gEDA-user: Re: How to convert a hole

[John Luciani <jluciani@xxxxxxxxx>]

That symbol does not have a hole. The #10 and 1/4" symbols do not have
holes only
a silkscreen cross to be used as a manual drill guide. Here is the
note from the hardware section of my webpage ---

   The symbols for the #10 and 1/4" screws have a copper cross in the
center. The copper     cross is meant to be used as a manual drill
guide. The larger drill sizes do not seem to be common at the low-cost
board vendors.

  I will clarify the wording.

To add a hole you would need to add a pin to the symbol. To add a plated hole
with a 152mil diameter and an annular ring of 23mils replace the two pad lines
with the following line:

   Pin(0 0 175 152 "" "1" 0x01)

(* jcl *)

P.S. You should also remove the last two ElementLine statements and
the ElementArc
statement. They are not needed when you have a hole.

On 2/8/06, toaster2@xxxxxxxxxxxx <toaster2@xxxxxxxxxxxx> wrote:
> John,
> I have a stupid question. I used a hex standoff footprint you created from:
> http://www.luciani.org/geda/pcb/footprints/hard-hex-standoff-10.
> It defines a .150" diameter NON-PLATED hole, which I must change to a PLATED
> hole of 0.152" diameter.
>
> I don't see anywhere the number 150 and I don't even understand how a hole was
> defined in the first place. If you have a minute please be kind to enlighten
> me and show me "how to fish".
> Thanks,
> Frank
>
> Element(0x0 "hard-hex-standoff-10" "" "" -169 -210 0 100 0x0)
> (
>    Pad(0 45 0 -45 30 "" "1" 0x0100)
>    Pad(-45 0 45 0 30 "" "2" 0x0100)
>    ElementLine(-144 0 -72 125 10)
>    ElementLine(-72 125 72 125 10)
>    ElementLine(72 125 144 0 10)
>    ElementLine(144 0 72 -125 10)
>    ElementLine(72 -125 -72 -125 10)
>    ElementLine(-72 -125 -144 0 10)
>    ElementLine(-20 0 20 0 10)
>    ElementLine(0 -20 0 20 10)
>    ElementArc(0 0 100 100 0 360 10)
>    Mark(0 0)
> )
>
>


--
http://www.luciani.org