Re: gEDA-user: How to make PCB 1 mm connector?

["harry eaton" <bumpelo@comcast.net>]

That datasheet is a little hard to understand, but I think this element file
is pretty much what you want. Sorry, I was very sloppy on the silkscreen
outline, but you get the idea. Note that there are two pads for mounting (I
think that's what they're for) that I named "MOUNT_A" and "MOUNT_B". I was
also didn't check the actual pin numbering, I just went with what I thought
was probably right.

This was done by drawing 10 lines for the pins, two for the mounting pads,
then the silkscreen. After converting to an element I made all of the pads
square (q key over the element body), then returned pad 1 to rounded for
identification.

Note that it is possible (and sometimes desireable) to make a composite pad
from multiple lines. In that case, just be sure to give all segments the
same pin number.

Element[0x00000000 "" "J1" "" 55002 70041 -9000 -7000 0 100 0x00000000]
(
 Pad[116 -7049 116 825 2400 2000 4400 "" "1" 0x00004000]
 Pad[4053 -7049 4053 825 2400 2000 4400 "" "2" 0x00004100]
 Pad[7990 -7049 7990 825 2400 2000 4400 "" "3" 0x00004100]
 Pad[11927 -7049 11927 825 2400 2000 4400 "" "4" 0x00004100]
 Pad[15864 -7049 15864 825 2400 2000 4400 "" "5" 0x00004100]
 Pad[19801 -7049 19801 825 2400 2000 4400 "" "6" 0x00004100]
 Pad[23738 -7049 23738 825 2400 2000 4400 "" "7" 0x00004100]
 Pad[27675 -7049 27675 825 2400 2000 4400 "" "8" 0x00004100]
 Pad[31612 -7049 31612 825 2400 2000 4400 "" "9" 0x00004100]
 Pad[35549 -7049 35549 825 2400 2000 4400 "" "10" 0x00004100]
 Pad[43700 -19550 46750 -19550 6700 2000 8700 "" "MOUNT_A" 0x00004100]
 Pad[-11200 -19500 -8050 -19500 6700 2000 8700 "" "MOUNT_B" 0x00000100]
 ElementLine [44000 -32000 -8000 -32000 1000]
 ElementLine [-3000 -10000 39000 -10000 1000]
 ElementLine [39000 -10000 39000 -25000 1000]
 ElementLine [39000 -25000 45000 -25000 1000]
 ElementLine [-3000 -25000 -3000 -10000 1000]
 ElementLine [-9000 -25000 -3000 -25000 1000]
 ElementArc [45000 -30000 5000 5000 90 90 1000]
 ElementArc [46000 -30000 4000 4000 180 90 1000]
 ElementArc [46000 -32000 2000 2000 270 90 1000]
 ElementArc [-9000 -30000 5000 5000 0 90 1000]
 ElementArc [-10000 -30000 4000 4000 270 90 1000]
 ElementArc [-10000 -32000 2000 2000 180 90 1000]
 )

----- Original Message -----
From: "Bob Paddock" <bpaddock@csonline.net>
To: <geda-user@seul.org>
Sent: Sunday, April 11, 2004 9:36 AM
Subject: gEDA-user: How to make PCB 1 mm connector?


>
> I've been trying to make a ten pin version of this 1 mm pitch connector
for
> PCB:
>
> http://www.jst-mfg.com/ProductGuideE/EFPZ.html
>
> http://www.jst-mfg.com/pdfE/eFPZ.pdf
>
> I've tried drawing it then converting it to a element, but the resulting
> element says it has > 200+ pins.  A pin for each line segment that
> made up the ten filed 1mm pads.
>
> Since you can't use rectangles for pad elements how do you make
> a filed rectangular pad out of line segments, that is only one pin,
> with 1mm spacing?
>
>
>
>