Parent page: PCB Panels
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:
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.
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.
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.
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)
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.
The following information is listed for each xSignal:
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.
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.
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_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.
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 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 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.