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 need to do some *fast* simulations of a mixer and after long searching I found out that the most stable is to do an ENV of the transient where some bias voltages settle (under LO pump, though), then use PAC right after.
I was quite pleased to find out today of this possiblity, I knew only PSS would allow this kind of simulation (but then its tstab transient would be quite long).
However, to set up this PAC after ENV, one has to open the 'options' window of the ENV, navigate to the 'Misc' tab, and here set two fields:
pactimes --> the time(s) at which you want a pac to be performed
pacnames --> the name of the pac(s) simulation(s)
now, I use ADEXL from the GUI, I am therefore not aware of any way of modifying the name of a simulation. For me, a PAC simulation has always 'pac' as name. From the fact that you can define multiple times, I gather that you could in principle run multiple PACs as well...but how to implement that is for me a complete mistery.
Anyways, I set the string 'pac' under 'pacnames' and that works.
Only for single point simulations, though.
I have to do MonteCarlo. For this, I get an error from the ENV itself, saying :
'The analysis `pac' cannot be referenced by multiple analyses'
So...from one ENV to the next, but not even for the first indeed, the 'nameforming' gets wrong.
I have no idea whatsoever how to tackle this. Probably some 'pre-running script' defining a name and then passing it?
Please, please help me with this, I am in desperate need for a solution fast!
This appears to be a bug in envlp when used within Monte Carlo. I tried also giving it the name mc1_pac but that didn't work either.
I think you'll need to report this via customer support (I managed to reproduce it myself). By all means put me on copy (I think you have my email address) when you file this and I'll pick it up.
I did also try an alternative strategy - which was to use a pss with tstabenvlp=yes and envlpname=envlp (these are not on the form, so have to be done as additional parameters) together with a long tstab (the idea is that it uses the envlp analysis for the tstab phase). This works fine in normal cases, but not within a monte carlo either. So that's a bug too (although tstabenvlp is not really being actively promoted/worked on).
In reply to Andrew Beckett:
I am in contact with the support and preparing a reply for you because actually the reason why I resorted to PAC after ENV was that I could not get a proper PAC after PSS after ENV. In fact, the post you link from here was an attempt to start a PSS from a definite state, be it a TRAN or another simulation like ENV.
This, for my circuit, is not working properly (details in the email to the support), so that's why I was pretty happy to be able to simulate PAC taking an ENV cycle as the operating point.
I am now on 18.104.22.1680.15, but also on the previous version I had a couple of days ago, you had those 'use envelope for tstab' options in the Misc tab.
Thank you for your support!!
In reply to MicheleA:
Er, yes, the "Use Envelope for tstab" is on the Misc tab. I was obviously being a bit blind... or having a senior moment...