EDIT | EDIT3D | ERC | ERRORS | EXPORT | EXPORTSTEP
Function
Loads an existing drawing to be edited or creates a new drawing.
Syntax
EDIT name
EDIT name.ext
EDIT .ext
EDIT .sX [ .sY ]
EDIT name.mod
EDIT name.m2
EDIT .m3
EDIT modX.m3 modY.m1
EDIT;
See also OPEN, CLOSE, BOARD, MODULE.
The EDIT command opens a drawing, or, if in an open Library, opens a package, symbol, or component, for editing.
The EDIT command is also used to create or edit modules within a schematic.
| EDIT name.brd | loads a board | |
| EDIT name.sch | loads a schematic | |
| EDIT name.fpt | loads a footprint (new in EAGLE 9.1) | |
| EDIT name.pac | loads a footprint (alternative suffix for backward compatibility with older EAGLE versions) | |
| EDIT name.sym | loads a symbol | |
| EDIT name.dev | loads a device | |
| EDIT name.dbl | loads a design block in preview dialog | |
| EDIT name.dbl; | loads a new design block into the editor(s) | |
| EDIT urn | loads a footprint|symbol|device by urn | |
| EDIT .s3 | loads sheet 3 of a schematic | |
| EDIT .s5 .s2 | moves sheet 5 before sheet 2 and loads it (if sheet 5 doesn't exist, a new sheet is inserted before sheet 2) | |
| EDIT .s2 .s5 | moves sheet 2 before sheet 5 and loads it (if sheet 5 doesn't exist, sheet 2 becomes the last sheet) | |
| EDIT name.mod | loads (or creates) a module within a schematic | |
| EDIT name.m2 | loads (or creates) sheet 2 of module | |
| EDIT .m3 | loads (or creates) sheet 3 of the current module | |
| EDIT .s2 modY.m1 | moves sheet 2 before sheet 1 of module 'modY' and loads it | |
| EDIT modX.m3 modY.m1 | moves sheet 3 of module 'modX' before sheet 1 of module 'modY' and loads it | |
| EDIT; | shows table of contents (in a library) |
Wildcards in the name are allowed (for example *.brd).
The EDIT command without parameters will cause a file dialog (in board or schematic mode) or a popup menu(in library mode) to appear from which you can select the file or object.
To switch from schematic to a board with the same name, the command
EDIT .brd
can be used. In the same way, to switch from board to schematic, use the command
EDIT .sch
It is also possible to switch from the library editor to board or schematic. To edit another sheet of a schematic, use the command
EDIT .sX
(where X is the sheet number) or the combo box in the action toolbar of the editor window. If the given sheet number doesn't exist, a new sheet is created. You can also switch between sheets by clicking an icon of the sheet thumbnail preview. Drag&drop in the thumbnail preview allows you to reorder sheets.
Symbols, components, or footprints may only be edited if a library is first opened with the OPEN command. To do this, it is possible to use the name or the urn of the component.
EDIT loads files from the project directory.
Function
Edit the 3D model of an element/part in the board/schematic editor.
Syntax
EDIT3D
Mouse keys
Left selects the element/part to apply the command to.
Function
Electrical Rule Check.
Syntax
ERC
ERC is used to test schematics for electrical errors. The result of the check is presented in the ERRORS dialog.
The ERC command also performs a Consistency Check between a schematic and its corresponding board, provided the board file has been loaded before starting the ERC. As a result of this check the automatic Forward&Back Annotation will be turned on or off, depending on whether the files have been found to be consistent or not. Note that the ERC detects inconsistencies between the implicit power and supply pins in the schematic and the actual signal connections in the board. Such inconsistencies can occur if the supply pin configuration is modified after the board has been created with the BOARD command. Since the power pins are only connected "implicitly", these changes can't always be forward annotated.
If such errors are detected, Forward&Back Annotation will still be performed, but the supply pin configuration should be checked!
Function
Shows the errors found by the ERC or DRC command.
Syntax
ERRORS
ERRORS CLEAR
Use ERRORS to show the errors found by the Electrical Rule Check (ERC) or the Design Rule Check (DRC). When selected, a window opens, showing all errors. If no ERC or DRC has yet been run for the loaded drawing, the respective check is started first.
The list view in the ERRORS dialog has up to four sections that contain Consistency errors, Errors, Warnings and Approved messages, respectively.
When you select an entry, the error is marked with a rectangle and a line from the upper left corner of the screen in the editor window.
Double-clicking an entry centers the drawing on the area where the error is located. This happens automatically if you select the "Centered" checkbox.
The Processed button marks a message as processed. It is still contained in the list, but there is no error indicator in the editor window anymore (except if the list entry is selected). This can be used to mark messages as "done" after fixing the related problem, without having to run the check again. After the next ERC/DRC the message will be either gone, or marked as unprocessed again if the problem still persists.
If an error or warning can't be fixed, but apparently doesn't matter (which the user has to decide), it can be moved to the Approved section by pressing the Approve button. Messages in that section will not draw error indicators in the editor window (except if the list entry is selected) and are implicitly marked as "processed". If any of these messages no longer apply after the next ERC/DRC, they will be deleted. All approved messages are stored in the drawing file, so that it is documented which ones have been explicitly approved by the user. Note that consistency errors can't be approved - they always have to be fixed in order to activate Forward&Back Annotation.
The Clear all button deletes all entries form the list, except for the approved messages. This can be used to get rid of the error indicators in the editor window. The next ERC/DRC will regenerate the messages again, if they still apply. The list can also be cleared by entering the command
ERRORS CLEAR
Function
Generation of data files.
Syntax
EXPORT SCRIPT filename;
EXPORT NETLIST filename;
EXPORT SPICENETLIST filename;
EXPORT NETSCRIPT filename;
EXPORT PARTLIST filename;
EXPORT PINLIST filename;
EXPORT DIRECTORY filename;
EXPORT IMAGE filename|CLIPBOARD [MONOCHROME|WINDOW] resolution;
The EXPORT command is used to provide you with ASCII text files which can be used, for example, 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.
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 you want to import it again with the SCRIPT command, a new library should be opened in order to avoid duplication - for example, when the same symbol is defined more than once. Reading script files can be accelerated if you first disable the undo log with the
Set Undo_Log Off;
command.
Generates a netlist for the loaded schematic or board. Only nets which are connected to elements are listed.
Generates a spice-formatted netlist for the loaded schematic. 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 previously routed tracks have been deleted with DELETE SIGNALS. Note that while reading such a script into a board no schematic that is consistent with this board may be loaded.
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 | |
| .tif | TIFF 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.
The optional keyword WINDOW creates an image of the currently visible area in the editor window. Without this keyword, the image will contain the entire drawing.
Many further formats like DXF or Hyperlynx can be exported by ULPs. They can be started from command line using the RUN command. Under 'File/Export' a number these format exports are also available.
Function
Exports the board into a STEP file.
Syntax
EXPORTSTEP
The EXPORTSTEP command can be used in the command line or from the Export/STEP menu in the Layout Editor window. EAGLE uses the cloud service for Fusion Sync to do the translation. The STEP file can be accessed on the Control Panel's home tab. It's listed in the Recent Generated 3D files section. Clicking an entry in the list opens the file manager folder with the relevant step file.