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

[Attila Kinali]

Hoi Bert,

On Sun, 29 Oct 2017 08:06:37 -0400
Bert Kehren via time-nuts  wrote:

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

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

[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,  
att...@kinali.ch writes:

On Tue,  24 Oct 2017 12:12:24 -0700
"Richard (Rick) Karlquist"   wrote:

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

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

[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.



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

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

[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

> On Oct 28, 2017, at 7:36 AM, Rafael Gajanec  wrote:
> 
> Hi Attila,
> 
> On 27-Oct-17 8:25 PM, Attila Kinali wrote:
>> Hi Rafael
>> 
>> On Sun, 22 Oct 2017 17:20:52 +0200
>> Rafael Gajanec  wrote:
>> 
>>> 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.
>> 
>>> but maybe the answer is Harmonic Balance.
>> Hmm.. I didn't know about Harmonic Balance. I have some reading up to do.
>> Thanks!
>> 
>>> 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.
> 
>> 
>>  Attila Kinali
> 
> Best regards,
> Rafael Gajanec
> ___
> time-nuts mailing list -- time-nuts@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-nuts@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

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

[Rafael Gajanec]

Hi Attila,

On 27-Oct-17 8:25 PM, Attila Kinali wrote:

Hi Rafael

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


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.



but maybe the answer is Harmonic Balance.

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


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.




Attila Kinali


Best regards,
Rafael Gajanec
___
time-nuts mailing list -- time-nuts@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

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

[Attila Kinali]

On Tue, 24 Oct 2017 12:12:24 -0700
"Richard (Rick) Karlquist"  wrote:

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

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

[Attila Kinali]

Hoi Bruce,

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

> 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." 

> 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!

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

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

[Attila Kinali]

Hi Rafael

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

> 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)

> but maybe the answer is Harmonic Balance.

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

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

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

[Attila Kinali]

Hoi Dana,

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

> 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

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

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

[jimlux]

On 10/24/17 11:54 AM, Bob kb8tq wrote:

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.





Bob


On Oct 24, 2017, at 2:10 PM, Hal Murray  wrote:


aph...@comcast.net said:

  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.



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

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

[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

> On Oct 24, 2017, at 2:10 PM, Hal Murray  wrote:
> 
> 
> aph...@comcast.net said:
>>  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.
> 
> 
> 
> ___
> time-nuts mailing list -- time-nuts@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-nuts@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

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

[Richard (Rick) Karlquist]

On 10/24/2017 11:10 AM, Hal Murray wrote:


aph...@comcast.net said:

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

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

[Hal Murray]

aph...@comcast.net said:
>   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.



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

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

[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)

On 10/24/2017 6:24 AM, Bob kb8tq wrote:

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


On Oct 24, 2017, at 6:09 AM, Anders Wallin  wrote:

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

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

[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

> On Oct 24, 2017, at 6:09 AM, Anders Wallin  
> wrote:
> 
> 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-nuts@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-nuts@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

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

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

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

[Gerhard Hoffmann]

Am 22.10.2017 um 22:58 schrieb 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 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-nuts@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

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

[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

> 
> On 23 October 2017 at 10:25 Bruce Griffiths  
> wrote:
> 
> 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
> 
> > > 
> > On 23 October 2017 at 03:23 Dana Whitlow  
> > wrote:
> > 
> > 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
> > 
> > On Sun, Oct 22, 2017 at 7:53 AM, Attila Kinali  
> > wrote:
> > 
> > > > > 
> > > > > > > 
> > > > 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
> > > 
> > > ___
> > > time-nuts mailing list -- time-nuts@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-nuts@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-nuts@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-nuts@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

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

[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

> 
> On 23 October 2017 at 03:23 Dana Whitlow  wrote:
> 
> 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
> 
> On Sun, Oct 22, 2017 at 7:53 AM, Attila Kinali  wrote:
> 
> > > 
> > 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
> > 
> > ___
> > time-nuts mailing list -- time-nuts@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-nuts@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-nuts@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

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

[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

> 
> On 23 October 2017 at 01:53 Attila Kinali  wrote:
> 
> 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
> 
> ___
> time-nuts mailing list -- time-nuts@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-nuts@febo.com
To unsubscribe, go to https://www.febo.com/cgi-bin/mailman/listinfo/time-nuts
and follow the instructions there.

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

[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


On 22-Oct-17 4:23 PM, Dana Whitlow wrote:

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

On Sun, Oct 22, 2017 at 7:53 AM, Attila Kinali  wrote:


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

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

[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

On Sun, Oct 22, 2017 at 7:53 AM, Attila Kinali  wrote:

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

[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

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