|
IsSpice4 is a derivative of Berkeley SPICE
3F.5 and XSPICE. There are a number of major differences between IsSpice4,
past IsSpice versions, and other competitive
versions of SPICE. (Top)
User
Interface
|
IsSpice4
is completely interactive.
Simulations can be started, stopped, paused and resumed on demand.
New analyses can be run at any time. Virtually any component or
model parameter can be hand tweaked, individually or in groups,
and the circuit can be instantly resimulated. Voltage, current,
and power dissipation waveforms may be displayed at any time.
IsSpice4 contains
hot links to schematic
entry programs and IntuScope,
allowing simulation data to be available to the schematic for
interactive cross-probing, or to the post-processor for instant
display even during an analysis.
IsSpice4 displays
multiple real time waveforms from the AC, DC, Transient, Distortion,
and Noise analyses while the simulation runs. This is in contrast
to other SPICE versions which display only the timestep and the
data for one waveform.
IsSpice4 contains
a powerful set of interactive commands that provide access to
Print Expressions, Device parameter summaries, Simulation Breakpoints,
and Control loops. Complete “Simulation Scripts” can
be written to perform multiple analyses, check for Simulation
Breakpoints, and alter various parameters between each analysis.
(Top)
|
Netlist
Construction
- Model names and reference designations
can use more than 8 characters. IsSpice4 input netlists may
be in upper or lower case, or a mixture of both.
- IsSpice4 accepts names in place
of node numbers.
- Negative capacitor and inductor
values may be used.
- IsSpice4 automatically converts
some behavioral PSpice® syntax and all SPICE 2 dependent
source (E, F, G, H) polynomial syntax to the (B) nonlinear dependent
source syntax, allowing backward compatibility with any model
library using dependent sources.
- Improved support for parameter
passing including .PARAM statements, multiple level passing
of parameters, expressions in the main circuit, and general
PSpice syntax compatibility. (Top)
|
Error
Checking
| Errors
are placed in the Errors and Status window and in a file with the
same name as the input netlist and the extension .ERR. For example,
if the input is Sample.Cir, the error file will be Sample.Err. Some
errors may also be repeated in the IsSpice4 output file. If the
simulation aborts or the data looks drastically incorrect, you should
check the filename.ERR file for a summary listing of errors. This
is in contrast to SPICE 2, which places the errors in the output
file. (Top) |
New
Models Written in C
| Code models
are a new type of SPICE model, created using a publicly available
AHDL (Hardware
Description Language) based on the C
programming language. The code describing the model’s behavior
is linked to the simulator via an external DLL file (CML.DLL) rather
than being bound within the executable program. This allows new
primitive models to be added to the simulator, and old models changed,
without having to recompile IsSpice4. You can add your own code
models to IsSpice4 using the Intusoft
Code Modeling Kit. The modeling kit produces a DLL which can
be read by any IsSpice4 program. Over 45 new analog, digital, real
and mixed analog/digital code models are included in IsSpice4. (Top) |
New
or Improved SPICE Elements
|
A variety of new analog behavioral capabilities
are included in IsSpice4. The nonlinear dependent source element
(B) allows you to access in-line equations using algebraic, trigonometric
or transcendental operators, node voltages and currents. If-Then-Else
functions and Boolean logic expressions, useful for mixed-mode
simulation, can also be entered directly.
A variety of new models are included
in the IsSpice4 program:
- Lossy transmission line model
using a distributed approach (RC, RG, LC, and RLC combinations)
- Uniformly distributed RC/RD transmission
line model
- Additional GaAs Mesfet models
based on Statz, Curtis-Ettenburg, Parker-Skellern, and others
- Mosfet models:BSIM3v3.2.4
assigned to level=7-8.
BSIMSOIv3.2 (Silicon-On-Insulator) assigned to level=10.
BSIM4.4.0 assigned to level=14-15.
- Smooth transition switch
- Voltage and current-controlled
switches with hysteresis
- Semiconductor resistor and capacitor
.MODEL statements
- Improved MOSFET level 2 model
(capacitance response)
- New JFET model (several new parameters)
- Improved lossless transmission
line model (Dynamic breakpoint table with minimum breakpoint
spacing control) (Top)
|
New
or Improved Analysis Capabilities
|
IsSpice4 includes a 12-state digital logic
simulator which provides Native Mixed-Mode simulation capability.
Event-driven
simulation algorithms are also provided for real data, which
allows sampled data filters to be simulated.
You can ask IsSpice4 to stop the
simulation when a voltage, current, or a computed device parameter
meets a particular condition. Simulation Breakpoints can be used
to test for a variety of conditions including device breakdown,
safe operating area, and time-dependent events, all while the
simulation is running.
IsSpice4 includes a Simulation
Template features that allows the simulation to be driven
via ICL scripts. Simulation Templates are included for RSS,
EVA, Worst
Case, and Sensitivity analyses.
All of these analyses can be used in conjunction with AC, DC,
Transient and operating analyses.
Pole-Zero transfer function analysis
has been added.
Automatic Stress Alarms and User-defined
Measurements.
The individual operating temperature
of a single device can be set to a different value than the overall
circuit temperature. This allows simulation of a “hot”
component. Temperature sweeps can be run for virtually any parameter.
Improvements have been made in the
DC analysis and distortion analysis (all active components have
distortion).
The DC and transient convergence
properties of IsSpice4 have been greatly improved through the
addition or enhancement of:
- Gmin stepping/Source Stepping
algorithms
- Independent Supply Ramping algorithms
- Improved program defaults, LIMPTS/ITL5
no longer needed
- Alternate UIC algorithm
- Automatic conductance from every
node to ground (Top)
|
Enhanced
Program Output Features
- Real-time viewing and printing of a
wide variety of computed device parameters such as device power
dissipation, inductor flux, BJT Vbe, and FET transconductance,
to name a few. (For BOTH the operating point AND the Transient
analysis, see Appendix B in the on-line help for a full summary
listing)
- Access to ALL node voltages, the
power dissipation of any component, and the current through
any component, without the need for extra voltage sources.
- Expressions using voltages, currents,
computed device parameters and a variety of mathematical functions
can be viewed on-screen immediately after the IsSpice4 run,
or saved to the output file for viewing in IntuScope.
- Computed device parameters, voltages,
currents and expressions are all available for devices which
are within subcircuits.
- Powerful “Show” and
“Showmod” functions provide summary printouts of device
and model operating point information.
- Save option using the CSDF format
for compatibility with Viewlogic ViewTrace, PSpice Probe and
other post processor products. (Top)
|
Additions
over Berkeley SPICE 3F.5
|
In addition to the enhancements over the
Berkeley SPICE 2G.6 version, Intusoft has added a number of major
features to IsSpice4 that are not found in Berkeley SPICE 3F.5.
- A graphical interface that allows
the user to easily interact with the simulator and pop-up help
menus to support all of the SPICE 3, Nutmeg, and ICL commands.
- IsSpice4 features “Real-Time
View Windows” that display voltage, current and computed
device parameters from the AC, DC, Transient, Distortion, and
Noise analyses as the program runs. A new control statement,
“.VIEW”, has been added to provide control of the
waveform scaling.
- XSPICE enhancements including:
full native mixed-mode simulation, support for user-defined
C subroutines (Code Models), AHDL language based on C, and over
40 new code model primitives.
- The Nutmeg and SPICE3 interactive
control commands (Alias, Alter, Let, Save, Set, Show, Showmod,
Stop, and Control Loop) have been vastly augmented.
- The SPICE 3 B element (arbitrary
dependent source) supports Boolean logic expressions and an
If-Then-Else statement which is useful for a variety of functions,
including table-type representations.
- New JFET and HEMT model, (Parker
model) based on the work of Macquarie University in Australia
has been added.
- A model current convergence test
has been added. This may make convergence more difficult in
some cases, but eliminates the need for the "OFF"
keyword in many instances.
- The Lossy Transmission Line has
frequency dependence (skin effect/dielectric loss) in the time
and frequency domains.
- R, L, C, B, and O expressions
can use frequency, time and temperature.
- B elements accept expressions
which are functions of device currents in the time and frequency
domains.
- A number of bugs in the interactive
control language, memory management, distortion analysis, device
models, and data output areas of Berkeley SPICE 3F.5 have also
been corrected. (Top)
|
Syntax
Changes
- Temperature coefficients are no longer
included on the resistor call line. Resistor temperature coefficients
are now inserted in a resistor .MODEL statement.
- The MOSFET parameter XQC is ignored
since an improved Meyer capacitance model is used all of the
time.
- The .NOISE and .DISTO statements
have new syntax requirements. SPICE 2 .NOISE and .DISTO syntax
is not compatible. See the .NOISE and .DISTO syntax in Chapter
10 for more information.
- The .TEMP statement is not recognized.
To change the circuit temperature, use the .OPTIONS TEMP= parameter
or the set temp = ICL command. Multiple runs at several temperatures
are fully supported. In addition, a different temperature can
be set on each individual device during a single simulation.
- Several .OPTIONS parameters have
been added to support the “Real-Time View Windows”
and the Boolean logic expressions in the analog behavioral element
B. See the .OPTIONS statement for more information.
- Several .OPTIONS parameters have
been added to support the native mixed-mode simulation features.
(Top)
|
Obsolete
SPICE 2 Functions
|
Polynomial capacitors/inductors (using
the POLY keyword) are not supported, although polynomial elements
can be created using behavioral expressions, subcircuits, the
new B element or code models.
Several unnecessary .OPTIONS parameters
(ITL5, LIMPTS, etc.) have also been removed.
Several separate input circuit netlists
may not be included in the same input file and simulated batch
style. (Top)
|
|
