Enhanced Footprint Compare and Update

Being able to compare and merge changes to the PCB and it's routing enable design team members - be they one or many - to keep track of design history and collaborate with each other very effectively. It is important to be able to do this, but it is not enough if the source of the components used in the design - the library - is also in a continuous state of development. The ability to check the PCB against the libraries the footprints came from now allows cell-based visual browsing of differences, and the ability to update and merge those changes into your current PCB design.

Comparing against the library and running an update

To use the footprint comparator, run the Update from PCB Libraries command from the PCB editor Tools menu. Next, you will be prompted to choose which layers of the PCB and library footprint you wish to compare. This is important, as in some designs certain layers of the footprint may not be used, and extra comparisons will take extra time to process:


Run the Update from PCB Libraries command.

Once you click OK, the comparison is executed and differences are shown in the Update from PCB Libraries dialog. A summary is given at the top showing all the components compared, with the Match status (pass or fail) indicating which components require updating. If no Match icon is shown next to a component, then that component's footprint has not been found in any of the libraries within the current Altium Designer workspace.
Under the list of components, the graphical comparison is shown. The footprint is divided up into square cells and each cell has been analyzed for the differences. Cells where differences exist are shown in full color, with the differences highlighted.


Wherever the compared cells of a component contain differences these will be highlighted.

The Layer tabs show how many primitive objects have differences for each layer that was compared, and clicking on a tab allows you to browse the differences more thoroughly. Primitive objects in the current PCB are shown full color, with the updated component primitives from the library shown as a "ghost" image over the top of them.


Browsing the differences allows you to drill-down and zoom to view each change up close.

From this dialog you can also click on Generate Report which will create and open an HTML report detailing all the differences.

Once you are satisfied with your exploration of the changes, you can click Accept Changes (Generate ECO) to run the ECO process and update the PCB with the newer footprints. You can disable change orders for specific components you do not wish to update. You can also generate an ECO report showing which components were updated.


Component updates are done through the ECO giving extra control over the process.

After this point the changes made to the components are implemented in the PCB document.


The updated component.

Footprint Comparator as a Validation Output

It is also possible to add this high-definition footprint comparator into Output Job Files as a Validation Output generator.


Add the Footprint Comparison Report output generator to your Validation Outputs.

The Footprint Comparison Report generator is configured to graphically compare footprints on the PCB to the libraries they came from in the same way as the Update from PCB Libraries process above. The difference being that it outputs an HTML report detailing the layers of each component that have differences, and which components are not linked to a library.