> On Jul 14, 2018, at 7:30 PM, Seth Hillbrand <s...@hillbrand.org> wrote: > > 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
Bug report with overly-verbose description is filed at https://bugs.launchpad.net/kicad/+bug/1781760 Thanks! FWIW, for this I just wanted to generate a Gerber file for the paste mask layer so I could get a correct stencil made. The board was fabbed and I had stencils made, and the stencil had just the one big hole for the exposed pad (not good). That’s why I edited the footprint in place. If the board needs a respin, I’ll use an updated footprint from my library. -a > Am Sa., 14. Juli 2018 um 18:26 Uhr schrieb Andy Peters <de...@latke.net>: > > > On Jul 14, 2018, at 3:33 PM, Seth Hillbrand <s...@hillbrand.org> 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 <de...@latke.net>: > > 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@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
