Showing Physical Differences - Going Graphical

The Project » Show Differences command provides for detection of the logical differences that exist between (typically) different documents - commonly the source documents in a project with the target PCB. These are component and connectivity comparisons. In addition to these, Altium Designer's Comparator caters for the physical comparison of schematic or PCB documents. This feature enables you to graphically compare two versions of the same schematic or PCB and, with the two documents open side-by-side in the workspace, view the physical differences between them.
Access to this feature can be made in one of the following ways:

The Differences panel can only display the differences that were listed in the Differences dialog.
Using the Project » Show Physical Differences command. Ensure that the previous version (typically a backup) of the document is saved with a different name before opening. The backup version of the document does not need to be added to the project, it can be opened as a free document. Then, run the command to access the Choose Documents To Compare dialog which, when configured in Advanced mode, can be used to select the two versions of the document for comparison.

• From within the Storage Manager panel. Select two versions of the document in the Local History region (or VCS Revisions region if your documents are under version control using CVS or SVN), right-click and choose Compare.
• Using the Project » Local History » Show Local History command. Select two versions of the document from the available list and click Compare.
• In all three cases the comparison will proceed - in accordance with the options defined for the Physical comparison types in the Comparator tab of the Options for Project dialog. Any detected physical differences will be listed in the Differences panel, with entries also appearing in the Messages panel. With the two versions of the document open side by side in the main design window, you can peruse the differences graphically. Clicking on a top-level folder for a detected difference (in the Differences panel) will highlight that difference on both documents simultaneously (Figure 1). Click on the sub-entry for an object to highlight it on its parent document separately.

Note that this feature is purely for visual comparison of differences between versions, neither of the documents can be updated by generation of ECOs.
Not all difference updates can be pushed from the PCB back to the schematic document(s). The right-click menu items will, in such cases, not allow the direction to be set to the left (i.e. the schematic document(s)). If you select this direction individually - by clicking on the associated entry in the Decision column - the ECO that is created will not contain the update, reinforcing the fact that such a change to the schematic document is not possible/supported.

Comparing Versions of ASCII Text Documents

Not part of the Comparator, but well worth a mention, is the ability to compare two versions of a text-based ASCII document. This feature is available when comparing documents from within the Storage Manager panel, or when using the Show Local History command. Comparison will open the CompareForm dialog (Figure 2), showing a graphical 'diff' of the two versions of the document. The dialog is for comparison only - no modifications to a loaded document can be made.