You choose a noise type of "timedomain" (noisetype=timedomain if you're using spectre standalone).

Ken refers to it as "strobed" noise, since that is a more descriptive way of describing what it does - however, it is called time domain noise in pnoise.

Regards,

Andrew.

Andrew,

I perform PSS simulation for a 8 divider. But it cannot converge. The result log is :

pss has reached the maximum iterations (20).
Error found by spectre during periodic steady state analysis `pss'.    pss analysis did not converge.

I tried more iterations and adding cmin in pss option but it still couldn't work.

It's a simple divider, consisting of 3 dff. I use a input pulse source with 192MHz.

Because this ckt is so simple, I cannot figure out what's the source making it unconverge.

But when I perform PFD/CP and VCO PSS simulation, it works well.

Is there some special requirment for divider PSS simulation?

Another Question:
I read through Ken's jitter+pnoise for the divider PSS simulation. It says "perform a PSS analysis to determine the threshold crossing times and the slew reate at these times".
I wonder how to dertermine the threshold crossing time by performing PSS analysis?

Any hint will be highly appreciated.

sorry for the unenough information

1. I dont use the Oscillator option

2. It seems I cannot set the fundmental frequency. As I mentioned, I  use a periodic pulse source as the input frequency. when I setup the PSS option, this periodic source automatically shown in the upper form, just above the "Beat Frequency" form (I cannot remember the name of the form coz I'm away from the Cadence GUI). I also remember I cannot set the Beat Frequency in this case.

3. When I perform PSS for the combination of VCO and divider, it converges with the maxstep 200ps. When I set the maxstep to 2ps, it wouldn't converge. So does it mean I shouldn't set the maxstep too small for PSS and Pnoise simulation.

Best Regards

Andrew,

sorry for the wrong information. I check the PSS option again and find I can set the Beat Frequency to 24MHz(i.e. 1/8 of 192M input signal). The PSS analysis can run now but I still have several questions:

1.      In the Pnoise Analysis, I set Maximum sideband to 20; Reference side-band: 1; Choose Noise Type to timedomain. But what’s the appropriate number for “Noise Skip Count” or “Number of Points”? I set Noise Skip Count to 100
2.      In PSS analysis, I set the maxstep to 20ps. Does it too large or too small? When I set 200ps, the result log shows:
“Convergence failure counts:
   70         _net0
   70         _net0
   71         avdd1p8v
   71         avdd1p8v
   71         avss1p8v
   71         avss1p8v
   1          out
   1          out
71      V0:p
…….
Maximum value achieved for any signal of each quantity:
   I: I(V2:p) = 508.1 uA
   V: V(I0.I77.I15.M1:int_d) = 1.97 V
pss: The steady-state solution was achieved in 3 iterations.
           
It seems it cannot reach convergence, but the steady-state solution was still achieved. Does it mean the following Pnoise analysis won’t be correct?

When I set maxstep to 20ps. The result log shows:

Convergence failure counts:
Maximum value achieved for any signal of each quantity:
   I: I(V2:p) = 508.1 uA
   V: V(I0.I77.I15.M1:int_d) = 1.97 V
pss: The steady-state solution was achieved in 3 iterations.

3.      After the Pnoise analysis, I cannot get the curve like Fig 10 in Ken’s paper “jitter + pnoise”. I use the result browser to observe timedomain pnoise. But the curve is totally different from what is shown in Fig 10. The unit of the Y axis is V/sqr(Hz).

Thanks in advance for your time and patience.

Hey Ken,
Thanks for your reply. I did the simulation as you indicated in your last post.  
 
1. My divider is a 1/8 ripple divider. As you wrote in your paper, I should only simulate one stage at one time. My input frequency is 200MHz. So after the fist stage, the frequency should be 100MHz.  
 
2.I set the beat frequency 100MHz in PSS form. In the pnoise form. I use timedomain option and add the cross time point 0.5ns. After I finished the simulation, I could only observe the result in the "Result Browser". The unit of the pnoise result is V/sqr(Hz). Then to get the variance of output noise, I should integrate the result from 0 to f0/2(i.e. 100M/2). Here is the question: I am not sure whether I should integrated the result directly since the unit is V/sqr(Hz)? I think I should firstly change the unit from V/sqr(Hz) to V**2/Hz. To do so, after I get the date of timedomain.pnoise from the result browser, I use the X**2 button on the calculator to squre the result. Then use Integ function to integrate it from 0 to 100M/2. Then I use Eq(54) to calculate Jee.
Am I right? If not, how to calculate the var(nv(tc)) with the "V/sqr(Hz)" result?    
 
3. With the method mentioned above. I get the jitter for the first stage: about 0.2 ps. Then I suppose the other two stages have the same jitter since these stages are all same and you said jitter was independent on the input frequency. Then I calculate the total jitter by Jee= sqr(0.2**2+0.2**2+0.2**2), resulting at 0.3xx ps. Is this too small for a 1/8 divider?    
 
Thanks for your time. your explanation will be highly appreciated.
 
Bests,
 
James