Sch_Cmd-CrossProbeChooseCrossProbeChoose_AD

Applied Parameters: None

Summary

This command is used to cross probe from a chosen object on the current schematic document to its corresponding counterpart on the PCB document. Cross-probing is a powerful searching tool to help locate objects in other editors by selecting the object in the current editor. Between the Schematic and PCB Editors, full cross-probing support is provided for documents, components, buses, nets, and pins/pads.

Access

This command can be accessed from the Schematic Editor by:

• Choosing the Tools » Cross Probe command from the main menus.
• Clicking the  button on the Schematic Standard toolbar.

Use

There are two cross-probing modes available:

• Continuous Mode – this mode allows remaining in the source document while cross-probing to different objects on the target document. Simply position the cursor over the required object within the workspace and click, or press Enter. The corresponding object will be highlighted on the target document. Continue cross-probing further objects, or right-click, or press Esc, to exit.

• Jump To Mode – this mode allows cross-probing to a single object (i.e., 'single-shot cross-probing'), making the target document the active document. Simply position the cursor over the required object within the workspace and Ctrl+click or press Ctrl+Enter. The corresponding object will be highlighted on the target document, with that document becoming the active document.

Tips

1. When using the command repeatedly in Continuous Mode, the last object chosen will be the one displayed/highlighted. Cross-probe filtering is not cumulative.
2. The cross-probed objects on the target document will be displayed in accordance with the Highlight Methods defined on the System - Navigation page of the Preferences dialog. Highlighting will not be applied to the originating document.

Applied Parameters: Action=ToggleFastCrossSelect

Summary

This feature facilitates dynamic, bi-directional object cross-selection. It is used to select corresponding objects between schematic and PCB documents. That is, when you select an object on a schematic document, the same object on the PCB document is also selected (and vice-versa). There are many uses for cross-selecting from the schematic to build up a selection of PCB components, three of which include:

• The ability to quickly create a PCB Component Class (Design » Classes; there is a button to take over selected components when defining a component class).
• The ability to cluster selected components into a user-defined rectangle using the Tools » Component Placement » Arrange Within Rectangle command, ideal for pulling a set of components out when the design is first transferred from schematic to PCB.
• The ability to select the schematic components in a specific order, then switch to the PCB Editor and run the Tools » Component Placement » Reposition Selected Components command - each PCB component can then be placed one-by-one, in the same order they were selected on the schematic.

Access

This feature is accessed from the Schematic Editor in one of the following ways:

• Click the Tools » Cross Select Mode command from the main menus.
• Enable the Cross Selection option in the Cross Select Mode region, on the System - Navigation page of the Preferences dialog.
• Click Shift+Ctrl+X.

Use

With this feature enabled, simply select one or more objects within the source schematic sheets of the design project. Those same objects will become selected on the PCB document.

Tips

1. When enabled, the icon for the feature on the main Tools menu will become highlighted.
2. Cross Select Mode display behavior is controlled using the Cross Select Mode options on the System - Navigation page of the Preferences dialog. This includes the option to Reposition selected component in PCB. With this enabled, when you click on a component on a schematic, the corresponding component will be attached to the cursor in the PCB, which is made active, ready for placement immediately.
3. If a document is closed and then reopened, the project must be re-compiled before the feature will work correctly for affected objects on that document.

Applied Parameters: Action=CrossSelect

Summary

This feature facilitates cross-selection between selected parts on one or more schematic source documents and the corresponding component footprints on the PCB document for the active project. This can be useful, for example, in selecting a set of parts on the source documents to create a new component class quickly in the PCB document.

Access

This feature is accessed from the Schematic Editor by choosing the Tools » Select PCB Components command from the main menus.

Use

First, ensure that the target PCB document is open and that the required components are selected on the applicable source schematic documents.

After launching the command, all schematic source documents will be automatically compiled, and the PCB document for the project will then be made the active document. All corresponding component footprints for the selection will become selected and zoomed (but not masked) in the workspace.

Tips

1. If the active project contains multiple PCB documents, you should open only the document upon which you wish to work/have the components selected. If more than one PCB document is opened, the command will interrogate all documents for a corresponding match to the components selected on the schematic document(s).

Applied Parameters: ContextSensitive=True|Action=CrossSelect

Summary

This feature facilitates cross-selection between selected parts on one or more schematic source documents, and the corresponding component footprints on the PCB document for the active project. This can be useful, for example, in selecting a set of parts on the source documents to create a new component class quickly in the PCB document.

Access

This feature is accessed from the Schematic Editor by right-clicking over the required part (or one part in a selection of parts) and choosing the Part Actions » Select PCB Components command from the context menu.

Use

First, ensure that the target PCB document is open, and that the required components are selected on the applicable source schematic documents. If cross selecting a single part, the part need not be selected.

After launching the command, all schematic source documents will be automatically compiled and the PCB document for the project will then be made the active document. All corresponding component footprints for the selection will become selected and zoomed (but not masked) in the workspace.

Tips

1. If the active project contains multiple PCB documents, you should open only the document upon which you wish to work/have the components selected. If more than one PCB document is opened, the command will interrogate all documents for a corresponding match to the components selected on the schematic document(s).