Altium NEXUS Documentation

AdvancedMultiRoute

Modified by Jason Howie on Sep 25, 2017

Parent page: PCB Commands

The following pre-packaged resource, derived from this base command, is available:


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 Route » Interactive Multi-Routing command, from the main menus.
  • Locating and using the Interactive Multi-Routing command () on the Active Bar.
If the command has been recently used from the Active Bar, it will become the active/visible button. Where other commands are available, this is indicated by a triangle at the bottom-right corner of the button. Click and hold on the active button to access a menu of all associated commands for that grouping.
  • Clicking the  button on the Wiring toolbar.

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.

Press Shift+F1 to display all of the available shortcuts for commands available to you while in interactive multi-routing mode. Shortcuts are also reflected in the Properties panel, which presents controls and options available while using the interactive multi-routing tool.

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 NEXUS 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.

This feature is employed by enabling the Automatically Remove Loops option - either from within the Properties panel (while in interactive multi-trace routing mode), or on the PCB Editor - Interactive Routing page of the Preferences dialog. To toggle this feature on or off while routing, use the Shift+D keyboard shortcut.

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 NEXUS 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 th at fall within a localized viewing circle.

The clearance around existing workspace objects is displayed dynamically, as you route. Use the Ctrl+W shortcut to enable/disable during routing.

This feature is employed by enabling the Display Clearance Boundaries option, on the PCB Editor - Interactive Routing page of the Preferences dialog. To toggle this feature on or off while routing, use the Ctrl+W keyboard shortcut. To show clearance boundaries only with a localized area, ensure to enable the Reduce Clearance Display Area sub-option.
The display of clearance boundaries is available in all routing modes except Ignore Obstacles.

Tips

  1. 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.
  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.
  3. For a high-level overview on routing multiple nets in Altium NEXUS, see Interactive Multi-Routing.

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.