footprinter.py — gEDA PCB Footprint Generator
version 0.1

footprinter.py gives you a set of classes for generating footprint files as used by the PCB program. By importing footprinter in a very small Python program, you have all the facilities of Python, when you need then, to create your part footprints.

Differences from version 0.0:

• The "clearance" parameter initializing the Pad and Pin classes has been renamed to "trace_clearance".
• The "mask" parameter initializing the Pad and Pin classes has been replaced by a "mask_clearance" parameter. The new parameter specifies the gap between the edge of the Pad or Pin and the solder mask.
• A "description" parameter initializing the Footprint class has been added to fill in the element's description field.

A simple source file looks like this:

#!/usr/bin/env python
'''Footprint -- Holes, outline for 4-lead cylindrical W02 bridge rectifier.
'''
from footprinter import inch, mil, mm, Footprint, Pad, Pin, ElementArc, ElementLine

fp = Footprint (
	[
	Pin (1, inch(-.2), inch(-.1), mil(100), mil(25), mil(2), mil(49), sflags='square'),	#+ positive
	Pin (2, inch(.2), inch(.1), mil(100), mil(25), mil(2), mil(49)),	#~ AC
	Pin (3, inch(.1), inch(-.2), mil(100), mil(25), mil(2), mil(49)),	#- negative
	Pin (4, inch(-.1), inch(.2), mil(100), mil(25), mil(2), mil(49)),	#~ AC
	],
	[
	ElementArc (0,0, inch(.27),inch(.27), 0,360, inch(.01))
	]
	, description="W02 bridge rectifier"
	)
	
fp.file_element ('W02.fp')

inch, mil, mm

give you functions to specify units of measure for sizes and coordinates.

Footprint

is a Python class that collects all the information describing a footprint. The arguments for Footprint are:

padpins

a Python list of all the Pad and Pin instances (see below) included in this footprint. Empty if omitted.

linearcs

a Python list of all the ElementArc and ElementLine instances (see below) included in this footprint. Empty if omitted.

sflags

the comma-separated flag symbols for the footprint file "Element" line. Blank if omitted.

description

A descriptive string for this footprint. Blank if omitted.

Pad

collects all the information describing a pad in the footprint. The parameters are

number

the part's pin number associated with this pad

padrect

a 4-item Python list or tuple containing the x- and y-coordinates of the diagonally opposite corners of this pad's copper rectangle: e.g. (x1,y1, x2,y2) for corner#1 and corner#2.

trace_clearance

the clearance value for the footprint file "Pad" line

mask_clearance

width of the gap between each edge of the copper pad and the solder mask. (In the older release, this parameter gave the entire width of the mask.)

name

the name value for the footprint file "Pad" line. Blank if omitted.

sflags

the comma-separated flag symbols for the footprint file "Pad" line. Blank if omitted.

Pin

collects all the information describing a pin in the footprint. The parameters are

number

the part's pin number associated with this pin

rx

the X-coordinate of the center of this pin

ry

the Y-coordinate of the center of this pin

thickness

the thickness value for the footprint file "Pin" line

trace_clearance

the clearance value for the footprint file "Pin" line

mask_clearance

width of the gap between the edge of the copper pin and the solder mask. (In the older release, this parameter gave the entire width of the mask.)

drill

the drill diameter value for the footprint file "Pin" line

name

the name value for the footprint file "Pin" line. Blank if omitted.

sflags

the comma-separated flag symbols for the footprint file "Pin" line. Blank if omitted.

ElementArc

collects all the information describing an arc in the footprint. The parameters are:

rx

the X-coordinate of the center of this arc

ry

the Y-coordinate of the center of this arc

width

the thickness value for the footprint file "ElementArc" line

height

the height value for the footprint file "ElementArc" line

start_angle

the start_angle value for the footprint file "ElementArc" line

delta_angle

the delta_angle value for the footprint file "ElementArc" line

thickness

the thickness value for the footprint file "ElementArc" line

ElementLine

collects all the information describing an arc in the footprint. The parameters are:

rx1

the X-coordinate of the start point of the line

ry1

the Y-coordinate of the start point of the line

rx2

the X-coordinate of the end point of the line

ry2

the Y-coordinate of the end point of the line

thickness

the thickness of the line

All coordinates are relative to the notional "center" of the part that you select.

Since the footprint source file is actually Python, you can make your specifications clearer by using named arguments, e.g.

ElementArc (rx=0,ry=0, width=inch(.27),height=inch(.27), start_angle=0,delta_angle=360, thickness=inch(.01))

You can also define functions and use if-statements and loops to avoid cumbersome boilerplate code in your definitions.

With all the information for the footprint complete, use the file_element method to write the .fp footprint file for PCB. The argument for the file_element method is the path to the file to be written.