PCB_Cmd-AdvancedMultiRouteAdvancedMultiRoute_AD

Applied Parameters: None

Summary

When routing a PCB it is fairly common for groups of signals to all need to be routed along the same path, such as for Address and Data busses. One option would be to route each of these signals individually but a much faster option is to route them collectively. This command allows you to do just that - route multiple nets simultaneously.

Access

This command can be accessed from the PCB Editor by:

• Choosing the Place » Interactive Multi-Routing command, from the main menus.
• Clicking the  button on the Wiring toolbar.
• Right-clicking in the workspace and choosing the Interactive Multi-Routing command from the context menu.

Use

First select the source pad of each net to be included in the route. Shift+click to select individual pads, Ctrl+click and drag to draw a selection rectangle and sub-select multiple child pads in a component. After launching the command, you will be prompted to click to begin multi-routing. Simply click within the workspace at the point where you require to lay down the first set of track segments, then continue routing as required toward your target destination.

As you route, 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.

Use the + and - keys on the numeric keypad to switch routing layers, and the B / Shift+B to decrease / increase bus spacing in increments of the current grid. Press C to converge bus spacing to the minimum allowed by the applicable routing rules.

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, or 2 segments per click. 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.

Loop Removal

Altium Designer provides support for Loop Removal when interactively routing multiple 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 Differential Pair 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.

Tips

1. Interactive routing preferences are defined on the PCB Editor - Interactive Routing page of the Preferences dialog. These preferences can be accessed while routing by using the Tab shortcut.
2. It is also possible to enter this mode of routing implicitly, by selecting a group of tracks and dragging their ends (sometimes referred to as Smart Drag). In this mode successive drags can be used to add new segments.