USB 3.0 Mode for the xSignals Wizard

Old Content - visit altium.com/documentation

Released in Altium Designer 15, the xSignals Wizard simplifies the process of creating multiple xSignals between multiple components, as a single process.

The xSignal Wizard creates 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 Lengths design rules targeting these xSignals.

The original xSignals Wizard supported creating custom xSignals for multiple components. The Wizard is being expanded to automatically create xSignals and xSignal classes for a number of different common interface and memory circuits.

This release sees the addition a USB3 mode to the xSignals Wizard. The goal of the USB 3.0 xSignal Wizard is to create the xSignals, xSignal Classes, and Matched Length rules for each USB 3.0 channel.

Running the xSignal Wizard

The xSignal Wizard can be launched by selecting:

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

USB 3.0

The Wizard can process all USB 3.0 channels between each controller–to-connector-pair specified by the user. The Wizard automatically evaluates Differential Pair nets connected to the controller, detecting those that span through to the connector. The span can include passive components and multiple nets. The Wizard identifies each of these pairs by an xSignal class, with each leg of the pair identified by a controller-to-connector xSignal.

Once you have selected USB 3.0, the page will include a setting for the Matched Length Tolerance Within Diff Pair, enter a suitable value. This value is used for the design rule created by the Wizard, and can be changed at any time in the PCB Rules and Constraints Editor. User-defined settings such as this are saved for future use.

For USB 3.0, each USB user port is referred to as a channel. As can be seen in the image, each channel includes 3 differential pairs: Transmit, Receive and Data.

For USB 3.0, the critical routing design requirement is to match the route lengths within each pair, between-pairs length matching is not as critical. Because of this requirement, and the fact that the Matched Length design rule requires differential pairs to check lengths within a pair of nets, the Wizard will check for Differential Pair definitions, and automatically create suitable differential pairs if there are none. The Matched Length design rule that the Wizard creates is then configured to check length matching Within Differential Pair Length. Note that the rule is configured to compare the leg lengths within the pair for the overall xSignal, it does not compare the leg lengths within each differential pair.


Select USB 3.0 to use the Wizard to automatically create xSignals and Differential Pairs for the important USB 3.0 nets.

Selecting the Source and Target Components

On the next page, the Wizard identifies all potential source components and target connectors, based on the designator prefix and the number of pins.

  1. Set the filter prefix for the Controller designator and the Connector designator, and the Min Pin Count values as required, then
  2. Select a single source component, then
  3. Select the target component(s).


Select the source controller component, and the target USB connectors.

If you select multiple target components, you should check the xSignal and Net Naming Syntax for each of these components, using the drop down in the next page of the Wizard.

Identifying the Channels and Creating the xSignals

On this page you define a naming syntax that the Wizard can use to identify the relevant Transmitter, Receiver and Data pair nets, which are then included in xSignals. Each pair of xSignals is then clustered into an xSignal class, and these classes are used to scope the Matched Length design rule.


Check, and if required, define suitable Naming Syntaxes for xSignals and Nets, then click to create the xSignals.

The functionality of this page is as follows:

  1. The designator of the Controller is displayed next to the Components label. Next to this, the dropdown includes all of the Connectors selected on the previous page of the Wizard.
  • The naming syntax options shown below apply to each of the connectors listed in the drop down, select each in turn and check that the chosen naming syntax is complete, and suitable.
  • As mentioned, for USB 3.0, each USB user-port is referred to as a channel. You can set the number of channels (Channels Total) from 1 to 32. Typically each connector has a single channel.
  1. Within each USB 3.0 channel there are 3 differential pair paths, Transmit, Receive and Data, that run from the Controller to the Connector. The Wizard will create an xSignal, spanning series components as required, for each positive net, and another xSignal for each negative net, and then an xSignal class to represent that Controller-to-Connector pair. The Define xSignal Class Syntax group is used to specify the names of these xSignal classes. the Wizard also creates suitable Differential Pairs, if there are none already defined.
  • Define xSignal Class Name Syntax - the xSignal classes that are created will be named as specified, with each channel assigned a numeric value in place of the [#]. Enter your preferred string as required.
  1. Channel <N> - these fields define the masks that are used to identify the relevant Transmitter / Receiver / Data net names.
  • The Wizard has a large template of predefined naming schemes that it checks, usually it will populate these fields automatically. If it does not, select the correct name from the dropdown, or type in a suitable net name syntax.
  1. Once the naming fields are configured, click the Analyze Nets & Create xSignal Classes button.
  • The Wizard will create the xSignals, xSignal Classes, and Matched Length rules for all of the channels. Note that these are created each time you re-run the Wizard, delete them if you plan to run the Wizard again.
  1. The resulting xSignal Class names and their member xSignals are detailed in the grid.
  2. Click the Create Spreadsheet button to generate an XLS-format spreadsheet of the xSignals created by the Wizard.
  3. Click Finish to complete the Wizard.

xSignals and xSignal Classes Created

As mentioned, the Wizard automatically creates:

  • xSignals - for each of the three pairs of controller-to-connector Transmit, Receive and Data signal paths, as identified by the Net Names Syntax masks.
  • xSignal Classes - xSignal classes are created for each of these pairs of xSignals, named in accordance with the naming specified in the Define xSignal Class Name Syntax controls.
  • Differential Pairs - to scope the Matched Length design rule so that it checks within a pair of nets, differential pairs are required. The Wizard checks for suitable pairs, and if none are detected, automatically creates them. Set the PCB panel to Differential Pairs Editor mode to examine the pairs and confirm that they are correct.

Design Rules Created

The Wizard then creates a single Matched Length design rule that targets all of the xSignal classes. Only one rule is required, because it is scoped to test all xSignal pairs, and compare the leg lengths within each pair. The rules use the Tolerance constraint entered into the second page of the Wizard. Adjust the tolerance if required.


Only one Matched Length rule needs to be created for checking all xSignals classes, because it is testing the leg-lengths within each pair.

 

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.

Sounds exciting! Did you know we offer special discounted student licenses? For more information, click here.

In the meantime, feel free to request a free trial by filling out the form below.

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.