kicad-developers team mailing list archive
Mailing list archive
Re: Kicad libraries for pcbnew
Sun, 11 Oct 2009 10:44:32 -0000
--- In kicad-devel@xxxxxxxxxxxxxxx, Vesa Solonen <vsolonen@...> wrote:
> On Thu, 8 Oct 2009, viking632 wrote:
> > I've been working on some pcbnew (physical package) libraries for kicad.
> I took a brief look at them and they are fine and very needed addition.
> Solder mask cutouts that overlap need some consideration I think. Should
> they be cut open in one piece to avoid manufacturing warnings? I don't
> certainly know what's the practice, but this just came to my mind.
> IMO the scripted method for making the land patterns is very much
> preferred to anyting else. Please keep up the good work.
The size of the soldermask (and the pastemask ?) seems to be hardcoded to be 6mils larger than the pad on all sides, and there is no way of specifyingthe masksize(s) in the component libs.
As you noticed, this causes overlapping masks on closely spaced components like QFP:
QFP packages with 0.5mm pitch have pins that are 0.22mm wide,
with 0.254mm wide pads on the recommended land pattern.
This, with the 6mil masks, causes an overlap of 0.059mm (2.32mils).
QFPs with 0.4mm pitch have 0.18mm wide pins, with 0.203mm recommended pad width, causing an even larger overlap of 0.108mm (4.25mils).
There are only two ways of changing this in kicad: Either lower the built-in default from 6mils to 3mils (4mils is too large), or enhance the pcbnew component libraries with two extra values: The masksize (relative to the padsize) in X and Y.
When doing a PCB Design Rules Check on my *QFP sample board, it doesn't complain about the overlapping masks, so are overlapping masks really a problem, or can they be ignored ?
I've searched the web for info on this, and the recommendation seems to be,that in general, pins should be NSMD (Non-Solder Mask Defined), i.e. have a soldermask that is 60-75um (2.4-3mils) _larger_ than the pad on all sides.
This seems to indicate, that the 6mil value in kicad should be lowered to 3mils, or has the 6mils been chosen to allow larger misalignment of the soldermask (for hobby production of PCBs) ?
Exposed thermal pads that are close to other pads should be SMD (Solder Mask Defined), with a mask that is 100um (4mils) _smaller_ than the pad, to reduce the risk of bridging when soldering.
Pads that are very close (or even "too close" together, as the QFP examplesabove), should use one big opening, as the soldermask alignment accuracy won't allow accurate enough placement, and the thin lines of the mask won't help much in prevent bridging anyway.
Overlapping masks will of course give this desired box opening result.
Pads that are a little farter apart could also benefit from a box opening as well, but achieving that would require a library change: The addition of masksize to the Pad definition.
Quidquid latine dictum sit, altum viditur.