[time-nuts] Spice simulation of PSRR and phase noise

[Attila Kinali]

Hi,

I have been looking into spice simulations of circuits, in particular
trying to extract PSRR and phase noise information. Unfortunatelly,
the obvious way of putting AC sources at the right places does not
work, as the (ideal) input signals are not small and drive the circuit
into non-linearities. Hence I have to do transient simulations.
But extracting PSRR and phase noise information out of a transient
simulation is cumbersome at best and takes a lot of simulation time
(we are talking about hours to days for simple circuits).

I am looking for guidelines and hints how to speed things up.
Maybe even being able to use standard DC and AC analysis for the
circuit instead of transient. Unfortunately, my google-foo was not
strong enough to find approriate documentation.

Does someone have any hints what I should read or search for?

Thanks in advance

Attila Kinali

[Dana Whitlow]

Hello Attila,

It seems to me that an AC simulation could never work since the
very generation of phase noise by the mechanisms that matter is
a modulation process at heart, automatically forcing one into the
realm of transient simulations.

But I am surprised about the simulation times that you speak of.
Would you be willing to post some information detailing your
methodology and an example "simple" circuit?

Dana

Post by Attila Kinali
Hi,
I have been looking into spice simulations of circuits, in particular
trying to extract PSRR and phase noise information. Unfortunatelly,
the obvious way of putting AC sources at the right places does not
work, as the (ideal) input signals are not small and drive the circuit
into non-linearities. Hence I have to do transient simulations.
But extracting PSRR and phase noise information out of a transient
simulation is cumbersome at best and takes a lot of simulation time
(we are talking about hours to days for simple circuits).
I am looking for guidelines and hints how to speed things up.
Maybe even being able to use standard DC and AC analysis for the
circuit instead of transient. Unfortunately, my google-foo was not
strong enough to find approriate documentation.
Does someone have any hints what I should read or search for?
Thanks in advance
Attila Kinali
--
It is upon moral qualities that a society is ultimately founded. All
the prosperity and technological sophistication in the world is of no
use without that foundation.
-- Miss Matheson, The Diamond Age, Neil Stephenson
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/
mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Rafael Gajanec]

Dear Attila,

you haven't specified what sort of circuits would you like to simulate,
but maybe the answer is Harmonic Balance. Have a look at
http://qucs.sourceforge.net/ and
http://qucs.sourceforge.net/tech/node36.html

HSPICE from Synopsis and ADS from Keysight (which I use) also have the
HB engine.

Best regards,
Rafael Gajanec

Post by Dana Whitlow
Hello Attila,
It seems to me that an AC simulation could never work since the
very generation of phase noise by the mechanisms that matter is
a modulation process at heart, automatically forcing one into the
realm of transient simulations.
But I am surprised about the simulation times that you speak of.
Would you be willing to post some information detailing your
methodology and an example "simple" circuit?
Dana

Post by Attila Kinali
Hi,
I have been looking into spice simulations of circuits, in particular
trying to extract PSRR and phase noise information. Unfortunatelly,
the obvious way of putting AC sources at the right places does not
work, as the (ideal) input signals are not small and drive the circuit
into non-linearities. Hence I have to do transient simulations.
But extracting PSRR and phase noise information out of a transient
simulation is cumbersome at best and takes a lot of simulation time
(we are talking about hours to days for simple circuits).
I am looking for guidelines and hints how to speed things up.
Maybe even being able to use standard DC and AC analysis for the
circuit instead of transient. Unfortunately, my google-foo was not
strong enough to find approriate documentation.
Does someone have any hints what I should read or search for?
Thanks in advance
Attila Kinali
--
It is upon moral qualities that a society is ultimately founded. All
the prosperity and technological sophistication in the world is of no
use without that foundation.
-- Miss Matheson, The Diamond Age, Neil Stephenson
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/
mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Attila Kinali]

Hi Rafael

On Sun, 22 Oct 2017 17:20:52 +0200

Post by Rafael Gajanec
you haven't specified what sort of circuits would you like to simulate,

Simplified, they are differential amplifiers driven into saturation.
A bit more detailed, I am looking at ring oscillator stages and sine-to-square
conversion circuits and their behaviour regarding various key factors
(note: I am not sure what the key factors are, yet)

Post by Rafael Gajanec
but maybe the answer is Harmonic Balance.

Hmm.. I didn't know about Harmonic Balance. I have some reading up to do.
Thanks!

Post by Rafael Gajanec
HSPICE from Synopsis and ADS from Keysight (which I use) also have the
HB engine.

I am mostly using ngpsice, because it's very easy to script (I have a bunch
of perl scripts that feed simulations into a Grid Engine cluster, extract
data and analyzse it). Is there any big advantage of the commercial spice
engines that would make them worth considering? And would the license alow
to run hundreds of instances in parallel?
(Yes, I am doing crazy things :-)

Attila Kinali

[Rafael Gajanec]

Hi Attila,

Post by Attila Kinali
Hi Rafael
On Sun, 22 Oct 2017 17:20:52 +0200

Post by Rafael Gajanec
you haven't specified what sort of circuits would you like to simulate,

Simplified, they are differential amplifiers driven into saturation.
A bit more detailed, I am looking at ring oscillator stages and sine-to-square
conversion circuits and their behaviour regarding various key factors
(note: I am not sure what the key factors are, yet)

Oscillator design - that's what I found HB simulation particularly
useful for. It gives you almost instant results, compared to the
transient simulation, say 10 seconds instead of 5 hours! Just imagine
what it means if you are trying to tune several parameters of an
oscillator... The only other reasonably fast and accurate way I can
think of is to build the bloody circuit and measure it using some
expensive equipment.

Post by Attila Kinali

Post by Rafael Gajanec
but maybe the answer is Harmonic Balance.

Hmm.. I didn't know about Harmonic Balance. I have some reading up to do.
Thanks!

Post by Rafael Gajanec
HSPICE from Synopsis and ADS from Keysight (which I use) also have the
HB engine.

I am mostly using ngpsice, because it's very easy to script (I have a bunch
of perl scripts that feed simulations into a Grid Engine cluster, extract
data and analyzse it). Is there any big advantage of the commercial spice
engines that would make them worth considering? And would the license alow
to run hundreds of instances in parallel?
(Yes, I am doing crazy things :-)

Attached are some results of a simple transient simulation using Hspice
M 2017.03, BBspice A/D 5.2.3 and ADS 2016.01. It's basically *V1 1 0 SIN
0 1 1Meg *and then *.FOUR 1Meg V(1)* in Hspice, VspecTran in ADS and
spectra computed using postprocessor in BBspice and ADS. As you can see,
there are some differences... To be fair, possibly there are some
simulator-specific settings/methods that could improve the results and
you should figure it out yourself what's the way to get the best results
from your spice. See
http://www.audio-perfection.com/spice-ltspice/distortion-measurements-with-ltspice.html

Commercial spice engines may have lower computational noise and shorter
simulation times. For example my out-dated BBspice (which is commercial
too by the way) crashed several times before I got some results, while
it used little RAM and only about 10-12% of available processor
resources... I intended to get you Pspice results of this simulation as
well, but I gave up after half an hour and about 1% of progress.

Post by Attila Kinali
Attila Kinali

Best regards,
Rafael Gajanec

[Bob kb8tq]

Hi

The “fun part” of harmonic balance is making sure you are not off in a corner
case where the results are not as good as they might otherwise be. Maybe not
as much an issue for a VCO as for some other structures.

Bob

Post by Rafael Gajanec
Hi Attila,

Post by Attila Kinali
Hi Rafael
On Sun, 22 Oct 2017 17:20:52 +0200

Post by Rafael Gajanec
you haven't specified what sort of circuits would you like to simulate,

Simplified, they are differential amplifiers driven into saturation.
A bit more detailed, I am looking at ring oscillator stages and sine-to-square
conversion circuits and their behaviour regarding various key factors
(note: I am not sure what the key factors are, yet)

Oscillator design - that's what I found HB simulation particularly useful for. It gives you almost instant results, compared to the transient simulation, say 10 seconds instead of 5 hours! Just imagine what it means if you are trying to tune several parameters of an oscillator... The only other reasonably fast and accurate way I can think of is to build the bloody circuit and measure it using some expensive equipment.

Post by Attila Kinali

Post by Rafael Gajanec
but maybe the answer is Harmonic Balance.

Hmm.. I didn't know about Harmonic Balance. I have some reading up to do.
Thanks!

Post by Rafael Gajanec
HSPICE from Synopsis and ADS from Keysight (which I use) also have the
HB engine.

I am mostly using ngpsice, because it's very easy to script (I have a bunch
of perl scripts that feed simulations into a Grid Engine cluster, extract
data and analyzse it). Is there any big advantage of the commercial spice
engines that would make them worth considering? And would the license alow
to run hundreds of instances in parallel?
(Yes, I am doing crazy things :-)

Attached are some results of a simple transient simulation using Hspice M 2017.03, BBspice A/D 5.2.3 and ADS 2016.01. It's basically *V1 1 0 SIN 0 1 1Meg *and then *.FOUR 1Meg V(1)* in Hspice, VspecTran in ADS and spectra computed using postprocessor in BBspice and ADS. As you can see, there are some differences... To be fair, possibly there are some simulator-specific settings/methods that could improve the results and you should figure it out yourself what's the way to get the best results from your spice. See http://www.audio-perfection.com/spice-ltspice/distortion-measurements-with-ltspice.html
Commercial spice engines may have lower computational noise and shorter simulation times. For example my out-dated BBspice (which is commercial too by the way) crashed several times before I got some results, while it used little RAM and only about 10-12% of available processor resources... I intended to get you Pspice results of this simulation as well, but I gave up after half an hour and about 1% of progress.

Post by Attila Kinali
Attila Kinali

Best regards,
Rafael Gajanec
<Hspice.png><BBspice.png><ADS.png>_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Bruce Griffiths]

If one for example wishes to estimate PN down to an offset of 1Hz then an equivalent filter noise bandwidth of 0.1Hz or perhaps less is desirable (the PN spectrum at low offsets is far from flat). To achive accurate noise estimates a simulation time of at least 100 x the reciprocal of the equivalent noise bandwidth is required. The resultant simulation for 1000 sec or more takes considerably longer than 1000 sec to run.

Bruce

Post by Dana Whitlow
Hello Attila,
It seems to me that an AC simulation could never work since the
very generation of phase noise by the mechanisms that matter is
a modulation process at heart, automatically forcing one into the
realm of transient simulations.
But I am surprised about the simulation times that you speak of.
Would you be willing to post some information detailing your
methodology and an example "simple" circuit?
Dana

Post by Attila Kinali
Hi,
I have been looking into spice simulations of circuits, in particular
trying to extract PSRR and phase noise information. Unfortunatelly,
the obvious way of putting AC sources at the right places does not
work, as the (ideal) input signals are not small and drive the circuit
into non-linearities. Hence I have to do transient simulations.
But extracting PSRR and phase noise information out of a transient
simulation is cumbersome at best and takes a lot of simulation time
(we are talking about hours to days for simple circuits).
I am looking for guidelines and hints how to speed things up.
Maybe even being able to use standard DC and AC analysis for the
circuit instead of transient. Unfortunately, my google-foo was not
strong enough to find approriate documentation.
Does someone have any hints what I should read or search for?
Thanks in advance
Attila Kinali
--
It is upon moral qualities that a society is ultimately founded. All
the prosperity and technological sophistication in the world is of no
use without that foundation.
-- Miss Matheson, The Diamond Age, Neil Stephenson
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/
mailman/listinfo/time-nuts
and follow the instructions there.
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Bruce Griffiths]

One has to provide noise models that work with the Spice transient simulation for all devices including resistors. Random number generators can be used but they need to be independent and must not repeat during the entire simulation.

Bruce

If one for example wishes to estimate PN down to an offset of 1Hz then an equivalent filter noise bandwidth of 0.1Hz or perhaps less is desirable (the PN spectrum at low offsets is far from flat). To achive accurate noise estimates a simulation time of at least 100 x the reciprocal of the equivalent noise bandwidth is required. The resultant simulation for 1000 sec or more takes considerably longer than 1000 sec to run.
Bruce

Post by Dana Whitlow
Hello Attila,
It seems to me that an AC simulation could never work since the
very generation of phase noise by the mechanisms that matter is
a modulation process at heart, automatically forcing one into the
realm of transient simulations.
But I am surprised about the simulation times that you speak of.
Would you be willing to post some information detailing your
methodology and an example "simple" circuit?
Dana

Post by Attila Kinali

Post by Attila Kinali
Hi,

I have been looking into spice simulations of circuits, in particular
trying to extract PSRR and phase noise information. Unfortunatelly,
the obvious way of putting AC sources at the right places does not
work, as the (ideal) input signals are not small and drive the circuit
into non-linearities. Hence I have to do transient simulations.
But extracting PSRR and phase noise information out of a transient
simulation is cumbersome at best and takes a lot of simulation time
(we are talking about hours to days for simple circuits).
I am looking for guidelines and hints how to speed things up.
Maybe even being able to use standard DC and AC analysis for the
circuit instead of transient. Unfortunately, my google-foo was not
strong enough to find approriate documentation.
Does someone have any hints what I should read or search for?
Thanks in advance
Attila Kinali
--
It is upon moral qualities that a society is ultimately founded. All
the prosperity and technological sophistication in the world is of no
use without that foundation.
-- Miss Matheson, The Diamond Age, Neil Stephenson
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/
mailman/listinfo/time-nuts
and follow the instructions there.
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

Post by Attila Kinali
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Attila Kinali]

Hoi Dana,

On Sun, 22 Oct 2017 09:23:26 -0500

Post by Dana Whitlow
But I am surprised about the simulation times that you speak of.
Would you be willing to post some information detailing your
methodology and an example "simple" circuit?

As Bruce already mentioned, the simulation times required for
getting decent results is 100-1000 times as long as the lowest
frequency considered. This is basically a statistical issue as
noise simulation, to be accurate, has to average over several
"runs" to remove effects of the noise source behaviour.

Another thing is, that, for the transient simulation to be accurate,
the maximum steps size has to be limited such that the maximum voltage
or current step seen is small. Ie if there is anything in the system
with high slew rates, then the step size has to be adapted to this
slew rate. This in turn makes it slower

Additionally, most spice implementations have quite short running
random number generators (usually with a state space of 2^16 to 2^32,
few with 2^64) which in turn requires some tricks to get decent results
out of it, that again make the simulation time longer.


Attila Kinali

[Bruce Griffiths]

Hoi Attila

Since close in phase noise can result from up conversion of supply noise etc via circuit non linearities, using an AC analysis won't work.

Only transient simulation or perhaps analytical modelling of the various non linearities will provide accurate estimates of upconverted PN. If you use transient simulation techniques increasing the level of the various noise sources above the actual levels encountered in real circuits and then correcting the resultant PN back to the level that would be encountered in the actual circuit (using the results of analytical modelling) may be a useful way to reduce simulation time or at least overcome some of the challenges associated with accurately determining low level PN from a simulation.

There are some in the LTSpice Yahoo group attempting this but they seem way out of touch with the amount of simulation data required. I've provided them with the appropriate formulae to extract PN from the the amplitude spectra. At the moment they appear bogged down with some somewhat trivial peripheral issues.

Bruce

Post by Attila Kinali
Hi,
I have been looking into spice simulations of circuits, in particular
trying to extract PSRR and phase noise information. Unfortunatelly,
the obvious way of putting AC sources at the right places does not
work, as the (ideal) input signals are not small and drive the circuit
into non-linearities. Hence I have to do transient simulations.
But extracting PSRR and phase noise information out of a transient
simulation is cumbersome at best and takes a lot of simulation time
(we are talking about hours to days for simple circuits).
I am looking for guidelines and hints how to speed things up.
Maybe even being able to use standard DC and AC analysis for the
circuit instead of transient. Unfortunately, my google-foo was not
strong enough to find approriate documentation.
Does someone have any hints what I should read or search for?
Thanks in advance
Attila Kinali
--
It is upon moral qualities that a society is ultimately founded. All
the prosperity and technological sophistication in the world is of no
use without that foundation.
-- Miss Matheson, The Diamond Age, Neil Stephenson
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Gerhard Hoffmann]

Post by Bruce Griffiths
Hoi Attila
Since close in phase noise can result from up conversion of supply noise etc via circuit non linearities, using an AC analysis won't work.
Only transient simulation or perhaps analytical modelling of the various non linearities will provide accurate estimates of upconverted PN. If you use transient simulation techniques increasing the level of the various noise sources above the actual levels encountered in real circuits and then correcting the resultant PN back to the level that would be encountered in the actual circuit (using the results of analytical modelling) may be a useful way to reduce simulation time or at least overcome some of the challenges associated with accurately determining low level PN from a simulation.
There are some in the LTSpice Yahoo group attempting this but they seem way out of touch with the amount of simulation data required. I've provided them with the appropriate formulae to extract PN from the the amplitude spectra. At the moment they appear bogged down with some somewhat trivial peripheral issues.

In a previous life, when I was an EE&CS student, we had to write all the
relevant algorithms ourselves, like building the conductance matrix,
finding the operating point, linearizing nonlinear devices around the
OP, doing the integration over time, companion models etc, b4 we were
given the Spice 2G4 sources...

(Attila, that was a few 100 meters from where you seem to work right
now. There was a beautiful TR440!)

Given that we often enough see convergence problems in integration over
time to the point that the simulator gives up altogether, especially
when there are high Q resonances or nonlinearities around, and that
these errors look like phase noise, I would never ever trust a FFT
result at, say, the -140 dBc level. And there it just starts to be
interesting.

As much as I like to use LTspice, it's easy availability blocks any fast
progress in the public spices like adding HB, s-params by diverting
people to experiment with add-ons instead of solving the fundamental
issues. X/Ngspice and QUCS are nice but understaffed for sure.

regards, Gerhard.

(who was designing a chopper amplifier in the 140 pV/rt Hz league this
rainy weekend and did not even try to simulate its noise. The
interesting part of it would never make it through the pot core
transformer.)



_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Anders Wallin]

FWIW I recently took a peek inside a commercial distribution-amplifier and
it seems to use two LMH6702 op-amps in parallel.
There are two of these dual-LMH6702 stages with a 1:2 splitter after the
first, and then a 1:4 splitter after the second stage. 8 outputs in total,
with an additional op-amp driving each output.
A simulation that shows the difference in PN between a single LMH6702 and
the dual-op-amp idea would be nice.
For far-out (>100Hz from carrier?) PN only SNR might matter, so a SPICE
noise-simulation giving noise PSD at relevant (5-10MHz) frequencies might
give something?

Anders
_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Bob kb8tq]

Hi

One would guess that they put them in parallel to get more drive. If that’s correct,
details of the loading are going to get into the simulation pretty quickly.

In a lot of cases, these amplifiers were designed against a specific need. If you have
a signal source that is in the -180 dbc / Hz range, they are unlikely do perform well.
In many cases a floor in the -140 dbc / Hz range was considered “good enough”.
If you are simply driving common test gear, it probably *is* good enough. If the
application was video rather than a standard the specs could have been very different.

In the case of an amp with a LMH6702, you are not going to get super close in
phase noise. The device is *very* noisy under 1 MHz. It also starts to increase distortion
by 10 MHz so you will see up conversion. It probably did quite well against the intended
design spec.

=====

If you need a system that will distribute one frequency today and a totally different
frequency tomorrow, broadband makes sense. For the more common task of
something like “only 10 MHz”, it does not make much sense at all. Gain other
frequencies is just going to spread around noise from this or that source
of crud. Driving filters with op amps can be problematic. It often is easier to go another
way.

Bob

Post by Anders Wallin
FWIW I recently took a peek inside a commercial distribution-amplifier and
it seems to use two LMH6702 op-amps in parallel.
There are two of these dual-LMH6702 stages with a 1:2 splitter after the
first, and then a 1:4 splitter after the second stage. 8 outputs in total,
with an additional op-amp driving each output.
A simulation that shows the difference in PN between a single LMH6702 and
the dual-op-amp idea would be nice.
For far-out (>100Hz from carrier?) PN only SNR might matter, so a SPICE
noise-simulation giving noise PSD at relevant (5-10MHz) frequencies might
give something?
Anders
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Bob Martin]

I never had much luck with current feedback amplifiers such as the
LMH6702. Their input current noise (at the time) was too high for
my needs and their output peaks at higher frequencies if the
feedback resistors aren't optimal for the part.

I had the best results with voltage feedback op amps like the
MAX4104/MAX3404 when I needed gain on the input stage and the
LMH6609 when I needed a buffer.

My applications were broadband. If I remember correctly,
aggressive bandwidth limiting can cause phase shift problems due to
temperature changes unless one is careful in the design of the filter.

I've successfully put as many as four op amps in parallel in an
input stage to reduce phase noise.


Bob M (another bob)

Post by Bob kb8tq
Hi
One would guess that they put them in parallel to get more drive. If that’s correct,
details of the loading are going to get into the simulation pretty quickly.
In a lot of cases, these amplifiers were designed against a specific need. If you have
a signal source that is in the -180 dbc / Hz range, they are unlikely do perform well.
In many cases a floor in the -140 dbc / Hz range was considered “good enough”.
If you are simply driving common test gear, it probably *is* good enough. If the
application was video rather than a standard the specs could have been very different.
In the case of an amp with a LMH6702, you are not going to get super close in
phase noise. The device is *very* noisy under 1 MHz. It also starts to increase distortion
by 10 MHz so you will see up conversion. It probably did quite well against the intended
design spec.
=====
If you need a system that will distribute one frequency today and a totally different
frequency tomorrow, broadband makes sense. For the more common task of
something like “only 10 MHz”, it does not make much sense at all. Gain other
frequencies is just going to spread around noise from this or that source
of crud. Driving filters with op amps can be problematic. It often is easier to go another
way.
Bob

Post by Anders Wallin
FWIW I recently took a peek inside a commercial distribution-amplifier and
it seems to use two LMH6702 op-amps in parallel.
There are two of these dual-LMH6702 stages with a 1:2 splitter after the
first, and then a 1:4 splitter after the second stage. 8 outputs in total,
with an additional op-amp driving each output.
A simulation that shows the difference in PN between a single LMH6702 and
the dual-op-amp idea would be nice.
For far-out (>100Hz from carrier?) PN only SNR might matter, so a SPICE
noise-simulation giving noise PSD at relevant (5-10MHz) frequencies might
give something?
Anders
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Attila Kinali]

Hoi Bruce,

On Mon, 23 Oct 2017 09:58:40 +1300 (NZDT)

Post by Bruce Griffiths
Since close in phase noise can result from up conversion of supply noise
etc via circuit non linearities, using an AC analysis won't work.
Only transient simulation or perhaps analytical modelling of the various
non linearities will provide accurate estimates of upconverted PN.

Unfortunately, my understanding of transistors is far from being good.
Hence doing accurate analytical analysis is beyond me. Hence my reliance
on spice to do the "hard work."

Post by Bruce Griffiths
If you use transient simulation techniques increasing the level of the
various noise sources above the actual levels encountered in real circuits
and then correcting the resultant PN back to the level that would be
encountered in the actual circuit (using the results of analytical modelling)
may be a useful way to reduce simulation time or at least overcome some of
the challenges associated with accurately determining low level PN from a
simulation.

This is a good idea, thanks!

Post by Bruce Griffiths
There are some in the LTSpice Yahoo group attempting this but they seem
way out of touch with the amount of simulation data required. I've provided
them with the appropriate formulae to extract PN from the the amplitude
spectra. At the moment they appear bogged down with some somewhat trivial
peripheral issues.

I tried to read the yahoo groups... but god! is the interface bad!
I only found a few mails from last August that go into that direction.
Is there anything else that might be interesting?


Attila Kinali

[Hal Murray]

My applications were broadband. If I remember correctly, aggressive
bandwidth limiting can cause phase shift problems due to temperature
changes unless one is careful in the design of the filter.

Does anybody ovenize amplifiers and filters to avoid that problem?

[Richard (Rick) Karlquist]

Post by Hal Murray

My applications were broadband. If I remember correctly, aggressive
bandwidth limiting can cause phase shift problems due to temperature
changes unless one is careful in the design of the filter.

Does anybody ovenize amplifiers and filters to avoid that problem?

This problem came up in the design of the 5071A.
I elected to avoid narrowband filters by using
some tricks described in my FCS paper of about
25 years ago. I didn't find it necessary to ovenize
the output section.

By contrast, the 5061 had numerous narrow band filters
that were problematical.

Rick N6RK
_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Attila Kinali]

On Tue, 24 Oct 2017 12:12:24 -0700

Post by Richard (Rick) Karlquist
This problem came up in the design of the 5071A.
I elected to avoid narrowband filters by using
some tricks described in my FCS paper of about
25 years ago. I didn't find it necessary to ovenize
the output section.

For those looking for the paper:
http://www.karlquist.com/FCS92.pdf


Attila Kinali

[Bob kb8tq]

Hi

If you have the money, almost anything can be (and has been) done. It’s rare to find a
real world application where this kind of thing is considered cost effective. Fancy
radar systems are about the only thing that comes to mind. Radar of
this sort is always high cost / low volume.

Bob

Post by Hal Murray

My applications were broadband. If I remember correctly, aggressive
bandwidth limiting can cause phase shift problems due to temperature
changes unless one is careful in the design of the filter.

Does anybody ovenize amplifiers and filters to avoid that problem?
--
These are my opinions. I hate spam.
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[jimlux]

Post by Bob kb8tq
Hi
If you have the money, almost anything can be (and has been) done. It’s rare to find a
real world application where this kind of thing is considered cost effective. Fancy
radar systems are about the only thing that comes to mind. Radar of
this sort is always high cost / low volume.

Deep Space Network stations or other applications (VLBI) where the
measurement uncertainty is like ADEV = 1E-12 in 1000 seconds. There's a
whole analysis of the temperature effects on the fiber optic
distribution components, for instance - and they're buried 2 meters down.

At "billions of dollars in 1960/1970" I think DSN fits in Bob's high
cost/low volume bucket.

Post by Bob kb8tq
Bob

Post by Hal Murray

My applications were broadband. If I remember correctly, aggressive
bandwidth limiting can cause phase shift problems due to temperature
changes unless one is careful in the design of the filter.

Does anybody ovenize amplifiers and filters to avoid that problem?
--
These are my opinions. I hate spam.
_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Mark Sims]

And it's the only way to be sure... never trust a simulation, particularly for such flighty and subtle things like noise. Simulations can be useful for pointing you in the right direction for a design, but where the rubber meets the road there is nothing like real hardware to get to the true answer.

----------------

Post by Rafael Gajanec
The only other reasonably fast and accurate way I can

think of is to build the bloody circuit and measure it using some
expensive equipment.
_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Bert Kehren via time-nuts]

Attila
Thank you for posting the link to Richard's excellent paper that does not
only apply to Cs. In my opinion it is a must read for any one serious in
doing any work on time and frequency issues.
Bert Kehren




In a message dated 10/27/2017 3:14:48 P.M. Eastern Daylight Time,
***@kinali.ch writes:

On Tue, 24 Oct 2017 12:12:24 -0700

This problem came up in the design of the 5071A.
I elected to avoid narrowband filters by using
some tricks described in my FCS paper of about
25 years ago. I didn't find it necessary to ovenize
the output section.

For those looking for the paper:
http://www.karlquist.com/FCS92.pdf


Attila Kinali
--
It is upon moral qualities that a society is ultimately founded. All
the prosperity and technological sophistication in the world is of no
use without that foundation.
-- Miss Matheson, The Diamond Age, Neil Stephenson
_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to
https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

_______________________________________________
time-nuts mailing list -- time-***@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

[Attila Kinali]

Hoi Bert,

On Sun, 29 Oct 2017 08:06:37 -0400

Post by Bert Kehren via time-nuts
Thank you for posting the link to Richard's excellent paper that does not
only apply to Cs. In my opinion it is a must read for any one serious in
doing any work on time and frequency issues.

Well, the way how the HP 5071 synthesis chain is designed is the way
one would do it today. Using SRDs went pretty much out of fashion,
and not only because they are hard to buy these days. Today we have
monolithic VCOs that give 9GHz in a tiny packages with good
phase noise performance. We have PLLs with integrated dividers that
can handle 10GHz inputs with 10MHz references directly. Ie you could
simplify the synthesis chain even further. You could build the complete
synthesis chain for the 5071 on a PCB of 5x5cm and still have space to spare.
Even using a DRO (for lower phase noise) would not make the circuit much bigger.

We kind of live in the golden age of electronics design, even if the constant
shrinking of parts makes them harder to handle for hobbyists.

Attila Kinali

[Hal Murray]

https://www.gps.gov/governance/advisory/meetings/2009-05/doherty.pdf

Thanks.

eLoran meets needs of all identified critical applications -- and others
-- 10-20 meter navigation accuracy for harbor entrance
-- 0.3 mile required navigation performance (RNP 0.3) & aviation integrity
-- Stratum 1 for precise frequency users & 50 ns time accuracy

Lots more info there. It wasn't expensive.
--
These are my opinions. I hate spam.




_______________________________________________
time-nuts mailing list -- time-***@lists.febo.com
To unsubscribe, go to http://lists.febo.com/mailman/listinfo/time-nuts_lists.febo.com
and follow the instructions there.