Stats

  • Locked Locked
  • Replies 17
  • Subscribers 125
  • Views 21841
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Noise Figure of track and hold circuit

Alok110

Hi, I am trying to get Noise Figure in track and hold circuit with RC>>Ts/2. My ckt is like RC low pass filter {Port(with res=50) + switch + cap to gnd }

NF= 10logF,  where F is Noise Factor
and F = (Ni+Nsys)/Ni.

In my circuit Nsys = 0 (Sys include only switch and cap, there is no res(noise generator)). so, F should be =1, so the Noise figure should be = 0.
But, cadence giving me F = 1.96  and NF = 2.92 dB. (I am measuring it with Pss+Pnoise)


what I am doing wrong?

                           

Fullscreen netlist.txt.txt Download 
// Library name: PHD22
// Cell name: switching
// View name: schematic
W0 (Prt net02 clk 0) relay vt1=1m vt2=500.0m ropen=1T rclosed=1.0
C1 (net02 0) capacitor c=c
V1 (clk 0) vsource type=pulse val0=0 val1=500.0m period=1/f width=1/(2*f) \
        fundname="CLK"
PORT1 (Prt 0) port r=r dc=DC/2 type=sine freq=frf ampl=Amp/2 mag=Ac_mag/2 \
        isnoisy=yes
Fullscreen Input(scs).txt Download 
// Generated for: spectre
// Generated on: Aug 14 21:28:57 2021
// Design library name: PHD22
// Design cell name: switching
// Design view name: schematic
simulator lang=spectre
global 0
parameters r=50 frf=50M f=50000k c=1000n DC=0 Amp=1 Ac_mag=0

// Library name: PHD22
// Cell name: switching
// View name: schematic
W0 (Prt net02 clk 0) relay vt1=1m vt2=500.0m ropen=1T rclosed=1.0
C1 (net02 0) capacitor c=c
V1 (clk 0) vsource type=pulse val0=0 val1=500.0m period=1/f width=1/(2*f) \
        fundname="CLK"
PORT1 (Prt 0) port r=r dc=DC/2 type=sine freq=frf ampl=Amp/2 mag=Ac_mag/2 \
        isnoisy=yes
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=50M  harms=20  errpreset=liberal  autotstab=yes
+    saveinit=yes  method=gear2only  tstabmethod=gear2only  maxacfreq=50G
+    annotate=status
pnoise  (  net02  0  )  pnoise  start=1  stop=25M
+       maxsideband=1000  iprobe=PORT1  refsideband=0
+       noisetype=timeaverage  noiseout=[usb]  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=all

 

Parents

  • Dear Alok110,

    Alok110 said:

    In my circuit Nsys = 0 (Sys include only switch and cap, there is no res(noise generator)). so, F should be =1, so the Noise figure should be = 0.
    But, cadence giving me F = 1.96  and NF = 2.92 dB. (I am measuring it with Pss+Pnoise)


    what I am doing wrong?

    Just reading your description, Alok110, does not really give me the full picture of your circuit and simulation results to be honest - I apologize if I am overlooking something!

    However, I do see a number of items that I consider "red flags" and list them below.

    1. Did you check to make sure the port resistance of 50 ohms has its noise term disabled? There is an option for it to produce noise and want to make sure it is, indeed, noiseless.

    2. You have set the number of "output harmonics" in your pss analysis GUI to 0. Is this really reasonable for a sampled signal (especially since you chose a "Shooting method" for your pss analysis)?

    3. I have personally never seen anyone select the "liberal" level of simulation accuracy for a css analysis. Why are you choosing such a relaxed tolerance (especially for such a small circuit). The accuracy of your steady-state solution may be compromised and this will clearly impact the accuracy of your estimated NF. Are you using spectre or spectre with +aps or ++aps or spectre X? You did not indicate and did not include any log files (which would be exceedingly useful to understand your results).

    4. With the "liberal" level of simulation accuracy, did you visually  inspect the pss solution? Did you run a companion conventional analysis and compare the estimated pss solution waveform to the transient waveform after it reaches steady-state to see if the pss solution appears close to that of the transient steady-state solution?

    5. In your PSS analysis, it appears you are not saving the transient results. Is there a reason you are not? It can be helpful. You also are not specifying a value for tstab. I would suggest you might consider setting it to a time when your conventional transient simulation appears to be close to its steady-state waveform.

    We recently had a similar set of discussions concerning a noise figure analysis for a track and hold circuit using pss and you might want to review its contents if you have not seen it. I think it may be provide you some added insights.

    community.cadence.com/.../question-on-pss-pnoise-simulation-for-a-track-and-hold-circuit

    Shawn

  • in reply to ShawnLogan

    Hi Shawn,

    I am really delighted to see such a detailed reply. Thank you for your time and efforts.

    I am fairly new with PSS and Pnoise analysis. I will try your suggestions.

    In my circuit RC>> Ts/2,I did PSD calculation for same circuit with this same settings (harmonics =0, no saving of transient result and all) and I got the expected PSD and total noise result .Port resistance is 50 ohms and I think it as source resistance which generate source noise. If I disable the noise from port then simulator doesn't calculate NF and F.

    I tried same circuit without switch (bypassing switch) and did noise sim, and my F and NF were coming as expected.

    I am using spectre +aps.

    Thank you again.

Reply
  • in reply to ShawnLogan

    Hi Shawn,

    I am really delighted to see such a detailed reply. Thank you for your time and efforts.

    I am fairly new with PSS and Pnoise analysis. I will try your suggestions.

    In my circuit RC>> Ts/2,I did PSD calculation for same circuit with this same settings (harmonics =0, no saving of transient result and all) and I got the expected PSD and total noise result .Port resistance is 50 ohms and I think it as source resistance which generate source noise. If I disable the noise from port then simulator doesn't calculate NF and F.

    I tried same circuit without switch (bypassing switch) and did noise sim, and my F and NF were coming as expected.

    I am using spectre +aps.

    Thank you again.

Children
No Data

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.