xSignals Multi-Chip Wizard

Now reading version 16.1. For the latest, read: xSignals Multi-Chip Wizard for version 22
Applies to Altium Designer versions: 16.1, 17.0 and 17.1

The first page of the xSignals Wizard.
The first page of the xSignals Wizard.

Summary

The xSignal Wizard is used to create xSignals between a single source component and multiple target components. The Wizard uses a component-oriented approach to identifying potential xSignals - you select a single source component, the nets of interest and the target components - it then analyzes all potential paths from the source component to the designation components, passing through series passive components and along any branches. As the designer you then get to choose the xSignals you would like to have generated, and you can also create Matched Length design rules if required. The xSignal Wizard can also be used to automatically create xSignals and xSignal classes for a number of different common interface and memory circuits.

 In this Wizard, an output pin is referred to as the Source, and the target input pin is referred to as the Destination.

Explore the xSignals in the PCB panel - note that the xSignals Wizard can create both end-to-end xSignals, and xSignals for connections within those end-to-end xSignals.

The Wizard is also a multiple-run tool - from the overall master group of xSignals you initially create on the xSignal Routes page, you can select a sub-set of these, define classes and rules, then return to the master group, choose another sub-set, define classes and rules for them, and so on.

One of the great strengths of the Wizard is the ease of working between the Wizard and the workspace, click on an xSignal on any page of the Wizard and the pads and any routing are highlighted in the workspace.

At this stage, the Wizard does not support the automatic addition of T-junction identifiers, often referred to as tie-points or branch-points. If your design includes branched routing, it is suggested that you:

  1. Tune the length from the source component to the passive component (such as a series termination resistor), if there are any.
  2. Tune the length in each branch, from the T-Junction to the destination component.
  3. If required, tune the remaining length between the passive component (or from the source if there are no passives) to the T-junction.
If you need to tune the lengths of just the branches, create a user-defined branch point by placing a single-layer, single-pad component within the routing at the T-junction. Refer to the Defining the Branch Point in a Balanced T Pattern topic in the Defining High Speed Signal Paths with xSignals page for more information.

Access

The xSignal Wizard can be launched by selecting:

  • Design » xSignals » Run xSignals Wizard
  • Component right-click » xSignals » Run xSignals Wizard

xSignals Multi-Chip Wizard Modes

Before beginning the xSignal Multi-Chip Wizard, you will be asked to select whether to use a custom multi-component interconnect, an on-board DDR3 / DDR4, or USB 3.0. The custom multi-component interconnect mode can be used to define multiple xSignals between a chosen source component and multiple target components, while the on-board DDR3 / DDR4 is used to create xSignals for your DDR3 or DDR4 memory. The USB 3.0 mode creates the xSignals, xSignal Classes, and Matched Length rules for each USB 3.0 channel.

Note

The features available depend on your level of Altium Designer Software Subscription.