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 want to make an ac model which has got sample and hold (zero-order). I found the block, zvcvs, for that. Can somebody suggest the suitable parameters' values to implement that.
I tried Polynomial argument = z or inversez
S to Z Transformation = default (I assume it means none)
Specification type = polynomial
And then I tried various polynomails (order 1 or 2) to get sample-and-hold fft output for a simple wideband spectrum signal-input but seems I am doing something somewhere wrong. I am not very good at digital and z and bilinear transforms, so I think the capability is there but somehow I am not able to implement it using zvcvs. Can somebody please help me with it - implementing sample and zero-order hold using zvcvs.
That's interesting - I am trying to use a zvcvs in a PLL model and it doesn't do what I assumed it would do!
I hope someone will be along soon ...
In reply to keble6:
In reply to agaurav:
If you are not getting an answer on the forum, I recommend contacting Cadence Customer Support at http://support.cadence.com and filing a Service Request.
Sr. Staff Support AE, Global Customer Support
Cadence Design Systems, Inc.
In reply to Tawna:
You can do an implementation of 1/(1-z^-1) by using:
//vsin (samp 0) vsource type=sine ampl=1 freq=20kr1 (samp 0) resistor r=1ksh (hold 0 samp 0) zvcvs ts=1u numer= denom=[1 -1] r2 (hold 0) resistor r=1ktran tran stop=3/20k
For example. Note that you can't simulate this in an "ac" analysis - this doesn't make any sense. And you can't simulate this with pss/pac (which might make some sense because it has a periodic operating point) because the z-domain controlled sources are not supported in the Shooting Newton method because they have "hidden states". It's not clear to me if that's what you wanted anyway...
In reply to Andrew Beckett:
Both ac and noise analyses perform a small-signal analysis around a DC operating point. For any circuit with periodic behaviour, simulating around a DC operating point is not terribly useful - it's not wrong, but almost certainly not what you're looking for. For example, if you have a switch capacitor filter, simulating the noise around a particular bias point, with some of the switches open and some closed will not tell you anything very useful - because you really need the time-averaged response, not the response about a single DC operating point. That's what pss/pac or pss/pnoise give you - the pss captures a periodic steady state (i.e. a periodic operating point) and then the small signal analysis gives you a time-averaged small-signal response over that period.
The same is true if you use a zvcvs - a single bias point is meaningless. It shouldn't error out - in the same way as it shouldn't error out if you try to analyse a circuit which relies on periodic behaviour in ac/noise. It does however error out if you try to analyse it using pss because the component has some internal "state" storage which is not visible to the PSS solver. The way you'd have to solve that is by using a suitable Verilog-A model as outlined in this paper on Hidden States.
I'm not sure what your question is from the above? I've explained why what you're trying to do doesn't make sense with a zvcvs.
If you had a laplace representation you could use svcvs, in which case all would be OK (because these do not require periodic behaviour). Maybe that's what you want? But if you really want a sample-and-hold, you'll have to use a Verilog-A based approach and use PSS and corresponding small-signal analyses. Or use the real circuit (and PSS)