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 |
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 |
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.
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
#
’-sign
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 |
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 |
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 |
Pad[-24606 14760 -19538 14760 1181 2000 3181 “” “16” “square”]
Pad[-14760 19538 -14760 24606 1181 2000 3181 “” “17” “square,edge2”]
Pin[0 0 12000 2000 12500 6400 “” “1” 0×00000001]
ElementArc [0 0 6800 6800 0 360 1000]
ElementLine [-26696 -26696 26696 -26696 1000]
# notes within PCB Footprints go after the pound sign