Cadence® system design and verification solutions, integrated under our Verification 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.
More Support Log In
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 technology. 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 have two questions about pnoise jitter calculation in SpectreRF.
1. What is the meaning of Freq. Multiplier in jitter calculator?
2. What is the optimum integration range of phase noise for jitter calculation?
Actually, I posted about similar subject last year, but I'm still confused..... : (
I need to calculate VCO's jitter to estimate the SNR limit of synchronous ADC by clock.
I've done PSS/PNOISE simulation like following condtion
- Free running VCO
- VCO clock speed : 10MS/s
- Total ADC conversion time : 100us(1000cycle)
Beat frequency : 10MHz
Output harmonics(Number of harmonics) : 0
Output Frequency Sweep Range : 1~500MHz(I have no idea what's the right sweep range. I just think it would be wide enough)
Maximum Sideband : 40(40 is enough to get accurate results in my case)
Noise type : Jitter(Typically, ADC needs only RMS jitter, not phase noise)
After PSS/PNOISE simulation, I caculated k-cycle jitter because the VCO is autonomous system and I need accumulated RMS jitter.
Following is what I did.
Results->Direct Plot->Main Form->select pnoise jitter(Analysis)->Jc(Function)->Number of cycles=1000->select RMS->
->Freq. Multiplier=1->Integration Limits:1kHz~20MHz
Here are two questions as I asked above.
I think the integration range of 1k~20MHz is enough, because total ADC's conversion time is 100us and 20MHz=10MHz(Fundamental X2)
Is it proper approach?
I believe the Freq Multiplier (which is really not clearly documented - it just says in various places that it defaults to 1, but gives no explanation, even in the documentation for the underlying functions drplRFJcc etc, as to what it actually means) is to allow you to say that you want the frequency used for the jitter calculation to be multiplied up from the frequency found in the PSS analysis. An example where that might be useful is when you have a divider and the PSS has found the divided frequency - but yet you are measuring the jitter elsewhere in the circuit (maybe on the divider input), and so you need to multiply the frequency of the PSS by the divide ratio of the divider to use the correct frequency in the calculations. However, I think you should log a service request to confirm this and request that it is properly documented.
If your PSS fundamental is 10MHz, and you are using the PMjitter mode, you should not sweep the pnoise beyond half the PSS fundamental (5MHz). This is because the PMjitter mode adds an ideal sampler to the output of the circuit and this is sampling at the PSS fundamental rate - sweeping beyond this will alias the noise and cause overcounting of the noise. Since the sampler is there, it will automatically fold any noise into the output band anyway, so it should be sufficient to have an upper limit of 5MHz. The lower limit of 1kHz is OK, but in practice if K is 1000 you are only including frequencies as low as 10MHz/1000 - i.e. 10kHz. The integration automatically takes this into account - so it's fine to leave it as 1kHz.
You might want to read the Jitter app note at <MMSIMinstDir>/tools/spectre/examples/SpectreRF_workshop/JitterAN.pdf
In reply to Andrew Beckett:
Your comment is really helpful to understand PSS sim.
Thank you for your reply, Andrew
I read the app note you suggested(for version MMSIM6.0, March 2006), and I'm little confused about k-cycle jitter.
From the note, section "Synchronous Jitter Versus Accumulating Jitter", autonomous circuits, e.g. VCO have only cycle-to-cycle jitter as the jitter performance as mentioned below
"For autonomous circuits where there are no ideal reference transitions, you are limited to using self-referred jitter metrics. This jitter is accumulating jitter. The next cycle transition is the result of the previous cycle output, so the jitter variance accumulates from cycle-to-cycle"
But, in the Figure 1-9 of the note, Cycle jitter is used as the jitter performance of VCO.
Could I use the K-cycle jitter as accumulating jitter of autonomous circuits?
Which is right?
Hi Andrew, I also have been stuck with the problem of selecting the proper fmin in long term ( accumulated ) jitter calculation in PSS/PNOISE sims. I would like to get some more clarification on the last statement "The lower limit of 1kHz is OK, but in practice if K is 1000 you are only including frequencies as low as 10MHz/1000 - i.e. 10kHz. The integration automatically takes this into account - so it's fine to leave it as 1kHz." Does spectre Jc(K) form always takes Fmin as "Fbeat / K" for integration, irrespective of what fmin value we give ..? Could you kindly point me to the theoretical basis for this "Fbeat / K"...? ( I am asking this because I have not found any literature which clearly specifies the Fmin of integration for K cycle accumulated long term jitter) Following is my specific scenario.: I have an experimental/simple RC relaxation oscillator operating at 10MHz. Ran PSS/PNOSE with Fbeat=10MHz. Want to find out the accumulated jitter for 100000 cycles. In the Jc(K) form, max integration range is set to =Fbeat/2 = 5MHz. I tried different fmin ( like 10Hz ,50Hz , 100Hz ). Follwing are the respective jitter values reported by spectre ==> 431nS , 132nS , 56nS. ==> The values are vastly different. Kindly let me know your thoughts/advice on this as this is inconsistent with the comment you have given. I am concerned about what value I should give as Fmin... ? Wondering if I am getting this issue due to some setting or version issue ? ( I use Virtuoso 6.1.6-64b ) ( Based on your comment, the Fmin in my case should have to be 10MHz/100000 = 100 and Jc(K=100000) values should have to be same if I input Fmin=100Hz or 50Hz or 10Hz ) Highly appreciate your help... Thanks and regards Soman