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.
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 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.
Q 1. Parameters AC magnitude and AC phase are only effective in an AC analysis. AC phase does not change the phase of vsin in a transient analysis - at least it does not in IC6.1. There is a parameter "Initial phase for sinusoid" than can be set to a non-zero value to set the phase of the source in a transient analysis. "DC voltage" sets the DC value of vsin in a DC operating point analysis or AV analysis. The vsin parameter "Offset voltage" sets the DC average of the vsin source in a transient analysis.
Q 2. The DC voltage parameter can be used to set the DC value of the vsin source in a DC operating point analysis. This value can be different than parameter "Offset voltage" which is the average value in a transient analysis.
This is what I observed from running a few test cases in IC6.1 and I hope this is useful.
In reply to smlogan:
Just to clarify what Shawn said. If you specify the DC voltage but not the "Offset voltage", when the DC voltage will be used as the mid-voltage of the sinusoid. If Offset voltage is specified, that is used instead (for the transient).
For a DC analysis (or for any small signal analysis that requires a DC operating point), the DC value of the source is taken as the DC voltage (if specified), or if not specified, it's the time-zero value of the source. These could of course be different...
Shawn is absolutely right in saying that the AC phase does not affect transient. It's the initial phase for sinusoid that affects that.
I would generally recommend using vsource rather than vsin (they're the same thing in spectre) because the parameters are better organized.
In reply to Andrew Beckett:
Thank you for your clarification concerning the use of parameter DC voltage in vsin during a transient analysis when "Offset voltage" is left blank. You are absolutely correct. I have noticed this and should have included it! Good poiint (again!).
One more question - maybe it's too trivial:
Does the properties of instances (e.g., "vsin" etc.) from "analogLib" used in the schematic change with the simulator (e.g., "spectre") being used?
In reply to jdp721:
Yes, they do. Not all properties on an analogLib component (e.g. vsin, vsource, isource, port, etc.) are supported by all simulators.
In fact, I recommend using vsource with sourcetype=sine instead of vsin if you are simulating with Spectre. vsin is a subset of vsource. New features are put into vsource. vsource has a much more intuitive GUI.
Similarly, if using spectre, I recommend port (instead of psin). All of the port properties are documented in the SpectreRF User Guide (version 13.1 and 13.1.1). Many of the port properties are the same as the vsource properties.
Customer Support Director - Analog/Mixed-Signal/RF AEs
Cadence Design Systems, Inc.
In reply to Tawna:
One more thing...
Use the Tool Filter (In IC616, go to Options-Tool Filter) to limit what parameters are displayed in the schematic and in the Edit Properties/Add Instance form.
For example, if you choose hspice (and deselect all others) and OK the form, you will see a different parameter set than if you check spectre (and deselect all others).