgs-Vth)^2/2+vds/rd; gm = k*(vgs-Vth); gd = 1/rd; endif a = zeros(4); b = [ 0 0 0 0; -gm (gm+gd) -gd 0; gm -(gm+gd) gd 0; 0 0 0 0]; c = [0 -id id 0]'; break; otherwise error(["Mnmosfet: unknown option " string]); endswitch endfunction

The model for the p-type devices is entirely analogous.

Below we show three methods for constructing the circuit data structure

• using an Octave script
• parsing a SPICE netlist
• parsing an IFF netlist

Once the circuit data structure is loaded the simulation can be started by the following commands

Code: Run the AND gate simulation

x = [.5 .5 .33 .66 .5 1 0 0 1 ]'; t = linspace (0, .5, 100); pltvars = {"Va", "Vb", "Va_and_b"}; dmp = .2; tol = 1e-15; maxit = 100; out = tst_backward_euler (outstruct, x, t, tol, maxit, pltvars);

Result of the CMOS AND gate switching simulation

Click on the figure to the right to see the simulation results

Build the AND GATE structure directly

Code: Build the AND GATE structure via an Octave script

## NLC # n-type outstruct.NLC(1).func = "Mnmosfet"; outstruct.NLC(1).section = "simple"; outstruct.NLC(1).nextvar = 4; outstruct.NLC(1).npar = 3; outstruct.NLC(1).nparnames = 3; outstruct.NLC(1).parnames = { "k", "Vth", "rd"}; outstruct.NLC(1).pvmatrix = [1.0000e-04 1.0000e-01 1.0000e+07 1.0000e-04 1.0000e-01 1.0000e+07 1.0000e-04 1.0000e-01 1.0000e+07]; outstruct.NLC(1).vnmatrix = [1 3 4 0 2 0 3 0 4 0 5 0]; outstruct.NLC(1).nintvar = [0 0 0]; outstruct.NLC(1).osintvar = [0 0 0]; # p-type outstruct.NLC(2).func = "Mpmosfet"; outstruct.NLC(2).section = "simple"; outstruct.NLC(2).nextvar = 4; outstruct.NLC(2).npar = 3; outstruct.NLC(2).nparnames = 3; outstruct.NLC(2).parnames = { "k", "Vth", "rd"}; outstruct.NLC(2).pvmatrix = [-1.0000e-04 -1.0000e-01 1.0000e+07 -1.0000e-04 -1.0000e-01 1.0000e+07 -1.0000e-04 -1.0000e-01 1.0000e+07]; outstruct.NLC(2).vnmatrix = [ 1 6 4 6 2 6 4 6 4 6 5 6]; outstruct.NLC(2).nintvar = [0 0 0]; outstruct.NLC(2).osintvar = [0 0 0]; # Va and Vb outstruct.NLC(3).func = "Mvoltagesources"; outstruct.NLC(3).section = "sinwave"; outstruct.NLC(3).nextvar = 2; outstruct.NLC(3).npar = 4; outstruct.NLC(3).nparnames = 4; outstruct.NLC(3).parnames = {"Ampl", "f", "delay", "shift"}; outstruct.NLC(3).pvmatrix = [0.50000 1.00000 0.00000 0.50000 0.50000 2.00000 0.25000 0.50000]; outstruct.NLC(3).vnmatrix = [ 1 0 2 0]; outstruct.NLC(3).nintvar = [1 1]; outstruct.NLC(3).osintvar = [0 0]; ## LCR # Vdd outstruct.LCR(1).func = "Mvoltagesources"; outstruct.LCR(1).section = "DC"; outstruct.LCR(1).nextvar = 2; outstruct.LCR(1).npar = 1; outstruct.LCR(1).nparnames = 1; outstruct.LCR(1).parnames = {"V"}; outstruct.LCR(1).pvmatrix = 1; outstruct.LCR(1).vnmatrix = [6 0]; outstruct.LCR(1).nintvar = 1; outstruct.LCR(1).osintvar = 2; ## outstruct.namesn = [1 2 5 6 7 8 9]; outstruct.namess = {"Va", "Vb", "Va_and_b", "Vdd", "I1", "I2", "I3"}; outstruct.totextvar = 6; outstruct.totintvar = 3;

Build the AND gate circuit structure parsing an IFF netlist

To parse an IFF format netlist of the CMOS AND gate we can use the following command

Code: Load the AND circuit structure parsing an IFF netlist

outstruct = prs_iff ("and");

The IFF netlist consists of the .cir file named "and.cir" shown below

Code: IFF netlist for the AND gate (.cir file)

% 0.1b1 % A Simple CMOS AND GATE % % N-Mosfets % There are 3 N-Mosfets Mnmosfet simple 4 3 3 3 k Vth rd 1e-4 0.1 1e7 1e-4 0.1 1e7 1e-4 0.1 1e7 1 3 4 0 2 0 3 0 4 0 5 0 % % P-Mosfets Mpmosfet simple 4 3 3 3 k Vth rd -1e-4 -0.1 1e7 -1e-4 -0.1 1e7 -1e-4 -0.1 1e7 1 6 4 6 2 6 4 6 4 6 5 6 % % Input voltage sources Mvoltagesources sinwave 2 4 2 4 Ampl f delay shift 0.5 1 0.0 0.5 0.5 2 0.25 0.5 1 0 2 0 END % % Power supply Mvoltagesources DC 2 1 1 1 V 1 6 0 END

and of the .nms file named "and.nms shown below

Code: IFF netlist for the AND gate (.nms file)

% 0.1b1 1 Va 2 Vb 5 Va_and_b 6 Vdd 7 I1 8 I2 9 I3

Build the AND gate circuit structure parsing a .spc file

Code: Load the AND circuit structure parsing a .spc file

outstruct = prs_spice ("and");

Code: The .spc file for the CMOS AND gate

* AND (simple Algebraic MOS-FET model) .MODEL mynmos NMOS(LEVEL=simple k=2.94e-05 Vth=0.08 rd=.957e7) .MODEL mypmos PMOS( k=-2.94e-05 Vth=-0.08 rd=.957e7) M1 Va 3 4 0 mynmos M2 Vb 0 3 0 mynmos * nside of the inverter M3 4 0 Va_and_b 0 mynmos M4 Va Vdd 4 Vdd mypmos M5 Vb Vdd 4 Vdd mypmos * pside of the inverter M6 4 Vdd Va_and_b Vdd mypmos V1 Va 0 SIN(0.5 0.5 1 0 0) V2 Vb 0 SIN(0.5 0.5 2 0.25 0) V3 Vdd 0 1 .END

Creating a model for a memristor device

To demonstrate how to write a model evaluator file (SBN file), we will discuss the simplest memristor model shown in this paper by KaKiLa et al. (KaKiLa, can you please add a reference to the paper?)

The device model is presented in the original paper as

$\left\{{\begin{array}{l}{\dot {x}}=\mu I(t)\\H(x)=\left\{{\begin{array}{l}R\qquad x\leq 0\\R-(R-r)x\qquad 0<x<1\\r\qquad x>1\end{array}}\right.\\V(t)=H(x)I(t)\end{array}}\right.$

The first thing to do is to change the model from impedance to admittance form and write the constitutive relation for the internal variable in an "implicit form"

$\left\{{\begin{array}{l}{\dfrac {1}{\mu }}{\dot {x}}+Q(V(t),x(t))={\dfrac {1}{\mu }}{\dot {x}}-I(t)=0\\H(x)=\left\{{\begin{array}{l}R\qquad x\leq 0\\R-(R-r)x\qquad 0<x<1\\r\qquad x>1\end{array}}\right.\\I(t)={\dfrac {V(t)}{H(x)}}\end{array}}\right.$

It is then useful to compute the derivatives for the current and for the constitutive relation

${\dfrac {\partial I}{\partial x}}=-{\dfrac {H'(x)}{H(x)^{2}}}$

${\dfrac {\partial I}{\partial V}}={\dfrac {1}{H}}$

$H'(x)=\left\{{\begin{array}{l}0\qquad x\leq 0\\-(R-r)\qquad 0<x<1\\0\qquad x>1\end{array}}\right.$

Next we define external variables (pin voltages) for the device and coupling variables (pin currents)

 N.B. the convention in existing device models is that pin currents are 
      assumed to be entering the device

${\begin{array}{l}i^{+}=I(t)\\i^{-}=-I(t)\\V(t)=v^{+}-v^{-}\end{array}}$

Now define the local state vector

$z=\left[{\begin{array}{l}v^{+}\\v^{-}\\x\end{array}}\right]$

and the local equations

$a{\dot {z}}+c(z)=0$

and finally define the local matrices for the memristor element

$a=\left[{\begin{array}{c c c}0&0&0\\0&0&0\\0&0&{\dfrac {1}{\mu }}\end{array}}\right]$

$c(z)=\left[{\begin{array}{c}{\dfrac {V}{H}}\\[2mm]-{\dfrac {V}{H}}\end{array}}\right]$

$b(z)={\dfrac {\partial c}{\partial z}}=\left[{\begin{array}{c c c}{\dfrac {\partial I}{\partial V}}&-{\dfrac {\partial I}{\partial V}}&{\dfrac {\partial I}{\partial x}}\\[2mm]-{\dfrac {\partial I}{\partial V}}&+{\dfrac {\partial I}{\partial V}}&-{\dfrac {\partial I}{\partial x}}\\[2mm]-{\dfrac {\partial I}{\partial V}}&+{\dfrac {\partial I}{\partial V}}&-{\dfrac {\partial I}{\partial x}}\\[2mm]\end{array}}\right]$

The resulting model implementation is the following

Code: memristor model implementation

function [a,b,c] = Mmemristors (string, parameters, parameternames, extvar, intvar, t) if isempty(intvar) intvar = 0; endif switch string case "STRUKOV" ## NLC part for ii=1:length(parameternames) eval([parameternames{ii} "=" num2str(parameters(ii)) ";"]) endfor v1 = extvar(1); v2 = extvar(2); x = intvar(1); if (x <= 0) H = RH; Hp = 0; elseif (x > 0 && x < 1) H = RH - (RH - RL) * x; Hp = - (RH - RL); else H = RL; Hp = 0; endif I = (v1-v2) / H; i1 = I; i2 = -I; dIdx = - Hp / H^2; dIdV = 1 / H; a = zeros (3); a(3, 3) = 1/ MU; b = [dIdV -dIdV dIdx; -dIdV dIdV -dIdx; -dIdV dIdV -dIdx]; c = [i1 i2 i2]'; break; otherwise error (["unknown section:" string]) endswitch endfunction

As an example let's run a simulation by applying a sinusoidal signal with varying frequency

Code: memristor model implementation

t = linspace (0, 1, 100); y = [(sin (2 * pi * t * 1.5)), (sin (2 * pi * t * 4))(2:end)]; t = [t, (linspace (1, 2, 100))(2:end)]; pwl = [t; y](:).'; c1.LCR = []; c1.totextvar = 1; c1.NLC(1).("func") = "Mvoltagesources"; c1.NLC(1).("section") = "pwl"; c1.NLC(1).("nextvar") = 2; c1.NLC(1).("npar") = 398; c1.NLC(1).("nrows") = 1; c1.NLC(1).("nparnames") = 0; c1.NLC(1).("parnames") = {}; c1.NLC(1).("pvmatrix") = pwl; c1.NLC(1).("vnmatrix") = [1 0]; c1.NLC(1).("nintvar") = 1; c1.NLC(1).("osintvar") = 0; c1.NLC(2).("func") = "Mmemristors"; c1.NLC(2).("section") = "STRUKOV"; c1.NLC(2).("nextvar") = 2; c1.NLC(2).("npar") = 3; c1.totintvar = 2; c1.namesn = [1 2 3]; c1.NLC(2).("nrows") = 1; c1.NLC(2).("nparnames") = 3; c1.NLC(2).("parnames") = {"MU", "RH", "RL"}; c1.NLC(2).("pvmatrix") = [1.8e3 1e3 1]; c1.NLC(2).("vnmatrix") = [1 0]; c1.NLC(2).("nintvar") = 1; c1.NLC(2).("osintvar") = 1; c1.namess = {"voltage", "current", "x"}; start = [0 0 0.1]; %% c = prs_iff ("memristor_example"); out = tst_backward_euler (c1, start.', t, 1e-2, 300, {'voltage', 'current'}); plot (out(1, 1:100), out (2, 1:100), 'r', out(1, 101:end), out(2, 101:end), 'k') legend ("frequency 1 Hz", "frequency 4 Hz")

Memristor simulation result

The results are shown in the figure to the right.