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.
Hello,I used "tran" analysis for a simulation, with simulation setup all correct (ie. same setup as my prev. known good ones). Indeed, simulation finished, and the tran.tran file was about 290 Giga. However, when I used plot to see nodes' voltage/current, it said the wavefore data was not available, and then it crashed the whole "icfb" tool kits. I am wondering if this is a bug, or a limitation that I was not aware before. This happened several times so I am wondering if there is a solution for it. Thank you !san
A simulator can sequentially write out the data to a massive file as it goes along.However, to plot the waveforms, it has to load the data for that waveform into memory. Given that the waveform tool is a 32 bit executable, the absolute maximum memory it can use is 4G (2^32 bytes). Given that there's some overhead over what is stored on disk, it's not hard for you to run out of memory... 290G is pretty massive. You might want to try to cut down the amount of data. Save less waveforms, and you might want to cut down the number of points in the results database (e.g. skipcount, starttime, strobeperiod - lots of options).Andrew.
After you pare down your data set from 290GB to something in the single digits you can get more mileage with these two points:a. Save to sst2 or psfbinf instead of psfbin. Psfbinf saves as floats instead of doubles, increasing (2x) your memory capacity. You will need a recent version of Spectre for this. To enable this, quit ADE, then set either of these options: .cdsenv: spectre.envOpts simOutputFormat string "psfbinf" .cdsinit: envSetVal("spectre.envOpts" "simOutputFormat" 'string "psfbinf")b. Only load a subset of the results into wavescan. From the Wavescan "Results Browser", use Settings->Select Data and select a range of results to load.-Samir Jafferali
My system is a true 64-bit linux version, though limited memory capacity. Seems even I did not save any waveform for any nodes or nets, it still generated a tran.tran.tra file about 40 G. This simulation is not very critical so I actually ignored this paracity-included simulation, instead, just use a purely schematic simulation. I also play a bit what Samir suggested. However, do not know why "Select Data" is not active in the Setting menu. I am using version 5.10.41. Thank you very much for very helpful suggestions.
In ADE, you probably have it set to save all voltages. Look at Outputs->Save All and change the voltages to "selected". Then save the nets you're interested in.Perhaps you're not using wavescan as the viewer, but using the older AWD viewer?Either way, you probably still need to resolve the huge file. No point producing enormous data files if you can't view them. Just because you have a 64-bit system, does not mean you'll be able to view the data if using a 32-bit application...Regards,Andrew.