I am designing a PCB with many pairs each consisting of an IC and a pin header. The autorouter does a lousy job, but I found good manual routes for one pair. How can I route all the other pairs the same way, without having to re-do the routing over and over again?
There's a way, but it's treacherous. Also tedious.
Complete the layout you wish to duplicate. Save your work. Probably make a backup copy of the .sch and .brd files here to be safe.
Close the schematic editor window, but keep the board layout editor open. The layout editor will warn you with the yellow-and-black banner saying "F/B Annotation has been severed!"
Use the group tool to highlight the components and routes of the layout you wish to duplicate. Use the copy tool to copy-paste as you would in the schematic editor. Since the schematic window is severed, Eagle will allow you to copy objects now.
Open the schematic screen again. The little circle in the button-right corner will now be purple, indicating there is a mismatch between the .sch file and .brd file.
Group the exact same components and nets in the schematic window and copy-paste them. If you're very lucky, Eagle will have auto-incremented the names of every component and net the same in the schematic window and the layout window. If not, you will need to manually rename every component and net/route to be exactly the same on both windows. This is the tedious part.
When you think you've gotten everything matched up between the two windows, run the ERC. It will warn you if anything is still mismatched. Otherwise, the circle in the bottom corner will turn green and you're good to go.