Seeed Studio has issued a new Seeed Design for Manufacturing Manual. For their pick-and-place machines, they require some new, very specific fiducial marks. See section 11.2.1:
It’s a 1mm copper circle surrounded by a 2mm hole in the solder mask. That, in turn, is surrounded by a copper octagon. They say “covering copper”, but I think they mean “covered copper”, under the solder mask.
I’ve tried making this in the footprint editor. Each octagon face is a trapezoidal SMD pad, and the octagon is a circular array of such pads. The problem is that that they’re pads to KiCAD. Even if I blank out the pad number, they’re treated as real pads - the solder mask doesn’t cover them, and design rule check complains that the pads are touching each other, which they are… Is there some way to tell KiCAD that this is non-functional copper? Thanks.
Here’s the result in Kicad’s 3D View. Seeed apparently wanted a target that couldn’t be mistaken for anything else. I’ll put this and the other Seeed markers on Github soon. They could be added to the standard Fiducials library.
I guess SEEED can request whatever they like, but i thought fiducials were somewhat “standardised”:
Round bare copper area, radius R, Solder Mask clearance (round), radius 2R or 3R regardess if they are local or global.
Just curious, do other fabs have requirements like this?
IPC suggests the same fiducial size/shape for panel, global and local fiducials. Seeed Studio’s suggested panel fiducial would still seem to be compatible with the IPC fiducial.
I think that’s what they had in mind with the octagon under the solder mask. It looks like a standard fiducial, but the octagon gives them something unambiguous to look for.
Might want to hold off on using those. Seeed’s DFM manual is ambiguous on whether the copper octagon is covered with solder mask. Their text reads
“Covering copper: an octagonal copper ring”.
“Covering” is confusing here. “Covered” or “Uncovered” would not be ambiguous. It’s not clear whether they want solder mask over the octagon or not. I sent Seeed support a message, and I’ll fix the footprints if they say the copper should be uncovered.
That’s a good alignment target. Nothing else usually seen on a PC board looks like that.
The octagon and dot are bare copper, no solder paste. 1mm copper dot, 2mm solder mask hole, 3mm octagon.
I also added footprints for Seeed’s local fiducial - 1mm copper dot, 2mm solder mask hole. They require those for some fine-pitched parts where the pick and place machine has to precision align. The ones in the KiCAD library have a 2.54mm solder mask hole.
Aren’t you worried about soldermask vs copper alignment errors for the octagon?
The center copper dot has got the 1mm clearance fro a reason I think… the octagon doesn’t have that and could become partly covered with soldermask.
Good point, usually the inner clearance is ‘quite generous’ to ensure the optics do grab the copper and not the soldermask.
The outer polygon is likely used to allow auto-find type smarts to work, (and less for final precise alignment), but it’s probably also a good idea to have a mask-excess on that outer outline too.
Would not need to be 1mm, just enough to tolerate usual mask alignments.
