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 have 100 copies of one cell in my high-level simulation and I wanted to define an initial condition for a node inside these cells.
I was wondering if there is a way that I can define an initial condition for the subcircuit (maybe in its schematic or symbol definition) and after instantiation that initial condition automatically applies to all?
I am using IC6.1.5.
If you need to have the same IC in all of your copies, just setup it in master cell of your inctances.
If you need different IC for each of your copiesyou could setup it manualy during your project simulation setup.
In reply to VKhlyupin:
I'm not sure what the previous response was trying to say, but in the spectre netlist you can do:
subckt block (d e) I1 (d f) myinv I2 (e g) myinv ic f=3 g=0ends block
However, ADE doesn't provide any way to do this - unless you created your own component to netlist an ic statement from an instance in the design, maybe.
You can however do this:
at the top level (so assuming that you have all your instances called BLOCK something, and the node inside called f, it will do an initial condition on all matching instances. ADE doesn't really have a way to define this through a form, but all you have to do is put the line in a file called "myIC.scs" (say; make sure it has a .scs suffix) and then reference this via Setup->Model Libraries or the Definition Files line on Setup->Simulation Files.
In reply to Andrew Beckett:
Thanks a lot for your response. I wasn't aware of that wildcard (*).
It solved my problem.