1. Flicker noise is problematic in that most jitter metrics are undefined in the presence of flicker noise.
2. You should choose to compute c at a frequency where flicker noise is negligible.
3. The flicker_noise function produces a non-zero onlyl during the small-signal noise analyses. During large signal analyses it always produces zero. So that any way that you have of observing its output will always give zero unless you observe it indirectly by looking at the output of a noise analysis. You can view the contributed noise summary produced by the noise analysis to confirm that it is operating properly.

-Ken

What is causing the difference?

-Ken

You could use Verilog-A to create a large-signal white noise source and then pass the output through a fracpole with a slope of 1/2.

-Ken

I just tried doing a pnoise analysis of the VCO including flicker and white noise as described below.
When plotting the phase_noise button I do not obtain the expected curve with 1/f^2 and 1/f^3 regions. Instead it is just a flat response at some dB value.
What might be the problem?

   freq = f0+Kvco*V(in);
   phase = 2*`M_PI*idtmod(freq, 0.0, 1.0, -0.5);
   phase = phase +  flicker_noise(n,2,"wpn") +                        
   flicker_noise(n*fc,3,"fpn");

I choose a c value of 82e-21, f0=1.1Ghz, and thus n=0.2 according eq. 29 in your paper "predicting noise in plls".

Here is how I configure the analysis.
pss  (out  0)  pss  fund=6e6  harms=3  errpreset=moderate tstab=120n  annotate=status
pnoise  (out  0)  pnoise  sweeptype=relative  relharmnum=1 start=1  stop=10M  log=100  maxsideband=15  annotate=status

Thanks,
svensl

Ken,
I had a look at the section in your book and modified my code as given below. However, I still obtain only a flat phase noise response. The model is as follows:

`include "disciplines.vams"
`include "constants.vams"
module sdvcoct (out, in);
input in; voltage in;                  
output out; voltage out;            
parameter real f0=1e6;
parameter real Kvco=50e5;
real freq, phase;
parameter real period=2.56e6;
parameter real n =0.2 from [0:inf);      
parameter real fc = 1e6  from [0:inf);  
analog begin
   freq = f0+Kvco*V(in);
   phase = 2*`M_PI*idtmod(freq, 0.0, 1.0, -0.5);
   V(out) <+ sin(phase) + flicker_noise(n,2,"wpn") +    
   flicker_noise(n*fc,3,"fpn");
end
endmodule

The VCO gain is set to 50e5 and the freq. to 1e6. The control voltage is set by a dc source (1V).
I choose a PSS analysis first with beat freq. 6e6, no. of harmonics 3, accuracy moderate, tstab 120n, check the oscillator button, choose vout and gnd! for the output node.
The pnoise analysis has sweeptype relative (harmonic 1), freq. range 1 to 10M, scale logarithmic with 100 steps, max. sidebands 15, and the pos. output node being out and the negative being gnd!.
When plotting I choose the main form, choose pnoise, and then the phase noise button.
Any ideas what might be wrong?
Cheers

Ken,

There is a warning saying that:
The Floquet eigenspace computed by Virtuoso(R) Spectre(R) PSS analysis appears  to be inaccurate. PNOISE computations may be inaccurate. Consider re-running the simulation with smaller reltol and `method=gear2only'.
I tried changing the settings for reltol and method but without any change. I saved the netlist to strip it down to:
simulator lang=spectre
global 0
ahdl_include "/home/sven/cadence/AHDL_CODE/VCO/veriloga/veriloga.va"
parameters crtl=1
V0 (net2 0) vsource dc=crtl pacmag=1 type=dc
I0 (out net2) sdvcoct
pss  (out  0)  pss  fund=1e6  harms=3  errpreset=conservative tstab=120n  reltol=1e-8 maxstep=1e-8 method=gear2only
pnoise  (out 0)  pnoise  sweeptype=absolute  start=1 stop=10M  log=500  maxsideband=15
saveOptions options save=allpub

But still no change in the output. I then switched from Spectre Version 5.1.0 05/24/2004 to Version 5.0.0 09/23/2003 and it works!
I still get the same warning, but the result is as expected. I did not change anything in the netlist or the veriloga model. Just a change in the Version. Why do I keep getting wrong results with the newer version of spectre? Please see also
http://www.designers-guide.org/Forum/?board=circuit;action=display;num=112391795...
I still have not solved that problem as well.

Any thoughts?
Thanks so much for any feedback.

From doing a quick search, it may have been due to this PCR (I'm not certain):

   PCR: 713247
 Title: white_noise does not work with integer argument

The second argument to your flicker_noise function is an integer (try making it a real by adding ".0" onto the end?) and that might be confusing the compiler. Anyway, it was fixed in an ISR soon after the CD version was released. The same bug was in IC5033 too. Sometimes bugs creep in, of course...

Try using IC5141 USR2 - or using the latest MMSIM60 simulator release (put MMSIM60 at the beginning of your path, in conjunction with IC5141 USR2, to get the latest version of spectre). If you use MMSIM60 you have access to a transient noise analysis too (with the usual warnings about the fact that these analyses are best for qualitative analysis of noise behaviour rather than quantatitive analysis, well, unless you run with the noise bandwidth set high enough and run the simulation for a very long time).

Regards,

Andrew.