SetupPreferences

Applied Parameters: Tab=PreferredWidths

Summary

This command is used to access the Favorite Interactive Routing Widths dialog, with which you can predefine your favorite track widths for use when interactively routing a board using the Interactive Router.

Access

This command is accessed from the PCB Editor by using the O keyboard shortcut then choosing the Favorite Routing Widths entry on the subsequent pop-up menu.

Use

After launching the command, the Favorite Interactive Routing Widths dialog will open. Use this dialog to configure a desired set of favorite routing widths, across metric and imperial measurement systems.

Tips

1. When you run the Interactive Routing command then click to start routing, a series of track objects are created from the nearest pad up to the current cursor location. The width of these tracks is either taken from your preferred width or the applicable routing width design rule. The former is referred to as User Choice and it is the Favorite Interactive Routing Widths dialog that provides the cornerstone of this feature.
2. When using the User Choice feature and predefined routing widths, you still have the full protection of the rules system. If a chosen predefined routing width is outside the applicable min-max rule setting, the width will be clipped back to the minimum or maximum, whichever is appropriate.
3. An incarnation of the Favorite Interactive Routing Widths dialog is accessed when wanting to change the current routing width to one of the predefined favorites. Press Shift+W while interactively routing to access the Choose Width dialog.

Applied Parameters: SingleLayerMode = Toggle

Summary

This command is used to cycle through the available single layer viewing modes. Viewing a single layer using one of these modes enables you to more easily see what you need on that layer without the clutter of other layers and their objects.

Access

This command is accessed from both PCB and PCB Library Editors by using the Shift+S keyboard shortcut.

Use

After launching the command, the next available single layer mode - in the following sequence of modes - will be employed in the design workspace, depending on the mode previously employed:

• Gray Scale Other Layers - displays the current layer; all primitives on other layers are displayed in gray. The shade of gray is based on a layer's color scheme.
• Monochrome Other Layers - displays the current layer; all primitives on other layers are displayed in the same shade of gray.
• Hide Other Layers - displays the current layer; all primitives on other layers are not displayed.
• Not In Single Layer Mode - displays all visible layers as normal.

Use the command repeatedly to cycle through the available modes.

Tips

1. The current single layer mode is reflected through the Single Layer Mode field in the General Settings region on the View Options tab of the View Configuration panel. Click the mode link (next to the On button) to access the PCB Editor - Board Insight Display page of the Preferences dialog from where you can configure the available single layer modes as required.

Applied Parameters: RoutingMode = Cycle

Summary

This command is used to cycle through the available routing conflict resolution modes while routing your board using the Interactive Router.

Access

While in an interactive routing mode (interactive routing, interactive differential pair routing, and interactive multi-routing), this command is accessed from the PCB Editor by using the Shift+R keyboard shortcut.

Use

After launching the command, the next available routing conflict resolution mode - in the following sequence of modes - will be employed in the design workspace, depending on the mode previously employed:

• Ignore Obstacles - enable this option to have the Interactive Router allow the track to pass through obstacles while routing.
• Walkaround Obstacles - enable this option to have the Interactive Router route around existing tracks, pads and vias while routing. If this mode cannot walkaround an obstacle without causing violation, an indicator appears to show the route is blocked.
• Push Obstacles - enable this option to have the Interactive Router move existing tracks out of the way while routing. This mode can also push vias to make way for the new routing. If this mode cannot push an obstacle without causing violation, an indicator appears to show the route is blocked.
• HugNPush Obstacles - enable this option to have the Interactive Router hug existing tracks, pads and vias as closely as possible while routing and, where necessary, push obstacles to continue the route. If this mode cannot hug or push an obstacle without causing violation, an indicator appears to show the route is blocked.
• Stop At First Obstacle - enable this option to have the Interactive Router stop routing when it encounters the first obstacle in its path.
• AutoRoute Current Layer - enable this option to have the Interactive Router autoroute to the current cursor location on the current layer.
• AutoRoute MultiLayer - enable this option to have the Interactive Router autoroute to the current cursor location across different layers. Vias will be placed as required to change to alternate signal layers.

Use the command repeatedly to cycle through the available modes.

Tips

1. The available modes are determined by enabling the corresponding options in the Routing Conflict Resolution region on the PCB Editor - Interactive Routing page of the Preferences dialog. The current routing conflict resolution mode is reflected (and can also be selected directly) through the Current Mode field located below these options
2. The current mode can also be changed on-the-fly from the Properties panel (accessed by pressing Tab while interactively routing). Use the Routing Mode drop-down field in the Interactive Routing Options section of the panel. Pressing Tab pauses routing, allowing you to interact with the panel (or other area of the software) directly. To resume, click the pause symbol that appears over the workspace or press Esc.

Applied Parameters: ShowDifferenceObjects=Toggle

Summary

This command is used to toggle the display of the Difference Map Overlay in the main design workspace On or Off. The overlay is used to display the resulting differences from performing a comparison through the Collaborate, Compare and Merge panel. This panel is command central for Altium Designer's collaborative PCB design features.

Access

This command can be accessed from the PCB Editor by:

• Choosing the View » Differences » Show/Hide Difference Overlay command from the main menus.
• Using the Shift+O keyboard shortcut.

Use

After launching the command, the difference map overlay will either be hidden, or displayed, depending on its previous state.