BOARD | BREAKOUTBUS | BUS
Function
Converts a schematic into a board.
Syntax
BOARD [ grid ]
See also EDIT.
Use the command BOARD to convert a schematic drawing into a board. If the board already exists, it is loaded into a board window. If the board does not exist, you are asked whether to create that new board. If a grid is given, the parts on the board are placed in the given raster, as in
BOARD 5mm
which places the parts in a 5-mm raster (default is 50 mil). The number must be given with a unit, and the maximum allowed value is 10 mm. The BOARD command never overwrites 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.
The first time you edit a board, the program checks if there is a schematic with the same name in the same directory and gives you the choice to create the board from that schematic.
If you have opened a schematic window and want to create a board, just type
edit .brd
in 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 160x100 mm (Light edition: 100x80mm). All packages and connections are shown on the left side of the board. Supply pins are already connected (see PIN).
If you need board outlines different to the ones that are generated by default, delete the respective lines and use the LINE command to draw your own outlines into the Dimension layer. The recommended width for these lines is 0.
A board file cannot be generated:
Function
Breakout member nets from a bus as new nets with labels.
Syntax
BREAKOUTBUS ..
The BREAKOUTBUS command is accessed from the context menu after right-clicking on a bus. The breakout types are given as choices in the menu: "All Nets", "Selected Nets", and "Single Net". The "Selected Nets" option will bring up a dialog where the user can choose which nets to breakout. "Single Net" is a submenu where all members of the bus are shown and a single net can be chosen. "All Nets" breaks out all members of the bus.
Once a breakout choice is made new nets with labels are created, spaced 1 grid apart, along the bus, and the user then clicks to finalize the placement of the new nets. Holding down SHIFT while placing the nets will freeze the shape of the new nets, and allow movement only along the bus.
Function
Draws buses in a schematic.
Syntax
BUS [? | {PREDEFINED_BUS_NAME} | bus_spec] [curve | @radius] ..
BUS {PREDEFINED_BUS_NAME=bus_spec}
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 INFO, BREAKOUTBUS, NET, NAME, SET.
A BUS is a collection of nets. A BUS has a specification and is drawn as one or more bus line segments. The bus specification may include a (strictly unique) alias, which is a short name used to identify the bus. The BUS command is used to draw buses onto the Bus layer of a schematic diagram.
EAGLE has the ability to save reusable bus specifications as "Predefined Busses" (PDBs). The PDBs are saved in the eaglerc file and can be used across projects, even shared with others (example: SPI:MISO,MOSI,CLK,CS). By including the PDB in braces after the BUS command, the bus will adopt this specification when drawn. The PDB name must be valid and exist in the eaglerc file to use in this way.
BUS {PREDEFINED_BUS_NAME}
The BUS toolbar command button supports a context menu, with quick access to existing PDBs. Choosing one from this menu is equivalent to using the command format above.
New PDBs can be also created from the command line using the format below. Note that the PDB name must be unique, and the bus_spec must be a valid bus specification as described in this section. PDBs are saved to eaglerc and are available immediately for use.
BUS {PREDEFINED_BUS_NAME=bus_spec}
If you type BUS ? on the command line (or choose "New" from the context menu on the BUS button in the command toolbar), the Predefined Bus dialog will open, where you can create and manage PDBs.
BUS ?
Bus_spec has the following form:
ALIAS:partbus,partbus,..
where ALIAS can be any name. Partbus is either a simple net name or a name range of the following form:
NetName[LowestIndex..HighestIndex]
where the following condition must be met: 0 <= LowestIndex <= HighestIndex <= 511
If a name is used with a range, that NetName 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 deselecting "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 LINE 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 specification is given, a specification of the form B$1 is automatically allocated. This can be changed with the NAME or INFO 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).
The name of an inverted signal ("active low") can be displayed overlined if it is preceded with an exclamation mark ('!'), as in
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.
Buses can be broken out automatically with new labeled nets using the BREAKOUTBUS command, available from the command line and by the bus object right-click context menu.