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.
I am trying to simulate the phase noise of a 25GHz LC oscillator using pss (flexible balance) and pnoise analysis. In the Direct Plot Form, there are two different Phase Noise options:
1) Analysis: pnoise Function:Phase Noise
2) Analysis: pnoise jitter Function: Phase Noise
The two above give different results (#1 is approximately ~2.3dBc lower than #2 @ 10MHz offset). What is the difference between these two functions?
I would like to note that #1 provides much more numerically stable results than #2.
You may want to take a look at the following solutions on Cadence On-Line Support:
1. Phase noise is not consistent for pnoise
sources and Jitter in ADE
2. FAQ: What is the equation that relates jitter to
3. Explain the differences between the 4 noisetype
settings for pnoise
In fact, there are a great deal of Solutions on phase noise, jitter, pnoise. The following solution summarizes many of them and where to find them:
4. Summary of existing documentation on various
RF related noise analyses
Sr. Staff Support AE, Global Customer Support
Cadence Design Systems, Inc.
In reply to Tawna:
Thanks for pointing out the solutions. I have a further question: What is the numerical noise floor for phase noise if we use harmonic balance? SpectreRF Theory states that the noise floor is -120 dB but I was not sure whether this applies to both shooting method and the harmonic balance.
In reply to Soner:
The numerical noise floor is not a fixed number for either engine. It will typically be lower with harmonic balance than shooting, but even saying that shooting has a numerical noise floor of some fixed number (e.g. -120dB) is a bit cavalier! However, I can pretty safely say that it will be something above about -300dB since that's the (approximate) limit of double precision floating point numbers ;-)
The numerical noise floor will depend upon the reltol and abstol (primarily) used, but there's a complex (and circuit dependent) relationship.
In reply to Andrew Beckett:
I am using reltol 1e-7, vabstol 1e-9 and iabstol 1e-12 and conservative in harmonic balance. I have an LC VCO with amplitude control (where I can change a bias voltage and increase the amplitude of oscillation). At two different bias voltages, (everything else the same) I observe phase noise of -117.7 and -125.7 dBc/Hz at 10MHz respectively. When I sweep tstab, I observe < 5mdBc/Hz numerical noise on -117 but I observe ~ 200mdBc/Hz numerical noise on -125.7 dBc/Hz. Based on your reply, 0.2 dBc noise is too much, isn't it? What other simulation parameters would you recommend me to adjust?
Thanks for your fast response and regards,
It is difficult to give exact advice without seeing your circuit and at the very least your options and analysis statements in your netlist.
I recommend that you contact Cadence Customer Support (support.cadence.com) and work with an AE on this.
A reltol of 1e-7 and vabstol of 1e-9 is very very tight (way moreso than typically necessary).
Other things will affect accuracy, such as the number of harmonics and sidebands specified.
Are you using augmented pnoise?
How have you set oversample? You may want to increase oversample from 1 to 2 when more accuracy is required (for example, you are running harmonic balance as the solver and seeing phase noise vary - particularly when varying tstab).
You also have not specified if you have any warning messages - they can be very helpful in diagnosing problems.