| EAGLE Help Version 7.1.0 | Copyright © 2014 CadSoft Computer GmbH |
You can also display an editor command's help page by entering
HELP commandreplacing "command" with, e.g., MOVE, which would display the help page for the MOVE command.
Anywhere else, pressing the F1 key will bring up a context sensitive help page for the menu, dialog or action that is currently active.
For detailed information on how to get started with EAGLE please read the following help pages:
The following editor commands can be used to customize the way EAGLE works. They can be given either directly from an editor window's command line, or in the eagle.scr file.
| Command menu | MENU command..; | |
| Assign keys | ASSIGN function_key command..; | |
| Snap function | SET SNAP_LENGTH number; | |
| SET CATCH_FACTOR value; | ||
| SET SELECT_FACTOR value; | ||
| Content of menus | SET USED_LAYERS name | number; | |
| SET WIDTH_MENU value..; | ||
| SET DIAMETER_MENU value..; | ||
| SET DRILL_MENU value..; | ||
| SET SMD_MENU value..; | ||
| SET SIZE_MENU value..; | ||
| SET ISOLATE_MENU value..; | ||
| SET SPACING_MENU value..; | ||
| SET MITER_MENU value..; | ||
| Wire bend | SET WIRE_BEND bend_nr; | |
| Beep on/off | SET BEEP OFF | ON; |
| Color for grid lines | SET COLOR_GRID color; | |
| Color for layer | SET COLOR_LAYER layer color; | |
| Fill style for layer | SET FILL_LAYER layer fill; | |
| Grid parameter | SET MIN_GRID_SIZE pixels; | |
| Min. text size displayed | SET MIN_TEXT_SIZE size; | |
| Display of net lines | SET NET_WIRE_WIDTH width; | |
| Display of pads | SET DISPLAY_MODE REAL | NODRILL; | |
| SET PAD_NAMES OFF | ON; | ||
| Display of bus lines | SET BUS_WIRE_WIDTH width; | |
| DRC fill style | SET DRC_FILL fill_name; | |
| Polygon processing | SET POLYGON_RATSNEST OFF | ON; | |
| Vector font | SET VECTOR_FONT OFF | ON; |
| Package check | SET CHECK_CONNECTS OFF | ON; | |
| Grid parameters | GRID options; | |
| Replace mode | SET REPLACE_SAME NAMES | COORDS; | |
| UNDO Buffer | SET UNDO_LOG OFF | ON; | |
| Wire Optimizing | SET OPTIMIZING OFF | ON; | |
| Net wire termination | SET AUTO_END_NET OFF | ON; | |
| Automatic junctions | SET AUTO_JUNCTION OFF | ON; |
| Pad shape | CHANGE SHAPE shape; | |
| Wire width | CHANGE WIDTH value; | |
| Pad/via diameter | CHANGE DIAMETER diameter; | |
| Pad/via/hole drill diam. | CHANGE DRILL value; | |
| Smd size | CHANGE SMD width height; | |
| Text height | CHANGE SIZE value; | |
| Text thickness | CHANGE RATIO ratio; | |
| Text font | CHANGE FONT font; | |
| Text alignment | CHANGE ALIGN align; | |
| Polygon parameter | CHANGE THERMALS OFF | ON; | |
| Polygon parameter | CHANGE ORPHANS OFF | ON; | |
| Polygon parameter | CHANGE ISOLATE distance; | |
| Polygon parameter | CHANGE POUR SOLID | HATCH | CUTOUT; | |
| Polygon parameter | CHANGE RANK value; | |
| Polygon parameter | CHANGE SPACING distance; | |
| Dimension type | CHANGE DTYPE value; |
eagle [ options [ filename [ layer ] ] ]
| -Axxx | Assembly variant | |
| -Cxxx | execute the given Command | |
| -Dxxx | Draw tolerance (0.1 = 10%) | |
| -Exxx | Drill tolerance (0.1 = 10%) | |
| -Fxxx | Flash tolerance (0.1 = 10%) | |
| -N- | no command line prompts | |
| -O+ | Optimize pen movement | |
| -Pxxx | plotter Pen (layer=pen) | |
| -Rxxx | drill Rack file | |
| -Sxxx | Scriptfile | |
| -Uxxx | User settings file | |
| -Wxxx | aperture Wheel file | |
| -X- | eXecute CAM Processor | |
| -c+ | positive Coordinates | |
| -dxxx | Device (-d? for list) | |
| -e- | Emulate apertures | |
| -f+ | Fill pads | |
| -hxxx | page Height (inch) | |
| -m- | Mirror output | |
| -oxxx | Output filename | |
| -pxxx | Pen diameter (mm) | |
| -q- | Quick plot | |
| -r- | Rotate output 90 degrees | |
| -sxxx | Scale factor | |
| -u- | output Upside down | |
| -vxxx | pen Velocity | |
| -wxxx | page Width (inch) | |
| -xxxx | offset X (inch) | |
| -yxxx | offset Y (inch) |
where xxx means that further data, e.g. a file name or a decimal number needs to be appended to the option character (without space or separated by a space), as in
-Wmywheel.whl -W mywheel.whl -e Aperture emulation on -e+ dto. -e- Aperture emulation offFor flag options, a '-' means that the option is off by default, while '+' means it is on by default.
Flag options (e.g. -e) can be used without repeating the '-' character:
| -ecfm | Aperture emulation on, positive oordinates on, fill pads on | |
| -ec-f+ | Aperture emulation on, positive oordinates off, fill pads on |
| On Windows it is stored in the file eaglerc.usr under the directory that is defined by the registry key "HKEY_CURRENT_USER\Software\Microsoft\Windows\CurrentVersion\Explorer\Shell Folders\AppData" if no environment variable named HOME is defined. |
If a '-' sign is given as the file name, as in -U-, no eaglerc file will be read or written.
| -D0.10 | adjusts the draw tolerance to ±10% | |
| -D+0.1 -D-0.05 | adjusts the draw toleranceto +10% and -5% |
eagle -C "window (1 1) (2 2);" myboard.brdEAGLE will load the given file and execute the command as if it had been typed into the editor window's command line.
The following conditions apply for the '-C' option:
eagle -C ""Note that in this special case there must be a blank between the option character and the quotes, so that the program will see the explicitly empty string. There also doesn't have to be a file name here, because no command will actually be executed.
Wherever coordinates or sizes (like width, diameter etc.) can be entered, they may
be given with units, as in 50mil or 0.8mm. If no unit is given, the current grid unit is used.
Drawing a Schematic
Create a Schematic File
Use File/New and Save as to create a schematic with a name of your
choice.
Load a Drawing Frame
Load library FRAMES with USE and place a frame of your choice with ADD.
All the components, together with their connections drawn as airwires, appear beside a blank board ready for placing. Power pins are automatically connected to the appropriate supply (if not connected by a net on the schematic).
The board is linked to the schematic via Forward&Back Annotation. This mechanism makes sure that schematic and board are consistent. When editing a drawing, board and schematic must be loaded to keep Forward&Back Annotation active.
To start, open a library. Use the File menu Open or New command (not the USE command).
Click the Edit Package icon and edit a new package by typing its name in the New field of the dialog box.
Set the proper distance GRID.
Add texts >NAME and >VALUE with the TEXT command (show actual name and value in the board) and draw package outlines (WIRE command) in the proper layers.
Click the Edit Symbol icon and edit a new symbol by typing its name in the New field of the dialog box.
Place and name pins with the commands PIN and NAME and provide pin parameters (CHANGE).
Add texts >NAME and >VALUE with the TEXT command (show actual name and value in the schematic) and draw symbol outlines (WIRE command) in the proper layers.
Click the Edit Device icon and edit a new device by typing its name in the New field of the dialog box.
Assign the package with the PACKAGE command.
Add the gate(s) with ADD, you can have as many gates as needed.
Use CONNECT to specify which of the packages pads are connected to the pins of each gate.
Save the library and you can USE it from the schematic or board
editor.
Control Panel
The Control Panel is the top level window of EAGLE.
It contains a tree view on the left side, and an information window on the right side.
Directories
The top level items of the tree view represent the various types of EAGLE files.
Each of these can point to one or more directories that contain files of that type.
The location of these directories can be defined with the directories dialog.
If a top level item points to a single directory, the contents of that directory will
appear if the item is opened (either by clicking on the little symbol to the left, or by
double clicking the item). If such an item points to more directories, all of these
directories will be listed when the item is opened.
| Directories | a file named DESCRIPTION in that directory | |
| Libraries | the description of the library | |
| Devices | the description of the device | |
| Packages | the description of the package | |
| Design Rules | the description of the design rules file | |
| User Language Programs | the text defined with the #usage directive | |
| Scripts | the comment at the beginning of the script file | |
| CAM Jobs | the description of the CAM job |
| New | create a new file | |
| Open | open an existing file | |
| Open recent projects | open a recently used project | |
| Save all | save all modified editor files | |
| Close project | close the current project | |
| Exit | exit from the program |
| Refresh | refresh the contents of the tree view | |
| Search in tree | search in the contents of the tree view (see below) | |
| Sort | change the sorting of the tree view |
| Directories... | opens the directories dialog | |
| Backup... | opens the backup dialog | |
| User interface... | opens the user interface dialog | |
| Window positions... | opens the window positions dialog |
| Control Panel | switch to the Control Panel | |
| 1 Schematic - ... | switch to window number 1 | |
| 2 Board - ... | switch to window number 2 |
| General | opens a general help page | |
| Context | opens the help page for the current context | |
| Control Panel | opens the help page you are currently looking at | |
| EAGLE License | opens the license dialog | |
| Check for Update | checks if a new version of EAGLE is available | |
| About EAGLE | displays details on your EAGLE version and license |
Printing a file through this context menu option will always print the file
as it is on disk, even if you have an open editor window in which you have
modified the file! Use the PRINT command to
print the drawing from an open editor window.
Please note that polygons in boards will not be automatically calculated
when printing via the context menu! Only the outlines will be drawn.
To print polygons in their calculated shape you have to load the drawing
into an editor window, enter RATSNEST
and then PRINT.
All entries may contain one or more directories, separated by a colon (':'), in which to look for the various types of files.
| On Windows the individual directory names are separated by a semicolon (';'). |
The special variables $HOME and $EAGLEDIR can be used to reference the user's home directory and the EAGLE program directory, respectively.
| On Windows the value of $HOME is either that of the environment variable HOME (if set), or the value of the registry key "HKEY_CURRENT_USER\Software\Microsoft\Windows\CurrentVersion\Explorer\Shell Folders\Personal", which contains the actual name of the "My Documents" directory. |
| Pulldown menu | activates the pulldown menu at the top of the editor window | |
| Action toolbar | activates the action toolbar containing buttons for "File", "Print" etc. | |
| Parameter toolbar | activates the dynamic parameter toolbar, which contains all the parameters that are available for the currently active command | |
| Command buttons | activates the command buttons | |
| Command texts | activates the textual command menu | |
| Sheet thumbnails | aktivates the sheet thumbnail preview |
| Background | selects a black, white or colored background for the layout mode | |
| Cursor | selects a small or large cursor for the layout mode |
| Background | selects a black, white or colored background for the schematic mode | |
| Cursor | selects a small or large cursor for the schematic mode |
| New drawings | selects the reading direction of vertical texts in newly created drawings | |
| This drawing | selects the reading direction of vertical texts in the currently loaded drawing |
| Bubble help | activates the "Bubble Help" function, which pops up a short hint about the meaning of several buttons when moving the cursor over them | |
| User guidance | activates the "User Guidance" function, which displays a helping text telling the user what would be the next meaningful action when a command is active |
| Always vector font | always displays texts in drawings with the builtin vector font, regardless of which font is actually set for a particular text | |
| Mouse wheel zoom | defines the zoom factor that will be used to zoom in and out of an editor window when the mouse wheel is turned ('0' disables this feature, the sign of this value defines the direction of the zoom operation) |
You can also delete all stored window positions, so that the window manager
can decide again where to place newly opened windows.
The Configure button opens a dialog in which you can specify if and
how often a check for new versions should be done automatically upon program
start (by default it checks once per day). If you need to use a proxy to access
the Internet, this can also be specified in the configuration dialog. In the "Host"
field enter the full name of the proxy host, without any
http:// prefix, and enter an optional port number in the "Port" field.
If you would like to be informed about beta versions of EAGLE, you can check
the "Also check for beta versions" box.
Check for Update
The option "Help/Check for Update" in the Control Panel's pulldown menu opens
a dialog that displays whether there is a new version of EAGLE available on
the CadSoft server.
Keyboard and Mouse
The modifier keys (Alt, Ctrl and Shift) are used
to modify the behavior of certain mouse actions.
Note that depending on which operating system or window manager you use, some of these
keys (in combination with mouse events) may not be delivered to applications, which means
that some of the functions described here may not be available.
Alt
Pressing the Alt key switches to an alternate GRID.
This can typically be a finer grid than the normal one, which allows you to quickly
do some fine positioning in a dense area, for instance, where the normal grid might
be too coarse.
The alternate grid remains active as long as the Alt key is held pressed down.
Ctrl
Pressing the Ctrl key while clicking on the right mouse button toggles
between corresponding wire bend styles (only applies to commands that support wire
bend styles, like, for instance, WIRE).
The Ctrl key together with the left mouse button controls special functionality of individual commands, like, for instance, selecting an object at its origin with the MOVE command.
If a command can select a group, the Ctrl key must be pressed together with the right mouse button when selecting the group (otherwise a context menu for the selected object would be opened).
| On Mac OS X the Cmd key has to be used instead of the Ctrl key. |
The Shift key together with the left mouse button controls special functionality of individual commands, like, for instance, deleting a higher level object with the DELETE command.
The following commands support the center mouse button:
| ADD | mirror part | |
| ARC | change active layer | |
| CIRCLE | change active layer | |
| COPY | mirror object | |
| INVOKE | mirror gate | |
| LABEL | change active layer | |
| MOVE | mirror object or group | |
| PASTE | mirror group | |
| POLYGON | change active layer | |
| RECT | change active layer | |
| ROUTE | change active layer | |
| SMD | change active layer | |
| TEXT | change active layer | |
| WIRE | change active layer |
Click&Drag with the center mouse button will pan the drawing within the editor window.
When selecting an object with the right mouse button, a context specific popup menu is displayed from which commands that apply to this object can be selected. If there is currently a command active that can be applied to a group, the popup menu will contain an entry for this.
The following commands support the right mouse button:
| ADD | rotate part | |
| ARC | change direction of arc | |
| BUS | change wire bend | |
| CHANGE | apply change to group | |
| DELETE | delete group | |
| GROUP | close polygon | |
| INVOKE | rotate gate | |
| LABEL | rotate label | |
| MIRROR | mirror group | |
| MOVE | rotate object, select group | |
| NET | change wire bend | |
| PAD | rotate pad | |
| PASTE | rotate group | |
| PIN | rotate pin | |
| POLYGON | change wire bend | |
| RIPUP | ripup group | |
| ROTATE | rotate group | |
| ROUTE | change wire bend | |
| SMD | rotate smd | |
| SPLIT | change wire bend | |
| TEXT | rotate text | |
| WIRE | change wire bend |
Select highlighted object? (left=yes, right=next, ESC=cancel)
indicates that you can now choose one of these objects.
Press the right mouse button to switch to the next object.
Press the left mouse button to select the highlighted object.
Press Esc to cancel the selection procedure.
The command
SET Select_Factor select_radius;defines the selection radius.
If the original selection was done with the right mouse button, a context specific
popup menu will be displayed which applies to the first selected object, and which
contains "Next" as the first entry. Clicking on this entry will cyclically switch
through the objects within the selection radius.
Editor Windows
EAGLE knows different types of data files, each of which has its own
type of editor window. By double clicking on one of the items in the
Control Panel or by selecting a file from the
File/Open menu, an editor
window suitable for that file will be opened.
After opening a new library editor window, the edit area will be empty and
you will have to use the EDIT command to select
which package, symbol or device you want to edit or create.
Package: the package definition.
Symbol: the symbol as it appears in the circuit diagram.
Device: definition of the whole component. Contains one or more
package variants and one or several symbols (e.g. gates).
The symbols can be different from each other.
Click on the Dev, Pac or
Sym button to select Device, Packages or Symbols,
respectively.
If you want to create a new object, write the name of the new object into
the New field. You can also edit an existing object
by typing its name into this field. If you omit the extension, an object
of the type indicated by the Choose... prompt will be
loaded. Otherwise an object of the type indicated by the extension will
be loaded.
If your license does not include
the Schematic Module, the object type buttons (Dev...)
will not appear in the menu.
When there is a schematic file (*.sch) with the same name as the
board file (in the same directory), opening a board editor window will
automatically open a Schematic Editor
window containing that file and will put it on the desktop
as an icon. This is necessary to have the schematic file loaded when editing
the board causes modifications that have to be
back-annotated
to the schematic.
When there is a board file (*.brd) with the same name as the
schematic file (in the same directory), opening a schematic editor window will
automatically open a Board Editor
window containing that file and will put it on the desktop
as an icon. This is necessary to have the board file loaded when editing
the schematic causes modifications that have to be
forward-annotated
to the board.
The combo box in the action toolbar of the schematic editor window allows
you to switch between the various sheets of the schematic, or to add new
sheets to the schematic (this can also be done using the
EDIT command).
The text must be a pure ASCII file and must not contain any control codes.
The main area of use for the text editor is writing
User Language Programs and
Script files.
Within that command the following placeholders will be replaced with
actual values:
Edit Library Object
In library edit mode you can edit packages, symbols, and devices.
Board Editor
The Board Editor is used to edit a board (*.brd).
Schematic Editor
The Schematic Editor is used to edit a schematic (*.sch).
Text Editor
The Text Editor is used to edit any kind of text.
Using an external text editor
If you prefer to use an external text editor instead of EAGLE's builtin text
editor, you can specify the command necessary to start that editor in the
"Options/User interface" dialog.
| %C | the column in which to place the cursor (currently always 1) | |
| %F | the name of the file to load | |
| %L | the line in which to place the cursor |
If the command consists only of a hyphen ('-'), EAGLE will never open a text editor window. This may be useful for people who always start their text editor by themselves.
The following restrictions apply when using an external text editor:
| CLOSE | Close drawing after editing | |
| EDIT | Load/create a drawing | |
| EXPORT | Generate ASCII list (e.g. netlist) | |
| OPEN | Open library for editing | |
| QUIT | Quit EAGLE | |
| REMOVE | Delete files/library elements | |
| SCRIPT | Execute command file | |
| USE | Load library for placing elements | |
| WRITE | Save drawing/library |
| ADD | Add element to drawing/symbol to device | |
| ARC | Draw arc | |
| ATTRIBUTE | Define attributes | |
| CIRCLE | Draw circle | |
| CLASS | Define net classes | |
| COPY | Copy objects/elements | |
| CUT | Cut previously defined group | |
| DELETE | Delete objects | |
| DESCRIPTION | Change an object's description | |
| GROUP | Define group for upcoming operation | |
| HOLE | Define non-conducting hole | |
| LAYER | Create/change layer | |
| MIRROR | Mirror objects | |
| MITER | Miter wire joints | |
| MODULE | Create module and add module instances | |
| MOVE | Move or rotate objects | |
| NAME | Name object | |
| PASTE | Paste previously cut group to a drawing | |
| PORT | Add port to module | |
| POLYGON | Draw polygon | |
| RECT | Draw rectangle | |
| ROTATE | Rotate objects | |
| SMASH | Prepare NAME/VALUE text for moving | |
| SPLIT | Bend wires/lines (tracks, nets, etc.) | |
| TEXT | Add text to a drawing | |
| VALUE | Enter/change value for component | |
| WIRE | Draw line or routed track |
| DRC | Perform design rule check | |
| ERRORS | Show DRC errors | |
| LOCK | Lock component's position | |
| RATSNEST | Show shortest air lines | |
| REPLACE | Replace component | |
| RIPUP | Ripup routed track | |
| ROUTE | Route signal | |
| SIGNAL | Define signal (air line) | |
| VIA | Place via-hole |
| BOARD | Create a board from a schematic | |
| BUS | Draw bus line | |
| ERC | Perform electrical rule check | |
| GATESWAP | Swap equivalent 'gates' | |
| INVOKE | Add certain 'gate' from a placed device | |
| JUNCTION | Place connection point | |
| LABEL | Provide label to bus or net | |
| NET | Define net | |
| PINSWAP | Swap equivalent pins |
| CONNECT | Define pin/pad assignment | |
| PACKAGE | Define package for device | |
| PAD | Add pad to a package | |
| PIN | Add pin to a symbol | |
| PREFIX | Define default prefix for device | |
| REMOVE | Delete library elements | |
| RENAME | Rename symbol/package/device | |
| SMD | Add smd pad to a package | |
| TECHNOLOGY | Define technologies for a device | |
| VALUE | Define if value text can be changed |
| ASSIGN | Assign keys | |
| CHANGE | Change parameters | |
| DISPLAY | Display/hide layers | |
| GRID | Define grid/unit | |
| MENU | Configure command menu | |
| SET | Set program parameters | |
| WINDOW | Choose screen window |
| AUTO | Start Autorouter | |
| HELP | Show help page | |
| INFO | Show information about object | |
| MARK | Set/remove mark (for measuring) | |
| OPTIMIZE | Optimize (join) wire segments | |
| Print to the system printer | ||
| REDO | Redo commands | |
| RUN | Run User Language Program | |
| SHOW | Highlight object | |
| UNDO | Undo commands | |
| UPDATE | Update library objects |
Commands and parameters in CAPITAL LETTERS are entered directly (or selected in the command menu with the mouse). For the input there is no difference between small and capital letters.
Parameters in lowercase letters are replaced by names, number values or key words. Example:
| Syntax: | GRID grid_size grid_multiple; | |
| Input: | GRID 1 10; |
| Syntax: | SET BEEP OFF | ON; | |
| Input: | SET BEEP OFF; | |
| or | ||
| SET BEEP ON; |
| Syntax: | DISPLAY option layer_name.. | |
| Input: | DISPLAY TOP PINS VIAS |
| Syntax: | MOVE .. | |
| Input: | MOVE | |
| Mouse click on the first element to be moved | ||
| Mouse click on the target position | ||
| Mouse click on the second element to be moved | ||
| etc. |
This example also explains the meaning of the repetition points for commands with mouse clicks.
For the program each mouse click is the input of a coordinate. If coordinates are to be entered as text, the input via the keyboard must be as follows:
(x y)x and y are numbers in the unit which has been selected with the GRID command. The input as text is mainly required for script files.
(100mil 200mil)Allowed units are mm, mic, mil and in. It is possible to use different units for x and y.
(@)can be used to reference the current position of the mouse cursor within the draw window. For example, the input
MOVE R1 (@)would move the part named R1 to the place currently pointed to with the mouse.
Any combination of the following modifiers may follow the opening brace in order to simulate a particular key that is held pressed with the "mouse click" or to change the type of coordinates:
| > | right mouse button click | |
| A | Alt key | |
| C | Ctrl key | |
| P | Polar coordinates (relative to the mark, x = radius, y = angle in degrees, counterclockwise) | |
| R | Relative coordinates (relative to the mark) | |
| S | Shift key |
(CR> 1 2)would result in a "right button mouse click" at (1 2) relative to the mark, with the Ctrl key held down (of course what happens with this kind of input will depend on the actual command). Note that if there is currently no mark defined, coordinates with R or P will be relative to the drawing's origin. Also, the modifier characters are not case sensitive, their sequence doesn't matter and there doesn't have to be a blank between them and the first coordinate digit. So the above example could also be written as (r>c1 2). Values entered as "polar coordinates" will be stored internally as the corresponding pair of (x y) coordinates.
As an example for entering coordinates as text let's assume you wish to enter the exact dimensions for board outlines:
GRID 1 MM; CHANGE LAYER DIMENSION; WIRE 0 (0 0) (160 0) (160 100) (0 100) (0 0); GRID LAST;
WINDOW;redraws the drawing window, whereas
WINDOW FITscales the drawing to fit entirely into the drawing window. There is no semicolon necessary here because it is already clear that the command is complete.
The ADD command fetches a circuit symbol (gate) or a package from the active library and places it into the drawing.
During device definition the ADD command fetches a symbol into the device.
Usually you click the ADD command and select the package or symbol from the menu which opens. If necessary, parameters can now be entered via the keyboard.
If device_name contains wildcard characters ('*' or '?') and more than one device matches the pattern, the ADD dialog will be opened and the specific device can be selected from the list. Note that the Description checkbox in the ADD dialog will be unchecked after any ADD command with a device_name has been given in the command line, no matter if it contains wildcards or not. This is because a device_name entered in the command line is only searched for in the device names, not in the descriptions.
The package or symbol is placed with the left button and rotated with the right button. After it has been placed another copy is immediately hanging from the cursor.
If there is already a device or package with the same name (from the same library) in the drawing, and the library has been modified after the original object was added, an automatic library update will be started and you will be asked whether objects in the drawing shall be replaced with their new versions. Note: You should always run a Design Rule Check (DRC) and an Electrical Rule Check (ERC) after a library update has been performed!
To add directly from a specific library, the command syntax
ADD devicename@librarynamecan be used. devicename may contain wildcards and libraryname can be either a plain library name (like "ttl" or "ttl.lbr") or a full file name (like "/home/mydir/myproject/ttl.lbr" or "../lbr/ttl"). In case of blanks in the file name the whole expression has to be enclosed by apostrophs (like ADD 'DEV1A@/home/my dir/ttl.lbr').
Example:
ADD DIL14 IC1 fetches the DIL14 package to the board and gives it the name IC1.
If no name is given in the schematic, the gate will receive the prefix that was specified in the device definition with PREFIX, expanded with a sequential number (e.g. IC1).
Example:
ADD 7400 This will place a sequence of five gates from 7400 type components. Assuming that the prefix is defined as "IC" and that the individual gates within a 7400 have the names A..D, the gates in the schematic will be named IC1A, IC1B, IC1C, IC1D, IC2A. (If elements with the same prefix have already been placed the counting will proceed from the next sequential number.) See also INVOKE.
While an object is attached to the cursor, you can change the name under which it will be added to the drawing. This allows you to add several parts of the same type, but with different, explicitly defined names:
Example:
ADD CAP C1 C5 C7
Example:
ADD 7400 IC1 A This is mainly useful if a schematic is to be generated through a script. Note that if a particular gate is added, no other gates with add level MUST or ALWAYS will be fetched automatically, and you will have to use the INVOKE command to invoke at least the MUST gates (otherwise the Electrical Rule Check will report them as missing).
[S][M]Rnnn
| S | sets the Spin flag, which disable keeping texts readable from the bottom or right side of the drawing (only available in a board context) | |
| M | sets the Mirror flag, which mirrors the object about the y-axis | |
| Rnnn | sets the Rotation to the given value, which may be in the range 0.0...359.9 (at a resolution of 0.1 degrees) in a board context, or one of 0, 90, 180 or 270 in a schematic context (angles may be given as negative values, which will be converted to the corresponding positive value) |
The key letters S, M and R may be given in upper- or lowercase, and there must be at least R followed by a number.
If the Mirror flag is set in an element as well as in a text within the element's package, they cancel each other out. The same applies to the Spin flag.
Examples:
| R0 | no rotation | |
| R90 | rotated 90° counterclockwise | |
| R-90 | rotated 90° clockwise (will be converted to 270°) | |
| MR0 | mirrored about the y-axis | |
| SR0 | spin texts | |
| SMR33.3 | rotated 33.3° counterclockwise, mirrored and spin texts |
Default: R0
ADD DIL16 R90 (0 0);places a 16-pin DIL package, rotated 90 degrees counterclockwise, at coordinates (0 0).
| 0: | The symbol (gate) can not be swapped with any other in the schematic. | |
| >0 | The symbol (gate) can be swapped with any other symbol of the same type in the schematic that has the same swaplevel (including swapping between different devices). |
Default: 0
| Next | If a device has more than one gate, the symbols are fetched into the schematic with Addlevel Next. | |
| Must | If any symbol from a device is fetched into the schematic, then a symbol defined with Addlevel Must must also appear. This happens automatically. It cannot be deleted until all the other symbols in the device have been deleted. If the only symbols remaining from a device are Must-symbols, the DELETE command will delete the entire device. | |
| Always | Like Must, although a symbol with Addlevel Always can be deleted and brought back into the schematic with INVOKE. | |
| Can | If a device contains Next-gates, then Can-gates are only fetched if explicitly called with INVOKE. A symbol with Addlevel Can is only then fetched into the schematic with ADD if the device only contains Can-gates and Request-gates. | |
| Request | This property is usefully applied to devices' power-symbols. Request-gates can only be explicitly fetched into the schematic (INVOKE) and are not internally counted. The effect of this is that in devices with only one gate and one voltage supply symbol, the gate name is not added to the component name. In the case of a 7400 with four gates (plus power supply) the individual gates in the schematic are called, for example, IC1A, IC1B, IC1C and IC1D. A 68000 with only one Gate, the processor symbol, might on the other hand be called IC1, since its separate voltage supply symbol is not counted as a gate. |
Example:
ADD PWR 0 REQUEST fetches the PWR symbol (e.g. a power pin symbol), and defines a Swaplevel of 0 (not swappable) and the Addlevel Request for it.
The ARC command, followed by three mouse clicks on a drawing, draws an arc of defined width. The first point defines a point on a circle, the second its diameter. Entering the second coordinate reduces the circle to a semi-circle, while the right button alters the direction from first to second point. Entry of a third coordinate truncates the semi-circle to an arc extending to a point defined by the intersection of the circumference and a line between the third point and the arc center.
The parameters CW and CCW enable you to define the direction of the arc (clockwise or counterclockwise). ROUND and FLAT define whether the arc endings are round or flat, respectively.
CHANGE WIDTH width;The adjusted width is identical to the line width for wires.
Arcs with angles of 0 or 360 degrees or a radius of 0 are not accepted.
Example for text input:
GRID inch 1; ARC CW (0 1) (0 -1) (1 0);generates a 90-degree arc with the center at the origin.
function_key = modifier+key
modifier = any combination of S (Shift), C (Control), A (Alt) and M (Cmd, Mac OS X only)
key = F1..F12, A-Z, 0-9, BS (Backspace)
The ASSIGN command can be used to define the meaning of the function keys F1 thru F12, the letter keys A thru Z, the (upper) digit keys 0 thru 9 and the backspace key (each also in combination with modifier keys).
The ASSIGN command without parameters displays the present key assignments in a dialog, which also allows you to modify these settings.
Keys can be assigned a single command or multiple commands. The command sequence to be assigned should be enclosed in apostrophes.
If key is one of A-Z or 0-9, the modifier must contain at least A, C or M.
| The M modifier is only available on Mac OS X. |
Please note that any special operating system function assigned to a function
key will be overwritten by the ASSIGN command
(depending on the operating system, ASSIGN may not be able to overwrite
certain function keys).
If you assign to a letter key together with the modifier A,
(e.g. A+F), a corresponding hotkey from the pulldown menu is
no longer available.
To remove an assignment from a key you can enter ASSIGN with only the function_key code, but no command.
ASSIGN F7 'change layer top; route'; ASS A+F7 'cha lay to; rou'; ASSIGN C+F10 menu add mov rou ''';''' edit; ASSIGN CA+R 'route';The first two examples have the same effect, since EAGLE allows abbreviations not only with commands but also with parameters (as long as they are unmistakable).
Please note that here, for instance, the change layer top command is terminated by a semicolon, but not the route command. The reason is that in the first case the command already contains all the necessary parameters, while in the second case coordinates still have to be added (usually with the mouse). Therefore the ROUTE command must not be deactivated by a semicolon.
| F1 HELP | Help function | |
| Alt+F2 WINDOW FIT | The whole drawing is displayed | |
| F2 WINDOW; | Screen redraw | |
| F3 WINDOW 2 | Zoom in by a factor of 2 | |
| F4 WINDOW 0.5 | Zoom out by a factor of 2 | |
| F5 WINDOW (@); | Cursor pos. is new center | |
| F6 GRID; | Grid on/off |
Further, many useful key assignments are contained in the initialisation script eagle.scr
and can be adjusted to your individual needs.
ATTRIBUTE
See also TECHNOLOGY,
NAME,
VALUE,
SMASH,
TEXT
ATTRIBUTE part_name attribute_name
ATTRIBUTE part_name attribute_name 'attribute_value' [ [ orientation ] ]
ATTRIBUTE part_name attribute_name DELETE
ATTRIBUTE * [ name [ 'value' ] ]
ATTRIBUTE * name DELETE
ATTRIBUTE ..
See the description of orientation at ADD.
An attribute is an arbitrary combination of a name and a value, that can be used to specify any kind of information for a given part.
Attributes can be defined in the library (for individual devices), in the schematic (for an actual part) or in the board (for an actual element). Attributes defined on the device level will be used for every part of that device type in the schematic. In a schematic, additional attributes can be defined for each part, and existing attributes from the devices can be overwritten with new values (if the attributes have been defined as variable). An element in the board has all the attributes of its corresponding part, and can have further attributes of its own.
ATTRIBUTE name [ 'value' ] [ options ]The name may consist of any letters, digits, '_', '#' and '-' and may have any length; the first character must not be '-', though. Names are treated case insensitive, so PartNo is the same as PARTNO. The value may contain any characters and must be enclosed in single quotes.
The valid options are:
| delete | Delete the attribute with the given name from all technology variants (in this case there must be no 'value'). | |
| variable | Mark this attribute as variable, so that it can be overwritten in the schematic (this is the default). | |
| constant | Attributes marked as constant cannot be overwritten in the schematic (unless the user insists). |
An already existing attribute can be switched between variable and constant without the need to repeat its value, as in
| ATTRIBUTE ABC '123' | (variable by default) | |
| ATTRIBUTE ABC constant | (ABC retains its value '123') |
The attribute name _EXTERNAL_ is reserved for marking of external devices (see PACKAGE).
Some special attribute names are not allowed, since they would interfere with the already existing text variables. If an attribute named VALUE is defined, its value will be used to initialize the actual value when placing a part in a schematic (in case the device set has 'Value On').
Selecting the ATTRIBUTE command and clicking on a part shows a dialog in which all attributes of that part are listed and can be edited.
For a fully textual definition of an attribute, the following syntax can be used:
ATTRIBUTE part_name attribute_name 'attribute_value' orientation Note that in case of a multi-gate part, actually one of the gates (i.e. "instances") is selected. When selecting it via a mouse click it is already clear which gate is meant, while when selecting it via part_name, the full name consisting of the part and gate name should be given. While a specific part can only have one attribute with a given name, the attribute can be attached to any or all of its gates. If only the part name is given, the first visible gate will be implicitly selected.
If no coordinates are given (and the command is terminated with a ';'), the behavior depends on whether the given attribute already exists for that part (either in the device or in the schematic). If the attribute already exists, only its value will be changed. If it doesn't exist yet, a new attribute with the given name and value will be placed at the origin of the selected gate of the part.
To delete an attribute from a part, the command
ATTRIBUTE part_name attribute_name DELETEcan be used.
When defining attributes via the command line or a script, use the CHANGE DISPLAY command to define which parts of the attribute (name, value, both or none of these) shall be visible.
Such an attribute could for instance be the author of a drawing, and can be used in the title block of a drawing's frame. It will be shown on every schematic sheet that has a drawing frame that contains a text variable with the same name.
LAYER layer; WIRE (1 2) (3 4);doesn't work here. The layer needs to be selected while the ATTRIBUTE command is already active, which can be done like this
ATTRIBUTE parameters LAYER layer more parameters;Note that the ATTRIBUTE line is not terminated with a ';', and that the LAYER command starts on a new line.
ATTRIBUTE LAYER layer;set the layer to use with subsequent ATTRIBUTE commands.
PACKAGE N; TECHNOLOGY LS; ATTRIBUTE PartNo '12345-ABC'; ATTRIBUTE Temp '100K' constant; ATTRIBUTE Remark 'mount manually';
The AUTO command activates the integrated Autorouter. If signal names are specified or signals are selected with the mouse, only these signals are routed. Without parameters the command will try to route all signals. If a "!" character is specified all signals are routed except the signals following the "!" character. The "!" character must be the first parameter and must show up only once.
The LOAD and SAVE options can be used to load the Autorouter parameters from or save them to the given file. If filename doesn't have the extension ".ctl" it will be appended automatically.
Without any parameters (or if no terminating ';' is given), the AUTO command opens a dialog in which the parameters that control the routing algorithm can be configured. The special option FOLLOWME opens this dialog in a mode where only the parameters controlling the Follow-me router can be modified.
AUTO ! GND VCC;In every case the semicolon is necessary as a terminator. A menu for adjusting the Autorouter control parameters opens if you select AUTO from the command menu or type in AUTO from the keyboard (followed by Return key).
| * | matches any number of any characters | |
| ? | matches exactly one character | |
| [...] | matches any of the characters between the brackets |
If any of these characters shall be matched exactly as such, it has to be enclosed in brackets. For example, abc[*]ghi would match abc*ghi and not abcdefghi.
A range of characters can be given as [a-z], which results in any character in the range 'a'...'z'.
In practice you draw the board outlines into the Dimension layer with the WIRE command and place the components within this area.
If you want the Autorouter not to use a layer, select "N/A" in the preferred direction field.
The command BOARD is used to convert a schematic drawing into a board.
If the board already exists, it will be loaded into a board window.
If the board does not exist, you will be asked whether to create that new board. If a grid is given, the parts on the board will be placed in the given raster, as in
BOARD 5mmwhich would place the parts in a 5 millimeter raster (default is 50mil). The number must be given with a unit, and the maximum allowed value is 10mm.
The BOARD command will never overwrite an existing board file. To create a new board file if there is already a file with that name, you have to remove that file first.
edit .brdin the editor window's command line.
All relevant data from the schematic file (name.sch) will be converted to a board file (name.brd). The new board is loaded automatically as an empty card with a size of 160x100mm (Light edition: 100x80mm). All packages and connections are shown on the left side of the board. Supply pins are already connected (see PIN command).
If you need board outlines different to the ones that are generated by default, simply delete the respective lines and use the WIRE command to draw your own outlines into the Dimension layer. The recommended width for these lines is 0.
A board file cannot be generated:
The command BUS is used to draw bus connections onto the Bus layer of a schematic diagram. Bus_name has the following form:
SYNONYM:partbus,partbus,..where SYNONYM can be any name. Partbus is either a simple net name or a bus name range of the following form:
Name[LowestIndex..HighestIndex]where the following condition must be met:
0 <= LowestIndex <= HighestIndex <= 511
If a name is used with a range, that name must not end with digits, because it would become unclear which digits belong to the Name and which belong to the range.
If a bus wire is placed at a point where there is already another bus wire, the current bus wire will be ended at that point. This function can be disabled with "SET AUTO_END_NET OFF;", or by unchecking "Options/Set/Misc/Auto end net and bus".
If the curve or @radius parameter is given, an arc can be drawn as part of the bus (see the detailed description in the WIRE command).
A[0..15] RESET DB[0..7],A[3..4] ATBUS:A[0..31],B[0..31],RESET,CLOCK,IOSEL[0..1]If no bus name is used, a name of the form B$1 is automatically allocated. This name can be changed with the NAME command at any time.
The line width used by the bus can be defined for example with
SET Bus_Wire_Width 40;to be 40 mil. (Default: 30 mil).
ATBUS:A[0..31],B[0..31],!RESET,CLOCK,IOSEL[0..1]which would result in
_____ ATBUS:A[0..31],B[0..31],RESET,CLOCK,IOSEL[0..1]You can find further details about this in the description of the TEXT command.
Parameters adjusted with the CHANGE command remain as preset properties for objects added later.
All values in the CHANGE command are used according to the actual grid unit.
| Layer | CHANGE LAYER name | number | |
| Text | CHANGE TEXT [ text ] | |
| Text height | CHANGE SIZE value | |
| Text thickness | CHANGE RATIO ratio | |
| Text line distance | CHANGE LINEDISTANCE value | |
| Text font | CHANGE FONT VECTOR | PROPORTIONAL | FIXED | |
| Text alignment | CHANGE ALIGN BOTTOM | LEFT | CENTER | TOP | RIGHT | |
| Wire width | CHANGE WIDTH value | |
| Wire style | CHANGE STYLE value | |
| Arc cap | CHANGE CAP ROUND | FLAT | |
| Pad shape | CHANGE SHAPE SQUARE | ROUND | OCTAGON | LONG | OFFSET | |
| Pad/via/smd flags | CHANGE STOP | CREAM | THERMALS | FIRST OFF | ON | |
| Pad/via diameter | CHANGE DIAMETER diameter | |
| Pad/via/hole drill | CHANGE DRILL value | |
| Via layers | CHANGE VIA from-to | |
| Smd dimensions | CHANGE SMD width height | |
| Smd roundness | CHANGE ROUNDNESS value | |
| Pin parameters | CHANGE DIRECTION NC | IN | OUT | IO | OC | HIZ | SUP | PAS | PWR | |
| CHANGE FUNCTION NONE | DOT | CLK | DOTCLK | ||
| CHANGE LENGTH POINT | SHORT | MIDDLE | LONG | ||
| CHANGE VISIBLE BOTH | PAD | PIN | OFF | ||
| CHANGE SWAPLEVEL number | ||
| Polygon parameters | CHANGE THERMALS OFF | ON | |
| CHANGE ORPHANS OFF | ON | ||
| CHANGE ISOLATE distance | ||
| CHANGE POUR SOLID | HATCH | CUTOUT | ||
| CHANGE RANK value | ||
| CHANGE SPACING distance | ||
| Gate parameters | CHANGE SWAPLEVEL number | |
| CHANGE ADDLEVEL NEXT | MUST | ALWAYS | CAN | REQUEST | ||
| Net class | CHANGE CLASS number | name | |
| Package | CHANGE PACKAGE part_name [device_name] | 'device_name' [part_name] | |
| Technology | CHANGE TECHNOLOGY part_name [device_name] | 'device_name' [part_name] | |
| Attribute display | CHANGE DISPLAY OFF | VALUE | NAME | BOTH | |
| Frame parameters | CHANGE COLUMS value | |
| CHANGE ROWS value | ||
| CHANGE BORDER NONE | BOTTOM | RIGHT | TOP | LEFT | ALL | ||
| Label | CHANGE XREF OFF | ON | |
| Dimension type | CHANGE DTYPE PARALLEL | HORIZONTAL | VERTICAL | RADIUS | DIAMETER | ANGLE | LEADER | |
| Dimension unit | CHANGE DUNIT [MIC | MM | MIL | INCH] [OFF | ON] [precision] | |
| Dimension line | CHANGE DLINE width [ extension_width [ extension_length [ extension_offset ]]] (extension values can be set to AUTO; unchanged preceding values can be skipped with '-') | |
| Populate | CHANGE POPULATE OFF | ON (only available in a board context without active f/b annotation) |
The CIRCLE command is used to create circles. Circles in the layers tRestrict, bRestrict, and vRestrict define restricted areas. They should be defined with a width of 0.
The width parameter defines the width of the circle's circumference and is the same parameter as used in the WIRE command. The width can be changed with the command:
CHANGE WIDTH width;where width is the desired value in the current unit.
A circle defined with a width of 0 will be filled.
GRID inch 1; CIRCLE (0 0) (1 0);generates a circle with a radius of 1 inch and the center at the origin.
The CLASS command is used to define or use net classes.
Without parameters, it offers a dialog in which the net classes can be defined.
If only a number or name is given, the net class with the given number or name is selected and will be used for subsequent NET and SIGNAL commands.
If both a number and a name are given, the net class with the given number will be assigned all the following values and will also be used for subsequent NET and SIGNAL commands. If any of the parameters following name are omitted, the net class will keep its respective value.
If number is negative, the net class with the absolute value of number will be cleared. The default net class 0 can't be cleared.
Net class names are handled case insensitive, so SUPPLY would be the same as Supply or SuPpLy.
Using several net classes in a drawing increases the time the Autorouter needs to do its job. Therefore it makes sense to use only as few net classes as necessary (only the number of net classes actually used by nets or signals count here, not the number of defined net classes).
In order to avoid conflicts when CUT/PASTEing between drawings it makes sense to define the same net classes under the same numbers in all drawings.
Modules are using the same set of net classes as the schematic itself.
If a net of a MODULE has an external connection through a PORT, the net class of the net on this port is overwriting the net class of the net in the module.
The Autorouter processes signals sorted by their total width requirements (Width plus Clearance), starting with those that require the most space. The bus router only routes signals with net class 0.
The net class of an existing net/signal can be changed with the CHANGE command.
CLASS 3 1:0.6mm 2:0.8mmdefines a minimum clearance of 0.6mm between signals in net classes 1 and 3, and one of 0.8mm between signals in net classes 2 and 3. Note that the numbers in number:clearance must be less than or equal to the number of the net class itself ('3' in the above example), so
CLASS 3 1:0.6mm 2:0.8mm 3:0.2mmwould also be valid, whereas
CLASS 3 1:0.6mm 2:0.8mm 3:0.2mm 4:0.5mmwould not be allowed.
The CLOSE command is used to close an editor window. If the drawing you are editing has been modified you will be prompted whether you wish to save it.
This command is mainly used in script files.
CONNECT
See also PREFIX,
OPEN,
CLOSE,
SCRIPT
CONNECT [ ALL | ANY ] gate_name.pin_name pad_name..
CONNECT [ ALL | ANY ] pin_name pad_name..
This command is used in the device editing mode in order to define the relationship between the pins of a gate and the pads of the corresponding package in the library. First of all, it is necessary to define which package is to be used by means of the PACKAGE command.
If the CONNECT command is invoked without parameters, a dialog is presented which allows you to interactively assign the connections.
CONNECT gnd 1 rdy 2 phi1 3 !irq 4 nc1 5...(Note: "!" is used to indicate inverted data signals.)
CONNECT A.I1 1 A.I2 2 A.O 3; CONNECT B.I1 4 B.I2 5 B.O 6; CONNECT C.I1 13 C.I2 12 C.O 11; CONNECT D.I1 10 D.I2 9 D.O 8; CONNECT PWR.gnd 7; CONNECT PWR.VCC 14;In this case, the connections for four NAND gates of a good old 7400 are allocated. The device includes five gates - A, B, C, D, and PWR. The gate inputs are named I1 and I2 while the output is named O.
The CONNECT command can be repeated as often as required. It may be used with all pin/pad connections or with only certain pins. Each new CONNECT command overwrites the previous conditions for the relevant pins.
Note that if you have a large number of connections in a single device, the CONNECT command works a lot faster if all connections are given in one single call, like shown in the example below.
CONNECT ALL I1 '1 3 5'; CONNECT ANY O1 '2 4 6';In the first example the pin I1 is connected to the three pads 1, 3 and 5. If the pin I1 is connected to a net in the schematic, all three pads must be explicitly connected to the corresponding signal in the board.
If a pin name would collide with one of the keywords ALL or ANY, the pin name needs to be enclosed with single quotes.
In the CONNECT dialog the "Connect" button creates a new connection between
the selected pin and the selected pads. There can be more than one pad selected,
in which case all of these pads will be connected to the selected pin. Use the
Ctrl and Shift keys in the usual way to mark more than one pad as selected.
The "Append" button adds the selected pads to the current connection.
The "Disconnect" button removes the selected connection and puts the pin and
pads back in their separate lists, keeping them selected so that it is easy to
make modifications. A Disconnect immediately followed by a Connect results in
the same configuration as before the Disconnect (and vice versa).
If a connection contains more than one pad, an icon indicates whether any or
all of these pads need to be externally connected to a signal. Click on this
icon to toggle the mode. When such a connection item is expanded, all the pads
are listed separately, and clicking on Disconnect with one of the pads selected
will only disconnect that one pad.
ed 6502.dev; prefix 'IC'; package dil40; connect gnd 1 rdy 2 phi1 3 !irq 4 nc1 5 !nmi 6 \ sync 7 vcc 8 a0 9 a1 10 a2 11 a3 12 a4 \ 13 a5 14 a6 15 a7 16 a8 17 a9 18 a10 19 \ a11 20 p$0 21 a12 22 a13 23 a14 24 a15 \ 25 d7 26 d6 27 d5 28 d4 29 d3 30 d2 31 \ d1 32 d0 33 r/w 34 nc2 35 nc3 36 phi0 37 \ so 38 phi2 39 !res 40;If a command is continued at the next line, it is advisable to insert the character "\" at the end of the line to ensure the following text cannot be confused with an EAGLE command.
Confusing parameters with commands can also be avoided
by enclosing the parameters in apostrophes.
COPY
See also GROUP,
CUT,
PASTE,
ADD,
INVOKE,
POLYGON
COPY deviceset@library [name]
COPY package@library [name]
The COPY command is used to copy objects within the same drawing, or between libraries. EAGLE will generate a new name for the copy but will retain the old value. When copying signals (wires), buses, and nets the names are retained, but in all other cases a new name is assigned.
SET Cmd.Copy.ClassicEagleMode 1to get back the original behavior of the COPY command (as well as the CUT command).
If you just want to use another gate of a multi-gate part, you should use the INVOKE command instead.
Note that any existing library objects (device sets, symbols or packages) used by the copied library object will be automatically updated.
Parts of a drawing (or even a whole board) can be copied onto other drawings by means of the commands CUT and PASTE.
To do this you first define a group (GROUP command). Then use the CUT command, followed by a reference point (mouse click or coordinates (x y)) to put the selected objects into the buffer. CUT; automatically puts the reference point at the center of the selected objects (snapped to the grid). Now you can change to an other drawing (EDIT) and copy the contents of the buffer onto the new drawing by executing the PASTE command.
SET Cmd.Copy.ClassicEagleMode 1to get back the original behavior of the CUT command (as well as the COPY command).
The DELETE command is used to delete the selected object.
Parts, pads, smds, pins and gates can also be selected by their name, which is especially useful if the object is outside the currently shown window area. Note that when selecting a multi-gate part in a schematic by name, you will need to enter the full instance name, consisting of part and gate name.
Attributes of parts can be selected by entering the concatenation of part name and attribute name, as in R5>VALUE.
Clicking the right mouse button deletes a previously defined GROUP.
After deleting a group it is possible that airwires which have been newly created due to the removal of a component may be "left over", because they have not been part of the original group. In such a case you should re-calculate the airwires with the RATSNEST command.
With active Forward&Back Annotation, no wires or vias can be deleted from a signal that is connected to components in a board. Also, no components can be deleted that have signals connected to them. Modifications like these have to be done in the schematic.
Use the RIPUP command to convert an already routed connection back into an airwire.
The DELETE command has no effect on layers that are not visible (refer to DISPLAY).
The DRC might generate error polygons which can only be deleted with DRC CLEAR.
DELETE SIGNALS can be used to delete all signals on a board. This is useful if you want to read in a new or changed netlist (see EXPORT). Only those signals are deleted which are connected to pads.
If you want to delete a part that has the name SIGNALS, you need to write the name in single quotes.
| Gate | Deletes the entire part containing this gate (even if the gates are spread over several sheets). If f/b annotation is active, the wires connected to the element in the board will not be ripped up (as opposed to deleting a single gate), except for those cases where a pin of the deleted part is only connected directly to one single other pin and no net wire | |
| Polygon Wire | Deletes the entire polygon | |
| Net/Bus Wire | Deletes the entire net or bus segment |
Don't forget: Deleting can be reversed by the
UNDO command!
DESCRIPTION
See also CONNECT,
PACKAGE,
VALUE
DESCRIPTION ** [ description_string; ]
This command is used to define or edit the description of a drawing or a library object.
The description_string may contain HTML tags.
The first non-blank line of description_string will be used as a short descriptive text (headline) in the Control Panel.
The DESCRIPTION command without a parameter opens a dialog in which the text can be edited. The upper pane of this dialog shows the formatted text, in case it contains HTML tags, while the lower pane is used to edit the raw text. At the very top of the dialog the headline is displayed as it would result from the first non-blank line of the description. The headline is stripped of any HTML tags.
By default the DESCRIPTION command works on the description of the object that is currently edited, like a device set, package, symbol, board or sheet. If, in a library, there is no currently edited object (as can be the case after it has been newly loaded) the description of the library will be changed.
To explicitly access the description of a library, even if a device, package or symbol is already being edited, enter the asterisk character ('*') as the first parameter to the DESCRIPTION command. This is also the way to access the description of a schematic, as opposed to the description of an individual sheet.
To access the description of the current MODULE, enter a pair of asterisk characters ('**') as the first parameter to the DESCRIPTION command.
DESCRIPTION '<b>Quad NAND</b><p>\nFour NAND gates with 2 inputs each.';This would result in
Quad NAND
Four NAND gates with 2 inputs each.
DIMENSION
See also WIRE,
CHANGE,
CIRCLE,
HOLE
The DIMENSION command adds dimensioning to a drawing. It can either be applied to an object, or it can draw arbitrary dimensions.
If the first point selects an object, a suitable dimension object is generated as follows:
| straight wire | linear dimension displaying the distance between the end points of the wire | |
| curved wire | radius dimension displaying the radius of the arc | |
| circle | diameter dimension displaying the diameter of the circle | |
| hole | diameter dimension displaying the diameter of the hole |
If no object is selected, or a wire is selected at one of its end points, a dimension object is generated according to the current dimension type. If this dimension type is not the one that is needed, the right mouse button can be clicked to loop through the various types.
To draw an arbitrary dimension even at close proximity to an object that would trigger a specific kind of dimension, press the Ctrl key with the first click. This may also be useful when using the DIMENSION command in a script (by adding the 'C' modifier to the first coordinate), to make sure the dimension appears exactly as intended.
The way in which a dimension object is drawn (line, unit, precision) can be configured with "CHANGE DLINE/DUNIT" or with its properties dialog. Note that the "Unit" parameter in this dialog refers to the unit in which the actual numbers of the dimension object will be displayed.
Parallel
A parallel dimension displays the distance between its first and second reference point. The dimension line is parallel to the line going through its reference points, and it runs through the given alignment point. The actual position of the alignment point doesn't matter, only its distance from the the line through its reference points is taken into account. When a parallel dimension object is newly created or modified, the alignment point is normalized, so that it lies in the middle of the dimension line.
Horizontal
Same as parallel, but the dimension line extends only in X direction, and it displays only the X distance between the reference points.
Vertical
Like horizontal, but for Y.
Radius
A radius dimension displays the distance between its first and second reference point. The first reference point is at the center of the arc this dimension is drawn for, while the second point is somewhere on the arc itself. If the alignment point is between the two reference points, the dimension line is drawn between the reference points, which is "inside" the arc. Otherwise the dimension line is drawn "outside" of the arc. If the measurement text is too long to fit on an inside radius dimension, the dimension line is drawn on the outside. A radius dimension automatically displays a cross at its first reference point (which is the center of the arc). When a radius dimension object is newly created or modified, the alignment point is normalized, so that it lies in the middle of the dimension line for an "inside" dimension, or just beyond the arrow for an "outside" dimension.
Diameter
A diameter dimension displays the distance between its first and second reference point. The two reference points are on opposite sides of the circle's circumference, so their distance measures the circle's diameter. If the alignment point is between the two reference points, the dimension line is drawn between the reference points, which is "inside" the circle. Otherwise the dimension line is drawn "outside" of the circle, much like a parallel dimension. If the measurement text is too long to fit on an inside diameter dimension, the dimension line is drawn on the outside. A diameter dimension automatically displays a cross in the middle between its two reference points (which is the center of the circle). When a diameter dimension object is newly created or modified, the alignment point is normalized, so that it lies at the same coordinates as its second reference point for an "inside" dimension, or in the middle of the dimension line for an "outside" dimension.
Angle
An angle dimension displays the angle between the second and third reference point, measured counterclockwise around the first reference point (which is the center of the arc). When an angle dimension object is newly created or modified, the second reference point is normalized, so that it has the same distance from the first point as the third one does.
Leader
A leader dimension can be used to point at something in a drawing. There is an arrow at the first point, and the second and third point define a (bent) line. The leader doesn't display any measurement. You can use the TEXT command to place any text you need.
Valid options are: ALL, NONE, LAST, ? and ??
The DISPLAY command is used to choose the visible layers. As parameters, the layer number and the layer name are allowed (even mixed). If the parameter ALL is chosen, all layers become visible. If the parameter NONE is used, all layers are switched off. For example:
DISPLAY NONE BOTTOM;Following this command only the Bottom layer is displayed.
If the parameter LAST is given, the previously visible layers will be displayed.
Please note that only those signal layers (1 through 16) are available that have been entered into the layer setup in the Design Rules.
If the layer name or the layer number includes a negative sign, it will be filtered out. For example:
DISPLAY TOP -BOTTOM -3;In this case the Top layer is displayed while the Bottom layer and the layer with the number 3 are not shown on the screen.
Avoid layer names ALL and NONE as well as names starting with a "-".
Some commands (PAD, SMD, SIGNAL, ROUTE) automatically activate certain layers.
If the DISPLAY command is invoked without parameters, a dialog is presented which allows you to adjust all layer settings.
DISPLAY TOP BOTTOM ? MYLAYER1 MYLAYER2 ?? OTHER WHATEVERIn the above example the two layers TOP and BOTTOM are required and will cause an error if either of them is missing. MYLAYER1 and MYLAYER2 will just be reported if missing, allowing the user to cancel the operation, and OTHER and WHATEVER will be displayed if they are there, otherwise they will be ignored.
The '?' and '??' options may appear any number of times and in any sequence.
If the color selected for layer 17 (Pads) or 18 (Vias) is 0 (which represents the current background color), the pads and vias are displayed in the color and fill style of the respective signal layers. If no signal layer is visible, pads and vias are not displayed.
If the color selected for layer 17 (Pads) or 18 (Vias) is not the background color and no signal layers are visible, pads and vias are displayed in the shape of the uppermost and undermost layer.
This also applies to printouts made with PRINT.
The syntax to handle these aliases is:
DISPLAY = MyLayers None Top Bottom Pads Vias Unrouted
Defines the alias "MyLayers" which, when used as in
DISPLAY myl
will display just the layers Top, Bottom, Pads, Vias and Unrouted
(without the "None" parameter the given layers would be displayed in
addition to the currently visible layers).
Note the abbreviated use of the alias and the case insensitivity.
DRC
See also Design Rules,
CLASS,
SET,
ERC,
ERRORS
DRC ;
DRC LOAD|MERGE|SAVE filename;
DRC *
The command DRC checks a board against the current set of Design Rules.
Please note that electrically irrelevant objects (wires in packages, rectangles, circles and texts) are not checked against each other for clearance errors.
The errors found are displayed as error polygons in the respective layers, and can be browsed through with the ERRORS command.
Without parameters the DRC command opens a Design Rules dialog in which the board's Design Rules can be defined, and from which the actual check can be started.
If two coordinates are given in the DRC command (or if the Select button is clicked in the Design Rules dialog) all checks will be performed solely in the defined rectangle. Only errors that occur (at least partly) in this area will be reported.
If you get DRC errors that don't go away, even if you modify the Design Rules, make sure you check the Net class of the reported object to see whether the error is caused by a specific parameter of that class.
To delete all error polygons use the command
ERRORS CLEAR
The LOAD and SAVE options can be used to load the Design Rules from or save them to the given file. If filename doesn't have the extension ".dru" it will be appended automatically. The MERGE option can be used to merge some additional Design Rules parameters (the others remain unchanged).
If the DRC command is given an asterisk character ('*') as the first parameter, the Design Rules dialog will be opened and allow editing the Design Rules, without triggering an actual check when the dialog is confirmed.
SET DRC_FILL fill_name;Defines the fill style used for the DRC error polygons. Default is LtSlash.
The EDIT command is used to load a drawing or if a library has been opened with the OPEN command, to load a package, symbol, or device 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.pac | loads a package | |
| EDIT name.sym | loads a symbol | |
| EDIT name.dev | loads a device | |
| 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 |
Wildcards in the name are allowed (e.g. *.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 change from schematic to a board with the same name the command
EDIT .brdcan be used. In the same way to change from board to schematic use the command
EDIT .schTo edit another sheet of a schematic the command
EDIT .sX(X is the sheet number) or the combo box in the action toolbar of the editor window can be used. If the given sheet number doesn't exist, a new sheet is created.
You can also switch between sheets by clicking on an icon of the sheet thumbnail preview. Drag&drop in the thumbnail preview allows you to reorder sheets.
Symbols, devices or packages may only be edited if a library is first opened with the OPEN command.
This command is used to test schematics for electrical errors. The result of the check is presented in the ERRORS dialog.
Please 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!
ERRORS
See also ERC,
DRC
ERRORS CLEAR
The command ERRORS is used to show the errors found by the Electrical Rule Check (ERC) or the Design Rule Check (DRC). If selected, a window is opened in which all errors are listed. If no ERC or DRC has been run for the loaded drawing, yet, the respective check will be started first.
The list view in the ERRORS dialog has up to four sections that contain Consistency errors, Errors, Warnings and Approved messages, respectively.
Selecting an entry with the mouse causes the error to be marked in the editor window with a rectangle and a line from the upper left corner of the screen.
Double clicking an entry centers the drawing to the area where the error is located. Checking the "Centered" checkbox causes this to happen automatically.
The list can also be cleared by entering the command
ERRORS CLEAR
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.
The command generates the following output files:
Set Undo_Log Off;is given before.
| .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.
The FRAME command draws a frame with numbered columns and rows. The two points define two opposite corners of the frame. Pressing the center mouse button changes the layer to which the frame is to be added.
The columns parameter defines the number of columns in the frame. There can be up to 127 columns. By default the columns are numbered from left to right. If the columns value is negative, they are numbered from right to left.
The rows parameter defines the number of rows in the frame. There can be up to 26 rows. Rows are marked from top to bottom with letters, beginning with 'A'. If the rows value is negative, they are marked from bottom to top. If rows is given, it must be preceeded by columns.
The borders parameter, if given, defines which sides of the frame will have a border with numbers or letters displayed. Valid options for this parameter are Left, Top, Right and Bottom. By default all four sides of the frame will have a border. If any of these options is given, only the requested sides will have a border. The special options None and All can be used to have no borders at all, or all sides marked.
Even though you can draw several frames in the same drawing, only the first one will be used for calculating the positions of parts and nets. These positions can be used, for instance, in a User Language Program to generate a list of parts with their locations in their respective frame. They are also used internally to automatically generate cross references for labels.
Due to the special nature of the frame object, it doesn't have a rotation of its own, and it doesn't get rotated with the ROTATE command.
A frame can be drawn directly into a board or schematic, but more typically you will want to create a special symbol or package drawing that perhaps also contains a title block, which you can then use in all your drawings. The "frames" library that comes with EAGLE contains several drawing frames.
FRAME 10 5 TOP LEFT draws a frame with 10 columns (numbered from left to right) and 5 rows (marked 'A' to 'E' from top to bottom) that has the column and row indicators drawn only at the top and left border.
Using this command two gates may be swapped within a schematic. Both gates must be identical with the same number of pins and must be allocated the same Swaplevel in the device definition. They do not, however, need to be in the same device.
The name used in the GATESWAP command is the displayed name on the schematic (e.g. U1A for gate A in device U1).
If a device is not used anymore after the GATESWAP command, it is
deleted automatically from the drawing.
GRID
See also SCRIPT
GRID;
The GRID command is used to specify the grid and the current unit. Given without an option, this command switches between GRID ON and GRID OFF.
The following options exist:
| GRID ON; | Displays the grid on the screen | |
| GRID OFF; | Turns off displayed grid | |
| GRID DOTS; | Displays the grid as dots | |
| GRID LINES; | Displays the grid as solid lines | |
| GRID MIC; | Sets the grid units to micron | |
| GRID MM; | Sets the grid units to mm | |
| GRID MIL; | Sets the grid units to mil | |
| GRID INCH; | Sets the grid units to inch | |
| GRID FINEST; | Sets the grid to the finest possible value | |
| GRID grid_size; | Defines the distance between | |
| the grid points in the actual unit | ||
| GRID LAST; | Sets grid to the most recently | |
| used values | ||
| GRID DEFAULT; | Sets grid to the standard values | |
| GRID grid_size grid_multiple; | ||
| grid_size = grid distance | ||
| grid_multiple = grid factor | ||
| GRID ALT ...; | Defines the alternate grid |
Grid mm; Set Diameter_Menu 1.0 1.27 2.54 5.08; Grid Last;In this case you can change back to the last grid definition although you don't know what the definition looked like.
GRID mm 1 10;for instance specifies that the distance between the grid points is 1 mm and that every 10th grid line will be displayed.
Note: The first number in the GRID command always represents the grid distance, the second - if existing - represents the grid multiple.
The GRID command may contain multiple parameters:
GRID inch 0.05 mm;In this case the grid distance is first defined as 0.05 inch. Then the coordinates of the cursor are chosen to be displayed in mm.
GRID DEFAULT;Sets grid to the standard value for the current drawing type.
GRID mil 50 2 lines on alt mm 1 mil;Defines a 50 mil grid displayed as lines (with only every other line visible), and sets the alternate grid size to 1 mm, but displays it in mil.
Pressing the Alt key switches to the alternate Grid. This can typically be a finer grid than the normal one, which allows you to quickly do some fine positioning in a dense area, for instance, where the normal grid might be too coarse. The alternate grid remains active as long as the Alt key is held pressed down.
The syntax to handle these aliases is:
GRID = MyGrid inch 0.1 lines on
Defines the alias "MyGrid" which, when used as in
GRID myg
will change the current grid to the given settings.
Note the abbreviated use of the alias and the case insensitivity.
GROUP
See also CHANGE,
CUT,
PASTE,
MIRROR,
DELETE
GROUP ALL
GROUP;
The GROUP command is used to define a group of objects for a successive command. Also a whole drawing or an element can be defined as a group. Objects are selected - after activating the GROUP command - by click&dragging a rectangle or by drawing a polygon with the mouse. The easiest way to close the polygon is to use the right mouse button. Only objects from displayed layers can become part of the group.
The keyword ALL can be used to define a group that includes the entire drawing area.
The group includes:
For instance: In order to change several pad shapes, select CHANGE and SHAPE with the left mouse button and select the group with the right mouse button.
The group definition remains until a new drawing is loaded or the command
GROUP;is executed.
A command name within the HELP command shows the help page of that command.
HELP GRID;displays the help page for the GRID command.
This command is used to define e.g. mounting holes (has no electrical connection between the different layers) in a board or in a package. The parameter drill defines the diameter of the hole in the actual unit. It may be up to 200 mm (7.7840 inch).
HOLE 0.20 If the actual unit is "inch", the hole will have a diameter of 0.20 inch.
The entered value for the diameter (also used for via-holes and pads) remains as a presetting for successive operations. It may be changed with the command:
CHANGE DRILL value A hole can only be selected if the Holes layer is displayed.
 The relation between certain diameters and symbols is defined in the "Options/Set/Drill" dialog. The circle in the Dimension layer is used by the Autorouter. As it will keep a (user-defined) minimum distance between via-holes/wires and dimension lines, it will automatically keep this distance to the hole.
In the layers tStop and bStop, holes generate the solder
stop mask, whose diameter is determined by the Design Rules.
INFO
See also CHANGE,
SHOW
INFO name ..
The INFO command displays further details about an object's properties on screen, e.g. wire width, layer number, text size etc. It is also possible to modify properties in this dialog.
Parts, pads, smds, pins and gates can also be selected by their name, which is especially useful if the object is outside the currently shown window area. Note that when selecting a multi-gate part in a schematic by name, you will need to enter the full instance name, consisting of part and gate name.
Attributes of parts can be selected by entering the concatenation of part name and attribute name, as in R5>VALUE.
The coordinates of a rotated rect are not changeable.
INVOKE
See also COPY,
ADD
INVOKE part_name gate_name orientation
See the ADD command for an explanation of Addlevel und Orientation.
The INVOKE command is used to select a particular gate from a device which is already in use and place it in the schematic (e.g. a power symbol with Addlevel = Request).
Gates are activated in the following way:
If an already invoked gate is selected in the dialog, the default button changes to "Show", and a click on it zooms the editor window in on the selected gate, switching to a different sheet if necessary.
This command is used to draw a connection dot at the intersection of nets which are to be connected to each other. Junction points may be placed only on a net. If placed on the intersection of different nets, the user is given the option to connect the nets.
If a net wire is placed at a point where there are at least two other net wires and/or pins, a junction will automatically be placed. This function can be disabled with "SET AUTO_JUNCTION OFF;", or by unchecking "Options/Set/Misc/Auto set junction".
On the screen junction points are displayed at least with a diameter
of five pixels.
LABEL
See also NAME,
BUS,
FRAME
Bus or net names may be placed on a schematic in any location by using the label command. When the bus or net is clicked on with the mouse, the relevant label attaches to the mouse cursor and may be rotated, changed to another layer, or moved to a different location. The second mouse click defines the location of the label.
The orientation of the label may be defined textually using the usual definitions as listed in the ADD command (R0, R90 etc.).
Buses and nets may have any number of labels.
Labels cannot be changed with "CHANGE TEXT".
Labels are handled by the program as text, but their value corresponds to the name of the appropriate bus or net. If a bus or net is renamed with the NAME command, all associated labels are renamed automatically.
If a bus, net, or label is selected with the SHOW command, all connected buses, nets and labels are highlighted.
The format in which a cross-reference label is displayed can be controlled through the "Xref label format" string, which is defined in the "Options/Set/Misc" dialog, or with the SET command. The following placeholders are defined, and can be used in any order:
| %F | enables drawing a flag border around the label | |
| %N | the name of the net | |
| %S | the next sheet number | |
| %C | the column on the next sheet | |
| %R | the row on the next sheet |
The default format string is "%F%N/%S.%C%R". Apart from the defined placeholders you can also use any other ASCII characters.
The column and row values only work if there is a frame on the next sheet on which the net appears. If %C or %R is used and there is no frame on that sheet, they will display a question mark ('?').
When determining the column and row of a net on a sheet, first the column and then the row within that column is taken into account. Here XREF labels take precedence over normal labels, which again take precedence over net wires. For a higher sheet number, the frame coordinates of the left- and topmost field are taken, while for a lower sheet number those of the right- and bottommost field are used.
The orientation of a cross-reference label defines whether it will point to a "higher" or a "lower" sheet number. Labels with an orientation of R0 or R270 point to the right or bottom border of the drawing, and will therefore refer to a higher sheet number. Accordingly, labels with an orientation of R90 or R180 will refer to a lower sheet number. If a label has an orientation of R0 or R270, but the net it is attached to is not present on any higher sheet, a reference to the next lower sheet is displayed instead (the same applies accordingly to R90 and R180). If the net appears only on the current sheet, no cross-reference is shown at all, and only the net name is displayed (surrounded by the flag border, if the format string contains the %F placeholder).
A cross-reference label that is placed on the end of a net wire will connect to the wire so that the wire is moved with the label, and vice versa.
The cross-reference label format string is stored within the schematic drawing file.
A cross-reference label can be changed to a normal label either through the CHANGE command or the label's Properties dialog.
LAYER layer; WIRE (1 2) (3 4);doesn't work here. The layer needs to be selected while the LABEL command is already active, which can be done like this
LABEL parameters LAYER layer more parameters;Note that the LABEL line is not terminated with a ';', and that the LAYER command starts on a new line.
LABEL LAYER layer;set the layer to use with subsequent LABEL commands.
Certain layers are not available in all modes.
Please note that only those signal layers (1 through 16) are available that have been entered into the layer setup in the Design Rules.
LAYER 101 SAMPLE;you define a new layer with layer number 101 and layer name SAMPLE.
If a package contains layers not yet specified in the board, these layers are added to the board as soon as you place the package into the board (ADD or REPLACE).
The predefined layers have a special function. You can change their names, but their functions (related with their number) remain the same.
If you define your own layers, you should use only numbers greater than 100. Numbers below may be assigned for special purposes in later EAGLE versions.
LAYER -103;deletes the layer number 103. Layers to be deleted must be empty. If this is not the case, the program generates the error message
"layer is not empty: #"
where "#" represents the layer number. If you want to avoid any error messages in a layer delete operation you can use the '??' option. This may be useful in scripts that try to delete certain layers, but don't consider it an error if any of these layers is not empty or not present at all.
| 1 Top | Tracks, top side | |
| 2 Route2 | Inner layer | |
| 3 Route3 | Inner layer | |
| 4 Route4 | Inner layer | |
| 5 Route5 | Inner layer | |
| 6 Route6 | Inner layer | |
| 7 Route7 | Inner layer | |
| 8 Route8 | Inner layer | |
| 9 Route9 | Inner layer | |
| 10 Route10 | Inner layer | |
| 11 Route11 | Inner layer | |
| 12 Route12 | Inner layer | |
| 13 Route13 | Inner layer | |
| 14 Route14 | Inner layer | |
| 15 Route15 | Inner layer | |
| 16 Bottom | Tracks, bottom side | |
| 17 Pads | Pads (through-hole) | |
| 18 Vias | Vias (through-hole) | |
| 19 Unrouted | Airwires (rubberbands) | |
| 20 Dimension | Board outlines (circles for holes) | |
| 21 tPlace | Silk screen, top side | |
| 22 bPlace | Silk screen, bottom side | |
| 23 tOrigins | Origins, top side | |
| 24 bOrigins | Origins, bottom side | |
| 25 tNames | Service print, top side | |
| 26 bNames | Service print, bottom side | |
| 27 tValues | Component VALUE, top side | |
| 28 bValues | Component VALUE, bottom side | |
| 29 tStop | Solder stop mask, top side | |
| 30 bStop | Solder stop mask, bottom side | |
| 31 tCream | Solder cream, top side | |
| 32 bCream | Solder cream, bottom side | |
| 33 tFinish | Finish, top side | |
| 34 bFinish | Finish, bottom side | |
| 35 tGlue | Glue mask, top side | |
| 36 bGlue | Glue mask, bottom side | |
| 37 tTest | Test and adjustment inf., top side | |
| 38 bTest | Test and adjustment inf. bottom side | |
| 39 tKeepout | Nogo areas for components, top side | |
| 40 bKeepout | Nogo areas for components, bottom side | |
| 41 tRestrict | Nogo areas for tracks, top side | |
| 42 bRestrict | Nogo areas for tracks, bottom side | |
| 43 vRestrict | Nogo areas for via-holes | |
| 44 Drills | Conducting through-holes | |
| 45 Holes | Non-conducting holes | |
| 46 Milling | Milling | |
| 47 Measures | Measures | |
| 48 Document | General documentation | |
| 49 Reference | Reference marks | |
| 51 tDocu | Part documentation, top side | |
| 52 bDocu | Part documentation, bottom side |
| 91 Nets | Nets | |
| 92 Busses | Buses | |
| 93 Pins | Connection points for component symbols | |
| with additional information | ||
| 94 Symbols | Shapes of component symbols | |
| 95 Names | Names of component symbols | |
| 96 Values | Values/component types | |
| 97 Info | General information | |
| 98 Guide | Guide lines |
The LOCK command can be applied to parts in a board, and prevents them from being moved, rotated, or mirrored. This is useful for things like connectors, which need to be mounted at a particular location and must not be inadvertently moved.
The origin of a locked part is displayed as an 'x' to have a visual indication that the part is locked.
If a group is moved and it contains locked parts, these parts (together with any wires ending at their pads) will not move with the group.
Detached texts of a locked part can still be moved individually, but they won't move with a group.
Parts can also be selected by their name, which is especially useful if the object is outside the currently shown window area.
A "locked" part can be made "unlocked" by clicking on it with the
Shift key pressed (and of course the LOCK command activated).
MARK
See also GRID
MARK;
The MARK command allows you to define a point on the drawing area and display the coordinates of the mouse cursor relative to that point at the upper left corner of the screen (with a leading 'R' character). This command is useful especially when board dimensions or cutouts are to be defined. Entering MARK; turns the mark on or off.
Please choose a grid fine enough before using the MARK command.
MEANDER
See also ROUTE
The MEANDER command can be used to balance the lengths of signals forming a differential pair. To do this, just click on a wire of a differential pair and move the mouse cursor away from the selection point. If there is a difference in the length of the two signals, and the current mouse position is far enough away from the selection point, a "meander" shaped sequence of wires will be drawn that increases the length of the shorter signal segment. An indicator attached to the mouse cursor shows the target length (which is the length of the longer signal segment), as well as the deviation (in percent) of the two signals from the target length.
The meander starts at the first click point and extends to the second point the mouse is moved to. The maximum (perpendicular) size of the meander is defined by the distance of the mouse to the meandered wire.
If a single meander isn't enough to balance the lengths, you can add further meanders at different locations.
At any time you can enter a value in the command line to set the target length. This can be used for all signals, not just for differential pairs.
When meandering a differential pair with a given target length, the meander first tries to balance the length of the two signal segments that form the differential pair, and then increases the total length of both segments.
To reset the target length you can either restart the MEANDER command or enter a value of 0 in the command line.
If you do the measuring with Ctrl+Shift pressed, the maximum length of this or any previously selected segments will be taken. This can be used to easily determine the maximum length of several bus signals and then meandering each of them to that length.
The MENU command can be used to create a user specific command menu.
The complete syntax specification for the option parameters is
option := command | submenu | delimiter command := [ icon ] text1 [ ':' text2 ] submenu := [ icon ] text '{' option [ '|' option ] '}' icon := '[' filename ']' delimiter := '---'A menu option can be a simple command, as in
MENU Display Grid;which would set the menu to the commands Display and Grid. Display and Grid are interpreted both as menu text and as commands.
MENU 'MyDisp : Display None Top Bottom Pads Vias;' 'MyGrid : Grid mil 100 lines on;';which would set the menu to show the command aliases MyDisp and MyGrid and actually execute the command sequence behind the ':' of each option (text2, see above) when the respective button is clicked.
MENU 'Grid { Fine : Grid inch 0.001; | Coarse : Grid inch 0.1; }';which would define a button labeled Grid that, when clicked opens a submenu with the two options Fine and Coarse.
The special option '---' can be used to insert a delimiter, which may be useful for grouping buttons.
A command button can display an icon by preceding the button text with the file name of an icon, enclosed in square brackets, as in
MENU '[/path/to/myicon.png] Set a fine grid : Grid inch 0.001;';Here the button will display only the given icon, and "Set a fine grid" will be used as a "tool tip" that gets displayed when the mouse cursor is moved over the button. The filename needs not be enquoted additionally (like for masking spaces).
MENU 'Grid { [/path/to/myicon.png] Set a fine grid : Grid inch 0.001; }';then both the icon and the text will be displayed, as with any other popup menu.
Note that any option that consists of more than a single word, or that might be interpreted as a command, must be enclosed in single quotes. If you want to use the MENU command in a script to define a complex menu, and would like to spread the menu definitions over several lines to make them more readable, you need to end the lines with a backslash character ('\') as in
MENU 'Grid {\ Fine : Grid inch 0.001; |\ Coarse : Grid inch 0.1;\ }';
MENU Move Delete Rotate Route ';' Edit;would create a command menu that contains the commands Move...Route, the semicolon, and the Edit command.
The command
MENU;switches back to the default menu. Note that the ';' entry should always be added to the menu. It is used to terminate many commands.
Complex example:
MENU '[draw.png] Draw {\ Wire {\ Continous : CHANGE STYLE Continuous; WIRE |\ DashDot : CHANGE STYLE DashDot; WIRE |\ Help : HELP WIRE;\ }|\ Rectangle {\ RECT |\ Help : HELP RECT; \ }\ }\ [export.png] Export {\ Script : EXPORT SCRIPT |\ Image : EXPORT IMAGE\ }\ MyScript : SCRIPT MyScript.scr;';This menu consists of the 3 entries Draw, Export and MyScript, whereat Draw and Export have submenus and are supplied with icons. Draw consists of the submenus Wire and Rectangle, whereat Wire consists of the entries Continous, DashDot and Help and Rectangle consists of the entries RECT (text and command RECT) and Help.
Using the MIRROR command, objects may be mirrored about the y axis. One application for this command is to mirror components to be placed on the reverse side of the board.
Parts, pads, smds and pins can also be selected by their name, which is especially useful if the object is outside the currently shown window area.
Attributes of parts can be selected by entering the concatenation of part name and attribute name, as in R5>VALUE.
Components can be mirrored only if the appropriate tOrigins/bOrigins layer is visible.
When packages are selected for use with the MIRROR command, connected wires on the outer layers are mirrored, too (beware of short circuits!).
Note that any objects on inner layers (2...15) don't change their layer when they are mirrored. The same applies to vias.
Parts cannot be mirrored if they are locked, or if any of their connected pads would extend outside the allowed area (in case you are using a limited edition of EAGLE).
Wires, circles, pads and polygons may not be individually mirrored unless included in a group.
Mirrored text in a schematic will be printed on the other side of its origin point,
but it will still remain normally readable.
MITER
See also SPLIT,
WIRE,
ROUTE,
POLYGON
The MITER command can be used to take the edge off a point where two wires join. The two existing wires need to be on the the same layer and must have the same width and wire style.
The MODULE command is used to create modules used in hierarchical schematics and add module instances into a sheet.
If +offset is given, the current module instance will use this offset for naming the elements. The value has to be a multiple of 100 (e.g. +100). Please note that this is only supported for module instances in the main schematic.
The orientation of the module instance may be defined textually using the usual definitions as listed in the ADD command (R0, R90 etc.).
The PORT command is used to add ports to a module.
A module instance adds the parts and nets of that module to the board. Net names are composed using the module name and the net name (e.g. 'MODULE1:N$1'). If a net is exported through a PORT, it could be overwritten with a net connected to this port. Part names of a module instance with an offset are generated by adding this offset (e.g. 'R17' with offset '100' becomes 'R117'). If no offset is set, part names are composed the same way as net names (e.g. 'MODULE1:R17').
In order to choose a specific assembly variant of the module, its name has to be predended the module name variant_name@module_name (e.g. 'V1@ABC').
The MOVE command is used to move objects.
Parts, pads, smds, pins and gates can also be selected by their name, which is especially useful if the object is outside the currently shown window area. Note that when selecting a multi-gate part in a schematic by name, you will need to enter the full instance name, consisting of part and gate name.
Attributes of parts can be selected by entering the concatenation of part name and attribute name, as in R5>VALUE.
Elements can be moved only if the appropriate tOrigins/bOrigins layer is visible.
The MOVE command has no effect on layers that are not visible (refer to DISPLAY).
The ends of wires (tracks) that are connected to an element cannot be moved at this point.
When moving elements, connected wires (tracks) that belong to a signal are moved too (beware of short circuits!).
If an object is selected with the left mouse button and the button is not released, the object can be moved immediately ("click&drag"). The same applies to groups when using the right mouse button. In this mode, however, it is not possible to rotate or mirror the object while moving it.
Parts cannot be moved if they are locked, or if any of their connected pads would extend outside the allowed area (in case you are using a limited edition of EAGLE).
Pins placed on each other are connected together.
If unconnected pins of an element are placed on nets or pins then they are connected with them.
If nets are moved over pins they are not connected with them.
If you select a wire somewhere in the middle (not at one of its end points) with Ctrl pressed, the end points stay fixed and you can bend the wire, which changes it into an arc. The same way the curvature of an arc (which is basically a wire) can be modified.
If you select a rectangle at one of its corners with Ctrl pressed, you can resize both the rectangle's width and height. Selecting an edge of the rectangle with Ctrl pressed lets you resize the rectangle's width or height, respectively. Selecting the rectangle at its center with Ctrl pressed pulls it towards the cursor and snaps it into the current grid.
If you select a circle at its circumference with Ctrl pressed, the center stays fixed and you can resize the circle's diameter. Selecting the center point this way pulls it towards the cursor and snaps it into the current grid.
Note that only wires that have both ends in the group will be transferred, and any part that is transferred takes all its electrical connections with it, even if a net wire attached to one of its pins is not transferred because its other end is not in the group. In case a pin in the new sheet has an electrical connection, but no other pin, wire or junction attached to it to make this visible, a junction will be automatically generated at this point.
This process can even be scripted. For instance
edit .s1 group (1 1) (1 2) (2 2) (2 1) (1 1) move (> 0 0) edit .s2 (0 0)would switch to the first sheet, define a group, select that group with MOVE, switch to the second sheet and place the group. Note the final (0 0), which are coordinates to the implicitly invoked MOVE command.
See the EDIT command if you want to just reorder the
sheets.
NAME
See also SHOW,
SMASH,
VALUE
NAME new_name
NAME old_name new_name
The NAME command is used to display or edit the name of the selected object.
Parts, elements, pads, smds, pins and gates can also be selected by their name, which is especially useful if the object is outside the currently shown window area. Other object types (e.g. nets, busses, signals) have to be clicked first.
This segment
Every segment on this sheet
All segments on all sheets
These questions appear in a popup menu if necessary and can be answered either by selecting the appropriate item with the mouse or by pressing the appropriate hot key (T, E, A).
The net command is used to draw individual connections (nets) onto the Net layer of a schematic drawing. The first mouse click marks the starting point for the net, the second marks the end point of a segment. Two mouse clicks on the same point end the net.
If a net wire is placed at a point where there is already another net or bus wire or a pin, the current net wire will be ended at that point. This function can be disabled with "SET AUTO_END_NET OFF;", or by unchecking "Options/Set/Misc/Auto end net and bus".
If a net wire is placed at a point where there are at least two other net wires and/or pins, a junction will automatically be placed. This function can be disabled with "SET AUTO_JUNCTION OFF;", or by unchecking "Options/Set/Misc/Auto set junction".
If the curve or @radius parameter is given, an arc can be drawn as part of the net (see the detailed description in the WIRE command).
If no net name is included in the command line and the net is not started on a bus, then a name in the form of N$1 is automatically allocated to the net.
Nets or net segments that run over different sheets of a schematic and use the same net name are connected.
Net names should not contain a comma (','), because this is the delimiting character in busses.
SET NET_WIRE_WIDTH width;(Default: 6 mil).
!RESETwhich would result in
_____ RESETYou can find further details about this in the description of the TEXT command.
The OPEN command is used to open an existing library or create a new library. Once the library has been opened or created, an existing or new symbol, device, or package may be edited.
This command is mainly used in script files.
OPTIMIZE
See also SET,
SPLIT,
MOVE,
ROUTE
OPTIMIZE signal_name ..
OPTIMIZE ..
The OPTIMIZE command (which is only applicable in a board drawing) joins wire segments which lie in one straight line. The individual segments must be on the same layer and have the same width. This command is useful to reduce the number of objects in a drawing and to facilitate moving a complete track instead of individual segments.
If signal names are given, or a signal is selected, the command affects only the respective signals.
Note that when selecting an object with the mouse (or selecting a group) only actual signal wires are optimized. To optimize all wires in a board drawing, do
OPTIMZE;
SET OPTIMIZING OFF;or you have clicked the same spot twice with the SPLIT command.
The OPTIMIZE command works in any case, no matter if Optimizing
is enabled or disabled.
PACKAGE
See also CONNECT,
TECHNOLOGY,
PREFIX
PACKAGE pname vname
PACKAGE pname@lname vname
PACKAGE name
PACKAGE -old_name new_name
PACKAGE -name
This command is used in the device edit mode to define, delete or rename a package variant. In the schematic or board editor the PACKAGE command behaves exactly like "CHANGE PACKAGE".
Without parameters a dialog is opened that allows you to select a package and define this variant's name.
The parameters pname vname assign the package pname to the new variant vname.
The notation pname@lname vname fetches the package pname from library lname and creates a new package variant. This can also be done through the library objects' context menu or via Drag&Drop from the Control Panel's tree view.
The single parameter name switches to the given existing package variant. If no package variants have been defined yet, and a package of the given name exists, a new package variant named '' (an "empty" name) with the given package will be created (this is for compatibility with version 3.5).
If -old_name new_name is given, the package variant old_name is renamed to new_name.
The single parameter -name deletes the given package variant.
The name of a package variant will be appended to the device set name to form the full device name. If the device set name contains the character '?', that character will be replaced by the package variant name. Note that the package variant is processed after the technology, so if the device set name contains neither a '*' nor a '?' character, the resulting device name will consist of device_set_name+technology+package_variant.
Following the PACKAGE command, the CONNECT command is used to define the correspondence of pins in the schematic device to pads on the package.
When the BOARD command is used in schematic editing mode to create a new board, each device is represented on a board layout with the appropriate package as already defined with the PACKAGE command.
Note that supply or external devices are no longer treated as such, as soon as packages are assigned.
The pins have to be connected with pads then.
PAD
See also SMD,
CHANGE,
DISPLAY,
SET,
NAME,
VIA,
Design Rules
The PAD command is used to add pads to a package. When the PAD command is active, a pad symbol is attached to the cursor and can be moved around the screen. Pressing the left mouse button places a pad at the current position. Entering a number changes the diameter of the pad (in the actual unit). Pad diameters can be up to 200 mm (7.7840 inch).
The orientation (see description in ADD) may be any angle in the range R0...R359.9. The S and M flags can't be used here.
PAD 0.06 The pad will have a diameter of 0.06 inch, provided the actual unit is "inch". This diameter remains as a presetting for successive operations.
| Square | ||
| Round | ||
| Octagon | octagonal | |
| Long | elongated | |
| Offset | elongated with offset |
These shapes only apply to the outer layers (Top and Bottom). In inner layers the shape is always "round".
With elongated pads, the given diameter defines the smaller side of the pad. The ratio between the two sides of elongated pads is given by the parameter Shapes/Elongation in the Design Rules of the board (default is 100%, which results in a ratio of 2:1).
The pad shape or diameter can be selected while the PAD command is active, or it can be changed with the CHANGE command, e.g.:
CHANGE SHAPE OCTAGON The drill size may also be changed using the CHANGE command. The existing values then remain in use for successive pads.
Because displaying different pad shapes and drill holes in their real size slows down the screen refresh, EAGLE lets you change between real and fast display mode by the use of the SET commands:
SET DISPLAY_MODE REAL | NODRILL;Note that the actual shape and diameter of a pad will be determined by the Design Rules of the board the part is used in.
The following conditions apply:
SET PAD_NAMES OFF | ON;This change will be visible after the next screen refresh.
| NOSTOP | don't generate solder stop mask | |
| NOTHERMALS | don't generate thermals | |
| FIRST | this is the "first" pad (which may be drawn with a special shape) |
By default a pad automatically generates solder stop mask and thermals as necessary.
However, in special cases it may be desirable to have particular pads not do this.
The above NO... flags can be used to suppress these features.
If the Design Rules of a given board specify that the
"first pad" of a package shall be drawn with a particular shape, the pad marked with
the FIRST flag will be displayed that way.
A newly started PAD command resets all flags to their defaults. Once a flag is given
in the command line, it applies to all following pads placed within this PAD command
(except for FIRST, which applies only to the pad immediately following this
option).
See the ADD command for an explanation of orientation.
Using the commands GROUP, CUT, and PASTE, parts of a drawing/library can be copied to the same or different drawings/libraries. When using the PASTE command, the following points should be observed:
Assume you have a consistent board/schematic pair that contains the design of an amplifier, where the schematic may consist of several sheets. Now if you want to place this amplifier several times into your project, you can simply do
PASTE 100 amplifier.sch PASTE 200 amplifier.sch This example also shows the use of an offset, which adds the given value to all part and net names in the pasted files (unless they retain their name, see below). So the first amplifier channel will have all parts and nets named starting at 100, while the second one will have them start at 200. If no offset is given, new names are generated as necessary.
Just like in a normal PASTE operation, when pasting from a file, nets that have a label or are connected to a supply pin, retain their name while all others will get newly generated names. It is enough for a net to retain its name if it is labeled or connected to a supply pin on one sheet, even if it appears on several sheets.
Unless the PASTE operation is done in a script file, you will be offered a dialog that shows all the net names. By clicking on the names in the "New name" column you can edit individual net names. Icons indicate whether a net in the pasted drawing has a label or a supply pin, and whether the net will be connected to an existing net with the same name in the edited drawing.
If you paste a schematic into a schematic drawing, all sheets of the pasted schematic will be added as separate new sheets to the edited drawing (this is not possible in the Light edition, which can handle only a single schematic sheet). The corresponding board (if any) will be placed below the existing content of the edited board drawing. If you want to have explicit control over where the board is placed, you can perform the PASTE operation in the board, in which case the schematic sheets will be added just the same, but the board will be attached to the mouse cursor and you will be able to place it exactly where you want it.
For global settings in the files like layer definitions, netclasses, design rules
and autorouter parameters this holds: The settings of the currently opened drawing
are kept. This means e.g., that for the pasted data the restring parameters of
current drawing are used which can lead to differences compared to source drawing.
Please consider running a DRC for this.
Additional settings like additioal layers or netclasses are added to the current
drawing, of course.
You can also paste from a file using Drag&Drop, by pressing the Ctrl key when dropping the file.
If the file name could be mistaken as an orientation or an offset value,
you can enclose it in single quotes.
PIN
See also NAME,
SHOW,
CHANGE
Direction
Function
Length
Orientation
Visible
Swaplevel
| NC | not connected | |
| In | input | |
| Out | output (totem-pole) | |
| IO | in/output (bidirectional) | |
| OC | open collector or open drain | |
| Hiz | high impedance output (e.g. 3-state) | |
| Pas | passive (for resistors, capacitors etc.) | |
| Pwr | power input pin (Vcc, Gnd, Vss, Vdd, etc.) | |
| Sup | general supply pin (e.g. for ground symbol) |
Default: IO
If Pwr pins are used on a symbol and a corresponding Sup pin exists on the schematic, nets are connected automatically. The Sup pin is not used for components.
| None | no special function | |
| Dot | inverter symbol | |
| Clk | clock symbol | |
| DotClk | inverted clock symbol |
Default: None
| Point | pin with no connection or name | |
| Short | 0.1 inch long connection | |
| Middle | 0.2 inch long connection | |
| Long | 0.3 inch long connection |
Default: Long
| R0 | connection point on the right | |
| R90 | connection point above | |
| R180 | connection point on the left | |
| R270 | connection point below |
Default: R0
| Off | pin and pad name not drawn | |
| Pad | pad name drawn, pin name not drawn | |
| Pin | pin name drawn, pad name not drawn | |
| Both | pin and pad name drawn |
Default: Both
Default: 0
If a name is used in the PIN command, it must be enclosed in apostrophes. Pin names can be changed in the symbol edit mode using the NAME command.
PIN 'D0' *and the location for the other pins defined with a mouse click for each.
The SHOW command may be used to show pin options such as Direction and Swaplevel.
For example, suppose that three pins are required for GND. The pins are allocated the names GND@1, GND@2 and GND@3 during the symbol definition. Then only the characters before the "@" sign appear in the schematic.
It is not possible to add or delete pins in symbols which are already used by a device because this would change the pin/pad allocation defined with the CONNECT command.
!RESETwhich would result in
_____ RESETYou can find further details about this in the description of the TEXT command.
The PINSWAP command is used to swap pins within the same symbol which have been allocated the same swaplevel (> 0). Swaplevel, see PIN command. If a board is tied to a schematic via Back Annotation two pads can only be swapped if the related pins are swappable.
On a board without a schematic this command permits two pads in the same package to be swapped. The Swaplevel is not checked in this case.
Wires attached to the swapped pins are moved with the pins so that
short circuits may appear. Please perform the DRC and correct possible
errors.
POLYGON
See also CHANGE,
DELETE,
RATSNEST,
RIPUP,
WIRE,
MITER
The POLYGON command is used to draw polygon areas. Polygons in the layers Top, Bottom, and Route2..15 are treated as signals. Polygons in the layers t/b/vRestrict are protected areas for the Autorouter.
If the curve or @radius parameter is given, an arc can be drawn as part of the polygon definition (see the detailed description in the WIRE command).
If you want to give the polygon a name that starts with a digit (as in 0V), you must enclose the name in single quotes to distinguish it from a width value.
The parameters Isolate and Rank only have a meaning for polygons in layers Top...Bottom.
| 1. Outlines | only the outlines as defined by the user are displayed. | |
| 2. Real mode | all of the areas are visible as calculated by the program. |
In "outlines" mode a polygon is drawn with dotted wires, so that it can be distinguished from other wires. The board file contains only the "outlines".
The default display mode is "outlines" as the calculation is a time consuming operation.
When a drawing is generated with the CAM Processor all polygons are calculated.
The RATSNEST command starts the calculation of the polygons (this can be turned off with SET POLYGON_RATSNEST OFF;). Clicking the STOP button terminates the calculation of the polygons. Already calculated polygons are shown in "real mode", all others are shown in "outline mode".
The RIPUP command changes the display mode of a polygon to "outline".
CHANGE operations re-calculate a polygon if it was shown in "real mode" before.
SPLIT: Inserts a new polygon edge.
DELETE: Deletes a polygon corner (if only three corners are left the whole polygon is deleted).
CHANGE LAYER: Changes the layer of the whole polygon.
CHANGE WIDTH: Changes the parameter width of the whole polygon.
MOVE: Moves a polygon edge or corner (like wire segments).
COPY: Copies the whole polygon.
NAME: If the polygon is located in a signal layer the name of the signal is changed.
Under certain circumstances, especially with Orphans = Off, a polygon can disappear completely. In that case the polygon's original outlines will be displayed on the screen, to make it possible to delete or otherwise modify it. When going to the printer or CAM Processor these outlines will not be drawn in order to avoid short circuits. A polygon is also displayed with its original outlines if there are other non-polygon objects in the signal, but none of them is connected to the polygon.
When calculating whether such an object is actually solidly connected to the hatched polygon, it is reduced to several "control points". For a round pad, for instance, these would be the north, east, west and south point on the pad's circumference, while for a wire it's the two end points. A solid connection is considered to exist if there is at least one line in the calculated polygon (outline or hatch line) that runs through these points with its center line.
Thermal and annulus rings inside a hatched polygon that do not have solid contact to any of the polygon lines are not generated.
Only polygons in signal layers can have the pour style "Cutout".
The outlines of a cutout polygon are always drawn as dotted lines on the screen, even after the signal polygons have been calculated using RATSNEST.
The wire width of a cutout polygon is taken into account when subtracting it from
other signal polygons. It may be arbitrarily small (even zero) without causing large
amounts of CAM data (as opposed to "solid" polygons, where the wire width should
not be too small).
PORT
See also MODULE
PORT 'module' 'net_name' options ..
PORT 'module' 'net_name' options|DELETE
The PORT command is used to add ports to modules used in hierarchical schematics.
The position and orientation are calculated automatically on the closest side of the module symbol.
A port exports a net of a module to the outside and defines a connection point for another net. The net connected to the port provides the common name and class.
A port with a bus name exports all nets of that bus at once to the outside and defines a connection point for a proper bus.
If a net of a MODULE has an external connection through a PORT, the net class of the net on this port is overwriting the net class of the net in the module.
| NC | not connected | |
| In | input | |
| Out | output (totem-pole) | |
| IO | in/output (bidirectional) | |
| OC | open collector or open drain | |
| Hiz | high impedance output (e.g. 3-state) | |
| Pas | passive (for resistors, capacitors etc.) | |
| Pwr | power input pin (Vcc, Gnd, Vss, Vdd, etc.) |
Default: IO
In module context the direction of already existing ports can be changed.
The INFO command can be used to get the port properties
by selecting it with PREFIX
See also CONNECT,
MODULE,
PACKAGE,
VALUE
This command is used in the device editor mode to determine the initial characters of automatically generated symbol names when a symbol is placed in a schematic using the ADD command.
This command can also be used if editing a sheet of a module to set the prefix of this module.
PREFIX U;If this command is used when editing, for example, a 7400 device, then gates which are later placed in a schematic using the ADD command will be allocated the names U1, U2, U3 in sequence. These names may be changed later with the NAME command.
The PRINT command prints the currently edited drawing to the system printer.
Colors and fill styles are used as set in the editor window. This can be changed with the SOLID and BLACK options. The color palette used for the printout is always that for white background.
If you want to print pads and vias "filled" (without the drill holes being visible), use the command
SET DISPLAY_MODE NODRILL;Please note that polygons in boards will not be automatically calculated when printing via the PRINT command! Only the outlines will be drawn. To print polygons in their calculated shape you have to use the RATSNEST command before printing.
You can enter a factor to scale the output.
The limit parameter is the maximum number of pages you want the output to use. The number has to be preceded with a '-' to distinguish it from the factor. In case the drawing does not fit on the given number of pages, the factor will be reduced until it fits. Set this parameter to -0 to allow any number of pages (and thus making sure the printout uses exactly the given scale factor).
If the PRINT command is not terminated with a ';', a print dialog will allow you to set print options. Note that options entered via the command line will not be stored permanently in the print setup unless they have been confirmed in the print dialog (i.e. if the command has not been terminated with a ';').
The following options exist:
| MIRROR | mirrors the output | |
| ROTATE | rotates the output by 90° | |
| UPSIDEDOWN | rotates the drawing by 180°. Together with ROTATE, the drawing is rotated by a total of 270° | |
| BLACK | ignores the color settings of the layers and prints everything in black | |
| SOLID | ignores the fill style settings of the layers and prints everything in solid | |
| CAPTION | prints a caption at the bottom of the page | |
| FILE | prints the output into a file; the file name must immediately follow this option | |
| PRINTER | prints to a specific printer; the printer name must immediately follow this option | |
| PAPER | prints on the given paper size; the paper size must immediately follow this option | |
| SHEETS | prints the given range of sheets; the range (from-to) must immediately follow this option | |
| WINDOW | prints the currently visible window selection of the drawing | |
| PORTRAIT | prints in portrait orientation | |
| LANDSCAPE | prints in landscape orientation | |
| HIERARCHY | prints sheets of modules in hierarchical use |
If any of the options MIRROR...CAPTION is preceeded with a '-', that option is turned off in case it is currently on (from a previous PRINT). A '-' by itself turns off all options.
If the output file name has an extension of ".pdf" (case insensitive), a PDF file will be created. A PDF file can also be created by selecting "Print to File (PDF)" from the "Printer" combo box in the print dialog. Texts in a PDF file can be searched in a PDF viewer, as long as they are not using the vector font.
If the output file name has an extension of ".ps" (case insensitive), a Postscript file will be created.
If the file name is only an "*" or "*.ext" (an asterisk followed by an extension, as in "*.pdf", for instance), a file dialog will be opened that allows the user to select or enter the actual file name.
If the file name is only an extension, as in ".pdf", the output file name will be the same as the drawing file name, with the extension changed to the given string.
The file name may contain one or more of the following placeholders, which will be replaced with the respective string:
| %E | the loaded file's extension (without the '.') | |
| %N | the loaded file's name (without path and extension) | |
| %P | the loaded file's directory path (without file name) | |
| %% | the character '%' |
For example, the file name
%N.cmp.pdf
would create boardname.cmp.pdf.
If both the FILE and the PRINTER option are present, only the last one given will be taken into account
Width x Height Unit(without blanks), as in
PRINT PAPER 200x300mm PRINT PAPER 8.0x11.5inchWidth and Height can be floating point numbers, and the Unit may be either mm or inch (the latter may be abbreviated as in). Paper names must be given in full, and are case insensitive. If both the PRINTER and PAPER option are used, the PRINTER option must be given first. Custom paper sizes may not work with all printers. They are mainly for use with Postscript or PDF output.
| opens the print dialog in which you can set print options | ||
| PRINT; | immediately prints the drawing with the default options | |
| PRINT - MIRROR BLACK SOLID; | prints the drawing mirrored, with everything in black and solid | |
| PRINT 2.5 -1; | prints the drawing enlarged by a factor of 2.5, but makes sure that it does not exceed one page | |
| PRINT FILE .pdf; | prints the drawing into a PDF file with the same name as the drawing file | |
| PRINT SHEETS 2-15 FILE .pdf; | prints the sheets 2 through 15 into a PDF file with the same name as the drawing file | |
| PRINT SHEETS ALL; | prints all sheets of the main schematic and of all modules as drawn | |
| PRINT HIERARCHY SHEETS ALL; | prints all sheets of the main schematic and all sheets of the modules according to their module instances |
You can also exit from EAGLE at any time by pressing Alt+X.
RATSNEST
See also SIGNAL,
MOVE,
POLYGON,
RIPUP
RATSNEST signal_name ..
RATSNEST ! signal_name ..
The RATSNEST command assesses the airwire connections in order to achieve the shortest possible paths, for instance, after components have been moved. After reading a netlist via the SCRIPT command, it is also useful to use the RATSNEST command to optimize the length of airwires.
The RATSNEST command also calculates all polygons belonging to a
signal. This is necessary in order to avoid the calculation of
airwires for pads already connected through polygons. All of the calculated
polygon areas are then being displayed in the "real mode".
You can switch back to the faster
"outline mode" with the RIPUP command.
The automatic calculation of the polygons can be turned off with
SET POLYGON_RATSNEST OFF;Note that RATSNEST doesn't mark the board drawing as modified, since the calculated polygon data (if any) is not stored in the board, and the recalculated airwires don't really constitute a modification of the drawing.
Such zero length airwires can be picked up with the ROUTE command just like ordinary airwires. They may also be handled by placing a VIA at that point.
Ratsnest: Nothing to do!Otherwise, if there are still airwires that have not been routed, the message
Ratsnest: xx airwires.will be displayed, where xx gives the number of unrouted airwires.
| * | matches any number of any characters | |
| ? | matches exactly one character | |
| [...] | matches any of the characters between the brackets |
If any of these characters shall be matched exactly as such, it has to be enclosed in brackets. For example, abc[*]ghi would match abc*ghi and not abcdefghi.
A range of characters can be given as [a-z], which results in any character in the range 'a'...'z'.
To hide airwires the RATSNEST command can be given the exclamation mark ('!'), followed by a list of signals, as in
RATSNEST ! GND VCCwhich would hide the airwires of the signals GND and VCC.
RATSNEST GND VCCThis will activate the display of the airwires of the signals GND and VCC and also recalculates them. You can also recalculate the airwires (and polygons) of particular signals this way.
The signal names may contain wildcards, and the two variants may be combined, as in
RATSNEST D* ! ?GND VCCwhich would recalculate and display the airwires of all signals with names beginning with 'D', and hide the airwires of all the various GND signals (like AGND, DGND etc.) and the VCC signal. Note that the command is processed from left to right, so in case there is a DGND signal the example would first process it for display, but then hide its airwires.
To make sure all airwires are displayed enter
RATSNEST *Note that the SIGNAL command will automatically make the airwires of a signal visible if a new airwire is created for that signal. The RIPUP command on the other hand will not change the state of hiding airwires if a wire of a signal is changed into an airwire.
The RECT command is used to add rectangles to a drawing. The two points define two opposite corners of the rectangle. Pressing the center mouse button changes the layer to which the rectangle is to be added.