ManagePinPairs

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 2 nodes - these can be 2 nodes within the same net, or they can be 2 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.

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 and choosing the xSignals » Create xSignal from selected pins 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 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.
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 2 nodes - these can be 2 nodes within the same net, or they can be 2 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.

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 appear. 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.

5. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
6. 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.
7. 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 2 nodes - these can be 2 nodes within the same net, or they can be 2 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.

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).

5. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
6. 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.
7. 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 2 nodes - these can be 2 nodes within the same net, or they can be 2 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.

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 appear. 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.

5. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
6. 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.
7. 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. 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. An xSignal (or extended Signal) is essentially a designer-defined signal path between 2 nodes - these can be 2 nodes within the same net, or they can be 2 nodes in associated nets separated by a component.

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 appear. 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, and you can also create Matched Net Lengths design rules if required.

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.

If the set of nets selected include series termination components extra Wizard pages will appear, giving you the opportunity to create additional xSignals and design rules for these sections of the nets (source output pin to series termination component and/or series termination component to destination input pin).

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. 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.