Cadence® system design and verification solutions, integrated under our Verification Suite, provide the simulation, acceleration, emulation, and management capabilities.
Verification 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.
More Support Log In
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 technology. 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.
yes...there is this support answer #11003524 which should address the topic.
I also learnt from Andrew some time ago about saving oppoints and/or specific info through a file and attaching it to the model libraries.
What I am experiencing now is that the method:
a) gives me the info out of a *tran*
b) gives me the info out of a *envlp_td*
c) for a *pss*, I get
1. a _constant_ value in the *pss_td* folder, if I use the shooting method (seems like a DCOP value)
2. nothing if I use the HB method
Just wondering whether that is the behavior to be expected, or shouldn't I get a (nice) plot of my wanted gm over a period, exactly like I get it for any other V/I in the circuit after a pss?
I seem to remember having done the same thing some 6 months ago and it worked fine..
Thanks for any help.
So...I must be growing older since I do not remember replying to myself in the past ;-)
Anyhow, I found out yesterday what the issue is. I was simulating using the 'High Performance Simulator -- APS'.
For some reason - I am in contact with the Support for this - it looks like the stored gm is just a DC value.
I had a glimpse yesterday and tried the same simulation with good ole Spectre and bam! My gm Vs. time was there!
Maybe this helps someone,
In reply to MicheleA:
That sounds like a bug to me. This ought to work, so support should ensure that a CCR is filed to get this fixed.
That said, I tried to reproduce it with MMSIM12.1 ISR14, and for me I get the gm value saved during shooting in the pss_td database (as a waveform) even when using APS. This isn't true with harmonic balance, but then again that doesn't surprise me - with harmonic balance it would need to solve the gm as a harmonic series and then convert it back into the time domain - and it only computes the voltages and currents as a harmonic series.
Here's the netlist I used:
// test of saving gm during a pss analysismodel nch bsim4 type=nmodel pch bsim4 type=pMP1 (z a vdd vdd) pch w=2u l=0.5uMN1 (z a 0 0) nch w=1u l=0.5uVz (a 0) vsource type=pulse period=40n width=20n rise=1n fall=1n val0=0 val1=1.5Vvdd (vdd 0) vsource type=dc dc=1.5save *:gm sigtype=dev devtype=bsim4tran tran stop=200npss pss period=40n outputtype=all // harmonicbalance=yes
In reply to Andrew Beckett:
yes I just sent my netlist to the Support via our internal channel. Will keep you posted here anyways.
I do not know which MMSIM version I am under (what's the command to see this?), just the Cadence version.
I could source from 500.4 to 500.15 but all gave me this (with APS).
By the way, I was under the impression that HB would not work for time rep of gm. Then why do you say 'harmonicbalance=yes' in your netlist?
Type "spectre -W" or look at the top of your spectre output log - it will tell you the subversion you're using.
The harmonicbalance=yes in my netlist is commented out (it's preceded by // which is a comment).
Surprised you're using the base MMSIM12.1 version - been quite a few hotfixes since then. However, with my netlist, that version works too - I get a waveform in the pss_td database for the gm.
Perhaps you can check? Run "spectre invpss.scs" and open the results in ViVA. Maybe there's some subtle difference in your testcase.
Of course I meant "spectre +aps invpss.scs".
I like to encourage people to live on the edge now and again ;-)
In general I'd expect you to be running from ADE; obviously the benefit of a small command line example is that it's a bit easier to share in a forum like this (and I can throw it together in a few seconds).
I look forward to hearing your findings!
Thank you for fostering my growth Andrew ;-)
...And indeed, your netlist works like a charm! But what a crappy gm :-D
I then tried to use ADE instead of ADEXL for my circuit, however the result is the same: I get a curve with Spectre only. APS gives a sort of DC value out.
Same thing if I sim my circuit from the command line (now I'm a master :-))
I also noted that the whole sim setup is waaay faster when using cmd line. Ok, the circuit is two transitors but I got the impression that the processes *before* actual simulation took a fraction of the time.
Can you please point me to the help entries containing - possibly an overview - of topics like 'running Spectre from the command line' and directory structure...things like that. Maybe the time has come for me to understand all this a little better.
MicheleAI also noted that the whole sim setup is waaay faster when using cmd line. Ok, the circuit is two transitors but I got the impression that the processes *before* actual simulation took a fraction of the time.Can you please point me to the help entries containing - possibly an overview - of topics like 'running Spectre from the command line' and directory structure...things like that. Maybe the time has come for me to understand all this a little better.Hi Michele,
Oh no! What have I done? ;-)
The actual simulation will be the same time - it's doing the same thing - but you've eliminated the overhead of starting the ICRP job, netlisting, managing the job and so on. There's been quite a bit of work on optimizing that recently though, so should be less significant in recent IC616 ISRs, at least for the case of having large numbers of jobs.
As for running spectre from the command line, this is covered in the Spectre User and Reference manuals. Also "spectre -h" is your friend...
As for the actual issue, it must be something to do with some other setting in your example - I don't know what that might be (without seeing the example).
Do you think you could start something if I attached the netlist...well..stripped of the actual devices and just options and simulations?
I'd be more than happy to do that :)
Ideally if you can include the transistor instances, and just omit the model files - presumably you can reproduce this with a simple circuit (similar to my inverter) - and also the options and analysis statements included. Then I can replace them with some other models and see what happens.