Re: High purity 1kHz oscillator

On 26/10/2024 10:31 pm, Bill Sloman wrote:

On 26/10/2024 8:40 pm, JM wrote:

On Sat, 26 Oct 2024 14:21:32 +1100, Bill Sloman <bill.sloman@ieee.org> wrote:
>

On 26/10/2024 3:41 am, JM wrote:

On Sat, 26 Oct 2024 01:27:27 +1100, Bill Sloman <bill.sloman@ieee.org> wrote:
>

On 26/10/2024 12:15 am, JM wrote:

On Fri, 25 Oct 2024 23:03:32 +1100, Bill Sloman <bill.sloman@ieee.org> wrote:
>

On 25/10/2024 7:45 pm, JM wrote:

On Fri, 25 Oct 2024 09:25:31 +0100, JM <sunaecoNoSpam@gmail.com> wrote:
>

On Fri, 25 Oct 2024 18:16:26 +1100, Bill Sloman <bill.sloman@ieee.org> wrote:
>

On 25/10/2024 3:25 pm, Bill Sloman wrote:

On 25/10/2024 4:48 am, JM wrote:

On Thu, 24 Oct 2024 16:16:49 +0100, JM <sunaecoNoSpam@gmail.com> wrote:
>

On Wed, 23 Oct 2024 02:05:52 +0100, JM <sunaecoNoSpam@gmail.com> wrote:
>

On Tue, 22 Oct 2024 01:10:41 -0400, "Edward Rawde"
<invalid@invalid.invalid> wrote:

>
<snip>
>

Maybe one of the connections got messed up in the process - you did say
that one of them was misplaced.
>
I am running LTSpice 17 (XVII) and it was updated recently.
>
My FFT on V(out) had the third harmonic -78dB below the fundamental, not
-118dB.
>
Checking again over the last one 1 second and the last 10 seconds, it's
only -46dB, which is very odd.
>
Viktor Mickevic's design does look pretty good, so I suspect that
LTSpice 17 might not be performing as well as it should.

>
Yes, the resistors have an offset - one of us must have a non standard symbol.

>
My resistor symbol  is the normal rectangular block. I don't recall
doing anything to select it,
>

The Q1 emitter/r14 node should connect to the D3 cathode (which is the schematic error I mentioned) so that may account for the different result (I can't see any other changes that needs to be made). I used ltspice 17.1.15 - as is usual with oscillators the integration method should be trapezoidal rather than gear.

>
Moving the connection did make a big difference. I'm now seeing both odd
and even harmonics, but 80dB below the fundamental. I collected data
from 1 second rather than 4sec, and the amplitude takes most of the
extra time to settle to a stable value. I'll have more of a dig tomorrow
- it's 1:20am here, and I should be in bed.
>
I'm using LTSpice XVII (x64) (17.0.37.0) running under Windows 7.

>
You are probably using modified trapezoidal (which is the default) rather than trapezpoidal.  To get anything vaguely sensible out of ltspice you have to turn off all of Engelhardt's "improvements".  Better yet use any other spice.

>
I was. Switching to trapezoidal made another big difference.
>
I'm still seeing both odd an even harmonics, but they are about 97dB
below the fundamental.
>
Mike Engelhardt wasn't trying to make a more perfect Spice - he was
making a version of Spice that Linear Technology could distribute free
as an advertising gimmick. It was a pretty a good version of Spice
despite this, and made a good deal of difference to what we could share
on sci.electronics.design.
>
It turned out that Mike and I had been working on opposite sides of the
electron-beam tester conflict at the end of the 1980's. Mike's side won
- my machine was more ambitious, but quite a bit more expensive, and
while we got it working, it wasn't worth spending the money to put it
into  even low-volume production.
>
http://sophia-elektronica.com/At_Cambridge.html
>
puts my project in context
>
http://sophia-elektronica.com/The_early_history_of_voltage_contrast.html
>
talks about voltage contrast, and mentions Mike Engelhardt.
>
http://sophia-elektronica.com/The_first_stage.html
>
is more specific.
>

Check the origin in your res.asy and EuropeanResistor.asy (if by box type you mean the IEC standard).  It should be one grid diagonal from pin A.  (Press control while right clicking on a placed resistor to locate and open the symbol).  If the origin is not correct resistors on any schematic sent to (or received from) you will be drawn with an offset.

>
I'll have a look sometime soon.
>
The point you made about the LTSpice op amp models echoes what the late
Jim Thompson used to say here. The op amp models that get distributed
aren't transistor level models but behavioral models, that do more or
less the right thing. depending on how carefully and expertly they had
been written. Jim Thompson touted himself - fairly convincingly - as an
expert on writing them.

>
Are you doing an FFT only over an interval where the output has settled down?

 I changed the simulation command to start it saving data at 0.1 sec and to simulate for 10 seconds. The settling behavior is interesting. It hasn't quite settled at 5 sec, and I ran the FFT from 6sec to 10 sec.
 

Since you have an interest in oscillators  I'll email you a version of the circuit next week (if I remember!) where all harmonics in the audio band are below -150dB wrt the fundamental.

 I look forward to it.
 

I won't post to the group since the design is proprietary.

 That makes sense. This is a public forum.

I've got the circuit and it was impressive - the LTSpice simulation gave a third harmonic that was 140dB below the fundamental, even though the circuit had been modified into a form that would simulate in a finite time.
I'm not all that happy with the amplitude control feedback loop - it clearly works but seems to have quite a few more components than it ought to need - but once you have a circuit that works that well it's tempting to stick with it.
--
Bill Sloman, Sydney