Ngspice User Manual V27

User Manual: Pdf

Open the PDF directly: View PDF PDF.
Page Count: 624 [warning: Documents this large are best viewed by clicking the View PDF Link!]

Ngspice Users Manual
Version 27
(Describes ngspice-27 release version)
Holger Vogt, Marcel Hendrix, Paolo Nenzi
August 31, 2017
2
Locations
The project and download pages of ngspice may be found at
Ngspice home page http://ngspice.sourceforge.net/
Project page at sourceforge http://sourceforge.net/projects/ngspice/
Download page at sourceforge http://sourceforge.net/projects/ngspice/files/
Git source download http://sourceforge.net/scm/?type=cvs&group_id=38962
Status
This manual is a work in progress. Some to-dos are listed in the following. More is surely
needed. You are invited to report bugs, missing items, wrongly described items, bad English
style etc.
To Do
1. Review of Chapt. 1.3
2. hfet1,2 model descriptions
How to use this manual
The manual is a ‘work in progress’. It may accompany a specific ngspice release, e.g. ngspice-
24 as manual version 24. If its name contains ‘Version xxplus’, it describes the actual code
status, found at the date of issue in the Git Source Code Management (SCM) tool. The manual is
intended to provide a complete description of the ngspice functionality, its features, commands,
or procedures. It is not a book about learning SPICE usage, but the novice user may find some
hints how to start using ngspice. Chapter 21.1 gives a short introduction how to set up and
simulate a small circuit. Chapter 32 is about compiling and installing ngspice from a tarball or
the actual Git source code, which you may find on the ngspice web pages. If you are running a
specific Linux distribution, you may check if it provides ngspice as part of the package. Some
are listed here.
Part I
Ngspice User Manual
3
Contents
I Ngspice User Manual 3
1 Introduction 35
1.1 Simulation Algorithms .............................. 36
1.1.1 Analog Simulation ............................ 36
1.1.2 Digital Simulation ............................ 37
1.1.3 Mixed-Mode Simulation ......................... 37
1.1.4 Mixed-Level Simulation ......................... 38
1.2 Supported Analyses ................................ 39
1.2.1 DC Analyses ............................... 39
1.2.2 AC Small-Signal Analysis ........................ 40
1.2.3 Transient Analysis ............................ 40
1.2.4 Pole-Zero Analysis ............................ 40
1.2.5 Small-Signal Distortion Analysis .................... 41
1.2.6 Sensitivity Analysis ........................... 41
1.2.7 Noise Analysis .............................. 42
1.2.8 Periodic Steady State Analysis ..................... 42
1.3 Analysis at Different Temperatures ........................ 42
1.4 Convergence ................................... 44
1.4.1 Voltage convergence criterion ...................... 44
1.4.2 Current convergence criterion ...................... 44
1.4.3 Convergence failure ........................... 45
2 Circuit Description 47
2.1 General Structure and Conventions ........................ 47
2.1.1 Input file structure ............................ 47
2.1.2 Circuit elements (device instances) ................... 47
2.1.3 Some naming conventions ........................ 49
5
6CONTENTS
2.2 Basic lines ..................................... 50
2.2.1 .TITLE line ................................ 50
2.2.2 .END Line ................................ 50
2.2.3 Comments ................................ 51
2.2.4 End-of-line comments .......................... 51
2.3 .MODEL Device Models ............................. 51
2.4 .SUBCKT Subcircuits ............................... 52
2.4.1 .SUBCKT Line .............................. 53
2.4.2 .ENDS Line ................................ 54
2.4.3 Subcircuit Calls .............................. 54
2.5 .GLOBAL ..................................... 54
2.6 .INCLUDE .................................... 55
2.7 .LIB ........................................ 55
2.8 .PARAM Parametric netlists ........................... 55
2.8.1 .param line ................................ 56
2.8.2 Brace expressions in circuit elements: .................. 56
2.8.3 Subcircuit parameters ........................... 57
2.8.4 Symbol scope ............................... 58
2.8.5 Syntax of expressions .......................... 58
2.8.6 Reserved words ............................. 61
2.8.7 Alternative syntax ............................ 61
2.9 .FUNC ....................................... 61
2.10 .CSPARAM .................................... 62
2.11 .TEMP ....................................... 63
2.12 .IF Condition-Controlled Netlist ......................... 63
2.13 Parameters, functions, expressions, and command scripts ............ 65
2.13.1 Parameters ................................ 65
2.13.2 Nonlinear sources ............................. 65
2.13.3 Control commands, Command scripts .................. 65
3 Circuit Elements and Models 67
3.1 General options and information ......................... 67
3.1.1 Paralleling devices with multiplier m .................. 67
3.1.2 Technology scaling ............................ 69
3.1.3 Model binning .............................. 69
CONTENTS 7
3.1.4 Initial conditions ............................. 69
3.2 Elementary Devices ................................ 70
3.2.1 Resistors ................................. 70
3.2.2 Semiconductor Resistors ......................... 71
3.2.3 Semiconductor Resistor Model (R) ................... 72
3.2.4 Resistors, dependent on expressions (behavioral resistor) ........ 73
3.2.5 Capacitors ................................ 74
3.2.6 Semiconductor Capacitors ........................ 75
3.2.7 Semiconductor Capacitor Model (C) ................... 75
3.2.8 Capacitors, dependent on expressions (behavioral capacitor) ...... 77
3.2.9 Inductors ................................. 78
3.2.10 Inductor model .............................. 78
3.2.11 Coupled (Mutual) Inductors ....................... 80
3.2.12 Inductors, dependent on expressions (behavioral inductor) ....... 80
3.2.13 Capacitor or inductor with initial conditions .............. 81
3.2.14 Switches ................................. 82
3.2.15 Switch Model (SW/CSW) ........................ 83
4 Voltage and Current Sources 85
4.1 Independent Sources for Voltage or Current ................... 85
4.1.1 Pulse ................................... 86
4.1.2 Sinusoidal ................................. 87
4.1.3 Exponential ................................ 87
4.1.4 Piece-Wise Linear ............................ 88
4.1.5 Single-Frequency FM .......................... 88
4.1.6 Amplitude modulated source (AM) ................... 89
4.1.7 Transient noise source .......................... 90
4.1.8 Random voltage source .......................... 91
4.1.9 External voltage or current input ..................... 91
4.1.10 Arbitrary Phase Sources ......................... 92
4.2 Linear Dependent Sources ............................ 92
4.2.1 Gxxxx: Linear Voltage-Controlled Current Sources (VCCS) ...... 92
4.2.2 Exxxx: Linear Voltage-Controlled Voltage Sources (VCVS) ...... 93
4.2.3 Fxxxx: Linear Current-Controlled Current Sources (CCCS) ...... 93
4.2.4 Hxxxx: Linear Current-Controlled Voltage Sources (CCVS) ...... 93
4.2.5 Polynomial Source Compatibility .................... 94
8CONTENTS
5 Non-linear Dependent Sources (Behavioral Sources) 95
5.1 Bxxxx: Nonlinear dependent source (ASRC) .................. 95
5.1.1 Syntax and usage ............................. 95
5.1.2 Special B-Source Variables time, temper, hertz ............. 98
5.1.3 par(’expression’)............................. 99
5.1.4 Piecewise Linear Function: pwl ..................... 99
5.2 Exxxx: non-linear voltage source1........................ 101
5.2.1 VOL ................................... 101
5.2.2 VALUE .................................. 101
5.2.3 TABLE .................................. 101
5.2.4 POLY ................................... 102
5.2.5 LAPLACE ................................ 103
5.3 Gxxxx: non-linear current source2........................ 104
5.3.1 CUR ................................... 104
5.3.2 VALUE .................................. 104
5.3.3 TABLE .................................. 104
5.3.4 POLY ................................... 105
5.3.5 LAPLACE ................................ 105
5.3.6 Example ................................. 105
5.4 Debugging a behavioral source .......................... 106
6 Transmission Lines 109
6.1 Lossless Transmission Lines ........................... 109
6.2 Lossy Transmission Lines ............................ 110
6.2.1 Lossy Transmission Line Model (LTRA) ................ 110
6.3 Uniform Distributed RC Lines .......................... 112
6.3.1 Uniform Distributed RC Model (URC) ................. 112
6.4 KSPICE Lossy Transmission Lines ........................ 113
6.4.1 Single Lossy Transmission Line (TXL) ................. 113
6.4.2 Coupled Multiconductor Line (CPL) ................... 114
7 Diodes 117
7.1 Junction Diodes .................................. 117
7.2 Diode Model (D) ................................. 117
7.3 Diode Equations .................................. 119
1To get this functionality, the compatibility mode has to be set in spinit or .spiceinit by set ngbehavior=all.
2To get this functionality, the compatibility mode has to be set in spinit or .spiceinit by set ngbehavior=all.
CONTENTS 9
8 BJTs 125
8.1 Bipolar Junction Transistors (BJTs) ....................... 125
8.2 BJT Models (NPN/PNP) ............................. 125
9 JFETs 131
9.1 Junction Field-Effect Transistors (JFETs) .................... 131
9.2 JFET Models (NJF/PJF) ............................. 131
9.2.1 JFET level 1 model with Parker Skellern modification ......... 131
9.2.2 JFET level 2 Parker Skellern model ................... 133
10 MESFETs 135
10.1 MESFETs ..................................... 135
10.2 MESFET Models (NMF/PMF) .......................... 135
10.2.1 Model by Statz e.a. ............................ 135
10.2.2 Model by Ytterdal e.a. .......................... 136
10.2.3 hfet1 ................................... 136
10.2.4 hfet2 ................................... 136
11 MOSFETs 137
11.1 MOSFET devices ................................. 137
11.2 MOSFET models (NMOS/PMOS) ........................ 138
11.2.1 MOS Level 1 ............................... 138
11.2.2 MOS Level 2 ............................... 140
11.2.3 MOS Level 3 ............................... 140
11.2.4 MOS Level 6 ............................... 140
11.2.5 Notes on Level 1-6 models ........................ 140
11.2.6 BSIM Models ............................... 143
11.2.7 BSIM1 model (level 4) .......................... 143
11.2.8 BSIM2 model (level 5) .......................... 145
11.2.9 BSIM3 model (levels 8, 49) ....................... 145
11.2.10 BSIM4 model (levels 14, 54) ....................... 146
11.2.11 EKV model ................................ 147
11.2.12 BSIMSOI models (levels 10, 58, 55, 56, 57) ............... 147
11.2.13 SOI3 model (level 60) .......................... 147
11.2.14 HiSIM models of the University of Hiroshima .............. 147
10 CONTENTS
12 Mixed-Mode and Behavioral Modeling with XSPICE 149
12.1 Code Model Element & .MODEL Cards .................... 149
12.1.1 Syntax .................................. 149
12.1.2 Examples ................................. 153
12.1.3 Search path for file input ......................... 153
12.2 Analog Models .................................. 154
12.2.1 Gain .................................... 154
12.2.2 Summer .................................. 155
12.2.3 Multiplier ................................. 156
12.2.4 Divider .................................. 157
12.2.5 Limiter .................................. 158
12.2.6 Controlled Limiter ............................ 160
12.2.7 PWL Controlled Source ......................... 161
12.2.8 Filesource ................................. 163
12.2.9 multi_input_pwl block .......................... 165
12.2.10 Analog Switch .............................. 166
12.2.11 Zener Diode ............................... 167
12.2.12 Current Limiter .............................. 169
12.2.13 Hysteresis Block ............................. 172
12.2.14 Differentiator ............................... 173
12.2.15 Integrator ................................. 174
12.2.16 S-Domain Transfer Function ....................... 176
12.2.17 Slew Rate Block ............................. 179
12.2.18 Inductive Coupling ............................ 180
12.2.19 Magnetic Core .............................. 181
12.2.20 Controlled Sine Wave Oscillator ..................... 184
12.2.21 Controlled Triangle Wave Oscillator ................... 185
12.2.22 Controlled Square Wave Oscillator .................... 186
12.2.23 Controlled One-Shot ........................... 188
12.2.24 Capacitance Meter ............................ 190
12.2.25 Inductance Meter ............................. 191
12.2.26 Memristor ................................. 192
12.2.27 2D table model .............................. 193
12.2.28 3D table model .............................. 194
12.3 Hybrid Models .................................. 197
CONTENTS 11
12.3.1 Digital-to-Analog Node Bridge ..................... 197
12.3.2 Analog-to-Digital Node Bridge ..................... 198
12.3.3 Controlled Digital Oscillator ....................... 200
12.3.4 Node bridge from digital to real with enable ............... 201
12.3.5 A Z**-1 block working on real data ................... 201
12.3.6 A gain block for event-driven real data .................. 202
12.3.7 Node bridge from real to analog voltage ................. 203
12.4 Digital Models .................................. 203
12.4.1 Buffer ................................... 203
12.4.2 Inverter .................................. 204
12.4.3 And .................................... 205
12.4.4 Nand ................................... 206
12.4.5 Or ..................................... 207
12.4.6 Nor .................................... 208
12.4.7 Xor .................................... 209
12.4.8 Xnor ................................... 210
12.4.9 Tristate .................................. 211
12.4.10 Pullup ................................... 213
12.4.11 Pulldown ................................. 213
12.4.12 D Flip Flop ................................ 214
12.4.13 JK Flip Flop ............................... 216
12.4.14 Toggle Flip Flop ............................. 218
12.4.15 Set-Reset Flip Flop ............................ 220
12.4.16 D Latch .................................. 223
12.4.17 Set-Reset Latch .............................. 225
12.4.18 State Machine ............................... 227
12.4.19 Frequency Divider ............................ 230
12.4.20 RAM ................................... 232
12.4.21 Digital Source .............................. 234
12.4.22 LUT .................................... 236
12.4.23 General LUT ............................... 237
12.5 Predefined Node Types for event driven simulation ............... 239
12.5.1 Digital Node Type ............................ 239
12.5.2 Real Node Type ............................. 239
12.5.3 Int Node Type .............................. 239
12.5.4 (Digital) Input/Output .......................... 239
12 CONTENTS
13 Verilog A Device models 241
13.1 Introduction .................................... 241
13.2 adms ........................................ 241
13.3 How to integrate a Verilog-A model into ngspice ................ 241
13.3.1 How to setup a *.va model for ngspice .................. 241
13.3.2 Adding admsXml to your build environment .............. 241
14 Mixed-Level Simulation (ngspice with TCAD) 243
14.1 Cider ....................................... 243
14.2 GSS, Genius .................................... 244
15 Analyses and Output Control (batch mode) 245
15.1 Simulator Variables (.options) .......................... 245
15.1.1 General Options ............................. 246
15.1.2 DC Solution Options ........................... 247
15.1.3 AC Solution Options ........................... 248
15.1.4 Transient Analysis Options ........................ 248
15.1.5 ELEMENT Specific options ....................... 249
15.1.6 Transmission Lines Specific Options ................... 250
15.1.7 Precedence of option and .options commands .............. 250
15.2 Initial Conditions ................................. 250
15.2.1 .NODESET: Specify Initial Node Voltage Guesses ........... 250
15.2.2 .IC: Set Initial Conditions ........................ 251
15.3 Analyses ...................................... 252
15.3.1 .AC: Small-Signal AC Analysis ..................... 252
15.3.2 .DC: DC Transfer Function ........................ 253
15.3.3 .DISTO: Distortion Analysis ....................... 253
15.3.4 .NOISE: Noise Analysis ......................... 255
15.3.5 .OP: Operating Point Analysis ...................... 255
15.3.6 .PZ: Pole-Zero Analysis ......................... 256
15.3.7 .SENS: DC or Small-Signal AC Sensitivity Analysis .......... 257
15.3.8 .TF: Transfer Function Analysis ..................... 257
15.3.9 .TRAN: Transient Analysis ........................ 258
15.3.10 Transient noise analysis (at low frequency) ............... 258
15.3.11 .PSS: Periodic Steady State Analysis .................. 262
15.4 Measurements after AC, DC and Transient Analysis ............... 263
CONTENTS 13
15.4.1 .meas(ure) ................................. 263
15.4.2 batch versus interactive mode ...................... 263
15.4.3 General remarks ............................. 263
15.4.4 Input ................................... 264
15.4.5 Trig Targ ................................. 264
15.4.6 Find ... When ............................... 266
15.4.7 AVG|MIN|MAX|PP|RMS|MIN_AT|MAX_AT ................ 267
15.4.8 Integ ................................... 267
15.4.9 param ................................... 268
15.4.10 par(’expression’)............................. 268
15.4.11 Deriv ................................... 269
15.4.12 More examples .............................. 269
15.5 Safe Operating Area (SOA) warning messages .................. 270
15.5.1 Resistor and Capacitor SOA model parameters ............. 271
15.5.2 Diode SOA model parameter ....................... 271
15.5.3 BJT SOA model parameter ........................ 271
15.5.4 MOS SOA model parameter ....................... 271
15.6 Batch Output ................................... 272
15.6.1 .SAVE: Name vector(s) to be saved in raw file .............. 272
15.6.2 .PRINT Lines ............................... 273
15.6.3 .PLOT Lines ............................... 273
15.6.4 .FOUR: Fourier Analysis of Transient Analysis Output ......... 274
15.6.5 .PROBE: Name vector(s) to be saved in raw file ............. 275
15.6.6 par(’expression’): Algebraic expressions for output ........... 275
15.6.7 .width ................................... 276
15.7 Measuring current through device terminals ................... 276
15.7.1 Adding a voltage source in series .................... 276
15.7.2 Using option ’savecurrents’ ....................... 276
16 Starting ngspice 279
16.1 Introduction .................................... 279
16.2 Where to obtain ngspice ............................. 279
16.3 Command line options for starting ngspice and ngnutmeg ............ 280
16.4 Starting options .................................. 282
16.4.1 Batch mode ................................ 282
14 CONTENTS
16.4.2 Interactive mode ............................. 282
16.4.3 Control mode (Interactive mode with control file or control section) . . 283
16.5 Standard configuration file spinit ......................... 284
16.6 User defined configuration file .spiceinit ..................... 285
16.7 Environmental variables ............................. 285
16.7.1 Ngspice specific variables ........................ 285
16.7.2 Common environment variables ..................... 286
16.8 Memory usage .................................. 286
16.9 Simulation time .................................. 287
16.10Ngspice on multi-core processors using OpenMP ................ 287
16.10.1 Introduction ................................ 287
16.10.2 Some results ............................... 288
16.10.3 Usage ................................... 289
16.10.4 Literature ................................. 289
16.11Server mode option -s ............................... 289
16.12Ngspice control via input, output fifos ...................... 291
16.13Compatibility ................................... 293
16.13.1 Compatibility mode ........................... 293
16.13.2 Missing functions ............................. 293
16.13.3 Devices .................................. 294
16.13.4 Controls and commands ......................... 294
16.14Tests ........................................ 295
16.15Reporting bugs and errors ............................. 296
17 Interactive Interpreter 297
17.1 Introduction .................................... 297
17.2 Expressions, Functions, and Constants ...................... 298
17.3 Plots ........................................ 302
17.4 Command Interpretation ............................. 303
17.4.1 On the console .............................. 303
17.4.2 Scripts .................................. 303
17.4.3 Add-on to circuit file ........................... 303
17.5 Commands .................................... 304
17.5.1 Ac*: Perform an AC, small-signal frequency response analysis . . . . . 304
17.5.2 Alias: Create an alias for a command .................. 305
CONTENTS 15
17.5.3 Alter*: Change a device or model parameter .............. 305
17.5.4 Altermod*: Change model parameter(s) ................ 306
17.5.5 Asciiplot: Plot values using old-style character plots .......... 308
17.5.6 Aspice*: Asynchronous ngspice run ................... 308
17.5.7 Bug: Mail a bug report .......................... 308
17.5.8 Cd: Change directory ........................... 308
17.5.9 Cdump: Dump the control flow to the screen .............. 309
17.5.10 Circbyline*: Enter a circuit line by line ................. 309
17.5.11 Codemodel*: Load an XSPICE code model library ........... 310
17.5.12 Compose: Compose a vector ....................... 310
17.5.13 Dc*: Perform a DC-sweep analysis ................... 311
17.5.14 Define: Define a function ......................... 311
17.5.15 Deftype: Define a new type for a vector or plot ............. 311
17.5.16 Delete*: Remove a trace or breakpoint .................. 312
17.5.17 Destroy: Delete an output data set .................... 312
17.5.18 Devhelp: information on available devices ................ 312
17.5.19 Diff: Compare vectors .......................... 313
17.5.20 Display: List known vectors and types .................. 313
17.5.21 Echo: Print text .............................. 313
17.5.22 Edit*: Edit the current circuit ...................... 313
17.5.23 Edisplay: Print a list of all the event nodes ............... 314
17.5.24 Eprint: Print an event driven node .................... 314
17.5.25 Eprvcd: Dump event nodes in VCD format ............... 314
17.5.26 FFT: fast Fourier transform of vectors .................. 314
17.5.27 Fourier: Perform a Fourier transform .................. 316
17.5.28 Gnuplot: Graphics output via gnuplot .................. 317
17.5.29 Hardcopy: Save a plot to a file for printing ............... 317
17.5.30 Help: Print summaries of Ngspice commands ............. 318
17.5.31 History: Review previous commands .................. 318
17.5.32 Inventory: Print circuit inventory ..................... 321
17.5.33 Iplot*: Incremental plot ......................... 321
17.5.34 Jobs*: List active asynchronous ngspice runs .............. 321
17.5.35 Let: Assign a value to a vector ...................... 321
17.5.36 Linearize*: Interpolate to a linear scale ................. 322
17.5.37 Listing*: Print a listing of the current circuit .............. 323
16 CONTENTS
17.5.38 Load: Load rawfile data ......................... 323
17.5.39 Meas*: Measurements on simulation data ................ 323
17.5.40 Mdump*: Dump the matrix values to a file (or to console) ....... 324
17.5.41 Mrdump*: Dump the matrix right hand side values to a file (or to console)324
17.5.42 Noise*: Noise analysis .......................... 324
17.5.43 Op*: Perform an operating point analysis ................ 325
17.5.44 Option*: Set a ngspice option ...................... 325
17.5.45 Plot: Plot vectors on the display ..................... 326
17.5.46 Pre_<command>: execute commands prior to parsing the circuit . . . . 327
17.5.47 Print: Print values ............................ 328
17.5.48 Quit: Leave Ngspice or Nutmeg ..................... 328
17.5.49 Rehash: Reset internal hash tables .................... 329
17.5.50 Remcirc*: Remove the current circuit .................. 329
17.5.51 Reset*: Reset an analysis ......................... 329
17.5.52 Reshape: Alter the dimensionality or dimensions of a vector ...... 329
17.5.53 Resume*: Continue a simulation after a stop .............. 330
17.5.54 Rspice*: Remote ngspice submission .................. 330
17.5.55 Run*: Run analysis from the input file .................. 330
17.5.56 Rusage: Resource usage ......................... 331
17.5.57 Save*: Save a set of outputs ....................... 332
17.5.58 Sens*: Run a sensitivity analysis ..................... 333
17.5.59 Set: Set the value of a variable ...................... 333
17.5.60 Setcirc*: Change the current circuit ................... 333
17.5.61 Setplot: Switch the current set of vectors ................ 334
17.5.62 Setscale: Set the scale vector for the current plot ............ 334
17.5.63 Settype: Set the type of a vector ..................... 334
17.5.64 Shell: Call the command interpreter ................... 335
17.5.65 Shift: Alter a list variable ......................... 335
17.5.66 Show*: List device state ......................... 335
17.5.67 Showmod*: List model parameter values ................ 335
17.5.68 Snload*: Load the snapshot file ..................... 336
17.5.69 Snsave*: Save a snapshot file ...................... 336
17.5.70 Source: Read a ngspice input file .................... 337
17.5.71 Spec: Create a frequency domain plot .................. 338
17.5.72 Status*: Display breakpoint information ................. 338
CONTENTS 17
17.5.73 Step*: Run a fixed number of time-points ................ 338
17.5.74 Stop*: Set a breakpoint .......................... 339
17.5.75 Strcmp: Compare two strings ...................... 339
17.5.76 Sysinfo*: Print system information ................... 340
17.5.77 Tf*: Run a Transfer Function analysis .................. 340
17.5.78 Trace*: Trace nodes ........................... 341
17.5.79 Tran*: Perform a transient analysis ................... 341
17.5.80 Transpose: Swap the elements in a multi-dimensional data set . . . . . 342
17.5.81 Unalias: Retract an alias ......................... 342
17.5.82 Undefine: Retract a definition ...................... 342
17.5.83 Unlet: Delete the specified vector(s) ................... 342
17.5.84 Unset: Clear a variable .......................... 343
17.5.85 Version: Print the version of ngspice ................... 343
17.5.86 Where*: Identify troublesome node or device .............. 344
17.5.87 Wrdata: Write data to a file (simple table) ................ 345
17.5.88 Write: Write data to a file (Spice3f5 format) ............... 345
17.5.89 Wrs2p: Write scattering parameters to file (Touchstone® format) . . . 346
17.5.90 Xgraph: use the xgraph(1) program for plotting. ............ 346
17.6 Control Structures ................................. 347
17.6.1 While - End ................................ 347
17.6.2 Repeat - End ............................... 347
17.6.3 Dowhile - End .............................. 347
17.6.4 Foreach - End ............................... 347
17.6.5 If - Then - Else .............................. 348
17.6.6 Label ................................... 348
17.6.7 Goto ................................... 348
17.6.8 Continue ................................. 349
17.6.9 Break ................................... 349
17.7 Internally predefined variables .......................... 349
17.8 Scripts ....................................... 354
17.8.1 Variables ................................. 354
17.8.2 Vectors .................................. 355
17.8.3 Commands ................................ 355
17.8.4 control structures ............................. 355
17.8.5 Example script ’spectrum’ ........................ 359
18 CONTENTS
17.8.6 Example script for random numbers ................... 361
17.8.7 Parameter sweep ............................. 362
17.8.8 Output redirection ............................ 362
17.9 Scattering parameters (s-parameters) ....................... 364
17.9.1 Intro .................................... 364
17.9.2 S-parameter measurement basics ..................... 364
17.9.3 Usage ................................... 366
17.10MISCELLANEOUS ............................... 366
17.11Bugs ........................................ 367
18 Ngspice User Interfaces 369
18.1 MS Windows Graphical User Interface ...................... 369
18.2 MS Windows Console .............................. 371
18.3 Linux ....................................... 372
18.4 CygWin ...................................... 372
18.5 Error handling ................................... 372
18.6 Postscript printing options ............................ 373
18.7 .......................................... 374
18.8 Integration with CAD software and ‘third party’ GUIs .............. 374
18.8.1 KJWaves ................................. 374
18.8.2 GNU Spice GUI ............................. 374
18.8.3 XCircuit ................................. 374
18.8.4 GEDA ................................... 374
18.8.5 CppSim .................................. 375
18.8.6 NGSPICE Online ............................. 375
18.8.7 Spicy Schematics ............................. 375
18.8.8 MSEspice ................................. 375
18.8.9 PartSim .................................. 375
19 ngspice as shared library or dynamic link library 377
19.1 Compile options .................................. 377
19.1.1 How to get the sources .......................... 377
19.1.2 Linux, MINGW, CYGWIN ....................... 377
19.1.3 MS Visual Studio ............................. 377
19.2 Linking shared ngspice to a calling application ................. 378
19.2.1 Linking during creating the caller .................... 378
CONTENTS 19
19.2.2 Loading at runtime ............................ 378
19.3 Shared ngspice API ................................ 378
19.3.1 structs and types defined for transporting data .............. 378
19.3.2 Exported functions ............................ 380
19.3.3 Callback functions ............................ 382
19.4 General remarks on using the API ........................ 384
19.4.1 Loading a netlist ............................. 384
19.4.2 Running the simulation .......................... 385
19.4.3 Accessing data .............................. 386
19.4.4 Altering model or device parameters ................... 386
19.4.5 Output .................................. 386
19.4.6 Error handling .............................. 387
19.5 Example applications ............................... 387
19.6 ngspice parallel .................................. 387
19.6.1 Go parallel! ................................ 388
19.6.2 Additional exported functions ...................... 389
19.6.3 Additional callback functions ...................... 390
19.6.4 Parallel ngspice example ......................... 391
20 TCLspice 393
20.1 tclspice framework ................................ 393
20.2 tclspice documentation .............................. 393
20.3 spicetoblt ..................................... 393
20.4 Running TCLspice ................................ 394
20.5 examples ..................................... 394
20.5.1 Active capacitor measurement ...................... 394
20.5.2 Optimization of a linearization circuit for a Thermistor ......... 397
20.5.3 Progressive display ............................ 401
20.6 Compiling ..................................... 402
20.6.1 Linux ................................... 402
20.6.2 MS Windows ............................... 402
20.7 MS Windows 32 Bit binaries ........................... 403
20 CONTENTS
21 Example Circuits 405
21.1 AC coupled transistor amplifier .......................... 405
21.2 Differential Pair .................................. 411
21.3 MOSFET Characterization ............................ 411
21.4 RTL Inverter .................................... 411
21.5 Four-Bit Binary Adder (Bipolar) ......................... 412
21.6 Four-Bit Binary Adder (MOS) .......................... 414
21.7 Transmission-Line Inverter ............................ 415
22 Statistical circuit analysis 417
22.1 Introduction .................................... 417
22.2 Using random param(eters) ............................ 417
22.3 Behavioral sources (B, E, G, R, L, C) with random control ........... 419
22.4 ngspice scripting language ............................ 420
22.5 Monte-Carlo Simulation ............................. 421
22.5.1 Example 1 ................................ 421
22.5.2 Example 2 ................................ 423
22.5.3 Example 3 ................................ 423
22.5.4 Example 4 ................................ 423
22.6 Data evaluation with ............................... 424
23 Circuit optimization with ngspice 427
23.1 Optimization of a circuit ............................. 427
23.2 ngspice optimizer using ngspice scripts ..................... 428
23.3 ngspice optimizer using tclspice ......................... 428
23.4 ngspice optimizer using a Python script ..................... 428
23.5 ngspice optimizer using ASCO .......................... 428
23.5.1 Three stage operational amplifier ..................... 429
23.5.2 Digital inverter .............................. 430
23.5.3 Bandpass ................................. 432
23.5.4 Class-E power amplifier ......................... 433
24 Notes 435
24.1 Glossary ...................................... 435
24.2 Acronyms and Abbreviations ........................... 436
CONTENTS 21
II XSPICE Software User’s Manual 439
25 XSPICE Basics 441
25.1 ngspice with the XSPICE option ......................... 441
25.2 The XSPICE Code Model Subsystem ...................... 441
25.3 XSPICE Top-Level Diagram ........................... 442
26 Execution Procedures 443
26.1 Simulation and Modeling Overview ....................... 443
26.1.1 Describing the Circuit .......................... 443
26.2 Circuit Description Syntax ............................ 449
26.2.1 XSPICE Syntax Extensions ....................... 449
26.3 How to create code models ............................ 451
27 Example circuits 455
27.1 Amplifier with XSPICE model ‘gain’ ...................... 455
27.2 XSPICE advanced usage ............................. 457
27.2.1 Circuit example C3 ............................ 457
27.2.2 Running example C3 ........................... 460
28 Code Models and User-Defined Nodes 465
28.1 Code Model Data Type Definitions ........................ 466
28.2 Creating Code Models .............................. 466
28.3 Creating User-Defined Nodes ........................... 467
28.4 Adding a new code model library ......................... 468
28.5 Compiling and loading the new code model (library) .............. 468
28.6 Interface Specification File ............................ 469
28.6.1 The Name Table ............................. 471
28.6.2 The Port Table .............................. 471
28.6.3 The Parameter Table ........................... 473
28.6.4 Static Variable Table ........................... 474
28.7 Model Definition File .............................. 476
28.7.1 Macros .................................. 476
28.7.2 Function Library ............................. 485
28.8 User-Defined Node Definition File ........................ 492
28.8.1 Macros .................................. 493
28.8.2 Function Library ............................. 493
28.8.3 Example UDN Definition File ...................... 496
22 CONTENTS
29 Error Messages 501
29.1 Preprocessor Error Messages ........................... 501
29.2 Simulator Error Messages ............................ 506
29.3 Code Model Error Messages ........................... 507
29.3.1 Code Model aswitch ........................... 507
29.3.2 Code Model climit ............................ 508
29.3.3 Code Model core ............................. 508
29.3.4 Code Model d_osc ............................ 508
29.3.5 Code Model d_source .......................... 509
29.3.6 Code Model d_state ........................... 509
29.3.7 Code Model oneshot ........................... 510
29.3.8 Code Model pwl ............................. 510
29.3.9 Code Model s_xfer ............................ 510
29.3.10 Code Model sine ............................. 511
29.3.11 Code Model square ........................... 511
29.3.12 Code Model triangle ........................... 512
III CIDER 513
30 CIDER User’s Manual 515
30.1 SPECIFICATION ................................. 515
30.1.1 Examples ................................. 516
30.2 BOUNDARY, INTERFACE ........................... 517
30.2.1 DESCRIPTION ............................. 517
30.2.2 PARAMETERS ............................. 518
30.2.3 EXAMPLES ............................... 518
30.3 COMMENT .................................... 518
30.3.1 DESCRIPTION ............................. 519
30.3.2 EXAMPLES ............................... 519
30.4 CONTACT .................................... 519
30.4.1 DESCRIPTION ............................. 519
30.4.2 PARAMETERS ............................. 519
30.4.3 EXAMPLES ............................... 519
30.4.4 SEE ALSO ................................ 520
30.5 DOMAIN, REGION ............................... 520
CONTENTS 23
30.5.1 DESCRIPTION ............................. 520
30.5.2 PARAMETERS ............................. 520
30.5.3 EXAMPLES ............................... 520
30.5.4 SEE ALSO ................................ 521
30.6 DOPING ..................................... 521
30.6.1 DESCRIPTION ............................. 521
30.6.2 PARAMETERS ............................. 524
30.6.3 EXAMPLES ............................... 524
30.6.4 SEE ALSO ................................ 525
30.7 ELECTRODE ................................... 525
30.7.1 DESCRIPTION ............................. 525
30.7.2 PARAMETERS ............................. 526
30.7.3 EXAMPLES ............................... 526
30.7.4 SEE ALSO ................................ 526
30.8 END ....................................... 526
30.8.1 DESCRIPTION ............................. 527
30.9 MATERIAL ................................... 527
30.9.1 DESCRIPTION ............................. 527
30.9.2 PARAMETERS ............................. 528
30.9.3 EXAMPLES ............................... 528
30.9.4 SEE ALSO ................................ 528
30.10METHOD .................................... 529
30.10.1 DESCRIPTION ............................. 529
30.10.2 Parameters ................................ 529
30.10.3 Examples ................................. 529
30.11Mobility ...................................... 530
30.11.1 Description ................................ 530
30.11.2 Parameters ................................ 531
30.11.3 Examples ................................. 531
30.11.4 SEE ALSO ................................ 531
30.11.5 BUGS .................................. 532
30.12MODELS ..................................... 532
30.12.1 DESCRIPTION ............................. 532
30.12.2 Parameters ................................ 532
30.12.3 Examples ................................. 532
24 CONTENTS
30.12.4 See also .................................. 533
30.12.5 Bugs ................................... 533
30.13OPTIONS .................................... 533
30.13.1 DESCRIPTION ............................. 533
30.13.2 Parameters ................................ 534
30.13.3 Examples ................................. 534
30.13.4 See also .................................. 534
30.14OUTPUT ..................................... 535
30.14.1 DESCRIPTION ............................. 535
30.14.2 Parameters ................................ 536
30.14.3 Examples ................................. 536
30.14.4 SEE ALSO ................................ 537
30.15TITLE ....................................... 537
30.15.1 DESCRIPTION ............................. 537
30.15.2 EXAMPLES ............................... 537
30.15.3 BUGS .................................. 537
30.16X.MESH, Y.MESH ................................ 537
30.16.1 DESCRIPTION ............................. 538
30.16.2 Parameters ................................ 539
30.16.3 EXAMPLES ............................... 539
30.16.4 SEE ALSO ................................ 539
30.17NUMD ...................................... 540
30.17.1 DESCRIPTION ............................. 540
30.17.2 Parameters ................................ 541
30.17.3 EXAMPLES ............................... 541
30.17.4 SEE ALSO ................................ 542
30.17.5 BUGS .................................. 542
30.18NBJT ....................................... 542
30.18.1 DESCRIPTION ............................. 542
30.18.2 Parameters ................................ 543
30.18.3 EXAMPLES ............................... 543
30.18.4 SEE ALSO ................................ 544
30.18.5 BUGS .................................. 544
30.19NUMOS ..................................... 544
30.19.1 DESCRIPTION ............................. 544
CONTENTS 25
30.19.2 Parameters ................................ 545
30.19.3 EXAMPLES ............................... 545
30.19.4 SEE ALSO ................................ 546
30.20Cider examples .................................. 546
IV Appendices 547
31 Model and Device Parameters 549
31.1 Accessing internal device parameters ....................... 549
31.2 Elementary Devices ................................ 551
31.2.1 Resistor .................................. 551
31.2.2 Capacitor - Fixed capacitor ........................ 553
31.2.3 Inductor - Fixed inductor ......................... 554
31.2.4 Mutual - Mutual Inductor ......................... 555
31.3 Voltage and current sources ............................ 556
31.3.1 ASRC - Arbitrary source ......................... 556
31.3.2 Isource - Independent current source ................... 557
31.3.3 Vsource - Independent voltage source .................. 558
31.3.4 CCCS - Current controlled current source ................ 559
31.3.5 CCVS - Current controlled voltage source ................ 559
31.3.6 VCCS - Voltage controlled current source ................ 560
31.3.7 VCVS - Voltage controlled voltage source ................ 560
31.4 Transmission Lines ................................ 561
31.4.1 CplLines - Simple Coupled Multiconductor Lines ............ 561
31.4.2 LTRA - Lossy transmission line ..................... 562
31.4.3 Tranline - Lossless transmission line ................... 563
31.4.4 TransLine - Simple Lossy Transmission Line .............. 564
31.4.5 URC - Uniform R. C. line ........................ 565
31.5 BJTs ........................................ 566
31.5.1 BJT - Bipolar Junction Transistor .................... 566
31.5.2 BJT - Bipolar Junction Transistor Level 2 ................ 569
31.5.3 VBIC - Vertical Bipolar Inter-Company Model ............. 572
31.6 MOSFETs ..................................... 576
31.6.1 MOS1 - Level 1 MOSFET model with Meyer capacitance model . . . . 576
31.6.2 MOS2 - Level 2 MOSFET model with Meyer capacitance model . . . . 579
26 CONTENTS
31.6.3 MOS3 - Level 3 MOSFET model with Meyer capacitance model . . . 583
31.6.4 MOS6 - Level 6 MOSFET model with Meyer capacitance model . . . 587
31.6.5 MOS9 - Modified Level 3 MOSFET model ............... 590
31.6.6 BSIM1 - Berkeley Short Channel IGFET Model ............ 594
31.6.7 BSIM2 - Berkeley Short Channel IGFET Model ............ 597
31.6.8 BSIM3 .................................. 601
31.6.9 BSIM4 .................................. 602
32 Compilation notes 605
32.1 Ngspice Installation under Linux (and other ’UNIXes’) ............. 605
32.1.1 Prerequisites ............................... 605
32.1.2 Install from Git .............................. 605
32.1.3 Install from a tarball, e.g. ngspice-rework-27.tgz ............ 607
32.1.4 Compilation using an user defined directory tree for object files . . . . 607
32.1.5 Advanced Install ............................. 607
32.1.6 Compilers and Options .......................... 609
32.1.7 Compiling For Multiple Architectures .................. 610
32.1.8 Installation Names ............................ 610
32.1.9 Optional Features ............................. 610
32.1.10 Specifying the System Type ....................... 611
32.1.11 Sharing Defaults ............................. 611
32.1.12 Operation Controls ............................ 611
32.2 Ngspice Compilation under Windows OS .................... 612
32.2.1 Compile ngspice with MS Visual Studio 2015 or 2017 ......... 612
32.2.2 How to make ngspice with MINGW and MSYS ............ 614
32.2.3 64 Bit executables with MINGW-w64 .................. 616
32.2.4 make ngspice with pure CYGWIN .................... 618
32.2.5 ngspice mingw or cygwin console executable w/o graphics ....... 618
32.2.6 ngspice for MS Windows, cross compiled from Linux ......... 618
32.2.7 make ngspice with CYGWIN and external MINGW32 ......... 619
32.2.8 make ngspice with CYGWIN and internal MINGW32 (use config.h
made above) ............................... 619
32.3 Reporting errors .................................. 619
CONTENTS 27
33 Copyrights and licenses 621
33.1 Documentation license .............................. 621
33.1.1 Spice documentation copyright ...................... 621
33.1.2 XSPICE SOFTWARE (documentation) copyright ............ 621
33.1.3 CIDER RESEARCH SOFTWARE AGREEMENT (superseded by 33.2.1)622
33.2 ngspice license .................................. 622
33.2.1 ‘Modified’ BSD license ......................... 623
33.2.2 XSPICE .................................. 624
33.2.3 tclspice, numparam ............................ 624
33.2.4 Linking to GPLd libraries (e.g. readline, fftw, table.cm): ........ 624
28 CONTENTS
Prefaces
Preface to the first edition
This manual has been assembled from different sources:
1. The spice3f5 manual,
2. the XSPICE user’s manual,
3. the CIDER user’s manual
and some original material needed to describe the new features and the newly implemented
models. This cut and paste approach, while not being orthodox, allowed ngspice to have a full
manual in a fraction of the time that writing a completely new text would have required. The use
of LaTex and Lyx instead of TeXinfo, which was the original encoding for the manual, further
helped to reduce the writing effort and improved the quality of the result, at the expense of an
on-line version of the manual but, due to the complexity of the software I hardly think that users
will ever want to read an on-line text version.
In writing this text I followed the spice3f5 manual, both in the chapter sequence and presentation
of material, mostly because that was already the user manual of SPICE.
Ngspice is an open source software, users can download the source code, compile, and run it.
This manual has an entire chapter describing program compilation and available options to help
users in building ngspice (see Chapt. 32). The source package already comes with all ‘safe’
options enabled by default, and activating the others can produce unpredictable results and thus
is recommended to expert users only. This is the first ngspice manual and I have removed all
the historical material that described the differences between ngspice and spice3, since it was
of no use for the user and not so useful for the developer who can look for it in the Changelogs
of in the revision control system.
I want to acknowledge the work done by Emmanuel Rouat and Arno W. Peters for converting the
original spice3f documentation to T
E
Xinfo. Their effort gave ngspice users the only available
documentation that described the changes for many years. A good source of ideas for this
manual came from the on-line spice3f manual written by Charles D.H. Williams (Spice3f5
User Guide), constantly updated and useful for its many insights.
As always, errors, omissions and unreadable phrases are only my fault.
Paolo Nenzi
Roma, March 24th 2001
29
30 CONTENTS
Indeed. At the end of the day, this is engineering, and one learns to live
within the limitations of the tools.
Kevin Aylward, Warden of the King’s Ale
Preface to the actual edition (as of January 2013)
Due to the wealth of new material and options in ngspice the actual order of chapters has been
revised. Several new chapters have been added. The L
Y
X text processor has allowed adding
internal cross references. The PDF format has become the standard format for distribution of
the manual. Within each new ngspice distribution (starting with ngspice-21) a manual edition
is provided reflecting the ngspice status at the time of distribution. At the same time, located
at ngspice manuals, the manual is constantly updated. Every new ngspice feature should enter
this manual as soon as it has been made available in the Git source code.
Holger Vogt
Mülheim, 2013
Acknowledgments
ngspice contributors
Spice was originally written at The University of California at Berkeley (USA).
XSPICE has been provided by Georgia Institute of Technology, Atlanta (USA).
Since then, there have been many people working on the software, most of them releasing
patches to the original code through the Internet.
The following people have contributed in some way:
Vera Albrecht,
Cecil Aswell,
Giles C. Billingsley,
Phil Barker,
Steven Borley,
Stuart Brorson,
Mansun Chan,
Wayne A. Christopher,
Al Davis,
Glao S. Dezai,
Jon Engelbert,
Daniele Foci,
Noah Friedman,
David A. Gates,
Alan Gillespie,
John Heidemann,
Marcel Hendrix,
Jeffrey M. Hsu,
JianHui Huang,
S. Hwang,
Chris Inbody,
Gordon M. Jacobs,
Min-Chie Jeng,
Beorn Johnson,
Stefan Jones,
Kenneth H. Keller,
Francesco Lannutti,
Robert Larice,
31
32 CONTENTS
Mathew Lew,
Robert Lindsell,
Weidong Liu,
Kartikeya Mayaram,
Richard D. McRoberts,
Manfred Metzger,
Wolfgang Muees,
Paolo Nenzi,
Gary W. Ng,
Hong June Park,
Stefano Perticaroli,
Arno Peters,
Serban-Mihai Popescu,
Georg Post,
Thomas L. Quarles,
Emmanuel Rouat,
Jean-Marc Routure,
Jaijeet S. Roychowdhury,
Lionel Sainte Cluque,
Takayasu Sakurai,
Amakawa Shuhei,
Kanwar Jit Singh,
Bill Swartz,
Hitoshi Tanaka,
Steve Tell,
Andrew Tuckey,
Andreas Unger,
Holger Vogt,
Dietmar Warning,
Michael Widlok,
Charles D.H. Williams,
Antony Wilson,
and many others...
If someone helped in the development and has not been inserted in this list then this omis-
sion was unintentional. If you feel you should be on this list then please write to <ngspice-
devel@lists.sourceforge.net>. Do not be shy, we would like to make a list as complete as
possible.
XSPICE
The XSPICE simulator, developed at Georgia Tech., is based on the SPICE3 program developed
by the Electronics Research Laboratory, Department of Electrical Engineering and Computer
Sciences, University of California at Berkeley. The authors of XSPICE gratefully acknowledge
UC Berkeley’s development and distribution of this software, and their licensing policies which
promote further improvements to simulation technology. They also gratefully acknowledge the
CONTENTS 33
participation and support of their U.S. Air Force sponsors, the Aeronautical Systems Center and
the Warner Robins Air Logistics Command, without which the development of XSPICE would
not have been possible.
34 CONTENTS
Chapter 1
Introduction
Ngspice is a general-purpose circuit simulation program for nonlinear and linear analyses. Ci-
rcuits may contain resistors, capacitors, inductors, mutual inductors, independent or dependent
voltage and current sources, loss-less and lossy transmission lines, switches, uniform distributed
RC lines, and the five most common semiconductor devices: diodes, BJTs, JFETs, MESFETs,
and MOSFETs.
Some introductory remarks on how to use ngspice may be found in Chapt. 21.
Ngspice is an update of Spice3f5, the last Berkeley’s release of Spice3 simulator family. Ng-
spice is being developed to include new features to existing Spice3f5 and to fix its bugs. Im-
proving a complex software like a circuit simulator is a very hard task and, while some impro-
vements have been made, most of the work has been done on bug fixing and code refactoring.
Ngspice has built-in models for the semiconductor devices, and the user need specify only the
pertinent model parameter values. There are three models for bipolar junction transistors, all
based on the integral-charge model of Gummel and Poon; however, if the Gummel-Poon pa-
rameters are not specified, the basic model (BJT) reduces to the simpler Ebers-Moll model.
In either case and in either models, charge storage effects, ohmic resistances, and a current-
dependent output conductance may be included. The second bipolar model BJT2 adds dc cur-
rent computation in the substrate diode. The third model (VBIC) contains further enhancements
for advanced bipolar devices.
The semiconductor diode model can be used for either junction diodes or Schottky barrier di-
odes. There are two models for JFET: the first (JFET) is based on the model of Shichman and
Hodges, the second (JFET2) is based on the Parker-Skellern model. All the original six MOS-
FET models are implemented: MOS1 is described by a square-law I-V characteristic, MOS2 [1]
is an analytical model, while MOS3 [1] is a semi-empirical model; MOS6 [2] is a simple analy-
tic model accurate in the short channel region; MOS9, is a slightly modified Level 3 MOSFET
model - not to confuse with Philips level 9; BSIM 1 [3, 4]; BSIM2 [5] are the old BSIM (Ber-
keley Short-channel IGFET Model) models. MOS2, MOS3, and BSIM include second-order
effects such as channel-length modulation, subthreshold conduction, scattering-limited velocity
saturation, small-size effects, and charge controlled capacitances. The recent MOS models for
submicron devices are the BSIM3 (Berkeley BSIM3 web page) and BSIM4 (Berkeley BSIM4
web page) models. Silicon-on-insulator MOS transistors are described by the SOI models from
the BSIMSOI family (Berkeley BSIMSOI web page) and the STAG [18] one. There is partial
support for a couple of HFET models and one model for MESA devices.
35
36 CHAPTER 1. INTRODUCTION
Ngspice supports mixed-level simulation and provides a direct link between technology para-
meters and circuit performance. A mixed-level circuit and device simulator can provide greater
simulation accuracy than a stand-alone circuit or device simulator by numerically modeling the
critical devices in a circuit. Compact models can be used for noncritical devices. The mixed-
level extensions to ngspice are two:
• CIDER: a mixed-level circuit and device simulator integrated into ngspice code. CIDER
was originally the name of the mixed-level extension made to spice3f5.
• GSS: GSS (now called GENIUS) TCAD is a 2D simulator developed independently from
ngspice. The device simulator itself is free and not included into ngspice, but a socket
interface is provided.
Ngspice supports mixed-signal simulation through the integration of XSPICE code into it.
XSPICE software, developed as an extension to Spice3C1 from GeorgiaTech, has been por-
ted to ngspice to provide ‘board’ level and mixed-signal simulation.
New devices can be added to ngspice by two means: the XSPICE code-model interface and the
ADMS interface based on Verilog-A and XML.
Finally, numerous small bugs have been discovered and fixed, and the program has been ported
to a wider variety of computing platforms.
1.1 Simulation Algorithms
Computer-based circuit simulation is often used as a tool by designers, test engineers, and
others who want to analyze the operation of a design without examining the physical circuit.
Simulation allows you to change quickly the parameters of many of the circuit elements to
determine how they affect the circuit response. Often it is difficult or impossible to change
these parameters in a physical circuit.
However, to be practical, a simulator must execute in a reasonable amount of time. The key to
efficient execution is choosing the proper level of modeling abstraction for a given problem. To
support a given modeling abstraction, the simulator must provide appropriate algorithms.
Historically, circuit simulators have supported either an analog simulation algorithm or a digital
simulation algorithm. Ngspice inherits the XSPICE framework and supports both analog and
digital algorithms and is a ‘mixed-mode’ simulator.
1.1.1 Analog Simulation
Analog simulation focuses on the linear and non-linear behavior of a circuit over a continuous
time or frequency interval. The circuit response is obtained by iteratively solving Kirchhoff’s
Laws for the circuit at time steps selected to ensure the solution has converged to a stable value
and that numerical approximations of integrations are sufficiently accurate. Since Kirchhoff’s
laws form a set of simultaneous equations, the simulator operates by solving a matrix of equa-
tions at each time point. This matrix processing generally results in slower simulation times
when compared to digital circuit simulators.
1.1. SIMULATION ALGORITHMS 37
The response of a circuit is a function of the applied sources. Ngspice offers a variety of
source types including DC, sine-wave, and pulse. In addition to specifying sources, the user
must define the type of simulation to be run. This is termed the ‘mode of analysis’. Analysis
modes include DC analysis, AC analysis, and transient analysis. For DC analysis, the time-
varying behavior of reactive elements is neglected and the simulator calculates the DC solution
of the circuit. Swept DC analysis may also be accomplished with ngspice. This is simply the
repeated application of DC analysis over a range of DC levels for the input sources. For AC
analysis, the simulator determines the response of the circuit, including reactive elements to
small-signal sinusoidal inputs over a range of frequencies. The simulator output in this case
includes amplitudes and phases as a function of frequency. For transient analysis, the circuit
response, including reactive elements, is analyzed to calculate the behavior of the circuit as a
function of time.
1.1.2 Digital Simulation
Digital circuit simulation differs from analog circuit simulation in several respects. A primary
difference is that a solution of Kirchhoff’s laws is not required. Instead, the simulator must only
determine whether a change in the logic state of a node has occurred and propagate this change
to connected elements. Such a change is called an ‘event’.
When an event occurs, the simulator examines only those circuit elements that are affected by
the event. As a result, matrix analysis is not required in digital simulators. By comparison,
analog simulators must iteratively solve for the behavior of the entire circuit because of the
forward and reverse transmission properties of analog components. This difference results in
a considerable computational advantage for digital circuit simulators, which is reflected in the
significantly greater speed of digital simulations.
1.1.3 Mixed-Mode Simulation
Modern circuits often contain a mix of analog and digital circuits. To simulate such circuits
efficiently and accurately a mix of analog and digital simulation techniques is required. When
analog simulation algorithms are combined with digital simulation algorithms, the result is
termed ‘mixed-mode simulation’.
Two basic methods of implementing mixed-mode simulation used in practice are the ‘native
mode’ and ‘glued mode’ approaches. Native mode simulators implement both an analog algo-
rithm and a digital algorithm in the same executable. Glued mode simulators actually use two
simulators, one of which is analog and the other digital. This type of simulator must define an
input/output protocol so that the two executables can communicate with each other effectively.
The communication constraints tend to reduce the speed, and sometimes the accuracy, of the
complete simulator. On the other hand, the use of a glued mode simulator allows the component
models developed for the separate executables to be used without modification.
Ngspice is a native mode simulator providing both analog and event-based simulation in the
same executable. The underlying algorithms of ngspice (coming from XSPICE and its Code
Model Subsystem) allow use of all the standard SPICE models, provide a pre-defined collection
of the most common analog and digital functions, and provide an extensible base on which to
build additional models.
38 CHAPTER 1. INTRODUCTION
1.1.3.1 User-Defined Nodes
Ngspice supports creation of ‘User-Defined Node’ types. User-Defined Node types allow you
to specify nodes that propagate data other than voltages, currents, and digital states. Like digital
nodes, User-Defined Nodes use event-driven simulation, but the state value may be an arbitrary
data type. A simple example application of User-Defined Nodes is the simulation of a digital
signal processing filter algorithm. In this application, each node could assume a real or integer
value. More complex applications may define types that involve complex data such as digital
data vectors or even non-electronic data.
Ngspice digital simulation is actually implemented as a special case of this User-Defined Node
capability where the digital state is defined by a data structure that holds a Boolean logic state
and a strength value.
1.1.4 Mixed-Level Simulation
Ngspice can simulate numerical device models for diodes and transistors in two different ways,
either through the integrated DSIM simulator or interfacing to GSS TCAD system. DSIM is an
internal C-based device simulator that is part of the CIDER simulator, the mixed-level simulator
based on SPICE3f5. CIDER within ngspice provides circuit analyses, compact models for
semiconductor devices, and one- or two-dimensional numerical device models.
1.1.4.1 CIDER (DSIM)
DSIM provides accurate, one- and two-dimensional numerical device models based on the so-
lution of Poisson’s equation, and the electron and hole current-continuity equations. DSIM
incorporates many of the same basic physical models found in the Stanford two-dimensional
device simulator PISCES. Input to CIDER consists of a SPICE-like description of the circuit
and its compact models, and PISCES-like descriptions of the structures of numerically modeled
devices. As a result, CIDER should seem familiar to designers already accustomed to these
two tools. CIDER is based on the mixed-level circuit and device simulator CODECS, and is a
replacement for this program. The basic algorithms of the two programs are the same. Some of
the differences between CIDER and CODECS are described below. The CIDER input format
has greater flexibility and allows increased access to physical model parameters. New physical
models have been added to allow simulation of state-of-the-art devices. These include trans-
verse field mobility degradation important in scaled-down MOSFETs and a polysilicon model
for poly-emitter bipolar transistors. Temperature dependence has been included over the range
from -50C to 150C. The numerical models can be used to simulate all the basic types of se-
miconductor devices: resistors, MOS capacitors, diodes, BJTs, JFETs and MOSFETs. BJTs
and JFETs can be modeled with or without a substrate contact. Support has been added for the
management of device internal states. Post-processing of device states can be performed using
the ngnutmeg user interface.
1.1.4.2 GSS TCAD
GSS is a TCAD software that enables two-dimensional numerical simulation of semiconductor
device with well-known drift-diffusion and hydrodynamic method. GSS has Basic DDM (drift-
diffusion method) solver, Lattice Temperature Corrected DDM solver, EBM (energy balance
1.2. SUPPORTED ANALYSES 39
method) solver and Quantum corrected DDM solver based on density-gradient theory. The GSS
program is directed via input statements by a user specified disk file. Supports triangle mesh
generation and adaptive mesh refinement. Employs PMI (physical model interface) to support
various materials, including compound semiconductor materials such as SiGe and AlGaAs.
Supports DC sweep, transient and AC sweep calculations. The device can be stimulated by
voltage or current source(s).
GSS is no longer updated, but is still available as open source as a limited edition of the com-
mercial GENIUS TCAD tool.
1.2 Supported Analyses
The ngspice simulator supports the following different types of analysis:
1. DC Analysis (Operating Point and DC Sweep)
2. AC Small-Signal Analysis
3. Transient Analysis
4. Pole-Zero Analysis
5. Small-Signal Distortion Analysis
6. Sensitivity Analysis
7. Noise Analysis
Applications that are exclusively analog can make use of all analysis modes with the exception
of Code Model subsystem that do not implements Pole-Zero, Distortion, Sensitivity and Noise
analyses. Event-driven applications that include digital and User-Defined Node types may make
use of DC (operating point and DC sweep) and Transient only.
In order to understand the relationship between the different analyses and the two underlying
simulation algorithms of ngspice, it is important to understand what is meant by each analysis
type. This is detailed below.
1.2.1 DC Analyses
The dc analysis portion of ngspice determines the dc operating point of the circuit with inductors
shorted and capacitors opened. The dc analysis options are specified on the .DC,.TF, and .OP
control lines.
There is assumed to be no time dependence on any of the sources within the system description.
The simulator algorithm subdivides the circuit into those portions that require the analog simu-
lator algorithm and such that require the event-driven algorithm. Each subsystem block is then
iterated to solution, with the interfaces between analog nodes and event-driven nodes iterated
for consistency across the entire system.
Once stable values are obtained for all nodes in the system, the analysis halts and the results
may be displayed or printed out as you request them.
40 CHAPTER 1. INTRODUCTION
A dc analysis is automatically performed prior to a transient analysis to determine the transient
initial conditions, and prior to an ac small-signal analysis to determine the linearized, small-
signal models for nonlinear devices. If requested, the dc small-signal value of a transfer function
(ratio of output variable to input source), input resistance, and output resistance is also computed
as a part of the dc solution. The dc analysis can also be used to generate dc transfer curves: a
specified independent voltage, current source, resistor or temperature1is stepped over a user-
specified range and the dc output variables are stored for each sequential source value.
1.2.2 AC Small-Signal Analysis
AC analysis is limited to analog nodes and represents the small signal, sinusoidal solution of the
analog system described at a particular frequency or set of frequencies. This analysis is similar
to the DC analysis in that it represents the steady-state behavior of the described system with a
single input node at a given set of stimulus frequencies.
The program first computes the dc operating point of the circuit and determines linearized,
small-signal models for all of the nonlinear devices in the circuit. The resultant linear circuit
is then analyzed over a user-specified range of frequencies. The desired output of an ac small-
signal analysis is usually a transfer function (voltage gain, transimpedance, etc). If the circuit
has only one ac input, it is convenient to set that input to unity and zero phase, so that output
variables have the same value as the transfer function of the output variable with respect to the
input.
1.2.3 Transient Analysis
Transient analysis is an extension of DC analysis to the time domain. A transient analysis be-
gins by obtaining a DC solution to provide a point of departure for simulating time-varying
behavior. Once the DC solution is obtained, the time-dependent aspects of the system are rein-
troduced, and the two simulator algorithms incrementally solve for the time varying behavior of
the entire system. Inconsistencies in node values are resolved by the two simulation algorithms
such that the time-dependent waveforms created by the analysis are consistent across the entire
simulated time interval. Resulting time-varying descriptions of node behavior for the specified
time interval are accessible to you.
All sources that are not time dependent (for example, power supplies) are set to their dc value.
The transient time interval is specified on a .TRAN control line.
1.2.4 Pole-Zero Analysis
The pole-zero analysis portion of Ngspice computes the poles and/or zeros in the small-signal
ac transfer function. The program first computes the dc operating point and then determines
the linearized, small-signal models for all the nonlinear devices in the circuit. This circuit is
then used to find the poles and zeros of the transfer function. Two types of transfer functions
are allowed: one of the form (output voltage)/(input voltage) and the other of the form (output
voltage)/(input current). These two types of transfer functions cover all the cases and one can
1Temperature (TEMP) and resistance sweeps have been introduced in Ngspice, they were not available in the
original code of Spice3f5.
1.2. SUPPORTED ANALYSES 41
find the poles/zeros of functions like input/output impedance and voltage gain. The input and
output ports are specified as two pairs of nodes. The pole-zero analysis works with resistors,
capacitors, inductors, linear-controlled sources, independent sources, BJTs, MOSFETs, JFETs
and diodes. Transmission lines are not supported. The method used in the analysis is a sub-
optimal numerical search. For large circuits it may take a considerable time or fail to find all
poles and zeros. For some circuits, the method becomes ‘lost’ and finds an excessive number
of poles or zeros.
1.2.5 Small-Signal Distortion Analysis
The distortion analysis portion of Ngspice computes steady-state harmonic and intermodulation
products for small input signal magnitudes. If signals of a single frequency are specified as the
input to the circuit, the complex values of the second and third harmonics are determined at
every point in the circuit. If there are signals of two frequencies input to the circuit, the analysis
finds out the complex values of the circuit variables at the sum and difference of the input
frequencies, and at the difference of the smaller frequency from the second harmonic of the
larger frequency. Distortion analysis is supported for the following nonlinear devices:
• Diodes (DIO),
• BJT,
• JFET (level 1),
• MOSFETs (levels 1, 2, 3, 9, and BSIM1),
• MESFET (level 1).
All linear devices are automatically supported by distortion analysis. If there are switches
present in the circuit, the analysis continues to be accurate provided the switches do not change
state under the small excitations used for distortion calculations.
If a device model does not support direct small signal distortion analysis, please use the Fourier
statement and evaluate the output per scripting.
1.2.6 Sensitivity Analysis
Ngspice will calculate either the DC operating-point sensitivity or the AC small-signal sen-
sitivity of an output variable with respect to all circuit variables, including model parameters.
Ngspice calculates the difference in an output variable (either a node voltage or a branch current)
by perturbing each parameter of each device independently. Since the method is a numerical
approximation, the results may demonstrate second order effects in highly sensitive parameters,
or may fail to show very low but non-zero sensitivity. Further, since each variable is perturb
by a small fraction of its value, zero-valued parameters are not analyzed (this has the benefit of
reducing what is usually a very large amount of data).
42 CHAPTER 1. INTRODUCTION
1.2.7 Noise Analysis
The noise analysis portion of Ngspice gives the device-generated noise for a given circuit. When
provided with an input source and an output port, the analysis calculates the noise contributions
of each device, and each noise generator within the device, to the output port voltage. It also
calculates the equivalent input noise of the circuit, based on the output noise. This is done for
every frequency point in a specified range - the calculated value of the noise corresponds to
the spectral density of the circuit variable viewed as a stationary Gaussian stochastic process.
After calculating the spectral densities, noise analysis integrates these values over the speci-
fied frequency range to arrive at the total noise voltage and current over this frequency range.
The calculated values correspond to the variance of the circuit variables viewed as stationary
Gaussian processes.
1.2.8 Periodic Steady State Analysis
Experimental code, not yet made publicly available.
PSS is a radio frequency periodical large-signal dedicated analysis. The implementation is
based on a time domain shooting method that make use of transient analysis. As it is in early
development stage, PSS performs analysis only on autonomous circuits, meaning that it is able
to predict fundamental frequency and (harmonic) amplitude(s) for oscillators, VCOs, etc.. The
algorithm is based on a search of the minimum error vector defined as the difference of RHS
vectors between two occurrences of an estimated period. Convergence is reached when the
mean of this error vector decreases below a given threshold parameter. Results of PSS are the
basis of periodical large-signal analyses like PAC or PNoise.
1.3 Analysis at Different Temperatures
Temperature, in ngspice, is a property associated to the entire circuit, rather than an analysis op-
tion. Circuit temperature has a default (nominal) value of 27°C (300.15 K) that can be changed
using the TEMP option in an .option control line (see 15.1.1) or by the .TEMP line (see 2.11),
which has precedence over the .option TEMP line. All analyses are, thus, performed at circuit
temperature, and if you want to simulate circuit behavior at different temperatures you should
prepare a netlist for each temperature.
All input data for ngspice is assumed to have been measured at the circuit nominal temperature.
This value can further be overridden for any device that models temperature effects by speci-
fying the TNOM parameter on the .model itself. Individual instances may further override the
circuit temperature through the specification of TEMP and DTEMP parameters on the instance.
The two options are not independent even if you can specify both on the instance line, the TEMP
option overrides DTEMP. The algorithm to compute instance temperature is described below:
IF TEMP is specified THEN
instance_temperature = TEMP
ELSE IF
instance_temperature = circuit_temperature + DTEMP
END IF
Algorithm 1: Instance temperature computation
1.3. ANALYSIS AT DIFFERENT TEMPERATURES 43
Temperature dependent support is provided for all devices except voltage and current sources
(either independent and controlled) and BSIM models. BSIM MOSFETs have an alternate
temperature dependency scheme that adjusts all of the model parameters before input to ngspice.
For details of the BSIM temperature adjustment, see [6] and [7]. Temperature appears explicitly
in the exponential terms of the BJT and diode model equations. In addition, saturation currents
have a built-in temperature dependence. The temperature dependence of the saturation current
in the BJT models is determined by:
IS(T1) = IS(T0)T1
T0XT I
expEgq(T1T0)
k(T1−T0)(1.1)
where kis Boltzmann’s constant, qis the electronic charge, Egis the energy gap model pa-
rameter, and XT I is the saturation current temperature exponent (also a model parameter, and
usually equal to 3).
The temperature dependence of forward and reverse beta is according to the formula:
B(T1) = B(T0)T1
T0XT B
(1.2)
where T0and T1are in degrees Kelvin, and X T B is a user-supplied model parameter. Tempera-
ture effects on beta are carried out by appropriate adjustment to the values of BF,ISE ,BR, and
ISC (SPICE model parameters BF, ISE, BR, and ISC, respectively).
Temperature dependence of the saturation current in the junction diode model is determined by:
IS(T1) = IS(T0)T1
T0X T I
N
expEgq(T1T0)
Nk (T1−T0)(1.3)
where Nis the emission coefficient model parameter, and the other symbols have the same
meaning as above. Note that for Schottky barrier diodes, the value of the saturation current
temperature exponent, XT I, is usually 2. Temperature appears explicitly in the value of junction
potential, U (in Ngspice PHI), for all the device models.
The temperature dependence is determined by:
U(T) = kT
qln NaNd
Ni(T)2!(1.4)
where kis Boltzmann’s constant, qis the electronic charge, Nais the acceptor impurity den-
sity, Ndis the donor impurity density, Niis the intrinsic carrier concentration, and Egis the
energy gap. Temperature appears explicitly in the value of surface mobility, M0(or U0), for the
MOSFET model.
The temperature dependence is determined by:
M0(T) = M0(T0)
T
T01.5(1.5)
44 CHAPTER 1. INTRODUCTION
The effects of temperature on resistors, capacitor and inductors is modeled by the formula:
R(T) = R(T0)h1+TC1(T−T0) + TC2(T−T0)2i(1.6)
where Tis the circuit temperature, T0is the nominal temperature, and TC1and TC2are the first
and second order temperature coefficients.
1.4 Convergence
Ngspice uses the Newton-Raphson algorithm to solve nonlinear equations arising from circuit
description. The NR algorithm is interactive and terminates when both of the following condi-
tions hold:
1. The nonlinear branch currents converge to within a tolerance of 0.1% or 1 picoamp (1.0e-
12 Amp), whichever is larger.
2. The node voltages converge to within a tolerance of 0.1% or 1 microvolt (1.0e-6 Volt),
whichever is larger.
1.4.1 Voltage convergence criterion
The algorithm has reached convergence when the difference between the last iteration kand the
current one (k+1)
v(k+1)
n−v(k)
n≤RELTOL vnmax +VNTOL,(1.7)
where
vnmax =maxv(k+1)
n,v(k)
n.(1.8)
The RELTOL (RELative TOLerance) parameter, which default value is 10−3, specifies how small
the solution update must be, relative to the node voltage, to consider the solution to have conver-
ged. The VNTOL (absolute convergence) parameter, which has 1µVas default value, becomes
important when node voltages have near zero values. The relative parameter alone, in such
case, would need too strict tolerances, perhaps lower than computer round-off error, and thus
convergence would never be achieved. VNTOL forces the algorithm to consider as converged any
node whose solution update is lower than its value.
1.4.2 Current convergence criterion
Ngspice checks the convergence on the non-linear functions that describe the non-linear bran-
ches in circuit elements. In semiconductor devices the functions defines currents through the
device and thus the name of the criterion.
1.4. CONVERGENCE 45
Ngspice computes the difference between the value of the nonlinear function computed for the
last voltage and the linear approximation of the same current computed with the actual voltage
\
i(k+1)
branch −i(k)
branch≤RELTOL ibrmax +ABSTOL,(1.9)
where
ibrmax =max\
i(k+1)
branch,i(k)
branch.(1.10)
In the two expressions above, the
\
ibranch indicates the linear approximation of the current.
1.4.3 Convergence failure
Although the algorithm used in ngspice has been found to be very reliable, in some cases it fails
to converge to a solution. When this failure occurs, the program terminates the job. Failure
to converge in dc analysis is usually due to an error in specifying circuit connections, element
values, or model parameter values. Regenerative switching circuits or circuits with positive
feedback probably will not converge in the dc analysis unless the OFF option is used for some
of the devices in the feedback path, .nodeset control line is used to force the circuit to converge
to the desired state.
46 CHAPTER 1. INTRODUCTION
Chapter 2
Circuit Description
2.1 General Structure and Conventions
2.1.1 Input file structure
The circuit to be analyzed is described to ngspice by a set of element instance lines, which
define the circuit topology and element instance values, and a set of control lines, which define
the model parameters and the run controls. All lines are assembled in an input file to be read by
ngspice. Two lines are essential:
• The first line in the input file must be the title, which is the only comment line that does
not need any special character in the first place.
• The last line must be .end.
The order of the remaining lines is arbitrary (except, of course, that continuation lines must
immediately follow the line being continued). This feature in the ngspice input language da-
tes back to the punched card times where elements were written on separate cards (and cards
frequently fell off). Leading white spaces in a line are ignored, as well as empty lines.
The lines decribed in sections 2.1 to 2.12 are typically used in the core of the input file, outside
of a .control section (see 16.4.3). An exception is the .include includefile line (2.6)
that may be placed anywhere in the input file. The contents of includefile will be inserted
exactly in place of the .include line.
2.1.2 Circuit elements (device instances)
Each element in the circuit is a device instance specified by an instance line that contains:
• the element instance name,
• the circuit nodes to which the element is connected,
• and the values of the parameters that determine the electrical characteristics of the ele-
ment.
47
48 CHAPTER 2. CIRCUIT DESCRIPTION
The first letter of the element instance name specifies the element type. The format for the
ngspice element types is given in the following manual chapters. In the rest of the manual, the
strings XXXXXXX,YYYYYYY, and ZZZZZZZ denote arbitrary alphanumeric strings.
For example, a resistor instance name must begin with the letter Rand can contain one or more
characters. Hence, R,R1,RSE,ROUT, and R3AC2ZY are valid resistor names. Details of each
type of device are supplied in a following section 3. Table 2.1 lists the element types available
in ngspice, sorted by their first letter.
First letter Element description Comments, links
A XSPICE code model
12
analog (12.2)
digital (12.4)
mixed signal (12.3)
B Behavioral (arbitrary) source 5.1
C Capacitor 3.2.5
D Diode 7
E Voltage-controlled voltage source (VCVS) linear (4.2.2),
non-linear (5.2)
F Current-controlled current source (CCCs) linear (4.2.3)
G Voltage-controlled current source (VCCS) linear (4.2.1),
non-linear (5.3)
H Current-controlled voltage source (CCVS) linear (4.2.4)
I Current source 4.1
J Junction field effect transistor (JFET) 9
K Coupled (Mutual) Inductors 3.2.11
L Inductor 3.2.9
M Metal oxide field effect transistor (MOSFET)
11
BSIM3 (11.2.9)
BSIM4 (11.2.10)
N Numerical device for GSS 14.2
O Lossy transmission line 6.2
P Coupled multiconductor line (CPL) 6.4.2
Q Bipolar junction transistor (BJT) 8
R Resistor 3.2.1
S Switch (voltage-controlled) 3.2.14
T Lossless transmission line 6.1
U Uniformly distributed RC line 6.3
V Voltage source 4.1
W Switch (current-controlled) 3.2.14
X Subcircuit 2.4.3
Y Single lossy transmission line (TXL) 6.4.1
Z Metal semiconductor field effect transistor (MESFET) 10
Table 2.1: ngspice element types
2.1. GENERAL STRUCTURE AND CONVENTIONS 49
2.1.3 Some naming conventions
Fields on a line are separated by one or more blanks, a comma, an equal (=) sign, or a left or
right parenthesis; extra spaces are ignored. A line may be continued by entering a ‘+’ (plus) in
column 1 of the following line; ngspice continues reading beginning with column 2. A name
field must begin with a letter (A through Z) and cannot contain any delimiters. A number field
may be an integer field (12, -44), a floating point field (3.14159), either an integer or floating
point number followed by an integer exponent (1e-14, 2.65e3), or either an integer or a floating
point number followed by one of the following scale factors:
Suffix Name Factor
T Tera 1012
G Giga 109
Meg Mega 106
K Kilo 103
mil Mil 25.4×10−6
m milli 10−3
u micro 10−6
n nano 10−9
p pico 10−12
f femto 10−15
Table 2.2: Ngspice scale factors
Letters immediately following a number that are not scale factors are ignored, and letters im-
mediately following a scale factor are ignored. Hence, 10, 10V, 10Volts, and 10Hz all represent
the same number, and M, MA, MSec, and MMhos all represent the same scale factor. Note that
1000, 1000.0, 1000Hz, 1e3, 1.0e3, 1kHz, and 1k all represent the same number. Note that ‘M’
or ‘m’ denote ‘milli’, i.e. 10−3. Suffix meg has to be used for 106.
Nodes names may be arbitrary character strings and are case insensitive, if ngspice is used in
batch mode (16.4.1). If in interactive (16.4.2) or control (16.4.3) mode, node names may either
be plain numbers or arbitrary character strings, not starting with a number. The ground node
must be named ‘0’ (zero). For compatibility reason gnd is accepted as ground node, and will
internally be treated as a global node and be converted to ‘0’. Each circuit has to have a ground
node (gnd or 0)! Note the difference in ngspice where the nodes are treated as character strings
and not evaluated as numbers, thus ‘0’ and 00 are distinct nodes in ngspice but not in SPICE2.
Ngspice requires that the following topological constraints are satisfied:
• The circuit cannot contain a loop of voltage sources and/or inductors and cannot contain
a cut-set of current sources and/or capacitors.
• Each node in the circuit must have a dc path to ground.
• Every node must have at least two connections except for transmission line nodes (to
permit unterminated transmission lines) and MOSFET substrate nodes (which have two
internal connections anyway).
50 CHAPTER 2. CIRCUIT DESCRIPTION
2.2 Basic lines
2.2.1 .TITLE line
Examples:
POWER AMPLIFIER CIRCUIT
* additional lines following
*...
Test of CAM cell
* additional lines following
*...
The title line must be the first in the input file. Its contents are printed verbatim as the heading
for each section of output.
As an alternative you may place a .TITLE <any title> line anywhere in your input deck.
The first line of your input deck will be overridden by the contents of this line following the
.TITLE statement.
.TITLE line example:
******************************
* additional lines following
*...
.TITLE Test of CAM cell
* additional lines following
*...
will internally be replaced by
Internal input deck:
Test of CAM cell
* additional lines following
*...
*TITLE Test of CAM cell
* additional lines following
*...
2.2.2 .END Line
Examples:
.end
The .end line must always be the last in the input file. Note that the period is an integral part
of the name.
2.3. .MODEL DEVICE MODELS 51
2.2.3 Comments
General Form:
* <any comment >
Examples:
* RF=1K Gain should be 100
* Check open - loop gain and phase margin
The asterisk in the first column indicates that this line is a comment line. Comment lines may
be placed anywhere in the circuit description.
2.2.4 End-of-line comments
General Form:
<any command > $ <any comment >
Examples:
RF2 =1K $ Gain should be 100
C1=10p $ Check open - loop gain and phase margin
.param n1 =1 // new value
ngspice supports comments that begin with double characters ‘$’ (dollar plus space) or ‘//’.
For readability you should precede each comment character with a space. ngspice will accept
the single character ‘$’.
Please note that in .control sections the ‘;’ character means ‘continuation’ and can be used
to put more than one statement on a line.
2.3 .MODEL Device Models
General form:
.model mname type( pname1 =pval1 pname2 = pval2 ... )
Examples:
. model MOD1 npn (bf =50 is =1e -13 vbf =50)
52 CHAPTER 2. CIRCUIT DESCRIPTION
Code Model Type
R Semiconductor resistor model
C Semiconductor capacitor model
L Inductor model
SW Voltage controlled switch
CSW Current controlled switch
URC Uniform distributed RC model
LTRA Lossy transmission line model
D Diode model
NPN NPN BJT model
PNP PNP BJT model
NJF N-channel JFET model
PJF P-channel JFET model
NMOS N-channel MOSFET model
PMOS P-channel MOSFET model
NMF N-channel MESFET model
PMF P-channel MESFET model
Table 2.3: Ngspice model types
Most simple circuit elements typically require only a few parameter values. However, some de-
vices (semiconductor devices in particular) that are included in ngspice require many parameter
values. Often, many devices in a circuit are defined by the same set of device model parameters.
For these reasons, a set of device model parameters is defined on a separate .model line and
assigned a unique model name. The device element lines in ngspice then refer to the model
name.
For these more complex device types, each device element line contains the device name, the
nodes the device is connected to, and the device model name. In addition, other optional para-
meters may be specified for some devices: geometric factors and an initial condition (see the
following section on Transistors (8to 11) and Diodes (7) for more details). mname in the above
is the model name, and type is one of the following fifteen types:
Parameter values are defined by appending the parameter name followed by an equal sign and
the parameter value. Model parameters that are not given a value are assigned the default values
given below for each model type. Models are listed in the section on each device along with
the description of device element lines. Model parameters and their default values are given in
Chapt. 31.
2.4 .SUBCKT Subcircuits
A subcircuit that consists of ngspice elements can be defined and referenced in a fashion similar
to device models. Subcircuits are the way ngspice implements hierarchical modeling, but this is
not entirely true because each subcircuit instance is flattened during parsing, and thus ngspice
is not a hierarchical simulator.
The subcircuit is defined in the input deck by a grouping of element cards delimited by the
.subckt and the .ends cards (or the keywords defined by the substart and subend options
2.4. .SUBCKT SUBCIRCUITS 53
(see 17.7)); the program then automatically inserts the defined group of elements wherever the
subcircuit is referenced. Instances of subcircuits within a larger circuit are defined through the
use of an instance card that begins with the letter ‘X’. A complete example of all three of these
cards follows:
Example:
* The following is the instance card :
*
xdiv1 10 7 0 vdivide
* The following are the subcircuit definition cards :
*
.subckt vdivide 1 2 3
r1 1 2 10K
r2 2 3 5K
.ends
The above specifies a subcircuit with ports numbered ‘1’, ‘2’ and ‘3’:
• Resistor ‘R1’ is connected from port ‘1’ to port ‘2’, and has value 10 kOhms.
• Resistor ‘R2’ is connected from port ‘2’ to port ‘3’, and has value 5 kOhms.
The instance card, when placed in an ngspice deck, will cause subcircuit port ‘1’ to be equated
to circuit node ‘10’, while port ‘2’ will be equated to node ‘7’ and port ‘3’ will equated to node
‘0’.
There is no limit on the size or complexity of subcircuits, and subcircuits may contain other
subcircuits. An example of subcircuit usage is given in Chapt. 21.6.
2.4.1 .SUBCKT Line
General form:
.SUBCKT subnam N1 <N2 N3 ...>
Examples:
.SUBCKT OPAMP 1 2 3 4
A circuit definition is begun with a .SUBCKT line. subnam is the subcircuit name, and N1, N2,
... are the external nodes, which cannot be zero. The group of element lines that immediately
follow the .SUBCKT line define the subcircuit. The last line in a subcircuit definition is the
.ENDS line (see below). Control lines may not appear within a subcircuit definition; however,
subcircuit definitions may contain anything else, including other subcircuit definitions, device
models, and subcircuit calls (see below). Note that any device models or subcircuit definitions
included as part of a subcircuit definition are strictly local (i.e., such models and definitions
54 CHAPTER 2. CIRCUIT DESCRIPTION
are not known outside the subcircuit definition). Also, any element nodes not included on the
.SUBCKT line are strictly local, with the exception of 0 (ground) that is always global. If you
use parameters, the .SUBCKT line will be extended (see 2.8.3).
2.4.2 .ENDS Line
General form:
.ENDS <SUBNAM >
Examples:
.ENDS OPAMP
The .ENDS line must be the last one for any subcircuit definition. The subcircuit name, if
included, indicates which subcircuit definition is being terminated; if omitted, all subcircuits
being defined are terminated. The name is needed only when nested subcircuit definitions are
being made.
2.4.3 Subcircuit Calls
General form:
XYYYYYYY N1 <N2 N3 ...> SUBNAM
Examples:
X1 2 4 17 3 1 MULTI
Subcircuits are used in ngspice by specifying pseudo-elements beginning with the letter X,
followed by the circuit nodes to be used in expanding the subcircuit. If you use parameters, the
subcircuit call will be modified (see 2.8.3).
2.5 .GLOBAL
General form:
.GLOBAL nodename
Examples:
.GLOBAL gnd vcc
2.6. .INCLUDE 55
Nodes defined in the .GLOBAL statement are available to all circuit and subcircuit blocks inde-
pendently from any circuit hierarchy. After parsing the circuit, these nodes are accessible from
top level.
2.6 .INCLUDE
General form:
.INCLUDE filename
Examples:
.INCLUDE / users/spice / common/bsim3 - param.mod
Frequently, portions of circuit descriptions will be reused in several input files, particularly with
common models and subcircuits. In any ngspice input file, the .INCLUDE line may be used to
copy some other file as if that second file appeared in place of the .INCLUDE line in the original
file.
There is no restriction on the file name imposed by ngspice beyond those imposed by the local
operating system.
2.7 .LIB
General form:
.LIB filename libname
Examples:
.LIB / users /spice / common/ mosfets .lib mos1
The .LIB statement allows to include library descriptions into the input file. Inside the *.lib
file a library libname will be selected. The statements of each library inside the *.lib file are
enclosed in .LIB libname <...> .ENDL statements.
If the compatibility mode (16.13) is set to ’ps’ by set ngbehavior=ps (17.7) in spinit (16.5)
or .spiceinit (16.6), then a simplified syntax .LIB filename is available: a warning is issued
and filename is simply included as described in Chapt. 2.6.
2.8 .PARAM Parametric netlists
Ngspice allows for the definition of parametric attributes in the netlists. This is an enhancement
of the ngspice front-end that adds arithmetic functionality to the circuit description language.
56 CHAPTER 2. CIRCUIT DESCRIPTION
2.8.1 .param line
General form:
.param <ident > = <expr > <ident > = <expr > ...
Examples:
. param pippo =5
. param po =6 pp =7.8 pap ={ AGAUSS (pippo , 1, 1.67)}
. param pippp ={ pippo + pp }
.param p={pp}
.param pop=’pp+p’
This line assigns numerical values to identifiers. More than one assignment per line is possible
using a separating space. Parameter identifier names must begin with an alphabetic character.
The other characters must be either alphabetic, a number, or ! #$%[]_as special cha-
racters. The variables time,temper, and hertz (see 5.1.1) are not valid identifier names. Other
restrictions on naming conventions apply as well, see 2.8.6.
The .param lines inside subcircuits are copied per call, like any other line. All assignments
are executed sequentially through the expanded circuit. Before its first use, a parameter name
must have been assigned a value. Expressions defining a parameter should be put within braces
{p+p2}, or alternatively within single quotes ’AGAUSS(pippo, 1, 1.67)’. An assignment
cannot be self-referential, something like .param pip = ’pip+3’ will not work.
The current ngspice version does not always need quotes or braces in expressions, especially
when spaces are used sparingly. However, it is recommended to do so, as the following exam-
ples demonstrate.
.param a = 123 * 3 b = sqrt (9) $ doesn ’t work , a <= 123
.param a = ’123 * 3’ b = sqrt (9) $ ok.
.param c = a + 123 $ won ’t work
.param c = ’a + 123 ’ $ ok.
.param c = a+123 $ ok.
2.8.2 Brace expressions in circuit elements:
General form:
{ <expr > }
Examples:
These are allowed in .model lines and in device lines. A SPICE number is a floating point
number with an optional scaling suffix, immediately glued to the numeric tokens (see Chapt.
2.8.5). Brace expressions ({..}) cannot be used to parametrize node names or parts of names.
2.8. .PARAM PARAMETRIC NETLISTS 57
All identifiers used within an <expr> must have known values at the time when the line is
evaluated, else an error is flagged.
2.8.3 Subcircuit parameters
General form:
.subckt <identn > node node ... <ident >=<value > <ident >=<value > ...
Examples:
. subckt myfilter in out rval =100 k cval =100 nF
<identn> is the name of the subcircuit given by the user. node is an integer number or an
identifier, for one of the external nodes. The first <ident>=<value> introduces an optional
section of the line. Each <ident> is a formal parameter, and each <value> is either a SPICE
number or a brace expression. Inside the .subckt ... .ends context, each formal parameter
may be used like any identifier that was defined on a .param control line. The <value> parts
are supposed to be default values of the parameters. However, in the current version of , they
are not used and each invocation of the subcircuit must supply the _exact_ number of actual
parameters.
The syntax of a subcircuit call (invocation) is:
General form:
X<name > node node ... <identn > <ident >=< value > <ident >=<value > ...
Examples:
X1 input output myfilter rval =1k cval =1 n
Here <name> is the symbolic name given to that instance of the subcircuit, <identn> is the
name of a subcircuit defined beforehand. node node ... is the list of actual nodes where the
subcircuit is connected. <value> is either a SPICE number or a brace expression { <expr> }
. The sequence of <value> items on the Xline must exactly match the number and the order of
formal parameters of the subcircuit.
58 CHAPTER 2. CIRCUIT DESCRIPTION
Subcircuit example with parameters:
* Param - example
.param amplitude = 1V
*
. subckt myfilter in out rval =100 k cval =100 nF
Ra in p1 {2* rval }
Rb p1 out {2* rval }
C1 p1 0 {2* cval }
Ca in p2 {cval }
Cb p2 out {cval }
R1 p2 0 {rval }
.ends myfilter
*
X1 input output myfilter rval =1k cval =1 n
V1 input 0 AC { amplitude }
.end
2.8.4 Symbol scope
All subcircuit and model names are considered global and must be unique. The .param symbols
that are defined outside of any .subckt ... .ends section are global. Inside such a section, the
pertaining params: symbols and any .param assignments are considered local: they mask any
global identical names, until the .ends line is encountered. You cannot reassign to a global
number inside a .subckt, a local copy is created instead. Scope nesting works up to a level of
10. For example, if the main circuit calls A that has a formal parameter xx, A calls B that has a
param. xx, and B calls C that also has a formal param. xx, there will be three versions of ‘xx’
in the symbol table but only the most local one - belonging to C - is visible.
2.8.5 Syntax of expressions
<expr> ( optional parts within [...] )
An expression may be one of:
<atom > where <atom > is either a spice number or an identifier
<unary -operator > <atom >
<function -name > ( <expr > [ , <expr > ...] )
<atom > <binary - operator > <expr >
( <expr > )
As expected, atoms, built-in function calls and stuff within parentheses are evaluated before
the other operators. The operators are evaluated following a list of precedence close to the one
of the C language. For equal precedence binary ops, evaluation goes left to right. Functions
operate on real values only!
2.8. .PARAM PARAMETRIC NETLISTS 59
Operator Alias Precedence Description
-1 unary -
!1 unary not
** ^ 2 power, like pwr
*3 multiply
/3 divide
%3 modulo
\3 integer divide
+4 add
-4 subtract
== 5 equality
!= <> 5 non-equal
<= 5 less or equal
>= 5 greater or equal
<5 less than
>5 greater than
&& 6 boolean and
|| 7 boolean or
c?x:y 8 ternary operator
The number zero is used to represent boolean False. Any other number represents boolean True.
The result of logical operators is 1 or 0. An example input file is shown below:
Example input file with logical operators:
* Logical operators
v1or 1 0 {1 || 0}
v1and 2 0 {1 && 0}
v1not 3 0 {! 1}
v1mod 4 0 {5 % 3}
v1div 5 0 {5 \ 3}
v0not 6 0 {! 0}
.control
op
print allv
.endc
.end
60 CHAPTER 2. CIRCUIT DESCRIPTION
Built-in function Notes
sqr(x) y=x*x
sqrt(x) y = sqrt(x)
sin(x), cos(x), tan(x)
sinh(x), cosh(x), tanh(x)
asin(x), acos(x), atan(x)
asinh(x), acosh(x), atanh(x)
arctan(x) atan(x), kept for compatibility
exp(x)
ln(x), log(x)
abs(x)
nint(x) Nearest integer, half integers towards even
int(x) Nearest integer rounded towards 0
floor(x) Nearest integer rounded towards -∞
ceil(x) Nearest integer rounded towards +∞
pow(x,y) x raised to the power of y (pow from C runtime library)
pwr(x,y) pow(fabs(x), y)
min(x, y)
max(x, y)
sgn(x) 1.0 for x > 0, 0.0 for x == 0, -1.0 for x < 0
ternary_fcn(x, y, z) x ? y : z
gauss(nom, rvar, sigma) nominal value plus variation drawn from Gaussian
distribution with mean 0 and standard deviation rvar
(relative to nominal), divided by sigma
agauss(nom, avar, sigma) nominal value plus variation drawn from Gaussian
distribution with mean 0 and standard deviation avar
(absolute), divided by sigma
unif(nom, rvar) nominal value plus relative variation (to nominal)
uniformly distributed between +/-rvar
aunif(nom, avar) nominal value plus absolute variation uniformly distributed
between +/-avar
limit(nom, avar) nominal value +/-avar, depending on random number in
[-1, 1) being > 0 or < 0
The scaling suffixes (any decorative alphanumeric string may follow):
suffix value
g 1e9
meg 1e6
k 1e3
m 1e-3
u 1e-6
n 1e-9
p 1e-12
f 1e-15
Note: there are intentional redundancies in expression syntax, e.g. x^y ,x**y and pwr(x,y)
all have nearly the same result.
2.9. .FUNC 61
2.8.6 Reserved words
In addition to the above function names and to the verbose operators ( not and or div mod
), other words are reserved and cannot be used as parameter names: or,defined,sqr,sqrt,
sin,cos,exp,ln,log, log10, arctan,abs,pwr,time,temper,hertz.
2.8.7 Alternative syntax
The & sign is tolerated to provide some ‘historical’ parameter notation: &as the first character
of a line is equivalent to: .param.
Inside a line, the notation &(....) is equivalent to {....}, and &identifier means the same
thing as {identifier} .
Comments in the style of C++ line trailers (//) are detected and erased.
Warning: this is not possible in embedded .control parts of a source file, these lines are
outside of this scope.
Confusion may arise in ngspice because of its multiple numerical expression features. The
.param lines and the brace expressions (see Chapt. 2.9) are evaluated in the front-end, that
is, just after the subcircuit expansion. (Technically, the X lines are kept as comments in the
expanded circuit so that the actual parameters can be correctly substituted). Therefore, after the
netlist expansion and before the internal data setup, all number attributes in the circuit are known
constants. However, there are circuit elements in Spice that accept arithmetic expressions not
evaluated at this point, but only later during circuit analysis. These are the arbitrary current
and voltage sources (B-sources, 5), as well as E- and G-sources and R-, L-, or C-devices.
The syntactic difference is that ‘compile-time’ expressions are within braces, but ‘run-time’
expressions have no braces. To make things more complicated, the back-end ngspice scripting
language accepts arithmetic/logic expressions that operate only on its own scalar or vector data
sets (17.2). Please see Chapt. 2.13.
It would be desirable to have the same expression syntax, operator and function set, and prece-
dence rules, for the three contexts mentioned above. In the current Numparam implementation,
that goal is not achieved.
2.9 .FUNC
This keyword defines a function. The syntax of the expression is the same as for a .param
(2.8.5).
62 CHAPTER 2. CIRCUIT DESCRIPTION
General form:
.func <ident > { <expr > }
.func <ident > = { <expr > }
Examples:
.func icos(x) {cos(x) - 1}
.func f(x ,y) {x*y}
.func foo(a,b) = {a + b}
.func will initiate a replacement operation. After reading the input files, and before parameters
are evaluated, all occurrences of the icos(x) function will be replaced by cos(x)-1. All
occurrences of f(x,y) will be replaced by x*y. Function statements may be nested to a depth
of t.b.d..
2.10 .CSPARAM
Create a constant vector (see 17.8.2) from a parameter in plot (17.3)const.
General form:
.csparam <ident > = <expr >
Examples:
. param pippo =5
.param pp =6
. csparam pippp ={ pippo + pp }
.param p={pp}
.csparam pap=’pp+p ’
In the example shown, vectors pippp, and pap are added to the constants that already reside
in plot const, having length one and real values. These vectors are generated during circuit
parsing and thus cannot be changed later (same as with ordinary parameters). They may be used
in ngspice scripts and .control sections (see Chapt. 17).
The use of .csparam is still experimental and has to be tested. A simple usage is shown below.
* test csparam
.param TEMPS = 27
.csparam newt = {3*TEMPS}
.csparam mytemp = ’2 + TEMPS’
.control
echo $&newt $&mytemp
.endc
.end
2.11. .TEMP 63
2.11 .TEMP
Sets the circuit temperature in degrees Celsius.
General form:
.temp value
Examples:
.temp 27
This card overrides the circuit temperature given in an .option line (15.1.1).
2.12 .IF Condition-Controlled Netlist
A simple .IF-.ELSE(IF) block allows condition-controlling of the netlist. boolean expression
is any expression according to Chapt. 2.8.5 that evaluates parameters and returns a boolean 1
or 0. The netlist block in between the .if ... .endif statements may contain device instances or
.model cards that are selected according to the logic condition.
64 CHAPTER 2. CIRCUIT DESCRIPTION
General form:
.if( boolean expression)
...
.elseif ( boolean expression )
...
.else
...
.endif
Example 1:
* device instance in IF - ELSE block
.param ok =0 ok2 =1
v1 1 0 1
R1 1 0 2
.if (ok && ok2)
R11 1 0 2
.else
R11 1 0 0.5 $ <-- selected
.endif
Example 2:
* . model in IF - ELSE block
.param m0 =0 m1=1
M1 1 2 3 4 N1 W=1 L =0.5
.if (m0 ==1)
.model N1 NMOS level =49 Version =3.1
. elseif ( m1 ==1)
.model N1 NMOS level =49 Version =3.2.4 $ <-- selected
.else
.model N1 NMOS level =49 Version =3.3.0
.endif
For now this is a very restricted version of an .IF-.ELSE(IF) block, so several netlist com-
ponents are currently not supported within the .IF-.ENDIF block: .SUBCKT,.INC,.LIB, and
.PARAM. Nesting of .IF-.ELSE(IF) blocks is not possible. Only one .elseif is allowed per
block.
2.13. PARAMETERS, FUNCTIONS, EXPRESSIONS, AND COMMAND SCRIPTS 65
2.13 Parameters, functions, expressions, and command scripts
In ngspice there are several ways to describe functional dependencies. In fact there are three
independent function parsers, being active before, during, and after the simulation. So it might
be due to have a few words on their interdependence.
2.13.1 Parameters
Parameters (Chapt. 2.8.1) and functions, either defined within the .param statement or with
the .func statement (Chapt. 2.9) are evaluated before any simulation is started, that is during
the setup of the input and the circuit. Therefore these statements may not contain any simu-
lation output (voltage or current vectors), because it is simply not yet available. The syntax is
described in Chapt. 2.8.5. During the circuit setup all functions are evaluated, all parameters
are replaced by their resulting numerical values. Thus it will not be possible to get feedback
from a later stage (during or after simulation) to change any of the parameters.
2.13.2 Nonlinear sources
During the simulation, the B source (Chapt. 5) and their associated E and G sources, as well
as some devices (R, C, L) may contain expressions. These expressions may contain parameters
from above (evaluated immediately upon ngspice start up), numerical data, predefined functi-
ons, but also node voltages and branch currents resulting from the simulation. The source or
device values are continuously updated during the simulation. Therefore the sources are po-
werful tools to define non-linear behavior, you may even create new ‘devices’ by yourself.
Unfortunately the expression syntax (see Chapt. 5.1) and the predefined functions may deviate
from the ones for parameters listed in 2.8.1.
2.13.3 Control commands, Command scripts
Commands, as described in detail in Chapt. 17.5, may be used interactively, but also as a com-
mand script enclosed in .control ... .endc lines. The scripts may contain expressions
(see Chapt. 17.2). The expressions may work upon simulation output vectors (of node volta-
ges, branch currents), as well as upon predefined or user defined vectors and variables, and are
invoked after the simulation. Parameters from 2.8.1 defined by the .param statement are not
allowed in these expressions. However you may define such parameters with .csparam (2.10).
Again the expression syntax (see Chapt. 17.2) will deviate from the one for parameters or B
sources listed in 2.8.1 and 5.1.
If you want to use parameters from 2.8.1 inside your control script, you may use .csparam
(2.10) or apply a trick by defining a voltage source with the parameter as its value, and then
have it available as a vector (e.g. after a transient simulation) with a then constant output (the
parameter). A feedback from here back into parameters (2.13.1) is never possible. Also you
cannot access non-linear sources of the preceding simulation. However you may start a first
simulation inside your control script, then evaluate its output using expressions, change some of
the element or model parameters with the alter and altermod statements (see Chapt. 17.5.3)
and then automatically start a new simulation.
66 CHAPTER 2. CIRCUIT DESCRIPTION
Expressions and scripting are powerful tools within ngspice, and we will enhance the examples
given in Chapt. 21 continuously to describe these features.
Chapter 3
Circuit Elements and Models
Data fields that are enclosed in less-than and greater-than signs (‘< >’) are optional. All indi-
cated punctuation (parentheses, equal signs, etc.) is optional but indicate the presence of any
delimiter. Further, future implementations may require the punctuation as stated. A consis-
tent style adhering to the punctuation shown here makes the input easier to understand. With
respect to branch voltages and currents, ngspice uniformly uses the associated reference con-
vention (current flows in the direction of voltage drop).
3.1 General options and information
3.1.1 Paralleling devices with multiplier m
When it is needed to simulate several devices of the same kind in parallel, use the ‘m’ (parallel
multiplier) instance parameter available for the devices listed in Table 3.1. This multiplies the
value of the element’s matrix stamp with m’s value. The netlist below shows how to correctly
use the parallel multiplier:
Multiple device example:
d1 2 0 mydiode m =10
d01 1 0 mydiode
d02 1 0 mydiode
d03 1 0 mydiode
d04 1 0 mydiode
d05 1 0 mydiode
d06 1 0 mydiode
d07 1 0 mydiode
d08 1 0 mydiode
d09 1 0 mydiode
d10 1 0 mydiode
...
The d1 instance connected between nodes 2 and 0 is equivalent to the 10 parallel devices
d01-d10 connected between nodes 1 and 0.
67
68 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
The following devices support the multiplier m:
First letter Element description
C Capacitor
D Diode
F Current-controlled current source (CCCs)
G Voltage-controlled current source (VCCS)
I Current source
J Junction field effect transistor (JFET)
L Inductor
M Metal oxide field effect transistor (MOSFET)
Q Bipolar junction transistor (BJT)
R Resistor
X Subcircuit (for details see below)
Z Metal semiconductor field effect transistor (MESFET)
Table 3.1: ngspice elements supporting multiplier ’m’
When the X line (e.g. x1 a b sub1 m=5) contains the token m=value (as shown) or m=expression,
subcircuit invocation is done in a special way. If an instance line of the subcircuit sub1 contains
any of the elements shown in table 3.1, then these elements are instantiated with the additional
parameter m(in this example having the value 5). If such an element already has an mmul-
tiplier parameter, the element mis multiplied with the mderived from the X line. This works
recursively, meaning that if a subcircuit contains another subcircuit (a nested X line), then the
latter mparameter will be multiplied by the former one, and so on.
Example 1:
.param madd = 6
X1 a b sub1 m=5
.subckt sub1 a1 b1
Cs1 a1 b1 C=5p m=’madd -2’
.ends
In example 1, the capacitance between nodes a and b will be C = 5pF*(madd-2)*5 = 100pF.
Example 2:
.param madd = 4
X1 a b sub1 m=3
.subckt sub1 a1 b1
X2 a1 b1 sub2 m=’ madd -2’
.ends
.subckt sub2 a2 b2
Cs2 a2 b2 3p m=2
.ends
In example 2, the capacitance between nodes a and b is C = 3pF*2*(madd-2)*3 = 36pF.
3.1. GENERAL OPTIONS AND INFORMATION 69
Using mmay fail to correctly describe geometrical properties for real devices like MOS transis-
tors.
M1 d g s nmos W=0.3u L=0.18u m=20
is probably not be the same as
M1 d g s nmos W=6u L=0.18u
because the former may suffer from small width (or edge) effects, whereas the latter is simply
a wide transistor.
3.1.2 Technology scaling
Still to be implemented and written.
3.1.3 Model binning
Binning is a kind of range partitioning for geometry dependent models like MOSFET’s. The
purpose is to cover larger geometry ranges (Width and Length) with higher accuracy then the
model built-in geometry formulas. Each size range described by the additional model parame-
ters LMIN, LMAX, WMIN and WMAX has its own model parameter set. These model cards
are defined by a number extension, like ‘nch.1’. NGSPICE has a algorithm to choose the right
model card by the requested W and L.
This is implemented for BSIM3 (11.2.9) and BSIM4 (11.2.10) models.
3.1.4 Initial conditions
Two different forms of initial conditions may be specified for some devices. The first form
is included to improve the dc convergence for circuits that contain more than one stable state.
If a device is specified OFF, the dc operating point is determined with the terminal voltages
for that device set to zero. After convergence is obtained, the program continues to iterate to
obtain the exact value for the terminal voltages. If a circuit has more than one dc stable state,
the OFF option can be used to force the solution to correspond to a desired state. If a device
is specified OFF when in reality the device is conducting, the program still obtains the correct
solution (assuming the solutions converge) but more iterations are required since the program
must independently converge to two separate solutions.
The .NODESET control line (see Chapt. 15.2.1) serves a similar purpose as the OFF option. The
.NODESET option is easier to apply and is the preferred means to aid convergence. The second
form of initial conditions are specified for use with the transient analysis. These are true ‘initial
conditions’ as opposed to the convergence aids above. See the description of the .IC control
line (Chapt. 15.2.2) and the .TRAN control line (Chapt. 15.3.9) for a detailed explanation of
initial conditions.
70 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
3.2 Elementary Devices
3.2.1 Resistors
General form:
RXXXXXXX n+ n- < resistance |r=>value <ac=val > <m=val >
+ <scale =val > <temp=val > <dtemp =val > <tc1=val > <tc2 =val >
+ <noisy =0|1 >
Examples:
R1 1 2 100
RC1 12 17 1K
R2 5 7 1K ac=2K
RL 1 4 2K m=2
Ngspice has a fairly complex model for resistors. It can simulate both discrete and semicon-
ductor resistors. Semiconductor resistors in ngspice means: resistors described by geometrical
parameters. So, do not expect detailed modeling of semiconductor effects.
n+ and n- are the two element nodes, value is the resistance (in ohms) and may be positive or
negative1but not zero.
Simulating small valued resistors: If you need to simulate very small resis-
tors (0.001 Ohm or less), you should use CCVS (transresistance), it is less
efficient but improves overall numerical accuracy. Think about that a small
resistance is a large conductance.
Ngspice can assign a resistor instance a different value for AC analysis, specified using the
ac keyword. This value must not be zero as described above. The AC resistance is used in
AC analysis only (neither Pole-Zero nor Noise). If you do not specify the ac parameter, it is
defaulted to value.
Ngspice calculates the nominal resistance as
Rnom =VALUE scale
m
Racnom =ac scale
m.
(3.1)
If you want to simulate temperature dependence of a resistor, you need to specify its temperature
coefficients, using a .model line or as instance parameters, like in the examples below:
1A negative resistor modeling an active element can cause convergence problems, please avoid it.
3.2. ELEMENTARY DEVICES 71
Examples:
RE1 1 2 800 newres dtemp =5
.MODEL newres R tc1 =0.001
RE2 a b 1.4k tc1 =2m tc2 =1.4 u
RE3 n1 n2 1 Meg tce =700 m
The temperature coefficients tc1 and tc2 describe a quadratic temperature dependence (see
equation 1.6) of the resistance. If given in the instance line (the R... line) their values will
override the tc1 and tc2 of the .model line (3.2.3). Ngspice has an additional temperature
model equation 3.2 parameterised by tce given in model or instance line. If all parameters are
given (quadratic and exponential) the exponential temperature model is choosen.
R(T) = R(T0)h1.01TCE·(T−T0)i(3.2)
where Tis the circuit temperature, T0is the nominal temperature, and TCE is the exponential
temperature coefficients.
Instance temperature is useful even if resistance does not vary with it, since the thermal noise
generated by a resistor depends on its absolute temperature. Resistors in ngspice generates two
different noises: thermal and flicker. While thermal noise is always generated in the resistor, to
add a flicker noise2source you have to add a .model card defining the flicker noise parameters.
It is possible to simulate resistors that do not generate any kind of noise using the noisy (or
noise) keyword and assigning zero to it, as in the following example:
Example:
Rmd 134 57 1.5 k noisy =0
If you are interested in temperature effects or noise equations, read the next section on semi-
conductor resistors.
3.2.2 Semiconductor Resistors
General form:
RXXXXXXX n+ n- <value > <mname > <l=length > <w=width >
+ <temp=val > <dtemp =val > <m=val > <ac=val > <scale=val >
+ <noisy = 0|1 >
Examples:
RLOAD 2 10 10K
RMOD 3 7 RMODEL L=10 u W=1u
2Flicker noise can be used to model carbon resistors.
72 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
This is the more general form of the resistor presented before (3.2.1) and allows the modeling of
temperature effects and for the calculation of the actual resistance value from strictly geometric
information and the specifications of the process. If value is specified, it overrides the geo-
metric information and defines the resistance. If mname is specified, then the resistance may be
calculated from the process information in the model mname and the given length and width.
If value is not specified, then mname and length must be specified. If width is not specified,
then it is taken from the default width given in the model.
The (optional) temp value is the temperature at which this device is to operate, and overrides
the temperature specification on the .option control line and the value specified in dtemp.
3.2.3 Semiconductor Resistor Model (R)
The resistor model consists of process-related device data that allow the resistance to be calcu-
lated from geometric information and to be corrected for temperature. The parameters available
are:
Name Parameter Units Default Example
TC1 first order temperature coeff. Ω
/◦C0.0 -
TC2 second order temperature coeff. Ω
/◦C20.0 -
RSH sheet resistance Ω
/- 50
DEFW default width m1e-6 2e-6
NARROW narrowing due to side etching m0.0 1e-7
SHORT shortening due to side etching m0.0 1e-7
TNOM parameter measurement temperature ◦C27 50
KF flicker noise coefficient 0.0 1e-25
AF flicker noise exponent 0.0 1.0
WF flicker noise width exponent 1.0
LF flicker noise length exponent 1.0
EF flicker noise frequnecy exponent 1.0
R (RES) default value if element value not given Ω- 1000
The sheet resistance is used with the narrowing parameter and land wfrom the resistor device
to determine the nominal resistance by the formula:
Rnom =rsh l−SHORT
w−NARROW (3.3)
DEFW is used to supply a default value for wif one is not specified for the device. If either rsh
or lis not specified, then the standard default resistance value of 1 mOhm is used. TNOM is used
to override the circuit-wide value given on the .options control line where the parameters
of this model have been measured at a different temperature. After the nominal resistance is
calculated, it is adjusted for temperature by the formula:
R(T) = R(TNOM)1+TC1(T−TNOM) + TC2(T−TNOM)2(3.4)
where R(TNOM) = Rnom|Racnom. In the above formula, ‘T’ represents the instance temperature,
which can be explicitly set using the temp keyword or calculated using the circuit temperature
and dtemp, if present. If both temp and dtemp are specified, the latter is ignored. Ngspice
3.2. ELEMENTARY DEVICES 73
improves SPICE’s resistors noise model, adding flicker noise (1
/f) to it and the noisy (or
noise) keyword to simulate noiseless resistors. The thermal noise in resistors is modeled
according to the equation:
¯
i2
R=4kT
R
∆f(3.5)
where ‘k’ is the Boltzmann’s constant, and ‘T’ the instance temperature.
Flicker noise model is:
¯
i2
R f n =KFIAF
R
WW F LLF fEF ∆f(3.6)
A small list of sheet resistances (in Ω
/) for conductors is shown below. The table represents
typical values for MOS processes in the 0.5 - 1 um
range. The table is taken from: N. Weste, K. Eshraghian - Principles of CMOS VLSI Design
2nd Edition, Addison Wesley.
Material Min. Typ. Max.
Inter-metal (metal1 - metal2) 0.005 0.007 0.1
Top-metal (metal3) 0.003 0.004 0.05
Polysilicon (poly) 15 20 30
Silicide 2 3 6
Diffusion (n+, p+) 10 25 100
Silicided diffusion 2 4 10
n-well 1000 2000 5000
3.2.4 Resistors, dependent on expressions (behavioral resistor)
General form:
RXXXXXXX n+ n- R = ’expression ’ <tc1=value > <tc2 =value >
RXXXXXXX n+ n- ’expression ’ <tc1 = value > <tc2=value >
Examples:
R1 rr 0 r = ’V(rr) < {Vt} ? {R0} : {2* R0 }’ tc1 =2e -03 tc2 =3.3e -06
R2 r2 rr r = {5k + 50* TEMPER}
Expression may be an equation or an expression containing node voltages or branch currents
(in the form of i(vm)) and any other terms as given for the B source and described in Chapt. 5.1.
It may contain parameters (2.8.1) and the special variables time,temper, and hertz (5.1.2).
An example file is given below.
74 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
Example input file for non-linear resistor:
Non - linear resistor
. param R0 =1 k Vi =1 Vt =0.5
* resistor depending on control voltage V(rr)
R1 rr 0 r = ’V(rr) < {Vt} ? {R0} : {2* R0 }’
* control voltage
V1 rr 0 PWL (0 0 100u {Vi})
.control
unset askquit
tran 100n 100 u uic
plot i(V1)
.endc
.end
3.2.5 Capacitors
General form:
CXXXXXXX n+ n- <value > <mname > <m=val > <scale =val > <temp =val >
+ <dtemp =val > <tc1=val > <tc2=val > <ic= init_condition >
Examples:
CBYP 13 0 1UF
COSC 17 23 10U IC=3V
Ngspice provides a detailed model for capacitors. Capacitors in the netlist can be specified
giving their capacitance or their geometrical and physical characteristics. Following the original
SPICE3 ‘convention’, capacitors specified by their geometrical or physical characteristics are
called ‘semiconductor capacitors’ and are described in the next section.
In this first form n+ and n- are the positive and negative element nodes, respectively and value
is the capacitance in Farads.
Capacitance can be specified in the instance line as in the examples above or in a .model line,
as in the example below:
C1 15 5 cstd
C2 2 7 cstd
.model cstd C cap =3n
Both capacitors have a capacitance of 3nF.
If you want to simulate temperature dependence of a capacitor, you need to specify its tempe-
rature coefficients, using a .model line, like in the example below:
3.2. ELEMENTARY DEVICES 75
CEB 1 2 1u cap1 dtemp =5
.MODEL cap1 C tc1 =0.001
The (optional) initial condition is the initial (time zero) value of capacitor voltage (in Volts).
Note that the initial conditions (if any) apply only if the uic option is specified on the .tran
control line.
Ngspice calculates the nominal capacitance as described below:
Cnom =value ·scale ·m(3.7)
The temperature coefficients tc1 and tc2 describe a quadratic temperature dependence (see
equation17.12) of the capacitance. If given in the instance line (the C... line) their values will
override the tc1 and tc2 of the .model line (3.2.7).
3.2.6 Semiconductor Capacitors
General form:
CXXXXXXX n+ n- <value > <mname > <l=length > <w=width > <m=val >
+ <scale =val > <temp=val > <dtemp =val > <ic=init_condition >
Examples:
CLOAD 2 10 10P
CMOD 3 7 CMODEL L=10 u W=1u
This is the more general form of the Capacitor presented in section (3.2.5), and allows for the
calculation of the actual capacitance value from strictly geometric information and the speci-
fications of the process. If value is specified, it defines the capacitance and both process and
geometrical information are discarded. If value is not specified, the capacitance is calcula-
ted from information contained model mname and the given length and width (l,wkeywords,
respectively).
It is possible to specify mname only, without geometrical dimensions and set the capacitance in
the .model line (3.2.5).
3.2.7 Semiconductor Capacitor Model (C)
The capacitor model contains process information that may be used to compute the capacitance
from strictly geometric information.
76 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
Name Parameter Units Default Example
CAP model capacitance F0.0 1e-6
CJ junction bottom capacitance F/m2- 5e-5
CJSW junction sidewall capacitance F/m- 2e-11
DEFW default device width m1e-6 2e-6
DEFL default device length m0.0 1e-6
NARROW narrowing due to side etching m0.0 1e-7
SHORT shortening due to side etching m0.0 1e-7
TC1 first order temperature coeff. F/◦C0.0 0.001
TC2 second order temperature coeff. F/◦C20.0 0.0001
TNOM parameter measurement temperature ◦C27 50
DI relative dielectric constant F/m- 1
THICK insulator thickness m0.0 1e-9
The capacitor has a capacitance computed as:
If value is specified on the instance line then
Cnom =value ·scale ·m(3.8)
If model capacitance is specified then
Cnom =CAP ·scale ·m(3.9)
If neither value nor CAP are specified, then geometrical and physical parameters are take into
account:
C0=CJ(l−SHORT)(w−NARROW) + 2CJSW(l−SHORT +w−NARROW)(3.10)
CJ can be explicitly given on the .model line or calculated by physical parameters. When CJ
is not given, is calculated as:
If THICK is not zero:
CJ =DI ε0
THICK if DI is specified,
CJ =εSiO2
THICK otherwise.
(3.11)
If the relative dielectric constant is not specified the one for SiO2 is used. The values of the
constants are: ε0=8.854214871e−12 F
mand εSiO2=3.4531479969e−11F
m. The nominal
capacitance is then computed as:
Cnom =C0scale m(3.12)
After the nominal capacitance is calculated, it is adjusted for temperature by the formula:
C(T) = C(TNOM)1+TC1(T−TNOM) + TC2(T−TNOM)2(3.13)
3.2. ELEMENTARY DEVICES 77
where C(TNOM) = Cnom.
In the above formula, ‘T’ represents the instance temperature, which can be explicitly set using
the temp keyword or calculated using the circuit temperature and dtemp, if present.
3.2.8 Capacitors, dependent on expressions (behavioral capacitor)
General form:
CXXXXXXX n+ n- C = ’expression ’ <tc1=value > <tc2 =value >
CXXXXXXX n+ n- ’expression ’ <tc1 = value > <tc2=value >
Examples:
C1 cc 0 c = ’V(cc) < {Vt} ? {C1} : {Ch }’ tc1 =-1e -03 tc2 =1.3e-05
Expression may be an equation or an expression containing node voltages or branch currents
(in the form of i(vm)) and any other terms as given for the B source and described in Chapt. 5.1.
It may contain parameters (2.8.1) and the special variables time,temper, and hertz (5.1.2).
Example input file:
Behavioral Capacitor
.param Cl =5n Ch =1n Vt =1m Il =100n
.ic v(cc) = 0 v(cc2 ) = 0
* capacitor depending on control voltage V(cc)
C1 cc 0 c = ’V(cc) < {Vt} ? {Cl} : {Ch }’
*C1 cc 0 c ={ Ch}
I1 0 1 {Il}
Exxx n1 - copy n2 n2 cc2 1
Cxxx n1 - copy n2 1
Bxxx cc2 n2 I = ’(V( cc2) < {Vt} ? {Cl} : {Ch})’ * i(Exxx )
I2 n2 22 {Il}
vn2 n2 0 DC 0
* measure charge by integrating current
aint1 %id (1 cc) 2 time_count
aint2 %id (22 cc2) 3 time_count
. model time_count int( in_offset =0.0 gain =1.0
+ out_lower_limit =-1 e12 out_upper_limit =1 e12
+ limit_range =1e -9 out_ic =0.0)
.control
unset askquit
tran 100n 100 u
plot v(2)
plot v(cc) v( cc2)
.endc
.end
78 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
3.2.9 Inductors
General form:
LYYYYYYY n+ n- <value > <mname > <nt=val > <m=val >
+ <scale =val > <temp=val > <dtemp =val > <tc1=val >
+ <tc2 =val > <ic=init_condition >
Examples:
LLINK 42 69 1UH
LSHUNT 23 51 10U IC =15.7 MA
The inductor device implemented into ngspice has many enhancements over the original one.n+
and n- are the positive and negative element nodes, respectively. value is the inductance in
Henry. Inductance can be specified in the instance line as in the examples above or in a .model
line, as in the example below:
L1 15 5 indmod1
L2 2 7 indmod1
.model indmod1 L ind =3n
Both inductors have an inductance of 3nH.
The nt is used in conjunction with a .model line, and is used to specify the number of turns
of the inductor. If you want to simulate temperature dependence of an inductor, you need to
specify its temperature coefficients, using a .model line, like in the example below:
Lload 1 2 1u ind1 dtemp =5
.MODEL ind1 L tc1 =0.001
The (optional) initial condition is the initial (time zero) value of inductor current (in Amps) that
flows from n+, through the inductor, to n-. Note that the initial conditions (if any) apply only if
the UIC option is specified on the .tran analysis line.
Ngspice calculates the nominal inductance as described below:
Lnom =value scale
m(3.14)
3.2.10 Inductor model
The inductor model contains physical and geometrical information that may be used to compute
the inductance of some common topologies like solenoids and toroids, wound in air or other
material with constant magnetic permeability.
3.2. ELEMENTARY DEVICES 79
Name Parameter Units Default Example
IND model inductance H0.0 1e-3
CSECT cross section m20.0 1e-3
LENGTH length m0.0 1e-2
TC1 first order temperature coeff. H/◦C0.0 0.001
TC2 second order temperature coeff. H/◦C20.0 0.0001
TNOM parameter measurement temperature ◦C27 50
NT number of turns - 0.0 10
MU relative magnetic permeability H/m0.0 -
The inductor has an inductance computed as:
If value is specified on the instance line then
Lnom =value scale
m(3.15)
If model inductance is specified then
Lnom =IND scale
m(3.16)
If neither value nor IND are specified, then geometrical and physical parameters are take into
account. In the following formulas
NT refers to both instance and model parameter (instance parameter overrides model parameter):
If LENGTH is not zero:
(Lnom =MU µ0NT2CSECT
LENGTH if MU is specified,
Lnom =µ0NT2CSECT
LENGTH otherwise.(3.17)
with µ0=1.25663706143592 µH
m. After the nominal inductance is calculated, it is adjusted for
temperature by the formula
L(T) = L(TNOM)1+TC1(T−TNOM) + TC2(T−TNOM)2,(3.18)
where L(TNOM) = Lnom. In the above formula, ‘T’ represents the instance temperature, which
can be explicitly set using the temp keyword or calculated using the circuit temperature and
dtemp, if present.
80 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
3.2.11 Coupled (Mutual) Inductors
General form:
KXXXXXXX LYYYYYYY LZZZZZZZ value
Examples:
K43 LAA LBB 0.999
KXFRMR L1 L2 0.87
LYYYYYYY and LZZZZZZZ are the names of the two coupled inductors, and value is the
coefficient of coupling, K, which must be greater than 0 and less than or equal to 1. Using the
‘dot’ convention, place a ‘dot’ on the first node of each inductor.
3.2.12 Inductors, dependent on expressions (behavioral inductor)
General form:
LXXXXXXX n+ n- L = ’expression ’ <tc1=value > <tc2 =value >
LXXXXXXX n+ n- ’expression ’ <tc1 = value > <tc2=value >
Examples:
L1 l2 lll L = ’i(Vm) < {It} ? {Ll} : {Lh}’ tc1 =-4e -03 tc2 =6e -05
Expression may be an equation or an expression containing node voltages or branch currents
(in the form of i(vm)) and any other terms as given for the B source and described in Chapt. 5.1.
It may contain parameters (2.8.1) and the special variables time,temper, and hertz (5.1.2).
3.2. ELEMENTARY DEVICES 81
Example input file:
Variable inductor
.param Ll =0.5 m Lh =5m It =50 u Vi =2m
.ic v(int21 ) = 0
* variable inductor depending on control current i(Vm)
L1 l2 lll L = ’i(Vm) < {It} ? {Ll} : {Lh}’
* measure current through inductor
vm lll 0 dc 0
* voltage on inductor
V1 l2 0 {Vi}
* fixed inductor
L3 33 331 {Ll}
* measure current through inductor
vm33 331 0 dc 0
* voltage on inductor
V3 33 0 {Vi}
* non linear inductor ( discrete setup )
F21 int21 0 B21 -1
L21 int21 0 1
B21 n1 n2 V = ’(i(Vm21 ) < {It} ? { Ll} : {Lh })’ * v( int21)
* measure current through inductor
vm21 n2 0 dc 0
V21 n1 0 {Vi}
.control
unset askquit
tran 1u 100u uic
plot i(Vm) i( vm33)
plot i(vm21 ) i( vm33)
plot i(vm)-i(vm21)
.endc
.end
3.2.13 Capacitor or inductor with initial conditions
The simulator supports the specification of voltage and current initial conditions on capaci-
tor and inductor models, respectively. These models are not the standard ones supplied with
SPICE3, but are in fact code models that can be substituted for the SPICE models when rea-
listic initial conditions are required. For details please refer to Chapter 12. A XSPICE deck
example using these models is shown below:
*
* This circuit contains a capacitor and an inductor with
82 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
* initial conditions on them. Each of the components
* has a parallel resistor so that an exponential decay
* of the initial condition occurs with a time constant of
* 1 second.
*
a1 1 0 cap
.model cap capacitor (c=1000uf ic=1)
r1 1 0 1k
*
a2 2 0 ind
.model ind inductor (l=1H ic=1)
r2 2 0 1.0
*
.control
tran 0.01 3
plot v(1) v(2)
.endc
.end
3.2.14 Switches
Two types of switches are available: a voltage controlled switch (type SXXXXXX, model SW)
and a current controlled switch (type WXXXXXXX, model CSW). A switching hysteresis may
be defined, as well as on- and off-resistances (0 <R<∞).
General form:
SXXXXXXX N+ N - NC+ NC - MODEL <ON ><OFF >
WYYYYYYY N+ N - VNAM MODEL <ON ><OFF >
Examples:
s1 1 2 3 4 switch1 ON
s2 5 6 3 0 sm2 off
Switch1 1 2 10 0 smodel1
w1 1 2 vclock switchmod1
W2 3 0 vramp sm1 ON
wreset 5 6 vclck lossyswitch OFF
Nodes 1 and 2 are the nodes between which the switch terminals are connected. The model
name is mandatory while the initial conditions are optional. For the voltage controlled switch,
nodes 3 and 4 are the positive and negative controlling nodes respectively. For the current
controlled switch, the controlling current is that through the specified voltage source. The
direction of positive controlling current flow is from the positive node, through the source, to
the negative node.
The instance parameters ON or OFF are required, when the controlling voltage (current) starts
inside the range of the hysteresis loop (different outputs during forward vs. backward voltage
or current ramp). Then ON or OFF determine the initial state of the switch.
3.2. ELEMENTARY DEVICES 83
3.2.15 Switch Model (SW/CSW)
The switch model allows an almost ideal switch to be described in ngspice. The switch is not
quite ideal, in that the resistance can not change from 0 to infinity, but must always have a finite
positive value. By proper selection of the on and off resistances, they can be effectively zero
and infinity in comparison to other circuit elements. The parameters available are:
Name Parameter Units Default Switch model
VT threshold voltage V 0.0 SW
IT threshold current A 0.0 CSW
VH hysteresis voltage V 0.0 SW
IH hysteresis current A 0.0 CSW
RON on resistance Ω1.0 SW,CSW
ROFF off resistance Ω1.0e+12 (*) SW,CSW
(*) Or 1/GMIN, if you have set GMIN to any other value, see the .OPTIONS control line
(15.1.2) for a description of GMIN, its default value results in an off-resistance of 1.0e+12
ohms.
The use of an ideal element that is highly nonlinear such as a switch can cause large discontinui-
ties to occur in the circuit node voltages. A rapid change such as that associated with a switch
changing state can cause numerical round-off or tolerance problems leading to erroneous results
or time step difficulties. The user of switches can improve the situation by taking the following
steps:
• First, it is wise to set ideal switch impedances just high or low enough to be negligible
with respect to other circuit elements. Using switch impedances that are close to ‘ideal’
in all cases aggravates the problem of discontinuities mentioned above. Of course, when
modeling real devices such as MOSFETS, the on resistance should be adjusted to a rea-
listic level depending on the size of the device being modeled.
• If a wide range of ON to OFF resistance must be used in the switches (ROFF/RON >
1e+12), then the tolerance on errors allowed during transient analysis should be decreased
by using the .OPTIONS control line and specifying TRTOL to be less than the default value
of 7.0.
• When switches are placed around capacitors, then the option CHGTOL should also be re-
duced. Suggested values for these two options are 1.0 and 1e-16 respectively. These
changes inform ngspice to be more careful around the switch points so that no errors are
made due to the rapid change in the circuit.
84 CHAPTER 3. CIRCUIT ELEMENTS AND MODELS
Example input file:
Switch test
.tran 2 us 5ms
*switch control voltage
v1 1 0 DC 0.0 PWL (0 0 2e -3 2 4e-3 0)
*switch control voltage starting inside hysteresis window
* please note influence of instance parameters ON , OFF
v2 2 0 DC 0.0 PWL (0 0.9 2e -3 2 4e -3 0.4)
*switch control current
i3 3 0 DC 0.0 PWL (0 0 2e -3 2m 4e-3 0) $ <--- switch control current
*load voltage
v4 4 0 DC 2.0
*input load for current source i3
r3 3 33 10k
vm3 33 0 dc 0 $ <--- measure the current
* ouput load resistors
r10 4 10 10k
r20 4 20 10k
r30 4 30 10k
r40 4 40 10k
*
s1 10 0 1 0 switch1 OFF
s2 20 0 2 0 switch1 OFF
s3 30 0 2 0 switch1 ON
.model switch1 sw vt =1 vh =0.2 ron =1 roff =10k
*
w1 40 0 vm3 wswitch1 off
. model wswitch1 csw it =1 m ih =0.2 m ron =1 roff =10 k
*
.control
run
plot v(1) v(10)
plot v (10) vs v(1) $ <-- get hysteresis loop
plot v(2) v (20) $ <--- different initial values
plot v (20) vs v(2) $ <-- get hysteresis loop
plot v(2) v (30) $ <--- different initial values
plot v (30) vs v(2) $ <-- get hysteresis loop
plot v(40) vs vm3#branch $ <--- current controlled switch hysteresis
.endc
.end
Chapter 4
Voltage and Current Sources
4.1 Independent Sources for Voltage or Current
General form:
VXXXXXXX N+ N - <<DC > DC /TRAN VALUE > <AC < ACMAG <ACPHASE >>>
+ <DISTOF1 <F1MAG <F1PHASE >>> <DISTOF2 <F2MAG <F2PHASE >>>
IYYYYYYY N+ N - <<DC > DC /TRAN VALUE > <AC < ACMAG <ACPHASE >>>
+ <DISTOF1 <F1MAG <F1PHASE >>> <DISTOF2 <F2MAG <F2PHASE >>>
Examples:
VCC 10 0 DC 6
VIN 13 2 0.001 AC 1 SIN (0 1 1MEG )
ISRC 23 21 AC 0.333 45.0 SFFM (0 1 10K 5 1K)
VMEAS 12 9
VCARRIER 1 0 DISTOF1 0.1 -90.0
VMODULATOR 2 0 DISTOF2 0.01
IIN1 1 5 AC 1 DISTOF1 DISTOF2 0.001
n+ and n- are the positive and negative nodes, respectively. Note that voltage sources need not
be grounded. Positive current is assumed to flow from the positive node, through the source, to
the negative node. A current source of positive value forces current to flow out of the n+ node,
through the source, and into the n- node. Voltage sources, in addition to being used for circuit
excitation, are the ‘ammeters’ for ngspice, that is, zero valued voltage sources may be inserted
into the circuit for the purpose of measuring current. They of course have no effect on circuit
operation since they represent short-circuits.
DC/TRAN is the dc and transient analysis value of the source. If the source value is zero both for
dc and transient analyses, this value may be omitted. If the source value is time-invariant (e.g.,
a power supply), then the value may optionally be preceded by the letters DC.
ACMAG is the ac magnitude and ACPHASE is the ac phase. The source is set to this value in the
ac analysis. If ACMAG is omitted following the keyword AC, a value of unity is assumed. If
ACPHASE is omitted, a value of zero is assumed. If the source is not an ac small-signal input,
the keyword AC and the ac values are omitted.
85
86 CHAPTER 4. VOLTAGE AND CURRENT SOURCES
DISTOF1 and DISTOF2 are the keywords that specify that the independent source has distortion
inputs at the frequencies F1 and F2 respectively (see the description of the .DISTO control line).
The keywords may be followed by an optional magnitude and phase. The default values of the
magnitude and phase are 1.0 and 0.0 respectively.
Any independent source can be assigned a time-dependent value for transient analysis. If a
source is assigned a time-dependent value, the time-zero value is used for dc analysis. There
are nine independent source functions:
• pulse,
• exponential,
• sinusoidal,
• piece-wise linear,
• single-frequency FM
• AM
• transient noise
• random voltages or currents
• and external data (only with ngspice shared library).
If parameters other than source values are omitted or set to zero, the default values shown are
assumed. TSTEP is the printing increment and TSTOP is the final time – see the .TRAN control
line for an explanation.
4.1.1 Pulse
General form (the PHASE parameter is only possible when XSPICE is enabled):
PULSE(V1 V2 TD TR TF PW PER PHASE )
Examples:
VIN 3 0 PULSE ( -1 1 2NS 2 NS 2NS 50 NS 100 NS )
Name Parameter Default Value Units
V1 Initial value - V,A
V2 Pulsed value - V,A
TD Delay time 0.0 sec
TR Rise time TSTEP sec
TF Fall time TSTEP sec
PW Pulse width TSTOP sec
PER Period TSTOP sec
PHASE Phase 0.0 degrees
4.1. INDEPENDENT SOURCES FOR VOLTAGE OR CURRENT 87
A single pulse, without phase offset, is described by the following table:
Time Value
0 V1
TD V1
TD+TR V2
TD+TR+PW V2
TD+TR+PW+TF V1
TSTOP V1
Intermediate points are determined by linear interpolation.
4.1.2 Sinusoidal
General form (the PHASE parameter is only possible when XSPICE is enabled):
SIN(VO VA FREQ TD THETA PHASE )
Examples:
VIN 3 0 SIN (0 1 100 MEG 1NS 1 E10)
Name Parameter Default Value Units
VO Offset - V,A
VA Amplitude - V,A
FREQ Frequency 1
/T ST OP Hz
TD Delay 0.0 sec
THETA Damping factor 0.0 1
/sec
PHASE Phase 0.0 degrees
The shape of the waveform is described by the following formula:
V(t) = (V0 if 0 ≤t<T D
V0+VA e−(t−T D)T HETA sin(2π·FREQ ·(t−T D) + PHASE)if T D ≤t<T ST OP.
(4.1)
4.1.3 Exponential
General Form:
EXP(V1 V2 TD1 TAU1 TD2 TAU2 )
Examples:
VIN 3 0 EXP(-4 -1 2NS 30 NS 60 NS 40 NS)
88 CHAPTER 4. VOLTAGE AND CURRENT SOURCES
Name Parameter Default Value Units
V1 Initial value - V,A
V2 pulsed value - V,A
TD1 rise delay time 0.0 sec
TAU1 rise time constant TSTEP sec
TD2 fall delay time TD1+TSTEP sec
TAU2 fall time constant TSTEP sec
The shape of the waveform is described by the following formula:
Let V21 =V2−V1,V12 =V1−V2:
V(t) =
V1 if 0 ≤t<T D1,
V1+V211−e−(t−T D1)
TAU 1if T D1≤t<T D2,
V1+V211−e−(t−T D1)
TAU 1+V121−e−(t−T D2)
TAU 2if T D2≤t<T ST OP.
(4.2)
4.1.4 Piece-Wise Linear
General Form:
PWL(T1 V1 <T2 V2 T3 V3 T4 V4 ... >) <r=value > <td=value >
Examples:
VCLOCK 7 5 PWL(0 -7 10 NS -7 11NS -3 17 NS -3 18NS -7 50 NS -7)
+ r=0 td =15 NS
Each pair of values (Ti,Vi) specifies that the value of the source is Vi(in Volts or Amps) at
time = Ti. The value of the source at intermediate values of time is determined by using linear
interpolation on the input values. The parameter rdetermines a repeat time point. If ris not
given, the whole sequence of values (Ti,Vi) is issued once, then the output stays at its final
value. If r = 0, the whole sequence from time 0 to time Tn is repeated forever. If r = 10ns, the
sequence between 10ns and 50ns is repeated forever. the rvalue has to be one of the time points
T1 to Tn of the PWL sequence. If td is given, the whole PWL sequence is delayed by the value
of td.
4.1.5 Single-Frequency FM
General Form (the PHASE parameters are only possible when XSPICE is enabled):
SFFM(VO VA FC MDI FS PHASEC PHASES )
Examples:
V1 12 0 SFFM (0 1M 20K 5 1K)
4.1. INDEPENDENT SOURCES FOR VOLTAGE OR CURRENT 89
Name Parameter Default value Units
VO Offset - V,A
VA Amplitude - V,A
FC Carrier frequency 1
/T ST OP Hz
MDI Modulation index -
FS Signal frequency 1
/T ST OP Hz
PHASEC carrier phase 0 degrees
PHASES signal phase 0 degrees
The shape of the waveform is described by the following equation:
V(t) = VO+VAsin (2π·FC ·t+MDI sin(2π·FS ·t+PHASES) + PHASEC)(4.3)
4.1.6 Amplitude modulated source (AM)
General Form (the PHASE parameter is only possible when XSPICE is enabled):
AM(VA VO MF FC TD PHASES)
Examples:
V1 12 0 AM (0.5 1 20K 5MEG 1m)
Name Parameter Default value Units
VA Amplitude - V,A
VO Offset - V,A
MF Modulating frequency - Hz
FC Carrier frequency 1
/T ST OP Hz
TD Signal delay - s
PHASES Phase 0.0 degrees
The shape of the waveform is described by the following equation:
V(t) = VA(VO +sin (2π·MF ·t) + PHASES)sin(2π·FC ·t+PHASES)(4.4)
90 CHAPTER 4. VOLTAGE AND CURRENT SOURCES
4.1.7 Transient noise source
General Form:
TRNOISE(NA NT NALPHA NAMP RTSAM RTSCAPT RTSEMT )
Examples:
VNoiw 1 0 DC 0 TRNOISE (20n 0.5n 0 0) $ white
VNoi1of 1 0 DC 0 TRNOISE (0 10 p 1.1 12p) $ 1/f
VNoiw1of 1 0 DC 0 TRNOISE (20 10p 1.1 12p) $ white and 1/f
IALL 10 0 DC 0 trnoise (1 m 1u 1.0 0.1m 15m 22u 50u)
$ white , 1/f, RTS
Transient noise is an experimental feature allowing (low frequency) transient noise injection
and analysis. See Chapt. 15.3.10 for a detailed description. NA is the Gaussian noise rms
voltage amplitude, NT is the time between sample values (breakpoints will be enforced on mul-
tiples of this value). NALPHA (exponent to the frequency dependency), NAMP (rms voltage or
current amplitude) are the parameters for 1/f noise, RTSAM the random telegraph signal ampli-
tude, RTSCAPT the mean of the exponential distribution of the trap capture time, and RTSEMT
its emission time mean. White Gaussian, 1/f, and RTS noise may be combined into a single
statement.
Name Parameter Default value Units
NA Rms noise amplitude (Gaussian) - V,A
NT Time step - sec
NALPHA 1/f exponent 0 <α<2 -
NAMP Amplitude (1/f) - V,A
RTSAM Amplitude - V,A
RTSCAPT Trap capture time - sec
RTSEMT Trap emission time - sec
If you set NT and RTSAM to 0, the noise option TRNOISE ... is ignored. Thus you may switch off
the noise contribution of an individual voltage source VNOI by the command
alter @vnoi[trnoise] = [ 0 0 0 0 ] $ no noise
alter @vrts[trnoise] = [ 0 0 0 0 0 0 0] $ no noise
See Chapt. 17.5.3 for the alter command.
You may switch off all TRNOISE noise sources by setting
set notrnoise
to your .spiceinit file (for all your simulations) or into your control section in front of the next
run or tran command (for this specific and all following simulations). The command
unset notrnoise
will reinstate all noise sources.
The noise generators are implemented into the independent voltage (vsrc) and current (isrc)
sources.
4.1. INDEPENDENT SOURCES FOR VOLTAGE OR CURRENT 91
4.1.8 Random voltage source
The TRRANDOM option yields statistically distributed voltage values, derived from the ngspice
random number generator. These values may be used in the transient simulation directly within
a circuit, e.g. for generating a specific noise voltage, but especially they may be used in the
control of behavioral sources (B, E, G sources 5, voltage controllable A sources 12, capacitors
3.2.8, inductors 3.2.12, or resistors 3.2.4) to simulate the circuit dependence on statistically va-
rying device parameters. A Monte-Carlo simulation may thus be handled in a single simulation
run.
General Form:
TRRANDOM ( TYPE TS <TD <PARAM1 <PARAM2 >>>)
Examples:
VR1 r1 0 dc 0 trrandom (2 10m 0 1) $ Gaussian
TYPE determines the random variates generated: 1 is uniformly distributed, 2 Gaussian, 3 ex-
ponential, 4 Poisson. TS is the duration of an individual voltage value. TD is a time delay with
0 V output before the random voltage values start up. PARAM1 and PARAM2 depend on the type
selected.
TYPE description PARAM1 default PARAM2 default
1 Uniform Range 1 Offset 0
2 Gaussian Standard Dev. 1 Mean 0
3 Exponential Mean 1 Offset 0
4 Poisson Lambda 1 Offset 0
4.1.9 External voltage or current input
General Form:
EXTERNAL
Examples:
Vex 1 0 dc 0 external
Iex i1 i2 dc 0 external <m = xx >
Voltages or currents may be set from the calling process, if ngspice is compiled as a shared
library and loaded by the process. See Chapt. 19.6.3 for an explanation.
92 CHAPTER 4. VOLTAGE AND CURRENT SOURCES
4.1.10 Arbitrary Phase Sources
The XSPICE option supports arbitrary phase independent sources that output at TIME=0.0 a
value corresponding to some specified phase shift. Other versions of SPICE use the TD (delay
time) parameter to set phase-shifted sources to their time-zero value until the delay time has
elapsed. The XSPICE phase parameter is specified in degrees and is included after the SPICE3
parameters normally used to specify an independent source. Partial XSPICE deck examples of
usage for pulse and sine waveforms are shown below:
* Phase shift is specified after Berkeley defined parameters
* on the independent source cards. Phase shift for both of the
* following is specified as +45 degrees
*
v1 1 0 0.0 sin(0 1 1k 0 0 45.0)
r1 1 0 1k
*
v2 2 0 0.0 pulse(-1 1 0 1e-5 1e-5 5e-4 1e-3 45.0)
r2 2 0 1k
*
4.2 Linear Dependent Sources
Ngspice allows circuits to contain linear dependent sources characterized by any of the four
equations
i=gv v =ev i =f i v =hi
where g,e,f, and hare constants representing transconductance, voltage gain, current gain,
and transresistance, respectively. Non-linear dependent sources for voltages or currents (B, E,
G) are described in Chapt. 5.
4.2.1 Gxxxx: Linear Voltage-Controlled Current Sources (VCCS)
General form:
GXXXXXXX N+ N - NC+ NC - VALUE <m= val >
Examples:
G1 2 0 5 0 0.1
n+ and n- are the positive and negative nodes, respectively. Current flow is from the positive
node, through the source, to the negative
node. nc+ and nc- are the positive and negative controlling nodes, respectively. value is the
transconductance (in mhos). mis an optional multiplier to the output current. val may be a
numerical value or an expression according to 2.8.5 containing references to other parameters.
4.2. LINEAR DEPENDENT SOURCES 93
4.2.2 Exxxx: Linear Voltage-Controlled Voltage Sources (VCVS)
General form:
EXXXXXXX N+ N - NC+ NC - VALUE
Examples:
E1 2 3 14 1 2.0
n+ is the positive node, and n- is the negative node. nc+ and nc- are the positive and negative
controlling nodes, respectively. value is the voltage gain.
4.2.3 Fxxxx: Linear Current-Controlled Current Sources (CCCS)
General form:
FXXXXXXX N+ N- VNAM VALUE <m=val >
Examples:
F1 13 5 VSENS 5 m=2
n+ and n- are the positive and negative nodes, respectively. Current flow is from the positive
node, through the source, to the negative node. vnam is the name of a voltage source through
which the controlling current flows. The direction of positive controlling current flow is from
the positive node, through the source, to the negative node of vnam.value is the current gain.
mis an optional multiplier to the output current.
4.2.4 Hxxxx: Linear Current-Controlled Voltage Sources (CCVS)
General form:
HXXXXXXX n+ n- vnam value
Examples:
HX 5 17 VZ 0.5K
n+ and n- are the positive and negative nodes, respectively. vnam is the name of a voltage source
through which the controlling current flows. The direction of positive controlling current flow
is from the positive node, through the source, to the negative node of vnam.value is the
transresistance (in ohms).
94 CHAPTER 4. VOLTAGE AND CURRENT SOURCES
4.2.5 Polynomial Source Compatibility
Dependent polynomial sources available in SPICE2G6 are fully supported in ngspice using the
XSPICE extension (25.1). The form used to specify these sources is shown in Table 4.1. For
details on its usage please see Chapt. 5.2.4.
Dependent Polynomial Sources
Source Type Instance Card
POLYNOMIAL VCVS EXXXXXXX N+ N- POLY(ND) NC1+ NC1- P0 (P1...)
POLYNOMIAL VCCS GXXXXXXX N+ N- POLY(ND) NC1+ NC1- P0 (P1...)
POLYNOMIAL CCCS FXXXXXXX N+ N- POLY(ND) VNAM1 !VNAM2...? P0 (P1...)
POLYNOMIAL CCVS HXXXXXXX N+ N- POLY(ND) VNAM1 !VNAM2...? P0 (P1...)
Table 4.1: Dependent Polynomial Sources
Chapter 5
Non-linear Dependent Sources (Behavioral
Sources)
The non-linear dependent sources B ( see Chapt. 5.1), E (see 5.2), G see (5.3) described in
this chapter allow to generate voltages or currents that result from evaluating a mathematical
expression. Internally E and G sources are converted to the more general B source. All three
sources may be used to introduce behavioral modeling and analysis.
5.1 Bxxxx: Nonlinear dependent source (ASRC)
5.1.1 Syntax and usage
General form:
BXXXXXXX n+ n- <i=expr > <v=expr > <tc1=value > <tc2=value >
+ <temp =value > <dtemp =value >
Examples:
B1 0 1 I= cos(v(1))+ sin(v(2))
B2 0 1 V=ln( cos (log (v (1 ,2)^2))) - v (3)^4+ v(2)^ v(1)
B3 3 4 I=17
B4 3 4 V= exp(pi^i(vdd))
B5 2 0 V = V(1) < {Vlow} ? {Vlow } :
+ V(1) > {Vhigh } ? { Vhigh} : V(1)
n+ is the positive node, and n- is the negative node. The values of the Vand Iparameters
determine the voltages and currents across and through the device, respectively. If Iis given
then the device is a current source, and if Vis given the device is a voltage source. One and only
one of these parameters must be given.
A simple model is implemented for temperature behavior by the formula:
I(T) = I(TNOM)1+TC1(T−TNOM) + TC2(T−TNOM)2(5.1)
95
96 CHAPTER 5. NON-LINEAR DEPENDENT SOURCES (BEHAVIORAL SOURCES)
or
V(T) = V(TNOM)1+TC1(T−TNOM) + TC2(T−TNOM)2(5.2)
In the above formula, ‘T’ represents the instance temperature, which can be explicitly set using
the temp keyword or calculated using the circuit temperature and dtemp, if present. If both
temp and dtemp are specified, the latter is ignored.
The small-signal AC behavior of the nonlinear source is a linear dependent source (or sources)
with a proportionality constant equal to the derivative (or derivatives) of the source at the DC
operating point. The expressions given for Vand Imay be any function of voltages and currents
through voltage sources in the system.
The following functions of a single real variable are defined:
Trigonometric functions: cos, sin, tan, acos, asin, atan
Hyperbolic functions: cosh, sinh, acosh, asinh, atanh
Exponential and logarithmic: exp, ln, log, log10 (ln, log with base e, log10 with base 10)
Other: abs, sqrt, u, u2, uramp, floor, ceil
Functions of two variables are: min, max, pow
Functions of three variables are: a ? b:c
The function ‘u’ is the unit step function, with a value of one for arguments greater than zero
and a value of zero for arguments less than zero. The function ‘u2’ returns a value of zero
for arguments less than zero, one for arguments greater than one and assumes the value of the
argument between these limits. The function ‘uramp’ is the integral of the unit step: for an
input x, the value is zero if x is less than zero, or if x is greater than zero the value is x. These
three functions are useful in synthesizing piece-wise non-linear functions, though convergence
may be adversely affected.
The following standard operators are defined: +,-,*,/,^, unary -
Logical operators are !=,<>,>=,<=,==,>,<,||,&&,!.
A ternary function is defined as a ? b : c , which means IF a, THEN b, ELSE c. Be
sure to place a space in front of ‘?’ to allow the parser distinguishing it from other tokens.
5.1. BXXXX: NONLINEAR DEPENDENT SOURCE (ASRC) 97
Example: Ternary function
* B source test Clamped voltage source
* C. P. Basso "Switched -mode power supplies ", New York , 2008
.param Vhigh = 4.6
.param Vlow = 0.4
Vin1 1 0 DC 0 PWL (0 0 1u 5)
Bcl 2 0 V = V(1) < Vlow ? Vlow : V(1) > Vhigh ? Vhigh : V(1)
.control
unset askquit
tran 5n 1u
plot V (2) vs V(1)
.endc
.end
If the argument of log, ln, or sqrt becomes less than zero, the absolute value of the argument is
used. If a divisor becomes zero or the argument of log or ln becomes zero, an error will result.
Other problems may occur when the argument for a function in a partial derivative enters a
region where that function is undefined.
Parameters may be used like {Vlow} shown in the example above. Parameters will be evaluated
upon set up of the circuit, vectors like V(1) will be evaluated during the simulation.
To get time into the expression you can integrate the current from a constant current source
with a capacitor and use the resulting voltage (don’t forget to set the initial voltage across the
capacitor).
Non-linear resistors, capacitors, and inductors may be synthesized with the nonlinear dependent
source. Nonlinear resistors, capacitors and inductors are implemented with their linear counter-
parts by a change of variables implemented with the nonlinear dependent source. The following
subcircuit will implement a nonlinear capacitor:
Example: Non linear capacitor
.Subckt nlcap pos neg
* Bx: calculate f(input voltage )
Bx 1 0 v = f(v(pos ,neg ))
* Cx: linear capacitance
Cx 2 0 1
* Vx: Ammeter to measure current into the capacitor
Vx 2 1 DC 0 Volts
* Drive the current through Cx back into the circuit
Fx pos neg Vx 1
.ends
Example for f(v(pos,neg)):
Bx 1 0 V = v(pos ,neg )*v(pos ,neg )
Non-linear resistors or inductors may be described in a similar manner. An example for a
nonlinear resistor using this template is shown below.
98 CHAPTER 5. NON-LINEAR DEPENDENT SOURCES (BEHAVIORAL SOURCES)
Example: Non linear resistor
* use of ’hertz ’ variable in nonlinear resistor
*. param rbase =1 k
* some tests
B1 1 0 V = hertz *v(33)
B2 2 0 V = v (33)* hertz
b3 3 0 V = 6.283 e3 /( hertz +6.283 e3 )*v(33)
V1 33 0 DC 0 AC 1
*** Translate R1 10 0 R=’1k/sqrt ( HERTZ)’ to B source ***
.Subckt nlres pos neg rb= rbase
* Bx: calculate f(input voltage )
Bx 1 0 v = -1 / {rb} / sqrt ( HERTZ) * v(pos , neg )
* Rx: linear resistance
Rx 2 0 1
Example: Non linear resistor (continued)
* Vx: Ammeter to measure current into the resistor
Vx 2 1 DC 0 Volts
* Drive the current through Rx back into the circuit
Fx pos neg Vx 1
.ends
Xres 33 10 nlres rb =1 k
*Rres 33 10 1k
Vres 10 0 DC 0
.control
define check(a,b) vecmax(abs (a - b))
ac lin 10 100 1k
* some checks
print v(1) v(2) v(3)
if check (v(1) , frequency ) < 1e -12
echo " INFO: ok"
end
plot vres # branch
.endc
.end
5.1.2 Special B-Source Variables time, temper, hertz
The special variables time and temper are available in a transient analysis, reflecting the actual
simulation time and circuit temperature. temper returns the circuit temperature, given in degree
C (see 2.11). The variable hertz is available in an AC analysis. time is zero in the AC analysis,
hertz is zero during transient analysis. Using the variable hertz may cost some CPU time if
you have a large circuit, because for each frequency the operating point has to be determined
before calculating the AC response.
5.1. BXXXX: NONLINEAR DEPENDENT SOURCE (ASRC) 99
5.1.3 par(’expression’)
The B source syntax may also be used in output lines like .plot as algebraic expressions for
output (see Chapt.15.6.6 ).
5.1.4 Piecewise Linear Function: pwl
Both B source types may contain a piece-wise linear dependency of one network variable:
Example: pwl_current
Bdio 1 0 I = pwl(v(A), 0,0, 33 ,10m, 100 ,33m, 200 ,50m)
v(A) is the independent variable x. Each pair of values following describes the x,y functional
relation: In this example at node A voltage of 0V the current of 0A is generated - next pair gives
10mA flowing from ground to node 1 at 33V on node A and so forth.
The same is possible for voltage sources:
Example: pwl_voltage
Blimit b 0 V = pwl(v(1), -4,0, -2,2, 2,4, 4,5, 6 ,5)
Monotony of the independent variable in the pwl definition is checked - non-monotonic x entries
will stop the program execution. v(1) may be replaced by a controlling current source. v(1) may
also be replaced by an expression, e.g. −2i(Vin). The value pairs may also be parameters, and
have to be predefined by a .param statement. An example for the pwl function using all of
these options is shown below.
100 CHAPTER 5. NON-LINEAR DEPENDENT SOURCES (BEHAVIORAL SOURCES)
Example: pwl function in B source
Demonstrates usage of the pwl function in an B source ( ASRC)
* Also emulates the TABLE function with limits
.param x0 = -4 y0 =0
.param x1 = -2 y1 =2
.param x2 =2 y2=-2
.param x3 =4 y3=1
.param xx0=x0 -1
.param xx3= x3 +1
Vin 1 0 DC=0V
R102
* no limits outside of the tabulated x values
* (continues linearily)
Btest2 2 0 I = pwl (v (1) ,’x0 ’,’y0 ’,’x1 ’ ,’y1 ’,’x2 ’ ,’y2 ’,’x3 ’ ,’y3 ’)
* like TABLE function with limits:
Btest3 3 0 I = (v(1) < ’x0 ’) ? ’y0 ’ :
(v(1) < ’x3 ’) ?
+ pwl (v (1) ,’x0 ’,’y0 ’,’x1 ’,’y1 ’ ,’x2 ’,’y2 ’ ,’x3 ’,’y3 ’) : ’y3 ’
* more efficient and elegant TABLE function with limits
*( voltage controlled ):
Btest4 4 0 I = pwl(v(1),
+ ’xx0 ’,’ y0 ’ , ’x0 ’,’y0 ’,
+ ’x1 ’,’y1 ’,
+ ’x2 ’,’y2 ’,
+ ’x3 ’,’y3 ’, ’xx3 ’ ,’y3 ’)
*
* more efficient and elegant TABLE function with limits
* ( controlled by current ):
Btest5 5 0 I = pwl ( -2*i( Vin),
+ ’xx0 ’,’ y0 ’ , ’x0 ’,’y0 ’,
+ ’x1 ’,’y1 ’,
+ ’x2 ’,’y2 ’,
+ ’x3 ’,’y3 ’, ’xx3 ’ ,’y3 ’)
Rint2 2 0 1
Rint3 3 0 1
Rint4 4 0 1
Rint5 5 0 1
.control
dc Vin -6 6 0.2
plot v(2) v(3) v(4) -0.5 v (5)+0.5
.endc
.end
5.2. EXXXX: NON-LINEAR VOLTAGE SOURCE2101
5.2 Exxxx: non-linear voltage source1
5.2.1 VOL
General form:
EXXXXXXX n+ n- vol=’expr ’
Examples:
E41 4 0 vol = ’V (3)* V(3) - Offs ’
Expression may be an equation or an expression containing node voltages or branch currents
(in the form of i(vm)) and any other terms as given for the B source and described in Chapt.
5.1. It may contain parameters (2.8.1) and the special variables time,temper,hertz (5.1.2).
’or { } may be used to delimit the function.
5.2.2 VALUE
Optional syntax:
EXXXXXXX n+ n - value ={ expr }
Examples:
E41 4 0 value = {V (3)* V (3) - Offs }
The ’=’ sign is optional.
5.2.3 TABLE
Data may be entered from the listings of a data table similar to the pwl B-Source (5.1.4). Data
are grouped into x, y pairs. Expression may be an equation or an expression containing node
voltages or branch currents (in the form of i(vm)) and any other terms as given for the B source
and described in Chapt. 5.1. It may contain parameters (2.8.1). ’or { } may be used to delimit
the function. Expression delivers the x-value, which is used to generate a corresponding y-
value according to the tabulated value pairs, using linear interpolation. If the x-value is below
x0 , y0 is returned, above x2 y2 is returned (limiting function). The value pairs have to be real
numbers, parameters are not allowed.
1To get this functionality, the compatibility mode has to be set in spinit or .spiceinit by set ngbehavior=all.
102 CHAPTER 5. NON-LINEAR DEPENDENT SOURCES (BEHAVIORAL SOURCES)
Syntax for data entry from table:
Exxx n1 n2 TABLE {expression } = (x0 , y0) (x1 , y1) (x2 , y2)
Example (simple comparator):
ECMP 11 0 TABLE {V (10 ,9)} = (-5mV , 0V) (5mV , 5V)
An ’=’ sign may follow the keyword TABLE.
5.2.4 POLY
Polynomial sources are only available when the XSPICE option (see 32) is enabled.
General form:
EXXXX N+ N- POLY(ND) NC1+ NC1 - (NC2+ NC2 -...) P0 (P1 ...)
Example:
ENONLIN 100 101 POLY (2) 3 0 4 0 0.0 13.6 0.2 0.005
POLY(ND) Specifies the number of dimensions of the polynomial. The number of pairs of
controlling nodes must be equal to the number of dimensions.
(N+) and (N-) nodes are output nodes. Positive current flows from the (+) node through the
source to the (-) node.
The <NC1+> and <NC1-> are in pairs and define a set of controlling voltages. A particular node
can appear more than once, and the output and controlling nodes need not be different.
The example yields a voltage output controlled by two input voltages v(3,0) and v(4,0). Four
polynomial coefficients are given. The equivalent function to generate the output is:
0 + 13.6 * v(3) + 0.2 * v(4) + 0.005 * v(3) * v(3)
Generally you will set the equation according to
POLY(1) y = p0 + k1*X1 + p2*X1*X1 + p3*X1*X1*X1 + ...
POLY(2) y = p0 + p1*X1 + p2*X2 +
+ p3*X1*X1 + p4*X2*X1 + p5*X2*X2 +
+ p6*X1*X1*X1 + p7*X2*X1*X1 + p8*X2*X2*X1 +
+ p9*X2*X2*X2 + ...
POLY(3) y = p0 + p1*X1 + p2*X2 + p3*X3 +
+ p4*X1*X1 + p5*X2*X1 + p6*X3*X1 +
+ p7*X2*X2 + p8*X2*X3 + p9*X3*X3 + ...
where X1 is the voltage difference of the first input node pair, X2 of the second pair and so on.
Keeping track of all polynomial coefficient is rather tedious for large polynomials.
5.2. EXXXX: NON-LINEAR VOLTAGE SOURCE4103
5.2.5 LAPLACE
Currently ngspice does not offer a direct E-Source element with the LAPLACE option. There
is however a XSPICE code model equivalent called s_xfer (see Chapt. 12.2.16), which you
may invoke manually. The XSPICE option has to be enabled (32.1). AC (15.3.1) and transient
analysis (15.3.9) is supported.
The following E-Source:
ELOPASS 4 0 LAPLACE {V (1)}
+ {5 * (s /100 + 1) / (s ^2/42000 + s/60 + 1)}
may be replaced by:
AELOPASS 1 int_4 filter1
. model filter1 s_xfer ( gain =5
+ num_coeff =[{1/100} 1]
+ den_coeff =[{1/42000} {1/60} 1]
+ int_ic =[0 0])
ELOPASS 4 0 int_4 0 1
where you have the voltage of node 1 as input, an intermediate output node int_4 and an E-
source as buffer to keep the name ‘ELOPASS’ available if further processing is required.
If the controlling expression is more complex than just a voltage node, you may add a B-Source
(5.1) for evaluating the expression before entering the A-device.
E-Source with complex controlling expression:
ELOPASS 4 0 LAPLACE {V (1)*v(2)} {10 / (s /6800 + 1)}
may be replaced by:
BELOPASS int_1 0 V=V (1)* v(2)
AELOPASS int_1 int_4 filter1
. model filter1 s_xfer ( gain =10
+ num_coeff =[1]
+ den_coeff =[{1/6800} 1]
+ int_ic =[0])
ELOPASS 4 0 int_4 0 1
104 CHAPTER 5. NON-LINEAR DEPENDENT SOURCES (BEHAVIORAL SOURCES)
5.3 Gxxxx: non-linear current source3
5.3.1 CUR
General form:
GXXXXXXX n+ n- cur=’expr ’ <m=val >
Examples:
G51 55 225 cur = ’V(3)* V (3) - Offs ’
Expression may be an equation or an expression containing node voltages or branch currents
(in the form of i(vm)) and any other terms as given for the B source and described in Chapt.
5.1. It may contain parameters (2.8.1) and special variables (5.1.2). mis an optional multiplier
to the output current. val may be a numerical value or an expression according to 2.8.5 con-
taining only references to other parameters (no node voltages or branch currents!), because it is
evaluated before the simulation commences.
5.3.2 VALUE
Optional syntax:
GXXXXXXX n+ n- value=’expr ’ <m=val >
Examples:
G51 55 225 value = ’V (3)*V(3) -Offs ’
The ’=’ sign is optional.
5.3.3 TABLE
A data entry by a tabulated listing is available with syntax similar to the E-Source (see Chapt.
5.2.3).
3To get this functionality, the compatibility mode has to be set in spinit or .spiceinit by set ngbehavior=all.
5.3. GXXXX: NON-LINEAR CURRENT SOURCE5105
Syntax for data entry from table:
Gxxx n1 n2 TABLE {expression } =
+ (x0 , y0) (x1 , y1) (x2 , y2) <m=val >
Example (simple comparator with current output and voltage control):
GCMP 0 11 TABLE {V (10 ,9)} = (-5MV , 0V) (5MV , 5V)
R 11 0 1k
mis an optional multiplier to the output current. val may be a numerical value or an expression
according to 2.8.5 containing only references to other parameters (no node voltages or branch
currents!), because it is evaluated before the simulation commences. An ’=’ sign may follow
the keyword TABLE.
5.3.4 POLY
see E-Source at Chapt. 5.2.4.
5.3.5 LAPLACE
See E-Source, Chapt. 5.2.5 , for an equivalent code model replacement.
5.3.6 Example
An example file is given below.
106 CHAPTER 5. NON-LINEAR DEPENDENT SOURCES (BEHAVIORAL SOURCES)
Example input file:
VCCS , VCVS , non - linear dependency
.param Vi =1
. param Offs = ’0.01* Vi ’
* VCCS depending on V(3)
B21 int1 0 V = V(3)*V(3)
G1 21 22 int1 0 1
* measure current through VCCS
vm 22 0 dc 0
R21 21 0 1
* new VCCS depending on V(3)
G51 55 225 cur = ’V(3)* V (3) - Offs ’
* measure current through VCCS
vm5 225 0 dc 0
R51 55 0 1
* VCVS depending on V(3)
B31 int2 0 V = V(3)*V(3)
E1 1 0 int2 0 1
R1 1 0 1
* new VCVS depending on V(3)
E41 4 0 vol = ’V (3)* V(3) - Offs ’
R4 4 0 1
* control voltage
V1 3 0 PWL (0 0 100u {Vi })
.control
unset askquit
tran 10n 100u uic
plot i(E1) i( E41)
plot i(vm) i( vm5)
.endc
.end
5.4 Debugging a behavioral source
The B, E, G, sources and the behavioral R, C, L elements are powerful tools to set up user
defined models. Unfortunately debugging these models is not very comfortable.
5.4. DEBUGGING A BEHAVIORAL SOURCE 107
Example input file with bug (log(-2)):
B source debugging
V1 1 0 1
V2 2 0 -2
E41 4 0 vol = ’V (1)* log(V(2)) ’
.control
tran 1 1
.endc
.end
The input file given above results in an error message:
Error: -2 out of range for log
In this trivial example, the reason and location for the bug is obvious. However, if you have
several equations using behavioral sources, and several occurrences of the log function, then
debugging is nearly impossible.
However, if the variable ngdebug (see 17.7) is set (e.g. in file .spiceinit), a more distinctive
error message is issued that (after some closer investigation) will reveal the location and value
of the buggy parameter.
Detailed error message for input file with bug (log(-2)):
Error: -2 out of range for log
calling PTeval , tree =
(v0) * (log (v1))
d / d v0 : log (v1)
d / d v1 : (v0) * ((0.434294) / (v1 ))
values: var0 = 1
var1 = -2
If variable strict_errorhandling (see 17.7) is set, ngspice exits after this message. If not,
gmin and source stepping may be started, typically without success.
108 CHAPTER 5. NON-LINEAR DEPENDENT SOURCES (BEHAVIORAL SOURCES)
Chapter 6
Transmission Lines
Ngspice implements both the original SPICE3f5 transmission lines models and the one introdu-
ced with KSPICE. The latter provide an improved transient analysis of lossy transmission lines.
Unlike SPICE models that use the state-based approach to simulate lossy transmission lines,
KSPICE simulates lossy transmission lines and coupled multiconductor line systems using the
recursive convolution method. The impulse response of an arbitrary transfer function can be
determined by deriving a recursive convolution from the Pade approximations of the function.
We use this approach for simulating each transmission line’s characteristics and each multi-
conductor line’s modal functions. This method of lossy transmission line simulation has been
proved to give a speedup of one to two orders of magnitude over SPICE3f5.
6.1 Lossless Transmission Lines
General form:
TXXXXXXX N1 N2 N3 N4 Z0 = VALUE <TD=VALUE >
+ <F= FREQ <NL =NRMLEN >> <IC= V1 , I1 , V2 , I2 >
Examples:
T1 1 0 2 0 Z0=50 TD =10 NS
n1 and n2 are the nodes at port 1; n3 and n4 are the nodes at port 2. z0 is the characteristic
impedance. The length of the line may be expressed in either of two forms. The transmission
delay, td, may be specified directly (as td=10ns, for example). Alternatively, a frequency f
may be given, together with nl, the normalized electrical length of the transmission line with
respect to the wavelength in the line at the frequency ‘f’. If a frequency is specified but nl is
omitted, 0.25 is assumed (that is, the frequency is assumed to be the quarter-wave frequency).
Note that although both forms for expressing the line length are indicated as optional, one of
the two must be specified.
Note that this element models only one propagating mode. If all four nodes are distinct in the ac-
tual circuit, then two modes may be excited. To simulate such a situation, two transmission-line
elements are required. (see the example in Chapt. 21.7 for further clarification.) The (optional)
109
110 CHAPTER 6. TRANSMISSION LINES
initial condition specification consists of the voltage and current at each of the transmission line
ports. Note that the initial conditions (if any) apply only if the UIC option is specified on the
.TRAN control line.
Note that a lossy transmission line (see below) with zero loss may be more accurate than the
lossless transmission line due to implementation details.
6.2 Lossy Transmission Lines
General form:
OXXXXXXX n1 n2 n3 n4 mname
Examples:
O23 1 0 2 0 LOSSYMOD
OCONNECT 10 5 20 5 INTERCONNECT
This is a two-port convolution model for single conductor lossy transmission lines. n1 and n2
are the nodes at port 1; n3 and n4 are the nodes at port 2. Note that a lossy transmission line
with zero loss may be more accurate than the lossless transmission line due to implementation
details.
6.2.1 Lossy Transmission Line Model (LTRA)
The uniform RLC/RC/LC/RG transmission line model (referred to as the LTRA model hen-
ceforth) models a uniform constant-parameter distributed transmission line. The RC and LC
cases may also be modeled using the URC and TRA models; however, the newer LTRA model
is usually faster and more accurate than the others. The operation of the LTRA model is based
on the convolution of the transmission line’s impulse responses with its inputs (see [8]). The
LTRA model takes a number of parameters, some of which must be given and some of which
are optional.
6.2. LOSSY TRANSMISSION LINES 111
Name Parameter Units/Type Default Example
R resistance/length Ω
/unit 0.0 0.2
L inductance/length H/unit 0.0 9.13e-9
G conductance/length mhos
/unit 0.0 0.0
C capacitance/length F/unit 0.0 3.65e-12
LEN length of line unit no default 1.0
REL breakpoint control arbitrary unit 1 0.5
ABS breakpoint control 1 5
NOSTEPLIMIT don’t limit time-step to less
than line delay
flag not set set
NO CONTROL don’t do complex time-step
control
flag not set set
LININTERP use linear interpolation flag not set set
MIXEDINTERP use linear when quadratic
seems bad
flag not set set
COMPACTREL special reltol for history
compaction
RELTOL 1.0e-3
COMPACTABS special abstol for history
compaction
ABSTOL 1.0e-9
TRUNCNR use Newton-Raphson method
for time-step control
flag not set set
TRUNCDONTCUT don’t limit time-step to keep
impulse-response errors low
flag not set set
The following types of lines have been implemented so far:
• RLC (uniform transmission line with series loss only),
• RC (uniform RC line),
• LC (lossless transmission line),
• RG (distributed series resistance and parallel conductance only).
Any other combination will yield erroneous results and should not be tried. The length LEN
of the line must be specified. NOSTEPLIMIT is a flag that will remove the default restriction
of limiting time-steps to less than the line delay in the RLC case. NO CONTROL is a flag that
prevents the default limiting of the time-step based on convolution error criteria in the RLC and
RC cases. This speeds up simulation but may in some cases reduce the accuracy of results.
LININTERP is a flag that, when specified, will use linear interpolation instead of the default
quadratic interpolation for calculating delayed signals. MIXEDINTERP is a flag that, when spe-
cified, uses a metric for judging whether quadratic interpolation is not applicable and if so uses
linear interpolation; otherwise it uses the default quadratic interpolation. TRUNCDONTCUT is a
flag that removes the default cutting of the time-step to limit errors in the actual calculation of
impulse-response related quantities. COMPACTREL and COMPACTABS are quantities that control
the compaction of the past history of values stored for convolution. Larger values of these lower
accuracy but usually increase simulation speed. These are to be used with the TRYTOCOMPACT
option, described in the .OPTIONS section. TRUNCNR is a flag that turns on the use of Newton-
Raphson iterations to determine an appropriate time-step in the time-step control routines. The
112 CHAPTER 6. TRANSMISSION LINES
default is a trial and error procedure by cutting the previous time-step in half. REL and ABS are
quantities that control the setting of breakpoints.
The option most worth experimenting with for increasing the speed of simulation is REL. The
default value of 1 is usually safe from the point of view of accuracy but occasionally increases
computation time. A value greater than 2 eliminates all breakpoints and may be worth trying
depending on the nature of the rest of the circuit, keeping in mind that it might not be safe from
the viewpoint of accuracy.
Breakpoints may usually be entirely eliminated if it is expected the circuit will not display
sharp discontinuities. Values between 0 and 1 are usually not required but may be used for
setting many breakpoints.
COMPACTREL may also be experimented with when the option TRYTOCOMPACT is specified in
a.OPTIONS card. The legal range is between 0 and 1. Larger values usually decrease the
accuracy of the simulation but in some cases improve speed. If TRYTOCOMPACT is not specified
on a .OPTIONS card, history compaction is not attempted and accuracy is high.
NO CONTROL,TRUNCDONTCUT and NOSTEPLIMIT also tend to increase speed at the expense of
accuracy.
6.3 Uniform Distributed RC Lines
General form:
UXXXXXXX n1 n2 n3 mname l=len <n=lumps >
Examples:
U1 1 2 0 URCMOD L =50U
URC2 1 12 2 UMODL l=1 MIL N=6
n1 and n2 are the two element nodes the RC line connects, while n3 is the node the capacitances
are connected to. mname is the model name, len is the length of the RC line in meters. lumps,
if specified, is the number of lumped segments to use in modeling the RC line (see the model
description for the action taken if this parameter is omitted).
6.3.1 Uniform Distributed RC Model (URC)
The URC model is derived from a model proposed by L. Gertzberg in 1974. The model is
accomplished by a subcircuit type expansion of the URC line into a network of lumped RC
segments with internally generated nodes. The RC segments are in a geometric progression,
increasing toward the middle of the URC line, with Kas a proportionality constant. The num-
ber of lumped segments used, if not specified for the URC line device, is determined by the
following formula:
N=
log
Fmax R
L
C
L2πL2
(K−1)
K
2
logK(6.1)
6.4. KSPICE LOSSY TRANSMISSION LINES 113
The URC line is made up strictly of resistor and capacitor segments unless the ISPERL parame-
ter is given a nonzero value, in which case the capacitors are replaced with reverse biased diodes
with a zero-bias junction capacitance equivalent to the capacitance replaced, and with a satu-
ration current of ISPERL amps per meter of transmission line and an optional series resistance
equivalent to RSPERL ohms per meter.
Name Parameter Units Default Example Area
K Propagation Constant - 2.0 1.2 -
FMAX Maximum Frequency of interest Hz 1.0 G 6.5 Meg -
RPERL Resistance per unit length Ω
/m1000 10 -
CPERL Capacitance per unit length F/m10e-15 1 p -
ISPERL Saturation Current per unit length A
/m0 - -
RSPERL Diode Resistance per unit length Ω
/m0 - -
6.4 KSPICE Lossy Transmission Lines
Unlike SPICE3, which uses the state-based approach to simulate lossy transmission lines,
KSPICE simulates lossy transmission lines and coupled multiconductor line systems using the
recursive convolution method. The impulse response of an arbitrary transfer function can be
determined by deriving a recursive convolution from the Pade approximations of the function.
NGSPICE is using this approach for simulating each transmission line’s characteristics and each
multiconductor line’s modal functions. This method of lossy transmission line simulation has
shown to give a speedup of one to two orders of magnitude over SPICE3E. Please note that the
following two models will support only transient simulation, no ac.
Additional Documentation Available:
• S. Lin and E. S. Kuh, ‘Pade Approximation Applied to Transient Simulation of Lossy
Coupled Transmission Lines,’ Proc. IEEE Multi-Chip Module Conference, 1992, pp.
52-55.
• S. Lin, M. Marek-Sadowska, and E. S. Kuh, ‘SWEC: A StepWise Equivalent Conduc-
tance Timing Simulator for CMOS VLSI Circuits,’ European Design Automation Conf.,
February 1991, pp. 142-148.
• S. Lin and E. S. Kuh, ‘Transient Simulation of Lossy Interconnect,’ Proc. Design Auto-
mation Conference, Anaheim, CA, June 1992, pp. 81-86.
6.4.1 Single Lossy Transmission Line (TXL)
General form:
YXXXXXXX N1 0 N2 0 mname <LEN=LENGTH >
Example:
Y1 1 0 2 0 ymod LEN =2
.MODEL ymod txl R =12.45 L =8.972e -9 G=0 C =0.468e -12 length =16
114 CHAPTER 6. TRANSMISSION LINES
n1 and n2 are the nodes of the two ports. The optional instance parameter len is the length of
the line and may be expressed in multiples of [unit]. Typically unit is given in meters. len will
override the model parameter length for the specific instance only.
The TXL model takes a number of parameters:
Name Parameter Units/Type Default Example
R resistance/length Ω
/unit 0.0 0.2
L inductance/length H/unit 0.0 9.13e-9
G conductance/length mhos
/unit 0.0 0.0
C capacitance/length F/unit 0.0 3.65e-12
LENGTH length of line unit no default 1.0
Model parameter length must be specified as a multiple of unit. Typically unit is given in [m].
For transient simulation only.
6.4.2 Coupled Multiconductor Line (CPL)
The CPL multiconductor line model is in theory similar to the RLGC model, but without fre-
quency dependent loss (neither skin effect nor frequency-dependent dielectric loss). Up to 8
coupled lines are supported in NGSPICE.
General form:
PXXXXXXX NI1 NI2 ... NIX GND1 NO1 NO2 ... NOX GND2 mname < LEN =LENGTH >
Example:
P1 in1 in2 0 b1 b2 0 PLINE
. model PLINE CPL length ={ Len }
+R=1 0 1
+L={ L11 } { L12} {L22}
+G=0 0 0
+C={ C11 } { C12} {C22}
.param Len =1 Rs =0
+ C11 =9.143579E -11 C12 = -9.78265E -12 C22 =9.143578 E-11
+ L11 =3.83572E -7 L12 =8.26253E -8 L22 =3.83572E-7
ni1 ... nix are the nodes at port 1 with gnd1; no1 ... nox are the nodes at port 2 with gnd2.
The optional instance parameter len is the length of the line and may be expressed in multiples
of [unit]. Typically unit is given in meters. len will override the model parameter length for
the specific instance only.
The CPL model takes a number of parameters:
Name Parameter Units/Type Default Example
R resistance/length Ω
/unit 0.0 0.2
L inductance/length H/unit 0.0 9.13e-9
G conductance/length mhos
/unit 0.0 0.0
C capacitance/length F/unit 0.0 3.65e-12
LENGTH length of line unit no default 1.0
6.4. KSPICE LOSSY TRANSMISSION LINES 115
All RLGC parameters are given in Maxwell matrix form. For the R and G matrices the diagonal
elements must be specified, for L and C matrices the lower or upper triangular elements must
specified. The parameter LENGTH is a scalar and is mandatory. For transient simulation only.
116 CHAPTER 6. TRANSMISSION LINES
Chapter 7
Diodes
7.1 Junction Diodes
General form:
DXXXXXXX n+ n- mname <area =val > <m=val > <pj=val > <off >
+ <ic=vd > <temp=val > <dtemp =val >
Examples:
DBRIDGE 2 10 DIODE1
DCLMP 3 7 DMOD AREA =3.0 IC =0.2
The pn junction (diode) implemented in ngspice expands the one found in SPICE3f5. Perimeter
effects and high injection level have been introduced into the original model and temperature
dependence of some parameters has been added. n+ and n- are the positive and negative nodes,
respectively. mname is the model name. Instance parameters may follow, dedicated to only
the diode described on the respective line. area is the area scale factor, which may scale
the saturation current given by the model parameters (and others, see table below). pj is the
perimeter scale factor, scaling the sidewall saturation current and its associated capacitance. m
is a multiplier of area and perimeter, and off indicates an (optional) starting condition on the
device for dc analysis. If the area factor is omitted, a value of 1.0 is assumed. The (optional)
initial condition specification using ic is intended for use with the uic option on the .tran
control line, when a transient analysis is desired starting from other than the quiescent operating
point. You should supply the initial voltage across the diode there. The (optional) temp value
is the temperature at which this device is to operate, and overrides the temperature specification
on the .option control line. The temperature of each instance can be specified as an offset to
the circuit temperature with the dtemp option.
7.2 Diode Model (D)
The dc characteristics of the diode are determined by the parameters is and n. An ohmic
resistance, rs, is included. Charge storage effects are modeled by a transit time, tt, and a
117
118 CHAPTER 7. DIODES
nonlinear depletion layer capacitance that is determined by the parameters cjo,vj, and m. The
temperature dependence of the saturation current is defined by the parameters eg, the energy,
and xti, the saturation current temperature exponent. The nominal temperature where these
parameters were measured is tnom, which defaults to the circuit-wide value specified on the
.options control line. Reverse breakdown is modeled by an exponential increase in the reverse
diode current and is determined by the parameters bv and ibv (both of which are positive
numbers).
Junction DC parameters
Name Parameter Units Default Example Scale factor
BV Reverse breakdown voltage V∞40
IBV Current at breakdown voltage A1.0e-3 1.0e-4
IK (IKF) Forward knee current A1.0e-3 1.0e-6
IKR Reverse knee current A1.0e-3 1.0e-6
IS (JS) Saturation current A1.0e-14 1.0e-16 area
JSW Sidewall saturation current A1.0e-14 1.0e-15 perimeter
N Emission coefficient - 1 1.5
RS Ohmic resistance Ω0.0 100 1
/area
Junction capacitance parameters
Name Parameter Units Default Example Scale factor
CJO (CJ0) Zero-bias junction bottom-wall
capacitance
F0.0 2pF area
CJP (CJSW) Zero-bias junction sidewall
capacitance
F0.0 .1pF perimeter
FC Coefficient for forward-bias
depletion bottom-wall capacitance
formula
- 0.5 -
FCS Coefficient for forward-bias
depletion sidewall capacitance
formula
- 0.5 -
M (MJ) Area junction grading coefficient - 0.5 0.5
MJSW Periphery junction grading
coefficient
- 0.33 0.5
VJ (PB) Junction potential V1 0.6
PHP Periphery junction potential V1 0.6
TT Transit-time sec 0 0.1ns
7.3. DIODE EQUATIONS 119
Temperature effects
Name Parameter Units Default Example
EG Activation energy eV 1.11
1.11 Si
0.69 Sbd
0.67 Ge
TM1 1st order tempco for MJ 1
/◦C0.0 -
TM2 2nd order tempco for MJ 1
/◦C20.0 -
TNOM (TREF) Parameter measurement temperature ◦C27 50
TRS1 (TRS) 1st order tempco for RS 1
/◦C0.0 -
TRS2 2nd order tempco for RS 1
/◦C20.0 -
TM1 1st order tempco for MJ 1
/◦C0.0 -
TM2 2nd order tempco for MJ 1
/◦C20.0 -
TTT1 1st order tempco for TT 1
/◦C0.0 -
TTT2 2nd order tempco for TT 1
/◦C20.0 -
XTI Saturation current temperature exponent - 3.0 3.0 pn
2.0 Sbd
TLEV Diode temperature equation selector - 0
TLEVC Diode capac. temperature equation selector - 0
CTA (CTC) Area junct. cap. temperature coefficient 1
/◦C0.0 -
CTP Perimeter junct. cap. temperature coefficient 1
/◦C0.0 -
TCV Breakdown voltage temperature coefficient 1
/◦C0.0 -
Noise modeling
Name Parameter Units Default Example Scale factor
KF Flicker noise coefficient - 0
AF Flicker noise exponent - 1
Diode models may be described in the input file (or an file included by .inc) according to the
following example:
General form:
.model mname type( pname1 =pval1 pname2 = pval2 ... )
Examples:
. model DMOD D ( bf =50 is =1e -13 vbf =50)
7.3 Diode Equations
The junction diode is the basic semiconductor device and the simplest one in ngspice, but its
model is quite complex, even when not all the physical phenomena affecting a pn junction are
handled. The diode is modeled in three different regions:
120 CHAPTER 7. DIODES
•Forward bias: the anode is more positive than the cathode, the diode is ‘on’ and can
conduct large currents. To avoid convergence problems and unrealistic high current, it is
prudent to specify a series resistance to limit current with the rs model parameter.
•Reverse bias: the cathode is more positive than the anode and the diode is ‘off’. A reverse
bias diode conducts a small leakage current.
•Breakdown: the breakdown region is modeled only if the bv model parameter is given.
When a diode enters breakdown the current increases exponentially (remember to limit
it); bv is a positive value.
Parameters Scaling
Model parameters are scaled using the unit-less parameters area and pj and the multiplier mas
depicted below:
AREAe f f =AREA m
PJe f f =PJ m
ISe f f =IS AREAe f f +JSW PJe f f
IBVe f f =IBV AREAe f f
IKe f f =IK AREAe f f
IKRe f f =IKR AREAe f f
CJe f f =CJ0 AREAe f f
CJP
e f f =CJP PJe f f
Diode DC, Transient and AC model equations
ID=
ISe f f (eqVD
NkT −1) +VD·GMIN,if VD≥ −3NkT
q
−ISe f f [1+ (3NkT
qVDe)3] +VD·GMIN,if −BVe f f <VD<−3NkT
q
−ISe f f (e−q(BVe f f +VD)
NkT ) +VD·GMIN,if VD≤ −BVe f f
(7.1)
The breakdown region must be described with more depth since the breakdown is not modeled
physically. As written before, the breakdown modeling is based on two model parameters: the
‘nominal breakdown voltage’ bv and the current at the onset of breakdown ibv. For the diode
model to be consistent, the current value cannot be arbitrarily chosen, since the reverse bias and
breakdown regions must match. When the diode enters breakdown region from reverse bias,
the current is calculated using the formula1:
Ibdwn =−ISe f f (e−qBV
NkT −1)(7.2)
The computed current is necessary to adjust the breakdown voltage making the two regions
match. The algorithm is a little bit convoluted and only a brief description is given here:
1if you look at the source code in file diotemp.c you will discover that the exponential relation is replaced
with a first order Taylor series expansion.
7.3. DIODE EQUATIONS 121
if IBVe f f <Ibdwn then
IBVe f f =Ibdwn
BVe f f =BV
else
BVe f f =BV −NVtln(IBVe f f
Ibdwn )
Algorithm 2: Diode breakdown current calculation
Most real diodes shows a current increase that, at high current levels, does not follow the expo-
nential relationship given above. This behavior is due to high level of carriers injected into the
junction. High injection effects (as they are called) are modeled with ik and ikr.
IDe f f =
ID
1+rID
IKe f f
,if VD≥ −3NkT
q
ID
1+rID
IKRe f f
,otherwise.(7.3)
Diode capacitance is divided into two different terms:
• Depletion capacitance
• Diffusion capacitance
Depletion capacitance is composed by two different contributes, one associated to the bottom
of the junction (bottom-wall depletion capacitance) and the other to the periphery (sidewall
depletion capacitance). The basic equations are:
CDiode =Cdi f f usion +Cdepletion
Where the depletion capacitance is defined as:
Cdepletion =Cdeplbw +Cdeplsw
The diffusion capacitance, due to the injected minority carriers, is modeled with the transit time
tt:
Cdi f f usion =TT∂IDe f f
∂VD
The depletion capacitance is more complex to model, since the function used to approximate it
diverges when the diode voltage become greater than the junction built-in potential. To avoid
function divergence, the capacitance function is approximated with a linear extrapolation for
applied voltage greater than a fraction of the junction built-in potential.
Cdeplbw =
CJe f f (1−VD
VJ )−MJ,if VD<FC ·VJ
CJe f f
1−FC(1+MJI)+MJVD
VJ
(1−FC)(1+MJ),otherwise.(7.4)
122 CHAPTER 7. DIODES
Cdeplsw =
CJP
e f f (1−VD
PHP )−MJSW,if VD<FCS ·PHP
CJP
e f f
1−FCS(1+MJSW)+MJSW·VD
PHP
(1−FCS)(1+MJSW),otherwise.(7.5)
Temperature dependence
The temperature affects many of the parameters in the equations above, and the following equa-
tions show how. One of the most significant parameters that varies with the temperature for a
semiconductor is the band-gap energy:
EGnom =1.16 −7.02e−4TNOM2
TNOM +1108.0(7.6)
EG(T) = 1.16 −7.02e−4T2
TNOM +1108.0(7.7)
The leakage current temperature’s dependence is:
IS(T) = IS elog f actor
N(7.8)
JSW (T) = JSW elog f actor
N(7.9)
where ‘logfactor’ is defined as
log f actor =EG
Vt(TNOM)−EG
Vt(T)+XTI ln(T
TNOM)(7.10)
The contact potentials (bottom-wall an sidewall) temperature dependence is:
V J(T) = VJ(T
TNOM)−Vt(T)3·ln(T
TNOM) + EGnom
Vt(TNOM)−EG(T)
Vt(T)(7.11)
PHP(T) = PHP(T
TNOM)−Vt(T)3·ln(T
TNOM) + EGnom
Vt(TNOM)−EG(T)
Vt(T)(7.12)
The depletion capacitances temperature dependence is:
CJ(T) = CJ 1+MJ(4.0e−4(T−TNOM)−V J(T)
VJ +1)(7.13)
CJSW (T) = CJSW 1+MJSW(4.0e−4(T−TNOM)−PHP(T)
PHP +1)(7.14)
The transit time temperature dependence is:
T T (T) = TT(1+TTT1(T−TNOM) + TTT2(T−TNOM)2)(7.15)
7.3. DIODE EQUATIONS 123
The junction grading coefficient temperature dependence is:
MJ(T) = MJ(1+TM1(T−TNOM) + TM2(T−TNOM)2)(7.16)
The series resistance temperature dependence is:
RS(T) = RS(1+TRS(T−TNOM) + TRS2(T−TNOM)2)(7.17)
Noise model
The diode has three noise contribution, one due to the presence of the parasitic resistance rs
and the other two (shot and flicker) due to the pn junction.
The thermal noise due to the parasitic resistance is:
i2
RS =4kT ∆f
RS (7.18)
The shot and flicker noise contributions are:
i2
d=2qID∆f+KF ·IAF
D
f
∆f(7.19)
124 CHAPTER 7. DIODES
Chapter 8
BJTs
8.1 Bipolar Junction Transistors (BJTs)
General form:
QXXXXXXX nc nb ne <ns > mname <area=val > <areac =val >
+ <areab =val > <m=val > <off > <ic=vbe ,vce > <temp =val >
+ <dtemp =val >
Examples:
Q23 10 24 13 QMOD IC=0.6 , 5.0
Q50A 11 26 4 20 MOD1
nc,nb, and ne are the collector, base, and emitter nodes, respectively. ns is the (optional) sub-
strate node. When unspecified, ground is used. mname is the model name, area,areab,areac
are the area factors (emitter, base and collector respectively), and off indicates an (optional)
initial condition on the device for the dc analysis. If the area factor is omitted, a value of 1.0 is
assumed.
The (optional) initial condition specification using ic=vbe,vce is intended for use with the
uic option on a .tran control line, when a transient analysis is desired to start from other
than the quiescent operating point. See the .ic control line description for a better way to set
transient initial conditions. The (optional) temp value is the temperature where this device is
to operate, and overrides the temperature specification on the .option control line. Using the
dtemp option one can specify the instance’s temperature relative to the circuit temperature.
8.2 BJT Models (NPN/PNP)
Ngspice provides three BJT device models, which are selected by the .model card.
.model QMOD1 BJT level=2
This is the minimal version, further optional parameters listed in the table below may replace
the ngspice default parameters. The level keyword specifies the model to be used:
125
126 CHAPTER 8. BJTS
• level=1 : This is the original SPICE BJT model, and it is the default model if the level
keyword is not specified on the .model line.
• level=2 : This is a modified version of the original SPICE BJT that models both vertical
and lateral devices and includes temperature corrections of collector, emitter and base
resistors.
• level=4: Advanced VBIC model (see http://www.designers-guide.org/VBIC/ for details)
The bipolar junction transistor model in ngspice is an adaptation of the integral charge control
model of Gummel and Poon. This modified Gummel-Poon model extends the original model
to include several effects at high bias levels. The model automatically simplifies to the simpler
Ebers-Moll model when certain parameters are not specified. The parameter names used in the
modified Gummel-Poon model have been chosen to be more easily understood by the user, and
to reflect better both physical and circuit design thinking.
The dc model is defined by the parameters is,bf,nf,ise,ikf, and ne, which determine
the forward current gain characteristics, is,br,nr,isc,ikr, and nc, which determine the
reverse current gain characteristics, and vaf and var, which determine the output conductance
for forward and reverse regions.
The level 1 model has among the standard temperature parameters an extension compatible with
most foundry provided process design kits (see parameter table below tlev).
The level 1 and 2 models include the substrate saturation current iss. Three ohmic resistances
rb,rc, and re are included, where rb can be high current dependent. Base charge storage is
modeled by forward and reverse transit times, tf and tr, where the forward transit time tf can
be bias dependent if desired. Nonlinear depletion layer capacitances are defined with cje,vje,
and nje for the B-E junction, cjc,vjc, and njc for the B-C junction and cjs,vjs, and mjs
for the C-S (collector-substrate) junction.
The level 1 and 2 model support a substrate capacitance that is connected to the device’s base or
collector, to model lateral or vertical devices dependent on the parameter subs. The temperature
dependence of the saturation currents, is and iss (for the level 2 model), is determined by the
energy-gap, eg, and the saturation current temperature exponent, xti.
In the new model, additional base current temperature dependence is modeled by the beta tem-
perature exponent xtb. The values specified are assumed to have been measured at the tempera-
ture tnom, which can be specified on the .options control line or overridden by a specification
on the .model line.
The level 4 model (VBIC) has the following improvements beyond the GP models: impro-
ved Early effect modeling, quasi-saturation modeling, parasitic substrate transistor modeling,
parasitic fixed (oxide) capacitance modeling, includes an avalanche multiplication model, im-
proved temperature modeling, base current is decoupled from collector current, electrothermal
modeling, smooth and continuous mode.
The BJT parameters used in the modified Gummel-Poon model are listed below. The parameter
names used in earlier versions of SPICE2 are still accepted.
Gummel-Poon BJT Parameters (incl. model extensions)
8.2. BJT MODELS (NPN/PNP) 127
Name Parameters Units Default Example Scale factor
SUBS Substrate connection: for vertical
geometry, -1 for lateral geometry
(level 2 only).
1
IS Transport saturation current. A1.0e-16 1.0e-15 area
ISS Reverse saturation current,
substrate-to-collector for vertical
device or substrate-to-base for
lateral (level 2 only).
A1.0e-16 1.0e-15 area
BF Ideal maximum forward beta. - 100 100
NF Forward current emission
coefficient.
- 1.0 1
VAF (VA) Forward Early voltage. V∞200
IKF Corner for forward beta current
roll-off.
A∞0.01 area
NKF High current Beta rolloff exponent - 0.5 0.58
ISE B-E leakage saturation current. A0.0 1e-13 area
NE B-E leakage emission coefficient. - 1.5 2
BR Ideal maximum reverse beta. - 1 0.1
NR Reverse current emission
coefficient.
- 1 1
VAR (VB) Reverse Early voltage. V∞200
IKR Corner for reverse beta high
current roll-off.
A∞0.01 area
ISC B-C leakage saturation current
(area is ‘areab’ for vertical devices
and ‘areac’ for lateral).
A0.0 1e-13 area
NC B-C leakage emission coefficient. - 2 1.5
RB Zero bias base resistance. Ω0 100 area
IRB Current where base resistance falls
halfway to its min value.
A∞0.1 area
RBM Minimum base resistance at high
currents.
ΩRB 10 area
RE Emitter resistance. Ω0 1 area
RC Collector resistance. Ω0 10 area
CJE B-E zero-bias depletion
capacitance.
F0 2pF area
VJE (PE) B-E built-in potential. V0.75 0.6
MJE (ME) B-E junction exponential factor. - 0.33 0.33
TF Ideal forward transit time. sec 0 0.1ns
XTF Coefficient for bias dependence of
TF.
- 0
VTF Voltage describing VBC
dependence of TF.
V∞
ITF High-current parameter for effect
on TF.
A0 - area
128 CHAPTER 8. BJTS
PTF Excess phase at freq= 1
2πT F Hz. deg 0
CJC B-C zero-bias depletion
capacitance (area is ‘areab’ for
vertical devices and ‘areac’ for
lateral).
F0 2pF area
VJC (PC) B-C built-in potential. V0.75 0.5
MJC B-C junction exponential factor. - 0.33 0.5
XCJC Fraction of B-C depletion
capacitance connected to internal
base node.
- 1
TR Ideal reverse transit time. sec 0 10ns
CJS Zero-bias collector-substrate
capacitance (area is ‘areac’ for
vertical devices and ‘areab’ for
lateral).
F0 2pF area
VJS (PS) Substrate junction built-in
potential.
V0.75
MJS (MS) Substrate junction exponential
factor.
- 0 0.5
XTB Forward and reverse beta
temperature exponent.
- 0
EG Energy gap for temperature effect
on IS.
eV 1.11
XTI Temperature exponent for effect on
IS.
- 3
KF Flicker-noise coefficient. - 0
AF Flicker-noise exponent. - 1
FC Coefficient for forward-bias
depletion capacitance formula.
- 0.5 0
TNOM (TREF) Parameter measurement
temperature.
◦C27 50
TLEV BJT temperature equation selector - 0
TLEVC BJT capac. temperature equation
selector
- 0
TRE1 1st order temperature coefficient
for RE.
1
/◦C0.0 1e-3
TRE2 2nd order temperature coefficient
for RE.
1
/◦C20.0 1e-5
TRC1 1st order temperature coefficient
for RC .
1
/◦C0.0 1e-3
TRC2 2nd order temperature coefficient
for RC.
1
/◦C20.0 1e-5
TRB1 1st order temperature coefficient
for RB.
1
/◦C0.0 1e-3
TRB2 2nd order temperature coefficient
for RB.
1
/◦C20.0 1e-5
8.2. BJT MODELS (NPN/PNP) 129
TRBM1 1st order temperature coefficient
for RBM
1
/◦C0.0 1e-3
TRBM2 2nd order temperature coefficient
for RBM
1
/◦C20.0 1e-5
TBF1 1st order temperature coefficient
for BF
1
/◦C0.0 1e-3
TBF2 2nd order temperature coefficient
for BF
1
/◦C20.0 1e-5
TBR1 1st order temperature coefficient
for BR
1
/◦C0.0 1e-3
TBR2 2nd order temperature coefficient
for BR
1
/◦C20.0 1e-5
TIKF1 1st order temperature coefficient
for IKF
1
/◦C0.0 1e-3
TIKF2 2nd order temperature coefficient
for IKF
1
/◦C20.0 1e-5
TIKR1 1st order temperature coefficient
for IKR
1
/◦C0.0 1e-3
TIKR2 2nd order temperature coefficient
for IKR
1
/◦C20.0 1e-5
TIRB1 1st order temperature coefficient
for IRB
1
/◦C0.0 1e-3
TIRB2 2nd order temperature coefficient
for IRB
1
/◦C20.0 1e-5
TNC1 1st order temperature coefficient
for NC
1
/◦C0.0 1e-3
TNC2 2nd order temperature coefficient
for NC
1
/◦C20.0 1e-5
TNE1 1st order temperature coefficient
for NE
1
/◦C0.0 1e-3
TNE2 2nd order temperature coefficient
for NE
1
/◦C20.0 1e-5
TNF1 1st order temperature coefficient
for NF
1
/◦C0.0 1e-3
TNF2 2nd order temperature coefficient
for NF
1
/◦C20.0 1e-5
TNR1 1st order temperature coefficient
for IKF
1
/◦C0.0 1e-3
TNR2 2nd order temperature coefficient
for IKF
1
/◦C20.0 1e-5
TVAF1 1st order temperature coefficient
for VAF
1
/◦C0.0 1e-3
TVAF2 2nd order temperature coefficient
for VAF
1
/◦C20.0 1e-5
TVAR1 1st order temperature coefficient
for VAR
1
/◦C0.0 1e-3
130 CHAPTER 8. BJTS
TVAR2 2nd order temperature coefficient
for VAR
1
/◦C20.0 1e-5
CTC 1st order temperature coefficient
for CJC
1
/◦C0.0 1e-3
CTE 1st order temperature coefficient
for CJE
1
/◦C0.0 1e-3
CTS 1st order temperature coefficient
for CJS
1
/◦C0.0 1e-3
TVJC 1st order temperature coefficient
for VJC
1
/◦C20.0 1e-5
TVJE 1st order temperature coefficient
for VJE
1
/◦C0.0 1e-3
TITF1 1st order temperature coefficient
for ITF
1
/◦C0.0 1e-3
TITF2 2nd order temperature coefficient
for ITF
1
/◦C20.0 1e-5
TTF1 1st order temperature coefficient
for TF
1
/◦C0.0 1e-3
TTF2 2nd order temperature coefficient
for TF
1
/◦C20.0 1e-5
TTR1 1st order temperature coefficient
for TR
1
/◦C0.0 1e-3
TTR2 2nd order temperature coefficient
for TR
1
/◦C20.0 1e-5
TMJE1 1st order temperature coefficient
for MJE
1
/◦C0.0 1e-3
TMJE2 2nd order temperature coefficient
for MJE
1
/◦C20.0 1e-5
TMJC1 1st order temperature coefficient
for MJC
1
/◦C0.0 1e-3
TMJC2 2nd order temperature coefficient
for MJC
1
/◦C20.0 1e-5
Chapter 9
JFETs
9.1 Junction Field-Effect Transistors (JFETs)
General form:
JXXXXXXX nd ng ns mname <area > <off > <ic=vds ,vgs > <temp =t >
Examples:
J1 7 2 3 JM1 OFF
nd,ng, and ns are the drain, gate, and source nodes, respectively. mname is the model name,
area is the area factor, and off indicates an (optional) initial condition on the device for dc
analysis. If the area factor is omitted, a value of 1.0 is assumed. The (optional) initial condition
specification, using ic=VDS,VGS is intended for use with the uic option on the .TRAN control
line, when a transient analysis is desired starting from other than the quiescent operating point.
See the .ic control line for a better way to set initial conditions. The (optional) temp value is
the temperature where this device is to operate, and overrides the temperature specification on
the .option control line.
9.2 JFET Models (NJF/PJF)
9.2.1 JFET level 1 model with Parker Skellern modification
The level 1 JFET model is derived from the FET model of Shichman and Hodges. The dc
characteristics are defined by the parameters VTO and BETA, which determine the variation
of drain current with gate voltage, LAMBDA, which determines the output conductance, and
IS, the saturation current of the two gate junctions. Two ohmic resistances, RD and RS, are
included.
vgst =vgs −V T O (9.1)
131
132 CHAPTER 9. JFETS
βp=BETA (1+LAMBDA vds)(9.2)
b f ac =1−B
PB −V T O (9.3)
IDrain =
vds ·GMIN,if vgst ≤0
βpvds (vds (b f ac vds −B)vgst (2B+3b f ac (vgst −vds))) + vds ·GMIN,if vgst ≥vds
βpvgst2(B+vgst b f ac) + vds ·GMIN,if vgst <vds
(9.4)
Note that in Spice3f and later, the fitting parameter B has been added by Parker and Skellern.
For details, see [9]. If parameter B is set to 1 equation above simplifies to
IDrain =
vds ·GMIN,if vgst ≤0
βpvds (2vgst −vds) + vds ·GMIN,if vgst ≥vds
βpvgst2+vds ·GMIN,if vgst <vds
(9.5)
Charge storage is modeled by nonlinear depletion layer capacitances for both gate junctions,
which vary as the −1
/2power of junction voltage and are defined by the parameters CGS, CGD,
and PB.
Name Parameter Units Default Example Scaling factor
VTO Threshold voltage VT0V-2.0 -2.0
BETA Transconductance parameter (β)A
/V”1.0e-4 1.0e-3 area
LAMBDA Channel-length modulation
parameter (λ)
1
/V0 1.0e-4
RD Drain ohmic resistance Ω0 100 area
RS Source ohmic resistance Ω0 100 area
CGS Zero-bias G-S junction capacitance
Cgs
F0 5pF area
CGD Zero-bias G-D junction
capacitance Cgd
F0 1pF area
PB Gate junction potential V1 0.6
IS Gate saturation current ISA1.0e-14 1.0e-14 area
B Doping tail parameter - 1 1.1
KF Flicker noise coefficient - 0
AF Flicker noise exponent - 1
NLEV Noise equation selector - 1 3
GDSNOI Channel noise coefficient for
nlev=3
1.0 2.0
FC Coefficient for forward-bias
depletion capacitance formula
0.5
TNOM Parameter measurement
temperature
◦C27 50
TCV Threshold voltage temperature
coefficient
1
/°C0.0 0.1
BEX Mobility temperature exponent - 0.0 1.1
9.2. JFET MODELS (NJF/PJF) 133
Additional to the standard thermal and flicker noise model an alternative thermal channel noise
model is implemented and is selectable by setting NLEV parameter to 3. This follows in a
correct channel thermal noise in the linear region.
Snoise =2
34kT ·BETA ·V gst (1+α+α2)
1+αGDSNOI (9.6)
with
α=(1−vds
vgs−V T O ,if vgs −V T O ≥vds
0,else (9.7)
9.2.2 JFET level 2 Parker Skellern model
The level 2 model is an improvement to level 1. Details are available from Macquarie Univer-
sity. Some important items are:
• The description maintains strict continuity in its high-order derivatives, which is essential
for prediction of distortion and intermodulation.
• Frequency dependence of output conductance and transconductance is described as a
function of bias.
• Both drain-gate and source-gate potentials modulate the pinch-off potential, which is con-
sistent with S-parameter and pulsed-bias measurements.
• Self-heating varies with frequency.
• Extreme operating regions - subthreshold, forward gate bias, controlled resistance, and
breakdown regions - are included.
• Parameters provide independent fitting to all operating regions. It is not necessary to
compromise one region in favor of another.
• Strict drain-source symmetry is maintained. The transition during drain-source potential
reversal is smooth and continuous.
The model equations are described in this pdf document and in [19].
134 CHAPTER 9. JFETS
Name Description Unit Type Default
ID Device IDText Text PF1
ACGAM Capacitance modulation None 0
BETA Linear-region transconductance scale None 10−4
CGD Zero-bias gate-source capacitance Capacitance 0 F
CGS Zero-bias gate-drain capacitance Capacitance 0 F
DELTA Thermal reduction coefficient None 0 W
FC Forward bias capacitance parameter None 0.5
HFETA High-frequency VGS feedback parameter None 0
HFE1 HFGAM modulation by VGD None 0V−1
HFE2 HFGAM modulation by VGS None 0 V−1
HFGAM High-frequency VGD feedback parameter None 0
HFG1 HFGAM modulation by VSG None 0 V−1
HFG2 HFGAM modulation by VDG None 0 V−1
IBD Gate-junction breakdown current Current 0 A
IS Gate-junction saturation current Current 10−14A
LFGAM Low-frequency feedback parameter None 0
LFG1 LFGAM modulation by VSG None 0 V−1
LFG2 LFGAM modulation by VDG None 0 V−1
MVST Subthreshold modulation None 0 V−1
N Gate-junction ideality factor None 1
P Linear-region power-law exponent None 2
Q Saturated-region power-law exponent None 2
RS Source ohmic resistance Resistance 0 Ohm
RD Drain ohmic resistance Resistance 0 Ohm
TAUD Relaxation time for thermal reduction Time 0 s
TAUG Relaxation time for gamma feedback Time 0 s
VBD Gate-junction breakdown potential Voltage 1 V
VBI Gate-junction potential Voltage 1 V
VST Subthreshold potential Voltage 0 V
VTO Threshold voltage Voltage -2.0 V
XC Capacitance pinch-off reduction factor None 0
XI Saturation-knee potential factor None 1000
Z Knee transition parameter None 0.5
RG Gate ohmic resistance Resistance 0 Ohm
LG Gate inductance Inductance 0 H
LS Source inductance Inductance 0 H
LD Drain inductance Inductance 0 H
CDSS Fixed Drain-source capacitance Capacitance 0 F
AFAC Gate-width scale factor None 1
NFING Number of gate fingers scale factor None 1
TNOM Nominal Temperature (Not implemented) Temperature 300 K
TEMP Temperature Temperature 300 K
Chapter 10
MESFETs
10.1 MESFETs
General form:
ZXXXXXXX ND NG NS MNAME <AREA > <OFF > <IC=VDS , VGS >
Examples:
Z1 7 2 3 ZM1 OFF
10.2 MESFET Models (NMF/PMF)
10.2.1 Model by Statz e.a.
The MESFET model level 1 is derived from the GaAs FET model of Statz et al. as described in
[11]. The dc characteristics are defined by the parameters VTO, B, and BETA, which determine
the variation of drain current with gate voltage, ALPHA, which determines saturation voltage,
and LAMBDA, which determines the output conductance. The formula are given by:
Id=
B(Vgs−VT)2
1+b(Vgs−VT)
1−1−AVds
3
3
(1+LVds)for 0 <Vds <3
A
B(Vgs−VT)2
1+b(Vgs−VT)(1+LVds)for V>3
A
(10.1)
Two ohmic resistances, rd and rs, are included. Charge storage is modeled by total gate charge
as a function of gate-drain and gate-source voltages and is defined by the parameters cgs,cgd,
and pb.
135
136 CHAPTER 10. MESFETS
Name Parameter Units Default Example Area
VTO Pinch-off voltage V-2.0 -2.0
BETA Transconductance parameter A
/V21.0e-4 1.0e-3 *
B Doping tail extending parameter 1
/V0.3 0.3 *
ALPHA Saturation voltage parameter 1
/V2 2 *
LAMBDA Channel-length modulation parameter 1
/V0 1.0e-4
RD Drain ohmic resistance Ω0 100 *
RS Source ohmic resistance Ω0 100 *
CGS Zero-bias G-S junction capacitance F0 5pF *
CGD Zero-bias G-D junction capacitance F0 1pF *
PB Gate junction potential V1 0.6
KF Flicker noise coefficient - 0
AF Flicker noise exponent - 1
FC Coefficient for forward-bias depletion
capacitance formula
- 0.5
Device instance:
z1 2 3 0 mesmod area =1.4
Model:
. model mesmod nmf level =1 rd =46 rs =46 vt0 = -1.3
+ lambda =0.03 alpha =3 beta =1.4e -3
10.2.2 Model by Ytterdal e.a.
level 2 (and levels 3,4) Copyright 1993: T. Ytterdal, K. Lee, M. Shur and T. A. Fjeldly
to be written
M. Shur, T.A. Fjeldly, T. Ytterdal, K. Lee, "Unified GaAs MESFET Model for Circuit Simula-
tion", Int. Journal of High Speed Electronics, vol. 3, no. 2, pp. 201-233, 1992
10.2.3 hfet1
level 5
to be written
no documentation available
10.2.4 hfet2
level6
to be written
no documentation available
Chapter 11
MOSFETs
Ngspice supports all the original mosfet models present in SPICE3f5 and almost all the newer
ones that have been published and made open-source. Both bulk and SOI (Silicon on Insula-
tor) models are available. When compiled with the cider option, ngspice implements the four
terminals numerical model that can be used to simulate a MOSFET (please refer to numerical
modeling documentation for additional information and examples).
11.1 MOSFET devices
General form:
MXXXXXXX nd ng ns nb mname <m=val > <l=val > <w=val >
+ <ad=val > <as=val > <pd=val > <ps =val > <nrd=val >
+ <nrs=val > <off > <ic=vds , vgs , vbs > <temp =t>
Examples:
M1 24 2 0 20 TYPE1
M31 2 17 6 10 MOSN L=5U W=2U
M1 2 9 3 0 MOSP L=10U W=5U AD =100 P AS =100P PD =40 U PS=40U
Note the suffixes in the example: the suffix ‘u’ specifies microns (1e-6 m) and ‘p’ sq-microns
(1e-12 m2).
The instance card for MOS devices starts with the letter ’M’. nd,ng,ns, and nb are the drain,
gate, source, and bulk (substrate) nodes, respectively. mname is the model name and mis the
multiplicity parameter, which simulates ‘m’ paralleled devices. All MOS models support the
‘m’ multiplier parameter. Instance parameters land w, channel length and width respectively,
are expressed in meters. The areas of drain and source diffusions: ad and as, in squared meters
(m2).
If any of l,w,ad, or as are not specified, default values are used. The use of defaults simplifies
input file preparation, as well as the editing required if device geometries are to be changed. pd
and ps are the perimeters of the drain and source junctions, in meters. nrd and nrs designate
the equivalent number of squares of the drain and source diffusions; these values multiply the
137
138 CHAPTER 11. MOSFETS
sheet resistance rsh specified on the .model control line for an accurate representation of the
parasitic series drain and source resistance of each transistor. pd and ps default to 0.0 while nrd
and nrs to 1.0. off indicates an (optional) initial condition on the device for dc analysis. The
(optional) initial condition specification using ic=vds,vgs,vbs is intended for use with the
uic option on the .tran control line, when a transient analysis is desired starting from other
than the quiescent operating point. See the .ic control line for a better and more convenient
way to specify transient initial conditions. The (optional) temp value is the temperature at
which this device is to operate, and overrides the temperature specification on the .option
control line.
The temperature specification is ONLY valid for level 1, 2, 3, and 6 MOSFETs, not for level 4
or 5 (BSIM) devices.
BSIM3.2 and BSIM4 (v4.7 and v4.8) models are also supporting the instance parameter delvto
and mulu0 for local mismatch and NBTI (negative bias temperature instability) modeling:
Name Parameter Units Default Example
delvto (delvt0) Threshold voltage shift V0.0 0.07
mulu0 Low-field mobility multiplier (U0) - 1.0 0.9
11.2 MOSFET models (NMOS/PMOS)
MOSFET models are the central part of ngspice, probably because they are the most widely
used devices in the electronics world. Ngspice provides all the MOSFETs implemented in the
original Spice3f and adds several models developed by UC Berkeley’s Device Group and other
independent groups.
Each model is invoked with a .model card. A minimal version is:
.model MOSN NMOS level=8 version=3.3.0
The model name MOSN corresponds to the model name in the instance card (see 11.1). Pa-
rameter NMOS selects an n-channel device, PMOS would point to a p-channel transistor. The
level and version parameters select the specific model. Further model parameters are op-
tional and replace ngspice default values. Due to the large number of parameters (more than
100 for modern models), model cards may be stored in extra files and loaded into the netlist by
the .include (2.6) command. Model cards are specific for a an IC manufacturing process and
are typically provided by the IC foundry. Some generic parameter sets, not linked to a specific
process, are made available by the model developers, e.g. UC Berkeley’s Device Group for
BSIM4 and BSIMSOI.
Ngspice provides several MOSFET device models, which differ in the formulation of the I-V
characteristic, and are of varying complexity. Models available are listed in table 11.1. Current
models for IC design are BSIM3 (11.2.9, down to channel length of 0.25 µm), BSIM4 (11.2.10,
below 0.25 µm), BSIMSOI (11.2.12, silicon-on-insulator devices), HiSIM2 and HiSIM_HV
(11.2.14, surface potential models for standard and high voltage/high power MOS devices).
11.2.1 MOS Level 1
This model is also known as the ‘Shichman-Hodges’ model. This is the first model written and
the one often described in the introductory textbooks for electronics. This model is applicable
11.2. MOSFET MODELS (NMOS/PMOS) 139
Level Name Model Version Developer References Notes
1 MOS1 Shichman-Hodges - Berkeley This is the classical quadratic model.
2 MOS2 Grove-Frohman - Berkeley Described in [2]
3 MOS3 Berkeley A semi-empirical model (see [1])
4 BSIM1 Berkeley Described in [3]
5 BSIM2 Berkeley Described in [5]
6 MOS6 Berkeley Described in [2]
9 MOS9 Alan Gillespie
8, 49 BSIM3v0 3.0 Berkeley extensions by Alan Gillespie
8, 49 BSIM3v1 3.1 Berkeley extensions by Serban Popescu
8, 49 BSIM3v32 3.2 - 3.2.4 Berkeley Multi version code
8, 49 BSIM3 3.3.0 Berkeley Described in [13]
10, 58 B4SOI 4.3.1 Berkeley
14, 54 BSIM4v5 4.0 - 4.5 Berkeley Multi version code
14, 54 BSIM4v6 4.6.5 Berkeley
14, 54 BSIM4v7 4.7.0 Berkeley
14, 54 BSIM4 4.8.0 Berkeley
44 EKV EPFL adms configured
45 PSP 1.0.2 Gildenblatt adms configured
55 B3SOIFD Berkeley
56 B3SOIDD Berkeley
57 B3SOIPD Berkeley
60 STAG SOI3 Southampton
68 HiSIM2 2.8.0 Hiroshima
73 HiSIM_HV 1.2.4/2.2.0 Hiroshima High Voltage Version for LDMOS
Table 11.1: MOSFET model summary
140 CHAPTER 11. MOSFETS
only to long channel devices. The use of Meyer’s model for the C-V part makes it non charge
conserving.
11.2.2 MOS Level 2
This model tries to overcome the limitations of the Level 1 model addressing several short-
channel effects, like velocity saturation. The implementation of this model is complicated and
this leads to many convergence problems. C-V calculations can be done with the original Meyer
model (non charge conserving).
11.2.3 MOS Level 3
This is a semi-empirical model derived from the Level 2 model. In the 80s this model has often
been used for digital design and, over the years, has proved to be robust. A discontinuity in the
model with respect to the KAPPA parameter has been detected (see [10]). The supplied fix has
been implemented in Spice3f2 and later. Since this fix may affect parameter fitting, the option
badmos3 may be set to use the old implementation (see the section on simulation variables and
the .options line). Ngspice level 3 implementation takes into account length and width mask
adjustments (xl and xw) and device width narrowing due to diffusion (wd).
11.2.4 MOS Level 6
This model is described in [2]. The model can express the current characteristics of short-
channel MOSFETs at least down to 0.25 µmchannel-length, GaAs FET, and resistance inserted
MOSFETs. The model evaluation time is about 1/3 of the evaluation time of the SPICE3 mos
level 3 model. The model also enables analytical treatments of circuits in short-channel region
and makes up for a missing link between a complicated MOSFET current characteristics and
circuit behaviors in the deep submicron region.
11.2.5 Notes on Level 1-6 models
The dc characteristics of the level 1 through level 3 MOSFETs are defined by the device para-
meters vto,kp,lambda,phi and gamma. These parameters are computed by ngspice if process
parameters (nsub,tox, ...) are given, but users specified values always override. vto is po-
sitive (negative) for enhancement mode and negative (positive) for depletion mode N-channel
(P-channel) devices.
Charge storage is modeled by three constant capacitors, cgso,cgdo, and cgbo, which represent
overlap capacitances, by the nonlinear thin-oxide capacitance that is distributed among the gate,
source, drain, and bulk regions, and by the nonlinear depletion-layer capacitances for both
substrate junctions divided into bottom and periphery, which vary as the mj and mjsw power
of junction voltage respectively, and are determined by the parameters cbd,cbs,cj,cjsw,mj,
mjsw and pb.
Charge storage effects are modeled by the piecewise linear voltages-dependent capacitance mo-
del proposed by Meyer. The thin-oxide charge-storage effects are treated slightly different for
11.2. MOSFET MODELS (NMOS/PMOS) 141
the level 1 model. These voltage-dependent capacitances are included only if tox is specified
in the input description and they are represented using Meyer’s formulation.
There is some overlap among the parameters describing the junctions, e.g. the reverse current
can be input either as is (in A) or as js (in A
/m2). Whereas the first is an absolute value the
second is multiplied by ad and as to give the reverse current of the drain and source junctions
respectively.
This methodology has been chosen since there is no sense in relating always junction charac-
teristics with ad and as entered on the device line; the areas can be defaulted. The same idea
applies also to the zero-bias junction capacitances cbd and cbs (in F) on one hand, and cj (in
F/m2) on the other.
The parasitic drain and source series resistance can be expressed as either rd and rs (in ohms)
or rsh (in ohms/sq.), the latter being multiplied by the number of squares nrd and nrs input on
the device line.
NGSPICE level 1, 2, 3 and 6 parameters
Name Parameter Units Default Example
LEVEL Model index - 1
VTO Zero-bias threshold voltage
(VT0)
V0.0 1.0
KP Transconductance
parameter
A
/V22.0e-5 3.1e-5
GAMMA Bulk threshold parameter √V0.0 0.37
PHI Surface potential (U) V0.6 0.65
LAMBDA Channel length modulation
(MOS1 and MOS2 only)
(λ)
1
/V0.0 0.02
RD Drain ohmic resistance Ω0.0 1.0
RS Source ohmic resistance Ω0.0 1.0
CBD Zero-bias B-D junction
capacitance
F0.0 20fF
CBS Zero-bias B-S junction
capacitance
F0.0 20fF
IS Bulk junction saturation
current (IS)
A1.0e-14 1.0e-15
PB Bulk junction potential V0.8 0.87
CGSO Gate-source overlap
capacitance per meter
channel width
F/m0.0 4.0e-11
CGDO Gate-drain overlap
capacitance per meter
channel width
F/m0.0 4.0e-11
CGBO Gate-bulk overlap
capacitance per meter
channel width
F/m0.0 2.0e-11
142 CHAPTER 11. MOSFETS
Name Parameter Units Default Example
RSH Drain and source diffusion
sheet resistance
Ω
/0.0 10
CJ Zero-bias bulk junction
bottom cap. per sq-meter of
junction area
F/m20.0 2.0e-4
MJ Bulk junction bottom
grading coeff.
- 0.5 0.5
CJSW Zero-bias bulk junction
sidewall cap. per meter of
junction perimeter
F/m0.0 1.0e-9
MJSW Bulk junction sidewall
grading coeff.
-0.50 (level1)
0.33 (level2,3)
JS Bulk junction saturation
current
TOX Oxide thickness m1.0e-7 1.0e-7
NSUB Substrate doping cm−30.0 4.0e15
NSS Surface state density cm−20.0 1.0e10
NFS Fast surface state density cm−20.0 1.0e10
TPG Type of gate material: +1
opp. to substrate, -1 same as
substrate, 0 Al gate
- 1.0
XJ Metallurgical junction depth m0.0 1M
LD Lateral diffusion m0.0 0.8M
UO Surface mobility cm2
/V·sec 600 700
UCRIT Critical field for mobility
degradation (MOS2 only)
V/cm 1.0e4 1.0e4
UEXP Critical field exponent in
mobility degradation
(MOS2 only)
- 0.0 0.1
UTRA Transverse field coeff.
(mobility) (deleted for
MOS2)
- 0.0 0.3
VMAX Maximum drift velocity of
carriers
m
/s0.0 5.0e4
NEFF Total channel-charge (fixed
and mobile) coefficient
(MOS2 only)
- 1.0 5.0
KF Flicker noise coefficient - 0.0 1.0e-26
AF Flicker noise exponent - 1.0 1.2
FC Coefficient for forward-bias
depletion capacitance
formula
- 0.5
DELTA Width effect on threshold
voltage (MOS2 and MOS3)
- 0.0 1.0
THETA Mobility modulation
(MOS3 only)
1
/V0.0 0.1
11.2. MOSFET MODELS (NMOS/PMOS) 143
Name Parameter Units Default Example
ETA Static feedback (MOS3
only)
- 0.0 1.0
KAPPA Saturation field factor
(MOS3 only)
- 0.2 0.5
TNOM Parameter measurement
temperature
◦C27 50
11.2.6 BSIM Models
Ngspice implements many of the BSIM models developed by Berkeley’s BSIM group. BSIM
stands for Berkeley Short-Channel IGFET Model and groups a class of models that is continu-
ously updated. In general, all parameters of BSIM models are obtained from process characte-
rization, in particular level 4 and level 5 (BSIM1 and BSIM2) parameters are can be generated
automatically. J. Pierret [4] describes a means of generating a ‘process’ file, and the program
ngproc2mod provided with ngspice converts this file into a sequence of BSIM1 .model lines
suitable for inclusion in an ngspice input file.
Parameters marked below with an *in the l/w column also have corresponding parameters with
a length and width dependency. For example, vfb is the basic parameter with units of Volts,
and lvfb and wvfb also exist and have units of Volt-meter.
The formula
P=P
0+P
L
Leffective
+P
W
Weffective
(11.1)
is used to evaluate the parameter for the actual device specified with
Leffective =Linput −DL (11.2)
Weffective =Winput −DW (11.3)
Note that unlike the other models in ngspice, the BSIM models are designed for use with a
process characterization system that provides all the parameters, thus there are no defaults for
the parameters, and leaving one out is considered an error. For an example set of parameters
and the format of a process file, see the SPICE2 implementation notes[3]. For more information
on BSIM2, see reference [5]. BSIM3 (11.2.9) and BSIM4 (11.2.10) represent state of the art
for submicron and deep submicron IC design.
11.2.7 BSIM1 model (level 4)
BSIM1 model (the first is a long series) is an empirical model. Developers placed less emp-
hasis on device physics and based the model on parametrical polynomial equations to model
the various physical effects. This approach pays in terms of circuit simulation behavior but the
accuracy degrades in the submicron region. A known problem of this model is the negative out-
put conductance and the convergence problems, both related to poor behavior of the polynomial
equations.
144 CHAPTER 11. MOSFETS
Ngspice BSIM (level 4) parameters
Name Parameter Units l/w
VFB Flat-band voltage V*
PHI Surface inversion potential V*
K1 Body effect coefficient √V*
K2 Drain/source depletion charge-sharing
coefficient
- *
ETA Zero-bias drain-induced barrier-lowering
coefficient
- *
MUZ Zero-bias mobility cm2
/V·sec
DL Shortening of channel µm
DW Narrowing of channel µm
U0 Zero-bias transverse-field mobility degradation
coefficient
1
/V*
U1 Zero-bias velocity saturation coefficient µ/V*
X2MZ Sens. of mobility to substrate bias at v=0 cm2
/V2·sec *
X2E Sens. of drain-induced barrier lowering effect
to substrate bias
1
/V*
X3E Sens. of drain-induced barrier lowering effect
to drain bias at Vds =Vdd
1
/V*
X2U0 Sens. of transverse field mobility degradation
effect to substrate bias
1
/V2*
X2U1 Sens. of velocity saturation effect to substrate
bias
µm
/V2*
MUS Mobility at zero substrate bias and at Vds =Vdd cm2
/V2sec
X2MS Sens. of mobility to substrate bias at Vds =Vdd cm2
/V2sec *
X3MS Sens. of mobility to drain bias at Vds =Vdd cm2
/V2sec *
X3U1 Sens. of velocity saturation effect on drain bias
at Vds=Vdd
µm
/V2*
TOX Gate oxide thickness µm
TEMP Temperature where parameters were measured ◦C
VDD Measurement bias range V
CGDO Gate-drain overlap capacitance per meter
channel width
F/m
CGSO Gate-source overlap capacitance per meter
channel width
F/m
CGBO Gate-bulk overlap capacitance per meter
channel length
F/m
XPART Gate-oxide capacitance-charge model flag -
N0 Zero-bias subthreshold slope coefficient - *
NB Sens. of subthreshold slope to substrate bias - *
ND Sens. of subthreshold slope to drain bias - *
RSH Drain and source diffusion sheet resistance Ω
/
JS Source drain junction current density A
/m2
PB Built in potential of source drain junction V
MJ Grading coefficient of source drain junction -
11.2. MOSFET MODELS (NMOS/PMOS) 145
Name Parameter Units l/w
PBSW Built in potential of source, drain junction
sidewall
V
MJSW Grading coefficient of source drain junction
sidewall
-
CJ Source drain junction capacitance per unit area F/m2
CJSW source drain junction sidewall capacitance per
unit length
F/m
WDF Source drain junction default width m
DELL Source drain junction length reduction m
xpart = 0 selects a 40/60 drain/source charge partition in saturation, while xpart=1 selects
a 0/100 drain/source charge partition. nd,ng, and ns are the drain, gate, and source nodes,
respectively. mname is the model name, area is the area factor, and off indicates an (optional)
initial condition on the device for dc analysis. If the area factor is omitted, a value of 1.0 is
assumed. The (optional) initial condition specification, using ic=vds,vgs is intended for use
with the uic option on the .tran control line, when a transient analysis is desired starting from
other than the quiescent operating point. See the .ic control line for a better way to set initial
conditions.
11.2.8 BSIM2 model (level 5)
This model contains many improvements over BSIM1 and is suitable for analog simulation.
Nevertheless, even BSIM2 breaks transistor operation into several distinct regions and this leads
to discontinuities in the first derivative in C-V and I-V characteristics that can cause numerical
problems during simulation.
11.2.9 BSIM3 model (levels 8, 49)
BSIM3 solves the numerical problems of previous models with the introduction of smoothing
functions. It adopts a single equation to describe device characteristics in the operating regions.
This approach eliminates the discontinuities in the I-V and C-V characteristics. The origi-
nal model, BSIM3 evolved through three versions: BSIM3v1, BSIM3v2 and BSIM3v3. Both
BSIM3v1 and BSIM3v2 had suffered from many mathematical problems and were replaced by
BSIM3v3. The latter is the only surviving release and has itself a long revision history.
The following table summarizes the story of this model:
Release Date Notes Version flag
BSIM3v3.0 10/30/1995 3.0
BSIM3v3.1 12/09/1996 3.1
BSIM3v3.2 06/16/1998 Revisions available: BSIM3v3.2.2,
BSIM3v3.2.3, and BSIM3v3.2.4
Parallel processing with OpenMP is available
for BSIM3v3.2.4.
3.2, 3.2.2,
3.2.3, 3.2.4
BSIM3v3.3 07/29/2005 Parallel processing with OpenMP is available
for this model.
3.3.0
146 CHAPTER 11. MOSFETS
BSIM3v2 and 3v3 models has proved for accurate use in 0.18 µmtechnologies. The model is
publicly available as source code form from University of California, Berkeley.
A detailed description is given in the user’s manual available from here .
We recommend that you use only the most recent BSIM3 model (version 3.3.0), because it
contains corrections to all known bugs. To achieve that, change the version parameter in your
modelcard files to
VERSION = 3.3.0.
If no version number is given in the .model card, this (newest) version is selected as the default.
The older models will not be supported, they are made available for reference only.
BSIM3v3.2.4 supports the extra model parameter lmlt on channel length scaling.
11.2.10 BSIM4 model (levels 14, 54)
This is the newest class of the BSIM family and introduces noise modeling and extrinsic para-
sitics. BSIM4, as the extension of BSIM3 model, addresses the MOSFET physical effects into
sub-100nm regime. It is a physics-based, accurate, scalable, robust and predictive MOSFET
SPICE model for circuit simulation and CMOS technology development. It is developed by
the BSIM Research Group in the Department of Electrical Engineering and Computer Sciences
(EECS) at the University of California, Berkeley (see BSIM4 home page). BSIM4 has a long
revision history, which is summarized below.
Release Date Notes Version flag
BSIM4.0.0 03/24/2000
BSIM4.1.0 10/11/2000
BSIM4.2.0 04/06/2001
BSIM4.2.1 10/05/2001 * 4.2.1
BSIM4.3.0 05/09/2003 * 4.3.0
BSIM4.4.0 03/04/2004 * 4.4.0
BSIM4.5.0 07/29/2005 * ** 4.5.0
BSIM4.6.0 12/13/2006
...
BSIM4.6.5 09/09/2009 * ** 4.6.5
BSIM4.7.0 04/08/2011 * ** 4.7
BSIM4.8.0 30/10/2013 * ** 4.8
*) supported in ngspice, using e.g. the version=<version flag> flag in the parameter file.
**) Parallel processing using OpenMP support is available for this model.
Details of any revision are to be found in the Berkeley user’s manuals, a pdf download of the
most recent edition is to be found here .
We recommend that you use only the most recent BSIM4 model (version 4.8.0), because it
contains corrections to all known bugs. To achieve that, change the version parameter in your
modelcard files to
VERSION = 4.8.
If no version number is given in the .model card, this (newest) version is selected as the default.
The older models will typically not be supported, they are made available for reference only.
11.2. MOSFET MODELS (NMOS/PMOS) 147
11.2.11 EKV model
Level 44 model (EKV) is not available in the standard distribution since it is not released in
source form by the EKV group. To obtain the code please refer to the (EKV model home page,
EKV group home page). A verilog-A version is available contributed by Ivan Riis Nielsen
11/2006.
11.2.12 BSIMSOI models (levels 10, 58, 55, 56, 57)
BSIMSOI is a SPICE compact model for SOI (Silicon-On-Insulator) circuit design, created by
University of California at Berkeley . This model is formulated on top of the BSIM3 frame-
work. It shares the same basic equations with the bulk model so that the physical nature and
smoothness of BSIM3v3 are retained. Four models are supported in ngspice, those based on
BSIM3 and modeling fully depleted (FD, level 55), partially depleted (PD, level 57) and both
(DD, level 56), as well as the modern BSIMSOI version 4 model (levels 10, 58). Detailed des-
criptions are beyond the scope of this manual, but see e.g. BSIMSOIv4.4 User Manual for a
very extensive description of the recent model version. OpenMP support is available for levels
10, 58, version 4.4.
11.2.13 SOI3 model (level 60)
see literature citation [18] for a description.
11.2.14 HiSIM models of the University of Hiroshima
There are two model implementations available - see also HiSIM Research Center:
1. HiSIM2 model: Surface-Potential-Based MOSFET Model for Circuit Simulation version
2.8.0 - level 68 (see link to HiSIM2 for source code and manual).
2. HiSIM_HV model: Surface-Potential-Based HV/LD-MOSFET Model for Circuit Simu-
lation version 1.2.4 and 2.2.0 - level 73 (see link to HiSIM_HV for source code and
manual).
148 CHAPTER 11. MOSFETS
Chapter 12
Mixed-Mode and Behavioral Modeling
with XSPICE
Ngspice implements XSPICE extensions for behavioral and mixed-mode (analog and digital)
modeling. In the XSPICE framework this is referred to as code level modeling. Behavioral
modeling may benefit dramatically because XSPICE offers a means to add analog functionality
programmed in C. Many examples (amplifiers, oscillators, filters ...) are presented in the follo-
wing. Even more flexibility is available because you may define your own models and use them
in addition and in combination with all the already existing ngspice functionality. Mixed mode
simulation is speeded up significantly by simulating the digital part in an event driven manner,
in that state equations use only a few allowed states and are evaluated only during switching,
and not continuously in time and signal as in a pure analog simulator.
This chapter describes the predefined models available in ngspice, stemming from the original
XSPICE simulator. The instructions for writing new code models are given in Chapt. 28.
To make use of the XSPICE extensions, you need to compile them in. Linux, CYGWIN,
MINGW and other users may add the flag --enable-xspice to their ./configure com-
mand and then recompile. The prebuilt ngspice for Windows distribution has XSPICE already
enabled. For detailed compiling instructions see Chapt. 32.1.
12.1 Code Model Element & .MODEL Cards
12.1.1 Syntax
Ngspice includes a library of predefined ‘Code Models’ that can be placed within any circuit
description in a manner similar to that used to place standard device models. Code model in-
stance cards always begin with the letter ‘A’, and always make use of a .MODEL card to describe
the code model desired. Section 28 of this document goes into greater detail as to how a code
model similar to the predefined models may be developed, but once any model is created and
linked into the simulator it may be placed using one instance card and one .MODEL card (note
here we conform to the SPICE custom of referring to a single logical line of information as a
‘card’). As an example, the following uses a predefined ‘gain’ code model taking as an input
some value on node 1, multiplies it by a gain of 5.0, and outputs the new value to node 2.
Note that, by convention, input ports are specified first on code models. Output ports follow the
inputs.
149
150 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Example:
a1 1 2 amp
.model amp gain(gain =5.0)
In this example the numerical values picked up from single-ended (i.e. ground referenced)
input node 1 and output to single-ended output node 2 will be voltages, since in the Interface
Specification File for this code model (i.e., gain), the default port type is specified as a voltage
(more on this later). However, if you didn’t know this, the following modifications to the
instance card could be used to insure it:
Example:
a1 %v(1) %v(2) amp
.model amp gain(gain =5.0)
The specification %v preceding the input and output node numbers of the instance card indicate
to the simulator that the inputs to the model should be single-ended voltage values. Other
possibilities exist, as described later.
Some of the other features of the instance and .MODEL cards are worth noting. Of particular
interest is the portion of the .MODEL card that specifies gain=5.0. This portion of the card
assigns a value to a parameter of the ‘gain’ model. There are other parameters that can be assig-
ned values for this model, and in general code models will have several. In addition to numeric
values, code model parameters can take non-numeric values (such as TRUE and FALSE), and
even vector values. All of these topics will be discussed at length in the following pages. In
general, however, the instance and .MODEL cards that define a code model will follow the ab-
stract form described below. This form illustrates that the number of inputs and outputs and the
number of parameters that can be specified is relatively open-ended and can be interpreted in a
variety of ways (note that angle-brackets ‘<’ and ‘>’ enclose optional inputs):
Example:
AXXXXXXX <%v ,%i ,% vd ,% id ,%g ,% gd ,%h,%hd , or %d>
+ <[> <~><%v ,%i,%vd ,%id ,%g ,%gd ,%h ,% hd , or %d>
+ <NIN1 or +NIN1 -NIN1 or "null">
+ <~ >... < NIN2 .. <]> >
+ <%v ,%i ,%vd ,% id ,%g,%gd ,%h ,%hd ,%d or %vnam >
+ <[> <~><%v ,%i,%vd ,%id ,%g ,%gd ,%h ,% hd ,
or %d><NOUT1 or +NOUT1 -NOUT1 >
+ <~ >... < NOUT2 .. <]>>
+ MODELNAME
.MODEL MODELNAME MODELTYPE
+ <( PARAMNAME1 = <[> VAL1 <VAL2 ... <]>> PARAMNAME2 ..>)>
12.1. CODE MODEL ELEMENT & .MODEL CARDS 151
Square brackets ([ ]) are used to enclose vector input nodes. In addition, these brackets are used
to delineate vectors of parameters.
The literal string ‘null’, when included in a node list, is interpreted as no connection at that input
to the model. ‘Null’ is not allowed as the name of a model’s input or output if the model only
has one input or one output. Also, ‘null’ should only be used to indicate a missing connection
for a code model; use on other XSPICE component is not interpreted as a missing connection,
but will be interpreted as an actual node name.
The tilde, ‘~’, when prepended to a digital node name, specifies that the logical value of that
node be inverted prior to being passed to the code model. This allows for simple inversion of
input and output polarities of a digital model in order to handle logically equivalent cases and
others that frequently arise in digital system design. The following example defines a NAND
gate, one input of which is inverted:
a1 [~1 2] 3 nand1
.model nand1 d_nand ( rise_delay =0.1 fall_delay =0.2)
The optional symbols %v, %i, %vd, etc. specify the type of port the simulator is to expect for
the subsequent port or port vector. The meaning of each symbol is given in Table 12.1.
The symbols described in Table 12.1 may be omitted if the default port type for the model is
desired. Note that non-default port types for multi-input or multi-output (vector) ports must be
specified by placing one of the symbols in front of EACH vector port. On the other hand, if all
ports of a vector port are to be declared as having the same non-default type, then a symbol may
be specified immediately prior to the opening bracket of the vector. The following examples
should make this clear:
Example 1: - Specifies two differential voltage connections, one
to nodes 1 & 2, and one to nodes 3 & 4.
%vd [1 2 3 4]
Example 2: - Specifies two single-ended connections to node 1 and
at node 2, and one differential connection to
nodes 3 & 4.
%v [1 2 %vd 3 4]
Example 3: - Identical to the previous example...parenthesis
are added for additional clarity.
%v [1 2 %vd(3 4)]
Example 4: - Specifies that the node numbers are to be treated in the
default fashion for the particular model.
If this model had ‘%v” as a default for this
port, then this notation would represent four single-ended
voltage connections.
[1 2 3 4]
152 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Port Type Modifiers
Modifier Interpretation
%v represents a single-ended voltage port - one node name or number is expected
for each port.
%i represents a single-ended current port - one node name or number is expected
for each port.
%g represents a single-ended voltage-input, current-output (VCCS) port - one
node name or number is expected for each port. This type of port is auto-
matically an input/output.
%h represents a single-ended current-input, voltage-output (CCVS) port - one
node name or number is expected for each port. This type of port is auto-
matically an input/output.
%d represents a digital port - one node name or number is expected for each port.
This type of port may be either an input or an output.
%vnam represents the name of a voltage source, the current through which is taken as
an input. This notation is provided primarily in order to allow models defined
using SPICE2G6 syntax to operate properly in XSPICE.
%vd represents a differential voltage port - two node names or numbers are ex-
pected for each port.
%id represents a differential current port - two node names or numbers are ex-
pected for each port.
%gd represents a differential VCCS port - two node names or numbers are expected
for each port.
%hd represents a differential CCVS port - two node names or numbers are expected
for each port.
Table 12.1: Port Type Modifiers
12.1. CODE MODEL ELEMENT & .MODEL CARDS 153
The parameter names listed on the .MODEL card must be identical to those named in the code
model itself. The parameters for each predefined code model are described in detail in Sections
12.2 (analog), 12.3 (Hybrid, A/D) and 12.4 (digital) . The steps required in order to specify
parameters for user-defined models are described in Chapter 28.
12.1.2 Examples
The following is a list of instance card and associated .MODEL card examples showing use of
predefined models within an XSPICE deck:
a1 1 2 amp
.model amp gain(in_offset=0.1 gain=5.0 out_offset=-0.01)
a2 %i[1 2] 3 sum1
.model sum1 summer(in_offset=[0.1 -0.2] in_gain=[2.0 1.0]
+ out_gain=5.0 out_offset=-0.01)
a21 %i[1 %vd(2 5) 7 10] 3 sum2
.model sum2 summer(out_gain=10.0)
a5 1 2 limit5
.model limit5 limit(in_offset=0.1 gain=2.5
+ out_lower.limit=-5.0 out_upper_limit=5.0 limit_domain=0.10
+ fraction=FALSE)
a7 2 %id(4 7) xfer.cntl1
.model xfer_cntl1 pwl(x_array=[-2.0 -1.0 2.0 4.0 5.0]
+ y_array=[-0.2 -0.2 0.1 2.0 10.0]
+ input_domain=0.05 fraction=TRUE)
a8 3 %gd(6 7) switch3
.model switch3 aswitch(cntl_off=0.0 cntl_on=5.0 r_off=1e6
+ r_on=10.0 log=TRUE)
12.1.3 Search path for file input
Several code models (filesource 12.2.8,d_source 12.4.21,d_state 12.4.18) call additional
files for supply of input data. A call to file="path/filename" (or input_file=, state_file=)
in the .model card will start a search sequence for finding the file. path may be an absolute
path. If path is omitted or is a relative path, filename is looked for according to the following
search list:
Infile_Path/<path/filename> (Infile_Path is the path of the input file *.sp containing the
netlist)
NGSPICE_INPUT_DIR/<path/filename> (where an additional path is set by the environmen-
tal variable)
<path/filename> (where the search is relativ to the current directory (OS dependant))
154 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
12.2 Analog Models
The following analog models are supplied with XSPICE. The descriptions included consist
of the model Interface Specification File and a description of the model’s operation. This is
followed by an example of a simulator-deck placement of the model, including the .MODEL
card and the specification of all available parameters.
12.2.1 Gain
NAME_TABLE:
C_Function_Name: cm_gain
Spice_Model_Name: gain
Description: "A simple gain block"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id]
Vector: no no
Vector.Bounds: - -
Null.Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset gain out_offset
Description: "input offset" "gain" "output offset"
Data_Type: real real real
Default_Value: 0.0 1.0 0.0
Limits: - - -
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: yes yes yes
Description: This function is a simple gain block with optional offsets on the input and the
output. The input offset is added to the input, the sum is then multiplied by the gain, and
the result is produced by adding the output offset. This model will operate in DC, AC,
and Transient analysis modes.
Example:
a1 1 2 amp
. model amp gain (in_offset =0.1 gain =5.0
+ out_offset = -0.01)
12.2. ANALOG MODELS 155
12.2.2 Summer
NAME_TABLE:
C_Function_Name: cm_summer
Spice_Model_Name: summer
Description: "A summer block"
PORT_TABLE:
Port Name: in out
Description: "input vector" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id]
Vector: yes no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset in_gain
Description: "input offset vector" "input gain vector"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: yes yes
Vector_Bounds: in in
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: out_gain out_offset
Description: "output gain" "output offset"
Data_Type: real real
Default_Value: 1.0 0.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: This function is a summer block with 2-to-N input ports. Individual gains and
offsets can be applied to each input and to the output. Each input is added to its respective
offset and then multiplied by its gain. The results are then summed, multiplied by the
output gain and added to the output offset. This model will operate in DC, AC, and
Transient analysis modes.
Example usage:
a2 [1 2] 3 sum1
.model sum1 summer( in_offset =[0.1 -0.2] in_gain =[2.0 1.0]
+ out_gain =5.0 out_offset = -0.01)
156 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
12.2.3 Multiplier
NAME_TABLE:
C_Function_Name: cm_mult
Spice_Model_Name: mult
Description: "multiplier block"
PORT_TABLE:
Port_Name: in out
Description: "input vector" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id]
Vector: yes no
Vector_Bounds: [2 -] -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset in_gain
Description: "input offset vector" "input gain vector"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: yes yes
Vector_Bounds: in in
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: out_gain out_offset
Description: "output gain" "output offset"
Data_Type: real real
Default_Value: 1.0 0.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: This function is a multiplier block with 2-to-N input ports. Individual gains and
offsets can be applied to each input and to the output. Each input is added to its respective
offset and then multiplied by its gain. The results are multiplied along with the output
gain and are added to the output offset. This model will operate in DC, AC, and Transient
analysis modes. However, in ac analysis it is important to remember that results are
invalid unless only one input of the multiplier is connected to a node that i connected to
an AC signal (this is exemplified by the use of a multiplier to perform a potentiometer
function: one input is DC, the other carries the AC signal).
Example SPICE Usage:
a3 [1 2 3] 4 sigmult
.model sigmult mult ( in_offset =[0.1 0.1 -0.1]
+ in_gain =[10.0 10.0 10.0] out_gain =5.0 out_offset =0.05)
12.2. ANALOG MODELS 157
12.2.4 Divider
NAME_TABLE:
C_Function_Name: cm_divide
Spice_Model_Name: divide
Description: "divider block"
PORT_TABLE:
Port_Name: num den out
Description: "numerator" "denominator" "output"
Direction: in in out
Default_Type: v v v
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id,vnam] [v,vd,i,id]
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: no no no
PARAMETER_TABLE:
Parameter_Name: num_offset num_gain
Description: "numerator offset" "numerator gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: den_offset den_gain
Description: "denominator offset" "denominator gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: den_lower_limit
Description: "denominator lower limit"
Data_Type: real
Default_Value: 1.0e-10
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: den_domain
Description: "denominator smoothing domain"
Data_Type: real
Default_Value: 1.0e-10
Limits: -
Vector: no
158 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: fraction
Description: "smoothing fraction/absolute value switch"
Data_Type: boolean
Default_Value: false
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: out_gain out_offset
Description: "output gain" "output offset"
Data_Type: real real
Default_Value: 1.0 0.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: This function is a two-quadrant divider. It takes two inputs; num (numerator) and
den (denominator). Divide offsets its inputs, multiplies them by their respective gains,
divides the results, multiplies the quotient by the output gain, and offsets the result. The
denominator is limited to a value above zero via a user specified lower limit. This limit
is approached through a quadratic smoothing function, the domain of which may be spe-
cified as a fraction of the lower limit value (default), or as an absolute value. This model
will operate in DC, AC and Transient analysis modes. However, in ac analysis it is impor-
tant to remember that results are invalid unless only one input of the divider is connected
to a node that is connected to an ac signal (this is exemplified by the use of the divider to
perform a potentiometer function: one input is dc, the other carries the ac signal).
Example SPICE Usage:
a4 1 2 4 divider
.model divider divide(num_offset=0.1 num_gain=2.5 den_offset=-0.1
+ den_gain=5.0 den_lower.limit=1e-5 den_domain=1e-6
+ fraction=FALSE out_gain=1.0 out_offset=0.0)
12.2.5 Limiter
NAME_TABLE:
C_Function_Name: cm_limit
Spice_Model_Name: limit
Description: "limit block"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
12.2. ANALOG MODELS 159
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset gain
Description: "input offset" "gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: out_lower_limit out_upper_limit
Description: "output lower limit" "output upper limit"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: limit_range
Description: "upper & lower smoothing range"
Data_Type: real
Default_Value: 1.0e-6
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: fraction
Description: "smoothing fraction/absolute value switch"
Data_Type: boolean
Default_Value: FALSE
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The Limiter is a single input, single output function similar to the Gain Block.
However, the output of the Limiter function is restricted to the range specified by the
output lower and upper limits. This model will operate in DC, AC and Transient analysis
modes. Note that the limit range is the value below the upper limit and above the lower
limit at which smoothing of the output begins. For this model, then, the limit range
represents the delta with respect to the output level at which smoothing occurs. Thus, for
160 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
an input gain of 2.0 and output limits of 1.0 and -1.0 volts, the output will begin to smooth
out at ±0.9 volts, which occurs when the input value is at ±0.4.
Example SPICE Usage:
a5 1 2 limit5
.model limit5 limit(in_offset=0.1 gain=2.5 out_lower_limit=-5.0
+ out_upper_limit=5.0 limit_range=0.10 fraction=FALSE)
12.2.6 Controlled Limiter
NAME_TABLE:
C_Function_Name: cm_climit
Spice_Model_Name: climit
Description: "controlled limiter block"
PORT_TABLE:
Port_Name: in cntl_upper
Description: "input" "upper lim. control input"
Direction: in in
Default_Type: v v
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id,vnam]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PORT_TABLE:
Port_Name: cntl_lower out
Description: "lower limit control input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset gain
Description: "input offset" "gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: upper_delta lower_delta
Description: "output upper delta" "output lower delta"
Data_Type: real real
Default_Value: 0.0 0.0
Limits: - -
Vector: no no
12.2. ANALOG MODELS 161
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: limit_range fraction
Description: "upper & lower sm. range" "smoothing %/abs switch"
Data_Type: real boolean
Default_Value: 1.0e-6 FALSE
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The Controlled Limiter is a single input, single output function similar to the Gain
Block. However, the output of the Limiter function is restricted to the range specified by
the output lower and upper limits. This model will operate in DC, AC, and Transient
analysis modes. Note that the limit range is the value below the cntl_upper limit and
above the cntl_lower limit at which smoothing of the output begins (minimum positive
value of voltage must exist between the cntl_upper input and the cntl_lower input at
all times). For this model, then, the limit range represents the delta with respect to the
output level at which smoothing occurs. Thus, for an input gain of 2.0 and output limits
of 1.0 and -1.0 volts, the output will begin to smooth out at ±0.9 volts, which occurs
when the input value is at ±0.4. Note also that the Controlled Limiter code tests the
input values of cntl_upper and cntl_lower to make sure that they are spaced far enough
apart to guarantee the existence of a linear range between them. The range is calculated
as the difference between (cntl_upper −upper_delta −limit_range) and (cntl_lower +
lower_delta +limit_range) and must be greater than or equal to zero. Note that when
the limit range is specified as a fractional value, the limit range used in the above is taken
as the calculated fraction of the difference between cntl_upper and cntl_lower. Still, the
potential exists for too great a limit range value to be specified for proper operation, in
which case the model will return an error message.
Example SPICE Usage:
a6 3 6 8 4 varlimit
.
.
.model varlimit climit(in_offset=0.1 gain=2.5 upper_delta=0.0
+ lower_delta=0.0 limit_range=0.10 fraction=FALSE)
12.2.7 PWL Controlled Source
NAME_TABLE:
C_Function_Name: cm_pwl
Spice_Model_Name: pwl
Description: "piecewise linear controlled source"
PORT_TABLE:
Port_Name: in out
Description: "input" "output"
Direction: in out
162 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Default_Type: v v
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: x_array y_array
Description: "x-element array" "y-element array"
Data_Type: real real
Default_Value: - -
Limits: - -
Vector: yes yes
Vector_Bounds: [2 -] [2 -]
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: input_domain fraction
Description: "input sm. domain" "smoothing %/abs switch"
Data_Type: real boolean
Default_Value: 0.01 TRUE
Limits: [1e-12 0.5] -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
STATIC_VAR_TABLE:
Static_Var_Name: last_x_value
Data_Type: pointer
Description: "iteration holding variable for limiting"
Description: The Piece-Wise Linear Controlled Source is a single input, single output function
similar to the Gain Block. However, the output of the PWL Source is not necessarily li-
near for all values of input. Instead, it follows an I/O relationship specified by you via the
x_array and y_array coordinates. This is detailed below.
The x_array and y_array values represent vectors of coordinate points on the x and
y axes, respectively. The x_array values are progressively increasing input coordinate
points, and the associated y_array values represent the outputs at those points. There
may be as few as two (x_array[n], y_array[n]) pairs specified, or as many as memory
and simulation speed allow. This permits you to very finely approximate a non-linear
function by capturing multiple input-output coordinate points.
Two aspects of the PWL Controlled Source warrant special attention. These are the hand-
ling of endpoints and the smoothing of the described transfer function near coordinate
points.
In order to fully specify outputs for values of in outside of the bounds of the PWL
function (i.e., less than x_array[0] or greater than x_array[n], where n is the largest
user-specified coordinate index), the PWL Controlled Source model extends the slope
found between the lowest two coordinate pairs and the highest two coordinate pairs.
This has the effect of making the transfer function completely linear for in less than
x_array[0] and in greater than x_array[n]. It also has the potentially subtle effect of
unrealistically causing an output to reach a very large or small value for large inputs. You
12.2. ANALOG MODELS 163
should thus keep in mind that the PWL Source does not inherently provide a limiting
capability.
In order to diminish the potential for non-convergence of simulations when using the
PWL block, a form of smoothing around the x_array,y_array coordinate points is ne-
cessary. This is due to the iterative nature of the simulator and its reliance on smooth first
derivatives of transfer functions in order to arrive at a matrix solution. Consequently, the
input_domain and fraction parameters are included to allow you some control over
the amount and nature of the smoothing performed.
Fraction is a switch that is either TRUE or FALSE. When TRUE (the default setting),
the simulator assumes that the specified input domain value is to be interpreted as a fracti-
onal figure. Otherwise, it is interpreted as an absolute value. Thus, if fraction=TRUE
and input_domain=0.10, The simulator assumes that the smoothing radius about each
coordinate point is to be set equal to 10% of the length of either the x_array segment
above each coordinate point, or the x_array segment below each coordinate point. The
specific segment length chosen will be the smallest of these two for each coordinate point.
On the other hand, if fraction=FALSE and input=0.10, then the simulator will begin
smoothing the transfer function at 0.10 volts (or amperes) below each x_array coordi-
nate and will continue the smoothing process for another 0.10 volts (or amperes) above
each x_array coordinate point. Since the overlap of smoothing domains is not allowed,
checking is done by the model to ensure that the specified input domain value is not ex-
cessive.
One subtle consequence of the use of the fraction=TRUE feature of the PWL Con-
trolled Source is that, in certain cases, you may inadvertently create extreme smoothing
of functions by choosing inappropriate coordinate value points. This can be demonstra-
ted by considering a function described by three coordinate pairs, such as (-1,-1), (1,1),
and (2,1). In this case, with a 10% input_domain value specified (fraction=TRUE,
input_domain=0.10), you would expect to see rounding occur between in=0.9 and
in=1.1, and nowhere else. On the other hand, if you were to specify the same function
using the coordinate pairs (-100,-100), (1,1) and (201,1), you would find that rounding
occurs between in=-19 and in=21. Clearly in the latter case the smoothing might cause
an excessive divergence from the intended linearity above and below in=1.
Example SPICE Usage:
a7 2 4 xfer_cntl1
.
.
.model xfer_cntl1 pwl(x_array=[-2.0 -1.0 2.0 4.0 5.0]
+ y_array=[-0.2 -0.2 0.1 2.0 10.0]
+ input_domain=0.05 fraction=TRUE)
12.2.8 Filesource
NAME_TABLE:
C_Function_Name: cm_filesource
Spice_Model_Name: filesource
Description: "File Source"
PORT_TABLE:
Port_Name: out
164 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Description: "output"
Direction: out
Default_Type: v
Allowed_Types: [v,vd,i,id]
Vector: yes
Vector_Bounds: [1 -]
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: timeoffset timescale
Description: "time offset" "timescale"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: timerelative amplstep
Description: "relative time" "step amplitude"
Data_Type: boolean boolean
Default_Value: FALSE FALSE
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: amploffset amplscale
Description: "ampl offset" "amplscale"
Data_Type: real real
Default_Value: - -
Limits: - -
Vector: yes yes
Vector_Bounds: [1 -] [1 -]
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: file
Description: "file name"
Data_Type: string
Default_Value: "filesource.txt"
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The File Source is similar to the Piece-Wise Linear Source, except that the wa-
veform data is read from a file instead of being taken from parameter vectors. The file
format is line oriented ASCII. ‘#’ and ‘;’ are comment characters; all characters from
a comment character until the end of the line are ignored. Each line consists of two or
12.2. ANALOG MODELS 165
more real values. The first value is the time; subsequent values correspond to the outputs.
Values are separated by spaces. Time values are absolute and must be monotonically in-
creasing, unless timerelative is set to TRUE, in which case the values specify the interval
between two samples and must be positive. Waveforms may be scaled and shifted in the
time dimension by setting timescale and timeoffset.
Amplitudes can also be scaled and shifted using amplscale and amploffset. Amplitudes
are normally interpolated between two samples, unless amplstep is set to TRUE.
Note: The file named by the parameter filename in file="filename" is sought after accor-
ding to a search list described in12.1.3.
Example SPICE Usage:
a8 %vd([1 0 2 0]) filesrc
.
.
.model filesrc filesource (file="sine.m" amploffset=[0 0] amplscale=[1 1]
+ timeoffset=0 timescale=1
+ timerelative=false amplstep=false)
Example input file:
# name: sine.m
# two output ports
# column 1: time
# columns 2, 3: values
001
3.90625e-09 0.02454122852291229 0.9996988186962042
7.8125e-09 0.04906767432741801 0.9987954562051724
1.171875e-08 0.07356456359966743 0.9972904566786902
...
12.2.9 multi_input_pwl block
NAME_TABLE:
C_Function_Name: cm_multi_input_pwl
Spice_Model_Name: multi_input_pwl
Description: "multi_input_pwl block"
PORT_TABLE:
Port_Name: in out
Description: "input array" "output"
Direction: in out
Default_Type: vd vd
Allowed_Types: [vd,id] [vd,id]
Vector: yes no
Vector_Bounds: [2 -] -
Null_Allowed: no no
PARAMETER_TABLE:
166 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Parameter_Name: x y
Description: "x array" "y array"
Data_Type: real real
Default_Value: 0.0 0.0
Limits: - -
Vector: yes yes
Vector_Bounds: [2 -] [2 -]
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: model
Description: "model type"
Data_Type: string
Default_Value: "and"
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: Multi-input gate voltage controlled voltage source that supports and or or gating.
The x’s and y’s represent the piecewise linear variation of output (y) as a function of input
(x). The type of gate is selectable by the parameter model. In case the model is and, the
smallest input determines the output value (i.e. the and function). In case the model is or,
the largest input determines the output value (i.e. the or function). The inverse of these
functions (i.e. nand and nor) is constructed by complementing the y array.
Example SPICE Usage:
a82[102030]70pwlm
.
.
.model pwlm multi_input_pwl((x=[-2.0 -1.0 2.0 4.0 5.0]
+ y=[-0.2 -0.2 0.1 2.0 10.0]
+ model="and")
12.2.10 Analog Switch
NAME_TABLE:
C_Function_Name: cm_aswitch
Spice_Model_Name: aswitch
Description: "analog switch"
PORT_TABLE:
Port Name: cntl_in out
Description: "input" "resistive output"
Direction: in out
Default_Type: v gd
Allowed_Types: [v,vd,i,id] [gd]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
12.2. ANALOG MODELS 167
PARAMETER_TABLE:
Parameter_Name: cntl_off cntl_on
Description: "control ‘off’ value" "control ‘on’ value"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: r_off log
Description: "off resistance" "log/linear switch"
Data_Type: real boolean
Default_Value: 1.0e12 TRUE
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: r_on
Description: "on resistance"
Data_Type: real
Default_Value: 1.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The Analog Switch is a resistor that varies either logarithmically or linearly be-
tween specified values of a controlling input voltage or current. Note that the input is
not internally limited. Therefore, if the controlling signal exceeds the specified OFF state
or ON state value, the resistance may become excessively large or excessively small (in
the case of logarithmic dependence), or may become negative (in the case of linear de-
pendence). For the experienced user, these excursions may prove valuable for modeling
certain devices, but in most cases you are advised to add limiting of the controlling input
if the possibility of excessive control value variation exists.
Example SPICE Usage:
a8 3 %gd(6 7) switch3
.
.
.model switch3 aswitch(cntl_off=0.0 cntl_on=5.0 r_off=1e6
+ r_on=10.0 log=TRUE)
12.2.11 Zener Diode
NAME_TABLE:
C_Function_Name: cm_zener
168 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Spice_Model_Name: zener
Description: "zener diode"
PORT_TABLE:
Port Name: z
Description: "zener"
Direction: inout
Default_Type: gd
Allowed_Types: [gd]
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: v_breakdown i_breakdown
Description: "breakdown voltage" "breakdown current"
Data_Type: real real
Default_Value: - 2.0e-2
Limits: [1.0e-6 1.0e6] [1.0e-9 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no yes
PARAMETER_TABLE:
Parameter_Name: i_sat n_forward
Description: "saturation current" "forward emission coefficient"
Data_Type: real real
Default_Value: 1.0e-12 1.0
Limits: [1.0e-15 -] [0.1 10]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: limit_switch
Description: "switch for on-board limiting (convergence aid)"
Data_Type: boolean
Default_Value: FALSE
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
STATIC_VAR_TABLE:
Static_Var_Name: previous_voltage
Data_Type: pointer
Description: "iteration holding variable for limiting"
Description: The Zener Diode models the DC characteristics of most zeners. This model
differs from the Diode/Rectifier by providing a user-defined dynamic resistance in the
reverse breakdown region. The forward characteristic is defined by only a single point,
since most data sheets for zener diodes do not give detailed characteristics in the forward
region.
12.2. ANALOG MODELS 169
The first three parameters define the DC characteristics of the zener in the breakdown
region and are usually explicitly given on the data sheet.
The saturation current refers to the relatively constant reverse current that is produced
when the voltage across the zener is negative, but breakdown has not been reached. The
reverse leakage current determines the slight increase in reverse current as the voltage
across the zener becomes more negative. It is modeled as a resistance parallel to the
zener with value v breakdown / i rev.
Note that the limit switch parameter engages an internal limiting function for the zener.
This can, in some cases, prevent the simulator from converging to an unrealistic solution
if the voltage across or current into the device is excessive. If use of this feature fails to
yield acceptable results, the convlimit option should be tried (add the following statement
to the SPICE input deck: .options convlimit)
Example SPICE Usage:
a9 3 4 vref10
.
.
.model vref10 zener(v_breakdown=10.0 i_breakdown=0.02
+ r_breakdown=1.0 i_rev=1e-6 i_sat=1e-12)
12.2.12 Current Limiter
NAME_TABLE:
C_Function_Name: cm_ilimit
Spice_Model_Name: ilimit
Description: "current limiter block"
PORT_TABLE:
Port Name: in pos_pwr
Description: "input" "positive power supply"
Direction: in inout
Default_Type: v g
Allowed_Types: [v,vd] [g,gd]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no yes
PORT_TABLE:
Port Name: neg_pwr out
Description: "negative power supply" "output"
Direction: inout inout
Default_Type: g g
Allowed_Types: [g,gd] [g,gd]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes no
PARAMETER_TABLE:
Parameter_Name: in_offset gain
Description: "input offset" "gain"
Data_Type: real real
170 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: r_out_source r_out_sink
Description: "sourcing resistance" "sinking resistance"
Data_Type: real real
Default_Value: 1.0 1.0
Limits: [1.0e-9 1.0e9] [1.0e-9 1.0e9]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: i_limit_source
Description: "current sourcing limit"
Data_Type: real
Default_Value: -
Limits: [1.0e-12 -]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: i_limit_sink
Description: "current sinking limit"
Data_Type: real
Default_Value: -
Limits: [1.0e-12 -]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: v_pwr_range i_source_range
Description: "upper & lower power "sourcing current
supply smoothing range" smoothing range"
Data_Type: real real
Default_Value: 1.0e-6 1.0e-9
Limits: [1.0e-15 -] [1.0e-15 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: i_sink_range
Description: "sinking current smoothing range"
Data_Type: real
Default_Value: 1.0e-9
Limits: [1.0e-15 -]
12.2. ANALOG MODELS 171
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: r_out_domain
Description: "internal/external voltage delta smoothing range"
Data_Type: real
Default_Value: 1.0e-9
Limits: [1.0e-15 -]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The Current Limiter models the behavior of an operational amplifier or compa-
rator device at a high level of abstraction. All of its pins act as inputs; three of the four
also act as outputs. The model takes as input a voltage value from the in connector. It
then applies an offset and a gain, and derives from it an equivalent internal voltage (veq),
which it limits to fall between pos_pwr and neg_pwr. If veq is greater than the output
voltage seen on the out connector, a sourcing current will flow from the output pin. Con-
versely, if the voltage is less than vout, a sinking current will flow into the output pin.
Depending on the polarity of the current flow, either a sourcing or a sinking resistance
value (r_out_source,r_out_sink) is applied to govern the vout/i_out relationship.
The chosen resistance will continue to control the output current until it reaches a max-
imum value specified by either i_limit_source or i_limit_sink. The latter mimics
the current limiting behavior of many operational amplifier output stages.
During all operation, the output current is reflected either in the pos_pwr connector cur-
rent or the neg_pwr current, depending on the polarity of i_out. Thus, realistic power
consumption as seen in the supply rails is included in the model.
The user-specified smoothing parameters relate to model operation as follows: v_pwr_range
controls the voltage below vpos_pwr and above vneg_pwr inputs beyond which veq =
gain(vin+vo f f set )is smoothed; i_source_range specifies the current below i_limit_source
at which smoothing begins, as well as specifying the current increment above i_out=0.0
at which i_pos_pwr begins to transition to zero; i_sink_range serves the same pur-
pose with respect to i_limit_sink and i_neg_pwr that i_source_range serves for
i_limit_source and i_pos_pwr;r_out_domain specifies the incremental value above
and below (veq-vout)=0.0 at which r_out will be set to r_out_source and r_out_sink,
respectively. For values of (veq-vout) less than r_out_domain and greater than -r_out_domain,
r_out is interpolated smoothly between r_out_source and r_out_sink.
Example SPICE Usage:
a10 3 10 20 4 amp3
.
.
.model amp3 ilimit(in_offset=0.0 gain=16.0 r_out_source=1.0
+ r_out_sink=1.0 i_limit_source=1e-3
+ i_limit_sink=10e-3 v_pwr_range=0.2
+ i_source_range=1e-6 i_sink_range=1e-6
+ r_out_domain=1e-6)
172 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
12.2.13 Hysteresis Block
NAME_TABLE:
C_Function_Name: cm_hyst
Spice_Model_Name: hyst
Description: "hysteresis block"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_low in_high
Description: "input low value" "input high value"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: hyst out_lower_limit
Description: "hysteresis" "output lower limit"
Data_Type: real real
Default_Value: 0.1 0.0
Limits: [0.0 -] -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: out_upper_limit input_domain
Description: "output upper limit" "input smoothing domain"
Data_Type: real real
Default_Value: 1.0 0.01
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: fraction
Description: "smoothing fraction/absolute value switch"
Data_Type: boolean
Default_Value: TRUE
Limits: -
Vector: no
12.2. ANALOG MODELS 173
Vector_Bounds: -
Null_Allowed: yes
Description: The Hysteresis block is a simple buffer stage that provides hysteresis of the output
with respect to the input. The in low and in high parameter values specify the center
voltage or current inputs about which the hysteresis effect operates. The output values
are limited to out lower limit and out upper limit. The value of hyst is added to the in
low and in high points in order to specify the points at which the slope of the hysteresis
function would normally change abruptly as the input transitions from a low to a high
value. Likewise, the value of hyst is subtracted from the in high and in low values in
order to specify the points at which the slope of the hysteresis function would normally
change abruptly as the input transitions from a high to a low value. In fact, the slope of the
hysteresis function is never allowed to change abruptly but is smoothly varied whenever
the input domain smoothing parameter is set greater than zero.
Example SPICE Usage:
a11 1 2 schmitt1
.
.
.model schmitt1 hyst(in_low=0.7 in_high=2.4 hyst=0.5
+ out_lower_limit=0.5 out_upper_limit=3.0
+ input_domain=0.01 fraction=TRUE)
12.2.14 Differentiator
NAME_TABLE:
C_Function_Name: cm_d_dt
Spice_Model_Name: d_dt
Description: "time-derivative block"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: gain out_offset
Description: "gain" "output offset"
Data_Type: real real
Default_Value: 1.0 0.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
174 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Parameter_Name: out_lower_limit out_upper_limit
Description: "output lower limit" "output upper limit"
Data_Type: real real
Default_Value: - -
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: limit_range
Description: "upper & lower limit smoothing range"
Data_Type: real
Default_Value: 1.0e-6
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The Differentiator block is a simple derivative stage that approximates the time
derivative of an input signal by calculating the incremental slope of that signal since the
previous time point. The block also includes gain and output offset parameters to allow
for tailoring of the required signal, and output upper and lower limits to prevent conver-
gence errors resulting from excessively large output values. The incremental value of
output below the output upper limit and above the output lower limit at which smoothing
begins is specified via the limit range parameter. In AC analysis, the value returned is
equal to the radian frequency of analysis multiplied by the gain.
Note that since truncation error checking is not included in the d_dt block, it is not re-
commended that the model be used to provide an integration function through the use
of a feedback loop. Such an arrangement could produce erroneous results. Instead, you
should make use of the "integrate" model, which does include truncation error checking
for enhanced accuracy.
Example SPICE Usage:
a12 7 12 slope_gen
.
.
.model slope_gen d_dt(out_offset=0.0 gain=1.0
+ out_lower_limit=1e-12 out_upper_limit=1e12
+ limit_range=1e-9)
12.2.15 Integrator
NAME_TABLE:
C_Function_Name: cm_int
Spice_Model_Name: int
Description: "time-integration block"
PORT_TABLE:
Port Name: in out
12.2. ANALOG MODELS 175
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset gain
Description: "input offset" "gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: out_lower_limit out_upper_limit
Description: "output lower limit" "output upper limit"
Data_Type: real real
Default_Value: - -
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: limit_range
Description: "upper & lower limit smoothing range"
Data_Type: real
Default_Value: 1.0e-6
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: out_ic
Description: "output initial condition"
Data_Type: real
Default_Value: 0.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The Integrator block is a simple integration stage that approximates the integral
with respect to time of an input signal. The block also includes gain and input offset
parameters to allow for tailoring of the required signal, and output upper and lower limits
to prevent convergence errors resulting from excessively large output values. Note that
176 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
these limits specify integrator behavior similar to that found in an operational amplifier-
based integration stage, in that once a limit is reached, additional storage does not occur.
Thus, the input of a negative value to an integrator that is currently driving at the out
upper limit level will immediately cause a drop in the output, regardless of how long
the integrator was previously summing positive inputs. The incremental value of output
below the output upper limit and above the output lower limit at which smoothing begins
is specified via the limit range parameter. In AC analysis, the value returned is equal to
the gain divided by the radian frequency of analysis.
Note that truncation error checking is included in the int block. This should provide
for a more accurate simulation of the time integration function, since the model will
inherently request smaller time increments between simulation points if truncation errors
would otherwise be excessive.
Example SPICE Usage:
a13 7 12 time_count
.
.
.model time_count int(in_offset=0.0 gain=1.0
+ out_lower_limit=-1e12 out_upper_limit=1e12
+ limit_range=1e-9 out_ic=0.0)
12.2.16 S-Domain Transfer Function
NAME_TABLE:
C_Function_Name: cm_s_xfer
Spice_Model_Name: s_xfer
Description: "s-domain transfer function"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset gain
Description: "input offset" "gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: num_coeff
Description: "numerator polynomial coefficients"
12.2. ANALOG MODELS 177
Data_Type: real
Default_Value: -
Limits: -
Vector: yes
Vector_Bounds: [1 -]
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: den_coeff
Description: "denominator polynomial coefficients"
Data_Type: real
Default_Value: -
Limits: -
Vector: yes
Vector_Bounds: [1 -]
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: int_ic
Description: "integrator stage initial conditions"
Data_Type: real
Default_Value: 0.0
Limits: -
Vector: yes
Vector_Bounds: den_coeff
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: denormalized_freq
Description: "denorm. corner freq.(radians) for 1 rad/s coeffs"
Data_Type: real
Default_Value: 1.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The s-domain transfer function is a single input, single output transfer function
in the Laplace transform variable ‘s’ that allows for flexible modulation of the frequency
domain characteristics of a signal. Ac and transient simulations are supported. The code
model may be configured to produce an arbitrary s-domain transfer function with the
following restrictions:
1. The degree of the numerator polynomial cannot exceed that
of the denominator polynomial in the variable "s".
2. The coefficients for a polynomial must be stated
explicitly. That is, if a coefficient is zero, it must be
included as an input to the num coeff or den coeff vector.
The order of the coefficient parameters is from that associated with the highest-powered term
decreasing to that of the lowest. Thus, for the coefficient parameters specified below, the equa-
tion in ‘s’ is shown:
178 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
.model filter s_xfer(gain=0.139713
+ num_coeff=[1.0 0.0 0.7464102]
+ den_coeff=[1.0 0.998942 0.001170077]
+ int_ic=[0 0])
...specifies a transfer function of the form...
N(s) = 0.139713 ·s2+0.7464102
s2+0.998942s+0.00117077
The s-domain transfer function includes gain and in_offset (input offset) parameters to allow
for tailoring of the required signal. There are no limits on the internal signal values or on
the output value of the s-domain transfer function, so you are cautioned to specify gain and
coefficient values that will not cause the model to produce excessively large values. In AC
analysis, the value returned is equal to the real and imaginary components of the total s-domain
transfer function at each frequency of interest.
The denormalized_freq term allows you to specify coefficients for a normalized filter (i.e. one
in which the frequency of interest is 1 rad/s). Once these coefficients are included, specifying
the denormalized frequency value ‘shifts’ the corner frequency to the actual one of interest. As
an example, the following transfer function describes a Chebyshev low-pass filter with a corner
(pass-band) frequency of 1 rad/s:
N(s) = 0.139713 ·1.0
s2+1.09773s+1.10251
In order to define an s_xfer model for the above, but with the corner frequency equal to 1500
rad/s (9425 Hz), the following instance and model lines would be needed:
a12 node1 node2 cheby1
.model cheby1 s_xfer(num_coeff=[1] den_coeff=[1 1.09773 1.10251]
+ int_ic=[0 0] denormalized_freq=1500)
In the above, you add the normalized coefficients and scale the filter through the use of the
denormalized freq parameter. Similar results could have been achieved by performing the de-
normalization prior to specification of the coefficients, and setting denormalized freq to the
value 1.0 (or not specifying the frequency, as the default is 1.0 rad/s) Note in the above that
frequencies are always specified as radians/second.
Truncation error checking is included in the s-domain transfer block. This should provide for
more accurate simulations, since the model will inherently request smaller time increments
between simulation points if truncation errors would otherwise be excessive.
The int_ic parameter is an array that must be of size one less as the array of values specified for
the den_coeff parameter. Even if a 0 start value is required, you have to add the specific int_ic
vector to the set of coefficients (see the examples above and below).
Example SPICE Usage:
a14 9 22 cheby_LP_3kHz
.
.
.model cheby_LP_3kHz s_xfer(in_offset=0.0 gain=1.0 int_ic=[0 0]
+ num_coeff=[1.0]
+ den_coeff=[1.0 1.42562 1.51620])
12.2. ANALOG MODELS 179
12.2.17 Slew Rate Block
NAME_TABLE:
C_Function_Name: cm_slew
Spice_Model_Name: slew
Description: "A simple slew rate follower block"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_slope
Description: "maximum rising slope value"
Data_Type: real
Default_Value: 1.0e9
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: fall_slope
Description: "maximum falling slope value"
Data_Type: real
Default_Value: 1.0e9
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: range
Description: "smoothing range"
Data_Type: real
Default_Value: 0.1
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: This function is a simple slew rate block that limits the absolute slope of the
output with respect to time to some maximum or value. The actual slew rate effects of
over-driving an amplifier circuit can thus be accurately modeled by cascading the ampli-
fier with this model. The units used to describe the maximum rising and falling slope
values are expressed in volts or amperes per second. Thus a desired slew rate of 0.5 V/µs
will be expressed as 0.5e+6, etc.
180 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
The slew rate block will continue to raise or lower its output until the difference between
the input and the output values is zero. Thereafter, it will resume following the input sig-
nal, unless the slope again exceeds its rise or fall slope limits. The range input specifies
a smoothing region above or below the input value. Whenever the model is slewing and
the output comes to within the input + or - the range value, the partial derivative of the
output with respect to the input will begin to smoothly transition from 0.0 to 1.0. When
the model is no longer slewing (output = input), dout/din will equal 1.0.
Example SPICE Usage:
a15 1 2 slew1
.model slew1 slew(rise_slope=0.5e6 fall_slope=0.5e6)
12.2.18 Inductive Coupling
NAME_TABLE:
C_Function_Name: cm_lcouple
Spice_Model_Name: lcouple
Description: "inductive coupling (for use with ’core’ model)"
PORT_TABLE:
Port_Name: l mmf_out
Description: "inductor" "mmf output (in ampere-turns)"
Direction: inout inout
Default_Type: hd hd
Allowed_Types: [h,hd] [hd]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: num_turns
Description: "number of inductor turns"
Data_Type: real
Default_Value: 1.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: This function is a conceptual model that is used as a building block to create a
wide variety of inductive and magnetic circuit models. This function is normally used in
conjunction with the core model, but can also be used with resistors, hysteresis blocks,
etc. to build up systems that mock the behavior of linear and nonlinear components.
The lcouple takes as an input (on the ‘l’ port), a current. This current value is multiplied
by the num_turns value, N, to produce an output value (a voltage value that appears on the
mmf_out port). The mmf_out acts similar to a magnetomotive force in a magnetic circuit;
when the lcouple is connected to the core model, or to some other resistive device, a
current will flow. This current value (which is modulated by whatever the lcouple is
connected to) is then used by the lcouple to calculate a voltage ‘seen’ at the lport. The
voltage is a function of the derivative with respect to time of the current value seen at
12.2. ANALOG MODELS 181
mmf_out.
The most common use for lcouples will be as a building block in the construction of
transformer models. To create a transformer with a single input and a single output, you
would require two lcouple models plus one core model. The process of building up
such a transformer is described under the description of the core model, below.
Example SPICE Usage:
a150 (7 0) (9 10) lcouple1
.model lcouple1 lcouple(num_turns=10.0)
12.2.19 Magnetic Core
NAME_TABLE:
C_Function_Name: cm_core
Spice_Model_Name: core
Description: "magnetic core"
PORT_TABLE:
Port_Name: mc
Description: "magnetic core"
Direction: inout
Default_Type: gd
Allowed_Types: [g,gd]
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: H_array B_array
Description: "magnetic field array" "flux density array"
Data_Type: real real
Default_Value: - -
Limits: - -
Vector: yes yes
Vector_Bounds: [2 -] [2 -]
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: area length
Description: "cross-sectional area" "core length"
Data_Type: real real
Default_Value: - -
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: input_domain
Description: "input sm. domain"
Data_Type: real
Default_Value: 0.01
182 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Limits: [1e-12 0.5]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: fraction
Description: "smoothing fraction/abs switch"
Data_Type: boolean
Default_Value: TRUE
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: mode
Description: "mode switch (1 = pwl, 2 = hyst)"
Data_Type: int
Default_Value: 1
Limits: [1 2]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: in_low in_high
Description: "input low value" "input high value"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: hyst out_lower_limit
Description: "hysteresis" "output lower limit"
Data_Type: real real
Default_Value: 0.1 0.0
Limits: [0 -] -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: out_upper_limit
Description: "output upper limit"
Data_Type: real
Default_Value: 1.0
Limits: -
Vector: no
Vector_Bounds: -
12.2. ANALOG MODELS 183
Null_Allowed: yes
Description: This function is a conceptual model that is used as a building block to create
a wide variety of inductive and magnetic circuit models. This function is almost always
expected to be used in conjunction with the lcouple model to build up systems that mock
the behavior of linear and nonlinear magnetic components. There are two fundamental
modes of operation for the core model. These are the pwl mode (which is the default, and
which is the most likely to be of use to you) and the hysteresis mode. These are detailed
below.
PWL Mode (mode = 1)
The core model in PWL mode takes as input a voltage that it treats as a magnetomotive force
(mmf) value. This value is divided by the total effective length of the core to produce a value
for the Magnetic Field Intensity, H. This value of H is then used to find the corresponding Flux
Density, B, using the piecewise linear relationship described by you in the H array / B array
coordinate pairs. B is then multiplied by the cross-sectional area of the core to find the Flux
value, which is output as a current. The pertinent mathematical equations are listed below:
H = mmf =L, where L = Length
Here H, the Magnetic Field Intensity, is expressed in ampere-turns/meter.
B = f (H)
The B value is derived from a piecewise linear transfer function described to the model via
the (H_array[],B_array[]) parameter coordinate pairs. This transfer function does not include
hysteretic effects; for that, you would need to substitute a HYST model for the core.
φ= BA, where A = Area
The final current allowed to flow through the core is equal to φ. This value in turn is used by
the "lcouple" code model to obtain a value for the voltage reflected back across its terminals to
the driving electrical circuit.
The following example code shows the use of two lcouple models and one core model to
produce a simple primary/secondary transformer.
Example SPICE Usage:
a1 (2 0) (3 0) primary
.model primary lcouple (num_turns = 155)
a2 (3 4) iron_core
.model iron_core core (H_array = [-1000 -500 -375 -250 -188 -125 -63 0
+ 63 125 188 250 375 500 1000]
+ B_array = [-3.13e-3 -2.63e-3 -2.33e-3 -1.93e-3
+ -1.5e-3 -6.25e-4 -2.5e-4 0 2.5e-4
+ 6.25e-4 1.5e-3 1.93e-3 2.33e-3
+ 2.63e-3 3.13e-3]
+ area = 0.01 length = 0.01)
a3 (5 0) (4 0) secondary
.model secondary lcouple (num_turns = 310)
184 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
HYSTERESIS Mode (mode = 2)
The core model in HYSTERESIS mode takes as input a voltage that it treats as a magnetomotive
force (mmf) value. This value is used as input to the equivalent of a hysteresis code model block.
The parameters defining the input low and high values, the output low and high values, and the
amount of hysteresis are as in that model. The output from this mode, as in PWL mode, is a
current value that is seen across the mc port. An example of the core model used in this fashion
is shown below:
Example SPICE Usage:
a1 (2 0) (3 0) primary
.model primary lcouple (num_turns = 155)
a2 (3 4) iron_core
.model iron_core core (mode = 2 in_low=-7.0 in_high=7.0
+ out_lower_limit=-2.5e-4 out_upper_limit=2.5e-4
+ hyst = 2.3 )
a3 (5 0) (4 0) secondary
.model secondary lcouple (num_turns = 310)
One final note to be made about the two core model nodes is that certain parameters are avai-
lable in one mode, but not in the other. In particular, the in_low, in_high, out_lower_limit,
out_upper_limit, and hysteresis parameters are not available in PWL mode. Likewise, the
H_array, B_array, area, and length values are unavailable in HYSTERESIS mode. The input
domain and fraction parameters are common to both modes (though their behavior is somewhat
different; for explanation of the input domain and fraction values for the HYSTERESIS mode,
you should refer to the hysteresis code model discussion).
12.2.20 Controlled Sine Wave Oscillator
NAME_TABLE:
C_Function_Name: cm_sine
Spice_Model_Name: sine
Description: "controlled sine wave oscillator"
PORT_TABLE:
Port Name: cntl_in out
Description: "control input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: cntl_array freq_array
Description: "control array" "frequency array"
Data_Type: real real
Default_Value: 0.0 1.0e3
12.2. ANALOG MODELS 185
Limits: - [0 -]
Vector: yes yes
Vector_Bounds: [2 -] cntl_array
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: out_low out_high
Description: "output peak low value" "output peak high value"
Data_Type: real real
Default_Value: -1.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: This function is a controlled sine wave oscillator with parametrizable values of
low and high peak output. It takes an input voltage or current value. This value is used as
the independent variable in the piecewise linear curve described by the coordinate points
of the cntl array and freq array pairs. From the curve, a frequency value is determined,
and the oscillator will output a sine wave at that frequency. From the above, it is easy
to see that array sizes of 2 for both the cntl array and the freq array will yield a linear
variation of the frequency with respect to the control input. Any sizes greater than 2 will
yield a piecewise linear transfer characteristic. For more detail, refer to the description of
the piecewise linear controlled source, which uses a similar method to derive an output
value given a control input.
Example SPICE Usage:
asine 1 2 in_sine
.model in_sine sine(cntl_array = [-1 0 5 6]
+ freq_array=[10 10 1000 1000] out_low = -5.0
+ out_high = 5.0)
12.2.21 Controlled Triangle Wave Oscillator
NAME_TABLE:
C_Function_Name: cm_triangle
Spice_Model_Name: triangle
Description: "controlled triangle wave oscillator"
PORT_TABLE:
Port Name: cntl_in out
Description: "control input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: cntl_array freq_array
186 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Description: "control array" "frequency array"
Data_Type: real real
Default_Value: 0.0 1.0e3
Limits: - [0 -]
Vector: yes yes
Vector_Bounds: [2 -] cntl_array
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: out_low out_high
Description: "output peak low value" "output peak high value"
Data_Type: real real
Default_Value: -1.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: duty_cycle
Description: "rise time duty cycle"
Data_Type: real
Default_Value: 0.5
Limits: [1e-10 0.999999999]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: This function is a controlled triangle/ramp wave oscillator with parametrizable
values of low and high peak output and rise time duty cycle. It takes an input voltage or
current value. This value is used as the independent variable in the piecewise linear curve
described by the coordinate points of the cntl_array and freq_array pairs.
From the curve, a frequency value is determined, and the oscillator will output a triangle
wave at that frequency. From the above, it is easy to see that array sizes of 2 for both the
cntl_array and the freq_array will yield a linear variation of the frequency with respect to
the control input. Any sizes greater than 2 will yield a piecewise linear transfer characte-
ristic. For more detail, refer to the description of the piecewise linear controlled source,
which uses a similar method to derive an output value given a control input.
Example SPICE Usage:
ain 1 2 ramp1
.model ramp1 triangle(cntl_array = [-1 0 5 6]
+ freq_array=[10 10 1000 1000] out_low = -5.0
+ out_high = 5.0 duty_cycle = 0.9)
12.2.22 Controlled Square Wave Oscillator
NAME_TABLE:
C_Function_Name: cm_square
Spice_Model_Name: square
12.2. ANALOG MODELS 187
Description: "controlled square wave oscillator"
PORT_TABLE:
Port Name: cntl_in out
Description: "control input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: cntl_array freq_array
Description: "control array" "frequency array"
Data_Type: real real
Default_Value: 0.0 1.0e3
Limits: - [0 -]
Vector: yes yes
Vector_Bounds: [2 -] cntl_array
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: out_low out_high
Description: "output peak low value" "output peak high value"
Data_Type: real real
Default_Value: -1.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER.TABLE:
Parameter_Name: duty_cycle rise_time
Description: "duty cycle" "output rise time"
Data_Type: real real
Default_Value: 0.5 1.0e-9
Limits: [1e-6 0.999999] -
Vector: no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: fall_time
Description: "output fall time"
Data_Type: real
Default_Value: 1.0e-9
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: This function is a controlled square wave oscillator with parametrizable values
of low and high peak output, duty cycle, rise time, and fall time. It takes an input voltage
188 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
or current value. This value is used as the independent variable in the piecewise linear
curve described by the coordinate points of the cntl_array and freq_array pairs. From the
curve, a frequency value is determined, and the oscillator will output a square wave at
that frequency.
From the above, it is easy to see that array sizes of 2 for both the cntl_array and the
freq_array will yield a linear variation of the frequency with respect to the control input.
Any sizes greater than 2 will yield a piecewise linear transfer characteristic. For more
detail, refer to the description of the piecewise linear controlled source, which uses a
similar method to derive an output value given a control input.
Example SPICE Usage:
ain 1 2 pulse1
.model pulse1 square(cntl_array = [-1 0 5 6]
+ freq_array=[10 10 1000 1000] out_low = 0.0
+ out_high = 4.5 duty_cycle = 0.2
+ rise_time = 1e-6 fall_time = 2e-6)
12.2.23 Controlled One-Shot
NAME_TABLE:
C_Function_Name: cm_oneshot
Spice_Model_Name: oneshot
Description: "controlled one-shot"
PORT_TABLE:
Port Name: clk cntl_in
Description: "clock input" "control input"
Direction: in in
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no yes
PORT_TABLE:
Port Name: clear out
Description: "clear signal" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes no
PARAMETER_TABLE:
Parameter_Name: clk_trig retrig
Description: "clock trigger value" "retrigger switch"
Data_Type: real boolean
Default_Value: 0.5 FALSE
Limits: - -
Vector: no no
12.2. ANALOG MODELS 189
Vector_Bounds: - -
Null_Allowed: no yes
PARAMETER_TABLE:
Parameter_Name: pos_edge_trig
Description: "positive/negative edge trigger switch"
Data_Type: boolean
Default_Value: TRUE
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: cntl_array pw_array
Description: "control array" "pulse width array"
Data_Type: real real
Default_Value: 0.0 1.0e-6
Limits: - [0.00 -]
Vector: yes yes
Vector_Bounds: - cntl_array
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: out_low out_high
Description: "output low value" "output high value"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: fall_time rise_time
Description: "output fall time" "output rise time"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: rise_delay
Description: "output delay from trigger"
Data_Type: real
Default_Value: 1.0e-9
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
190 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Parameter_Name: fall_delay
Description: "output delay from pw"
Data_Type: real
Default_Value: 1.0e-9
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: This function is a controlled oneshot with parametrizable values of low and high
peak output, input trigger value level, delay, and output rise and fall times. It takes an
input voltage or current value. This value is used as the independent variable in the
piecewise linear curve described by the coordinate points of the cntl_array and pw_array
pairs. From the curve, a pulse width value is determined. The one-shot will output a
pulse of that width, triggered by the clock signal (rising or falling edge), delayed by the
delay value, and with specified rise and fall times. A positive slope on the clear input will
immediately terminate the pulse, which resets with its fall time.
From the above, it is easy to see that array sizes of 2 for both the cntl_array and the
pw_array will yield a linear variation of the pulse width with respect to the control input.
Any sizes greater than 2 will yield a piecewise linear transfer characteristic. For more
detail, refer to the description of the piecewise linear controlled source, which uses a
similar method to derive an output value given a control input.
Example SPICE Usage:
ain 1 2 3 4 pulse2
.model pulse2 oneshot(cntl_array = [-1 0 10 11]
+ pw_array=[1e-6 1e-6 1e-4 1e-4]
+ clk_trig = 0.9 pos_edge_trig = FALSE
+ out_low = 0.0 out_high = 4.5
+ rise_delay = 20.0-9 fall_delay = 35.0e-9)
12.2.24 Capacitance Meter
NAME_TABLE:
C_Function_Name: cm_cmeter
Spice_Model_Name: cmeter
Description: "capacitance meter"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: gain
12.2. ANALOG MODELS 191
Description: "gain"
Data_Type: real
Default_Value: 1.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The capacitance meter is a sensing device that is attached to a circuit node and
produces as an output a scaled value equal to the total capacitance seen on its input mul-
tiplied by the gain parameter. This model is primarily intended as a building block for
other models that must sense a capacitance value and alter their behavior based upon it.
Example SPICE Usage:
atest1 1 2 ctest
.model ctest cmeter(gain=1.0e12)
12.2.25 Inductance Meter
NAME_TABLE:
C_Function_Name: cm_lmeter
Spice_Model_Name: lmeter
Description: "inductance meter"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: gain
Description: "gain"
Data_Type: real
Default_Value: 1.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The inductance meter is a sensing device that is attached to a circuit node and
produces as an output a scaled value equal to the total inductance seen on its input mul-
tiplied by the gain parameter. This model is primarily intended as a building block for
other models that must sense an inductance value and alter their behavior based upon it.
192 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Example SPICE Usage:
atest2 1 2 ltest
.model ltest lmeter(gain=1.0e6)
12.2.26 Memristor
NAME_TABLE:
C_Function_Name: cm_memristor
Spice_Model_Name: memristor
Description: "Memristor Interface"
PORT_TABLE:
Port_Name: memris
Description: "memristor terminals"
Direction: inout
Default_Type: gd
Allowed_Types: [gd]
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: rmin rmax
Description: "minimum resistance" "maximum resistance"
Data_Type: real real
Default_Value: 10.0 10000.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rinit vt
Description: "initial resistance" "threshold"
Data_Type: real real
Default_Value: 7000.0 0.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: alpha beta
Description: "model parameter 1" "model parameter 2"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
Description: The memristor is a two-terminal resistor with memory, whose resistance depends
12.2. ANALOG MODELS 193
on the time integral of the voltage across its terminals. rmin and rmax provide the lower
and upper limits of the resistance, rinit is its starting value (no voltage applied so far).
The voltage has to be above a threshold vt to become effective in changing the resistance.
alpha and beta are two model parameters. The memristor code model is derived from a
SPICE subcircuit published in [23].
Example SPICE Usage:
amen 1 2 memr
.model memr memristor (rmin=1k rmax=10k rinit=7k
+ alpha=0 beta=2e13 vt=1.6)
12.2.27 2D table model
NAME_TABLE:
C_Function_Name: cm_table2D
Spice_Model_Name: table2D
Description: "2D table model"
PORT_TABLE:
Port_Name: inx iny out
Description: "inputx" "inputy" "output"
Direction: in in out
Default_Type: v v i
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id,vnam] [v,vd,i,id]
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: no no no
PARAMETER_TABLE:
Parameter_Name: order verbose
Description: "order" "verbose"
Data_Type: int int
Default_Value: 3 0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: offset gain
Description: "offset" "gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: file
Description: "file name"
Data_Type: string
194 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Default_Value: "2D-table-model.txt"
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The 2D table model reads a matrix from file "file name" (default 2D-table-
model.txt) which has x columns and y rows. Each x,y pair, addressed by inx and iny,
yields an output value out. Linear interpolation is used for out, eno (essentially non
oscillating) interpolation for its derivatives. Parameters offset (default 0) and gain (de-
fault 1) modify the output table values according to o f f set +gain out. Parameter order
(default 3) influences the calculation of the derivatives. Parameter verbose (default 0)
yields test outputs, if set to 1 or 2. The table format is shown below. Be careful to include
the data point inx = 0, iny = 0 into your table, because ngspice uses these during .OP
computations. The x horizontal and y vertical address values have to increase monoto-
nically. The usage example consists of two input voltages referenced to ground and a
current source output with two floating nodes.
Table Example:
* table source
* number of columns (x)
8
* number of rows (y)
9
* x horizontal (column) address values (real numbers)
-10123456
* y vertical (row) address values (real numbers)
-0.6 0 0.6 1.2 1.8 2.4 3.0 3.6 4.2
* table with output data (horizontally addressed by x, vertically by y)
1 0.9 0.8 0.7 0.6 0.5 0.4 0.3
11111111
1 1.2 1.4 1.6 1.8 2 2.2 2.4
1 1.5 2 2.5 3 3.5 4 4.5
12345678
1 2.5 4 5.5 7 8.5 10 11.5
13579111315
1 3.5 6 8.5 11 13.5 16 18.5
1471013161922
Example SPICE Usage:
atab inx iny %id(out1 out2) tabmod
.model tabmod table2d (offset=0.0 gain=1 order=3 file="table-simple.txt")
12.2.28 3D table model
NAME_TABLE:
C_Function_Name: cm_table3D
Spice_Model_Name: table3D
Description: "3D table model"
12.2. ANALOG MODELS 195
PORT_TABLE:
Port_Name: inx iny inz
Description: "inputx" "inputy" "inputz"
Direction: in in in
Default_Type: v v v
Allowed_Types: [v,vd,i,id,vnam] [v,vd,i,id,vnam] [v,vd,i,id,vnam]
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: no no no
PORT_TABLE:
Port_Name: out
Description: "output"
Direction: out
Default_Type: i
Allowed_Types: [v,vd,i,id]
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: order verbose
Description: "order" "verbose"
Data_Type: int int
Default_Value: 3 0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: offset gain
Description: "offset" "gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: file
Description: "file name"
Data_Type: string
Default_Value: "3D-table-model.txt"
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The 3D table model reads a matrix from file "file name" (default 3D-table-
model.txt) which has x columns, y rows per table and z tables. Each x,y,z triple, ad-
dressed by inx, iny, and inz, yields an output value out. Linear interpolation is used
196 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
for out, eno (essentially non oscillating) interpolation for its derivatives. Parameters
offset (default 0) and gain (default 1) modify the output table values according to
o f f set +gain out. Parameter order (default 3) influences the calculation of the deri-
vatives. Parameter verbose (default 0) yields test outputs, if set to 1 or 2. The table
format is shown below. Be careful to include the data point inx = 0, iny = 0, inz = 0 into
your table, because ngspice needs these to for the .OP calculation. The x horizontal, y
vertical, and z table address values have to increase monotonically. The usage example
simulates a NMOS transistor with independent drain, gate and bulk nodes, referenced to
source. Parameter gain may be used to emulate transistor width, with respect to the table
transistor.
Table Example:
* 3D table for nmos bsim 4, W=10um, L=0.13um
*x
39
*y
39
*z
11
*x (drain voltage)
-0.1 -0.05 0 0.05 0.1 0.15 0.2 0.25 ...
*y (gate voltage)
-0.1 -0.05 0 0.05 0.1 0.15 0.2 0.25 ...
*z (substrate voltage)
-1.8 -1.6 -1.4 -1.2 -1 -0.8 -0.6 -0.4 -0.2 0 0.2
*table -1.8
-4.50688E-10 -4.50613E-10 -4.50601E-10 -4.50599E-10 ...
-4.49622E-10 -4.49267E-10 -4.4921E-10 -4.49202E-10 ...
-4.50672E-10 -4.49099E-10 -4.48838E-10 -4.48795E-10 ...
-4.55575E-10 -4.4953E-10 -4.48435E-10 -4.48217E-10 ...
...
*table -1.6
-3.10015E-10 -3.09767E-10 -3.0973E-10 -3.09724E-10 ...
-3.09748E-10 -3.08524E-10 -3.08339E-10 -3.08312E-10 ...
...
*table -1.4
-2.04848E-10 -2.04008E-10 -2.03882E-10 ...
-2.07275E-10 -2.03117E-10 -2.02491E-10 ...
...
Example SPICE Usage:
amos1 %vd(d s) %vd(g s) %vd(b s) %id(d s) mostable1
.model mostable1 table3d (offset=0.0 gain=0.5 order=3
+ verbose=1 file="table-3D-bsim4n.txt")
12.3. HYBRID MODELS 197
12.3 Hybrid Models
The following hybrid models are supplied with XSPICE. The descriptions included below con-
sist of the model Interface Specification File and a description of the model’s operation. This
is followed by an example of a simulator-deck placement of the model, including the .MODEL
card and the specification of all available parameters.
A note should be made with respect to the use of hybrid models for other than simple digital-to-
analog and analog-to-digital translations. The hybrid models represented in this section address
that specific need, but in the development of user-defined nodes you may find a need to translate
not only between digital and analog nodes, but also between real and digital, real and int, etc.
In most cases such translations will not need to be as involved or as detailed as shown in the
following.
12.3.1 Digital-to-Analog Node Bridge
NAME_TABLE:
C_Function_Name: cm_dac_bridge
Spice_Model_Name: dac_bridge
Description: "digital-to-analog node bridge"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: d v
Allowed_Types: [d] [v,vd,i,id,d]
Vector: yes yes
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: out_low
Description: "0-valued analog output"
Data_Type: real
Default_Value: 0.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: out_high
Description: "1-valued analog output"
Data_Type: real
Default_Value: 1.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
198 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Parameter_Name: out_undef input_load
Description: "U-valued analog output" "input load (F)"
Data_Type: real real
Default_Value: 0.5 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: t_rise t_fall
Description: "rise time 0->1" "fall time 1->0"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The dac_bridge is the first of two node bridge devices designed to allow for
the ready transfer of digital information to analog values and back again. The second
device is the adc_bridge (which takes an analog value and maps it to a digital one).The
dac_bridge takes as input a digital value from a digital node. This value by definition
may take on only one of the values ‘0’, ‘1’ or ‘U’. The dac_bridge then outputs the value
out_low,out_high or out_undef, or ramps linearly toward one of these ‘final’ values
from its current analog output level. The speed at which this ramping occurs depends
on the values of t_rise and t_fall. These parameters are interpreted by the model
such that the rise or fall slope generated is always constant. Note that the dac_bridge
includes test code in its cfunc.mod file for determining the presence of the out_undef para-
meter. If this parameter is not specified by you, and if out_high and out_low values are
specified, then out_undef is assigned the value of the arithmetic mean of out_high and
out_low.This simplifies coding of output buffers, where typically a logic family will
include an out_low and out_high voltage, but not an out_undef value. This model
also posts an input load value (in farads) based on the parameter input load.
Example SPICE Usage:
abridge1 [7] [2] dac1
.model dac1 dac_bridge(out_low = 0.7 out_high = 3.5 out_undef = 2.2
+ input_load = 5.0e-12 t_rise = 50e-9
+ t_fall = 20e-9)
12.3.2 Analog-to-Digital Node Bridge
NAME_TABLE:
C_Function_Name: cm_adc_bridge
Spice_Model_Name: adc_bridge
Description: "analog-to-digital node bridge"
PORT_TABLE:
Port Name: in out
12.3. HYBRID MODELS 199
Description: "input" "output"
Direction: in out
Default_Type: v d
Allowed_Types: [v,vd,i,id,d] [d]
Vector: yes yes
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_low
Description: "maximum 0-valued analog input"
Data_Type: real
Default_Value: 1.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: in_high
Description: "minimum 1-valued analog input"
Data_Type: real
Default_Value: 2.0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The adc_bridge is one of two node bridge devices designed to allow for the
ready transfer of analog information to digital values and back again. The second device
is the dac_bridge (which takes a digital value and maps it to an analog one). The
adc_bridge takes as input an analog value from an analog node. This value by definition
may be in the form of a voltage, or a current. If the input value is less than or equal to
in_low, then a digital output value of ‘0’ is generated. If the input is greater than or equal
to in_high, a digital output value of ‘1’ is generated. If neither of these is true, then
a digital ‘UNKNOWN’ value is output. Note that unlike the case of the dac_bridge,
no ramping time or delay is associated with the adc_bridge. Rather, the continuous
ramping of the input value provides for any associated delays in the digitized signal.
Example SPICE Usage:
abridge2 [1] [8] adc_buff
.model adc_buff adc_bridge(in_low = 0.3 in_high = 3.5)
200 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
12.3.3 Controlled Digital Oscillator
NAME_TABLE:
C_Function_Name: cm_d_osc
Spice_Model_Name: d_osc
Description: "controlled digital oscillator"
PORT_TABLE:
Port Name: cntl_in out
Description: "control input" "output"
Direction: in out
Default_Type: v d
Allowed_Types: [v,vd,i,id] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: cntl_array freq_array
Description: "control array" "frequency array"
Data_Type: real real
Default_Value: 0.0 1.0e6
Limits: - [0 -]
Vector: yes yes
Vector_Bounds: [2 -] cntl_array
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: duty_cycle init_phase
Description: "duty cycle" "initial phase of output"
Data_Type: real real
Default_Value: 0.5 0
Limits: [1e-6 0.999999] [-180.0 +360.0]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1e-9 1e-9
Limits: [0 -] [0 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The digital oscillator is a hybrid model that accepts as input a voltage or current.
This input is compared to the voltage-to-frequency transfer characteristic specified by the
cntl_array/freq_array coordinate pairs, and a frequency is obtained that represents
a linear interpolation or extrapolation based on those pairs. A digital time-varying signal
is then produced with this fundamental frequency.
The output waveform, which is the equivalent of a digital clock signal, has rise and fall
12.3. HYBRID MODELS 201
delays that can be specified independently. In addition, the duty cycle and the phase of
the waveform are also variable and can be set by you.
Example SPICE Usage:
a5 1 8 var_clock
.model var_clock d_osc(cntl_array = [-2 -1 1 2]
+ freq_array = [1e3 1e3 10e3 10e3]
+ duty_cycle = 0.4 init_phase = 180.0
+ rise_delay = 10e-9 fall_delay=8e-9)
12.3.4 Node bridge from digital to real with enable
NAME_TABLE:
Spice_Model_Name: d_to_real
C_Function_Name: ucm_d_to_real
Description: "Node bridge from digital to real with enable"
PORT_TABLE:
Port_Name: in enable out
Description: "input" "enable" "output"
Direction: in in out
Default_Type: d d real
Allowed_Types: [d] [d] [real]
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: no yes no
PARAMETER_TABLE:
Parameter_Name: zero one delay
Description: "value for 0" "value for 1" "delay"
Data_Type: real real real
Default_Value: 0.0 1.0 1e-9
Limits: - - [1e-15 -]
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: yes yes yes
12.3.5 A Z**-1 block working on real data
NAME_TABLE:
Spice_Model_Name: real_delay
C_Function_Name: ucm_real_delay
Description: "A Z ** -1 block working on real data"
PORT_TABLE:
Port_Name: in clk out
Description: "input" "clock" "output"
Direction: in in out
Default_Type: real d real
Allowed_Types: [real] [d] [real]
202 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: no no no
PARAMETER_TABLE:
Parameter_Name: delay
Description: "delay from clk to out"
Data_Type: real
Default_Value: 1e-9
Limits: [1e-15 -]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
12.3.6 A gain block for event-driven real data
NAME_TABLE:
Spice_Model_Name: real_gain
C_Function_Name: ucm_real_gain
Description: "A gain block for event-driven real data"
PORT_TABLE:
Port_Name: in out
Description: "input" "output"
Direction: in out
Default_Type: real real
Allowed_Types: [real] [real]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset gain out_offset
Description: "input offset" "gain" "output offset"
Data_Type: real real real
Default_Value: 0.0 1.0 0.0
Limits: - - -
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: yes yes yes
PARAMETER_TABLE:
Parameter_Name: delay ic
Description: "delay" "initial condition"
Data_Type: real real
Default_Value: 1.0e-9 0.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
12.4. DIGITAL MODELS 203
12.3.7 Node bridge from real to analog voltage
NAME_TABLE:
Spice_Model_Name: real_to_v
C_Function_Name: ucm_real_to_v
Description: "Node bridge from real to analog voltage"
PORT_TABLE:
Port_Name: in out
Description: "input" "output"
Direction: in out
Default_Type: real v
Allowed_Types: [real] [v, vd, i, id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: gain transition_time
Description: "gain" "output transition time"
Data_Type: real real
Default_Value: 1.0 1e-9
Limits: - [1e-15 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
12.4 Digital Models
The following digital models are supplied with XSPICE. The descriptions included below con-
sist of an example model Interface Specification File and a description of the model’s opera-
tion. This is followed by an example of a simulator-deck placement of the model, including the
.MODEL card and the specification of all available parameters. Note that these models have not
been finalized at this time.
Some information common to all digital models and/or digital nodes is included here. The fol-
lowing are general rules that should make working with digital nodes and models more straig-
htforward:
1. All digital nodes are initialized to ZERO at the start of a simulation (i.e., when INIT=TRUE).
This means that a model need not post an explicit value to an output node upon initia-
lization if its output would normally be a ZERO (although posting such would certainly
cause no harm).
12.4.1 Buffer
NAME_TABLE:
C_Function_Name: cm_d_buffer
Spice_Model_Name: d_buffer
Description: "digital one-bit-wide buffer"
204 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The buffer is a single-input, single-output digital buffer that produces as output
a time-delayed copy of its input. The delays associated with an output rise and those
associated with an output fall may be different. The model also posts an input load value
(in farads) based on the parameter input load. The output of this model does not, however,
respond to the total loading it sees on its output; it will always drive the output strongly
with the specified delays.
Example SPICE Usage:
a6 1 8 buff1
.model buff1 d_buffer(rise_delay = 0.5e-9 fall_delay = 0.3e-9
+ input_load = 0.5e-12)
12.4.2 Inverter
NAME_TABLE:
C_Function_Name: cm_d_inverter
Spice_Model_Name: d_inverter
Description: "digital one-bit-wide inverter"
PORT_TABLE:
Port Name: in out
12.4. DIGITAL MODELS 205
Description: "input" "output"
Direction: in out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The inverter is a single-input, single-output digital inverter that produces as out-
put an inverted, time-delayed copy of its input. The delays associated with an output rise
and those associated with an output fall may be specified independently. The model also
posts an input load value (in farads) based on the parameter input load. The output of this
model does not, however, respond to the total loading it sees on its output; it will always
drive the output strongly with the specified delays.
Example SPICE Usage:
a6 1 8 inv1
.model inv1 d_inverter(rise_delay = 0.5e-9 fall_delay = 0.3e-9
+ input_load = 0.5e-12)
12.4.3 And
NAME_TABLE:
C_Function_Name: cm_d_and
Spice_Model_Name: d_and
Description: "digital ‘and’ gate"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
206 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [2 -] -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital and gate is an n-input, single-output and gate that produces an active
‘1’ value if, and only if, all of its inputs are also ‘1’ values. If ANY of the inputs is a
‘0’, the output will also be a ‘0’; if neither of these conditions holds, the output will be
unknown. The delays associated with an output rise and those associated with an output
fall may be specified independently. The model also posts an input load value (in farads)
based on the parameter input load. The output of this model does not, however, respond
to the total loading it sees on its output; it will always drive the output strongly with the
specified delays.
Example SPICE Usage:
a6 [1 2] 8 and1
.model and1 d_and(rise_delay = 0.5e-9 fall_delay = 0.3e-9
+ input_load = 0.5e-12)
12.4.4 Nand
NAME_TABLE:
C_Function_Name: cm_d_nand
Spice_Model_Name: d_nand
Description: "digital ‘nand’ gate"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
12.4. DIGITAL MODELS 207
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [2 -] -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital nand gate is an n-input, single-output nand gate that produces an
active ‘0’ value if and only if all of its inputs are ‘1’ values. If ANY of the inputs is a ‘0’,
the output will be a ‘1’; if neither of these conditions holds, the output will be unknown.
The delays associated with an output rise and those associated with an output fall may be
specified independently. The model also posts an input load value (in farads) based on
the parameter input load. The output of this model does not, however, respond to the total
loading it sees on its output; it will always drive the output strongly with the specified
delays.
Example SPICE Usage:
a6 [1 2 3] 8 nand1
.model nand1 d_nand(rise_delay = 0.5e-9 fall_delay = 0.3e-9
+ input_load = 0.5e-12)
12.4.5 Or
NAME_TABLE:
C_Function_Name: cm_d_or
Spice_Model_Name: d_or
Description: "digital ‘or’ gate"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
208 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [2 -] -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital or gate is an n-input, single-output or gate that produces an active
‘1’ value if at least one of its inputs is a ‘1’ value. The gate produces a ‘0’ value if
all inputs are ‘0’; if neither of these two conditions holds, the output is unknown. The
delays associated with an output rise and those associated with an output fall may be
specified independently. The model also posts an input load value (in farads) based on
the parameter input load. The output of this model does not, however, respond to the total
loading it sees on its output; it will always drive the output strongly with the specified
delays.
Example SPICE Usage:
a6 [1 2 3] 8 or1
.model or1 d_or(rise_delay = 0.5e-9 fall_delay = 0.3e-9
+ input_load = 0.5e-12)
12.4.6 Nor
NAME_TABLE:
C_Function_Name: cm_d_nor
Spice_Model_Name: d_nor
Description: "digital ‘nor’ gate"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
12.4. DIGITAL MODELS 209
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [2 -] -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital nor gate is an n-input, single-output nor gate that produces an active
‘0’ value if at least one of its inputs is a ‘1’ value. The gate produces a ‘0’ value if
all inputs are ‘0’; if neither of these two conditions holds, the output is unknown. The
delays associated with an output rise and those associated with an output fall may be
specified independently. The model also posts an input load value (in farads) based on
the parameter input load. The output of this model does not, however, respond to the total
loading it sees on its output; it will always drive the output strongly with the specified
delays.
Example SPICE Usage:
anor12 [1 2 3 4] 8 nor12
.model nor12 d_or(rise_delay = 0.5e-9 fall_delay = 0.3e-9
+ input_load = 0.5e-12)
12.4.7 Xor
NAME_TABLE:
C_Function_Name: cm_d_xor
Spice_Model_Name: d_xor
Description: "digital exclusive-or gate"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
210 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [2 -] -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital xor gate is an n-input, single-output xor gate that produces an active
‘1’ value if an odd number of its inputs are also ‘1’ values. The delays associated with an
output rise and those associated with an output fall may be specified independently.
The model also posts an input load value (in farads) based on the parameter input load.
The output of this model does not, however, respond to the total loading it sees on its
output; it will always drive the output strongly with the specified delays. Note also that
to maintain the technology-independence of the model, any UNKNOWN input, or any
floating input causes the output to also go UNKNOWN.
Example SPICE Usage:
a9 [1 2] 8 xor3
.model xor3 d_xor(rise_delay = 0.5e-9 fall_delay = 0.3e-9
+ input_load = 0.5e-12)
12.4.8 Xnor
NAME_TABLE:
C_Function_Name: cm_d_xnor
Spice_Model_Name: d_xnor
Description: "digital exclusive-nor gate"
PORT_TABLE:
Port Name: in out
Description: "input" "output"
Direction: in out
12.4. DIGITAL MODELS 211
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [2 -] -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital xnor gate is an n-input, single-output xnor gate that produces an
active ‘0’ value if an odd number of its inputs are also ‘1’ values. It produces a ‘1’ output
when an even number of ‘1’ values occurs on its inputs. The delays associated with an
output rise and those associated with an output fall may be specified independently. The
model also posts an input load value (in farads) based on the parameter input load. The
output of this model does not, however, respond to the total loading it sees on its output; it
will always drive the output strongly with the specified delays. Note also that to maintain
the technology-independence of the model, any UNKNOWN input, or any floating input
causes the output to also go UNKNOWN.
Example SPICE Usage:
a9 [1 2] 8 xnor3
.model xnor3 d_xnor(rise_delay = 0.5e-9 fall_delay = 0.3e-9
+ input_load = 0.5e-12)
12.4.9 Tristate
NAME_TABLE:
C_Function_Name: cm_d_tristate
Spice_Model_Name: d_tristate
Description: "digital tristate buffer"
PORT_TABLE:
Port Name: in enable out
Description: "input" "enable" "output"
212 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Direction: in in out
Default_Type: d d d
Allowed_Types: [d] [d] [d]
Vector: no no no
Vector_Bounds: - - -
Null_Allowed: no no no
PARAMETER_TABLE:
Parameter_Name: delay
Description: "delay"
Data_Type: real
Default_Value: 1.0e-9
Limits: [1.0e-12 -]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: enable_load
Description: "enable load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital tristate is a simple tristate gate that can be configured to allow for
open-collector behavior, as well as standard tristate behavior. The state seen on the input
line is reflected in the output. The state seen on the enable line determines the strength of
the output. Thus, a ONE forces the output to its state with a STRONG strength. A ZERO
forces the output to go to a HI_IMPEDANCE strength. The delays associated with an
output state or strength change cannot be specified independently, nor may they be spe-
cified independently for rise or fall conditions; other gate models may be used to provide
such delays if needed. The model posts input and enable load values (in farads) based
on the parameters input load and enable. The output of this model does not, however,
respond to the total loading it sees on its output; it will always drive the output with the
specified delay. Note also that to maintain the technology-independence of the model,
any UNKNOWN input, or any floating input causes the output to also go UNKNOWN.
Likewise, any UNKNOWN input on the enable line causes the output to go to an UNDE-
TERMINED strength value.
12.4. DIGITAL MODELS 213
Example SPICE Usage:
a9 1 2 8 tri7
.model tri7 d_tristate(delay = 0.5e-9 input_load = 0.5e-12
+ enable_load = 0.5e-12)
12.4.10 Pullup
NAME_TABLE:
C_Function_Name: cm_d_pullup
Spice_Model_Name: d_pullup
Description: "digital pullup resistor"
PORT_TABLE:
Port Name: out
Description: "output"
Direction: out
Default_Type: d
Allowed_Types: [d]
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: load
Description: "load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital pullup resistor is a device that emulates the behavior of an analog
resistance value tied to a high voltage level. The pullup may be used in conjunction
with tristate buffers to provide open-collector wired or constructs, or any other logical
constructs that rely on a resistive pullup common to many tristated output devices. The
model posts an input load value (in farads) based on the parameter load.
Example SPICE Usage:
a2 9 pullup1
.model pullup1 d_pullup(load = 20.0e-12)
12.4.11 Pulldown
NAME_TABLE:
C_Function_Name: cm_d_pulldown
Spice_Model_Name: d_pulldown
Description: "digital pulldown resistor"
PORT_TABLE:
214 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Port Name: out
Description: "output"
Direction: out
Default_Type: d
Allowed_Types: [d]
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: load
Description: "load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital pulldown resistor is a device that emulates the behavior of an analog
resistance value tied to a low voltage level. The pulldown may be used in conjunction
with tristate buffers to provide open-collector wired or constructs, or any other logical
constructs that rely on a resistive pulldown common to many tristated output devices.
The model posts an input load value (in farads) based on the parameter load.
Example SPICE Usage:
a4 9 pulldown1
.model pulldown1 d_pulldown(load = 20.0e-12)
12.4.12 D Flip Flop
NAME_TABLE:
C_Function_Name: cm_d_dff
Spice_Model_Name: d_dff
Description: "digital d-type flip flop"
PORT_TABLE:
Port Name: data clk
Description: "input data" "clock"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PORT_TABLE:
Port Name: set reset
Description: "asynch. set" "asynch. reset"
Direction: in in
Default_Type: d d
12.4. DIGITAL MODELS 215
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PORT_TABLE:
Port Name: out Nout
Description: "data output" "inverted data output"
Direction: out out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: clk_delay set_delay
Description: "delay from clk" "delay from set"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: reset_delay ic
Description: "delay from reset" "output initial state"
Data_Type: real int
Default_Value: 1.0e-9 0
Limits: [1.0e-12 -] [0 2]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: data_load clk_load
Description: "data load value (F)" "clk load value (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: set_load reset_load
Description: "set load value (F)" "reset load (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector.Bounds: - -
216 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The digital d-type flip flop is a one-bit, edge-triggered storage element that will
store data whenever the clk input line transitions from low to high (ZERO to ONE). In
addition, asynchronous set and reset signals exist, and each of the three methods of chan-
ging the stored output of the d_dff have separate load values and delays associated with
them. Additionally, you may specify separate rise and fall delay values that are added to
those specified for the input lines; these allow for more faithful reproduction of the output
characteristics of different IC fabrication technologies.
Note that any UNKNOWN input on the set or reset lines immediately results in an
UNKNOWN output.
Example SPICE Usage:
a7123456flop1
.model flop1 d_dff(clk_delay = 13.0e-9 set_delay = 25.0e-9
+ reset_delay = 27.0e-9 ic = 2 rise_delay = 10.0e-9
+ fall_delay = 3e-9)
12.4.13 JK Flip Flop
NAME_TABLE:
C_Function_Name: cm_d_jkff
Spice_Model_Name: d_jkff
Description: "digital jk-type flip flop"
PORT_TABLE:
Port Name: j k
Description: "j input" "k input"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PORT_TABLE:
Port Name: clk
Description: "clock"
Direction: in
Default_Type: d
Allowed_Types: [d]
12.4. DIGITAL MODELS 217
Vector: no
Vector_Bounds: -
Null_Allowed: no
PORT_TABLE:
Port Name: set reset
Description: "asynchronous set" "asynchronous reset"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PORT_TABLE:
Port Name: out Nout
Description: "data output" "inverted data output"
Direction: out out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: clk_delay set_delay
Description: "delay from clk" "delay from set"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: reset_delay ic
Description: "delay from reset" "output initial state"
Data_Type: real int
Default_Value: 1.0e-9 0
Limits: [1.0e-12 -] [0 2]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: jk_load clk_load
Description: "j,k load values (F)" "clk load value (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
218 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
PARAMETER_TABLE:
Parameter_Name: set_load reset_load
Description: "set load value (F)" "reset load (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The digital jk-type flip flop is a one-bit, edge-triggered storage element that will
store data whenever the clk input line transitions from low to high (ZERO to ONE).
In addition, asynchronous set and reset signals exist, and each of the three methods of
changing the stored output of the d_jkff have separate load values and delays associated
with them. Additionally, you may specify separate rise and fall delay values that are
added to those specified for the input lines; these allow for more faithful reproduction of
the output characteristics of different IC fabrication technologies.
Note that any UNKNOWN inputs other than j or k cause the output to go UNKNOWN
automatically.
Example SPICE Usage:
a81234567flop2
.model flop2 d_jkff(clk_delay = 13.0e-9 set_delay = 25.0e-9
+ reset_delay = 27.0e-9 ic = 2 rise_delay = 10.0e-9
+ fall_delay = 3e-9)
12.4.14 Toggle Flip Flop
NAME_TABLE:
C_Function_Name: cm_d_tff
Spice_Model_Name: d_tff
Description: "digital toggle flip flop"
PORT_TABLE:
Port Name: t clk
Description: "toggle input" "clock"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
12.4. DIGITAL MODELS 219
Vector_Bounds: - -
Null_Allowed: no no
PORT_TABLE:
Port Name: set reset
Description: "set" "reset"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PORT.TABLE:
Port Name: out Nout
Description: "data output" "inverted data output"
Direction: out out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: clk_delay set_delay
Description: "delay from clk" "delay from set"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: reset_delay ic
Description: "delay from reset" "output initial state"
Data_Type: real int
Default_Value: 1.0e-9 0
Limits: [1.0e-12 -] [0 2]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: t_load clk_load
Description: "toggle load value (F)" "clk load value (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
220 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Parameter_Name: set_load reset_load
Description: "set load value (F)" "reset load (F)"
Data_Type: real real
Default.Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The digital toggle-type flip flop is a one-bit, edge-triggered storage element that
will toggle its current state whenever the clk input line transitions from low to high (ZERO
to ONE). In addition, asynchronous set and reset signals exist, and each of the three met-
hods of changing the stored output of the d_tff have separate load values and delays
associated with them. Additionally, you may specify separate rise and fall delay values
that are added to those specified for the input lines; these allow for more faithful repro-
duction of the output characteristics of different IC fabrication technologies.
Note that any UNKNOWN inputs other than t immediately cause the output to go UNKNOWN.
Example SPICE Usage:
a8 2 12 4 5 6 3 flop3
.model flop3 d_tff(clk_delay = 13.0e-9 set_delay = 25.0e-9
+ reset_delay = 27.0e-9 ic = 2 rise_delay = 10.0e-9
+ fall_delay = 3e-9 t_load = 0.2e-12)
12.4.15 Set-Reset Flip Flop
NAME_TABLE:
C_Function_Name: cm_d_srff
Spice_Model_Name: d_srff
Description: "digital set-reset flip flop"
PORT_TABLE:
Port Name: s r
Description: "set input" "reset input"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
12.4. DIGITAL MODELS 221
PORT_TABLE:
Port Name: clk
Description: "clock"
Direction: in
Default_Type: d
Allowed_Types: [d]
Vector: no
Vector_Bounds: -
Null_Allowed: no
PORT_TABLE:
Port Name: set reset
Description: "asynchronous set" "asynchronous reset"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PORT_TABLE:
Port Name: out Nout
Description: "data output" "inverted data output"
Direction: out out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: clk_delay set_delay
Description: "delay from clk" "delay from set"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: reset_delay ic
Description: "delay from reset" "output initial state"
Data_Type: real int
Default_Value: 1.0e-9 0
Limits: [1.0e-12 -] [0 2]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: sr_load clk_load
Description: "set/reset loads (F)" "clk load value (F)"
222 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: set_load reset_load
Description: "set load value (F)" "reset load (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The digital sr-type flip flop is a one-bit, edge-triggered storage element that will
store data whenever the clk input line transitions from low to high (ZERO to ONE). The
value stored (i.e., the out value) will depend on the s and r input pin values, and will be:
out=ONE if s=ONE and r=ZERO;
out=ZERO if s=ZERO and r=ONE;
out=previous value if s=ZERO and r=ZERO;
out=UNKNOWN if s=ONE and r=ONE;
In addition, asynchronous set and reset signals exist, and each of the three methods of changing
the stored output of the d_srff have separate load values and delays associated with them. You
may also specify separate rise and fall delay values that are added to those specified for the
input lines; these allow for more faithful reproduction of the output characteristics of different
IC fabrication technologies.
Note that any UNKNOWN inputs other than s and r immediately cause the output to go UNKNOWN.
Example SPICE Usage:
a8 2 12 4 5 6 3 14 flop7
.model flop7 d_srff(clk_delay = 13.0e-9 set_delay = 25.0e-9
+ reset_delay = 27.0e-9 ic = 2 rise_delay = 10.0e-9
+ fall_delay = 3e-9)
12.4. DIGITAL MODELS 223
12.4.16 D Latch
NAME_TABLE:
C_Function_Name: cm_d_dlatch
Spice_Model_Name: d_dlatch
Description: "digital d-type latch"
PORT_TABLE:
Port Name: data enable
Description: "input data" "enable input"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PORT_TABLE:
Port Name: set reset
Description: "set" "reset"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PORT_TABLE:
Port Name: out Nout
Description: "data output" "inverter data output"
Direction: out out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: data_delay
Description: "delay from data"
Data_Type: real
Default_Value: 1.0e-9
Limits: [1.0e-12 -]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: enable_delay set_delay
Description: "delay from enable" "delay from SET"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
224 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: reset_delay ic
Description: "delay from RESET" "output initial state"
Data_Type: real boolean
Default_Value: 1.0e-9 0
Limits: [1.0e-12 -] -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: data_load enable_load
Description: "data load (F)" "enable load value (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: set_load reset_load
Description: "set load value (F)" "reset load (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The digital d-type latch is a one-bit, level-sensitive storage element that will out-
put the value on the data line whenever the enable input line is high (ONE). The value on
the data line is stored (i.e., held on the out line) whenever the enable line is low (ZERO).
In addition, asynchronous set and reset signals exist, and each of the four methods of
changing the stored output of the d_dlatch (i.e., data changing with enable=ONE, enable
changing to ONE from ZERO with a new value on data, raising set and raising reset) have
separate delays associated with them. You may also specify separate rise and fall delay
values that are added to those specified for the input lines; these allow for more faithful
reproduction of the output characteristics of different IC fabrication technologies.
12.4. DIGITAL MODELS 225
Note that any UNKNOWN inputs other than on the data line when enable=ZERO imme-
diately cause the output to go UNKNOWN.
Example SPICE Usage:
a4 12 4 5 6 3 14 latch1
.model latch1 d_dlatch(data_delay = 13.0e-9 enable_delay = 22.0e-9
+ set_delay = 25.0e-9
+ reset_delay = 27.0e-9 ic = 2
+ rise_delay = 10.0e-9 fall_delay = 3e-9)
12.4.17 Set-Reset Latch
NAME_TABLE:
C_Function_Name: cm_d_srlatch
Spice_Model_Name: d_srlatch
Description: "digital sr-type latch"
PORT_TABLE:
Port Name: s r
Description: "set" "reset"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PORT_TABLE:
Port Name: enable
Description: "enable"
Direction: in
Default_Type: d
Allowed_Types: [d]
Vector: no
Vector_Bounds: -
Null_Allowed: no
PORT_TABLE:
Port Name: set reset
Description: "set" "reset"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PORT_TABLE:
Port Name: out Nout
Description: "data output" "inverted data output"
Direction: out out
Default_Type: d d
226 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: sr_delay
Description: "delay from s or r input change"
Data_Type: real
Default_Value: 1.0e-9
Limits: [1.0e-12 -]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: enable_delay set_delay
Description: "delay from enable" "delay from SET"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: reset_delay ic
Description: "delay from RESET" "output initial state"
Data_Type: real boolean
Default_Value: 1.0e-9 0
Limits: [1.0e-12 -] -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: sr_load enable_load
Description: "s & r input loads (F)" "enable load value (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: set_load reset_load
Description: "set load value (F)" "reset load (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
12.4. DIGITAL MODELS 227
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
Description: The digital sr-type latch is a one-bit, level-sensitive storage element that will
output the value dictated by the state of the s and r pins whenever the enable input line
is high (ONE). This value is stored (i.e., held on the out line) whenever the enable line is
low (ZERO). The particular value chosen is as shown below:
s=ZERO, r=ZERO => out=current value (i.e., not change in output)
s=ZERO, r=ONE => out=ZERO
s=ONE, r=ZERO => out=ONE
s=ONE, r=ONE => out=UNKNOWN
Asynchronous set and reset signals exist, and each of the four methods of changing the sto-
red output of the d srlatch (i.e., s/r combination changing with enable=ONE, enable changing
to ONE from ZERO with an output-changing combination of s and r, raising set and raising
reset) have separate delays associated with them. You may also specify separate rise and fall
delay values that are added to those specified for the input lines; these allow for more faithful
reproduction of the output characteristics of different IC fabrication technologies.
Note that any UNKNOWN inputs other than on the s and r lines when enable=ZERO immedi-
ately cause the output to go UNKNOWN.
Example SPICE Usage:
a4 12 4 5 6 3 14 16 latch2
.model latch2 d_srlatch(sr_delay = 13.0e-9 enable_delay = 22.0e-9
+ set_delay = 25.0e-9
+ reset_delay = 27.0e-9 ic = 2
+ rise_delay = 10.0e-9 fall_delay = 3e-9)
12.4.18 State Machine
NAME_TABLE:
C_Function_Name: cm_d_state
Spice_Model_Name: d_state
Description: "digital state machine"
PORT_TABLE:
Port Name: in clk
Description: "input" "clock"
228 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [1 -] -
Null_Allowed: yes no
PORT_TABLE:
Port Name: reset out
Description: "reset" "output"
Direction: in out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no yes
Vector_Bounds: - [1 -]
Null_Allowed: yes no
PARAMETER_TABLE:
Parameter_Name: clk_delay reset_delay
Description: "delay from CLK" "delay from RESET"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE: Parameter_Name: state_file
Description: "state transition specification file name"
Data_Type: string
Default_Value: "state.txt"
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: reset_state
Description: "default state on RESET & at DC"
Data_Type: int
Default_Value: 0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input loading capacitance (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
12.4. DIGITAL MODELS 229
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: clk_load
Description: "clock loading capacitance (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: reset_load
Description: "reset loading capacitance (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital state machine provides for straightforward descriptions of clocked
combinatorial logic blocks with a variable number of inputs and outputs and with an
unlimited number of possible states. The model can be configured to behave as virtually
any type of counter or clocked combinatorial logic block and can be used to replace very
large digital circuit schematics with an identically functional but faster representation.
The d state model is configured through the use of a state definition file (state.in) that
resides in a directory of your choosing. The file defines all states to be understood by the
model, plus input bit combinations that trigger changes in state. An example state.in file
is shown below:
----------- begin file -------------
* This is an example state.in file. This file
* defines a simple 2-bit counter with one input. The
* value of this input determines whether the counter counts
* up (in = 1) or down (in = 0).
00s0s0->3
1 -> 1
10s1z0->0
1 -> 2
21z0s0->1
1 -> 3
31z1z0->2
31z1z1->0
------------------ end file ---------------
Several attributes of the above file structure should be noted. First, all lines in the file must be
one of four types. These are:
230 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
1. A comment, beginning with a ‘*’ in the first column.
2. A header line, which is a complete description of the current state, the outputs correspon-
ding to that state, an input value, and the state that the model will assume should that
input be encountered. The first line of a state definition must always be a header line.
3. A continuation line, which is a partial description of a state, consisting of an input value
and the state that the model will assume should that input be encountered. Note that
continuation lines may only be used after the initial header line definition for a state.
4. A line containing nothing but white-spaces (space, form-feed, newline, carriage return,
tab, vertical tab).
A line that is not one of the above will cause a file-loading error. Note that in the example
shown, whitespace (any combination of blanks, tabs, commas) is used to separate values, and
that the character -> is used to underline the state transition implied by the input preceding it.
This particular character is not critical in of itself, and can be replaced with any other character
or non-broken combination of characters that you prefer (e.g. ==>,>>, ‘:’, resolves_to, etc.)
The order of the output and input bits in the file is important; the first column is always inter-
preted to refer to the ‘zeroth’ bit of input and output. Thus, in the file above, the output from
state 1 sets out[0] to 0s, and out[1] to 1z.
The state numbers need not be in any particular order, but a state definition (which consists of
the sum total of all lines that define the state, its outputs, and all methods by which a state can
be exited) must be made on contiguous line numbers; a state definition cannot be broken into
sub-blocks and distributed randomly throughout the file. On the other hand, the state definition
can be broken up by as many comment lines as you desire.
Header files may be used throughout the state.in file, and continuation lines can be discarded
completely if you so choose: continuation lines are primarily provided as a convenience.
Example SPICE Usage:
a4 [2 3 4 5] 1 12 [22 23 24 25 26 27 28 29] state1
.model state1 d_state(clk_delay = 13.0e-9 reset_delay = 27.0e-9
+ state_file = "newstate.txt" reset_state = 2)
Note: The file named by the parameter filename in state_file="filename" is sought after
according to a search list described in12.1.3.
12.4.19 Frequency Divider
NAME_TABLE:
C_Function_Name: cm_d_fdiv
Spice_Model_Name: d_fdiv
Description: "digital frequency divider"
PORT_TABLE:
Port Name: freq_in freq_out
Description: "frequency input" "frequency output"
Direction: in out
12.4. DIGITAL MODELS 231
Default_Type: d d
Allowed_Types: [d] [d]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: div_factor high_cycles
Description: "divide factor" "# of cycles for high out"
Data_Type: int int
Default_Value: 2 1
Limits: [1 -] [1 div_factor-1]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: i_count
Description: "divider initial count value"
Data_Type: int
Default_Value: 0
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: yes yes
Vector_Bounds: in in
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: freq_in_load
Description: "freq_in load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital frequency divider is a programmable step-down divider that accepts
an arbitrary divisor (div_factor), a duty-cycle term (high_cycles), and an initial count
value (i_count). The generated output is synchronized to the rising edges of the input
signal. Rise delay and fall delay on the outputs may also be specified independently.
Example SPICE Usage:
232 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
a4 3 7 divider
.model divider d_fdiv(div_factor = 5 high_cycles = 3
+ i_count = 4 rise_delay = 23e-9
+ fall_delay = 9e-9)
12.4.20 RAM
NAME_TABLE:
C_Function_Name: cm_d_ram
Spice_Model_Name: d_ram
Description: "digital random-access memory"
PORT_TABLE:
Port Name: data_in data_out
Description: "data input line(s)" "data output line(s)"
Direction: in out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes yes
Vector_Bounds: [1 -] data_in
Null_Allowed: no no
PORT_TABLE:
Port Name: address write_en
Description: "address input line(s)" "write enable line"
Direction: in in
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [1 -] -
Null_Allowed: no no
PORT_TABLE:
Port Name: select
Description: "chip select line(s)"
Direction: in
Default_Type: d
Allowed_Types: [d]
Vector: yes
Vector_Bounds: [1 16]
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: select_value
Description: "decimal active value for select line comparison"
Data_Type: int
Default_Value: 1
Limits: [0 32767]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
12.4. DIGITAL MODELS 233
Parameter_Name: ic
Description: "initial bit state @ dc"
Data_Type: int
Default_Value: 2
Limits: [0 2]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: read_delay
Description: "read delay from address/select/write.en active"
Data_Type: real
Default_Value: 100.0e-9
Limits: [1.0e-12 -]
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: data_load address_load
Description: "data_in load value (F)" "addr. load value (F)"
Data_Type: real real
Default_Value: 1.0e-12 1.0e-12
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: select_load
Description: "select load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: enable_load
Description: "enable line load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
Description: The digital RAM is an M-wide, N-deep random access memory element with
programmable select lines, tristated data out lines, and a single write/~read line. The
width of the RAM words (M) is set through the use of the word width parameter. The
234 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
depth of the RAM (N) is set by the number of address lines input to the device. The value
of N is related to the number of address input lines (P) by the following equation:
2P=N
There is no reset line into the device. However, an initial value for all bits may be specified
by setting the ic parameter to either 0 or 1. In reading a word from the ram, the read delay
value is invoked, and output will not appear until that delay has been satisfied. Separate
rise and fall delays are not supported for this device.
Note that UNKNOWN inputs on the address lines are not allowed during a write. In the
event that an address line does indeed go unknown during a write, the entire contents
of the ram will be set to unknown. This is in contrast to the data in lines being set to
unknown during a write; in that case, only the selected word will be corrupted, and this is
corrected once the data lines settle back to a known value. Note that protection is added
to the write en line such that extended UNKNOWN values on that line are interpreted as
ZERO values. This is the equivalent of a read operation and will not corrupt the contents
of the RAM. A similar mechanism exists for the select lines. If they are unknown, then it
is assumed that the chip is not selected.
Detailed timing-checking routines are not provided in this model, other than for the enable
delay and select delay restrictions on read operations. You are advised, therefore, to
carefully check the timing into and out of the RAM for correct read and write cycle
times, setup and hold times, etc. for the particular device they are attempting to model.
Example SPICE Usage:
a4 [3 4 5 6] [3 4 5 6] [12 13 14 15 16 17 18 19] 30 [22 23 24] ram2
.model ram2 d_ram(select_value = 2 ic = 2 read_delay = 80e-9)
12.4.21 Digital Source
NAME_TABLE:
C_Function_Name: cm_d_source
Spice_Model_Name: d_source
Description: "digital signal source"
PORT_TABLE:
Port Name: out
Description: "output"
Direction: out
Default_Type: d
Allowed_Types: [d]
Vector: yes
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: input_file
Description: "digital input vector filename"
Data_Type: string
Default_Value: "source.txt"
Limits: -
12.4. DIGITAL MODELS 235
Vector: no
Vector_Bounds: -
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input loading capacitance (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: no
Description: The digital source provides for straightforward descriptions of digital signal vec-
tors in a tabular format. The model reads input from the input file and, at the times
specified in the file, generates the inputs along with the strengths listed. The format of
the input file is as shown below. Note that comment lines are delineated through the use
of a single ‘*’ character in the first column of a line. This is similar to the way the SPICE
program handles comments.
* T c n n n . . .
* i l o o o . . .
* m o d d d . . .
* e c e e e . . .
* k a b c . . .
0.0000 Uu Uu Us Uu . . .
1.234e-9 0s 1s 1s 0z . . .
1.376e-9 0s 0s 1s 0z . . .
2.5e-7 1s 0s 1s 0z . . .
2.5006e-7 1s 1s 1s 0z . . .
5.0e-7 0s 1s 1s 0z . . .
Note that in the example shown, whitespace (any combination of blanks, tabs, commas) is used
to separate the time and state/strength tokens. The order of the input columns is important; the
first column is always interpreted to mean ‘time’. The second through the N’th columns map
to the out[0] through out[N-2] output nodes. A non-commented line that does not contain
enough tokens to completely define all outputs for the digital source will cause an error. Also,
time values must increase monotonically or an error will result in reading the source file.
Errors will also occur if a line exists in source.txt that is neither a comment nor vector line.
The only exception to this is in the case of a line that is completely blank; this is treated as
a comment (note that such lines often occur at the end of text within a file; ignoring these in
particular prevents nuisance errors on the part of the simulator).
Example SPICE Usage:
a3 [2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17] input_vector
.model input_vector d_source(input_file = "source_simple.text")
Note: The file named by the parameter filename in input_file="filename" is sought after
according to a search list described in12.1.3.
236 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
12.4.22 LUT
NAME_TABLE:
C_Function_Name: cm_d_lut
Spice_Model_Name: d_lut
Description: "digital n-input look-up table gate"
PORT_TABLE:
Port_Name: in out
Description: "input" "output"
Direction: in out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes no
Vector_Bounds: [1 -] -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load
Description: "input load value (F)"
Data_Type: real
Default_Value: 1.0e-12
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: yes
PARAMETER_TABLE:
Parameter_Name: table_values
Description: "lookup table values"
Data_Type: string
Default_Value: "0"
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: no
12.4. DIGITAL MODELS 237
Description: The lookup table provides a way to map any arbitrary n-input, 1-output combi-
national logic block to XSPICE. The inputs are mapped to the output using a string of length
2^n. The string may contain values "0", "1" or "X", corresponding to an output of low, high,
or unknown, respectively. The outputs are only mapped for inputs which are valid logic le-
vels. Any unknown bit in the input vector will always produce an unknown output. The first
character of the string table_values corresponds to all inputs value zero, and the last (2^n)
character corresponds to all inputs value one, with the first signal in the input vector being the
least significant bit. For example, a 2-input lookup table representing the function (A * B)
(that is, A AND B), with input vector [A B] can be constructed with a table_values string of
"0001"; function (~A * B) with input vector [A B] can be constructed with a table_values
string of "0010". The delays associated with an output rise and those associated with an output
fall may be specified independently. The model also posts an input load value (in farads) based
on the parameter input_load. The output of this model does not respond to the total loading
it sees on the output; it will always drive the output strongly with the specified delays.
Example SPICE Usage:
* LUT encoding 3-bit parity function
a4 [1 2 3] 5 lut_pty3_1
.model lut_pty3_1 d_lut(table_values = "01101001"
+ input_load 2.0e-12)
12.4.23 General LUT
NAME_TABLE:
C_Function_Name: cm_d_genlut
Spice_Model_Name: d_genlut
Description: "digital n-input x m-output look-up table gate"
PORT_TABLE:
Port_Name: in out
Description: "input" "output"
Direction: in out
Default_Type: d d
Allowed_Types: [d] [d]
Vector: yes yes
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: rise_delay fall_delay
Description: "rise delay" "fall delay"
Data_Type: real real
Default_Value: 1.0e-9 1.0e-9
Limits: [1.0e-12 -] [1.0e-12 -]
Vector: yes yes
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: input_load input_delay
Description: "input load value (F)" "input delay"
238 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Data_Type: real real
Default_Value: 1.0e-12 0.0
Limits: - -
Vector: yes yes
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: table_values
Description: "lookup table values"
Data_Type: string
Default_Value: "0"
Limits: -
Vector: no
Vector_Bounds: -
Null_Allowed: no
Description: The lookup table provides a way to map any arbitrary n-input, m-output combi-
national logic block to XSPICE. The inputs are mapped to the output using a string of length m
* (2^n). The string may contain values "0", "1", "X", or "Z", corresponding to an output of low,
high, unknown, or high-impedance, respectively. The outputs are only mapped for inputs which
are valid logic levels. Any unknown bit in the input vector will always produce an unknown
output. The character string is in groups of (2^n) characters, one group corresponding to each
output pin, in order. The first character of a group in the string table_values corresponds to
all inputs value zero, and the last (2^n) character in the group corresponds to all inputs value
one, with the first signal in the input vector being the least significant bit. For example, a 2-input
lookup table representing the function (A * B) (that is, A AND B), with input vector [A B] can
be constructed with a table_values string of "0001"; function (~A * B) with input vector
[A B] can be constructed with a "table_values" string of "0010". The delays associated with
each output pin’s rise and those associated with each output pin’s fall may be specified indepen-
dently. The model also posts independent input load values per input pin (in farads) based on
the parameter input_load. The parameter input_delay provides a way to specify additional
delay between each input pin and the output. This delay is added to the rise- or fall-time of the
output. The output of this model does not respond to the total loading it sees on the output; it
will always drive the output strongly with the specified delays.
Example SPICE Usage:
* LUT encoding 3-bit parity function
a4 [1 2 3] [5] lut_pty3_1
.model lut_pty3_1 d_genlut(table_values = "01101001"
+ input_load [2.0e-12])
* LUT encoding a tristate inverter function (en in out)
a2 [1 2] [3] lut_triinv_1
.model lut_triinv_1 d_genlut(table_values = "Z1Z0")
* LUT encoding a half-adder function (A B Carry Sum)
a8 [1 2] [3 4] lut_halfadd_1
.model lut_halfadd_1 d_genlut(table_values = "00010110"
+ rise_delay [ 1.5e-9 1.0e-9 ] fall_delay [ 1.5e-9 1.0e-9 ])
12.5. PREDEFINED NODE TYPES FOR EVENT DRIVEN SIMULATION 239
12.5 Predefined Node Types for event driven simulation
The following prewritten node types are included with the XSPICE simulator. These should
provide you not only with valuable event-driven modeling capabilities, but also with examples
to use for guidance in creating new UDN (user defined node) types. You may access these node
data by the plot (17.5.45) or eprint (17.5.24) commands.
12.5.1 Digital Node Type
The ‘digital’ node type is directly built into the simulator. 12 digital node values are available.
They are described by a two character string (the state/strength token). The first character (0,
1, or U) gives the state of the node (logic zero, logic one, or unknown logic state). The second
character (s, r, z, u) gives the "strength" of the logic state (strong, resistive, hi-impedance, or
undetermined). So these are the values we have: 0s, 1s, Us, 0r, 1r, Ur, 0z, 1z, Uz, 0u, 1u, Uu.
12.5.2 Real Node Type
The ‘real’ node type provides for event-driven simulation with double-precision floating point
data. This type is useful for evaluating sampled-data filters and systems. The type implements
all optional functions for User-Defined Nodes, including inversion and node resolution. For
inversion, the sign of the value is reversed. For node resolution, the resultant value at a node is
the sum of all values output to that node. The node is implemented as a user defined node in
ngspice/src/xspice/icm/xtraevt/real.
12.5.3 Int Node Type
The ‘int’ node type provides for event-driven simulation with integer data. This type is useful
for evaluating round-off error effects in sampled-data systems. The type implements all optional
functions for User-Defined Nodes, including inversion and node resolution. For inversion, the
sign of the integer value is reversed. For node resolution, the resultant value at a node is the
sum of all values output to that node. The node is implemented as a user defined node in
ngspice/src/xspice/icm/xtraevt/int.
12.5.4 (Digital) Input/Output
The analog code models use the standard (analog) nodes provided by ngspice and thus are using
all the commands for sourcing, storing, printing, and plotting data.
I/O for event nodes (digital, real, int, and UDNs) currently is much more limited to a few tools.
For output you may use the plot (17.5.45) or eprint (17.5.24) commands. For input, you may
create a test bench with existing code models (oscillator (12.3.3), frequency divider (12.4.19),
state machine (12.4.18) etc.). Reading data from a file is offered by d_source (12.4.21). Some
comments and hints have been provided by Sdaau. You may also use the analog input from file,
(filesource 12.2.8) and convert its analog input to the digital type by the adc_bridge (12.3.2).
If you want reading data from a VCD file, you may have a look at ngspice-users forum and
apply a python script provided by Sdaau to translate the VCD data to d_source or filesource
input.
240 CHAPTER 12. MIXED-MODE AND BEHAVIORAL MODELING WITH XSPICE
Chapter 13
Verilog A Device models
13.1 Introduction
The ngspice-adms interface will implement extra HICUM level0 and level2 (HICUM model
web page), MEXTRAM(MEXTRAM model web page), EKV(EKV model web page) and
PSP(NXP MOS model 9 web page) models written in Verilog-A behavior language.
13.2 adms
To compile Verilog-A compact models into ngspice-ready C models the the program admsXml
is required. Details of this software are described in adms home page.
13.3 How to integrate a Verilog-A model into ngspice
13.3.1 How to setup a *.va model for ngspice
The root entry for new Verilog-A models is \src\spicelib\devices\adms. Below the model-
name entry the Verilog-A code should reside in folder admsva
(e.g.: ngspice\src\spicelib\devices\adms\ekv\admsva\ekv.va). The file extension is fixed
to .va.
Certain files must modified to create the interface to ngspice - see the guideline README.adms
in the ngspice root.
13.3.2 Adding admsXml to your build environment
To facilitate the installation of adms, a source code package has been assembled for use with ng-
spice, available as a zip file for download. It is based on adms source code from the subversion
repository downloaded on August 1st, 2010, and has been slightly modified (see ChangeLog).
Under OS Linux (tested with SUSE 11.2, 64 bit) you may expand the zip file and run
./autogen_lin.sh, followed by ’make’ and ’make install’.
241
242 CHAPTER 13. VERILOG A DEVICE MODELS
Under OS CYGWIN (tested with actual CYGWIN on MS Windows 7, 64 bit), please use
./autogen_cyg.sh, followed by ’make’ and ’make install’.
Under OS MINGW, a direct compilation would require the additional installation of perl module
XML-LibXML, which is not as straightforward as it should be. However you may start with a
CYGWIN compile as described above. If you then go to your MSYS window, cd to the adms
top directory and start ./mingw-compile.sh, you will obtain admsXml.exe, copied to MSYS
/bin, and you are ready to go. To facilitate installation under MS Windows, a admsXml.exe
zipped binary is available. Just copy it to MSYS /bin directory and start working on your verilog
models.
A short test of a successful installation is:
$ admsXml -v
$ [usage..] release name="admsXml" version="2.3.0" date="Aug 4 2010"
time="10:24:18"
Compilation of admsXml with MS Visual Studio is not possible, because the source code has
variable declarations not only at the top of a block, but deliberately also in the following lines.
This is ok by the C99 standard, but not supported by MS Visual Studio.
Chapter 14
Mixed-Level Simulation (ngspice with
TCAD)
14.1 Cider
Ngspice implements mixed-level simulation through the merging of its code with CIDER (de-
tails see Chapt. 30).
CIDER is a mixed-level circuit and device simulator that provides a direct link between techno-
logy parameters and circuit performance. A mixed-level circuit and device simulator can pro-
vide greater simulation accuracy than a stand-alone circuit or device simulator by numerically
modeling the critical devices in a circuit. Compact models can be used for noncritical devices.
CIDER couples the latest version of SPICE3 (version 3F.2) [JOHN92] to a internal C-based
device simulator, DSIM. SPICE3 provides circuit analyses, compact models for semiconductor
devices, and an interactive user interface. DSIM provides accurate, one- and two-dimensional
numerical device models based on the solution of Poisson’s equation, and the electron and
hole current-continuity equations. DSIM incorporates many of the same basic physical models
found in the the Stanford two-dimensional device simulator PISCES [PINT85]. Input to CIDER
consists of a SPICE-like description of the circuit and its compact models, and PISCES-like
descriptions of the structures of numerically modeled devices. As a result, CIDER should seem
familiar to designers already accustomed to these two tools. For example, SPICE3F.2 input files
should run without modification, producing identical results.
CIDER is based on the mixed-level circuit and device simulator CODECS [MAYA88] and is a
replacement for this program. The basic algorithms of the two programs are the same. Some of
the differences between CIDER and CODECS are described below. The CIDER input format
has greater flexibility and allows increased access to physical model parameters. New physical
models have been added to allow simulation of state-of-the-art devices. These include trans-
verse field mobility degradation [GATE90] that is important in scaled-down MOSFETs and a
polysilicon model for poly-emitter bipolar transistors. Temperature dependence has been inclu-
ded for most physical models over the range from -50°C to 150°C. The numerical models can
be used to simulate all the basic types of semiconductor devices: resistors, MOS capacitors, di-
odes, BJTs, JFETs and MOSFETs. BJTs and JFETs can be modeled with or without a substrate
contact. Support has been added for the management of device internal states. Post-processing
of device states can be performed using the NUTMEG user interface of SPICE3. Previously
243
244 CHAPTER 14. MIXED-LEVEL SIMULATION (NGSPICE WITH TCAD)
computed states can be loaded into the program to provide accurate initial guesses for subse-
quent analyses. Finally, numerous small bugs have been discovered and fixed, and the program
has been ported to a wider variety of computing platforms.
Berkeley tradition calls for the naming of new versions of programs by affixing a (number,
letter, number) triplet to the end of the program name. Under this scheme, CIDER should
instead be named CODECS2A.l. However, tradition has been broken in this case because major
incompatibilities exist between the two programs and because it was observed that the acronym
CODECS is already used in the analog design community to refer to coder-decoder circuits.
Details of the basic semiconductor equations and the physical models used by CIDER are not
provided in this manual. Unfortunately, no other single source exists that describes all of the
relevant background material. Comprehensive reviews of device simulation can be found in
[PINT90] and the book [SELB84]. CODECS and its inversion-layer mobility model are des-
cribed in [MAYA88] and LGATE90], respectively. PISCES and its models are described in
[PINT85]. Temperature dependencies for the PISCES models used by CIDER are available in
[SOLL90].
14.2 GSS, Genius
For Linux users the cooperation of the TCAD software GSS with ngspice might be of interest,
see http://ngspice.sourceforge.net/gss.html. This project is no longer maintained however, but
has moved into the Genius simulator, still available as open source cogenda genius.
Chapter 15
Analyses and Output Control (batch
mode)
The command lines described in this chapter are specifying analyses and outputs within the
circuit description file. They start with a ‘.’ (dot commands). Specifying analyses and plots
(or tables) in the input file with dot commands is used with batch runs. Batch mode is entered
when either the -b option is given upon starting ngspice
ngspice -b -r rawfile.raw circuitfile.cir
or when the default input source is redirected from a file (see also Chapt. 16.4.1).
ngspice < circuitfile.cir
In batch mode, the analyses specified by the control lines in the input file (e.g. .ac,.tran, etc.)
are immediately executed. If the -r rawfile option is given then all data generated is written to
a ngspice rawfile. The rawfile may later be read by the interactive mode of ngspice using the
load command (see 17.5.38). In this case, the .save line (see 15.6) may be used to record the
value of internal device variables (see Appendix, Chapt. 31).
If a rawfile is not specified, then output plots (in ‘line-printer’ form) and tables can be printed
according to the .print,.plot, and .four control lines, described in Chapt. 15.6.
If ngspice is started in interactive mode (see Chapt. 16.4.2), like
ngspice circuitfile.cir
and no control section (.control ... .endc, see 16.4.3) is provided in the circuit file, the dot
commands are not executed immediately, but are waiting for manually receiving the command
run.
15.1 Simulator Variables (.options)
Various parameters of the simulations available in Ngspice can be altered to control the accu-
racy, speed, or default values for some devices. These parameters may be changed via the
option command (described in Chapt. 17.5.44) or via the .options line:
245
246 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
General form:
.options opt1 opt2 ... (or opt=optval ...)
Examples:
. options reltol =.005 trtol =8
The options line allows the user to reset program control and user options for specific simulation
purposes. Options specified to Ngspice via the option command (see Chapt. ) are also passed
on as if specified on a .options line. Any combination of the following options may be
included, in any order. ‘x’ (below) represents some positive number.
15.1.1 General Options
ACCT causes accounting and run time statistics to be printed.
NOACCT no printing of statistics, no printing of the Initial Transient Solution.
NOINIT suppresses only printing of the Initial Transient Solution, maybe combined with
ACCT.
LIST causes the summary listing of the input data to be printed.
NOMOD suppresses the printout of the model parameters.
NOPAGE suppresses page ejects.
NODE causes the printing of the node table.
OPTS causes the option values to be printed.
TEMP=x Resets the operating temperature of the circuit. The default value is 27 ◦C(300K).
TEMP can be overridden per device by a temperature specification on any temperature
dependent instance. May also be generally overridden by a .TEMP card (2.11).
TNOM=x resets the nominal temperature at which device parameters are measured. The de-
fault value is 27 ◦C(300 deg K). TNOM can be overridden by a specification on any
temperature dependent device model.
WARN=1|0 enables or turns of SOA (Safe Operating Area) voltage warning messages (default:
0).
MAXWARNS=x specifies the maximum number of SOA (Safe Operating Area) warning mes-
sages per model (default: 5).
SAVECURRENTS save currents through all terminals of the following devices: M, J, Q, D,
R, C, L, B, F, G, W, S, I (see 2.1.2). Recommended only for small circuits, because
otherwise memory requirements explode and simulation speed suffers. See 15.7 for more
details.
15.1. SIMULATOR VARIABLES (.OPTIONS) 247
15.1.2 DC Solution Options
The following options controls properties pertaining to DC analysis and algorithms. Since
transient analysis is based on DC many of the options affect the latter one.
ABSTOL=x resets the absolute current error tolerance of the program. The default value is 1
pA.
GMIN=x resets the value of GMIN, the minimum conductance allowed by the program. The
default value is 1.0e-12.
ITL1=x resets the dc iteration limit. The default is 100.
ITL2=x resets the dc transfer curve iteration limit. The default is 50.
KEEPOPINFO Retain the operating point information when either an AC, Distortion, or Pole-
Zero analysis is run. This is particularly useful if the circuit is large and you do not want
to run a (redundant) .OP analysis.
PIVREL=x resets the relative ratio between the largest column entry and an acceptable pivot
value. The default value is 1.0e-3. In the numerical pivoting algorithm the allowed mi-
nimum pivot value is determined by EPSREL =AMAX1(PIVREL ·MAXVAL,PIVTOL)where
MAXVAL is the maximum element in the column where a pivot is sought (partial pivo-
ting).
PIVTOL=x resets the absolute minimum value for a matrix entry to be accepted as a pivot.
The default value is 1.0e-13.
RELTOL=x resets the relative error tolerance of the program. The default value is 0.001
(0.1%).
RSHUNT=x introduces a resistor from each analog node to ground. The value of the resistor
should be high enough to not interfere with circuit operations. The XSPICE option has to
be enabled (see 32.1.5) .
VNTOL=x resets the absolute voltage error tolerance of the program. The default value is 1
µV.
15.1.2.1 Matrix Conditioning info
In most SPICE-based simulators, problems can arise with certain circuit topologies. One of
the most common problems is the absence of a DC path to ground at some node. This may
happen, for example, when two capacitors are connected in series with no other connection at
the common node or when certain code models are cascaded. The result is an ill-conditioned
or nearly singular matrix that prevents the simulation from completing. The XSPICE option
introduces the rshunt option to help eliminate this problem. When used, this option inserts
resistors to ground at all the analog nodes in the circuit. In general, the value of rshunt should
be set to some very high resistance (e.g. 1000 Meg Ohms or greater) so that the operation of the
circuit is essentially unaffected, but the matrix problems are corrected. If you should encounter
a ‘no DC path to ground’ or a ‘matrix is nearly singular’ error message with your circuit, you
should try adding the following .option card to your circuit description deck.
248 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
.option rshunt = 1.0e12
Usually a value of 1.0e12 is sufficient to correct the matrix problems. However, if you still have
problems, you may wish to try lowering this value to 1.0e10 or 1.0e9.
Another matrix conditioning problem might occur if you try to place an inductor in parallel to
a voltage source. An ac simulation will fail, because it is preceded by an op analysis. Option
noopac (15.1.3) will help if the circuit is linear. If the circuit is non-linear, you will need the
op analysis. Then adding a small resistor (e.g. 1e-4 Ohms) in series to the inductor will help to
obtain convergence.
.option rseries = 1.0e-4
will add a series resistor to each inductor in the circuit. Be careful if you use behavioral induc-
tors (see 3.2.12), because the result may become unpredictable.
15.1.3 AC Solution Options
NOOPAC Do not do an operating point (OP) analysis before the AC analysis. To become
valid, this option requires that the circuit is linear, thus consists only of R, L, and C
devices, independent V, I sources and linear dependent E, G, H, and F sources (without
poly statement, non-behavioral). If a non-linear device is detected, the OP analysis will
be executed automatically. This option is of interest for example in nested LC circuits,
where there is no series resistance for the L device given, which during OP analysis may
result in an ill formed matrix, yields an error message and aborts the simulation.
15.1.4 Transient Analysis Options
AUTOSTOP stops a transient analysis after successfully calculating all measure functions
(15.4) specified with the dot command .meas. Autostop is not available with meas
(17.5.39) used in control mode.
CHGTOL=x resets the charge tolerance of the program. The default value is 1.0e-14.
CONVSTEP=x relative step limit applied to code models.
CONVABSSTEP=x absolute step limit applied to code models.
GMINSTEPS=x [*] sets number of Gmin steps to be attempted. If the value is set to zero, the
gmin stepping algorithm is disabled. In such case the source stepping algorithm becomes
the standard when the standard procedure fails to converge to a solution.
INTERP interpolates output data onto fixed time steps, detemined by TSTEP (15.3.9). Uses
linear interpolation between previous and next time value. Simulation itself is not in-
fluenced by this option. May be used in all simulation modes (batch, control or inte-
ractive, 16.4). This option may drastically reduce memory requirements in control mode
or file size in batch mode, but be careful not to choose a too large TSTEP value, other-
wise your output data may be corrupted by undersampling. See command ’linearize’
(17.5.36) in control or interactive mode to achieve similar outputs by post-processing of
data. See ngspice/examples/xspice/delta-sigma/delta-sigma-1.cir how INTERP will
reduce memory requirements and speeds up plotting.
15.1. SIMULATOR VARIABLES (.OPTIONS) 249
ITL3=x resets the lower transient analysis iteration limit. the default value is 4. (Note: not
implemented in Spice3).
ITL4=x resets the transient analysis time-point iteration limit. the default is 10.
ITL5=x resets the transient analysis total iteration limit. the default is 5000. Set ITL5=0 to
omit this test. (Note: not implemented in Spice3).
ITL6=x [*] synonym for SRCSTEPS.
MAXEVITER=x sets the number of event iterations that are allowed at an analysis point
MAXOPALTER=x specifies the maximum number of analog/event alternations that the simu-
lator can use in solving a hybrid circuit.
MAXORD=x [*] specifies the maximum order for the numerical integration method used by
SPICE. Possible values for the Gear method are from 2 (the default) to 6. Using the value
1 with the trapezoidal method specifies backward Euler integration.
METHOD=name sets the numerical integration method used by SPICE. Possible names are
‘Gear’ or ‘trapezoidal’ (or just ‘trap’). The default is trapezoidal.
NOOPALTER=TRUE|FALSE if set to false alternations between analog/event are enabled.
RAMPTIME=x this options sets the rate of change of independent supplies and code model
inductors and capacitors with initial conditions specified.
SRCSTEPS=x [*] a non-zero value causes SPICE to use a source-stepping method to find the
DC operating point. Its value specifies the number of steps.
TRTOL=x resets the transient error tolerance. The default value is 7. This parameter is an esti-
mate of the factor by which ngspice overestimates the actual truncation error. If XSPICE
is enabled and ’A’ devices included, the value is internally set to 1 for higher precision.
This will cost a factor of two in CPU time during transient analysis.
XMU=x sets a damping factor for trapezoidal integration. The default value is XMU=0.5. A
value <0.5 may be chosen. Even a small reduction, e.g. to 0.495, may suppress trap
ringing. The reduction has to be set carefully in order not to excessively damp circuits
that are prone to ringing, and lead the simulation (and the user) to believe that the circuit
is stable.
15.1.5 ELEMENT Specific options
BADMOS3 Use the older version of the MOS3 model with the ‘kappa’ discontinuity.
DEFAD=x resets the value for MOS drain diffusion area; the default is 0.0.
DEFAS=x resets the value for MOS source diffusion area; the default is 0.0.
DEFL=x resets the value for MOS channel length; the default is 100.0 µm.
DEFW=x resets the value for MOS channel width; the default is 100.0 µm.
250 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
SCALE=x set the element scaling factor for geometric element parameters whose default unit
is meters. As an example: scale=1u and a MOSFET instance parameter W=10 will result
in a width of 10µmfor this device. An area parameter AD=20 will result in 20e-12 m2.
Following instance parameters are scaled:
• Resistors and Capacitors: W, L
• Diodes: W, L, Area
• JFET, MESFET: W, L, Area
• MOSFET: W, L, AS, AD, PS, PD, SA, SB, SC, SD
15.1.6 Transmission Lines Specific Options
TRYTOCOMPACT Applicable only to the LTRA model (see 6.2.1). When specified, the
simulator tries to condense LTRA transmission line’s past history of input voltages and
currents.
15.1.7 Precedence of option and .options commands
There are various ways to set the above mentioned options in Ngspice. If no option or
.options lines are set by the user, internal default values are given for each of the simula-
tor variables.
You may set options in the init files spinit or .spiceinit via the option command (see Chapt.
17.5.44). The values given here will supersede the default values. If you set options via the
.options line in your input file, their values will supersede the default and init file data. Finally
if you set options inside a .control ... .endc section, these values will supersede any values
of the respective simulator variables given so far.
15.2 Initial Conditions
15.2.1 .NODESET: Specify Initial Node Voltage Guesses
General form:
. NODESET V( NODNUM )= VAL V( NODNUM )= VAL ...
.NODESET ALL=VAL
Examples:
.NODESET V (12)=4.5 V(4)=2.23
. NODESET ALL =1.5
15.2. INITIAL CONDITIONS 251
The .nodeset line helps the program find the dc or initial transient solution by making a
preliminary pass with the specified nodes held to the given voltages. The restriction is then
released and the iteration continues to the true solution. The .nodeset line may be necessary
for convergence on bistable or a-stable circuits. .nodeset all=val allows to set all starting
node voltages (except for the ground node) in a single line. In general, the .nodeset line
should not be necessary.
15.2.2 .IC: Set Initial Conditions
General form:
.ic v( nodnum )= val v( nodnum )= val ...
Examples:
.ic v (11)=5 v (4)= -5 v (2)=2.2
The .ic line is for setting transient initial conditions. It has two different interpretations, de-
pending on whether the uic parameter is specified on the .tran control line. Also, one should
not confuse this line with the .nodeset line. The .nodeset line is only to help dc conver-
gence, and does not affect the final bias solution (except for multi-stable circuits). The two
interpretations of this line are as follows:
1. When the uic parameter is specified on the .tran line, then the node voltages specified
on the .ic control line are used to compute the capacitor, diode, BJT, JFET, and MOSFET
initial conditions. This is equivalent to specifying the ic=... parameter on each device
line, but is much more convenient. The ic=... parameter can still be specified and takes
precedence over the .ic values. Since no dc bias (initial transient) solution is computed
before the transient analysis, one should take care to specify all dc source voltages on the
.ic control line if they are to be used to compute device initial conditions.
2. When the uic parameter is not specified on the .tran control line, the dc bias (initial
transient) solution is computed before the transient analysis. In this case, the node volta-
ges specified on the .ic control lines are forced to the desired initial values during the
bias solution. During transient analysis, the constraint on these node voltages is removed.
This is the preferred method since it allows ngspice to compute a consistent dc solution.
252 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
15.3 Analyses
15.3.1 .AC: Small-Signal AC Analysis
General form:
.ac dec nd fstart fstop
.ac oct no fstart fstop
.ac lin np fstart fstop
Examples:
.ac dec 10 1 10K
.ac dec 10 1K 100 MEG
.ac lin 100 1 100 HZ
dec stands for decade variation, and nd is the number of points per decade. oct stands for
octave variation, and no is the number of points per octave. lin stands for linear variation, and
np is the number of points. fstart is the starting frequency, and fstop is the final frequency.
If this line is included in the input file, ngspice performs an AC analysis of the circuit over the
specified frequency range. Note that in order for this analysis to be meaningful, at least one
independent source must have been specified with an ac value. Typically it does not make much
sense to specify more than one ac source. If you do, the result will be a superposition of all
sources, thus difficult to interpret.
Example:
Basic RC circuit
r 1 2 1.0
c 2 0 1.0
vin 1 0 dc 0 ac 1 $ <--- the ac source
.options noacct
.ac dec 10 .01 10
. plot ac vdb (2) xlog
.end
In this ac (or ’small signal’) analysis all non-linear devices are linearized around their actual dc
operating point. All Ls and Cs get their imaginary value, depending on the actual frequency
step. Each output vector will be calculated relative to the input voltage (current) given by the ac
value (Vin equals to 1 in the example above). The resulting node voltages (and branch currents)
are complex vectors. Therefore you have to be careful using the plot command. Especially
you may use the variants of vxx(node) described in Chapt. 15.6.2 like vdb(2) (see example
above).
15.3. ANALYSES 253
15.3.2 .DC: DC Transfer Function
General form:
.dc srcnam vstart vstop vincr [src2 start2 stop2 incr2]
Examples:
.dc VIN 0.25 5.0 0.25
.dc VDS 0 10 .5 VGS 0 5 1
.dc VCE 0 10 .25 IB 0 10u 1u
.dc RLoad 1k 2k 100
.dc TEMP -15 75 5
The .dc line defines the dc transfer curve source and sweep limits (again with capacitors open
and inductors shorted). srcnam is the name of an independent voltage or current source, a
resistor or the circuit temperature. vstart,vstop, and vincr are the starting, final, and in-
crementing values respectively. The first example causes the value of the voltage source VIN
to be swept from 0.25 Volts to 5.0 Volts in increments of 0.25 Volts. A second source (src2)
may optionally be specified with associated sweep parameters. In this case, the first source is
swept over its range for each value of the second source. This option can be useful for obtaining
semiconductor device output characteristics. See the example circuit description on transistor
characteristics (21.3).
15.3.3 .DISTO: Distortion Analysis
General form:
.disto dec nd fstart fstop <f2overf1 >
.disto oct no fstart fstop <f2overf1 >
.disto lin np fstart fstop <f2overf1 >
Examples:
. disto dec 10 1 kHz 100 MEG
.disto dec 10 1 kHz 100 MEG 0.9
The .disto line does a small-signal distortion analysis of the circuit. A multi-dimensional Vol-
terra series analysis is done using multi-dimensional Taylor series to represent the nonlinearities
at the operating point. Terms of up to third order are used in the series expansions.
If the optional parameter f2overf1 is not specified, .disto does a harmonic analysis - i.e.,
it analyses distortion in the circuit using only a single input frequency F1, which is swept as
specified by arguments of the .disto command exactly as in the .ac command. Inputs at this
frequency may be present at more than one input source, and their magnitudes and phases are
specified by the arguments of the distof1 keyword in the input file lines for the input sources
254 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
(see the description for independent sources). (The arguments of the distof2 keyword are not
relevant in this case).
The analysis produces information about the AC values of all node voltages and branch currents
at the harmonic frequencies 2F1and , vs. the input frequency F1as it is swept. (A value of 1
(as a complex distortion output) signifies cos(2π(2F1)t)at 2F1and cos(2π(3F1)t)at 3F1, using
the convention that 1 at the input fundamental frequency is equivalent to cos(2πF1t).) The
distortion component desired (2F1or 3F1) can be selected using commands in ngnutmeg, and
then printed or plotted. (Normally, one is interested primarily in the magnitude of the harmonic
components, so the magnitude of the AC distortion value is looked at). It should be noted that
these are the AC values of the actual harmonic components, and are not equal to HD2 and HD3.
To obtain HD2 and HD3, one must divide by the corresponding AC values at F1, obtained from
an .ac line. This division can be done using ngnutmeg commands.
If the optional f2overf1 parameter is specified, it should be a real number between (and not
equal to) 0.0 and 1.0; in this case, .disto does a spectral analysis. It considers the circuit with
sinusoidal inputs at two different frequencies F1and F2.F1is swept according to the .disto
control line options exactly as in the .ac control line. F2is kept fixed at a single frequency
as F1sweeps - the value at which it is kept fixed is equal to f2overf1 times fstart. Each
independent source in the circuit may potentially have two (superimposed) sinusoidal inputs
for distortion, at the frequencies F1and F2. The magnitude and phase of the F1component are
specified by the arguments of the distof1 keyword in the source’s input line (see the descrip-
tion of independent sources); the magnitude and phase of the F2component are specified by the
arguments of the distof2 keyword. The analysis produces plots of all node voltages/branch
currents at the intermodulation product frequencies F1+F2,F1−F2, and (2F1)−F2, vs the
swept frequency F1. The IM product of interest may be selected using the setplot command,
and displayed with the print and plot commands. It is to be noted as in the harmonic analysis
case, the results are the actual AC voltages and currents at the intermodulation frequencies, and
need to be normalized with respect to .ac values to obtain the IM parameters.
If the distof1 or distof2 keywords are missing from the description of an independent
source, then that source is assumed to have no input at the corresponding frequency. The default
values of the magnitude and phase are 1.0 and 0.0 respectively. The phase should be specified
in degrees.
It should be carefully noted that the number f2overf1 should ideally be an irrational number,
and that since this is not possible in practice, efforts should be made to keep the denominator
in its fractional representation as large as possible, certainly above 3, for accurate results (i.e.,
if f2overf1 is represented as a fraction A
/B, where Aand Bare integers with no common
factors, Bshould be as large as possible; note that A<Bbecause f2overf1 is constrained
to be <1). To illustrate why, consider the cases where f2overf1 is 49/100 and 1/2. In a
spectral analysis, the outputs produced are at F1+F2,F1−F2and 2F1−F2. In the latter case,
F1−F2=F2, so the result at the F1−F2component is erroneous because there is the strong
fundamental F2component at the same frequency. Also, F1+F2=2F1−F2in the latter case,
and each result is erroneous individually. This problem is not there in the case where f2overf1
= 49/100, because F1−F2=51/100 F1<> 49/100 F1=F2. In this case, there are two very
closely spaced frequency components at F2and F1−F2. One of the advantages of the Volterra
series technique is that it computes distortions at mix frequencies expressed symbolically (i.e.
nF1+mF2), therefore one is able to obtain the strengths of distortion components accurately
even if the separation between them is very small, as opposed to transient analysis for example.
The disadvantage is of course that if two of the mix frequencies coincide, the results are not
15.3. ANALYSES 255
merged together and presented (though this could presumably be done as a postprocessing step).
Currently, the interested user should keep track of the mix frequencies himself or herself and
add the distortions at coinciding mix frequencies together should it be necessary.
Only a subset of the ngspice nonlinear device models supports distortion analysis. These are
• Diodes (DIO),
• BJT,
• JFET (level 1),
• MOSFETs (levels 1, 2, 3, 9, and BSIM1),
• MESFET (level 1).
15.3.4 .NOISE: Noise Analysis
General form:
.noise v( output <,ref >) src ( dec | lin | oct ) pts fstart fstop
+ <pts_per_summary>
Examples:
.noise v(5) VIN dec 10 1kHz 100 MEG
.noise v(5 ,3) V1 oct 8 1.0 1.0 e6 1
The .noise line does a noise analysis of the circuit. output is the node at which the total
output noise is desired; if ref is specified, then the noise voltage v(output) - v(ref) is
calculated. By default, ref is assumed to be ground. src is the name of an independent source
to which input noise is referred. pts,fstart and fstop are .ac type parameters that specify
the frequency range over which plots are desired. pts_per_summary is an optional integer; if
specified, the noise contributions of each noise generator is produced every pts_per_summary
frequency points. The .noise control line produces two plots:
1. one for the Noise Spectral Density (in V/√Hz or A
/√Hz ) curves and
2. one for the total Integrated Noise (in Vor A) over the specified frequency range.
15.3.5 .OP: Operating Point Analysis
General form:
.op
The inclusion of this line in an input file directs ngspice to determine the dc operating point of
the circuit with inductors shorted and capacitors opened.
256 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
Note: a DC analysis is automatically performed prior to a transient analysis to determine the
transient initial conditions, and prior to an AC small-signal, Noise, and Pole-Zero analysis
to determine the linearized, small-signal models for nonlinear devices (see the KEEPOPINFO
variable 15.1.2).
15.3.6 .PZ: Pole-Zero Analysis
General form:
.pz node1 node2 node3 node4 cur pol
.pz node1 node2 node3 node4 cur zer
.pz node1 node2 node3 node4 cur pz
.pz node1 node2 node3 node4 vol pol
.pz node1 node2 NODE3 node4 vol zer
.pz node1 node2 node3 node4 vol pz
Examples:
.pz 1 0 3 0 cur pol
.pz 2 3 5 0 vol zer
.pz 4 1 4 1 cur pz
cur stands for a transfer function of the type (output voltage)/(input current) while vol stands
for a transfer function of the type (output voltage)/(input voltage). pol stands for pole analysis
only, zer for zero analysis only and pz for both. This feature is provided mainly because
if there is a nonconvergence in finding poles or zeros, then, at least the other can be found.
Finally, node1 and node2 are the two input nodes and node3 and node4 are the two output
nodes. Thus, there is complete freedom regarding the output and input ports and the type of
transfer function.
In interactive mode, the command syntax is the same except that the first field is pz instead of
.pz. To print the results, one should use the command print all.
15.3. ANALYSES 257
15.3.7 .SENS: DC or Small-Signal AC Sensitivity Analysis
General form:
.SENS OUTVAR
.SENS OUTVAR AC DEC ND FSTART FSTOP
.SENS OUTVAR AC OCT NO FSTART FSTOP
.SENS OUTVAR AC LIN NP FSTART FSTOP
Examples:
.SENS V(1, OUT)
.SENS V(OUT) AC DEC 10 100 100 k
.SENS I( VTEST)
The sensitivity of OUTVAR to all non-zero device parameters is calculated when the SENS
analysis is specified. OUTVAR is a circuit variable (node voltage or voltage-source branch
current). The first form calculates sensitivity of the DC operating-point value of OUTVAR.
The second form calculates sensitivity of the AC values of OUTVAR. The parameters listed
for AC sensitivity are the same as in an AC analysis (see .AC above). The output values are in
dimensions of change in output per unit change of input (as opposed to percent change in output
or per percent change of input).
15.3.8 .TF: Transfer Function Analysis
General form:
.tf outvar insrc
Examples:
.tf v(5, 3) VIN
.tf i( VLOAD) VIN
The .tf line defines the small-signal output and input for the dc small-signal analysis. outvar
is the small signal output variable and insrc is the small-signal input source. If this line is
included, ngspice computes the dc small-signal value of the transfer function (output/input),
input resistance, and output resistance. For the first example, ngspice would compute the ratio
of V(5, 3) to VIN, the small-signal input resistance at VIN, and the small signal output resistance
measured across nodes 5 and 3.
258 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
15.3.9 .TRAN: Transient Analysis
General form:
.tran tstep tstop <tstart <tmax >> <uic >
Examples:
.tran 1ns 100ns
. tran 1 ns 1000 ns 500 ns
.tran 10 ns 1us
tstep is the printing or plotting increment for line-printer output. For use with the post-
processor, tstep is the suggested computing increment. tstop is the final time, and tstart
is the initial time. If tstart is omitted, it is assumed to be zero. The transient analysis always
begins at time zero. In the interval <zero, tstart>, the circuit is analyzed (to reach a steady
state), but no outputs are stored. In the interval <tstart,tstop>, the circuit is analyzed and
outputs are stored. tmax is the maximum stepsize that ngspice uses; for default, the program
chooses either tstep or (tstop-tstart)/50.0, whichever is smaller. tmax is useful when one
wishes to guarantee a computing interval that is smaller than the printer increment, tstep.
An initial transient operating point at time zero is calculated according to the following proce-
dure: all independent voltages and currents are applied with their time zero values, all capacitan-
ces are opened, inductances are shorted, the non linear device equations are solved iteratively.
uic (use initial conditions) is an optional keyword that indicates that the user does not want
ngspice to solve for the quiescent operating point before beginning the transient analysis. If this
keyword is specified, ngspice uses the values specified using IC=... on the various elements as
the initial transient condition and proceeds with the analysis. If the .ic control line has been
specified (see 15.2.2), then the node voltages on the .ic line are used to compute the initial
conditions for the devices. IC=... will take precedence over the values given in the .ic control
line. If neither IC=... nor the .ic control line is given for a specific node, node voltage zero is
assumed.
Look at the description on the .ic control line (15.2.2) for its interpretation when uic is not
specified.
15.3.10 Transient noise analysis (at low frequency)
In contrast to the analysis types described above the transient noise simulation (noise current or
voltage versus time) is not implemented as a dot command, but is integrated with the indepen-
dent voltage source vsrc (isrc not yet available) (see 4.1.7) and used in combination with the
.tran transient analysis (15.3.9).
Transient noise analysis deals with noise currents or voltages added to your circuits as a time
dependent signal of randomly generated voltage excursion on top of a fixed dc voltage. The
sequence of voltage values has random amplitude, but equidistant time intervals, selectable by
the user (parameter NT). The resulting voltage waveform is differentiable and thus does not
require any modifications of the matrix solving algorithms.
15.3. ANALYSES 259
White noise is generated by the ngspice random number generator, applying the Box-Muller
transform. Values are generated on the fly, each time when a breakpoint is hit.
The 1/f noise is generated with an algorithm provided by N. J. Kasdin (‘Discrete simulation of
colored noise and stochastic processes and 1/fapower law noise generation’, Proceedings of
the IEEE, Volume 83, Issue 5, May 1995 Page(s):802–827). The noise sequence (one for each
voltage/current source with 1/f selected) is generated upon start up of the simulator and stored
for later use. The number of points is determined by the total simulation time divided by NT,
rounded up the the nearest power of 2. Each time a breakpoint (n?NT , relevant to the noise
signal) is hit, the next value is retrieved from the sequence.
If you want a random, but reproducible sequence, you may select a seed value for the random
number generator by adding
set rndseed=nn
to the spinit or .spiceinit file, nn being a positive integer number.
The transient noise analysis will allow the simulation of the three most important noise sources.
Thermal noise is described by the Gaussian white noise. Flicker noise (pink noise or 1 over
f noise) with an exponent between 0 and 2 is provided as well. Shot noise is dependent on
the current flowing through a device and may be simulated by applying a non-linear source as
demonstrated in the following example:
Example:
* Shot noise test with B source , diode
* voltage on device (diode , forward )
Vdev out 0 DC 0 PULSE (0.4 0.45 10 u)
* diode , forward direction , to be modeled with noise
D1 mess 0 DMOD
.model DMOD D IS =1e-14 N=1
X1 0 mess out ishot
* device between 1 and 2
* new output terminals of device including noise : 1 and 3
.subckt ishot 1 2 3
* white noise source with rms 1V
* 20000 sample points
VNG 0 11 DC 0 TRNOISE (1 1n 0 0)
*measure the current i(v1)
V1 2 3 DC 0
* calculate the shot noise
* sqrt (2* current *q* bandwidth )
BI 1 3 I= sqrt (2* abs (i( v1 ))*1.6e -19*1 e7 )* v(11)
.ends ishot
.tran 1n 20u
.control
run
plot ( -1)*i(vdev )
.endc
.end
260 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
The selection of the delta time step (NT) is worth discussing. Gaussian white noise has unlimited
bandwidth and thus unlimited energy content. This is unrealistic. The bandwidth of real noise
is limited, but it is still called ‘White’ if it is the same level throughout the frequency range
of interest, e.g. the bandwidth of your system. Thus you may select NT to be a factor of 10
smaller than the frequency limit of your circuit. A thorough analysis is still needed to clarify the
appropriate factor. The transient method is probably most suited to circuits including switches,
which are not amenable to the small signal .NOISE analysis (Chapt. 15.3.4).
There is a price you have to pay for transient noise analysis: the number of required time steps,
and thus the simulation time, increases.
In addition to white and 1/f noise the independent voltage and current sources offer a random
telegraph signal (RTS) noise source, also known as burst noise or popcorn noise, again for
transient analysis. For each voltage (current) source offering RTS noise an individual noise
amplitude is required for input, as well as a mean capture time and a mean emission time.
The amplitude resembles the influence of a single trap on the current or voltage. The capture
and emission times emulate the filling and emptying of the trap, typically following a Poisson
process. They are generated from an random exponential distribution with respective mean
values given by the user. To simulate an ensemble of traps, you may combine several current or
voltage sources with different parameters.
All three sources (white, 1/f, and RTS) may be combined in a single command line.
15.3. ANALYSES 261
RTS noise example:
* white noise , 1/f noise , RTS noise
* voltage source
VRTS2 13 12 DC 0 trnoise (0 0 0 0 5m 18u 30u)
VRTS3 11 0 DC 0 trnoise (0 0 0 0 10m 20u 40u)
VALL 12 11 DC 0 trnoise (1m 1u 1.0 0.1m 15m 22u 50u)
VW1of 21 0 DC trnoise (1 m 1u 1.0 0.1m)
* current source
IRTS2 10 0 DC 0 trnoise (0 0 0 0 5m 18u 30u)
IRTS3 10 0 DC 0 trnoise (0 0 0 0 10m 20u 40u)
IALL 10 0 DC 0 trnoise (1 m 1u 1.0 0.1m 15m 22u 50u)
R10 10 0 1
IW1of 9 0 DC trnoise (1m 1u 1.0 0.1m)
Rall 9 0 1
* sample points
.tran 1u 500u
.control
run
plot v(13) v(21)
plot v(10) v (9)
.endc
.end
Some details on RTS noise modeling are available in a recent article [20], available here.
This transient noise feature is still experimental.
The following questions (among others) are to be solved:
• clarify the theoretical background
• noise limit of plain ngspice (numerical solver, fft etc.)
• time step (NT) selection
• calibration of noise spectral density
• how to generate noise from a transistor model
• application benefits and limits
262 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
15.3.11 .PSS: Periodic Steady State Analysis
Experimental code, not yet made publicly available.
General form:
.pss gfreq tstab oscnob psspoints harms sciter steadycoeff <uic >
Examples:
.pss 150 200e -3 2 1024 11 50 5e -3 uic
.pss 624 e6 1u v_plus 1024 10 150 5e-3 uic
.pss 624 e6 500n bout 1024 10 100 5e -3 uic
gfreq is guessed frequency of fundamental suggested by user. When performing transient
analysis the PSS algorithm tries to infer a new rough guess rgfreq on the fundamental. If
gfreq is out of ±10% with respect to rgfreq then gfreq is discarded.
tstab is stabilization time before the shooting begin to search for the PSS. It has to be noticed
that this parameter heavily influence the possibility to reach the PSS. Thus is a good practice to
ensure a circuit to have a right tstab, e.g. performing a separate TRAN analysis before to run
PSS analysis.
oscnob is the node or branch where the oscillation dynamic is expected. PSS analysis will give
a brief report of harmonic content at this node or branch.
psspoints is number of step in evaluating predicted period after convergence is reached. It
is useful only in Time Domain plots. However this number should be higher than 2 times the
requested harms. Otherwise the PSS analysis will properly adjust it.
harms number of harmonics to be calculated as requested by the user.
sciter number of allowed shooting cycle iterations. Default is 50.
steady_coeff is the weighting coefficient for calculating the Global Convergence Error (GCE),
which is the reference value in order to infer is convergence is reached. The lower steady_coeff
is set, the higher the accuracy of predicted frequency can be reached but at longer analysis time
and sciter number. Default is 1e-3.
uic (use initial conditions) is an optional keyword that indicates that the user does not want
ngspice to solve for the quiescent operating point before beginning the transient analysis. If this
keyword is specified, ngspice uses the values specified using IC=... on the various elements as
the initial transient condition and proceeds with the analysis. If the .ic control line has been
specified, then the node voltages on the .ic line are used to compute the initial conditions for
the devices. Look at the description on the .ic control line for its interpretation when uic is
not specified.
15.4. MEASUREMENTS AFTER AC, DC AND TRANSIENT ANALYSIS 263
15.4 Measurements after AC, DC and Transient Analysis
15.4.1 .meas(ure)
The .meas or .measure statement (and its equivalent meas command, see Chapt. 17.5.39)
are used to analyze the output data of a tran, ac, or dc simulation. The command is executed
immediately after the simulation has finished.
15.4.2 batch versus interactive mode
.meas analysis may not be used in batch mode (-b command line option), if an output file
(rawfile) is given at the same time (-r rawfile command line option). In this batch mode
ngspice will write its simulation output data directly to the output file. The data is not kept in
memory, thus is no longer available for further analysis. This is made to allow a very large
output stream with only a relatively small memory usage. For .meas to be active you need to
run the batch mode with a .plot or .print command. A better alternative may be to start
ngspice in interactive mode.
If you need batch like operation, you may add a .control ... .endc section to the input
file:
Example:
*input file
...
. tran 1 ns 1000 ns
...
*********************************
.control
run
write outputfile data
.endc
*********************************
.end
and start ngspice in interactive mode, e.g. by running the command
ngspice inputfile .
.meas<ure> then prints its user-defined data analysis to the standard output. The analysis
includes propagation, delay, rise time, fall time, peak-to-peak voltage, minimum or maximum
voltage, the integral or derivative over a specified period and several other user defined values.
15.4.3 General remarks
The measure type {DC|AC|TRAN|SP} depends on the data that is to be evaluated, either origi-
nating from a dc analysis, an ac analysis, or a transient simulation. The type SP to analyze a
spectrum from the spec or fft commands is only available when executed in a meas command,
see 17.5.39.
264 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
result will be a vector containing the result of the measurement. trig_variable,targ_variable,
and out_variable are vectors stemming from the simulation, e.g. a voltage vector v(out).
VAL=val expects a real number val. It may be as well a parameter delimited by ” or {}
expanding to a real number.
TD=td and AT=time expect a time value if measure type is tran. For ac and sp AT will be a
frequency value, TD is ignored. For dc analysis AT is a voltage (or current), TD is ignored as
well.
CROSS=# requires an integer number #. CROSS=LAST is possible as well. The same is expected
by RISE and FALL.
Frequency and time values may start at 0 and extend to positive real numbers. Voltage (or
current) inputs for the independent (scale) axis in a dc analysis may start or end at arbitrary real
valued numbers.
Please note that not all of the .measure commands have been implemented.
15.4.4 Input
In the following lines you will get some explanation on the .measure commands. A simple
simulation file with two sines of different frequencies may serve as an example. The transient
simulation delivers time as the independent variable and two voltages as output (dependent
variables).
Input file:
File: simple - meas - tran .sp
* Simple .measure examples
* transient simulation of two sine
* signals with different frequencies
vac1 1 0 DC 0 sin (0 1 1k 0 0)
vac2 2 0 DC 0 sin (0 1.2 0.9k 0 0)
.tran 10u 5m
*
.measure tran ... $ for the different inputs see below!
*
.control
run
plot v(1) v(2)
.endc
.end
After displaying the general syntax of the .measure statement, some examples are posted,
referring to the input file given above.
15.4.5 Trig Targ
.measure according to general form 1 measures the difference in dc voltage, frequency or time
between two points selected from one or two output vectors. The current examples all are using
15.4. MEASUREMENTS AFTER AC, DC AND TRANSIENT ANALYSIS 265
transient simulation. Measurements for tran analysis start after a delay time td. If you run
other examples with ac simulation or spectrum analysis, time may be replaced by frequency,
after a dc simulation the independent variable may become a voltage or current.
General form 1:
.MEASURE {DC|AC|TRAN |SP} result TRIG trig_variable VAL =
val
+ <TD=td > <CROSS =# | CROSS = LAST > <RISE =# | RISE=LAST >
+ <FALL =# | FALL =LAST > <TRIG AT =time > TARG
targ_variable
+ VAL = val <TD=td > <CROSS =# | CROSS=LAST > <RISE =# |
+ RISE=LAST > <FALL =# | FALL=LAST > <TARG AT=time >
Measure statement example (for use in the input file given above):
.measure tran tdiff TRIG v(1) VAL=0.5 RISE=1 TARG v(1) VAL=0.5 RISE=2
measures the time difference between v(1) reaching 0.5 V for the first time on its first rising
slope (TRIG) versus reaching 0.5 V again on its second rising slope (TARG), i.e. it measures
the signal period.
Output:
tdiff = 1.000000e-003 targ= 1.083343e-003 trig= 8.334295e-005
Measure statement example:
.measure tran tdiff TRIG v(1) VAL=0.5 RISE=1 TARG v(1) VAL=0.5 RISE=3
measures the time difference between v(1) reaching 0.5 V for the first time on its rising slope
versus reaching 0.5 V on its rising slope for the third time (i.e. two periods).
Measure statement:
.measure tran tdiff TRIG v(1) VAL=0.5 RISE=1 TARG v(1) VAL=0.5 FALL=1
measures the time difference between v(1) reaching 0.5V for the first time on its rising slope
versus reaching 0.5 V on its first falling slope.
Measure statement:
.measure tran tdiff TRIG v(1) VAL=0 FALL=3 TARG v(2) VAL=0 FALL=3
measures the time difference between v(1) reaching 0V its third falling slope versus v(2) rea-
ching 0 V on its third falling slope.
Measure statement:
.measure tran tdiff TRIG v(1) VAL=-0.6 CROSS=1 TARG v(2) VAL=-0.8 CROSS=1
measures the time difference between v(1) crossing -0.6 V for the first time (any slope) versus
v(2) crossing -0.8 V for the first time (any slope).
Measure statement:
.measure tran tdiff TRIG AT=1m TARG v(2) VAL=-0.8 CROSS=3
measures the time difference between the time point 1ms versus the time when v(2) crosses -0.8
V for the third time (any slope).
266 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
15.4.6 Find ... When
The FIND and WHEN functions allow to measure any dependent or independent time, frequency,
or dc parameter, when two signals cross each other or a signal crosses a given value. Measure-
ments start after a delay TD and may be restricted to a range between FROM and TO.
General form 2:
.MEASURE {DC|AC|TRAN |SP} result WHEN out_variable = val
+ <TD=td > <FROM =val > <TO=val > <CROSS =# | CROSS =LAST >
+ <RISE =# | RISE = LAST > <FALL =# | FALL =LAST >
Measure statement:
.measure tran teval WHEN v(2)=0.7 CROSS=LAST
measures the time point when v(2) crosses 0.7 V for the last time (any slope).
General form 3:
.MEASURE {DC|AC|TRAN |SP} result
+ WHEN out_variable = out_variable2
+ <TD=td > <FROM =val > <TO=val > <CROSS =# | CROSS =LAST >
+ <RISE =# | RISE = LAST > <FALL =# | FALL =LAST >
Measure statement:
.measure tran teval WHEN v(2)=v(1) RISE=LAST
measures the time point when v(2) and v(1) are equal, v(2) rising for the last time.
General form 4:
.MEASURE {DC|AC|TRAN |SP} result FIND out_variable
+ WHEN out_variable2 =val <TD=td > <FROM =val > <TO=val >
+ <CROSS =# | CROSS =LAST > <RISE =# | RISE=LAST >
+ <FALL =# | FALL = LAST >
Measure statement:
.measure tran yeval FIND v(2) WHEN v(1)=-0.4 FALL=LAST
returns the dependent (y) variable drawn from v(2) at the time point when v(1) equals a value
of -0.4, v(1) falling for the last time.
General form 5:
.MEASURE {DC|AC|TRAN |SP} result FIND out_variable
+ WHEN out_variable2 = out_variable3 <TD =td >
+ <CROSS =# | CROSS = LAST >
+ <RISE =#| RISE =LAST > <FALL =#| FALL =LAST >
Measure statement:
.measure tran yeval FIND v(2) WHEN v(1)=v(3) FALL=2
15.4. MEASUREMENTS AFTER AC, DC AND TRANSIENT ANALYSIS 267
returns the dependent (y) variable drawn from v(2) at the time point when v(1) crosses v(3),
v(1) falling for the second time.
General form 6:
.MEASURE {DC|AC|TRAN |SP} result FIND out_variable AT =
val
Measure statement:
.measure tran yeval FIND v(2) AT=2m
returns the dependent (y) variable drawn from v(2) at the time point 2 ms (given by AT=time).
15.4.7 AVG|MIN|MAX|PP|RMS|MIN_AT|MAX_AT
General form 7:
.MEASURE {DC|AC|TRAN |SP} result
+ {AVG|MIN | MAX|PP|RMS | MIN_AT| MAX_AT }
+ out_variable <TD=td > <FROM =val > <TO =val >
Measure statements:
.measure tran ymax MAX v(2) from=2m to=3m
returns the maximum value of v(2) inside the time interval between 2 ms and 3 ms.
.measure tran tymax MAX_AT v(2) from=2m to=3m
returns the time point of the maximum value of v(2) inside the time interval between 2 ms and
3 ms.
.measure tran ypp PP v(1) from=2m to=4m
returns the peak to peak value of v(1) inside the time interval between 2 ms and 4 ms.
.measure tran yrms RMS v(1) from=2m to=4m
returns the root mean square value of v(1) inside the time interval between 2 ms and 4 ms.
.measure tran yavg AVG v(1) from=2m to=4m
returns the average value of v(1) inside the time interval between 2 ms and 4 ms.
15.4.8 Integ
General form 8:
.MEASURE {DC| AC| TRAN|SP} result INTEG <RAL > out_variable
+ <TD=td > <FROM =val > <TO=val >
Measure statement:
.measure tran yint INTEG v(2) from=2m to=3m
returns the area under v(2) inside the time interval between 2 ms and 3 ms.
268 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
15.4.9 param
General form 9:
.MEASURE {DC|AC|TRAN |SP} result param=’ expression ’
Measure statement:
.param fval=5
.measure tran yadd param=’fval + 7’
will evaluate the given expression fval + 7 and return the value 12.
’Expression’ is evaluated according to the rules given in Chapt. 2.8.5 during start up of ngspice.
It may contain parameters defined with the .param statement. It may also contain parameters
resulting from preceding .meas statements.
.param vout_diff=50u
...
.measure tran tdiff TRIG AT=1m TARG v(2) VAL=-0.8 CROSS=3
.meas tran bw_chk param=’(tdiff < vout_diff) ? 1 : 0’
will evaluate the given ternary function and return the value 1 in bw_chk, if tdiff measured is
smaller than parameter vout_diff.
The expression may not contain vectors like v(10), e.g. anything resulting directly from a
simulation. This may be handled with the following .meas command option.
15.4.10 par(’expression’)
The par(’expression’)option (15.6.6) allows to use algebraic expressions on the .measure
lines. Every out_variable may be replaced by par(’expression’) using the general forms 1. . . 9
described above. Internally par(’expression’) is substituted by a vector according to the rules
of the B source (Chapt. 5.1). A typical example of the general form is shown below:
General form 10:
.MEASURE {DC| TRAN|AC|SP} result
+ FIND par(’ expression ’) AT=val
The measure statement
.measure tran vtest find par(’(v(2)*v(1))’) AT=2.3m
returns the product of the two voltages at time point 2.3 ms.
Note that a B-source, and therefore the par(’...’) feature, operates on values of type complex
in AC analysis mode.
15.4. MEASUREMENTS AFTER AC, DC AND TRANSIENT ANALYSIS 269
15.4.11 Deriv
General form:
.MEASURE {DC|AC|TRAN |SP} result DERIV <ATIVE >
out_variable
+ AT= val
.MEASURE {DC|AC|TRAN |SP} result DERIV <ATIVE >
out_variable
+ WHEN out_variable2 = val <TD =td >
+ <CROSS =# | CROSS =LAST > <RISE =#| RISE=LAST >
+ <FALL =#| FALL =LAST >
.MEASURE {DC|AC|TRAN |SP} result DERIV <ATIVE >
out_variable
+ WHEN out_variable2 = out_variable3
+ <TD=td > <CROSS =# | CROSS = LAST >
+ <RISE =#| RISE =LAST > <FALL =#| FALL =LAST >
15.4.12 More examples
Some other examples, also showing the use of parameters, are given below. Corresponding
demonstration input files are distributed with ngspice in folder /examples/measure.
270 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
Other examples:
.meas tran inv_delay2 trig v(in) val =’vp/2’ td =1n fall
=1
+ targ v( out ) val =’ vp /2 ’ rise =1
.meas tran test_data1 trig AT = 1n targ v(out )
+ val =’ vp /2 ’ rise =3
. meas tran out_slew trig v( out ) val = ’0.2* vp ’ rise =2
+ targ v( out ) val = ’0.8* vp ’ rise =2
.meas tran delay_chk param =’( inv_delay < 100 ps) ? 1 :
0’
.meas tran skew when v(out)=0.6
.meas tran skew2 when v(out)= skew_meas
. meas tran skew3 when v( out )= skew_meas fall =2
.meas tran skew4 when v(out)= skew_meas fall= LAST
.meas tran skew5 FIND v(out) AT=2n
.meas tran v0_min min i(v0)
+ from =’ dfall ’ to=’ dfall+period ’
.meas tran v0_avg avg i(v0)
+ from =’ dfall ’ to=’ dfall+period ’
.meas tran v0_integ integ i(v0)
+ from =’ dfall ’ to=’ dfall+period ’
.meas tran v0_rms rms i(v0)
+ from =’ dfall ’ to=’ dfall+period ’
.meas dc is_at FIND i(vs) AT =1
. meas dc is_max max i( vs ) from =0 to =3.5
.meas dc vds_at when i(vs) =0.01
.meas ac vout_at FIND v( out) AT=1 MEG
.meas ac vout_atd FIND vdb ( out) AT =1 MEG
. meas ac vout_max max v( out ) from =1k to =10 MEG
.meas ac freq_at when v(out ) =0.1
.meas ac vout_diff trig v( out) val =0.1 rise =1 targ v(
out)
+ val =0.1 fall =1
.meas ac fixed_diff trig AT = 10k targ v(out)
+ val =0.1 rise =1
. meas ac vout_avg avg v( out ) from =10 k to =1 MEG
. meas ac vout_integ integ v( out ) from =20 k to =500 k
.meas ac freq_at2 when v(out)=0.1 fall=LAST
.meas ac bw_chk param =’( vout_diff < 100k) ? 1 : 0’
. meas ac vout_rms rms v( out) from =10 to =1G
15.5 Safe Operating Area (SOA) warning messages
By setting .option warn=1 the Safe Operation Area check algorithm is enabled. In this case
for .op,.dc and .tran analysis warning messages are issued if the branch voltages of devices
15.5. SAFE OPERATING AREA (SOA) WARNING MESSAGES 271
(Resistors, Capacitors, Diodes, BJTs and MOSFETs) exceed limits that are specified by model
parameters. All these parameters are positive with default value of infinity.
The check is executed after Newton-Raphson iteration is finished i.e. in transient analysis in
each time step. The user can specify an additional .option maxwarns (default: 5) to limit the
count of messages.
The output goes on default to stdout or alternatively to a file specified by command line option
--soa-log=filename.
15.5.1 Resistor and Capacitor SOA model parameters
1. Bv_max: if |Vr| or |Vc| exceed Bv_max, SOA warning is issued.
15.5.2 Diode SOA model parameter
1. Bv_max: if |Vj| exceeds Bv_max, SOA warning is issued.
2. Fv_max: if |Vf| exceeds Fv_max, SOA warning is issued.
15.5.3 BJT SOA model parameter
1. Vbe_max: if |Vbe| exceeds Vbe_max, SOA warning is issued.
2. Vbc_max: if |Vbc| exceeds Vbc_max, SOA warning is issued.
3. Vce_max: if |Vce| exceeds Vce_max, SOA warning is issued.
4. Vcs_max: if |Vcs| exceeds Vcs_max, SOA warning is issued.
15.5.4 MOS SOA model parameter
1. Vgs_max: if |Vgs| exceeds Vgs_max, SOA warning is issued.
2. Vgd_max: if |Vgd| exceeds Vgd_max, SOA warning is issued.
3. Vgb_max: if |Vgb| exceeds Vgb_max, SOA warning is issued.
4. Vds_max: if |Vds| exceeds Vds_max, SOA warning is issued.
5. Vbs_max: if |Vbs| exceeds Vbs_max, SOA warning is issued.
6. Vbd_max: if |Vbd| exceeds Vbd_max, SOA warning is issued.
272 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
15.6 Batch Output
The following commands .print (15.6.2), .plot (15.6.3) and .four (15.6.4) are valid only
if ngspice is started in batch mode (see 16.4.1), whereas .save and the equivalent .probe are
aknowledged in all operating modes.
If you start ngspice in batch mode using the -b command line option, the outputs of .print,
.plot, and .four are printed to the console output. You may use the output redirection of your
shell to direct this printout into a file (not available with MS Windows GUI). As an alternative
you may extend the ngspice command by specifying an output file:
ngspice -b -o output.log input.cir
If you however add the command line option -r to create a rawfile, .print and .plot are
ignored. If you want to involve the graphics plot output of ngspice, use the control mode
(16.4.3) instead of the -b batch mode option.
15.6.1 .SAVE: Name vector(s) to be saved in raw file
General form:
.save vector vector vector ...
Examples:
.save i(vin ) node1 v(node2 )
.save @m1[id] vsource #branch
.save all @m2 [ vdsat ]
The vectors listed on the .SAVE line are recorded in the rawfile for use later with ngspice or ng-
nutmeg (ngnutmeg is just the data-analysis half of ngspice, without the ability to simulate). The
standard vector names are accepted. Node voltages may be saved by giving the nodename or
v(nodename). Currents through an independent voltage source are given by i(sourcename)
or sourcename#branch. Internal device data are accepted as @dev[param].
If no .SAVE line is given, then the default set of vectors is saved (node voltages and voltage
source branch currents). If .SAVE lines are given, only those vectors specified are saved. For
more discussion on internal device data, e.g. @m1[id], see Appendix, Chapt. 31.1. If you want
to save internal data in addition to the default vector set, add the parameter all to the additional
vectors to be saved. If the command .save vm(out) is given, and you store the data in a raw-
file, only the original data v(out)are stored. The request for storing the magnitude is ignored,
because this may be added later during rawfile data evaluation with ngnutmeg or ngspice. See
also the section on the interactive command interpreter (Chapt. 17.5) for information on how to
use the rawfile.
15.6. BATCH OUTPUT 273
15.6.2 .PRINT Lines
General form:
.print prtype ov1 <ov2 ... ov8 >
Examples:
.print tran v(4) i(vin)
.print dc v(2) i( vsrc ) v(23 , 17)
.print ac vm (4, 2) vr (7) vp (8, 3)
The .print line defines the contents of a tabular listing of one to eight output variables. prtype
is the type of the analysis (DC,AC,TRAN,NOISE, or DISTO) for which the specified outputs are
desired. The form for voltage or current output variables is the same as given in the previous
section for the print command; Spice2 restricts the output variable to the following forms
(though this restriction is not enforced by ngspice):
V(N1<,N2>) specifies the voltage difference between nodes N1 and N2.
If N2 (and the preceding comma) is omitted, ground (0) is
assumed. See the print command in the previous section
for more details. For compatibility with SPICE2, the
following five additional values can be accessed for the ac
analysis by replacing the ‘V’ in V(N1,N2) with:
VR Real part
VI Imaginary part
VM Magnitude
VP Phase
VDB 20log10(magnitude)
I(VXXXXXXX) specifies the current flowing in the independent voltage
source named VXXXXXXX. Positive current flows from
the positive node, through the source, to the negative node.
(Not yet implemented: For the ac analysis, the
corresponding replacements for the letter Imay be made
in the same way as described for voltage outputs.)
Output variables for the noise and distortion analyses have a different general form from that of
the other analyses. There is no limit on the number of .print lines for each type of analysis.
The par(’expression’)option (15.6.6) allows to use algebraic expressions in the .print lines.
.width (15.6.7) selects the maximum number of characters per line.
15.6.3 .PLOT Lines
.plot creates a printer plot output.
274 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
General form:
.plot pltype ov1 <( plo1 , phi1 )> <ov2 <(plo2 , phi2 )> ... ov8 >
Examples:
.plot dc v(4) v (5) v(1)
.plot tran v(17, 5) (2, 5) i( vin) v(17) (1, 9)
.plot ac vm (5) vm(31 , 24) vdb (5) vp (5)
.plot disto hd2 hd3(R) sim2
.plot tran v(5, 3) v(4) (0, 5) v (7) (0, 10)
The .plot line defines the contents of one plot of from one to eight output variables. pltype is
the type of analysis (DC,AC,TRAN,NOISE, or DISTO) for which the specified outputs are desired.
The syntax for the oviis identical to that for the .print line and for the plot command in the
interactive mode.
The overlap of two or more traces on any plot is indicated by the letter ‘X’. When more than
one output variable appears on the same plot, the first variable specified is printed as well
as plotted. If a printout of all variables is desired, then a companion .print line should be
included. There is no limit on the number of .plot lines specified for each type of analysis.
The par(’expression’)option (15.6.6) allows to use algebraic expressions in the .plot lines.
15.6.4 .FOUR: Fourier Analysis of Transient Analysis Output
General form:
.four freq ov1 <ov2 ov3 ... >
Examples:
.four 100K v(5)
The .four (or Fourier) line controls whether ngspice performs a Fourier analysis as a part of
the transient analysis. freq is the fundamental frequency, and ov1 is the desired vector to
be analyzed. The Fourier analysis is performed over the interval <TSTOP-period, TSTOP>,
where TSTOP is the final time specified for the transient analysis, and period is one period of
the fundamental frequency. The dc component and the first nine harmonics are determined. For
maximum accuracy, TMAX (see the .tran line) should be set to period/100.0 (or less for very
high-Q circuits). The par(’expression’)option (15.6.6) allows to use algebraic expressions in
the .four lines.
15.6. BATCH OUTPUT 275
15.6.5 .PROBE: Name vector(s) to be saved in raw file
General form:
.probe vector <vector vector ...>
Examples:
.probe i(vin) input output
.probe @m1[ id]
Same as .SAVE (see Chapt. 15.6.1).
15.6.6 par(’expression’): Algebraic expressions for output
General form:
par(’ expression ’)
output=par (’ expression ’) $ not in .measure ac
Examples:
. four 1001 sq1 = par (’v (1)* v (1) ’)
. measure tran vtest find par (’( v(2)* v (1)) ’) AT =2.3 m
. print tran output = par (’ v(1)/ v (2) ’) v(1) v (2)
.plot dc v(1) diff=par (’(v(4) -v (2))/0.01 ’) out222
With the output lines .four, .plot, .print, .save and in .measure evaluation it is pos-
sible to add algebraic expressions for output, in addition to vectors. All of these output lines
accept par(’expression’), where expression is any expression valid for a B source (see Chapt.
5.1). Thus expression may contain predefined functions, numerical values, constants, simula-
tor output like v(n1) or i(vdb), parameters predefined by a .param statement, and the variables
hertz,temper, and time. Note that a B-source, and therefore the par(’...’) feature, ope-
rates on values of type complex in AC analysis mode.
Internally the expression is replaced by a generated voltage node that is the output of a B source,
one node, and the B source implementing par(’...’). Several par(’...’) are allowed in each line,
up to 99 per input file. The internal nodes are named pa_00 to pa_99. An error will occur if
the input file contains any of these reserved node names.
In .four, .plot, .print, .save, but not in .measure, an alternative syntax
output=par(’expression’)is possible. par(’expression’)may be used as described above.
output is the name of the new node to replace the expression. So output has to be unique and
a valid node name.
The syntax of output=par(expression)is strict, no spaces between par and (’, or between (
and ’are allowed, (’ and ’) both are required. Also there is not much error checking on your
input, if there is a typo, for example, an error may pop up at an unexpected place.
276 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
15.6.7 .width
Set the width of a print-out or plot with the following card:
.with out = 256
Parameter out yields the maximum number of characters plotted in a row, if printing in columns
or an ASCII-plot is selected.
15.7 Measuring current through device terminals
15.7.1 Adding a voltage source in series
Originally the ngspice matrix solver delivers node voltages and currents through independent
voltage sources. So to measure the currents through a resistor you may add a voltage source in
series with dc voltage 0.
Current measurement with series voltage source
*measure current through R1
V1 1 0 1
R1 1 0 5
R2 1 0 10
* will become
V1 1 0 1
R1 1 11 5
Vmess 11 0 dc 0
R2 1 0 10
15.7.2 Using option ’savecurrents’
Current measurement with series voltage source
*measure current through R1 and R2
V1 1 0 1
R1 1 0 5
R2 1 0 10
.options savecurrents
The option savecurrents will add .save lines (15.6.1) like
.save @r1[i]
.save @r2[i]
to your input file information read during circuit parsing. These newly created vectors contain
the terminal currents of the devices R1 and R2.
You will find information of the nomenclature in Chapt. 31, also how to plot these vectors. The
following devices are supported: M, J, Q, D, R, C, L, B, F, G, W, S, I (see 2.1.2). For M only
15.7. MEASURING CURRENT THROUGH DEVICE TERMINALS 277
MOSFET models MOS1 to MOS9 are included so far. Devices in subcircuits are supported as
well. Be careful when choosing this option in larger circuits, because 1 to 4 additional output
vectors are created per device and this may consume lots of memory.
278 CHAPTER 15. ANALYSES AND OUTPUT CONTROL (BATCH MODE)
Chapter 16
Starting ngspice
16.1 Introduction
Ngspice consists of the simulator and a front-end for data analysis and plotting. Input to the
simulator is a netlist file, including commands for circuit analysis and output control. Interactive
ngspice can plot data from a simulation on a PC or a workstation display.
Ngspice on Linux (and OSs like Cygwin, BCD, Solaris ...) uses the X Window System for
plotting (see Chapt. 18.3) if the environment variable DISPLAY is available. Otherwise, a con-
sole mode (non-graphical) interface is used. If you are using X on a workstation, the DISPLAY
variable should already be set; if you want to display graphics on a system different from the
one you are running ngspice or ngutmeg on, DISPLAY should be of the form machine:0.0. See
the appropriate documentation on the X Window System for more details.
The MS Windows versions of ngspice and ngnutmeg will have a native graphics interface (see
Chapt. 18.1).
The front-end may be run as a separate ‘stand-alone’ program under the name ngnutmeg. ng-
nutmeg is a subset of ngspice dedicated to data evaluation, still made available for historical
reasons. Ngnutmeg will read in the ‘raw’ data output file created by ngspice -r or by the write
command during an interactive ngspice session.
16.2 Where to obtain ngspice
The actual distribution of ngspice may be downloaded from the ngspice download web page.
The installation for Linux or MS Windows is described in the file INSTALL to be found in
the top level directory. You may also have a look at Chapt. 32 of this manual for compiling
instructions.
If you want to check out the source code that is actually under development, you may have a
look at the ngspice source code repository, which is stored using the Git Source Code Mana-
gement (SCM) tool. The Git repository may be browsed on the Git web page, also useful for
downloading individual files. You may however download (or clone) the complete repository
including all source code trees from the console window (Linux, CYGWIN or MSYS/MINGW)
by issuing the command (in a single line)
279
280 CHAPTER 16. STARTING NGSPICE
git clone git://ngspice.git.sourceforge.net/gitroot/ngspice/ngspice
You need to have Git installed, which is available for all three OSs. The whole source tree
is then available in <current directory>/ngspice. Compilation and local installation is again
described in INSTALL (or Chapt. 32). If you later want to update your files and download the
recent changes from sourceforge into your local repository, cd into the ngspice directory and
just type
git pull
git pull will deny to overwrite modified files in your working directory. To drop your local
changes first, you can run
git reset --hard
To learn more about git, which can be both powerful and difficult to master, please consult
http://git-scm.com/, especially: http://git-scm.com/documentation, which has pointers to docu-
mentation and tutorials.
16.3 Command line options for starting ngspice and ngnut-
meg
Command Synopsis:
ngspice [ -o logfile ] [ -r rawfile ] [ -b ] [ -i ] [ input files ]
ngnutmeg [ - ] [ datafile ... ]
Options are:
16.3. COMMAND LINE OPTIONS FOR STARTING NGSPICE AND NGNUTMEG 281
Option Long option Meaning
-Don’t try to load the default data file ("rawspice.raw") if no
other files are given (ngnutmeg only).
-n --no-spiceinit Don’t try to source the file .spiceinit upon start-up.
Normally ngspice and ngnutmeg try to find the file in the
current directory, and if it is not found then in the user’s
home directory (obsolete).
-t TERM --terminal=TERM The program is being run on a terminal with mfb name
term (obsolete).
-b --batch Run in batch mode. Ngspice reads the default input source
(e.g. keyboard) or reads the given input file and performs
the analyses specified; output is either Spice2-like
line-printer plots ("ascii plots") or a ngspice rawfile. See
the following section for details. Note that if the input
source is not a terminal (e.g. using the IO redirection
notation of "<") ngspice defaults to batch mode (-i
overrides). This option is valid for ngspice only.
-s --server Run in server mode. This is like batch mode, except that a
temporary rawfile is used and then written to the standard
output, preceded by a line with a single "@", after the
simulation is done. This mode is used by the ngspice
daemon. This option is valid for ngspice only.
Example for using pipes from the console window:
cat adder.cir|ngspice -s|more
-i --interactive Run in interactive mode. This is useful if the standard input
is not a terminal but interactive mode is desired. Command
completion is not available unless the standard input is a
terminal, however. This option is valid for ngspice only.
-r FILE --rawfile=FILE Use rawfile as the default file into which the results of the
simulation are saved. This option is valid for ngspice only.
-p --pipe Allow a program (e.g., xcircuit) to act as a GUI frontend
for ngspice through a pipe. Thus ngspice will assume that
the input pipe is a tty and allows to run in interactive mode.
-o FILE --output=FILE All logs generated during a batch run (-b) will be saved in
outfile.
-h --help A short help statement of the command line syntax.
-v --version Prints a version information.
-a --autorun Start simulation immediately, as if a control section
.control
run
.endc
had been added to the input file.
--soa-log=FILE output from Safe Operating Area (SOA) check
Further arguments to ngspice are taken to be ngspice input files, which are read and saved (if
running in batch mode then they are run immediately). Ngspice accepts Spice3 (and also most
Spice2) input files, and outputs ASCII plots, Fourier analyses, and node printouts as specified
in .plot,.four, and .print cards. If an out parameter is given on a .width card (15.6.7),
282 CHAPTER 16. STARTING NGSPICE
the effect is the same as set width = .... Since ngspice ASCII plots do not use multiple ranges,
however, if vectors together on a .plot card have different ranges they do not provide as much
information as they do in a scalable graphics plot.
For ngnutmeg, further arguments are taken to be data files in binary or ASCII raw file format
(generated with -r in batch mode or the write (see 17.5.88) command) that are loaded into ng-
nutmeg. If the file is in binary format, it may be only partially completed (useful for examining
output before the simulation is finished). One file may contain any number of data sets from
different analyses.
16.4 Starting options
16.4.1 Batch mode
Let’s take as an example the Four-Bit binary adder MOS circuit shown in Chapt. 21.6, stored
in a file adder-mos.cir. You may start the simulation immediately by calling
ngspice -b -r adder.raw -o adder.log adder-mos.cir
ngspice will start, simulate according to the .tran command and store the output data in a
rawfile adder.raw. Comments, warnings and infos go to log file adder.log. Commands for batch
mode operation are described in Chapt. 15.
16.4.2 Interactive mode
If you call
ngspice
ngspice will start, load spinit (16.5) and .spiceinit (16.6, if available), and then waits for your
manual input. Any of the commands described in 17.5 may be chosen, but many of them are
useful only after a circuit has been loaded by
ngspice 1 -> source adder-mos.cir
others require the simulation being done already (e.g. plot):
ngspice 2 ->run
ngspice 3 ->plot allv
If you call ngspice from the command line with a circuit file as parameter:
ngspice adder-mos.cir
ngspice will start, load the circuit file, parse the circuit (same circuit file as above, containing
only dot commands (see Chapt. 15) for analysis and output control). ngspice then just waits for
your input. You may start the simulation by issuing the run command. Following completion
of the simulation you may analyze the data by any of the commands given in Chapt. 17.5.
16.4. STARTING OPTIONS 283
16.4.3 Control mode (Interactive mode with control file or control section)
If you add the following control section to your input file adder-mos.cir, you may call
ngspice adder-mos.cir
from the command line and see ngspice starting, simulating and then plotting immediately.
Control section:
* ADDER - 4 BIT ALL - NAND - GATE BINARY ADDER
.control
unset askquit
save vcc # branch
run
plot vcc # branch
rusage all
.endc
Any suitable command listed in Chapt. 17.5 may be added to the control section, as well as
control structures described in Chapt. 17.6. Batch-like behavior may be obtained by changing
the control section to
Control section with batch-like behavior:
* ADDER - 4 BIT ALL - NAND - GATE BINARY ADDER
.control
unset askquit
save vcc # branch
run
write adder.raw vcc#branch
quit
.endc
If you put this control section into a file, say adder-start.sp, you may just add the line
.include adder-start.sp
to your input file adder-mos.cir to obtain the batch-like behavior. In the following example
the line .tran ... from the input file is overridden by the tran command given in the control
section.
Control section overriding the .tran command:
* ADDER - 4 BIT ALL - NAND - GATE BINARY ADDER
.control
unset askquit
save vcc # branch
tran 1n 500n
plot vcc # branch
rusage all
.endc
284 CHAPTER 16. STARTING NGSPICE
The commands within the .control section are executed in the order they are listed and only
after the circuit has been read in and parsed. If you want to have a command being executed
before circuit parsing, you may use the prefix pre_ (17.5.46) to the command.
A warning is due however: If your circuit file contains such a control section (.control ...
.endc), you should not start ngspice in batch mode (with -b as parameter). The outcome may
be unpredictable!
16.5 Standard configuration file spinit
At startup ngspice reads its configuration file spinit.spinit may be found in a path relative to
the location of the ngspice executable
..\share\ngspice\scripts. The path may be overridden by setting the environmental variable
SPICE_SCRIPTS to a path where spinit is located. Ngspice for Windows will additionally
search for spinit in the directory where ngspice.exe resides. If spinit is not found a warning
message is issued, but ngspice continues.
Standard spinit contents:
* Standard ngspice init file
alias exit quit
alias acct rusage all
** set the number of threads in openmp
** default ( if compiled with --enable -openmp ) is: 2
set num_threads =4
if $? sharedmode
unset interactive
unset moremode
else
set interactive
set x11lineararcs
end
strcmp __flag $program " ngspice "
if $__flag = 0
codemodel ../ lib /spice / spice2poly .cm
codemodel ../ lib /spice / analog .cm
codemodel ../ lib /spice / digital . cm
codemodel ../ lib /spice / xtradev . cm
codemodel ../ lib /spice / xtraevt . cm
codemodel ../ lib /spice / table .cm
end
unset __flag
spinit contains a script, made of commands from chapt. 17.5, that is run upon start up of
16.6. USER DEFINED CONFIGURATION FILE .SPICEINIT 285
ngspice. Aliases (name equivalences) can be set. The asterisk ‘*’ comments out a line. If
used by ngspice, spinit will then load the XSPICE code models from a path relative to the
current directory where the ngspice executable resides. You may also define absolute paths.
The compatibility mode of ngspice can be set in spinit with set ngbehavior=all.
If the standard path for the libraries (see standard spinit above or /usr/local/lib/spice un-
der CYGWIN and Linux) is not adequate, you can add the ./configure options --prefix=/usr
--libdir=/usr/lib64 to set the codemodel search path to /usr/lib64/spice. Besides the
standard lib only lib64 is acknowledged.
Special care has to be taken when using the ngspice shared library. If you apply ngspice.dll
under Windows OS, the standard is to use relative paths for the code models as shown above.
However, the path is relative to the calling program, not to the dll. This is fine when ngspice.dll
and the calling program reside in the same directory. If ngspice.dll is placed in a different
directory, please check chapt. 32.2.
The Linux shared library ... t.b.d.
16.6 User defined configuration file .spiceinit
In addition to spinit you may define a (personal) file .spiceinit and put it into the current di-
rectory or in your home directory. The typical search sequence for .spiceinit is: current di-
rectory, HOME (Linux) and then USERPROFILE (Windows). USERPROFILE is typically
C:\Users\<User name>. This file will be read in and executed after spinit, but before any
other input file is read. It may contain further scripts, set variables, or issue commands from
chapt.17.5 to override commands given in spinit. For example set filetype=ascii will
yield ASCII output in the output data file (rawfile), instead of the compact binary format that is
used by default. set ngdebug will yield a lot of additional debug output. Any other contents
of the script, e.g. plotting preferences, may be included here also. If the command line option
-n is used upon ngspice start up, this file will be ignored.
.spiceinit may contain:
* User defined ngspice init file
set filetype =ascii
*set ngdebug
set numthreads = 8
*set outputpath =C:\ Spice64 \out
16.7 Environmental variables
16.7.1 Ngspice specific variables
SPICE_LIB_DIR default: /usr/local/share/ngspice (Linux, CYGWIN), C:\Spice\share\ngspice
(Windows)
SPICE_EXEC_DIR default: /usr/local/bin (Linux, CYGWIN), C:\Spice\bin (Windows)
286 CHAPTER 16. STARTING NGSPICE
SPICE_BUGADDR default: http://ngspice.sourceforge.net/bugrep.html
Where to send bug reports on ngspice.
SPICE_EDITOR default: vi (Linux, CYGWIN), notepad.exe (MINGW, Visual Studio)
Set the editor called in the edit command. Always overrides the EDITOR env. variable.
SPICE_ASCIIRAWFILE default: 0
Format of the rawfile. 0 for binary, and 1 for ascii.
SPICE_NEWS default: $SPICE_LIB_DIR/news
A file that is copied verbatim to stdout when ngspice starts in interactive mode.
SPICE_HELP_DIR default: $SPICE_LIB_DIR/helpdir
Help directory, not used in Windows mode
SPICE_HOST default: empty string
Used in the rspice command (probably obsolete, to be documented)
SPICE_SCRIPTS default: $SPICE_LIB_DIR/scripts
In this directory the spinit file will be searched.
SPICE_PATH default: $SPICE_EXEC_DIR/ngspice
Used in the aspice command (probably obsolete, to be documented)
NGSPICE_MEAS_PRECISION default: 5
Sets the number of digits if output values are printed by the meas(ure) command.
SPICE_NO_DATASEG_CHECK default: undefined
If defined, will suppress memory resource info (probably obsolete, not used on Windows
or where the /proc information system is available.)
NGSPICE_INPUT_DIR default: undefined
If defined, using a valid directory name, will add the given directory to the search path
when looking for input files (*.cir,*.inc,*.lib).
16.7.2 Common environment variables
TERM LINES COLS DISPLAY HOME PATH EDITOR SHELL POSIXLY_CORRECT
16.8 Memory usage
Ngspice started with batch option (-b) and rawfile output (-r rawfile) will store all simulation
data immediately into the rawfile without keeping them in memory. Thus very large circuits
may be simulated, the memory requested upon ngspice start up will depend on the circuit size,
but will not increase during simulation.
If you start ngspice in interactive mode or interactively with control section, all data will be kept
in memory, to be available for later evaluation. A large circuit may outgrow even Gigabytes of
memory. The same may happen after a very long simulation run with many vectors and many
time steps to be stored. Issuing the save <nodes> command will help to reduce memory
requirements by saving only the data defined by the command. You may alos choose option
INTERP (15.1.4) to reduce memory usage.
16.9. SIMULATION TIME 287
16.9 Simulation time
Simulating large circuits may take an considerable amount of CPU time. If this is of importance,
you should compile ngspice with the flags for optimum speed, set during configuring ngspice
compilation. Under Linux, MINGW, and CYGWIN you should select the following option to
disable the debug mode, which slows down ngspice:
./configure --disable-debug
Adding --disable-debug will set the -O2 optimization flag for compiling and linking.
Under MS Visual Studio, you will have to select the release version, which includes optimiza-
tion for speed.
If you have selected XSPICE (see Chapt. 12 and II) as part of your compilation configuration
(by adding the option --enable-xspice to your ./configure command), the value of trtol
(see 15.1.4) is set internally to 1 (instead of default 7) for higher precision if XSPICE code
model ’A’ devices included in the circuit. This may double or even triple the CPU time needed
for any transient simulation, because the amount of time steps and thus iteration steps is more
than doubled. For MS Visual Studio compilation there is currently no simple way to exclude
XSPICE during compilation.
You may enforce higher speed during XSPICE usage by setting the variable xtrtol in your
.spiceinit initialization file or in the .control section in front of the tran command (via set
xtrtol=2 using the set command 17.5.59) and override the above trtol reduction. Beware
however of precision or convergence issues if you use XSPICE ’A’ devices, especially if xtrtol
is set to values larger than 2.
If your circuit comprises mostly of MOS transistors, and you have a multi-core processor at
hand, you may benefit from OpenMP parallel processing, as described next (16.10).
16.10 Ngspice on multi-core processors using OpenMP
16.10.1 Introduction
Today’s computers typically come with CPUs having more than one core. It will thus be useful
to enhance ngspice to make use of such multi-core processors.
Using circuits comprising mostly of transistors and e.g. the BSIM3 model, around 2/3 of the
CPU time is spent in evaluating the model equations (e.g. in the BSIM3Load() function). The
same happens with other advanced transistor models. Thus this function should be paralleled, if
possible. Resulting from that the parallel processing has to be within a dedicated device model.
Interestingly solving the matrix takes only about 10% of the CPU time, so paralleling the matrix
solver is of secondary interest here!
A recent publication [1] has described a way to exactly do that using OpenMP, which is available
on many platforms and is easy to use, especially if you want to parallel processing of a for-loop.
To explain the implemented approach BSIM3 version 3.3.0 model was chosen, located in the
BSIM3 directory, as the first example. The BSIM3load() function in b3ld.c contains two nested
for-loops using linked lists (models and instances, e.g. individual transistors). Unfortunately
288 CHAPTER 16. STARTING NGSPICE
Table 16.1: OpenMP performance
Threads CPU time [s] CPU time [s]
Windows Linux
1 (standard) 167 165
1 (OpenMP) 174 167
2 110 110
3 95 94-120
4 83 107
6 94 90
8 93 91
OpenMP requires a loop with an integer index. So in file B3set.c an array is defined, filled with
pointers to all instances of BSIM3 and stored in model->BSIM3InstanceArray.
BSIM3load() is now a wrapper function, calling the for-loop, which runs through functions
BSIM3LoadOMP(), once per instance. Inside BSIM3LoadOMP() the model equations are cal-
culated.
Typically need it is needed to synchronize the activities, in that storing the results into the
matrix has to be guarded. The trick offered by the authors now is that the storage is moved out
of the BSIM3LoadOMP() function. Inside BSIM3LoadOMP() the updated data are stored in
extra locations locally per instance, defined in bsim3def.h. Only after the complete for-loop
is exercised, the update to the matrix is done in an extra function BSIM3LoadRhsMat() in the
main thread after the paralleled loop. No extra synchronization is required.
Then the thread programming needed is only a single line!!
#pragma omp parallel for
introducing the for-loop over the device instances.
This of course is made possible only thanks to the OpenMP guys and the clever trick on no
synchronization introduced by the above cited authors.
The time-measuring function getrusage() used with Linux or Cygwin to determine the CPU
time usage (with the rusage option enabled) counts tics from every core, adds them up, and
thus reports a CPU time value enlarged by a factor of 8 if 8 threads have been chosen. So now
ngspice is forced to use ftime for time measuring if OpenMP is selected.
16.10.2 Some results
Some results on an inverter chain with 627 CMOS inverters, running for 200ns, compiled with
Visual Studio professional 2008 on Windows 7 (full optimization) or gcc 4.4, SUSE Linux 11.2,
-O2, on a i7 860 machine with four real cores (and 4 virtuals using hyperthreading) are shown
in table 16.1.
So we see a ngspice speed up of nearly a factor of two! Even on an older notebook with a dual
core processor, more than 1.5x improvement using two threads was attained. Similar results are
to be expected from BSIM4.
16.11. SERVER MODE OPTION -S 289
16.10.3 Usage
To state it clearly: OpenMP is installed inside the model equations of a particular model. So for
the moment it is available only in BSIM3 version 3.3.0, not in version 3.2.4 nor in any other
BSIM3 model, in BSIM4 versions 4.6.5 or 4.8, not in any other BSIM4 model, and in B4SOI,
version 4.3.1, not in any other SOI model. Older parameter files of version 4.6.x (x any number
up to 5) are accepted, you have to check for compatibility.
Under Linux you may run
./autogen.sh
./configure ... --enable-openmp
make install
The same has been tested under MS Windows with CYGWIN and MINGW as well and deli-
vers similar results.
Under MS Windows with Visual Studio Professional you have to place an additional prepro-
cessor flag USE_OMP, and then enable /openmp. Visual Studio Express allone is not sufficient
due to lack of OpenMP support. But OpenMP is provided after installation of the Microsoft
SDK version 7.1. Even Visual Studio Professional lacks debugging support for OpenMP.
The number of threads has to be set manually by placing
set num_threads=4
into spinit or .spiceinit or in the control section of the SPICE input file. If OpenMP is enabled,
but num_threads not set, a default value num_threads=2 is set internally.
If you run a circuit, please keep in mind to select BSIM3 (levels 8, 49) version 3.3.0 (11.2.9),
by placing this version number into your parameter files, BSIM4 (levels 14, 54) version 4.6.5
or 4.8 (11.2.10), or B4SOI (levels 10, 58) version 4.3.1 (11.2.12).
If you run ./configure without --enable-openmp (or without USE_OMP preprocessor flag un-
der MS Windows), you will get the standard, not paralleled BSIM3 and BSIM4 model, as has
been available from Berkeley. If OpenMP is selected and the number of threads set to 1, there
will be only a very slight CPU time disadvantage (typ. 3%) compared to the standard, non
OpenMP build.
16.10.4 Literature
[1] R.K. Perng, T.-H. Weng, and K.-C. Li: "On Performance Enhancement of Circuit Simulation
Using Multithreaded Techniques", IEEE International Conference on Computational Science
and Engineering, 2009, pp. 158-165
16.11 Server mode option -s
A program may write the SPICE input to the console. This output is redirected to ngspice via
‘|’. ngspice called with the -s option writes its output to the console, which again is redirected
to a receiving program by ‘|’. In the following simple example cat reads the input file and
290 CHAPTER 16. STARTING NGSPICE
prints it content to the console, which is redirected to ngspice by a first pipe, ngspice transfers
its output (similar to a raw file, see below) to less via another pipe.
Example command line:
cat input .cir| ngspice -s| less
Under MS Windows you will need to compile ngspice as a console application (see Chapt.
32.2.5) for this server mode usage.
Example input file:
test -s
v1 1 0 1
r1 1 0 2k
.options filetype =ascii
.save i(v1)
.dc v1 -1 1 0.5
.end
If you start ngspice console with
ngspice -s
you may type in the above circuit line by line (not to forget the first line, which is a title and
will be ignored). If you close your input with ctrl Z, and return, you will get the following
output (this is valid for MINGW only) on the console, like a raw file:
Circuit: test -s
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
Title: test -s
Date: Sun Jan 15 18:57:13 2012
Plotname: DC transfer characteristic
Flags: real
No. Variables: 2
No. Points: 0
Variables:
No. of Data Columns : 2
0 v(v-sweep) voltage
1 i(v1) current
Values:
0 -1.000000000000000e+000
5.000000000000000e-004
1 -5.000000000000000e-001
2.500000000000000e-004
2 0.000000000000000e+000
0.000000000000000e+000
16.12. NGSPICE CONTROL VIA INPUT, OUTPUT FIFOS 291
3 5.000000000000000e-001
-2.500000000000000e-004
4 1.000000000000000e+000
-5.000000000000000e-004
@@@ 122 5
The number 5of the last line @@@ 122 5 shows the number of data points, which is missing in
the above line No. Points: 0 because at the time of writing to the console it has not yet
been available.
ctrl Z is not usable here in Linux, a patch to install ctrl D instead is being evaluated.
16.12 Ngspice control via input, output fifos
The following bash script (under Linux)
- launches ngspice in another thread.
- writes some commands in ngspice input
- reads the output and prints them on the console.
292 CHAPTER 16. STARTING NGSPICE
Example:
#!/ usr /bin /env bash
NGSPICE_COMMAND =" ngspice "
rm input.fifo
rm output. fifo
mkfifo input . fifo
mkfifo output . fifo
$NGSPICE_COMMAND -p -i < input . fifo >output . fifo &
exec 3> input .fifo
echo "I can write to input .fifo"
echo "Start processing ..."
echo ""
echo " source circuit .cir " >&3
echo " unset askquit " >&3
echo "set nobreak " >&3
echo " tran 0.01 ms 0.1 ms " >&3
echo " print n0" >&3
echo "quit " >&3
echo "Try to open output.fifo ..."
exec 4< output .fifo
echo "I can read from output.fifo "
echo " Ready to read ..."
while read output
do
echo $output
done <&4
exec 3>&-
exec 4>&-
echo "End processing "
The input file for SPICE is:
16.13. COMPATIBILITY 293
Circuit.cir:
* Circuit.cir
V1 n0 0 SIN (0 10 1 kHz)
C1 n1 n0 3.3 nF
R1 0 n1 1k
.end
16.13 Compatibility
ngspice is a direct derivative of spice3f5 from UC Berkeley and thus inherits all of the com-
mands available in its predecessor. Thanks to the open source policy of UCB (original spice3
from 1994 is still available here), several commercial variants have sprung off, either being more
dedicated to IC design or more concentrating on simulating discrete and board level electronics.
None of the commercial and almost none of the freely downloadable SPICE providers publishes
the source code. All of them have proceeded with the development, by adding functionality, or
by adding a more dedicated user interface. Some have kept the original SPICE syntax for their
netlist description, others have quickly changed some if not many of the commands, functions
and procedures. Thus it is difficult, if not impossible, to offer a simulator that acknowledges
all of these netlist dialects. ngspice includes some features that enhance compatibility that are
included automatically. This selection may be controlled to some extend by setting the com-
patibility mode. Others may be invoked by the user by small additions to the netlist input file.
Some of them are listed in this chapter, some will be integrated into ngspice at a later stage,
others will be added if they are reported by users.
16.13.1 Compatibility mode
The variable (17.7) ngbehavior sets the compatibility mode. ’all’ is set as the default value.
’spice3’ as invoked by the command
set ngbehavior=spice3
in spinit or .spiceinit will disable some of the advanced ngspice features. ’ps’ will enable
including a library by a simple .lib <lib_filename> statement that is not compatible to the
more comfortable library handling described in Chapt. 2.7.
16.13.2 Missing functions
You may add one or more function definitions to your input file, as listed below.
.func LIMIT(x,a,b) {min(max(x, a), b)}
.func PWR(x,a) {abs(x) ** a}
.func PWRS(x,a) {sgn(x) * PWR(x,a)}
.func stp(x) {u(x)}
294 CHAPTER 16. STARTING NGSPICE
16.13.3 Devices
16.13.3.1 E Source with LAPLACE
see Chapt. 5.2.5.
16.13.3.2 VSwitch
The VSwitch
S123110SW
.MODEL SW VSWITCH(VON=5V VOFF=0V RON=0.1 ROFF=100K)
may become
a1 %v(11) %gd(2 3) sw
.MODEL SW aswitch(cntl_off=0.0 cntl_on=5.0 r_off=1e5
+ r_on=0.1 log=TRUE)
The XSPICE option has to be enabled.
16.13.4 Controls and commands
16.13.4.1 .lib
The ngspice .lib command (see 2.7) requires two parameters, a file name followed by a library
name. If no library name is given, the line
.lib filename
should be replaced by
.inc filename
Alternatively, the compatibility mode (16.13.1) may be set to ’ps’.
16.13.4.2 .step
Repeated analysis in ngspice if offered by a short script inside of a .control section (see
Chapt. 17.8.7) added to the input file. A simple application (multiple dc sweeps) is shown
below.
16.14. TESTS 295
Input file with parameter sweep
parameter sweep
* resistive divider , R1 swept from start_r to stop_r
* replaces .STEP R1 1k 10k 1k
R1 1 2 1k
R2 2 0 1k
VDD 1 0 DC 1
.dc VDD 0 1 .1
.control
let start_r = 1k
let stop_r = 10k
let delta_r = 1k
let r_act = start_r
* loop
while r_act le stop_r
alter r1 r_act
run
write dc - sweep . out v (2)
set appendwrite
let r_act = r_act + delta_r
end
plot dc1.v(2) dc2.v(2) dc3.v(2) dc4.v(2) dc5.v(2)
+ dc6 .v (2) dc7 .v (2) dc8 .v (2) dc9 .v (2) dc10 .v (2)
.endc
.end
16.14 Tests
The ngspice distribution is accompanied by a suite of test input and output files, located in the
directory ngspice/tests. Originally this suite was meant to see if ngspice with all models was
made and installed properly. It is started by
$ make check
from within your compilation and development shell. A sequence of simulations is thus started,
its outputs compared to given output files by comparisons string by string. This feature is
momentarily used only to check for the BSIM3 model (11.2.9) and the XSPICE extension (12).
Several other input files located in directory ngspice/tests may serve as light-weight examples
for invoking devices and simple circuits.
Today’s very complex device models (BSIM4 (see 11.2.10), HiSIM (see 11.2.14) and others)
require a different strategy for verification. Under development for ngspice is the CMC Regres-
sion test by Colin McAndrew, which accompanies every new model. These tests cover a large
296 CHAPTER 16. STARTING NGSPICE
range of different DC, AC and noise simulations with different geometry ranges and operating
conditions and are more meaningful the transient simulations with their step size dependencies.
A major advantage is the scalability of the diff comparisons, which check for equality within a
given tolerance. A set of Perl modules cares for input, output and comparisons of the models.
Currently BSIM3, BSIM4, BSIMSOI4, HiSIM, and HiSIM_HV models implement the new
test. You may invoke it by running the command given above or by
$ make -i check 2>&1 | tee results
-i will make make to ignore any errors, tee will provide console output as well as printing to
file ’results’. Be aware that under MS Windows you will need the console binary (see 32.2.5)
to run the CMC tests, and you have to have Perl installed!
16.15 Reporting bugs and errors
Ngspice is a complex piece of software. The source code contains over 1500 files. Various
models and simulation procedures are provided, some of them not used and tested intensively.
Therefore errors may be found, some still evolving from the original spice3f5 code, others
introduced during the ongoing code enhancements.
If you happen to experience an error during the usage of ngspice, please send a report to the
development team. Ngspice is hosted on sourceforge, the preferred place to post a bug report is
the ngspice bug tracker. We would prefer to have your bug tested against the actual source code
available at Git, but of course a report using the most recent ngspice release is welcome! Please
provide the following information with your report:
Ngspice version
Operating system
Small input file to reproduce the bug
Actual output versus the expected output
Chapter 17
Interactive Interpreter
17.1 Introduction
The simulation flow in ngspice (input, simulation, output) may be controlled by dot commands
(see Chapt. 15 and 16.4.1) in batch mode. There is, however, a much more powerful control
scheme available in ngspice, traditionally coined ‘Interactive Interpreter’, but being much more
than just that. In fact there are several ways to use this feature, truly interactively by typing
commands to the input, but also running command sequences as scripts or as part of your input
deck in a quasi batch mode.
You may type in expressions, functions (17.2) or commands (17.5) into the input console to
elaborate on data already achieved from the interactive simulation session.
Sequences of commands, functions and control structures (17.6) may be assembled as a script
(17.8) into a file, and then activated by just typing the file name into the console input of an
interactive ngspice session.
Finally, and most useful, is it to add a script to the input file, in addition the the netlist and dot
commands. This is achieved by enclosing the script into .control ... .endc (see 16.4.3,
and 17.8.7 for an example). This feature enables a wealth of control options. You may set
internal (17.7) and other variables, start a simulation, evaluate the simulation output, start a new
simulation based on these data, and finally make use of many options for outputting the data
(graphically or into output files).
Historical note: The final releases of Berkeley Spice introduced a command shell and scripting
possibilities. The former releases were not interactive. The choice for the scripting language
was an early version of ‘csh’, the C-shell, which was en vogue back then as an improvement
over the ubiquitous Bourne Shell. Berkely Spice incorporated a modified csh source code that,
instead of invoking the unix ‘exec’ system call, executed internal SPICE C subroutines. Apart
from bug fixes, this is still how ngspice works.
The csh-like scripting language is active in .control sections. It works on ‘strings’, and does
string substitution of ‘environment’ variables. You see the csh at work in ngspice with set foo
= "bar"; set baz = "bar$foo", and in if,repeat,for, ... constructs. However, ngspice
processes mainly numerical data, and support for this was not available in the c-sh implementa-
tion. Therefore, Berkeley implemented an additional type of variables, with different syntax, to
access double and complex double vectors (possibly of length 1). This new variable type is mo-
dified with let, and can be used without special syntax in places where a numerical expression
297
298 CHAPTER 17. INTERACTIVE INTERPRETER
is expected: let bar = 4 * 5; let zoo = bar * 4 works. Unfortunately, occasionally
one has to cross the boundary between the numeric and the string domain. For this purpose the
$& construct is available – it queries a variable in the numerical let domain, and expands it to
a c-sh string denoting the value. This lets you do do something like set another = "this
is $&bar". It is important to remember that set can only operate on (c-sh) strings, and that
let operates only on numeric data. Convert from numeric to string with $&, and from string to
numeric with $.
17.2 Expressions, Functions, and Constants
Ngspice and ngnutmeg store data in the form of vectors: time, voltage, etc. Each vector has a
type, and vectors can be operated on and combined algebraically in ways consistent with their
types. Vectors are normally created as the output of a simulation, or when a data file (output raw
file) is read in again (ngspice, ngnutmeg, see the load command 17.5.38), or when the initial
data-file is loaded directly into ngnutmeg. They can also be created with the let command
817.5.35).
An expression is an algebraic formula involving vectors and scalars (a scalar is a vector of
length 1) and the following operations:
+ - * / ^ % ,
% is the modulo operator, and the comma operator has two meanings: if it is present in the
argument list of a user definable function, it serves to separate the arguments. Otherwise, the
term x,yis synonymous with x + j(y). Also available are the logical operations & (and),
| (or), ! (not), and the relational operations <, >, >=, <=, =, and <> (not equal). If used in an
algebraic expression they work like they would in C, producing values of 0 or 1. The relational
operators have the following synonyms:
Operator Synonym
gt >
lt <
ge >=
le <=
ne <>
and &
or |
not !
eq =
The operators are useful when < and > might be confused with the internal IO redirection (see
17.4, which is almost always happening). It is however safe to use < and > with the define
command (17.5.14).
The following functions are available:
17.2. EXPRESSIONS, FUNCTIONS, AND CONSTANTS 299
Name Function
mag(vector) Magnitude of vector (same as abs(vector)).
ph(vector) Phase of vector.
cph(vector) Phase of vector. Continuous values, no discontinuity at ±π.
unwrap(vector) Phase of vector. Continuous values, no discontinuity at ±π.
Real phase vector in degrees as input.
j(vector) i(sqrt(-1)) times vector.
real(vector The real component of vector.
imag(vector) The imaginary part of vector.
db(vector) 20 log10(mag(vector)).
log10(vector) The logarithm (base 10) of vector.
ln(vector) The natural logarithm (base e) of vector.
exp(vector) e to the vector power.
abs(vector) The absolute value of vector (same as mag).
sqrt(vector) The square root of vector.
sin(vector) The sine of vector.
cos(vector) The cosine of vector.
tan(vector) The tangent of vector.
atan(vector) The inverse tangent of vector.
sinh(vector) The hyperbolic sine of vector.
cosh(vector) The hyperbolic cosine of vector.
tanh(vector) The hyperbolic tangent of vector.
floor(vector) Largest integer that is less than or equal to vector.
ceil(vector) Smallest integer that is greater than or equal to vector.
norm(vector) The vector normalized to 1 (i.e, the largest magnitude of
any component is 1).
mean(vector) The result is a scalar (a length 1 vector) that is the mean of
the elements of vector (elements values added, divided by
number of elements).
avg(vector) The average of a vector.
Returns a vector where each element is the mean of the
preceding elements of the input vector (including the
actual element).
stddev(vector) The result is a scalar (a length 1 vector) that is the standard
deviation of the elements of vector .
group_delay(vector) Calculates the group delay -dphase[rad]/dω[rad/s]. Input is
the complex vector of a system transfer function versus
frequency, resembling damping and phase per frequency
value. Output is a vector of group delay values (real values
of delay times) versus frequency.
vector(number) The result is a vector of length number, with elements 0, 1,
... number - 1. If number is a vector then just the first
element is taken, and if it isn’t an integer then the floor of
the magnitude is used.
unitvec(number) The result is a vector of length number, all elements having
a value 1.
300 CHAPTER 17. INTERACTIVE INTERPRETER
Name Function
length(vector) The length of vector.
interpolate(plot.vector) The result of interpolating the named vector onto the scale
of the current plot. This function uses the variable
polydegree to determine the degree of interpolation.
deriv(vector) Calculates the derivative of the given vector. This uses
numeric differentiation by interpolating a polynomial and
may not produce satisfactory results (particularly with
iterated differentiation). The implementation only
calculates the derivative with respect to the real component
of that vector’s scale.
vecd(vector) Compute the differential of a vector.
vecmin(vector) Returns the value of the vector element with minimum
value. Same as minimum.
minimum(vector) Returns the value of the vector element with minimum
value. Same as vecmin.
vecmax(vector) Returns the value of the vector element with maximum
value. Same as maximum.
maximum(vector) Returns the value of the vector element with maximum
value. Same as vecmax.
fft(vector) fast fourier transform (17.5.26)
ifft(vector) inverse fast fourier transform (17.5.26)
sortorder(vector) Returns a vector with the positions of the elements in a real
vector after they have been sorted into increasing order
using a stable method (qsort).
timer(vector) Returns CPU-time minus the value of the first vector
element.
clock(vector) Returns wall-time minus the value of the first vector
element.
Several functions offering statistical procedures are listed in the following table:
17.2. EXPRESSIONS, FUNCTIONS, AND CONSTANTS 301
Name Function
rnd(vector) A vector with each component a random integer between 0
and the absolute value of the input vector’s corresponding
integer element value.
sgauss(vector) Returns a vector of random numbers drawn from a
Gaussian distribution (real value, mean = 0 , standard
deviation = 1). The length of the vector returned is
determined by the input vector. The contents of the input
vector will not be used. A call to sgauss(0) will return a
single value of a random number as a vector of length 1..
sunif(vector) Returns a vector of random real numbers uniformly
distributed in the interval [-1 .. 1[. The length of the vector
returned is determined by the input vector. The contents of
the input vector will not be used. A call to sunif(0) will
return a single value of a random number as a vector of
length 1.
poisson(vector) Returns a vector with its elements being integers drawn
from a Poisson distribution. The elements of the input
vector (real numbers) are the expected numbers λ.
Complex vectors are allowed, real and imaginary values
are treated separately.
exponential(vector) Returns a vector with its elements (real numbers) drawn
from an exponential distribution. The elements of the input
vector are the respective mean values (real numbers).
Complex vectors are allowed, real and imaginary values
are treated separately.
An input vector may be either the name of a vector already defined or a floating-point number
(a scalar). A scalar will result in an output vector of length 1. A number may be written in
any format acceptable to ngspice, such as 14.6Meg or -1.231e-4. Note that you can either use
scientific notation or one of the abbreviations like MEG or G, but not both. As with ngspice, a
number may have trailing alphabetic characters.
The notation expr [num] denotes the num’th element of expr. For multi-dimensional vectors,
a vector of one less dimension is returned. Also for multi-dimensional vectors, the notation
expr[m][n] will return the nth element of the mth subvector. To get a subrange of a vector, use
the form expr[lower, upper]. To reference vectors in a plot that is not the current plot (see the
setplot command, below), the notation plotname.vecname can be used. Either a plotname or
a vector name may be the wildcard all. If the plotname is all, matching vectors from all plots
are specified, and if the vector name is all, all vectors in the specified plots are referenced. Note
that you may not use binary operations on expressions involving wildcards - it is not obvious
what all + all should denote, for instance. Thus some (contrived) examples of expressions are:
302 CHAPTER 17. INTERACTIVE INTERPRETER
Expressions examples:
cos( TIME ) + db(v(3))
sin(cos ( log ([1 2 3 4 5 6 7 8 9 10])))
TIME * rnd(v(9)) - 15 * cos (vin# branch ) ^ [7.9 e5 8]
not (( ac3 . FREQ [32] & tran1 . TIME [10]) gt 3)
(sunif (0) ge 0) ? 1.0 : 2.0
mag(fft (v (18)))
Vector names in ngspice may look like @dname[param], where dname is either the name of
a device instance or of a device model. The vector contains the value of the parameter of the
device or model. See Appendix, Chapt. 31 for details of which parameters are available. The
returned value is a vector of length 1. Please note that finding the value of device and device
model parameters can also be done with the show command (e.g. show v1 : dc).
There are a number of pre-defined constants in ngspice, which you may use by their name. They
are stored in plot (17.3)const and are listed in the table below:
Name Description Value
pi π3.14159...
ee(the base of natural logarithms) 2.71828...
cc(the speed of light) 299,792,500 m
/sec
i i (the square root of -1) √−1
kelvin (absolute zero in centigrade) -273.15◦C
echarge q (the charge of an electron) 1.60219e-19 C
boltz k (Boltzmann’s constant) 1.38062e-23J/K
planck h (Planck’s constant) 6.62620e-34
yes boolean 1
no boolean 0
TRUE boolean 1
FALSE boolean 0
These constants are all given in MKS units. If you define another variable with a name that
conflicts with one of these then it takes precedence.
Additional constants may be generated during circuit setup (see .csparam,2.10).
17.3 Plots
The output vectors of any analysis are stored in plots, a traditional SPICE notion. A plot is a
group of vectors. A first tran command will generate several vectors within a plot tran1. A
subsequent tran command will store their vectors in tran2. Then a linearize command will
linearize all vectors from tran2 and store them in tran3, which then becomes the current plot. A
fft will generate a plot spec1, again now the current plot. The display command always will
show all vectors in the current plot. Echo $plots followed by Return lists all plots generated
so far.Setplot followed by Return will show all plots and ask for a (new) plot to become
current. A simple Return will end the command. Setplot name will change the current plot
to ’name’ (e.g. setplot tran2 will make tran2 the current plot). A sequence name.vector
may be used to access the vector from a foreign plot.
17.4. COMMAND INTERPRETATION 303
You may generate plots by yourself: setplot new will generate a new plot named unknown1,
set curplottitle=”a new plot” will set a title, set curplotname=myplot will set its
name as a short description, set curplotdate=”Sat Aug 28 10:49:42 2010” will set its
date. Note that strings with spaces have to be given with double quotes.
Of course the notion ’plot’ will be used by this manual also in its more common meaning,
denoting a graphics plot or being a plot command. Be careful to get the correct meaning.
17.4 Command Interpretation
17.4.1 On the console
On the ngspice console window (or into the Windows GUI) you may directly type in any com-
mand from 17.5. Within a command sequence Input/output redirection is available (see Chapt.
17.8.8 for an example) - the symbols >,>>,>&,>>&, and <have the same effects as in the
C-shell. This I/O-redirection is internal to ngspice commands, and should not be mixed up with
the ‘external’ I/O-redirection offered by the usual shells (Linux, MSYS etc.), see 17.5.64. You
may type multiple commands on one line, separated by semicolons.
17.4.2 Scripts
If a word is typed as a command, and there is no built-in command with that name, the directo-
ries in the sourcepath list are searched in order for a file with the name given by the word. If
it is found, it is read in as a command file (as if it were sourced). Before it is read, however, the
variables argc and argv are set to the number of words following the file-name on the com-
mand line, and a list of those words respectively. After the file is finished, these variables are
unset. Note that if a command file calls another, it must save its argv and argc since they are
altered. Also, command files may not be re-entrant since there are no local variables. Of course,
the procedures may explicitly manipulate a stack.... This way one can write scripts analogous
to shell scripts for ngnutmeg and ngspice.
Note that for the script to work with ngspice, it must begin with a blank line (or whatever else,
since it is thrown away) and then a line with .control on it. This is an unfortunate result
of the source command being used for both circuit input and command file execution. Note
also that this allows the user to merely type the name of a circuit file as a command and it is
automatically run. The commands are executed immediately, without running any analyses that
may be specified in the circuit (to execute the analyses before the script executes, include a run
command in the script).
There are various command scripts installed in /usr/local/lib/spice/scripts (or whate-
ver the path is on your machine), and the default sourcepath includes this directory, so you
can use these command files (almost) like built-in commands.
17.4.3 Add-on to circuit file
The problably most common way to invoke the commands described in the following Chapt.
17.5 is to add a .control ... .endc section to the circuit input file (see 16.4.3).
304 CHAPTER 17. INTERACTIVE INTERPRETER
Example:
.control
pre_set strict_errorhandling
unset ngdebug
*save outputs and specials
save x1 .x1.x1 .7 V(9) V(10) V (11) V(12) V (13)
run
display
* plot the inputs , use offset to plot on top of each other
plot v(1) v(2)+4 v(3)+8 v (4)+12 v(5)+16 v (6)+20 v (7)+24 v (8)+28
* plot the outputs , use offset to plot on top of each other
plot v(9) v(10)+4 v (11)+8 v (12)+12 v (13)+16
.endc
17.5 Commands
Commands marked with a * are only available in ngspice, not in ngnutmeg.
17.5.1 Ac*: Perform an AC, small-signal frequency response analysis
General Form:
ac ( DEC | OCT | LIN ) N Fstart Fstop
Do an small signal ac analysis (see also Chapt. 15.3.1) over the specified frequency range.
DEC decade variation, and Nis the number of points per decade.
OCT stands for octave variation, and Nis the number of points per octave.
LIN stands for linear variation, and Nis the number of points.
fstart is the starting frequency, and fstop is the final frequency.
Note that in order for this analysis to be meaningful, at least one independent source must have
been specified with an ac value.
In this ac analysis all non-linear devices are linearized around their actual dc operating point.
All Ls and Cs get their imaginary value, depending on the actual frequency step. Each output
vector will be calculated relative to the input voltage (current) given by the ac value (Iin equals
to 1 in the example below). The resulting node voltages (and branch currents) are complex
vectors. Therefore you have to be careful using the plot command.
17.5. COMMANDS 305
Example:
* AC test
Iin 1 0 AC 1
R1 1 2 100
L1 2 0 1
.control
AC LIN 101 10 10K
plot v(2) $ real part !
plot mag(v(2)) $ magnitude
plot db(v(2)) $ same as vdb (2)
plot imag(v(2)) $ imaginary part of v(2)
plot real(v(2)) $ same as plot v(2)
plot phase(v (2)) $ phase in rad
plot cph(v(2)) $ phase in rad , continuous beyond pi
plot 180/ PI *phase (v (2)) $ phase in deg
.endc
.end
In addition to the plot examples given above you may use the variants of vxx(node) described in
Chapt. 15.6.2 like vdb(2). An option to suppress OP analysis before AC may be set for linear
circuits (15.1.3).
17.5.2 Alias: Create an alias for a command
General Form:
alias [word ] [ text ...]
Causes word to be aliased to text. History substitutions may be used, as in C-shell aliases.
17.5.3 Alter*: Change a device or model parameter
Alter changes the value for a device or a specified parameter of a device or model.
General Form:
alter dev = <expression >
alter dev param = <expression >
alter @dev[param ] = <expression >
<expression> must be real (complex isn’t handled right now, integer is fine though, but no
strings. For booleans, use 0/1).
306 CHAPTER 17. INTERACTIVE INTERPRETER
Old style (pre 3f4):
alter device value
alter device parameter value [ parameter value ]
Using the old style, its first form is used by simple devices that have one principal value (resis-
tors, capacitors, etc.) where the second form is for more complex devices (bjt’s, etc.). Model
parameters can be changed with the second form if the name contains a ‘#’. For specifying a
list of parameters as values, start it with ‘[’, followed by the values in the list, and end with ‘]’.
Be sure to place a space between each of the values and before and after the ‘[’ and ‘]’.
Some examples are given below:
Examples (Spice3f4 style):
alter vd = 0.1
alter vg dc = 0.6
alter @m1[w]= 15e-06
alter @vg[sin] [ -1 1.5 2MEG ]
alter @Vi[pwl] = [ 0 1.2 100p 0 ]
alter may have vectors (17.8.2) or variables (17.8.1) as parameters.
Examples (vector or variable in parameter list):
let newfreq = 10k
alter @vg[sin] [ -1 1.5 $& newfreq ] $ vector
set newperiod = 150u
alter @Vi[pwl] = [ 0 1.2 $newperiod 0 ] $ variable
You may change a parameter of a device residing in a subcircuit, e.g. of MOS transistor msub1
in subcircuit xm1 (see also Chapt. 31.1).
Examples (parameter of device in subcircuit):
alter m.xm1 . msub1 w = 20u
alter @m.xm1 . msub1[w] = 20u
17.5.4 Altermod*: Change model parameter(s)
General form:
altermod mod param = < expression >
altermod @mod[ param ] = <expression >
Example:
altermod nc1 tox = 10e -9
altermod @nc1[tox ] = 10e-9
17.5. COMMANDS 307
Altermod operates on models and is used to change model parameters. The above example
will change the parameter tox in all devices using the model nc1, which is defined as
*** BSIM3v3 model
.MODEL nc1 nmos LEVEL=8 version = 3.2.2
+ acm = 2 mobmod = 1 capmod = 1 noimod = 1
+ rs = 2.84E+03 rd = 2.84E+03 rsh = 45
+ tox = 20E-9 xj = 0.25E-6 nch = 1.7E+17
+ ...
If you invoke the model by the MOS device
M1 d g s b nc1 w=10u l=1u
you might also insert the device name M1 for mod as in
altermod M1 tox = 10e-9
The model parameter tox will be modified, however not only for device M1, but for all devices
using the associated MOS model nc1!
If you want to run corner simulations within a single simulation flow, the following option of
altermod may be of help. The parameter set with name modn may be overrun by the altermod
command specifying a model file. All parameter values fitting to the existing model modn will
be modified. As usual the ’reset’ command (see 17.5.51) restores the original values. The model
file (see 2.3) has to use the standard specifications for an input file, the .model section is the
relevant part. However the first line in the model file will be ignored by the input parser, so it
should contain only some title information. The .model statement should appear then in the
second or any later line. More than one .model section may reside in the file.
General form:
altermod mod1 [mod2 .. mod15] file = <model file name >
altermod mod1 [mod2 .. mod15 ] file <model file name >
Example:
altermod nch file = BSIM3_nmos .mod
altermod pch nch file BSIM4_mos.mod
Be careful that the new model file corresponds to the existing model selected by modn. The ex-
isting models are defined during circuit setup at start up of ngspice. Models have been included
by .model statements (2.3) in your input file or included by the .include command. In the
example given above, the models nch (or nch and pch) have to be already available before cal-
ling altermod. If they are not found in the active circuit, ngspice will terminate with an error
message. There is no checking however of the version and level parameters! So you have to
be responsible for offering model data of the same model level (e.g. level 8 for BSIM3). Thus
no new model is selectable by altermod, but the parameters of the existing model(s) may be
changed (partially, completely, temporarily).
308 CHAPTER 17. INTERACTIVE INTERPRETER
17.5.5 Asciiplot: Plot values using old-style character plots
General Form:
asciiplot plotargs
Produce a line printer plot of the vectors. The plot is sent to the standard output, or you can
put it into a file with asciiplot args ... > file. The set options width, height, and nobreak
determine the width and height of the plot, and whether there are page breaks, respectively.
The ’more’ mode is the standard mode if printing to the screen, that is after a number of lines
given by height, and after a page break printing stops with request for answering the prompt
by <return>, ’c’ or ’q’. If everything shall be printed without stopping, put the command set
nomoremode into .spiceinit 16.6 (or spinit 16.5). Note that you will have problems if you try
to asciiplot something with an X-scale that isn’t monotonic (i.e, something like sin(TIME)
), because asciiplot uses a simple-minded linear interpolation. The asciiplot command
doesn’t deal with log scales or the delta keywords.
17.5.6 Aspice*: Asynchronous ngspice run
General Form:
aspice input - file [output -file ]
Start an ngspice run, and when it is finished load the resulting data. The raw data is kept in
a temporary file. If output-file is specified then the diagnostic output is directed into that file,
otherwise it is thrown away.
17.5.7 Bug: Mail a bug report
General Form:
bug
Send a bug report. Please include a short summary of the problem, the version number and
name of the operating system that you are running, the version of ngspice that you are running,
and the relevant ngspice input file. (If you have defined BUGADDR, the mail is delivered to there.)
17.5.8 Cd: Change directory
General Form:
cd [directory ]
Change the current working directory to directory, or to the user’s home directory if none is
given.
17.5. COMMANDS 309
17.5.9 Cdump: Dump the control flow to the screen
General Form:
cdump
Dumps the control sequence to the screen (all statements inside the .control ... .endc struc-
ture before the line with cdump). Indentations show the structure of the sequence. The example
below is printed if you add cdump to /examples/Monte_Carlo/MonteCarlo.sp.
Example (abbreviated):
let mc_runs =5
let run =0
...
define agauss(nom , avar , sig) (nom + avar /sig * sgauss (0))
define limit(nom , avar ) (nom + (( sgauss (0) >=0) ? avar : -avar ))
dowhile run < mc_runs
alter c1 = unif (1 e-09 , 0.1)
...
ac oct 100 250k 10 meg
meas ac bw trig vdb(out) val = -10 rise =1 targ vdb( out)
+ val = -10 fall =1
set run ="$&run "
...
let run=run + 1
end
plot db ({ $scratch }. allv )
echo
print { $scratch }. bwh
cdump
17.5.10 Circbyline*: Enter a circuit line by line
General Form:
circbyline line
Enter a circuit line by line. line is any circuit line, as found in the *.cir ngspice input files. The
first line is a title line. The entry will be finished by entering .end. Circuit parsing is then
started automatically.
310 CHAPTER 17. INTERACTIVE INTERPRETER
Example:
circbyline test circuit
circbyline v1 1 0 1
circbyline r1 1 0 1
circbyline .dc v1 0.5 1.5 0.1
circbyline .end
run
plot i(v1)
17.5.11 Codemodel*: Load an XSPICE code model library
General Form:
codemodel [ library file ]
Load a XSPICE code model shared library file (e.g. analog.cm ...). Only available if ngspice
is compiled with the XSPICE option (--enable-xspice) or with the Windows executable
distributed since ngspice21. This command has to be called from spinit (see Chapt. 16.5) (or
.spiceinit for personal code models, 16.6).
17.5.12 Compose: Compose a vector
General Form:
compose name values value1 [ value2 ... ]
compose name param = val [ param = val ... ]
The first form takes the values and creates a new vector, where the values may be arbitrary
expressions.
The second form has the following possible parameters:
start The value of name[0]
stop The last value of name
step The difference between successive elements of the created vector
lin How many linearly spaced elements the new vector should have
log The number of points, logarithmically spaced (not working)
dec The number of points per decade, logarithmically spaced (not working)
center Where to center the range of points (not working)
span The size of the range of points (not working)
gauss The nominal value for the used gaussian distribution
sd The standard deviation for the used gaussian distribution
sigma The sigma for the used gaussian distribution
random The nominal value for a uniform random distribution
rvar The percentage variation for the uniform random distribution
17.5. COMMANDS 311
17.5.13 Dc*: Perform a DC-sweep analysis
General Form:
dc Source Vstart Vstop Vincr [ Source2 Vstart2 Vstop2 Vincr2 ]
Do a dc transfer curve analysis. See the previous Chapt. 15.3.2 for more details. Several options
may be set (15.1.2).
17.5.14 Define: Define a function
General Form:
define function (arg1 , arg2 , ...) expression
Define the function with the name function and arguments arg1, arg2, ... to be expression,
which may involve the arguments. When the function is later used, the arguments it is given
are substituted for the formal arguments when it was parsed. If expression is not present, any
existing definition for function is printed, and if there are no arguments then all expressions for
all currently active definitions are printed. Note that you may have different functions defined
with the same name but different arities. Some useful definitions are:
Example:
define max(x,y) (x > y) * x + (x <= y) * y
define min(x,y) (x < y) * x + (x >= y) * y
define limit(nom , avar ) (nom + (( sgauss (0) >= 0) ? avar : -avar ))
17.5.15 Deftype: Define a new type for a vector or plot
General Form:
deftype [v | p] typename abbrev
defines types for vectors and plots. abbrev will be used to parse things like abbrev(name) and
to label axes with M<abbrev>, instead of numbers. It may be omitted. Also, the command
‘deftype p plottype pattern ...’ will assign plottype as the name to any plot with one of the
patterns in its Name: field.
Example:
deftype v capacitance F
settype capacitance moscap
plot moscap vs v(cc)
312 CHAPTER 17. INTERACTIVE INTERPRETER
17.5.16 Delete*: Remove a trace or breakpoint
General Form:
delete [ debug - number ... ]
Delete the specified saved nodes and parameters, breakpoints and traces. The debug numbers
are those shown by the status command (unless you do status > file, in which case the debug
numbers are not printed).
17.5.17 Destroy: Delete an output data set
General Form:
destroy [ plotnames | all]
Release the memory holding the output data (the given plot or all plots) for the specified runs.
17.5.18 Devhelp: information on available devices
General Form:
devhelp [[- csv ] device_name [parameter ]]
Devhelp command shows the user information about the devices available in the simulator. If
called without arguments, it simply displays the list of available devices in the simulator. The
name of the device is the name used inside the simulator to access that device. If the user spe-
cifies a device name, then all the parameters of that device (model and instance parameters)
will be printed. Parameter description includes the internal ID of the parameter (id#), the name
used in the model card or on the instance line (Name), the direction (Dir) and the description
of the parameter (Description). All the fields are self-explanatory, except the ‘direction’. Di-
rection can be in,out or inout and corresponds to a ‘write-only’, ‘read-only’ or a ‘read/write’
parameter. Read-only parameters can be read but not set, write only can be set but not read and
read/write can be both set and read by the user.
The -csv option prints the fields separated by a comma, for direct import into a spreadsheet.
This option is used to generate the simulator documentation.
Example:
devhelp
devhelp resistor
devhelp capacitor ic
17.5. COMMANDS 313
17.5.19 Diff: Compare vectors
General Form:
diff plot1 plot2 [vec ...]
Compare all the vectors in the specified plots, or only the named vectors if any are given. If
there are different vectors in the two plots, or any values in the vectors differ significantly,
the difference is reported. The variables diff_abstol,diff_reltol, and diff_vntol are used to
determine a significant difference.
17.5.20 Display: List known vectors and types
General Form:
display [varname ...]
Prints a summary of currently defined vectors, or of the names specified. The vectors are sorted
by name unless the variable nosort is set. The information given is the name of the vector, the
length, the type of the vector, and whether it is real or complex data. Additionally, one vector
is labeled [scale]. When a command such as plot is given without a vs argument, this scale is
used for the X-axis. It is always the first vector in a rawfile, or the first vector defined in a new
plot. If you undefine the scale (i.e, let TIME = []), one of the remaining vectors becomes the
new scale (which one is unpredictable). You may set the scale to another vector of the plot with
the command setscale (17.5.62).
17.5.21 Echo: Print text
General Form:
echo [text ...] [$variable ] ["$& vector "]
Echos the given text, variable or vector to the screen. echo without parameters issues a blank
line.
17.5.22 Edit*: Edit the current circuit
General Form:
edit [ file - name ]
Print the current ngspice input file into a file, call up the editor on that file and allow the user to
modify it, and then read it back in, replacing the original file. If a file-name is given, then edit
that file and load it, making the circuit the current one. The editor may be defined in .spiceinit
or spinit by a command line like
set editor=emacs
314 CHAPTER 17. INTERACTIVE INTERPRETER
Using MS Windows, to allow the edit command calling an editor, you will have to add the
editor’s path to the PATH variable of the command prompt windows (see here). edit then calls
cmd.exe with e.g. notepad++ and file-name as parameter, if you have set
set editor=notepad++.exe
in .spiceinit or spinit.
17.5.23 Edisplay: Print a list of all the event nodes
General Form:
edisplay
Print the names of all event driven nodes generated or used by XSPICE ’A’ devices. See
eprint,eprvcd, and 27.2.2 for an example.
17.5.24 Eprint: Print an event driven node
General Form:
eprint node [node ]
eprint node [ node] > nodeout . txt $ output redirected
Print an event driven node generated or used by an XSPICE ’A’ device. These nodes are vectors
not organized in plots. See edisplay,eprvcd, and Chapt. 27.2.2 for an example. Output
redirection into a file is available.
17.5.25 Eprvcd: Dump event nodes in VCD format
General Form:
eprvcd node1 node2 .. noden [ > filename ]
Dump the data of the specified event driven nodes to a .vcd file. Such files may be viewed
with an vcd viewer, for example ’gtkwave.’ See edisplay,eprint,eprvcd, and 27.2.2 for
an example.
17.5.26 FFT: fast Fourier transform of vectors
General Form:
fft vector1 [ vector2] ...
This analysis provides a fast Fourier transform of the input vector(s) in forward direction. fft
is much faster than spec (17.5.71) (about a factor of 50 to 100 for larger vectors).
17.5. COMMANDS 315
The fft command will create a new plot consisting of the Fourier transforms of the vectors
given on the command line. Each vector given should be a transient analysis result, i.e. it
should have time as a scale. You will have got these vectors by the tran Tstep Tstop
Tstart command.
The vector should have a linear equidistant time scale. Therefore linearization using the linearize
command is recommended before running fft. Be careful selecting a Tstep value small
enough for good interpolation, e.g. much smaller than any signal period to be resolved by fft
(see linearize command). The Fast Fourier Transform will be computed using a window
function as given with the specwindow variable. A new plot named specx will be generated
with a new vector (having the same name as the input vector, see command above) containing
the transformed data.
Ngspice has two FFT implementations:
1. Standard code is based on the FFT function provided by John Green ‘FFTs for RISC 2.0‘,
downloaded 2012, now to be found here. These are a power-of-two routines for fft and
ifft. If the input size doesn’t fit this requirement the remaining data will be zero padded
upto the next 2Nfield size. You have to take care of the correlated change in the scale
vector.
2. If available on the operating system (see Chapter 32) ngspice can be linked to the famous
FFTW-3 package, found here. This high performance package has advantages in speed
and accuracy compared to most of the freely available FFT libraries. It makes arbitrary
size transforms for even and odd data.
How to compute the fft from a transient simulation output:
ngspice 8 -> setplot tran1
ngspice 9 -> linearize V(2)
ngspice 9 -> set specwindow =blackman
ngspice 10 -> fft V(2)
ngspice 11 -> plot mag(V (2))
Linearize will create a new vector V(2) in a new plot tran2. The command fft V(2) will
create a new plot spec1 with vector V(2) holding the resulting data.
The variables listed in the following table control operation of the fft command. Each can be
set with the set command before calling fft.
specwindow: This variable is set to one of the following strings, which will determine the
type of windowing used for the Fourier transform in the spec and fft command. If not set, the
default is hanning.
none No windowing
rectangular Rectangular window
bartlet Bartlett (also triangle) window
blackman Blackman window
316 CHAPTER 17. INTERACTIVE INTERPRETER
hanning Hanning (also hann or cosine) window
hamming Hamming window
gaussian Gaussian window
flattop Flat top window
Figure 17.1: Spec and FFT window functions (Gaussian order = 4)
specwindoworder: This can be set to an integer in the range 2-8. This sets the order when
the Gaussian window is used in the spec and fft commands. If not set, order 2 is used.
17.5.27 Fourier: Perform a Fourier transform
General Form:
fourier fundamental_frequency [ expression ...]
Fourier is used to analyse the output vector(s) of a preceeding transient analysis (see 17.5.79).
It does a Fourier analysis of each of the given values, using the first 10 multiples of the funda-
mental frequency (or the first nfreqs multiples, if that variable is set - see 17.7). The printed
output is like that of the .four ngspice line (Chapt. 15.6.4). The expressions may be any valid
expression (see 17.2), e.g. v(2). The evaluated expression values are interpolated onto a fixed-
space grid with the number of points given by the fourgridsize variable, or 200 if it is not set.
The interpolation is of degree polydegree if that variable is set, or 1. If polydegree is 0, then no
interpolation is done. This is likely to give erroneous results if the time scale is not monotonic,
though.
The fourier command not only issues a printout, but also generates vectors, one per expression.
The size of the vector is 3 x nfreqs (per default 3 x 10). The name of the new vector is fouriermn,
17.5. COMMANDS 317
where m is set by the mth call to the fourier command, n is the nth expression given in the actual
fourier command. fouriermn[0] is the vector of the 10 (nfreqs) frequency values, fouriermn[1]
contains the 10 (nfreqs) magnitude values, fouriermn[2] the 10 (nfreqs) phase values of the
result.
Example:
* do the transient analysis
tran 1n 1m
* do the fourier analysis
fourier 3.34 e6 v(2) v(3) $ first call
fourier 100 e6 v (2) v(3) $ second call
* get individual values
let newt1 = fourier11 [0][1]
let newt2 = fourier11 [1][1]
let newt3 = fourier11 [2][1]
let newt4 = fourier12 [0][4]
let newt5 = fourier12 [1][4]
let newt6 = fourier12 [2][4]
* plot magnitude of second expression (v(3))
* from first call versus frequency
plot fourier12 [1] vs fourier12 [0]
The plot command from the example plots the vector of the magnitude values, obtained by
the first call to fourier and evaluating the first expression in this call, against the vector of the
frequency values.
17.5.28 Gnuplot: Graphics output via gnuplot
General Form:
gnuplot file plotargs
Like plot, but using for graphics output and further data manipulation. ngspice creates a file
called file.plt containing the command sequence, a file called file.data containing the data to be
plotted, and a file called either file.eps (Postscript, this is the default) or file.png (the compres-
sed binary png format, when the variable gnuplot_terminal is set to png). It is possible to
suppress the latter hardcopy file by using a file name that starts with ’np_’. On Linux gnuplot
is called via xterm, and offers a console to manipulate the data. On Windows a plot window is
opened and the command console window is available with a mouse click. Of course you have
to have gnuplot installed on your system.
17.5.29 Hardcopy: Save a plot to a file for printing
General Form:
hardcopy file plotargs
318 CHAPTER 17. INTERACTIVE INTERPRETER
Just like plot, except that it creates a file called file containing the plot. The file is a postscript
image. As an alternative the plot(5) format is available by setting the hcopydevtype variable
to plot5, and can be printed by either the plot(1) program or lpr with the -g flag. See also
Chapt. 18.6 for more details (color etc.).
17.5.30 Help: Print summaries of Ngspice commands
Prints help. This help information, however, is spice3f5-like, stemming from 1991 and thus
is outdated. If commands are given, descriptions of those commands are printed. Otherwise
help for only a few major commands is printed. On Windows this help command is no longer
available. Spice3f5 compatible help may be found in the Spice 3 User manual. For ngspice
please use this manual.
17.5.31 History: Review previous commands
General Form:
history [-r] [ number]
Print out the history, or the last (first if -r is specified) number commands typed at the keyboard.
A history substitution enables you to reuse a portion of a previous command as you type the
current command. History substitutions save typing. A history substitution normally starts
with a ’!’. A history substitution has three parts: an event that specifies a previous command,
a selector that selects one or more words of the event, and some modifiers that modify the
selected words. The selector and modifiers are optional. A history substitution has the form
![event][:]selector[:modifier] ...]The event is required unless it is followed by a
selector that does not start with a digit. The ’:’ can be omitted before the selector if this
selector does not begin with a digit. History substitutions are interpreted before anything else
even before quotations and command substitutions. The only way to quote the ’!’ of a
history substitution is to escape it with a preceding backslash. A ’!’ need not be escaped if it
is followed by whitespace, ’=’, or ’(’.
Ngspice saves each command that you type on a history list, provided that the command con-
tains at least one word. The commands on the history list are called events. The events are
numbered, with the first command that you issue when you start Ngspice being number one.
The history variable specifies how many events are retained on the history list.
These are the forms of an event in a history substitution:
!! The preceding event. Typing ’!!’ is an easy way to reissue the previous command.
!n Event number n.
!-n The nth previous event. For example, !-1 refers to the immediately preceding event and
is equivalent to !!.
!str The unique previous event whose name starts with str.
!?str[?] The unique previous event containing the string str. The closing ’?’ can be omitted if it
is followed by a newline.
17.5. COMMANDS 319
You can modify the words of an event by attaching one or more modifiers. Each modifier must
be preceded by a colon. The following modifiers assume that the first selected word is a file
name:
:r Removes the trailing .str extension from the first selected word.
:h Removes a trailing path name component from the first selected word.
:t Removes all leading path name components from the first selected word.
:e Remove all but the trailing suffix.
:p Print the new command but do not execute it.
s/old/new Substitute new for the first occurrence of old in the event line. Any delimiter may be
used in place of ‘/’. The delimiter may be quoted in old and new with a single backslash.
If ‘&’ appears in new, it is replaced by old. A single backslash will quote the ‘&’. The
final delimiter is optional if it is the last character on the input line.
&Repeat the previous substitution.
g a Cause changes to be applied over the entire event line. Used in conjunction with ‘s’, as
in gs/old/new/, or with ‘&’.
GApply the following ‘s’ modifier once to each word in the event.
For example, if the command ls /usr/elsa/toys.txt has just been executed, then the command
echo !!^:r !!^:h !!^:t !!^:t:r produces the output /usr/elsa/toys /usr/elsa toys.txt toys . The ’^’
command is explained in the table below.
You can select a subset of the words of an event by attaching a selector to the event. A history
substitution without a selector includes all of the words of the event. These are the possible
selectors for selecting words of the event:
:0 The command name
[:]^ The first argument
[:]$ The last argument
:n The nth argument (n≥1)
:n1-n2 Words n1 through n2
[:]* Words 1 through $
:x* Words xthrough $
:x- Words xthrough ($ - 1)
[:]-x Words 0 through x
[:]% The word matched by the last ?str? search used
The colon preceding a selector can be omitted if the selector does not start with a digit.
The following additional special conventions provide abbreviations for commonly used forms
of history substitution:
• An event specification can be omitted from a history substitution if it is followed by a
selector that does not start with a digit. In this case the event is taken to be the event
used in the most recent history reference on the same line if there is one, or the preceding
event otherwise. For example, the command echo !?qucs?^ !$ echoes the first and last
arguments of the most recent command containing the string qucs .
• If the first nonblank character of an input line is ’^’, the ’^’ is taken as an abbreviation
for !:s^ . This form provides a convenient way to correct a simple spelling error in the
320 CHAPTER 17. INTERACTIVE INTERPRETER
previous line. For example, if by mistake you typed the command cat /etc/lasswd you
could re-execute the command with lasswd changed to passwd by typing ^l^p .
• You can enclose a history substitution in braces to prevent it from absorbing the following
characters. In this case the entire substitution except for the starting ’!’ must be within
the braces. For example, suppose that you previously issued the command cp accounts
../money . Then the command !cps looks for a previous command starting with cps
while the command !{cp}s turns into a command cp accounts ../moneys .
Some characters are handled specially as follows:
~Expands to the home directory
*Matches any string of characters in a filename
?Matches any single character in a filename
[] Matches any of the characters enclosed in a filename
-Used within [] to specify a range of characters. For example, [b-k] matches on any
character between and including ‘b’ through to ‘k’.
^If the ^is included within [] as the first character, then it negates the following characters
matching on anything but those. For example, [^agm] would match on anything other
than ‘a’,‘g’ and ‘m’.[^a-zA-Z] would match on anything other than an alphabetic
character.
The wildcard characters *,?,[, and ]can be used, but only if you unset noglob first. This
makes them rather useless for typing algebraic expressions, so you should set noglob again
after you are done with wildcard expansion.
When the environment variable HOME exists (on Unix, Linux, or CYGWIN), history per-
manently stores previous command lines in the file $HOME/._ngspice_history. When this
variable does not exist (typically on Windows when the readline library is not officially instal-
led), the history file is called .history and put in the current working directory.
The history command is part of the readline or editline package. The readline program pro-
vides a command line editor that is configurable through the file .inputrc. The path to this
configuration file is either found in the shell variable INPUTRC, or it is (on Unix/Linux/CYG-
WIN) the file ~/.inputrc in the user’s home directory. On Windows systems the configuration
file is /Users/<username>/.inputrc, unless the readline library was officially installed. In that
case the filename is taken from the Windows registry and points to a location that the user speci-
fied during installation. See https://cnswww.cns.cwru.edu/php/chet/readline/rltop.html for
detailed documentation. Some useful commands are:
Left/Right arrow Move one character to the left or right
Home/End Move to beginning or end of line
Up/Down arrow Cycle through the history buffer
C-_- Undo last editing command
C-r Incremental search backward
TAB completion of a file name
C-ak Erase the command line (kill)
C-y Retrieve last kill (yank)
C-u Erase from cursor to start of line
17.5. COMMANDS 321
17.5.32 Inventory: Print circuit inventory
General Form:
inventory
This commands accepts no argument and simply prints the number of instances of a particular
device in a loaded netlist.
17.5.33 Iplot*: Incremental plot
General Form:
iplot [ node ...]
Incrementally plot the values of the nodes while ngspice runs. The iplot command can be used
with the where command to find trouble spots in a transient simulation.
The @name[param] notation (31.1) might not work yet.
17.5.34 Jobs*: List active asynchronous ngspice runs
General Form:
jobs
Report on the asynchronous ngspice jobs currently running. Ngnutmeg checks to see if the
jobs are finished every time you execute a command. If it is done then the data is loaded and
becomes available.
17.5.35 Let: Assign a value to a vector
General Form:
let name = expr
Creates a new vector called name with the value specified by expr, an expression as described
above. If expr is [] (a zero-length vector) then the vector becomes undefined. Individual ele-
ments of a vector may be modified by appending a subscript to name (ex. name[0]). If there are
no arguments, let is the same as display.
The command let creates a vector in the current plot. Use setplot (17.5.61) to create a new plot.
There is no straightforward way to initialize a new vector. In general, one might want let
initialize a slice (i.e. name[4:4,21:23] = [ 1 2 3 ]) of a multi-dimensional matrix of arbitrary
type (i.e. real, complex ..), where all values and indexes are arbitrary expressions. This will
fail. The procedure is to first allocate a real vector of the appropriate size with either vector(),
unitvec(), or [ n1 n2 n3 ... ]. The second step is to optionally change the type of the
322 CHAPTER 17. INTERACTIVE INTERPRETER
new vector (to complex) with the j() function. The third step reshapes the dimensions, and
the final step (re)initializes the contents, like so:
let a = j(vector(10))
reshape a [2][5]
let a[0][0] = (pi,pi)
Initialization of real vectors can be done quite efficiently with compose:
compose a values (pi, pi) (1,1) (2,sqrt(7)) (boltz,e)
reshape a [2][2]
See also unlet (17.5.83), compose (17.5.12).
17.5.36 Linearize*: Interpolate to a linear scale
General Form:
linearize vec ...
Create a new plot with all of the vectors in the current plot, or only those mentioned as argu-
ments to the command, all data linearized onto an equidistant time scale.
How to compute the fft from a transient simulation output:
ngspice 8 -> setplot tran1
ngspice 9 -> linearize V(2)
ngspice 9 -> set specwindow =blackman
ngspice 10 -> fft V(2)
ngspice 11 -> plot mag(V (2)) tstep
Linearize will redo the vectors vec or renew all vectors of the current plot (e.g. tran3) if no
arguments are given and store them into a new plot (e.g. tran4). The new vectors are interpolated
onto a linear time scale, which is determined by the values of tstep,tstart, and tstop in
the currently active transient analysis. The currently loaded input file must include a transient
analysis (a tran command may be run interactively before the last reset, alternately), and
the current plot must be from this transient analysis. The length of the new vector is (tstop
- tstart) / tstep + 1.5. This command is needed for example if you want to do a fft
analysis (17.5.26). Please note that the parameter tstep of your transient analysis (see Chapt.
15.3.9) has to be small enough to get adequate resolution, otherwise the command linearize
will do sub-sampling of your signal. If no circuit is loaded and the data have been aquired by the
load (17.5.38) command, Linearize will take time data from transient analysis scale vector.
17.5. COMMANDS 323
17.5.37 Listing*: Print a listing of the current circuit
General Form:
listing [ logical ] [physical ] [deck] [ expand ] [param ]
If the logical argument is given, the listing is with all continuation lines collapsed into one line,
and if the physical argument is given the lines are printed out as they were found in the file. The
default is logical. A deck listing is just like the physical listing, except without the line numbers
it recreates the input file verbatim (except that it does not preserve case). If the word expand is
present, the circuit is printed with all subcircuits expanded. The option param allows to print
all parameters and their actual values.
17.5.38 Load: Load rawfile data
General Form:
load [ filename] ...
Loads either binary or ascii format rawfile data from the files named. The default file-name is
rawspice.raw, or the argument to the -r flag if there was one.
17.5.39 Meas*: Measurements on simulation data
General Form (example):
MEAS {DC |AC |TRAN |SP } result TRIG trig_variable VAL =val <TD =td >
<CROSS =# | CROSS =LAST > <RISE =#| RISE =LAST > <FALL =#| FALL =LAST >
<TRIG AT= time > TARG targ_variable VAL =val <TD =td >
<CROSS =# | CROSS =LAST > <RISE =#| RISE =LAST >
<FALL =#| FALL =LAST > <TRIG AT= time >
Most of the input forms found in 15.4 may be used here with the command meas instead of
.meas(ure). Using meas inside the .control ... .endc section offers additional features
compared to the .meas use. meas will print the results as usual, but in addition will store
its measurement result (typically the token result given in the command line) in a vector.
This vector may be used in following command lines of the script as an input value of another
command. For details of the command see Chapt. 15.4. The measurement type SP is only
available here, because a fft command will prepare the data for SP measurement. Option
autostop (15.1.4) is not available.
Unfortunately par(’expression’)(15.6.6) will not work here, i.e. inside the .control section.
You may use an expression by the let command instead, giving let vec_new = expression.
324 CHAPTER 17. INTERACTIVE INTERPRETER
Replacement for par(’expression’) in meas inside the .control section
let vdiff = v(n1)-v( n0)
meas tran vtest find vdiff at =0.04e -3
*the following will not do here:
* meas tran vtest find par (’v( n1 )- v( n0 )’) at =0.04e -3
17.5.40 Mdump*: Dump the matrix values to a file (or to console)
General Form:
mdump <filename >
If <filename> is given, the output will be stored in file <filename>, otherwise dumped to
your console.
17.5.41 Mrdump*: Dump the matrix right hand side values to a file (or
to console)
General Form:
mrdump <filename >
If <filename> is given, the output will be appended to file <filename>, otherwise dumped to
your console.
Example usage after ngspice has started:
* Dump matrix and RHS values after 10 and 20 steps
* of a transient simulation
source rc. cir
step 10
mdump m1. txt
mrdump mr1 . txt
step 10
mdump m2. txt
mrdump mr2 . txt
* just to continue to the end
step 10000
You may create a loop using the control structures (Chapt. 17.6).
17.5.42 Noise*: Noise analysis
See the .NOISE analysis (15.3.4) for details.
17.5. COMMANDS 325
The noise command will generate two plots (typically named noise1 and noise2) with Noise
Spectral Density Curves and Integrated Noise data. To write these data into output file(s), you
may use the following command sequence:
Command sequence for writing noise data to file(s):
.control
tran 1e-6 1e-3
write test_tran . raw
noise V(out ) vinp dec 333 1 1e8 16
print inoise_total onoise_total
*first option to get all of the output (two files )
setplot noise1
write test_noise1 .raw all
setplot noise2
write test_noise2 .raw all
* second option (all in one raw -file )
write testall .raw noise1 . all noise2 . all
.endc
17.5.43 Op*: Perform an operating point analysis
General Form:
op
Do an operating point analysis. See Chapt. 15.3.5 for more details.
17.5.44 Option*: Set a ngspice option
General Form:
option [option = val] [option = val] ...
Set any of the simulator variables as listed in Chapt. 15.1. See this chapter also for more
information on the available options. The option command without any argument lists the
actual options set in the simulator (to be verified). Multiple options may be set in a single line.
The following example demonstrates a control section, which may be added to your circuit file
to test the influence of variable trtol on the number of iterations and on the simulation time.
326 CHAPTER 17. INTERACTIVE INTERPRETER
Command sequence for testing option trtol:
.control
set noinit
option trtol =1
echo
echo trtol =1
run
rusage traniter trantime
reset
option trtol =3
echo
echo trtol =3
run
rusage traniter trantime
reset
option trtol =5
echo
echo trtol =5
run
rusage traniter trantime
reset
option trtol =7
echo
echo trtol =7
run
rusage traniter trantime
plot tran1.v( out25) tran1.v( out50) v( out25 ) v( out50 )
.endc
17.5.45 Plot: Plot vectors on the display
General Form:
plot exprs [ylimit ylo yhi] [ xlimit xlo xhi] [ xindices xilo xihi]
[xcompress comp ] [ xdelta xdel] [ ydelta ydel ]
[xlog] [ ylog ] [ loglog ] [ nogrid] [vs xname_expr]
[linplot ] [ combplot ] [ pointplot ] [ nointerp ]
[xlabel word ] [ ylabel word] [title word] [ samep ] [linear ]
Plot the given vectors or exprs on the screen (if you are on a graphics terminal). The xlimit
and ylimit arguments determine the high and low x- and y-limits of the axes, respectively. The
xindices arguments determine what range of points are to be plotted - everything between the
xilo’th point and the xihi’th point is plotted. The xcompress argument specifies that only
one out of every comp points should be plotted. If an xdelta or a ydelta parameter is present,
it specifies the spacing between grid lines on the X- and Y-axis. These parameter names may
17.5. COMMANDS 327
be abbreviated to xl,yl,xind,xcomp,xdel, and ydel respectively.
The xname_expr argument is an expression to use as the scale on the x-axis. If xlog or ylog are
present then the X or Y scale, respectively, are logarithmic (loglog is the same as specifying
both). The xlabel and ylabel arguments cause the specified labels to be used for the X and
Y axes, respectively.
If samep is given, the values of the other parameters (other than xname_expr) from the previous
plot,hardcopy, or asciiplot command are used unless re-defined on the command line.
The title argument is used in the headline of the plot window and replaces the default text,
which is ‘actual plot: first line of input file’.
The linear keyword is used to override a default logscale plot (as in the output for an AC
analysis).
The keywords linplot,combplot and pointplot select different plot styles. The keyword
nointerp turns of interpolation of the vector data, nogrid suppresses the drawing of gridlines.
Finally, the keyword polar generates a polar plot. To produce a smith plot, use the keyword
smith. Note that the data is transformed, so for smith plots you will see the data transformed
by the function (x-1)/(x+1). To produce a polar plot with a smith grid but without performing
the smith transform, use the keyword smithgrid.
If you specify plot all, all vectors (including the scale vector) are plotted versus the scale
vector (see commands display (17.5.20) or setscale (17.5.62) on viewing the vectors of the
current plot). The command plot ally will not plot the scale vector, but all other ’real’ y
values. The command plot alli selects all current vectors, the command plot allv all
voltage vectors.
If the vector name to be plotted contains -,/or other tokens that may be taken for opera-
tors of an expression, and plotting fails, try enclosing the name in double quotes, e.g. plot
“/vout”.
Plotting of complex vectors, as may occur after an ac simulation, requires special considerati-
ons. Please see Chapt. 17.5.1 for details.
17.5.46 Pre_<command>: execute commands prior to parsing the circuit
General Form:
pre_ <command >
All commands in a .control ... .endc section are executed after the circuit has been parsed.
If you need command execution before circuit parsing, you may add these commands to the
general spinit or local .spiceinit files. Another possibility is adding a leading pre_ to a com-
mand within the .control section of an ordinary input file, which forces the command to be
executed before circuit parsing. Basically <command> may be any command listed in Chapt.
17.5, however only a few commands are indeed useful here. Some examples are given below:
328 CHAPTER 17. INTERACTIVE INTERPRETER
Examples:
pre_unset ngdebug
pre_set strict_errorhandling
pre_codemodel mymod . cm
pre_<command> is available only in the .control mode (see 16.4.3), not in interactive mode,
where the user may determine herself when a circuit is to be parsed, using the source command
(17.5.70) .
17.5.47 Print: Print values
General Form:
print [col ] [ line ] expr ...
Prints the vector(s) described by the expression expr. If the col argument is present, print the
vectors named side by side. If line is given, the vectors are printed horizontally. col is the
default, unless all the vectors named have a length of one, in which case line is the default.
The options width (default 80) and height (default 24) are effective for this command (see
asciiplot 17.5.5). The ’more’ mode is the standard mode if printing to the screen, that is after
a number of lines given by height, and after a page break printing stops with request for answe-
ring the prompt by <return> (print next page), ’c’ (print rest) or ’q’ (quit printing). If everything
shall be printed without stopping, put the command set nomoremode into .spiceinit 16.6 (or
spinit 16.5). If the expression is all, all of the vectors available are printed. Thus print col
all > filename prints everything into the file filename in SPICE2 format. The scale vector
(time, frequency) is always in the first column unless the variable noprintscale is true. You
may use the vectors alli, allv, ally with the print command, but then the scale vector
will not be printed.
Examples:
print all
set width =300
print v (1) > outfile.out
17.5.48 Quit: Leave Ngspice or Nutmeg
General Form:
quit
quit [ exitcode ]
Quit ngnutmeg or ngspice. Ngspice will ask for an acknowledgment if parameters have not
been saved. If unset askquit is specified, ngspice will terminate immediately.
The optional parameter exitcode is an integer that sets the exit code for ngspice. This is useful
to return a success/fail value to the operating system.
17.5. COMMANDS 329
17.5.49 Rehash: Reset internal hash tables
General Form:
rehash
Recalculate the internal hash tables used when looking up UNIX commands, and make all
UNIX commands in the user’s PATH available for command completion. This is useless unless
you have set unixcom first (see above).
17.5.50 Remcirc*: Remove the current circuit
General Form:
remcirc
This command removes the current circuit from the list of circuits sourced into ngspice. To se-
lect a specific circuit, use setcirc (17.5.60). To load another circuit, refer to source (17.5.70).
The new actual circuit will be the circuit on top of the list of the remaining circuits.
17.5.51 Reset*: Reset an analysis
General Form:
reset
Throw out any intermediate data in the circuit (e.g, after a breakpoint or after one or more
analyses have been done), and re-parse the input file. The circuit can then be re-run from it’s
initial state, overriding the effect of any set or alter commands.
Reset may be required in simulation loops preceding any run (or tran ...) command.
17.5.52 Reshape: Alter the dimensionality or dimensions of a vector
General Form:
reshape vector vector ...
or
reshape vector vector ... [ dimension , dimension , ... ]
or
reshape vector vector ... [ dimension ][ dimension ] ...
This command changes the dimensions of a vector or a set of vectors. The final dimension
may be left off and it will be filled in automatically. If no dimensions are specified, then the
dimensions of the first vector are copied to the other vectors. An error message of the form
’dimensions of x were inconsistent’ can be ignored.
330 CHAPTER 17. INTERACTIVE INTERPRETER
Example:
* generate vector with all (here 30) elements
let newvec =vector (30)
* reshape vector to format 3 x 10
reshape newvec [3][10]
* access elements of the reshaped vector
print newvec [0][9]
print newvec [1][5]
let newt = newvec [2][4]
17.5.53 Resume*: Continue a simulation after a stop
General Form:
resume
Resume a simulation after a stop or interruption (control-C).
17.5.54 Rspice*: Remote ngspice submission
General Form:
rspice <input file >
Runs a ngspice remotely taking the input file as a ngspice input file, or the current circuit if
no argument is given. Ngnutmeg or ngspice waits for the job to complete, and passes output
from the remote job to the user’s standard output. When the job is finished the data is loaded
in as with aspice. If the variable rhost is set, ngnutmeg connects to this host instead of the
default remote ngspice server machine. This command uses the rsh command and thereby
requires authentication via a .rhosts file or other equivalent method. Note that rsh refers to
the ‘remote shell’ program, which may be remsh on your system; to override the default name
of rsh, set the variable remote_shell. If the variable rprogram is set, then rspice uses this
as the pathname to the program to run on the remote system.
Note: rspice will not acknowledge elements that have been changed via the alter or altermod
commands.
17.5.55 Run*: Run analysis from the input file
General Form:
run [ rawfile]
Run the simulation as specified in the input file. If there were any of the control lines .ac,.op,
.tran, or .dc, they are executed. The output is put in rawfile if it was given, in addition to
being available interactively.
17.5. COMMANDS 331
17.5.56 Rusage: Resource usage
General Form:
rusage [ resource ...]
Print resource usage statistics. If any resources are given, just print the usage of that resource.
Most resources require that a circuit be loaded. Currently valid resources are:
decklineno Number of lines in deck
netloadtime Nelist loading time
netparsetime Netlist parsing time
elapsed The amount of time elapsed since the last rusage elapsed call.
faults Number of page faults and context switches (BSD only).
space Data space used.
time CPU time used so far.
temp Operating temperature.
tnom Temperature at which device parameters were measured.
equations Circuit Equations
time Total Analysis Time
totiter Total iterations
accept Accepted time-points
rejected Rejected time-points
loadtime Time spent loading the circuit matrix and RHS.
reordertime Matrix reordering time
lutime L-U decomposition time
solvetime Matrix solve time
trantime Transient analysis time
tranpoints Transient time-points
traniter Transient iterations
trancuriters Transient iterations for the last time point*
tranlutime Transient L-U decomposition time
transolvetime Transient matrix solve time
everything All of the above.
* listed incorrectly as ‘Transient iterations per point’.
332 CHAPTER 17. INTERACTIVE INTERPRETER
17.5.57 Save*: Save a set of outputs
General Form:
save [all | outvec ...]
Save a set of outputs, discarding the rest (if not keyword all is given). Maybe used to dramati-
cally reduce memory (RAM) requirements if only a few useful node voltages or branch currents
are saved.
Node voltages may be saved by giving the nodename or v(nodename). Currents through an
independent voltage source are given by i(sourcename) or sourcename#branch. Internal de-
vice data (31.1) are accepted as @dev[param]. The syntax is identical to the .save command
(15.6.1).
Note: In the .control .... .endc section save must occur before the run or tran com-
mand to become effective.
If a node has been mentioned in a save command, it appears in the working plot after a run has
completed, or in the rawfile written by the write (17.5.88) command. For backward compatibi-
lity, if there are no save commands given, all outputs are saved. If you want to trace (17.5.78)
or plot (17.5.45) a node, you have to save it explicitly, except for all given or no save command
at all.
When the keyword all appears in the save command, all node voltages, voltage source currents
and inductor currents are saved in addition to any other vectors listed.
Save voltage and current:
save vd_node vs # branch v(vs_node ) i(vs2)
Save allows to store and later access internal device parameters. e.g. in a command like
Save internal parameters:
save all @mn1[gm]
saves all standard analysis output data plus gm of transistor mn1 to internal memory (see also
31.1).
save may store data from nodes or devices residing inside of a subcircuit:
Save voltage on node 3 (top level), node 8 (from inside subcircuit x2) and current through vmeas
(from subcircuit x1):
save 3 x1.x2.x1.x2 .8 v.x1.x1.x1. vmeas# branch
Save internal parameters within subcircuit:
save @m.xmos3 .mn1[gm]
Use commands listing expand (17.5.37,before the simulation) or display (17.5.20, af-
ter simulation) to obtain a list of all nodes and currents available. Please see Chapt. 31 for an
explanation of the syntax for internal parameters.
17.5. COMMANDS 333
Entering several save lines in a single .control section will accumulate the nodes and parame-
ters to be saved. If you want to exclude a node, you have to get its number by calling status
(17.5.72) and then calling delete number (17.5.16).
17.5.58 Sens*: Run a sensitivity analysis
General Form:
sens output_variable
sens output_variable ac ( DEC | OCT | LIN ) N Fstart Fstop
Perform a Sensitivity analysis. output_variable is either a node voltage (ex. v(1) or
v(A,out)) or a current through a voltage source (e.g. i(vtest)). The first form calcula-
tes DC sensitivities, the second form AC sensitivities. The output values are in dimensions of
change in output per unit change of input (as opposed to percent change in output or per percent
change of input).
17.5.59 Set: Set the value of a variable
General Form:
set [ word]
set [ word = value ] ...
Set the value of word to value, if it is present. You can set any word to be any value, numeric or
string. If no value is given then the value is the Boolean ‘true’. If you enter a string, you have
to enclose it in double quotes. Set save the lower case version of a word string.
The value of word may be inserted into a command by writing $word. If a variable is set to
a list of values that are enclosed in parentheses (which must be separated from their values by
white space), the value of the variable is the list.
The variables used by ngspice are listed in section 17.7.
Set entered without any parameter will list all variables set, and their values, if applicable.
Be advised that set sets the lower case variant of word. If this is not desired, please use setcf
(see ?? below).
17.5.60 Setcirc*: Change the current circuit
General Form:
setcirc [circuit number ]
The current circuit is the one that is used for the simulation commands below. When a circuit
is loaded with the source command (see below, 17.5.70) it becomes the current circuit.
Setcirc followed by ’return’ without any parameters lists all circuits loaded.
334 CHAPTER 17. INTERACTIVE INTERPRETER
17.5.61 Setplot: Switch the current set of vectors
General Form:
setplot [ plotname ]
Set the current plot to the plot with the given name, or if no name is given, prompt the user
with a menu. (Note that the plots are named as they are loaded, with names like tran1 or op2.
These names are shown by the setplot and display commands and are used by diff, below.)
If the ‘New plot’ item is selected, the current plot becomes one with no vectors defined.
Note that here the word plot refers to a group of vectors that are the result of one ngspice run.
When more than one file is loaded in, or more than one plot is present in one file, ngspice keeps
them separate and only shows you the vectors in the current plot.
17.5.62 Setscale: Set the scale vector for the current plot
General Form:
setscale [vector ]
Defines the scale vector for the current plot. If no argument is given, the current scale vector is
printed. The scale vector delivers the values for the x-axis in a 2D plot.
17.5.63 Settype: Set the type of a vector
General Form:
settype type vector ...
Change the type of the named vectors to type. Type names can be found in the following table.
Type Unit Type Unit
notype pole
time s zero
frequency Hz s-param
voltage V temp-sweep Celsius
current A res-sweep Ohms
onoise-spectrum (V or A)/√Hz impedance Ohms
onoise-integrated V or A admittance Mhos
inoise-spectrum (V or A)/√Hz power W
inoise-integrated V or A phase Degree
decibel dB
17.5. COMMANDS 335
17.5.64 Shell: Call the command interpreter
General Form:
shell [ command ]
Call the operating system’s command interpreter; execute the specified command or call for
interactive use.
17.5.65 Shift: Alter a list variable
General Form:
shift [varname ] [number ]
If varname is the name of a list variable, it is shifted to the left by number elements (i.e, the
number leftmost elements are removed). The default varname is argv, and the default number
is 1.
17.5.66 Show*: List device state
General Form:
show devices [ : parameters ] , ...
The show command prints out tables summarizing the operating condition of selected devices.
If devices is missing, a default set of devices are listed, if devices is a single letter, devices
of that type are listed. A device’s full name may be specified to list only that device. Finally,
devices may be selected by model by using the form #modelname.
If no parameters are specified, the values for a standard set of parameters are listed. If the list of
parameters contains a ‘+’, the default set of parameters is listed along with any other specified
parameters.
For both devices and parameters, the word all has the obvious meaning.
Note: there must be spaces separating the ‘:’ that divides the device list from the parameter list.
17.5.67 Showmod*: List model parameter values
General Form:
showmod models [ : parameters ] , ...
The showmod command operates like the show command (above) but prints out model parame-
ter values. The applicable forms for models are a single letter specifying the device type letter
(e.g. m, or c), a device name (e.g. m.xbuf22.m4b), or #modelname (e.g. #p1).
336 CHAPTER 17. INTERACTIVE INTERPRETER
17.5.68 Snload*: Load the snapshot file
General Form:
snload circuit -file file
snload reads the snapshot file generated by snsave (17.5.69). circuit-file is the original circuit
input file. After reading, the simulation may be continued by resume (17.5.53).
An input script for loading circuit and intermediate data, resuming simulation and plotting is
shown below:
Typical usage:
* SCRIPT : ADDER - 4 BIT BINARY
* script to reload circuit and continue the simulation
* begin with editing the file location
* to be started with ’ngspice adder_snload .script ’
.control
* cd to where all files are located
cd D:\ Spice_g ene ral \ ngspice \ exa mples \ snapshot
* load circuit and snpashot file
snload adder_mos_circ . cir adder500 . snap
* continue simulation
resume
* plot some node voltages
plot v(10) v(11) v(12)
.endc
Due to a bug we currently need the term ’script’ in the title line (first line) of the script.
17.5.69 Snsave*: Save a snapshot file
General Form:
snsave file
If you run a transient simulation and interrupt it by e.g. a stop breakpoint (17.5.74), you may
resume simulation immediately (17.5.53) or store the intermediate status in a snapshot file by
snsave for resuming simulation later (using snload (17.5.68)), even with a new instance of
ngspice.
17.5. COMMANDS 337
Typical usage:
Example input file for snsave
* load a circuit (including transistor models and .tran command )
* starts transient simulation until stop point
* store intermediate data to file
* begin with editing the file location
* to be run with ’ngspice adder_mos .cir ’
.include adder_mos_circ .cir
.control
*cd to where all files are located
cd D:\ Spice_g ene ral \ ngspice \ exa mples \ snapshot
unset askquit
set noinit
*interrupt condition for the simulation
stop when time > 500n
* simulate
run
* store snapshot to file
snsave adder500 . snap
quit
.endc
.END
adder_mos_circ.cir is a circuit input file, including the netlist, .model and .tran statements.
Unfortunately snsave/snload will not work if you have XSPICE devices (or V/I sources with
polynomial statements) in your input deck.
17.5.70 Source: Read a ngspice input file
General Form:
source infile
For ngspice: read the ngspice input file infile, containing a circuit netlist. Ngnutmeg and ngspice
commands may be included in the file, and must be enclosed between the lines .control and
.endc. These commands are executed immediately after the circuit is loaded, so a control
line of ac ... works the same as the corresponding .ac card. The first line in any input file
is considered a title line and not parsed but kept as the name of the circuit. Thus, a ngspice
command script in infile must begin with a blank line and then with a .control line. Also,
any line starting with the string ‘*#’ is considered as a control line (.control and .endc is
placed around this line automatically.). The exception to these rules are the files spinit (16.5)
and .spiceinit (16.6).
338 CHAPTER 17. INTERACTIVE INTERPRETER
For ngutmeg: reads commands from the file infile. Lines beginning with the character ‘*’ are
considered comments and are ignored.
The following search path is executed to find infile: current directory (OS dependent), <pre-
fix>/share/ngspice/scripts, env. variable NGSPICE_INPUT_DIR (if defined), see 16.7. This
sequence may be overriden by setting the internal sourcepath variable (see 17.7) before cal-
ling source infile.
17.5.71 Spec: Create a frequency domain plot
General Form:
spec start_freq stop_freq step_freq vector [ vector ...]
Calculates a new complex vector containing the Fourier transform of the input vector (typi-
cally the linearized result of a transient analysis). The default behavior is to use a Hanning
window, but this can be changed by setting the variables specwindow and specwindoworder
appropriately.
Typical usage:
ngspice 13 -> linearize
ngspice 14 -> set specwindow = " blackman"
ngspice 15 -> spec 10 1000000 1000 v(out )
ngspice 16 -> plot mag(v( out ))
Possible values for specwindow are: none,hanning,cosine,rectangular,hamming,triangle,
bartlet,blackman,gaussian and flattop. In the case of a gaussian window specwindoworder
is a number specifying its order. For a list of window functions see 17.5.26.
17.5.72 Status*: Display breakpoint information
General Form:
status
Display all of the saved nodes and parameters, traces and breakpoints currently in effect.
17.5.73 Step*: Run a fixed number of time-points
General Form:
step [ number ]
Iterate number times, or once, and then stop.
17.5. COMMANDS 339
17.5.74 Stop*: Set a breakpoint
General Form:
stop [ after n] [ when value cond value ] ...
Set a breakpoint. The argument after nmeans stop after iteration number ‘n’, and the argument
when value cond value means stop when the first value is in the given relation with the
second value, the possible relations being
Symbol Alias Meaning
= eq equal to
<> ne not equal
> gt greater than
< lt less than
>= ge greater than or equal to
<= le less than or equal to
Symbol or alias may be used alternatively. All stop commands have to be given in the control
flow before the run command. The values above may be node names in the running circuit, or
real values. If more than one condition is given, e.g.
stop after 4 when v(1) > 4 when v(2) < 2,
the conjunction of the conditions is implied. If the condition is met, the simulation and control
flow are interrupted, and ngspice waits for user input.
In a transient simulation the ‘=’ or eq will only work with vector time in commands like
stop when time = 200n.
Internally a breakpoint will be set at the time requested. Multiple breakpoints may be set. If the
first stop condition is met, the simulation is interrupted, the commands following run or tran
(e.g. alter or altermod) are executed, then the simulation may continue at the first resume
command. The next breakpoint requires another resume to continue automatically. Otherwise
the simulation stops and ngspice waits for user input.
If you try to stop at
stop when V(1) eq 1
(or similar) during a transient simulation, you probably will miss this point, because it is not
very likely that at any time step the vector v(1) will have the exact value of 1. Then ngspice
simply will not stop.
17.5.75 Strcmp: Compare two strings
General Form:
strcmp _flag $string1 " string2 "
The command compares two strings, either given by a variable (string1) or as a string in quotes
(‘string2’). _flag is set as an output variable to ’0’, if both strings are equal. A value greater
than zero indicates that the first character that does not match has a greater value in str1 than in
str2; and a value less than zero indicates the opposite (like the C strcmp function).
340 CHAPTER 17. INTERACTIVE INTERPRETER
17.5.76 Sysinfo*: Print system information
General Form:
sysinfo
The command prints system information useful for sending bug report to developers. Informa-
tion consists of:
• Name of the operating system,
• CPU type,
• Number of physical processors (not available under Windows OS), number of logical
processors,
• Total amount of DRAM available,
• DRAM currently available.
The example below shows the use of this command.
ngspice 1 -> sysinfo
OS: CYGWIN_NT -5.1 1.5.25(0.156/4/2) 2008 -06 -12 19:34
CPU : Intel (R) Pentium (R) 4 CPU 3.40 GHz
Logical processors : 2
Total DRAM available = 1535.480469 MB.
DRAM currently available = 984.683594 MB.
ngspice 2 ->
This command has been tested under Windows OS and Linux. It may not be available in your
operating system environment.
17.5.77 Tf*: Run a Transfer Function analysis
General Form:
tf output_node input_source
The tf command performs a transfer function analysis, returning:
• the transfer function (output/input),
• output resistance,
• and input resistance
17.5. COMMANDS 341
between the given output node and the given input source. The analysis assumes a small-signal
DC (slowly varying) input. The following example file
Example input file:
* Tf test circuit
vs 1 0 dc 5
r1 1 2 100
r2 2 3 50
r3 3 0 150
r4 2 0 200
.control
tf v(3,5) vs
print all
.endc
.end
will yield the following output:
transfer_function = 3.750000e-001
output_impedance_at_v(3,5) = 6.662500e+001
vs#input_impedance = 2.000000e+002
17.5.78 Trace*: Trace nodes
General Form:
trace [ node ...]
For every step of an analysis, the value of the node is printed. Several traces may be active at
once. Tracing is not applicable for all analyses. To remove a trace, use the delete (17.5.16)
command.
17.5.79 Tran*: Perform a transient analysis
General Form:
tran Tstep Tstop [ Tstart [ Tmax ] ] [ UIC ]
Perform a transient analysis. See Chapt. 15.3.9 of this manual for more details.
An interactive transient analysis may be interrupted by issuing a ctrl-c (control-C) command.
The analysis then can be resumed by the resume command (17.5.53). Several options may be
set to control the simulation (15.1.4).
342 CHAPTER 17. INTERACTIVE INTERPRETER
17.5.80 Transpose: Swap the elements in a multi-dimensional data set
General Form:
transpose vector vector ...
This command transposes a multidimensional vector. No analysis in ngspice produces multidi-
mensional vectors, although the DC transfer curve may be run with two varying sources. You
must use the reshape command to reform the one-dimensional vectors into two dimensional
vectors. In addition, the default scale is incorrect for plotting. You must plot versus the vec-
tor corresponding to the second source, but you must also refer only to the first segment of
this second source vector. For example (circuit to produce the transfer characteristic of a MOS
transistor):
How to produce the transfer characteristic of a MOS transistor:
ngspice > dc vgg 0 5 1 vdd 0 5 1
ngspice > plot i( vdd)
ngspice > reshape all [6,6]
ngspice > transpose i( vdd) v( drain )
ngspice > plot i(vdd ) vs v(drain )[0]
17.5.81 Unalias: Retract an alias
General Form:
unalias [word ...]
Removes any aliases present for the words.
17.5.82 Undefine: Retract a definition
General Form:
undefine function
Definitions for the named user-defined functions are deleted.
17.5.83 Unlet: Delete the specified vector(s)
General Form:
unlet vector [ vector ... ]
Delete the specified vector(s). See also let (17.5.35).
17.5. COMMANDS 343
17.5.84 Unset: Clear a variable
General Form:
unset [word ...]
Clear the value of the specified variable(s) (word).
17.5.85 Version: Print the version of ngspice
General Form:
version [-s | -f | <version id >]
Print out the version of ngnutmeg that is running, if invoked without argument or with -s or -f.
If the argument is a <version id> (any string different from -s or -f is considered a <version id>
), the command checks to make sure that the arguments match the current version of ngspice.
(This is mainly used as a Command: line in rawfiles.)
Options description:
• No option: The output of the command is the message you can see when running ngspice
from the command line, no more no less.
•-s(hort): A shorter version of the message you see when calling ngspice from the com-
mand line.
•-f(ull): You may want to use this option if you want to know what extensions are included
into the simulator and what compilation switches are active. A list of compilation options
and included extensions is appended to the normal (not short) message. May be useful
when sending bug reports.
The following example shows what the command returns in some situations:
344 CHAPTER 17. INTERACTIVE INTERPRETER
Use of the version command:
ngspice 10 -> version
******
** ngspice -24 : Circuit level simulation program
** The U. C. Berkeley CAD Group
** Copyright 1985 -1994 , Regents of the University of California.
** Please get your ngspice manual from
http :// ngspice . sourceforge . net /docs .html
** Please file your bug - reports at
http :// ngspice . sourceforge . net / bugrep .html
** Creation Date: Jan 1 2011 13:36:34
******
ngspice 2 ->
ngspice 11 -> version 14
Note: rawfile is version 14 (current version is 24)
ngspice 12 -> version 24
ngspice 13 ->
Note for developers: The option listing returned when version is called with the
-f flag is built at compile time using #ifdef blocks. When new compile switches
are added, if you want them to appear on the list, you have to modify the code in
misccoms.c.
17.5.86 Where*: Identify troublesome node or device
General Form:
where
When performing a transient or operating point analysis, the name of the last node or device to
cause non-convergence is saved. The where command prints out this information so that you
can examine the circuit and either correct the problem or generate a bug report. You may do this
either in the middle of a run or after the simulator has given up on the analysis. For transient
simulation, the iplot command can be used to monitor the progress of the analysis. When the
analysis slows down severely or hangs, interrupt the simulator (with control-C) and issue the
where command. Note that only one node or device is printed; there may be problems with
more than one node.
17.5. COMMANDS 345
17.5.87 Wrdata: Write data to a file (simple table)
General Form:
<set wr_singlescale >
<set wr_vecnames >
< option numdgt =7 >
...
wrdata [file ] [ vecs]
Writes out the vectors to file.
This is a very simple printout of data in array form. Variables are written in pairs: scale vector,
value vector. If variable is complex, a triple is printed (scale, real, imag). If more than one
vector is given, the third column again is the default scale, the fourth the data of the second
vector. The default format is ASCII. All vectors have to stem from the same plot, otherwise a
segfault may occur. Setting wr_singlescale as variable, the scale vector will be printed only
once, if scale vectors are of the same length (you have to take care of that yourself). Setting
wr_vecnames as variable, scale and data vector names are printed on the first row. The number
of significant digits is set with option numdgt.
output example from two vectors:
0.000000 e+00 -1.845890e -06 0.000000e+00 0.000000e+00
7.629471 e+06 4.243518e -06 7.629471 e+06 -4.930171e -06
1.525894 e+07 -5.794628e -06 1.525894e+07 4.769020e-06
2.288841 e+07 5.086875e -06 2.288841 e+07 -3.670687e -06
3.051788 e+07 -3.683623e -06 3.051788e+07 1.754215e-06
3.814735 e+07 1.330798e -06 3.814735 e+07 -1.091843e -06
4.577682 e+07 -3.804620e -07 4.577682e+07 2.274678e-06
5.340630 e+07 9.047444e -07 5.340630 e+07 -3.815083e -06
6.103577 e+07 -2.792511e -06 6.103577e+07 4.766727e-06
6.866524 e+07 5.657498e -06 6.866524 e+07 -2.397679e -06
....
If variable appendwrite is set, the data may be added to an existing file.
17.5.88 Write: Write data to a file (Spice3f5 format)
General Form:
write [file ] [ exprs]
Writes out the expressions to file.
First vectors are grouped together by plots, and written out as such (i.e. if the expression list
contained three vectors from one plot and two from another, then two plots are written, one
with three vectors and one with two). Additionally, if the scale for a vector isn’t present it is
automatically written out as well.
346 CHAPTER 17. INTERACTIVE INTERPRETER
The default format is a compact binary, but this can be changed to ASCII with the set file-
type=ascii command. The default file name is either rawspice.raw or the argument of the
optional -r flag on the command line, and the default expression list is all.
If variable appendwrite is set, the data may be added to an existing file.
17.5.89 Wrs2p: Write scattering parameters to file (Touchstone® format)
General Form:
wrs2p [file ]
Writes out the s-parameters of a two-port to file.
In the active plot the following is required: vectors frequency, S11 S12 S21 S22, all having the
same length and complex values (as a result of an ac analysis), and vector Rbase. For details
how to generate these data see Chapt. 17.9.
The file format is Touchstone® Version 1, ASCII, frequency in Hz, real and imaginary parts of
Snn versus frequency.
The default file name is s-param.s2p.
output example:
!2 - port S-parameter file
!Title : test for scattering parameters
!Generated by ngspice at Sat Oct 16 13:51:18 2010
# Hz S RI R 50
!freq ReS11 ImS11 ReS21
...
2.500000 e+06 -1.358762e -03 -1.726349e -02 9.966563e-01
5.000000 e+06 -5.439573e -03 -3.397117e -02 9.867253e-01 ...
17.5.90 Xgraph: use the xgraph(1) program for plotting.
General Form:
xgraph file [exprs ] [plot options ]
The ngspice/ngnutmeg xgraph command plots data like the plot command but via xgraph, a
popular X11 plotting program. If file is either temp or tmp a temporary file is used to hold the
data while being plotted. For available plot options, see the plot command. All options except
for polar or smith plots are supported.
17.6. CONTROL STRUCTURES 347
17.6 Control Structures
17.6.1 While - End
General Form:
while condition
statement
...
end
While condition, an arbitrary algebraic expression, is true, execute the statements.
17.6.2 Repeat - End
General Form:
repeat [number]
statement
...
end
Execute the statements number times, or forever if no argument is given.
17.6.3 Dowhile - End
General Form:
dowhile condition
statement
...
end
The same as while, except that the condition is tested after the statements are executed.
17.6.4 Foreach - End
General Form:
foreach var value ...
statement
...
end
The statements are executed once for each of the values, each time with the variable var set to
the current one. (var can be accessed by the $var notation - see below).
348 CHAPTER 17. INTERACTIVE INTERPRETER
17.6.5 If - Then - Else
General Form:
if condition
statement
...
else
statement
...
end
If the condition is non-zero then the first set of statements are executed, otherwise the second
set. The else and the second set of statements may be omitted.
17.6.6 Label
General Form:
label word
If a statement of the form goto word is encountered, control is transferred to this point, other-
wise this is a no-op.
17.6.7 Goto
General Form:
goto word
If a statement of the form label word is present in the block or an enclosing block, control is
transferred there. Note that if the label is at the top level, it must be before the goto statement
(i.e, a forward goto may occur only within a block). A block to just include goto on the top
level may look like the following example.
Example noop block to include forward goto on top level:
if (1)
...
goto gohere
...
label gohere
end
17.7. INTERNALLY PREDEFINED VARIABLES 349
17.6.8 Continue
General Form:
continue
If there is a while,dowhile, or foreach block enclosing this statement, control passes to the
test, or in the case of foreach, the next value is taken. Otherwise an error results.
17.6.9 Break
General Form:
break
If there is a while,dowhile, or foreach block enclosing this statement, control passes out of
the block. Otherwise an error results.
Of course, control structures may be nested. When a block is entered and the input is the
terminal, the prompt becomes a number of >’s corresponding to the number of blocks the user
has entered. The current control structures may be examined with the debugging command
cdump (see 17.5.9).
17.7 Internally predefined variables
The operation of both ngutmeg and ngspice may be affected by setting variables with the set
command (17.5.59). In addition to the variables mentioned below, the set command also
affects the behavior of the simulator via the options previously described under the section
on .OPTIONS (15.1). You also may define new variables or alter existing variables inside
.control ... .endc for later use in a user-defined script (see Chapt. 17.8).
The following list is in alphabetical order. All of these variables are acknowledged by ngspice.
Frontend variables (e.g. on circuits and simulation) are not defined in ngnutmeg. The predefined
variables that may be set or altered by the set command are:
appendwrite Append to the file when a write command is issued, if one already exists.
askquit Check to make sure that there are circuits suspended or plots unsaved. ngspice warns
the user when he tries to quit if this is the case.brief If set to FALSE, the netlist will be
printed.
batchmode Set by ngspice if run with the -b command line parameter. May be used in input
files to suppress plotting if ngspice runs in batch mode.
colorN These variables determine the colors used, if X is being run on a color display. N may
be between 0 and 15. Color 0 is the background, color 1 is the grid and text color, and
colors 2 through 15 are used in order for vectors plotted. The value of the color variables
should be names of colors, which may be found in the file /usr/lib/rgb.txt. ngspice
for Windows does support only white background (color0=”white” with black grid and
text) or or color0=”black” with white grid and text.
350 CHAPTER 17. INTERACTIVE INTERPRETER
cpdebug Print control debugging information.
curplotdate Sets the date of the current plot.
curplotname Sets the name of the current plot.
curplottitle Sets the title (a short description) of the current plot.
debug If set then a lot of debugging information is printed.
device The name (/dev/tty??) of the graphics device. If this variable isn’t set then the
user’s terminal is used. To do plotting on another monitor you probably have to set both
the device and term variables. (If device is set to the name of a file, nutmeg dumps the
graphics control codes into this file – this is useful for saving plots.)
diff_abstol The relative tolerance used by the diff command (default is 1e-12).
diff_reltol The relative tolerance used by the diff command (default is 0.001).
diff_vntol The absolute tolerance for voltage type vectors used by the diff command (default
is 1e-6).
echo Print out each command before it is executed.
editor The editor to use for the edit command.
filetype This can be either ascii or binary, and determines the format of the raw file
(compact binary or text editor readable ascii). The default is binary.
fourgridsize How many points to use for interpolating into when doing Fourier analysis.
gridsize If this variable is set to an integer, this number is used as the number of equally
spaced points to use for the Y axis when plotting. Otherwise the current scale is used
(which may not have equally spaced points). If the current scale isn’t strictly monotonic,
then this option has no effect.
gridstyle Sets the grid during plotting with the plot command. Will be overridden by direct
entry of gridstyle in the plot command. A linear grid is standard for both x and
y axis. Allowed values are lingrid loglog xlog ylog smith smithgrid polar
nogrid.
hcopydev If this is set, when the hardcopy command is run the resulting file is automatically
printed on the printer named hcopydev with the command lpr -Phcopydev -g file.
hcopyfont This variable specifies the font name for hardcopy output plots. The value is device
dependent.
hcopyfontsize This is a scaling factor for the font used in hardcopy plots.
hcopydevtype This variable specifies the type of the printer output to use in the hardcopy
command. If hcopydevtype is not set, Postscript format is assumed. plot (5) is re-
cognized as an alternative output format. When used in conjunction with hcopydev,
hcopydevtype should specify a format supported by the printer.
hcopyscale This is a scaling factor for the font used in hardcopy plots (between 0 and 10).
17.7. INTERNALLY PREDEFINED VARIABLES 351
hcopywidth Sets width of the hardcopy plot.
hcopyheight Sets height of the hardcopy plot.
hcopypscolor Sets the color of the hardcopy output. If not set, black & white plotting is
assumed with different linestyles for each output vector. A valid color integer value yields
a colored plot background (0: black 1: white, others see below). and colored solid lines.
This is valid for Postscript only.
hcopypstxcolor This variable sets the color of the text in the Postscript hardcopy output. If
not set, black on white background is assumed, else it will be white on black background.
Valid colors are 0: black 1: white 2: red 3: blue 4: orange 5: green 6: pink 7: brown 8:
khaki 9: plum 10: orchid 11: violet 12: maroon 13: turquoise 14: sienna 15: coral 16:
cyan 17: magenta 18: gray (for smith grid) 19: gray (for smith grid) 20: gray (for normal
grid).
height The length of the page for asciiplot and print col.
history The number of events to save in the history list.
interactive If interactive is set, numparam error handling may be done manually with
user input from the console. If not, ngspice will exit upon a numparam error.
lprplot5 This is a printf(3s) style format string used to specify the command to use for
sending plot(5)-style plots to a printer or plotter. The first parameter supplied is the
printer name, the second parameter is a file name containing the plot. Both parameters
are strings.
lprps This is a printf(3s) style format string used to specify the command to use for sen-
ding Postscript plots to a printer or plotter. The first parameter supplied is the printer
name, the second parameter is the file name containing the plot. Both parameters are
strings.
modelcard The name of the model card (normally .MODEL)
moremode If moremode is set, whenever a large amount of data is being printed to the screen
(e.g, the print or asciiplot commands), the output is stopped every screenful and
continues when a carriage return is typed. If moremode is unset, then data scrolls off the
screen without pausing.
nfreqs The number of frequencies to compute in the Fourier command. (Defaults to 10.)
ngbehavior Sets the compatibility mode of ngspice. To be set in spinit (16.5) or .spiceinit
(16.6). A value of ’all’ improves compatibility with commercial simulators. Full com-
patibility is however not the intention of ngspice! The values ’ps’,’hs’ and ’spice3’
are available. See Chapt. 16.13.
nobjthack BJTs can have either 3 or 4 nodes, which makes it difficult for the subcircuit ex-
pansion routines to decide what to rename. If the fourth parameter has been declared as a
model name, then it is assumed that there are 3 nodes, otherwise it is considered a node.
To disable this, you can set the variable nobjthack and force BJTs to have 4 nodes (for
the purposes of subcircuit expansion, at least).
352 CHAPTER 17. INTERACTIVE INTERPRETER
nobreak Don’t have asciiplot and print col break between pages.
noasciiplotvalue Don’t print the first vector plotted to the left when doing an asciiplot.
nobjthack Assume that BJTs have 4 nodes.
noclobber Don’t overwrite existing files when doing IO redirection.
noglob Don’t expand the global characters ‘*’, ‘?’, ‘[’, and ‘]’. This is the default.
nonomatch If noglob is unset and a global expression cannot be matched, use the global
characters literally instead of complaining.
noparse Don’t attempt to parse input files when they are read in (useful for debugging). Of
course, they cannot be run if they are not parsed.
noprintscale Don’t print the scale in the leftmost column when a print col command is
given.
nosort Don’t let display sort the variable names.
nosubckt Don’t expand subcircuits.
notrnoise Switch off the transient noise sources (Chapt. 4.1.7).
numdgt The number of digits to use when printing tables of data (print col). The default
precision is 6 digits. On the VAX, approximately 16 decimal digits are available using
double precision, so p should not be more than 16. If the number is negative, one fewer
digit is printed to ensure constant widths in tables.
num_threads The number of of threads to be used if OpenMP (see Chapt. 16.10) is selected.
The default value is 2.
outputpath Set the path for all ngspice outputs that are written to files. The directory must
exist. Path names with spaces are set in single quotes ’ ’, like set outputpath =
’C:\My Path’.
plotstyle This should be one of linplot,combplot, or pointplot.linplot, the default,
causes points to be plotted as parts of connected lines. combplot causes a comb plot
to be done. It plots vectors by drawing a vertical line from each point to the X-axis, as
opposed to joining the points. pointplot causes each point to be plotted separately.
pointchars Set a string as a list of characters to be used as points in a point plot. Standard is
‘ox*+#abcdefhgijklmnpqrstuvwyz’. Some characters are forbidden.
polydegree The degree of the polynomial that the plot command should fit to the data. If
polydegree is N, then nutmeg fits a degree N polynomial to every set of N points and
draws 10 intermediate points in between each end point. If the points aren’t monotonic,
then nutmeg tries to rotate the curve and reduce the degree until a fit is achieved.
polysteps The number of points to interpolate between every pair of points available when
doing curve fitting. The default is 10.
program The name of the current program (argv[0]).
17.7. INTERNALLY PREDEFINED VARIABLES 353
prompt The prompt, with the character ‘!’ replaced by the current event number. Single quotes
’ ’ are required around the specified string unless you really want it expanded.
rawfile The default name for created rawfiles.
remote_shell Overrides the name used for generating rspice runs (default is rsh).
renumber Renumber input lines when an input file has .includes.
rndseed Seed value for random number generator (used by sgauss,sunif, and rnd functi-
ons). If not set, the process Id is used as seed value.
rhost The machine to use for remote ngspice runs, instead of the default one (see the descrip-
tion of the rspice command, below).
rprogram The name of the remote program to use in the rspice command.
sharedmode Variable is set when ngspice runs in its shared mode (from ngspice.dll or ng-
spice_xx.so). May be used in universal input files to suppress plotting because a graphics
interface is lacking.
sourcepath A list of the directories to search when a source command is given. The default
is the current directory and the standard ngspice library (/usr/local/lib/ngspice, or
whatever LIBPATH is #defined to in the ngspice source). The command
set sourcepath = ( e:/ D:/ . c:/spice/examples )
will overwrite the default. The search sequence now is: current directory, e:/,d:/, current
directory (again due to .), c:/spice/examples. ’Current directory’ is depending on the
OS.
specwindow Windowing for commands spec (17.5.71) or fft (17.5.26). May be one of the
following: bartlet blackman cosine gaussian hamming hanning none rectangular
triangle.
specwindoworder Integer value 2 - 8 (default 2), used by commands spec or fft.
spicepath The program to use for the aspice command. The default is /cad/bin/spice.
sqrnoise If set, noise data outputs will be given as V^2/Hz or A^2/Hz, otherwise as the usual
V/√Hz or A/√Hz.
strict_errorhandling If set by the user, an error detected during circuit parsing will im-
mediately lead ngspice to exit with exit code 1 (see 18.5). May be set in files spinit (16.5)
or .spiceinit (16.6) only.
subend The card to end subcircuits (normally .ends).
subinvoke The prefix to invoke subcircuits (normally X).
substart The card to begin subcircuits (normally .subckt).
term The mfb name of the current terminal.
ticmarks An integer value n, n tics (a small ’x’) will be set on your graph.
ticlist A list of integers, e.g. ( 4 14 24 ) to set tics (small ’x’) on your graph.
354 CHAPTER 17. INTERACTIVE INTERPRETER
units If this is degrees, then all the trig functions will use degrees instead of radians.
unixcom If a command isn’t defined, try to execute it as a UNIX command. Setting this option
has the effect of giving a rehash command, below. This is useful for people who want
to use ngnutmeg as a login shell.
wfont Set the font for the graphics plot in MS Windows. Typical fonts are courier, times,
arial and all others found on your machine. Default is courier.
wfont_size The size of the windows font. The default depends on system settings.
width The width of the page for asciiplot and print col (see also 15.6.7).
win_console is set when ngspice runs in a console under Windows.
x11lineararcs Some X11 implementations have poor arc drawing. If you set this option,
ngspice will plot using an approximation to the curve using straight lines.
xbrushwidth Linewidth for grid, border and graph.
xfont Set the font for the graphics plot in X11 (Linux, Cygwin, etc.). Input format still has to
be checked.
xtrtol Set trtol, e.g. to 7, to avoid the default speed reduction (accuracy increase) for
XSPICE (see 16.9). Be aware of potential precision degradation or convergence issues
using this option.
17.8 Scripts
Expressions, functions, constants, commands, variables, vectors, and control structures may be
assembled into scripts within a .control ... .endc section of the input file. The script allows
to automate any ngspice task: simulations to perform, output data to analyze, repeat simulations
with modified parameters, assemble output plot vectors. The ngspice scripting language is not
very powerful, but well integrated into the simulation flow.
The ngspice script input file contains the usual circuit netlist, modelcards, and the actual script,
enclosed in a .control .. .endc section. Ngspice is started in interactive mode with the
input file on the command line (or sourced later with the source command). After reading the
input file the command sequence is immediately processed. Variables or vectors set by previous
commands may be referenced by the commands following them. Data can be stored, plotted or
grouped into new vectors for either plotting or other means of data evaluation.
The input file may contain only the .control .. .endc section. To notify ngspice about this
(not mandatory), the script may start with *ng_script in the first line.
17.8.1 Variables
Variables are defined and initialized with the set command (17.5). set output=10 defines
the variable output and sets it to the (real) number 10. Predefined variables, which are used
inside ngspice for specific purposes, are listed in Chapt. 17.7. Variables are accessible globally.
17.8. SCRIPTS 355
The values of variables may be used in commands by writing $varname where the value of
the variable is to appear, e.g. $output. The special variable $$ refers to the process ID of the
program. With $< a line of input is read from the terminal. If a variable is assigned with to
with $&word, then word must be a vector (see below), and word’s numeric value is taken to be
the new value of the variable. If foo is a valid variable, and is of type list, then the expression
$foo[low-high] expands to a range of elements. Either the upper or lower index may be left
out, and in addition to slicing also reversing of a list is possible through $foo[len-0] (len
is the length of the list, the first valid index is always 1). Furthermore, the notation $?foo
evaluates to 1 if the variable foo is defined, 0 otherwise, and $#foo evaluates to the number of
elements in foo if it is a list, 1 if it is a number or string, and 0 if it is a Boolean variable.
17.8.2 Vectors
Ngspice and ngnutmeg data is in the form of vectors: time, voltage, etc. Each vector has a
type, and vectors can be operated on and combined algebraically in ways consistent with their
types. Vectors are normally created as a result of a transient or dc simulation. They are also
established when a data file is read in (see the load command 17.5.38), or they are created
with the let command 17.5.35 inside a script. If a variable xis assigned something of the form
$&word, then word has to be a vector, and the numeric value of word is transferred into the
variable x.
17.8.3 Commands
Commands have been described in Chapt. 17.5.
17.8.4 control structures
Control structures have been described in Chapt. 17.6. Some simple examples will be given
below.
356 CHAPTER 17. INTERACTIVE INTERPRETER
Control structure examples:
Test sequences for ngspice control structures
*vectors are used ( except foreach )
*start in interactive mode
.control
* test sequence for while , dowhile
let loop = 0
echo
echo enter loop with "$&loop "
dowhile loop < 3
echo within dowhile loop "$& loop"
let loop = loop + 1
end
echo after dowhile loop "$& loop "
echo
let loop = 0
while loop < 3
echo within while loop "$&loop "
let loop = loop + 1
end
echo after while loop "$&loop "
let loop = 3
echo
echo enter loop with "$&loop "
dowhile loop < 3
echo within dowhile loop "$& loop"
$ output expected
let loop = loop + 1
end
echo after dowhile loop "$& loop "
echo
let loop = 3
while loop < 3
echo within while loop "$&loop "
$ no output expected
let loop = loop + 1
end
echo after while loop "$&loop "
17.8. SCRIPTS 357
Control structure examples (continued):
* test for while , repeat , if , break
let loop = 0
while loop < 4
let index = 0
repeat
let index = index + 1
if index > 4
break
end
end
echo index "$& index " loop "$&loop "
let loop = loop + 1
end
* test sequence for foreach
echo
foreach outvar 0 0.5 1 1.5
echo parameters : $outvar $ foreach parameters are variables ,
$ not vectors !
end
* test for if ... else ... end
echo
let loop = 0
let index = 1
dowhile loop < 10
let index = index * 2
if index < 128
echo "$&index " lt 128
else
echo "$& index" ge 128
end
let loop = loop + 1
end
* simple test for label , goto
echo
let loop = 0
label starthere
echo start "$&loop "
let loop = loop + 1
if loop < 3
goto starthere
end
echo end "$&loop "
358 CHAPTER 17. INTERACTIVE INTERPRETER
Control structure examples (continued):
* test for label , nested goto
echo
let loop = 0
label starthere1
echo start nested "$&loop "
let loop = loop + 1
if loop < 3
if loop < 3
goto starthere1
end
end
echo end "$&loop "
* test for label , goto
echo
let index = 0
label starthere2
let loop = 0
echo We are at start with index "$& index " and loop "$& loop"
if index < 6
label inhere
let index = index + 1
if loop < 3
let loop = loop + 1
if index > 1
echo jump2
goto starthere2
end
end
echo jump
goto inhere
end
echo We are at end with index "$&index " and loop "$&loop "
17.8. SCRIPTS 359
Control structure examples (continued):
* test goto in while loop
let loop = 0
if 1 $ outer loop to allow nested forward label ’endlabel ’
while loop < 10
if loop > 5
echo jump
goto endlabel
end
let loop = loop + 1
end
echo before $ never reached
label endlabel
echo after "$&loop "
end
* test for using variables , simple test for label , goto
set loop = 0
label starthe
echo start $loop
let loop = $loop + 1 $ expression needs vector at lhs
set loop = "$& loop" $ convert vector contents to variable
if $loop < 3
goto starthe
end
echo end $loop
.endc
17.8.5 Example script ’spectrum’
A typical example script named spectrum is delivered with the ngspice distribution. Even if
it is made obsolete by the internal spec command (see 17.5.71), and especially by the much
faster fft command (see 17.5.26), it is a good example for getting acquainted with the ngspice
(or nutmeg) post-processor language.
As a suitable input for spectrum you may run a ring-oscillator, delivered with ngspice in e.g.
test/bsim3soi/ring51_41.cir. For an adequate resolution a simulation time of 1µs is needed. A
small control script starts ngspice by loading the R.O. simulation data and executing spectrum.
Small script to start ngspice, read the simulation data and start spectrum:
* test for script ’spectrum ’
.control
load ring51_41 .out
spectrum 10 MEG 2500 MEG 1MEG v( out25) v( out50 )
.endc
360 CHAPTER 17. INTERACTIVE INTERPRETER
17.8. SCRIPTS 361
17.8.6 Example script for random numbers
Generation and test of random numbers with Gaussian distribution
* agauss test in ngspice
* generate a sequence of gaussian distributed random numbers .
* test the distribution by sorting the numbers into
* a histogram ( buckets)
.control
define agauss(nom , avar , sig) (nom + avar /sig * sgauss (0))
let mc_runs = 200
let run = 0
let no_buck = 8 $ number of buckets
let bucket = unitvec (no_buck ) $ each element contains 1
let delta = 3e -11 $ width of each bucket , depends
$ on avar and sig
let lolimit = 1e-09 - 3* delta
let hilimit = 1e -09 + 3* delta
dowhile run < mc_runs
let val = agauss (1e -09 , 1e -10 , 3) $ get the random number
if (val < lolimit)
let bucket [0] = bucket [0] + 1 $ ’lowest ’ bucket
end
let part = 1
dowhile part < ( no_buck - 1)
if (( val < ( lolimit + part * delta )) &
+ ( val > (lolimit + ( part -1)* delta )))
let bucket[ part ] = bucket[part ] + 1
break
end
let part = part + 1
end
if (val > hilimit)
* ’highest ’ bucket
let bucket[ no_buck - 1] = bucket[ no_buck - 1] + 1
end
let run = run + 1
end
let part = 0
dowhile part < no_buck
let value = bucket [ part] - 1
set value = "$& value "
* print the bucket ’s contents
echo $value
let part = part + 1
end
.endc
.end
362 CHAPTER 17. INTERACTIVE INTERPRETER
17.8.7 Parameter sweep
While there is no direct command to sweep a device parameter during simulation, you may use
a script to emulate such behavior. The example input file contains of an resistive divider with
R1 and R2, where R1 is swept from a start to a stop value inside of the control section, using
the alter command (see 17.5.3).
Input file with parameter sweep
parameter sweep
* resistive divider , R1 swept from start_r to stop_r
VDD 1 0 DC 1
R1 1 2 1k
R2 2 0 1k
.control
let start_r = 1k
let stop_r = 10k
let delta_r = 1k
let r_act = start_r
* loop
while r_act le stop_r
alter r1 r_act
op
print v(2)
let r_act = r_act + delta_r
end
.endc
.end
17.8.8 Output redirection
The console outputs delivered by commands like print (17.5.47), echo (17.5.21), or others may
be redirected into a text file. ’print vec > filename’ will generate a new file or overwrite
an existing file named ’filename’, ’echo text >> filename’ will append the new data to
the file ’filename’. Output redirection may be mixed with commands like wrdata.
17.8. SCRIPTS 363
Input file with output redirection >and >>
** MOSFET Gain Stage (AC):
** Benchmarking Implementation of BSIM4 .0.0
** by Weidong Liu 5/16/2000.
** output redirection into file
M1 3 2 0 0 N1 L=1u W=4u
Rsource 1 2 100k
Rload 3 vdd 25k
Vdd vdd 0 1.8
Vin 1 0 1.2 ac 0.1
.control
ac dec 10 100 1000 Meg
plot v(2) v(3)
let flen = length( frequency) $ length of the vector
let loopcounter = 0
echo output test > text .txt $ start new file test.txt
* loop
while loopcounter lt flen
let vout2 = v(2)[ loopcounter ] $ generate a single point
$ complex vector
let vout2re = real ( vout2) $ generate a single point
$ real vector
let vout2im = imag ( vout2) $ generate a single point
$ imaginary vector
let vout3 = v(3)[ loopcounter ] $ generate a single
$ point complex vector
let vout3re = real ( vout3) $ generate a single point
$ real vector
let vout3im = imag ( vout3) $ generate a single point
$ imaginary vector
let freq = frequency [ loopcounter ] $ generate a single point vector
echo bbb "$&freq " "$& vout2re " "$& vout2im "
+ "$& vout3re " "$& vout3im " >> text.txt
$ append text and
$ data to file
$ (continued from line above )
let loopcounter = loopcounter + 1
end
.endc
.MODEL N1 NMOS LEVEL =14 VERSION =4.8.1 TNOM =27
.end
364 CHAPTER 17. INTERACTIVE INTERPRETER
17.9 Scattering parameters (s-parameters)
17.9.1 Intro
A command line script, available from the ngspice distribution at examples/control_structs/s-
param.cir, together with the command wrs2p (see Chapt. 17.5.89) allows to calculate, print
and plot the scattering parameters S11, S21, S12, and S22 of any two port circuit at varying
frequencies.
The printed output using wrs2p is a Touchstone® version 1 format file. The file follows the
format according to The Touchstone File Format Specification, Version 2.0, available from here.
An example is given as number 13 on page 15 of that specification.
17.9.2 S-parameter measurement basics
S-parameters allow a two-port description not just by permuting I1,U1,I2,U2, but using a
superposition, leading to a power view of the port (We only look at two-ports here, because
multi-ports are not (yet?) implemented.).
You may start with the effective power, being negative or positive
P=u·i(17.1)
The value of Pmay be the difference of two real numbers, with Kbeing another real number.
ui =P=a2−b2= (a+b)(a−b)=(a+b)(KK−1)(a−b) = {K(a+b)}K−1(a−b)(17.2)
Thus you get
K−1u=a+b(17.3)
Ki =a−b(17.4)
and finally
a=u+K2i
2K(17.5)
b=u−K2i
2K(17.6)
By introducing the reference resistance Z0:=K2>0 we get finally the Heaviside transformation
a=u+Z0i
2√Z0
,b=u−Z0i
2√Z0
(17.7)
17.9. SCATTERING PARAMETERS (S-PARAMETERS) 365
In case of our two-port we subject our variables to a Heaviside transformation
a1=U1+Z0I1
2√Z0
b1=U1−Z0I1
2√Z0
(17.8)
a2=U2+Z0I2
2√Z0
b2=U2−Z0I2
2√Z0
(17.9)
The s-matrix for a two-port then is
b1
b2=s11 s12
s21 s22 a1
a2(17.10)
Two obtain s11 we have to set a2=0. This is accomplished by loading the output port exactly
with the reference resistance Z0,which sinks a current I2=−U2/Z0from the port.
s11 =b1
a1a2=0
(17.11)
s11 =U1−Z0I1
U1+Z0I1
(17.12)
Loading the input port from an ac source U0via a resistor with resistance value Z0, we obtain
the relation
U0=Z0I1+U1(17.13)
Entering this into 17.12, we get
s11 =2U1−U0
U0
(17.14)
For s21 we obtain similarly
s21 =b2
a1a2=0
(17.15)
s21 =U2−Z0I2
U1+Z0I1
=2U2
U0
(17.16)
Equations 17.14 and 17.16 now tell us how to measure s11 and s21: Measure U1at the input port,
multiply by 2 using an E source, subtracting U0, which for simplicity is set to 1, and divide by
U0. At the same time measure U2at the output port, multiply by 2 and divide by U0. Biasing and
measuring is done by subcircuit S_PARAM. To obtain s22 and s12, you have to exchange the
input and output ports of your two-port and do the same measurement again. This is achieved
by switching resistors from low (1mΩ) to high (1TΩ) and thus switching the input and output
ports.
366 CHAPTER 17. INTERACTIVE INTERPRETER
17.9.3 Usage
Copy and then edit s-param.cir. You will find this file in directory /examples/control_structs
of the ngspice distribution.
The reference resistance (often called characteristic impedance) for the measurements is added
as a parameter
.param Rbase=50
The bias voltages at the input and output ports of the circuit are set as parameters as well:
.param Vbias_in=1 Vbias_out=2
Place your circuit at the appropriate place in the input file, e.g. replacing the existing example
circuits. The input port of your circuit has two nodes in, 0. The output port has the two nodes
out, 0. The bias voltages are connected to your circuit via the resistances of value Rbase at the
input and output respectively. This may be of importance for the operating point calculations if
your circuit draws a large dc current.
Now edit the ac commands (see 17.5.1) according to the circuit provided, e.g.
ac lin 100 2.5MEG 250MEG $ use for Tschebyschef
Be careful to keep both ac lines in the .control ... .endc section the same and only change
both in equal measure!
Select the plot commands (lin/log, or smithgrid) or the ’write to file’ commands (write,
wrdata, or wrs2p) according to your needs.
Run ngspice in interactive mode
ngspice s-param.cir
17.10 MISCELLANEOUS
C-shell type quoting with ’and ’, and backquote substitution may be used. Within single
quotes, no further substitution (like history substitution) is done, and within double quotes,
the words are kept together but further substitution is done. Any text between backquotes is
replaced by the result of executing the text as a command to the shell.
History substitutions, similar to C-shell history substitutions, are also available - see the
C-shell manual page for all of the details. The characters ~, @{, and @} have the same effects
as they do in the C-Shell, i.e., home directory and alternative expansion. It is possible to use the
wildcard characters *, ?, [, and ] also, but only if you unset noglob first. This makes them rather
useless for typing algebraic expressions, so you should set noglob again after you are done with
wildcard expansion. Note that the pattern [^abc] matches all characters except a, b, and c.
If X is being used, the cursor may be positioned at any point on the screen when the window
is up and characters typed at the keyboard are added to the window at that point. The window
may then be sent to a printer using the xpr(1) program.
17.11. BUGS 367
17.11 Bugs
When defining aliases like alias pdb plot db(!:1 -!:2 ) you must be careful to quote the
argument list substitutions in this manner. If you quote the whole argument it might not work
properly.
In a user-defined function, the arguments cannot be part of a name that uses the plot.vec syntax.
For example: define check(v(1)) cos(tran1.v(1)) does not work.
368 CHAPTER 17. INTERACTIVE INTERPRETER
Chapter 18
Ngspice User Interfaces
ngspice offers a variety of user interfaces. For an overview (several screen shots) please have a
look at the ngspice web page.
18.1 MS Windows Graphical User Interface
If compiled properly (e.g. using the --with-wingui flag for ./configure under MINGW),
ngspice for Windows offers a simple graphical user interface. In fact this interface does not
offer much more for data input than a console would offer, e.g. command line inputs, command
history and program text output. First of all it applies the Windows api for data plotting. If you
run the sample input file given below, you will get an output as shown in Fig. 18.1.
Input file:
***** Single NMOS Transistor For BSIM3V3 .1
***** general purpose check (Id -Vd) ***
*
*** circuit description ***
m1 2 1 3 0 n1 L =0.6 u W=10.0 u
vgs 1 0 3.5
vds 2 0 3.5
vss 3 0 0
*
.dc vds 0 3.5 0.05 vgs 0 3.5 0.5
*
.control
run
plot vss # branch
.endc
*
* UCB parameters BSIM3v3 .2
.include ../ Exam_BSIM3 / Modelcards /modelcard .nmos
.include ../ Exam_BSIM3 / Modelcards /modelcard .pmos
*
.end
369
370 CHAPTER 18. NGSPICE USER INTERFACES
The GUI consists of an I/O port (lower window) and a graphics window, created by the plot
command.
Figure 18.1: MS Windows GUI
The output window displays messages issued by ngspice. You may scroll the window to get
more of the text. The input box (white box) may be activated by a mouse click to accept any
of the valid ngspice commends. The lower left output bar displays the actual input file. ngspice
progress during setup and simulation is shown in the progress window (--ready--). The Quit
button allow to interrupt ngspice. If ngspice is actively simulating, due to using only a single
thread, this interrupt has to wait until the window is accessible from within ngspice, e.g. during
an update of the progress window.
In the plot window there is the upper left button, which activated a drop down menu. You may
select to print the plot window shown (a very simple printer interface, to be improved), set
up any of the printers available on your computer, or issue a postscript file of the actual plot
window, either black&white or colored.
18.2. MS WINDOWS CONSOLE 371
Instead of plotting with black background, you may set the background to any other color,
preferably to ‘white’ using the command shown below.
Input file modification for white background:
.control
run
* white background
set color0 =white
* black grid and text (only needed with X11 , automatic with MS Win)
set color1 =black
* wider grid and plot lines
set xbrushwidth =2
plot vss # branch
.endc
Figure 18.2: Plotting with white background
18.2 MS Windows Console
If the --with-wingui flag for ./configure under MINGW is omitted (see 32.2.5) or con-
sole_debug or console_release is selected in the MS Visual Studio configuration manager, then
ngspice will compile without any internal graphical input or output capability. This may be use-
ful if you apply ngspice in a pipe inside the MSYS window, or use it being called from another
program, and just generating output files from a given input. The plot (17.5.45) command will
not do and leads to an error message.
372 CHAPTER 18. NGSPICE USER INTERFACES
Only on the ngspice console binary in MS Windows input/output redirection is possible, if
ngspice is called (e.g. within a MSYS shell or from a shell script) like
$ ngspice < input.
This feature is used in the new CMC model test suite (to be described elsewhere), thus requires
a console binary.
You still may generate graphics output plots or prints by (17.5.28), if installed properly (18.7),
or by selecting a suitable printing option (18.6).
18.3 Linux
The standard user interface is a console for input and the X11 graphics system for output with
the interactive plot (17.5.45) command. If ngspice is compiled with the –without-x flag for
./configure, a console application without graphical interface results. For more sophisticated
input user interfaces please have a look at Chapt. 18.8.
18.4 CygWin
The CygWin interface is similar to the Linux interface (18.3), i.e. console input and X11
graphics output. To avoid the warning of a missing graphical user interface, you have to start
the X11 window manager by issuing the commands
$ export DISPLAY=:0.0
$ xwin -multiwindow -clipboard &
inside of the CygWin window before starting ngspice.
18.5 Error handling
Error messages and error handling in ngspice have grown over the years, include a lot of ‘tradi-
tional’ behavior and thus are not very systematic and consistent.
Error messages may occur with the token ‘Error:’. Often the errors are non-recoverable and will
lead to exiting ngspice with error code 1. Sometimes, however, you will get an error message,
but ngspice will continue, and may either bail out later because the error has propagated into
the simulation, sometimes ngspice will continue, deliver wrong results and exit with error code
0 (no error detected!).
In addition ngspice may issue warning messages like ‘Warning: ...’. These should cover reco-
verable errors only.
So there is still work to be done to define a consistent error messaging, recovery or exiting. A
first step is the user definable variable strict_errorhandling. This variable may be set in files
spinit (16.5) or .spiceinit (16.6) to immediately stop ngspice, after an error is detected during
parsing the circuit. An error message is sent, the ngspice exit code is 1. This behavior deviates
from traditional SPICE error handling and thus is introduced as an option only.
XSPICE error messages are explained in Chapt. 29.
18.6. POSTSCRIPT PRINTING OPTIONS 373
18.6 Postscript printing options
This info is compiled from Roger L. Traylor’s web page. All the commands and variables you
can set are described in Chapt. 17.5. The corresponding input file for the examples given below
is listed in Chapt. 21.1. Just add the .control section to this file and run in interactive mode
by
$ ngspice xspice_c1_print.cir
One way is to setup your printing like this:
.control
set hcopydevtype=postscript
op
run
plot vcc coll emit
hardcopy temp.ps vcc coll emit
.endc
Then print the postscript file temp.ps to a postscript printer.
You can add color traces to it if you wish:
.control
set hcopydevtype=postscript
* allow color and set background color if set to value > 0
set hcopypscolor=1
*color0 is background color
*color1 is the grid and text color
*colors 2-15 are for the vectors
set color0=rgb:f/f/f
set color1=rgb:0/0/0
op
run
hardcopy temp.ps vcc coll emit
.endc
Then print the postscript file temp.ps to a postscript printer.
You can also direct your output directly to a designated printer (not available in MS Windows):
.control
set hcopydevtype=postscript
*send output to the printer kec3112-clr
set hcopydev=kec3112-clr
hardcopy out.tmp vcc coll emit
374 CHAPTER 18. NGSPICE USER INTERFACES
18.7
Install (on Linux available from the distribution, on Windows available here). On Windows
expand the zip file to a directory of your choice, add the path <any directory>//bin to the
PATH variable, and go... The command to invoke (17.5.28) is limited however to x/y plots (no
polar etc.).
18.8 Integration with CAD software and ‘third party’ GUIs
In this chapter you will find some links and comments on GUIs for ngspice offered from other
projects and on the integration of ngspice into a circuit development flow. The data given rely
mostly on information available from the web and thus is out of our control. It also may be far
from complete. The GUIs KJWaves and GNUSpiceGUI help you to navigate the commands
to need to perform your simulation. XCircuit and the GEDA tools gschem and gnetlist offer
integrating schematic capture and simulation.
18.8.1 KJWaves
KJWaves was written to be a cross-platform SPICE tool in pure Java. It aids in viewing,
modifying, and simulating SPICE CIRCUIT files. Output from SPICE3 (ngspice) can be
read and displayed. Resulting graphs may be printed and saved. The Java executable will
run under Linux and Windows (and maybe other OSs). The development site is available at
http://sourceforge.net/projects/kjwaves/. You may find the project home page at http://www.comefly.us/.
18.8.2 GNU Spice GUI
Another GUI, to be found at http://sourceforge.net/projects/gspiceui/.
18.8.3 XCircuit
CYGWIN and especially Linux users may find XCircuit valuable to establish a development
flow including schematic capture and circuit simulation.
18.8.4 GEDA
The gEDA project is developing a full GPL‘d suite and toolkit of Electronic Design Automation
tools for use with a Linux. Ngspice may be integrated into the development flow. Two web sites
offer tutorials using gschem and gnetlist with ngspice:
http://geda.seul.org/wiki/geda:csygas
http://geda.seul.org/wiki/geda:ngspice_and_gschem
18.8. INTEGRATION WITH CAD SOFTWARE AND ‘THIRD PARTY’ GUIS 375
18.8.5 CppSim
A complete simulation environment called CppSim has been developed and made available for
system level simulation of complex mixed signal circuits. ngspice has been integrated into the
simulation flow, as described here.
18.8.6 NGSPICE Online
A web browser based interface is offered here. Simulation is performed on a remote server. The
project is not directly linked to our ngspice development project.
18.8.7 Spicy Schematics
An IPAD and web interface (including schematics entry) to ngspice is offered here.Simulation
is performed on a remote server.
18.8.8 MSEspice
Agraphical front end to ngspice, using the Free Pascal cross platform RAD environment
MSEide+MSEgui.
18.8.9 PartSim
Aweb based guiin your browser, including schematics entry. Simulation is performed on a
remote server.
376 CHAPTER 18. NGSPICE USER INTERFACES
Chapter 19
ngspice as shared library or dynamic link
library
ngspice may be compiled as a shared library. This allows adding ngspice to an application
that then gains control over the simulator. The shared module offers an interface that exports
functions controlling the simulator and callback functions for feedback.
So you may send an input ‘file’ with a netlist to ngspice, start the simulation in a separate thread,
read back simulation data at each time point, stop the simulator depending on some condition,
alter device or model parameters and then resume the simulation.
Shared ngspice does not have any user interface. The calling process is responsible for this. It
may offer a graphical user interface, add plotting capability or any other interactive element.
You may develop and optimize these user interface elements without a need to alter the ngspice
source code itself, using a console application or GUIs like gtk, Delphi, Qt or others.
19.1 Compile options
19.1.1 How to get the sources
Currently (as of ngspice-26 being the actual release), you will have to use the direct loading of
the sources from the git repository (see Chapt. 32.1.2).
19.1.2 Linux, MINGW, CYGWIN
Compilation is done as described in chapts. 32.1 or 32.2.2.Use the configure option --with-ngshared
instead of --with-x or --with-wingui.
Other operation systems (Mac OS, BSD, ...) have not been tested so far. Your input is welcome!
19.1.3 MS Visual Studio
Compilation is similar to what has been described in Chapt. ??. However, there is a dedicated
project file coming with the source code to generate ngspice.dll. Go to the directory visualc
and start the project with double clicking on sharedspice.vcxproj.
377
378 CHAPTER 19. NGSPICE AS SHARED LIBRARY OR DYNAMIC LINK LIBRARY
19.2 Linking shared ngspice to a calling application
Basically there are two methods (as with all *.so,*.dll libraries). The caller may link to a (small)
library file during compiling/linking, and then immediately search for the shared library upon
being started. It is also possible to dynamically load the ngspice shared library at runtime using
the dlopen/LoadLibrary mechanisms.
19.2.1 Linking during creating the caller
While creating the ngspice shared lib, not only the *.so (*.dll) file is created, but also a small
library file, which just includes references to the exported symbols. Depending on the OS,
these may be called libngspice.dll.a,ngspice.lib. Linux and MINGW also allow linking to the
shared object itself. The shared object is not included into the executable component but is tied
to the execution.
19.2.2 Loading at runtime
dlopen (Linux) or LoadLibrary (MS Windows) will load libngspice.so or ngspice.dll into
the address space of the caller at runtime. The functions return a handle that may be used to
acquire the pointers to the functions exported by libngspice.so. Detaching ngspice at runtime
is equally possible (using dlclose/FreeLibrary), after the background thread has been stopped
and all callbacks have returned.
19.3 Shared ngspice API
The sources for the ngspice shared library API are contained in a single C file (sharedspice.c)
and a corresponding header file sharedspice.h. The type and function declarations are contai-
ned in sharedspice.h, which may be directly added to the calling application, if written in C
or C++.
19.3.1 structs and types defined for transporting data
pvector_info is returned by the exported function ngGet_Vec_Info (see 19.3.2.5). Adresses of
the vector name, type, real or complex data are transferred and may be read asynchronously
during or after the simulation.
vector_info
typedef struct vector_info {
char *v_name; /* Same as so_vname */
int v_type; /* Same as so_vtype */
short v_flags ; /* Flags (a combination of VF_ *) */
double *v_realdata ; /* Real data */
ngcomplex_t * v_compdata ;/* Complex data */
int v_length ; /* Length of the vector */
} vector_info , * pvector_info ;
19.3. SHARED NGSPICE API 379
The next two structures are used by the callback function SendInitData (see 19.3.3.5). Each time
a new plot is generated during simulation, e.g. when a sequence of op, ac or tran is used, or
commands like linearize or fft are invoked, the function is called once by ngspice. Among
its parameters you find a pointer to a struct vecinfoall, which includes an array of vecinfo, one
for each vector. Pointers to the struct dvec, containing the vector, are included.
vecinfo
typedef struct vecinfo
{
int number; /* number of vector , as position in the
linked list of vectors , starts with 0 */
char *vecname ; /* name of the actual vector */
bool is_real ; /* TRUE if the actual vector has real data */
void * pdvec ; /* a void pointer to struct dvec *d, the
actual vector */
void * pdvecscale; /* a void pointer to struct dvec *ds ,
the scale vector */
} vecinfo , * pvecinfo;
vecinfoall
typedef struct vecinfoall
{
/* the plot */
char *name;
char * title ;
char *date;
char *type;
int veccount ;
/* the data as an array of vecinfo with
length equal to the number of vectors
in the plot */
pvecinfo *vecs ;
} vecinfoall , * pvecinfoall ;
The next two structures are used by the callback function SendData (see 19.3.3.4). Each time a
new data point (e.g. time value and simulation output value(s)) is added to the vector structure
of the current plot, the function SendData is called by ngspice, among its parameters the actual
pointer pvecvaluesall, which contains an array of pointers to pvecvalues, one for each vector.
380 CHAPTER 19. NGSPICE AS SHARED LIBRARY OR DYNAMIC LINK LIBRARY
vecvalues
typedef struct vecvalues {
char* name; /* name of a specific vector */
double creal; /* actual data value */
double cimag; /* actual data value */
bool is_scale ; /* if ’name ’ is the scale vector */
bool is_complex ; /* if the data are complex numbers */
} vecvalues , * pvecvalues;
Pointer vecvaluesall to be found as parameter to callback function SendData.
vecvaluesall
typedef struct vecvaluesall {
int veccount ; /* number of vectors in plot */
int vecindex ; /* index of actual set of vectors , i.e.
the number of accepted data points */
pvecvalues *vecsa; /* values of actual set of vectors ,
indexed from 0 to veccount - 1 */
} vecvaluesall , * pvecvaluesall ;
19.3.2 Exported functions
The functions listed in this chapter are the (only) symbols exported by the shared library.
19.3.2.1 int ngSpice_Init(SendChar*, SendStat*, ControlledExit*, SendData*, SendInit-
Data*, BGThreadRunning*, void)
After caller has loaded ngspice.dll, the simulator has to be initialized by calling ngSpice_Init(...).
Address pointers of several callback functions (see 19.3.3), which are to be defined in the caller,
are sent to ngspice.dll. The int return value is not used.
Pointers to callback functions (details see 19.3.3):
SendChar* callback function for reading printf, fprintf, fputs (NULL allowed)
SendStat* callback function for reading status string and percent value (NULL allowed)
ControlledExit* callback function for transferring a flag to caller, generated by ngspice upon
a call to function controlled_exit. May be used by caller to detach ngspice.dll, if dyna-
mically loaded or to try any other recovery method, or to exit. (required)
SendData* callback function for sending an array of structs containing data values of all vec-
tors in the current plot (simulation output) (NULL allowed)
SendInitData* callback function for sending an array of structs containing info on all vectors
in the current plot (immediately before simulation starts) (NULL allowed)
19.3. SHARED NGSPICE API 381
BGThreadRunning* callback function for sending a boolean signal (true if thread is running)
(NULL allowed)
void* Using the void pointer, you may send the object address of the calling function (’self’ or
’this’ pointer) to ngspice.dll. This pointer will be returned unmodified by any callback
function (see the *void pointers in Chapt. 19.3.3). Callback functions are to be defined
in the global section of the caller. Because they now have got the object address of the
calling function, they may direct their actions to the calling object.
19.3.2.2 int ngSpice_Init_Sync(GetVSRCData* , GetISRCData* , GetSyncData* , int*,
void*)
see Chapt. 19.6.
19.3.2.3 int ngSpice_Command(char*)
Send a valid command (see the control or interactive commands) from caller to ngspice.dll.
Will be executed immediately (as if in interactive mode). Some commands are rejected (e.g.
’plot’, because there is no graphics interface). Command ’quit’ will remove internal data, and
then send a notice to caller via ngexit(). The function returns a ’1’ upon error, otherwise ’0’.
19.3.2.4 bool ngSpice_running (void)
Checks if ngspice is running in its background thread (returning ’true’).
19.3.2.5 pvector_info ngGet_Vec_Info(char*)
uses the name of a vector (may be in the form ’vectorname’ or <plotname>.vectorname) as
parameter and returns a pointer to a vector_info struct. The caller may then directly assess the
vector data (but better should not modify them).
19.3.2.6 int ngSpice_Circ(char**)
sends an array of null-terminated char* to ngspice.dll. Each char* contains a single line of a
circuit (Each line is like it is found in an input file *.sp.). The last entry to char** has to be
NULL. Upon receiving the array, ngspice.dll will immediately parse the input and set up the
circuit structure (as if the circuit is loaded from a file by the ’source’ command). The function
returns a ’1’ upon error, otherwise ’0’.
19.3.2.7 char* ngSpice_CurPlot(void)
returns to the caller a pointer to the name of the current plot. For a definition of the term ’plot’
see Chapt. 17.3.
382 CHAPTER 19. NGSPICE AS SHARED LIBRARY OR DYNAMIC LINK LIBRARY
19.3.2.8 char** ngSpice_AllPlots(void)
returns to the caller a pointer to an array of all plots (listed by their typename).
19.3.2.9 char** ngSpice_AllVecs(char*)
returns to the caller a pointer to an array of all vector names in the plot named by the string in
the argument.
19.3.2.10 bool ngSpice_SetBkpt(double)
see Chapt. 19.6.
19.3.3 Callback functions
Callback functions are a means to return data from ngspice to the caller. These functions are
defined as global functions in the caller, so to be reachable by the C-coded ngspice. They are
declared according to the typedefs given below. ngspice receives their addresses from the caller
upon initialization with the ngSpice_Init(...) function (see 19.3.2.1). If the caller will not make
use of a callback, it may send NULL instead of the address (except for ControlledExit, which
is always required).
If ngspice is run in the background thread (19.4.2), the callback functions (defined in the caller)
also are called from within that thread. One has to be carefully judging how this behavior might
influence the caller, where now you have the primary and the background thread running in
parallel. So make the callback function thread safe. The integer identification number is only
used if you run several shared libraries in parallel (see Chapt. 19.6). Three additional callback
function are described in Chapt. 19.6.3.
19.3.3.1 typedef int (SendChar)(char*, int, void*)
char* string to be sent to caller output
int identification number of calling ngspice shared lib (default is 0, see Chapt. 19.6)
void* return pointer received from caller during initialization, e.g. pointer to object having sent
the request
Sending output from stdout, stderr to caller. ngspice printf, fprintf, fputs, fputc functions are
redirected to this function. The char* string is generated by assembling the print outputs of
the above mentioned functions according to the following rules: The string commences with
‘stdout ’, if directed to stdout by ngspice (with ‘stderr ’ respectively); all tokens are as-
sembled in sequence, taking the printf format specifiers into account, until ‘\n’ is hit. If set
addescape is given in .spiceinit, the escape character \is added to any character from $[]\"
found in the string.
Each callback function has a void pointer as the last parameter. This is useful in object oriented
programming. You may have sent the this (or self) pointer of the caller’s class object to ng-
spice.dll during calling ngSpice_Init (19.3.2.1). The pointer is returned unmodified by each
callback, so the callback function may identify the class object that has initialized ngspice.dll.
19.3. SHARED NGSPICE API 383
19.3.3.2 typedef int (SendStat)(char*, int, void*)
char* simulation status and value (in percent) to be sent to caller
int identification number of calling ngspice shared lib (default is 0, see Chapt. 19.6)
void* return pointer received from caller
sending simulation status to caller, e.g. the string tran 34.5%.
19.3.3.3 typedef int (ControlledExit)(int, bool, bool, int, void*)
int exit status
bool if true: immediate unloading dll, if false: just set flag, unload is done when function has
returned
bool if true: exit upon ’quit’, if false: exit due to ngspice.dll error
int identification number of calling ngspice shared lib (default is 0, see Chapt. 19.6)
void* return pointer received from caller
asking for a reaction after controlled exit.
19.3.3.4 typedef int (SendData)(pvecvaluesall, int, int, void*
vecvaluesall* pointer to array of structs containing actual values from all vectors
int number of structs (one per vector)
int identification number of calling ngspice shared lib (default is 0, see Chapt. 19.6)
void* return pointer received from caller
send back actual vector data.
19.3.3.5 typedef int (SendInitData)(pvecinfoall, int, void*)
vecinfoall* pointer to array of structs containing data from all vectors right after initialization
int identification number of calling ngspice shared lib (default is 0, see Chapt. 19.6)
void* return pointer received from caller
send back initialization vector data.
384 CHAPTER 19. NGSPICE AS SHARED LIBRARY OR DYNAMIC LINK LIBRARY
19.3.3.6 typedef int (BGThreadRunning)(bool, int, void*)
bool true if background thread is running
int identification number of calling ngspice shared lib (default is 0, see Chapt. 19.6)
void* return pointer received from caller
indicate if background thread is running
19.4 General remarks on using the API
19.4.1 Loading a netlist
Basically the input to shared ngspice is the same as if you would start a ngspice batch job, e.g.
you enter a netlist and the simulation command (any .dot analysis command like .tran,.op,
or .dc etc. as found in Chapt. 15.3), as well as suitable options.
Typically you should not include a .control section in your input file. Any script described
in a .control section for standard ngspice should better be emulated by the caller and be sent
directly to ngspice.dll. Start the simulation according to Chapt. 19.4.2 in an extra thread.
As an alternative, only the netlist has to be entered (without analysis command), then you may
use any interactive command as listed in Chapt. 17.5 (except for the plot command).
The ‘typical usage’ examples given below are excerpted from a caller written in C.
19.4.1.1 Loading from file
As with interactive ngspice, you may use the ngspice internal command source (17.5.70) to
load a complete netlist from a file.
Typical usage:
ngSpice_Comm and (" source ../ examples / adder_mos . cir ");
19.4.1.2 Loading line by line
As with interactive ngspice, you may use the ngspice internal command circbyline (17.5.10) to
send a netlist line by line to the ngspice circuit parser.
Typical usage:
ngSpice_Command (" circbyline fail test ");
ngSpice_Command (" circbyline V1 1 0 1");
ngSpice_Command (" circbyline R1 1 0 1");
ngSpice_Command (" circbyline .dc V1 0 1 0.1");
ngSpice_Comm and (" circbyline . end ");
The first line is a title line, which will be ignored during circuit parsing. As soon as the line
.end has been sent to ngspice, circuit parsing commences.
19.4. GENERAL REMARKS ON USING THE API 385
19.4.1.3 Loading as a string array
Typical usage:
circarray = ( char **) malloc ( sizeof ( char *) * 7);
circarray [0] = strdup (" test array ");
circarray [1] = strdup (" V1 1 0 1");
circarray [2] = strdup (" R1 1 2 1");
circarray [3] = strdup (" C1 2 0 1 ic =0");
circarray [4] = strdup (". tran 10u 3 uic ");
circarray [5] = strdup (". end ");
circarray [6] = NULL ;
ngSpice_Circ ( circarray );
An array of char pointers is malloc’d, each netlist line is then copied to the array. strdup will
care for the memory allocation. The first entry to the array is a title line, the last entry has to
contain NULL. ngSpice_Circ(circarray); sends the array to ngspice, where circuit parsing is
started immediately. Don’t forget to free the array after sending it, to avoid a memory leak.
19.4.2 Running the simulation
The following commands are used to start the simulator in its own thread, halt the simulation
and resume it again. The extra (background) thread enables the caller to continue with other
tasks in the main thread, e.g. watching its own event loop. Of course you have to take care
that the caller will not exit before ngspice is finished, otherwise you immediately will loose all
data. After having halted the simulator by suspending the background thread, you may assess
data, change ngspice parameters, or read output data using the caller’s main thread, before you
resume simulation using a background thread again. While the background thread is running,
ngspice will reject any other command sent by ngSpice_Command.
Typical usage:
ngSpice_Command (" bg_run ");
...
ngSpice_Command (" bg_halt ");
...
ngSpice_Command (" bg_resume ");
Basically you may send the commands ’run’ or ’resume’ (no prefix bg_), starting ngspice within
the main thread. The caller then has to wait until ngspice returns from simulation. A command
’halt’ is not available then.
After simulation is finished (test with callback 19.3.3.6), you may send other commands from
Chapt. 17.5, emulating any .control script. These commands are executed in the main thread,
which should be okay because execution time is typically short.
386 CHAPTER 19. NGSPICE AS SHARED LIBRARY OR DYNAMIC LINK LIBRARY
19.4.3 Accessing data
19.4.3.1 Synchronous access
The callback functions SendInitData (19.3.3.5) and SendData (19.3.3.4) allow access to si-
mulator output data synchronized with the simulation progress.
Each time a new plot is generated during simulation, e.g. when a sequence of op, ac and tran is
used or commands like linearize or fft are invoked, the callback SendInitData is called by
ngspice. Immediately after setting up the vector structure of the new plot, the function is called
once. Its parameter is a pointer to the structure vecinfoall (19.3.1), which contains an array of
structures vecinfo, one for each vector in the actual plot. You may simply use vecname to get
the name of any vector. This time the vectors are still empty, but pointers to the vector structure
are available.
Each time a new data point (e.g. time value and simulation output value(s)) is added to the
vector structure of the current plot, the function SendData is called by ngspice. This allows
you to immediately access the simulation output synchronized with the simulation time, e.g.
to interface it to a runtime plot or to use it for some controlled simulation by stopping the
simulation based on a condition, altering parameters and resume the simulation. SendData
returns a structure vecvaluesall as parameter, which contains an array of structures vecvalues,
one for each vector.
Some code to demonstrate the callback function usage is referenced below (19.5).
19.4.3.2 Asynchronous access
During simulation, while the background thread is running, or after it is finished, you may
use the functions ngSpice_CurPlot (19.3.2.7), ngSpice_AllPlots (19.3.2.8), ngSpice_AllVecs
(19.3.2.9) to retrieve information about vectors available, and function ngGet_Vec_Info (19.3.2.5)
to obtain data from a vector and its corresponding scale vector. The timing of the caller and the
simulation progress are independent from each other and not synchronized.
Again some code to demonstrate the callback function usage is referenced below (19.5).
19.4.4 Altering model or device parameters
After halting ngspice by stopping the background thread (19.4.2), nearly all ngspice commands
are available. Especially alter (17.5.3) and altermod (17.5.4) may be used to change device
or model parameters. After the modification, the simulation may be resumed immediately.
Changes to a circuit netlist, however, are not possible. You would need to load a complete new
netlist (19.4.1) and restart the simulation from the beginning.
19.4.5 Output
After the simulation is finished, use the ngspice commands write (17.5.88) or wrdata (17.5.87)
to output data to a file as usual, use the print command (17.5.47) to retrieve data via callback
SendChar (19.3.3.1), or refer to accessing the data as described in Chapt. 19.4.3.
19.5. EXAMPLE APPLICATIONS 387
Typical usage:
ngSpice_Comm and (" write testout . raw V (2)");
ngSpice_Comm and (" print V (2)");
19.4.6 Error handling
There are several occasions where standard ngspice suffers from an error, cannot recover inter-
nally and then exits. If this is happening to the shared module this would mean that the parent
application, the caller, is also forced to exit. Therefore (if not suffering from a seg fault) ng-
spice.dll will call the function controlled_exit as usual, this now calls the callback function
’ControlledExit’ (19.3.3.3), which hands over the request for exiting to the caller. The caller
now has the task to handle the exit code for ngspice.
If ngspice has been linked at runtime by dlopen/LoadLibrary (see 19.2.2), the callback may
close all threads, and then detach ngspice.dll by invoking dlclose/FreeLibrary. The caller
may then restart ngspice by another loading and initialization (19.3.2.1).
If ngspice is included during linking the caller (see 19.2.1), there is not yet a good and general
solution to error handling, if the error is non-recoverable from inside ngspice.
19.5 Example applications
Three executables (coming with source code) serve as examples for controlling ngspice. These
are not meant to be ‘production’ programs, but just give some commented example usages of
the interface.
ng_start.exe is a MS Windows application loading ngspice.dll dynamically. All functions
and callbacks of the interface are assessed. The source code, generated with Turbo Delphi
2006, may be found here, the binaries compiled for 32 Bit are here.
Two console applications, compilable with Linux, CYGWIN, MINGW or MS Visual Studio,
are available here, demonstrating either linking upon start-up or loading shared ngspice dyna-
mically at runtime. A simple feedback loop is shown in tests 3 and 4, where a device parameter
is changed upon having an output vector value crossing a limit.
19.6 ngspice parallel
The following chapter describes an offer to the advanced user and developer community. If you
are interested in evaluating the parallel and synchronized operation of several ngspice instances,
this may be one way to go. However, no ready to use implementation is available. You will
find a toolbox and some hints how to use it. Parallelization and synchronization is your task by
developing a suitable caller! And of course another major input has to come from partitioning
the circuit into suitable, loosely coupled pieces, each with its own netlist, one netlist per ngspice
instance. And you have to define the coupling between the circuit blocks. Both are not provided
by ngspice, but are again your responsibility. Both are under active research, and the toolbox
described below is an offer to join that research.
388 CHAPTER 19. NGSPICE AS SHARED LIBRARY OR DYNAMIC LINK LIBRARY
19.6.1 Go parallel!
A simple way to run several invocations of ngspice in parallel for transient simulation is to define
a caller that loads two or more ngspice shared libraries. There is one prerequisite however
to do so: the shared libraries have to have different names. So compile ngspice shared lib
(see 19.1), then copy and rename the library file, e.g. ngspice.dll may become ngspice1.dll,
ngspice2.dll etc. Then dynamically load ngspice1.dll, retrieve its address, initialize it by
calling ngSpice_init() (see 19.3.2.1), then continue initialization by calling ngSpice_init_Sync()
(see 19.6.2.1). An integer identification number may be sent during this step to later uniquely
identify each invocation of the shared library, e.g. by having any callback use this identifier.
Repeat the sequence with ngspice2.dll and so on.
Inter-process communication and synchronization is now done by using three callback functi-
ons. To understand their interdependency, it might be useful to have a look at the transient
simulation sequence as defined in the ngspice source file dctran.c. The following listing in-
cludes the shared library option (It differs somewhat from standard procedure) and disregards
XSPICE.
1. initialization
2. calculation of operating point
3. next time step: set new breakpoints (VSRC, ISRC, TRA, LTRA)
4. send simulation data to output, callback function SendData* datfcn
5. check for autostop and other end conditions
6. check for interrupting simulation (e.g. by bg_halt)
7. breakpoint handling (e.g. enforce breakpoint, set new small cktdelta if directly after the
breakpoint)
8. calling ngspice internal function sharedsync() that invokes callback function GetSyn-
cData* getsync with location flag loc = 0
9. save the previous states
10. start endless loop
11. save cktdelta to olddelta, set new time point by adding cktdelta to ckttime
12. new iteration of circuit at new time point, which uses callback functions GetVSRCData*
getvdat and GetISRCData* getidat to retrieve external voltage or current inputs, returns
redostep=0, if converged, redostep=1 if not converged
13. if not converged, divide cktdelta by 8
14. check for truncation error with all non-linear devices, if necessary create a new (smaller)
cktdelta to limit the error, optionally change integration order
15. calling ngspice internal function sharedsync() that invokes callback function GetSyn-
cData* getsync with location flag loc = 1: as a result either goto 3 (next time step) or to
10 (loop start), depending on ngspice and user data, see the next paragraph.
19.6. NGSPICE PARALLEL 389
The code of the synchronization procedure is handled in the ngspice internal function shared-
sync() and its companion user defined callback function GetSyncData* getsync. The actual
setup is as follows:
If no synchronization is asked for (GetSyncData* set to NULL), program control jumps to ’next
time step’ (3) if redostep==0, or subtracts olddelta from ckttime and jumps to ’loop start’ (9) if
redostep <> 0. This is the standard ngspice behavior.
If GetSyncData* has been set to a valid address by ngSpice_Init_Sync(), the callback function
getsync is involved. If redostep <> 0, olddelta is subtracted from ckttime, getsync is called,
either the cktdelta time suggested by ngspice is kept or the user provides his own deltatime,
and the program execution jumps to (9) for redoing the last step with the new deltatime. The
return value of getsync is not used. If redostep == 0, getsync is called. The user may keep
the deltatime suggested by ngspice or define a new value. If the user sets the return value of
getsync to 0, the program execution then jumps to ’next time step’ (3). If the return value of
getsync is 1, olddelta is subtracted from ckttime, and the program execution jumps to (9) for
redoing the last step with the new deltatime. Typically the user provided deltatime should be
smaller than the value suggested by ngspice.
19.6.2 Additional exported functions
The following functions (exported or callback) are designed to support the parallel action of
several ngspice invocations. They may be useful, however, also when only a single library
is loaded into a caller, if you want to use external voltage or current sources or ’play’ with
advancing simulation time.
19.6.2.1 int ngSpice_Init_Sync(GetVSRCData* , GetISRCData* , GetSyncData* , int*,
void*)
Pointers to callback functions (details see 19.3.3):
GetVSRCData* callback function for retrieving a voltage source value from caller (NULL
allowed)
GetISRCData* callback function for retrieving a current source value from caller (NULL al-
lowed)
GetSyncData* callback function for synchronization (NULL allowed)
More pointers
int* pointer to integer unique to this shared library (defaults to 0)
void* pointer to user-defined data, will not be modified, but handed over back to caller during
Callback, e.g. address of calling object. If NULL is sent here, userdata info from ng-
Spice_Init() will be kept, otherwise userdata will be overridden by new value from here.
390 CHAPTER 19. NGSPICE AS SHARED LIBRARY OR DYNAMIC LINK LIBRARY
19.6.2.2 bool ngSpice_SetBkpt(double)
Sets a breakpoint in ngspice, a time point that the simulator is enforced to hit during the transient
simulation. After the breakpoint time has been hit, the next delta time starts with a small value
and is ramped up again. A breakpoint should be set only when the background thread in ngspice
is not running (before the simulation has started, or after the simulation has been paused by
bg_halt). The time sent to ngspice should be larger than the current time (which is either 0
before start or given by the callback GetSyncData (19.6.3.3). Several breakpoints may be set.
19.6.3 Additional callback functions
19.6.3.1 typedef int (GetVSRCData)(double*, double, char*, int, void*)
double* return voltage value
double actual time
char* node name
int identification number of calling ngspice shared lib
void* return pointer received from caller
Ask for a VSRC EXTERNAL voltage value. The independent voltage source (see Chapt. 4.1)
with EXTERNAL option allows to set a voltage value to the node defined in the netlist and
named here at the time returned by the simulator.
19.6.3.2 typedef int (GetISRCData)(double*, double, char*, int, void*)
double* return current value
double actual time
char* node name
int identification number of calling ngspice shared lib
void* return pointer received from caller
Ask for ISRC EXTERNAL value. The independent current source (see Chapt. 4.1) with EX-
TERNAL option allows to set a current value to the node defined by the netlist and named here
at the time returned by the simulator.
19.6. NGSPICE PARALLEL 391
19.6.3.3 typedef int (GetSyncData)(double, double*, double, int, void*)
double actual time (ckt->CKTtime)
double* delta time (ckt->CKTdelta)
double old delta time (olddelta)
int identification number of calling ngspice shared lib
int location of call for synchronization in dctran.c
void* return pointer received from caller
Ask for new delta time depending on synchronization requirements. See 19.6.1 for an explana-
tion.
19.6.4 Parallel ngspice example
A first example is available as a compacted 7z archive. It contains the source code of a control-
ling application, as well as its compiled executable and ngspice.dll (for MS Windows). As the
input circuit an inverter chain has been divided into three parts. Three ngspice shared libraries
are loaded, each simulates one partition of the circuit. Interconnections between the partitions
are provided via a callback function. The simulation time is synchronized among the three
ngspice invocations by another callback function.
392 CHAPTER 19. NGSPICE AS SHARED LIBRARY OR DYNAMIC LINK LIBRARY
Chapter 20
TCLspice
Spice historically comes as a simulation engine with a Command Line Interface. The Spice
engine can also be used with a Graphical User Interface. Tclspice represents a third approach
to interfacing ngspice simulation functionality. Tclspice is nothing more than a new way of
compiling and using SPICE source code. Spice is no longer considered as a standalone program
but as a library invoked by a TCL interpreter. It either permits direct simulation in a TCL shell
(this is quite analogous to the command line interface of ngspice), or it permits the elaboration
of more complex, more specific, or more user friendly simulation programs, by writing TCL
scripts.
20.1 tclspice framework
The technical difference between the ngspice CLI interface and tclspice is that the CLI interface
is compiled as a standalone program, whereas tclspice is a shared object. Tclspice is designed to
work with tools that expand the capabilities of ngspice: TCL for the scripting and programming
language interface and BLT for data processing and display. This two tools give tclspice all of
its relevance, with the insurance that the functionality is maintained by competent people.
Making tclspice (see 20.6) produces two files: libspice.so and pkgIndex.tcl.libspice.so is the
executable binary that the TCL interpreter calls to handle SPICE commands. pkgIndex.tcl take
place in the TCL directory tree, providing the SPICE package1to the TCL user.
BLT is a TCL package. It is quite well documented. It permits to handle mathematical vector
data structures for calculus and display, in a Tk interpreter like wish.
20.2 tclspice documentation
A detailed documentation on tclspice commands is available on the original tclspice web page.
20.3 spicetoblt
Tclspice opens its doors to TCL and BLT with a single specific command spicetoblt.
1package has to be understood as the TCL package
393
394 CHAPTER 20. TCLSPICE
TCLspice gets its identity in the command spice::vectoblt . This command copies data com-
puted by the simulation engine into a tcl variable. vectoblt is composed of three words: vec,
to and blt. Vec means SPICE vector data. To is the English preposition, and blt is a useful tcl
package providing a vector data structure. Example:
blt :: vector create Iex
spice :: vectoblt Vex # branch Iex
Here an empty blt vector is created. It is then filled with the vector representation of the current
flowing out of source Vex.Vex#branch is native SPICE syntax. Iex is the name of the BLT
vector.
The reverse operation is handled by native SPICE commands, such as alter,let and set.
20.4 Running TCLspice
TCLspice consists of a library or a package to include in your tcl console or script:
load / somepath / libspice .so
package require spice
Then you can execute any native SPICE command by preceding it with spice::. For example
if you want to source the testCapa.cir netlist, type the following:
spice :: source testCapa . cir
spice :: spicetoblt example ...
Plotting data is not a matter of SPICE, but of tcl. Once the data is stored in a blt vector, it can
be plotted. Example:
blt :: graph .cimvd - title " Cim = f(Vd)"
pack . cimvd
.cimvd element create line1 -xdata Vcmd -ydata Cim
With blt::graph a plotting structure is allocated in memory. With pack it is placed into the
output window, and becomes visible. The last command, and not the least, plots the function
Cim =f(Vcmd ), where Cim and Vcmd are two BLT vectors.
20.5 examples
20.5.1 Active capacitor measurement
This is a crude implementation of a circuit described by Marc Kodrnja, in his PhD thesis that
was found on the Internet. The simulation outputs a graph representing virtual capacitance
versus a control voltage. The function C=f(V)is calculated point by point. For each control
20.5. EXAMPLES 395
voltage value, the virtual capacitance is calculated in a frequency simulation. A control value
that should be as close to zero as possible is calculated to assess simulation success.
20.5.1.1 Invocation:
This script can be invoked by typing wish testbench1.tcl
20.5.1.2 testbench1.tcl
This line loads the simulator capabilities
package require spice
This is a comment (Quite useful if you intend to live with other Human beings)
# Test of virtual capacitor circuit
# Vary the control voltage and log the resulting capacitance
A good example of the calling of a SPICE command: precede it with spice::
spice :: source " testCapa .cir "
This reminds that any regular TCL command is of course possible
set n 30 set dv 0.2
set vmax [ expr $dv /2]
set vmin [ expr -1 * $dv /2]
set pas [ expr $dv/ $n]
BLT vector is the structure used to manipulate data. Instantiate the vectors
blt :: vector create Ctmp
blt :: vector create Cim
blt :: vector create check
blt :: vector create Vcmd
Data is, in my coding style, plotted into graph objects. Instantiate the graph
396 CHAPTER 20. TCLSPICE
blt :: graph .cimvd - title " Cim = f(Vd)"
blt :: graph .checkvd -title " Rim = f(Vd)"
blt :: vector create Iex
blt :: vector create freq
blt :: graph .freqanal -title " Analyse frequentielle "
#
# First simulation : A simple AC plot
#
set v [expr {$vmin + $n * $pas / 4}]
spice :: alter vd = $v
spice :: op
spice ::ac dec 10 100 100k
Retrieve a the intensity of the current across Vex source
spice :: vectoblt { Vex #branch } Iex
Retrieve the frequency at which the current have been assessed
spice :: vectoblt { frequency } freq
Room the graph in the display window
pack . freqanal
Plot the function Iex =f(V)
.freqanal element create line1 -xdata freq -ydata Iex
#
# Second simulation : Capacitance versus voltage control
# for {set i 0} {[ expr $n - $i]} {incr i }
# { set v [expr {$vmin + $i * $pas }]
spice :: alter vd = $v
spice :: op spice :: ac dec 10 100 100 k
Image capacitance is calculated by SPICE, instead of TCL there is no objective reason
spice :: let Cim = real ( mean ( Vex #branch /(2* Pi *i* frequency *( V(5) -V (6)))))
spice :: vectoblt Cim Ctmp
Build function vector point by point
Cim append $Ctmp (0: end )
Build a control vector to check simulation success
20.5. EXAMPLES 397
spice :: let err = real ( mean ( sqrt (( Vex #branch -
(2* Pi*i* frequency * Cim*V(5)-V (6)))^2)))
spice :: vectoblt err Ctmp check
append $Ctmp (0: end )
Build abscissa vector
FALTA ALGO ... Vcmd append $v }
Plot
pack . cimvd
.cimvd element create line1 -xdata Vcmd -ydata Cim
pack . checkvd
.checkvd element create line1 - xdata Vcmd -ydata check
20.5.2 Optimization of a linearization circuit for a Thermistor
This example is both the first and the last optimization program written for an electronic circuit.
It is far from perfect.
The temperature response of a CTN is exponential. It is thus nonlinear. In a battery charger
application floating voltage varies linearly with temperature. A TL431 voltage reference sees
its output voltage controlled by two resistors (r10, r12) and a thermistor (r11). The simulation
is run at a given temperature. The thermistor is modeled in SPICE by a regular resistor. Its
resistivity is assessed by the TCL script. It is set with a spice::alter command before running
the simulation. This script uses an iterative optimization approach to try to converge to a set
of two resistor values that minimizes the error between the expected floating voltage and the
TL431 output.
20.5.2.1 Invocation:
This script can be executed by the user by simply executing the file in a terminal.
./ testbench3 .tcl
Two issues2are important to point out:
2For those who are really interested in optimizing circuits: Some parameters are very important for quick and
correct convergence. The optimizer walks step by step to a local minimum of the cost function you define. Starting
from an initial vector you provide, it converges step by step. Consider trying another start vector if the result is not
the one you expected.
The optimizer will carry on walking until it reaches a vector whose resulting cost is smaller than the target cost
you provided. You must also provide a maximum iteration count in case the target can not be achieved. Balance
time, specifications, and every other parameter. For a balance between quick and accurate convergence adjust the
‘factor’ variable, at the beginning of minimumSteepestDescent in the file differentiate.tcl.
398 CHAPTER 20. TCLSPICE
• During optimization loop, graphical display of the current temperature response is not yet
possible and I don’t know why. Each time a simulation is performed, some memory is
allocated for it.
• The simulation result remains in memory until the libspice library is unloaded (typically:
when the tcl script ends) or when a spice::clean command is performed. In this kind of
simulation, not cleaning the memory space will freeze your computer and you’ll have to
restart it. Be aware of that.
20.5.2.2 testbench3.tcl
This calls the shell sh who then runs wish with the file itself.
#!/ bin /sh
# WishFix \
exec wish "$0 " $ {1+" $@ "}
#
#
#
Regular package for simulation
package require spice
Here the important line is source differentiate.tcl that contains the optimization library
source differentiate .tcl
Generates a temperature vector
proc temperatures_calc {temp_inf temp_sup points } {
set tstep [ expr " ( $temp_sup - $temp_inf ) / $points " ]
set t $temp_inf
set temperatures ""
for { set i 0 } { $i < $points } { incr i } {
set t [ expr { $t + $tstep } ]
set temp era tur es " $te mper atu res $t "
}
return $temperatures }
generates thermistor resistivity as a vector, typically run: thermistance_calc res B [ temperatu-
res_calc temp_inf temp_sup points ]
20.5. EXAMPLES 399
proc thermistance_calc { res B points } {
set tzero 273.15
set tref 25
set thermistance ""
foreach t $points {
set res_temp [ expr " $res *
+ exp ( $B * ( 1 / ($tzero + $t) -
+ 1 / ( $tzero + $tref ) ) ) " ]
set thermistance " $thermistance $res_temp "
}
return $thermistance }
generates the expected floating value as a vector, typically run: tref_calc res B [ temperatu-
res_calc temp_inf temp_sup points ]
proc tref_calc { points } {
set tref ""
foreach t $points {
set tref "$tref [expr "6*(2.275 -0.005*( $t -20)) -9"]"
}
return $tref }
In the optimization algorithm, this function computes the effective floating voltage at the given
temperature.
### NOTE :
### As component values are modified by a spice :: alter
### Component values can be considered as global
variable.
### R10 and R12 are not passed to iteration function
### because it is expected to be correct , i.e. to
### have been modified soon before
proc iteration { t } { set tzero 273.15 spice :: alter
r11 = [ thermistance_calc 10000 3900 $t ]
# Temperature simulation often crashes. Comment it out
...
#spice :: set temp = [ expr " $tzero + $t " ]
spice :: op
spice :: vectoblt vref_temp tref_tmp
### NOTE :
### As the library is executed once for the
### whole script execution , it is important to manage
the memory
### and regularly destroy unused data set. The data
### computed here will not be reused. Clean it
spice :: destroy all return [ tref_tmp range 0 0 ] }
400 CHAPTER 20. TCLSPICE
This is the cost function optimization algorithm will try to minimize. It is a 2-norm (Euclidean
norm) of the error across the temperature range [-25:75]°C.
proc cost { r10 r12 } {
tref_blt length 0
spice :: alter r10 = $r10
spice :: alter r12 = $r12
foreach point [ temperatures_blt range 0
+ [ expr " [ temperatures_blt length ] - 1" ] ] {
+ tref_blt append [ iteration $point ]
}
set result [ blt :: vector expr " 1000 *
sum (( tref_blt - expected_blt )^2 )" ]
disp_curve $r10 $r12
return $result }
This function displays the expected and effective value of the voltage, as well as the r10 and r12
resistor values
proc disp_curve { r10 r12 }
+ { .g configure -title "Valeurs optimales : R10 = $r10
R12 = $r12" }
Main loop starts here
#
# Optimization
# blt :: vector create tref_tmp
blt :: vector create tref_blt
blt :: vector create expected_blt
blt :: vector create temperatures_blt temperatures_blt
append [ temperatures_calc -25 75 30 ] expected_blt
append [ tref_calc [ temperatures_blt range 0
+ [ expr " [ temperatures_blt length ] - 1" ] ] ]
blt :: graph .g
pack .g -side top -fill both - expand true
.g element create real -pixels 4 -xdata
temperatures_blt
+ -ydata tref_blt
.g element create expected -fill red -pixels 0 -dashes
+ dot -xdata temperatures_blt -ydata expected_blt
Source the circuit and optimize it. The result is retrieved in the variable r10r12e and put into
r10 and r12 with a regular expression. A bit ugly.
20.5. EXAMPLES 401
spice :: source FB14 .cir
set r10r12 [ :: math :: optimize :: minimu mSteepestDe scent
+ cost { 10000 10000 } 0.1 50 ]
regexp {([0 -9.]*) ([0 -9.]*) } $r10r12 r10r12 r10 r12
Outputs optimization result
#
# Results
# spice :: alter r10 = $r10
spice :: alter r12 = $r12
foreach point [ temperatures_blt range 0
+ [ expr " [temperatures_blt length ] - 1" ] ] {
tref_blt append [ iteration $point ]
}
disp_curve $r10 $r12
20.5.3 Progressive display
This example is quite simple but it is very interesting. It displays a transient simulation result
on the fly. You may now be familiar with most of the lines of this script. It uses the ability of
BLT objects to automatically update. When the vector data is modified, the strip-chart display
is modified accordingly.
20.5.3.1 testbench2.tcl
#!/ bin /sh
# WishFix \
exec wish -f "$0" ${1+" $@ "}
###
package require BLT package require spice
this avoids to type blt:: before the blt class commands
namespace import blt ::*
wm title . "Vector Test script"
wm geometry . 800 x600 +40+40 pack propagate . false
A strip chart with labels but without data is created and displayed (packed)
402 CHAPTER 20. TCLSPICE
stripchart .chart
pack . chart -side top -fill both - expand true
.chart axis configure x -title "Time" spice :: source example . cir
spice :: bg
run after 1000 vector
create a0 vector
create b0 vectorry
create a1 vector
create b1 vector
create stime
proc bltupdate {} {
puts [ spice :: spice_data ]
spice :: spicetoblt a0 a0
spice :: spicetoblt b0 b0
spice :: spicetoblt a1 a1
spice :: spicetoblt b1 b1
spice :: spicetoblt time stime
after 100 bltupdate }
bltupdate . chart element create a0 -color red -xdata
+ stime -ydata a0
.chart element create b0 -color blue -xdata stime -ydata b0
.chart element create a1 -color yellow -xdata stime -ydata a1
.chart element create b1 -color black -xdata stime -ydata b1
20.6 Compiling
20.6.1 Linux
Get tcl8.4 from your distribution. You will need the blt plotting package (compatible to the old
tcl 8.4 only) from here. See also the actual blt wiki.
./configure --with-tcl ..
make
sudo make install
20.6.2 MS Windows
Can be done, but is tedious. Here it is described by a procedure on Windows 7, 64 Bit Home
Edition.
20.6.2.1 Downloads
download tcl8.6b2-src.zip from http://www.tcl.tk/software/tcltk/download.html
download tk8.6b2-src.zip
20.7. MS WINDOWS 32 BIT BINARIES 403
download blt from http://ngspice.sourceforge.net/experimental/blt2.4z.7z
expand all to d:\software
20.6.2.2 Tcl
double click on D:\software\tcl8.6b2\win\tcl.dsw
convert to MS Visual Studio 2008 project
select release or debug
create tcl as tcl86t.dll.
20.6.2.3 Tk
edit D:\software\tk8.6b2\win\buildall.vc.bat
line 31 to
call C:\Program Files (x86)\Microsoft Visual Studio 9.0\VC\vcvarsall.bat
line 53 to
if "%TCLDIR%" == "" set TCLDIR=..\..\tcl8.6b2
open cmd window
cd to
d:\software\tk8.6b2\win>
then
d:\software\tk8.6b2\win> buildall.vc.bat debug
tk will be made as tk86t.dll, in addition wish86t.exe is generated.
20.6.2.4 blt
blt source files have been downloaded from the blt web page and modified for compatibility
with TCL8.6. To facilitate making blt24.dll, the modified source code is available as a 7z
compressed file, including a project file for MS Visual Studio 2008.
20.6.2.5 tclspice
ngspice is compiled and linked into a dll called spice.dll that may be loaded by wish86t.exe.
MS Visual Studio 2008 is the compiler applied. A project file may be downloaded as a 7z
compressed file. Expand this file in the ngspice main directory. The links to tcl and tk are hard-
coded, so both have to be installed in the places described above (d:\software\...). spice.dll
may be generated in Debug, Release or ReleaseOMP mode.
20.7 MS Windows 32 Bit binaries
You may download the compiled binaries, including tcl, tk, blt and tclspice, plus the examples,
slightly modified, from http://ngspice.sourceforge.net/experimental/tclspice-25.7z.
404 CHAPTER 20. TCLSPICE
Chapter 21
Example Circuits
This section starts with an ngspice example to walk you through the basic features of ngspice
using its command line user interface. The operation of ngspice will be illustrated through
several examples (Chapt. 20.1 to 20.7).
The first example uses the simple one-transistor amplifier circuit illustrated in Fig. 21.1. This
circuit is constructed entirely with ngspice compatible devices and is used to introduce basic
concepts, including:
• Invoking the simulator:
• Running simulations in different analysis modes
• Printing and plotting analog results
• Examining status, including execution time and memory usage
• Exiting the simulator
The remainder of the section (from Chapt. 21.2 onwards) lists several circuits, which have been
accompanying any ngspice distribution, and may be regarded as the ‘classical’ SPICE circuits.
21.1 AC coupled transistor amplifier
The circuit shown in Fig. 21.1 is a simple one-transistor amplifier. The input signal is amplified
with a gain of approximately -(Rc/Re) = -(3.9K/1K) = -3.9. The circuit description file for this
example is shown below.
405
406 CHAPTER 21. EXAMPLE CIRCUITS
Figure 21.1: Transistor Amplifier Simulation Example
Example:
A Berkeley SPICE3 compatible circuit
*
* This circuit contains only Berkeley SPICE3 components .
*
* The circuit is an AC coupled transistor amplifier with
* a sinewave input at node "1" , a gain of approximately -3.9,
* and output on node " coll ".
*
.tran 1e -5 2e-3
*
vcc vcc 0 12.0
vin 1 0 0.0 ac 1.0 sin (0 1 1k)
ccouple 1 base 10uF
rbias1 vcc base 100k
rbias2 base 0 24k
q1 coll base emit generic
rcollector vcc coll 3.9k
remitter emit 0 1k
*
.model generic npn
*
.end
To simulate this circuit, move into a directory under your user account and copy the file xspice_c1.cir
21.1. AC COUPLED TRANSISTOR AMPLIFIER 407
from directory /examples/xspice/. This file stems from the original XSPICE introduction,
therefore its name, but you do not need installing the XSPICE option to run it.
$ cp /examples/xspice/xspice_c1.cir xspice_c1.cir
Now invoke the simulator on this circuit as follows:
$ ngspice xspice_c1.cir
After a few moments, you should see the ngspice prompt:
ngspice 1 ->
At this point, ngspice has read-in the circuit description and checked it for errors. If any errors
had been encountered, messages describing them would have been output to your terminal.
Since no messages were printed for this circuit, the syntax of the circuit description was correct.
To see the circuit description read by the simulator you can issue the following command:
ngspice 1 -> listing
The simulator shows you the circuit description currently in memory:
a berkeley spice3 compatible circuit
1 : a berkeley spice3 compatible circuit
2 : .global gnd
10 : .tran 1e-5 2e-3
12 : vcc vcc 0 12.0
13 : vin 1 0 0.0 ac 1.0 sin(0 1 1k)
14 : ccouple 1 base 10uf
15 : rbias1 vcc base 100k
16 : rbias2 base 0 24k
17 : q1 coll base emit generic
18 : rcollector vcc coll 3.9k
19 : remitter emit 0 1k
21 : .model generic npn
24 : .end
The title of this circuit is ‘A Berkeley SPICE3 compatible circuit’. The circuit description
contains a transient analysis control command .TRAN 1E-5 2E-3 requesting a total simulated
time of 2ms with a maximum time-step of 10us. The remainder of the lines in the circuit
description describe the circuit of Fig. 21.1.
Now, execute the simulation by entering the run command:
ngspice 1 -> run
408 CHAPTER 21. EXAMPLE CIRCUITS
The simulator will run the simulation and when execution is completed, will return with the
ngspice prompt. When the prompt returns, issue the rusage command again to see how much
time and memory has been used now.
To examine the results of this transient analysis, we can use the plot command. First we will
plot the nodes labeled ‘1’ and ‘base’.
ngspice 2 -> plot v(1) base
The simulator responds by displaying an X Window System plot similar to that shown in Fig.
21.2.
Figure 21.2: node 1 and node ’base’ versus time
Notice that we have named one of the nodes in the circuit description with a number (‘1’),
while the others are words (‘base’). This was done to illustrate ngspice’s special requirements
for plotting nodes labeled with numbers. Numeric labels are allowed in ngspice for backwards
compatibility with SPICE2. However, they require special treatment in some commands such
as plot. The plot command is designed to allow expressions in its argument list in addition
to names of results data to be plotted. For example, the expression plot (base - 1) would
plot the result of subtracting 1 from the value of node ‘base’.
If we had desired to plot the difference between the voltage at node ‘base’ and node ‘1’, we
would need to enclose the node name ‘1’ in the construction v( ) producing a command such
as plot (base - v(1)).
Now, issue the following command to examine the voltages on two of the internal nodes of the
transistor amplifier circuit:
21.1. AC COUPLED TRANSISTOR AMPLIFIER 409
ngspice 3 -> plot vcc coll emit
The plot shown in Fig. 21.3 should appear. Notice in the circuit description that the power
supply voltage source and the node it is connected to both have the name ‘vcc’. The plot
command above has plotted the node voltage ‘vcc’. However, it is also possible to plot branch
currents through voltage sources in a circuit. ngspice always adds the special suffix #branch to
voltage source names. Hence, to plot the current into the voltage source named vcc, we would
use a command such as plot vcc#branch.
Figure 21.3: VCC, Collector and Emitter Voltages
Now let’s run a simple DC simulation of this circuit and examine the bias voltages with the
print command. One way to do this is to quit the simulator using the quit command, edit
the input file to change the .tran line to .op (for ’operating point analysis’), re-invoke the
simulator, and then issue the run command. However, ngspice allows analysis mode changes
directly from the ngspice prompt. All that is required is to enter the control line, e.g. op (without
the leading ‘.’). ngspice will interpret the information on the line and start the new analysis run
immediately, without the need to enter a new run command.
To run the DC simulation of the transistor amplifier, issue the following command:
ngspice 4 -> op
After a moment the ngspice prompt returns. Now issue the print command to examine the
emitter, base, and collector DC bias voltages.
ngspice 5 -> print emit base coll
410 CHAPTER 21. EXAMPLE CIRCUITS
ngspice responds with:
emit = 1.293993e+00 base = 2.074610e+00 coll = 7.003393e+00
To run an AC analysis, enter the following command:
ngspice 6 -> ac dec 10 0.01 100
This command runs a small-signal swept AC analysis of the circuit to compute the magnitude
and phase responses. In this example, the sweep is logarithmic with ‘decade’ scaling, 10 points
per decade, and lower and upper frequencies of 0.01 Hz and 100 Hz. Since the command
sweeps through a range of frequencies, the results are vectors of values and are examined with
the plot command. Issue to the following command to plot the response curve at node ‘coll’:
ngspice 7 -> plot coll
This plot shows the AC gain from input to the collector. (Note that our input source in the circuit
description ‘vin’ contained parameters of the form ‘AC 1.0’ designating that a unit-amplitude
AC signal was applied at this point.) For plotting data from an AC analysis, ngspice chooses
automatically a logarithmic scaling for the frequency (x) axis.
To produce a more traditional ‘Bode’ gain phase plot (again with automatic logarithmic scaling
on the frequency axis), we use the expression capability of the plot command and the built-in
Nutmeg functions db( ) and ph( ):
ngspice 8 -> plot db(coll) ph(coll)
The last analysis supported by ngspice is a swept DC analysis. To perform this analysis, issue
the following command:
ngspice 9 -> dc vcc 0 15 0.1
This command sweeps the supply voltage ‘vcc’ from 0 to 15 volts in 0.1 volt increments. To
plot the results, issue the command:
ngspice 10 -> plot emit base coll
Finally, to exit the simulator, use the quit command, and you will be returned to the operating
system prompt.
ngspice 11 -> quit
So long.
21.2. DIFFERENTIAL PAIR 411
21.2 Differential Pair
The following deck determines the dc operating point of a simple differential pair. In addition,
the ac small-signal response is computed over the frequency range 1Hz to 100MEGHz.
Example:
SIMPLE DIFFERENTIAL PAIR
VCC 7 0 12
VEE 8 0 -12
VIN 1 0 AC 1
RS1 1 2 1K
RS2 6 0 1K
Q1 3 2 4 MOD1
Q2 5 6 4 MOD1
RC1 7 3 10K
RC2 7 5 10K
RE 4 8 10K
.MODEL MOD1 NPN BF =50 VAF =50 IS =1.E -12 RB =100 CJC =.5 PF TF=.6NS
.TF V (5) VIN
.AC DEC 10 1 100 MEG
.END
21.3 MOSFET Characterization
The following deck computes the output characteristics of a MOSFET device over the range
0-10V for VDS and 0-5V for VGS.
Example:
MOS OUTPUT CHARACTERISTICS
.OPTIONS NODE NOPAGE
VDS 3 0
VGS 2 0
M1 1 2 0 0 MOD1 L=4U W=6U AD =10 P AS=10 P
* VIDS MEASURES ID , WE COULD HAVE USED VDS ,
* BUT ID WOULD BE NEGATIVE
VIDS 3 1
. MODEL MOD1 NMOS VTO = -2 NSUB =1.0 E15 UO =550
.DC VDS 0 10 .5 VGS 0 5 1
.END
21.4 RTL Inverter
The following deck determines the dc transfer curve and the transient pulse response of a simple
RTL inverter. The input is a pulse from 0 to 5 Volts with delay, rise, and fall times of 2ns and
412 CHAPTER 21. EXAMPLE CIRCUITS
a pulse width of 30ns. The transient interval is 0 to 100ns, with printing to be done every
nanosecond.
Example:
SIMPLE RTL INVERTER
VCC 4 0 5
VIN 1 0 PULSE 0 5 2NS 2NS 2NS 30NS
RB 1 2 10K
Q1 3 2 0 Q1
RC 3 4 1K
.MODEL Q1 NPN BF 20 RB 100 TF .1 NS CJC 2PF
.DC VIN 0 5 0.1
.TRAN 1NS 100NS
.END
21.5 Four-Bit Binary Adder (Bipolar)
The following deck simulates a four-bit binary adder, using several subcircuits to describe vari-
ous pieces of the overall circuit.
Example:
ADDER - 4 BIT ALL -NAND - GATE BINARY ADDER
*** SUBCIRCUIT DEFINITIONS
.SUBCKT NAND 1 2 3 4
* NODES: INPUT (2) , OUTPUT , VCC
Q1 9 5 1 QMOD
D1CLAMP 0 1 DMOD
Q2 9 5 2 QMOD
D2CLAMP 0 2 DMOD
RB 4 5 4K
R1 4 6 1.6 K
Q3 6 9 8 QMOD
R2 8 0 1K
RC 4 7 130
Q4 7 6 10 QMOD
DVBEDROP 10 3 DMOD
Q5 3 8 0 QMOD
.ENDS NAND
21.5. FOUR-BIT BINARY ADDER (BIPOLAR) 413
Continue 4 Bit adder:
.SUBCKT ONEBIT 1 2 3 4 5 6
* NODES: INPUT (2), CARRY -IN , OUTPUT , CARRY -OUT , VCC
X1 1 2 7 6 NAND
X2 1 7 8 6 NAND
X3 2 7 9 6 NAND
X4 8 9 10 6 NAND
X5 3 10 11 6 NAND
X6 3 11 12 6 NAND
X7 10 11 13 6 NAND
X8 12 13 4 6 NAND
X9 11 7 5 6 NAND
.ENDS ONEBIT
.SUBCKT TWOBIT 1 2 3 4 5 6 7 8 9
* NODES : INPUT - BIT0 (2) / BIT1 (2) , OUTPUT - BIT0 / BIT1 ,
* CARRY -IN , CARRY -OUT , VCC
X1 1 2 7 5 10 9 ONEBIT
X2 3 4 10 6 8 9 ONEBIT
.ENDS TWOBIT
.SUBCKT FOURBIT 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15
* NODES : INPUT - BIT0 (2) / BIT1 (2) / BIT2 (2) / BIT3 (2) ,
* OUTPUT - BIT0 / BIT1 / BIT2 / BIT3 , CARRY -IN , CARRY -OUT , VCC
X1 1 2 3 4 9 10 13 16 15 TWOBIT
X2 5 6 7 8 11 12 16 14 15 TWOBIT
.ENDS FOURBIT
*** DEFINE NOMINAL CIRCUIT
.MODEL DMOD D
.MODEL QMOD NPN(BF =75 RB =100 CJE =1 PF CJC =3 PF)
VCC 99 0 DC 5V
VIN1A 1 0 PULSE (0 3 0 10 NS 10 NS 10NS 50NS)
VIN1B 2 0 PULSE (0 3 0 10 NS 10 NS 20NS 100 NS)
VIN2A 3 0 PULSE (0 3 0 10 NS 10 NS 40NS 200 NS)
VIN2B 4 0 PULSE (0 3 0 10 NS 10 NS 80NS 400 NS)
VIN3A 5 0 PULSE (0 3 0 10 NS 10 NS 160 NS 800NS)
VIN3B 6 0 PULSE (0 3 0 10 NS 10 NS 320 NS 1600 NS)
VIN4A 7 0 PULSE (0 3 0 10 NS 10 NS 640 NS 3200 NS)
VIN4B 8 0 PULSE (0 3 0 10 NS 10 NS 1280 NS 6400 NS)
X1 1 2 3 4 5 6 7 8 9 10 11 12 0 13 99 FOURBIT
RBIT0 9 0 1K
RBIT1 10 0 1K
RBIT2 11 0 1K
RBIT3 12 0 1K
RCOUT 13 0 1K
*** ( FOR THOSE WITH MONEY ( AND MEMORY ) TO BURN )
. TRAN 1 NS 6400 NS
.END
414 CHAPTER 21. EXAMPLE CIRCUITS
21.6 Four-Bit Binary Adder (MOS)
The following deck simulates a four-bit binary adder, using several subcircuits to describe vari-
ous pieces of the overall circuit.
Example:
ADDER - 4 BIT ALL -NAND - GATE BINARY ADDER
*** SUBCIRCUIT DEFINITIONS
.SUBCKT NAND in1 in2 out VDD
* NODES : INPUT (2) , OUTPUT , VCC
M1 out in2 Vdd Vdd p1 W=7.5u L =0.35u pd =13.5u ad =22.5 p
+ ps =13.5 u as =22.5 p
M2 net .1 in2 0 0 n1 W=3u L =0.35 u pd=9u ad=9p
+ ps=9u as=9p
M3 out in1 Vdd Vdd p1 W=7.5u L =0.35u pd =13.5u ad =22.5 p
+ ps =13.5 u as =22.5 p
M4 out in1 net .1 0 n1 W=3u L=0.35u pd =9u ad =9p
+ ps=9u as=9p
.ENDS NAND
.SUBCKT ONEBIT 1 2 3 4 5 6 AND
X2 1 7 8 6 NAND
X3 2 7 9 6 NAND
X4 8 9 10 6 NAND
X5 3 10 11 6 NAND
X6 3 11 12 6 NAND
X7 10 11 13 6 NAND
X8 12 13 4 6 NAND
X9 11 7 5 6 NAND
.ENDS ONEBIT
.SUBCKT TWOBIT 1 2 3 4 5 6 7 8 9
* NODES : INPUT - BIT0 (2) / BIT1 (2), OUTPUT - BIT0 / BIT1 ,
* CARRY - IN , CARRY -OUT , VCC
X1 1 2 7 5 10 9 ONEBIT
X2 3 4 10 6 8 9 ONEBIT
.ENDS TWOBIT
.SUBCKT FOURBIT 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15
* NODES : INPUT - BIT0 (2) / BIT1 (2) / BIT2 (2) / BIT3 (2) ,
* OUTPUT - BIT0 / BIT1 / BIT2 / BIT3 , CARRY -IN ,
* CARRY -OUT , VCC
X1 1 2 3 4 9 10 13 16 15 TWOBIT
X2 5 6 7 8 11 12 16 14 15 TWOBIT
.ENDS FOURBIT
21.7. TRANSMISSION-LINE INVERTER 415
Continue 4 Bit adder MOS:
*** POWER
VCC 99 0 DC 3.3V
*** INPUTS
VIN1A 1 0 DC 0 PULSE (0 3 0 5NS 5NS 20 NS 50 NS)
VIN1B 2 0 DC 0 PULSE (0 3 0 5NS 5NS 30 NS 100 NS)
VIN2A 3 0 DC 0 PULSE (0 3 0 5NS 5NS 50 NS 200 NS)
VIN2B 4 0 DC 0 PULSE (0 3 0 5NS 5NS 90 NS 400 NS)
VIN3A 5 0 DC 0 PULSE (0 3 0 5NS 5NS 170 NS 800 NS)
VIN3B 6 0 DC 0 PULSE (0 3 0 5NS 5NS 330 NS 1600 NS)
VIN4A 7 0 DC 0 PULSE (0 3 0 5NS 5NS 650 NS 3200 NS)
VIN4B 8 0 DC 0 PULSE (0 3 0 5NS 5NS 1290 NS 6400 NS)
*** DEFINE NOMINAL CIRCUIT
X1 1 2 3 4 5 6 7 8 9 10 11 12
0 13 99 FOURBIT
.option acct
.save V(1) V(2) V(3) V (4) V(5) V (6) V(7) V (8) $ INPUTS
.save V(9) V (10) V(11) V (12) V(13) $ OUTPUTS
. TRAN 1 NS 6400 NS
* use BSIM3 model with default parameters
.model n1 nmos level =49 version =3.3.0
.model p1 pmos level =49 version =3.3.0
.END
21.7 Transmission-Line Inverter
The following deck simulates a transmission-line inverter. Two transmission-line elements are
required since two propagation modes are excited. In the case of a coaxial line, the first line
(T1) models the inner conductor with respect to the shield, and the second line (T2) models the
shield with respect to the outside world.
416 CHAPTER 21. EXAMPLE CIRCUITS
Example:
Transmission -line inverter
v1 1 0 pulse (0 1 0 0.1n)
r1 1 2 50
x1 2 0 0 4 tline
r2 4 0 50
.subckt tline 1 2 3 4
t1 1 2 3 4 z0=50 td =1.5 ns
t2 2 0 4 0 z0 =100 td=1ns
.ends tline
.tran 0.1 ns 20 ns
.end
Chapter 22
Statistical circuit analysis
22.1 Introduction
Real circuits do not operate in a world with fixed values of device parameters, power supplies
and environmental data. Even if a ngspice output offers 5 digits or more of precision, this
should not mislead you thinking that your circuits will behave exactly the same. All physical
parameters influencing a circuit (e.g. MOS Source/drain resistance, threshold voltage, transcon-
ductance) are distributed parameters, often following a Gaussian distribution with a mean value
µand a standard deviation σ.
To obtain circuits operating reliably under varying parameters, it might be necessary to simulate
them taking certain parameter spreads into account. ngspice offers several methods supporting
this task. A powerful random number generator is working in the background. Its seed va-
lue is derived from the process id upon start-up of ngspice. If you need reproducible random
numbers, you may start ngspice setting the command set rndseed=<int value> into spinit
or .spiceinit. The following three chapters offer a short introduction to the statistical methods
available in ngspice. The diversity of approaches stems from historical reasons, and from some
efforts to make ngspice compatible to other simulators.
22.2 Using random param(eters)
The ngspice frontend (with its ’numparam’ parser) contains the .param (see Chapt. 2.8.1) and
.func (see Chapt. 2.9) commands. Among the built-in functions supported (see 2.8.5) you will
find the following statistical functions:
417
418 CHAPTER 22. STATISTICAL CIRCUIT ANALYSIS
Built-in function Notes
gauss(nom, rvar, sigma) nominal value plus variation drawn from Gaussian
distribution with mean 0 and standard deviation rvar
(relative to nominal), divided by sigma
agauss(nom, avar, sigma) nominal value plus variation drawn from Gaussian
distribution with mean 0 and standard deviation avar
(absolute), divided by sigma
unif(nom, rvar) nominal value plus relative variation (to nominal)
uniformly distributed between +/-rvar
aunif(nom, avar) nominal value plus absolute variation uniformly distributed
between +/-avar
limit(nom, avar) nominal value +/-avar, depending on random number in
[-1, 1) being > 0 or < 0
The frontend parser evaluates all .param or .func statements upon start-up of ngspice, before
the circuit is evaluated. The parameters aga, aga2, lim obtain their numerical values once. If the
random function appears in a device card (e.g. v11 11 0 ’agauss(1,2,3)’), a new random
number is generated.
Random number example using parameters:
* random number tests
. param aga = agauss (1 ,2 ,3)
. param aga2 = ’2* aga ’
. param lim =limit (0 ,1.2)
. func rgauss (a,b ,c) ’5* agauss (a ,b,c )’
* always same value as defined above
v1 1 0 ’lim ’
v2 2 0 ’lim ’
* may be a different value
v3 3 0 ’ limit (0 ,1.2) ’
* always new random values
v11 11 0 ’agauss (1 ,2 ,3) ’
v12 12 0 ’agauss (1 ,2 ,3) ’
v13 13 0 ’agauss (1 ,2 ,3) ’
* same value as defined above
v14 14 0 ’aga ’
v15 15 0 ’aga ’
v16 16 0 ’aga2 ’
* using .func , new random values
v17 17 0 ’rgauss (0 ,2 ,3) ’
v18 18 0 ’rgauss (0 ,2 ,3) ’
.op
.control
run
print v(1) v(2) v(3) v (11) v(12) v (13)
print v(14) v (15) v(16) v (17) v(18)
.endc
.end
22.3. BEHAVIORAL SOURCES (B, E, G, R, L, C) WITH RANDOM CONTROL 419
So v1, v2, and v3 will get the same value, whereas v4 might differ. v11, v12, and v13 will get
different values, v14, v15, and v16 will obtain the values set above in the .param statements.
.func will start its replacement algorithm, rgauss(a,b,c) will be replaced everywhere by
5*agauss(a,b,c).
Thus device and model parameters may obtain statistically distributed starting values. You
simply set a model parameter not to a fixed numerical value, but insert a ’parameter’ instead,
which may consist of a token defined in a .param card, by calling .func or by using a built-
in function, including the statistical functions described above. The parameter values will be
evaluated once immediately after reading the input file.
22.3 Behavioral sources (B, E, G, R, L, C) with random con-
trol
All sources listed in the section header may contain parameters, which will be evaluated before
simulation starts, as described in the previous section (22.2). In addition the nonlinear voltage
or current sources (B-source, 5) as well as their derivatives E and G, but also the behavioral R,
L, and C may be controlled during simulation by a random independent voltage source V with
TRRANDOM option (Chapt. 4.1.8).
An example circuit, a Wien bridge oscillator from input file /examples/Monte_Carlo/OpWien.sp
is distributed with ngspice or available at Git. The two frequency determining pairs of R and
C are varied statistically using four independent Gaussian voltage sources as the controlling
units. An excerpt of this command sequence is shown below. The total simulation time ttime
is divided into 100 equally spaced blocks. Each block will get a new set of control voltages,
e.g. VR2, which is Gaussian distributed, mean 0 and absolute deviation 1. The resistor value
is calculated with ±10% spread, the factor 0.033 will set this 10% to be a deviation of 1 sigma
from nominal value.
Examples for control of a behavioral resistor:
* random resistor
.param res = 10k
.param ttime =12000 m
.param varia =100
.param ttime10 = ’ttime /varia ’
* random control voltage ( Gaussian distribution )
VR2 r2 0 dc 0 trrandom (2 ’ttime10 ’ 0 1)
* behavioral resistor
R2 4 6 R = ’res + 0.033 * res*V(r2)’
So within a single simulation run you will obtain 100 different frequency values issued by the
Wien bridge oscillator. The voltage sequence VR2 is shown below.
420 CHAPTER 22. STATISTICAL CIRCUIT ANALYSIS
22.4 ngspice scripting language
The ngspice scripting language is described in detail in Chapt. 17.8. All commands listed in
Chapt. 17.5 are available, as well as the built-in functions described in Chapt. 17.2, the control
structures listed in Chapt. 17.6, and the predefined variables from Chapt. 17.7. Variables and
functions are typically evaluated after a simulation run. You may created loops with several
simulation runs and change device and model parameters with the alter (17.5.3) or altermod
(17.5.4) commands, as shown in the next section 22.5. You may even interrupt a simulation run
by proper usage of the stop (17.5.74) and resume (17.5.53) commands. After stop you may
change device or model parameters and then go on with resume, continuing the simulation with
the new parameter values.
The statistical functions provided for scripting are listed in the following table:
22.5. MONTE-CARLO SIMULATION 421
Name Function
rnd(vector) A vector with each component a random integer between 0
and the absolute value of the input vector’s corresponding
integer element value.
sgauss(vector) Returns a vector of random numbers drawn from a
Gaussian distribution (real value, mean = 0 , standard
deviation = 1). The length of the vector returned is
determined by the input vector. The contents of the input
vector will not be used. A call to sgauss(0) will return a
single value of a random number as a vector of length 1..
sunif(vector) Returns a vector of random real numbers uniformly
distributed in the interval [-1 .. 1[. The length of the vector
returned is determined by the input vector. The contents of
the input vector will not be used. A call to sunif(0) will
return a single value of a random number as a vector of
length 1.
poisson(vector) Returns a vector with its elements being integers drawn
from a Poisson distribution. The elements of the input
vector (real numbers) are the expected numbers λ.
Complex vectors are allowed, real and imaginary values
are treated separately.
exponential(vector) Returns a vector with its elements (real numbers) drawn
from an exponential distribution. The elements of the input
vector are the respective mean values (real numbers).
Complex vectors are allowed, real and imaginary values
are treated separately.
22.5 Monte-Carlo Simulation
The ngspice scripting language may be used to run Monte-Carlo simulations with statistically
varying device or model parameters. Calls to the functions sgauss(0) or sunif(0) (see 17.2) will
return Gaussian or uniform distributed random numbers (real numbers), stored in a vector. You
may define (see 17.5.14) your own function using sgauss or sunif, e.g. to change the mean or
range. In a loop (see 17.6) then you may call the alter (17.5.3) or altermod (17.5.4) statements
with random parameters followed by an analysis like op, dc, ac, tran or other.
22.5.1 Example 1
The first examples is a LC band pass filter, where L and C device parameters will be changed 100
times. Each change is followed by an ac analysis. All graphs of output voltage versus frequency
are plotted. The file is available in the distribution as /examples/Monte_Carlo/MonteCarlo.sp
as well as from the CVS repository.
422 CHAPTER 22. STATISTICAL CIRCUIT ANALYSIS
Monte-Carlo example 1
Perform Monte Carlo simulation in ngspice
V1 N001 0 AC 1 DC 0
R1 N002 N001 141
*
C1 OUT 0 1e-09
L1 OUT 0 10e -06
C2 N002 0 1e -09
L2 N002 0 10e -06
L3 N003 N002 40e -06
C3 OUT N003 250e -12
*
R2 0 OUT 141
*
.control
let mc_runs = 100
let run = 1
set curplot = new $ create a new plot
set scratch = $curplot $ store its name to ’scratch ’
*
define unif(nom , var) (nom + nom*var * sunif (0))
define aunif(nom , avar) (nom + avar * sunif (0))
define gauss(nom , var , sig) ( nom + nom*var /sig * sgauss (0))
define agauss(nom , avar , sig) (nom + avar /sig * sgauss (0))
*
dowhile run <= mc_runs
* alter c1 = unif (1e -09 , 0.1)
* alter l1 = aunif (10e -06 , 2e -06)
* alter c2 = aunif (1e -09 , 100e -12)
* alter l2 = unif (10 e-06 , 0.2)
* alter l3 = aunif (40e -06 , 8e -06)
* alter c3 = unif (250e -12 , 0.15)
alter c1 = gauss (1e-09 , 0.1 , 3)
alter l1 = agauss (10e-06, 2e -06, 3)
alter c2 = agauss (1e -09 , 100 e-12 , 3)
alter l2 = gauss (10e -06 , 0.2 , 3)
alter l3 = agauss (40e-06, 8e -06, 3)
alter c3 = gauss (250e -12 , 0.15 , 3)
ac oct 100 250K 10 Meg
set run ="$&run " $ create a variable from the vector
set dt = $curplot $ store the current plot to dt
setplot $scratch $ make ’scratch ’ the active plot
* store the output vector to plot ’scratch ’
let vout {$run }={ $dt }.v (out )
setplot $dt $ go back to the previous plot
let run = run + 1
end
plot db ({ $scratch }. all )
.endc
.end
22.5. MONTE-CARLO SIMULATION 423
22.5.2 Example 2
A more sophisticated input file for Monte Carlo simulation is distributed with the file /exam-
ples/Monte_Carlo/MC_ring.sp (or git repository). Due to its length it is not reproduced here,
but some comments on its enhancements over example 1 (22.5.1) are presented in the following.
A 25-stage ring oscillator is the circuit used with a transient simulation. It comprises of CMOS
inverters, modeled with BSIM3. Several model parameters (vth, u0, tox, L, and W) shall be
varied statistically between each simulation run. The frequency of oscillation will be measured
by a fft and stored. Finally a histogram of all measured frequencies will be plotted.
The function calls to sunif(0) and sgauss(0) return uniformly or Gaussian distributed random
numbers. A function unif, defined by the line
define unif(nom, var) (nom + (nom*var) * sunif(0))
will return a value with mean nom and deviation var relative to nom.
The line
set n1vth0=@n1[vth0]
will store the threshold voltage vth0, given by the model parameter set, into a variable n1vth0,
ready to be used by unif,aunif,gauss, or agauss function calls.
In the simulation loop the altermod command changes the model parameters before a call to
tran. After the transient simulation the resulting vector is linearized, a fft is calculated, and the
maximum of the fft signal is measured by the meas command and stored in a vector maxffts.
Finally the contents of the vector maxffts is plotted in a histogram.
For more details, please have a look at the strongly commented input file MC_ring.sp.
22.5.3 Example 3
The next example is contained in the files MC_2_control.sp and MC_2_circ.sp from folder
/examples/Monte_Carlo/. MC_2_control.sp is a ngspice script (see 17.8). It starts a loop
by setting the random number generator seed value to the value of the loop counter, sources
the circuit file MC_2_circ.sp, runs the simulation, stores a raw file, makes an fft, saves the
oscillator frequency thus measured, deletes all outputs, increases the loop counter and restarts
the loop. The netlist file MC_2_circ.sp contains the circuit, which is the same ring oscillator
as of example 2. However, now the MOS model parameter set, which is included with this
netlist file, inherits some AGAUSS functions (see 2.8.5) to vary threshold voltage, mobility and
gate oxide thickness of the NMOS and PMOS transistors. This is an approach similar to what
commercial foundries deliver within their device libraries. So this example may be your source
for running Monte Carlo with commercial libs. Start example 3 by calling
ngspice -o MC_2_control.log MC_2_control.sp
22.5.4 Example 4
The next example, contained in the files MC_ring_ts.sp from folder /examples/Monte_Carlo/,
makes use of several advanced ngspice features supporting MonteCarlo simulation of circuits
with foundry transistor parameters. The current example has been checked with an X-FAB
424 CHAPTER 22. STATISTICAL CIRCUIT ANALYSIS
XH018 library and a TSMC library. You will have to obtain these libraries directly from the
foundry or an associated service organisation (MOSIS, CMP, Europractise etc.). To simplify
the evaluation, a simple BSIM3 model parameter set may be used instead. MC_ring_ts.sp is
a ngspice script (see 17.8). It sets some variables, i.e. sourcepath and outputpath, sources
the circuit file mc_ring_circ.net, starts a loop by setting the random number generator seed
value to the value of the loop counter, re-sources the circuit file from internal storage, runs the
simulation, stores some data, skips non-converging simulations, makes an fft, saves the oscil-
lator frequency thus measured, deletes all outputs, increases the loop counter and restarts the
loop. The netlist file mc_ring_circ.net contains the circuit, which is the same ring oscillator as
in example 2. However, now the MOS model parameter set is taken from a foundry library. As
an alternative a simple BSIM3 model set, which is included with this netlist file, inherits some
AGAUSS functions (see 2.8.5) to vary threshold voltages of the NMOS and PMOS transistors.
Start example 4 by calling
ngspice -o MC_ring_ts.log MC_ring_ts.sp
When using the shared library ngspice or the Windows console (both don’t have a graphics
interface), (see 22.6 below) is used for plotting.
22.6 Data evaluation with
Run the example file /examples/Monte_Carlo/OpWien.sp, described in Chapt. 22.3. Gene-
rate a plot with by the ngspice command
pl4mag v4mag xlimit 500 1500
Open and run the command file in the command line window by
load ’pl-v4mag.p’
A Gaussian curve will be fitted to the simulation data. The mean oscillator frequency and its
deviation are printed in the curve fitting log in the window.
22.6. DATA EVALUATION WITH 425
script for data evaluation:
# This file : pl - v4mag .p
# ngspice file OpWien.sp
# ngspice command :
# pl4mag v4mag xlimit 500 1500
# a manual :
# http :// www . duke . edu /~ hpgavin /. html
# Gauss function to be fitted
f1(x )=( c1 /( a1 *sqrt (2*3.14159))* exp ( -((x -b1 )**2)/(2* a1 **2)))
# Gauss function to plot start graph
f2(x )=( c2 /( a2 *sqrt (2*3.14159))* exp ( -((x -b2 )**2)/(2* a2 **2)))
# start values
a1=50 ; b1 =900 ; c1 =50
# keep start values in a2 , b2 , c2
a2=a1 b2=b1 ; c2=c1
# curve fitting
fit f1 (x ) ’ pl4mag .data ’ using 1:2 via a1 , b1 , c1
# plot original and fitted curves with new a1 , b1 , c1
plot " pl4mag. data " using 1:2 with lines , f1(x), f2(x)
pl4mag.data is the simulation data, f2(x) the starting curve, f1(x) the fitted Gaussian distribution.
This is just a simple example. You might explore the powerful built-in functions of to do a much
426 CHAPTER 22. STATISTICAL CIRCUIT ANALYSIS
more sophisticated statistical data analysis.
Chapter 23
Circuit optimization with ngspice
23.1 Optimization of a circuit
Your circuit design (analog, maybe mixed-signal) has already the best circuit topology. There
might be still some room for parameter selection, e.g. the geometries of transistors or values of
passive elements, to best fit the specific purpose. This is, what (automatic) circuit optimization
will deliver. In addition you may fine-tune, optimize and verify the circuit over voltage, process
or temperature corners. So circuit optimization is a valuable tool in the hands of an experienced
designer. It will relieve you from the routine task of ’endless’ repetitions of re-simulating your
design.
You have to choose circuit variables as parameters to be varied during optimization (e.g. device
size, component values, bias inputs etc.). Then you may pose performance constraints onto
you circuits (e.g. Vnode < 1.2V, gain > 50 etc.). Optimization objectives are the variables to be
minimized or maximized. The n objectives and m constraints are assembled into a cost function.
The optimization flow is now the following: The circuit is loaded. Several (perhaps only one)
simulations are started with a suitable starter set of variables. Measurements are done on the
simulator output to check for the performance constraints and optimization objectives. These
data are fed into the optimizer to evaluate the cost function. A sophisticated algorithm now
determines a new set of circuit variables for the next simulator run(s). Stop conditions have to
be defined by the user to tell the simulator when to finish (e.g. fall below a cost function value,
parameter changes fall below a certain threshold, number of iterations exceeded).
The optimizer algorithms, its parameters and the starting point influence the convergence beha-
vior. The algorithms have to provide measures to reaching the global optimum, not to stick to a
local one, and thus are tantamount for the quality of the optimizer.
ngspice does not have an integral optimization processor. Thus this chapter will rely on work
done by third parties to introduce ngspice optimization capability.ngspice provides the simula-
tion engine, a script or program controls the simulator and provides the optimizer functionality.
Four optimizers are presented here, using ngspice scripting language, using tclspice, using a
Python script, and using ASCO, a c-coded optimization program.
427
428 CHAPTER 23. CIRCUIT OPTIMIZATION WITH NGSPICE
23.2 ngspice optimizer using ngspice scripts
Friedrich Schmidt (see his web site) has intensively used circuit optimization during his deve-
lopment of Nonlinear loadflow computation with Spice based simulators. He has provided an
optimizer using the internal ngspice scripting language (see Chapt. 17.8). His original scripts
are found here. A slightly modified and concentrated set of his scripts is available from the
ngspice optimizer directory.
The simple example given in the scripts is ok with current ngspice. Real circuits have still to be
tested.
23.3 ngspice optimizer using tclspice
ngspice offers another scripting capability, namely the tcl/tk based tclspice option (see Chapt.
20). An optimization procedure may be written using a tcl script. An example is provided in
Chapt. 20.5.2.
23.4 ngspice optimizer using a Python script
Werner Hoch has developed a ngspice optimization procedure based on the ’differential evolu-
tion’ algorithm [21]. On his web page he provides a Python script containing the control flow
and algorithms.
23.5 ngspice optimizer using ASCO
The ASCO optimizer, developed by Joao Ramos, also applies the ’differential evolution’ al-
gorithm [21]. An enhanced version 0.4.7.1, adding ngspice as a simulation engine, may be
downloaded here (7z archive format). Included are executable files (asco, asco-mpi, ngspice-c
for MS Windows). The source code should also compile and function under Linux (not yet
tested).
ASCO is a standalone executable, which communicates with ngspice via ngspice input and out-
put files. Several optimization examples, originally provided by J. Ramos for other simulators,
are prepared for use with ngspice. Parallel processing on a multi-core computer has been tested
using MPI (MPICH2) under MS Windows. A processor network will be supported as well.
A MS Windows console application ngspice_c.exe is included in the archive. Several stand
alone tools are provided, but not tested yet.
Setting up an optimization project with ASCO requires advanced know-how of using ngspice.
There are several sources of information. First of all the examples provided with the distribu-
tion give hints how to start with ASCO. The original ASCO manual is provided as well, or is
available here. It elaborates on the examples, using a commercial simulator, and provides a
detailed description how to set up ASCO. Installation of ASCO and MPI (under Windows) is
described in a file INSTALL.
23.5. NGSPICE OPTIMIZER USING ASCO 429
Some remarks on how to set up ASCO for ngspice are given in the following sections (more
to be added). These a meant not as a complete description, but are an addition the the ASCO
manual.
23.5.1 Three stage operational amplifier
This example is taken from Chapt. 6.2.2 ‘Tutorial #2’ from the ASCO manual. The directory
examples /ngspice/amp3 contains four files:
amp3.cfg This file contains all configuration data for this optimization. Of special interest is
the following section, which sets the required measurements and the constraints on the measured
parameters:
# Measurements #
ac_power:VDD:MIN:0
dc_gain:VOUT:GE:122
unity_gain_frequency:VOUT:GE:3.15E6
phase_margin:VOUT:GE:51.8
phase_margin:VOUT:LE:70
amp3_slew_rate:VOUT:GE:0.777E6
#
Each of these entries is linked to a file in the /extract subdirectory, having exactly the same na-
mes as given here, e.g. ac_power,dc_gain,unity_gain,phase_margin, and amp3_slew_rate.
Each of these files contains an # Info # section, which is currently not used. The # Commands
#section may contain a measurement command (including ASCO parameter #SYMBOL#, see
file /extract/unity_gain_frequency). It also may contain a .control section (see file /ex-
tract/phase_margin_min). During set-up #SYMBOL# is replaced by the file name, a leading
‘z’, and a trailing number according to the above sequence, starting with 0.
amp3.sp This is the basic circuit description. Entries like #LM2# are ASCO-specific, defined
in the # Parameters # section of file amp3.cfg. ASCO will replace these parameter placehol-
ders with real values for simulation, determined by the optimization algorithm. The .control
... .endc section is specific to ngspice. Entries to this section may deliver workarounds of
some commands not available in ngspice, but used in other simulators. You may also define
additional measurements, get access to variables and vectors, or define some data manipulation.
In this example the .control section contains an op measurement, required later for slew rate
calculation, as well as the ac simulation, which has to occur before any further data evaluation.
Data from the op simulation are stored in a plot op1. Its name is saved in variable dt. The ac
measurements sets another plot ac1. To retrieve op data from the former plot, you have to use
the {$dt}.<vector> notation (see file /extract/amp3_slew_rate).
n.typ, p.typ MOSFET parameter files, to be included by amp3.sp.
430 CHAPTER 23. CIRCUIT OPTIMIZATION WITH NGSPICE
Testing the set-up
Copy asco-test.exe and ngspice_c.exe (console executable of ngspice) into the directory, and
run
$ asco-test -ngspice amp3
from the console window. Several files will be created during checking. If you look at <computer-
name>.sp: this is the input file for ngspice_c, generated by ASCO. You will find the ad-
ditional .measure commands and .control sections. The quit command will be added
automatically just before the .endc command in its own .control section. asco-test will
display error messages on the console, if the simulation or communication with ASCO is not
ok. The output file <computer-name>.out, generated by ngspice during each simulation, con-
tains symbols like zac_power0,zdc_gain1,zunity_gain_frequency2,zphase_margin3,
zphase_margin4, and zamp3_slew_rate5. These are used to communicate the ngspice
output data to ASCO. ASCO is searching for something like zdc_gain1 =, and then takes
the next token as the input value. Calling phase_margin twice in amp3.cfg has lead to
two measurements in two .control sections with different symbols (zphase_margin3,zp-
hase_margin4).
A failing test may result in an error message from ASCO. Sometimes, however, ASCO freezes
after some output statements. This may happen if ngspice issues an error message that cannot
be handled by ASCO. Here it may help calling ngspice directly with the input file generated by
ASCO:
$ ngspice_c <computer-name>.sp
Thus you may evaluate the ngspice messages directly.
Running the simulation
Copy (w)asco.exe, (w)asco-mpi.exe and ngspice_c.exe (console executable of ngspice)
into the directory, and run
$ asco -ngspice amp3
or alternatively (if MPICH is installed)
$ mpiexec -n 7 asco-mpi -ngspice amp3
The following graph 23.1 shows the acceleration of the optimization simulation on a multi-core
processor (i7 with 4 real or 8 virtual cores), 500 generations, if -n is varied. Speed is tripled, a
mere 15 min suffices to optimize 21 parameters of the amplifier.
23.5.2 Digital inverter
This example is taken from Chapt. 6.2.1 Tutorial #1 from the ASCO manual. In addition to the
features already mentioned above, it adds Monte-Carlo and corner simulations. The file inv.cfg
contains the following section:
#Optimization Flow#
Alter:yes $ do we want to do corner analysis?
23.5. NGSPICE OPTIMIZER USING ASCO 431
Figure 23.1: Optimization speed
MonteCarlo:yes $ do we want to do MonteCarlo analysis?
AlterMC cost:3.00 $ point at which we want to start ALTER and/or
$ MONTECARLO
ExecuteRF:no $ Execute or no the RF module to add RF parasitics?
SomethingElse:
#
Monte Carlo is switched on. It uses the AGAUSS function (see Chapt. 22.2). Its parameters
are generated by ASCO from the data supplied by the inv.cfg section #Monte Carlo#. Accor-
ding to the paper by Pelgrom on MOS transistor matching [22] the AGAUSS parameters are
calculated as
W=AGAU SS W,ABeta
√2·W·L·m·W
100 ·10−6,1(23.1)
delvto =AGAU SS 0,AV T
√2·W·L·m·10−9,1(23.2)
The .ALTER command is not available in ngspice. However, a new option in ngspice to the
altermod command (17.5.4) enables the simulation of design corners. The #Alter# section in
inv.cfg gives details. Specific to ngspice, again several .control section are used.
# ALTER #
.control
* gate oxide thickness varied
altermod nm pm file [b3.min b3.typ b3.max]
.endc
.control
* power supply variation
alter vdd=[2.0 2.1 2.2]
.endc
432 CHAPTER 23. CIRCUIT OPTIMIZATION WITH NGSPICE
.control
run
.endc
#
NMOS (nm) and PMOS (pm) model parameter sets are loaded from three different model files,
each containing both NMOS and PMOS sets. b3.typ is assembled from the original parameter
files n.typ and p.typ, provided with original ASCO, with some adaptation to ngspice BSIM3.
The min and max sets are artificially created in that only the gate oxide thickness deviates ±1
nm from what is found in model file b3.typ. In addition the power supply voltage is varied,
so in total you will find 3 x 3 simulation combinations in the input file <computer-name>.sp
(after running asco-test).
23.5.3 Bandpass
This example is taken from Chapt. 6.2.4 Tutorial #4 from the ASCO manual. S11 in the
passband is to be maximised. S21 is used to extract side lobe parameters. The .net command
is not available in ngspice, so S11 and S21 are derived with a script in file bandpass.sp as
described in Chapt. 17.9. The measurements requested in bandpass.cfg as
# Measurements #
Left_Side_Lobe:---:LE:-20
Pass_Band_Ripple:---:GE:-1
Right_Side_Lobe:---:LE:-20
S11_In_Band:---:MAX:---
#
are realized as ’measure’ commands inside of control sections (see files in directory extract).
The result of a measure statement is a vector, which may be processed by commands in the
following lines. In file extract/S1_In_Band #Symbol# is made available only after a short
calculation (inversion of sign), using the print command. quit has been added to this entry
because it will become the final control section in <computer-name>.sp. A disadvantage of
measure inside of a .control section is that parameters from .param statements may not be
used (as is done in example 23.5.4).
The bandpass example includes the calculation of RF parasitic elements defined in rfmodule.cfg
(see Chapt. 7.5 of the ASCO manual). This calculation is invoked by setting
ExecuteRF:yes $Execute or no the RF module to add RF parasitics?
in bandpass.cfg. The two subcircuits LBOND_sub and CSMD_sub are generated in <computer-
name>.sp to simulate these effects.
23.5. NGSPICE OPTIMIZER USING ASCO 433
23.5.4 Class-E power amplifier
This example is taken from Chapt. 6.2.3 Tutorial #3 from the ASCO manual. In this example
the ASCO post processing is applied in file extract/P_OUT (see Chapt. 7.4 of the ASCO
manual.). In this example .measure statements are used. They allow using parameters from
.param statements, because they will be located outside of .control sections, but do not allow
to do data post processing inside of ngspice. You may use ASCO post processing instead.
434 CHAPTER 23. CIRCUIT OPTIMIZATION WITH NGSPICE
Chapter 24
Notes
24.1 Glossary
card A logical SPICE input line. A card may be extended through the use of the ‘+’ sign in
SPICE, thereby allowing it to take up multiple lines in a SPICE deck.
code model A model of a device, function, component, etc. which is based solely on a C
programming language-based function. In addition to the code models included with the
XSPICE option of the ngspice simulator, you can use code models that you develop for
circuit modeling.
deck A collection of SPICE cards that together specify all input information required in order
to perform an analysis. A ‘deck’ of ‘cards’ will in fact be contained within a file on the
host computer system.
element card A single, logical line in an ngspice circuit deck that describes a circuit element.
Circuit elements are connected to each other to form circuits (e.g., a logical card that
describes a resistor, such as R1 2 0 10K, is an element card).
instance A unique occurrence of a circuit element. See ‘element card’, in which the instance
R1 is specified as a unique element (instance) in a hypothetical circuit description.
macro A macro, in the context of this document, refers to a C language macro that supports the
construction of user-defined models by simplifying input/output and parameter-passing
operations within the Model Definition File.
.mod Refers to the Model Definition File in XSPICE. The file suffix reflects the file-name of
the model definition file: cfunc.mod.
.model Refers to a model card associated with an element card in ngspice. A model card allows
for data defining an instance to be conveniently located in the ngspice deck such that the
general layout of the elements is more readable.
Nutmeg The ngspice default post-processor. This provides a simple stand-alone simulator
interface that can be used with the ngspice simulator to display and plot simulator raw
files.
subcircuit A ‘device’ within an ngspice deck that is defined in terms of a group of element
cards and that can be referenced in other parts of the ngspice deck through element cards.
435
436 CHAPTER 24. NOTES
24.2 Acronyms and Abbreviations
ATE Automatic Test Equipment
CAE Computer-Aided Engineering
CCCS Current Controlled Current Source.
CCVS Current Controlled Voltage Source.
FET Field Effect Transistor
IDD Interface Design Document
IFS Refers to the Interface Specification File. The abbreviation reflects the file name of the
Interface Specification File: ifspec.ifs.
MNA Modified Nodal Analysis
MOSFET Metal Oxide Semiconductor Field Effect Transistor
PWL Piece-Wise Linear
RAM Random Access Memory
ROM Read Only Memory
SDD Software Design Document
SI Simulator Interface
SPICE Simulation Program with Integrated Circuit Emphasis. This program was developed at
the University of California at Berkeley and is the origin of ngspice.
SPICE3 Version 3 of SPICE.
SRS Software Requirements Specification
SUM Software User’s Manual
UCB University of California at Berkeley
UDN User-Defined Node(s)
VCCS Voltage Controlled Current Source.
VCVS Voltage Controlled Voltage Source
XSPICE Extended SPICE; option to ngspice, integrating predefined or user defined code mo-
dels for event-driven mixed-signal simulation.
Bibliography
[1] A. Vladimirescu and S. Liu, ‘The Simulation of MOS Integrated Circuits Using SPICE2’
ERL Memo No. ERL M80/7, Electronics Research Laboratory University of California,
Berkeley, October 1980
[2] T. Sakurai and A. R. Newton, ‘A Simple MOSFET Model for Circuit Analysis and its ap-
plication to CMOS gate delay analysis and series-connected MOSFET Structure’ERL
Memo No. ERL M90/19, Electronics Research Laboratory, University of California, Ber-
keley, March 1990
[3] B. J. Sheu, D. L. Scharfetter, and P. K. Ko, ‘SPICE2 Implementation of BSIM’ ERL Memo
No. ERL M85/42, Electronics Research Laboratory University of California, Berkeley,
May 1985
[4] J. R. Pierret, ‘A MOS Parameter Extraction Program for the BSIM Model’ ERL Memo
Nos. ERL M84/99 and M84/100, Electronics Research Laboratory University of Califor-
nia, Berkeley, November 1984
[5] Min-Chie Jeng, ‘Design and Modeling of Deep Submicrometer MOSFETSs’ ERL Memo
Nos. ERL M90/90, Electronics Research Laboratory, University of California, Berkeley,
October 1990
[6] Soyeon Park, ‘Analysis and SPICE implementation of High Temperature Effects on MOS-
FET’, Master’s thesis, University of California, Berkeley, December 1986.
[7] Clement Szeto, ‘Simulation of Temperature Effects in MOSFETs (STEIM)’, Master’s the-
sis, University of California, Berkeley, May 1988.
[8] J.S. Roychowdhury and D.O. Pederson, ‘Efficient Transient Simulation of Lossy Intercon-
nect’, Proc. of the 28th ACM/IEEE Design Automation Conference, June 17-21 1991, San
Francisco
[9] A. E. Parker and D. J. Skellern, ‘An Improved FET Model for Computer Simulators’, IEEE
Trans CAD, vol. 9, no. 5, pp. 551-553, May 1990.
[10] R. Saleh and A. Yang, Editors, ‘Simulation and Modeling’, IEEE Circuits and Devices,
vol. 8, no. 3, pp. 7-8 and 49, May 1992.
[11] H.Statz et al., ‘GaAs FET Device and Circuit Simulation in SPICE’, IEEE Transactions
on Electron Devices, V34, Number 2, February 1987, pp160-169.
[12] Weidong Liu et al.: ‘BSIM3v3.2.3 MOSFET Model User’s Manual’, BSIM3v3.2.3
437
438 BIBLIOGRAPHY
[13] Weidong Lui et al.: ‘BSIM3.v3.3.0 MOSFET Model User’s Manual’, BSIM3v3.3.0
[14] ‘SPICE3.C1 Nutmeg Programmer’s Manual’, Department of Electrical Engineering and
Computer Sciences, University of California, Berkeley, California, April, 1987.
[15] Thomas L. Quarles: SPICE3 Version 3C1 User’s Guide, Department of Electrical En-
gineering and Computer Sciences, University of California, Berkeley, California, April,
1989.
[16] Brian Kernighan and Dennis Ritchie: ‘The C Programming Language’, Second Edition,
Prentice-Hall, Englewood Cliffs, New Jersey, 1988.
[17] ‘Code-Level Modeling in XSPICE’, F.L. Cox, W.B. Kuhn, J.P. Murray, and S.D. Tynor, pu-
blished in the Proceedings of the 1992 International Symposium on Circuits and Systems,
San Diego, CA, May 1992, vol 2, pp. 871-874.
[18] ‘A Physically Based Compact Model of Partially Depleted SOI MOSFETs for Analog Ci-
rcuit Simulation’, Mike S. L. Lee, Bernard M. Tenbroek, William Redman-White, James
Benson, and Michael J. Uren, IEEE JOURNAL OF SOLID-STATE CIRCUITS, VOL. 36,
NO. 1, JANUARY 2001, pp. 110-121
[19] ‘A Realistic Large-signal MESFET Model for SPICE’, A. E. Parker, and D. J. Skellern,
IEEE Transactions on Microwave Theory and Techniques, vol. 45, no. 9, Sept. 1997, pp.
1563-1571.
[20] ‘Integrating RTS Noise into Circuit Analysis’, T. B. Tang and A. F. Murray, IEEE ISCAS,
2009, Proc. of IEEE ISCAS, Taipei, Taiwan, May 2009, pp 585-588 (link)
[21] R. Storn, and K. Price: ‘Differential Evolution’, technical report TR-95-012, ICSI, March
1995, see report download, or the DE web page
[22] M. J. M. Pelgrom e.a.: ‘Matching Properties of MOS Transistors’, IEEE J. Sol. State Circ,
vol. 24, no. 5, Oct. 1989, pp. 1433-1440
[23] Y. V. Pershin, M. Di Ventra: ‘SPICE model of memristive devices with threshold’,
arXiv:1204.2600v1 [physics.comp-ph] 12 Apr 2012, http://arxiv.org/pdf/1204.2600.pdf
Part II
XSPICE Software User’s Manual
439
Chapter 25
XSPICE Basics
25.1 ngspice with the XSPICE option
The XSPICE option allows you to add event-driven simulation capabilities to NGSPICE. NG-
SPICE now is the main software program that performs mathematical simulation of a circuit
specified by you, the user. It takes input in the form of commands and circuit descriptions and
produces output data (e.g. voltages, currents, digital states, and waveforms) that describe the
circuit’s behavior.
Plain NGSPICE is designed for analog simulation and is based exclusively on matrix solution
techniques. The XSPICE option adds even-driven simulation capabilities. Thus, designs that
contain significant portions of digital circuitry can be efficiently simulated together with analog
components. NGSPICE with XSPICE option also includes a ‘User-Defined Node’ capability
that allows event-driven simulations to be carried out with any type of data.
The XSPICE option has been developed by the Computer Science and Information Technology
Laboratory at Georgia Tech Research Institute of the Georgia Institute of Technology, Atlanta,
Georgia 30332 at around 1990 and enhanced by the NGSPICE team. The manual is based on
the original XSPICE user’s manual, made available from Georgia Tech.
In the following, the term ‘XSPICE’ may be read as ‘NGSPICE with XSPICE code mo-
del subsystem enabled’. You may enable the option by adding --enable-xspice to the
./configure command. The MS Windows distribution already contains the XSPICE option.
25.2 The XSPICE Code Model Subsystem
The new component of ngspice, the Code Model Subsystem, provides the tools needed to model
the various parts of your system. While NGSPICE is targeted primarily at integrated circuit (IC)
analysis, XSPICE includes features to model and simulate board-level and system-level designs
as well. The Code Model Subsystem is central to this new capability, providing XSPICE with
an extensive set of models to use in designs and allowing you to add your own models to this
model set.
The NGSPICE simulator at the core of XSPICE includes built-in models for discrete compo-
nents commonly found within integrated circuits. These ‘model primitives’ include components
441
442 CHAPTER 25. XSPICE BASICS
such as resistors, capacitors, diodes, and transistors. The XSPICE Code Model Subsystem ex-
tends this set of primitives in two ways. First, it provides a library of over 40 additional pri-
mitives, including summers, integrators, digital gates, controlled oscillators, s-domain transfer
functions, and digital state machines. See Chapt. 12 for a description of the library entries.
Second, it adds a code model generator to ngspice that provides a set of programming utili-
ties to make it easy for you to create your own models by writing them in the C programming
language.
The code models are generated upon compiling ngspice. They are stored in shared libraries,
which may be distributed independently from the ngspice sources. Upon runtime ngspice will
load the code model libraries and make the code model instances available for simulation.
25.3 XSPICE Top-Level Diagram
A top-level diagram of the XSPICE system integrated into ngspice is shown in Fig. 25.1.
The XSPICE Simulator is made up of the NGSPICE core, the event-driven algorithm, circuit
description syntax parser extensions, a loading routine for code models, and the Nutmeg user
interface. The XSPICE Code Model Subsystem consists of the Code Model Generator, 5 stan-
dard code model library sources with more than 40 code models, the sources for Node Type
Libraries, and all the interfaces to User-Defined Code Models and to User-Defined Node Types.
Figure 25.1: ngspice/XSPICE Top-Level Diagram
Chapter 26
Execution Procedures
This chapter covers operation of the XSPICE simulator and the Code Model Subsystem. It
begins with background material on simulation and modeling and then discusses the analysis
modes supported in XSPICE and the circuit description syntax used for modeling. Detailed
descriptions of the predefined Code Models and Node Types provided in the XSPICE libraries
are also included.
26.1 Simulation and Modeling Overview
This section introduces the concepts of circuit simulation and modeling. It is intended primarily
for users who have little or no previous experience with circuit simulators, and also for those
who have not used circuit simulators recently. However, experienced SPICE users may wish to
scan the material presented here since it provides background for new Code Model and User-
Defined Node capabilities of the XSPICE option.
26.1.1 Describing the Circuit
This section provides an overview of the circuit description syntax expected by the XSPICE
simulator. A general understanding of circuit description syntax will be helpful to you should
you encounter problems with your circuit and need to examine the simulator’s error messages,
or should you wish to develop your own models.
This section will introduce you to the creation of circuit description input files using the Nutmeg
user interface. Note that this material is presented in an overview form. Details of circuit
description syntax are given later in this chapter and in the previous chapters of this manual.
26.1.1.1 Example Circuit Description Input
Although different SPICE-based simulators may include various enhancements to the basic
version from the University of California at Berkeley, most use a similar approach in describing
circuits. This approach involves capturing the information present in a circuit schematic in
the form of a text file that follows a defined format. This format requires the assignment of
alphanumeric identifiers to each circuit node, the assignment of component identifiers to each
443
444 CHAPTER 26. EXECUTION PROCEDURES
Figure 26.1: Example Circuit 1
circuit device, and the definition of the significant parameters for each device. For example, the
circuit description below shows the equivalent input file for the circuit shown in Fig. 26.1.
Examples for control of a behavioral resistor:
Small Signal Amplifier
*
* This circuit simulates a simple small signal amplifier .
*
Vin Input 0
0 SIN (0 .1 500 Hz)
R_source Input Amp_In 100
C1 Amp_In 0 1uF
R_Amp_Input Amp_In 0 1MEG
E1 (Amp_Out 0) ( Amp_In 0) -10
R_Load Amp_Out 0 1000
.Tran 1.0u 0.01
.end
This file exhibits many of the most important properties common to all SPICE circuit descrip-
tion files including the following:
• The first line of the file is always interpreted as the title of the circuit. The title may
consist of any text string.
• Lines that provide user comments, but no circuit information, are begun by an asterisk.
• A circuit device is specified by a device name, followed by the node(s) to which it is
connected, and then by any required parameter information.
• The first character of a device name tells the simulator what kind of device it is (e.g. R =
resistor, C = capacitor, E = voltage controlled voltage source).
• Nodes may be labeled with any alphanumeric identifier. The only specific labeling requi-
rement is that 0 must be used for ground.
26.1. SIMULATION AND MODELING OVERVIEW 445
• A line that begins with a dot is a ‘control directive’ Control directives are used most
frequently for specifying the type of analysis the simulator is to carry out.
• An .end statement must be included at the end of the file.
• With the exception of the Title and .end statements, the order in which the circuit file is
defined is arbitrary.
• All identifiers are case insensitive - the identifier ‘npn’ is equivalent to ‘NPN’ and to
‘nPn’.
• Spaces and parenthesis are treated as white space.
• Long lines may be continued on a succeeding line by beginning the next line with a ‘+’
in the first column.
In this example, the title of the circuit is ‘Small Signal Amplifier’. Three comment lines are
included before the actual circuit description begins. The first device in the circuit is voltage
source Vin, which is connected between node Input and ‘0’ (ground). The parameters after
the nodes specify that the source has an initial value of 0, a wave shape of SIN, and a DC offset,
amplitude, and frequency of 0, .1, and 500 respectively. The next device in the circuit is resistor
R_Source, which is connected between nodes Input and Amp_In, with a value of 100 Ohms.
The remaining device lines in the file are interpreted similarly.
The control directive that begins with .tran specifies that the simulator should carry out a
simulation using the Transient analysis mode. In this example, the parameters to the transient
analysis control directive specify that the maximum time-step allowed is 1 microsecond and
that the circuit should be simulated for 0.01 seconds of circuit time.
Other control cards are used for other analysis modes. For example, if a frequency response plot
is desired, perhaps to determine the effect of the capacitor in the circuit, the following statement
will instruct the simulator to perform a frequency analysis from 100 Hz to 10 MHz in decade
intervals with ten points per decade.
.ac dec 10 100 10meg
To determine the quiescent operating point of the circuit, the following statement may be inser-
ted in the file.
.op
A fourth analysis type supported by ngspice is swept DC analysis. An example control state-
ment for the analysis mode is
.dc Vin -0.1 0.2 .05
This statement specifies a DC sweep that varies the source Vin from -100 millivolts to +200
millivolts in steps of 50 millivolts.
446 CHAPTER 26. EXECUTION PROCEDURES
26.1.1.2 Models and Subcircuits
The file discussed in the previous section illustrated the most basic syntax rules of a circuit des-
cription file. However, ngspice (and other SPICE-based simulators) include many other features
that allow for accurate modeling of semiconductor devices such as diodes and transistors and
for grouping elements of a circuit into a macro or ‘subcircuit’ description that can be reused
throughout a circuit description. For instance, the file shown below is a representation of the
schematic shown in Fig. 26.2.
Examples for control of a behavioral resistor:
Small Signal Amplifier with Limit Diodes
*
* This circuit simulates a small signal amplifier
* with a diode limiter .
*
.dc Vin -1 1 .05
Vin Input 0 DC 0
R_source Input Amp_In 100
D_Neg 0 Amp_In 1 n4148
D_Pos Amp_In 0 1n4148
C1 Amp_In 0 1uF
X1 Amp_In 0 Amp_Out Amplifier
R_Load Amp_Out 0 1000
. model 1 n4148 D ( is =2.495 e -09 rs =4.755e -01 n =1.679 e+00
+ tt =3.030 e -09 cjo =1.700 e-12 vj =1 m=1.959 e -01 bv =1.000 e +02
+ ibv =1.000 e -04)
.subckt Amplifier Input Common Output
E1 ( Output Common ) (Input Common ) -10
R_Input Input Common 1meg
.ends Amplifier
.end
This is the same basic circuit as in the initial example, with the addition of two components and
some changes to the simulation file. The two diodes have been included to illustrate the use of
device models, and the amplifier is implemented with a subcircuit. Additionally, this file shows
the use of the swept DC control card.
Device Models Device models allow you to specify, when required, many of the parameters
of the devices being simulated. In this example, model statements are used to define the silicon
diodes. Electrically, the diodes serve to limit the voltage at the amplifier input to values between
about ±700 millivolts. The diode is simulated by first declaring the ‘instance’ of each diode
with a device statement. Instead of attempting to provide parameter information separately for
both diodes, the label ‘1n4148’ alerts the simulator that a separate model statement is included
26.1. SIMULATION AND MODELING OVERVIEW 447
Figure 26.2: Example Circuit 2
in the file that provides the necessary electrical specifications for the device (‘1n4148’ is the
part number for the type of diode the model is meant to simulate).
The model statement that provides this information is:
. model 1 n4148 D ( is =2.495 e -09 rs =4.755e -01 n =1.679 e+00
+ tt =3.030 e -09 cjo =1.700 e-12 vj =1 m=1.959 e -01
+ bv =1.000 e +02 ibv =1.000 e -04)
The model statement always begins with the string .model followed by an identifier and the
model type (D for diode, NPN for NPN transistors, etc).
The optional parameters (‘is’, ‘rs’, ‘n’, . . . ) shown in this example configure the simulator’s
mathematical model of the diode to match the specific behavior of a particular part (e.g. a
‘1n4148’).
Subcircuits In some applications, describing a device by embedding the required elements
in the main circuit file, as is done for the amplifier in Fig. 26.1, is not desirable. A hierarchical
approach may be taken by using subcircuits. An example of a subcircuit statement is shown in
the second circuit file:
X1 Amp_In 0 Amp_Out
Amplifier Subcircuits are always identified by a device label beginning with ‘X’. Just as with
other devices, all of the connected nodes are specified. Notice, in this example, that three nodes
are used. Finally, the name of the subcircuit is specified. Elsewhere in the circuit file, the
simulator looks for a statement of the form:
.subckt <Name > <Node1 > <Node2 > <Node3 > ...
This statement specifies that the lines that follow are part of the Amplifier subcircuit, and that the
three nodes listed are to be treated wherever they occur in the subcircuit definition as referring,
respectively, to the nodes on the main circuit from which the subcircuit was called. Normal
device, model, and comment statements may then follow. The subcircuit definition is concluded
with a statement of the form:
448 CHAPTER 26. EXECUTION PROCEDURES
.ends <Name >
26.1.1.3 XSPICE Code Models
In the previous example, the specification of the amplifier was accomplished by using a NG-
SPICE Voltage Controlled Voltage Source device. This is an idealization of the actual amplifier.
Practical amplifiers include numerous non-ideal effects, such as offset error voltages and non-
ideal input and output impedances. The accurate simulation of complex, real-world components
can lead to cumbersome subcircuit files, long simulation run times, and difficulties in synthesi-
zing the behavior to be modeled from a limited set of internal devices known to the simulator.
To address these problems, XSPICE allows you to create Code Models that simulate complex,
non-ideal effects without the need to develop a subcircuit design. For example, the following file
provides simulation of the circuit in Fig. 26.2, but with the subcircuit amplifier replaced with
a Code Model called ‘Amp’ that models several non-ideal effects including input and output
impedance and input offset voltage.
Small Signal Amplifier
*
* This circuit simulates a small signal amplifier
* with a diode limiter .
*
.dc Vin -1 1 .05
Vin Input 0 DC 0
R_source Input Amp_In 100
D_Neg 0 Amp_In 1n4148
D_Pos Amp_In 0 1n4148
C1 Amp_In 0 1uF
A1 Amp_In 0 Amp_Out Amplifier
R_Load Amp_Out 0 1000
. model 1 n4148 D ( is =2.495 e -09 rs =4.755e -01 n =1.679 e+00
+ tt =3.030 e -09 cjo =1.700 e-12 vj =1 m=1.959 e -01 bv =1.000 e +02
+ ibv =1.000 e -04)
.model Amplifier Amp ( gain = -10 in_offset = 1e-3
+ rin = 1 meg rout = 0.4)
.end
A statement with a device label beginning with ‘A’ alerts the simulator that the device uses
a Code Model. The model statement is similar in form to the one used to specify the diode.
The model label ‘Amp’ directs XSPICE to use the code model with that name. Parameter
information has been added to specify a gain of -10, an input offset of 1 millivolt, an input
impedance of 1 meg ohm, and an output impedance of 0.4 ohm. Subsequent sections of this
document detail the steps required to create such a Code Model and include it in the XSPICE
simulator.
26.2. CIRCUIT DESCRIPTION SYNTAX 449
26.1.1.4 Node Bridge Models
When a mixed-mode simulator is used, some method must be provided for translating data
between the different simulation algorithms. XSPICE’s Code Model support allows you to
develop models that work under the analog simulation algorithm, the event-driven simulation
algorithm, or both at once.
In XSPICE, models developed for the express purpose of translating between the different al-
gorithms or between different User-Defined Node types are called ‘Node Bridge’ models. For
translations between the built-in analog and digital types, predefined node bridge models are
included in the XSPICE Code Model Library.
26.1.1.5 Practical Model Development
In practice, developing models often involves using a combination of NGSPICE passive devi-
ces, device models, subcircuits, and XSPICE Code Models. XSPICE’s Code Models may be
seen as an extension to the set of device models offered in standard NGSPICE. The collection
of over 40 predefined Code Models included with XSPICE provides you with an enriched set of
modeling primitives with which to build subcircuit models. In general, you should first attempt
to construct your models from these available primitives. This is often the quickest and easiest
method.
If you find that you cannot easily design a subcircuit to accomplish your goal using the available
primitives, then you should turn to the code modeling approach. Because they are written in a
general purpose programming language (C), code models enable you to simulate virtually any
behavior for which you can develop a set of equations or algorithms.
26.2 Circuit Description Syntax
If you need to debug a simulation, if you are planning to develop your own models, or if you
are using the XSPICE simulator through the Nutmeg user interface, you will need to become
familiar with the circuit description language.
The previous sections presented example circuit description input files. The following sections
provide more detail on XSPICE circuit descriptions with particular emphasis on the syntax
for creating and using models. First, the language and syntax of the NGSPICE simulator are
described and references to additional information are given. Next, XSPICE extensions to the
ngspice syntax are detailed. Finally, various enhancements to NGSPICE operation are discussed
including polynomial sources, arbitrary phase sources, supply ramping, matrix conditioning,
convergence options, and debugging support.
26.2.1 XSPICE Syntax Extensions
In the preceding discussion, NGSPICE syntax was reviewed, and those features of NGSPICE
that are specifically supported by the XSPICE simulator were enumerated. In addition to these
features, there exist extensions to the NGSPICE capabilities that provide much more flexibility
in describing and simulating a circuit. The following sections describe these capabilities, as
well as the syntax required to make use of them.
450 CHAPTER 26. EXECUTION PROCEDURES
26.2.1.1 Convergence Debugging Support
When a simulation is failing to converge, the simulator can be asked to return convergence diag-
nostic information that may be useful in identifying the areas of the circuit in which convergence
problems are occurring. When running through the Nutmeg user interface, these messages are
written directly to the terminal.
26.2.1.2 Digital Nodes
Support is included for digital nodes that are simulated by an event-driven algorithm. Because
the event-driven algorithm is faster than the standard SPICE matrix solution algorithm, and
because all digital,real,int and User-Defined Node types make use of the event-driven
algorithm, reduced simulation time for circuits that include these models can be anticipated
compared to simulation of the same circuit using analog code models and nodes.
26.2.1.3 User-Defined Nodes
Support is provided for User Defined Nodes that operate with the event-driven algorithm. These
nodes allow the passing of arbitrary data structures among models. The real and integer node
types supplied with XSPICE are actually predefined User-Defined Node types.
26.2.1.4 Supply Ramping
A supply ramping function is provided by the simulator as an option to a transient analysis
to simulate the turn-on of power supplies to a board level circuit. To enable this option, the
compile time flag XSPICE_EXP has to be set, e.g. by adding CFLAGS="-DXSPICE_EXP" to
the ./configure command line. The supply ramping function linearly ramps the values of all
independent sources and the capacitor and inductor code models (code model extension) with
initial conditions toward their final value at a rate that you define. A complete ngspice deck
example of usage of the ramptime option is shown below.
26.3. HOW TO CREATE CODE MODELS 451
Example:
Supply ramping option
*
* This circuit demonstrates the use of the option
* " ramptime" that ramps independent sources and the
* capacitor and inductor initial conditions from
* zero to their final value during the time period
* specified .
*
*
.tran 0.1 5
.option ramptime =0.2
* a1 1 0 cap
. model cap capacitor (c =1000 uf ic =1)
r1 1 0 1k
*
a2 2 0 ind
.model ind inductor (l=1H ic =1)
r2 2 0 1.0
*
v1 3 0 1.0
r3 3 0 1k
*
i1 4 0 1e-3
r4 4 0 1k
*
v2 5 0 0.0 sin (0 1 0.3 0 0 45.0)
r5 5 0 1k
*
.end
26.3 How to create code models
The following instruction to create an additional code model uses the ngspice infrastructure and
some ’intelligent’ copy and paste. As an example an extra code model d_xxor is created in the
xtradev shared library, reusing the existing d_xor model from the digital library. More detailed
information will be made available in Chapt. 28.
You should have downloaded ngspice, either the most recent distribution or from the Git re-
pository, and compiled and installed it properly according to your operating system and the
instructions given in Chapt. 32 of the Appendix, especially Chapt. 32.1.4 (for Linux users), or
Chapt. 32.2.2 for MINGW and MS Windows (MS Visual Studio will not do, because we not
yet have integrated the code model generator into this compiler! You may however use all code
models later with any ngspice executable.) . Then change into directory ngspice/src/xspice/i-
cm/xtradev.
Create a new directory
452 CHAPTER 26. EXECUTION PROCEDURES
mkdir d_xxor
Copy the two files cfunc.mod and ifspec.ifs from ngspice/src/xspice/icm/digital/d_xor to ng-
spice/src/xspice/icm/xtradev/d_xxor. These two files may serve as a template for your new
model!
For simplicity reasons we do only a very simple editing to these files here, in fact the functiona-
lity is not changed, just the name translated to a new model. Edit the new cfunc.mod: In lines
5, 28, 122, 138, 167, 178 replace the old name (d_xor) by the new name d_xxor. Edit the new
ifspec.ifs: In lines 16, 23, 24 replace cm_d_xor by cm_d_xxor and d_xor by d_xxor.
Make ngspice aware of the new code model by editing file
ngspice/src/xspice/icm/xtradev/modpath.lst:
Add a line with the new model name d_xxor.
Redo ngspice by entering directory ngspice/release, and issuing the commands:
make
sudo make install
And that’s it! In ngspice/release/src/xspice/icm/xtradev/ you now will find cfunc.c and
ifspec.c and the corresponding object files. The new code model d_xxor resides in the shared
library xtradev.cm, and is available after ngspice is started. As a test example you may edit
ngspice/src/xspice/examples/digital_models1.deck, and change line 60 to the new model:
.model d_xor1 d_xxor (rise_delay=1.0e-6 fall_delay=2.0e-6 input_load=1.0e-12)
The complete input file follows:
26.3. HOW TO CREATE CODE MODELS 453
Code Model Test: new xxor
*
*** analysis type ***
.tran .01s 4s
*
*** input sources ***
*
v2 200 0 DC PWL( (0 0.0) (2 0.0) (2.0000000001 1.0) (3 1.0) )
*
v1 100 0 DC PWL( (0 0.0) (1.0 0.0) (1.0000000001 1.0) (2 1.0)
+ (2.0000000001 0.0) (3 0.0) (3.0000000001 1.0) (4 1.0) )
*
*** resistors to ground ***
r1 100 0 1k
r2 200 0 1k
*
*** adc_bridge blocks ***
aconverter [200 100] [2 1] adc_bridge1
.model adc_bridge1 adc_bridge ( in_low =0.1 in_high =0.9
+ rise_delay =1.0 e -12 fall _delay =1.0 e -12)
*
*** xor block ***
a7 [1 2] 70 d_xor1
.model d_xor1 d_xxor ( rise_delay =1.0e -6 fall_delay =2.0e-6
+ input_load =1.0e -12)
*
*** dac_bridge blocks ****
abridge1 [70] [out ] dac1
.model dac1 dac_bridge ( out_low = 0.7 out_high = 3.5
+ out_undef = 2.2 input_load = 5.0e -12 t_rise = 50e -9
+ t_fall = 20e -9)
*
*** simulation and plotting ***
.control
run
plot allv
.endc
*
.end
An analog input, delivered by the pwl voltage sources, is transformed into the digital domain
by an adc_bridge, processed by the new code model d_xxor, and then translated back into the
analog domain.
If you want to change the functionality of the new model, you have to edit ifspec.ifs for the
code model interface and cfunc.mod for the detailed functionality of the new model. Please see
Chapt. 28, especially Chapt. 28.6 ff. for any details. And of course you may take the existing
454 CHAPTER 26. EXECUTION PROCEDURES
analog, digital, mixed signal and other existing code models (to be found in the subdirectories
to ngspice/release/src/xspice/icm) as stimulating examples for your work.
Chapter 27
Example circuits
The following chapter is designed to demonstrate XSPICE features. The first example circuit
models the circuit of Fig. 26.2 using the XSPICE gain block code model to substitute for the
more complex and computationally expensive ngspice transistor model. This example illustra-
tes one way in which XSPICE code models can be used to raise the level of abstraction in circuit
modeling to improve simulation speed.
The next example, shown in Fig. 27.1, illustrates many of the more advanced features offered by
XSPICE. This circuit is a mixed-mode design incorporating digital data, analog data, and User-
Defined Node data together in the same simulation. Some of the important features illustrated
include:
• Creating and compiling Code Models
• Creating an XSPICE executable that incorporates these new models
• The use of ‘node bridge’ models to translate data between the data types in the simulation
• Plotting analog and event-driven (digital and User-Defined Node) data
• Using the eprint command to print event-driven data
Throughout these examples, we assume that ngspice with XSPICE option has already been
installed on your system and that your user account has been set up with the proper search path
and environment variable data.
The examples also assume that you are running under Linux and will use standard Linux com-
mands such as cp for copying files, etc. If you are using a different set up, with different ope-
rating system command names, you should be able to translate the commands shown into those
suitable for your installation. Finally, file system path-names given in the examples assume
that ngspice + XSPICE has been installed on your system in directory /usr/local/xspice-1-0.
If your installation is different, you should substitute the appropriate root path-name where
appropriate.
27.1 Amplifier with XSPICE model ‘gain’
The circuit, as has been shown in Fig. 26.2, is extended here by using the XSPICE code model
gain. The ngspice circuit description for this circuit is shown below.
455
456 CHAPTER 27. EXAMPLE CIRCUITS
Example:
A transistor amplifier circuit
*
.tran 1e -5 2e-3
*
vin 1 0 0.0 ac 1.0 sin (0 1 1k)
*
ccouple 1 in 10 uF
rzin in 0 19.35 k
*
aamp in aout gain_block
.model gain_block gain ( gain = -3.9 out_offset = 7.003)
*
rzout aout coll 3.9k
rbig coll 0 1e12
*
.end
Notice the component ‘aamp’. This is an XSPICE code model device. All XSPICE code model
devices begin with the letter ‘a’ to distinguish them from other ngspice devices. The actual
code model used is referenced through a user-defined identifier at the end of the line - in this
case gain_block. The type of code model used and its parameters appear on the associated
.model card. In this example, the gain has been specified as -3.9 to approximate the gain of the
transistor amplifier, and the output offset (out_offset) has been set to 7.003 according to the DC
bias point information obtained from the DC analysis in Example 1.
Notice also that input and output impedances of the one-transistor amplifier circuit are modeled
with the resistors ‘rzin’ and ‘rzout’, since the gain code model defaults to an ideal voltage-
input, voltage-output device with infinite input impedance and zero output impedance.
Lastly, note that a special resistor ‘rbig’ with value ‘1e12’ has been included at the opposite side
of the output impedance resistor ‘rzout’. This resistor is required by ngspice’s matrix solution
formula. Without it, the resistor ‘rzout’ would have only one connection to the circuit, and
an ill-formed matrix could result. One way to avoid such problems without adding resistors
explicitly is to use the ngspice ‘rshunt’ option described in this document under ngspice Syntax
Extensions/General Enhancements.
To simulate this circuit, copy the file xspice_c2.cir from the directory /src/xspice/exam-
ples into a directory in your account.
$ cp /examples/xspice/xspice_c2.cir xspice_c2.cir
Invoke the simulator on this circuit:
$ ngspice xspice_c2.cir
After a few moments, you should see the ngspice prompt:
ngspice 1 ->
27.2. XSPICE ADVANCED USAGE 457
Now issue the run command and when the prompt returns, issue the plot command to examine
the voltage at the node ‘coll’.
ngspice 1 -> run
ngspice 2 -> plot coll
The resulting waveform closely matches that from the original transistor amplifier circuit simu-
lated in Example 1.
When you are done, enter the quit command to leave the simulator and return to the command
line.
ngspice 3 -> quit
Using the rusage command, you can verify that this abstract model of the transistor amplifier
runs somewhat faster than the full circuit of Example 1. This is because the code model is less
complex computationally. This demonstrates one important use of XSPICE code models - to
reduce run time by modeling circuits at a higher level of abstraction. Speed improvements vary
and are most pronounced when a large amount of low-level circuitry can be replaced by a small
number of code models and additional components.
27.2 XSPICE advanced usage
27.2.1 Circuit example C3
An equally important use of code models is in creating models for circuits and systems that do
not easily lend themselves to synthesis using standard ngspice primitives (resistors, capacitors,
diodes, transistors, etc.). This occurs often when trying to create models of ICs for use in simu-
lating board-level designs. Creating models of operational amplifiers such as an LM741 or timer
ICs such as an LM555 is greatly simplified through the use of XSPICE code models. Another
example of code model use is shown in the next example where a complete sampled-data system
is simulated using XSPICE analog, digital, and User-Defined Node types simultaneously.
The circuit shown in Fig. 27.1 is designed to demonstrate several of the more advanced features
of XSPICE. In this example, you will be introduced to the process of creating code models and
linking them into ngspice. You will also learn how to print and plot the results of event-driven
analysis data. The ngspice/XSPICE circuit description for this example is shown below.
458 CHAPTER 27. EXAMPLE CIRCUITS
Figure 27.1: Example Circuit C3
Example:
Mixed IO types
* This circuit contains a mixture of IO types , including
* analog , digital , user -defined ( real), and ’null ’.
*
* The circuit demonstrates the use of the digital and
* user - defined node capability to model system - level designs
* such as sampled -data filters . The simulated circuit
* contains a digital oscillator enabled after 100 us. The
* square wave oscillator output is divided by 8 with a
* ripple counter . The result is passed through a digital
* filter to convert it to a sine wave .
*
.tran 1e -5 1e-3
*
v1 1 0 0.0 pulse (0 1 1e -4 1e -6)
r1 1 0 1k
*
abridge1 [1] [ enable ] atod
.model atod adc_bridge
*
aclk [ enable clk] clk nand
. model nand d_nand ( rise_delay =1e -5 fall_delay =1e -5)
*
adiv2 div2_out clk NULL NULL NULL div2_out dff
adiv4 div4_out div2_out NULL NULL NULL div4_out dff
adiv8 div8_out div4_out NULL NULL NULL div8_out dff
.model dff d_dff
27.2. XSPICE ADVANCED USAGE 459
Example (continued):
abridge2 div8_out enable filt_in node_bridge2
. model node_bridge2 d_to_real ( zero = -1 one =1)
*
xfilter filt_in clk filt_out dig_filter
*
abridge3 filt_out a_out node_bridge3
.model node_bridge3 real_to_v
*
rlpf1 a_out oa_minus 10 k
*
xlpf 0 oa_minus lpf_out opamp
*
rlpf2 oa_minus lpf_out 10 k
clpf lpf_out oa_minus 0.01 uF
***************************************
.subckt dig_filter filt_in clk filt_out
.model n0 real_gain ( gain =1.0)
.model n1 real_gain ( gain =2.0)
.model n2 real_gain ( gain =1.0)
.model g1 real_gain ( gain =0.125)
.model zm1 real_delay
. model d0a real_gain ( gain = -0.75)
.model d1a real_gain ( gain =0.5625)
.model d0b real_gain ( gain = -0.3438)
.model d1b real_gain ( gain =1.0)
*
an0a filt_in x0a n0
an1a filt_in x1a n1
an2a filt_in x2a n2
*
az0a x0a clk x1a zm1
az1a x1a clk x2a zm1
*
ad0a x2a x0a d0a
ad1a x2a x1a d1a
*
az2a x2a filt1_out g1
az3a filt1_out clk filt2_in zm1
*
an0b filt2_in x0b n0
an1b filt2_in x1b n1
an2b filt2_in x2b n2
*
az0b x0b clk x1b zm1
az1b x1b clk x2b zm1
*
ad0 x2b x0b d0b
ad1 x2b x1b d1b
*
az2b x2b clk filt_out zm1
.ends dig_filter
460 CHAPTER 27. EXAMPLE CIRCUITS
Example (continued):
.subckt opamp plus minus out
*
r1 plus minus 300k
a1 %vd ( plus minus ) outint lim
.model lim limit (out_lower_limit = -12 out_upper_limit = 12
+ fraction = true limit_range = 0.2 gain =300 e3)
r3 outint out 50.0
r2 out 0 1e12
*
.ends opamp
*
.end
This circuit is a high-level design of a sampled-data filter. An analog step waveform (created
from a ngspice pulse waveform) is introduced as ‘v1’ and converted to digital by code model
instance ‘abridge’. This digital data is used to enable a Nand-Gate oscillator (‘aclk’) after a
short delay. The Nand-Gate oscillator generates a square-wave clock signal with a period of
approximately two times the gate delay, which is specified as 1e-5 seconds. This 50 kHz clock
is divided by a series of D Flip Flops (‘adiv2’, ‘adiv4’, ‘adiv8’) to produce a square-wave at
approximately 6.25 kHz. Note particularly the use of the reserved word ‘NULL’ for certain
nodes on the D Flip Flops. This tells the code model that there is no node connected to these
ports of the flip flop.
The divide-by-8 and enable waveforms are converted by the instance ‘abridge2’ to the format
required by the User-Defined Node type ‘real’, which expected real-valued data. The output of
this instance on node filt_in is a real valued square wave that oscillates between values of -1
and 1. Note that the associated code model d_to_real is not part of the original XSPICE code
model library but has been added later to ngspice.
This signal is then passed through subcircuit ‘xfilter’ that contains a digital low-pass filter cloc-
ked by node ‘clk’. The result of passing this square-wave through the digital low-pass filter is
the production of a sampled sine wave (the filter passes only the fundamental of the square-
wave input) on node filt_out. This signal is then converted back to ngspice analog data on
node a_out by node bridge instance ‘abridge3’.
The resulting analog waveform is then passed through an op-amp-based low-pass analog filter
constructed around subcircuit ‘xlpf’ to produce the final output at analog node ‘lpf_out’.
27.2.2 Running example C3
Now copy the file xspice_c3.cir from directory /examples/xspice/ into the current directory:
$ cp /examples/xspice/xspice_c3.cir xspice_c3.cir
and invoke the new simulator executable as you did in the previous examples.
$ ngspice xspice_c3.cir
27.2. XSPICE ADVANCED USAGE 461
Execute the simulation with the run command.
ngspice 1 -> run
After a short time, the ngspice prompt should return. Results of this simulation are examined
in the manner illustrated in the previous two examples. You can use the plot command to plot
either analog nodes, event-driven nodes, or both. For example, you can plot the values of the
sampled-data filter input node and the analog low-pass filter output node as follows:
ngspice 2 -> plot filt_in lpf_out
The plot shown in Fig. 27.2 should appear.
Figure 27.2: Nutmeg Plot of Filter Input and Output
You can also plot data from nodes inside a subcircuit. For example, to plot the data on node
‘x1a’ in subcircuit ‘xfilter’, create a pathname to this node with a dot separator.
ngspice 3 -> plot xfilter.x1a
The output from this command is shown in Fig. 27.3. Note that the waveform contains vertical
segments. These segments are caused by the non-zero delays in the ‘real gain’ models used
within the subcircuit. Each vertical segment is actually a step with a width equal to the model
delay (1e-9 seconds).
Plotting nodes internal to subcircuits works for both analog and event-driven nodes.
To examine data such as the closely spaced events inside the subcircuit at node ‘xfilter.x1a’, it
is often convenient to use the eprint command to produce a tabular listing of events. Try this
by entering the following command:
462 CHAPTER 27. EXAMPLE CIRCUITS
Figure 27.3: Nutmeg Plot of Subcircuit Internal Node
ngspice 4 -> eprint xfilter.x1a
**** Results Data ****
Time or Step
xfilter.x1a
0.000000000e+000 0.000000e+000 1.010030000e-004 2.000000e+000
1.010040000e-004 2.562500e+000 1.210020000e-004 2.812500e+000
1.210030000e-004 4.253906e+000 1.410020000e-004 2.332031e+000
1.410030000e-004 3.283447e+000 1.610020000e-004 2.014893e+000
1.610030000e-004 1.469009e+000 1.810020000e-004 2.196854e+000
1.810030000e-004 1.176232e+000
...
9.610030000e-004 3.006294e-001 9.810020000e-004 2.304755e+000
9.810030000e-004 9.506230e-001
9.810090000e-004 -3.049377e+000
9.810100000e-004 -4.174377e+000
**** Messages ****
**** Statistics ****
Operating point analog/event alternations: 1
Operating point load calls: 37
Operating point event passes: 2
Transient analysis load calls: 4299
Transient analysis timestep backups: 87
This command produces a tabular listing of event-times in the first column and node values in
the second column. The 1 ns delays can be clearly seen in the fifth decimal place of the event
times.
Note that the eprint command also gives statistics from the event-driven algorithm portion of
XSPICE. For this example, the simulator alternated between the analog solution algorithm and
27.2. XSPICE ADVANCED USAGE 463
the event-driven algorithm one time while performing the initial DC operating point solution
prior to the start of the transient analysis. During this operating point analysis, 37 total calls were
made to event-driven code model functions, and two separate event passes or iterations were
required before the event nodes obtained stable values. Once the transient analysis commenced,
there were 4299 total calls to event-driven code model functions. Lastly, the analog simulation
algorithm performed 87 time-step backups that forced the event-driven simulator to backup its
state data and its event queues.
A similar output is obtained when printing the values of digital nodes. For example, print the
values of the node ‘div8 out’ as follows:
ngspice 5 -> eprint div8_out
**** Results Data ****
Time or Step
div8_out
0.000000000e+000 1s
1.810070000e-004 0s
2.610070000e-004 1s
...
9.010070000e-004 1s
9.810070000e-004 0s
**** Messages ****
**** Statistics ****
Operating point analog/event alternations: 1
Operating point load calls: 37
Operating point event passes: 2
Transient analysis load calls: 4299
Transient analysis timestep backups: 87
From this printout, we see that digital node values are composed of a two character string. The
first character (0, 1, or U) gives the state of the node (logic zero, logic one, or unknown logic
state). The second character (s, r, z, u) gives the ‘strength’ of the logic state (strong, resistive,
hi-impedance, or undetermined).
If you wish, examine other nodes in this circuit with either the plot or eprint commands.
When you are done, enter the quit command to exit the simulator and return to the operating
system prompt:
ngspice 6 -> quit
So long.
464 CHAPTER 27. EXAMPLE CIRCUITS
Chapter 28
Code Models and User-Defined Nodes
The following sections explain the steps required to create code models and User-Defined Nodes
(UDNs), store them in shared libraries and load them into the simulator at runtime. The ngspice
simulator already includes XSPICE libraries of predefined models and node types that span the
analog and digital domains. These have been detailed earlier in this document (see Sections
12.2,12.3, and 12.4). However, the real power of the XSPICE is in its support for extending
these libraries with new models written by users. ngspice includes an XSPICE code model
generator. Adding code models to ngspice will require a model definition plus some simple file
operations, which are explained in this chapter.
The original manual cited an XSPICE ‘Code Model Toolkit’ that enabled one to define new
models and node data types to be passed between them offline, independent from ngspice.
Whereas this Toolkit is still available in the original source code distribution at the XSPICE
web page, it is neither required nor supported any more.
So we make use of the existing XSPICE infrastructure provided with ngspice to create new
code models. With an ’intelligent’ copy and paste, and the many available code models serving
as a guide you will be quickly able to create your own models. You have to have a compiler
(gcc) available under Linux, MS Windows (Cygwin, MINGW), maybe also for other OSs,
including supporting software (Flex, Bison, and the autotools if you start from Git sources).
The compilation procedures for ngspice are described in detail in Chapt. 32. Adding a code
model may then require defining the functionality , interface, and eventually user defined nodes.
Compiling into a shared library is only a simple ’make’, loading the shared lib(s) into ngspice is
done by the ngspice command codemodel... (see Chapt. 17.5.11). This will allow you to either
add some code model to an existing library, or you may generate a new library with your own
code models. The latter is of interest if you want to distribute your code models independently
from the ngspice sources or executables.
These new code models are handled by ngspice in a manner analogous to its treating of SPICE
devices and XSPICE Predefined Code Models. The basic steps required to create sources for
new code models or User-Defined Nodes, compile them and load them into ngspice are simi-
lar. They consist of 1) creating the code model or UserDefined Node (UDN) directory and
its associated model or data files, 2) inform ngspice about the code model or UDN directories
that have to be compiled and linked into ngspice, 3) compile them into a shared lib, and 4)
load them into the ngspice simulator upon runtime. All code models finally reside in dynami-
cally linkable shared libraries (*.cm), which in fact are .so files under Linux or dlls under MS
Windows. Currently we have 5 of them (analog.cm,digital.cm,spice2poly.cm,xtradev.cm,
465
466 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
xtraevt.cm). Upon start up of ngspice they are dynamically loaded into the simulator by the
ngspice codemodel command (which is located in file spinit (see Chapt. 16.5) for the stan-
dard code models). Once you have added your new code model into one of these libraries (or
have created a new library file, e.g. my-own.cm), instances of the model can be placed into
any simulator deck that describes a circuit of interest and simulated along with all of the other
components in that circuit.
A quick entry to get a new code model has already been presented in Chapt. 26.3. You may
find the details of the XSPICE language in Chapt. 28.6 ff.
28.1 Code Model Data Type Definitions
There are several data types that you can incorporate into a model. These have already been
used extensively in the code model library included with the simulator. They are detailed below:
Boolean_t The Boolean type is an enumerated type that can take on values of FALSE (integer
value 0) or TRUE (integer value 1). Alternative names for these enumerations are MIF FALSE
and MIF TRUE, respectively.
Complex_t The Complex type is a structure composed of two double values. The first of
these is the .real type, and the second is the .imag type. Typically these values are accessed as
shown:
For complex value ‘data’, the real portion is ‘data.real’, and the imaginary portion is ‘data.imag’.
Digital_State_t The Digital State type is an enumerated value that can be either ZERO (in-
teger value 0), ONE (integer value 1), or UNKNOWN (integer value 2).
Digital_Strength_t The Digital Strength type is an enumerated value that can be either
STRONG (integer value 0), RESISTIVE (integer value 1), HI IMPEDANCE (integer value
2) or UNDETERMINED (integer value 3).
Digital_t The Digital type is a composite of the Digital_State_t and Digital_Strength_t enu-
merated data types. The actual variable names within the Digital type are .state and .strength
and are accessed as shown below:
For Digital_t value ‘data’, the state portion is ‘data.state’, and the strength portion is ‘data.strength’.
28.2 Creating Code Models
The following description deals with extending one of the five existing code model libraries.
Adding a new library is described in Chapt. 28.4. The first step in creating a new code model
within XSPICE is to create a model directory inside of the selected library directory. The new
directory name is the name of the new code model. As an example you may add a directory
d_counter to the library directory digital.
28.3. CREATING USER-DEFINED NODES 467
cd ngspice/src/xspice/icm/digital
mkdir d_counter
Into this new directory you copy the following template files:
• Interface Specification File (ifspec.ifs)
• Model Definition File (cfunc.mod)
You may choose existing files that are similar to the new code model you intend to integrate.
The template Interface Specification File (ifspec.ifs) is edited to define the model’s inputs, out-
puts, parameters, etc (see Chapt. 28.6). You then edit the template Model Definition File
(cfunc.mod) to include the C-language source code that defines the model behavior (see Chapt.
28.7). As a final step you have to notify ngspice of the new code model. You have to edit the
file modpath.lst that resides in the library directory ngspice/src/xspice/icm/digital. Just add
the entry d_counter to this file.
The Interface Specification File is a text file that describes, in a tabular format, information
needed for the code model to be properly interpreted by the simulator when it is placed with
other circuit components into a SPICE deck. This information includes such things as the
parameter names, parameter default values, and the name of the model itself. The specific
format presented to you in the Interface Specification File template must be followed exactly,
but is quite straightforward. A detailed description of the required syntax, along with numerous
examples, is included in Section 28.6.
The Model Definition File contains a C programming language function definition. This function
specifies the operations to be performed within the model on the data passed to it by the simula-
tor. Special macros are provided that allow the function to retrieve input data and return output
data. Similarly, macros are provided to allow for such things as storage of information bet-
ween iteration time-points and sending of error messages. Section 28.7 describes the form and
function of the Model Definition File in detail and lists the support macros provided within the
simulator for use in code models.
To allow compiling and linking (see Chapt. 28.5) you have at least to adapt the names of the
functions inside of the two copied files to get unique function and model names. If for example
you have chosen ifspec.ifs and cfunc.mod from model d_fdiv as your template, simply replace
all entries d_fdiv by d_counter inside of the two files.
28.3 Creating User-Defined Nodes
In addition to providing the capability of adding new models to the simulator, a facility exists
that allows node types other than those found in standard SPICE to be created. Models may be
constructed that pass information back and forth via these nodes. Such models are constructed
in the manner described in the previous sections, with appropriate changes to the Interface
Specification and Model Definition Files.
Because of the need of electrical engineers to have ready access to both digital and analog
simulation capabilities, the digital node type is provided as a built-in node type along with
standard SPICE analog nodes. For digital nodes, extensive support is provided in the form
468 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
of macros and functions so that you can treat this node type as a standard type analogous to
standard SPICE analog nodes when creating and using code models. In addition to analog and
digital nodes, the node types real and int are also provided with the simulator. These were
created using the User-Defined Node (UDN) creation facilities described below and may serve
as a template for further node types.
The first step in creating a new node type within XSPICE is to set up a node type directory
along with the appropriate template files needed.
cd ngspice/src/xspice/icm/xtraevt
mkdir <directory name>
<directory name> should be the name of the new type to be defined. Copy file udnfunc.c
from /icm/xtraevt/int into the new directory. Edit this file according to the new type you want
to create.
Notify ngspice about this new UDN directory by editing
ngspice/src/xspice/icm/xtraevt/udnpath.lst. Add a new line containing <directory name>.
For compiling and linking see Chapt. 28.5.
The UDN Definition File contains a set of C language functions. These functions perform
operations such as allocating space for data structures, initializing them, and comparing them to
each other. Section 28.8 describes the form and function of the User-Defined Node Definition
File in detail and includes an example UDN Definition File.
28.4 Adding a new code model library
A group of code models may be assembled into a library. A new library is a means to distribute
new code models, independently from the existing ones. This is the way to generate a new code
model library:
cd ngspice/src/xspice/icm/
mkdir <directory name>
<directory name> is the name of the new library. Copy empty files modpath.lst and udnpath.lst
into this directory.
Edit file ngspice/src/xspice/icm/GNUmakefile.in, add <directory name> to the end of line
10, which starts with CMDIRS = ... .
That’s all you have to do about a new library! Of course it is empty right now, so you have to
define at least one code model according to the procedure described in Chapt. 28.2.
28.5 Compiling and loading the new code model (library)
Compiling is now as simple as issuing the commands
28.6. INTERFACE SPECIFICATION FILE 469
cd ngspice/release
make
sudo make install
if you have installed ngspice according to Chapt. 32.1.4. This procedure will install the code
model libraries into a directory <prefix>/lib/spice/, e.g. C:/Spice/lib/spice/ for standard Win-
dows install or /usr/local/lib/spice/ for Linux.
Thus the code model libraries are not linked into ngspice at compile time, but may be loaded
at runtime using the codemodel command (see Chapt. 17.5.11). This is done automatically
for the predefined code model libraries upon starting ngspice. The appropriate commands are
provided in the start up file spinit (see Chapt. 16.5). So if you have added a new code model
inside of one of the existing libraries, nothing has to be done, you will have immediate access
to your new model.
If you have generated a new code model library, e.g. new_lib.cm, then you have to add the line
@XSPICEINIT@ codemodel @prefix@/@libname@/spice/new_lib.cm
to spinit.in in ngspice/src. This will create a new spinit if ngspice is recompiled from scratch.
To avoid the need for recompilation of ngspice, you also may directly edit the file spinit by
adding the line
codemodel C:/Spice/lib/spice/new_lib.cm
(OS MS Windows) or the appropriate Linux equivalent. Upon starting ngspice, the new library
will be loaded and you have access to the new code model(s). The codemodel command has to
be executed upon start-up of ngspice, so that the model information is available as soon as the
circuit is parsed. Failing to do so will lead to an error message of a model missing. So spinit
(or .spiceinit for personal code model libraries) is the correct place for codemodel.
28.6 Interface Specification File
The Interface Specification (IFS) file is a text file that describes the model’s naming informa-
tion, its expected input and output ports, its expected parameters, and any variables within the
model that are to be used for storage of data across an entire simulation. These four types
of data are described to the simulator in IFS file sections labeled NAME_TABLE,PORT_TABLE,
PARAMETER_TABLE and STATIC_VAR_TABLE, respectively. An example IFS file is given below.
The example is followed by detailed descriptions of each of the entries, what they signify, and
what values are acceptable for them. Keywords are case insensitive.
NAME_TABLE:
C_Function_Name: ucm_xfer
Spice_Model_Name: xfer
Description: "arbitrary transfer function"
PORT_TABLE:
470 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
Port_Name: in out
Description: "input" "output"
Direction: in out
Default_Type: v v
Allowed_Types: [v,vd,i,id] [v,vd,i,id]
Vector: no no
Vector_Bounds: - -
Null_Allowed: no no
PARAMETER_TABLE:
Parameter_Name: in_offset gain
Description: "input offset" "gain"
Data_Type: real real
Default_Value: 0.0 1.0
Limits: - -
Vector: no no
Vector_Bounds: - -
Null_Allowed: yes yes
PARAMETER_TABLE:
Parameter_Name: num_coeff
Description: "numerator polynomial coefficients"
Data_Type: real
Default_Value: -
Limits: -
Vector: yes
Vector_Bounds: [1 -]
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: den_coeff
Description: "denominator polynomial coefficients"
Data_Type: real
Default_Value: -
Limits: -
Vector: yes
Vector_Bounds: [1 -]
Null_Allowed: no
PARAMETER_TABLE:
Parameter_Name: int_ic
Description: "integrator stage initial conditions"
Data_Type: real
Default_Value: 0.0
Limits: -
Vector: yes
Vector_Bounds: den_coeff
Null_Allowed: yes
STATIC_VAR_TABLE:
Static_Var_Name: x
Data_Type: pointer
Description: "x-coefficient array"
28.6. INTERFACE SPECIFICATION FILE 471
28.6.1 The Name Table
The name table is introduced by the Name_Table: keyword. It defines the code model’s C
function name, the name used on a .MODEL card, and an optional textual description. The
following sections define the valid fields that may be specified in the Name Table.
28.6.1.1 C Function Name
The C function name is a valid C identifier that is the name of the function for the code model. It
is introduced by the C_Function_Name: keyword followed by a valid C identifier. To reduce
the chance of name conflicts, it is recommended that user-written code model names use the
prefix ucm_ for this entry. Thus, in the example given above, the model name is xfer, but the C
function is ucm_xfer. Note that when you subsequently write the model function in the Model
Definition File, this name must agree with that of the function (i.e., ucm_xfer), or an error will
result in the linking step.
28.6.1.2 SPICE Model Name
The SPICE model name is a valid SPICE identifier that will be used on SPICE .MODEL cards to
refer to this code model. It may or may not be the same as the C function name. It is introduced
by the Spice_Model_Name: keyword followed by a valid SPICE identifier.
Description The description string is used to describe the purpose and function of the code
model. It is introduced by the Description: keyword followed by a C string literal.
28.6.2 The Port Table
The port table is introduced by the Port_Table: keyword. It defines the set of valid ports
available to the code model. The following sections define the valid fields that may be specified
in the port table.
28.6.2.1 Port Name
The port name is a valid SPICE identifier. It is introduced by the Port_Name: keyword follo-
wed by the name of the port. Note that this port name will be used to obtain and return input
and output values within the model function. This will be discussed in more detail in the next
section.
28.6.2.2 Description
The description string is used to describe the purpose and function of the code model. It is
introduced by the Description: keyword followed by a C string literal.
472 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
Default Types
Type Description Valid Directions
d digital in or out
g conductance (VCCS) inout
gd differential conductance (VCCS) inout
h resistance (CCVS) inout
hd differential resistance (CCVS) inout
i current in or out
id differential current in or out
v voltage in or out
vd differential voltage in or out
<identifier> user-defined type in or out
Table 28.1: Port Types
28.6.2.3 Direction
The direction of a port specifies the data flow direction through the port. A direction must be
one of n,out, or inout. It is introduced by the Direction: keyword followed by a valid
direction value.
28.6.2.4 Default Type
The Default_Type field specifies the type of a port. These types are identical to those used to
define the port types on a SPICE deck instance card (see Table 12.1), but without the percent
sign (%) preceding them. Table 28.1 summarizes the allowable types.
28.6.2.5 Allowed Types
A port must specify the types it is allowed to assume. An allowed type value must be a list of
type names (a blank or comma separated list of names delimited by square brackets, e.g. [v vd
i id] or [d]). The type names must be taken from those listed in Table 28.1.
28.6.2.6 Vector
A port that is a vector can be thought of as a bus. The Vector field is introduced with the
Vector: keyword followed by a Boolean value: YES, TRUE, NO or FALSE.
The values YES and TRUE are equivalent and specify that this port is a vector. Likewise, NO
and FALSE specify that the port is not a vector. Vector ports must have a corresponding vector
bounds field that specifies valid sizes of the vector port.
28.6.2.7 Vector Bounds
If a port is a vector, limits on its size must be specified in the vector bounds field. The Vector
Bounds field specifies the upper and lower bounds on the size of a vector. The Vector Bounds
28.6. INTERFACE SPECIFICATION FILE 473
field is usually introduced by the Vector_Bounds: keyword followed by a range of integers
(e.g. ‘[1 7]’ or ‘[3, 20]’). The lower bound of the vector specifies the minimum number of
elements in the vector; the upper bound specifies the maximum number of elements. If the
range is unconstrained, or the associated port is not a vector, the vector bounds may be specified
by a hyphen (‘-’). Using the hyphen convention, partial constraints on the vector bound may be
defined (e.g., ‘[2, -]’ indicates that the least number of port elements allowed is two, but there
is no maximum number).
28.6.2.8 Null Allowed
In some cases, it is desirable to permit a port to remain unconnected to any electrical node in
a circuit. The Null_Allowed field specifies whether this constitutes an error for a particular
port. The Null_Allowed field is introduced by the ‘Null_Allowed:’ keyword and is followed
by a boolean constant: ‘YES’, ‘TRUE’, ‘NO’ or ‘FALSE’. The values ‘YES’ and ‘TRUE’ are
equivalent and specify that it is legal to leave this port unconnected. ‘NO’ or ‘FALSE’ specify
that the port must be connected.
28.6.3 The Parameter Table
The parameter table is introduced by the Parameter_Table: keyword. It defines the set of
valid parameters available to the code model. The following sections define the valid fields that
may be specified in the parameter table.
28.6.3.1 Parameter Name
A parameter name is a valid SPICE identifier that will be used on SPICE .MODEL cards to
refer to this parameter. It is introduced by the Parameter_Name: keyword followed by a valid
SPICE identifier.
28.6.3.2 Description
The description string is used to describe the purpose and function of the parameter. It is
introduced by the ‘Description:’ keyword followed by a string literal.
28.6.3.3 Data Type
The parameter’s data type is specified by the Data Type field. The Data Type field is introduced
by the keyword ‘Data_Type:’ and is followed by a valid data type. Valid data types include
boolean, complex, int, real, and string.
28.6.3.4 Null Allowed
The Null_Allowed field is introduced by the ‘Null_Allowed:’ keyword and is followed by a
boolean literal. A value of ‘TRUE’ or ‘YES’ specify that it is valid for the corresponding SPICE
.MODEL card to omit a value for this parameter. If the parameter is omitted, the default value
474 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
is used. If there is no default value, an undefined value is passed to the code model, and the
PARAM_NULL( ) macro will return a value of ‘TRUE’ so that defaulting can be handled within
the model itself. If the value of Null_Allowed is ‘FALSE’ or ‘NO’, then the simulator will
flag an error if the SPICE .MODEL card omits a value for this parameter.
28.6.3.5 Default Value
If the Null_Allowed field specifies ‘TRUE’ for this parameter, then a default value may be
specified. This value is supplied for the parameter in the event that the SPICE .MODEL card
does not supply a value for the parameter. The default value must be of the correct type. The
Default Value field is introduced by the ‘Default_Value:’ keyword and is followed by a
numeric, boolean, complex, or string literal, as appropriate.
28.6.3.6 Limits
Integer and real parameters may be constrained to accept a limited range of values. The fol-
lowing range syntax is used whenever such a range of values is required. A range is specified
by a square bracket followed by a value representing a lower bound separated by space from
another value representing an upper bound and terminated with a closing square bracket (e.g.”[0
10]”). The lower and upper bounds are inclusive. Either the lower or the upper bound may be
replaced by a hyphen (‘-’) to indicate that the bound is unconstrained (e.g. ‘[10 -]’ is read
as ‘the range of values greater than or equal to 10’). For a totally unconstrained range, a single
hyphen with no surrounding brackets may be used. The parameter value limit is introduced by
the ‘Limits:’ keyword and is followed by a range.
28.6.3.7 Vector
The Vector field is used to specify whether a parameter is a vector or a scalar. Like the PORT
TABLE Vector field, it is introduced by the ‘Vector:’ keyword and followed by a boolean
value. ‘TRUE’ or ‘YES’ specify that the parameter is a vector. ‘FALSE’ or ‘NO’ specify that it
is a scalar.
28.6.3.8 Vector Bounds
The valid sizes for a vector parameter are specified in the same manner as are port sizes (see
Section 28.6.2.7). However, in place of using a numeric range to specify valid vector bounds it
is also possible to specify the name of a port. When a parameter’s vector bounds are specified
in this way, the size of the vector parameter must be the same as the associated vector port.
28.6.4 Static Variable Table
The Static Variable table is introduced by the ‘Static_Var_Table:’ keyword. It defines the
set of valid static variables available to the code model. These are variables whose values are
retained between successive invocations of the code model by the simulator. The following
sections define the valid fields that may be specified in the Static Variable Table.
28.6. INTERFACE SPECIFICATION FILE 475
28.6.4.1 Name
The Static variable name is a valid C identifier that will be used in the code model to refer to
this static variable. It is introduced by the ‘Static_Var_Name:’ keyword followed by a valid
C identifier.
28.6.4.2 Description
The description string is used to describe the purpose and function of the static variable. It is
introduced by the ‘Description:’ keyword followed by a string literal.
28.6.4.3 Data Type
The static variable’s data type is specified by the Data Type field. The Data Type field is in-
troduced by the keyword Data_Type: and is followed by a valid data type. Valid data types
include boolean, complex, int, real, string and pointer.
Note that pointer types are used to specify vector values; in such cases, the allocation of memory
for vectors must be handled by the code model through the use of the malloc() or calloc() C
function. Such allocation must only occur during the initialization cycle of the model (which
is identified in the code model by testing the INIT macro for a value of TRUE). Otherwise,
memory will be unnecessarily allocated each time the model is called.
Following is an example of the method used to allocate memory to be referenced by a static
pointer variable ‘x’ and subsequently use the allocated memory. The example assumes that the
value of ‘size’ is at least 2, else an error would result. The references to STATIC_VAR(x) that
appear in the example illustrate how to set the value of, and then access, a static variable named
‘x’. In order to use the variable ‘x’ in this manner, it must be declared in the Static Variable
Table of the code model’s Interface Specification File.
/* Define local pointer variable */
double *local .x;
/* Allocate storage to be referenced by the static variable x. */
/* Do this only if this is the initial call of the code model. */
if (INIT == TRUE) {
STATIC_VAR (x) = calloc (size , sizeof (double ));
}
/* Assign the value from the static pointer value to the local */
/* pointer variable. */
local_x = STATIC_VAR (x);
/* Assign values to first two members of the array */
local_x [0] = 1.234;
local_x [1] = 5.678;
476 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
28.7 Model Definition File
The Model Definition File is a C source code file that defines a code model’s behavior given
input values that are passed to it by the simulator. The file itself is always given the name
cfunc.mod. In order to allow for maximum flexibility, passing of input, output, and simulator-
specific information is handled through accessor macros, which are described below. In ad-
dition, certain predefined library functions (e.g. smoothing interpolators, complex arithmetic
routines) are included in the simulator in order to ease the burden of the code model program-
mer. These are also described below.
28.7.1 Macros
The use of the accessor macros is illustrated in the following example. Note that the argument
to most accessor macros is the name of a parameter or port as defined in the Interface Specifi-
cation File. Note also that all accessor macros except ‘ARGS’ resolve to an lvalue (C language
terminology for something that can be assigned a value). Accessor macros do not implement
expressions or assignments.
void code .model( ARGS ) /* private structure accessed by
accessor macros */
{
/* The following code fragments are intended to show how
information in the argument list is accessed . The reader
should not attempt to relate one fragment to another .
Consider each fragment as a separate example .
*/
double p,/* variable for use in the following code fragments */
x, /* variable for use in the following code fragments */
y; /* variable for use in the following code fragments */
int i, /* indexing variable for use in the following */
j; /* indexing variable for use in the following */
UDN_Example_Type *a_ptr , /* A pointer used to access a
User -Defined Node type */
*y_ptr ; /* A pointer used to access a
User -Defined Node type */
/* Initializing and outputting a User -Defined Node result */
if( INIT) {
OUTPUT (y) = malloc (sizeof (user . defined .struct ));
y_ptr = OUTPUT (y);
y_ptr -> component1 = 0.0;
y_ptr -> component2 = 0.0;
}
28.7. MODEL DEFINITION FILE 477
else {
y_ptr = OUTPUT (y);
y_ptr -> component1 = x1;
y_ptr -> component2 = x2;
}
/* Determining analysis type */
if( ANALYSIS == AC) {
/* Perform AC analysis - dependent operations here */
}
/* Accessing a parameter value from the .model card */
p = PARAM ( gain );
/* Accessing a vector parameter from the .model card */
for(i = 0; i < PARAM_SIZE (in_offset ); i ++)
p = PARAM( in_offset[i]);
/* Accessing the value of a simple real -valued input */
x = INPUT(a);
/* Accessing a vector input and checking for null port */
if( ! PORT_NULL(a))
for(i = 0; i < PORT_SIZE (a); i ++)
x = INPUT(a[i ]);
/* Accessing a digital input */
x = INPUT(a);
/* Accessing the value of a User - Defined Node input ...
*/
/* This node type includes two elements in its definition . */
a_ptr = INPUT (a);
x = a_ptr -> component1 ;
y = a_ptr -> component2 ;
/* Outputting a simple real - valued result */
OUTPUT( out1 ) = 0.0;
/* Outputting a vector result and checking for null */
if( ! PORT_NULL(a))
for(i = 0; i < PORT.SIZE (a); i ++)
OUTPUT(a[i]) = 0.0;
/* Outputting the partial of output out1 w.r.t. input a */
PARTIAL (out1 ,a) = PARAM ( gain );
/* Outputting the partial of output out2(i) w.r.t. input b(j) */
478 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
for(i = 0; i < PORT_SIZE (out2 ); i++) {
for(j = 0; j < PORT_SIZE (b); j ++) {
PARTIAL( out2 [i],b[j]) = 0.0;
}
}
/* Outputting gain from input c to output out3 in an
AC analysis */
complex_gain_real = 1.0;
complex_gain_imag = 0.0;
AC_GAIN(out3 ,c) = complex_gain ;
/* Outputting a digital result */
OUTPUT_STATE ( out4) = ONE;
/* Outputting the delay for a digital or user - defined output */
OUTPUT_DELAY ( out5) = 1.0e-9;
}
28.7.1.1 Macro Definitions
The full set of accessor macros is listed below. Arguments shown in parenthesis are examples
only. Explanations of the accessor macros are provided in the subsections below.
Circuit Data:
ARGS
CALL_TYPE
INIT
ANALYSIS
FIRST_TIMEPOINT
TIME
T(n)
RAD_FREQ
TEMPERATURE
Parameter Data:
PARAM(gain)
PARAM_SIZE(gain)
PARAM_NULL(gain)
Port Data:
PORT_SIZE(a)
PORT_NULL(a)
LOAD(a)
TOTAL_LOAD(a)
Input Data:
INPUT(a)
INPUT_STATE(a)
INPUT_STRENGTH(a)
28.7. MODEL DEFINITION FILE 479
Output Data:
OUTPUT(y)
OUTPUT_CHANGED(a)
OUTPUT_DELAY(y)
OUTPUT_STATE(a)
OUTPUT_STRENGTH(a)
Partial Derivatives:
PARTIAL(y,a)
AC Gains:
AC_GAIN(y,a)
Static Variable:
STATIC_VAR(x)
28.7.1.2 Circuit Data
ARGS
CALL_TYPE
INIT
ANALYSIS
FIRST_TIMEPOINT
TIME
T(n)
RAD_FREQ
TEMPERATURE
ARGS is a macro that is passed in the argument list of every code model. It is there to provide
a way of referencing each model to all of the remaining macro values. It must be present
in the argument list of every code model; it must also be the only argument present in the
argument list of every code model.
CALL_TYPE is a macro that returns one of two possible symbolic constants. These are
EVENT and ANALOG. Testing may be performed by a model using CALL TYPE to
determine whether it is being called by the analog simulator or the event-driven simula-
tor. This will, in general, only be of value to a hybrid model such as the adc bridge or the
dac bridge.
INIT is an integer (int) that takes the value 1 or 0 depending on whether this is the first call to
the code model instance or not, respectively.
ANALYSIS is an enumerated integer that takes values of DC, AC, or TRANSIENT.
FIRST TIMEPOINT is an integer that takes the value 1 or 0 depending on whether this is the
first call for this instance at the current analysis step (i.e., time-point) or not, respectively.
TIME is a double representing the current analysis time in a transient analysis. T(n) is a double
vector giving the analysis time for a specified time-point in a transient analysis, where n
takes the value 0 or 1. T(0) is equal to TIME. T(1) is the last accepted time-point. (T(0) -
T(1)) is the time-step (i.e., the delta-time value) associated with the current time.
RAD_FREQ is a double representing the current analysis frequency in an AC analysis expres-
sed in units of radians per second.
480 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
TEMPERATURE is a double representing the current analysis temperature.
28.7.1.3 Parameter Data
PARAM(gain)
PARAM_SIZE(gain)
PARAM_NULL(gain)
PARAM(gain) resolves to the value of the scalar (i.e., non-vector) parameter ‘gain’ that was
defined in the Interface Specification File tables. The type of ‘gain’ is the type given in
the ifspec.ifs file. The same accessor macro can be used regardless of type. If ‘gain’ is a
string, then PARAM(gain) would resolve to a pointer. PARAM(gain[n]) resolves to the
value of the nth element of a vector parameter ‘gain’.
PARAM_SIZE(gain) resolves to an integer (int) representing the size of the ‘gain’ vector
(which was dynamically determined when the SPICE deck was read). PARAM_SIZE(gain)
is undefined if ‘gain’ is a scalar.
PARAM_NULL(gain) resolves to an integer with value 0 or 1 depending on whether a value
was specified for gain, or whether the value is defaulted, respectively.
28.7.1.4 Port Data
PORT_SIZE(a)
PORT_NULL(a)
LOAD(a)
TOTAL_LOAD(a)
PORT_SIZE(a) resolves to an integer (int) representing the size of the ‘a’ port (which was
dynamically determined when the SPICE deck was read). PORT_SIZE(a) is undefined if
gain is a scalar.
PORT_NULL(a) resolves to an integer (int) with value 0 or 1 depending on whether the SPICE
deck has a node specified for this port, or has specified that the port is null, respectively.
LOAD(a) is used in a digital model to post a capacitive load value to a particular input or output
port during the INIT pass of the simulator. All values posted for a particular event-driven
node using the LOAD() macro are summed, producing a total load value.
TOTAL_LOAD(a) returns a double value that represents the total capacitive load seen on a
specified node to which a digital code model is connected. This information may be used
after the INIT pass by the code model to modify the delays it posts with its output states
and strengths. Note that this macro can also be used by non-digital event-driven code
models (see LOAD(), above).
28.7. MODEL DEFINITION FILE 481
28.7.1.5 Input Data
INPUT(a)
INPUT_STATE(a)
INPUT_STRENGTH(a)
INPUT(a) resolves to the value of the scalar input athat was defined in the Interface Specifi-
cation File tables (acan be either a scalar port or a port value from a vector; in the latter
case, the notation used would be a[i], where iis the index value for the port). The
type of ais the type given in the ifspec.ifs file. The same accessor macro can be used
regardless of type.
INPUT_STATE(a) resolves to the state value defined for digital node types. These will be one
of the symbolic constants ZERO, ONE, or UNKNOWN.
INPUT_STRENGTH(a) resolves to the strength with which a digital input node is being dri-
ven. This is determined by a resolution algorithm that looks at all outputs to a node and
determines its final driven strength. This value in turn is passed to a code model when
requested by this macro. Possible strength values are:
1. STRONG
2. RESISTIVE
3. HI_IMPEDANCE
4. UNDETERMINED
28.7.1.6 Output Data
OUTPUT(y)
OUTPUT_CHANGED(a)
OUTPUT_DELAY(y)
OUTPUT_STATE(a)
OUTPUT_STRENGTH(a)
OUTPUT(y) resolves to the value of the scalar output ‘y’ that was defined in the Interface
Specification File tables. The type of ‘y’ is the type given in the ifspec.ifs file. The same
accessor macro can be used regardless of type. If ‘y’ is a vector, then OUTPUT(y) would
resolve to a pointer.
OUTPUT_CHANGED(a) may be assigned one of two values for any particular output from
a digital code model. If assigned the value TRUE (the default), then an output state,
strength and delay must be posted by the model during the call. If, on the other hand, no
change has occurred during that pass, the OUTPUT_CHANGED(a) value for an output
can be set to FALSE. In this case, no state, strength or delay values need subsequently
be posted by the model. Remember that this macro applies to a single output port. If a
model has multiple outputs that have not changed, OUTPUT_CHANGED(a) must be set
to FALSE for each of them.
OUTPUT_DELAY(y) may be assigned a double value representing a delay associated with
a particular digital or User-Defined Node output port. Note that this macro must be set
for each digital or User-Defined Node output from a model during each pass, unless the
482 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
OUTPUT_CHANGED(a) macro is invoked (see above). Note also that a non-zero value
must be assigned to OUTPUT_DELAY(). Assigning a value of zero (or a negative value)
will cause an error.
OUTPUT_STATE(a) may be assigned a state value for a digital output node. Valid values are
ZERO, ONE, and UNKNOWN. This is the normal way of posting an output state from a
digital code model.
OUTPUT_STRENGTH(a) may be assigned a strength value for a digital output node. This
is the normal way of posting an output strength from a digital code model. Valid values
are:
1. STRONG
2. RESISTIVE
3. HI_IMPEDANCE
4. UNDETERMINED
28.7.1.7 Partial Derivatives
PARTIAL(y,a)
PARTIAL(y[n],a)
PARTIAL(y,a[m])
PARTIAL(y[n],a[m])
PARTIAL(y,a) resolves to the value of the partial derivative of scalar output ‘y’ with respect
to scalar input ‘a’. The type is always double since partial derivatives are only defined for
nodes with real valued quantities (i.e., analog nodes).
The remaining uses of PARTIAL are shown for the cases in which either the output, the input,
or both are vectors.
Partial derivatives are required by the simulator to allow it to solve the non-linear equations
that describe circuit behavior for analog nodes. Since coding of partial derivatives can become
difficult and error-prone for complex analog models, you may wish to consider using the cm
analog auto partial() code model support function instead of using this macro.
28.7.1.8 AC Gains
AC_GAIN(y,a)
AC_GAIN(y[n],a)
AC_GAIN(y,a[m])
AC_GAIN(y[n],a[m])
AC_GAIN(y,a) resolves to the value of the AC analysis gain of scalar output ‘y’ from scalar
input ‘a’. The type is always a structure (Complex_t) defined in the standard code model
header file:
typedef struct Complex_s {
double real; /* The real part of the complex number */
double imag; /* The imaginary part of the complex number */
}Complex_t;
28.7. MODEL DEFINITION FILE 483
The remaining uses of AC_GAIN are shown for the cases in which either the output, the input,
or both are vectors.
28.7.1.9 Static Variables
STATIC_VAR(x)
STATIC_VAR(x) resolves to an lvalue or a pointer that is assigned the value of some scalar
code model result or state defined in the Interface Spec File tables, or a pointer to a value
or a vector of values. The type of ‘x’ is the type given in the Interface Specification
File. The same accessor macro can be used regardless of type since it simply resolves
to an lvalue. If ‘x’ is a vector, then STATIC_VAR(x) would resolve to a pointer. In this
case, the code model is responsible for allocating storage for the vector and assigning the
pointer to the allocated storage to STATIC_VAR(x).
28.7.1.10 Accessor Macros
Table 28.3 describes the accessor macros available to the Model Definition File programmer and
their C types. The PARAM and STATIC_VAR macros, whose types are labeled CD (context
dependent), return the type defined in the Interface Specification File. Arguments listed with
‘[i]’ take an optional square bracket delimited index if the corresponding port or parameter is a
vector. The index may be any C expression - possibly involving calls to other accessor macros
(e.g.,” OUTPUT(out[PORT_SIZE(out)-1])”)
Name Type Args Description
AC_GAIN Complex_t y[i],x[i] AC gain of output y with respect to
input x.
ANALYSIS enum <none> Type of analysis: DC, AC,
TRANSIENT.
ARGS Mif_Private_t <none> Standard argument to all code
model function.
CALL_TYPE enum <none> Type of model evaluation call:
ANALOG or EVENT.
INIT Boolean_t <none> Is this the first call to the model?
INPUT double or void* name[i] Value of analog input port, or value
of structure pointer for
User-Defined Node port.
INPUT_STATE enum name[i] State of a digital input: ZERO,
ONE, or UNKNOWN.
INPUT_STRENGHT enum name[i] Strength of digital input:
STRONG, RESISTIVE, HI
IMPEDANCE, or
UNDETERMINED.
INPUT_TYPE char* name[i] The port type of the input.
LOAD double name[i] The digital load value placed on a
port by this model.
484 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
Table 28.3: Accessor macros
MESSAGE char* name[i] A message output by a model on
an event-driven node.
OUTPUT double or void* name[i] Value of the analog output port or
value of structure pointer for
User-Defined Node port.
OUTPUT_CHANGED Boolean_t name[i] Has a new value been assigned to
this event-driven output by the
model?
OUTPUT_DELAY double name[i] Delay in seconds for an
event-driven output.
OUTPUT_STATE enum name[i] State of a digital output: ZERO,
ONE, or UNKNOWN.
OUTPUT_STRENGTH enum name[i] Strength of digital output:
STRONG, RESISTIVE,
HI_IMPEDANCE, or
UNDETERMINED.
OUTPUT_TYPE char* name[i] The port type of the output.
PARAM CD name[i] Value of the parameter.
PARAM_NULL Boolean_t name[i] Was the parameter not included on
the SPICE .model card ?
PARAM_SIZE int name Size of parameter vector.
PARTIAL double y[i],x[i] Partial derivative of output y with
respect to input x.
PORT_NULL Mif_Boolean_t name Has this port been specified as
unconnected?
PORT_SIZE int name Size of port vector.
RAD_FREQ double <none> Current analysis frequency in
radians per second.
STATIC_VAR CD name Value of a static variable.
STATIC_VAR_SIZE int name Size of static var vector (currently
unused).
T(n) int index Current and previous analysis
times (T(0) = TIME = current
analysis time, T(1) = previous
analysis time).
TEMPERATURE double <none> Current analysis temperature.
TIME double <none> Current analysis time (same as
T(0)).
TOTAL_LOAD double name[i] The total of all loads on the node
attached to this event driven port.
28.7. MODEL DEFINITION FILE 485
28.7.2 Function Library
28.7.2.1 Overview
Aside from the accessor macros, the simulator also provides a library of functions callable from
within code models. The header file containing prototypes to these functions is automatically
inserted into the Model Definition File for you. The complete list of available functions follows:
Smoothing Functions:
void cm_smooth_corner
void cm_smooth_discontinuity
double cm_smooth_pwl
Model State Storage Functions:
void cm_analog_alloc
void cm_event_alloc
void *cm_analog_get_ptr
void *cm_event_get_ptr
Integration and Convergence Functions:
int cm_analog_integrate
int cm_analog_converge
void cm_analog_not_converged
void cm_analog_auto_partial
double cm_analog_ramp_factor
Message Handling Functions:
char *cm_message_get_errmsg
void cm_message_send
Breakpoint Handling Functions:
int cm_analog_set_temp_bkpt
int cm_analog_set_perm_bkpt
int cm_event_queue
Special Purpose Functions:
void cm_climit_fcn
double cm_netlist_get_c
double cm_netlist_get_l
char *cm_get_path
Complex Math Functions:
complex_t cm_complex_set
complex_t cm_complex_add
complex_t cm_complex_sub
complex_t cm_complex_mult
complex_t cm_complex_div
28.7.2.2 Smoothing Functions
void
cm_smooth_corner(x_input, x_center, y_center, domain,
lower_slope, upper_slope, y_output, dy_dx)
486 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
double x_input; /* The value of the x input */
double x_center; /* The x intercept of the two slopes */
double y_center; /* The y intercept of the two slopes */
double domain; /* The smoothing domain */
double lower_slope; /* The lower slope */
double upper_slope; /* The upper slope */
double *y_output; /* The smoothed y output */
double *dy_dx; /* The partial of y wrt x */
void
cm_smooth_discontinuity(x_input, x_lower, y_lower, x_upper, y_upper
y_output, dy_dx)
double x_input; /* The x value at which to compute y */
double x_lower; /* The x value of the lower corner */
double y_lower; /* The y value of the lower corner */
double x_upper; /* The x value of the upper corner */
double y_upper; /* The y value of the upper corner */
double *y_output; /* The computed smoothed y value */
double *dy_dx; /* The partial of y wrt x */
double
cm_smooth_pwl(x_input, x, y, size, input_domain, dout_din)
double x_input; /* The x input value */
double *x; /* The vector of x values */
double *y; /* The vector of y values */
int size; /* The size of the xy vectors */
double input_domain; /* The smoothing domain */
double *dout_din; /* The partial of the output wrt the input */
cm_smooth_corner() automates smoothing between two arbitrarily-sloped lines that meet
at a single center point. You specify the center point (x_center,y_center), plus a dom-
ain (x-valued delta) above and below x_center. This defines a smoothing region about the
center point. Then, the slopes of the meeting lines outside of this smoothing region are speci-
fied (lower_slope,upper_slope). The function then interpolates a smoothly-varying output
(*y_output) and its derivative (*dy_dx) for the x_input value. This function helps to au-
tomate the smoothing of piecewise-linear functions, for example. Such smoothing aids the
simulator in achieving convergence.
cm_smooth_discontinuity() allows you to obtain a smoothly-transitioning output (*y_output)
that varies between two static values (y_lower,y_upper) as an independent variable (x_input)
transitions between two values (x_lower,x_upper). This function is useful in interpolating
between resistances or voltage levels that change abruptly between two values.
cm_smooth_pwl() duplicates much of the functionality of the predefined pwl code model. The
cm smooth pwl() takes an input value plus x-coordinate and y-coordinate vector values along
with the total number of coordinate points used to describe the piecewise linear transfer function
and returns the interpolated or extrapolated value of the output based on that transfer function.
28.7. MODEL DEFINITION FILE 487
More detail is available by looking at the description of the pwl code model. Note that the
output value is the function’s returned value.
28.7.2.3 Model State Storage Functions
void cm_analog_alloc(tag, size)
int tag; /* The user-specified tag for this block of memory */
int size; /* The number of bytes to allocate */
void cm_event_alloc(tag, size)
int tag; /* The user-specified tag for the memory block */
int size; /* The number of bytes to be allocated */
void *cm_analog_get_ptr(tag, timepoint)
int tag; /* The user-specified tag for this block of memory */
int timepoint; /* The timepoint of interest - 0=current 1=previous */
void *cm_event_get_ptr(tag, timepoint)
int tag; /* The user-specified tag for the memory block */
int timepoint; /* The timepoint - 0=current, 1=previous */
cm_analog_alloc() and cm_event_alloc() allow you to allocate storage space for analog
and event-driven model state information. The storage space is not static, but rather represents
a storage vector of two values that rotate with each accepted simulator time-point evaluation.
This is explained more fully below. The ‘tag’ parameter allows you to specify an integer tag
when allocating space. This allows more than one rotational storage location per model to be
allocated. The ‘size’ parameter specifies the size in bytes of the storage (computed by the C
language sizeof() operator). Both cm_analog_alloc() and cm_event_alloc() will not re-
turn pointers to the allocated space, as has been available (and buggy) from the original XSPICE
code. cm_analog_alloc() should be used by an analog model; cm_event_alloc() should
be used by an event-driven model.
*cm_analog_get_ptr() and *cm_event_get_ptr() retrieve the pointer location of the ro-
tational storage space previously allocated by cm_analog_alloc() or cm_event_alloc().
Important notice: These functions must be called only after all memory allocation (all calls to
cm_analog_alloc() or cm_event_alloc()) have been done. All pointers returned between
calls to memory allocation will become obsolete (point to freed memory because of an internal
realloc). The functions take the integer ‘tag’ used to allocate the space, and an integer from 0 to
1 that specifies the time-point with which the desired state variable is associated (e.g. timepoint
= 0 will retrieve the address of storage for the current time-point; timepoint = 1 will retrieve
the address of storage for the last accepted time-point). Note that once a model is exited,
storage to the current time-point state storage location (i.e., timepoint = 0) will, upon the
next time-point iteration, be rotated to the previous location (i.e., timepoint = 1). When
rotation is done, a copy of the old ‘timepoint = 0’ storage value is placed in the new ‘timepoint
= 0’ storage location. Thus, if a value does not change for a particular iteration, specific writing
488 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
to ‘timepoint = 0’ storage is not required. These features allow a model coder to constantly
know which piece of state information is being dealt with within the model function at each
time-point.
28.7.2.4 Integration and Convergence Functions
int cm_analog_integrate(integrand, integral, partial)
double integrand; /* The integrand */
double *integral; /* The current and returned value of integral */
double *partial; /* The partial derivative of integral wrt integrand */
int cm_analog_converge(state)
double *state; /* The state to be converged */
void cm_analog_not_converged()
void cm_analog_auto_partial()
double cm_ramp_factor()
cm_analog_integrate() takes as input the integrand (the input to the integrator) and produ-
ces as output the integral value and the partial of the integral with respect to the integrand. The
integration itself is with respect to time, and the pointer to the integral value must have been
previously allocated using cm_analog_alloc() and *cm_analog_get_ptr(). This is requi-
red because of the need for the integrate routine itself to have access to previously-computed
values of the integral.
cm_analog_converge() takes as an input the address of a state variable that was previously
allocated using cm_analog_alloc() and *cm_analog_get_ptr(). The function itself serves
to notify the simulator that for each time-step taken, that variable must be iterated upon until it
converges.
cm_analog_not_converged() is a function that can and should be called by an analog model
whenever it performs internal limiting of one or more of its inputs to aid in reaching conver-
gence. This causes the simulator to call the model again at the current time-point and continue
solving the circuit matrix. A new time-point will not be attempted until the code model returns
without calling the cm_analog_not_converged() function. For circuits that have trouble re-
aching a converged state (often due to multiple inputs changing too quickly for the model to
react in a reasonable fashion), the use of this function is virtually mandatory.
cm_analog_auto_partial() may be called at the end of a code model function in lieu of
calculating the values of partial derivatives explicitly in the function. When this function is cal-
led, no values should be assigned to the PARTIAL macro since these values will be computed
automatically by the simulator. The automatic calculation of partial derivatives can save consi-
derable time in designing and coding a model, since manual computation of partial derivatives
can become very complex and error-prone for some models. However, the automatic evaluation
may also increase simulation run time significantly. Function cm_analog_auto_partial()
causes the model to be called N additional times (for a model with N inputs) with each input
varied by a small amount (1e-6 for voltage inputs and 1e-12 for current inputs). The values
28.7. MODEL DEFINITION FILE 489
of the partial derivatives of the outputs with respect to the inputs are then approximated by the
simulator through divided difference calculations.
cm_analog_ramp_factor() will then return a value from 0.0 to 1.0 that indicates whether
or not a ramp time value requested in the SPICE analysis deck (with the use of .option
ramptime=<duration>) has elapsed. If the RAMPTIME option is used, then cm_analog_ramp_factor
returns a 0.0 value during the DC operating point solution and a value that is between 0.0 and
1.0 during the ramp. A 1.0 value is returned after the ramp is over or if the RAMPTIME op-
tion is not used. This value is intended as a multiplication factor to be used with all model
outputs that would ordinarily experience a ‘power-up’ transition. Currently, all sources within
the simulator are automatically ramped to the ‘final’ time-zero value if a RAMPTIME option is
specified.
28.7.2.5 Message Handling Functions
char *cm_message_get_errmsg()
int cm_message_send(char *msg)
char *msg; /* The message to output. */
*cm_message_get_errmsg() is a function designed to be used with other library functions
to provide a way for models to handle error situations. More specifically, whenever a library
function that returns type int is executed from a model, it will return an integer value, n. If this
value is not equal to zero (0), then an error condition has occurred (likewise, functions that re-
turn pointers will return a NULL value if an error has occurred). At that point, the model can in-
voke *cm_message_get_errmsg to obtain a pointer to an error message. This can then in turn
be displayed to the user or passed to the simulator interface through the cm_message_send()
function. The C code required for this is as follows:
err = cm_analog_integrate(in, &out, &dout_din);
if (err) {
cm_message_send(cm_message_get_errmsg());
}
else { ...
cm_message_send() sends messages to either the standard output screen or to the simulator
interface, depending on which is in use.
28.7.2.6 Breakpoint Handling Functions
int cm_analog_set_perm_bkpt(time)
double time; /* The time of the breakpoint to be set */
int cm_analog_set_temp_bkpt(time)
double time; /* The time of the breakpoint to be set */
int cm_event_queue(time)
double time; /* The time of the event to be queued */
490 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
cm_analog_set_perm_bkpt() takes as input a time value. This value is posted to the analog
simulator algorithm and is used to force the simulator to choose that value as a breakpoint at
some time in the future. The simulator may choose as the next time-point a value less than the
input, but not greater. Also, regardless of how many time-points pass before the breakpoint is
reached, it will not be removed from posting. Thus, a breakpoint is guaranteed at the passed
time value. Note that a breakpoint may also be set for a time prior to the current time, but this
will result in an error if the posted breakpoint is prior to the last accepted time (i.e., T(1)).
cm_analog_set_temp_bkpt() takes as input a time value. This value is posted to the simu-
lator and is used to force the simulator, for the next time-step only, to not exceed the passed
time value. The simulator may choose as the next time-point a value less than the input, but not
greater. In addition, once the next time-step is chosen, the posted value is removed regardless
of whether it caused the break at the given time-point. This function is useful in the event that
a time-point needs to be retracted after its first posting in order to recalculate a new breakpoint
based on new input data (for controlled oscillators, controlled one-shots, etc), since temporary
breakpoints automatically ‘go away’ if not reposted each time-step. Note that a breakpoint may
also be set for a time prior to the current time, but this will result in an error if the posted
breakpoint is prior to the last accepted time (i.e., T(1)).
cm_event_queue() is similar to cm_analog_set_perm_bkpt(), but functions with event-
driven models. When invoked, this function causes the model to be queued for calling at the
specified time. All other details applicable to cm_analog_set_perm_bkpt() apply to this
function as well.
28.7.2.7 Special Purpose Functions
void
cm_climit_fcn(in, in_offset, cntl_upper, cntl_lower, lower_delta, upper_delta,
limit_range, gain, fraction, out_final, pout_pin_final,
pout_pcntl_lower_final, pout_pcntl_upper_final)
double in; /* The input value */
double in-offset; /* The input offset */
double cntl_upper; /* The upper control input value */
double cntl_lower; /* The lower control input value */
double lower_delta; /* The delta from control to limit value */
double upper_delta; /* The delta from control to limit value */
double limit_range; /* The limiting range */
double gain; /* The gain from input to output */
int percent; /* The fraction vs. absolute range flag */
double *out_final; /* The output value */
double *pout_pin_final; /* The partial of output wrt input */
double *pout_pcntl_lower_final; /* The partial of output wrt lower
control input */
double *pout_pcntl_upper:final; /* The partial of output wrt upper
control input */
double cm_netlist_get_c()
28.7. MODEL DEFINITION FILE 491
double cm_netlist_get_l()
char* cm_get_path()
cm_climit_fcn() is a very specific function that mimics the behavior of the climit code model
(see the Predefined Models section). In brief, the cm_climit_fcn() takes as input an in value,
an offset, and controlling upper and lower values. Parameter values include delta values for
the controlling inputs, a smoothing range, gain, and fraction switch values. Outputs include
the final value, plus the partial derivatives of the output with respect to signal input, and both
control inputs. These all operate identically to the similarly-named inputs and parameters of the
climit model.
The function performs a limit on the in value, holding it to within some delta of the control-
ling inputs, and handling smoothing, etc. The cm_climit_fcn() was originally used in the
ilimit code model to handle much of the primary limiting in that model, and can be used by a
code model developer to take care of limiting in larger models that require it. See the detailed
description of the climit model for more in-depth description.
cm_netlist_get_c() and cm_netlist_get_l() functions search the analog circuitry to
which their input is connected, and total the capacitance or inductance, respectively, found
at that node. The functions, as they are currently written, assume they are called by a model
that has only one single-ended analog input port.
cm_get_path() fetches the path of the first netlist input file found on the ngspice command
line or in the source command, which ngspice saves to the global variable Infile_Path.
28.7.2.8 Complex Math Functions
Complex_t cm_complex_set (real_part, imag_part)
double real_part; /* The real part of the complex number */
double imag_part; /* The imaginary part of the complex number */
Complex_t cm_complex_add (x, y)
Complex_t x; /* The first operand of x + y */
Complex_t y; /* The second operand of x + y */
Complex_t cm_complex_sub (x, y)
Complex_t x; /* The first operand of x - y */
Complex_t y; /* The second operand of x - y */
Complex_t cm_complex_mult (x, y)
Complex_t x; /* The first operand of x * y */
Complex_t y; /* The second operand of x * y */
Complex_t cm_complex_div (x, y)
Complex_t x; /* The first operand of x / y */
492 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
Complex_t y; /* The second operand of x / y */
cm_complex_set() takes as input two doubles, and converts these to a Complex_t. The first
double is taken as the real part, and the second is taken as the imaginary part of the resulting
complex value.
cm_complex_add(),cm_complex_sub(),cm_complex_mult(), and cm_complex_div()
each take two complex values as inputs and return the result of a complex addition, subtraction,
multiplication, or division, respectively.
28.8 User-Defined Node Definition File
The User-Defined Node Definition File (udnfunc.c) defines the C functions that implement
basic operations on user-defined nodes such as data structure creation, initialization, copying,
and comparison. Unlike the Model Definition File that uses the Code Model Preprocessor to
translate Accessor Macros, the User-Defined Node Definition file is a pure C language file. This
file uses macros to isolate you from data structure definitions, but the macros are defined in a
standard header file (EVTudn.h), and translations are performed by the standard C Preproces-
sor.
When you create a directory for a new User-Defined Node, e.g. /ngspice/src/xspice/icm/xtraevt/new_type/,
add a new User-Defined Node Definition File udnfunc.c (see the example in Chapt. 28.8.3),
and place a structure of type ’Evt_Udn_Info_t’ at its bottom.
This structure contains the type name for the node, a description string, and pointers to each
of the functions that define the node. This structure is complete except for a text string that
describes the node type. This string is stubbed out and may be edited by you if desired.
28.8. USER-DEFINED NODE DEFINITION FILE 493
28.8.1 Macros
Name Type Description
MALLOCED_PTR void * Assign pointer to allocated structure
to this macro
STRUCT_PTR void * A pointer to a structure of the defined
type
STRUCT_PTR_1 void * A pointer to a structure of the defined
type
STRUCT_PTR_2 void * A pointer to a structure of the defined
type
EQUAL Mif_Boolean_t Assign TRUE or FALSE to this macro
according to the results of structure
comparison
INPUT_STRUCT_PTR void * A pointer to a structure of the defined
type
OUTPUT_STRUCT_PTR void * A pointer to a structure of the defined
type
INPUT_STRUCT_PTR_ARRAY void ** An array of pointers to structures of
the defined type
INPUT_STRUCT_PTR_ARRAY_SIZE int The size of the array
STRUCT_MEMBER_ID char * A string naming some part of the
structure
PLOT_VAL double The value of the specified structure
member for plotting purposes
PRINT_VAL char * The value of the specified structure
member for printing purposes
Table 28.4: User-Defined Node Macros
You must code the functions described in the following section using the macros appropriate
for the particular function. You may elect whether not to provide the optional functions.
It is an error to use a macro not defined for a function. Note that a review of the sample
directories for the real and int UDN types will make the function usage clearer.
The macros used in the User-Defined Node Definition File to access and assign data values
are defined in Table 28.4. The translations of the macros and of macros used in the function
argument lists are defined in the Interface Diesign Document for the XSPICE Simulator.
28.8.2 Function Library
The functions (required and optional) that define a User-Defined Node are listed below. For
optional functions not used, the pointer in the Evt_Udn_Info_t structure can be changed to
NULL.
Required functions:
494 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
create Allocate data structure used as inputs and outputs to
code models.
initialize Set structure to appropriate initial value for first use as
model input.
copy Make a copy of the contents into created but possibly
uninitialized structure.
compare Determine if two structures are equal in value.
Optional functions:
dismantle Free allocations inside structure (but not structure itself).
invert Invert logical value of structure.
resolve Determine the resultant when multiple outputs are connected
to a node.
plot_val Output a real value for specified structure component for
plotting purposes.
print_val Output a string value for specified structure component for
printing.
ipc_val Output a binary representation of the structure suitable
for sending over the IPC channel.
The required actions for each of these functions are described in the following subsections. In
each function, you have to replace the XXX with the node type name specified. The macros
used in implementing the functions are described in a later section.
28.8.2.1 Function udn_XXX_create
Allocate space for the data structure defined for the User-Defined Node to pass data between
models. Then assign pointer created by the storage allocator (e.g. malloc) to MALLOCED_PTR.
28.8.2.2 Function udn_XXX_initialize
Assign STRUCT_PTR to a pointer variable of defined type and then initialize the value of the
structure.
28.8. USER-DEFINED NODE DEFINITION FILE 495
28.8.2.3 Function udn_XXX_compare
Assign STRUCT_PTR_1 and STRUCT_PTR_2 to pointer variables of the defined type. Com-
pare the two structures and assign either TRUE or FALSE to EQUAL.
28.8.2.4 Function udn_XXX_copy
Assign INPUT_STRUCT_PTR and OUTPUT_STRUCT_PTR to pointer variables of the defi-
ned type and then copy the elements of the input structure to the output structure.
28.8.2.5 Function udn_XXX_dismantle
Assign STRUCT_PTR to a pointer variable of defined type and then free any allocated sub-
structures (but not the structure itself!). If there are no substructures, the body of this function
may be left null.
28.8.2.6 Function udn_XXX_invert
Assign STRUCT_PTR to a pointer variable of the defined type, and then invert the logical value
of the structure.
28.8.2.7 Function udn_XXX_resolve
Assign INPUT_STRUCT_PTR_ARRAY to a variable declared as an array of pointers of the
defined type - e.g.:
<type> **struct_array;
struct_array = INPUT_STRUCT_PTR_ARRAY;
Then, the number of elements in the array may be determined from the integer valued IN-
PUT_STRUCT_PTR_ARRAY_SIZE macro.
Assign OUTPUT_STRUCT_PTR to a pointer variable of the defined type. Scan through the
array of structures, compute the resolved value, and assign it into the output structure.
28.8.2.8 Function udn_XXX_plot_val
Assign STRUCT_PTR to a pointer variable of the defined type. Then, access the member of
the structure specified by the string in STRUCT_MEMBER_ID and assign some real valued
quantity for this member to PLOT_VALUE.
28.8.2.9 Function udn_XXX_print_val
Assign STRUCT_PTR to a pointer variable of the defined type. Then, access the member of
the structure specified by the string in STRUCT_MEMBER_ID and assign some string valued
quantity for this member to PRINT_VALUE.
If the string is not static, a new string should be allocated on each call. Do not free the allocated
strings.
496 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
28.8.2.10 Function udn_XXX_ipc_val
Use STRUCT_PTR to access the value of the node data. Assign to IPC_VAL a binary repre-
sentation of the data. Typically this can be accomplished by simply assigning STRUCT_PTR
to IPC_VAL.
Assign to IPC_VAL_SIZE an integer representing the size of the binary data in bytes.
28.8.3 Example UDN Definition File
The following is an example UDN Definition File that is included with the XSPICE system. It
illustrates the definition of the functions described above for a User-Defined Node type int (for
integer node type), to be found in file /ngspice/src/xspice/icm/xtraevt/int/udnfunc.c.
#include <stdio.h>
#include " ngspice/cm.h"
#include " ngspice/ evtudn .h"
void * tmalloc ( size_t );
# define TMALLOC (t ,n) (t *) tmalloc ( sizeof (t )*( size_t )( n))
/* macro to ignore unused variables and parameters */
#define NG_IGNORE (x) ( void)x
/* ************************************************* */
static void udn_int_create ( CREATE_ARGS )
{
/* Malloc space for an int */
MALLOCED_PTR = TMALLOC (int , 1);
}
/* ************************************************* */
static void udn_i nt_dis mantl e ( DISMA NTL E_AR GS )
{
NG_IGNORE(STRUCT_PTR);
/* Do nothing . There are no internally malloc ’ed
things to dismantle */
}
/* ************************************************* */
static void udn_in t_init ialize ( IN ITIA LIZE_ ARGS )
{
int *int_struct = ( int *) STRUCT_PTR ;
/* Initialize to zero */
28.8. USER-DEFINED NODE DEFINITION FILE 497
*int_struct = 0;
}
/* ************************************************* */
static void udn_int_invert ( INVERT_ARGS )
{
int *int_struct = ( int *) STRUCT_PTR ;
/* Invert the state */
*int_struct = -(*int_struct);
}
/* ************************************************* */
static void udn_int_copy ( COPY_ARGS )
{
int * in t_f rom_s truc t = ( int *) INPUT_STRUC T_PTR ;
int * int_to_struct = ( int *) OUTPUT_S TRUCT _PTR ;
/* Copy the structure */
*int_to_struct = *int_from_struct;
}
/* ************************************************* */
static void udn_int_resolve ( RESOLVE_ARGS )
{
int ** array = ( int **) INPUT_S TRUCT_P TR_ARRAY ;
int * out = ( int *) OU TPUT_S TRUCT_ PTR ;
int num_struct = IN PUT_STRUCT_PTR_ARRAY_SIZ E ;
int sum;
int i;
/* Sum the values */
for(i = 0, sum = 0; i < num_struct; i++)
sum += *( array [i ]);
/* Assign the result */
*out = sum;
}
/* ************************************************* */
static void udn_int_compare ( COMPARE_ARGS )
{
int *int_struct1 = (int *) STRUCT_PTR_1 ;
498 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
int *int_struct2 = (int *) STRUCT_PTR_2 ;
/* Compare the structures */
if ((* int_struct1 ) == (* int_struct2 ))
EQUAL = TRUE ;
else
EQUAL = FALSE ;
}
/* ************************************************* */
static void udn_ int_p lot_v al ( PLO T_VA L_A RGS )
{
int *int_struct = ( int *) STRUCT_PTR ;
NG_IGN ORE ( STRUCT_M EMBER_ ID );
/* Output a value for the int struct */
PLOT_VAL = * int_struct;
}
/* ************************************************* */
static void udn_i nt_pri nt_va l ( PRINT _VA L_AR GS )
{
int *int_struct = ( int *) STRUCT_PTR ;
NG_IGN ORE ( STRUCT_M EMBER_ ID );
/* Allocate space for the printed value */
PRINT_VAL = TMALLOC (char , 30);
/* Print the value into the string */
sprintf (PRINT_VAL , "%8 d", * int_struct );
}
/* ************************************************* */
static void udn_int_ipc_val ( IPC_VAL_ARGS )
{
/* Simply return the structure and its size */
IPC_VAL = STRUCT_PTR ;
IPC_VAL_SIZE = sizeof (int );
}
Evt_Udn_Info_t udn_int_info = {
"int",
"integer valued data",
udn_int_create,
28.8. USER-DEFINED NODE DEFINITION FILE 499
udn_int_dismantle,
udn_int_initialize ,
udn_int_invert,
udn_int_copy,
udn_int_resolve,
udn_int_compare,
udn_int_plot_val,
udn_int_print_val,
udn_int_ipc_val
};
500 CHAPTER 28. CODE MODELS AND USER-DEFINED NODES
Chapter 29
Error Messages
Error messages may be subdivided into three categories. These are:
1. Error messages generated during the development of a code model (Preprocessor Error
Messages).
2. Error messages generated by the simulator during a simulation run (Simulator Error Mes-
sages).
3. Error messages generated by individual code models (Code Model Error Messages).
These messages will be explained in detail in the following subsections.
29.1 Preprocessor Error Messages
The following is a list of error messages that may be encountered when invoking the directory-
creation and code modeling preprocessor tools. These are listed individually, and explanations
follow the name/listing.
Usage: cmpp [-ifs] [-mod [<filename>]] [-lst]
The Code Model Preprocessor (cmpp) command was invoked incorrectly.
ERROR - Too few arguments
The Code Model Preprocessor (cmpp) command was invoked with too few arguments.
ERROR - Too many arguments
The Code Model Preprocessor (cmpp) command was invoked with too many arguments.
ERROR - Unrecognized argument
501
502 CHAPTER 29. ERROR MESSAGES
The Code Model Preprocessor (cmpp) command was invoked with an invalid argument.
ERROR - File not found: s<filename>
The specified file was not found, or could not be opened for read access.
ERROR - Line <line number> of <filename> exceeds XX characters
The specified line was too long.
ERROR - Pathname on line <line number> of <filename>
exceeds XX characters.
The specified line was too long.
ERROR - No pathnames found in file: <filename>
The indicated modpath.lst file does not have pathnames properly listed.
ERROR - Problems reading ifspec.ifs in directory <pathname>
The Interface Specification File (ifspec.ifs) for the code model could not be read.
ERROR - Model name <model name> is same as internal SPICE model name
A model has been given the same name as an intrinsic SPICE device.
ERROR - Model name ’<model name>’ in directory: <pathname>
is same as
model name ’<model name>’ in directory: <pathname>
Two models in different directories have the same name.
ERROR - C function name ’<function name>’ in directory: <pathname>,
is same as
C function name ’<function name>’ in directory: <pathname>
Two C language functions in separate model directories have the same names; these would
cause a collision when linking the final executable.
ERROR - Problems opening CMextrn.h for write
29.1. PREPROCESSOR ERROR MESSAGES 503
The temporary file CMextern.h used in building the XSPICE simulator executable could not
be created or opened. Check permissions on directory.
ERROR - Problems opening CMinfo.h for write
The temporary file CMinfo.h used in building the XSPICE simulator executable could not be
created or opened. Check permissions on directory.
ERROR - Problems opening objects.inc file for write
The temporary file objects.inc used in building the XSPICE simulator executable could not be
created or opened. Check permissions on directory.
ERROR - Could not open input .mod file: <filename>
The Model Definition File that contains the definition of the Code Model’s behavior (usually
cfunc.mod) was not found or could not be read.
ERROR - Could not open output .c: <filename>
The indicated C language file that the preprocessor creates could not be created or opened.
Check permissions on directory.
Error parsing .mod file: <filename>
Problems were encountered by the preprocessor in interpreting the indicated Model Definition
File.
ERROR - File not found: <filename>
The indicated file was not found or could not be opened.
Error parsing interface specification file
Problems were encountered by the preprocessor in interpreting the indicated Interface Specifi-
cation File.
ERROR - Can’t create file: <filename>
The indicated file could not be created or opened. Check permissions on directory.
ERROR - write.port.info() - Number of allowed types cannot be zero
There must be at least one port type specified in the list of allowed types.
504 CHAPTER 29. ERROR MESSAGES
illegal quoted character in string (expected "\" or "\\")
A string was found with an illegal quoted character in it.
unterminated string literal
A string was found that was not terminated.
Unterminated comment
A comment was found that was not terminated.
Port ’<port name>’ not found
The indicated port name was not found in the Interface Specification File.
Port type ’vnam’ is only valid for ’in’ ports
The port type vnam was used for a port with direction out or inout. This type is only allowed
on in ports.
Port types ’g’, ’gd’, ’h’, ’hd’ are only valid for ’inout’ ports
Port type g,gd,h, or hd was used for a port with direction out or in. These types are only
allowed on inout ports.
Invalid parameter type - POINTER type valid only for STATIC_VARs
The type POINTER was used in a section of the Interface Specification file other than the
STATIC_VAR section.
Port default type is not an allowed type
A default type was specified that is not one of the allowed types for the port.
Incompatible port types in ‘allowed_types’ clause
Port types listed under ‘Allowed_Types’ in the Interface Specification File must all have the
same underlying data type. It is illegal to mix analog and eventdriven types in a list of allowed
types.
Invalid parameter type (saw <parameter type 1> - expected <parameter type 2>)
29.1. PREPROCESSOR ERROR MESSAGES 505
A parameter value was not compatible with the specified type for the parameter.
Named range not allowed for limits
A name was found where numeric limits were expected.
Direction of port ’<port number>’ in <port name>()
is not <IN or OUT> or INOUT
A problem exists with the direction of one of the elements of a port vector.
Port ’<port name>’ is an array - subscript required
A port was referenced that is specified as an array (vector) in the Interface Specification File. A
subscript is required (e.g. myport[i])
Parameter ’<parameter name>’ is an array - subscript required
A parameter was referenced that is specified as an array (vector) in the Interface Specification
File. A subscript is required (e.g. myparam[i])
Port ’<port name>’ is not an array - subscript prohibited
A port was referenced that is not specified as an array (vector) in the Interface Specification
File. A subscript is not allowed.
Parameter ’<parameter name>’ is not an array - subscript prohibited
A parameter was referenced that is not specified as an array (vector) in the Interface Specifica-
tion File. A subscript is not allowed.
Static variable ’<static variable name>’ is not an array - subscript prohibited
Array static variables are not supported. Use a POINTER type for the static variable.
Buffer overflow - try reducing the complexity of CM-macro array subscripts
The argument to a code model accessor macro was too long.
Unmatched )
An open ( was found with no corresponding closing ).
Unmatched ]
An open [ was found with no corresponding closing ].
506 CHAPTER 29. ERROR MESSAGES
29.2 Simulator Error Messages
The following is a list of error messages that may be encountered while attempting to run a
simulation (with the exception of those error messages generated by individual code models).
Most of these errors are generated by the simulator while attempting to parse a SPICE deck.
These are listed individually, and explanations follow the name/listing.
ERROR - Scalar port expected, [ found
A scalar connection was expected for a particular port on the code model, but the symbol [,
which is used to begin a vector connection list, was found.
ERROR - Unexpected ]
A ] was found where not expected. Most likely caused by a missing [.
ERROR - Unexpected [ - Arrays of arrays not allowed
A [ character was found within an array list already begun with another [ character.
ERROR - Tilde not allowed on analog nodes
The tilde character ~ was found on an analog connection. This symbol, which performs state
inversion, is only allowed on digital nodes and on User-Defined Nodes only if the node type
definition allows it.
ERROR - Not enough ports
An insufficient number of node connections was supplied on the instance line. Check the Inter-
face Specification File for the model to determine the required connections and their types.
ERROR - Expected node/instance identifier
A special token (e.g. []<>...) was found when not expected.
ERROR - Expected node identifier
A special token (e.g. []<>...) was found when not expected.
ERROR - unable to find definition of model <name>
A.model line for the referenced model was not found.
ERROR - model: %s - Array parameter expected - No array delimiter found
29.3. CODE MODEL ERROR MESSAGES 507
An array (vector) parameter was expected on the .model card, but enclosing [ ] characters were
not found to delimit its values.
ERROR - model: %s - Unexpected end of model card
The end of the indicated .model line was reached before all required information was supplied.
ERROR - model: %s - Array parameter must have at least one value
An array parameter was encountered that had no values.
ERROR - model: %s - Bad boolean value
A bad values was supplied for a Boolean. Value used must be TRUE, FALSE, T, or F.
ERROR - model: %s - Bad integer, octal, or hex value
A badly formed integer value was found.
ERROR - model: %s - Bad real value
A badly formed real value was found.
ERROR - model: %s - Bad complex value
A badly formed complex number was found. Complex numbers must be enclosed in < > deli-
miters.
29.3 Code Model Error Messages
The following is a list of error messages that may be encountered while attempting to run a
simulation with certain code models. These are listed alphabetically based on the name of the
code model, and explanations follow the name and listing.
29.3.1 Code Model aswitch
cntl_error:
*****ERROR*****
ASWITCH: CONTROL voltage delta less than 1.0e-12
This message occurs as a result of the cntl_off and cntl_on values being less than 1.0e-12 volt-
s/amperes apart.
508 CHAPTER 29. ERROR MESSAGES
29.3.2 Code Model climit
climit_range_error:
**** ERROR ****
* CLIMIT function linear range less than zero. *
This message occurs whenever the difference between the upper and lower control input values
are close enough that there is no effective room for proper limiting to occur; this indicates an
error in the control input values.
29.3.3 Code Model core
allocation_error:
***ERROR***
CORE: Allocation calloc failed!
This message is a generic message related to allocating sufficient storage for the H and B array
values.
limit_error:
***ERROR***
CORE: Violation of 50% rule in breakpoints!
This message occurs whenever the input domain value is an absolute value and the H coordinate
points are spaced too closely together (overlap of the smoothing regions will occur unless the
H values are redefined).
29.3.4 Code Model d_osc
d_osc_allocation_error:
**** Error ****
D_OSC: Error allocating VCO block storage
Generic block storage allocation error.
d_osc_array_error:
**** Error ****
D_OSC: Size of control array different than frequency array
Error occurs when there is a different number of control array members than frequency array
members.
d_osc_negative_freq_error:
**** Error ****
D_OSC: The extrapolated value for frequency
has been found to be negative...
Lower frequency level has been clamped to 0.0 Hz.
Occurs whenever a control voltage is input to a model that would ordinarily (given the specified
control/freq coordinate points) cause that model to attempt to generate an output oscillating at
zero frequency. In this case, the output will be clamped to some DC value until the control
voltage returns to a more reasonable value.
29.3. CODE MODEL ERROR MESSAGES 509
29.3.5 Code Model d_source
loading_error:
***ERROR***
D_SOURCE: source.txt file was not read successfully.
This message occurs whenever the d source model has experienced any difficulty in loading the
source.txt (or user-specified) file. This will occur with any of the following problems:
• Width of a vector line of the source file is incorrect.
• A time-point value is duplicated or is otherwise not monotonically increasing.
• One of the output values was not a valid 12-State value (0s, 1s, Us, 0r, 1r, Ur, 0z, 1z, Uz,
0u, 1u, Uu).
29.3.6 Code Model d_state
loading_error:
***ERROR***
D_STATE: state.in file was not read successfully.
The most common cause of this problem is a trailing
blank line in the state.in file
This error occurs when the state.in file (or user-named state machine input file) has not been
read successfully. This is due to one of the following:
• The counted number of tokens in one of the file’s input lines does not equal that required
to define either a state header or a continuation line (Note that all comment lines are
ignored, so these will never cause the error to occur).
• An output state value was defined using a symbol that was invalid (i.e., it was not one of
the following: 0s, 1s, Us, 0r, 1r, Ur, 0z, 1z, Uz, 0u, 1u, Uu).
• An input value was defined using a symbol that was invalid (i.e., it was not one of the
following: 0, 1, X, or x).
index_error:
***ERROR***
D_STATE: An error exists in the ordering of states values
in the states->state[] array. This is usually caused
by non-contiguous state definitions in the state.in file
This error is caused by the different state definitions in the input file being non-contiguous. In
general, it will refer to the different states not being defined uniquely, or being ‘broken up’ in
some fashion within the state.in file.
510 CHAPTER 29. ERROR MESSAGES
29.3.7 Code Model oneshot
oneshot_allocation_error:
**** Error ****
ONESHOT: Error allocating oneshot block storage
Generic storage allocation error.
oneshot_array_error:
**** Error ****
ONESHOT: Size of control array different than pulse-width array
This error indicates that the control array and pulse-width arrays are of different sizes.
oneshot_pw_clamp:
**** Warning ****
ONESHOT: Extrapolated Pulse-Width Limited to zero
This error indicates that for the current control input, a pulse-width of less than zero is indicated.
The model will consequently limit the pulse width to zero until the control input returns to a
more reasonable value.
29.3.8 Code Model pwl
allocation_error:
***ERROR***
PWL: Allocation calloc failed!
Generic storage allocation error.
limit_error:
***ERROR***
PWL: Violation of 50% rule in breakpoints!
This error message indicates that the pwl model has an absolute value for its input domain, and
that the x_array coordinates are so close together that the required smoothing regions would
overlap. To fix the problem, you can either spread the x_array coordinates out or make the
input domain value smaller.
29.3.9 Code Model s_xfer
num_size_error:
***ERROR***
S_XFER: Numerator coefficient array size greater than
denominator coefficient array size.
This error message indicates that the order of the numerator polynomial specified is greater
than that of the denominator. For the s_xfer model, the orders of numerator and denominator
polynomials must be equal, or the order of the denominator polynomial must be greater than
that or the numerator.
29.3. CODE MODEL ERROR MESSAGES 511
29.3.10 Code Model sine
allocation_error:
**** Error ****
SINE: Error allocating sine block storage
Generic storage allocation error.
sine_freq_clamp:
**** Warning ****
SINE: Extrapolated frequency limited to 1e-16 Hz
This error occurs whenever the controlling input value is such that the output frequency ordina-
rily would be set to a negative value. Consequently, the output frequency has been clamped to
a near-zero value.
array_error:
**** Error ****
SINE: Size of control array different than frequency array
This error message normally occurs whenever the controlling input array and the frequency
array are different sizes.
29.3.11 Code Model square
square_allocation_error:
**** Error ****
SQUARE: Error allocating square block storage
Generic storage allocation error.
square_freq_clamp:
**** WARNING ****
SQUARE: Frequency extrapolation limited to 1e-16
This error occurs whenever the controlling input value is such that the output frequency ordina-
rily would be set to a negative value. Consequently, the output frequency has been clamped to
a near-zero value.
square_array_error:
**** Error ****
SQUARE: Size of control array different than frequency array
This error message normally occurs whenever the controlling input array and the frequency
array are different sizes.
512 CHAPTER 29. ERROR MESSAGES
29.3.12 Code Model triangle
triangle_allocation_error:
**** Error ****
TRIANGLE: Error allocating triangle block storage
Generic storage allocation error.
triangle_freq_clamp:
**** Warning ****
TRIANGLE: Extrapolated Minimum Frequency Set to 1e-16 Hz
This error occurs whenever the controlling input value is such that the output frequency ordina-
rily would be set to a negative value. Consequently, the output frequency has been clamped to
a near-zero value.
triangle_array_error:
**** Error ****
TRIANGLE: Size of control array different than frequency array
This error message normally occurs whenever the controlling input array and the frequency
array are different sizes.
Part III
CIDER
513
Chapter 30
CIDER User’s Manual
The CIDER User’s Manual that follows is derived from the original manual being part of the
PhD thesis from David A. Gates from UC Berkeley. Unfortunately the manual here is not yet
complete, so please refer to the thesis for detailed information. Literature on CODECS, the
predecessor of CIDER, is available here from UCB: TechRpt ERL-90-96 and TechRpt ERL-
88-71.
30.1 SPECIFICATION
Overview of numerical-device specification
The input to CIDER consists of a SPICE-like description of a circuit, its analyses and its com-
pact device models, and PISCES-like descriptions of numerically analyzed device models. For
a description of the SPICE input format, consult the SPICE3 Users Manual [JOHN92].
To simulate devices numerically, two types of input must be added to the input file. The first
is a model description in which the common characteristics of a device class are collected. In
the case of numerical models, this provides all the information needed to construct a device
cross-section, such as, for example, the doping profile. The second type of input consists of one
or more element lines that specify instances of a numerical model, describe their connection to
the rest of the circuit, and provide additional element-specific information such as device layout
dimensions ans initial bias information.
The format of a numerical device model description differs from the standard approach used
for SPICE3 compact models. It begins the same way with one line containing the .MODEL
keyword followed by the name of the model, device type and modeling level. However, instead
of providing a single long list of parameters and their values, numerical model parameters are
grouped onto cards. Each type of card has its own set of valid parameters. In all cases, the
relative ordering of different types of cards is unimportant. However, for cards of the same type
(such as mesh-specification cards), their order in the input file can be important in determining
the device structure.
Each card begins on a separate line of the input file. In order to let CIDER know that card
lines are continuations of a numerical model description, each must begin with the continuation
character ‘+’. If there are too many parameters on a given card to allow it fit on a single line,
the card can be continued by adding a second ‘+’ to the beginning of the next line. However,
the name and value of a parameter should always appear on the same line.
515
516 CHAPTER 30. CIDER USER’S MANUAL
Several features are provided to make the numerical model format more convenient.
Blank space can follow the initial ‘+’ to separate it from the name of a card or the card con-
tinuation ‘+’. Blank lines are also permitted, as long as they also begin with an initial ‘+’.
Parentheses and commas can be used to visually group or separate parameter definitions. In
addition, while it is common to add an equal sign between a parameter and its value, this is not
strictly necessary.
The name of any card can be abbreviated, provided that the abbreviation is unique. Parameter
name abbreviations can also be used if they are unique in the list of a card’s parameters. Numeric
parameter values are treated identically as in SPICE3, so exponential notation, engineering
scale factors and units can be attached to parameter values: tau=10ns, nc=3.0e19cm^-3. In
SPICE3, the value of a FLAG model parameter is changed to TRUE simply by listing its name
on the model line. In CIDER, the value of a numerical model FLAG parameter can be turned
back to FALSE by preceding it by a caret ‘^’. This minimizes the amount of input change
needed when features such as debugging are turned on and off. In certain cases it is necessary
to include file names in the input description and these names may contain capital letters. If
the file name is part of an element line, the inout parser will convert these capitals to lowercase
letters. To protect capitalization at any time, simply enclose the string in double quotes ‘”’.
The remainder of this manual describes how numerically analyzed elements and models can be
used in CIDER simulations. The manual consists of three parts. First, all of the model cards and
their parameters are described. This is followed by a section describing the three basic types of
numerical models and their corresponding element lines. In the final section, several complete
examples of CIDER simulations are presented.
Several conventions are used in the card descriptions. In the card synopses, the name of a
card is followed by a list of parameter classes. Each class is represented by a section in the
card parameter table, in the same order as it appears in the synopsis line. Classes that contain
optional parameters are surrounded by brackets: [...]. Sometimes it only makes sense for a
single parameter to take effect. (For example, a material can not simultaneously be both Si
and SiO2.) In such cases, the various choices are listed sequentially, separated by colons. The
same parameter often has a number of different acceptable names, some of which are listed in
the parameter tables.1These aliases are separated by vertical bars: ‘|’. Finally, in the card
examples, the model continuation pluses have been removed from the card lines for clarity’s
sake.
30.1.1 Examples
The model description for a two-dimensional numerical diode might look something like what
follows. This example demonstrates many of the features of the input format described above.
Notice how the .MODEL line and the leading pluses form a border around the model description:
1Some of the possibilities are not listed in order to shorten the lengths of the parameter tables. This makes
the use of parameter abbreviations somewhat troublesome since an unlisted parameter may abbreviate to the same
name as one that is listed. CIDER will produce a warning when this occurs. Many of the undocumented parameter
names are the PISCES names for the same parameters. The adventurous soul can discover these names by delving
through the ‘cards’ directory of the source code distribution looking for the C parameter tables.
30.2. BOUNDARY, INTERFACE 517
Example: Numerical diode
. MODEL M_NUMERICAL NUPD LEVEL =2
+ cardnamel numberl =val1 (number2 val2 ), ( number3 = val3 )
+ cardname2 numberl =val1 string1 = name1
+
+ cardname3 numberl =val1 , flag1 , ^ flag2
+ + number2 =val2 , flag3
The element line for an instance of this model might look something like the following. Double
quotes are used to protect the file name from decapitalization:
dl 1 2 M_NUMERICAL area= lOOpm ^2 ic.file = "diode .IC"
30.2 BOUNDARY, INTERFACE
Specify properties of a domain boundary or the interface between two boundaries.
SYNOPSIS
boundary domain [bounding -box] [ properties]
interface domain neighbor [ bounding - box] [ properties ]
30.2.1 DESCRIPTION
The boundary and interface cards are used to set surface physics parameters along the boundary
of a specified domain. Normally, the parameters apply to the entire boundary, but there are two
ways to restrict the area of interest. If a neighboring domain is also specified, the parameters
are only set on the interface between the two domains. In addition, if a bounding box is given,
only that portion of the boundary or interface inside the bounding box will be set.
If a semiconductor-insulator interface is specified, then an estimate of the width of any inversion
or accumulation layer that may form at the interface can be provided. If the surface mobility
model (cf. models card) is enabled, then the model will apply to all semiconductor portions of
the device within this estimated distance of the interface. If a point lies within the estimated
layer width of more than one interface, it belong to the interface specified first in the input file.
If the layer width given is less than or equal to zero, it is automatically replaced by an estimate
calculated from the doping near the interface. As a consequence, if the doping varies so will the
layer width estimate.
Each edge of the bounding box can be specified in terms of its location or its mesh-index in the
relevant dimension, or defaulted to the respective boundary of the simulation mesh.
518 CHAPTER 30. CIDER USER’S MANUAL
30.2.2 PARAMETERS
Name Type Description Units
Domain Integer ID number of primary domain
Neighbor Integer ID number of neighboring domain
X.Low Real Lowest X location of bounding box µm
: IX.Low Integer Lowest X mesh-index of bounding box
X.High Real Highest X location of bounding box µm
: IX.High Integer Highest X mesh-index of bounding box
Y.Low Real Lowest Y location of bounding box µm
: IY.Low Integer Lowest Y mesh-index of bounding box
Y.High Real Highest Y location of bounding box µm
:IY.High Integer Highest Y mesh-index of bounding box
Qf Real Fixed interface charge C
/cm2
SN Real Surface recombination velocity - electrons cm
/s
SP Real Surface recombination velocity - holes cm
/s
Layer.Width Real Width of surface layer µm
30.2.3 EXAMPLES
The following shows how the surface recombination velocities at an Si-SiO2 interface might be
set:
interface dom=l neigh =2 sn=l.Oe4 sp =l. Oe4
In a MOSFET with a 2.0µmgate width and 0.1µmsource and drain overlap, the surface channel
can be restricted to the region between the metallurgical junctions and within 100 ˙
A(0.01 µm)
of the interface:
interface dom =l neigh =2 x.l=l. l x .h =2.9 layer .w =0.01
The inversion layer width in the previous example can be automatically determined by setting
the estimate to 0.0:
interface dom =l neigh =% x.l=l. l x .h =2.9 layer .w =0.0
30.3 COMMENT
Add explanatory comments to a device definition.
SYNOPSIS
comment [text ]
* [text]
$ [text]
# [text]
30.4. CONTACT 519
30.3.1 DESCRIPTION
Annotations can be added to a device definition using the comment card. All text on a comment
card is ignored. Several popular commenting characters are also supported as aliases: ‘*’ from
SPICE, ‘$’ from PISCES, and ‘#’ from Linux shell scripts.
30.3.2 EXAMPLES
A SPICE-like comment is followed by a PISCES-like comment and shell script comment:
* CIDER and SPICE would ignore this input line
$ CIDER and PISCES would ignore this , but SPICE wouldn ’t
# CIDER and Linux Shell scripts would ignore this input line
30.4 CONTACT
Specify properties of an electrode
SYNOPSIS
contact number [ workfunction ]
30.4.1 DESCRIPTION
The properties of an electrode can be set using the contact card. The only changeable property is
the work-function of the electrode material and this only affects contacts made to an insulating
material. All contacts to semiconductor material are assumed to be ohmic in nature.
30.4.2 PARAMETERS
Name Type Description
Number Integer ID number of the electrode
Work-function Real Work-function of electrode material. ( eV )
30.4.3 EXAMPLES
The following shows how the work-function of the gate contact of a MOSFET might be changed
to a value appropriate for a P+ polysilicon gate:
contact num =2 workf =5.29
520 CHAPTER 30. CIDER USER’S MANUAL
30.4.4 SEE ALSO
electrode, material
30.5 DOMAIN, REGION
Identify material-type for section of a device
SYNOPSIS
domain number material [ position]
region number material [ position]
30.5.1 DESCRIPTION
A device is divided into one or more rectilinear domains, each of which has a unique identifica-
tion number and is composed of a particular material.
Domain (aka region) cards are used to build up domains by associating a material type with a
box-shaped section of the device. A single domain may be the union of multiple boxes. When
multiple domain cards overlap in space, the one occurring last in the input file will determine
the ID number and material type of the overlapped region.
Each edge of a domain box can be specified in terms of its location or mesh-index in the relevant
dimension, or defaulted to the respective boundary of the simulation mesh.
30.5.2 PARAMETERS
Name Type Description
Number Integer ID number of this domain
Material Integer ID number of material used by this domain
X.Low Real Lowest X location of domain box, ( µm)
:IX.Low Integer Lowest X mesh-index of domain box
X.High Real Highest X location of domain box, ( µm)
:IX-High Integer Highest X mesh-index of domain box
Y.Low Real Lowest Y location of domain box, ( µm)
:IY.Low Integer Lowest Y mesh-index of domain box
Y.High Real Highest Y location of domain box, ( µm)
:IY.High Integer Highest Y mesh-index of domain box
30.5.3 EXAMPLES
Create a 4.0 pm wide by 2.0 pm high domain out of material #1:
domain num=l material =l x.l=O.O x.h =4.0 y.l=O.O y.h=2.0
30.6. DOPING 521
The next example defines the two domains that would be typical of a planar MOSFET simula-
tion. One occupies all of the mesh below y = 0 and the other occupies the mesh above y = 0.
Because the x values are left unspecified, the low and high x boundaries default to the edges of
the mesh:
domain n=l m=l y.l=O.O
domain n=2 m=2 y.h=O.O
30.5.4 SEE ALSO
x.mesh, material
30.6 DOPING
Add dopant to regions of a device
SYNOPSIS
doping [domains ] profile -type [lateral -profile - type] [ axis ]
[impurity -type1 [ constant - box] [profile - specifications ]
30.6.1 DESCRIPTION
Doping cards are used to add impurities to the various domains of a device. Initially each
domain is dopant-free. Each new doping card creates a new doping profile that defines the
dopant concentration as a function of position. The doping at a particular location is then the
sum over all profiles of the concentration values at that position. Each profile can be restricted
to a subset of a device’s domains by supplying a list of the desired domains.
Otherwise, all domains are doped by each profile.
A profile has uniform concentration inside the constant box. Outside this region, it varies accor-
ding to the primary an lateral profile shapes. In 1D devices the lateral shape is unused and in 2D
devices the y-axis is the default axis for the primary profile. Several analytic functions can be
used to define the primary profile shape. Alternatively, empirical or simulated profile data can
be extracted from a file. For the analytic profiles, the doping is the product of a profile function
(e.g. Gaussian) and a reference concentration, which is either the constant concentration of a
uniform profile, or the peak concentration for any of the other functions. If concentration data
is used instead take from an ASCII file containing a list of location-concentration pairs or a
SUPREM3 exported file, the name of the file must be provided. If necessary, the final concen-
tration at a point is then found by multiplying the primary profile concentration by the value of
the lateral profile function at that point. Empirical profiles must first be normalized by the value
at 0.0 to provide a usable profile functions. Alternatively, the second dimension can be included
by assigning the same concentration to all points equidistant from the edges of the constant box.
The contours of the profile are the circular.
522 CHAPTER 30. CIDER USER’S MANUAL
Figure 30.1: 1D doping profiles with location > 0.
Unless otherwise specified, the added impurities are assumes to be N type. However, the name
of a specific dopant species is needed when extracting concentration information for that impu-
rity from a SUPREM3 exported file.
Several parameters are used to adjust the basic shape of a profile functions so that the final,
constructed profile, matches the doping profile in the real device. The constant box region
should coincide with a region of constant concentration in the device. For uniform profiles its
boundaries default to the mesh boundaries. For the other profiles the constant box starts as a
point and only acquires width or height if both the appropriate edges are specified. The location
of the peak of the primary profile can be moved away from the edge of the constant box. A
positive location places the peak outside the constant box (cf. Fig. 30.1), and a negative value
puts it inside the constant box (cf. Fig. 30.2). The concentration in the constant box is then
equal to the value of the profile when it intersects the edge of the constant box. The argument
of the profile function is a distance expressed in terms of the characteristic length (by default
equal to 1µm). The longer this length, the more gradually the profile will change. For example,
in Fig. 30.1 and Fig. 30.2, the profiles marked (a) have characteristic lengths twice those of the
profiles marked (b). The location and characteristic length for the lateral profile are multiplied
by the lateral ratio. This allows the use of different length scales for the primary and lateral
profiles. For rotated profiles, this scaling is taken into account, and the profile contours are
elliptical rather than circular.
30.6. DOPING 523
Figure 30.2: 1D doping profiles with location < 0.
524 CHAPTER 30. CIDER USER’S MANUAL
30.6.2 PARAMETERS
Name Type Description
Domains Int List List of domains to dope
Uniform: Flag Primary profile type
Linear:
Erfc:
Exponential:
Suprem3:
Ascii:
Ascii Suprem3
InFile String Name of Suprem3, Ascii or Ascii Suprem3 input file
Lat.Rotate: Flag Lateral profile type
Lat.Unif:
Lat.Lin:
Lat.Gauss:
Lat.Erfc:
Lat.Exp
X.Axis:Y.Axis Flag Primary profile direction
N.Type: P.Type: Flag Impurity type
Donor: Acceptor:
Phosphorus:
Arsenic:
Antimony:
Boron
X.Low Real Lowest X location of constant box, (µm)
X.High Real Highest X location of constant box, (µm)
Y.Low Real Lowest Y location of constant box, (µm)
Y.High Real Highest Y location of constant box, (µm)
Conic | Peak.conic Real Dopant concentration, (cm−3)
Location | Range Real Location of profile edge/peak, (µm)
Char.Length Real Characteristic length of profile, (µm)
Ratio.Lat Real Ratio of lateral to primary distances
30.6.3 EXAMPLES
This first example adds a uniform background P-type doping of 1.0×1016cm−3to an entire
device:
doping uniform p.type conc =l.0 el6
A Gaussian implantation with rotated lateral falloff, such as might be used for a MOSFET
source, is then added:
doping gauss lat.rotate n. type conc=l.0el9
+ x.l =0.0 x.h=0.5 y.l =0.0 y.h =0.2 ratio =0.7
30.7. ELECTRODE 525
Alternatively, an error-function falloff could be used:
doping gauss lat.erfc conc=l.0 el9
+ x.l =0.0 x.h=0.5 y.l =0.0 y.h =0.2 ratio =0.7
Finally, the MOSFET channel implant is extracted from an ASCII-format SUPREM3 file. The
lateral profile is uniform, so that the implant is confined between X=1µmand X=3µm. The
profile begins at Y=0µm(the high Y value defaults equal to the low Y value):
doping ascii suprem3 infile = implant.s3 lat. unif boron
+ x.l =1.0 x.h=3.0 y.l =0.0
30.6.4 SEE ALSO
domain, mobility, contact, boundary
30.7 ELECTRODE
Set location of a contact to the device
SYNOPSIS
electrode [ number ] [position ]
30.7.1 DESCRIPTION
Each device has several electrodes that are used to connect the device to the rest of the circuit.
The number of electrodes depends on the type of device. For example, a MOSFET needs 4
electrodes. A particular electrode can be identified by its position in the list of circuit nodes
on the device element line. For example, the drain node of a MOSFET is electrode number 1,
while the bulk node is electrode number 4. Electrodes for which an ID number has not been
specified are assigned values sequentially in the order they appear in the input file.
For lD devices, the positions of two of the electrodes are predefined to be at the ends of the
simulation mesh. The first electrode is at the low end of the mesh, and the last electrode is at
the high end. The position of the special lD BJT base contact is set on the options card. Thus,
electrode cards are used exclusively for 2D devices.
Each card associates a portion of the simulation mesh with a particular electrode. In contrast to
domains, which are specified only in terms of boxes, electrodes can also be specified in terms of
line segments. Boxes and segments for the same electrode do not have to overlap. If they don’t,
it is assumed that the electrode is wired together outside the area covered by the simulation
mesh. However, pieces of different electrodes must not overlap, since this would represent
a short circuit. Each electrode box or segment can be specified in terms of the locations or
mesh-indices of its boundaries. A missing value defaults to the corresponding mesh boundary.
526 CHAPTER 30. CIDER USER’S MANUAL
30.7.2 PARAMETERS
Name Type Description
Number Integer ID number of this domain
X.Low Real Lowest X location of electrode, (µm)
:IX.Low Integer Lowest X mesh-index of electrode
X.High Real Highest X location of electrode, (µm)
:IX.High Integer Highest X mesh-index of electrode
Y.Low Real Lowest Y location of electrode, (µm)
:IY.Low Integer Lowest Y mesh-index of electrode
Y.High Real Highest Y location of electrode, (µm)
:IY.High Integer Highest Y mesh-index of electrode
30.7.3 EXAMPLES
The following shows how the four contacts of a MOSFET might be specified:
* DRAIN
electrode x.l =0.0 x.h =0.5 y.l=0.0 y.h =0.0
* GATE
electrode x.l =1.0 x.h =3.0 iy.l=0 iy.h=0
* SOURCE
electrode x.l =3.0 x.h =4.0 y.l=0.0 y.h =0.0
* BULK
electrode x.l =0.0 x.h =4.0 y.l=2.0 y.h =2.0
The numbering option can be used when specifying bipolar transistors with dual base contacts:
* EMITTER
electrode num =3 x.l =1.0 x.h=2.0 y.l=0.0 y.h =0.0
* BASE
electrode num =2 x.l =0.0 x.h=0.5 y.l=0.0 y.h =0.0
electrode num =2 x.l =2.5 x.h=3.0 y.l=0.0 y.h =0.0
* COLLECTOR
electrode num =1 x.l =0.0 x.h=3.0 y.l=1.0 y.h =1.0
30.7.4 SEE ALSO
domain, contact
30.8 END
Terminate processing of a device definition
30.9. MATERIAL 527
SYNOPSIS
end
30.8.1 DESCRIPTION
The end card stops processing of a device definition. It may appear anywhere within a definition.
Subsequent continuation lines of the definition will be ignored. If no end card is supplied, all
the cards will be processed.
30.9 MATERIAL
Specify physical properties of a material
SYNOPSIS
material number type [physical - constants]
30.9.1 DESCRIPTION
The material card is used to create an entry in the list of materials used in a device. Each entry
needs a unique identification number and the type of the material. Default values are assigned
to the physical properties of the material. Most material parameters are accessible either here
or on the mobility or contact cards. However, some parameters remain inaccessible (e.g.
the ionization coefficient parameters). Parameters for most physical effect models are collected
here. Mobility parameters are handled separately by the mobility card. Properties of electrode
materials are set using the contact card.
528 CHAPTER 30. CIDER USER’S MANUAL
30.9.2 PARAMETERS
Name Type Description
Number Integer ID number of this material
Semiconductor : Silicon Flag Type of this material
: Polysilicon : GaAs
: Insulator : Oxide
: Nitride
Affinity Real Electron affinity (eV)
Permittivity Real Dielectric permittivity (F/cm)
Nc Real Conduction band density (cm−3)
Nv Real Valence band density (cm−3)
Eg Real Energy band gap (eV)
dEg.dT Real Bandgap narrowing with temperature (eV/◦K)
Eg.Tref Real Bandgap reference temperature, ( °K )
dEg.dN Real Bandgap narrowing with N doping, (eV/cm−3)
Eg.Nref Real Bandgap reference concentration - N type, (cm−3)
dEg.dP Real Bandgap narrowing with P doping, (eV/cm−3)
Eg.Pref Real Bandgap reference concentration - P type, (cm−3)
TN Real SRH lifetime - electrons, (sec)
SRH.Nref Real SRH reference concentration - electrons (cm−3)
TP Real SRH lifetime - holes, (sec)
SRH.Pref Real SRH reference concentration - holes (cm−3)
CN Real Auger coefficient - electrons (cm6
/sec)
CP Real Auger coefficient - holes (cm6
/sec)
ARichN Real Richardson constant - electrons, ( A
/cm2
◦K2)
ARichP Real Richardson constant - holes, ( A
/cm2
◦K2)
30.9.3 EXAMPLES
Set the type of material #1 to silicon, then adjust the values of the temperature-dependent band-
gap model parameters:
material num =1 silicon eg =1.12 deg .dt =4.7 e-4 eg . tref =640.0
The recombination lifetimes can be set to extremely short values to simulate imperfect semi-
conductor material:
material num =2 silicon tn =1ps tp=1 ps
30.9.4 SEE ALSO
domain, mobility, contact, boundary
30.10. METHOD 529
30.10 METHOD
Choose types and parameters of numerical methods
SYNOPSIS
method [types ] [ parameters ]
30.10.1 DESCRIPTION
The method card controls which numerical methods are used during a simulation and the pa-
rameters of these methods. Most of these methods are optimizations that reduce run time, but
may sacrifice accuracy or reliable convergence.
For majority-carrier devices such as MOSFETs, one carrier simulations can be used to save
simulation time. The systems of equations in AC analysis may be solved using either direct or
successive-over-relaxation techniques. Successive-over-relaxation is faster, but at high frequen-
cies, it may fail to converge or may converge to the wrong answer. In some cases, it is desirable
to obtain AC parameters as functions of DC bias conditions. If necessary, a one-point AC analy-
sis is performed at a predefined frequency in order to obtain these small-signal parameters. The
default for this frequency is 1 Hz. The Jacobian matrix for DC and transient analyses can be
simplified by ignoring the derivatives of the mobility with respect to the solution variables. Ho-
wever, the resulting analysis may have convergence problems. Additionally, if they are ignored
during AC analyses, incorrect results may be obtained.
A damped Newton method is used as the primary solution technique for the device-level partial
differential equations. This algorithm is based on an iterative loop that terminates when the error
in the solution is small enough or the iteration limit is reached. Error tolerances are used when
determining if the error is ‘small enough’. The tolerances are expressed in terms of an absolute,
solution-independent error and a relative, solution-dependent error. The absolute-error limit can
be set on this card. The relative error is computed by multiplying the size of the solution by the
circuit level SPICE parameter RELTOL.
30.10.2 Parameters
Name Type Description
OneCarrier Flag Solve for majority carriers only
AC analysis String AC analysis method, ( either DIRECT or SOR)
NoMobDeriv Flag Ignore mobility derivatives
Frequency Real AC analysis frequency, ( Hz )
ItLim Integer Newton iteration limit
DevTol Real Maximum residual error in device equations
30.10.3 Examples
Use one carrier simulation for a MOSFET, and choose direct method AC analysis to ensure
accurate, high frequency results:
530 CHAPTER 30. CIDER USER’S MANUAL
method onec ac.an=direct
Tolerate no more than 10−10 as the absolute error in device-level equations, and perform no
more than 15 Newton iterations in any one loop:
method devtol =1e -10 itlim =15
30.11 Mobility
Specify types and parameters of mobility models
SYNOPSIS
mobility material [ carrier] [ parameters ] [ models] [ initialize ]
30.11.1 Description
The mobility model is one of the most complicated models of a material’s physical properties.
As a result, separate cards are needed to set up this model for a given material.
Mobile carriers in a device are divided into a number of different classes, each of which has
different mobility modelling. There are three levels of division. First, electrons and holes are
obviously handled separately. Second, carriers in surface inversion or accumulation layers are
treated differently than carriers in the bulk. Finally, bulk carriers can be either majority or
minority carriers.
For surface carriers, the normal-field mobility degradation model has three user-modifiable pa-
rameters. For bulk carriers, the ionized impurity scattering model has four controllable para-
meters. Different sets of parameters are maintained for each of the four bulk carrier types:
majority-electron, minority-electron, majority-hole and minority-hole. Velocity saturation mo-
deling can be applied to both surface and bulk carriers. However, only two sets of parameters
are maintained: one for electrons and one for holes. These must be changed on a majority
carrier card (i.e. when the majority flag is set).
Several models for the physical effects are available, along with appropriate default values.
Initially, a universal set of default parameters usable with all models is provided. These can be
overridden by defaults specific to a particular model by setting the initialization flag. These can
then be changed directly on the card itself. The bulk ionized impurity models are the Caughey-
Thomas (CT) model and the Scharfetter-Gummel (SG) model [CAUG671, [SCHA69]. Three
alternative sets of defaults are available for the Caughey-Thomas expression. They are the Arora
(AR) parameters for Si [AROR82], the University of Florida (UF) parameters for minority
carriers in Si [SOLL90], and a set of parameters appropriate for GaAs (GA). The velocity-
saturation models are the Caughey-Thomas (CT) and Scharfetter-Gummel (SG) models for Si,
and the PISCES model for GaAs (GA). There is also a set of Arora (AR) parameters for the
Caughey-Thomas model.
30.11. MOBILITY 531
30.11.2 Parameters
Name Type Description
Material Integer ID number of material
Electron : Hole Flag Mobile carrier
Majority : Minority Flag Mobile carrier type
MUS Real Maximum surface mobility, ( cm2/Vs )
EC.A Real Surface mobility 1st-order critical field, ( V/cm )
EC.B Real Real Surface mobility 2nd-order critical field, ( V2/cm2 )
MuMax Real Maximum bulk mobility, ( cm2/Vs )
MuMin Real Minimum bulk mobility, ( cm2/Vs)
NtRef Real Ionized impurity reference concentration, ( cm-3 )
NtExp Real Ionized impurity exponent
Vsat Real Saturation velocity, ( cm/s )
Vwarm Real Warm carrier reference velocity, ( cm/s )
ConcModel String Ionized impurity model, ( CT, AR, UF, SG, Dr GA )
FieldModel String Velocity saturation model, ( CT, AR, SG, or GA )
Init Flag Copy model-specific defaults
30.11.3 Examples
The following set of cards completely updates the bulk mobility parameters for material #1:
mobility mat=l concmod =sg fieldmod=sg
mobility mat =l elec major mumax =1000.0 mumin = l00 .0
+ ntref =l.0 el6 ntexp =0.8 vsat =l.0 e7 vwarm =3.0 e6
mobility mat =l elec minor mumax =1000.0 mumin =200.O
+ ntref =l.0 el7 ntexp =0.9
mobility mat =l hole major mumax =500.0 mumin =50.0
+ ntref =l .0 el6 ntexp =0.7 vsat =8.0 e6 vwarm =l .0 e6
mobility mat=l hole minor mumax =500.0 mumin =150.0
+ ntref =l.0 el7 ntexp =0.8
The electron surface mobility is changed by the following:
mobility mat =l elec mus =800.0 ec .a =3.0 e5 ec .b =9.0 e5
Finally, the default Scharfetter-Gummel parameters can be used in Si with the GaAs velocity-
saturation model (even though it doesn’t make physical sense!):
mobility mat =l init elec major fieldmodel=sg
mobility mat =l init hole major fieldmodel=sg
mobility mat=l fieldmodel =ga
30.11.4 SEE ALSO
material
532 CHAPTER 30. CIDER USER’S MANUAL
30.11.5 BUGS
The surface mobility model does not include temperature-dependence for the transverse-field
parameters. Those parameters will need to be adjusted by hand.
30.12 MODELS
Specify which physical models should be simulated
SYNOPSIS
models [model flags ]
30.12.1 DESCRIPTION
The models card indicates which physical effects should be modeled during a simulation. Initi-
ally, none of the effects are included. A flag can be set false by preceding by a caret.
30.12.2 Parameters
Name Type Description
BGN Flag Bandgap narrowing
SRH Flag Shockley-Reed-Hall recombination
ConcTau Flag Concentration-dependent SRH lifetimes
Auger Flag Auger recombination
Avalanche Flag Local avalanche generation
TempMob Flag Temperature-dependent mobility
ConcMob Flag Concentration-dependent mobility
FieldMob Flag Lateral-field-dependent mobility
TransMob Flag Transverse-field-dependent surface mobility
SurfMob Flag Activate surface mobility model
30.12.3 Examples
Turn on bandgap narrowing, and all of the generation-recombination effects:
models bgn srh conctau auger aval
Amend the first card by turning on lateral- and transverse-field-dependent mobility in surface
charge layers, and lateral-field-dependent mobility in the bulk. Also, this line turns avalanche
generation modeling off.
models surfmob transmob fieldmob ^ aval
30.13. OPTIONS 533
30.12.4 See also
material, mobility
30.12.5 Bugs
The local avalanche generation model for 2D devices does not compute the necessary contri-
butions to the device-level Jacobian matrix. If this model is used, it may cause convergence
difficulties and it will cause AC analyses to produce incorrect results.
30.13 OPTIONS
Provide optional device-specific information
SYNOPSIS
options [device -type] [initial - state ] [dimensions ]
[measurement - temperature]
30.13.1 DESCRIPTION
The options card functions as a catch-all for various information related to the circuit-device
interface. The type of a device can be specified here, but will be defaulted if none is given.
Device type is used primarily to determine how to limit the changes in voltage between the
terminals of a device. It also helps determine what kind of boundary conditions are used as
defaults for the device electrodes.
A previously calculated state, stored in the named initial-conditions file, can be loaded at the
beginning of an analysis. If it is necessary for each instance of a numerical model to start in a
different state, then the unique flag can be used to generate unique filenames for each instance
by appending the instance name to the given filename. This is the same method used by CIDER
to generate unique filenames when the states are originally saved. If a particular state file does
not fit. this pattern, the filename can be entered directly on the instance line.
Mask dimension defaults can be set so that device sizes can be specified in terms of area or
width. Dimensions for the special lD BJT base contact can also be controlled. The measurement
temperature of material parameters, normally taken to be the circuit default, can be overridden.
534 CHAPTER 30. CIDER USER’S MANUAL
30.13.2 Parameters
Name Type Description
Resistor Flag Resistor
: Capacitor Flag Capacitor
: Diode Flag Diode
: Bipolar|BJT Flag Bipolar transistor
: MOSFET Flag MOS field-effect transistor
: JFET Flag Junction field-effect transistor
: MESFET Flag MES field-effect transistor
IC.File String Initial-conditions filename
Unique Flag Append instance name to filename
DefA Real Default Mask Area, (m²)
DefW Real Default Mask Width, (m)
DefL Real Default Mask Length, (m)
Base.Area Real lD BJT base area relative to emitter area
Base.Length Real Real lD BJT base contact length, (µm)
Base.Depth Real lD BJT base contact depth, (µm)
TNom Real Nominal measurement temperature, (°C)
30.13.3 Examples
Normally, a ’numos’ device model is used for MOSFET devices. However, it can be changed
into a bipolar-with-substrate-contact model, by specifying a bipolar structure using the other
cards, and indicating the device-structure type as shown here. The default length is set to 1.0
µm so that when mask area is specified on the element line it can be divided by this default to
obtain the device width.
options bipolar defl =1.0
Specify that a 1D BJT has base area 1/10th that of the emitter, has an effective depth of 0.2 µm
and a length between the internal and external base contacts
options base . area =0.1 base .depth =0.2 base.len =1.5
If a circuit contains two instances of a bipolar transistor model named ’q1’ and ’q2’, the fol-
lowing line tells the simulator to look for initial conditions in the ’OP1.q2’, respectively. The
period in the middle of the names is added automatically:
options unique ic . file =" OP1 "
30.13.4 See also
numd, nbjt, numos
30.14. OUTPUT 535
30.14 OUTPUT
Identify information to be printed or saved
SYNOPSIS
output [debugging -flags ] [ general - info] [saved - solutions ]
30.14.1 DESCRIPTION
The output card is used to control the amount of information that is either presented to or saved
for the user. Three types of information are available. Debugging information is available as
a means to monitor program execution. This is useful during long simulations when one is
unsure about whether the program has become trapped at some stage of the simulation. General
information about a device such as material parameters and resource usage can be obtained.
Finally, information about the internal and external states of a device is available. Since this
data is best interpreted using a post-processor, a facility is available for saving device solutions
in auxiliary output files. Solution filenames are automatically generated by the simulator. If the
named file already exists, the file will be overwritten. A filename unique to a particular circuit
or run can be generated by providing a root filename. This root name will be added onto the
beginning of the automatically generated name. This feature can be used to store solutions in
a directory other than the current one by specifying the root filename as the path of the desired
directory. Solutions are only saved for those devices that specify the ‘save’ parameter on their
instance lines.
The various physical values that can be saved are named below. By default, the following values
are saved: the doping, the electron and hole concentrations, the potential, the electric field, the
electron and hole current densities, and the displacement current density. Values can be added
to or deleted from this list by turning the appropriate flag on or off. For vector-valued quantities
in two dimensions, both the X and Y components are saved. The vector magnitude can be
obtained during post-processing.
Saved solutions can be used in conjunction with the options card and instance lines to reuse
previously calculated solutions as initial guesses for new solutions.For example, it is typical to
initialize the device to a known state prior to beginning any DC transfer curve or operating point
analysis. This state is an ideal candidate to be saved for later use when it is known that many
analyses will be performed on a particular device structure.
536 CHAPTER 30. CIDER USER’S MANUAL
30.14.2 Parameters
Name Type Description
All.Debug Flag Debug all analyses
OP.Debug Flag .OP analyses
DC.Debug Flag .DC analyses
TRAN.Debug Flag .TRAN analyses
AC.Debug Flag .AC analyses
PZ.Debug Flag .PZ analyses
Material Flag Physical material information
Statistics | Resources Flag Resource usage information
RootFile String Root of output file names
Psi Flag Potential ( V )
Equ.Psi Flag Equilibrium potential ( V )
Vac.Psi Flag Vacuum potential ( V )
Doping Flag Net doping ( cm³ )
N.Conc Flag Electron concentration ( cm³ )
P.Conc Flag Hole concentration ( cm³ )
PhiN Flag Electron quasi-fermi potential ( V )
PhiP Flag Hole quasi-fermi potential ( V )
PhiC Flag Conduction band potential ( V )
PhiV Flag Valence band potential ( V )
E.Field Flag Electric field ( V/cm )
JC Flag Conduction current density ( A/cm² )
JD Flag Displacement current density ( A/cm² )
JN Flag Electron current density ( A/cm² )
JP Flag Hole current density ( A/cm² )
JT Flag Total current density ( A/cm² )
Unet Flag Net recombination ( 1/cm³ s )
MuN Flag Electron mobility (low-field) ( cm²/Vs )
MuP Flag Hole mobility (low-field) ( cm²/Vs )
30.14.3 Examples
The following example activates all potentially valuable diagnostic output:
output all . debug mater stat
Energy band diagrams generally contain the potential, the quasi-fermi levels, the energies and
the vacuum energy. The following example enables saving of the r values needed to make
energy band diagrams:
output phin phjp phic phiv vac.psi
Sometimes it is desirable to save certain key solutions, and then reload them for use in subse-
quent simulations. In such cases only the essential values ( Ψ, n, and p ) need to be saved. This
example turns off the nonessential default values (and indicates the essential ones explicitly):
30.15. TITLE 537
output psi n. conc p. conc ^e.f ^jn ^jp ^jd
30.14.4 SEE ALSO
options, numd, nbjt, numos
30.15 TITLE
Provide a label for this device’s output
SYNOPSIS
title [text ]
30.15.1 DESCRIPTION
The title card provides a label for use as a heading in various output files. The text can be any
length, but titles that fit on a single line will produce more aesthetically pleasing output.
30.15.2 EXAMPLES
Set the title for a minimum gate length NMOSFET in a 1.0µm BiCMOS process
title L =1.0 um NMOS Device , 1.0 um BiCMOS Process
30.15.3 BUGS
The title is currently treated like a comment.
30.16 X.MESH, Y.MESH
Define locations of lines and nodes in a mesh
SYNOPSIS
x.mesh position numbering - method [spacing - parameters]
y.mesh position numbering - method [spacing - parameters]
538 CHAPTER 30. CIDER USER’S MANUAL
30.16.1 DESCRIPTION
The domains of a device are discretized onto a rectangular finite-difference mesh using x.mesh
cards for 1D devices, or x.mesh and y.mesh cards for 2D devices. Both uniform and non-
uniform meshes can be specified.
A typical mesh for a 2D device is shown in Fig. 30.3.
Figure 30.3: Typical mesh for 2D devices
The mesh is divided into intervals by the reference lines. The other lines in each interval are
automatically generated by CIDER using the mesh spacing parameters. In general, each new
mesh card adds one reference line and multiple automatic lines to the mesh. Conceptually, a 1D
mesh is similar to a 2D mesh except that there are no reference or automatic lines needed in the
second dimension.
The location of a reference line in the mesh must either be given explicitly (using Location) or
defined implicitly relative to the location of the previous reference line (by using Width). (If the
first card in either direction is specified using Width, an initial reference line is automatically
generated at location 0.0.) The line number of the reference line can be given explicitly, in
which case the automatic lines are evenly spaced within the interval, and the number of lines
is determined from the difference between the current line number and that of the previous
reference line. However, if the interval width is given, then the line number is interpreted
directly as the number of additional lines to add to the mesh.
For a nonuniformly spaced interval, the number of automatic lines has to be determined using
the mesh spacing parameters. Nonuniform spacing is triggered by providing a desired ratio for
the lengths of the spaces between adjacent pairs of lines. This ratio should always be greater
than one, indicating the ratio of larger spaces to smaller spaces. In addition to the ratio, one
or both of the space widths at the ends of the interval must be provided. If only one is given,
30.16. X.MESH, Y.MESH 539
it will be the smallest space and the largest space will be at the opposite end of the interval.
If both are given, the largest space will be in the middle of the interval. In certain cases it is
desirable to limit the growth of space widths in order to control the solution accuracy. This can
be accomplished by specifying a maximum space size, but this option is only available when
one of the two end lengths is given. Note that once the number of new lines is determined
using the desired ratio, the actual spacing ratio may be adjusted so that the spaces exactly fill
the interval.
30.16.2 Parameters
Name Type Description
Location Real Location of this mesh line, ( µm )
:Width Real Width between this and previous mesh lines, ( µm )
Number | Node Integer Number of this mesh line
:Ratio Real Ratio of sizes of adjacent spaces
H.Start | H1 Real Space size at start of interval, ( µm )
H.End | H2 Real Space size at end of interval, ( µm )
H.Max | H3 Real Maximum space size inside interval, ( µm )
30.16.3 EXAMPLES
A 50 node, uniform mesh for a 5 µm long semiconductor resistor can be specified as:
x. mesh loc =0.0 n =1
x. mesh loc =5.0 n =50
An accurate mesh for a 1D diode needs fine spacing near the junction. In this example, the
junction is assumed to be 0.75 µm deep. The spacing near the diode ends is limited to a maxi-
mum of 0.1 µm:
x.mesh w =0.75 h.e=0.001 h.m =0.l ratio =1.5
x.mesh w =2.25 h.s=0.001 h.m =0.l ratio =1.5
The vertical mesh spacing of a MOSFET can generally be specified as uniform through the gate
oxide, very fine for the surface inversion layer, moderate down to the so source/drain junction
depth, and then increasing all the way to the bulk contact:
y. mesh loc = -0.04 node =1
y. mesh loc =0.0 node =6
y.mesh width =0.5 h. start =0.001 h. max =.05 ratio =2.0
y.mesh width =2.5 h. start =0.05 ratio =2.0
30.16.4 SEE ALSO
domain
540 CHAPTER 30. CIDER USER’S MANUAL
30.17 NUMD
Diode / two-terminal numerical models and elements
SYNOPSIS Model:
.MODEL model -name NUMD [ level ]
+ ...
SYNOPSIS Element:
DXXXXXXX nl n2 model - name [geometry ] [ temperature ] [initial - conditions ]
SYNOPSIS Output:
.SAVE [small - signal values]
30.17.1 DESCRIPTION
NUMD is the name for a diode numerical model. In addition, this same model can be used
to simulate other two-terminal structures such as semiconductor resistors and MOS capacitors.
See the options card for more information on how to customize the device type.
Both 1D and 2D devices are supported. These correspond to the LEVEL=l and LEVEL=2
models, respectively. If left unspecified, it is assumed that the device is one-dimensional.
All numerical two-terminal element names begin with the letter ‘D. The element name is then
followed by the names of the positive (n1) and negative (n2) nodes. After this must come the
name of the model used for the element. The remaining information can come in any order. The
layout dimensions of an element are specified relative to the geometry of a default device. For
1D devices, the default device has an area of 1m², and for 2D devices, the default device has
a width of 1 m. However, these defaults can be overridden on an options card. The operating
temperature of a device can be set independently from that of the rest of the circuit in order to
simulate non-isothermal circuit operation. Finally, the name of a file containing an initial state
for the device can be specified. Remember that if the filename contains capital letters, they
must be protected by surrounding the filename with double quotes. Alternatively, the device
can be placed in an OFF state (thermal equilibrium) at the beginning of the analysis. For more
information on the use of initial conditions, see the NGSPICE User’s Manual, Chapt. 7.1.
In addition to the element input parameters, there are output-only parameters that can be shown
using the NGSPICE show command (17.5.66) or captured using the save/.SAVE (17.5.57/15.6.1)
command. These parameters are the elements of the indefinite conductance (G), capacitance
(C), and admittance (Y) matrices where Y=G+jωC. By default, the parameters are compu-
ted at 1 Hz. Each element is accessed using the name of the matrix (g, c or y) followed by the
node indices of the output terminal and the input terminal (e.g. g11). Beware that names are
case-sensitive for save/show, so lower-case letters must be used.
30.17. NUMD 541
30.17.2 Parameters
Name Type Description
Level Integer Dimensionality of numerical model
Area Real Multiplicative area factor
W Real Multiplicative width factor
Temp Real Element operating temperature
IC.File String Initial-conditions filename
Off Flag Device initially in OFF state
gIJ Flag Conductance element Gi j, ( Ω)
cIJ Flag Capacitance element Ci j,(F)
yIJ Flag Admittance element Yi j, ( Ω)
30.17.3 EXAMPLES
A one-dimensional numerical switching-diode element/model pair with an area twice that of
the default device (which has a size of l µm x 1 µm) can be specified using:
DSWITCH 1 2 M _SW ITC H_D IOD E AREA =2
.MODEL M_SWITCH_DIODE NUMD
+ options defa =1 p ...
+ ...
A two-dimensional two-terminal MOS capacitor with a width of 20 µm and an initial condition
of 3 V is created by:
DMOSCAP 11 12 M_MOSCAP W =20um IC =3v
. MODEL M_MOSCAP NUMD LEVEL =2
+ options moscap defw =1 m
+ ...
The next example shows how both the width and area factors can be used to create a power
diode with area twice that of a 6µm-wide device (i.e. a 12µm-wide device). The device is
assumed to be operating at a temperature of 100°C:
D1 POSN NEGN POWERMOD AREA =2 W=6 um TEMP =100.0
. MODEL POWERMOD NUMD LEVEL =2
+ ...
This example saves all the small-signal parameters of the previous diode:
.SAVE @d1[g11 ] @d1[g12] @d1 [ g21] @d1 [g22]
.SAVE @d1[c11 ] @d1[c12] @d1 [ c21] @d1 [c22]
.SAVE @d1[y11 ] @d1[y12] @d1 [ y21] @d1 [y22]
542 CHAPTER 30. CIDER USER’S MANUAL
30.17.4 SEE ALSO
options, output
30.17.5 BUGS
Convergence problems may be experienced when simulating MOS capacitors due to singulari-
ties in the current-continuity equations.
30.18 NBJT
Bipolar / three-terminal numerical models and elements
SYNOPSIS Model:
.MODEL model -name NBJT [ level ]
+ ...
SYNOPSIS Element:
QXXXXXXX nl n2 n3 model - name [ geometry ]
+ [temperature ] [initial - conditions ]
SYNOPSIS Output:
.SAVE [small - signal values]
30.18.1 DESCRIPTION
NBJT is the name for a bipolar transistor numerical model. In addition, the 2D model can be
used to simulate other three-terminal structures such as a JFET or MESFET. However, the 1D
model is customized with a special base contact, and cannot be used for other purposes. See the
options card for more information on how to customize the device type and setup the 1D base
contact.
Both 1”and 2D devices are supported. These correspond to the LEVEL=l and models, respecti-
vely. If left unspecified, it is assumed that the device is one-dimensional.
All numerical three-terminal element names begin with the letter ’Q’. If the device is a bipolar
transistor, then the nodes are specified in the order: collector (nl), base (n2), emitter (n3). For
a JFET or MESFET, the node order is: drain (n1), gate (n2), source (n3). After this must come
the name of the model used for the element. The remaining information can come in any order.
The layout dimensions of an element are specified relative to the geometry of a default device.
For the 1D BJT, the default device has an area of lm², and for 2D devices, the default device has
a width of lm. In addition, it is assumed that the default 1D BJT has a base contact with area
equal to the emitter area, length of 1µm and a depth automatically determined from the device
doping profile. However, all these defaults can be overridden on an options card.
30.18. NBJT 543
The operating temperature of a device can be set independently from the rest of that of the circuit
in order to simulate non-isothermal circuit operation. Finally, the name of a file containing an
initial state for the device can be specified. Remember that if the filename contains capital
letters, they must be protected by surrounding the filename with double quotes. Alternatively,
the device can be placed in an OFF state (thermal equilibrium) at the beginning of the analysis.
For more information on the use of initial conditions, see the NGSPICE User’s Manual.
In addition to the element input parameters, there are output-only parameters that can be shown
using the SPICE show command or captured using the save/.SAVE command. These para-
meters are the elements of the indefinite conductance (G), capacitance (C), and admittance (Y)
matrices where Y=G+jωC. By default, the parameters are computed at 1Hz. Each element
is accessed using the name of the matrix (g, c or y) followed by the node indices of the output
terminal and the input terminal (e.g. g11). Beware that parameter names are case-sensitive for
save/show, so lower-case letters must be used.
30.18.2 Parameters
Name Type Description
Level Integer Dimensionality of numerical model
Area Real Multiplicative area factor
W Real Multiplicative width factor
Temp Real Element operating temperature
IC.File String Initial-conditions filename
Off Flag Device initially in OFF state
gIJ Flag Conductance element Gi j, ( Ω)
cIJ Flag Capacitance element Ci j,(F)
yIJ Flag Admittance element Yi j, ( Ω)
30.18.3 EXAMPLES
A one-dimensional numerical bipolar transistor with an emitter stripe 4 times as wide as the
default device is created using:
Q2 1 2 3 M_BJT AREA =4
This example saves the output conductance (go), transconductance (gm) and input conductance
(gpi) of the previous transistor in that order:
.SAVE @q2[g11 ] @q2[g12] @q2 [ g22]
The second example is for a two-dimensional JFET with a width of 5pm and initial conditions
obtained from file IC.jfet:
QJ1 11 12 13 M_JFET W=5um IC. FILE =" IC. jfet"
. MODEL M_JFET NBJT LEVEL =2
+ options jfet
+ ...
544 CHAPTER 30. CIDER USER’S MANUAL
A final example shows how to use symmetry to simulate half of a 2D BJT, avoiding having the
user double the area of each instance:
Q2 NC2 NB2 NE2 BJTMOD AREA =1
Q3 NC3 NB3 NE3 BJTMOD AREA =1
. MODEL BJTMOD NBJT LEVEL =2
+ options defw =2 um
+ * Define half of the device now
+ ...
30.18.4 SEE ALSO
options, output
30.18.5 BUGS
MESFETs cannot be simulated properly yet because Schottky contacts have not been imple-
mented.
30.19 NUMOS
MOSFET / four-terminal numerical models and elements
SYNOPSIS Model:
.MODEL model -name NUMOS [ level ]
+ ...
SYNOPSIS Element:
MXXXXXXX nl n2 n3 n4 model - name [ geometry ]
+ [temperature ] [initial - conditions ]
SYNOPSIS Output:
.SAVE [small - signal values]
30.19.1 DESCRIPTION
NUMOS is the name for a MOSFET numerical model. In addition, the 2D model can be used
to simulate other four-terminal structures such as integrated bipolar and JFET devices with
substrate contacts. However, silicon controlled rectifiers (SCRs) cannot be simulated because
of the snapback in the transfer characteristic. See the options card for more information on
how to customize the device type. The LEVEL parameter of two- and three-terminal devices is
30.19. NUMOS 545
not needed, because only 2D devices are supported. However, it will accepted and ignored if
provided.
All numerical four-terminal element names begin with the letter ‘M’. If the device is a MOSFET,
or JFET with a bulk contact, then the nodes are specified in the order: drain (n1), gate (n2),
source (n3), bulk (n4). If the device is a BJT, the node order is: collector (n1), base (n2),
emitter (n3), substrate (n4). After this must come the name of the model 1used for the element.
The remaining information can come in any order. The layout dimensions of an element are
specified relative to the geometry of a default device. The default device has a width of lm.
However, this default can be overridden on an options card. In addition, the element line will
accept a length parameter, L, but does not use it in any calculations. This is provided to enable
somewhat greater compatibility between numerical MOSFET models and the standard SPICE3
compact MOSFET models.
The operating temperature of a device can be set independently from that of the rest of the circuit
in order to simulate non-isothermal circuit operation. Finally, the name of a file containing an
initial state for the device can be specified. Remember that if the filename contains capital
letters, they must be protected by surrounding the filename with double quotes. Alternatively,
the device can be placed in an OFF state (thermal equilibrium) at the beginning of the analysis.
For more information on the use of initial conditions, see the NGSPICE User’s Manual.
In addition to the element input parameters, there are output-only parameters that can be shown
using the SPICE show command or captured using the save/.SAVE command.
These parameters are the elements of the indefinite conductance (G), capacitance (C), and ad-
mittance (Y) matrices where Y=G+jωC. By default, the parameters are computed at 1 Hz.
Each element is accessed using the name of the matrix (g, c or y) followed by the node indi-
ces of the output terminal and the input terminal (e.g. g11). Beware that parameter names are
case-sensitive for save/show, so lower-case letters must be used.
30.19.2 Parameters
Name Type Description
Level Integer Dimensionality of numerical model
Area Real Multiplicative area factor
W Real Multiplicative width factor
L Real Unused length factor
Temp Real Element operating temperature
IC.File String Initial-conditions filename
Off Flag Device initially in OFF state
gIJ Flag Conductance element Gi j, ( Ω)
cIJ Flag Capacitance element Ci j,(F)
yIJ Flag Admittance element Yi j, ( Ω)
30.19.3 EXAMPLES
A numerical MOSFET with a gate width of 5µm and length of 1µm is described below. Howe-
ver, the model can only be used for lµm length devices, so the length parameter is redundant.
The device is initially biased near its threshold by taking an initial state from the file NM1.vth.
546 CHAPTER 30. CIDER USER’S MANUAL
M1 1 2 3 4 M_NMOS_1UM W=5 um L=1um IC.FILE ="NM1. vth"
.MODEL MNMOS_1UM NUMOS
+ * Description of a lum device
+ ...
This example saves the definite admittance matrix of the previous MOSFET where the source
terminal (3) is used as the reference. (The definite admittance matrix is formed by deleting the
third row and column from the indefinite admittance matrix.)
.SAVE @m1[y11 ] @m1[y12] @ml [ y14]
.SAVE @m1[y21 ] @m1[y22] @ml [ y24]
.SAVE @m1[y41 ] @m1[y42] @ml [ y44]
Bipolar transistors are usually specified in terms of their area relative to a unit device. The
following example creates a unit-sized device:
MQ1 NC NB NE NS N_BJT
.MODEL M_BJT NUMOS LEVEL =2
+ options bipolar defw =5 um
+ ...
30.19.4 SEE ALSO
options, output
30.20 Cider examples
The original Cider User’s manual, in its Appendix A, lists a lot of examples, starting at page
226. We do not reproduce these pages here, but ask you to refer to the original document. If
you experience any difficulties downloading it, please send a note to the ngspice users’ mailing
list.
Part IV
Appendices
547
Chapter 31
Model and Device Parameters
The following tables summarize the parameters available on each of the devices and models in
ngspice. There are two tables for each type of device supported by ngspice. Input parameters
to instances and models are parameters that can occur on an instance or model definition line in
the form keyword=value where keyword is the parameter name as given in the tables. Default
input parameters (such as the resistance of a resistor or the capacitance of a capacitor) obviously
do not need the keyword specified.
31.1 Accessing internal device parameters
Output parameters are those additional parameters that are available for many types of instances
for the output of operating point and debugging information. These parameters are specified as
@device[keyword] and are available for the most recent point computed or, if specified in
a.save statement, for an entire simulation as a normal output vector. Thus, to monitor the
gate-to-source capacitance of a MOSFET, a command
save @m1 [ cgs]
given before a transient simulation causes the specified capacitance value to be saved at each
time-point, and a subsequent command such as
plot @m1 [ cgs]
produces the desired plot. (Note that the show command does not use this format).
Some variables are listed as both input and output, and their output simply returns the previously
input value, or the default value after the simulation has been run. Some parameters are input
only because the output system can not handle variables of the given type yet, or the need for
them as output variables has not been apparent. Many such input variables are available as
output variables in a different format, such as the initial condition vectors that can be retrieved
as individual initial condition values. Finally, internally derived values are output only and are
provided for debugging and operating point output purposes.
549
550 CHAPTER 31. MODEL AND DEVICE PARAMETERS
If you want to access a device parameter of a device used inside of a subcircuit, you may use
the syntax as shown below.
General form:
@de vice_i dentifi er . subc ircui t_na me .< su bcircuit_name_nn >
+. device_name [ parameter ]
Example input file:
* transistor output characteristics
* two nested subcircuits
vdd d1 0 2.0
vss vsss 0 0
vsig g1 vsss 0
xmos1 d1 g1 vsss level1
.subckt level1 d3 g3 v3
xmos2 d3 g3 v3 level2
.ends
.subckt level2 d4 g4 v4
m1 d4 g4 v4 v4 nmos w=1e -5 l=3.5e -007
.ends
.dc vdd 0 5 0.1 vsig 0 5 1
.control
save all @m.xmos1 . xmos2.m1[ vdsat ]
run
plot vss # branch $ current measured at the top level
plot @m.xmos1 . xmos2.m1[ vdsat ]
.endc
.MODEL NMOS NMOS LEVEL = 8
+VERSION = 3.2.4 TNOM = 27 TOX = 7.4E -9
.end
The device identifier is the first letter extracted from the device name, e.g. m for a MOS tran-
sistor.
Please note that the parameter tables presented below do not provide the detailed information
available about the parameters provided in the section on each device and model, but are provi-
ded as a quick reference guide.
31.2. ELEMENTARY DEVICES 551
31.2 Elementary Devices
31.2.1 Resistor
31.2.1.1 Resistor instance parameters
# Name Direction Type Description
1 resistance (r) InOut real Resistance
10 ac InOut real AC resistance value
8 temp InOut real Instance operating temperature
14 dtemp InOut real Instance temperature difference
with the rest of the circuit
3 l InOut real Length
2 w InOut real Width
12 m InOut real Multiplication factor
16 tc InOut real First order temp. coefficient
16 tc1 InOut real First order temp. coefficient
17 tc2 InOut real Second order temp. coefficient
13 scale InOut real Scale factor
15 noisy (noise) InOut integer Resistor generate noise
5 sens_resist In flag flag to request sensitivity WRT
resistance
6 i Out real Current
7 p Out real Power
206 sens_dc Out real dc sensitivity
201 sens_real Out real dc sensitivity and real part of ac
sensitivity
202 sens_imag Out real dc sensitivity and imag part of ac
sensitivity
203 sens_mag Out real ac sensitivity of magnitude
204 sens_ph Out real ac sensitivity of phase
205 sens_cplx Out complex ac sensitivity
552 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.2.1.2 Resistor model parameters
# Name Direction Type Description
103 rsh InOut real Sheet resistance
106 narrow InOut real Narrowing of resistor
106 dw InOut real
109 short InOut real Shortening of resistor
109 dlr InOut real
101 tc1 InOut real First order temp. coefficient
102 tc2 InOut real Second order temp. coefficient
104 defw InOut real Default device width
104 w InOut real Default device width
105 l InOut real Default device length
110 kf InOut real Flicker noise coefficient
111 af InOut real Flicker noise exponent
108 tnom InOut real Parameter measurement temperature
107 r InOut real Resistance
107 res InOut real Resistance
wf InOut real Flicker noise width exponent
lf InOut real Flicker noise length exponent
ef InOut real Flicker noise frequency exponent
r In flag Device is a resistor model
31.2. ELEMENTARY DEVICES 553
31.2.2 Capacitor - Fixed capacitor
31.2.2.1 Capacitor instance parameters
# Name Direction Type Description
1 capacitance InOut real Device capacitance
1 cap InOut real Device capacitance
1 c InOut real Device capacitance
2 ic InOut real Initial capacitor voltage
8 temp InOut real Instance operating temperature
9 dtemp InOut real Instance temperature difference
from the rest of the circuit
3 w InOut real Device width
4 l InOut real Device length
11 m InOut real Parallel multiplier
10 scale InOut real Scale factor
5 sens_cap In flag flag to request sens. WRT cap.
6 i Out real Device current
7 p Out real Instantaneous device power
206 sens_dc Out real dc sensitivity
201 sens_real Out real real part of ac sensitivity
202 sens_imag Out real dc sens. & imag part of ac sens.
203 sens_mag Out real sensitivity of ac magnitude
204 sens_ph Out real sensitivity of ac phase
205 sens_cplx Out complex ac sensitivity
31.2.2.2 Capacitor model parameters
# Name Direction Type Description
112 cap InOut real Model capacitance
101 cj InOut real Bottom Capacitance per area
102 cjsw InOut real Sidewall capacitance per meter
103 defw InOut real Default width
113 defl InOut real Default length
105 narrow InOut real width correction factor
106 short InOut real length correction factor
107 tc1 InOut real First order temp. coefficient
108 tc2 InOut real Second order temp. coefficient
109 tnom InOut real Parameter measurement temperature
110 di InOut real Relative dielectric constant
111 thick InOut real Insulator thickness
104 c In flag Capacitor model
554 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.2.3 Inductor - Fixed inductor
31.2.3.1 Inductor instance parameters
# Name Direction Type Description
1 inductance InOut real Inductance of inductor
2 ic InOut real Initial current through inductor
5 sens_ind In flag flag to request sensitivity WRT
inductance
9 temp InOut real Instance operating temperature
10 dtemp InOut real Instance temperature difference with the
rest of the circuit
8 m InOut real Multiplication Factor
11 scale InOut real Scale factor
12 nt InOut real Number of turns
3 flux Out real Flux through inductor
4 v Out real Terminal voltage of inductor
4 volt Out real
6 i Out real Current through the inductor
6 current Out real
7 p Out real instantaneous power dissipated by the
inductor
206 sens_dc Out real dc sensitivity sensitivity
201 sens_real Out real real part of ac sensitivity
202 sens_imag Out real dc sensitivity and imag part of ac
sensitivty
203 sens_mag Out real sensitivity of AC magnitude
204 sens_ph Out real sensitivity of AC phase
205 sens_cplx Out complex ac sensitivity
31.2.3.2 Inductor model parameters
# Name Direction Type Description
100 ind InOut real Model inductance
101 tc1 InOut real First order temp. coefficient
102 tc2 InOut real Second order temp. coefficient
103 tnom InOut real Parameter measurement temperature
104 csect InOut real Inductor cross section
105 length InOut real Inductor length
106 nt InOut real Model number of turns
107 mu InOut real Relative magnetic permeability
108 l In flag Inductor model
31.2. ELEMENTARY DEVICES 555
31.2.4 Mutual - Mutual Inductor
31.2.4.1 Mutual instance parameters
# Name Direction Type Description
401 k InOut real Mutual inductance
401 coefficient InOut real
402 inductor1 InOut instance First coupled inductor
403 inductor2 InOut instance Second coupled inductor
404 sens_coeff In flag flag to request sensitivity WRT coupling factor
606 sens_dc Out real dc sensitivity
601 sens_real Out real real part of ac sensitivity
602 sens_imag Out real dc sensitivity and imag part of ac sensitivty
603 sens_mag Out real sensitivity of AC magnitude
604 sens_ph Out real sensitivity of AC phase
605 sens_cplx Out complex mutual model parameters:
556 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.3 Voltage and current sources
31.3.1 ASRC - Arbitrary source
31.3.1.1 ASRC instance parameters
# Name Direction Type Description
2 i In parsetree Current source
1 v In parsetree Voltage source
7 i Out real Current through source
6 v Out real Voltage across source
3 pos_node Out integer Positive Node
4 neg_node Out integer Negative Node
31.3. VOLTAGE AND CURRENT SOURCES 557
31.3.2 Isource - Independent current source
31.3.2.1 Isource instance parameters
# Name Direction Type Description
1 dc InOut real DC value of source
2 acmag InOut real AC magnitude
3 acphase InOut real AC phase
5 pulse In real vector Pulse description
6 sine In real vector Sinusoidal source description
6 sin In real vector Sinusoidal source description
7 exp In real vector Exponential source description
8 pwl In real vector Piecewise linear description
9 sffm In real vector Single freq. FM description
21 am In real vector Amplitude modulation description
10 neg_node Out integer Negative node of source
11 pos_node Out integer Positive node of source
12 acreal Out real AC real part
13 acimag Out real AC imaginary part
14 function Out integer Function of the source
15 order Out integer Order of the source function
16 coeffs Out real vector Coefficients of the source
20 v Out real Voltage across the supply
17 p Out real Power supplied by the source
4 ac In real vector AC magnitude,phase vector
1 c In real Current through current source
22 current Out real Current in DC or Transient mode
18 distof1 In real vector f1 input for distortion
19 distof2 In real vector f2 input for distortion
558 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.3.3 Vsource - Independent voltage source
31.3.3.1 Vsource instance parameters
# Name Direction Type Description
1 dc InOut real D.C. source value
3 acmag InOut real A.C. Magnitude
4 acphase InOut real A.C. Phase
5 pulse In real vector Pulse description
6 sine In real vector Sinusoidal source description
6 sin In real vector Sinusoidal source description
7 exp In real vector Exponential source description
8 pwl In real vector Piecewise linear description
9 sffm In real vector Single freq. FM descripton
22 am In real vector Amplitude modulation descripton
16 pos_node Out integer Positive node of source
17 neg_node Out integer Negative node of source
11 function Out integer Function of the source
12 order Out integer Order of the source function
13 coeffs Out real vector Coefficients for the function
14 acreal Out real AC real part
15 acimag Out real AC imaginary part
2 ac In real vector AC magnitude, phase vector
18 i Out real Voltage source current
19 p Out real Instantaneous power
20 distof1 In real vector f1 input for distortion
21 distof2 In real vector f2 input for distortion
23 r In real pwl repeat start time value
24 td In real pwl delay time value
31.3. VOLTAGE AND CURRENT SOURCES 559
31.3.4 CCCS - Current controlled current source
31.3.4.1 CCCS instance parameters
# Name Direction Type Description
1 gain InOut real Gain of source
2 control InOut instance Name of controlling source
6 sens_gain In flag flag to request sensitivity WRT gain
4 neg_node Out integer Negative node of source
3 pos_node Out integer Positive node of source
7 i Out real CCCS output current
9 v Out real CCCS voltage at output
8 p Out real CCCS power
206 sens_dc Out real dc sensitivity
201 sens_real Out real real part of ac sensitivity
202 sens_imag Out real imag part of ac sensitivity
203 sens_mag Out real sensitivity of ac magnitude
204 sens_ph Out real sensitivity of ac phase
205 sens_cplx Out complex ac sensitivity
31.3.5 CCVS - Current controlled voltage source
31.3.5.1 CCVS instance parameters
# Name Direction Type Description
1 gain InOut real Transresistance (gain)
2 control InOut instance Controlling voltage source
7 sens_trans In flag flag to request sens. WRT transimpedance
3 pos_node Out integer Positive node of source
4 neg_node Out integer Negative node of source
8 i Out real CCVS output current
10 v Out real CCVS output voltage
9 p Out real CCVS power
206 sens_dc Out real dc sensitivity
201 sens_real Out real real part of ac sensitivity
202 sens_imag Out real imag part of ac sensitivity
203 sens_mag Out real sensitivity of ac magnitude
204 sens_ph Out real sensitivity of ac phase
205 sens_cplx Out complex ac sensitivity
560 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.3.6 VCCS - Voltage controlled current source
31.3.6.1 VCCS instance parameters
# Name Direction Type Description
1 gain InOut real Transconductance of source (gain)
8 sens_trans In flag flag to request sensitivity WRT transconductance
3 pos_node Out integer Positive node of source
4 neg_node Out integer Negative node of source
5 cont_p_node Out integer Positive node of contr. source
6 cont_n_node Out integer Negative node of contr. source
2 ic In real Initial condition of controlling source
9 i Out real Output current
11 v Out real Voltage across output
10 p Out real Power
206 sens_dc Out real dc sensitivity
201 sens_real Out real real part of ac sensitivity
202 sens_imag Out real imag part of ac sensitivity
203 sens_mag Out real sensitivity of ac magnitude
204 sens_ph Out real sensitivity of ac phase
205 sens_cplx Out complex ac sensitivity
31.3.7 VCVS - Voltage controlled voltage source
31.3.7.1 VCVS instance parameters
# Name Direction Type Description
1 gain InOut real Voltage gain
9 sens_gain In flag flag to request sensitivity WRT gain
2 pos_node Out integer Positive node of source
3 neg_node Out integer Negative node of source
4 cont_p_node Out integer Positive node of contr. source
5 cont_n_node Out integer Negative node of contr. source
7 ic In real Initial condition of controlling source
10 i Out real Output current
12 v Out real Output voltage
11 p Out real Power
206 sens_dc Out real dc sensitivity
201 sens_real Out real real part of ac sensitivity
202 sens_imag Out real imag part of ac sensitivity
203 sens_mag Out real sensitivity of ac magnitude
204 sens_ph Out real sensitivity of ac phase
205 sens_cplx Out complex ac sensitivity
31.4. TRANSMISSION LINES 561
31.4 Transmission Lines
31.4.1 CplLines - Simple Coupled Multiconductor Lines
31.4.1.1 CplLines instance parameters
# Name Direction Type Description
1 pos_nodes InOut string vector in nodes
2 neg_nodes InOut string vector out nodes
3 dimension InOut integer number of coupled lines
4 length InOut real length of lines
31.4.1.2 CplLines model parameters
# Name Direction Type Description
101 r InOut real vector resistance per length
104 l InOut real vector inductance per length
102 c InOut real vector capacitance per length
103 g InOut real vector conductance per length
105 length InOut real length
106 cpl In flag Device is a cpl model
562 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.4.2 LTRA - Lossy transmission line
31.4.2.1 LTRA instance parameters
# Name Direction Type Description
6 v1 InOut real Initial voltage at end 1
8 v2 InOut real Initial voltage at end 2
7 i1 InOut real Initial current at end 1
9 i2 InOut real Initial current at end 2
10 ic In real vector Initial condition vector:v1,i1,v2,i2
13 pos_node1 Out integer Positive node of end 1 of t-line
14 neg_node1 Out integer Negative node of end 1 of t.line
15 pos_node2 Out integer Positive node of end 2 of t-line
16 neg_node2 Out integer Negative node of end 2 of t-line
31.4.2.2 LTRA model parameters
# Name Direction Type Description
0 ltra InOut flag LTRA model
1 r InOut real Resistance per meter
2 l InOut real Inductance per meter
3 g InOut real
4 c InOut real Capacitance per meter
5 len InOut real length of line
11 rel Out real Rel. rate of change of deriv. for bkpt
12 abs Out real Abs. rate of change of deriv. for bkpt
28 nocontrol InOut flag No timestep control
32 steplimit InOut flag always limit timestep to 0.8*(delay of line)
33 nosteplimit InOut flag don’t always limit timestep to 0.8*(delay of
line)
34 lininterp InOut flag use linear interpolation
35 quadinterp InOut flag use quadratic interpolation
36 mixedinterp InOut flag use linear interpolation if quadratic results look
unacceptable
46 truncnr InOut flag use N-R iterations for step calculation in
LTRAtrunc
47 truncdontcut InOut flag don’t limit timestep to keep impulse response
calculation errors low
42 compactrel InOut real special reltol for straight line checking
43 compactabs InOut real special abstol for straight line checking
31.4. TRANSMISSION LINES 563
31.4.3 Tranline - Lossless transmission line
31.4.3.1 Tranline instance parameters
# Name Direction Type Description
1 z0 InOut real Characteristic impedance
1 zo InOut real
4 f InOut real Frequency
2 td InOut real Transmission delay
3 nl InOut real Normalized length at frequency given
5 v1 InOut real Initial voltage at end 1
7 v2 InOut real Initial voltage at end 2
6 i1 InOut real Initial current at end 1
8 i2 InOut real Initial current at end 2
9 ic In real vector Initial condition vector:v1,i1,v2,i2
10 rel Out real Rel. rate of change of deriv. for bkpt
11 abs Out real Abs. rate of change of deriv. for bkpt
12 pos_node1 Out integer Positive node of end 1 of t. line
13 neg_node1 Out integer Negative node of end 1 of t. line
14 pos_node2 Out integer Positive node of end 2 of t. line
15 neg_node2 Out integer Negative node of end 2 of t. line
18 delays Out real vector Delayed values of excitation
564 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.4.4 TransLine - Simple Lossy Transmission Line
31.4.4.1 TransLine instance parameters
# Name Direction Type Description
1 pos_node In integer Positive node of txl
2 neg_node In integer Negative node of txl
3 length InOut real length of line
31.4.4.2 TransLine model parameters
# Name Direction Type Description
101 r InOut real resistance per length
104 l InOut real inductance per length
102 c InOut real capacitance per length
103 g InOut real conductance per length
105 length InOut real length
106 txl In flag Device is a txl model
31.4. TRANSMISSION LINES 565
31.4.5 URC - Uniform R. C. line
31.4.5.1 URC instance parameters
# Name Direction Type Description
1 l InOut real Length of transmission line
2 n InOut real Number of lumps
3 pos_node Out integer Positive node of URC
4 neg_node Out integer Negative node of URC
5 gnd Out integer Ground node of URC
31.4.5.2 URC model parameters
# Name Direction Type Description
101 k InOut real Propagation constant
102 fmax InOut real Maximum frequency of interest
103 rperl InOut real Resistance per unit length
104 cperl InOut real Capacitance per unit length
105 isperl InOut real Saturation current per length
106 rsperl InOut real Diode resistance per length
107 urc In flag Uniform R.C. line model
566 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.5 BJTs
31.5.1 BJT - Bipolar Junction Transistor
31.5.1.1 BJT instance parameters
# Name Direction Type Description
2 off InOut flag Device initially off
3 icvbe InOut real Initial B-E voltage
4 icvce InOut real Initial C-E voltage
1 area InOut real (Emitter) Area factor
10 areab InOut real Base area factor
11 areac InOut real Collector area factor
9 m InOut real Parallel Multiplier
5 ic In real vector Initial condition vector
6 sens_area In flag flag to request sensitivity WRT area
202 colnode Out integer Number of collector node
203 basenode Out integer Number of base node
204 emitnode Out integer Number of emitter node
205 substnode Out integer Number of substrate node
206 colprimenode Out integer Internal collector node
207 baseprimenode Out integer Internal base node
208 emitprimenode Out integer Internal emitter node
211 ic Out real Current at collector node
212 ib Out real Current at base node
236 ie Out real Emitter current
237 is Out real Substrate current
209 vbe Out real B-E voltage
210 vbc Out real B-C voltage
215 gm Out real Small signal transconductance
213 gpi Out real Small signal input conductance - pi
214 gmu Out real Small signal conductance - mu
225 gx Out real Conductance from base to internal base
216 go Out real Small signal output conductance
227 geqcb Out real d(Ibe)/d(Vbc)
228 gccs Out real Internal C-S cap. equiv. cond.
229 geqbx Out real Internal C-B-base cap. equiv. cond.
239 cpi Out real Internal base to emitter capactance
240 cmu Out real Internal base to collector capactiance
241 cbx Out real Base to collector capacitance
242 ccs Out real Collector to substrate capacitance
218 cqbe Out real Cap. due to charge storage in B-E jct.
220 cqbc Out real Cap. due to charge storage in B-C jct.
222 cqcs Out real Cap. due to charge storage in C-S jct.
224 cqbx Out real Cap. due to charge storage in B-X jct.
226 cexbc Out real Total Capacitance in B-X junction
31.5. BJTS 567
217 qbe Out real Charge storage B-E junction
219 qbc Out real Charge storage B-C junction
221 qcs Out real Charge storage C-S junction
223 qbx Out real Charge storage B-X junction
238 p Out real Power dissipation
235 sens_dc Out real dc sensitivity
230 sens_real Out real real part of ac sensitivity
231 sens_imag Out real dc sens. & imag part of ac sens.
232 sens_mag Out real sensitivity of ac magnitude
233 sens_ph Out real sensitivity of ac phase
234 sens_cplx Out complex ac sensitivity
7 temp InOut real instance temperature
8 dtemp InOut real instance temperature delta from circuit
31.5.1.2 BJT model parameters
# Name Direction Type Description
309 type Out string NPN or PNP
101 npn InOut flag NPN type device
102 pnp InOut flag PNP type device
103 is InOut real Saturation Current
104 bf InOut real Ideal forward beta
105 nf InOut real Forward emission coefficient
106 vaf InOut real Forward Early voltage
106 va InOut real
107 ikf InOut real Forward beta roll-off corner current
107 ik InOut real
108 ise InOut real B-E leakage saturation current
110 ne InOut real B-E leakage emission coefficient
111 br InOut real Ideal reverse beta
112 nr InOut real Reverse emission coefficient
113 var InOut real Reverse Early voltage
113 vb InOut real
114 ikr InOut real reverse beta roll-off corner current
115 isc InOut real B-C leakage saturation current
117 nc InOut real B-C leakage emission coefficient
118 rb InOut real Zero bias base resistance
119 irb InOut real Current for base resistance=(rb+rbm)/2
120 rbm InOut real Minimum base resistance
121 re InOut real Emitter resistance
122 rc InOut real Collector resistance
123 cje InOut real Zero bias B-E depletion capacitance
124 vje InOut real B-E built in potential
124 pe InOut real
125 mje InOut real B-E junction grading coefficient
125 me InOut real
568 CHAPTER 31. MODEL AND DEVICE PARAMETERS
126 tf InOut real Ideal forward transit time
127 xtf InOut real Coefficient for bias dependence of TF
128 vtf InOut real Voltage giving VBC dependence of TF
129 itf InOut real High current dependence of TF
130 ptf InOut real Excess phase
131 cjc InOut real Zero bias B-C depletion capacitance
132 vjc InOut real B-C built in potential
132 pc InOut real
133 mjc InOut real B-C junction grading coefficient
133 mc InOut real
134 xcjc InOut real Fraction of B-C cap to internal base
135 tr InOut real Ideal reverse transit time
136 cjs InOut real Zero bias C-S capacitance
136 ccs InOut real Zero bias C-S capacitance
137 vjs InOut real Substrate junction built in potential
137 ps InOut real
138 mjs InOut real Substrate junction grading coefficient
138 ms InOut real
139 xtb InOut real Forward and reverse beta temp. exp.
140 eg InOut real Energy gap for IS temp. dependency
141 xti InOut real Temp. exponent for IS
142 fc InOut real Forward bias junction fit parameter
301 invearlyvoltf Out real Inverse early voltage:forward
302 invearlyvoltr Out real Inverse early voltage:reverse
303 invrollofff Out real Inverse roll off - forward
304 invrolloffr Out real Inverse roll off - reverse
305 collectorconduct Out real Collector conductance
306 emitterconduct Out real Emitter conductance
307 transtimevbcfact Out real Transit time VBC factor
308 excessphasefactor Out real Excess phase fact.
143 tnom InOut real Parameter measurement temperature
145 kf InOut real Flicker Noise Coefficient
144 af InOut real Flicker Noise Exponent
31.5. BJTS 569
31.5.2 BJT - Bipolar Junction Transistor Level 2
31.5.2.1 BJT2 instance parameters
# Name Direction Type Description
2 off InOut flag Device initially off
3 icvbe InOut real Initial B-E voltage
4 icvce InOut real Initial C-E voltage
1 area InOut real (Emitter) Area factor
10 areab InOut real Base area factor
11 areac InOut real Collector area factor
9 m InOut real Parallel Multiplier
5 ic In real vector Initial condition vector
6 sens_area In flag flag to request sensitivity WRT area
202 colnode Out integer Number of collector node
203 basenode Out integer Number of base node
204 emitnode Out integer Number of emitter node
205 substnode Out integer Number of substrate node
206 colprimenode Out integer Internal collector node
207 baseprimenode Out integer Internal base node
208 emitprimenode Out integer Internal emitter node
211 ic Out real Current at collector node
212 ib Out real Current at base node
236 ie Out real Emitter current
237 is Out real Substrate current
209 vbe Out real B-E voltage
210 vbc Out real B-C voltage
215 gm Out real Small signal transconductance
213 gpi Out real Small signal input conductance - pi
214 gmu Out real Small signal conductance - mu
225 gx Out real Conductance from base to internal base
216 go Out real Small signal output conductance
227 geqcb Out real d(Ibe)/d(Vbc)
228 gcsub Out real Internal Subs. cap. equiv. cond.
243 gdsub Out real Internal Subs. Diode equiv. cond.
229 geqbx Out real Internal C-B-base cap. equiv. cond.
239 cpi Out real Internal base to emitter capactance
240 cmu Out real Internal base to collector capactiance
241 cbx Out real Base to collector capacitance
242 csub Out real Substrate capacitance
218 cqbe Out real Cap. due to charge storage in B-E jct.
220 cqbc Out real Cap. due to charge storage in B-C jct.
222 cqsub Out real Cap. due to charge storage in Subs. jct.
224 cqbx Out real Cap. due to charge storage in B-X jct.
226 cexbc Out real Total Capacitance in B-X junction
217 qbe Out real Charge storage B-E junction
219 qbc Out real Charge storage B-C junction
570 CHAPTER 31. MODEL AND DEVICE PARAMETERS
221 qsub Out real Charge storage Subs. junction
223 qbx Out real Charge storage B-X junction
238 p Out real Power dissipation
235 sens_dc Out real dc sensitivity
230 sens_real Out real real part of ac sensitivity
231 sens_imag Out real dc sens. & imag part of ac sens.
232 sens_mag Out real sensitivity of ac magnitude
233 sens_ph Out real sensitivity of ac phase
234 sens_cplx Out complex ac sensitivity
7 temp InOut real instance temperature
8 dtemp InOut real instance temperature delta from circuit
31.5.2.2 BJT2 model parameters
# Name Direction Type Description
309 type Out string NPN or PNP
101 npn InOut flag NPN type device
102 pnp InOut flag PNP type device
147 subs InOut integer Vertical or Lateral device
103 is InOut real Saturation Current
146 iss InOut real Substrate Jct. Saturation Current
104 bf InOut real Ideal forward beta
105 nf InOut real Forward emission coefficient
106 vaf InOut real Forward Early voltage
106 va InOut real
107 ikf InOut real Forward beta roll-off corner current
107 ik InOut real
108 ise InOut real B-E leakage saturation current
110 ne InOut real B-E leakage emission coefficient
111 br InOut real Ideal reverse beta
112 nr InOut real Reverse emission coefficient
113 var InOut real Reverse Early voltage
113 vb InOut real
114 ikr InOut real reverse beta roll-off corner current
115 isc InOut real B-C leakage saturation current
117 nc InOut real B-C leakage emission coefficient
118 rb InOut real Zero bias base resistance
119 irb InOut real Current for base resistance=(rb+rbm)/2
120 rbm InOut real Minimum base resistance
121 re InOut real Emitter resistance
122 rc InOut real Collector resistance
123 cje InOut real Zero bias B-E depletion capacitance
124 vje InOut real B-E built in potential
124 pe InOut real
125 mje InOut real B-E junction grading coefficient
125 me InOut real
31.5. BJTS 571
126 tf InOut real Ideal forward transit time
127 xtf InOut real Coefficient for bias dependence of TF
128 vtf InOut real Voltage giving VBC dependence of TF
129 itf InOut real High current dependence of TF
130 ptf InOut real Excess phase
131 cjc InOut real Zero bias B-C depletion capacitance
132 vjc InOut real B-C built in potential
132 pc InOut real
133 mjc InOut real B-C junction grading coefficient
133 mc InOut real
134 xcjc InOut real Fraction of B-C cap to internal base
135 tr InOut real Ideal reverse transit time
136 cjs InOut real Zero bias Substrate capacitance
136 csub InOut real
137 vjs InOut real Substrate junction built in potential
137 ps InOut real
138 mjs InOut real Substrate junction grading coefficient
138 ms InOut real
139 xtb InOut real Forward and reverse beta temp. exp.
140 eg InOut real Energy gap for IS temp. dependency
141 xti InOut real Temp. exponent for IS
148 tre1 InOut real Temp. coefficient 1 for RE
149 tre2 InOut real Temp. coefficient 2 for RE
150 trc1 InOut real Temp. coefficient 1 for RC
151 trc2 InOut real Temp. coefficient 2 for RC
152 trb1 InOut real Temp. coefficient 1 for RB
153 trb2 InOut real Temp. coefficient 2 for RB
154 trbm1 InOut real Temp. coefficient 1 for RBM
155 trbm2 InOut real Temp. coefficient 2 for RBM
142 fc InOut real Forward bias junction fit parameter
301 invearlyvoltf Out real Inverse early voltage:forward
302 invearlyvoltr Out real Inverse early voltage:reverse
303 invrollofff Out real Inverse roll off - forward
304 invrolloffr Out real Inverse roll off - reverse
305 collectorconduct Out real Collector conductance
306 emitterconduct Out real Emitter conductance
307 transtimevbcfact Out real Transit time VBC factor
308 excessphasefactor Out real Excess phase fact.
143 tnom InOut real Parameter measurement temperature
145 kf InOut real Flicker Noise Coefficient
144 af InOut real Flicker Noise Exponent
572 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.5.3 VBIC - Vertical Bipolar Inter-Company Model
31.5.3.1 VBIC instance parameters
# Name Direction Type Description
1 area InOut real Area factor
2 off InOut flag Device initially off
3 ic In real vector Initial condition vector
4 icvbe InOut real Initial B-E voltage
5 icvce InOut real Initial C-E voltage
6 temp InOut real Instance temperature
7 dtemp InOut real Instance delta temperature
8 m InOut real Multiplier
212 collnode Out integer Number of collector node
213 basenode Out integer Number of base node
214 emitnode Out integer Number of emitter node
215 subsnode Out integer Number of substrate node
216 collCXnode Out integer Internal collector node
217 collCInode Out integer Internal collector node
218 baseBXnode Out integer Internal base node
219 baseBInode Out integer Internal base node
220 baseBPnode Out integer Internal base node
221 emitEInode Out integer Internal emitter node
222 subsSInode Out integer Internal substrate node
223 vbe Out real B-E voltage
224 vbc Out real B-C voltage
225 ic Out real Collector current
226 ib Out real Base current
227 ie Out real Emitter current
228 is Out real Substrate current
229 gm Out real Small signal transconductance dIc/dVbe
230 go Out real Small signal output conductance dIc/dVbc
231 gpi Out real Small signal input conductance dIb/dVbe
232 gmu Out real Small signal conductance dIb/dVbc
233 gx Out real Conductance from base to internal base
247 cbe Out real Internal base to emitter capacitance
248 cbex Out real External base to emitter capacitance
249 cbc Out real Internal base to collector capacitance
250 cbcx Out real External Base to collector capacitance
251 cbep Out real Parasitic Base to emitter capacitance
252 cbcp Out real Parasitic Base to collector capacitance
259 p Out real Power dissipation
243 geqcb Out real Internal C-B-base cap. equiv. cond.
246 geqbx Out real External C-B-base cap. equiv. cond.
234 qbe Out real Charge storage B-E junction
235 cqbe Out real Cap. due to charge storage in B-E jct.
236 qbc Out real Charge storage B-C junction
31.5. BJTS 573
237 cqbc Out real Cap. due to charge storage in B-C jct.
238 qbx Out real Charge storage B-X junction
239 cqbx Out real Cap. due to charge storage in B-X jct.
258 sens_dc Out real DC sensitivity
253 sens_real Out real Real part of AC sensitivity
254 sens_imag Out real DC sens. & imag part of AC sens.
255 sens_mag Out real Sensitivity of AC magnitude
256 sens_ph Out real Sensitivity of AC phase
257 sens_cplx Out complex AC sensitivity
31.5.3.2 VBIC model parameters
# Name Direction Type Description
305 type Out string NPN or PNP
101 npn InOut flag NPN type device
102 pnp InOut flag PNP type device
103 tnom (tref) InOut real Parameter measurement temperature
104 rcx InOut real Extrinsic coll resistance
105 rci InOut real Intrinsic coll resistance
106 vo InOut real Epi drift saturation voltage
107 gamm InOut real Epi doping parameter
108 hrcf InOut real High current RC factor
109 rbx InOut real Extrinsic base resistance
110 rbi InOut real Intrinsic base resistance
111 re InOut real Intrinsic emitter resistance
112 rs InOut real Intrinsic substrate resistance
113 rbp InOut real Parasitic base resistance
114 is InOut real Transport saturation current
115 nf InOut real Forward emission coefficient
116 nr InOut real Reverse emission coefficient
117 fc InOut real Fwd bias depletion capacitance limit
118 cbeo InOut real Extrinsic B-E overlap capacitance
119 cje InOut real Zero bias B-E depletion capacitance
120 pe InOut real B-E built in potential
121 me InOut real B-E junction grading coefficient
122 aje InOut real B-E capacitance smoothing factor
123 cbco InOut real Extrinsic B-C overlap capacitance
124 cjc InOut real Zero bias B-C depletion capacitance
125 qco InOut real Epi charge parameter
126 cjep InOut real B-C extrinsic zero bias capacitance
127 pc InOut real B-C built in potential
128 mc InOut real B-C junction grading coefficient
129 ajc InOut real B-C capacitance smoothing factor
130 cjcp InOut real Zero bias S-C capacitance
131 ps InOut real S-C junction built in potential
132 ms InOut real S-C junction grading coefficient
574 CHAPTER 31. MODEL AND DEVICE PARAMETERS
133 ajs InOut real S-C capacitance smoothing factor
134 ibei InOut real Ideal B-E saturation current
135 wbe InOut real Portion of IBEI from Vbei, 1-WBE from Vbex
136 nei InOut real Ideal B-E emission coefficient
137 iben InOut real Non-ideal B-E saturation current
138 nen InOut real Non-ideal B-E emission coefficient
139 ibci InOut real Ideal B-C saturation current
140 nci InOut real Ideal B-C emission coefficient
141 ibcn InOut real Non-ideal B-C saturation current
142 ncn InOut real Non-ideal B-C emission coefficient
143 avc1 InOut real B-C weak avalanche parameter 1
144 avc2 InOut real B-C weak avalanche parameter 2
145 isp InOut real Parasitic transport saturation current
146 wsp InOut real Portion of ICCP
147 nfp InOut real Parasitic fwd emission coefficient
148 ibeip InOut real Ideal parasitic B-E saturation current
149 ibenp InOut real Non-ideal parasitic B-E saturation current
150 ibcip InOut real Ideal parasitic B-C saturation current
151 ncip InOut real Ideal parasitic B-C emission coefficient
152 ibcnp InOut real Nonideal parasitic B-C saturation current
153 ncnp InOut real Nonideal parasitic B-C emission coefficient
154 vef InOut real Forward Early voltage
155 ver InOut real Reverse Early voltage
156 ikf InOut real Forward knee current
157 ikr InOut real Reverse knee current
158 ikp InOut real Parasitic knee current
159 tf InOut real Ideal forward transit time
160 qtf InOut real Variation of TF with base-width modulation
161 xtf InOut real Coefficient for bias dependence of TF
162 vtf InOut real Voltage giving VBC dependence of TF
163 itf InOut real High current dependence of TF
164 tr InOut real Ideal reverse transit time
165 td InOut real Forward excess-phase delay time
166 kfn InOut real B-E Flicker Noise Coefficient
167 afn InOut real B-E Flicker Noise Exponent
168 bfn InOut real B-E Flicker Noise 1/f dependence
169 xre InOut real Temperature exponent of RE
170 xrb InOut real Temperature exponent of RB
171 xrbi InOut real Temperature exponent of RBI
172 xrc InOut real Temperature exponent of RC
173 xrci InOut real Temperature exponent of RCI
174 xrs InOut real Temperature exponent of RS
175 xvo InOut real Temperature exponent of VO
176 ea InOut real Activation energy for IS
177 eaie InOut real Activation energy for IBEI
179 eaic InOut real Activation energy for IBCI/IBEIP
31.5. BJTS 575
179 eais InOut real Activation energy for IBCIP
180 eane InOut real Activation energy for IBEN
181 eanc InOut real Activation energy for IBCN/IBENP
182 eans InOut real Activation energy for IBCNP
183 xis InOut real Temperature exponent of IS
184 xii InOut real Temperature exponent of IBEI,IBCI,IBEIP,IBCIP
185 xin InOut real Temperature exponent of IBEN,IBCN,IBENP,IBCNP
186 tnf InOut real Temperature exponent of NF
187 tavc InOut real Temperature exponent of AVC2
188 rth InOut real Thermal resistance
189 cth InOut real Thermal capacitance
190 vrt InOut real Punch-through voltage of internal B-C junction
191 art InOut real Smoothing parameter for reach-through
192 ccso InOut real Fixed C-S capacitance
193 qbm InOut real Select SGP qb formulation
194 nkf InOut real High current beta rolloff
195 xikf InOut real Temperature exponent of IKF
196 xrcx InOut real Temperature exponent of RCX
197 xrbx InOut real Temperature exponent of RBX
198 xrbp InOut real Temperature exponent of RBP
199 isrr InOut real Separate IS for fwd and rev
200 xisr InOut real Temperature exponent of ISR
201 dear InOut real Delta activation energy for ISRR
202 eap InOut real Exitivation energy for ISP
203 vbbe InOut real B-E breakdown voltage
204 nbbe InOut real B-E breakdown emission coefficient
205 ibbe InOut real B-E breakdown current
206 tvbbe1 InOut real Linear temperature coefficient of VBBE
207 tvbbe2 InOut real Quadratic temperature coefficient of VBBE
208 tnbbe InOut real Temperature coefficient of NBBE
209 ebbe InOut real exp(-VBBE/(NBBE*Vtv))
210 dtemp InOut real Locale Temperature difference
211 vers InOut real Revision Version
212 vref InOut real Reference Version
576 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.6 MOSFETs
31.6.1 MOS1 - Level 1 MOSFET model with Meyer capacitance model
31.6.1.1 MOS1 instance parameters
# Name Direction Type Description
21 m InOut real Multiplier
2 l InOut real Length
1 w InOut real Width
4 ad InOut real Drain area
3 as InOut real Source area
6 pd InOut real Drain perimeter
5 ps InOut real Source perimeter
8 nrd InOut real Drain squares
7 nrs InOut real Source squares
9 off In flag Device initially off
12 icvds InOut real Initial D-S voltage
13 icvgs InOut real Initial G-S voltage
11 icvbs InOut real Initial B-S voltage
20 temp InOut real Instance temperature
22 dtemp InOut real Instance temperature difference
10 ic In real vector Vector of D-S, G-S, B-S voltages
15 sens_l In flag flag to request sensitivity WRT length
14 sens_w In flag flag to request sensitivity WRT width
215 id Out real Drain current
18 is Out real Source current
17 ig Out real Gate current
16 ib Out real Bulk current
217 ibd Out real B-D junction current
216 ibs Out real B-S junction current
231 vgs Out real Gate-Source voltage
232 vds Out real Drain-Source voltage
230 vbs Out real Bulk-Source voltage
229 vbd Out real Bulk-Drain voltage
203 dnode Out integer Number of the drain node
204 gnode Out integer Number of the gate node
205 snode Out integer Number of the source node
206 bnode Out integer Number of the node
207 dnodeprime Out integer Number of int. drain node
208 snodeprime Out integer Number of int. source node
211 von Out real
212 vdsat Out real Saturation drain voltage
213 sourcevcrit Out real Critical source voltage
214 drainvcrit Out real Critical drain voltage
# Name Direction Type Description
31.6. MOSFETS 577
# Name Direction Type Description
258 rs Out real Source resistance
209 sourceconductance Out real Conductance of source
259 rd Out real Drain conductance
210 drainconductance Out real Conductance of drain
219 gm Out real Transconductance
220 gds Out real Drain-Source conductance
218 gmb Out real Bulk-Source transconductance
218 gmbs Out real
221 gbd Out real Bulk-Drain conductance
222 gbs Out real Bulk-Source conductance
223 cbd Out real Bulk-Drain capacitance
224 cbs Out real Bulk-Source capacitance
233 cgs Out real Gate-Source capacitance
236 cgd Out real Gate-Drain capacitance
239 cgb Out real Gate-Bulk capacitance
235 cqgs Out real Capacitance due to gate-source charge storage
238 cqgd Out real Capacitance due to gate-drain charge storage
241 cqgb Out real Capacitance due to gate-bulk charge storage
243 cqbd Out real Capacitance due to bulk-drain charge storage
245 cqbs Out real Capacitance due to bulk-source charge storage
225 cbd0 Out real Zero-Bias B-D junction capacitance
226 cbdsw0 Out real
227 cbs0 Out real Zero-Bias B-S junction capacitance
228 cbssw0 Out real
234 qgs Out real Gate-Source charge storage
237 qgd Out real Gate-Drain charge storage
240 qgb Out real Gate-Bulk charge storage
242 qbd Out real Bulk-Drain charge storage
244 qbs Out real Bulk-Source charge storage
19 p Out real Instaneous power
256 sens_l_dc Out real dc sensitivity wrt length
246 sens_l_real Out real real part of ac sensitivity wrt length
247 sens_l_imag Out real imag part of ac sensitivity wrt length
248 sens_l_mag Out real sensitivity wrt l of ac magnitude
249 sens_l_ph Out real sensitivity wrt l of ac phase
250 sens_l_cplx Out complex ac sensitivity wrt length
257 sens_w_dc Out real dc sensitivity wrt width
251 sens_w_real Out real real part of ac sensitivity wrt width
252 sens_w_imag Out real imag part of ac sensitivity wrt width
253 sens_w_mag Out real sensitivity wrt w of ac magnitude
254 sens_w_ph Out real sensitivity wrt w of ac phase
255 sens_w_cplx Out complex ac sensitivity wrt width
# Name Direction Type Description
31.6.1.2 MOS1 model parameters
578 CHAPTER 31. MODEL AND DEVICE PARAMETERS
# Name Direction Type Description
133 type Out string N-channel or P-channel MOS
101 vto InOut real Threshold voltage
101 vt0 InOut real
102 kp InOut real Transconductance parameter
103 gamma InOut real Bulk threshold parameter
104 phi InOut real Surface potential
105 lambda InOut real Channel length modulation
106 rd InOut real Drain ohmic resistance
107 rs InOut real Source ohmic resistance
108 cbd InOut real B-D junction capacitance
109 cbs InOut real B-S junction capacitance
110 is InOut real Bulk junction sat. current
111 pb InOut real Bulk junction potential
112 cgso InOut real Gate-source overlap cap.
113 cgdo InOut real Gate-drain overlap cap.
114 cgbo InOut real Gate-bulk overlap cap.
122 rsh InOut real Sheet resistance
115 cj InOut real Bottom junction cap per area
116 mj InOut real Bottom grading coefficient
117 cjsw InOut real Side junction cap per area
118 mjsw InOut real Side grading coefficient
119 js InOut real Bulk jct. sat. current density
120 tox InOut real Oxide thickness
121 ld InOut real Lateral diffusion
123 u0 InOut real Surface mobility
123 uo InOut real
124 fc InOut real Forward bias jct. fit parm.
128 nmos In flag N type MOSfet model
129 pmos In flag P type MOSfet model
125 nsub InOut real Substrate doping
126 tpg InOut integer Gate type
127 nss InOut real Surface state density
130 tnom InOut real Parameter measurement temperature
131 kf InOut real Flicker noise coefficient
132 af InOut real Flicker noise exponent
31.6. MOSFETS 579
31.6.2 MOS2 - Level 2 MOSFET model with Meyer capacitance model
31.6.2.1 MOS 2 instance parameters
# Name Direction Type Description
80 m InOut real Multiplier
2 l InOut real Length
1 w InOut real Width
4 ad InOut real Drain area
3 as InOut real Source area
6 pd InOut real Drain perimeter
5 ps InOut real Source perimeter
34 id Out real Drain current
34 cd Out real
36 ibd Out real B-D junction current
35 ibs Out real B-S junction current
18 is Out real Source current
17 ig Out real Gate current
16 ib Out real Bulk current
50 vgs Out real Gate-Source voltage
51 vds Out real Drain-Source voltage
49 vbs Out real Bulk-Source voltage
48 vbd Out real Bulk-Drain voltage
8 nrd InOut real Drain squares
7 nrs InOut real Source squares
9 off In flag Device initially off
12 icvds InOut real Initial D-S voltage
13 icvgs InOut real Initial G-S voltage
11 icvbs InOut real Initial B-S voltage
77 temp InOut real Instance operating temperature
81 dtemp InOut real Instance temperature difference
10 ic In real vector Vector of D-S, G-S, B-S voltages
15 sens_l In flag flag to request sensitivity WRT
length
14 sens_w In flag flag to request sensitivity WRT
width
22 dnode Out integer Number of drain node
23 gnode Out integer Number of gate node
24 snode Out integer Number of source node
25 bnode Out integer Number of bulk node
26 dnodeprime Out integer Number of internal drain node
27 snodeprime Out integer Number of internal source node
30 von Out real
31 vdsat Out real Saturation drain voltage
32 sourcevcrit Out real Critical source voltage
33 drainvcrit Out real Critical drain voltage
78 rs Out real Source resistance
580 CHAPTER 31. MODEL AND DEVICE PARAMETERS
28 sourceconductance Out real Source conductance
79 rd Out real Drain resistance
29 drainconductance Out real Drain conductance
38 gm Out real Transconductance
39 gds Out real Drain-Source conductance
37 gmb Out real Bulk-Source transconductance
37 gmbs Out real
40 gbd Out real Bulk-Drain conductance
41 gbs Out real Bulk-Source conductance
42 cbd Out real Bulk-Drain capacitance
43 cbs Out real Bulk-Source capacitance
52 cgs Out real Gate-Source capacitance
55 cgd Out real Gate-Drain capacitance
58 cgb Out real Gate-Bulk capacitance
44 cbd0 Out real Zero-Bias B-D junction
capacitance
45 cbdsw0 Out real
46 cbs0 Out real Zero-Bias B-S junction capacitance
47 cbssw0 Out real
54 cqgs Out real Capacitance due to gate-source
charge storage
57 cqgd Out real Capacitance due to gate-drain
charge storage
60 cqgb Out real Capacitance due to gate-bulk
charge storage
62 cqbd Out real Capacitance due to bulk-drain
charge storage
64 cqbs Out real Capacitance due to bulk-source
charge storage
53 qgs Out real Gate-Source charge storage
56 qgd Out real Gate-Drain charge storage
59 qgb Out real Gate-Bulk charge storage
61 qbd Out real Bulk-Drain charge storage
63 qbs Out real Bulk-Source charge storage
19 p Out real Instantaneous power
75 sens_l_dc Out real dc sensitivity wrt length
70 sens_l_real Out real real part of ac sensitivity wrt length
71 sens_l_imag Out real imag part of ac sensitivity wrt
length
74 sens_l_cplx Out complex ac sensitivity wrt length
72 sens_l_mag Out real sensitivity wrt l of ac magnitude
73 sens_l_ph Out real sensitivity wrt l of ac phase
76 sens_w_dc Out real dc sensitivity wrt width
65 sens_w_real Out real dc sensitivity and real part of ac
sensitivity wrt width
31.6. MOSFETS 581
66 sens_w_imag Out real imag part of ac sensitivity wrt
width
67 sens_w_mag Out real sensitivity wrt w of ac magnitude
68 sens_w_ph Out real sensitivity wrt w of ac phase
69 sens_w_cplx Out complex ac sensitivity wrt width
31.6.2.2 MOS2 model parameters
# Name Direction Type Description
141 type Out string N-channel or P-channel MOS
101 vto InOut real Threshold voltage
101 vt0 InOut real
102 kp InOut real Transconductance parameter
103 gamma InOut real Bulk threshold parameter
104 phi InOut real Surface potential
105 lambda InOut real Channel length modulation
106 rd InOut real Drain ohmic resistance
107 rs InOut real Source ohmic resistance
108 cbd InOut real B-D junction capacitance
109 cbs InOut real B-S junction capacitance
110 is InOut real Bulk junction sat. current
111 pb InOut real Bulk junction potential
112 cgso InOut real Gate-source overlap cap.
113 cgdo InOut real Gate-drain overlap cap.
114 cgbo InOut real Gate-bulk overlap cap.
122 rsh InOut real Sheet resistance
115 cj InOut real Bottom junction cap per area
116 mj InOut real Bottom grading coefficient
117 cjsw InOut real Side junction cap per area
118 mjsw InOut real Side grading coefficient
119 js InOut real Bulk jct. sat. current density
120 tox InOut real Oxide thickness
121 ld InOut real Lateral diffusion
123 u0 InOut real Surface mobility
123 uo InOut real
124 fc InOut real Forward bias jct. fit parm.
135 nmos In flag N type MOSfet model
136 pmos In flag P type MOSfet model
125 nsub InOut real Substrate doping
126 tpg InOut integer Gate type
127 nss InOut real Surface state density
129 delta InOut real Width effect on threshold
130 uexp InOut real Crit. field exp for mob. deg.
134 ucrit InOut real Crit. field for mob. degradation
131 vmax InOut real Maximum carrier drift velocity
132 xj InOut real Junction depth
582 CHAPTER 31. MODEL AND DEVICE PARAMETERS
133 neff InOut real Total channel charge coeff.
128 nfs InOut real Fast surface state density
137 tnom InOut real Parameter measurement temperature
139 kf InOut real Flicker noise coefficient
140 af InOut real Flicker noise exponent
31.6. MOSFETS 583
31.6.3 MOS3 - Level 3 MOSFET model with Meyer capacitance model
31.6.3.1 MOS3 instance parameters
# Name Direction Type Description
80 m InOut real Multiplier
2 l InOut real Length
1 w InOut real Width
4 ad InOut real Drain area
3 as InOut real Source area
6 pd InOut real Drain perimeter
5 ps InOut real Source perimeter
34 id Out real Drain current
34 cd Out real Drain current
36 ibd Out real B-D junction current
35 ibs Out real B-S junction current
18 is Out real Source current
17 ig Out real Gate current
16 ib Out real Bulk current
50 vgs Out real Gate-Source voltage
51 vds Out real Drain-Source voltage
49 vbs Out real Bulk-Source voltage
48 vbd Out real Bulk-Drain voltage
8 nrd InOut real Drain squares
7 nrs InOut real Source squares
9 off In flag Device initially off
12 icvds InOut real Initial D-S voltage
13 icvgs InOut real Initial G-S voltage
11 icvbs InOut real Initial B-S voltage
10 ic InOut real vector Vector of D-S, G-S, B-S voltages
77 temp InOut real Instance operating temperature
81 dtemp InOut real Instance temperature difference
15 sens_l In flag flag to request sensitivity WRT length
14 sens_w In flag flag to request sensitivity WRT width
22 dnode Out integer Number of drain node
23 gnode Out integer Number of gate node
24 snode Out integer Number of source node
25 bnode Out integer Number of bulk node
26 dnodeprime Out integer Number of internal drain node
27 snodeprime Out integer Number of internal source node
30 von Out real Turn-on voltage
31 vdsat Out real Saturation drain voltage
32 sourcevcrit Out real Critical source voltage
33 drainvcrit Out real Critical drain voltage
78 rs Out real Source resistance
28 sourceconductance Out real Source conductance
79 rd Out real Drain resistance
584 CHAPTER 31. MODEL AND DEVICE PARAMETERS
29 drainconductance Out real Drain conductance
38 gm Out real Transconductance
39 gds Out real Drain-Source conductance
37 gmb Out real Bulk-Source transconductance
37 gmbs Out real Bulk-Source transconductance
40 gbd Out real Bulk-Drain conductance
41 gbs Out real Bulk-Source conductance
42 cbd Out real Bulk-Drain capacitance
43 cbs Out real Bulk-Source capacitance
52 cgs Out real Gate-Source capacitance
55 cgd Out real Gate-Drain capacitance
58 cgb Out real Gate-Bulk capacitance
54 cqgs Out real Capacitance due to gate-source charge storage
57 cqgd Out real Capacitance due to gate-drain charge storage
60 cqgb Out real Capacitance due to gate-bulk charge storage
62 cqbd Out real Capacitance due to bulk-drain charge storage
64 cqbs Out real Capacitance due to bulk-source charge storage
44 cbd0 Out real Zero-Bias B-D junction capacitance
45 cbdsw0 Out real Zero-Bias B-D sidewall capacitance
46 cbs0 Out real Zero-Bias B-S junction capacitance
47 cbssw0 Out real Zero-Bias B-S sidewall capacitance
63 qbs Out real Bulk-Source charge storage
53 qgs Out real Gate-Source charge storage
56 qgd Out real Gate-Drain charge storage
59 qgb Out real Gate-Bulk charge storage
61 qbd Out real Bulk-Drain charge storage
19 p Out real Instantaneous power
76 sens_l_dc Out real dc sensitivity wrt length
70 sens_l_real Out real real part of ac sensitivity wrt length
71 sens_l_imag Out real imag part of ac sensitivity wrt length
74 sens_l_cplx Out complex ac sensitivity wrt length
72 sens_l_mag Out real sensitivity wrt l of ac magnitude
73 sens_l_ph Out real sensitivity wrt l of ac phase
75 sens_w_dc Out real dc sensitivity wrt width
65 sens_w_real Out real real part of ac sensitivity wrt width
66 sens_w_imag Out real imag part of ac sensitivity wrt width
67 sens_w_mag Out real sensitivity wrt w of ac magnitude
68 sens_w_ph Out real sensitivity wrt w of ac phase
69 sens_w_cplx Out complex ac sensitivity wrt width
31.6. MOSFETS 585
586 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.6.3.2 MOS3 model parameters
# Name Direction Type Description
144 type Out string N-channel or P-channel MOS
133 nmos In flag N type MOSfet model
134 pmos In flag P type MOSfet model
101 vto InOut real Threshold voltage
101 vt0 InOut real
102 kp InOut real Transconductance parameter
103 gamma InOut real Bulk threshold parameter
104 phi InOut real Surface potential
105 rd InOut real Drain ohmic resistance
106 rs InOut real Source ohmic resistance
107 cbd InOut real B-D junction capacitance
108 cbs InOut real B-S junction capacitance
109 is InOut real Bulk junction sat. current
110 pb InOut real Bulk junction potential
111 cgso InOut real Gate-source overlap cap.
112 cgdo InOut real Gate-drain overlap cap.
113 cgbo InOut real Gate-bulk overlap cap.
114 rsh InOut real Sheet resistance
115 cj InOut real Bottom junction cap per area
116 mj InOut real Bottom grading coefficient
117 cjsw InOut real Side junction cap per area
118 mjsw InOut real Side grading coefficient
119 js InOut real Bulk jct. sat. current density
120 tox InOut real Oxide thickness
121 ld InOut real Lateral diffusion
145 xl InOut real Length mask adjustment
146 wd InOut real Width Narrowing (Diffusion)
147 xw InOut real Width mask adjustment
148 delvto InOut real Threshold voltage Adjust
148 delvt0 InOut real
122 u0 InOut real Surface mobility
122 uo InOut real
123 fc InOut real Forward bias jct. fit parm.
124 nsub InOut real Substrate doping
125 tpg InOut integer Gate type
126 nss InOut real Surface state density
131 vmax InOut real Maximum carrier drift velocity
135 xj InOut real Junction depth
129 nfs InOut real Fast surface state density
138 xd InOut real Depletion layer width
139 alpha InOut real Alpha
127 eta InOut real Vds dependence of threshold voltage
128 delta InOut real Width effect on threshold
140 input_delta InOut real
130 theta InOut real Vgs dependence on mobility
132 kappa InOut real Kappa
141 tnom InOut real Parameter measurement temperature
142 kf InOut real Flicker noise coefficient
143 af InOut real Flicker noise exponent
31.6. MOSFETS 587
31.6.4 MOS6 - Level 6 MOSFET model with Meyer capacitance model
31.6.4.1 MOS6 instance parameters
# Name Direction Type Description
2 l InOut real Length
1 w InOut real Width
22 m InOut real Parallel Multiplier
4 ad InOut real Drain area
3 as InOut real Source area
6 pd InOut real Drain perimeter
5 ps InOut real Source perimeter
215 id Out real Drain current
215 cd Out real Drain current
18 is Out real Source current
17 ig Out real Gate current
16 ib Out real Bulk current
216 ibs Out real B-S junction capacitance
217 ibd Out real B-D junction capacitance
231 vgs Out real Gate-Source voltage
232 vds Out real Drain-Source voltage
230 vbs Out real Bulk-Source voltage
229 vbd Out real Bulk-Drain voltage
8 nrd InOut real Drain squares
7 nrs InOut real Source squares
9 off In flag Device initially off
12 icvds InOut real Initial D-S voltage
13 icvgs InOut real Initial G-S voltage
11 icvbs InOut real Initial B-S voltage
20 temp InOut real Instance temperature
21 dtemp InOut real Instance temperature difference
10 ic In real vector Vector of D-S, G-S, B-S voltages
15 sens_l In flag flag to request sensitivity WRT length
14 sens_w In flag flag to request sensitivity WRT width
203 dnode Out integer Number of the drain node
204 gnode Out integer Number of the gate node
205 snode Out integer Number of the source node
206 bnode Out integer Number of the node
207 dnodeprime Out integer Number of int. drain node
208 snodeprime Out integer Number of int. source node
258 rs Out real Source resistance
209 sourceconductance Out real Source conductance
259 rd Out real Drain resistance
210 drainconductance Out real Drain conductance
211 von Out real Turn-on voltage
212 vdsat Out real Saturation drain voltage
213 sourcevcrit Out real Critical source voltage
588 CHAPTER 31. MODEL AND DEVICE PARAMETERS
214 drainvcrit Out real Critical drain voltage
218 gmbs Out real Bulk-Source transconductance
219 gm Out real Transconductance
220 gds Out real Drain-Source conductance
221 gbd Out real Bulk-Drain conductance
222 gbs Out real Bulk-Source conductance
233 cgs Out real Gate-Source capacitance
236 cgd Out real Gate-Drain capacitance
239 cgb Out real Gate-Bulk capacitance
223 cbd Out real Bulk-Drain capacitance
224 cbs Out real Bulk-Source capacitance
225 cbd0 Out real Zero-Bias B-D junction capacitance
226 cbdsw0 Out real
227 cbs0 Out real Zero-Bias B-S junction capacitance
228 cbssw0 Out real
235 cqgs Out real Capacitance due to gate-source charge storage
238 cqgd Out real Capacitance due to gate-drain charge storage
241 cqgb Out real Capacitance due to gate-bulk charge storage
243 cqbd Out real Capacitance due to bulk-drain charge storage
245 cqbs Out real Capacitance due to bulk-source charge storage
234 qgs Out real Gate-Source charge storage
237 qgd Out real Gate-Drain charge storage
240 qgb Out real Gate-Bulk charge storage
242 qbd Out real Bulk-Drain charge storage
244 qbs Out real Bulk-Source charge storage
19 p Out real Instaneous power
256 sens_l_dc Out real dc sensitivity wrt length
246 sens_l_real Out real real part of ac sensitivity wrt length
247 sens_l_imag Out real imag part of ac sensitivity wrt length
248 sens_l_mag Out real sensitivity wrt l of ac magnitude
249 sens_l_ph Out real sensitivity wrt l of ac phase
250 sens_l_cplx Out complex ac sensitivity wrt length
257 sens_w_dc Out real dc sensitivity wrt width
251 sens_w_real Out real real part of ac sensitivity wrt width
252 sens_w_imag Out real imag part of ac sensitivity wrt width
253 sens_w_mag Out real sensitivity wrt w of ac magnitude
254 sens_w_ph Out real sensitivity wrt w of ac phase
255 sens_w_cplx Out complex ac sensitivity wrt width
31.6. MOSFETS 589
31.6.4.2 MOS6 model parameters
# Name Direction Type Description
140 type Out string N-channel or P-channel MOS
101 vto InOut real Threshold voltage
101 vt0 InOut real
102 kv InOut real Saturation voltage factor
103 nv InOut real Saturation voltage coeff.
104 kc InOut real Saturation current factor
105 nc InOut real Saturation current coeff.
106 nvth InOut real Threshold voltage coeff.
107 ps InOut real Sat. current modification par.
108 gamma InOut real Bulk threshold parameter
109 gamma1 InOut real Bulk threshold parameter 1
110 sigma InOut real Static feedback effect par.
111 phi InOut real Surface potential
112 lambda InOut real Channel length modulation param.
113 lambda0 InOut real Channel length modulation param. 0
114 lambda1 InOut real Channel length modulation param. 1
115 rd InOut real Drain ohmic resistance
116 rs InOut real Source ohmic resistance
117 cbd InOut real B-D junction capacitance
118 cbs InOut real B-S junction capacitance
119 is InOut real Bulk junction sat. current
120 pb InOut real Bulk junction potential
121 cgso InOut real Gate-source overlap cap.
122 cgdo InOut real Gate-drain overlap cap.
123 cgbo InOut real Gate-bulk overlap cap.
131 rsh InOut real Sheet resistance
124 cj InOut real Bottom junction cap per area
125 mj InOut real Bottom grading coefficient
126 cjsw InOut real Side junction cap per area
127 mjsw InOut real Side grading coefficient
128 js InOut real Bulk jct. sat. current density
130 ld InOut real Lateral diffusion
129 tox InOut real Oxide thickness
132 u0 InOut real Surface mobility
132 uo InOut real
133 fc InOut real Forward bias jct. fit parm.
137 nmos In flag N type MOSfet model
138 pmos In flag P type MOSfet model
135 tpg InOut integer Gate type
134 nsub InOut real Substrate doping
136 nss InOut real Surface state density
139 tnom InOut real Parameter measurement temperature
590 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.6.5 MOS9 - Modified Level 3 MOSFET model
31.6.5.1 MOS9 instance parameters
# Name Direction Type Description
80 m InOut real Multiplier
2 l InOut real Length
1 w InOut real Width
4 ad InOut real Drain area
3 as InOut real Source area
6 pd InOut real Drain perimeter
5 ps InOut real Source perimeter
34 id Out real Drain current
34 cd Out real Drain current
36 ibd Out real B-D junction current
35 ibs Out real B-S junction current
18 is Out real Source current
17 ig Out real Gate current
16 ib Out real Bulk current
50 vgs Out real Gate-Source voltage
51 vds Out real Drain-Source voltage
49 vbs Out real Bulk-Source voltage
48 vbd Out real Bulk-Drain voltage
8 nrd InOut real Drain squares
7 nrs InOut real Source squares
9 off In flag Device initially off
12 icvds InOut real Initial D-S voltage
13 icvgs InOut real Initial G-S voltage
11 icvbs InOut real Initial B-S voltage
10 ic InOut real vector Vector of D-S, G-S, B-S voltages
77 temp InOut real Instance operating temperature
81 dtemp InOut real Instance operating temperature difference
15 sens_l In flag flag to request sensitivity WRT length
14 sens_w In flag flag to request sensitivity WRT width
22 dnode Out integer Number of drain node
23 gnode Out integer Number of gate node
24 snode Out integer Number of source node
25 bnode Out integer Number of bulk node
26 dnodeprime Out integer Number of internal drain node
27 snodeprime Out integer Number of internal source node
30 von Out real Turn-on voltage
31 vdsat Out real Saturation drain voltage
32 sourcevcrit Out real Critical source voltage
33 drainvcrit Out real Critical drain voltage
78 rs Out real Source resistance
28 sourceconductance Out real Source conductance
79 rd Out real Drain resistance
31.6. MOSFETS 591
29 drainconductance Out real Drain conductance
38 gm Out real Transconductance
39 gds Out real Drain-Source conductance
37 gmb Out real Bulk-Source transconductance
37 gmbs Out real Bulk-Source transconductance
40 gbd Out real Bulk-Drain conductance
41 gbs Out real Bulk-Source conductance
42 cbd Out real Bulk-Drain capacitance
43 cbs Out real Bulk-Source capacitance
52 cgs Out real Gate-Source capacitance
55 cgd Out real Gate-Drain capacitance
58 cgb Out real Gate-Bulk capacitance
54 cqgs Out real Capacitance due to gate-source charge storage
57 cqgd Out real Capacitance due to gate-drain charge storage
60 cqgb Out real Capacitance due to gate-bulk charge storage
62 cqbd Out real Capacitance due to bulk-drain charge storage
64 cqbs Out real Capacitance due to bulk-source charge storage
44 cbd0 Out real Zero-Bias B-D junction capacitance
45 cbdsw0 Out real Zero-Bias B-D sidewall capacitance
46 cbs0 Out real Zero-Bias B-S junction capacitance
47 cbssw0 Out real Zero-Bias B-S sidewall capacitance
63 qbs Out real Bulk-Source charge storage
53 qgs Out real Gate-Source charge storage
56 qgd Out real Gate-Drain charge storage
59 qgb Out real Gate-Bulk charge storage
61 qbd Out real Bulk-Drain charge storage
19 p Out real Instantaneous power
76 sens_l_dc Out real dc sensitivity wrt length
70 sens_l_real Out real real part of ac sensitivity wrt length
71 sens_l_imag Out real imag part of ac sensitivity wrt length
74 sens_l_cplx Out complex ac sensitivity wrt length
72 sens_l_mag Out real sensitivity wrt l of ac magnitude
73 sens_l_ph Out real sensitivity wrt l of ac phase
75 sens_w_dc Out real dc sensitivity wrt width
65 sens_w_real Out real real part of ac sensitivity wrt width
66 sens_w_imag Out real imag part of ac sensitivity wrt width
67 sens_w_mag Out real sensitivity wrt w of ac magnitude
68 sens_w_ph Out real sensitivity wrt w of ac phase
69 sens_w_cplx Out complex ac sensitivity wrt width
592 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.6. MOSFETS 593
31.6.5.2 MOS9 model parameters
# Name Direction Type Description
144 type Out string N-channel or P-channel MOS
133 nmos In flag N type MOSfet model
134 pmos In flag P type MOSfet model
101 vto InOut real Threshold voltage
101 vt0 InOut real
102 kp InOut real Transconductance parameter
103 gamma InOut real Bulk threshold parameter
104 phi InOut real Surface potential
105 rd InOut real Drain ohmic resistance
106 rs InOut real Source ohmic resistance
107 cbd InOut real B-D junction capacitance
108 cbs InOut real B-S junction capacitance
109 is InOut real Bulk junction sat. current
110 pb InOut real Bulk junction potential
111 cgso InOut real Gate-source overlap cap.
112 cgdo InOut real Gate-drain overlap cap.
113 cgbo InOut real Gate-bulk overlap cap.
114 rsh InOut real Sheet resistance
115 cj InOut real Bottom junction cap per area
116 mj InOut real Bottom grading coefficient
117 cjsw InOut real Side junction cap per area
118 mjsw InOut real Side grading coefficient
119 js InOut real Bulk jct. sat. current density
120 tox InOut real Oxide thickness
121 ld InOut real Lateral diffusion
145 xl InOut real Length mask adjustment
146 wd InOut real Width Narrowing (Diffusion)
147 xw InOut real Width mask adjustment
148 delvto InOut real Threshold voltage Adjust
148 delvt0 InOut real
122 u0 InOut real Surface mobility
122 uo InOut real
123 fc InOut real Forward bias jct. fit parm.
124 nsub InOut real Substrate doping
125 tpg InOut integer Gate type
126 nss InOut real Surface state density
131 vmax InOut real Maximum carrier drift velocity
135 xj InOut real Junction depth
129 nfs InOut real Fast surface state density
138 xd InOut real Depletion layer width
139 alpha InOut real Alpha
127 eta InOut real Vds dependence of threshold voltage
128 delta InOut real Width effect on threshold
140 input_delta InOut real
130 theta InOut real Vgs dependence on mobility
132 kappa InOut real Kappa
141 tnom InOut real Parameter measurement temperature
142 kf InOut real Flicker noise coefficient
143 af InOut real Flicker noise exponent
594 CHAPTER 31. MODEL AND DEVICE PARAMETERS
31.6.6 BSIM1 - Berkeley Short Channel IGFET Model
31.6.6.1 BSIM1 instance parameters
# Name Direction Type Description
2 l InOut real Length
1 w InOut real Width
14 m InOut real Parallel Multiplier
4 ad InOut real Drain area
3 as InOut real Source area
6 pd InOut real Drain perimeter
5 ps InOut real Source perimeter
8 nrd InOut real Number of squares in drain
7 nrs InOut real Number of squares in source
9 off InOut flag Device is initially off
11 vds InOut real Initial D-S voltage
12 vgs InOut real Initial G-S voltage
10 vbs InOut real Initial B-S voltage
13 ic In unknown vector Vector of DS,GS,BS initial voltages
31.6.6.2 BSIM1 Model Parameters
# Name Direction Type Description
101 vfb InOut real Flat band voltage
102 lvfb InOut real Length dependence of vfb
103 wvfb InOut real Width dependence of vfb
104 phi InOut real Strong inversion surface potential
105 lphi InOut real Length dependence of phi
106 wphi InOut real Width dependence of phi
107 k1 InOut real Bulk effect coefficient 1
108 lk1 InOut real Length dependence of k1
109 wk1 InOut real Width dependence of k1
110 k2 InOut real Bulk effect coefficient 2
111 lk2 InOut real Length dependence of k2
112 wk2 InOut real Width dependence of k2
113 eta InOut real VDS dependence of threshold voltage
114 leta InOut real Length dependence of eta
115 weta InOut real Width dependence of eta
116 x2e InOut real VBS dependence of eta
117 lx2e InOut real Length dependence of x2e
118 wx2e InOut real Width dependence of x2e
119 x3e InOut real VDS dependence of eta
120 lx3e InOut real Length dependence of x3e
121 wx3e InOut real Width dependence of x3e
122 dl InOut real Channel length reduction in um
123 dw InOut real Channel width reduction in um
31.6. MOSFETS 595
124 muz InOut real Zero field mobility at VDS=0 VGS=VTH
125 x2mz InOut real VBS dependence of muz
126 lx2mz InOut real Length dependence of x2mz
127 wx2mz InOut real Width dependence of x2mz
128 mus InOut real Mobility at VDS=VDD VGS=VTH, channel length modulation
129 lmus InOut real Length dependence of mus
130 wmus InOut real Width dependence of mus
131 x2ms InOut real VBS dependence of mus
132 lx2ms InOut real Length dependence of x2ms
133 wx2ms InOut real Width dependence of x2ms
134 x3ms InOut real VDS dependence of mus
135 lx3ms InOut real Length dependence of x3ms
136 wx3ms InOut real Width dependence of x3ms
137 u0 InOut real VGS dependence of mobility
138 lu0 InOut real Length dependence of u0
139 wu0 InOut real Width dependence of u0
140 x2u0 InOut real VBS dependence of u0
141 lx2u0 InOut real Length dependence of x2u0
142 wx2u0 InOut real Width dependence of x2u0
143 u1 InOut real VDS depence of mobility, velocity saturation
144 lu1 InOut real Length dependence of u1
145 wu1 InOut real Width dependence of u1
146 x2u1 InOut real VBS depence of u1
147 lx2u1 InOut real Length depence of x2u1
148 wx2u1 InOut real Width depence of x2u1
149 x3u1 InOut real VDS depence of u1
150 lx3u1 InOut real Length dependence of x3u1
151 wx3u1 InOut real Width depence of x3u1
152 n0 InOut real Subthreshold slope
153 ln0 InOut real Length dependence of n0
154 wn0 InOut real Width dependence of n0
155 nb InOut real VBS dependence of subthreshold slope
156 lnb InOut real Length dependence of nb
157 wnb InOut real Width dependence of nb
158 nd InOut real VDS dependence of subthreshold slope
159 lnd InOut real Length dependence of nd
160 wnd InOut real Width dependence of nd
161 tox InOut real Gate oxide thickness in um
162 temp InOut real Temperature in degree Celcius
163 vdd InOut real Supply voltage to specify mus
164 cgso InOut real Gate source overlap capacitance per unit channel width(m)
165 cgdo InOut real Gate drain overlap capacitance per unit channel width(m)
166 cgbo InOut real Gate bulk overlap capacitance per unit channel length(m)
167 xpart InOut real Flag for channel charge partitioning
168 rsh InOut real Source drain diffusion sheet resistance in ohm per square
169 js InOut real Source drain junction saturation current per unit area
596 CHAPTER 31. MODEL AND DEVICE PARAMETERS
170 pb InOut real Source drain junction built in potential
171 mj InOut real Source drain bottom junction capacitance grading coefficient
172 pbsw InOut real Source drain side junction capacitance built in potential
173 mjsw InOut real Source drain side junction capacitance grading coefficient
174 cj InOut real Source drain bottom junction capacitance per unit area
175 cjsw InOut real Source drain side junction capacitance per unit area
176 wdf InOut real Default width of source drain diffusion in um
177 dell InOut real Length reduction of source drain diffusion
180 kf InOut real Flicker noise coefficient
181 af InOut real Flicker noise exponent
178 nmos In flag Flag to indicate NMOS
179 pmos In flag Flag to indicate PMOS
31.6. MOSFETS 597
31.6.7 BSIM2 - Berkeley Short Channel IGFET Model
31.6.7.1 BSIM2 instance parameters
# Name Direction Type Description
2 l InOut real Length
1 w InOut real Width
14 m InOut real Parallel Multiplier
4 ad InOut real Drain area
3 as InOut real Source area
6 pd InOut real Drain perimeter
5 ps InOut real Source perimeter
8 nrd InOut real Number of squares in drain
7 nrs InOut real Number of squares in source
9 off InOut flag Device is initially off
11 vds InOut real Initial D-S voltage
12 vgs InOut real Initial G-S voltage
10 vbs InOut real Initial B-S voltage
13 ic In unknown vector Vector of DS,GS,BS initial voltages
31.6.7.2 BSIM2 model parameters
# Name Direction Type Description
101 vfb InOut real Flat band voltage
102 lvfb InOut real Length dependence of vfb
103 wvfb InOut real Width dependence of vfb
104 phi InOut real Strong inversion surface potential
105 lphi InOut real Length dependence of phi
106 wphi InOut real Width dependence of phi
107 k1 InOut real Bulk effect coefficient 1
108 lk1 InOut real Length dependence of k1
109 wk1 InOut real Width dependence of k1
110 k2 InOut real Bulk effect coefficient 2
111 lk2 InOut real Length dependence of k2
112 wk2 InOut real Width dependence of k2
113 eta0 InOut real VDS dependence of threshold voltage at VDD=0
114 leta0 InOut real Length dependence of eta0
115 weta0 InOut real Width dependence of eta0
116 etab InOut real VBS dependence of eta
117 letab InOut real Length dependence of etab
118 wetab InOut real Width dependence of etab
119 dl InOut real Channel length reduction in um
120 dw InOut real Channel width reduction in um
121 mu0 InOut real Low-field mobility, at VDS=0 VGS=VTH
122 mu0b InOut real VBS dependence of low-field mobility
123 lmu0b InOut real Length dependence of mu0b
598 CHAPTER 31. MODEL AND DEVICE PARAMETERS
124 wmu0b InOut real Width dependence of mu0b
125 mus0 InOut real Mobility at VDS=VDD VGS=VTH
126 lmus0 InOut real Length dependence of mus0
127 wmus0 InOut real Width dependence of mus
128 musb InOut real VBS dependence of mus
129 lmusb InOut real Length dependence of musb
130 wmusb InOut real Width dependence of musb
131 mu20 InOut real VDS dependence of mu in tanh term
132 lmu20 InOut real Length dependence of mu20
133 wmu20 InOut real Width dependence of mu20
134 mu2b InOut real VBS dependence of mu2
135 lmu2b InOut real Length dependence of mu2b
136 wmu2b InOut real Width dependence of mu2b
137 mu2g InOut real VGS dependence of mu2
138 lmu2g InOut real Length dependence of mu2g
139 wmu2g InOut real Width dependence of mu2g
140 mu30 InOut real VDS dependence of mu in linear term
141 lmu30 InOut real Length dependence of mu30
142 wmu30 InOut real Width dependence of mu30
143 mu3b InOut real VBS dependence of mu3
144 lmu3b InOut real Length dependence of mu3b
145 wmu3b InOut real Width dependence of mu3b
146 mu3g InOut real VGS dependence of mu3
147 lmu3g InOut real Length dependence of mu3g
148 wmu3g InOut real Width dependence of mu3g
149 mu40 InOut real VDS dependence of mu in linear term
150 lmu40 InOut real Length dependence of mu40
151 wmu40 InOut real Width dependence of mu40
152 mu4b InOut real VBS dependence of mu4
153 lmu4b InOut real Length dependence of mu4b
154 wmu4b InOut real Width dependence of mu4b
155 mu4g InOut real VGS dependence of mu4
156 lmu4g InOut real Length dependence of mu4g
157 wmu4g InOut real Width dependence of mu4g
158 ua0 InOut real Linear VGS dependence of mobility
159 lua0 InOut real Length dependence of ua0
160 wua0 InOut real Width dependence of ua0
161 uab InOut real VBS dependence of ua
162 luab InOut real Length dependence of uab
163 wuab InOut real Width dependence of uab
164 ub0 InOut real Quadratic VGS dependence of mobility
165 lub0 InOut real Length dependence of ub0
166 wub0 InOut real Width dependence of ub0
167 ubb InOut real VBS dependence of ub
168 lubb InOut real Length dependence of ubb
169 wubb InOut real Width dependence of ubb
31.6. MOSFETS 599
170 u10 InOut real VDS depence of mobility
171 lu10 InOut real Length dependence of u10
172 wu10 InOut real Width dependence of u10
173 u1b InOut real VBS depence of u1
174 lu1b InOut real Length depence of u1b
175 wu1b InOut real Width depence of u1b
176 u1d InOut real VDS depence of u1
177 lu1d InOut real Length depence of u1d
178 wu1d InOut real Width depence of u1d
179 n0 InOut real Subthreshold slope at VDS=0 VBS=0
180 ln0 InOut real Length dependence of n0
181 wn0 InOut real Width dependence of n0
182 nb InOut real VBS dependence of n
183 lnb InOut real Length dependence of nb
184 wnb InOut real Width dependence of nb
185 nd InOut real VDS dependence of n
186 lnd InOut real Length dependence of nd
187 wnd InOut real Width dependence of nd
188 vof0 InOut real Threshold voltage offset AT VDS=0 VBS=0
189 lvof0 InOut real Length dependence of vof0
190 wvof0 InOut real Width dependence of vof0
191 vofb InOut real VBS dependence of vof
192 lvofb InOut real Length dependence of vofb
193 wvofb InOut real Width dependence of vofb
194 vofd InOut real VDS dependence of vof
195 lvofd InOut real Length dependence of vofd
196 wvofd InOut real Width dependence of vofd
197 ai0 InOut real Pre-factor of hot-electron effect.
198 lai0 InOut real Length dependence of ai0
199 wai0 InOut real Width dependence of ai0
200 aib InOut real VBS dependence of ai
201 laib InOut real Length dependence of aib
202 waib InOut real Width dependence of aib
203 bi0 InOut real Exponential factor of hot-electron effect.
204 lbi0 InOut real Length dependence of bi0
205 wbi0 InOut real Width dependence of bi0
206 bib InOut real VBS dependence of bi
207 lbib InOut real Length dependence of bib
208 wbib InOut real Width dependence of bib
209 vghigh InOut real Upper bound of the cubic spline function.
210 lvghigh InOut real Length dependence of vghigh
211 wvghigh InOut real Width dependence of vghigh
212 vglow InOut real Lower bound of the cubic spline function.
213 lvglow InOut real Length dependence of vglow
214 wvglow InOut real Width dependence of vglow
215 tox InOut real Gate oxide thickness in um
600 CHAPTER 31. MODEL AND DEVICE PARAMETERS
216 temp InOut real Temperature in degree Celcius
217 vdd InOut real Maximum Vds
218 vgg InOut real Maximum Vgs
219 vbb InOut real Maximum Vbs
220 cgso InOut real Gate source overlap capacitance per unit channel width(m)
221 cgdo InOut real Gate drain overlap capacitance per unit channel width(m)
222 cgbo InOut real Gate bulk overlap capacitance per unit channel length(m)
223 xpart InOut real Flag for channel charge partitioning
224 rsh InOut real Source drain diffusion sheet resistance in ohm per square
225 js InOut real Source drain junction saturation current per unit area
226 pb InOut real Source drain junction built in potential
227 mj InOut real Source drain bottom junction capacitance grading coefficient
228 pbsw InOut real Source drain side junction capacitance built in potential
229 mjsw InOut real Source drain side junction capacitance grading coefficient
230 cj InOut real Source drain bottom junction capacitance per unit area
231 cjsw InOut real Source drain side junction capacitance per unit area
232 wdf InOut real Default width of source drain diffusion in um
233 dell InOut real Length reduction of source drain diffusion
236 kf InOut real Flicker noise coefficient
237 af InOut real Flicker noise exponent
234 nmos In flag Flag to indicate NMOS
235 pmos In flag Flag to indicate PMOS
31.6. MOSFETS 601
31.6.8 BSIM3
The accessible device parameters (see Chapt. 31.1 for the syntax) are listed here.
31.6.8.1 BSIM3 accessible instance parameters
# Name Direction Type Description
1 id Out real Drain current
2 vgs Out real Gate-Source voltage
3 vds Out real Drain-Source voltage
4 vbs Out real Bulk-Source voltage
5 gm Out real Transconductance
6 gds Out real Drain-Source conductance
7 gmbs Out real Bulk-Source transconductance
8 vdsat Out real Saturation voltage
9 vth Out real Threshold voltage
10 ibd Out real
11 ibs Out real
12 gbd Out real
13 gbs Out real
14 qb Out real Qbulk
15 cqb Out real
16 qg Out real Qgate
17 cqg Out real
18 qd Out real Qdrain
19 cqd Out real
20 cgg Out real
21 cgd Out real
22 cgs Out real
23 cdg Out real
24 cdd Out real
25 cds Out real
26 cbg Out real
27 cbd Out real
28 cbs Out real
29 capbd Out real Diode capacitance
30 capbs Out real Diode capacitance
The parameters are available in the BSIM3 models (level=8 or level=49) version=3.2.4 and ver-
sion=3.3.0 only. Negative capacitance values may occur, depending on the internal calculation.
Please see the note in Chapt. 31.6.9.1.
31.6.8.2 BSIM3 manual
Further detailed descriptions will not be given here. Unfortunately the details on these para-
meters are not documented, even not in the otherwise excellent pdf manual (tarred) issued by
602 CHAPTER 31. MODEL AND DEVICE PARAMETERS
University of California at Berkeley.
31.6.9 BSIM4
The accessible device parameters (see Chapt. 31.1 for the syntax) are listed here.
31.6.9.1 BSIM4 accessible instance parameters
# Name Direction Type Description
gmbs Out real Body effect (Back gate) transconductance
gm Out real Transconductance
gds Out real Drain-Source conductance
vdsat Out real Saturation voltage
vth Out real Threshold voltage
id Out real Drain current
ibd Out real Diode current
ibs Out real Diode current
gbd Out real Diode conductance
gbs Out real Diode conductance
isub Out real Substrate current
igidl Out real Gate-Induced Drain Leakage current
igisl Out real Gate-Induced Source Leakage current
igs Out real Gate-Source current
igd Out real Gate-drain current
igb Out real Gate-Bulk current
igcs Out real
vbs Out real Bulk-Source voltage
vgs Out real Gate-Source voltage
vds Out real Drain-Source voltage
cgg Out real
cgs Out real
cgd Out real
cbg Out real
cbd Out real
cbs Out real
cdg Out real
cdd Out real
cds Out real
csg Out real
csd Out real
css Out real
cgb Out real
cdb Out real
csb Out real
cbb Out real
31.6. MOSFETS 603
capbd Out real Diode capacitance
capbs Out real Diode capacitance
qg Out real Gate charge
qb Out real Bulk charge
qd Out real Drain charge
qs Out real
qinv Out real
qdef Out real
gcrg Out real
gtau Out real
The parameters are available in all BSIM4 models (level=14 or level=54) version=4.2.1 to ver-
sion=4.8.
Negative capacitance values may occur, depending on the internal calculation. To comparing
with measured data, please just use the absolute values of the capacitance data. For an expla-
nation of negative values and the basics on how capacitance values are evaluated in a BSIM
model, please refer to the book BSIM4 and MOSFET modeling by Liu and Hu, Chapt. 5.2.
31.6.9.2 BSIM4 manual
Detailed descriptions will not be given here. Unfortunately the details on these parameters
are not documented, even not in the otherwise excellent pdf manual issued by University of
California at Berkeley.
604 CHAPTER 31. MODEL AND DEVICE PARAMETERS
Chapter 32
Compilation notes
This file describes the procedures to install ngspice from sources.
32.1 Ngspice Installation under Linux (and other ’UNIXes’)
32.1.1 Prerequisites
Ngspice is written in C and thus a complete C compilation environment is needed. Almost any
UNIX comes with a complete C development environment. Ngspice is developed on GNU/Li-
nux with gcc and GNU make.
The following software must be installed in your system to compile ngspice: bison, flex,
and X11 headers and libs.
The X11 headers and libraries are typically available in an X11 development package from your
Linux distribution.
If you want to compile the Git source you need additional software: autoconf, automake,
libtool, texinfo.
The following software may be needed when enabling additional features: readline,editline,
tcl/tk,blt.
If you want have high performance and accurate FFT’s you should install: fftw-3.Ngspice
configure script will find the library and will induce the build process to link against it.
32.1.2 Install from Git
This section describes how to install from source code taken direct from Git. This will give
you access to the most recent enhancements and corrections. However be careful as the code
in Git may be under development and thus still unstable. For user install instructions using
source from released distributions, please see the sections titled ’Install from tarball’ (32.1.3)
and ’Advanced Install’ (32.1.5).
Download source from Git as described on the sourceforge ngspice Git page. Define and enter
a directory of your choice, e.g. /home/myname/software/. Download the complete ngspice
repository from Git, for example by anonymous access issuing the command
605
606 CHAPTER 32. COMPILATION NOTES
git clone git://git.code.sf.net/p/ngspice/ngspice
or via http protocol
git clone http://git.code.sf.net/p/ngspice/ngspice
You will find the sources in directory /home/myname/software/ngspice. Now enter the
ngspice top level directory ngspice (where the installation instruction file INSTALL can be
found).
The project uses the GNU build process. You should be able to do the following:
$ ./autogen.sh
$ ./configure --enable-xspice --enable-cider
--disable-debug --with-readline=yes
$ make
$ sudo make install
See the section titled ’Advanced Install’ (32.1.5) for instructions about arguments that can be
passed to ./configure to customize the build and installation. The following arguments are
already used here and may be called sort of ‘standard’:
--enable-xspice Include the XSPICE extensions (see Chapt. 12 and 28)
--enable-cider Include CIDER numerical device simulator (see Chapt. 30)
--disable-debug No debugging information included (optimized and compact code)
--with-readline=yes Include an editor for the input command line (command history, backspace,
insert etc.). If readline is not available, editline may be used.
--enable-openmp Compile ngspice for multi-core processors. Paralleling is done by OpenMP
(see Chapt. 16.10), and is enabled for certain MOS models.
If a problem is found with the build process, please submit a report to the Ngspice development
team. Please provide information about your system and any ./configure arguments you
are using, together with any error messages. Ideally you would have tried to fix the problem
yourself first. If you have fixed the problem then the development team will love to hear from
you.
If you need updating your local source code tree from Git, just enter ngspice directory and
issue the command
git pull
git pull will deny to overwrite modified files in your working directory. To drop your local
changes first, you can run
git reset --hard
To learn more about Git, which can be both powerful and difficult to master, please consult
http://git-scm.com/, especially: http://git-scm.com/documentation, which has pointers to docu-
mentation and tutorials.
32.1. NGSPICE INSTALLATION UNDER LINUX (AND OTHER ’UNIXES’) 607
32.1.3 Install from a tarball, e.g. ngspice-rework-27.tgz
This covers installation from a tarball (for example ngspice-rework-27.tgz, to be found at
http://sourceforge.net/projects/ngspice/files/). After downloading the tar ball to a local di-
rectory unpack it using:
$ tar -zxvf ngspice-rework-27.tgz
Now change directories in to the top-level source directory (where this text from the INSTALL
file can be found).
You should be able to do:
$ ./configure --enable-xspice --disable-debug --with-readline=yes
$ make
$ sudo make install
The default install dir is /usr/local/bin
See the section titled ’Advanced Install’ (32.1.5) for instructions about arguments that can be
passed to ./configure to customize the build and installation.
32.1.4 Compilation using an user defined directory tree for object files
The procedures described above will store the *.o files (output of the compilation step) into the
directories where the sources (*.c) are located. This may not be the best option if you want for
example to maintain a debug version and in parallel a release version of ngspice (./configure
--disable-debug). So if you intend to create a separate object file tree like ngspice/ngbuil-
d/release, you may do the following, starting from the default directory ngspice:
mkdir -p release
cd release
../configure --enable-xspice --disable-debug --with-readline=yes <more options>
make install
This will create an object file directory tree, similar to the source file directory tree, the object
files are now separated from the source files. For the debug version, you may do the same
as described above, replacing ’release’ by ’debug’, and obtain another separated object file
directory tree. If you already have run ./configure in ngspice, you have to do a maintainer-
clean, before the above procedure will work.
32.1.5 Advanced Install
Some extra options can be provided to ./configure. To get all available options do:
$ ./configure --help
Some of these options are generic to the GNU build process that is used by Ngspice, other are
specific to Ngspice.
The following sections provide some guidance and descriptions for many, but not all, of these
options.
608 CHAPTER 32. COMPILATION NOTES
32.1.5.1 Options Specific to Using Ngspice
--enable-openmp Compile ngspice for multi-core processors. Paralleling is done by OpenMP
(see Chapt. 16.10).
--enable-xspice Enable XSPICE enhancements, yielding a mixed signal simulator integra-
ted into ngspice with codemodel dynamic loading support. See Chapt. 12 and section II for
details.
--with-readline=yes Enable GNU readline support for the command line interface.
--enable-cider Cider is a mixed-level simulator that couples Spice3 and DSIM to simulate
devices from their technological parameters. This part of the simulator is not compiled by
default.
--enable-adms ADMS is an experimental model compiler that translates Verilog-A compact
models into C code that can be compiled into ngspice. This is still experimental, but working
with some limitations to the models (e.g. no noise models). If you want to use it, please refer
to the ADMS section on ngspice web site .
--with-editline=yes Enables the use of the BSD editline library (libedit).
See http://www.thrysoee.dk/editline/.
--without-x Disable the X-Windows graphical system. Compile without needing X headers
and X libraries. The plot command (17.5.45) is now disabled. You may use (17.5.28) instead.
--with-tcl=tcldir When configured with this option the tcl module ‘tclspice’ is compiled
and installed instead of plain ngspice.
--with-ngshared This option will create a shared library (*.so in Linux) or dynamic link
library (*.dll) instead of plain ngspice.
--enable-relpath This options introduces a searchpath for spinit relative to the calling exe-
cutable (ngspice or the caller using the ngspice shared library) as ../share/ngspice. In spinit
the search path for code models is also set as relative as ../lib.
The following options are seldom used today, not tested, some may even no longer be imple-
mented.
--enable-capbypass Bypass calculation of cbd/cbs in the mosfets if the vbs/vbd voltages are
unchanged.
--enable-capzerobypass Bypass all the cbd/cbs calculations if Czero is zero. This is ena-
bled by default since rework-18.
--enable-cluster Clustering code for distributed simulation. This is a contribution never
tested. This code comes from TCLspice implementation and is implemented for transient ana-
lysis only.
--enable-expdevices Enable experimental devices. This option is used by developers to
mask devices under development. Almost useless for users.
--enable-experimental This enables some experimental code. Specifically it enables: *
support for altering options in interactive mode by adding the interactive keyword ’options’. *
The ability to save and load snapshots: adds interactive keywords ’savesnap’ and ’loadsnap’.
--enable-help Force building nghelp. This is deprecated.
--enable-newpred Enable the NEWPRED symbol in the code.
32.1. NGSPICE INSTALLATION UNDER LINUX (AND OTHER ’UNIXES’) 609
--enable-newtrunc Enable the newtrunc option
--enable-ndev Enable NDEV interface, (experimental) A TCP/IP interface to external device
simulator such as GSS. For more information, please visit the homepage of GSS at http://gss-
tcad.sourceforge.net
--enable-nodelimiting Experimental damping scheme
--enable-nobypass Don’t bypass recalculations of slowly changing variables
--enable-nosqrt Use always log/exp for non-linear capacitances --enable-predictor
Enable a predictor method for convergence
--enable-sense2 Use spice2 sensitivity analysis
--enable-xgraph Compile the Xgraph plotting program. Xgraph is a plotting package for
X11 and was once very popular.
32.1.5.2 Options Useful for Debugging Ngspice
--disable-debug This option will remove the ’-g’ option passed to the compiler. This speeds
up execution time, creates a small executable, and is recommended for normal use. If you want
to run ngspice in a debugger (e.g. gdb), you should not select this option.
The following options are seldom used today, not tested, some may even no longer be imple-
mented.
--enable-ansi Configure will try to find an option for your compiler so that it expects ansi-C.
--enable-asdebug Debug sensitivity code *ASDEBUG*.
--enable-blktmsdebug Debug distortion code *BLOCKTIMES*
--enable-checkergcc Option for compilation with checkergcc.
--enable-cpdebug Enable ngspice shell code debug.
--enable-ftedebug Enable ngspice frontend debug.
--enable-gc Enable the Boehm-Weiser Conservative Garbage Collector.
--enable-pzdebug Debug pole/zero code.
--enable-sensdebug Debug sensitivity code *SENSDEBUG*.
--enable-smltmsdebug Debug distortion code *SMALLTIMES*
--enable-smoketest Enable smoketest compile.
--enable-stepdebug Turns on debugging of convergence steps in transient analysis
32.1.6 Compilers and Options
Some systems require unusual options for compilation or linking that the configure script does
not know about. You can give configure initial values for variables by setting them in the
environment. Using a Bourne-compatible shell, you can do that on the command line like this:
CC=c89
CFLAGS=-O2
610 CHAPTER 32. COMPILATION NOTES
LIBS=-lposix
./configure
Or on systems that have the env program, you can do it like this:
env CPPFLAGS=-I/usr/local/include
LDFLAGS=-s
./configure
32.1.7 Compiling For Multiple Architectures
You can compile the package for more than one kind of computer at the same time, by pla-
cing the object files for each architecture in their own directory. To do this, you must use a
version of make that supports the VPATH variable, such as GNU make.cd to the directory
where you want the object files and executables to go and run the configure script. configure
automatically checks for the source code in the directory that configure is in and in ‘..’.
If you have to use a make that does not supports the VPATH variable, you have to compile the
package for one architecture at a time in the source code directory. After you have installed the
package for one architecture, use make distclean before reconfiguring for another architecture.
32.1.8 Installation Names
By default, make install will install the package’s files in /usr/local/bin,/usr/local/man, etc.
You can specify an installation prefix other than /usr/local by giving configure the option –
prefix=PATH.
You can specify separate installation prefixes for architecture-specific files and architecture-
independent files. If you give configure the option –exec-prefix=PATH, the package will use
PATH as the prefix for installing programs and libraries. Documentation and other data files
will still use the regular prefix.
In addition, if you use an unusual directory layout you can give options like –bindir=PATH
to specify different values for particular kinds of files. Run configure –help for a list of the
directories you can set and what kinds of files go in them.
If the package supports it, you can cause programs to be installed with an extra prefix or suf-
fix on their names by giving configure the option –program-prefix=PREFIX or –program-
suffix=SUFFIX.
When installed on MinGW with MSYS alternative paths are not fully supported. See ‘How to
make ngspice with MINGW and MSYS’ below for details.
32.1.9 Optional Features
Some packages pay attention to –enable-FEATURE options to configure, where FEATURE
indicates an optional part of the package. They may also pay attention to –with-PACKAGE
options, where PACKAGE is something like gnu-as or ‘x’ (for the X Window System). The
README should mention any –enable- and –with- options that the package recognizes.
32.1. NGSPICE INSTALLATION UNDER LINUX (AND OTHER ’UNIXES’) 611
For packages that use the X Window System, configure can usually find the X include and
library files automatically, but if it doesn’t, you can use the configure options –x-includes=DIR
and –x-libraries=DIR to specify their locations.
32.1.10 Specifying the System Type
There may be some features configure can not figure out automatically, but needs to determine
by the type of host the package will run on. Usually configure can figure that out, but if it
prints a message saying it can not guess the host type, give it the –host=TYPE option. TYPE
can either be a short name for the system type, such as ‘sun4’, or a canonical name with three
fields: CPU-COMPANY-SYSTEM
See the file config.sub for the possible values of each field. If config.sub isn’t included in this
package, then this package doesn’t need to know the host type.
If you are building compiler tools for cross-compiling, you can also use the –target=TYPE
option to select the type of system they will produce code for and the –build=TYPE option to
select the type of system on which you are compiling the package.
32.1.11 Sharing Defaults
If you want to set default values for configure scripts to share, you can create a site shell
script called config.site that gives default values for variables like CC,cache_file, and prefix.
configure looks for PREFIX/share/config.site if it exists, then PREFIX/etc/config.site if it
exists. Or, you can set the CONFIG_SITE environment variable to the location of the site
script. A warning: not all configure scripts look for a site script.
32.1.12 Operation Controls
configure recognizes the following options to control how it operates.
--cache-file=FILE Use and save the results of the tests in FILE instead of ./config.cache.
Set FILE to /dev/null to disable caching, for debugging configure.
--help Print a summary of the options to configure, and exit.
--quiet --silent -q Do not print messages saying which checks are being made. To sup-
press all normal output, redirect it to /dev/null (any error messages will still be shown).
--srcdir=DIR Look for the package’s source code in directory DIR. Usually configure can
determine that directory automatically.
--version Print the version of Autoconf used to generate the configure script, and exit.
configure also accepts some other, not widely useful, options.
612 CHAPTER 32. COMPILATION NOTES
32.2 Ngspice Compilation under Windows OS
32.2.1 Compile ngspice with MS Visual Studio 2015 or 2017
ngspice may be compiled with MS Visual Studio 2015 or 2017. A free version is offered by
Microsoft with the Visual Studio Community Edition. XSPICE project files are located in
visualc/XSPICE and are automatically invoked if you start the build procedure.
CIDER and XSPICE are included, as well as the code models for XSPICE (*.cm). Verilog-A
models compiled with ADMS however are not available.
After compilation the executable, code models and initialization files are available in direc-
tory C: as C:\Spice, C:\Spice64 etc., as described in the installation tree below. A true Win-
dows installer is however not yet available. The ’home’ directory for Windows OS (ngspice-
ngspice/visualc) with its files vngspice.sln (project starter) and vngspice.vcxproj (project
contents) allows to compile and link ngspice with MS Visual Studio.
/visualc/src/include/ngspice contains a dedicated config.h file with the preprocessor definiti-
ons required to properly compile the code.
Install Microsoft Visual Studio 2017. The MS Visual Studio Community Edition (which is
available at no cost from https://www.microsoft.com/en-us/download/details.aspx?id=48146)
is fully adequate. It will generate a 32 bit Release with or without OpenMP support and a
Debug version of ngspice, using the Win32 flag. In addition you may select a console version
without graphics interface. The same is available for 64 bit (flag x64). Standard for every day
use are the ReleaseOMP variants for 32 or 64 bit.
Compilation of the ngspice and XSPICE codes requires the installation of FLEX and BISON.
They may be downloaded as Windows executables from winflexbison. Please unzip the zip
file and copy its content into a directory named flex-bison at the same level as the ngspice
directory.
Procedure:
Download ngspice. You may obtain a snapshot from ngspice git page at SourceForge, where
you will find on top of the page a link named ’Download Snapshot’. On the left you may select
any of the branches which are of interest. Branch ’master’ is the most mature code selection,
branch ’scope-inpcom-16’ is an actual development branch. Another approach is to install ’git’
from git-scm and installing ngspice source code with the command
git clone git://git.code.sf.net/p/ngspice/ngspice ngspice-ngspice
as described in chapter 32.1.2.
Go to directory /ngspice/visualc.
Start MS Visual Studio by double click on vngspice.sln. After MS Visual Studio opens,
select the debug or release version (with or without OpenMP support) by checking Build,
Configuration-Manager, Debug, Release or ReleaseOMP. Start making ngspice.exe by
selecting Build and Build Solution. The executable will be created and stored in visualc/vng-
spice/<configuration.platform>. Object files will be stored to visualc/vngspice/<configuration.platform>/obj.
A simplified installation tree is created in parallel:
32.2. NGSPICE COMPILATION UNDER WINDOWS OS 613
C:\Spice\
bin\
ngspice.exe
vcomp14xx.dll
lib\
ngspice\
analog.cm
digital.cm
spice2poly.cm
extradev.cm
extravt.cm
table.cm
share\
ngspice\
scripts\
spinit
Table 32.1: ngspice Visual Studio installation tree under MS Windows
The exact directory names depend on the configuration and platform you have selected (C:\Spice,
C:\Spice64,C:\Spiced,C:\Spice64d). If you intend to install ngspice into another directory,
e.g. D:\MySpice, you may simply copy the contents from C:\Spice to the new location. This
becomes possible because the paths to the code models or spinit are set relative to ngspice.exe.
As an alternative you may edit make-install-vngspice.bat and alter the following entries from:
set dst=c:\Spice
set dst=c:\Spice64
to
set dst=D:\MySpice
set dst=D:\MySpice64
To use the FFTW-3 library for a ’calibrated’ fast fourier analysis with the fft command (see
17.5.26), download the precompiled MS Windows FFTW distribution (either 32 bit or 64
bit) from http://www.fftw.org/install/windows.html. Extract at least the files fftw3.h,libfftw3-
3.def, and libfftw3-3.dll to directory ../../fftw-3.3.4-dll32 (from 32 bit fftw3 for ngspice 32
bit), or to directory ../../fftw-3.3.4-dll64 (from 64 bit fftw3 for ngspice 64 bit). So both di-
rectories are at the same level as the ngspice directory. Then select the MS VC++ project
file visualc/vngspice-fftw.vcxproj for starting VC++, select the appropriate configuration and
platform, and off you go. This is how the installed directory tree looks like:
614 CHAPTER 32. COMPILATION NOTES
D:\MySpiceSources\
ngspice\
visualc\
...
flex-bison\
...
fftw-3.3.4-dll32\
...
fftw-3.3.4-dll64\
...
Table 32.2: ngspice source tree under MS Windows
If you use the debugging features of Visual Studio, ngspice is started with a special spinit file
located in visualc\vngspice\share\ngspice\scripts. Your user-defined start-up commands are
best addressed in a .spiceinit file located in C:\users\<username>.
32.2.2 How to make ngspice with MINGW and MSYS
Creating ngspice with MINGW is a straight forward procedure, if you have MSYS/MINGW
installed properly. Unfortunately the installation is rather tedious because you will need several
enhancements to the standard install, especially if you want to include XSpice. Some links are
given below that describe the procedures. The default installation location of ngspice is the
Windows path C:\spice. The install path can be altered by passing --prefix=NEWPATH as an
argument to ./configure during the build process.
Put the install path you desire inside ‘’, e.g. "D:/NewSpice". Be careful to use forward slashes
‘/’, not backward slashes ‘\’ (something still to be fixed). Then add --prefix="D:/NewSpice"
as an argument to ./configure in the normal way.
The procedure of compiling a distribution (for example, the most recent stable distribution from
the ngspice website, e.g. ngspice-26.tar.gz), is as follows:
$ cd ngspice
$ cd release
$ ../configure --with-wingui ...and other options
$ make
$ make install
The useful options are:
--enable-xspice (this requires FLEX and BISON available in MSYS, see below).
--enable-cider
--disable-debug (-O2 optimization, no debug information)
A complete ngspice (release version, no debug info, optimized executable) may be made avai-
lable just by
$ cd ngspice
32.2. NGSPICE COMPILATION UNDER WINDOWS OS 615
$ ./compile_min.sh
If you want to compile the Git source you need additional software packages autoconf,auto-
make,libtool,available from the MSYS distribution and git,available for example here.
Download source from Git as described on the sourceforge ngspice Git page. Define and enter
a directory of your choice, e.g. /d/spice/. Download the complete ngspice repository from Git,
for example by anonymous access issuing the command
git clone git://ngspice.git.sourceforge.net/gitroot/ngspice/ngspice
You will find the sources in directory /d/spice/ngspice/. Now enter the ngspice top level
directory ngspice. This is the procedure for compilation:
$ cd ngspice
$ ./autogen.sh
$ mkdir release
$ cd release
$ ../configure --with-wingui ...and other options
$ make
$ make install
The user defined build tree saves the object files, instead of putting them into the source tree, in
a release (and a debug) tree. Please see Chapt. 32.1.4 for instructions.
If you need updating your local source code tree from Git, just enter ngspice directory and
issue the command
git pull
git pull will deny to overwrite modified files in your working directory. To drop your local
changes first, you can run
git reset --hard
To learn more about Git, which can be both powerful and difficult to master, please consult
http://git-scm.com/, especially: http://git-scm.com/documentation, which has pointers to docu-
mentation and tutorials.
MINGW and MSYS can be downloaded from http://www.mingw.org/. The making of the code
models *.cm for XSpice and one of the ngspice parsers require the installation of BISON and
FLEX to MSYS. A typical installation was tested with: bison-2.0-MSYS.tar.gz flex-2.5.4a-
1-bin.zip libiconv-1.9.2-1-bin.zip libintl-0.14.4-bin.zip
Bison 2.0 is now superseded by newer releases
(Bison 2.3, see http://sourceforge.net/project/showfiles.php?group_id=2435&package_id=67879)
The last three are fromhttp://sourceforge.net/project/showfiles.php?group_id=23617.
You may also look at
http://www.mingw.org/wiki/HOWTO_Install_the_MinGW_GCC_Compiler_Suite
http://www.mingw.org/wiki/MSYS
http://www.mingw.org/wiki/HOWTO_Create_an_MSYS_Build_Environment.
616 CHAPTER 32. COMPILATION NOTES
32.2.3 64 Bit executables with MINGW-w64
Procedure:
Install MSYS or preferently the newer MSYS2, plus bison,flex,auto tools,perl, libiconv,
libintl
Install MINGW-w64, activate OpenMP support
See either http://mingw-w64.sourceforge.net/ or http://tdm-gcc.tdragon.net/
(allows to generate both 32 or 64 bit executables by setting flag -m32 or -m64)
Set path to compiler in msys/xx/etc/fstab (e.g. c:/MinGW64 /mingw), if not set automatically
as in MSYS2.
Start compiling with
./compile_min.sh or ./compile_min.sh 64
Options used in the script:
–adms and –enable-adms ADMS is an experimental model compiler that translates Verilog-
A compact models into C code that can be compiled into ngspice. This is still experimental,
but working with some limitations to the models (e.g. no noise models). If you want to use it,
please refer to the ADMS section on ngspice web site .
CIDER, XSPICE, and OpenMP may be selected at will.
–disable-debug will give O2 optimization (versus O0 for debug) and removes all debugging
info.
The install script will copy all files to C:\Spice or C:\Spice64, the code models for XSPICE
will be stored in C:\Spice\lib\spice or C:\Spice64\lib\spice respectively.
make install will create a directory tree as shown below:
32.2. NGSPICE COMPILATION UNDER WINDOWS OS 617
C:\Spice\
bin\
ngspice.exe
nghelp.exe
ngmakeidx.exe
ngnutmeg.exe
cmpp.exe
lib\
ngspice\
analog.cm
digital.cm
spice2poly.cm
extradev.cm
extravt.cm
share\
info\
dir
ngspice.info
ngspice.info-1
..
ngspice.info-10
man\
man1\
ngmultidec.1
ngnutmeg.1
ngsconvert.1
ngspice.1
ngspice\
helpdir\
ngspice.idx
ngspice.txt
scripts\
ciderinit
devaxis
devload
setplot
spectrum
spinit
Table 32.3: ngspice standard installation tree under MS Windows
The ./configure flag --enable-relpath may be useful if the install path (e.g. C:\Spice64) is
only preliminary, because a Windows installer is preferred. Then all search paths for spinit and
code models are made relative to the executable (either ngspice.exe or the caller to ngspice.dll),
see 32.1.5.
618 CHAPTER 32. COMPILATION NOTES
32.2.4 make ngspice with pure CYGWIN
The procedure of compiling is the same as with Linux (see Chapt. 32.1). After you have moved
to the ngspice directory, the following command sequence may do the work for you:
$ ./autogen.sh
$ mkdir release-cyg
$ cd release-cyg
$ ../configure --with-x --disable-debug --with-readline=yes --enable-xspice
--enable-pss --enable-cider --enable-openmp
$ make clean 2>&1 | tee make_clean.log
$ make 2>&1 | tee make.log
$ make install 2>&1 | tee make_install.log
The CYGWIN console executable you have been creating is an X11 application. This is a not
a Windows native environment. So you have to add an X11 graphics interface by installing the
XServer from the CYGWIN project. Before starting ngspice, you have to start the XServer by
the following commands within the CYGWIN window:
$ export DISPLAY=:0.0
$ xwin -multiwindow -clipboard &
If you don’t have libdl.a you may need to link libcygwin.a to libdl.a symbolically, for example:
$ cd /lib $ ln -s libcygwin.a libdl.a.
32.2.5 ngspice mingw or cygwin console executable w/o graphics
If you omit the configure flag –with-wingui or –with-x, you will obtain a console application
without graphics interface.
./configure --enable-xspice --enable-cider --enable-openmp
--disable-debug CFLAGS=-m32 LDFLAGS=-m32 prefix=C:/Spice
is an example for TDM mingw, 32 Bit ngspice console. No graphics interface is provided. A
warning message will be issued upon starting ngspice. However, you may invoke for plotting
(see 17.5.28).
32.2.6 ngspice for MS Windows, cross compiled from Linux
The ngspice main directory contains two scripts that provide cross compiling ngspice.exe or ng-
spice.dll from a Linux setup. For details and prerequisites please have a look at cross-compile.sh
or cross-compile-shared.sh.
32.3. REPORTING ERRORS 619
32.2.7 make ngspice with CYGWIN and external MINGW32
The next two compilation options are deprecated and not tested any more!
according to http://www.geocrawler.com/lists/3/SourceForge/6013/0/7321042/
$ cd ngspice
$ export PATH="/cygdrive/g/gcc_mingw/bin:$PATH"
$ autoconf
$ rm config.cache
$ ./configure --with-wingui --prefix="/cygdrive/g/gcc_mingw/bin"
$ make clean
$ make 2> make.err
$ cp config.h config_ming.h
ngspice.exe is ok, but make tests does not work (cannot direct console output into file).
Needs to add .save ‘what’ ‘where.test’ to every input (*.cir) file. Also all given output files
have to be adapted to Windows (CR/LF instead of only LF at each line ending) for allowing
proper comparison.
32.2.8 make ngspice with CYGWIN and internal MINGW32 (use con-
fig.h made above)
$ cd ngspice
$ rm config.cache
$ export CFLAGS="-mno-cygwin -g -O2"
$ export LDFLAGS="-L/lib/mingw"
$ export CPPFLAGS="-I/usr/include/mingw"
$ ./configure --with-wingui
$ cp config_ming.h config.h
$ make clean
$ make 2> make.err
./configure does not work correctly: It finds headers and libs that are not really available in
the -mno-cygwin port of MINGW32. Therefore config.h is not ok.
To-Do: find appropriate presets for variables ? rewrite tests for headers and libs (search exclu-
sively in mingw directories)
32.3 Reporting errors
Setting up ngspice is a complex task. The source code contains over 1500 files. ngspice should
run on various operating systems. Therefore errors may be found, some still evolving from the
original spice3f5 code, others introduced during the ongoing code enhancements.
620 CHAPTER 32. COMPILATION NOTES
If you happen to experience an error during compilation of ngspice, please send a report to the
development team. Ngspice is hosted on sourceforge, the preferred place to post a bug report is
the ngspice bug tracker. We would prefer to have your bug tested against the actual source code
available at Git, but of course a report using the most recent ngspice release is welcome! Please
provide the following information with your report: Ngspice version, Operating system, Small
input file to reproduce the bug (if to report a runtime error), Actual output versus the expected
output.
Chapter 33
Copyrights and licenses
33.1 Documentation license
33.1.1 Spice documentation copyright
Copyright 1996 The Regents of the University of California.
Permission to use, copy, modify, and distribute this software and its documentation for educati-
onal, research and non-profit purposes, without fee, and without a written agreement is hereby
granted, provided that the above copyright notice, this paragraph and the following three para-
graphs appear in all copies. This software program and documentation are copyrighted by The
Regents of the University of California. The software program and documentation are supplied
‘as is’, without any accompanying services from The Regents. The Regents does not warrant
that the operation of the program will be uninterrupted or error-free. The end-user understands
that the program was developed for research purposes and is advised not to rely exclusively on
the program for any reason.
IN NO EVENT SHALL THE UNIVERSITY OF CALIFORNIA BE LIABLE TO ANY PARTY
FOR DIRECT, INDIRECT, SPECIAL, INCIDENTAL, OR CONSEQUENTIAL DAMAGES,
INCLUDING LOST PROFITS, ARISING OUT OF THE USE OF THIS SOFTWARE AND
ITS DOCUMENTATION, EVEN IF THE UNIVERSITY OF CALIFORNIA HAS BEEN AD-
VISED OF THE POSSIBILITY OF SUCH DAMAGE. THE UNIVERSITY OF CALIFORNIA
SPECIFICALLY DISCLAIMS ANY WARRANTIES, INCLUDING, BUT NOT LIMITED
TO, THE IMPLIED WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PAR-
TICULAR PURPOSE. THE SOFTWARE PROVIDED HEREUNDER IS ON AN "AS IS" BA-
SIS, AND THE UNIVERSITY OF CALIFORNIA HAS NO OBLIGATIONS TO PROVIDE
MAINTENANCE, SUPPORT, UPDATES, ENHANCEMENTS, OR MODIFICATIONS.
33.1.2 XSPICE SOFTWARE (documentation) copyright
Code added to SPICE3 to create the XSPICE Simulator and the XSPICE Code Model Subsy-
stem was developed at the Computer Science and Information Technology Laboratory, Georgia
Tech Research Institute, Atlanta GA, and is covered by license agreement the following copy-
right:
621
622 CHAPTER 33. COPYRIGHTS AND LICENSES
Copyright © 1992 Georgia Tech Research Corporation All Rights Reserved. This material may
be reproduced by or for the U.S. Government pursuant to the copyright license under the clause
at DFARS 252.227-7013 (Oct. 1988)
Refer to U.C. Berkeley and Georgia Tech license agreements for additional information.
This license is now superseded by Chapt. 33.2.2
33.1.3 CIDER RESEARCH SOFTWARE AGREEMENT (superseded by
33.2.1)
This chapter specifies the terms under which the CIDER software and documentation coming
with the original distribution are provided. This agreement is superseded by 33.2.1, the ‘modi-
fied’ BSD license.
Software is distributed as is, completely without warranty or service support. The University of
California and its employees are not liable for the condition or performance of the software.
The University does not warrant that it owns the copyright or other proprietary rights to all soft-
ware and documentation provided under this agreement, notwithstanding any copyright notice,
and shall not be liable for any infringement of copyright or proprietary rights brought by third
parties against the recipient of the software and documentation provided under this agreement.
THE UNIVERSITY OF CALIFORNIA HEREBY DISCLAIMS ALL IMPLIED WARRAN-
TIES, INCLUDING THE IMPLIED WARRANTIES OF MERCHANTABILITY AND FIT-
NESS FOR A PARTICULAR PURPOSE. THE UNIVERSITY IS NOT LIABLE FOR ANY
DAMAGES INCURRED BY THE RECIPIENT IN USE OF THE SOFTWARE AND DOCU-
MENTATION, INCLUDING DIRECT, INDIRECT, SPECIAL, INCIDENTAL, OR CONSE-
QUENTIAL DAMAGES.
The University of California grants the recipient the right to modify, copy, and redistribute the
software and documentation, both within the recipient’s organization and externally, subject to
the following restrictions:
(a) The recipient agrees not to charge for the University of California code itself. The recipient
may, however, charge for additions, extensions, or support.
(b) In any product based on the software, the recipient agrees to acknowledge the research group
that developed the software. This acknowledgment shall appear in the product documentation.
(c) The recipient agrees to obey all U.S. Government restrictions governing redistribution or
export of the software and documentation.
All BSD licenses have been changed to the ‘modified’ BSD license by UCB in 1999 (see Chapt.
33.2.1).
33.2 ngspice license
The SPICE license is the ‘Modified’ BSD license, (see http://embedded.eecs.berkeley.edu/pubs/downloads/spice/index.htm).
ngspice adopts this ‘Modified’ BSD license as well for all of its source code (except for tclspice
and numparam that are under LGPLv2, and XSPICE, which is public domain (see 33.2.2)).
*****************************************************************************
33.2. NGSPICE LICENSE 623
Copyright (c) 1985-1991 The Regents of the University of California.
All rights reserved.
Permission is hereby granted, without written agreement and without license or royalty fees, to
use, copy, modify, and distribute this software and its documentation for any purpose, provided
that the above copyright notice and the following two paragraphs appear in all copies of this
software.
IN NO EVENT SHALL THE UNIVERSITY OF CALIFORNIA BE LIABLE TO ANY PARTY
FOR DIRECT, INDIRECT, SPECIAL, INCIDENTAL, OR CONSEQUENTIAL DAMAGES
ARISING OUT OF THE USE OF THIS SOFTWARE AND ITS DOCUMENTATION, EVEN
IF THE UNIVERSITY OF CALIFORNIA HAS BEEN ADVISED OF THE POSSIBILITY
OF SUCH DAMAGE. THE UNIVERSITY OF CALIFORNIA SPECIFICALLY DISCLAIMS
ANY WARRANTIES, INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRAN-
TIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE. THE
SOFTWARE PROVIDED HEREUNDER IS ON AN "AS IS" BASIS, AND THE UNIVER-
SITY OF CALIFORNIA HAS NO OBLIGATION TO PROVIDE MAINTENANCE, SUP-
PORT, UPDATES, ENHANCEMENTS, OR MODIFICATIONS.
*****************************************************************************
33.2.1 ‘Modified’ BSD license
All ‘old’ BSD licenses (of SPICE or CIDER) have been changed to the ‘modified’ BSD license
according to the following publication
(see ftp://ftp.cs.berkeley.edu/pub/4bsd/README.Impt.License.Change):
July 22, 1999
To All Licensees, Distributors of Any Version of BSD:
As you know, certain of the Berkeley Software Distribution (‘BSD’) source code files require
that further distributions of products containing all or portions of the software, acknowledge
within their advertising materials that such products contain software developed by UC Berke-
ley and its contributors.
Specifically, the provision reads:
‘3. All advertising materials mentioning features or use of this software must display the follo-
wing acknowledgment: This product includes software developed by the University of Califor-
nia, Berkeley and its contributors.’
Effective immediately, licensees and distributors are no longer required to include the ackno-
wledgment within advertising materials. Accordingly, the foregoing paragraph of those BSD
Unix files containing it is hereby deleted in its entirety.
William Hoskins
Director, Office of Technology Licensing
University of California, Berkeley
624 CHAPTER 33. COPYRIGHTS AND LICENSES
33.2.2 XSPICE
According to http://users.ece.gatech.edu/mrichard/Xspice/ (as of Feb. 2012) the XSPICE source
code and documentation have been put into the public domain by the Georgia Institute of
Technology.
33.2.3 tclspice, numparam
Both software packages are copyrighted and are released under LGPLv2
(see http://www.gnu.org/licenses/lgpl-2.1.html).
33.2.4 Linking to GPLd libraries (e.g. readline, fftw, table.cm):
The readline manual at http://tiswww.case.edu/php/chet/readline/rltop.html states: Readline is
free software, distributed under the terms of the GNU General Public License, version 3. This
means that if you want to use Readline in a program that you release or distribute to anyone, the
program must be free software and have a GPL-compatible license.
According to http://www.gnu.org/licenses/license-list.html, the modified BSD license, thus
also the ngspice license, belongs to the family of GPL-Compatible Free Software Licen-
ses. Therefore the linking restrictions to readline, which have existed with the old BSD license,
are no longer in effect.

Navigation menu