Applied Parameters: ObjectKind=Project
This command is used to detect the logical differences that exist between (typically) different documents, by performing component and connectivity comparisons. It launches the Choose Documents To Compare dialog, with which to choose which documents to compare when using Altium NEXUS's powerful Comparator. Typically the dialog will be run to compare the design hierarchy of the active project, with a target PCB document. The advantage of running a comparison in this way, instead of one of the direct synchronization commands, is that it gives you full control over the synchronization process - providing the ability to view the list of differences detected and built by the Comparator. This is especially true when needing to control which, and in what direction, any updates (changes) are made, in order to (re)attain synchronicity.
This command is accessed from any editor by choosing the Project » Show Differences command, from the main menus.
When wanting to quickly show the differences between source schematics and target PCB, either make a source schematic for the project the active document, or make the target PCB for the project the active document.
After launching the command, the Choose Documents To Compare dialog will appear. By default, the dialog opens in simple (non-advanced) mode, allowing the user to quickly select the target PCB document to compare against the project's source document hierarchy. Enable the Advanced option to be able to select different document/project combinations to compare as required.
After clicking OK, and when comparing a project's source document hierarchy against the target PCB, the source documents will be recompiled automatically before the comparison is made. If any differences exist between these and the PCB document, the Differences between dialog will appear.
The Synchronizer is bi-directional. This means that updates to both source and target documents can be specified in the same Engineering Change Order (ECO). In order to synchronize the designs the aim now is to determine, for each difference, whether or not to take action and in which direction the change is made – specifying which document should be updated in order to remedy the difference. Even if differences are detected, you are under no obligation to take action on them. When the Differences between dialog is generated, the default update decision of No Change is assigned to each entry. Altium NEXUS will only synchronize the elements specified. To sweep all changes one way or another, simply right-click anywhere in the dialog and choose from a range of commands that act on all difference entries, all selected entries, or all entries of a particular comparison type. Alternatively, click in the Update column to make decisions on an individual basis.
From the Difference between dialog, you can:
- Explore differences - cross-probing directly to an object responsible for a difference on its parent document. This can be performed directly from the dialog, or by calling up the Differences panel.
- Report differences - set up and print/export a report for the differences found by the Comparator, the update decisions specified and the actions that will be included in the generated ECO.
- Create an ECO - with the update actions defined as required, the Engineering Change Order can be created, after which the Engineering Change Order dialog will appear. The dialog provides a list of modifications needed to resolve the differences detected between the PCB and source documents. Use this dialog to enable/disable individual modifications as required, before validating and ultimately executing the ECO, thereby implementing the required changes necessary to achieve synchronization.
- All schematic source documents are required to be open for compilation and comparison (the latter requires the PCB to be open too). These documents are opened and automatically hidden in order to prevent clutter in the tabbed area of the main design window. When a document is hidden, it is still open from the point of view of processes such as compilation/synchronization/annotation, It is just not displayed as a tabbed-document in the main design window. When a project is opened, and the first schematic sheet is opened, the PCB document will always be opened and hidden.
- To display the current status of documents in the Projects panel, click the button at the top-right of the panel, then enable the Show open/modified status option within the General grouping of pop-up controls. Hidden documents are given the blank document icon - .
- At the heart of the synchronization process is a user-configurable Comparator (or difference engine). It is this Comparator that is used to compare the source design documents and target PCB, and compile a list of differences. As a user, complete control is provided over the kinds of differences that the Comparator will detect. Controls for the Comparator are accessed from the Comparator tab of the Options for Project dialog, with all settings stored as part of the project.
- As with the Comparator, Altium NEXUS affords you control over which modification types can be contained in a generated ECO. ECO-related options are accessed from the ECO Generation tab of the Options for Project dialog, with all settings again stored as part of the project.
- For initial transfer of the design from source project documents to a blank PCB document, use of a direct synchronization command is by far the most expedient method. When component information is transferred for the first time between schematic source documents and the blank PCB design document, using the Synchronizer, all components will automatically be linked by unique ID – the ID information from each schematic component being assigned to the corresponding component footprint.
- Comparator-related messages will be displayed in the Messages panel.