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.
I uses a scripts to analyze phase noise of a VCO at different control voltage. I found some data points are significantly different from ADE produced. Then I saved script in ADE and load the script in ocean. The phase noise calculated with ocean script is -80. But at ADE, it is -100. Anyone can tell me how to solve this problem? Thanks! The save script is attached as below. The frequency calculated are consisten, but phase noise are different from ocean script.
ocnWaveformTool( 'wavescan )fp=outfile(sprintf(nil "%s/tmp.csv" resultPATH) "a")fprintf(fp "vc ts cf wc freq amp vcom phasenoise\n")simulator( 'spectre )design( "/users/dtgong/simulation/testLCVCO/spectre/schematic/netlist/netlist")resultsDir( "/users/dtgong/simulation/testLCVCO/spectre/schematic" )modelFile( '("/home/dtgong/peregrine/PSC_Release_3.8.1/Rel_3.8.1/gc/models/psa/spectre/modellib.scs" "Nominal"))analysis('tran ?stop "200n" ?errpreset "conservative" )analysis('pnoise ?sweeptype "relative" ?relharmnum "1" ?start "10K" ?stop "100M" ?maxsideband "7" ?p "/vp0" ?n "/vn0" ?oprobe "" ?iprobe "" ?refsideband "" ?ppv "" )analysis('pss ?fund "5.0G" ?harms "7" ?errpreset "conservative" ?tstab "500n" ?p "/vp0" ?n "/vn0" ?ppv "" )desVar( "wc" 30u )desVar( "wb" 10u )desVar( "cf" 220p )desVar( "r" 10 )desVar( "global_use_preLPE" 1 )desVar( "vc" 1.1 )desVar( "cl" 60f )envOption( 'autoDisplay nil )save( 'i "/I0/I0/R0/MINUS" "/I0/I0/L0/PLUS" "/I0/I0/L1/PLUS" )converge( 'ic "/vn0" "0.01" )temp( 27 ) run()selectResult( 'tran );plot(getData("/vp0") getData("/vn0") getData("/I0/vb") getData("/I0/I0/R0/MINUS") getData("/I0/I0/L0/PLUS") getData("/I0/I0/L1/PLUS") getData("/I0/I0/vtail") )freq = frequency(clip((VT("/vp0") - VT("/vn0")) 1e-08 4e-08));plot( freq ?expr '( "freq" ) )Phase\ Noise\;\ dBc\/Hz\,\ Relative\ Harmonic\ \=\ 1 = phaseNoise(1 "pss_fd" ?result "pnoise");plot( Phase\ Noise\;\ dBc\/Hz\,\ Relative\ Harmonic\ \=\ 1 ?expr '( "Phase Noise; dBc/Hz, Relative Harmonic = 1" ) )ph_1M = value(phaseNoise(1 "pss_fd" ?result "pnoise") 1000000.0);plot( ph_1M ?expr '( "ph_1M" ) );freq0 = (freq (VT("/vp0") - VT("/vn0")) "rising" ?xName "time" ?mode "auto" ?threshold 0.0 ?histoDisplay nil ?noOfHistoBins nil);plot( freq0 ?expr '( "freq0" ) )fprintf(fp "%.3fGHz %f\n" freq*1e-9 ph_1M)close(fp)
Thanks a lot,
Given that in both cases a netlist for spectre is assembled and simulated, I would take the "input.scs" in the netlist directory as simulated in ADE - copy it elsewhere - and then do the same for the OCEAN script - and do a "diff" between the two to see what differences there are. There is bound to be some difference (otherwise the results would be the same) - maybe that will pinpoint the reason and it will become clear if there's something missing (or different) in the OCEAN script.
In reply to Andrew Beckett:
I moved input.scs to a temporary directory. Then I ran simulation at ADE by press button "netlist and run", the phase noise at 1 MHz offset is -98.6. There is no input.scs in netlist direction created after the simulation. Then I ran the same job at OCEAN, the phase noise at 1MHz offset is -77 and input.scs is created, which is same as the one I moved to temporary directory. Any more comments on that?
I am still confused.
Thanks a lot,
In reply to datao:
Make sure you're not running OCEAN and ADE at the same time. Quite likely the ADE run was using spectre's interactive mode - so you had the previous netlist still in spectre's memory.
So to be sure, start ADE from scratch and run the simulation; copy the input.scs. Close ADE and then run your OCEAN script - and then compare the input.scs in both cases.
Check also the spectre.out from both runs - are you using the same versions?
I quite ADE and run OCEAN script, I still get the phase noise at -77. Then I remove input.scs and start ADE. This time the phase noise from ADE is -77! But if I re-run the job in ADE by press button "netlist and run", it is -98.6. The third time run is also -98.6. Now, I at least partially reproduce the results at ADE. But which number is correct?
How to check their version, OCEAN and ADE?
Thanks a lot,
When you hit the run button the second time, spectre will be re-running from what is in memory. It's possible that you have multiple operating points and your circuit is converging on a different solution after the first run.
In order to find out the spectre version - this will appear at the top of the spectre output log, and also "spectre -W" will tell you from the UNIX command line - but I'd check the log file.
You can also try setting "rebuildmatrix=yes" on the Simulator->Options->Analog form (if it's not on the form, type it in the additional parameters field). That said, if there is more than one operating point, maybe you need to investigate that. Perhaps you can check if the PSS simulation is finding the same oscillation frequency the first and second time you run it in ADE? It should tell you at the end of the PSS simulation what the final oscillation frequency is (and you can get this on the direct plot form too) - maybe it's converged on a different solution for the oscillation frequency?
I checked the logFile, the spectre version is 22.214.171.1246. In the spectre.out, I do not find the fundemental frequency change in pss analysis. When the option "rebuildmatrix=yes" is checked, I simulated 4 times with ADE, the phase noise is not change, always -77.
If I set "rebuildmatrix=no", then the first simulation get -77, the second simulation I get -98.6. Since frequency does not change, which number is more reasonable?