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.
Subject: Re: Transient Analysis in SPICE
Date: Thu, 09 Jan 2003 13:18:22 -0800
X-Newsreader: Forte Agent 1.93/32.576 English (American)
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)
Go Back To The Cyber-Spy.Com
Usenet Web Archive Index Of
The sci.electronics.design Newsgroup