交叉探测和选定
Altium provides various powerful cross-probing and cross-selecting capabilities enabling fast, efficient navigation between schematic and PCB design domains. The Cross-Probing and Cross Selecting features are powerful search tools to help locate objects in other editors by selecting the object in the current editor.
Cross-probing is used to point to a chosen object on the current document then "jump to" its corresponding counterpart in the target document. Between the PCB and schematic editors, full cross-probing support is provided for documents, components, buses, nets, and pins/pads(s). Literally, with a single click, you can select a supported object in either domain and see it highlighted in both.
Cross selecting enables you to select an object(s) on the source document and by enabling the cross select command, the same object(s) will be selected on the target document.
Unified Data Model And Project Compilation
A Unified Data Model (UDM) is automatically created in the computer’s memory. The UDM models every aspect of the design, including the components, the connectivity, the component footprints, the relationships between the PCB project and a connected FPGA project, etc. It is this Unified Data Model that enables cross-probing functionality between different design domains. Cross-probing features use auto-compilation, ensuring the very latest model of the data is being used. Dynamic compilation also can be performed manually at any time by clicking Project » Validate PCB Project. This function checks for logical, electrical, and drafting errors between the UDM and compiler settings.
Document Setup
Many of the features of Cross-Probing and Cross Selecting either require, or are more easily utilized, viewing both the schematic and PCB documents at the same time. You can view both documents at the same time by performing one of the following:
- Right-click on the document tab then select Split Vertical or Split Horizontal depending on your viewing preference.
- If you are using more than one screen, you can drag the document tab onto another monitor.
Cross-Probing
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.
The cross-probing feature is accessed from either the schematic or PCB editor using the Tools » Cross Probe command or by clicking the 
button from an editor's Standard toolbar.
There are two cross-probing modes, Continuous Mode and Jump-To Mode, which are both described in the following sections.
Continuous Cross-Probing Mode
The Continuous Mode allows you to stay in the source document while cross-probing to different objects on the target document. For this mode, ensure that the schematic and PCB documents are open side-by-side in the main design window.
After launching the cross-probe command by clicking Tools » Cross Probe, the cursor will change to a cross-hair and you will be prompted to choose the object that you wish to navigate. Position the cursor over the required object within the design space and click or press Enter. The corresponding object will be highlighted on the target document.
Cross-probing from the source (e.g., schematic) with corresponding object highlighted on the PCB.
You can continue to cross-probe additional objects or right-click or press Esc to exit.
Jump To Cross-Probing Mode
The Jump To Mode allows you to cross-probe to a single object and make the target document the active document.
After launching the cross-probe command by clicking Tools » Cross Probe, the cursor will change to a cross-hair and you will be prompted to choose the object that you wish to navigate. Position the cursor over the required object within the workspace then Ctrl+click or press Ctrl+Enter. The corresponding object will be highlighted on the target document which will be made the active document.
Cross-Probing from Additional Locations in the Software
Cross-Probing also can be accomplished in various additional places in the software. These additional locations enable you to use the cross-probe function even as you are building your design without the need to use the Tools » Cross Probe command.
Probing Within the Engineering Change Order Dialog
You can cross probe from the Engineering Change Order dialog by right-clicking to access cross probe commands to locate the Reference component in the schematic or the target component in the PCB as shown in the image below:
Probing Within the Differences Between Dialog
The Differences between dialog can be used to cross-probe to a selected component on the schematic or PCB. Double-click on an entry to cross probe to that component on the schematic or PCB.
Cross-Probing From the Variant Management Dialog
You can use the Variant Management dialog to cross probe to a chosen component on the schematic or the PCB. Double-click on the component in the Variant Management dialog or right-click then select Cross Probe from the menu.
Probing Within the Differences Panel
To cross probe to the schematic or PCB from the Differences panel (click the Explore Differences button in the Differences between dialog to access this panel), double-click on an entry in the panel.
Probing Within the BomDoc
Cross-Probing also can be done within the BomDoc. In the BomDoc, right-click, choose Cross Probe then select to which item you wish to navigate from the sub-menu.
Cross-Probing From the Projects Panel
To cross probe to a chosen component or net on the schematic or the PCB from the Projects panel, right-click on an entry in the Components or Nets sub-folder and then select the Cross Probe to Schematic or Cross Probe to PCB command.
Cross Selecting
This feature facilitates dynamic, bi-directional component cross-selection. It is used to select corresponding objects between PCB and schematic documents. In other words, when you select an object on the PCB document, the same object on the source schematic 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.
This feature is accessed by:
-
Clicking Tools » Cross Select Mode from the main menus. This command toggles the feature on and off and the status of the command is displayed in the Tools menu. Cross Select Mode is enabled when a blue box appears around the Cross Select Mode icon in the Tools menu as shown in the image below.
Cross Select Mode in the Tools menu shown disabled (left) and enabled (right). - Checking or un-checking the Cross Selection option in the System - Navigation page of the Preferences dialog.
- Clicking Shift+Ctrl+X.
With Cross Select Mode enabled, click to select one or more objects within the design space. Those same objects will become selected on the corresponding document.
Selecting PCB Components from the Schematic
It is possible to cross-select between selected parts on one or more schematic source documents and the corresponding component footprints on the PCB document for the active project. As an example, this can be useful when selecting a set of parts on the source documents to create a new component class quickly on the PCB document.
To use this feature:
- Ensure the target PCB document is open.
- Select the required part(s) on the source schematic document(s).
- Choose the Tools » Select PCB Components command.
After launching the command 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 design space.
To create the new component class once the part or set of parts has been selected on the PCB using the Select PCB Components command:
- Click Design » Classes to open the Object Class Explorer dialog.
- Right-click Component Classes then select Add Class by right-clicking in the left column. Enter the desired name of the new class.
- Click the button between the Non-Members and Members region of the dialog to add the desired and selected part(s) to the right-hand column.
- Click Cancel to close the Object Class Explorer dialog and return to the workspace.