Re: A variation on my current mirror low distortion sine wave oscillator - 10dB less distortion and much the same number of components

"JM" <sunaecoNoChoppedPork@gmail.com> wrote in message news:637vqjpics9oqi4gsv4vv200cf7t3kovb6@4ax.com...

On Fri, 14 Feb 2025 13:03:46 -0500, "Edward Rawde"
<invalid@invalid.invalid> wrote:
>

"Bill Sloman" <bill.sloman@ieee.org> wrote in message news:vompa5$3bjpm$1@dont-email.me...

On 14/02/2025 5:24 am, Edward Rawde wrote:

"Bill Sloman" <bill.sloman@ieee.org> wrote in message news:vol49p$2vd0d$1@dont-email.me...

On 14/02/2025 1:45 am, Edward Rawde wrote:

"Bill Sloman" <bill.sloman@ieee.org> wrote in message news:voh7a5$26aqj$1@dont-email.me...

On 10/02/2025 5:18 pm, Bill Sloman wrote:

Basically same idea, but two separate controllable asymmetric current mirrors, rather than one, and no current steering.
The
half-wave rectifier still seems to be the source of the distortion in the stabilised output.
>
C25 and C26 take out as much of it as I can. Increasing them - from 15nF to 33nF makes the distortion worse. Splitting the
resistors into three rather than two and adding two more capacitors might help, but what this circuit needs is more
insight,
rather than more components.

>
Splitting the resistors did help, and the optimum capacitor value at C25, C26, C27 and C28 turned out to be 4.7nF. The
second
and
fifth harmonics were just 80dB below the fundamental and the third 91dB down. Not dramatically good, but respectable.
>
Other changes were less successful - the current mirror approach does suffer from the need to split the waveform in order to
generate the amplitude correction waveform and minimising the 2usec wide switching spikes that show up at cross-over is what
it
takes to get it to work tolerably well
>
I've swapped out the LT1115 for the LT1678 - that doesn't seem to suffer from parasitic oscillations in LTSpice 24, so it
should
simulate tolerably fast.
>

After fixing line wraps I had to move U1 down into position.
I then noticed an issue with C10 so I converted to ANSI in Notepad++ and saved the file.

>
When I picked up your text file, I noted that C10 (on the output of U4, the LTC6655-1.25 voltage reference) had gone back to
3.3 -
no suffix. I set it back to 3300n(F) and the circuit worked as it did for me with the harmonics mostly 80dB down with the
third
harmonic about 91dB down
>

Simulation then failed without giving any clue what was wrong.
But instead of spending hours tracing the problem I removed .ENDS from the BAS70 model.

>
I put it back in again. and it didn't make any difference to my simulation.

>
It will for anyone else using 24.1.2.
>
I note that the model for MMBF4391 is still present and does not have .ENDS so why should BAS70 need it?
In 24.1.2 you get errors which make no sense and do not mention BAS70.

>
The BAS70 model dates back to 2015. It's a classic Spice model - and LTSpice is supposed to run them.

>
Online searching finds "A SPICE model starts with a .SUBCKT statement and ends with an .ENDS statement" which does not seem to be
applicable here.
>
24.1.2 seems to simulate just fine if .ENDS is removed from the BAS70 model.
But if .ENDS is included then the simulation does not run and the following log is produced.
Now tested on two different computers running 24.1.2
>
LTspice 24.1.2 for Windows
Circuit: C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net
Start Time: Fri Feb 14 11:10:46 2025
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(2): This sub-circuit name is not defined.
X§U1 N040 N035 N006 N052 N039 LT1360
                             ^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(22): This sub-circuit name is not defined.
X§U5 N037 N019 Vcc Vee N002 LT1056
                           ^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(25): This sub-circuit name is not defined.
X§U2 0 N033 N017 N051 N030 OP27
                          ^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(47): This sub-circuit name is not defined.
X§U4 N038 N038 0 N037 N037 LTC6655-1.25
                          ^^^^^^^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(57): This sub-circuit name is not defined.
X§U6 N032 N021 Vcc Vee filt1 LT1013
                            ^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(62): This sub-circuit name is not defined.
X§U7 N029 N013 Vcc Vee filter2 LT1013
                              ^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(80): This sub-circuit name is not defined.
X§U9 0 N025 Vcc Vee N034 LT1013
                        ^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(81): This sub-circuit name is not defined.
X§U10 0 N044 Vcc Vee N001 LT1056
                         ^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(87): This sub-circuit name is not defined.
X§U11 0 N022 Vcc Vee N023 LT1013
                         ^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(102): This sub-circuit name is not defined.
X§U3 0 N011 N024 N004 N045 LT1678
                          ^^^^^^^
C:\Users\Edward\Desktop\sloman 14 Feb 2025\sloman.net(103): This sub-circuit name is not defined.
X§U8 0 N014 Vout N005 N046 LT1678
                          ^^^^^^^
The ^^ characters are positioned under the device type.
Under LT1360 for the first error.
Formatting differences may not show this correctly.
>
It took me a while not long ago to slowly add/remove parts of your circuit until I found out that removing .ENDS in the BAS70
model
on the schematic eliminated the above issues and the simulation in 24.1.0 ran fine.
>

>

Simulation now runs fine at about 44 ms/s in LTSPice 24.1.2

FFT is approaching 60dB

>
Not having the right value capacitor at C10 usually totally messes it up. We've had that issue before.

>
C10 is 3.3uF
Changing to 3300n and resimulating makes no difference. Definitely only 60dB difference between 1kHz and 2,3,4,5kHz
Exact circuit I'm simulating (in 24.1.2) included below.

>
And when I run it (after having put U1 back where I intended it to go and restored it's connection to the negative rail) I got
the
second to the fifth harmonics harmonics 80dB below the fundamental with the third 91dB down. When I stretched the frequency
display out to 100kHz the higher harmonics were going down.

>
I ran your circuit to 10 seconds on 24.1.2 (about 4 minutes) and took a sample of about 60 cycles near 10 seconds.
I then did an FFT on Vout (U8 output) and selected current zoom extent and Blackman-Harris Window.
The vertical scale has 20dB at the top with 1kHz at 0dB one square down.
Another three squares down are 2,3,4,5 kHz approaching the 60dB line.
>
So let's copy the asc file to another computer with LTSPice 17.0.34.0 and no component updates since installation.
Fix the position of U1 and add .ENDS to the BAS70 model. Simulate.
Speed is about the same 44ms/s but drops to 7ms/s after about 2 seconds simulated and then goes back to 44ms/s
Appearance is as above. 3.2V pk initial transient then settling at 1.6V pk.
Same FFT as above.
Approaching 80dB at 2kHz, 3kHz 4kHz 75dB, 5kHz 65dB
Remove .ENDS from BAS70 model and resimulate.
Similar result depends a little on exact sample taken, maybe a little worse at 2kHz.
Put .ENDS back again and resimulate. Exactly the same FFT result so .ENDS as used here is best removed to avoid issues when
upgrading to 24.1.x
.ENDS is only an issue in 24.1.0 or later and only in the context described above.
>
So I wonder which simulation is closer to the truth.
>

>
I did let it settle down for two seconds before taking the FFT of V(out) onver the next second or so.
>

Simulated circuit included below.
I can get 80dB by adding an LC tuned circuit to a simple phase shift oscillator of the type which turns up here:
https://www.google.com/search?q=sine+wave+oscillator&udm=2

>
Where? There's a lot of stuff there.

>
Phase shift oscillator with feedback from the collector through CRCRCRCR to the base.

>
That is the simplest phase shift oscillator. Why didn't you identify it when you first mentioned it?

>
Because it didn't matter and there is more than one example of that type of circuit.
Most circuits which turn up there can't manage more than 60dB and those which can are unlikely to manage more than 90dB.
It's not long ago when I didn't think I'd do better than 90dB in simulation, but I kept at it. Now I can do 135dB in simulation
with
all simulated real (yes ok that's a contradiction) components.
>

>

No gain control yet but for unknown reasons it does run at constant (unpredictable) amplitude with very critical emitter
resistor
adjustment.

>
It's probably relying on the change in current gain with changing collector-base voltage. It is a small effect - the Early
effect - and non-linear.
>

I'm thinking of trying the sample/hold method posted by JM but with real components.
So I need to turn a FET on (not sure for how long yet) at the peaks of the sine wave.

>
Sample and holds tend to put spikes on the supply rails. Keeping them out of the output can take a lot of work.

>
Yeah I've had that problem before, decades ago.
A capacitively coupled inverted sampling signal was able to sufficiently remove the problem of  the sampling signal appearing
in
the
output.

>
Reduce rather than remove. Cancellation schemes rarely work perfectly.
>

But that may not work at 140dB down.
>
Here is the exact version of your circuit from my most recent simulation of it.

>
Give or take the usual problems.
>
-- Bill Sloman, Sydney
>

>

>
.ends is only used to end a .subckt so ltspice is correct to warn
about it.

 Yes I came to that conclusion a few minutes ago.
In versions prior to 24.1.0 .ENDS appears to be ignored when used without .SUBCKT
But In 24.1.0 or later the use of .ENDS without .SUBCKT can cause a simulation to fail with warnings which are not helpful when
tracing the cause of the problem.