P Reference

PACKAGE | PAD | PADARRAY | PAINTROLLER | PASTE | PATTERN | PIN | PINARRAY | PINBREAKOUT | PINSWAP | PINTOBUS | POLYGON | POLYGONIZE | PORT | PREFIX | PRINT

PACKAGE

Function

 Defines a package variant for a device.

Syntax

 PACKAGE

 PACKAGE pname vname

 PACKAGE pname.fpt vname (new in EAGLE 9.1)

 PACKAGE pname.pac vname (alternative for backward compatibility)

 PACKAGE pname.p3d vname

 PACKAGE urn vname

 PACKAGE pname@lname vname

 PACKAGE name

 PACKAGE -old_name new_name

 PACKAGE -name

 PACKAGE @vname

 PACKAGE @vname pname

 PACKAGE @vname pname.pac

 PACKAGE @vname pname.3d

 PACKAGE @vname urn

See also CONNECT, ATTRIBUTE SET, PREFIX.

This command is used in the device edit mode to define, delete, or rename a package variant (footprint and optional 3D package). 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 footprint (and 3D package) and define this variant's name.

The parameters pname vname assign the footprint pname to the new variant vname. If there's exactly one 3D package in the current library that references that footprint, and the 3D package references only that footprint, the 3D package will also be added to the new variant. To avoid including such a 3D package in the variant, use the notation pname.fpt vname (or pname.fpt vname). Use the notation pname.p3d vname to specify a 3D package in the library; this will create a new variant for each footprint in the 3D package. Each variant will also include the 3D package.

The notation urn vname creates a new variant for each footprint in the 3D package with the given urn. (The urn should be of the form urn:adsk.eagle:package:123/1, where 123 is the id of the 3D package and 1 is the version of the 3D package.) If the specified 3D package is not already present in the library, it will be downloaded and added to the library prior to creation of the variant(s).

The notation pname@lname vname fetches the footprint pname from library lname and creates a new package variant. This can also be done through the library objects' context menu or with Drag&Drop from the Control Panel's tree view.

The single parameter name switches to the given existing package variant.

Compatibility with version 3.5:

If no package variants have been defined yet, and a footprint of the given name exists, a new package variant named '' (an "empty" name) with the given footprint will be created.

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 @vname syntax allows an existing package variant to be updated by replacing its current footprint and 3D package with a different footprint and 3D package. The variant's existing connections and attributes will be retained. If @vname pname is given, the variant's existing footprint will be replaced with the footprint specified by pname. If there's exactly one 3D package in the current library that references that footprint, and the 3D package references only that footprint, the 3D package will also be added to the variant. To avoid including such a 3D package in the variant, use the notation @vname pname.fpt (or @vname pname.pac). Use the notation @vname pname.p3d or @vname urn to specify a 3D package in the library; if there's only one footprint in the 3D package, the footprint and 3D package will be assigned to the variant. (It's not currently possible to assign a 3D package with more than one footprint to a variant.) If just @vname is given, a dialog is opened that allows you to select the replacement footprint and 3D package. Note that in all cases, the replacement footprint and 3D package must already be present in the library.

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 attribute set, so if the device set name contains neither a '*' nor a '?' character, the resulting device name will consist of device_set_name+attribute_set+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.

Devices without packages

Devices can also be created without assigning a package, for example for frames, supply devices, external or other devices that only make sense in a schematic. This can be done by creating a device set with adequate gates, technologies, and attributes (if necessary) without using the PACKAGE command. If saved, a packageless variant is created (with empty string as variant name). As soon as a package is assigned, the packageless variant gets overwritten by this and no further packageless variants can be created.

As soon as gates contain pins, packageless devices only make limited sense (see below).

Supply devices

In order to use supply symbols in schematics, packageless supply devices are common. The device usually consists of exactly one symbol with a Sup pin (see PIN command).

External devices

These are for documenting assemblies in schematic that are not relevant for the board because they are externally added, for example for simulation or test purposes.

Such devices must be marked with the attribute EXTERNAL (see ATTRIBUTE command). The value is not relevant. In this case, any gates with pins can be defined without a package. The attribute must have been assigned in the library, not in schematic or board. 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.

Top

PAD

Function

 Adds pads to a footprint.

Syntax

 PAD [diameter] [shape] [orientation] [flags] ['name'] ..

Mouse keys

Right rotates the pad.

Shift+Right reverses the direction of rotating.

See also SMD, CHANGE, DISPLAY, SET, NAME, VIA.

The PAD command is used to add pads to a footprint. 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.

Example

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.

Pad Shapes

A pad can have one of the following shapes:

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, for example:

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 are determined by the Design Rules of the board on which the part is used.

Arbitrary Pad Shapes

If the standard pad shapes are not sufficient for a particular footprint, you can create arbitrary pad shapes by drawing a polygon around a pad, or by drawing wires that have one end connected to the pad. The following conditions apply:

Pad Names

Pad names are generated by the program automatically and can be changed with the NAME command. The name can also be defined in the PAD command. Pad name display can be turned on or off by means of the commands:

SET PAD_NAMES OFF | ON;

Flags

The following flags can be used to control the appearance of a pad:

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 footprint 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 on 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).

Single Pads

Single pads in boards can be used only by defining a footprint with one pad. Via-holes can be placed in board but they don't have an element name and therefore don't show up in the netlist.

Top

PADARRAY

Function

 Create arrays of pads.

Syntax

 PADARRAY [sides base start count dx dy unit drawrect includename includevalue deleteobjs]

See also PAD.

The PADARRAY command allows to create an array of pads in the Library Footprint Editor. If the command is started from the icon in the PAD parameter toolbar, a dialog pops up where the options for sides, basename, start index, number of pads, and others are set before creating the array. If the command is started from the command line and arguments are provided, the same options are available as specified below.

Options

If the arguments are provided after the command, all need to be present:

sides This can be L, R, LR, T, B, or TB, which indicates onto which sides of a rectangle to draw the pads, where L=Left, R=Right, T=Top, and B=Bottom.
base This is the base name to use when naming pads, where pads are named such that the first pin is and subsequent pad are named with an increasing numerical suffix (i.e, ADDR1, ADDR2, .. ADDRN). The last pad placed with have a name given by
start The is the start index for pad naming. The first pad starts with a name
count The number of pads to place.
dx The distance in X direction between pads.
dy The distance in Y direction between pads.
unit Valid values are: MIC (for micron), MM (millimeter), MIL (mil = 0.001 inch), INCH.
drawrect ON or OFF, indicates whether or not to draw a rectangle in the SilkscreenTop layer as part of the operation
includename ON or OFF, indicates whether or not to place a text object with >NAME as the value
includevalue ON or OFF, indicates whether or not to place a text object with >VALUE as the value
deleteobjs ON or OFF, indicates whether or not to delete pads,labels,and line objects before placing the array

Top

PAINTROLLER

Function

 Transfers selected properties of an object to other objects of the same type.

Syntax

 PAINTROLLER

 PAINTROLLER

 PAINTROLLER [propertyname]

The PAINTROLLER command can be started on the command line or with the PAINTROLLER icon in the commands toolbar. Select the properties you want to transfer to other objects of the same type in the Copy Properties dialog of the selected object, then close the dialog with OK, and click the target objects.

Top

PASTE

Function

 Copies the contents of the clipboard or a drawing or a design block file to a drawing.

Syntax

 PASTE [ orientation ]

 PASTE [ orientation ] [ offset ] filename

 PASTE [ DBL ][ orientation ] [ offset ] filename

Mouse keys

Center mirrors the contents of the clipboard.

Right rotates the contents of the clipboard.

Shift+Right reverses the direction of rotating.

Ctrl+V pastes the contents of the clipboard.

See also CUT, COPY, GROUP.

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:

If there are modified versions of devices or footprints in the clipboard, an automatic library update will be started to replace the objects in the schematic or board with the ones from the clipboard.

Note: You should always run a Design Rule Check (DRC) and an Electrical Rule Check (ERC) after a library update has been performed!

Pasting from a file

If a file name is given on the command line, the complete content of that file is pasted into the current drawing. If the given file is one of a consistent board/schematic pair and a consistent board/schematic pair is being edited, both files will be pasted into the corresponding drawings. If you set * instead of the file name or just a directory, a file dialog opens in the project directory or the set directory. 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 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. 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, for example, that for the pasted data the restring parameters of current drawing are used which can lead to differences compared to source drawing. Consider running a DRC for this.

Additional settings like additional 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.

For cases where the file name could be mistaken as an orientation or an offset value, enclose it in single quotes.

Pasting a Design Block (DBL)

If the DBL option is used, it pastes a design block by file name. If no file name is given, a dialog similar to the ADD dialog pops up. In general, this option is equal to pasting from a drawing file or a consistent pair of drawing files. A design block may contain a board and a schematic. It will paste all data it can. If there is only an opened schematic, it will paste only the schematic part of the design block, accordingly for boards. To paste both, a consistent pair has to be loaded. If the command is started from board editor, it has the same behavior as pasting from a drawing file. The board can be placed by a mouse click and new sheets are added to schematic. If the command is started from schematic editor and the design block has only one sheet, it can be placed by a mouse click into the current sheet as well. No automatic placement into new sheets is done in that case.

Pasting a Pin List from external source

This option is only available in symbol editor. Source of pins can be any application that copies data as comma, tab, or space separated text to clipboard, this includes various PDF viewers, spreadsheet, and text editors. For best results, format your data in a tabular manner with header row containing column names and cells containing pin attribute values as described in PIN section.

An example of correctly formatted pin table data:

Name Length Function Direction
IO_L1N_VREF_0 Middle None In
TCK Middle DotClk Io
GND Short None Sup
GND Short None Sup
gnd Long None Pwr
gnd Long None Pwr
Vcc Middle Dot Pwr
VCC Middle Dot Pwr
VCC Middle Dot Pwr

Copying pin lists directly from other sources

Copying directly from sources like PDF datasheets is also supported in either a single column or multicolumn data modes. Hint: to copy only a single column from PDF use system supported PDF viewer and hold Alt key while selecting the data. In single column mode it is assumed that every row shall contain a single word representing a pin name. In multicolumn mode, accessible by holding Ctrl key while starting a paste command, data is analyzed for the column that contains pin names. Success in these two modes highly depends on the formatting of input data, some PDF sheets apply unusual formatting styles. If you experience problems in this mode, paste data to text editor first to inspect data layout formatting and correct it if needed.

Dealing with non compliant pin data

PIN section describes general requirements about names of the pins. Default pin attribute values are used whenever values can't be inferred from input data. Following changes are applied to non compliant pin names.

Description Before After
Space characters are replaced by underscores "A A" "A_A"
Spaces surrounding forward slash are removed "A / B" "A/B"
Lowercase characters are promoted to uppercase "ABcde" "ABCDE"
Duplicate names are resolved using @ notation "GND" in symbol and "Gnd, gnd" in input data "GND@1, GND@2, GND@3"

Top

PATTERN

Function

 Make multiple copies of an object and arrange them in a linear or circular pattern.

Syntax

 PATTERN ..

 PATTERN LINEAR item-count x-spacing x-unit y-spacing y-unit object-location first-item-location

 PATTERN CIRCULAR item-count degree [ rotate ] object-location circle-center-location first-item-location

Mouse keys

Right rotates the selected object.

Shift+Right reverses the direction of rotation.

The PATTERN command can be started on the command line or with the PATTERN icon in the commands toolbar. A dialog opens where you decide about the number of copies and the X and Y spacing in the linear mode. Click OK to close the dialog, then click the object to be duplicated. The next click on the drawing area fixes the position of the first object to be placed. The further duplicates will be placed according to the given parameters.

If you choose the circular mode, the number of items, and the angle steps in the dialog, the first click on the drawing area selects the object to be duplicated, the second determines the center of the circle, and the third click fixes the position of the first object to be placed. Further copies are placed automatically according to the given parameters in the dialog.

The PATTERN command may be used in the Schematic, Layout, and Library Editor.

Options

Linear Pattern

ITEM-COUNT Number of copies in the pattern.
X-SPACING Value of the distance between two copies in the pattern in x direction.
X-UNIT INCH or MIL or MM or MIC. Unit of X-SPACING.
Y-SPACING Value of the distance between two copies in the pattern in y direction.
Y-UNIT INCH or MIL or MM or MIC. Unit of Y-SPACING.
OBJECT-LOCATION Location of the object to be copied.
CIRCLE-CENTER-LOCATION Location of the circle center of the circular pattern.
FIRST-ITEM-LOCATION Location of the first item in the pattern.

Circular Pattern

ITEM-COUNT Number of copies in the pattern. DEGREE Value of the angle (in degree) between two copies in the pattern. ROTATE Optional. By adding the "OPTIONAL" keyword, the items in the pattern will be rotated. OBJECT-LOCATION Location of the object to be copied. FIRST-ITEM-LOCATION Location of the first item in the pattern.

Example

PATTERN CIRCULAR 20 45.0 ROTATE (1.5 1.6) (2.0 2.0) (3.0 2.0)

This will generate a circular pattern consisting of 20 copies of the object from (1.5 1.6). The pattern center will be at (2.0 2.0), the first item of the pattern is at (3.0 2.0), the angle between two items is 45.0°, every item is rotated.

PATTERN LINEAR 5 1.5 INCH 200 MIL (1.5 1.5) (3.0 2.5)

This will generate a linear pattern consisting of 5 copies of the object at (1.5 1.5). The pattern will start at (3.0 2.5) with x spacing of 1.5 inch and y spacing of 200 mil.

Top

PIN

Function

 Defines connection points for symbols.

Syntax

 PIN 'name' options ..

Mouse keys

Right rotates the pin.

Shift+Right reverses the direction of rotating.

See also NAME, SHOW, CHANGE, PASTE, PINARRAY.

Options

There are six possible options: Direction

Function

Length

Orientation

Visible

Swaplevel

Direction

The logical direction of signal flow. It is essential for the Electrical Rule Check (ERC) and for the automatic wiring of the power supply pins. The following possibilities may be used:

NC not connected
In input
Out output (totem-pole)
IO in/output (bidirectional)
OC open collector or open drain
Hiz high impedance output (for example 3-state)
Pas passive (for resistors, capacitors etc.)
Pwr power input pin (Vcc, Gnd, Vss, Vdd, etc.)
Sup general supply pin (for example 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.

Function

The graphic representation of the pin:

None no special function
Dot inverter symbol
Clk clock symbol
DotClk inverted clock symbol

Default: None

Length

Length of the pin symbol:

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

Orientation

The orientation of the pin. When placing pins manually the right mouse button rotates the pin. The parameter "orientation" is mainly used in script files:

R0 connection point on the right
R90 connection point above
R180 connection point on the left
R270 connection point below

Default: R0

Visible

This parameter defines if pin and/or pad name are visible in the schematic:

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

Swaplevel

An integer number. Swaplevel = 0 indicates that a pin can't be swapped with another. The allocation of a number greater than 0 indicates that a pin may be swapped with any other in the same symbol with the same swaplevel number. For example: The inputs of a NAND gate could be allocated the same swaplevel number as they are all identical. Default: 0

Using the PIN Command

The PIN command is used to define connection points on a symbol for nets. Pins are drawn onto the Symbols layer while additional information appears on the Pins layer. Individual pins may be assigned various options on the command line. The options can be listed in any order or omitted. In this case the default options are valid. 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.

Automatic Naming

Pins may be automatically numbered in the following way. In order to place the pins D0...D7 on a symbol, the first pin is placed with the following command:

PIN 'D0' *

and the location for the other pins defined with a mouse click for each.

Predefine options with CHANGE

All options may be predefined with CHANGE commands. The options remain in use until edited by a new PIN or CHANGE command. The SHOW command may be used to show pin options such as Direction and Swaplevel.

Pins with the same Name

If it is required to define several pins in a component with the same name, the following procedure can be used. 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.

Pin Lettering

The position of pin and pad names on a symbol relative to the pin connection point can't be changed, nor can the text size. When defining new symbols please ensure their size is consistent with existing symbols.

Inverted pins

The name of an inverted pin ("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.

Top

PINARRAY

Function

 Create an array of pins.

Syntax

 PINARRAY [sides base start numpins drawrect includename includevalue deleteobjs]

See also PIN.

The PINARRAY command allows to create an array of pins in the Symbol editor. If the command is started from the icon in the PIN parameter toolbar, a dialog pops up where the options for sides, basename, start index, number of pins, and others are set before creating the array. If the command is started from the command line and arguments are provided, the same options are available as specified below.

Options

If the arguments are provided after the command, all need to be present:

SIDES This can be L|R|T|B, or any combination of these, which indicates onto which sides of a rectangle to draw the pins, where L=Left, R=Right, T=Top, and B=Bottom.
BASE This is the base name to use for the pin names. Pins are named such that the first pin is and subsequent pins are named with an increasing numerical suffix (i.e, ADDR1, ADDR2, .. ADDRn). The last pin placed has a name given by .
START This is the start index for pin naming. The first pin's name is .
NUMPINS The number of pins to place.
DRAWRECT ON or OFF. Determines whether a rectangle should be drawn in the layer Symbols as part of the operation.
INCLUDENAME ON or OFF. Determines whether a >NAME text object should be placed.
INCLUDEVALUE ON or OFF. Determines whether a >VALUE should be placed.
DELETEOBJS ON or OFF. Determines whether pins, labels, and wire objects should be deleted before placing the array.

Top

PINBREAKOUT

Function

 Creates nets with or without labels extending from all pins on the selected part.

Syntax

 PINBREAKOUT name type

The PINBREAKOUT command breaks out each part selected by extending nets from the part's pins, out a short distance from the pins, optionally named, and with labels.

The name parameter must match a part in schematic, and type is a number from 1 to 4 corresponding to the options below:

Note: The command with its various options is accessible on the right-click context menu when clicking a part in schematic.

Top

PINSWAP

Function

 Swap pins or pads.

Syntax

 PINSWAP ..

See also PIN.

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 footprint 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 can appear. It is recommended to run a DRC and correct possible errors.

Top

POLYGON

Function

 Draws polygon areas.

Syntax

 POLYGON [signal_name] [width] [curve | @radius] ..

Mouse keys

Center selects the layer.

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.

Ctrl+Left when placing a wire end point defines arc radius.

Left twice at the same point closes the polygon.

See also CHANGE, DELETE, RATSNEST, RIPUP, LINE, MITER, POLYGONIZE.

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 RestrictTop/Bottom/Vias 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 LINE command).

Note

You should avoid using very small values for the width of a polygon, because this can cause extremely large amounts of data when processing a drawing with the CAM Processor.

The polygon width should always be larger than the hardware resolution of the output device. For example, when using a Gerber photoplotter with a typical resolution of 1 mil, the polygon width should not be smaller than, say, 6 mil. Typically you should keep the polygon width in the same range as your other wires. 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 the signal layers.

To withdraw a mistake, always the last wire piece of the polygon can be removed with the ESCape key.

Outlines or Real Mode

Polygons belonging to a signal can be displayed in two different modes:

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 recalculate a polygon if it was shown in "real mode" before.

Other commands and Polygons

Polygons are selected at their edges (like wires).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.

Parameters

Width

Line width of the polygon edges. Also used for filling.

Layer

Polygons can be drawn into any layer. Polygons in signal layers belong to a signal and keep the distance defined in the design rules and net classes from other signals. Objects in the RestrictTop layer are subtracted from polygons in the Top layer (the same applies to RestrictBottom and the Bottom layer). This allows you, for instance, to generate "negative" text on a ground area.

Pour

Fill mode (Solid [default], Hatch or Cutout).

Rank

Defines how polygons are subtracted from each other. Polygons with a lower 'rank' appear "first" and thus get subtracted from polygons with a higher 'rank'.

Valid ranks are 1..6. Polygons with the same rank are checked against each other by the Design Rule Check. The rank parameter only has a meaning for polygons in signal layers (1..16) drawn in a board and will be ignored for any other polygons. The default is 1.

Thermals

Defines how pads and smds are connected (On = thermals are generated [default], Off = no thermals).

Spacing

Distance between fill lines when Pour = Hatch (default: 50 Mil).

Isolate

Distance between polygon areas and other signals or objects in the Dimension or according restrict layer (default: 0). If a particular polygon is given an Isolate value that exceeds that from the design rules and net classes, the larger value will be taken. See also Design Rules under Distance and Supply, respectively.

Note that if you give a polygon an Isolate value that exceeds that from the design rules and net classes, small gaps can result between the calculated polygon and objects belonging to the same signal as the polygon itself, which may lead to problems during manufacturing! It is therefore recommended to leave this parameter at 0 in most cases.

Orphans

As a polygon automatically keeps a certain distance to other signals it can happen that the polygon is separated into a number of smaller polygons. If such a polygon has no electrical connection to any other (non-polygon) object of its signal, the user might want it to disappear. With the parameter Orphans = Off [default] these isolated zones will disappear. With Orphans = On they will remain. If a signal consists only of polygons and has no other electrically connected objects, all polygon parts will remain, independent of the setting of the Orphans parameter. 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.

Thermal dimensions

The width of the conducting path in the thermal symbol is calculated as follows:

Outlines data

The special signal name OUTLINES gives a polygon certain properties that are used to generate outline data (for example for milling prototype boards). This name should not be used otherwise.

Hatched polygons and airwires

Depending on the value of the spacing parameter, pads, smds, vias and wires inside a hatched polygon that are connected to the same signal as the polygon may "fall through" the raster and thus have airwires generated to indicate their connection to the signal. 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.

Polygon cutouts

The special pour style "Cutout" makes a polygon be subtracted from all other signal polygons within the same layer, independent of their Rank. 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).

Top

PINTOBUS

Function

 Automatically connect part instance pins to a nearby bus that includes the pin name in the bus specification with labeled nets.

Syntax

 PINTOBUS name

The PINTOBUS command is used to extend nets from all pins on a part instance, out to a nearby bus, where the bus specification includes a member that matches the pin name on the part.

This command can be run from the command line, but is also available from the right-click context menu when clicking parts in schematic.

please note that the bus you wish to connect to has to be drawn either horizontally or vertically, and the pins must point into the direction of the bus.

As an example, consider a part with pins named VDD and GND at one side, and VIN and VOUT on the other side. If you were to draw a bus on one side with a spec that includes the names VDD and GND, and another bus on the other side that includes VIN and VOUT, then this command automatically creates nets with labels named VDD,GND,VIN, and VOUT extending from the respective pins to the corresponding busses.

Note: You have to select the part and all busses you want to connect to before using the command, or EAGLE will prompt you to do so. The recommended way to use this command is to incrementally select the busses and the part you wish to connect with Ctrl + left click, then run PINTOBUS from the context menu or command line.

Top

POLYGONIZE

Function

 Converts a closed set of wires into a polygon or vice versa.

Syntax

 POLYGONIZE

See also POLYGON.

The POLYGONIZE command is used to convert a closed set of wires into a polygon or vice versa. When converting wires into a polygon, execute POLYGONIZE and click one of the wires to be converted. When converting a polygon into wires, execute POLYGONIZE and click the outline of the polygon to be converted. Holding Alt while clicking will add the polygon as a new object, whereas not holding alt will replace the original object(s) with the new one(s).

An alternative way of invoking POLYGONIZE is by right clicking a wire or a polygon edge and choose "Convert To Polygon" or "Convert To Wires". After that you will get the option to either "Copy" or "Replace".

Top

PORT

Function

 Adds ports to modules.

Syntax

 PORT 'module_instance_name' 'net_name' options ..

 PORT 'module' 'net_name' options ..

 PORT 'module' 'net_name' options|DELETE

See also MODULE.

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.

If a simple bus name for net_name is used (see Names), this port 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.

Names

The port name have to be chosen according to the net name within that module, which should be exported. The port name can even be a simple bus name with a single range like 'PA[0..7]' (aliases are not allowed).

Options

Direction

The logical direction of signal flow. It is essential for the Electrical Rule Check (ERC) and for the automatic wiring of the power supply pins. The following possibilities may be used:

NC not connected
In input
Out output (totem-pole)
IO in/output (bidirectional)
OC open collector or open drain
Hiz high impedance output (for example 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.

DELETE

The option DELETE is used to delete an already existing port in module context.

Edit

The MOVE command can be used to edit the module symbol. A port of a module symbol can be selected with Ctrl+Left at it's connecting end for moving it along the module instance's border. The INFO command can be used to get the port properties by selecting it with Ctrl+Left.

The DELETE command can be used to delete a port by selecting it with Ctrl+Left.

If connected with a net, the selection can be ambiguous. Use Ctrl+Right in order to switch to the requested object (port in this case).

Top

PREFIX

Function

 Defines the prefix for a symbol or module name.

Syntax

 PREFIX prefix_string;

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.

Example

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.

Top

PRINT

Function

 Prints a drawing to the system printer.

Syntax

 PRINT [factor] [-limit] [options] [;]

See also CAM Processor, printing to the system printer.

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](ECD-CLI-S.html#set) DISPLAY_MODE NODRILL;

Note that polygons in boards are not automatically calculated when printing with the PRINT command! Only the outlines are drawn. To print polygons in their calculated shape, 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 with 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
ALIGN prints in a given alignment; the alignment setting 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 preceded with a '-', that option is turned off in case it is currently on (from a previous PRINT). A '-' by itself turns off all options.

Printing to a file

The FILE option can be used to print the output into a file. If this option is present, it must be immediately followed by the name of the output file. If the output file name has an extension of ".pdf" (not case-sensitive), 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" (not case-sensitive), 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.

Printing to a given paper size

The PAPER option defines the size of the paper to print on. It must be immediately followed by one of the paper size names listed in the Paper combo box of the PRINT dialog, like A4, Letter etc. If a custom paper size shall be set, it has to be given in the format

Width x Height Unit

(without blanks), as in

PRINT PAPER 200x300mm
PRINT PAPER 8.0x11.5inch

Width 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 not case-sensitive. If both the PRINTER and PAPER options 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.

Printing a range of sheets

The SHEETS option can be used to print a range of sheets from a schematic. The range is given as two numbers, delimited by a '-', as in 2-15. Without this option, only the currently edited sheet is printed. To print all sheets, the range ALL can be used (which is not case-sensitive, but must be written in full). A range can also consist of just a single number, as in 42, which will print exactly that sheet. If no schematic is loaded, this option has no meaning.

Printing with an alignment

For the ALIGN option, there are the settings T (top), C (center) and B (bottom) for vertical and R (right), C (center) and L (left) for horizontal alignment. For example, PRINT ALIGN TL; prints in alignment top left. If only one direction is specified, the other direction is assumed center (like in PRINT ALIGN B;, for printing with alignment bottom center). The order of settings is not relevant.

Printing sheets of modules

If the currently edited sheet is part of a module, the range of sheets applies to the module. With the option SHEETS ALL, all sheets of the main schematic and all sheets of all modules are printed. If the option HIERARCHY is given additionally, sheets of a module are printed for each use in a module instance with the according part and net names.

Examples

PRINT 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

Top