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.
Is it possible to do a Spectre sens analysis for a subcircuit? For instance having ..
subckt inv ( a b ) M1 ( a b vdd vdd ) pmos l=0.1u w=0.1u M2 ( 0 b a 0 ) nmos l=0.1u w=0.1u ends
X1 (a b) inv
.. I'd like to get the sensitivity of the current I(X1:a) against the voltage of a. Using a line such as ..
sens ( X1:a ) to ( a ) for (dcOp )
.. gives the error message "`X1': Not a signal, device instance or a model."
Is there a way to achieve that?
I don't think this is possible. For a start, the to part has to be a component or instance parameter - it cannot be a voltage. Secondly, the output variable can't be a subcircuit current.
I did manage to do it this way though:
// global 0 vdd model nmos bsim4 type=n model pmos bsim4 type=p subckt inv ( a b ) prb (a aint) iprobe M1 ( aint b vdd vdd ) pmos l=0.1u w=0.1u M2 ( 0 b aint 0 ) nmos l=0.1u w=0.1u ends X1 (a b) inv v1 (a 0) vsource dc=0.5 vdd (vdd 0) vsource dc=1 dcOp dc opts options sensfile="sens.out" sens (X1.prb:1) to (v1:dc) for (dcOp)
But this may not be exactly what you want...
In reply to Andrew Beckett:
Thanks, Andrew. This comes pretty close to what I was trying to do. Actually, my workaround was exactly that (unless that I've put prb outside the subcircuit). So if there's no other way of doing it, I'll stick with that. Thanks.