Table of Contents

PCB: Quick Reference

Key Mapping

PCB Keystrokes

KEY MNEMONIC DESCRIPTION
esc panner enter panning mode
insert insert point enter insert point mode. Click and drag on track to insert a point
space select enter select mode
tab flip view view: flip board
shift-del del-cu deletes connected copper (rats are considered a connection)
\ thin-draw toggles thin draw mode
shift-alt-a unselect clear selection
b to other side flip object to the other side of the board
shift-b flip view view: flip 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
shift-f un-find un-highlight found connections
g increase grid increment grid by configured grid increment
shift-g decrease grid decrement grid by configured grid increment
h hide toggle the visiblity of the refdes or value attached to the current component
ctrl-h holeplate toggle plating of a via. Used to produce non metalized mounting holes
k klearance increment clearance (soldermask to copper edge)
shift-k klear (-) decrement clearance (soldermask to copper edge (NOTE: can go negative!))
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
shift-p polygon close connect the first point of a polygon with the last
q square toggle toggle square/round corners on pads
ctrl-r report show object report
s size increment size
shift-s size (-) decrement size
alt-s sizehole increase the hole size
alt-shift-s sizehole (-) decrease the hole size
ctrl-s sizehole increase the hole size
ctrl-shift-s sizehole (-) decrease the hole size
v view extents global view of working area
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])
F12 lock enter lock mode

Viewport Keystrokes

KEY MNEMONIC DESCRIPTION
esc panner
v view extents global view of working area
c center centers view on cursor
z zoom zoom in
shift-z un-zoom
\ thin-draw on/off toggles thin draw mode
tab flip view flip board
shift-b flip view flip board

Footprint 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:

Elements

Element [element_flags, description, pcb-name, value, mark_x, mark_y, text_x, text_y, text_direction, text_scale, text_flags]

item allowed value explanation comment
element_flags unsigned hex value
description string text description of footprint written by footprint author
pcb name string refdes used on this particular pcb xxx
value string value of component on this particular pcb layout xxx
mark_x 1/100th mils
mark_y 1/100th mils
text_x 1/100th mils
text_y 1/100th mils
text direction decimal integer 0=horiz; 1=ccw90; 2=180; 3=cw90
text_scale decimal integer usu. set 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 mils x(1st point)
y1 1/100th mils y(1st point)
x2 1/100th mils 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 value xxx

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