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 noticed that in my SP simulations the following warning occurs when a DC operating point simulation doesn't precede it:
WARNING (CMI-2015): Unable to open nodeset file `spectre.dc'. No such file or directory.
Could someone please clarify what the function of the spectre.dc file in performing a SP simulation? Also, why is this a warning instead of an error?
Thanks for the help.
Most likely you have the readns parameter on one of the analyses (for example the sp analysis) set to "spectre.dc". This tells whichever analysis it is to try to read the nodeset file as a hint for the DC algorithm that precedes the analysis (pretty much every analysis requires a DC operating point to start from, including an S-parameter analysis). If the file is missing, it will solve the DC operating point as usual - the file is just a hint.
The reason why it's not an error is that quite often you do things like this:
dc dc readns="spectre.dc" write="spectre.dc"
Which means the first time it will give you a warning, then write the DC operating point at the end of the simulation. The second run, the file will exist, and it will use that as a starting point. We try to make it not too critical if the file doesn't exist - since it is a hint.
If you really want it to error out, you can do that by adding this option into your netlist:
increaseSeverity options warning_change_severity=error warning_id=[CMI-2015]
And then it will fail:
Error found by spectre during DC solution estimation, during DC analysis `dc'. ERROR (CMI-2015): Unable to open nodeset file `spectre.dc'. No such file or directory.
In reply to Andrew Beckett: