CHANGE | CIRCLE | CLASS | CLOSE | CONNECT | COPY | CUSTOM3D | CUT
Function
Changes parameters.
Syntax
CHANGE option ..
Mouse keys
Ctrl+Right changes parameter of the group.
The CHANGE command is used to change or preset properties of objects. To apply the change, pick the desired parameters from the CHANGE command menu or enter them from the keyboard, and then click the selected objects. 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.
When using the CHANGE command with a group, the group is first identified with the GROUP command before entering the CHANGE command with appropriate parameters. Use the right mouse button to execute the changes.
CUSTOM font uses any installed True Type / Clear Type fonts. The associated font family can be chosen using the FONTFAMILY property.
Changes the font family (FONTFAMILY) for any subsequent user text to the value specified in the 'new-fontfamily'. The Text Properties dialog displays the available font families in the Font Family drop-down menu. In Microsoft Windows, Font settings lists the available fonts. In MacOS, All Fonts lists the available fonts. The font family maps to the Full Name font property that can be found when searching for fonts in either operating system.
CHANGE DLINE 0.1mm;
changes dimension line width to 0.1 mm. Extension parameters are left unchanged.
CHANGE DLINE 0.2mm - 0.5mm AUTO;
changes dimension line width to 0.2 mm, extension line length to 0.5 mm and extension offset to AUTO. The extension line width is left unchanged.
CHANGE FONT CUSTOM
changes font type to CUSTOM (use true type / clear type fonts)
CHANGE FONTFAMILY 'Arial'
changes the current font family to 'Arial'. Note: single quotes are required.
Function
Adds circles to a drawing.
Syntax
CIRCLE .. [center, circumference]
CIRCLE width ..
Mouse keys
Center selects the layer.
Use CIRCLE to create circles. Circles in the layers RestrictTop, RestrictBottom, and RestrictVias 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 LINE 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.
The radius of the resulting circle is limited to 1000 mm.
GRID inch 1; CIRCLE (0 0) (1 0);
generates a circle with a radius of 1 inch and the center at the origin.
Function
Define and use net classes.
Syntax
CLASS
CLASS number|name
CLASS number [ name [ width [ clearance [ drill ] ] ] ] [ number:clearance .. ]
Use CLASS 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 used for subsequent NET and SIGNAL commands.
If both a number and a name are given, the net class with the given number is assigned all the following values and is also used for subsequent NET and SIGNAL commands. If any of the parameters following name are omitted, the net class keeps its respective value.
If number is negative, the net class with the absolute value of number is cleared. The default net class 0 can't be cleared.
Net class names are handled not case-sensitive, 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.
The width parameter defines a minimum width that all objects in this net class must have.
The clearance parameter defines the minimum clearance between objects of different signals in this net class and objects in other net classes.
The drill parameter defines a minimum drill size that all objects in this net class must have (only applies to objects that actually have a drill parameter, like pads and vias).
If a clearance is given in the form number:clearance, it defines the minimum clearance between signals in this net class and signals in the net class with the given number. The command
CLASS 3 1:0.6mm 2:0.8mm
defines 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 3:0.2mm
would also be valid, whereas
CLASS 3 1:0.6mm 2:0.8mm 3:0.2mm 4:0.5mm
would not be allowed. A clearance value of '0' between two net classes means, there is no specific value. Then the higher value of the participating net classes will be used.
Function
Closes an editor window.
Syntax
CLOSE
See also OPEN, EDIT, WRITE, SCRIPT.
Use CLOSE to close an editor window. If the drawing you are editing has been modified, you are prompted whether to save it.
This command is mainly used in script files.
Function
Assigns pads to pins.
Syntax
CONNECT
CONNECT [ ALL | ANY ] gate_name.pin_name pad_name..
CONNECT [ ALL | ANY ] pin_name pad_name..
See also PREFIX, OPEN, CLOSE, SCRIPT.
Use CONNECT in the device editing mode to define the relationship between the pins of a gate and the pads of the corresponding footprint in the library. First of all, it is necessary to define which package to use with the PACKAGE command.
If the CONNECT command is invoked without parameters, a dialog is presented which allows you to interactively assign the connections.
If only one gate is included in a device, the parameter gate_name can be dropped, for example:
CONNECT gnd 1 rdy 2 phi1 3 !irq 4 nc1 5...
(Note: "!" is used to indicate inverted data signals.)
If several gates are present in a device, parameters must be entered with gate_name, pin_name and pad_name each time. For example:
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.
Some parts, like power amplifiers or BGA chips, may have several pads that are connected internally. This may be done for better heat dissipation or to allow for higher currents. The CONNECT command can handle these cases by simply listing all related pad names, separated by blanks (and therefore enclosed in single quotes), as in
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.
In the second example, the keyword ANY indicates that any one (or even all) of the pads 2, 4 or 6 can be connected to the signal. It is even allowed to use this internal connection as a "bridge" by connecting one segment of the signal to, say, pad 2, while connecting the rest of the signal to pad 6, without any explicit external connection between these two pads. Of course, when designing a library part and using ANY in a CONNECT command, you need to be sure that the part will be able to handle cross currents running through its pads. If in doubt, use ALL (which is the default and may be omitted). If a pin name would collide with one of the keywords ALL or ANY, the pin name needs to be enclosed with single quotes. As soon as one of these keywords appears in a CONNECT command, it applies to all pin/pad connections that follow it, until a different keyword is seen, as in
CONNECT 'A' '1' 'B' '2' ANY 'C' '3 4 5 6' 'D' '7 8' ALL 'E' '9 10 11';
The RATSNEST and AUTO command will handle the ALL and ANY cases appropriately.
In the CONNECT dialog, the "Connect" button creates a 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 this icon to toggle the mode. When such a connection item is expanded, all the pads are listed separately, and clicking Disconnect with one of the pads selected will only disconnect that one pad.
If a gate or pin name contains a period, simply enter them without any special consideration (no quoting or escape characters are necessary).
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.
Function
Copy objects.
Syntax
COPY ..
COPY deviceset@[library] [name]
COPY footprint@[library] [name]
COPY package3d@[library] [name]
COPY symbol@[library] [name]
Mouse keys
Ctrl+C copies currently selected objects.
Ctrl+Left selects an object at its origin.
Ctrl+Right selects the group.
Center mirrors the selected object or the group.
Right rotates the selected object or the group.
Shift+Right reverses the direction of rotating.
See also GROUP, CUT, PASTE, ADD, INVOKE, POLYGON.
Use COPY to copy objects within the same drawing, or between libraries. Electronics generates a new name for the copy but retains the old value. When copying signals (wires), buses, and nets the names are retained, but in all other cases a new name is assigned.
The COPY command in EAGLE traditionally could only be used to copy objects by clicking them and placing their instances within the same drawing, or to copy library objects between libraries. However, before version 6 it did not send the current group selection to the system's clipboard. In EAGLE, the CUT command was used for this, but beginning with version 6, the COPY command also copies the selected group of objects to the clipboard, while still retaining the full functionality of previous versions. If you don't like this, you can use the SET command
SET Cmd.Copy.ClassicEagleMode 1
to get back the original behavior of the COPY command (as well as the CUT command).
If you copy wires or polygons, belonging to a signal, the copy will belong to the same signal. Note, for this reason, if two wires overlap after the use of the COPY command, the DRC will not register an error.
If one of the endpoints of the copied wire lies on the source segment, the wire is connected to this segment. If not, an extra segment is created for this wire (see also 'Copy and connectivity').
When copying a part in a schematic, there will always be a new instance of the complete part added, even if only a single gate of a multi-gate part is selected. In addition to the selected gate, any other gates of that device which have Add-Level MUST or ALWAYS will automatically be invoked. If you just want to use another gate of a multi-gate part, you should use the INVOKE command instead.
By writing COPY deviceset@[library], COPY footprint@[library], COPY package3d@[library], or COPY symbol@[library], you can copy a device set, footprint, 3D package or symbol from a given library into the currently loaded library. The library attribute can be either a plain library name, a file path (see ADD command), the URN of a downloaded managed library, or be omitted. If it's a library name, it is searched for in the currently set library path(s) and among the downloaded managed libraries. If it's a URN, it searched for among the downloaded managed libraries. If library is omitted, the currently loaded library is taken as source. In case of ambiguity, you can add the suffix .dev/.fpt/.p3d/.sym to the object name. (Note that the use of ".fpt" to specify a footprint is new as of EAGLE 9.1. For compatibility with previous versions, ".pac" is also supported.) If an additional name is given, the copied object will be given that name. This can also be done through the library objects' context menu or with Drag&Drop from the Control Panel's tree view. Note that any existing library objects (device sets, symbols, footprints, 3D packages) used by the copied library object will be automatically updated.
By writing COPY device [name], COPY footprint [name], COPY package [name], or COPY symbol [name] you can copy a device set, footprint, 3D package or symbol from a design into the currently loaded library. Name is either a part name (in schematic) or an element name (in board). COPY symbol [name] is supported in schematic window, COPY footprint [name] and COPY package [name] are supported in board window, and COPY device [name] is supported in both windows. Device can be copied from board if the corresponding schematic is available. If name is not specified in the command, you can select any valid object by mouse left click in the design to copy to loaded library.
Copying a group by selecting it with the right mouse button is actually done by doing an implicit CUT operation, immediately followed by a PASTE.
To copy objects to an other sheet of the same schematic, you need to GROUP the objects, do a COPY (or CUT), switch to the target sheet and then do PASTE.
Copying of wires does not change their connectivity. For instance, if you copy a net and position it at another net, it doesn't get connected to this net. The same is for segments of the same net, busses etc. For connections use NAME or JUNCTION.
If objects are copied using Ctrl+C, it works differently for a single object compared to more than one (a GROUP). If a single object is copied, the origin is used as the reference point when pasting the object later. If you copy a group of objects, it allows you to define an anchor, here called a "free anchor".
This means EAGLE will remember this point within the selected group you used for copying and will use that point for pasting. Typical example is large group of objects, you want to place relative to a certain point within those objects (as opposed to the default center position).
In this case, you would use Ctrl+C after placing the mouse cursor at the location of your choice, and this point will be used for pasting. In other words, for groups of objects, Ctrl+C remembers where your cursor was when you copied the objects, and uses it for pasting.
Function
Add a 3D model to element/part in the board/schematic editor.
Syntax
CUSTOM3D
Mouse keys
Left selects the element/part to apply the command to.
Function
Copies a group into the clipboard.
Syntax
CUT
CUT;
Use CUT and PASTE to copy parts of a drawing (or even a whole board) onto other drawings.
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.
If you click the mouse after selecting the CUT command, the position of the mouse cursor defines a reference point for the group, i.e. when using the PASTE command, the mouse cursor will be at the exact position of the group.
Unlike other (Windows-) programs, the Electronics CUT command does not physically remove the marked group from the drawing; it only copies the group into the clipboard. Beginning with EAGLE version 6, the CUT command no longer appears in the main drop-down menu or the toolbar (it is still available from the command line and within scripts). Windows users can use the COPY command to copy the selected group of objects into the system's clipboard. This, however, does not allow them to define an explicit reference point for the selected group. It will always be selected at the center of the group's bounding rectangle. Using a reference point is only possible with the CUT command. An alternative is to use the SET command
SET Cmd.Copy.ClassicEagleMode 1
to get back the original behavior of the CUT command (as well as the COPY command).