Applied Parameters: Action=CreatePinPairsFromConnectedNets
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.
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.
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:
- The chosen source component(s) will appear selected in the Source Component region.
- 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.
- Click the Analyze button - the software attempts to identify potential xSignals that exist for the selected nets emanating from the chosen component(s).
- All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
- 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.
- 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.
- Created xSignals can be browsed and managed through the PCB panel when configured in xSignals mode.
- 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.
- 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.