Browsing a Design using the Navigator Panel in Altium Designer

The Navigator panel showing results for a specific schematic document.

Summary

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.

Panel Access

The Navigator panel is accessed in the following ways:

• Click View » Workspace Panels » Design Compiler » Navigator from the main menus.
• Click Design Compiler at the bottom-right of the editor then select Navigator from the pop-up menu.

Interactive Navigation

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. 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.

Highlight Methods

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:

• Zooming - when enabled, the filtered objects will be zoomed and centered (where possible) in the design editor window. The zoom level - the extent of zooming applied when navigating from either the panel or interactively within the design document - can be controlled using the Zoom Precision slider bar. A greater zoom level is achieved by moving the slider to the right. (The zoom facility has no effect when the target object is a port and resides in a VHDL file).
• Selecting - when enabled, the filtered objects will be selected in the workspace.
• Masking - when enabled, filtered objects will appear fully visible in the design editor window, with all other objects becoming dimmed. Control over the contrast between filtered and masked objects is provided using the Mask Level button at the bottom right of the workspace.
• Connective Graph - enabling this option displays the connective relationship between objects (on the active document in the design editor window). The visual connections will be green when navigating by components and red when navigating by nets. Enable the Include Power Parts sub-option if you wish to also graph the connectivity of power objects.

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.

Panel Sections

Documents Section

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:

• A single source document (schematic or VHDL).
• A single target PCB document.
• All source documents in the project.

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.

Components Section

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 Preferences dialog, 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 and all pins for that parent net will be listed in the bottom section of the panel. A filter will also 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.

Nets and Buses Section

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 Options 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 options button, however you also can right-click in the Navigator panel and enable or disable them individually through the Show submenu.

Signal Section

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:

• SignalName Driven By Pin X - where X represents the component-pin designator.

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:

• Driving Node Pin X - where again, X represents the component-pin designator.

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:

• Driven By Node Sheet Entry SignalName

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:

• Driving Node Sheet Entry X - where X represents the sheet symbol-sheet entry name.

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.

Clicking on a sub-entry in the main signals list will populate the bottom section of the panel with all net objects associated with the parent net for that signal.

Sheet Symbols

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.

Browsing a VHDL Source Document

When the selected document to be browsed is a VHDL file, the panel will initially become populated as shown in the following image, where:

• The second list section of the panel - normally populated with component instances - will be empty.
• The third list section of the panel will contain the associated nets and buses for the design.
• The bottom section of the panel will contain all ports that are declared in the entity section of the VHDL file.

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.

Browsing a PCB Document

When the selected document to be browsed is a PCB, the panel will initially become populated as shown in the following image:

• the second list section of the panel will contain all component instances within the PCB design.
• the third list section of the panel will contain the associated nets and buses for the design.
• the bottom section of the panel will initially be empty.

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.

Right-click Menu

The right-click menu for the panel provides the following commands:

• Compile All - compile all source documents for the active project.
• Analyze - compile the active document only.
• Jump to xx - sensitive to the object entry under the cursor when the right-click menu is accessed. Will jump to the object on the relevant document in the design editor window, following the defined highlight methods.
• Show Graph - toggles the Connective Graph highlight option On or Off when browsing schematic documents. When enabled, a tick symbol will appear to the left of the menu entry. The corresponding option in the Highlight Methods region of the Interactive Navigation options pop-up will be updated accordingly.
• Zoom on Objects - toggles the Zooming highlight option On or Off.  The corresponding checkbox in the Highlight Methods region of the Interactive Navigation options pop-up will be updated accordingly.
• Mask Objects - toggles the Masking highlight option On or Off.  The corresponding checkbox in the Highlight Methods region of the Interactive Navigation options pop-up will be updated accordingly.
• Select Objects - toggles the Selecting highlight option On or Off. The corresponding option in the Highlight Methods region of the Interactive Navigation options pop-up will be updated accordingly.
• Report - generate a report in context with the section of the panel the menu is accessed from. After launching the command, the Report Preview dialog will appear from where you can peruse, print and export the report in various file formats.
• Port Cross References - provides commands for adding or removing port cross reference information for the current schematic document or all schematic documents in the active project. Choices available for port cross references include:
  • Add To Current Sheet 
  • Add To Entire Project 
  • Remove From Current Sheet 
  • Remove From Entire Project 
• Show - provides commands for toggling the display of objects in the panel. Objects available on the sub-menu are: Net Labels, Pins, Sheet Entries, Ports, Sheet Symbols, and Cross-Sheet connectors. The corresponding checkbox in the Objects To Highlight region of the System - Navigation page of the Preferences dialog will be updated accordingly.

Tips

• The document(s) must be compiled before the panel can be effectively used. The Interactive Navigation feature allows you to navigate the entire set of source documents in the active PCB or FPGA project. As such, clicking the Interactive Navigation button will compile all source documents in the active project and cannot be used to compile and navigate just the active document. To use the panel to browse the connective model for a single source document only, right-click on the document's entry in the panel and choose the Analyze command.
• The Signals list will not be available if Flattened Hierarchy has been chosen in the top section of the panel.
• The Highlight Methods, Zoom Precision, Objects To Display, and Cross Select Zoom Options can be defined on the System - Navigation page of the Preferences dialog (DXP » Preferences).

• When the Connective Graph option is enabled and you are browsing net objects on a schematic sheet, a solid red line in the design editor window indicates a physical connection between net objects. A dotted red line indicates a logical connection between objects in the net.
• When navigating a compiled FPGA project, interface ports - those ports that represent connection to the physical pins of an FPGA device - will be listed under a separate Interface Ports sub-folder in the Net/Bus section of the panel. Their inclusion in the panel is dependent upon the Ports option being enabled in the Objects To Display region.
• The keyboard shortcuts Up Arrow, Home, End, and Down Arrow can be used to display the previous, first, last, and next entry in a list section of the panel, respectively. Use the Right Arrow and Left Arrow keys to expand and collapse a top-level entry or sub-folder.
• In sections of the panel where multiple columns of data exist, the data may be sorted by any column by clicking on the header for that column. Clicking once will sort in ascending order. Click again to sort in descending order.
• You can change the order in which columns of data are displayed. To move a column, click on its header and drag it horizontally to the required position. A valid position is indicated by the appearance of two green positional arrows.
• Direct filtering is available for all list regions in the panel, allowing you to quickly jump to an entry by directly typing within the area of the list. Masking is not applied, leaving the full content of the list visible at all times. To use this feature, click within the relevant list section of the panel and type the first letter of the object/entry you wish to jump to. The first entry in the list starting with the letter you type will become selected and the letter will be highlighted to show that filtering of the list is based upon it, as illustrated below:

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.

Filtering

• The filtering applied when browsing design objects on a schematic sheet using the Navigator panel or Interactive Navigation feature is temporary. Clicking inside the design editor window will clear the filter, therefore, you are not prevented from selecting or editing design objects that fall outside the scope of the filter when the Masking option is enabled on the System - Navigation page of the Preferences dialog. If the Masking option has been enabled, the extent of masking can be manually adjusted using the Dim slider bar, accessed by clicking the Mask Level button to the immediate left of the Clear button at the bottom-right of the design editor window.
• The filtering applied when browsing ports in a VHDL file using the Navigator panel is permanent. If the Masking option has been enabled on the System - Navigation page of the Preferences dialog, all objects not falling under the scope of the filter will become faded in the workspace and are not available for selection or editing. Clicking inside the design editor window will not clear the filter. A permanent filter must be cleared by clicking on a corresponding Clear button (e.g., at the bottom-right of the design editor window). If the Masking option has been enabled, the extent of masking can be manually adjusted using the masking controls, accessed by clicking the Mask Level button to the immediate left of the Clear button at the bottom-right of the design editor window.
• The filtering applied when browsing components, nets, and pads on a PCB document using the Navigator panel is permanent. If the Masking option has been enabled on the System - Navigation page of the Preferences dialog, all objects not falling under the scope of the filter will become faded in the workspace and are not available for selection or editing. Clicking inside the design editor window will not clear the filter. A permanent filter must be cleared by clicking on a corresponding Clear button (e.g., at the bottom-right of the design editor window). If the Masking option has been enabled, the extent of masking can be manually adjusted using the masking controls, accessed by clicking the Mask Level button to the immediate left of the Clear button at the bottom-right of the design editor window.