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.
Get email delivery of the Cadence blog featured here
Say you have a design with 4 input frequencies: 3164M (vco), 1449M (tone0), 1456M (tone1), 1442M (tone2). Currently when you do a qpss analysis, you are inserting a total of 4 separate ports in your schematic and running a simulation. There is a divide by 2 in your circuit, so one of the frequencies of interest is 1582M. You'd like to take advantage of the multi-tone port and run a qpss analysis using 2 sources, rather than having to set up 4 individual ports.
What you'll want to use is the CTB source (composite triple beat source) feature. In the port/vsource components, CTB allows one to compose a set of evenly and closely spaced tones by using only two frequencies. This is useful in qpss analysis and greatly speeds up simulation time.Here is an example of what the port or vsource looks like in the netlist: PORT1 (net1 net2) port r=50 type=sine + freq=fcenter freq2=fspacing+ fundname="fcenter" fundname2=fspacing" + freqvec=[fcenter (fcenter+fspacing) (fcenter+2*fspacing) + (fcenter+3*fspacing)] dbmvec=[p0 p1 p2 p3]V1 (net1 net2) vsource type=sine + freq=fcenter freq2=fspacing+ fundname="fcenter" fundname2="fspacing" + freqvec=[fcenter (fcenter+fspacing) (fcenter+2*fspacing) + (fcenter+3*fspacing)] amplvec=[v0 v1 v2 v3]Note that ( ) and [ ] are needed around vector expressions, such as freqvec/amplvec for parsing purposes.
It is easiest to show how to use the CTB source by example. So, for your particular example....
1. Here's how you set up your CTB port:See the screen shots below. The center frequency is put as the first sinusoid. The spacing frequency is put as the second sinusoid. Note that the "display multi sinusoid" button is selected.
In particular, note when you select "Display multi sinusoid", the form expands to allow you to select multiple frequencies. Here, enter the frequency, magnitude, phase, and maximum number of harmonics for each tone:
2. Next, here's how to set up your Choosing Analyses form for Harmonic Balance qpss or hb analyses:
Or, if you are using Harmonic Balance QPSS, your Choosing Analyses form setup will look like this:
3. If you are using a frequency divider in your circuit, remember to set the large signal frequency division parameter in the Options form:
4. Comparing your original netlist snippet with the CTB netlist snippet:
This is how your ports and qpss statements look in the original netlist:PORT5 (net058 0) port r=50 type=sine dbm=-20 freq=1456M fundname="tone1"PORT7 (net060 0) port r=50 type=sine dbm=-20 freq=1442M fundname="tone2"PORT8 (net062 0) port r=50 type=sine dbm=-20 sinephase=90 freq=1.449G fundname="tone0"V8 (net081 0) vsource type=sine ampl=1 freq=3164M fundname="vco"
...qpss qpss funds=["vco" "tone1" "tone0" "tone2"] maxharms=[20+ 3 3 3] errpreset=conservative tstab=0 annotate=status+ flexbalance=yes freqdivide=2
And your new netlist (showing both qpss and hb analyses) will look like this:
PORT0 (net058 0) port r=50 num=1 type=sine freq=1.449G freq2=7M \ fundname="Fcenter" fundname2="Fspacing" freqvec=[ 1449M+7M \ 1449M-7M 1.449M+7M ] dbmvec=[ -20 -20 -20 ] phasevec=[ 90 0 0 ] \ maxharms=[ 3 3 3 ]VCOsource (net081 0) vsource type=sine freq=7M*226*2 ampl=1 fundname="vco"...qpss qpss flexbalance=yes oversample=[1 1 1] funds=["vco"+ "Fcenter" "Fspacing"] maxharms=[20 3 3] errpreset=moderate+ annotate=status freqdivide=2hb hb oversample=[1 1 1] funds=["vco" "Fcenter" "Fspacing"]+ maxharms=[20 3 3] errpreset=moderate freqdivide=2 + annotate=status
Have fun with your simulations!
The netlist shows a single net (net058) for PORT0. Then how are the connections to circuit done. In case of 4 ports there are separate nets for separate inputs.
This is described in more detail in support.cadence.com solution 11575904:
What is the difference between hb/hbac/hbnoise and the harmonic balance Q/PSS Q/PAC, Q/Pnoise ?
A brief summary of the solution:
In mmsim 7.1, we introduced new analyses: hb, hbac, and hbnoise. We recommend using these analyses in MMSIM 7.1 and onward. The analyses are essentially the same as the old harmonic balance Q/PSS and small signal analyses, but the hb/hbac/hbnoise GUIs are easier and more intuitive to use.
A good way to get started using the new analyses is to go through the RF Workshops located in the hierarchy at mmsim_hierarchy/tools/spectre/examples/SpectreRF_workshop/rfworkshop_hb.tar.gz
Can you explain if doing (a) hb analysis or, (b) QPSS analysis with hb engine one and the same thing? If so why there are two options?