Stats

  • Locked Locked
  • Replies 3
  • Subscribers 63
  • Views 16274
  • 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 discrepancies in LNA design

pswirhun

This question is regarding noise figure in a simple common-emitter LNA in the W-Band. There are two main simulations that I am using:

A) sp analysis with noise set to "yes" and the input/output ports specified.

B) noise analysis with the input port specified, and the output specified as a voltage between two nets: the net connected to the output port and ground. 

The problem is that these simulations seem to interfere with one another. If I enable (A), (B), or (A and B), I get different noise figures. Including only A gives NF ~= 20dB. Including only B gives NF ~= 220dB (clearly not right). Including A and B gives two different noise results: the sp-simulation gives roughly 3dB higher noise figure than the noise-simulation. However, the difference is not exactly 3dB. One is around 5.5dB in-band, and the other about 8.8dB in-band.

I am wondering whether one of these methods is taking into account the input matching / reflected signals, whether they are just different definitions of the same thing, or if I just do not understand the differences between these two simulations. In any case, it seems odd how the results change dramatically for one simulation depending on whether the other is enabled. 

I have printed noise summaries using both methods, and they include the same noise generators of the devices, resistances, and ports; however their absolute noise values differ across the two simulation methods--even for the same physical noise generator. 

I am using Cadence 6.15 and MMSIM 10.1. (Somewhat related: Are Spectre and SpectreRF distinct products?)

Thank you for your help,

Paul 

  • Paul,

    I suggest you contact customer support - I can't see why you should get different answers depending on whether two or one analysis is included.

    One thing that will make a difference is the fact that the noise analysis you should specify that the  output noise is a "probe" not a "voltage" - and then specify the output port as the component that is being probed. If you don't do this, then the noise of the load port will be included as part of the circuit noise; if you specify the output as being "voltage" then it has no idea which device represents the noise (noise figure should not include the noise of the load, since that's part of the "test equipment").

    SpectreRF is not a separate simulator - it is a licensed option of the Spectre circuit simulator. It's a distinct product, but there are many ways that it is licensed - you could have Multimode Simulation - which uses a token-based approach to licensing the capabilities. Here you're only using spectre capabilities, not spectreRF.

    Regards,

    Andrew.

  • Andrew,

    Thanks for the help. After changing the output of the noise analysis from a voltage to a probe of the output port, the noise figure results using the two simulations agree.

    Paul 

  • Paul,

    That's good - if you can contact customer support about the B-only simulation where you were getting the 220dB noise figure, that would be good (unless you've found the reason for it and it's a setup issue).

    Regards,

    Andrew.

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.