Stats

  • Locked Locked
  • Replies 12
  • Subscribers 63
  • Views 22537
  • 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

Problem of Nport PSS shooting simulation

Hubertastra

Hello,

I have some problem when doing the PSS/PAC/PSP simulation with Nport from the analoglib.

I'm using Spectre Version 19.1.0.373.isr7 64bit and Virtuoso IC6.1.8-64b.

I wrote a S4P touchstone file to model an ideal IQ coupler and simulated it with Nport component from analoglib.

I tried PSS/PSP/PAC simulations with both shooting and HB engine.

The result of HB engine is correct, funtioning exactly as an ideal IQ coupler. While the result of shooting engine is completely wrong.

I used the PSS shooting engine for NPORT simulation with Spectre 14 and Virtuoso IC6.1.6 before. It works very well.

I wonder whether there is a way to get NPORT works with PSS shooting engine in the new Spectre/Virtuoso version.

For the Nport setup, I  tried nearly all the options for passivity, causilty, interpolation methods.

One weird thing is that no matter which interpolation methods I chose (linear, rational), the final fitting is always based on BBspice.

Any comment is appreciated. Thank you.

 

Best regards,

Yang

  • in reply to ShawnLogan

    I only took a very quick look (I don't have the PDK to hand, so I can't really try out the circuit). However, just from running a simple instantiation of the nport (terminated with ports) with either linear or bbspice gives messages like this:

    Warning from spectre during initial setup.
    WARNING (CMI-2835): In file
    `/export/home/andrewb/tools/spectre/HBC_6_ports_0_180G.s7p', the
    maximum passivity violation is 31.963652% at 180 GHz. Data may be
    non-passive.

    (it's worse with bbspice). BBSPICE in SPECTRE19.1 really struggles to find a fit (probably because it's not a great fit), and it just gives up pretty quickly in SPECTRE20.1. Just opening the s-parameter file in ViVA and plotting all the s-parameters, you can see it's pretty discontinuous - so not a great s-parameter file, which is probably the root of your troubles with trying to do any time-domain based simulation:

  • in reply to Andrew Beckett

    Dear Andrew,

    Thank you for your response. I think you are right. After 70GHz, the EM simulation step I set was 5GHz. We can also observe that the discontinuity mainly occur around 120GHz, which I suspect is my inductor‘s’ self-resonate frequency. Due to the coarse frequency sweeping aroud this self-resonate frequency, large discontinuity occurs and cause time-domain simulation problem. I think this is the root of my problem.

    Thank you very much again.

    Best regards,

    Yang

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.