Dec 302017
 
PSPICE for OS/2. Part 1 of 2. For designing electronic circuitry. A PC Classic.
File PSPICEP1.ZIP from The Programmer’s Corner in
Category OS/2 Files
PSPICE for OS/2. Part 1 of 2. For designing electronic circuitry. A PC Classic.
File Name File Size Zip Size Zip Type
EXAMPLE1.OUT 40536 9152 deflated
PSPICE.CMD 73 69 deflated
PSPICE.HLP 34062 11519 deflated
PSPICE.NDX 2357 1049 deflated
PSPICE1.EXE 830894 334964 deflated
README.DOC 15316 5673 deflated
STMED.EXE 455636 190451 deflated
STMED.HLP 6755 2162 deflated

Download File PSPICEP1.ZIP Here

Contents of the README.DOC file


1.0) Introduction

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
completion.

Execute PSpice by using the following command format:

PSPICE [] [] [/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.


 December 30, 2017  Add comments

Leave a Reply