The Edit Component Links dialog provides controls to check and control the status of the links between components in the schematic and PCB domains. When a component is placed on a schematic sheet, it is automatically given a unique ID. As a precursor to comparison, Altium Designer scans the source schematic and target PCB documents for linked components. These are components that have been previously synchronized with one another and share a unique ID. This dialog provides controls to manually match and link components between the two domains.
It is a good idea to have all components matched using unique IDs so that annotation of designators in either the schematic or PCB document can be carried out with the knowledge that the documents can still be re-synchronized at any stage.
When component information is transferred for the first time between schematic source documents and a blank PCB design document using the Synchronizer, all components will automatically be linked by unique ID and the ID information from each schematic component is linked to the corresponding component footprint. Refer to Design Synchronization for more information.
The dialog is accessed by clicking Project » Component Links from the PCB Editor.
Manual linking of components is only carried out from within the PCB document since only the PCB component footprints need to be updated with the unique ID information – it is already present on the schematic side.
Un-Matched Components - the left-hand side of the dialog lists components that are currently unmatched. Two lists are used for unmatched components: on the source schematic documents (left) and those unmatched components on the target PCB document (right). Each component is listed in terms of its designator, footprint name, and comment.
As you type within one of the Mask fields below a list, the list is filtered to show only strings that match the Mask string. You can use "?" and "*" wild cards in the string. For example, "*" to display all components, or "D?" to display all components that start with the letter D.
Matched Components - the right-hand side of the dialog lists all components that are currently matched. The region's two columns list the schematic components on the left and the PCB components on the right, with each entry consisting of designator, footprint name, and comment.
Keep in mind that any components that are manually matched using this dialog will be moved from the Un-Matched Components to Matched Components regions immediately, however, the actual links are not created until the Perform Update button is clicked.
Right arrow (match selected) - click to manually match the currently selected unmatched schematic component, with the currently selected unmatched PCB component. The entries will disappear from their respective Un-Matched Components lists, and a single entry for the two will be added to the Matched Components region.
Left arrow (un-match selected) - click to 'un-match' the currently selected component entries in the Matched Components region. The entries will be removed from the region, and the constituent components added back to their respective Un-MatchedComponents region lists.
Double arrow (un-match all) - click to 'un-match' all components currently listed in the Matched Components region. The entries will be removed from the region, and the constituent components added back to their respective Un-MatchedComponents region lists.
Add Pairs Matched By - click to automatically match unmatched components in accordance with the selected options to the right. Matching can be attempted by selecting any combination of Designator, Comment, and Footprint. Successful matching will result in applicable entries disappearing from their respective Un-Matched Components list and a single entry for each linked couple being added to the Matched Components region.
Perform Update - click to effect changes made to linking. If there are un-matched any components, a confirmation dialog will appear alerting you that some existing component associations will be broken by proceeding. To continue, click Yes. An information dialog will appear showing how many links were modified and/or how many links were removed.
Adding a component link (matching unmatched components) adds the unique ID of the schematic component to the linked PCB component. Conversely, removing a component link will remove the unique ID from the corresponding PCB component only. The schematic component retains the unique ID unless a new one is generated (using a reset unique ID-related command).