PSS simulation for VCO

Dear yefj,

A few suggestions follow...

1. Let spectre compute the frequency since you have specified this is an oscillator. I noticed you are entering the beat freuqency. There is a check box to allow spectre to compute the frequency.

2. With an LC or other higher Q based oscillator, you need to guarantee that sufficient samples are taken over the period of oscillation. You are using an errpreset of "moderate" and I don't see that you have specified a value for maxstep (maximum time step for integration). With an errpreset of "moderate", the maximum integration step size is determined by dividing the time of the simulation (30.48 ns?) by 50. In your example, this is 30.48 ns/50 = 609 ps. However, the period of your oscillator is 74 ps. Hence, the maximum time step is far too large and may result in simulator accuracy errors. I would suggest including a maximum integration time step of, perhaps, 1 or 2 ps (maxstep = 1 ps, for example).

3. Your oscillator waveform is near sinusoidal. Hence, you might consider the use of harmonic balance in lieu of the shooting algorithm.

Shawn

Hi yefj,

There are examples of how to setup an oscillator - both ring (strongly_nonlinear) and sinusoidal (linear) in the RF_Doc_Database

​database located in <SPECTRE17.1 hierarchy>/tools.lnx86/spectre/examples/SpectreRF_workshop/RF_Doc_Database.tar.gz

And I believe the instructions are located here: <SPECTRE17.1>/doc/spectreRFexplorerWorkshop/spectreRFexplorerWorkshop.pdf

The best part is...it explains the "why" about how set up the analysis.   Great step-by-step tutorials.    Also see:  Article 2046330 SpectreRF AppNotes and Tutorials - One of Our Best Kept Secrets! on https://support.cadence.com .

Best regards,

Tawna

Unknown said:

1. Let spectre compute the frequency since you have specified this is an oscillator. I noticed you are entering the beat freuqency. There is a check box to allow spectre to compute the frequency.

Hello Shawn,as you suggested i was  able to check this option when i switched my PSS to harmonic balance instead of shooting.

after checking this option it still gives me an error that i must specify a value,although it disables this option when the box checked.

it doesnt allow me to auto calculate the beat frequency.

Unknown said:

However, the period of your oscillator is 74 ps. Hence, the maximum time step is far too large and may result in simulator accuracy errors. I would suggest including a maximum integration time step of, perhaps, 1 or 2 ps (maxstep = 1 ps, for example).

There is no maxstep option in the PSS window as shown bellow.

also spectreRF manual says(shown bellow) that for highly non linear oscillator (i have diodes an transistors) i should use shooting PSS.

what could be done to make it work properly? (i showed bellow my pss window)

Thanks

Hello Tawna,Yes i am following the spectrerf manual , i am showing quotes of definitions in my first post to justify the numbers i used, and a step by step of how it was done, in order to see where my implementation differs from the spectre rf manual.

Thanks

Several points here:

1. Shawn made a small mistake - the auto-calculate for the beat frequency doesn't work with oscillators, since it uses the frequencies on sources in the schematic and you don't have that, so you have to enter a number which is an estimate of the oscillation frequency (or the lowest frequency in the circuit if you have dividers as well)
2. maxstep is on the Options form at the bottom of the PSS (or hb) form. It's a good idea to ensure enough points that the oscillation builds up
3. The presence of diodes or transistors in your circuit isn't enough that you then couldn't use harmonic balance - that doesn't necessarily make it "strongly nonlinear". So you might still want to try hb with the harmonics set to "auto". If using hb, use the hb analysis rather than the harmonic balance on PSS - it has better automation (the simulator algorithms are the same, but it's a bit more usable).
4. Make sure you have a long enough transient assist time - you can turn on the option Detect Steady State. 
5. Whether you need 1 or 2 in the relative harmonic for the noise analysis depends on the frequency you want to measure the noise at. If  your oscillator oscillates at 13GHz, but you have a frequency doubler and you want to use it (and measure the noise) at 26GHz, then  you'd enter 2. If you wish to use the oscillation frequency at 13GHz, then enter 1. What it means is that you are measuring the output noise at relHarm*PSSfund+outputFreq where outputFreq is what you're sweeping
6. It would be much easier if you uploaded (ideally as an attachment) the entire spectre.out log file rather than just the bits you think are important - there is a lot of info in there which would have captured important parameters, how it had been converging (or not). Just reporting the final error isn't very helpful...

Regards,

Andrew.

Dear Andrew,

Thank you for correcting my error! I appreciate, very much, your insight and correction - as always - I have a lot to learn.

Shawn

Andrew Beckett said:

It would be much easier if you uploaded (ideally as an attachment) the entire spectre.out log file rather than just the bits you think are important - there is a lot of info in there which would have captured important parameters, how it had been converging (or not). Just reporting the final error isn't very helpful...

Hello Andrew,i am still digesting and implemeting your guidance with the manual, i got a perfect harmonic balance as shown bellow.

in my personal folder i only have files like

ASSURA_TECH.LIB

CDS.LIB

cdsLibEditor.log

and my schematic files that i created using library manager.

where can i find SPECTRE.OUT file?

Thanks

When you run a spectre simulation, you normally have a log file appear (you've copied and pasted info from it in your first post above). In the banner of that window, it gives the path to the file.

If running in ADE L, and when you've not changed the project directory (on Setup->Simulator/Dir/Host), it will be in ~/simulation/cellName/spectre/schematic/psf/spectre.out - the three in italics are the test bench cell name, the simulator name, and the view being simulated (so might be a config, might be something else, but commonly is schematic).

Anyway, glad you've got it working.

Regards,

Andrew.