kicad-developers team mailing list archive

[Eeli Kaikkonen <eeli.kaikkonen@xxxxxxxxx>]

Do I see some kind of gap in communication here? I know what Rene is
talking about because I have designed solder mask defined pads. Wayne talks
about "tolerances". But this is not about tolerances.  It's about designing
a mask-only (or paste-only) pad with certain dimensions and then those
dimensions changing according to some global value which is not fitting for
that pad. For example 0.3x0.3mm mask area becomes 0.4x0.4mm while the
purpose was to always have 0.3x0.3mm. It's OK with copper pads which have
solder mask and paste defined, but not for mask-only or paste-only. The
problem is that mask-only pad is handled as if it was a normal copper pad:
the mask area is changed because it has a value 0 and there's also a global
value > 0.

Eeli Kaikkonen

2018-04-27 23:15 GMT+03:00 Rene Pöschl <poeschlr@xxxxxxxxx>:

> Forwarded as i accidentally pressed on "Answer" instead of "Answer mailing
> list":
>
> How would you then design a footprint where you need the paste not to be
> centered on the copper area (0201 resistors need this.)?
> How would you design a footprint for a part including an exposed pad?
> There the paste needs to be split up. (And yes we know our 65% paste
> coverage rule will not be right for everyone but it should be ok for
> most users.)
>
> How would you design a footprint for a part with a large "exposed" pad
> for thermal reasons that has a reduced are where the copper is actually
> exposed. (such footprints typically require a different mask clearance
> in x and y direction.)
>
> How would you design a part where the copper pad should be a circle but
> the paste pad a square? (It seems BGA footprints should be made that way
> as it results in better paste stencil separation behavior)
>
> How would you define mask defined pads for example for a BGA? (if 0 is
> not a good idea for a clearance setting why should any other number be ok?)
>
>
>
>
> On 27/04/18 21:36, Wayne Stambaugh wrote:
>
>> The smallest unit in board file geometry is 1nm.  However, all
>> tolerances are really determined by the capabilities of the board
>> manufacturer.  I think setting all the default pad and footprint
>> tolerances to zero and using the user's global settings is the proper
>> way to go.  The problem I see with setting the tolerance on these paste
>> and/or mask pads is the user may not notice that the tolerances are too
>> small for the board manufacturer.  The best case scenario is the boards
>> will be rejected by the manufacturer's DRC or in the worst case the
>> boards will not reflect what the user had intended and possibly fail.
>>
>> On 04/27/2018 03:16 PM, Rene Pöschl wrote:
>>
>>> We (the librarians) discovered that our workflow (or is it a workaround
>>> for missing features) of defining special paste or mask areas does not
>>> work as intended.
>>>
>>> We use paste or mask only pads (no copper, only past or mask selected,
>>> no pin number assigned) to specify mask/paste areas if we can not use
>>> the normal way of defining them. (example a large exposed pad needs
>>> split up paste areas.) These pads naturally have a clearance setting of
>>> 0 which tells kicad that the project settings should be applied. (We did
>>> not think about that.)
>>>
>>> To avoid this i assume we will need to set a small clearance in such
>>> pads as a workaround. What is the smallest value possible that can be
>>> used?
>>>
>>>
>>> ---
>>>
>>>
>>> And a strange observation i made regarding polygon pads. One can not set
>>> a negative soldermask clearance on the pad level. (soldermask defined
>>> pad) But a negative clearance on the footprint level is possible. (and
>>> results in the expected mask area reduction.)
>>>
>>>
>>> _______________________________________________
>>> 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
>>>
>> _______________________________________________
>> 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
>>
>
>
>
> _______________________________________________
> 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
>