Extracting footprint existing PCB in Altium
Go to your board.
Select what you want to get. (Use Shift+S to set only the current layer visible and selectable)
Ctrl+C (and don't forget to mouse-click an origin after, or nothing gets copied - make it the new component origin if you like planning ahead like I do)
Go to the PCBLibrary (or make a new one)
Tools -&gt; New Blank Component
Ctrl+V
Click where you want your pads.
Edit the component properties and 3D model as required.
Ctrl+S
Done.
EDIT: Following our chat
For posterity, to quickly select a group of objects with same or similar properties, you can use:
Right-Click on object: Select &quot;Find Similar Objects&quot;
In the menu find the properties that are unique to the group of objects and select &quot;same&quot; from the dropdown.
Select Apply and then Ok and you get a listing for all the items matching your parameters, while they also become selected. (Technically usually only Ok works, but it may sometimes give the dreaded DLL based pop-up of doom, while preceding it with apply never gave me that).
To select on part of a parameter you can use an Asterisk (), like selecting all objects with a name that starts with JP, you can select &quot;same&quot; in &quot;Name&quot; and type &quot;JP&quot; and all JP1, JP101, JP2938, etc will become selected.