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.
Reply-To: "fred bartoli"
From: "fred bartoli"
Subject: Re: Flash a string of LEDs
Date: Thu, 5 Dec 2002 11:13:32 +0100
X-Newsreader: Microsoft Outlook Express 5.00.2314.1300
Organization: Guest of ProXad - France
NNTP-Posting-Date: 05 Dec 2002 11:10:30 MET
Terry Pinnell a écrit dans le message :
> "fred bartoli" wrote:
> >Terry Pinnell a écrit dans le message :
> >> It's a Spice issue, as it worked fine on breadboard with component
> >> values as per your/my circuit schematic (about 1 Hz).
> >> If Helmut Sennewald or Fred Bartoli see this and have the time and
> >> inclination, it would be educational to see how they get it simulating
> >> in SWCAD III and ICAP respectively. Probably too much to hope for
> >> anyone else with CircuitMaker.
> >> I scattered .IC parts around liberally, rang the changes on step
> >> times, and even kicked my desk, but still no regular output.
> >the circuit works nice... once you have settled the UIC (use initial
> >conditions) flag on the .TRAN line and given an initial condition of 0V
> >the 22uF capacitor.
> >Otherwise the circuit have (with the original values) a stable state that
> >found at the initial bias point calculation. Common startup problem of
> >oscillators with spice.
> Thanks Fred. I had another try with UIC enabled, as well as IC=0 at
> the top of the 220uF cap. (BTW, I note you said '22uF'. Are you using
> the identical circuit to me, as posted at
> http://www.terrypin.dial.pipex.com/Images/SP-LEDFlash.gif ?)
> But still couldn't get it working. What step and stop time did you
Yes, the same. I've just set the cap value to 22uF as I recall something
like that from an earlier exchange between you and Spehro. However it should
not change anything about the behaviour, except the flash period of course.
The simulation time is set to 10 seconds.
The time step has nothing to do with simulation. It has effects after the
simulation is done and gives the sampling period of the raw datas, *after*
the simulation is done, for the ascii output file. I don't know about CM but
I guess almost all todays spices don't use this file as the interface with
the scope program as this leads to lots of artifacts problems
(undersampling...). So if CM directly use raw data, simply set TimeStep to a
reasonably low value (don't generate huge text files) and all should be OK.
You can test this by setting a simple simulation file with a sine wave and
running 2 sims varying the timestep parameter and looking at what you have
in your scope.
For your simulation still not working don't forget that the oscillator, as
all, has a start up time (in my case with 22uF it's about 5 seconds), so let
enough simulation time.
Hmmm, wait a minute...
Ok, that's it. I've set the cap to 220 uF. It also refuse to start and
instead gently settle to the DC bias point I obtain without using the UIC
Now build an AC analysis to measure the circuit loop gain (there was a
recent thread about this but I can't remember what it was). Then vary the
cap and see what happens to your loop gain.
In my case with a 22uF cap the loop gain goes above 0dB somewhere -> the
When setting the cap to 220uF the loop gain *never* go above 0dB -> no
Then I set the 1uF cap to 10uF, the loop gain rise again above 0dB somewhere
and the circuit starts again.
Setting back to 220uF/1uF but increasing the 220R value to 1K, the loop gain
rise again above 0dB somewhere and the circuit still starts.
> Terry Pinnell
> Hobbyist, West Sussex, UK
Go Back To The Cyber-Spy.Com
Usenet Web Archive Index Of
The sci.electronics.design Newsgroup