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.
Hi, It is true that we can get Jitter from Phase noise simulated from the Spectre by integrating over a noise band of interest. It evident that from the tool that we can get Jcc(cycle to Cycle Jitter) and Jee(Edge to Edge) and Jc.But I want to know wether we can get "long term jitter" from the SpectreRF's Phase noise simulation. kindly tell me wether we have any other ways to measure the long term jitter from the spectre.I beleive the eyediagram technique with transient analysis will not include random noise and other noises.Also in the Direct plot menu after Pnoise analysis. we have the term "K"( no of cycles). Can you pls tell me what is it.Can we set k=3000 or (like that number ) to het the longterm jitter?kindly reply.Thanks & regardsSavithRu
Long term jitter is normally determined for a specified number of cycles - so yes, entering the number of cycles is the way to do it.Of course, you need to make sure you simulate the noise low enough in frequency to include noise over the total number of cycles you want to capture the long term jitter. The calculations will ensure that the integration is done properly over the number of cycles you want.You can do transient with an eye-diagram, and turn on transient noise, but this is a much less effective way of measuring jitter (it's less efficient, and less accurate, unless your circuit is non-periodic in nature or has a large signal response to the noise) than pnoise.Regards,Andrew.
Dear Andrew,Thank you very much for your kind reply. Thanks for clarifying me.""you need to make sure you simulate the noise low enough in frequency to include noise over the total number of cycles you want to capture the long term jitter"' .... here noise, in low enough in frequency, meanse what? I have taken it as 10KHz (up to 100M) . Is that value is fine enough to my clock synthesizer driving CPU.While simulation, there is no option for giving the time for simulation or simulation of no. of cycles. I beleive the tool will do simulations only for few cycles, And later it only extrapolates for other k=higher values. If this is the case, I doubt that wether this Jitter for k= say 3000 is not realistc.Also can you please tell how I can measure the PFD+CP phase noise from Spectre. I want to compare the phase noise of CP+PFd+Divider+LPF with that of VCO.Kindly guide me.Thanks & RegardsSavithRu
I can't tell whether 10kHz is low enough in frequency from the information you've given. If you want 3000 cycles, you need to go down as low as Fcycle/3000 - so if your clock is above 30MHz, you'll be OK.Since the jitter is coming from the noise analysis that is done, there is no need to simulate more cycles in the time domain. A single cycle of the output clock will be enough to capture the non-linearities so that pnoise can include all the noise folding that occurs in the circuit. It can then compute the noise response over frequency, and the k-cycle jitter will be dependent on integrating over that number of cycles (but in the frequency domain). So provided you have simulated the pnoise low enough in frequency to capture the noise at that fraction of your clock frequency, you'll be OK. The integration itself is far from trivial, but the pnoise form takes care of that - you just need to ensure that the frequency range is wide enough, and that it you've asked for the number of cycles you want.The result should be realistic (in terms of the the random jitter). You won't of course be capturing any deterministic jitter this way.Regards,Andrew.