kicad-developers team mailing list archive

[Andy Peters <devel@xxxxxxxxx>]

> On Jul 14, 2018, at 7:30 PM, Seth Hillbrand <seth@xxxxxxxxxxxxx> 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 <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 ...