This file describes the version modifications to the
PSpice software and installation and operation instructions
for the IBM OS/2 evaluation package.
2.0) System Requirements
PSpice will run on any 80286/80386/80486 based PC with an
8087/'287/'387 floating-point coprocessor (optional for the
evaluation version), the OS/2 operating system, and a minimum
of 2 megabytes of memory (for the OS/2 operating system).
PSpice will run on a system with 2 megabytes of memory, but the
program will be swapping back and forth to disk due to the
virtual memory. We recommend that your system have 4 megabytes
of memory in order for the PSpice package to run efficiently.
An IBM hardware-level compatible color graphics display must
be used (CGA, EGA, or VGA) and no special brand of printer or
special printer features are needed.
PSpice will also run on IBM-compatible systems as long as they
meet the above requirements.
3.0) Installation Instructions
Installing PSpice from either the 5" or 3" diskettes is
similar. Copy all of the files from the diskettes onto the
fixed disk in the directory where you normally keep your
program files. For the 3" diskettes only, you need to rebuild
PSPICE1.EXE by invoking the MAKESPIC command in that directory,
and observing that the MAKESPIC command terminates successfully.
The CONFIG.SYS file in the ROOT directory configures the system
when it is booted. If you do not have a CONFIG.SYS (some
versions of OS/2 use the file CONFIG.OS2) file currently on
your system, use the one included with the PSpice package.
Otherwise, update your CONFIG.SYS file to contain the commands
in the PSpice CONFIG.SYS file, in order for the PSpice package
to execute properly.
A PROBE.DEV file needs to be created defining the display type,
printer port, and printer type of your computer system. This
can be done very easilyby running the Control Shell (PS.EXE),
selecting the Probe Menu, and then choosing the Setup option.
Menus will guide you through the operation allowing you to
select the appropriate devices.
4.0) Operating Instructions
Running PSpice is straightforward. The file PSPICE.CMD must be
in either the default directory, or a directory which was
included in an earlier PATH command (see your OS/2 User's Guide
for using the PATH command).
Running PSpice causes PSPICE.CMD to first call PSPICE1.EXE
and then PROBE.EXE, if you have included a .PROBE statement in
your circuit file. PSPICE1.EXE creates several temporary files
for storing intermediate results, but deletes them on
Execute PSpice by using the following command format:
] [ ] [/B] By default, the input file has the extension of .CIR and the output file has the extension of .OUT. The name of the output file defaults to the name of the input file. So, these are all equivalent: PSPICE EXAMPLE1 PSPICE EXAMPLE1.CIR PSPICE EXAMPLE1.CIR EXAMPLE1 PSPICE EXAMPLE1.CIR EXAMPLE1.OUT PSPICE EXAMPLE1.CIR EXAMPLE1.OUT PROBE.DAT The output file can also be the name of your system's printer by using the printer name for the output name, for example PSPICE EXAMPLE1 PRN Try running PSpice using the example circuit file, EXAMPLE1.CIR, which was included with the package. Type PSPICE EXAMPLE1 After a short time, the screen should be cleared and redrawn with a status display. If this does not happen, verify - that PSPICE1.EXE is in the default directory or in a directory contained in the current path, - that EXAMPLE1.CIR exists in the default directory, and - that PSPICE.CMD is in a directory that OS/2 will search for programs and commands. Let EXAMPLE1 run to completion (about 5 minutes on an IBM-PC/AT). PSpice generates an output file with the same filename as the input file, but with a .OUT extension (in this case EXAMPLE1.OUT). Compare the generated EXAMPLE1.OUT file with the EXAMPLE1.OUT file that was included with your package. 5.0) Program changes from version 4.00 to the present 4.03January 1990 PSpiceOver 160 Zener diode models, 30 opamps from Linear Technology, 106 opamps from Texas Instruments, and over 30 three terminal regulators have been added to the library. New diode model parameters have been added: Model Parameters Units Default ---------------------------------------------------------------------------- NBV reverse breakdown ideality factor 1 IBVL low-level reverse breakdown "knee" current amp 0 NBVL low-level reverse breakdown ideality factor 1 TBV1 BV temperature coefficient (linear) C-1 0 TBV2 BV temperature coefficient (quadratic) C-2 0 New Bipolar Transistor model parameters have been added: Model Parameters Units Default ---------------------------------------------------------------------------- QCO epitaxial region charge factor coulomb 0 RCO epitaxial region resistance ohm 0 VO carrier mobility "knee" voltage volt 10 GAMMA epitaxial region doping factor 1E-11 If the model parameter RCO is specified, then quasi-saturation effects are included. MonteThe Worst Case analysis has changed so that it will honor CarloLOT/n and LOT tolerance tracking model parameters. The LIST option is now valid for .WCASE. Specifying LIST will print out a list of devices and model parameters, and their associated values. The distributions on tolerances will be taken into account during the worst case run. The DEV/n form of tolerances is ignored by .WCASE and is treated as a DEV tolerance. .MC treats DEV/n as it did before. Note that the DEV/n form might be eliminated in a future release. The BY keyword is syntactically legal but has no effect on the simulation. BY will be eliminated in a future release. The Monte Carlo, Sensitivity, and Worst Case Summaries provide additional information: the Monte Carlo and Worst Case Summaries print the current run's value as a percentage of the nominal run. The Sensitivity Summary prints the percent change of the output value per percent change in the model parameter. StmedWhen used with an existing circuit file, the Stimulus Editor will initially display only the first four analog and the first four digital stimuli. To display or modify other stimuli in the file, use the Display_stimulus command in the Plot Control Menu. An "All" option has been added to the Display_stimulus, Undisplay_stimulus, and Delete_stimulus menu commands. ProbeThe use of macros has been added. Minimum and maximum (MIN(x) and MAX(x)) arithmetic functions have been added. Some of the Display Control functions have been slightly modified. When requesting a RESTORE, before the restoration is done, the screen attributes are automatically saved under the display name LAST_DISPLAY, even when there is not a trace on the display. When you exit Probe with any traces displayed, the screen attributes are automatically saved under the display name LAST_SESSION. In the X_axis selection, a calculation range can now be specified instead of the calculation being done on the entire data set. The command is Restrict_data and will set a range for any range oriented function, such as an FFT, s(x), AVG(x), etc. When defining a trace, an existing trace can be used as a variable within the new trace expression. The existing trace is defined as # . When a trace is requested to be deleted, a check is done on whether the trace is used within another trace expression. If it is, a warning message is displayed asking you to verify the delete. If you choose to delete a trace used within other trace expressions, the trace is deleted along with all the trace expressions using that trace. When a trace is deleted, the other traces will be renumbered as needed. Under the Start-up Menu, a Section Selection Menu appears when multiple sections exist for the analysis selected. This displays all of the available sections and provides an easy access menu to make your selections. The optional use of a mouse has been added to position the cursor. The Mid-Analysis "Snoop" of Results allows you to look at digital waveforms as well as analog. The fast cursor for the DOS/16M version of PSpice has been fixed. ControlThe file size within the Browse function has been increased Shellfrom 16Kbytes to 1.5Mbytes, which is typically 32,000 lines. The editor file size has been increased from 16Kbytes to 32Kbytes. An external browser can be defined, just like an external editor. The menu selections have been modified to include an ellipsis (...) for those selections which have further menu prompts. Those functions without an ellipsis will execute upon selection. Probe no longer executes automatically within the Control Shell unless the Auto_run selection has been chosen in the Probe menu. When in the editor, the line and column numbers are displayed indicating the cursor position within the file. Also while in the editor, a flag is displayed indicating whether in insert or overstrike mode. The PSpice version number is now displayed at the top of the screen. DigitalPrimitives have been generated for both a Multi-Bit Analog Simulationto Digital converter and a Multi-Bit Digital to Analog converter. CD4000 series CMOS parts and miscellaneous TTL parts have been added to the digital library. 4.02July 1989 PSpiceAn optocoupler library was added to PSpice. The library index system was re-written. There are no changes in how to use the libraries, but searching the library files is now much faster. A .FUNC command was added. This allows functions to be defined for use in expressions. Functions can take up to 10 arguments. The internal numerics of the non-linear magnetics (K device) were improved. StmedA new program, STMED (STiMulus EDitor), was added for creating, deleting, and editing V and I devices. On the PC it can be invoked from the PSpice control shell. ProbeThe menus in Probe, Parts, and Stmed were changed to select items by first letter and by arrow keys. In Probe a new menu was added to allow a screen's attributes to be saved and restored. New drivers were added for the DEC GPX and IBM 8514 graphics displays. The LaserJet driver was augmented to handle A4 (metric) size paper. The first two characters output when the PostScript (PS) driver is used are "%!". When used in a system running TranScript the file will be automatically recognized as being a PostScript file. 4.01January 1989 Several corrections were made to PSpice, Probe, and Parts from version 4.00. There are no functional changes between versions 4.00 and 4.01. 4.00November 1988 PSpiceTwo new options, Analog Behavioral Modeling and Digital Simulation, were released. Worst Case and Sensitivity analysis was added to the Monte Carlo option. New collating functions - MAX, MIN, RISE_EDGE, FALL_EDGE - were added for both .MC and .WCASE. The device libraries were expanded to about 2200 analog components. PSpice now uses index files to find devices in a library file. If an index file does not exist or does match the library file, PSpice builds a new index file. On the PC (DOS and OS/2) and NEC PC an interactive control shell was added. The shell provides menus, on-line help, and interactive operation of PSpice. The MOS model has added a device "multiplier" parameter (M) which may be specified for each device (default = 1) in the netlist. The effect of "M" is like including M devices in in the netlist. In the following example: M17 3 5 9 9 W=20u L=1.2u M18 7 5 9 9 W=20u L=1.2u M=5 M18 is five times "bigger" than M17, which includes device currents and capacitances. Other modeling enhancements were made to support the expanded device libraries. The diode model has added parameters: IKFhigh-injection "knee" current (default = 0) If IKF > 0, the diode's forward current becomes Id' = Id * sqrt( IKF/(IKF+Id) ) ISRrecombination current parameter (default = 0) If ISR > 0, the diode's forward current becomes Id' = Id + area * ISR * exp( Vd/(NR*Vt) - 1 ) which simulates the generation current, and the diode's reverse current becomes inversely proportional to the junction capacitance (GMIN is not used) Id = area * ISR * ( 1-Vd/VJ )^M which simulates the recombination current. Temperature compensation for ISR follows the form of IS. NRemission coefficient for ISR (default = 2) TIKFlinear tempco for IKF TRS1linear tempco for RS TRS2quadratic tempco for RS The JFET model has added parameters: Njunction emission coefficient (default = 1) ISRrecombination current parameter (default = 0), see diode model (above) for explanation. NRemission coefficient for ISR (default = 2) ALPHAionization coefficient for "active" gate leakage. If ALPHA > 0 then the gate current, when the device is in saturation, has an added component Ig = Ig + ALPHA * vdif * exp( -VK/vdif ) where vdif = vds - vdsat This current is due to impact ionization from the channel carriers. VKionization "knee" voltage (default = 0) A .PARAM command was added to define parameters. The parameters can be used in expressions throughout the circuit file. Global nodes were added. Any node starting with "#" is treated as global. ProbeThe cursors were re-done. Instead of a command, the shift key chooses between the two cursors. Expressions with mistakes do not need to be re-typed. They can be edited instead. PartsAdditions to diode modeling that track advances in the PSpice diode model: IKF, ISR (see changes in PSpice). Added two-point data input for capacitance modeling. Additions to JFET modeling that track advances in the PSpice JFET model: ISR, VK, ALPHA, M (see changes in PSpice). Changes to bipolar transistor modeling: added two-point data input for capacitance modeling.