Parent page: System & Environment Panels
The Navigator panel allows you to browse either the compiled active source document or all compiled source documents in the active project. The source document(s) can be schematic and/or HDL in nature. The panel utilizes the connective model of the design, created upon compilation, as its foundation for navigation. The panel can also be used as a means to browse components, nets and pads on a compiled/analyzed PCB document.
The Navigator panel is accessed in the following ways:
When browsing source documents for a project (i.e., schematics and/or VHDL files), click the Interactive Navigation button at the top of the panel to enter interactive navigation mode. This mode allows you to spatially navigate the design directly on the document(s). All source documents in the active project are compiled and the cursor changes to a cross-hair ready for navigation. The cursor will remain in navigation mode until you right-click or press the Esc key. This gives you a spatial alternative to the logical list presented in the panel itself.
As you navigate a design document, the Navigator panel will update with the information relative to your selection in the design editor window. Located on either side of the Interactive Navigation button are direction arrows for browsing back and forth through the browse path (providing a simple history of your recent browsing).
To the right of the Interactive Navigation button is the Interactive Navigation Options button ( ). Click this button to open the System - Navigation page of the Preferences dialog, which provides options for controlling which objects are highlighted and the highlight methods to be used.
The Highlight Methods region provides the following four options that control the visual result of temporary filtering that is applied to the document, when navigation is performed from both the panel and within the document itself:
Any combination of these options can be enabled. For example, you might want to have all filtered objects zoomed, centered and selected in the design editor window, whilst applying masking to take away the clutter of other design objects.
The Objects To Display region allows you greater control over which objects are included in the Navigator panel. Enable an option for an object type; if objects of that type exist in the active design, they will be included in the information available in the panel.
Depending on whether you have chosen to compile/analyze the active document or compile the entire hierarchy of source documents in the active project, the first list section in the panel will contain either:
In the last case, three views of the compiled design are available - individual compiled sheets, a flattened hierarchy and a full design hierarchy, as shown in the image below.
For each schematic sheet entry in the full design hierarchy, the Sheet Name and File Name are listed - the former appearing as a tab at the bottom of the design editor window, the latter appearing as the main tab at the top of the design window.
Clicking on the entry for an individual document will populate the lower sections of the panel with component Instance and Net/Bus information local to that document and where such information exists. Selecting the Flattened Hierarchy entry will allow you to peruse all design objects across the entire compiled model of the design.
Notice that it is not just the bottom section that updates when you click on an object. Each section of the panel will jump to the corresponding item in its list when a navigated object pertains specifically to it. The workspace will also update. As you click on an object in the Navigator panel, filtering will be applied, the visual result of which is controlled by a number of Highlight Methods specified on the System - Navigation page of the Preferences dialog.
The following sections provide detailed information on the use of the Navigator panel and the different objects that may be browsed. The first four sections concentrate on use of the panel from the perspective of browsing a schematic source document. For information relating specifically to navigation when the browsed document is a VHDL file or target PCB, see the Browsing a VHDL Source Document and Browsing a PCB Document sections below.
The second list section in the Navigator panel contains all of the instances of components that exist for the selected document entry in the first section. As you select a top-level component instance entry in the list, a filter will be applied based on that entry, the visual result of which is determined by the highlighting methods chosen. If you have enabled the Connective Graph option on the System - Navigation page of the Preferences dialog, all other components that are connected to the component you have selected will be visible (the filter having been extended to include them). The connected components are visually highlighted by the green graph connection lines.
For each component entry, sub-folders containing additional information for defined parameters and linked models (Implementations) are available. If the Pins option is enabled in the Objects To Highlight region of the System - Navigation page of the Preferences dialog, a Pins sub-folder will also be available.
As you click on a pin entry in the Component Instance list, the corresponding entry for that pin will become selected in the Net/Bus section of the panel and all pins for that parent net will be listed in the bottom section of the panel. A filter also will be applied based on the pin entry you have chosen, the visual result of which is, again, determined by the highlighting methods chosen on the System - Navigation page of the Preferences dialog (Zooming, Selecting, Masking).
If you have enabled the Connective Graph option, all other pins that are connected to the parent net of the pin you have selected will be visible (the filter having been extended to include them). The parent net for the connected pins is visually highlighted by the use of red graph connection lines, as shown in the image below.
The third section of the panel lists each of the nets and buses used in the document (or flattened hierarchy) being browsed. As you click on an entry, all objects associated to the net/bus - Pins, Net Labels, Ports, Sheet Entries and Cross-Sheet Connectors - will be displayed in the design editor window in accordance with the highlighting methods enabled.
The various object types associated to a net are listed in sub-folders. The display/inclusion of each folder in the panel is dependent upon whether the corresponding option for each has been enabled in the Objects To Highlight region of the System - Navigation page of the Preferences dialog, which can be directly accessed via the Interactive Navigation button () at the top of the Navigator panel.
For each net/bus, a further sub-folder can be included which lists any graphical lines used to connect associated pins/ports/net labels/sheet entries/cross-sheet connectors. Click on a line entry to filter just that line object and apply the visual control settings.
All net objects that have been enabled for display in the panel (with the exception of graphical lines) will be summarily displayed in the bottom section of the panel, as shown below. Again, clicking on any of these will apply filtering in accordance with the highlighting methods chosen.
Note that the contents of the final section of the panel depends upon two things: the object you are navigating and the objects you have set for display. The master list of objects you want displayed can be accessed in the System - Navigator page of the Preferences dialog associated with the panel's Interactive Navigation button, however you also can right-click in the Navigator panel and enable or disable them individually through the Show submenu.
If the document being browsed is a schematic, enabling the Show Signals option at the top left of the panel causes the third list section of the panel to change to show all signals for that document. Click on a signal entry to apply a filter and the nodes for that signal (pins/ports/net labels/sheet entries/cross-sheet connectors) will be displayed in the design editor window, in accordance with the highlighting methods enabled.
For each signal in the list, the node pins, sheet entries or cross-sheet connectors associated with that signal will be listed. These entries will be displayed, regardless of whether the corresponding display option for that object type has been enabled or not.
If a node pin associated with a signal is an output pin or an IO pin, then it is driving the signal and the corresponding entry in the list will be of the format:
If a node pin associated with a signal is an input pin, then it is being driven by the signal and the corresponding entry in the list will be of the format:
Similarly, if the electrical type of a sheet entry node is output or IO, the entry is driving the signal and the entry will appear in the form:
If the electrical type of the sheet entry is Input, then the entry is being driven by the signal and the format of the entry will be:
Click on a top-level signal entry to populate the bottom section of the panel with all signal nodes associated with that signal. These can include Pins, Net Labels, Ports, Sheet Entries, and Cross-Sheet Connectors. Entries will only be displayed if the corresponding option to display that object type has been enabled.
Click on a sub-entry in the main signals list to populate the bottom section of the panel with all net objects associated with the parent net for that signal.
For hierarchical compiled designs, each sheet symbol can also be browsed (if enabled for display in the panel) and information viewed with respect to associated sheet entries and any defined parameters.
Clicking on the entry for a sheet symbol will again apply filtering in the design editor window in accordance with the defined visual controls. All sheet entries for the symbol will appear summarized in the bottom section of the panel.
Click on a sheet entry for a symbol in the main Instances list to populate the bottom section of the panel with all net objects associated with the parent net for that symbol.
When the selected document to be browsed is a VHDL file, the panel will initially become populated as shown in the following image where:
As you click on a top-level entry in the Net/Bus section, the corresponding port declaration will be displayed within the VHDL code of the document in the design editor window in accordance with the highlighting methods enabled. Note that when browsing VHDL files, only the Selecting, Zooming and Masking highlighting methods are applicable.
All net objects associated with the chosen net/bus that have been enabled for display in the panel (with the exception of graphical lines) will be summarily displayed in the bottom section of the panel, as illustrated in the image below. Again, clicking on any of these will navigate to the object on the relevant source document in the design editor window and with filtering applied in accordance with the highlighting methods chosen.
When the selected document to be browsed is a PCB, the panel will initially become populated as shown in the following image:
The Interactive Navigation feature is not available when specifically browsing a PCB document. As such, the options for object display in the panel, as well as visual highlighting controls cannot be accessed from the associated Options button (). However, the navigation options can be enabled/disabled from the right-click menu.
Note that only Pins and Net Labels can be included for display when browsing a PCB document.
Clicking on the PCB document entry in the top list of the panel, with the Select Objects option enabled will effectively select all components in the design, as shown above in the panel.
As you select a top-level Component entry in the Instance section of the panel, a filter will be applied based on that entry, the visual result of which is determined by the highlighting methods chosen. All pins for that component will be listed in the bottom (fourth) section of the panel with the heading of Component Pins.
For each component entry, a sub-folder containing additional information for defined parameters is available, as well as an entry for the footprint used to represent that component on the PCB. If the Show » Pins option is selected from the right-click menu, then a Pins sub-folder will also be available.
As you click on a pin entry in the Component Instance list, the corresponding entry for that pin will become selected in the Net/Bus section of the panel. A filter will also be applied based on the pin entry you have chosen, with the corresponding pad highlighted on the PCB document in the design editor window, the visual result of which is again determined by the highlighting methods chosen (Zoom, Mask, and Select).
As you click on a top-level entry in the Net/Bus section of the panel, all objects associated to that net/bus - e.g., pads, vias, tracks - will be highlighted in the design editor window, in accordance with the highlighting methods chosen. Note that when browsing a PCB document by nets, the Select Objects option has option has no effect.
Note that Pin and Net Label information for a selected net entry is listed under sub-folders, the inclusion in the panel of which is determined by whether the respective Show » Pins and Show » Net Labels options are enabled on the right-click menu. The full listing of pins and net label for the selected net is displayed in the bottom section of the panel (Net Pins). Clicking on a pin entry in either section will display the corresponding pad for the design in the design editor window, in accordance with the visual highlighting controls enabled.
The right-click menu for the panel provides the following commands:
If a list contains multiple entries starting with the same letter, narrow your search by typing additional letters as required. To clear the current filtering to allow you to filter using a different starting letter, press Esc. Use the Backspace key to clear the previously entered filter characters.
Note: The filtered entry will appear selected but in order to navigate to the object on the associated document, you will need to either click on the entry or press Enter. Additionally, the filtering feature will not find object entries listed in sub-folders unless the parent (top-level) entry is expanded to reveal those sub-folders and those sub-folders are expanded to reveal their object entries.
Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.