PCB_Cmd-AdvancedRouteAdvancedRoute_AD

Applied Parameters: None

Summary

This command is used to interactively route the connections on your board. Routing is the process of connecting the nodes in each net by placing a series of track segments and vias to define a path from one node to the next. Altium Designer includes a sophisticated interactive routing engine, that greatly enhances the designer's routing efficiency. Capabilities include:

• A number of routing modes, such as: stop at first obstacle, walkaround, and push and shove.
• Powerful dragging capabilities that maintains track angles and orthogonality.
• A loop removal feature that makes re-routing a quick and easy process.

The Interactive Routing tools help maximize routing efficiency and flexibility in an intuitive way, including following cursor path for laying route sections, single-click routing completion, pushing or walking around obstacles, and automatically following existing connections, all in accordance with applicable design rules.

Access

This command can be accessed from the PCB Editor by:

• Choosing the Route » Interactive Routing command, from the main menus.
• Locating and using the Interactive Routing command () on the Active Bar.

• Using the Ctrl+W keyboard shortcut.
• Choosing the Place » Track command from the main menus.
• Clicking the  button on the Wiring toolbar.
• Right-clicking in the workspace and choosing the Interactive Routing command from the context menu.
• Right-clicking in the workspace and choosing the Place » Track command from the context menu.

Use

After launching the command, the cursor will change to a cross-hair, and you will enter Interactive Routing mode. Click on a pad to begin routing from. Once you have clicked on the start location for the route, the current mode is shown on the Status Bar or in the Heads Up Display (HUD), if it is enabled. To place a track, move the cursor to where you want the current section of track segments to end and click or press Enter - the track will be placed up to the current cursor position. Using your cursor path as a guidance system for the route provides you with high degrees of flexibility in controlling the path that the routing will take, with the minimum number of actions required to commit the route.

When you start interactive routing, the PCB Editor will not only let you start placing track objects, it will:

• Monitor cursor position and mouse-clicks, applying all applicable design rules.
• Follow your cursor path, minimizing the number of actions required to place sections of routing.
• Monitor the connectivity and update connection lines as soon as you finish a route.
• Supports routing-specific shortcuts, for example pressing the * key on the numeric keypad to push to the next signal layer, inserting a via in accordance with the routing via style design rule.

As you route the net, the standard conflict resolutions modes are available, including Walkaround Obstacles, Push Obstacles, Hug and Push Obstacles, Ignore obstacles, and Stop at First Obstacle. Use Shift+R to cycle through the modes.

The following basic keyboard shortcuts can be used at any time:

• Click or Enter - commits the routing up to the current cursor position and places the tracks.
• Right-click or Esc - terminates the current route. Any routing that has been committed before calling the termination is retained.
• Backspace - unwinds the last committed route back to its starting point. If any objects had been pushed through placing the last segment, they are moved back to their original positions. This feature is not available after using Auto-Complete.
• 7 - cycles through the connections available for routing if the current pad has multiple connections.
• 9 - switches the cursor position from the currently selected pad or track to the target pad or track. If the location of the object being switched to is not in the current window, the view jumps and centers around the new cursor position.
• + and - keys (on the numeric keypad) - switch routing layers.

Placement Modes

While placing track segments there are 5 available corner modes, 4 of which also have corner direction sub-modes. During placement:

• Press Shift+Spacebar to cycle through the 5 available corner modes: 45 degree, 45 degree with arc, 90 degree, 90 degree with arc, and Any Angle.
• Press Spacebar to toggle between the two corner direction sub-modes.
• When in either of the arc corner modes, hold the  or  keys to shrink or grow the arc. Hold the Shift key as you press to accelerate arc resizing.
• Press the 1 shortcut key to toggle between placing 1 segment per click (the first 5 images just below), or 2 segments per click (the last image in the set just below). In the first mode the hollow track segment is referred to as the look-ahead segment.
• Press the Backspace key to remove the last vertex.

Press Shift+Spacebar to cycle through the 5 available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to
toggle placement between 1 segment or 2 segments.

Automatic Connection Completion

The Interactive Router is able to attempt automatic completion (Auto-Complete) of connections to the target pad, hold Ctrl and Left Click to instruct the Interactive Router to attempt to complete the current connection. This can make routing much faster than placing individual track segments, however, there are some limitations to the Auto-Complete feature, as follows:

• The start point and target pad must reside on the same layer.
• The route can be completed in accordance with design rules (provided that routing conflicts are not being ignored).

Auto-Complete is available at any time, and you can even Ctrl+click directly on a pad or connection line to route it, there is no need to select it first. You can use Auto-Complete on connections that are partially routed as well. To do this, Ctrl+click on the end of the last track segment, or the remaining connection line, to complete it to the target.

Loop Removal

Altium Designer provides support for Loop Removal when interactively routing your nets. As you route there will be many instances where you need to change some of the existing routing. Rather than attempting to change the existing routing using a drafting type approach of clicking and dragging track segments, you re-route. To do this, launch the Interactive Routing command, click on the existing routing to start, and then route the new path, coming back to meet the existing routing. This will create a loop with the old path and the new path - no need to worry though, as soon as you right-click or press Esc to terminate the route, the redundant segments are automatically removed, including any redundant vias.

Displaying Clearance Boundaries

As you route, it can be extremely beneficial to have an indication of just how much space you really do have available to you. Altium Designer provides this very aid, through dynamic display of clearance boundaries. As you interactively route, the no-go clearance area defined by the existing objects + the applicable clearance rule is displayed as shaded polygons. By default, all clearance boundaries are displayed, but you can opt to reduce the clearance display area - only viewing boundaries that fall within a localized viewing circle.

Tips

1. Tracks on a PCB are made from a series of straight segments. Each time there is a change of direction, a new track segment begins. Also, by default, the PCB editor constrains tracks to a vertical, horizontal or 45° orientation, allowing you to easily produce professional results. This behavior can be customized to suit your needs.
2. Interactive routing preferences are defined on the PCB Editor - Interactive Routing page of the Preferences dialog. In addition, and while routing, applicable options can be accessed through the Properties panel. While many controls are accessed through a corresponding keyboard shortcut (indicated in the panel), you can also pause routing in order to interact with the panel (or other area of the software) directly. To pause routing, simply press the Tab key. To resume, click the pause symbol that appears over the workspace, or press Esc.
3. For a high-level overview on interactively routing nets in Altium Designer, see Interactive Routing.

Applied Parameters: AutoRoute=True

Summary

This command is used to route a specific pad-to-pad connection within the current design, using the Situs Autorouter.

Access

This command is accessed from the PCB Editor by choosing the Route » Auto Route » Connection command, from the main menus.

Use

After launching the command, the Autorouter will initialize and the cursor will change to a crosshair. Position the cursor over the connection you wish to route and click or press Enter. The connection will be routed. Continue routing further connections, or right-click, or press Esc, to exit.

Tips

1. All Autorouter event and routing information will appear as messages in the Messages panel.
2. It is important to ensure that any relevant routing design rules are set up prior to running the Autorouter.