I wonder what you would do when tackling this footprint suggestion.
It’s the land pattern example for Texas Instruments’ LM708x0 chip, a 29 pin VQFN.
In particular there is exposed copper that connects multiple pads, roughly polygon shaped but with some filleted corners.
I opted to draw a standard QFN pad pattern, and add a polygon to the F.Cu and F.Mask layers, like so (Mask and Cu layers are the same):
However I wasn’t able to capture the filleted corners. The “Shape Modification → Fillet Lines” command works nicely, but produces an outline rather than a filled shape. And the inner fillets in particular are hard to replicate with standard fill and line tools.
I think it probably doesn’t matter, but I wonder if I’ve missed an option here?
I did a short experiment in KiCad V8 with the footprint editor.
- Draw a graphical polygon.
- Right click, Shape Modification / Fillet Lines.
- Right click, Create from Selection / Create Polygon from Selection.
And this seems to work, although the fillets are not real arcs, but made up out of line segments.
But for the rest, I probably would not have bothered to do this, and at most draw chamfers in the polygon. There is no need to exactly follow the contours of the exposed metal. With small pads, there is a benefit with rounded corners (more accurate stencil manufacturing, and more reliable solder paste release). But for such big pads, these effects are much smaller.
2 Likes
Oh wow, yep, step 3 does the trick (in v9)! Thanks.
Yes, it’s hard to imagine any starvation effect given the total area. And I’ve opted for more traditional rounded rects for the paste layer.
But the less departure from recommendations, the less nervous I feel. So this is good to know!
For those playing along at home, don’t forget to also do the cmd/ctrl-e, cmd/ctrl-e trick to join the polygon to one of the pads!
That is, after steps 1, 2 and 3 in @paulvdh 's fine suggestion, select one of the pads the polygon overlaps. Then hit ctrl-e (cmd-e on Mac) to enter “Edit custom pad” mode, and hit it again to exit. The polygon will magically become part of the pad you selected.
This is required so you can route to it, otherwise the polygon would be considered copper to stay clear of.
I suspect if you haven’t joined all the other pads in your schematic you’ll also get a DRC error. But provided they’re all the same net, you’ll be able to route and fill as expected:
2 Likes
@Heath_Raftery Please don’t ping people (by placing an @ in front of their name) unless you have a good reason for wanting to draw their attention. This forum software also sends alerts to those people when you do so, and there is no need to do so in this (and in most other) cases.
