Re: Current mirror version of the lowish distortion 1kHz sine wave osillator

On 23/01/2025 10:56 am, Edward Rawde wrote:

"Bill Sloman" <bill.sloman@ieee.org> wrote in message news:vmpj6v$i521$1@dont-email.me...

On 22/01/2025 12:32 pm, Bill Sloman wrote:

On 22/01/2025 3:58 am, Edward Rawde wrote:

"Edward Rawde" <invalid@invalid.invalid> wrote in message news:vmogqg$23tl$1@nnrp.usenet.blueworldhosting.com...

"Bill Sloman" <bill.sloman@ieee.org> wrote in message news:vmninh$3t6oi$1@dont-email.me...

On 21/01/2025 2:19 am, Bill Sloman wrote:

On 15/01/2025 11:33 pm, Bill Sloman wrote:

>
<snip>
>

It is running on LTSpice 17.0 on Windows 7, and I do have to download 17.1, which I'm going to do right now.

>
What you get if you are running Windows 7 is version 17.0.36.0, which may explain the difference. The sim runs just as fast on the
newly uploaded software. It's unlikely that John May has stuck to Window 7. and he has reported here that he is getting the same
kind of speed.
>
Don posted much the same observation earlier.

 I put LTSpice XVII(X64) (17.0.34.0) in the administrator account of an older core i5 2.8GHz (not SSD) running Windows 11 home 23H2.
I'll be upgrading it to Windows 10 pro when I get a chance.
I didn't install any suggested LTSpice updates.
U1 was out of position but this time I had to move it up and connect the -ve power rail.
Simulation speed varies between about 6ms/s and 15 ms/s.
Vout shows a single transient at startup which peaks at about 600mv pk and settles to a constant level of around 100mV pk in a few
hundred ms.
FFT of a sample of about 100ms near 10s with Blackman Harris window shows 1kHz a little below -20dB,
2kHz -90dB (so at least 70 dB down on 1 kHz)
3kHz -70dB
4kHz -85dB
5kHz  -75dB
There are no higher peaks or crud at higher frequencies.
The raw file didn't go above 1.1 GB
 Now move exactly the same circuit to LTSpice 24.1.0 on a core i7 SSD Windows 10 pro 22H2.
LTSpice component updates available today 22 Jan 2025 were also installed.
U1 now has to be moved down and the +ve rail has to be connected.
Note that after saving the file in 24.1.0 the version at the top of the file becomes 4.1
Take a sample of about 10us of Vout between 300-350us and do FFT with Blackman-Harris window.
This shows a peak of -43dB at 24MHz and the next highest peak -93dB at 400MHz.
Zoom to fit and watch progress. Reported speed is about 25us/s.
Leave simulation running and do some other work.
Come back after an hour and find it has peaked at 600mV pk after 86ms simulation time and is now falling.
Take a sample of a few cycles at 86ms and run FFT with Blackman-Harris window.
1kHz -9dB
2kHz -95dB
3kHz -85dB
4kHz -110dB
24MHz -63dB
raw file has reached 40GB and simulation time is now 130ms. Level is 200mv pk and still falling
Level seems reasonably stable (100mv pk) at 220ms but take a sample and you can see it has parasitic HF crud in it.
raw file has now reached 74GB. Stop simulation.
 All signal amplitude levels given are pk. pk-pk would be twice.
 To avoid any doubt of what I'm simulating, it's below.

And the problem with your version of the circuit is that C10 on the output of U4 was 3.3? rather than 3.3u, We've had that problem before.
The LTC6655-1.25 at U1 is an an excellent voltage reference if it is loaded with at least 2.7uF. Technically speaking I should be using the Greek symbol. Using 3300nF is safer, because not every LTSpice user takes advantage of the option to treat "u" as if was the correct Greek alphabet look-alike.
Without enough output capacitance the LTSpice model for the LTC6655-1.25 behaves oddly. I screwed up early on and only used 1uF and the part oscillated.
In your version of the circuit it presents a slowly rising ramp starting at 0V which had crept up to 10mV after 2 seconds.
This doesn't produce the behaviour I intended.
There's also a problem with the BAS70L diode model - your version leaves off the .ENDS line at the end of the Spice directive. The simulation appears to run fine without it, at 30msec/sec, but I'm still nervous about it.
--
Bill Sloman, Sydney