Skip to main content
How To PCBPCB DesignSignal IntegrityVideosWebinars

Unlock Your Signal Integrity Analysis Potential

Signal integrity analysis provides the measurement of the amount of signal degradation when the signal travels from the driver to the receiver. In other words, it signifies the signal’s ability to propagate along PCB traces without distortion.


Author headshot: The Keysight ADS Team

By The Keysight ADS Team

May 11, 2021  |  0 Comments

Signal integrity analysis provides the measurement of the amount of signal degradation when the signal travels from the driver to the receiver. In other words, it signifies the signal’s ability to propagate along PCB traces without distortion.

 

Watch Now Button

 

What is PCB simulation?

PCB simulation and signal integrity analysis
PCB simulation and signal integrity analysis

Simulation of a PCB is carried out to understand the actual behavior of the circuit board. It basically increases the efficiency of fabrication by providing a quick preview of how the printed circuit board is going to perform. Simulation (3D electromagnetic simulation)  is performed once the PCB layout is ready. This is followed by signal integrity analysis.

Once the board is fabricated, scope measurement and SI analysis are performed. SI analysis is performed twice, once in the layout stage and once after the board is fabricated.

Read about circuit simulation in How Does Circuit Simulation Work?

How to unlock your signal integrity analysis potential?

There are three aspects to be considered here:

  1. Understand the root causes of SI problems
  2. Have a realistic virtual prototype
  3. Rely on dependable PCB manufacturer

Let us see how these three points come together in a PCB design workflow.

PCB design workflow
PCB design workflow

Circuit board design workflow has three main phases. They are early design, PCB layout, and PCB fabrication. The system block diagram is drawn during the early design phase. PCB layout phase has stack-up and layout design. Finally, the manufacturing and assembly of a board are carried out in the fabrication phase. Sierra Circuits and Keysight Technologies provide assistance throughout all these phases. Virtual prototypes are generally sent to the manufacturers before the fabrication process begins.

 

sierra-circuits-pcb-stack-up-designer

 

Example of a virtual prototype

A virtual prototype allows the designers to identify and address issues related to signal integrity, thermal management, and manufacturability before the fabrication of the PCB prototype. The below image shows a virtual prototype of Xilinx FPGA ZCU104.

Virtual PCB Prototype
Virtual PCB prototype

The simulation is carried out by considering a net. Here we consider the signal flowing from the CPU (transmitter) to the HDMI retimer. The signal flow is shown in the image below.

Signal flow in PCB simulation
Signal flow in PCB simulation

Metrics to anticipate the signal loss

Before we begin the simulation, it is very important for us to anticipate the signal losses. The losses can be manually calculated using loss metrics.

Calculation of signal loss

The length of the trace is about 3 inches and the loss is 0.1 to 0.2 dB/in/GHz.  The signal loss can be calculated as shown below:

0.1 x (3 inches) x (10 GHz) = 3 dB;

0.2 x (6 inches) x (10 GHz) = 6 dB

Therefore we can expect a loss of 3 to 6 dB.

Calculation of time delay

We use signal speed in FR4 to anticipate the time delay. That is 6 inches/nanosecond.  The time delay can be calculated as shown below:

Time delay = (length of the trace)/(signal speed in FR4);

(3 inches)/ 6 ns = 0.5 ns . The expected time delay is about 0.5 nanosecond.

Calculation of differential impedance (Zdiff)

We use the impedance rule of thumb to anticipate the Zdiff.

Before we get into that, let us have detailed information on the HDMI traces.

Width and spacing of HDMI traces
Width and spacing of HDMI traces
Stackup of HDMI traces
Stack-up of HDMI traces

The stack-up says the H1 is 3mils and the H2 is 2.9mils. The differential impedance can be calculated using the impedance rule of thumb.

Impedance rule of thumb: If the width over the minimum (H1, H2) is about 1 and the spacing is around 3W then the differential impedance is equal to 100 ohms.

The differential impedance can be calculated as shown below:

Zdiff   = 100 ohms if; W / {min (H1, H2)} is equivalent to 1 and S is greater than 3W. Where W is the trace width. Here, the first condition (W/ {min (H1, H2)} is equivalent to 1) is almost satisfied. For the second condition (S should be greater than 3W) to be satisfied, the spacing should be around 9 mils. The spacing in this case is around 4 mils. That means the differential impedance is going to be less than a hundred ohms.  Let us assume that the impedance is around 90 ohms.

 

impedance-calculator.jpg

 

Now, we have all the anticipated values. These values can be cross-verified by performing a quick RapidScan.  Follow the below steps to run a 2D RapidScan in Keysight EDS.

  1. Import the board into the software. Keysight ADS SIPro will show all the nets of the board imported
  2. Select the HDMI nets (signal propagating from CPU to retimer).
  3. Right-click and choose the options RapidScan-Z0 > Analyze transmission. The steps are shown in the image below.
Steps to run RapidScan in Keysight EDS
Steps to run the RapidScan-Z0 in Keysight EDS

Transient analysis is one of the key aspects to ensure signal integrity in your design. To learn more about it, see Transient Analysis for Non-Sinusoidal Signals.

The image below shows the comparison between the expected and actual results of the simulation.

Comparison between expected and actual results of the simulation
Comparison between expected and actual results of the simulation

Robust signal integrity simulation workflow

A robust signal integrity workflow includes extracting the channel Electromagnetic (EM) model, dissecting channel data, and exploring design space. The flow chart below shows the robust signal integrity simulation process.

Robust signal integrity simulation workflow
Robust signal integrity simulation workflow

 

Signal Integrity eBook - Cover Image

Signal Integrity eBook

3 Chapters - 12 Pages - 20 Minute Read
What's Inside:
  • Impedance discontinuities
  • Crosstalk
  • Reflections, ringing, overshoot and undershoot
  • Via stubs

 

 

Extracting the channel EM model

The first step of the simulation workflow is to extract the channel EM model. Before we do that, we need to anticipate the values. We now convert the known values into S parameters. The image below shows the converted values.

Expected values for S parameters
The expected values for S parameters

The images below show that the expected and the resultant values of S parameters are consistent for low and high frequencies.

Values of S parameters at high frequency SI analysis
Comparison of expected and resultant values at high frequency
S parameter values at low frequency
Comparison of expected and resultant values at low frequency

Dissect your channel data

The first step is to convert single-ended trace to differential pair. The image below shows the setup to convert single-ended trace to differential pair.

Conversion of single-ended trace to differential pair

S parameters and SIPro simulation data
Comparison of expected S parameters and SIPro simulation data

Delay and skew calculations

The setup below can be used to extract the time delay.

Setup to extract the time delay for signal integrity analysis
Setup to extract the time delay

The image below shows that the expected values are consistent with the simulation data.

Time delay and the simulation data
Comparison between expected time delay and the simulation data

Channel simulation

The channel simulation will use PRBS (pseudo-random binary sequence) to evaluate the signal integrity. The image below shows the setup for the channel simulation.

Signal integrity analysis channel simulation
Setup for channel simulation

The comparison between the expected eye diagram and the simulation data is shown below.

Signal integrity analysis eye diagram and simulation data
Comparison between eye diagram expectation and the simulation data

The eye diagram clearly shows that the simulation result has an open eye. Therefore the expectation is consistent with the simulation data.

Explore design space

In this step, we perform equalization and other advanced analyses on the virtual prototype.

Watch the whole webinar to get more practical knowledge of SI analysis. If you want to learn more about any particular aspect of signal integrity simulation then let us know in the comment section.

 

Watch Now Button

 

High-Speed PCB Design Guide - Cover Image

High-Speed PCB Design Guide

8 Chapters - 115 Pages - 150 Minute Read
What's Inside:
  • Explanations of signal integrity issues
  • Understanding transmission lines and controlled impedance
  • Selection process of high-speed PCB materials
  • High-speed layout guidelines

 

What is 1900 + 86?

Subscribe
Notify of
guest
0 Comments
Inline Feedbacks
View all comments
Share this article
Zero Defects guaranteed on all PCB fabrication

Reduce Re-Spins with our Zero Defect Guarantee.

Our platform sources the whole package, creating a thread from design to delivery. Fabricating PCBs. Procuring parts. Assembling your boards.

Once you upload your BOM, Our best-in-class software automatically checks for errors and cleans your file for you. After you place an order, your dedicated CAM engineer will run a full DFM and DFA check to ensure your prototype achieves Zero Defect every time—all at no additional cost to you.

Get to market faster and spend less time troubleshooting.


Start Quote

Talk to a Sierra Circuits PCB Expert today

24 hours a day, 7 days a week.

Call us: +1 (800) 763-7503
Email us: through our Customer Care form