The Designer's Guide Community
Forum
Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.
May 20th, 2019, 9:28am
Pages: 1 2 3 
Send Topic Print
Question about phase noise simulation result (Read 36562 times)
Ken Kundert
Global Moderator
*****
Offline



Posts: 2161
Silicon Valley
Re: Question about phase noise simulation result
Reply #15 - Jul 02nd, 2011, 9:04am
 
YCY,
    One obvious difference is that the modulated noise analysis extracts the phase noise SΦ in units of radians2/Hertz whereas jitter analysis extracts the jitter in units of seconds2/Hertz. But the difference between the two is deeper than that. To see the difference between modulated noise and jitter, consider white noise added to a sine wave.

The modulated noise analysis will see equal amounts of AM and PM noise. The jitter analysis will pass the signal through an internal limiter to determine the jitter. That limiter will have the effect of converting the noise in the signal (both the AM and PM components as appropriate given the level of the threshold) to jitter. So the modulated noise analysis examines the entire signal to determine the PM noise whereas the jitter analysis only examines the noise at the threshold.

Further consider the case where you have a noise free signal that is amplitude modulated with noise. The modulated noise analysis will examine this signal and find no PM noise. But if the threshold is not at zero, the jitter analysis will find jitter.

Conversely, consider the case were you have a signal that consists of white noise and a large square wave with infinitely fast transitions. The white noise will cause the modulated noise analysis to report equal amounts of AM and PM noise, whereas the jitter analysis will find no jitter because the small amount of noise cannot affect the time of the threshold crossing because of the infinitely fast transition times of the square wave.

On your second question about noise correlation, the point is not that there is no frequency translation, but rather than the translated signals cannot be correlated because they must have different original source frequencies. In other words, because of the constraints on the passband of the filter, there is no frequency where the original source frequencies of the various translations is the same, therefore the various translations cannot be correlated.

-Ken
Back to top
 
 
View Profile WWW   IP Logged
Frank Wiedmann
Community Fellow
*****
Offline



Posts: 642
Munich, Germany
Re: Question about phase noise simulation result
Reply #16 - Jul 4th, 2011, 4:06am
 
In this context, the discussion I had with Ken a long time ago at http://www.designers-guide.org/Forum/YaBB.pl?num=1036850366 might also be interesting. AM and PM noise as calculated by SpectreRF are probably most meaningful for sinusoidal signals.

When you simulate the jitter of autonomous circuits (oscillators etc.) with SpectreRF, you should be aware that the default FM jitter analysis is based on modulated noise. In order to get the same analysis type as in the jitter analysis for driven circuits, you must select PM jitter. It took Andrew Beckett and me several years to get this option into ADE (see http://www.designers-guide.org/Forum/YaBB.pl?num=1158924743/4#4). See also http://www.cadence.com/community/forums/T/17940.aspx for how to interpret the simulation results.
Back to top
 
 
View Profile WWW   IP Logged
YCY
Community Member
***
Offline



Posts: 32

Re: Question about phase noise simulation result
Reply #17 - Jul 4th, 2011, 7:03pm
 
Hi, Ken and Frank

Thanks for your detailed description, I believe I have a further
understanding of phase noise and how SpectreRF calculate it now.
On the other hand, after going through the thread Frank provided,
I have some other questions:

1.How to determine the "threshold" in Pnoise jitter mode?
  We usually set the threshold to Vdd/2 in logic circuits.
  However this is an ideal value. In reality the threshold value
  may vary according to many causes, like Vdd ripple, devices mismatches...and so on.
  How can we precisely choose the threshold value?
  Or the threshold value doesn't affect the result much?
  (I myself have tried a chain of inverts with Vdd=1.2 V, and
  set the threshold value from 0.4 to 0.8 V, the resulting jitter
  doesn't have significant difference, the largest difference is less than 3 dB.)

2.It seems PM jitter in jitter mode is used to simulate oscillator followed by driven circuits, like buffer or divider.
   Then what is FM jitter for? Is it like the PM noise in the modulated mode but just reported in the unit of second/sqrt(Hz)?

3.In the thread http://www.designers-guide.org/Forum/YaBB.pl?num=1158788102;start=all, Ken said
   "...If you are in the 1/Δf 2 region, then the noise from the phase mode in the oscillator is dominating.
   In this case, using strobed noise to determine the phase noise should give the same result as using
   the time-averaged noise..."
   I don't understand what's the meaning of "if your are in the 1/Δf 2 region".
   Does it mean that we concern about the spot phase noise at a certain frequency which is in the 1/Δf 2 region?

Regards,

YCY
Back to top
 
 
View Profile   IP Logged
neoflash
Community Fellow
*****
Offline

Mixed-Signal
Designer

Posts: 382

Re: Question about phase noise simulation result
Reply #18 - Jul 4th, 2011, 7:44pm
 
It seems that as long as the block is followed by a thresholding circuit ( which seems to be always the case), strobed noise analysis is always more accurate than time-averaged analysis in phase noise and jitter analysis.

- Neo

YCY wrote on Jul 4th, 2011, 7:03pm:
   "...If you are in the 1/Δf 2 region, then the noise from the phase mode in the oscillator is dominating.
   In this case, using strobed noise to determine the phase noise should give the same result as using the time-averaged noise..."
 

Back to top
 
 
View Profile   IP Logged
YCY
Community Member
***
Offline



Posts: 32

Re: Question about phase noise simulation result
Reply #19 - Jul 5th, 2011, 12:34am
 
One more question,
Ken said when the divider is followed by a mixer, which is a thresholding
circuit, one should use "time domain" to strobe the noise at the threshold crossings.
(http://www.designers-guide.org/Forum/YaBB.pl?num=1158788102;start=all)
But in a receiver, shouldn't we simulate the sideband noise to carrier ratio (phase noise in the source mode)
to see the effect of reciprocal mixing?

So my question is what simulation (source or jitter mode) should we do to measure the phase noise
when the VCO is followed by a divider to change the output frequency, if this output signal is sent to a mixer as an LO?
Back to top
 
 
View Profile   IP Logged
neoflash
Community Fellow
*****
Offline

Mixed-Signal
Designer

Posts: 382

Re: Question about phase noise simulation result
Reply #20 - Jul 5th, 2011, 10:39am
 
Finally, we need Ken to confirm this.

However, I believe if your VCO + divider are clamped by some ideal voltage sources, such as an inverter biased at an ideal voltage supply, you should get the identical result since there is no AM noise left in source mode.

Otherwise, you should get more accurate result in jitter mode.

It seems that we should always use jitter mode.

Is this right, Ken?


YCY wrote on Jul 5th, 2011, 12:34am:
One more question,
Ken said when the divider is followed by a mixer, which is a thresholding
circuit, one should use "time domain" to strobe the noise at the threshold crossings.
(http://www.designers-guide.org/Forum/YaBB.pl?num=1158788102;start=all)
But in a receiver, shouldn't we simulate the sideband noise to carrier ratio (phase noise in the source mode)
to see the effect of reciprocal mixing?

So my question is what simulation (source or jitter mode) should we do to measure the phase noise
when the VCO is followed by a divider to change the output frequency, if this output signal is sent to a mixer as an LO?

Back to top
 
 
View Profile   IP Logged
Ken Kundert
Global Moderator
*****
Offline



Posts: 2161
Silicon Valley
Re: Question about phase noise simulation result
Reply #21 - Jul 5th, 2011, 1:02pm
 
Let me clarify. My advice was for the case where you were simulating just the divider while anticipating that when placed in the larger circuit it would be followed by a thresholding circuit such as a mixer. In otherwords, the noise measurement you make should depend on the circuit that will eventually be affected by the noise. In the case of a divider that will be followed by a mixer, you should use sampled noise option ('time domain') because it only includes noise that occurs at or near the threshold crossings, which is the only noise that will affect the subsequent mixer.

Since the underlying noise analysis is the same, reciprocal mixing would be included in either the 'time-domain' or 'sources' noise analysis if (and only if) you include a large interfering tone at the input to the mixer. Since the mixer is not included when simulating divider alone, the question of reciprocal mixing is moot in the case I was talking about. If you include the mixer and the divider in one simulation, then my advice does not apply. In that case, the type of noise analysis you would use would be determined on the type of circuit that followed the mixer. Since continuous time filters normally follow the mixer, you would probably use 'sources' if the mixer were not included in the simulation. If the filter was included, then the type of noise analysis is determined by what follows the filter, which is presumably a sample and hold, in which case you would use a 'time-domain' noise analysis. Etc.

Hopefully you can see that you are not really tailoring your noise analysis to what is in the circuit, but rather by what follows the circuit, because you need to measure the output noise in a way that is compatible with the way the next stage would see it.

-Ken
Back to top
 
 
View Profile WWW   IP Logged
YCY
Community Member
***
Offline



Posts: 32

Re: Question about phase noise simulation result
Reply #22 - Jul 5th, 2011, 7:08pm
 
neoflash wrote on Jul 5th, 2011, 10:39am:
However, I believe if your VCO + divider are clamped by some ideal voltage sources, such as an inverter biased at an ideal voltage supply, you should get the identical result since there is no AM noise left in source mode.


Hi, Neo

Yes I think you are right. No AM noise left in that situation.
But when you said "you should get the identical result",
do you mean the two results from "jitter" and "source" mode?
If so, I think we will not get the same result.

I've tried a VCO followed by a limiting amplifier and simulated
the phase noise by jitter, modulated, and source mode.
The results are different.
I think this is because the noise is calculated at the threshold crossing
in the PM jitter mode, whereas in the source mode noise is calculated in
the time-average method.
Here is my simulation result:


regards,

YCY
Back to top
 
 
View Profile   IP Logged
YCY
Community Member
***
Offline



Posts: 32

Re: Question about phase noise simulation result
Reply #23 - Jul 5th, 2011, 8:05pm
 
Hi, Ken

Thanks for your response.
I try to rephrase your reply in the following to confirm if I really understand what you meant.

1. If VCO alone is simulated, both source or  time-domain (FM jitter) analysis can be used to simulate phase noise.
    Because VCO compresses the AM noise, source and time-domain analyses will give identical result.

2. If VCO+buffer is simulated and the following stage is a divider, time-domain (PM jitter) is used.
   Because divider is a thresholding circuit.

3. If VCO+buffer+divider is simulated and the following stage is mixer or PFD, time-domain (PM jitter) is used.
   Because mixer and PFD are thresholding circuits.

4. If a continuous-time circuit is followed, the source mode is applied.

In conclusion, the type of noise simulation depends on the circuit that follows.

BTW, could you please also answer my questions in reply#17?
I still have no idea about the answers of them, especially #1.
Thanks a lot, your help is really appreciated.

regards,

YCY
Back to top
 
 
View Profile   IP Logged
Ken Kundert
Global Moderator
*****
Offline



Posts: 2161
Silicon Valley
Re: Question about phase noise simulation result
Reply #24 - Jul 5th, 2011, 10:29pm
 
YCY,
    Why, I'd think it would be obvious at this point. You set the threshold equal to the threshold of the subsequent circuit. If you want to determine the threshold of the subsequent circuit, sweep the input voltage to the circuit while calculating the gain, the threshold would be where the gain is the maximum.

-Ken
Back to top
 
 
View Profile WWW   IP Logged
neoflash
Community Fellow
*****
Offline

Mixed-Signal
Designer

Posts: 382

Re: Question about phase noise simulation result
Reply #25 - Jul 5th, 2011, 10:53pm
 
If YCY is concerned with uncertainty of the threshold voltage, I suggest you do some simulation with different values.

They should not vary too much. And the variation is also something that your design should cover.

- Neo

Ken Kundert wrote on Jul 5th, 2011, 10:29pm:
YCY,
    Why, I'd think it would be obvious at this point. You set the threshold equal to the threshold of the subsequent circuit. If you want to determine the threshold of the subsequent circuit, sweep the input voltage to the circuit while calculating the gain, the threshold would be where the gain is the maximum.

-Ken

Back to top
 
 
View Profile   IP Logged
YCY
Community Member
***
Offline



Posts: 32

Re: Question about phase noise simulation result
Reply #26 - Jul 6th, 2011, 12:31am
 
Ken Kundert wrote on Jul 5th, 2011, 10:29pm:
YCY,
    Why, I'd think it would be obvious at this point. You set the threshold equal to the threshold of the subsequent circuit. If you want to determine the threshold of the subsequent circuit, sweep the input voltage to the circuit while calculating the gain, the threshold would be where the gain is the maximum.

-Ken


Hi, Ken

Thanks, that's what I want to know.

Hi, Neo

Thanks, your suggestion is also useful.

regards,

YCY
Back to top
 
 
View Profile   IP Logged
Frank Wiedmann
Community Fellow
*****
Offline



Posts: 642
Munich, Germany
Re: Question about phase noise simulation result
Reply #27 - Jul 6th, 2011, 2:19am
 
There are a few more things to watch out for when using modulated pnoise.

First, the definition for AM and PM noise in the formulas used by ADE has been changed recently (in IC 5.10.41.500.6.144 and IC6.1.4.500.7, see http://support.cadence.com/wps/mypoc/cos?uri=deeplinkmin:ViewSolution;solutionNu...). For an ideal sine source with white additive noise, AM and PM noise now have the same value as USB and LSB noise. Before that, AM and PM noise were 3 dB lower.

Second, there may be a bug in the formulas that ADE uses to compute AM and PM noise. So far, I have never used modulated pnoise because jitter analysis is generally more useful in my designs. However, due to the recent discussions, I wanted to examine modulated pnoise a little more closely. So I created the attached test circuit (the box is the multiplier from ahdlLib), expecting only AM noise at node am and only PM noise at node pm. However, this is not the result I get from SpectreRF and ADE. Looking at the results more closely, it seems like the correlation between the sidebands might be taken into account with only half of the correct value. I have submitted this to Cadence as Service Request 42540676, they are currently looking into it.

If there is a bug in modulated pnoise, it probably also applies to FM jitter for autonomous circuits, which is based on modulated pnoise. I have not checked this, though.

Here is the netlist for the test circuit:
Code:
// Generated for: spectre
// Generated on: Jul  6 10:43:58 2011
// Design library name: fw_test
// Design cell name: test_mod_noise_am_pm
// Design view name: schematic
simulator lang=spectre
global 0

// Library name: fw_test
// Cell name: test_mod_noise_am_pm
// View name: schematic
Vam (m_am 0) vsource type=sine sinedc=0 ampl=1 sinephase=0 freq=1G
Vpm (m_pm 0) vsource type=sine sinedc=0 ampl=1 sinephase=90 freq=1G
Vsig_pm (pm mn_pm) vsource type=sine ampl=1 freq=1G
Vsig_am (am mn_am) vsource type=sine ampl=1 freq=1G
mult_pm (n_pm m_pm mn_pm) multiplier
mult_am (n_am m_am mn_am) multiplier
Rpm (n_pm 0) resistor r=1K
Ram (n_am 0) resistor r=1K
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
    tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
    digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
    checklimitdest=psf
pss  pss  fund=1G  harms=1  errpreset=conservative  annotate=status
mod1  (  am  0  )  pnoise  sweeptype=relative  relharmnum=1
+       start=0  stop=500M  maxsideband=5  annotate=status
mod2  (  am  0  )  pnoise  sweeptype=relative  relharmnum=1
+       start=-(0)  stop=-(500M)  maxsideband=5  noisetype=correlations
+       cycles=[0  -2]  annotate=status
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts  where=rawfile
saveOptions options save=allpub currents=all subcktprobelvl=5 \
    saveahdlvars=all
ahdl_include "/tools/ic5141isr148/tools/dfII/samples/artist/ahdlLib/multiplier/veriloga/veriloga.va"
 

Back to top
 
View Profile WWW   IP Logged
Frank Wiedmann
Community Fellow
*****
Offline



Posts: 642
Munich, Germany
Re: Question about phase noise simulation result
Reply #28 - Jul 14th, 2011, 1:51am
 
I have now received an answer from Cadence. As it turns out, the formulas used for calculating AM and PM noise assume bandlimited noise. If I limit the bandwidth of the noise source to less than the modulation frequency before modulating it, I get the correct result.

Here is the netlist for the modified circuit:
Code:
// Generated for: spectre
// Generated on: Jul 14 10:26:54 2011
// Design library name: fw_test
// Design cell name: test_mod_noise_am_pm
// Design view name: schematic
simulator lang=spectre
global 0

// Library name: fw_test
// Cell name: test_mod_noise_am_pm
// View name: schematic
Vnpm (n_pm 0) vsource type=dc noisevec=[ 0 1 900M 1 950M 0 ]
Vnam (n_am 0) vsource type=dc noisevec=[ 0 1 900M 1 950M 0 ]
Vsig_pm (pm mn_pm) vsource type=sine ampl=1 freq=1G
Vsig_am (am mn_am) vsource type=sine ampl=1 freq=1G
Vpm (m_pm 0) vsource type=sine sinedc=0 ampl=1 sinephase=90 freq=1G
Vam (m_am 0) vsource type=sine sinedc=0 ampl=1 sinephase=0 freq=1G
mult_pm (n_pm m_pm mn_pm) multiplier
mult_am (n_am m_am mn_am) multiplier
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
    tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
    digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
    checklimitdest=psf
pss  pss  fund=1G  harms=1  errpreset=conservative  annotate=status
mod1  (  am  0  )  pnoise  sweeptype=relative  relharmnum=1
+       start=0  stop=1G  maxsideband=5  annotate=status
mod2  (  am  0  )  pnoise  sweeptype=relative  relharmnum=1
+       start=-(0)  stop=-(1G)  maxsideband=5  noisetype=correlations
+       cycles=[0  -2]  annotate=status
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts  where=rawfile
saveOptions options save=allpub currents=all subcktprobelvl=5 \
    saveahdlvars=all
ahdl_include "/tools/ic5141isr148/tools/dfII/samples/artist/ahdlLib/multiplier/veriloga/veriloga.va"
 

Back to top
 
 
View Profile WWW   IP Logged
radiohead
New Member
*
Offline



Posts: 1

Re: Question about phase noise simulation result
Reply #29 - Nov 24th, 2015, 3:44am
 
Hi all,

Very interesting and helpful comments. Following the discussion, i use strobed PNoise (time domain) with spectreRF to find the jitter of a frequency divider. In an effort to correlate time domain pnoise with sources pnoise i would expect that if i average the total noise (V^2/Hz) at a certain frequency offset, then this quantity must equal the output noise in (V^2/Hz) estimated using the sources method. Although this is not what i get from spectreRF.
Back to top
 
 
View Profile   IP Logged
Pages: 1 2 3 
Send Topic Print
Copyright 2002-2019 Designer’s Guide Consulting, Inc. Designer’s Guide® is a registered trademark of Designer’s Guide Consulting, Inc. All rights reserved. Send comments or questions to editor@designers-guide.org. Consider submitting a paper or model.