SPICE 2/IsSpice4 Differences | User Interface | Netlist Construction | Error Checking | New Models Written in C |
New or Improved SPICE Elements | New or Improved Analysis Capabilities | Enhanced Program Output Features |
Additions over Berkeley SPICE 3F.5 | Syntax Changes | Obsolete SPICE Syntax

IsSpice4 Enhancements
Differences Between IsSpice4 and Berkeley SPICE

About IsSpice4

Berkeley SPICE 3A.7 was released in 1984. It was one of the first attempts by the University of California at Berkeley to enhance the standard version of SPICE used around the world, SPICE 2G.6. Since that time, “version 3” has gone through a number of major revisions. However, it was not until version 3E.2, which was released in early 1992, that there was a viable replacement for SPICE 2G.6. This is due to the fact that 3E.2 was the first version of Berkeley SPICE 3 to contain virtually all of the capabilities of SPICE 2G.6. IsSpice3 was the first SPICE program in the marketplace to be based on SPICE 3E.2 when it was released in 1992. Some SPICE vendors have chosen to upgrade their SPICE 2G.6 versions by adding pieces of SPICE 3. Intusoft has chosen to provide a simple and powerful one-step upgrade to the new standard in simulation.

With IsSpice4, Intusoft has added a variety of interactive features, making it the only SPICE 3 simulator with truly interactive performance. The latest revision of IsSpice4 now includes a number of extensions available in XSPICE, a derivative of Berkeley SPICE produced by the Georgia Technology Research Institute.

In addition to porting SPICE3 to the PC, and a command-line version for UNIX, Intusoft has added vast enhancement above and beyond Berkeley's version. The following paragraph detail some of the differences between Intusoft’s implementation, IsSpice4, which is currently based on Berkeley SPICE 3F.5, and previous versions of SPICE.

SPICE 2/IsSpice4 Differences

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)