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.
Signals are subject to degradation when they are transmitted through a channel. High speed signals are especially susceptible to degradation as loss and distortions tend to be frequency dependent. Channel characterization and multi-million bit simulations can be used to investigate these issues in greater detail. However, such investigations are time consuming for PCBs with several high speed nets.
Signal Quality Screening is used to determine signal quality of a system. It determines the signal and background noise intervals introduced by the system or channel. Extensive simulation is most beneficial when applied to the noisiest channel(s) in a given group. Signal quality screening determines the noisiest channel that needs further investigation. This focused analysis results in improved designs in a shorter time. In SPB16.3 Allegro PCB SI GXL, you can perform signal quality screening on a set of nets, which could either be single-ended or part of a differential pair.
Read on for more details…
How Signal Quality Screening Works
The Signal Quality Screening engine uses the frequency domain simulation capability of TLSim. An AC simulation generates the frequency response of the channel from which an impulse response can be generated. This impulse response is the characterization of the channel. Signal to Noise Ratio can be found by taking the ratio of the area of the signal bit and the rest of the impulse response (noise), as shown below.
The signal quality screening engine uses the frequency domain simulation capability of TLSim. A clean bit is sent to a channel to be analyzed. Its response is measured at the end of the channel, or input of a receiver. The response spreads in a much wider time interval than the original bit period. In the figure below, a window is placed on the time interval, in which the white portion represents signal while the gray portion represents noise.
The energy in the signal portion and the noise portions is then quantified by the areas under the waveform curve. The energy is calculated by root-square summations of the difference between the signal voltages and the reference voltage at every sampling point, or time step. The reference voltage is taken to be the final value at the end of the simulation when the signal is finally settled.
The bit period is derived from the Pulse Clock Frequency set in the Analyze — SI/EMI Sim — Preference — Simulation Tab.
This value of bitp is checked against the cutoff frequency (discussed in the next section). If the value of the bit period is substantially less than the bit period obtained from the cutoff frequency, a warning is issued.
Calculating the Signal Quality ValueThe signal quality value, which determines signal quality of a system, is calculated by taking the ratio of the energy of the signal and the rest of the waveform. Signal energy is derived by taking the sum of the square of voltage differences between the voltage instance and the reference voltage.
The cutoff frequency specified for the routed interconnect models in Analyze — SI — Preferences — InterconnectModels Tab is used as the default frequency for the AC simulations. If this frequency is 0 (or any number less than 5 GHz), a warning is issued and simulations are performed for a default value of 20 GHz.
A new button has been added to the Signal Analysis dialog:
Nets are selected in the same manner as if a Report or Waveform was being generated:
The Signal Quality Screening engine starts with the selected nets as input. Once all values have been determined, a results table with the net names and their corresponding signal quality values is displayed.
These values are sorted from lowest to highest signal quality value. Filter boxes are available that allow you to display a particular list of nets based on the net name. You can save this list of nets by selecting Save List of Nets... You can view and save a text version of the report by selecting View Report.
I look forward to your feedback on this PCB SI capability.
Jerry "GenPart" Grzenia