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.
I used a verilogA module in my schematic which measures the period of the output waveform of a block.
The verilogA code is as follows:-
`include "disciplines.vams"(*instrument_module*)module frequency_meter(in); parameter real thresh=0; // threshold (V) parameter integer dir = 1 from [-1:1] exclude 0; // 1 for rising edges, -1 for falling input in; voltage in; integer timing; real t0, t, period, freq; analog begin t = last_crossing(V(in) - thresh, dir); @(cross(V(in) - thresh, dir)) begin if (timing) begin period = t - t0; freq = 1/period; $strobe("period = %rs (measured at %rs).\n", t - t0, $abstime); end t0 = t; timing = 1; end endendmodule
I want to plot freq versus time using OCEAN script.
Can anybody please tell how it can be done.
I did :
save I5:period I5:freqplot(I5:freq).
This gives error in OCEAN script.
But in input.scs file I worte:-
save I5:period I5:freq
I ran the simulation and in the wavescan I was able to plot freq-vs-time.
In the spectre netlist, you can add:
myOpts options saveahdlvars=all
or in OCEAN you could say:
saveOption( ?saveahdlvars "all" )
And then to reference the freq signal, you'd do:
plot(getData("I5:freq" ?result 'tran))
Or you could make the frequency an output pin of the meter instead - but that involves changing it a bit so that you are contributing to a node - for your needs the above is probably sufficient?
In reply to Andrew Beckett:
Thanks a lot.
Now, I am beginner to verilogA coding.
I have some doubt regarding the above verliogA code.
1:- $Strobe prints at what instants
2:- Looks like it is printing even if there is NO thresold cross
In reply to RFStuff :
It should print when there's a threshold crossing and timing==1. That's what I see. Are you sure you don't have threshold crossings?
Theree are thresold crossings. But it is printing ( what is inside $strobe )even between the zero crossings.
To me it looks like it is being printed at the end of each simulation time step ? This I am not able to understand.
Can you put together a simple example (just with voltage sources, analogLib res/cap) which shows the problem? Then post the input.scs (also the version of spectre that you're using).
I misinterpreted the result. It is printing as you have mentioned.
1:- I have some doubt regarding the initial parameter value of "t0" and "timing" in the 1st iteration.
2:- Could you please tell what change I have to make to make freq as an output node in the code ?
3:- Could you please tell how to plot it in GHz unit instead of GV ?
1. The initial values will be 0 - this is in the VerilogAMS language definition.
2 & 3 - see the model below. By specifying the output as a frequency discipline, the graph comes out with the right units too (I'd not seen your third point until I'd updated the model, but it solves 3 too...)
`include "disciplines.vams"// could specify the fout signal as being electrical// but it's nicer to do it as the specific discipline - this// way we can have a custom abstol and blowup, since the// magnitude of the frequency will be much larger than // voltages in the circuitnature Frequency units="Hz"; access=Freq; abstol=1; blowup=100G;endnaturediscipline frequency potential Frequency;enddiscipline (*instrument_module*)module frequency_meter(in,fout); parameter real thresh=0; // threshold (V) parameter integer dir = 1 from [-1:1] exclude 0; // 1 for rising edges, -1 for falling input in; voltage in; output fout; frequency fout; integer timing; real t0, t, period, freq; analog begin t = last_crossing(V(in) - thresh, dir); @(cross(V(in) - thresh, dir)) begin if (timing) begin period = t - t0; freq = 1/period; $strobe("period = %rs (measured at %rs).\n", t - t0, $abstime); end t0 = t; timing = 1; end // use a transition filter to ensure that the frequency doesn't // change discontinuously Freq(fout) <+ transition(freq,0,100p); endendmodule
Whether setting abstol and blowup in this code affects the accuracy.
Actually, I am seeing some differnece in the frequency plots ( i.e. periodic spike ) in this code as compared to the code ( without having a pin)
blowup won't, abstol might. Depends on what frequencies you're dealing with - ideally abstol should be about a millionth of a typical frequency that is being measured.
Also, the transition time should not be excessively sharp if the frequency is low. Or it may be too short - I don't know what frequency ranges you're dealing with.