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.
Get email delivery of the Cadence blog featured here
Simulating crystal oscillators got a lot easier in MMSIM12.1...We have made enhancements to both Harmonic Balance and transient analyses.
In Part 1, I discussed Improvements to the Harmonic Balance use model. With the new streamlined Choosing Analyses form, you now can focus on getting your simulation results, rather than the setup of the analysis.
Now, in Part 2, I'll cover Improvements to transient analysis. We’ve added a new feature to transient analysis that allows you to reach steady state more quickly should you decide to simulate your crystal oscillator using transient analysis.
Important: Be sure to use IC615 ISR14 or later to see the new MMSIM12.1 features in the GUI.
Part 2: Spectre Transient Analysis Enhancement
Here is the new method that you can use to speed up transient analyses of crystal oscillators.
First, we’ll simulate without using the new parameters…then we’ll add them in and show the difference.
· Set up a transient analysis in the Choosing Analyses form:
· Set the stop time to 10K periods of oscillation - in this case, 1m (1 millisecond).
· For crystal oscillators, I always use errpreset = conservative.
· Click on the Apply button. Then click on the Options button.
Set the following transient analysis options:
· Set the Time Step parameter maxstep to about 20 timepoints per period. Note that Spectre accepts expressions (see the form below), which simplifies things for you.
Set the following Algorithm Parameters:
· For Integration Method, select traponly. By default, when errpreset=conservative, the integration method is gear2only. However, gear2only can dampen oscillations and shouldn’t be used – you want your oscillator to oscillate! So, I recommend using either trap or traponly when simulating crystal oscillators.
· Set Accuracy Parameter relref to alllocal. Note that this is one of the options that are set by default when you select errpreset=conservative.
· Leave all of the other parameters at their default values.
For more information on the transient parameters, type spectre -h transient in an xterm window.
· OK the Transient Options form. OK the Transient analysis form.
· Run the analysis (Simulation->Run or green arrow ).
The transient analysis output is shown below. Access the results by selecting Results – Direct Plot – Main Form, select tran in the Analysis section, voltage in the Function section, and select the resonator net in the Schematic).
Note that in 10K cycles, this oscillator is still ramping up – it will take quite a while to start. The peak voltage is approximately 1.47V (yes, that is volts, not KV).
As a comparison: Since we know that harmonic balance solves for the periodic steady state solution, we can use this as a check. How far away from steady state are the above transient analysis results? We will look at the transient assisted (tstab) and steady state waveforms from a harmonic balance simulation. Below is the tstab waveform (Transient assisted waveform) from the harmonic balance analysis:
Note that the peak voltage is about 900V. Compare this to the transient output voltage from previous simulation where the voltage was on the order of 1.47V. This is quite a significant difference.
Harmonic balance simulates to convergence and the ifft (inverse fast Fourier transform) is plotted below.
Notice that the actual peak voltage at steady state is about 1.3KV. This is significantly larger in amplitude compared to the transient analysis. You can see that we have a ways to go before reaching steady state in the transient analysis.
Now, we’ll use the two new transient parameters linearic and oscfreq.
· In the transient options form, select the misc tab. At the bottom of the form in the Additional Parameters section, you see a type-in field called additionalParams.
· In that field, type linearic=yes oscfreq=<actual_oscillator_freq>. Here, the actual_osc_freq is 10M.
· Note the space between the two keyword=value pairs. This is needed to separate the statements.
· Now re-run the simulation for 10ms, and plot the transient waveform.
· The output of the transient analysis without specifying linearic and oscfreq is above in green. The voltage is at roughly 1.5 volts and is nowhere near steady state at 10ms.
· The output of the transient analysis using linearic=yes oscfreq=10M is in orange. Steady state was reached in approximately 3ms. Note that the voltage starts at about 900 Volts peak and at steady state is approximately 1.3kV.
We have enhanced transient analysis to improve convergence. When using the new transient options linearic and oscfreq, transient analysis starts with a solution closer to the steady state value, and the transient simulation converges much faster. Although you do need to do some typing (filling in of fields), in the end the time saving is well worth it.
Have fun simulating!
Hi all! I write to get a very important info for me: I want to simulate an oscillator for a MEMS gyroscope; so I need to introduce the RLC equivalent model of the MEMS in my schematic. The problem is that the equivalent inductance is of 1MH! I see that with default simulation parameters it is impossible to compute the solution; how can I do to have a correct simulation (for example a transient) with so high inductances? Please somebody help me! thanks in advance! Federico
e have enhanced transient analysis to improve convergence. When using the new transient options linearic and oscfreq, transient analysis starts with a solution closer to the steady
Hi Tawna, This feature is exciting . One question I have is if we use linearic = yes and give approximate oscfreq is there any chance that even the oscillator closed loop gain is less than 0dB(but close to 0dB) and circuit shows that it will oscillate.Bharath
It doesn't work for me :-(
This is what I see:Warning from spectre during transient analysis `tran'.
WARNING: Linear IC: Fail to find out initial frequency. [ Early Reject ]
Can't find linear initial condition. Running transient from DC with the specified initial conditions. Can you contact me privately about it?