Edit Net

Modified by Jason Howie on Feb 13, 2015
Contents
Other Related Resources
Netlist Manager (Dialog)
PCB Editor - Interactive Routing (Preferences)
Favorite Interactive Routing Widths (Dialog)
Favorite Interactive Via Sizes (Dialog)
Interactive Routing (Dialog)
Interactive Routing

Parent page: PCB Dialogs

The Edit Net dialog.

Summary

This dialog allows the designer to browse the properties of the focused net, manage which pins (pads) of components in the design are part of the net, and also change the preferred routing widths and via sizes, for use when interactively routing the net.

Access

The dialog is accessed through the PCB Editor in the following ways:

  • Double-clicking on the net of interest, in the Nets region of the PCB panel (when configured in Nets mode).
  • In the design workspace, right-clicking over an object in the net of interest, and choosing Net Actions » Properties, from the context menu.
  • Double-clicking on the net of interest (or selecting the net and clicking the Edit button) in the Netlist Manager dialog.
The Netlist Manager dialog is accessed using the Tools | Netlist |  » Edit Nets command, from the main menus.

Options/Controls

Properties

  • Net Name - the current name for the net. This can be changed as required.
  • Connection Color - the current color used for the (unrouted) connection lines associated to this net. By default, all new nets are colored the same, with the color specified in the Default Color for New Nets field, on the Board Layers And Colors tab of the View Configurations dialog. Click the color sample to change the color as required, using the standard Choose Color dialog.
The chosen net color is reflected in the far left field for the net's entry, in the Nets region of the PCB panel. This field also presents a checkbox, which is used to enable the color-override feature for that net. This feature allows you to highlight the net (it's associated design objects) using the color assigned to the net itself, rather than simply using the associated layer coloring. The assigned net color is displayed using small squares, leaving the default layer color also visible, in a 'checkerboard' fashion. As the board is zoomed further out in the workspace, the net's connection color becomes more dominant, until the layer color is not noticeable.
As well as setting the connection line color for individual nets, you can also display the connection lines using the colors of the start and end layers that the connection line travels between. These connection lines are displayed as dashed lines, using the colors of both the start and end layers. This feature is ideal when you are routing a multi-layer board, as you can easily tell the target layer that connection being routed must get to. Note that this dashed color override is only applied to nets that travel from one layer to another, if the connection starts and ends on the same layer it retains its defined color. To use the color-by-layer feature, enable the Use Layer Colors for Connection Drawing option on the View Options tab of the View Configurations dialog.
  • Hide Connections - enable this option to hide all connection lines for the net.
  • Hide Jumpers - enable this option to hide all jumpers displayed for components whose jumpered pins are members of this net.
  • Remove Loops - this option controls whether redundant loop segments of routed track (and associated redundant vias), for this net, are removed when re-routing to modify existing route paths. Disable this option to exclude the net from automatic loop removal.
Automatic loop removal is controlled globally using the Automatically Remove Loops option, on the PCB Editor - Interactive Routing page of the Preferences dialog.

Pin Management

The controls in this region of the dialog allow the designer to manage the pins (component pads) belonging to this net:

  • Pins in Other Nets - this is a listing of all component pins (pads) that are not currently part of this net.
  • Pins in This Net - this is a listing of all component pins (pads) that are currently part of this net.
  •  (Add All) - click this button to quickly transfer all pins from the Pins in Other Nets list, over to the Pins in This Net list.
  •  (Add Selected) - click this button to quickly transfer those pins currently selected in the Pins in Other Nets list, over to the Pins in This Net list.
  •  (Remove Selected) - click this button to quickly transfer those pins currently selected in the Pins in This Net list, over to the Pins in Other Nets list.
  •  (Remove All) - click this button to quickly transfer all pins from the Pins in This Net list, over to the Pins in Other Nets list.
Multiple pins can be selected for transfer between lists using standard multi-select techniques (Ctrl+click and Shift+click).

Current Interactive Routing Settings

This region of the dialog gets loaded with information when:

  • The designer selects a predefined favorite track width and/or via sizing, when interactively routing the net. Choice is made using the Choose Width dialog (Shift+W) or Choose Via Size dialog (Shift+V) respectively. The predefined widths and sizes themselves are configured in the Favorite Interactive Routing Widths, and Favorite Interactive Via Sizes dialogs, respectively.
  • The designer sets a specific track width and/or via sizing on-the-fly, while interactively routing the net (pressing Tab to access the Interactive Routing dialog).

The designer also has the ability to change settings directly here in the dialog.

Selecting a predefined favorite track width and/or via sizing while interactively routing, or specifying a value on-the-fly while routing, is referred to as User Choice. It allows the designer to be more agile with their routing, while remaining within the boundaries of the applicable routing rules.
Whatever values are loaded/set in the dialog, you still have the full protection of the rules system. If a chosen/specified routing width and/or routing via size is outside the applicable min-max rule setting, the width and/or hole size and/or diameter will be clipped back to the minimum or maximum, whichever is appropriate.
  • Track Widths - this is a list of the available routing (signal) layers for the board, and the current track width used when routing the net on a layer. When the User Choice feature is used, and the designer chooses a favorite routing track width (Shift+W while interactively routing), that width will be loaded here. The same is true for a value specified on-the-fly while routing. If the designer chose to apply that width to all layers, then the value will be loaded into this field for all layers. If not, only the entry for the layer on which the routing was being performed, will get loaded with the value.
There are two different layer references - the Layer Stack Reference, which lists the layers in terms of their position within the layer stack, and the Absolute Layer reference, which lists the layers according to their order in the system.

The track width for each layer can be modified directly, adjusting whatever has been previously loaded.

When setting values directly in the dialog, for use when continuing routing, ensure the option to Pickup Track Width From Existing Routes is disabled (on the PCB Editor - Interactive Routing tab of the Preferences dialog). If this is not done, the dialog will simply be reloaded with the value for track width from an existing route.
  • Via Hole Size - the current via hole size used, when dropping a via while routing this net. When the User Choice feature is used, and the designer chooses a favorite routing via size (Shift+V while interactively routing), the hole size portion of that choice will be loaded here. The same is true for a value specified on-the-fly while routing. The hole size can be modified directly, adjusting whatever has been previously loaded.
  • Via Diameter - the current via diameter used, when dropping a via while routing this net. When the User Choice feature is used, and the designer chooses a favorite routing via size (Shift+V while interactively routing), the diameter portion of that choice will be loaded here. The same is true for a value specified on-the-fly while routing. The diameter can be modified directly, adjusting whatever has been previously loaded.
  • All Widths - if the User Choice feature is used, and the designer chose to apply a predefined favorite/on-the-fly routing track width to all layers, then the chosen/specified value will be loaded into this field. If the chosen/specified value was intended for the active routing layer only, then an entry of zero will appear in this field (and all Track Width fields for the other layers).
  • Layers in Layer-Stack only - enable this option to have User Choice values loaded for layers in the layer stack only.

 

You are reporting an issue with the following selected text and/or image within the active document: