Function
Displays and changes names.
Syntax
NAME ..
NAME new_name
NAME old_name new_name
See also LABEL, SHOW, REPOSITION, VALUE.
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 (for example nets, busses, signals) have to be clicked first.
When in library edit mode, the NAME command is used to display or edit the name of the selected pad, smd, pin, or gate.
EAGLE generates names automatically: N$.. for nets, E$.. for elements, S$.. for signals, P$.. for pads, pins and smds. In general, it is convenient to substitute commonly used names (for example 1...14 for a 14-pin dual inline package) in place of these automatically generated names. Automatic naming of parts can be controlled with PREFIX.
Letters for EAGLE object names are automatically converted to uppercase. Beside normal characters, EAGLE tolerates most other special characters except blank and semicolon (';'). For nets, parts, module instances, signals, and elements the colon (':') is also not supported because it is needed for automatic naming of objects in hierarchical designs in a unique way.
For example, element AMP1:IC1 can only relate to a part IC1 in the module which is used by module instance AMP1, assuming consistency. Beside the main schematic, each module has its own namespace. So it's no problem to have parts R1-R9 in main schematic and also in some modules. See also MODULE command, naming section.
If nets or busses are to be renamed, the program has to distinguish between three cases because they can consist of several segments placed on different sheets. Thus a menu will ask the user: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).
When changing nets and busses, there is a checkbox to confirm if the user wants to place a label on the same net or bus after the NAME change is complete, which is checked by default if a LABEL does not yet exist. If the user confirms the NAME change with this box checked, the LABEL command will start and once done, control will return to the NAME command.
When renaming a signal polygon in a board, you can choose whether to rename only this polygon (and thus move it from one signal into another), or to give the entire signal a different name.
Function
Draws nets on a schematic.
Syntax
NET [net_name] [curve | @radius] ..
NET BREAKOUT [PIN | UNIQUE] [LENGTH=VALUE] ..
NET BREAKOUT [AUTOINCR] [LENGTH=VALUE] net_name ..
Mouse keys
Right changes the wire bend style (see SET Wire_Bend).
Shift+Right reverses the direction of switching bend styles.
Ctrl+Right toggles between corresponding bend styles.
See also BUS, BREAKOUTBUS, CLASS, NAME, PINBREAKOUT, SET.
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.
Net wires snap to the tips of pins. When the mouse is within SNAP_LENGTH of any portion of a pin (either before or after grid snapping), a small circle will appear at the tip of the pin. This indicates that if the mouse is clicked, the resulting net wire point will be placed at the pin tip, creating a connection to the pin.
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 deselecting "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 LINE command).
If a net is started on a bus, a popup menu opens from which one of the bus signals can be selected. The net then is named correspondingly and becomes part of the same signal. If the bus includes several part buses, a further popup menu opens from which the relevant part bus can be selected.
If the NET command is used with a net name, then the net is named accordingly. If no net name is included on 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. Net names should also not contain '[' and ']', because they are used to specify a range in a bus. Nets from such a range have the index w/o these brackets. (For example the bus D[0..15] has the according nets: D0, D1, ...)
The NET command includes breakout options that allow you to select any part pins in your schematic (from any number of parts) and create new nets that breakout from the chosen pins, and with the specified label format. The UI version of that command is available by clicking the "Pin Breakout" button in the NET parameter toolbar, or by using NET BREAKOUT from the CLI. Start the command without any parameters (or by NET parameter toolbar button) and you can specify the breakout type in the user interface. Then click any pins from any parts in schematic to breakout out new nets with labels matching the chosen option.
The other command line options allow you to supply the type of label which can be PIN, UNIQUE, or net_name. If a net_name is supplied, this will be used for the net name regardless of what pin is connected.
Keywords PIN, UNIQUE, and AUTOINCR have special meanings and cannot be used as a net_name value: using keyword PIN means the new net with be named after the pin it is connected to. Choosing UNIQUE will create a label string with format: part_gate_pin, where the part, gate, and pin name are concatenated into a unique string for that net based on these values from the selected parts/pins.
The optional keyword AUTOINCR goes before a custom net name, and indicates that, if the user keeps adding pins, they should autoincrement, provided that the last character in the net_name is a number. For example, using ADDR1 with AUTOINCR before net_name results in ADDR2, ADDR3, etc as the nets are placed on pins.
The optional keyword LENGTH allows to set a minimum length, in # of grid units, for the new net segments created. This length of the new nets will be this min length, or the length calculated for the width of the label text, whichever is larger.
Buses can be broken out automatically with new labeled nets using the BREAKOUTBUS command, available from the command line and in the bus object right-click context menu. See BREAKOUTBUS for details.
Parts can be broken out automatically with new labeled nets using the PINBREAKOUT command, available from the command line and in the part instance right-click context menu. See PINBREAKOUT for details.
The width of the line drawn by the net command may be changed with the command:
SET NET_WIRE_WIDTH width;
(Default: 6 mil).
The name of an inverted signal ("active low") can be displayed overlined if it is preceded with an exclamation mark ('!'), as in
!RESET
which would result in
_____ RESET
You can find further details about this in the description of the TEXT command.