SI Analyzer by Keysight

More and more modern electronic devices incorporate high-speed PCB designs, and signal speeds grow as the technologies evolve (17 GHz in DDR6, 400 Gbps in QSFP++, etc.). Ensuring signal integrity (SI) is a crucial step in the high-speed design. Failure to meet the requirements of the interface developer is very likely to cause problems in further design stages, manufacturing, and performance.

To perform a Signal Integrity analysis right in the Altium Designer environment, the SI Analyzer by Keysight solution is available. Provided as a software extension, the SI Analyzer by Keysight integrates directly with Altium Designer to allow the performing of a range of SI post-layout checks to cover the most important high-speed design parameters:

• Impedance

• Delay

• Insertion Losses (IL)

• Return Losses (RL)

Installing the SI Analyzer by Keysight

There are two stages to setting up to perform signal analysis using SI Analyzer by Keysight in Altium Designer:

• Installing the SI Analyzer by Keysight extension.

• Adding a valid SI Analyzer by Keysight license.

Installing the SI Analyzer by Keysight Extension

To access the SI Analyzer by Keysight functionality in Altium Designer, the SI Analyzer by Keysight extension must be installed for your installation of Altium Designer. The extension is located on the Purchased tab of the Extensions and Updates page, which can be accessed by selecting the Extensions and Updates command from the menu of the Current User control (e.g., ) at the top right of the design space. To install the extension, hover the cursor of the extension icon and click the download icon that appears ( ).

When you click to download and install the extension, the End-User License Agreement will open. Clicking Accept indicates your acceptance of the EULA terms and conditions; when you do, the installation will continue. Clicking Close indicates that you do not accept the EULA terms and conditions, and the installation process will cease.

Restart Altium Designer after installing the extension.

Refer to the Extending & Updating Your Installation page to learn more.

Licensing the SI Analyzer by Keysight

Use of the SI Analyzer by Keysight requires a license. Once you have installed the SI Analyzer by Keysight extension, head over to the License Management view within Altium Designer accessed by clicking on the  Current User control (e.g., ) at the top-right of the design space and choosing the Licenses command from the menu. Find the Signal Analyzer by Keysight license entry and click the Use License button to activate that license.

Refer to the License Management page to learn more.

Launching the SI Analyzer by Keysight

To start signal integrity analysis, open the project's PCB document and select Tools » SI Analyzer by Keysight from the main menus.

Preparing for Analysis

Adding Nets to be Analyzed

After launching the SI Analyzer by Keysight, the PCB data are imported (in the ODB++ format) to the solver. At this stage, you can define the list of nets to be analyzed and assign specifications to them. To do this, click the Manage Nets button at the top of the SI Analyzer by Keysight document or use the Edit » Manage Nets command from the main menus (alternatively, if there are no nets in the document, the Manage Nets button is also available in the center of the document). The Manage Nets dialog opens, presenting the list of the PCB's net, differential pair and xSignal classes.

Enable the check box for each required class (or use the checkbox in the grid header to select all classes). Optionally, click the cell in the Specifications column to display a pop-up and select the required specification(s) that will define constraints for the selected class (which can be redefined later if required – learn more). You can select from built-in or user-defined specifications (the Specifications tab of the pop-up) or, for a class, define the required constraint values manually (the Custom Constraints tab of the pop-up).  

Refer to the Managing Specifications section to learn more about managing built-in or user-defined specifications.

You can also expand the All Nets list at the bottom of the dialog to select and assign specification(s) to individual nets in the design.

After clicking OK in the dialog, selected classes will be shown in the SI Analyzer by Keysight document. If a net was selected in the All Nets region of the Manage Nets dialog, it will be shown in the All Nets class entry. Expand a class entry to see its nets/xSignals.

Expand an entry for a net/xSignal or differential pair to see its constituent objects (pads, tracks, arcs and vias) in the Transmission Line region. Hover the cursor over an object's tile and click the  icon to cross-probe to this object in the PCB.

To remove a class or an individually added net from the document, click the  button at the right of its entry.

Managing Specifications

The Manage Specifications dialog, accessed by clicking the Manage Specifications button at the top of the SI Analyzer by Keysight document, allows you to manage both built-in and user-defined specifications. Specifications can then be assigned to a class or net to quickly define constraints for it as described in the previous section.

• The left-hand side of the dialog presents the list of currently defined specifications. Each specification is listed in terms of its name and one or more types of constraints it defines.

  Use the Search field at the top of the specification list to find the required specifications. As you type your search string, the list will be filtered to present only the specifications with relevant names.
• Select a specification in the list to display its details (name, whether it is a Built-In or User-Defined specification, and constraints) on the right-hand side of the dialog.
• To create a new specification, click the Add New button at the bottom-left of the specification list. The right-hand side of the dialog will be presented with controls to define the specification:

  • Define the name of the new constraint using the Specification Name field.

  • Select constraint type(s) you would like this specification to define using checkboxes: Impedance, Delay, Insertion Losses (IL), and/or Return Losses (RL).

  • For enabled constraint types, define their constraint values. For constraints of the Impedance and Delay types, use the text fields provided. For constraints of the Insertion Losses (IL) and Return Losses (RL) types, you can add, edit, and remove bounds to form an area of restricted and allowed loss values in the required frequency range.

    

  • Once the specification is defined as required, click the Save button at the top of the right-hand side of the dialog to create it, or click Cancel to quit without creating.

    Note that it is not possible to create a new specification with a name already used or with invalid constraint values in enabled constraints.
• A new specification can also be created by duplicating an existing one (either user-defined or built-in). Select a specification to be duplicated in the list and then click the Duplicate button at the bottom-left of the specification list. A new specification initially named <OriginalSpecificationName>(Copy) and with the same constraints as the original one will be created and ready for editing on the right-hand side of the dialog. Make changes as required and click the Save button at the top to create the specification or click Cancel to quit without creating.
• To edit a user-defined specification, click the  button on the right-hand side of the dialog when the specification is selected in the list. Make changes as required and click the Save button at the top to save the changes or click Cancel to quit without applying any changes.
• To remove a specification (either user-defined or built-in), click the  button on the right-hand side of the dialog when the specification is selected in the list.
• Removed built-in specifications can be restored by right-clicking in the specification list and selecting the Restore Built-In Spec command. Used-defined specifications will not be affected by this command.

Defining Constraints

Each net will be analyzed to determine if it is sufficient against the specified constraints. If a specification has been selected for the parent class, constraints are defined by this specification.

To explore the current constraints of a net/xSignal or differential pair, select the Constraints tab when its entry is expanded.

Click a constraint value to edit this constraint in the pop-up that appears.

Note that if a constraint value has been changed manually, the Custom constraints are used warning message will be shown in the corresponding entry.

Running an Analysis

With the configuration complete, you can run an analysis for all added nets, a specific class, or a specific net. Click the Analyze All button at the top-right of the SI Analyzer by Keysight document to analyze all nets or the Analyze button for an entry of a specific class or net to analyze only this class/net.

Exploring the Results

Once the analysis is finished, its results are presented in the SI Analyzer by Keysight document. The Analyzed message will be shown at the top-right of the document. If all analyzed nets suffice the constraints, the All Passed text will be shown next to the message. Otherwise, the Failed text will be shown, with the number of the nets that do not meet the constraints.

If all nets in a class pass the analysis, the Success text will be shown for its entry. Otherwise, the Failed text will be shown.

Expand a class entry to see the calculated values (impedance, delay, insertion losses, and return losses) for each analyzed net in that class. Values that meet the constraints are shown in green; values that do not meet the constraints are shown in red.

Expand a net entry to see the calculated values for this net on the Results tab. Also, tiles of net objects that do not meet the constraints have a red border in the Transmission Line region, and the failed value is shown in red.

To see the analysis results for a class or net/xSignal/differential pair within the PCB, click the associated Show on PCB button.

The SI Analyzer by Keysight Panel

In the PCB editor, the analysis process and results are controlled through the SI Analyzer by Keysight panel. Note that the panel is added to the list of available panels (via the Panels button) after a signal integrity analysis has been performed and the  Show on PCB button has been clicked.

Simulated Signal

• Simulated Signal – use to select the class or net/xSignal/differential pair you want to be displayed as a heatmap in the design space.
• Only nets with violations – when this option is on, only entities that currently have a violation are available in the drop-down. Clear this option to list all analyzed entities.
• Show Heatmap – when this option is on, a heatmap is displayed in the design space for the entity currently selected in the Simulated Signal drop-down.

Below these controls, the panel has two tabs, General and Heatmap. The options in these tabs apply to the entity currently selected in the Simulated Signal drop-down.

Heatmap

The Heatmap tab on the SI Analyzer by Keysight panel is used to control what data is presented as a heatmap, either the impedance or delay, and how color is applied to the impedance/delay. Note that these heatmap setting controls are only available when the Show Heatmap option is enabled.

Use the Impedance and Delay buttons to switch between two modes. The entire net is colored to reflect the impedance/delay at every location along the net as follows:

• For impedance, the closer the impedance to the Z0 target, the greener the color, and the further the impedance from the Z0 target, the redder the color. Calculated values below the minimum and above the maximum are displayed in red. 
• For delay, the larger the delay, the hotter (redder) the color, and the smaller the delay, the colder the color. Calculated values below the minimum are displayed in blue, and values above the maximum are displayed in red.

The colored scale reflects how the color is applied. The min and max values can be adjusted by clicking and dragging on the slider, or by entering a new value in the fields below. The scale is also displayed as a colored bar in the design space, below the PCB.

Enable the Color focus on results option to highlight the entity currently selected in the Simulated Signal drop-down and filter out other objects in the PCB.

An example of a heatmap shown for impedance calculations.

An example of a heatmap shown for delay calculations.

Violation Detection

If the analysis detects a constraint violation for the entity currently selected in the Simulated Signal drop-down, they are listed in the Violations region of the General tab of the SI Analyzer by Keysight panel.

• Use the buttons at the top of the region to define which violation types should be displayed in the list.
• Use the Analyze button at the bottom of the region to rerun the SI analysis. This can be used to quickly check if the entity suffices the constraint after changes are applied in the PCB editor, without returning to the SI Analyzer by Keysight document.

Probes

The Probes region of the SI Analyzer by Keysight panel is used to place measurement probes directly on the PCB. Probes can either measure impedance or delay, the type of measurement is determined by the current heatmap mode of the board.

Probes can either be a single probe, to measure an absolute value at the probe site, or a difference probe, to measure the difference between the two probe sites. Both types of probes are placed by clicking the Add button in the Probes region of the panel. To place a single probe, click at the required location then right-mouse click (or press Esc). To place a difference probe, click once to define the first probe site, then click a second time to define the second probe site. Once a probe has been defined, the measurement results will be displayed in the panel.

An example of a single probe

An example of a difference probe

Click a probe entry in the panel to show its location(s) on the PCB. Select a probe entry in the panel and click the  button at the bottom of the region to remove the probe.

Click the Add to Report button to create an image of the PCB at the selected probe location. The image will display in the Image Captures region of the panel, identified by a Probe badge. Hover the cursor over the screenshot to display the probe details.

Image Captures

The image capture functionality in the SI Analyzer by Keysight panel can be used to capture a design-specific screenshot, which can then be included in a report.

To take a picture of a specific area of the board, first, arrange the view of the board in the design space so that the elements you want to be included in the capture are visible. Once ready, click the Add button in the Image Captures region of the panel to capture the screenshot. You can continue to change your view of the board and add more images.

 To delete an image, hover the cursor over the image to reveal the  button, then click it to delete.

Reporting the Results

To generate a full analysis report, click the Full Report button at the top of the SI Analyzer by Keysight document. The full report includes a section for each class (and the All Nets entry for individually added nets outside of net classes).

Within the full report, click a net class name (or the net name in the All Nets list) to see a detailed report for it, including:

• Name of the net class or net.
• Assigned specification(s).
• Constraint check summary. Click a failed check entry to see recommendations for fixing related issues.
• Layer Stackup for the board.
• Constraint checks for each net. Expand a net entry to see constraint checks for each object of this net.
• Insertion losses chart.
• Return losses chart.

When exploring a detailed report, click the Show on PCB button to open the PCB and the SI Analyzer by Keysight panel to explore the class/net.

Working with Charts

The insertion losses and return losses charts show the corresponding waveforms for each net in the class being explored. The red area on the chart indicates the restricted zone defined by the constraints.

• Use the drop-down at the top-right of the insertion losses or return losses chart to manage the nets shown in the chart. All nets, failed nets, or specific net(s) can be shown.

• Click a waveform name at the right of the chart to highlight it by dimming other waveforms. Click a waveform name again to clear highlighting.

• Scroll the mouse wheel to zoom relative to the mouse pointer position on a chart. When the mouse pointer is on a chart axis, scroll the mouse to zoom relative to the pointer position on this axis only (the scale of the other axis will not change).

• Data measurements can be taken by using measurement cursors. Two cursors are available, which can be added to the same or different waveforms on a chart. Right-click a waveform name at the right of the chart and use the Cursor A and Cursor B commands from the context menu to enable/disable the cursors. Move the cursor by clicking and dragging its tab. Measured data for an enabled cursor is shown at the bottom of the chart.

  
  An example of cursors A and B added to the same waveform.

Exporting the Report

Click the Save Report button to save the report in HTML format. Use the subsequent Report Settings dialog to configure which nets (when the dialog is accessed from the full report) and specific data will be included in the report.

After clicking the Generate Report button, the report is stored in a sub-folder in the project folder named \SiAnalyzerByKeysight_Output\HTMLReport\<ProjectName>.sik_<CurrentDate>_<CurrentTime>. All of the images in the report are stored in an \Images sub-folder.