Re: gEDA-user: footprints needed

["Phil Taylor" <phil@xxxxxxxxxxxxxxxxxxxxxxxx>]

PCB's footprints are totally cartesian.  You can make newlib footprints with
your calculator's trig functions to find the x,y positions of the holes.  

This is a footprint best done in text.

It IS possible to make arcs with angles other than 0 or 90 in PCB.  You'll use
your text editor and specify the starting angle and the angle to be covered.

You may want to put arcs around the outsides of the holes as well.

For example here is a toroidal inductor with it's mounting pins on a 45 deg.
angle:

Element[0x00000000 "1000uH" "L?" "" 100000 100000 0 0 0 100 0x00000000]
(
	Pin[42430 -42430 10000 2000 10600 4900 "" "2" 0x00004001]
	Pin[-42430 42430 10000 2000 10600 4900 "" "1" 0x00004001]
	ElementArc [0 0 60000 60000 51 168 1000]
	ElementArc [0 0 60000 60000 231 168 1000]
	ElementArc [42430 -42430 6000 6000 135 180 1000]
	ElementArc [-42430 42430 6000 6000 315 180 1000]
	)

Phil Taylor





"Dominique Michel" <dominiquemichel@xxxxxxxxxxx> wrote:

> Hi,
> 
> I need to use footprints for vacuum tubes sockets as in 
> http://www.belton.co.kr/jack/vacuum-3.html
> For the noval socket, it is 9 VIAs on a circle of 21 mm diameter, 36° 
> between each VIA.
> I need other sockets too as in http://www.tube-shop.com/sockets.asp, so I 
> don't know if it is a way with pcb to write an arc that don't have 90° 
> aperture. Another way would be to use the old library file format.
> 
> Have somebody  any clue on how to do that, or an existing file to share?
> 
> Best,
> Dominique
> 
> _________________________________________________________________
> MSN Messenger : discutez en direct avec vos amis ! 
> http://www.msn.fr/msger/default.asp
> 
>