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 am trying to generate a plot of one of the capacitance values generated by captab. My approach is as follows:
1. Use stimulusFile to include the instruction: Cap_dcInfo info what=captab detail=nodetonode sort=name threshold=0 where=logfile
2. Set up captab analysis: Analysis( 'dc ?captab t ?detail "nodetonode")
3. Run parameteric analysis across voltage to generate multiple cap. tables:
paramAnalysis( "vdd" ?start vstart ?stop vstop ?step vstep)
This seems to work when I only run step 2 and 3 meaning I see the multiple cap. tables in the spectre.out file. However, I am having trouble figuring out how to plot a specific capacitance value from the generated tables with the independent variable being "vdd". Although an example exists in a previous post /forums/p/21764/1309486.aspx, it does not include the stimulus used and it did not attempt to plot multiple values but rather only print a single value.
Any help will be greatly appreciated.
A better discussion would be to look at /forums/t/20426.aspx?PageIndex=2(although that's more to do with seeing it over time)
You don't really need to use stimulusFile to turn on captab. Just do steps 2 and 3, and then if you do:
you'll see all the available outputs. You can also access it from the results browser and then send to the calculator to find the right expression. For example:
pv("out : net9" "Total" ?result 'captab) ; don't need the ?result bit if you've used selectResult first
The second arg for pv could be "Variable", "Fixed", or "Total". Because it was a parametric sweep, you'll see the capacitance value versus your swept variable.
In reply to Andrew Beckett: