kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxx>]

Hey Andrzej,

This makes sense now.  SnapEDA should have already resolved this issue.
They contacted me at the end of April about this problem and I explained
the problem with their NPTH generation.  If they are still producing
footprints with NPTHs that do not have any layers defined, I will ping
them to see what is going on.  I would say this is not an issue with
KiCad (other than maybe our file format documentation) but rather an
issue with SnapEDA's footprint generator.

Cheers,

Wayne

On 6/25/2018 5:19 PM, Andrzej Wolski wrote:
> Hi,
> 
> if by submitter you mean me, then this is a board I found on Github, I
> don't know if it was manually edited.
> 
> But I have done a little investigation, and I think I've found the
> source of this problem.
> The problematic footprint is identical to the one that can be downloaded
> from SnapEDA:
> https://www.snapeda.com/parts/67910-5700/Molex/view-part/
> The footprint is in legacy format and has NPTH holes defined with zero
> layer mask:
> 
> $PAD
> Sh "Hole" C 1.1 1.1 0 0 0
> Dr 1.1 0 0
> At HOLE N 0
> Po 14.3 0
> $EndPAD
> 
> So it looks like SnapEDA has a bug in their export-to-kicad script.
> 
> Maybe someone could inform them about this (I don't know how layer mask
> should look in legacy format).
> 
> Andrzej
> 
> 
> W dniu 2018-06-25 o 20:25, Wayne Stambaugh pisze:
>> Hey Seth,
>>
>> I would agree with you if this was our error.  If I'm reading JP's
>> analysis correctly, he could not create this board error using KiCad so
>> I'm working on the assumption that this was not our board file output
>> formatter causing the problem.  Using defensive measures such as
>> assertions and test cases to ensure our board file output formatter is
>> correct makes sense.  Adding code to our parser to fix board files that
>> are broken due to manual editing or broken scripts is a slippery slope.
>> Where do we draw the line?  This isn't the first time this has happened.
>>   In the past, we have chosen not to allow this so I am leaning in that
>> direction.  It would be nice if the submitter of the broken board would
>> confirm if the board was manually edited with a text editor or
>> manipulated with a script.  I'm not completely dismissing the patch but
>> it would be easier to make an informed decision if I knew how the broken
>> board was created.
>>
>> Cheers,
>>
>> Wayne
>>
>> On 6/25/2018 10:25 AM, Seth Hillbrand wrote:
>>> ​Hi Wayne-
>>>
>>> I would view this patch more as defensive coding than trying to fix
>>> others' errors.  The alternatives are to refuse to parse the file or (as
>>> we currently do) parse as written and encounter errors in display and
>>> routing.  JP's approach provides a clear and predictable response to a
>>> modified file.
>>>
>>> -Seth​
>>>
>>>
>>> Am Mo., 25. Juni 2018 um 06:16 Uhr schrieb Wayne Stambaugh
>>> <stambaughw@xxxxxxxxx <mailto:stambaughw@xxxxxxxxx>>:
>>>
>>>      On 6/25/2018 8:12 AM, jp charras wrote:
>>>      > Le 24/06/2018 à 21:52, Wayne Stambaugh a écrit :
>>>      >> Are we planning on fixing this for rc3?  If so, what is
>>>      required.  I'm fine with waiting a day or
>>>      >> two to tag rc3.
>>>      >>
>>>      >
>>>      > Attached a possible fix.
>>>      >
>>>      > The board test file shows really broken layer set in a few pads:
>>>      > - no layers for some pads (the layers section is empty).
>>>      > This make no sense for me.
>>>      >
>>>      > After tests, It is not possible to create this empty layer set
>>>      from Pcbnew (even with old 2013
>>>      > stable version).
>>>      >
>>>      > My opinion is the board (or the footprints) was modified by hand
>>>      (or by a script).
>>>
>>>      If this is the case, then I'm not thrilled about applying this
>>> patch
>>>      even if it does solve the problem.  We should not be modifying
>>> KiCad to
>>>      fix other people's coding errors.
>>>
>>>      >
>>>      > This patch is short and fixes silently this kind of issues.
>>>      > (I am not sure it is worth to try a better fix, because this
>>> issue
>>>      cannot happens when editing a
>>>      > board from pcbnew)
>>>      >
>>>      >
>>>      >
>>>      > _______________________________________________
>>>      > Mailing list: https://launchpad.net/~kicad-developers
>>>      > Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>      <mailto: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
>>>      <mailto: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