PCB: Quick Reference
- Additional information
- Default Key Mapping
Footprint Quick Reference
- General syntax
- PCB Units
- Elements
- Pads
- Pins
- Examples
PCB Command Line Action Reference (abridged)
PCB Physical Layer Reference

Translations of this page are also available in the following languages: Français, Русский.

PCB: Quick Reference

Additional information

More information on PCB you can find in the PCB Command reference (refcard.pdf) containing description of all PCB shortcuts and in the PCB Manual (pcb.pdf or pcb.html) residing in the doc/ directory of your PCB installation (its path may vary on various systems).

Default Key Mapping

All Keystrokes

Key	Mnemonic	Description
`Esc`	select	enter select mode (same as `Space`, or `F11`)
`Esc`	end of action	terminate the current action, e.g. stop drawing tracks
`Insert`	insert point	enter insert point mode. Click and drag on track to insert a point
`Return`	click	same as a click on the left mouse button
`Space`	select	enter select mode (same as `Esc`, or `F11`)
`Tab`	flip up/down	view: vertical flip
`Shift`+`Tab`	flip left/right	view: horizontal flip
`Ctrl`+`Shift`+`Tab`	far side	view: exchange the roles of front side and far side
`Del`	delete	delete object under the mouse cursor
`Ctrl`+`Shift` L-Mouse	delete	delete object under the mouse cursor (fast)
`Shift`+`Del`	del-sel	delete objects in selection
`Backspace`	del-sel	delete objects in selection
`Shift`+`Backspace`	del-copper	deletes connected copper under the cursor. Rats are considered a connection.
`\|`	thin-draw	toggles thin draw mode
`A`	set same	read the parameters to use for new objects from the object below the cursor.
`Alt`+`A`	select-all	select all objects on active layers. Deactivated layers are ignored.
`Shift`+`Alt`+`A`	unselect	clear selection
`B`	to other side	flip object to the other side of the board
`C`	center	view: center display at cursor position
`Ctrl`+`C`	copy to buffer	copy selection to buffer and unselect
`D`	display name	display pin or pad name
`Shift`+`D`	pinout dialog	open pinout window for element under mouse cursor
`E`	eliminate rats	delete all rats
`Shift`+`E`	eliminate some rats	delete selected rats
`F`	find	highlight connections to object under mouse cursor. This includes rats and objects on invisible layers
`Ctrl`+`F`	add to found	add connections to object under mouse cursor to the set of found objects
`Shift`+`F`	un-find	un-highlight found connections
`G`	incr grid mil	increment grid by configured imperial increment
`Shift`+`G`	decr grid mil	decrement grid by configured imperial increment
`Ctrl`+`G`	incr grid mm	increment grid by configured metric increment
`Ctrl`+`Shift`+`G`	decr grid mm	decrement grid by configured metric increment
`H`	hide	toggle the visibility of the refdes or value attached to the component under the cursor
`Shift`+`H`	hide sel	toggle the visibility of the refdes or value attached to selected components
`Ctrl`+`H`	holeplate	toggle plating of a via. Used to produce non metalized mounting holes
`J`	lineclear	toggle the polygon clear flag of the line under the cursor
`Shift`+`J`	lineclear sel	toggle the polygon clear flag of selected lines
`K`	klear	increment clearance (soldermask to copper edge)
`Shift`+`K`	klear (-)	decrement clearance (soldermask to copper edge (NOTE: can go negative!))
`Ctrl`+`K`	klear sel	increment clearance of selected objects (soldermask to copper edge)
`Shift`+`Ctrl`+`K`	klear sel (-)	decrement clearance of selected objects (soldermask to copper edge)
`L`	increase line	increment width of the line tool, adds to the settings of the current line style
`Shift`+`L`	decrease line	reduce the current linewidth
`M`	move to layer	move the object under the cursor to the current layer
`Shift`+`M`	move selection to layer	move selected objects to the current working layer (see pcb tip)
`Ctrl`+`M`	move origin	set the origin to the current position of the mouse pointer
`N`	name	show object refdes / pin number at mouse pointer
`Shift`+`N`	next	Select the shortest unselected rat on the board
`O`	optimize rats	optimize and redraw all rats
`Shift`+`O`	optimize some rats	optimize and redraw selected nets only
`Ctrl`+`O`	octagon	toggle the octagon flag of the object under the cursor
`Shift`+`P`	polygon close	connect the first point of a polygon with the last
`Q`	square toggle	toggle square/round corners on pads
`Shift`+`R`	redo	redo what was undone with undo
`Ctrl`+`R`	report	show object report
`S`	size	increment size of the object under the cursor
`Shift`+`S`	size (-)	decrement size of the object under the cursor
`Alt`+`S`	sizehole	increase the hole of the object under the cursor
`Alt`+`Shift`+`S`	sizehole (-)	decrease the hole of the object under the cursor
`Ctrl`+`S`	sizehole	increase the hole of the object under the cursor
`Ctrl`+`Shift`+`S`	sizehole (-)	decrease the hole size
`T`	text tool size	increase the size of new text by 10 mil
`Shift`+`T`	text tool size (-)	decrease the size of new text by 10 mil
`V`	view extents	global view of working area
`Shift`+`V`	via tool dia	increase the diameter of new vias by 5 mil
`Ctrl`+`V`	paste buffer	paste from buffer
`Ctrl`+`Shift`+`V`	via tool dia (-)	decrease the diameter of new vias by 5 mil
`Alt`+`V`	via tool drill	increase the drill diameter of new vias by 5 mil
`Shift`+`Alt`+`V`	via tool drill (-)	decrease the drill diameter of new vias by 5 mil
`Ctrl`+`X`	cut to buffer	cut selection to buffer
`Z`	zoom	view: zoom in
`Shift`+`Z`	un-zoom	view: zoom out
`F1`	via	enter via tool
`F2`	line	enter line tool
`F3`	arc	enter arc tool
`F4`	text	enter text tool
`F5`	rectangle	enter rectangle tool
`F6`	polygon	enter polygon tool
`F7`	buffer	enter buffer mode
`F8`	delete	enter remove mode
`F9`	rotate	enter rotate mode
`F10`	file menu	file menu
`F11`	select	enter select mode (same as `Space`, or `Esc`)
`F12`	lock	enter lock mode

Viewport Keystrokes

Key	Mnemonic	Description
`V`	view extents	global view of working area
`C`	center	centers view on cursor
`Z`	zoom	zoom in
`Shift`+`Z`	un-zoom	zoom out
`\|`	thin-draw	toggles thin draw mode
`Tab`	flip up/down	vertical flip
`Shift`+`Tab`	flip left/right	horizontal flip
`Ctrl`+`Shift`+`Tab`	far side	exchange the roles of front and far side

Layers

Key	Mnemonic	Description
`1` to `9`	-	select layers 1 to 9
`0`	-	select layer 10^*
`Alt`+`1` to `Alt`+`9`	-	select layers 11 to 19^*
`Alt`+`0`	-	select layer 20^*
`Ctrl`+`1` to `Ctrl`+`9`	-	toggle visibility of layers 1 to 9^*
`Ctrl`+`0`	-	toggle visibility of layer 10^*
`Ctrl`+`Alt`+`1` to `Ctrl`+`Alt`+`9`	-	toggle visibility of 11 to 19^*
`Ctrl`+`Alt`+`0`	-	toggle visibility of 20^*

^* _{These accels are available in PCB, GTK GUI in versions after August 2011}

Footprint Quick Reference

The Master document for footprint creation is the PCB Manual. There is also Stuart Brorson’s Footprint Creation for the Open-Source Layout Program PCB.

General syntax

A pcb footprint file may contain any of the following commands:

Element [element_flags, description, pcb_name, value, mark_x, mark_y, text_x, text_y, text_direction, text_scale, text_flags]
Pad [x1 y1 x2 y2 thickness clearance mask name pad_number flags]
Pin [x y thickness clearance mask drillholedia name number flags]
ElementArc [x y r1 r2 startangle sweepangle thickness]
ElementLine [x1 y1 x2 y2 thickness] –> thickness != 1000 = 10 mils almost for all footprints
Comment lines start with the ‘#’-sign

PCB Units

PCB handles metric and imperial units in the following way:

The base Imperial unit is the “centimil”, or 1/100 of a thousandth, or 1/100,000 inch, or 0.00001 inch.
Allowable imperial value range: “0.04” (0.0000004 inches) to approx. “78740000” (about 78-3/4“)
The base Metric unit is 1nm (one nanometer). PCB parses in metric if the number has a “mm” behind it.
Allowable metric value range: “0.000001mm” to “2000mm”
NOTES:
- use “mm” after number to specify metric
- imperial and metric may be mixed within a footprint (!)

Elements

Element [element_flags, description, pcb_name, value, mark_x, mark_y, text_x, text_y, text_direction, text_scale, text_flags]

	Allowed value (unit = 1e-5 inches)	Allowed Value (mm)	explanation	comment
element_flags	unsigned hex value
description	string		text description of footprint	user-defined
pcb_name	string		generic refdes (R?, U? etc.)	user-defined
value	string		component value (layout specific)	user-defined (blank)
mark_x	“1” to ~ “78740000”	“0.000001mm” to “2000mm”	(x,y) loc. of center mark
mark_y	“1” to ~ “78740000”	“0.000001mm” to “2000mm”
text_x	“1” to ~ “78740000”	“0.000001mm” to “2000mm”	(x,y) loc. of REFDES
text_y	“1” to ~ “78740000”	“0.000001mm” to “2000mm”
text_direction	decimal integer		0=horiz; 1=ccw90; 2=180; 3=cw90
text_scale	decimal integer			usu. set to 100
text_flags	unsigned hex

Pads

Pad[x1 y1 x2 y2 thickness clearance mask name pad_number flags]

Item	Allowed Value	Explanation	Comment
x1	1/100th mil	x (1st point)
y1	1/100th mil	y (1st point)
x2	1/100th mil	x (2nd point)
y2	1/100th mils	y (2nd point)
thickness	1/100 mils	width of metal surrounding line segment	see Brorson .pdf
clearance	1/100 mils	distance to any other copper on any layer	actually 1/2 of this number is used!
mask	1/100th mils	width of mask relief	actual width of the mask centered on pad copper
name	string	name of pad (arb. string)	e.g. "pad_1" or "positive" or any other string
pad_number	string	pad #	used for nets. it MUST be consistent with the definitions on the netlist.
flags	hex or string		examples:

Pins

Pin[x y thickness clearance mask drillholedia name number flags]

Item	Allowed Value	Explanation	Comment
x	1/100th mils	pin x coord.
y	1/100th mils	pin y coord.
thickness	1/100th mils	copper diameter
clearance	1/100th mils	2*(cu to cu clearance)	if you want a 10 mil clearance, put 2000 (20 mils) here
mask	1/100th mils	diameter of mask aperture	actual dia. of hole in mask
drillholedia	1/100th mils	dia. of hole
name	string	arb. pin name
number	decimal integer	pin number used by nets/rats
flags	hex	xxx

Examples

Pad[-24606 14760 -19538 14760 1181 2000 3181 "" "16" "square"]
Pad[-14760 19538 -14760 24606 1181 2000 3181 "" "17" "square,edge2"]
Pad[-240.00mil 0.0000 -80.00mil 0.0000 40.00mil 20.00mil 46.00mil "2" "2" "onsolder,square"]
Pad[80.00mil 0.0000 240.00mil 0.0000 40.00mil 20.00mil 46.00mil "1" "1" "onsolder,square,edge2"]
Pin[0 0 12000 2000 12500 6400 "" "1" 0×00000001]
Pin[0 0 11500 11800 35000 12500 "" "1" 0x08] ←- unplated / nonplated hole
ElementArc [0 0 6800 6800 0 360 1000]
ElementLine [-26696 -26696 26696 -26696 1000]
# notes within PCB Footprints go after the pound sign

PCB Command Line Action Reference (abridged)

:FreeRotateBuffer(degrees)		Rotate buffer arbitrarily
:MoveObject(x,y,unit)		Move Absolute (x,y,mil) or Relative(+x,-y,mil)
:ChangeClearSize(Selected,<amount>,<unit>)		Clearance Size
:ChangeSize(SelectedPins, SIZE)		Pin Size
:ChangeSize(SelectedLines,+N,mils)		Line Size
:MinClearGap(Selected,<amount>,<unit>)		Clearance Gap

units can be specified as mm or mil.
Action Reference from the PCB Manual

PCB Physical Layer Reference

outline layer reference
physical layer how-to (outline, direct (x,y) footprint placement, part insertion)

Table of Contents