This thread is now locked - but you can still ask Richard by posting your questions here. If you'd rather browse other member's questions you can read the CadSoft EAGLE Forums for past questions and answers. Enjoy!
Browse past Q&A help on anything technical relating to CadSoft EAGLE!
Richard Hammerl
Richard is an engineer with 16 years experience in EAGLE customer support and is waiting for your questions.
Hi Marc,
this question was asked recently, I believe in the same thread. But since there more than 700 entries this thread begins (since a long time) to become more and more unreadable...... 
But here a possible solution for your request:
The Procedure:
--------------------------------------------------
Sometimes circuit boards will have duplicate sections of schematic that you
want to layout identically. You could do this by laying out each section
separately, but for large or complex layouts this would be very time
consuming. Eagle does not have a function that allows you to directly
duplicate your layouts, so you have to use this workaround:
1. Create the schematic for the section you want to duplicate. You can have
additional schematic done at that time too if you like.
2. Create the layout for that section. You can have additional layout done
at that time if you like.
3. Close the layout so that you only have the schematic open.
4. Use the window selection tool to surround the section of schematic you
want to duplicate in the layout.
5. Use the scissors tool to copy the selection to the buffer.
6. Use the dropdown EDIT: PASTE to finish the copy operation.
7. Save the schematic and close it.
8. Open the layout. Click OK to acknowledge the warning about the schematic
and board not being consistent. Close the schematic that opened when you
opened the layout so that you only have the layout open.
9. Do the same window select, scissors, paste operation on the layout. YOU
MUST COPY EXACTLY THE SAME ITEMS AS YOU DID IN THE SCHEMATIC. THIS INCLUDES
COMPONENTS AND NETS.
10. Save the layout and open the schematic. You should have both the
schematic and layout open at this point.
11. In the layout, run ERC and you'll get a long list of nets that don't
match. Don't worry: you only have to fix each net once. This is usually
only 5 or 6 nets to fix the whole list.
12. The original section of layout will have nets named GND. The new
section will have them named GND1. The original section of the schematic
will have the nets named GND. The new section will also have them named
GND. The task here is to rename the net GND1 to GND in the layout.
13. Type "show GND1" in the command line. This will highlight GND1.
14. Use the name tool (R2 Icon) to change the name GND1 to GND. If
prompted, the rename applies to all nets.
15. If you run ERC again, you'll find that all of the GND/GND1 errors are
gone. Redo this renaming process a few more times for the remaining name1
nets and you're done.
Additional note: If you don't have any airwires for the net you're trying to
rename then you'll have to create one using the line tool and the name tool:
Create a line. Rename that line using the R2 tool to the net name you need
to rename (e.g. GND1). This will connect the line to the pad that was
previously un-airwired. Now you can rename the airwire or line to the right
name (e.g. GND) to fix that net.
--------------------------------------------------
This was initially posted in the eagle.support.eng forum....
Regards,
Richard
