The Cyber-Spy.Com Usenet Archive Feeds Directly
From The Open And Publicly Available Newsgroup
This Group And Thousands Of Others Are Available
On Most IS NNTP News Servers On Port 119.
Cyber-Spy.Com Is NOT Responsible For Any Topic,
Opinions Or Content Posted To This Or Any Other
Newsgroup. This Web Archive Of The Newsgroup And
Posts Are For Informational Purposes Only.
From: Jim Thompson
Subject: Re: Transient Analysis in SPICE
X-Newsreader: Forte Agent 1.91/32.564
Date: Fri, 10 Jan 2003 21:42:06 GMT
NNTP-Posting-Date: Fri, 10 Jan 2003 16:42:06 EST
Organization: Cox Communications
On Thu, 09 Jan 2003 13:18:22 -0800,
In Newsgroup: sci.electronics.cad,
Entitled: "Re: Transient Analysis in SPICE",
Wrote the following:
|On Thu, 09 Jan 2003 16:09:02 +0000, Paul Burridge
|>I'm having to carry out several simulations on an RF amplifier that
|>takes typically seems to take at least 0.2 seconds to 'settle down' to
|>a steady output signal. So I'm looking to sample the output from say
|>from 0.2s to 0.202s at a small enough time-step to be able to just
|>about see individual cycles. So I set my start time for 0.2 seconds
|>and enter the other time commands as above. Problem is, I'm staring at
|>a blank screen for anything up to 15 minutes before the program
|>reaches the bit I'm interested in and starts to plot it. This is very
|>frustrating. Does anyone know of a way of 'fast-forwarding' to the
|>desired stretch of waveform without racing past it too fast to see
|>what's going on in detail within the actual desired section?
|>When you have to do this over and over again it's enough to drive you
|I ran into this when doing transient testing on switching power
|supplies. It was frustrating to wait for the circuit to settle down.
|I devised a way to quicken settling time, and typed myself an
|application note so I could remember what to do.
|Although these steps are PSPICE specific, other engines may similar
|TRANSIENT RESPONSE AND SETTLING TIME
|Transient response tests proceed quicker if the nodes are pre-charged.
|The 'IC=' attributes can be set for each inductor & capacitor on the
|schematic, but this becomes a cumbersome process if many nodes are
|involved, or the desired pre-charge needs to be changed.
|PSPICE does not have an automated way to do this. The 'SAVE BIAS'
|function in PSPICE SCHEMATICS creates a SPICE '.NODESET' file, which
|is not used in TRANSIENT simulations.
|However, the following procedure creates an IC table by using a data
|file that PSPICE generates, with changes to make it function as a
|SPICE '.IC' table.
|1) Clear any IC values assigned to capacitors and inductors.
|2) Set up a transient analysis that will settle out when finished (ie,
|fixed conditions and/or a 'long' simulation time).
|3) In the 'Transient Analysis' window, clear the option for 'Skip
|initial transient solution' (an intitial transient solution _should_
|4) Set PSPICE to record node voltages and currents at the end of the
|transient analysis by:
|- Selecting 'ANALYSIS-SETUP', and check the box next to 'SAVE BIAS
|- Press the 'SAVE BIAS POINT' button.
|- Enter a descriptive name in the TRAN filename box, such as
|- Enter the time at which the node voltages should be saved in the
|'Time' box. This is usually the same time as the length of the
|transient analysis. If the simulation is a switching power supply, it
|helps to make the 'save time' a whole number of PWM cycles.
|- Press 'OK' and 'Close' to exit the windows.
|5) Run the transient analysis.
|6) Using a text editor, open the file PSPICE created (in this case
|'NOMINAL.BP'), and replace the SPICE keyword '.NODESET' with the
|Save the altered file under another name, such as 'NOMINAL.IC'.
|7) In PSPICE SCHEMATICS, include this new file in the next simulation
|run by selecting the menu entry 'ANALYSIS-LIBRARY AND INCLUDE FILES'.
|Enter the file name 'NOMINAL.IC' as an 'INCLUDE' file.
|If no other node voltage recording is required, the 'SAVE BIAS POINT'
|function can be cleared.
|The next time the simulation is run, PSPICE will take the '.IC' values
|and insert them into the file for processing.
|(remove .spamtrap to reply)
The only thing I would do differently... I tend to put only globally
used libraries and includes files in the Analysis/Library and Include
Files area. For schematic-specific files I use the "LIB" and
"INCLUDE" parts and place them on the simulation page of the
schematic. (I'm often varying these entries to handle process
corners, and I use "INCLUDE" to pass client-provided cells/subcircuits
into my portion of the system.)
Pat, Drop me an E-mail and I'll provide you with a contact name in
PSpice support. You should send this in to them, maybe they'll post
it on their solutions page. (They ought to make this a feature by
adding check boxes in the SAVE/LOAD Bias areas.)
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| Jim-T@analog_innovations.com Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
For proper E-mail replies SWAP "-" and "_"
I love to cook with wine. Sometimes I even put it in the food.
Go Back To The Cyber-Spy.Com
Usenet Web Archive Index Of
The sci.electronics.design Newsgroup