gEDA-user: PCB SMD footprint creation guidelines

[Karel Kulhavy <clock@xxxxxxxxxxxxx>]

Because creating a PCB footprint in gEDA is a rocket science and I made
always a million mistakes, I wrote myself guidelines. Please put it into
the gEDA user manual as example procedure so that inexperienced users
can draw a correct SMD footprint in 10 minutes and not an incorrect one
in 1 hour.

<li>Set grid to unit according to source drawing
<li>Draw the pads. User CTRL-M to measure on component layer
<li>Draw the silkscreen with 0.2mm line thickness on silk layer. The outline
of the component is the outer edge of the silkscreen (not the center of the
line nor the inner edge).
<li>Draw an alignment cross in the future component reference point
using two rectangles placed on "unused" or "unused1" layer
<li>Check all dimensions according to drawing using CTRL-M
<li>Go over each pad, press 'n' and enter number of the pad.
<li>Select everything
<li>Copy selection to buffer
<li>Click on the alignment cross
<li>Convert buffer to element
<li>Set the grid to maximum
<li>Place the element somewhere apart from the original drawing
<li>Press Q on pads which shall be square
<li>Go over every pad, press 'n' and enter the number again.
<li>Now you need to change soldermask for all pads. Always select all pads with
the same thickness (measure using CTRL-M). If you are working in milimeters,
issue then "changeclearsize(selectedobjects, thickness/2+0.1mm)". If in mils,
"changeclearsize(selectedobjects, thickness/2+4mil)".
<li>Unselect all
<li>Turn off soldermask
<li>Turn off silk
<li>Select component layer
<li>Draw a big rectangle over the footprint
<li>Select all pads
<li>"changeclearsize(selectedobjects, 0.35, mm)"
<li>Remove the big rectangle
<li>Turn on silk
<li>Press 'n' over the silk and enter for resistor R000, capacitor C000,
coil L000, transistor Q000, soldering point T000, diode D000 etc.
<li>Place the label suitably near the footprint
<li>Press 'd' over the footprint, check the numbers, press 'd' again
<li>Select the whole footprint
<li>Copy selection to buffer
<li>Click exactly over the middle of the diamond
<li>Save buffer elements to file, enter the filename
<li>File, Quit Program, OK to lose data? OK.
<li>pcb
<li>Load element data to buffer
<li>Enter the name of the file
<li>Click somewhere and check the footprint looks as expected

CL<