kicad-developers team mailing list archive

[Seth Hillbrand <seth@xxxxxxxxxxxxx>]

That's valid.  Would you mind submitting the issue to our bug tracker and
we'll fix that in 5.0.1?  I have a fix for the non-copper connectivity
issue queued but we should address the array pad numbering issue as well.
If memory serves, there are a few issues with that dialog outstanding...

-S

Am Sa., 14. Juli 2018 um 18:26 Uhr schrieb Andy Peters <devel@xxxxxxxxx>:

>
> > On Jul 14, 2018, at 3:33 PM, Seth Hillbrand <seth@xxxxxxxxxxxxx> wrote:
> >
> > Hi Andy-
> >
> > You don't provide enough information to help you here.  You'll need to
> show a larger image of your board with other layers enabled and, ideally
> set with some transparency so that we can see what's happening.
> >
> > Connectivity _only_ applies to copper.  So the paste-only pads shouldn't
> have any connections unless you also made them copper.  Did you follow
> Rene's instructions on the user forum?
>
> "Connectivity _only_ applies to copper.” Yes, that’s true, and that’s what
> baffled me. These pads were explicitly set to Layer Copper as None, only
> the F.Paste layer was checked.
>
> I did follow Rene’s instructions, except for one point. I created one of
> the paste-mask-only pads, made sure it had no pad number and no net name,
> placed it, and then used the array feature to create the needed 3x3 array.
> His recommendation is to just duplicate pads.
>
> And that’s what broke it. It assigned pad numbers to all of the pads. The
> pad numbers assigned are like such:
>
> +__+__+__+
> |33|23|13|
> +__+__+__+
> |32|22|12|
> +__+__+__+
> |31|21|11|
> +__+__+__+
>
> and the pads inherited the net name associated with the pad number, since
> those pad numbers were already on the footprint.
>
> When no copper layer is indicated in the pad, then the pad number vanishes
> from the display. After creating the array, I didn’t see any pad numbers,
> so I thought that all was well, and did not look at each of the pads to see
> that, yes, indeed, they _were_ assigned pad numbers, and as such inherited
> the pad’s net name.
>
> I can see why the array function would create pad numbers for footprint
> pins which have a copper layer. It surprised me that it created them for
> these aperture pads, especially since the pad from which the array was
> created had no number. Rene does say that "Using the array function is not
> really possible in this case as it does not allow us to assign no pad
> number to the resulting pads,” but I didn’t appreciate what that actually
> meant.
>
> The DRC wants the user to connect a trace to a non-existent copper part of
> a pad, and that’s not right.
>
> Could the array function be modified such that if the original pad has no
> number, then it should not assign pad numbers to the cloned pads?
>
> -a
>
>
> > -S
> >
> > Am Sa., 14. Juli 2018 um 14:00 Uhr schrieb <devel@xxxxxxxxx>:
> > I'm on yesterday's unified package of 5.0.0 rc3 on a mac.
> >
> > Following my question about why the footprint editor wouldn't let me
> create an arbitrary shape for a solder-paste-mask pad, which was not
> actually answered but the workaround was actually what I wanted (and I
> figured out what I was doing wrong, the pad shape has to be set to Custom),
> I went and edited my footprint in place to add the paste-mask-only pads (no
> copper layer). They're called aperture pads, I believe, and the footprint
> looks as shown in QFN-paste.png.
> >
> > Then I save it back to the layout, and I get a few connection errors, on
> a board which was fully routed. The connection errors refer to traces which
> now want to connect to those new aperture pads. I don't know why this
> should happen, and I don't know how to fix it! It seems like the
> connectivity is borked. I know about the change in the clearances (from
> http://kicad-pcb.org/blog/2018/05/Mask-Clearance-Generation-Changes/) but
> that doesn't seem to apply here, as it's a connectivity issue. This is
> shown in QFN-DRC-fail.png.
> >
> > I'm willing to believe that I did something wrong, but what!
> >
> > Thanks ...
> >
> >
>
>
> _______________________________________________
> 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
>