Andrzej-
I would prefer that this be fixed when reading the malformed file, not
displaying. We fix it there, the display issue goes away. This also
protects from unintended side effects rather than trying to code work
arounds for a malformed board in multiple parts of the code.
-S
Am Sa., 23. Juni 2018 um 13:18 Uhr schrieb Andrzej Wolski
<awolski.kicad@xxxxxxxxx <mailto:awolski.kicad@xxxxxxxxx>>:
When you generate gerbers from a valid NPTH pad with hole size = pad
size, there will be no shape plotted on copper layers, so in my
opinion,
this pad does not exist on copper layers. But this is more
philosophical
discussion :)
Regarding clearance for router, you could just take the merged shape of
both pad and hole. This would solve problems you mentioned, and perhaps
some other edge cases.
This is just my opinion, I'm not proposing to change anything in kicad
(at least not in the near future).
So if you agree to GAL fix, can this patch be merged?
Cheers,
Andrzej
W dniu 2018-06-23 o 08:54, jp charras pisze:
> Le 22/06/2018 à 21:54, Andrzej Wolski a écrit :
>> No, this IS an error in the board :)
>> If you open pad properties and click OK, it won't let you save
it as is, you will have to enable
>> copper layers.
>> NPTH pads also HAVE TO exists on copper layers (I don't
understand why, but they do).
> Just because they *are* on these copper layers, regardless the
hole has removed the visible copper area.
>
> A pad is not only a copper area. It also define a clearance area,
that is not necessary the hole area.
> If you say: this pad is not on this copper layer, it means you
have no obstacle to draw a track.
> This is obviously false: the hole in on this layer.
>
> If a NPTH is removed from copper layers (malformed pad), the PnS
router will happily route a track
> crossing the hole, because it is the mathematical result of "this
pad is not here".
> You can think: there is a bug in PnS router.
> But the Truth is the pad is broken and has incorrect layer
setting, therefore incorrect routing
> constraints (and incorrect fill zone param).
>
> Therefore regardless the GAL fix, the malformed pad (like any
malformed item) need a fix when
> reading the file, because it this king of issue can create
problems, even crashes.
>
> Of course, the GAL draw issue needs also to be fixed: it must
show the hole, even for malformed pads.
>
>> Also, as I already mentioned, current GAL behavior is different
from 4.0 GAL and legacy, so this is
>> a regression.
>>
>> Andrzej
>>
>> W dniu 2018-06-22 o 21:44, Seth Hillbrand pisze:
>>> Ah. This is not an error in the board. This is just an NPTH.
If you click on it in GAL, you
>>> will see it.
>>>
>>> I think the correct patch to this should check the pad type
instead of drawing one with no layers.
>>>
>>> -S
>>>
>>> Am Fr., 22. Juni 2018 um 12:33 Uhr schrieb Andrzej Wolski
<awolski.kicad@xxxxxxxxx <mailto:awolski.kicad@xxxxxxxxx>
>>> <mailto:awolski.kicad@xxxxxxxxx <mailto:awolski.kicad@xxxxxxxxx>>>:
>>>
>>> IIRC you have to leave (layers) to reproduce this.
>>>
>>> This is a board where I found the issue:
>>>
https://github.com/mntmn/reform/blob/master/electronics/reform-motherboard.kicad_pcb
>>> There are two mPCIE connectors in the center, they have
NPTH alignment holes, you can see them
>>> in legacy mode.
>>>
>>> Andrzej
>>>
>>> W dniu 2018-06-22 o 20:06, Seth Hillbrand pisze:
>>>> Andrzej-
>>>>
>>>> I just tested this, editing a file to remove the layers
from a pad and KiCad automatically
>>>> adds the pad back to all copper layers. I see the pad in
pcbnew and can edit it.
>>>>
>>>> Can you provide a board that demonstrates the issue?
Maybe it was only the test board I used?
>>>>
>>>> -S
>>>>
>>>> Am Fr., 22. Juni 2018 um 10:51 Uhr schrieb Andrzej Wolski
<awolski.kicad@xxxxxxxxx <mailto:awolski.kicad@xxxxxxxxx>
>>>> <mailto:awolski.kicad@xxxxxxxxx
<mailto:awolski.kicad@xxxxxxxxx>>>:
>>>>
>>>> Hi Seth,
>>>>
>>>> current behavior is that malformed pad holes are
always hidden, so you can't see on the
>>>> screen something that exists on your PCB and will be
plotted in drill files. This patch
>>>> makes those holes visible.
>>>>
>>>> Andrzej
>>>>
>>>> W dniu 2018-06-22 o 17:46, Seth Hillbrand pisze:
>>>>> Andrzej-
>>>>>
>>>>> Can you explain the issue that this patch
addresses? I read the commit message but it
>>>>> looks like malformed pads (GetLayerSet().any() == 0)
are no longer hidden. This seems
>>>>> counter-intuitive but maybe I'm just not seeing the
problem.
>>>>>
>>>>> Thanks!
>>>>> Seth
_______________________________________________
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
