kicad-developers team mailing list archive

[Eeli Kaikkonen <eeli.kaikkonen@xxxxxxxxx>]

It still looks to me that the original problem wasn't understood, and I
wasn't able to make it clear. A Solder Mask Defined footprint means that
the solder mask opening is smaller than the underlying copper area. It may
also be differently shaped than the underlying copper pad. Also the paste
area may be differently shaped than the copper or solder mask. In these
cases it should be possible to define the mask and paste areas exactly,
without adding or removing anything. The logical way of doing it, if KiCad
had took it into consideration, would be to draw the pad shape and set the
clearances to 0, and the pad would always keep the exact dimensions. But
now, because 0 is a special case and means "add here some other value" the
pad dimensions - we are talking about non-copper pads - will change
unpredictably. This works for normal Non Solder Mask Defined pads with
copper, but not for pads which are mask only or paste only.

The only possible solution ATM is to give very small clearance values so
that the original size of a mask-only pad is for example 0.3x0.45mm and the
efficient value will be 0.300001x0.450001mm. If the clearances are left to
0 they can be anything, depending on the project's values, and the
footprint doesn't work anymore. Remember that modern Solder Mask Defined
footprints are mostly very small and tolerances are small. You can't add or
remove 0.05mm without it going wrong.

See for example http://www.ti.com/lit/ug/slra003d/slra003d.pdf

Eeli Kaikkonen

2018-04-28 10:28 GMT+03:00 jp charras <jp.charras@xxxxxxxxxx>:

> Some info about these masks:
>
> For custom shaped pads, building a solder mask shape with a negative
> margin can create issues
> (unpredictable shape for non convex polygons).
> So it is not allowed.
>
> Margin in solder mask layers is needed because there are always
> registration issues between the
> copper layers and the solder mask layer.
>
> Therefore, because the X and Y registration position error, you need a
> actual mask size bigger than
> the area defined by a pad, to be sure the actual solder mask does not
> cover the pad (the hole in
> mask always covers the pad area).
> X/Y max error depends on your board house, so this is the reason to have
> the registration tolerance
> defined for the whole board (unless you know your board house, you cannot
> reliably use a defined
> tolerance: it could be too small or too large)
>
> I am guessing there are also similar registration problems for the solder
> mask, but I don't know them.
>
> --
> Jean-Pierre CHARRAS
>
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp
>