The EXPORT command is used to provide you with ASCII text files which can be used e.g. to transfer data from EAGLE to other programs, or to generate an image file from the current drawing.
By default the output file is written into the Project directory as defined in the directories dialog.
The command generates the following output files:
A library previously opened with the OPEN command will be output as a script file. When a library has been exported and is to be imported again with the SCRIPT command, a new library should be opened in order to avoid duplication - e.g. the same symbol is defined more than once. Reading script files can be accelerated if the command
Set Undo_Log Off;is given before.
Generates a netlist for the loaded schematic or board. Only nets which are connected to elements are listed.
Generates a netlist for the loaded schematic in the form of a script file. This file can be used to read a new or changed netlist into a board where elements have already been placed or a previously routed track have been deleted with DELETE SIGNALS.
Generates a component list for schematics or boards. Only elements with pins/pads are included.
Generates a list with pads and pins, containing the pin directions and the names of the nets connected to the pins.
Lists the directory of the currently opened library.
Exporting an IMAGE generates an image file with a format corresponding to the given filename extension. The following image formats are available:
|.bmp||Windows Bitmap Files|
|.png||Portable Network Graphics Files|
|.pbm||Portable Bitmap Files|
|.pgm||Portable Grayscale Bitmap Files|
|.ppm||Portable Pixelmap Files|
|.xbm||X Bitmap Files|
|.xpm||X Pixmap Files|
The resolution parameter defines the image resolution (in 'dpi').
If filename is the special name CLIPBOARD (upper or lowercase doesn't matter) the image will be copied into the system's clipboard.
The optional keyword MONOCHROME creates a black&white image.
|Index||Copyright © 2005 CadSoft Computer GmbH|