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.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
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'm about to simulate a power amplifier with spectre using mmsim 10.1 and cadence ic 5141. I want to analyze if it oscillates in transient simulations. Therefore I gave an inductor a initial condition which is not 0 so that there is a stimulation.
I read the following recommandation to simulate oscillators in a cadence blog post: (/blogs/rf/archive/2012/12/20/mmsim12-1-speed-up-transient-analysis-of-crystal-oscillators.aspx)
"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."
So I choose traponly and got problems with conversion. (The timestep was reduced to a few attoseconds) Even if I choose liberal as error preset. The simulation result is shown here:
First I thought there is an oscillation and zoomed in, which you see here:
Then I thought that there are some issues with undersampling or something like that, but if you look at the timestep, then the frequency would be higher than 500 GHz because the period of this triangle signal is about 2ps.
But I'm using a SiGe Technology with a transit frequency of 200 GHz.
Then I simulated the circuit using gear2 method and got the following result:
Which seems to be ok. Because nothin is oscillating at the end and the oscillation from my inductors initial condition is dampened very fast.
It also works if I set the errorpreset to conservative as I do usually.
I also read in the spectre reference about the different envelope integration methods like gear2, trap, etc. But I only saw that there are different presets in the timesteps, tolerances, steadyratios and so on which doesn't help me in understanding when do I have to use which method? And how do they work. What is the problem with using traponly?
I hope anyone can help.
What you are seeing here is a phenomenon called trapezoidal ringing. It's a numerical oscillation - the indication that it is numerical is that the oscillation is between adjacent timepoints (if you show all timepoints in the waveform, there should be none between the peaks of the oscillation).
The typical ways to cure trapezoidal ringing are to use a gear method (e.g. gear2only) because this introduces (amongst other things) a small amount of numerical damping, or you could tighten reltol. The downside of gear2only is that the small numerical damping can artificially damp out oscillation, and hence it can make it hard to simulate oscillators and also it can make unstable circuits appear more stable.
So you might also try tightening reltol (e.g. to 1e-5) and see if that helps.
However, maybe gear2only is fine with your circuit - it rather depends on what you are expecting!
You can find some more background information in http://www.kenkundert.com/docs/bctm98-MSsim.pdf (starting on page 18, with trapezoidal ringing explained on page 22) and in Ken Kundert's book "The Designer's Guide to SPICE and Spectre", see http://www.designers-guide.org/Books/dg-spice/index.html.
I would also like to point out that the Spectre version you are using is rather old (the current version is MMSIM 13.1).