Wishlist: Gerber export: Use RectRounded aperture shape for rounded rectangle pads

[Artsiom Shchatsko]

As KiCad supports rounded rectangle pads now it would be a cleaner implementation if the "RectRounded" aperture shape was used for such pads when generating Gerber data. Currently a polygon with multiple points is used.

[Novak Tamas (novak-7)]

Confirmed. "O" oval/obround is used, but "Q" for founded rectangle is not.
Anyway it goes to wishlist, as generated gerber is fine...only may be smaller is Q aperture was used.

[jean-pierre charras (jp-charras)]

AFAIK, rounded rect aperture does no exist (I never see a Q aperture).
Rounded rect shapes need to define one aperture macro, which is different, and one aperture by size and orientation, with a poor benefit, because Pcbnew generates also solder mask and paste.

[Novak Tamas (novak-7)]

You are right, Jean-Pierre. In latest https://www.ucamco.com/files/downloads/file/81/the_gerber_file_format_specification.pdf there are only "Standard apertures are pre-defined: the circle (C), rectangle (R), obround (O) and regular polygon (P)"
In my gerber viewer/editing tool there is a Q rounded rectangle aperture, but it is not standard, so rather not to use it.

On the other hand I've seen "home rules" to make all SMD resistor pads rectangles, and all SMD capacitors with rounded rectangle pads (it was just fashion, or to make them visually distinguishable?). In that case gerber size could be huge if all pads are defined as many-segment-poligons. Maybe it would worth using aperture macros or arcs.
I don't know if to set to Invalid or to leave as Wishlist.

[jean-pierre charras (jp-charras)]

Leave it as Wishlist.
In Gerber files, the best practice is using flashes for pads.

[Artsiom Shchatsko (cioma)]

I concur with Jean-Pierre: let's leave it as Wishlist.

I also got confused by my CAM tool (FAB 3000) as it supports aperture named "RectRounded". Now I actually tried it and when I checked the Gerber text it was defined as macro (as expected per Gerber format specification).

Indeed using flashes for pads is a cleaner approach as it represents the same entity but in a simpler way. That might be a more robust approach as some CAM tools might have some corner cases when handling thousands of pads defined as polygons. It also might take (much?) longer to do DFM checks.

[Fredrik Atmer (fredrikatmer)]

I used to define my own rounded rectangle pads from rectangular pads and a polygon to get the rounded outline. I must admit it is much handier and cleaner to define a roundrect pad with a single row in a kicad_mod file.

I.e. compare
  (pad 1 smd roundrect (at -0.6800 0.0000) (size 0.6000 0.9600) (layers F.Cu F.Mask F.Paste) (roundrect_rratio 0.20) (solder_mask_margin 0.1) (solder_paste_margin 0.1))

to
  (pad 5 smd rect (at 4.325 -1.30) (size 1.65 0.3) (layers F.Cu))
  (fp_poly (pts (xy 3.50 -1.15) (xy 5.15 -1.15) (xy 5.15 -1.45) (xy 3.50 -1.45)) (layer F.Cu) (width 0.1))
  (fp_poly (pts (xy 3.50 -1.15) (xy 5.15 -1.15) (xy 5.15 -1.45) (xy 3.50 -1.45)) (layer F.Mask) (width 0.1))
  (fp_poly (pts (xy 3.50 -1.15) (xy 5.15 -1.15) (xy 5.15 -1.45) (xy 3.50 -1.45)) (layer F.Paste) (width 0.1))

When exporting to gerbers I think it would be cleaner to use the rectangle + outline segments approach (sort of like how filled polygons are handled) rather than the way the roundrects are "polygonized" today.

[KiCad Janitor (kicad-janitor)]

KiCad bug tracker has moved to Gitlab. This report is now available here: https://gitlab.com/kicad/code/kicad/-/issues/2020