Re: gEDA-user: Footprint with asymmetric solder mask

[SZABO Tamas <sza2king@xxxxxxxxxxx>]

Thanks,
 
>> I would like to create a footprint where the pad is not in the center, and it is not symmetric for all sides.


> Unfortunately not. PCB derives the solder mask from the pad and mask
> clearance. The file format needs to be extended to allow for the type
> of mask you would like.

> I think you might be misinterpreting the diagram though. They are
> indicating that there should be a > 18mm^2 copper plane around the pad
> which must have solder resist (mask) on it.

I may tired to describe my problem short shortly. So I think I understand it:-)

> So set the relevant pads'
> mask clearance to 0, and place a polygon down around the pad. Remove
> the clear lines/pads flag by putting your cursor over the polygon and
> pressing "s" in PCB. Just note that no lines or pads will be cleared
> by that polygon. What I usually do is make a small polygon/rectangle
> that fits just around the pad and set that to "solid", and then use a
> normal polygon around that.

Can I use polygon in footprints?

I need to place ~600 pieces of this part (actually LEDs) to the board.

Well, I prefer hand editing the .fp file :-)

My solution:

Element["" "DDW-WJG-X6X7-R-CS0284" "D0" "" 0 0 0 0 0 100 ""]
(
        Pad[-1.50mm -0.55mm -1.50mm  0.55mm 1.50mm 1.00mm 1.50mm "CATHODE" "1" "square"]
        Pad[-2.75mm -1.30mm -2.75mm  1.30mm 1.00mm 1.00mm 0.00mm "CATHODE" "1" "square,nopaste"]
        Pad[-1.00mm -1.55mm -2.00mm -1.55mm 0.50mm 1.00mm 0.00mm "CATHODE" "1" "square,nopaste"]
        Pad[-1.00mm  1.55mm -2.00mm  1.55mm 0.50mm 1.00mm 0.00mm "CATHODE" "1" "square,nopaste"]

        Pad[ 1.50mm -0.55mm  1.50mm  0.55mm 1.50mm 1.00mm 1.50mm "ANODE" "2" "square"]
        Pad[ 2.75mm -1.30mm  2.75mm  1.30mm 1.00mm 1.00mm 0.00mm "ANODE" "2" "square,nopaste"]
        Pad[ 1.00mm -1.55mm  2.00mm -1.55mm 0.50mm 1.00mm 0.00mm "ANODE" "2" "square,nopaste"]
        Pad[ 1.00mm  1.55mm  2.00mm  1.55mm 0.50mm 1.00mm 0.00mm "ANODE" "2" "square,nopaste"]
        ElementLine[-3.5mm -1.8mm -3.5mm 1.8mm 1000]
)

I don't know whether is it an acceptable solution or not...

> HTH,
> Duncan

Thanks again,

/sza2


<a href="http://ad.adverticum.net/b/cl,1,73468,1601554,1592431/click.prm"; target="_blank">________________________________________________________<br>25-70% kedvezmény április 14-én éjfélig több mint 400 féle szépirodalmi, ismeretterjesztéső és tudományos könyvre. Tekintse meg választékunkat!<br></a>


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user