[gta02-core] The 1000 faces of 0402 (1005)

[Rene Harder]

Werner Almesberger wrote:
> Rene Harder wrote:
>   
>> I think the keepout area should meet our minimum trace clearance so we
>> do not get into any trouble during production.
>>     
>
>   
> Using the package width and t = 0.127 mm, we get:
>
> 			r	p	(1)	(3)	My value
> Panasonic 0402, width	0.5	0.5	0.75	0.63	0.85
> Vishay 0402, width	0.5	0.6	0.75	0.68	=
> Panasonic 0402, length	1.0	1.5	1.25	1.38	1.55
> Vishay 0402, length	1.0	1.3	1.25	1.28	=
> Panasonic 0603, width	0.8	0.8	1.05	0.93	1.15
> Vishay 0603, width	0.85	0.9	1.1	1.00	=
> Panasonic 0603, length	1.6	2.1	1.85	1.98	2.25
> Vishay 0603, length	1.55	2.0	1.8	1.90	=
>
> So this looks good, doesn't it ?
>   

I've not even considered all the points you mentioned above but you are
absolutely right and that's sounds good to me.

>> Does anyone know, how Kicad handles the solder stop mask, is it
>> generating the mask from the solder lands and what's their clearance?
>>     
>
> The clearance is set in Dimensions/Tracks and Vias/Mask clearance.
> The effective solder mask is the solder mark layer of the footprint,
> plus the clearance. If the footprint doesn't specify a solder mask,
> the land will have no opening in the solder mask !
>
> The usual setting is that all pads have the same shape and side in
> their solder mask layer as they have in their copper and solder
> paste layer.
>
>   

If the solder mask openings have the same size as the solder lands,
that's probably not a good idea because that means through tolerances in
the fabrication process you might end up with an overlapping stop mask.
This would cause stress to the solder joint which could lead to solder
cracking. So it's preferable to make the solder mask openings bigger
than the actual pad size. I think around 2-3mil to each edge of the
solder land should be fine.