XSpice To Spice3 Converter

This program is free software; you may redistribute and/or modify it under the terms of the GNU General Public License Version 2 as published by the Free Software Foundation.

This program is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY, without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for complete details.

spicepp README

WHAT

spicepp is a preprocessor for berkeley spice3f5. It adds support for some structures commercial spices provide. Useful additions include .meas, .param, .lib, .globals, inline comments and equations Check out spicrprm also as a complementary package. Written under linux with perl 5.005_03, but any version will probably work.

WHY

These are good features that make spice easier to use. And I had some decks to run.

WHERE

Install .spicepp and measure_spice in a directory in your search path. I keep them in ~/bin. You will need perl. If you don't have perl (or a link to it) in /usr/local/bin , then edit the first line of these two scripts to point to your perl. Remember to make both these executable.

HOW

spicepp preprocesses a spice deck for spice version 3. It translates commands that hspice recognises into spice3f5 syntax. Use spicepp to translate your input spicedeck into a intermediate file, then process that intermediate file to spice3. for example:

spicepp  -i file.cir > file.ckt
spice3 file.ckt

spicepp (v1.3) preprocesses the spice deck.

measure_spice (v1.2) is invoked by spice to perform measurements on a data fils [meas.data] written by spice using control information written to meas.ctl. measure_spice logs results to the file spice.log.

You need to grab both. You can check the version number of each of these with the -h commandline flag.

Commands

The following commands may be used in the input spice deck.

.lib 'libfile' model

The library libfile is read. The content between the .lib and the .endl lines is included in the output spicedeck. This is often used for subckts, but may be any valid spice input. libfile should include path. There can be multiple .lib entries in library. Single quotes are required around the file name. Syntax within the library is:

   .LIB model
   <stuff>
   .ENDL

libraries can use parameters and equations - these have global scope. Global signals are also enforced through library code and subckts.

.param name=value [name2=value2 ....];

adds the ability to parametrize spice data. This may include component values, voltages, currents, etc. Equations are supported. Nodes are not. A value (data) used several times in the deck can be entered once (dataval) in the deck in the .param card.

.global nodel [node2 [node3 ... ]]

You may include the .globals card to allow global nodes in subckts This permits you to (typically) not worry about power supplies for subckts. global signals are automatically added to the instantiate line for subckts that use them.

.temp temperature

You may define temprature using the .temp card instead of the .options card.

$

As usual '*' in the first column is permitted for comments. Also - you can use '$' to comment to end of line.

.meas

You can have spice calculate the delay from one point to another. This may be useful for measuring the propogation delay for a circuit element, or ramptime for example Syntax is:

   .MEAS TRAN IO_LH_DELAY TRIG ADATA VAL=1.2 RISE=1
   +  TARG PIN   VAL=1.7  TD=20n      FALL=2

TRAN implies transient analysis (which is the only analysis currently supported) IO_LH_DELAY is the reported name of the measurement performed. Measurements are performed from the TRIGger time to the TARGet time. In the above example the trigger point is calculated as when the ADATA vector gets to a VALue of 1.2 volts RISEing for the first time. The Target value point is calculated when the PIN vector FALLs past a VALue of 1.7 volts for the second time (fall=2). Counting of target transitions starts at the TD time of 20 nS. The value reported is the difference the target time minus the trigger time. Measurements are recorded into the file spice.log. Spice records time and linearized waveforms into a temporary file, then invokes measure.spice to make the measurement. The measurement, the current time, and the analysis heading line are recorded in the 'spice.log' logfile.

Following are features rather than keywords.

-h

help flag may be given to spicepp to get version information.

-i

interactive flag may be given to spicepp. This just means spice does not exit automatically. You can use nutmeg to see whats happening and draw plots. Be aware that vectors are linearized prior to measurements being made, so if you have .meas lines you may need to repeat the tran analysis to be able to plot.

tran tstep tend will achieve your goal.

m=nn

Including the term m=5 in a component instantiation line includes 5 (for example) components in parallel in the final deck.

level

For a bsim3v3 mosfet model model, the level=49 statement is changed to the Berkeley level=8. Not all model parameters are recognised.

equations

Equations are supported. Surround equations with single quotes. For example val='vdd*0.50' In the above vdd is a parameter - which will be substituted before evaluation. Equations are not supported in .lib cards, they are ok in the library contents. Only one pass of equation expansion is performed, nested parameter equations probably won't work.

This is beta code - but I use it. Released under GPL. Please tell me about any bugs, or improvements.you make. john@reptechnic.com.au

John Sheahan

Last modified: Sat Jan 22 21:03:39 EST 2000