Altium NEXUS Documentation

ManagePinPairs

Modified by Susan Riege on Aug 1, 2018

Parent page: PCB Commands

The following pre-packaged resources, derived from this base command, are available:


Applied Parameters: Action=CreatePinPair

Summary

This command is used to create a single xSignal between two specified component pins (pads) in the workspace. An xSignal (or extended Signal) is essentially a designer-defined signal path between two nodes - these can be two nodes within the same net, or they can be two nodes in associated nets separated by a component. The xSignal can then be used to scope relevant design rules such as Length and Matched Net Lengths, which will then be obeyed during design tasks, such as interactive length tuning.

For a conceptual overview of xSignals and their use, see the dedicated page xSignals, part of the documentation related to High Speed Design in Altium NEXUS.

Access

With the source and destination pads selected in the workspace, this command can be accessed from the PCB Editor by:

  • Choosing the Design » xSignals » Create xSignal from selected pins command from the main menus.
  • Right-clicking in the design workspace then choosing the xSignals » Create xSignal from selected pins command from the context menu.
A single xSignal can also be created directly from within the PCB panel. When configured in Nets mode, browse and select the required two pads, then right-click and choose the Create xSignal command from the context menu.

Use

First, ensure that the start and end pads are selected in the design workspace. These can be in the same net or different nets if the signal is through a series termination component.

After launching the command, the xSignal will be created.

Tips

  1. Created xSignals can be browsed and managed through the PCB panel, when configured in xSignals mode.
  2. If the start and end pads are in the same net, the xSignal will take a name in the form <NetName>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net. If the start and end pads are in different nets, the xSignal will take a name in the form <StartNet>_<EndNet>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net combination.
  3. An xSignal will actually follow the path of the connection lines that run between its start and end pads - indicating that this is the path the software assumes the xSignal will be routed. The reason it does this is because it is obeying the topology defined for that net.
  4. xSignals can be quickly and efficiently created, en masse, using the xSignals Multi-Chip Wizard. As well as defining the end-to-end xSignals for multiple nets between components, the Wizard also allows you to create xSignals for sections of those end-to-end signals. Based on the settings you enable, the Wizard can also create xSignal classes and Matched Net Lengths design rules targeting those xSignals. When the Wizard is complete, you can then start the length tuning process.


Applied Parameters: Action=CreatePinPairsBetweenComponents

Summary

This command is used to create one or more xSignals between a chosen source component and chosen destination component(s) for specific net(s) emanating from the source component in a single operation. An xSignal (or extended Signal) is essentially a designer-defined signal path between two nodes - these can be two nodes within the same net, or they can be two nodes in associated nets separated by a component. The xSignal can then be used to scope relevant design rules such as Length and Matched Net Lengths, which will then be obeyed during design tasks, such as interactive length tuning.

For a conceptual overview of xSignals and their use, see the dedicated page xSignals, part of the documentation related to High Speed Design in Altium NEXUS.

Access

With at least one component selected in the workspace, this command can be accessed from the PCB Editor by:

  • Choosing the Design » xSignals » Create xSignals between components command from the main menus.
  • Right-clicking in the design workspace and choosing the xSignals » Create xSignals between components command from the context menu.

Use

First, ensure that at least one component is selected in the design workspace. This will be used as the source component. If you select multiple components, the first will be used as the source with the other(s) used as the destination components.

After launching the command, the Create xSignals Between Components dialog will open. Use the dialog to create your xSignals as follows:

  1. The chosen source component will appear selected in the Source Component region.
  2. Any other component(s) selected in the workspace will appear selected in the Destination Components region. If not, make your choice(s) now.
  3. By default, all nets associated with the pads of the source component will be selected (in the Source Component Nets region). Adjust this selection as required.
  4. Click the Analyze button - the software attempts to identify potential xSignals that exist between the chosen source and destination components, for the selected nets.
Note that the analysis algorithm follows the current topology of the chosen nets.
The software can also search through series components if required, by selecting the appropriate mode from the button's associated drop-down menu. Modes available are: Search for direct connections, Through 1 series component, Through 2 series components, and Multipath coupled nets.
  1. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
  2. You can optionally have the created xSignals associated to an xSignal class. Either choose an existing xSignal class or enter a name for a new class. You can leave the field blank if you wish; the xSignals can always be added as members to the required class at a later stage.
  3. Click OK to create the xSignals. The dialog will close and you will be returned to the workspace, which presents a filtered view showing the newly created xSignals. If an xSignal class was specified, this will be created (if not existing) and the xSignals associated to it.

Tips

  1. Created xSignals can be browsed and managed through the PCB panel when configured in xSignals mode.
  2. If the start and end pads are in the same net, an xSignal will take a name in the form <NetName>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net. If the start and end pads are in different nets, an xSignal will take a name in the form <StartNet>_<EndNet>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net combination.
  3. xSignals can be quickly and efficiently created, en masse, using the xSignals Multi-Chip Wizard. As well as defining the end-to-end xSignals for multiple nets between components, the Wizard also allows you to create xSignals for sections of those end-to-end signals. Based on the settings you enable, the Wizard can also create xSignal classes and Matched Net Lengths design rules targeting those xSignals. When the Wizard is complete, you can then start the length tuning process.


Applied Parameters: Action=CreatePinPairsFromConnectedNets

Summary

This command is used to build xSignals outward from a selected series termination component, such as a resistor or capacitor. It supports both one or more discrete components, and one or more multi-instance pack-style components, such as resistor networks. An xSignal (or extended Signal) is essentially a designer-defined signal path between two nodes - these can be two nodes within the same net, or they can be two nodes in associated nets separated by a component. The xSignal can then be used to scope relevant design rules such as Length and Matched Net Lengths, which will then be obeyed during design tasks, such as interactive length tuning.

For a conceptual overview of xSignals and their use, see the dedicated page xSignals, part of the documentation related to High Speed Design in Altium NEXUS.

Access

With at least one component selected in the workspace, this command can be accessed from the PCB Editor by:

  • Choosing the Design » xSignals » Create xSignals from connected nets command from the main menus.
  • Right-clicking in the design workspace and choosing the xSignals » Create xSignals from connected nets command from the context menu.

Use

First, ensure that at least one series termination component is selected in the design workspace. This will be used as the source component.

After launching the command, the Create xSignals From Connected Nets dialog will appear. Use the dialog to create your xSignals as follows:

  1. The chosen source component(s) will appear selected in the Source Component region.
  2. By default, all nets associated with the pads of the source component(s) will be selected (in the Source Component Nets region). Adjust this selection as required.
  3. Click the Analyze button - the software attempts to identify potential xSignals that exist for the selected nets emanating from the chosen component(s).
Note that the analysis algorithm follows the current topology of the chosen nets.
  1. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
  2. You can optionally have the created xSignals associated to an xSignal class. Either choose an existing xSignal class or enter a name for a new class. You can leave the field blank if you wish; the xSignals can always be added as members to the required class at a later stage.
  3. Click OK to create the xSignals. The dialog will close and you will be returned to the workspace, which presents a filtered view showing the newly created xSignals. If an xSignal class was specified, this will be created (if not existing) and the xSignals associated to it.

Tips

  1. Created xSignals can be browsed and managed through the PCB panel when configured in xSignals mode.
  2. If the start and end pads are in the same net, an xSignal will take a name in the form <NetName>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net. If the start and end pads are in different nets, an xSignal will take a name in the form <StartNet>_<EndNet>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net combination.
  3. xSignals can be quickly and efficiently created, en masse, using the xSignals Multi-Chip Wizard. As well as defining the end-to-end xSignals for multiple nets between components, the Wizard also allows you to create xSignals for sections of those end-to-end signals. Based on the settings you enable, the Wizard can also create xSignal classes and Matched Net Lengths design rules targeting those xSignals. When the Wizard is complete, you can then start the length tuning process.


Applied Parameters: Action=ManagePinPairs

Summary

This command is used to create one or more xSignals between a chosen source component, and chosen destination component(s) - for specific net(s) emanating from the source component. An xSignal (or extended Signal) is essentially a designer-defined signal path between two nodes - these can be two nodes within the same net, or they can be two nodes in associated nets separated by a component. The xSignal can then be used to scope relevant design rules such as Length and Matched Net Lengths, which will then be obeyed during design tasks, such as interactive length tuning.

For a conceptual overview of xSignals and their use, see the dedicated page xSignals, part of the documentation related to High Speed Design in Altium NEXUS.

Access

This command is accessed from the PCB Editor by choosing the Design » xSignals » Create xSignals command from the main menus.

Use

After launching the command, the Create xSignals Between Components dialog will open. Use the dialog to create your xSignals as follows:

  1. Choose a source component in the Source Component region.
  2. Choose one or more destination components in the Destination Components region.
  3. All nets associated with the pads of the source component will be listed in the Source Component Nets region. Select the nets of interest.
  4. Click the Analyze button - the software attempts to identify potential xSignals that exist between the chosen source and destination components for the selected nets.
Note that the analysis algorithm follows the current topology of the chosen nets.
The software can also search through series components if required, by selecting the appropriate mode from the button's associated drop-down menu. Modes available are: Search for direct connections, Through 1 series component, Through 2 series components, and Multipath coupled nets.
  1. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
  2. You can optionally have the created xSignals associated to an xSignal class. Either choose an existing xSignal class or enter a name for a new class. You can leave the field blank if you wish; the xSignals can always be added as members to the required class at a later stage.
  3. Click OK to create the xSignals. The dialog will close and you will be returned to the workspace, which presents a filtered view showing the newly created xSignals. If an xSignal class was specified, this will be created (if not existing) and the xSignals associated to it.

Tips

  1. Created xSignals can be browsed and managed through the PCB panel when configured in xSignals mode.
  2. If the start and end pads are in the same net, an xSignal will take a name in the form <NetName>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net. If the start and end pads are in different nets, an xSignal will take a name in the form <StartNet>_<EndNet>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net combination.
  3. xSignals can be quickly and efficiently created, en masse, using the xSignals Multi-Chip Wizard. As well as defining the end-to-end xSignals for multiple nets between components, the Wizard also allows you to create xSignals for sections of those end-to-end signals. Based on the settings you enable, the Wizard can also create xSignal classes and Matched Net Lengths design rules targeting those xSignals. When the Wizard is complete, you can then start the length tuning process.


Applied Parameters: Action=xSignalsWizard

Summary

This command is used to run the xSignals Multi-Chip Wizard. Use the Wizard to either create xSignals for common interface and memory circuits or create custom xSignals for multiple components. An xSignal (or extended Signal) is essentially a designer-defined signal path between two nodes - these can be two nodes within the same net, or they can be two nodes in associated nets separated by a component.

For a conceptual overview of xSignals and their use, see the dedicated page xSignals, part of the documentation related to High Speed Design in Altium NEXUS.

Access

This command can be accessed from the PCB Editor by:

  • Choosing the Design » xSignals » Run xSignals Wizard command from the main menus.
  • Right-clicking in the design workspace and choosing the xSignals » Run xSignals Wizard command from the context menu.

Use

After launching the command, the xSignals Multi-Chip Wizard will open. Choose which xSignal creation mode you wish to use, then follow the Wizard's intuitive pages through to xSignal generation. The following modes of use are supported:

  • On-Board DDR3/DDR4 - use the Wizard to create xSignals for your DDR3 or DDR4 memory. In this mode, the Wizard will automatically create the xSignals, xSignal Classes, Matched Length Groups, Diff Pair Matched Lengths rules, and Fly-By topology for on-board DDR3/4. The Wizard assumes that a fly-by routing topology will be used.
  • USB 3.0 - use the Wizard to create xSignals for your USB 3.0 interface circuitry.  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.
  • Custom Multi-Component Interconnect - use the Wizard to create xSignals between a single source component and multiple destination components. The Wizard uses a component-oriented approach to identifying potential xSignals; you select a single source component, the nets of interest and the destination components; it then analyzes all potential paths from the source component to the destination 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. As well as defining the end-to-end xSignals for multiple nets between components, the Wizard also allows you to create xSignals for sections of those end-to-end signals (from source output pin to series termination component, and from series termination component to destination input pin). Based on the settings you enable, the Wizard can also create xSignal classes and Matched Net Lengths design rules targeting those xSignals. When the Wizard is complete, you can then start the length tuning process.

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.

Tips

  1. Created xSignals can be browsed and managed through the PCB panel when configured in xSignals mode.
  2. The Wizard creates xSignals, xSignal classes and design rules. Performing an Undo will remove xSignals created by the Wizard but not the design rules.
  3. When creating custom xSignals for multiple components:
    1. If the start and end pads are in the same net, an xSignal will take a name in the form <NetName>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net. If the start and end pads are in different nets, an xSignal will take a name in the form <StartNet>_<EndNet>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net combination.
    2. An xSignal will actually follow the path of the connection lines that run between its start and end pads - indicating that this is the path that the software assumes the xSignal will be routed. The reason it does this is because it is obeying the topology defined for that net.

 

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.