Have a question about CadSoft EAGLE?  Ask our Expert, Richard! (Archive)

Frequently I have the need to replicate a subcircit in a schematic/board, perhaps with 10~30 parts;  now while this works fine on the schematic to select-cut/copy, it does however only dump the parts onto the layout/board and then they all need to be suitably placed/routed - my question is - "Is there a way to cut-copy from the schematic and have Eagle also replicate the board/routing of the existing copy? (obviously offset to some other part of the layout screen)"

Hi Paul,

This can be done with the help of the commands GROUP, CUT, and PASTE.

Assumed you have consistent pair of schematic and board and you would like to use one of your existing designs (also a consistent pair of sch and brd) in the current project you could begin, for example, with the schematic:

* Open the schematic you want to use in your project and use the commands GROUP and CUT to copy it into the clipboard

* Now open the schematic of your current project. You will notice that the layout editor opens the consistent layout file, too.  BUT YOU HAVE TO CLOSE IT AGAIN!
* Now use the PASTE command in the schematic and place the previously selected group.

That's it for the schematic.

Now the same procedure for the layout:
* Open the board you want to put into the clipboard and use DISPLAY ALL first to activate all layers.
* Now: GROUP, CUT. Open the "target" layout and PASTE.

Run the ERC which compares schematic and layout. This is necessary because it might happen that the names of parts or nets are renamed while pasting them into the existing project. ERC can check whether the new numbering in SCH and BRD is all the same. In the case there are differences ERC reports this and you have to adjust this manually. Until ERC reports consistency again.

=============================

There is also an explicit description in on of the CadSoft forums written by one of our useres...... I would like to add it here, as well:

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.
--------------------------------------------------

Regards,

Richard

Hi Paul,

This can be done with the help of the commands GROUP, CUT, and PASTE.

Assumed you have consistent pair of schematic and board and you would like to use one of your existing designs (also a consistent pair of sch and brd) in the current project you could begin, for example, with the schematic:

* Open the schematic you want to use in your project and use the commands GROUP and CUT to copy it into the clipboard

* Now open the schematic of your current project. You will notice that the layout editor opens the consistent layout file, too.  BUT YOU HAVE TO CLOSE IT AGAIN!
* Now use the PASTE command in the schematic and place the previously selected group.

That's it for the schematic.

Now the same procedure for the layout:
* Open the board you want to put into the clipboard and use DISPLAY ALL first to activate all layers.
* Now: GROUP, CUT. Open the "target" layout and PASTE.

Run the ERC which compares schematic and layout. This is necessary because it might happen that the names of parts or nets are renamed while pasting them into the existing project. ERC can check whether the new numbering in SCH and BRD is all the same. In the case there are differences ERC reports this and you have to adjust this manually. Until ERC reports consistency again.

=============================

There is also an explicit description in on of the CadSoft forums written by one of our useres...... I would like to add it here, as well:

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.
--------------------------------------------------

Regards,

Richard

Many thanks for that Richard.