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 am designing an injection locked vco. My simulation scenario for the phase noise is as follows:
1. Run the vco without the injection signal for 2 microseconds ; let it setttle to the free running frequency;
2. Start the injection signal and observe the phase noise...
Well, I need a periodic vsine source to generate the injection signal in the schematic; and this is the very source of an error in my pss simulation:
" 'V0' is a periodic input signal, which is inconsistent with autonomous circuits. "
this is what happens if I set cadence for phase noise simulation using the instructions given in the cadence Spectre manual.
I know... the instructions are for a 'normal' vco; but I was hoping that it would work for my injection locking case as well.
Question, as obvious it is by now :), how do we simulate the injection locked oscillator phase noise ?
Is there a way to conceal the periodic voltage source in the circuit so as not to piss the pss off ?
Hi Calp, If you have access to Cadence Online Support website then there is a solution on how to simulate such vco – http://support.cadence.com/wps/mypoc/cos?uri=deeplinkmin:ViewSolution;solutionNumber=11182082
For such oscillators you shouldn’t be using the Oscillator button in the PSS form as this is considered a driven circuit since it is driven by an injection source. That is the reason you are receiving the error message. Once you set the PSS form accordingly, set the tstab to 100 periods (and can also use the saveinit button to save the initial transient waveform before steady state). You should now be able to run the simulation. With Regards,Ashish
In reply to Ashish Patni:
thanks ashish.. looks like we are getting somewhere. :)
Unfortunately, I don't have access to the link. Would you mind telling me more abt the pss/pnoise setup for these driven cct cases?
vco free running freq : 106 MHz.
injection freq: 111MHz.
In reply to Aprameya:
Please login to http://support.cadence.com and do a search on 11182082 . That should take you to the solution that Ashish is referring to:
I just verified this myself.
Sr. Staff Support AE, Global Customer Support
Cadence Design Systems, Inc.
In reply to Tawna:
In reply to woodyrfic:
Here is the article:
When simulating an injection locked oscillator and looking at the startup waveform, you are looking for the point where the timing of the oscillator output is stable with reference to the injection source. Note that the amplitude must be at steady-state as well.
When you set up your PSS analysis you:
- Do NOT select the oscillator button.
You are applying a signal (vsource) to your ring oscillator which causes the oscillator to oscillate at the injection frequency. Thus it is a driven circuit - as it is driven by the injection source. This is why you don't push the oscillator button on the PSS choosing analysis form. SpectreRF considers this a driven circuit and will error out if you select the oscillator button on the PSS choosing analyses form.
- Set tstab to 100 periods.
You want the circuit to be stabilized, i.e. you need to get it close enough to the final oscillation frequency so that PSS can converge. This will depend on the time constant of the circuit. A high Q oscillator will take a long time to settle. A ring oscillator is lower Q by definition, so it should not be as problematic.
- Check the saveinit button.
The waveforms for the initial transient before steady state are saved and you can view them with the results browser.
- You may even want to try to run the circuit using transient analysis.
Look at the oscillator output compared to the injection source. Look for variations in the timing of the oscillator output compared to the locking source. Hopefully, the circuit will settle fairly quickly.
Now, once you can get PSS to successfully converge, you can look at things like pnoise jitter
May I know what would be the best way to simulate an injection locked VCO where there is no external source used for injection. In this case, there will be two identical LC VCOs that will start oscillating and inject signals in to each other, there by being injection locked. Transient takes a lot of time, may i know if PSS, QPSS and/or envelope analysis support Quadrature VCO simulation for simulating steady state/start up.
In reply to Vijay Sunil Madaka:
I think you may need to open a new thread for this topic as I believe your question is different than that in the original thread. However, I will let Andrew decide.
> May I know what would be the best way to simulate an injection locked VCO where there is no external source used for injection.
It sounds as if you are looking to study the coupling between two LC VCO. Studying the coupling is a very difficult simulation problem. When coupling exists it will be at a frequency determined by the frequency difference between the two oscillators, their relative phase, and the source and strength of the coupling mechanism. I have used conventional transient simulations to study this phenomena. However, I have resorted to simplified models of some of the circuits involved to save computation time. Since the phenomena also depends on the relative phase of the two oscillators, I do not believe PSS will be very helpful as it is looking for a steady-state solution and the relative phase of the two waveforms may change as it iterates its solution.
If there a specific item you are looking to study, perhaps myself and others could provide some better insight as the question you pose is pretty broad.
In reply to smlogan:
Thank you for your inputs. I have created a new thread and mentioned what I am trying to do.
Looking forward to your suggestions,