I’d create footprint for UFQFPN28 package, where 0.55x0.3mm pad are so close at the corners, that the corners of the pad are cut in recommended FP (see attached image).
My best guess is creating pin as 0.4x0.3mm square and a dis-named (pin 1 and 1B) trapozoid supplement 0.15mm long. Is there any better way for asymmetric pad problems?
As you already discovered complicated pad shapes can be created by overlapping different pins (with the same number.)
So change your pin 1b to pin 1 and it will be handled by drc as a single pin.
There is currently no better way to do something like this.
That’s the best I can come up with (5 pads, 3 rectangles, 2 tapers), the solder mask clearance outline is not the smartest… 0.05 mm pictured. Ideally those solder mask corners should become rounded, as otherwise the sharp corners stick out extremely (the larger the solder mask clearance is set to the worse it gets).
pad-w-edge-missing.kicad_mod (1.2 KB)
Well i can do the same with 3 pads.
The file to play with:
But i don’t like the mask layer either.
It would be nice if one could have more control over the soldermask (especially for trapezoid/triangle pads)
As I said, I was careful to have the sharp edges not produce too large extends on the soldermask layer…
Ideally the soldermask clearance (bottom row, opengl canvas) should look like the pad/track clearance in legacy canvas (top row).
Unfortunately it doesn’t…
How does the soldermask look like in legacy?
(is there something comparable to that in legacy?)
To be honest i looked at your screenshot and wondered why you used so many pads.
Well i have a second idea. remove the soldermask from the trapezoid and create the missing part of the soldermask via a soldermask only (no copper) pad.
my_test_2.kicad_mod (758 Bytes)
optimized for 75um soldermask clearance.
Designed with this freecad document. (maybe help-full for designing this pad with other clearances.)
pad design.fcstd (9.2 KB)
If I remember correctly it doesn’t show, only in the 3D viewer. Back when the 3D viewer stopped using the current pcbnew settings for soldermask clearance (esp in the footprint editor) one could get really scared.
Last one to fall for this was @ArtG…
As for your alternative, yeah, if that works for him.
I guess the pads of the future will get ‘wilder’ and sooner or later someone is p**d off enough to sit down and hack some code together to allow arbitrary pads - just guessing. On the other hand I’m sure the devs are aware of this and it just hasn’t been tackled as the interactions with other code isn’t solved that easily.
Is this thread about Tangram?
LOL, this is so fun…
How to make a square hole (drill) BTW ?
You can’t drill square holes. They need to be routed. This means you simply put a square onto the edge cuts layer.
(By the way this would have been better as a separate question.)
They are aware of it and there is work actually trying to get this into Kicad, but as you say. It has some strange interactions to other code.