Edit Component Links

Old Content - visit altium.com/documentation

Modified by Admin on Nov 6, 2013

The Edit Component Links Dialog.

Summary

The Edit Component Links between ... dialog enables you to check and control the status of the links between schematic components and their corresponding PCB component footprints.

Access

In PCB editor, click Project » Component Links to access this dialog.

Options/Controls

Un-Matched Reference Components - This list displays the components of schematic documents that do not have a unique ID assigned to them. When the schematics and the corresponding PCB have been synchronized, matched Schematic and PCB components can be re-annotated at any time and ECO is executed to maintain the integrity of the project design.

Un-Matched Target Components - This list displays the components of PCB documents that do not have a unique ID assigned to them. When the schematics and the corresponding PCB have been synchronized, matched Schematic and PCB components can be re-annotated at any time and ECO is executed to maintain the integrity of the project design.

Reference Mask - In this field enter string search mask for the unmatched schematic components. As you type, the list is filtered to only show strings that match the mask string. You can use the ? (any single character) and * (any characters) wildcards in the Mask string. For example, * to display all designators, D? to display all designators that start with the letter D.

Target Mask - In this field enter string search mask for the unmatched PCB components. As you type, the list is filtered to only show strings that match the mask string. You can use the ? (any single character) and * (any characters) wildcards in the Mask string. For example, * to display all designators, D? to display all designators that start with the letter D.

Matched Components - This list displays the component links between the flattened project of schematic documents and the board design. Matched components from the PCB and Schematic documents are linked by their component designators or their respective IDs are mapped in the design project file. When the schematics and the corresponding PCB have been synchronized by clicking the Perform Update button, matched Schematic and PCB components can be re-annotated at any time and ECO is executed to maintain the integrity of the project design.

Buttons

Create Soft Match - Use these buttons to add or remove components from the matched components list.
Destroy Soft Match - Use these buttons to add or remove components from the matched components list.
Remove All Matches - Use these buttons to add or remove components from the matched components list.
Add Paris Match By - Clicking this button attempts to match the schematic components and the PCB footprints depending on what options are enabled (Designators, Footprints and Comments) to add these pairs into the Matched Componentslist of the dialog.
- Designators - Clicking this button attempts to match the schematic components and the PCB footprints depending on what options are enabled (Designators, Footprints and Comments) to add these pairs into the Matched Components list of the dialog.
- Comment - When the Comment option along with other options are enabled, and the Add Pairs Matched By » button is pressed, these components are matched by their designators, comments and/or footprints depending on which options are enabled.
- Footprint - When only this Footprint option along with other options are enabled, and the Add Pairs Matched By » button is pressed, these components are matched by their designators, comments and/or footprints depending on which options are enabled.
Perform Update - Select one of the following matching methods. Update the links through the use of schematic and PCB components' unique IDs, or update the designators of PCB or schematic documents.

When a component is placed on a schematic sheet, it is given a unique ID automatically. That is why, when adding matched components in the dialog, only the PCB components need to be updated with the unique ID information.

It is a good idea to have all components matched using unique IDs, so that annotation of designators in either schematic or PCB document can be carried out, with the safe knowledge that the documents can still be resynchronized at any stage. The documents can still be synchronized even if components aren't matched by unique IDs, but in this case, you will be prompted to match the components by designators only - comment and footprint is not taken into account and therefore it is possible that matching of some components is carried out incorrectly.

Use the dialog at any stage during the design, to view the linking between components and to reassure yourself that the components on the schematic source documents are indeed correctly matched to the corresponding component footprints in the PCB design.

Unique IDs can be removed at any time by moving the linked components back to the unmatched regions of the dialog. Removing a component link will remove the unique ID from the corresponding PCB footprint only. The schematic component retains the unique ID, unless a new one is generated (using a reset unique ID-related command at either the schematic or component level).

All component information that is transferred for the first time between schematic source documents and a blank PCB design document, using the Synchronizer, will automatically link all components by unique ID.