Re: gEDA-user: Thermal pads overlapping regular SMD pads and solder mask

[DJ Delorie <dj@xxxxxxxxxxx>]

> contact areas, presumably important to assist accurate placement of
> the LED.

Turns out resist is a better black-body emitter than shiny metals.

> It looks like I can in fact set different solder mask clearances for
> overlapping pads, but I have not been able to make a pad entirely
> covered with solder mask.  Is this possible?  I found that
> doing changeclearsize to 1 mil gave almost complete solder mask
> coverage, but some copper was exposed.

You should be able to set the mask to exactly zero, although it might
be easier to edit the .fp file than do it in PCB itself.  You'll also
need this bug fixed:

https://sourceforge.net/tracker/?func=detail&aid=3100510&group_id=73743&atid=538813

> Does anyone have any recommendations or tips for me on creating a pcb
> footprint like the one on page 10 of the data sheet?

Three pads per terminal.  One big one for the resist-covered parts,
two overlapping small ones to make the T shape.  Something like this:

Element["" "" "" "" 181102 181102 0 0 0 100 ""]
(
	Pad[-3543 4724 3543 4724 3937 1200 4537 "" "1" "square"]
	Pad[0 7481 0 7874 2362 1200 2962 "" "1" "square,edge2"]
	Pad[-11811 10630 11811 10630 15748 1200 0 "" "1" "square"]
	Pad[-3544 -4725 3542 -4725 3937 1200 4537 "" "2" "square"]
	Pad[0 -7874 0 -7481 2362 1200 2962 "" "2" "square"]
	Pad[-11811 -10630 11811 -10630 15748 1200 0 "" "2" "square"]
	ElementLine [-7874 -7874 7874 -7874 600]
	ElementLine [7874 -7874 7874 7874 600]
	ElementLine [7874 7874 -7874 7874 600]
	ElementLine [-7874 7874 -7874 -7874 600]
	ElementLine [5512 -7874 7874 -5512 600]

	)


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