Re: gEDA-user: PCB PKG CONNECTOR

[Stephen Meier <smeier@AlchemyResearch.com>]

Mikey Sklar wrote:

> On Sat, 9 Aug 2003, Terry Porter wrote:
>  
> > Using the graphical footprint design technique in the 1.99 series, just
> > use a make your own part and save it to your local pcb parts directory. I
> > havent used M4 to make a part since I started using the 1.99 series. 
> >    
> This works fine within PCB.
>
> Btw, the exact terminal block I needed did come with PCB.
>
> /usr/local/pcb_lib/connectors/3terminal_screw_block
>
> Its still not clear to me how to make a new FOOTPRINT on per project
> basis for gschem2pcb automation. I realize I could mess with the system
> wide pcb files under:
>
> /usr/X11R6/lib/X11/pcb/m4
>
> Creating a custom .list, .m4, and .inc. Followed by modifications to
> common.m4 to include the fresh .inc file. Seems like enugh work, that
> I'm taking the wrong approach.
>
> Is anyone able to easily able to generate fresh footprints for usage
> within gschem and PCB without this sort of system wide hackery?
>
>
>  
Yes, I generate land patterns for pcb at least every other week. Take a 
look at my document

www.meierrippin.com/pcb_landpattern_design.pdf

I created a directory within /usr/local/share/pcb/newlib

giving me /usr/local/share/pcb/newlib/MeierRippin

I put my good landpatterns in this new directory where I can easily get 
at them. Enclosed is my pattern for a R0603 surface mount resistor.

#-----------------------------------------------------------------------------------
#  0603 surface mount resistor landpattern
#
#  Author:  Stephen Meier
#
#  email: smeier@meierrippin.com
#
#  Version: 0.01 2/21/2003   Original
#
#  Copyright (c) 2003 Meier Rippin L.L.C.
#
# This land pattern is distributed in the hope that it will be useful,
# but WITHOUT ANY WARRANTY; without even the implied warranty of
# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.
#
#-----------------------------------------------------------------------------------

# Element( Flags "Description" "LayoutName" "Value" TextX TextY direction scale TextFlags)

#   Element Flags 

#     bit 4:  the element name is hidden
#     bit 6:  element has been selected
#     bit 7:  element is located on the solder side

#   TextFlags

# PAD  x1, y1, x2, y2, thickness, clearance, mask, name , pad number, flags
# Pad (StartX StartY EndX EndY XWidth YWidth ShadowMaskSize "Name" "Pin Number" Flags)

#   Pad Flags

#     bit 2:  set if pad was found during a connection search
#     bit 3:  set if pad has courners
#     bit 5:  display the pads name - this dosn't work
#     bit 6:  pad has been selected
#     bit 7:  pad is located on the solder side

#-----------------------------------------------------------------------------------

Element(0x00 "Surface Mount Chip Resistor 0603" "R1" "" 0 0 -31 -82 2 100 0x00)
(
	Pad(-2 0  2 0 39 30 50 "pad 1" "1" 0x00000100)
	Pad(65 0 69 0 39 30 50 "pad 2" "2" 0x00000100)
	ElementLine(-21 -35  87 -35 5)
	ElementLine( 87 -35  87  35 5)
	ElementLine( 87  35 -21  35 5)
	ElementLine(-21  35 -21 -35 5)
)