I've been using eagle 6.3 for some time and I am really frustrated about copy/pasting different projects to one board file so I can send them for manufacture.
I need to panelize different projects into one.
I used to do that by cut/pasting in Eagle 5 but now the cut command is missing.
Is there any solution to that? It's a shame that Eagle Team doesn't support this action.
I've also found some downloadable ULPs from the offcial Eagle site but I dont know if there is any that does what I need.
If anyone of you, have found a workaround to this issue, please share it with us.
In older versions of EAGLE the COPY command was used solely to copy objects
within a drawing, as opposed to the Windows behavior, where COPY places a
copy of the selected objects (i.e. the GROUP) into the system's clipboard.
As of version 6, EAGLE's COPY command primarily behaves the same way as in
other Windows applications, by putting a copy of the current group into the
clipboard. The original functionality of copying selected objects, or
copying library objects between libraries, is still fully available, which
is especially important to keep existing scripts and ULPs working.
What has also often irritated Windows users is that in EAGLE the CUT
command has only copied the current group to the clipboard, but did not
actually delete the group from the drawing. Since a CUT command that
deletes the group would not be of much use in a board/schematic pair that
is connected via forward-&backannotation, the CUT command has been
removed from the main pulldown menu and the command button toolbar. It is
still fully available from the command line or within scripts. The command
SET Cmd.Copy.ClassicEagleMode 1
restores the old behavior of both the COPY and the CUT command. Note that
this setting only takes effect the next time you open an editor window.
Added a note to the online help of COPY about how to copy objects from
one schematic sheet to an other.
I think I have been able to do it by opening another instance of Eagle. Basically have 2 Eagle schem/brd files open at once. If you copy from one and close it to open another, the copy doesn't work. It's been awhile since I've had to do this, but I think that is how I did it.
You can copy-paste between two instances of Eagle. You can also copy the board, close Eagle completely, re-open Eagle, start a new board, and paste what you copied back in. I just did both methods with Eagle 6.4.0.
One thing to remember is that you have to close the schematic window (if it's open) before you paste in the board window. Otherwise Eagle will not allow you to do that - it has no way of adding to do a backwards update to the schematic.
