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.
Get email delivery of the Cadence blog featured here
I'm first going to address how
you can perform a large-signal phase noise analysis on a design block such as a
VCO using our transient noise analysis capability in our Spectre circuit simulator.
This approach is in addition to our small signal phase noise
analysis which is available using either pnoise or hbnoise analysis in the
SpectreRF option to Spectre.
Here are the steps to obtain a phase noise plot from transient noise analysis:
1. Set up your oscillator testbench circuit for a transient noise analysis (See sourcelink for the Transient Noise appNote - it doesn't discuss the phase noise measurement, but describes how to properly set up the simulation analysis
2. Add the block freq_meter from the pllMMLib library ($CDSHOME/tools//dfII/samples/artist/pllMMLib) to the testbench circuit. Important: The instance name for this block must be 'vco_freq'.
If the oscillator output is differential, connect it to the vin_p and vin_n pins on the freq_meter block. If the oscillator output is single ended, connect it to the vin_p pin and connect the vin_n pin to ground. Connect a noConn cell from the basic library to the out_freq pin.
The parameters for this block are (set Tools Filter to veriloga in the CDF parameter form:
Vthup: Threshold voltage to determine the rise edge of the input waveform. The input waveform period is determined by two adjacent rise edges. Default is 0.
ttol: The tolerance of the time where the rise edge is determined. Default is 1p.
outStart: The time-dependent period of the input waveform is output to the file when the time is greater than outStart. Default is 0. To get accurate phase noise measurements, set this to past the time when the oscillator is fully powered up and oscillating at the design frequency.
outfile: The name of a file to contain time-dependent periods for use in later psd calculations. Specify just the file name, not a path. If outfile is left blank, the default name is periods.txt.
3. Before starting the simulation, in the ADE window, Select Tools->RF->PLL. In the PLL Macro Model Wizard window, enable PLL Macro Model and select PLL Bench as the Bench Type. Then OK this form.
4. Run the simulation. The simulation must run successfully to completion in order to get to the phase noise results.
5. In the Direct Plot form for transient noise there should be a PLL PSD Noise option. This will allow you to plot the phase noise results. If a message appears saying that the PLL Noise PSD data is not available, check steps 3) and 4). If you make any corrections, you will need to re-run the simulation.
The phase noise plot will extend from fmin = 4/tstop to fmax = fosc/2, where tstop is the transient noise simulation stop time and fosc is the oscillation frequency of the circuit.
Important note: You will need to use MMSIM701 and IC5141USR5 or IC613 (or latersubversions) to obtain a phase noise plot from transient noise analysis.
do i have to run this simulation on MMSIM701?
i found this function on MMSIM188.8.131.520 as well
and run this flow as you post, however ending up failure.
why?? can i use this function on MMSIM184.108.40.2060 ??