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.
Get email delivery of the Cadence blog featured here
In the previous appends, we looked at using Shooting Newton Periodic Steady-State analysis to analyze analog circuits. In this append, we will look at using Harmonic Balance Periodic Steady-State, HBPSS, to analyze analog circuits. HBPSS is widely used for RF and microwave circuit design. However, designers often do not realize that it can also be useful for analog circuit design, in particular, when they would like to analyze distortion. As an example, we will simulate the Total Harmonic Distortion, THD, of an amplifier. We will compare and contrast using transient analysis with the Fourier transform and using HBPSS to analyze distortion. The test circuit is a simple Audio Amplifier for headphones built from an LM386 op-amp, shown in Figure 1.
Figure 1: LM386 Audio Amplifier
Typically, transient analysis with the Fourier transform is used to simulate the THD of an audio amplifier. The challenge with using transient analysis is to optimize the transient analysis simulation configuration for accurate Fourier analysis. Fourier analysis requires that the circuit has reached sinusoidal steady-state, that is, we need to measure the response after the start-up transient of the system has completed settling. Achieving sinusoidal steady-state can require settling for many periods in audio designs because of the large time constants due to the large off-chip capacitors for dc blocking. Of course performing Fourier analysis can alter the spectrum of the amplifier unless designers are careful with their simulation and Fourier analysis setup.
To illustrate the limitations of Fourier analysis and the benefit of steady-state analysis for this application, the several simulations were run. In each case the THD was calculated for one period of the fundamental frequency, in this case 1kHz. Four transient simulations were performed with different amounts of delay allowed to settle the start-up transients of the circuit before performing the Fourier analysis. The delay times were: 0 periods of the fundamental frequency, 1 period of the fundamental frequency, 3 periods of the fundamental frequency, and 10 periods of the fundamental frequency. The THD for each simulation condition is shown is Table I. In this case, the simulation is performed using the Spectre's conservative error preset. The conversion from the time domain to the frequency domain was performed using the ViVA Waveform Calculator FFT function and the Spectre Fourier Integral.
Table 1: THD Results for Various Simulation Conditions
For this simple example, the simulation time using harmonic balance PSS analysis is >5x faster than using transient analysis with the Fourier Transform. As circuit become larger and especially for post-layout simulations, we would expect to see that the difference in the transient analysis time and the dc operating point calculation become larger and HBPSS becomes even more effective. Reducing simulation enables designers to analyze THD across process variations, with corner and Monte Carlo analysis, or to optimize THD.
One question maybe why didn't we use Shooting Newton for the periodic steady-state analysis? The short answer is that Shooting Newton is not required in this case. Harmonic Balance analysis provides the steady state solution in terms of finite Fourier series and is very effective for simulating distortion. If time domain waveforms were more non-linear, for example, when simulating a Switched Capacitor circuit or a DC-to-DC Converter then Shooting Newton would be appropriate.
To help illustrate the need to settle the initial start-up transient, I have plotted the non-periodicity, on of the outputs of the Spectre's Fourier Integral analysis, as a function of settling time, see Figure 2. The non-periodicity measures the difference between the initial value and final value. When the response is in sinusoidal steady-state the non-periodicity will be 0.
Figure 2: Effect of Settling Time on Periodicity
This approach, using harmonic balance analysis for periodic steady-state analysis to supplement transient analysis with the FFT, can be applied whenever you need to measure the distortion of a linear amplifier. In the next append, we will look at extending this approach to using PSS for distortion analysis of non-linear circuits, for example.
Hope you found this append useful, please let me know!
Great post. Like Andy1959 said, 'nice article. Clear concise, and to the point."
We, at Pinter Electronics Consultants, write similar content.
Check it out: www.pinterec.ca/.../blog
Nice article. Clear concise, and to the point. A nonlinear example like a mixer or a sigma delta would also be very useful.
An application note would a couple of basic examples would work well. A methodology that works for both switched cap and continuous time implementations would be very nice. Longer term a measurement test box may be the way to go. However having a good document as a reference to refer too is always a good thing. Hope this helps.
The request is has come up often recently. As the tools have advanced, it is difficult for designers to know when to use which technology for what problem. It is definitely something that we need to do more systematically. One question for you as a user, how would you like to see the guidelines provided: Published as application notes? As measurement testboxes? ...?
Good post. Anything that reduces sim time and allows things like corners and montecarlo is good. In paticular the non-linear topic will be interesting. Switched cap circuits take a while for transient simulations and improving these will help greatly. In particular sigma-delta designs would greatly benefit. I have seen some documents on how to check noise for sigma-delta ADC's with spectre-RF, however I have never been able to get accurate results. A comprehensive guide on noise and distortion simulations with sprectre-RF for these type of circuits would be of great benefit.