Altium Designer 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.
When an Altium Designer project is compiled, a Unified Data Model (UDM) is 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. Many of the cross-probing features use auto-compilation, ensuring the very latest model of the data is being used. Compilation also can be performed manually at any time by clicking Project » Compile PCB Project.
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:
There are two cross-probing modes, Continuous Mode and Jump-To Mode, which are both described in the following sections.
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 workspace and click or press Enter. The corresponding object will be highlighted on the target document.
You can continue to cross-probe additional objects, or right-click or press Esc to exit.
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 and 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 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.
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:
The Differences between dialog can be used to cross-probe to a selected component on the schematic or PCB. Use the Project » Show Differences command to open the Differences between dialog then double-click on an entry to cross probe to that component on the schematic or PCB.
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.
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.
Cross-Probing also can be done within the BomDoc. On the BOM Components tab of the BomDoc, right-click then choose Navigate to and select to which item you wish to navigate: the schematic component, the BOM Catalog entry, or The Vault component.
The Navigator panel is populated and refreshed each time the design is compiled. It provides a structured view of all documents, sheets, components, nets, parameters, and component pins in the currently focused project. In the context of editing, this panel provides a helpful means for navigating across the entire design and locating objects of interest.
You can use the Navigator panel to probe between schematic and PCB documents. With both the PCB and schematic documents open, click on a component in the Navigator panel to highlight it on both the schematic and PCB.
In order for the cross-probing feature of the Navigator panel to highlight correctly in both the schematic and PCB, ensure that the Cross Select Mode in the Tools menu is enabled and the Cross Selection option is enabled on the System - Navigation page of the Preferences dialog as shown in the following images. On the Preferences dialog, you also can enable the objects you want to use for cross selection in the Objects for cross selection region. Choices include: Components, Nets, and Pins and you can choose none, one, all, or any combination.
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.
This feature is accessed by:
To use the Cross Select Mode, the command must be enabled in both editors.
With Cross Select Mode enabled, click to select one or more objects within the workspace. Those same objects will become selected on the corresponding document.
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:
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.
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:
You can see the resulting new component class in the PCB - Components panel. The following video illustrates this process.
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.
好的，您可以下载免费的Altium Designer Viewer查看文档，有效期6个月。
好的，您可以下载免费的Altium Designer Viewer查看文档，有效期6个月。