On Sat, 9 Aug 2003, Terry Porter wrote:Yes, I generate land patterns for pcb at least every other week. Take a look at my document
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?
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: [EMAIL PROTECTED] # # 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)
)
