Managing xSignals using the PCB Panel in Altium Designer
xSignals mode of the PCB panel.
Summary
The PCB panel allows you to browse the current PCB design using a range of filter modes to determine which object types or design elements are listed, highlighted or selected. The panel also has editing modes for specific object types or design elements that provide dedicated controls for editing procedures. Note that you can access the properties for any element listed in the panel.
In the PCB panel’s xSignals mode, its three main list regions change to reflect the xSignal object hierarchy, in order from the top:
- xSignal Classes.
- Individual xSignal definition within a class.
- Individual primitives that constitute an xSignal (pads, tracks and vias).
Panel Access
When the PCB Editor is active, click the 
button at the bottom-right corner of the workspace and select PCB from the context menu. Alternatively, you can access the panel through the View » Workspace Panels » PCB » PCB sub-menu.
Once the PCB panel has been opened, select the xSignals option from the dropdown menu at the top of the PCB panel to enter xSignals mode.
Managing xSignals
xSignal Classes region
The xSignal Classes region lists any xSignal class collections that have been defined, or simply all available classes (<All xSignals>).
Select a class to see its xSignals list in the middle panel region (xSignals) and to display them in the PCB workspace.
Selecting an xSignal class will list its members in the panel's xSignals region and highlight them in the PCB workspace.
To create a new xSignal class from the existing xSignal collection, right-click in the region and select Add Class from the context menu. The Edit xSignal Class dialog lists the available xSignals which can be added or removed as members to the new class using the management buttons – use the Name field to define a suitable name for the new xSignal class.
Create or add to an xSignal class by adding/removing xSignal members via the Edit xSignal Class dialog.
The panel region’s right-click context menu also offers the ability to remove (Delete) or rename (Properties) an xSignal class, and change its visual representation in the PCB workspace (for example, Change xSignal Color)
xSignals region
The panel’s xSignals region lists all defined xSignals for the design, and their individual details such as signal/routing lengths and number of nodes. Note that multiple xSignals can be selected using standard Shift and Ctrl –click techniques – the multiple selections are visually shown in the PCB workspace.
Defined xSignals can be selected and managed in the panel's xSignal region.
The following information is listed for each xSignal:
- Node Count - This value reflects the total number of defined nodes in that xSignal.
- Signal Length - The distance traveled using the new length calculation engine, which detects and excludes overlaps and wiggles inside pads. It also copes with routing paths that use objects other than tracks or acs (for example, a region or fill). Signal Length also includes: the vertical distance through vias (applicable layers), pin/package lengths (defined as a pad property), as well as the length of any section still to be routed. For the un-routed section, it uses the Manhattan Length.
- Total Pin/Package Length - Sum of all the Pin/Pkg length values in all pads in that net.
- Routed Length - The distance traveled if you follow the centerline of the objects, including overlaps or routing wiggles inside pads.
- Un-Routed (Manhattan) Length - This length is the vertical or horizontal X+Y distance from here to there.
Right-click and navigate through the Columns sub-menu control the column visibility.
The option to change an xSignal's color is also available from the right-click menu in this section by selecting Change xSignal Color to open the Choose Color dialog.
xSignal Primitives region
The PCB panel’s third region, xSignal Primitives, lists all the constituent elements (primitives) of the currently selected xSignal.
Select the region’s Show nodes only checkbox to restrict the primitives listing to pads that are the xSignal start/end point nodes. In this mode the selected xSignal will be shown in the PCB workspace as node pads joined by a thin trace (rather than tracks) that represents the xSignal path.
The lower xSignal Primitives region lists all elements of the selected xSignal, such as pads, vias and tracks.
Create xSignals in Nets mode
While xSignals are generally defined through the Create xSignals dialog (Design » xSignals » Create xSignals), they can also be defined manually using the PCB panel in Nets mode.
The below diagram shows two nets that form one half of a differential pair that couples a processor to a high-speed connector. As a high-speed connection, we want the two nets and series component defined as a one xSignal, so it can be used to scope design rules.
The two highlighted nets, LCD_DB0 and LCD_DB2, are joined by series component UI. When selected in the PCB panel in Nets mode, the two nets are highlighted in the PCB workspace, as shown.
The complete path for one side of a differential pair is two nets joined by a series component.
To create a suitable xSignal, select the source and destination pads in the panel’s Primitives region, right-click on the selection and choose Create xSignal from the context menu. Note that the source is a pad on U1 (the processor) and the destination pad is on RA3.
The source and destination pads (pin pairs) for the desired path are used for creating a singular xSignal definition.
The newly created xSignal will now be available in the PCB panel’s xSignals mode – its default name can be changed by selecting Properties from the right-click context menu. Note that xSignal path incorporates both nets and the series component as a single entity.
The created xSignal selected in the PCB panel and displayed in the workspace.
Panel mini-viewer
The bottom section of the PCB panel provides a mini-viewer for the current document, with an image of the PCB board central to its window. A white viewing box is imposed on the image to show the area currently displayed in the design editor window. As the editor display automatically pans and zooms in response to the PCB panel filter selections, the box moves and expands accordingly to indicate the board viewing area.
As you manually pan around the document in the design editor window - using the editor's horizontal and vertical scroll bars or the right-click panning hand - the viewing box in the panel will also move accordingly. Conversely, if you click inside the viewing box and drag it around the board image, the document in the design editor window will be panned accordingly, and at the current zoom level.
As you zoom in or out in the design editor window, the viewing box will be resized accordingly in the panel. Conversely, resizing the viewing box in the panel, by clicking and dragging on any of its vertices, will cause the zoom level to change in the design editor window. The smaller the size of the viewing box, the more the actual document has been zoomed-in.