Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
Exchange ideas, news, technical information, and best practices.
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.
It's not all about the technlogy. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
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,
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.
In reply to Andrew Beckett:
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.
In reply to pswirhun:
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).