Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
Verification 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.
The Cadence Academic Network helps build strong relationships between academia and industry, and promotes the proliferation of leading-edge technologies and methodologies at universities renowned for their engineering and design excellence.
Participate in CDNLive
A huge knowledge exchange platform for academia to network with industry. We are looking for academic speakers to talk about their research to the industry attendees at the Academic Track at CDNLive EMEA and Silicon Valley.
Come & Meet Us @ Events
A huge knowledge exchange platform for academia. We are looking for academic speakers to talk about their research to industry attendees.
Americas University Software Program
Join the 250+ qualified Americas member universities who have already incorporated Cadence EDA software into their classrooms and academic research projects.
EMEA University Software Program
In EMEA, Cadence works with EUROPRACTICE to ensure cost-effective availability of our extensive electronic design automation (EDA) tools for non-commercial activities.
Apply Now For Jobs
If you are a recent college graduate or a student looking for internship. Visit our exclusive job search page for interns and recent college graduate jobs.
Cadence is a Great Place to do great work
Learn more about our internship program and visit our careers page to do meaningful work and make a great impact.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
Overview All Courses Asia Pacific EMEANorth America
Instructor-led training [ILT] are live classes that are offered in our state-of-the-art classrooms at our worldwide training centers, at your site, or as a Virtual classroom.
Online Training is delivered over the web to let you proceed at your own pace, anytime and anywhere.
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.
Get email delivery of the Cadence blog featured here
When you need to include noisy oscillators in SpectreRF transceiver simulations, you have at least 3 options:
1) Semi-autonomous simulation is the most accurate approach, recommended whenever the transistor-level model of the oscillator is available.
2) rfLib/osc model is less accurate but it’s well-suited for "what-if" design exploration. Since rfLib/osc uses Leeson’s noise formula, it doesn’t allow for arbitrary specification of phase noise profiles as a function of frequency.
3) Use PORTs and other sources with noisefiles. This approach lets users specify arbitrary noise profiles, but it omits sideband correlation data. In practice, this means that AM and PM components of the noise are modeled incorrectly. For oscillators in particular, the AM component is grossly exaggerated and the PM component of the noise is underestimated. As a result, this approach isn’t recommend for oscillator noise modeling.
One strategy is:
Use a frequency-dependent noise source which directly phase-modulates an otherwise ideal oscillator.
The noise source is modeled using a voltage source + noisefile.
This gives us two main benefits:
1. By virtue of direct phase modulation the oscillator’s noise is now all PM, which a good model of near-carrier oscillator noise.
2. By virtue of using noisefiles, we can now specify arbitrary noise profiles as a function of frequency.
A Simple Mathematical Model of the Oscillator
Below is a simple mathematical model of the oscillator.
Using the small noise assumption, and remembering that sin(x+y)=cos(x)sin(y)+sin(x)cos(y),
An equivalent system model of the above equation (1) is shown below:
Below is the Verilog-A Implementation
`include "disciplines.vams"// power: available power (dBm) default: 10 dBm// freq: output frequency (Hz) default: 1 GHz// rout: output impedance (Ohm) default: 50 Ohm`define db10_real(x) pow(10, (x)/10)`define dbm2pow(x) `db10_real( ((x)-30) )`define pow2v(x,r) sqrt(8*(r)*(x))module oscwphnoise(out, ph);inout out;input ph;electrical out;electrical ph;electrical gnd;ground gnd;electrical int;parameter real power = 10 ;parameter real rout = 50 ;parameter real freq = 1e+09 ;isource #(.type("sine"), .ampl(`pow2v(`dbm2pow(power),rout)/rout), .freq(freq) ) is1(gnd,out);vsource #(.type("sine"), .ampl(`pow2v(`dbm2pow(power),rout)/rout), .sinephase(-90), .freq(freq) ) vs1(gnd,int);analog beginI(out) <+ -V(int)*V(ph);I(out) <+ V(out)/rout;endendmodule
// power: available power (dBm) default: 10 dBm
// freq: output frequency (Hz) default: 1 GHz
// rout: output impedance (Ohm) default: 50 Ohm
`define db10_real(x) pow(10, (x)/10)
`define dbm2pow(x) `db10_real( ((x)-30) )
`define pow2v(x,r) sqrt(8*(r)*(x))
module oscwphnoise(out, ph);
parameter real power = 10 ;
parameter real rout = 50 ;
parameter real freq = 1e+09 ;
isource #(.type("sine"), .ampl(`pow2v(`dbm2pow(power),rout)/rout), .freq(freq) ) is1(gnd,out);
vsource #(.type("sine"), .ampl(`pow2v(`dbm2pow(power),rout)/rout), .sinephase(-90), .freq(freq) ) vs1(gnd,int);
I(out) <+ -V(int)*V(ph);
I(out) <+ V(out)/rout;
What Do We Apply to the Terminal φ to Model Noise?
Use the well-known relationship between the single sideband noise to carrier ratio and the spectral density of φ(t), which is valid for small offsets f:
L(f) = 0.5*Sφ(f)
So the phase φ(t) is a signal whose noise spectrum is given by:
To model this in Spectre, use a DC voltage source and specify the noise spectrum in a noisefile. You calculate the noisefile using Excel.
Calculating the Noisefile Contents in Excel
A Complete Model
The complete model is shown below:
Below are results showing hb and hbnoise (phase noise) results:
To explore this further, login into Cadence Online Support and see https://support.cadence.com/ Solution 11775686.
Have fun simulating!
Hi, thanks for positing this. I tried to follow using the verilog-A and noise file with the same PM spectral density values at the same offsets (1 to 1e8 Hz) but when I run pss and pnoise, the pnoise spectrum shows up as a flat line at -170.8dBc/Hz across the entire offset range instead of the roll off you got. It seems the -170.8dBc PN level corresponds to the highest offset/noise pair listed in the noise file or typed into the vdc form. Would you happen to know where I went wrong? Thanks!
I need Cadence to help me be designing rf power amplifier circuit for my our use.