Связаться с нами
Связаться с нашими Представительствами напрямую
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.
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.
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:
Cross-probing is a powerful searching tool to help locate objects in other editors by selecting the object in the current editor. There are numerous places you can cross probe in Altium Designer. For example, once you have launched cross probing from the PCB editor, you can click on a component on the PCB to display the same component on the schematic. Between the schematic and PCB editors, full cross-probing support is provided for documents, components, buses, nets, and pins/pads.
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 design space 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 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 also can be accomplished in various additional places in Altium Designer. 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. Double-click on an entry to cross probe to that component on the schematic or PCB.
You can use the Variant Manager or Variant Management dialog to cross probe to a chosen component on the schematic. Double-click on the component in the Variant Manager or 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. In the BomDoc, right-click, choose Cross Probe then select to which item you wish to navigate from the sub-menu.
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.
After validating the schematic project, you can right-click then choose Cross Probe or double-click on an error message in the Messages panel to jump to that error condition on the schematic.
To cross probe to an object from the Constraint Manager, right-click on its entry, then choose the Cross Probe option from the context menu or select Cross Probe from a custom rule's menu.
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. It is an ideal tool for building a set of selected objects ready for a design action. For example, you might be looking at a number of components on the schematic and would like to locate them in the PCB editor space so you can position them on the board.
There are many uses for cross-selecting from the schematic to build up a selection of PCB components, three of which include:
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.
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.
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 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:
Связаться с нашими Представительствами напрямую