How to Perform Simulation Analysis with Cadence SPECCTRAQuest

In electronic circuits, the schematic serves as a blueprint outlining the connections between signal lines. While many designers may hold the belief that meeting the physical and electrical alignment rules and establishing functional connections suffice to complete the PCB design process, this notion does not hold true in the realm of high-speed circuits. In high-speed circuits, a rudimentary approach can give rise to significant signal integrity issues, including problems like signal reflections and crosstalk, and in severe cases, circuit failure.

Advanced Reading: Signal Integrity Issues and Countermeasures

To preempt and mitigate these challenges, specialized signal integrity tools have been developed. In this TechSparks article, we will use Cadence SPECCTRAQuest as an illustrative example to elucidate the simulation processes both before and after the PCB design phase. Let’s commence our exploration!

Step 1: Acquiring an Accurate IBIS Model for the Component

To achieve precise simulation results, it’s imperative to start with a meticulously accurate electrical model of the component. This is a fundamental principle shared by all circuit analysis software. While it’s conceivable for a designer to construct such a model based on test results, this approach is undeniably challenging. Consequently, it is highly recommended to utilize the component manufacturer’s provided model whenever feasible.

The IBIS model is used in SPECCTRAQuest, no matter which manufacturer you use, you must request the IBIS model corresponding to the component. In instances where this proves unattainable, one can resort to utilizing similar component models for simulation experiments to derive approximate results. It’s important to note that this step may be dispensable for certain components, such as EEPROMs in memory modules, where functional aspects are not of primary concern.

Step 2: Converting the IBIS File Format and Importing Models

  1. Open SPECCTRAQuest and load the “.brd” file you want to analyze.
  2. In the SPECCTRAQuest interface, click on “Analyze” -> “SI/EMI Sim” -> “Library.”
  3. In the popup window, locate the “Translate” function button at the bottom right.
  4. Click on “ibis2signoise” to select the IBIS file format conversion tool.
  5. Choose the directory path where your IBIS model file is located. Once the conversion is complete, you will see the corresponding dml file in the library browser.
  6. If you already have a converted dml file, you can also add it directly by clicking “Add Existing Library” and specifying the directory path.

Step 3: Loading the Appropriate Model for the Component

  1. Navigate to the SI/EMI Sim menu and select “Model Assign.”
  2. A window titled “Signal Model Assignment” will appear. Here, select the relevant component and click “Find Model.”
  3. In the ensuing “Model Browser” window, choose the required model.

To streamline the process, you can specify the library where the model resides by selecting “Show Model From.” Next, identify the model type under “Model Type Filter,” and input “*” in the “Model Name Pattern” field to display all models within the selected library and type.

For certain passive components, it may be necessary to construct a custom model. In such cases, click “Create Model” and follow the prompts to input values and define the function of each pin. To facilitate future tasks, it is advisable to save and generate *.dat files. These files can be conveniently loaded when conducting simulation analyses using SPECCTRAQuest in subsequent work sessions.

Step 4: Specify the Power Supply Voltage

This step involves establishing the power supply voltage and ground level to enable the retrieval of the power supply model when extracting the topology model. It’s important to note that this step may be unnecessary for both forward and reverse simulations if the signal lines required for simulation analysis are unrelated to power and ground. The procedure is as follows:

  1. In SPECCTRAQuest, go to Logic -> Identify DC Nets.
  2. This action triggers the appearance of the “Identify DC Nets” dialog box. Here, select the power signal, input the corresponding voltage in the Voltage column, and confirm by clicking “OK” or “Apply.”
Identify DC Nets Dialog

Step 5: PCB Stackup Configuration

In SPECCTRAQuest, access the PCB stackup setup by selecting “Setup” and then “Cross-section.” This action will launch the Layout Cross Section dialog box, granting you control over stack layer management and the adjustment of layer parameters such as material, thickness, and conductivity.

Typically, the number and order of PCB stack layers, as well as the specific layer parameters, are predetermined and need only be aligned with project requirements. To attain the desired characteristic impedance, you have the flexibility to make adjustments to PCB trace width or substrate thickness as necessary.

It’s worth noting that when using the Cadence PSD 14.2 version for stack settings, occasional program anomalies may occur. This issue can be resolved by opting for Script commands as a workaround to manual configuration.

Step 6: Defining Simulation Parameters

Prior to commencing the simulation experiment, it is essential to configure various parameters, which can also be adjusted during the simulation analysis if necessary. To accomplish this, navigate to the SPECCTRAQuest interface and select “Analyze” -> “SI/EMI Sim” -> “Preferences” (or choose “Analyze” -> “Preferences” in Sigxplore). Within this menu, you can fine-tune parameters such as simulation cycle count, clock frequency, offset, and more.

Typically, the software provides default values for these parameters, which you can then modify to align with the specific requirements of your project.

Step 7: Signal Line Selection

  1. Go to “Analyze” -> “SI/EMI Sim” -> “Probe” (or use the provided shortcut key). This action triggers the appearance of the Signal Analysis dialog box.
  2. Within the Net column, enter “*” to display all available nets in the left box. Alternatively, you can opt to load an existing netlist file.
  3. In the sections labeled “Driver Pins,” “Load Pins,” and “Other Pins,” pins associated with the selected net will be presented based on their input-output relationships.
  4. Designers can adjust the pin type for each device by selecting “Logic” -> “Pin Type” in SPECCTRAQuest if needed.

Step 8: Circuit Topology Extraction

Once you’ve selected the target Net within the Signal Analysis dialog box, proceed by clicking “View Topology” located at the bottom right corner. This action transitions SPECCTRAQuest into Sigxplorer.

In the Sigxplorer interface, the topology template of the extracted circuit is displayed. The “View Topology” button acts as a bridge connecting SI Expert and Sigxplorer seamlessly.

It is crucial to review the extracted circuit’s topology template to prevent potential errors stemming from incomplete Via models or excessive use of arbitrary-angle traces in the PCB design.

To access specific modules, click on “Parameters,” “Measurements,” “Results,” or “comman” (depending on the context) located below the circuit’s topology template to display the corresponding data in the table.

Step 9: Choose Drive Stimulus and Configure Component Parameters for Simulation

Analysis and simulation must align with the designer’s specified environment. Sigxplorer offers a range of drive excitation modes and provides comprehensive, editable parameters for various components, including support for parameter sweep analysis.

  1. Click on the “TRISTATE” label in the second row, just above the driving source in the circuit.
  2. In the pop-up window, select the appropriate drive mode, typically “Pulse.”
  3. If adjustments to mode parameters are needed, you can make them by navigating to “Analyze” -> “Preferences.”
  4. To modify specific component parameters, click on the component’s name.
  5. Once parameters are set, select “Analyze” -> “Simulate.”
  6. The Sigxplorer spreadsheet interface will automatically shift to the Results column, displaying the simulation outcomes.
  7. In cases where parameter sweep simulation is not conducted, SigWave’s waveform will be loaded automatically to showcase the simulation results.

Step 10: Analyzing Simulation Results

Let’s consider reflection analysis as an example, which includes essential details like SIM ID, driver information, cycle data, FTS MODE, Noise Margin, overshoot high, overshoot low, and Propagation Delay. Typically, designers place significant emphasis on the SigWave-generated waveform results.

Designers often have specific requirements, such as ensuring an adequate noise margin, avoiding excessive overshoot and undershoot beyond specified voltage levels, eliminating noticeable ringing phenomena, preventing significant waveform distortion, and ensuring monotonic rising and falling edges of the waveform.

However, it’s important to acknowledge that different circuits may introduce unique considerations, such as requirements for transmission delay time or the speed of rise time. Addressing these specific issues demands the designer’s careful analysis and expertise.

Step 11: Wrapping Up

Upon completing the simulation of a Net in Sigxplorer, you can exit the program and return to SI Expert. If you intend to perform a new signal integrity simulation and compare it with previous results, you have the option to select a new Net and extract it within the Signal Analysis dialog box of SI Expert via window switching.

However, it’s important to exercise caution here. SPECCTRAQuest may experience bugs that lead to model confusion, potentially resulting in the failure of the new Net’s topology template simulation. To circumvent this, it’s advisable to generate a simulation report before closing Sigxplorer.

As a general practice, you should save the extracted topology template in the .top file format, along with the waveform file in the graphical .sim format for future reference and convenience.

More content you may be interested in

Flexible PCB Testing Guide
Flexible PCB Testing Guide

Dive into the world of flexible PCB testing with TechSparks! Explore the methods, challenges, and IPC standards essential for ensuring the reliability and functionality of

hard drive pcb replacement
Hard Drive PCB Replacement Guide

The guide outlines the importance of Hard Drive PCBs, providing insights into diagnosis and repair/replacement options. It emphasizes BIOS chip compatibility and cautious PCB replacement

what is a short circuit
Fundamentals of Short Circuit

Short circuits, prevalent in electronics, pose serious risks like fires, damage, and shocks. Identifying causes such as wire damage or component failure is crucial for

pcb soldering defects
PCB Soldering Defects

PCB solder defects, like bridging, fillet issues, virtual soldering, voiding, and tombstoning, arise from factors such as temperature control and component placement. Prevention involves planning,

solder bridge
Basic Guide to PCB Solder Bridges

Solder bridges in PCBs are unintended connections between circuit paths or pads, leading to short circuits and device malfunctions. They stem from design flaws, process

Scroll to Top