it is possible to make a hole like this?
if not are there ways to get arround it?
the octagon is 2,3mm on each side
In KiCad you would probably use Edge.Cut layer and draw it as an inner cutout, unless the manufacturer wants something else.
Whether it can be produced is a different matter. You have to ask the manufacturer. The cheap ones won’t most likely do it. They would route it with a router bit which is so large that the hole wouldn’t be rectangular but (almost) oval.
Yet another matter is whether you actually need that kind of hole. Very often an oval hole is good enough. But it depends on your use case.
1 Like
the hole itself is easy enough, i have that in plate, its the pad arround it i cant figure how to make
Then why first post:
There are a few different ways to make an octagonal pad, although your pad does not look octagonal at all, but a solid zone with just an octagonal cutout in the solder mask layer.
In KiCad it is very common to make complicated pads out of overlapping pads. Have a look for example at the Footprints for IC’s with thermal pads under them. When doing it this way, you can use a rectangular SMD pad for the center part and 2 trapezoidal pads for the top and bottom.
Or 4 rectangular pads on the same location, but rotated 45 degrees each time.
A more involved way is to draw our shape into an external application, import it in kicad as a dxf (or .svg) and make a custom pad out of it.e
You can also do it directly with the “Custom Shape Primitives” although the procedure is not very user friendly. It sort of works like:
- Open Footprint editor, create new footprint (in a library)
- Place / Place Pad, and place a random pad on the canvas.
- Hover the mouse cursor over the pad and press e for edit.
- Set the “Pad Type” to SMD, and “Shape” to: “Custom( Rect. Anchor)”
- On the Tab: “Custom Shape Primitives” -> Add Primitivy -> Polygon.
*Click on the + a few times until you have 8 corners.
Then enter coordinates something like:
1 Like
i tried that but could not quite figure out what size the retangular pad should have to end up with 8 sides that all are 2,3mm
figured it
2,3x5.553 mm
FWIW.
My experience is from ordering at JLCPCB’s. (No, I don’t work for JLCPCB nor do I receive benefits 
). But then, it’s not much different with other boardhouses when it comes to (cheap) prototype boards.
A perfectly square hole extactly like you want it cannot be produced. Such “holes” in effect are slots (drawn on edge.cuts) which are routed out. So you always have the radius of the routing tool. The minimum slot width is 0.5mm for plated and 0.8mm for unplated slots at JLCPCB’s. Or, the other way round, corners will always have a radius of 0.25mm plated or 0.4mm unplated.
This said, they will do it, even for their $2 boards, no questions asked.
Except for that the example shown is pretty much rectangular with sharp corners.
One way of producing these is by punching instead of milling, but that is a procees that’s mostly suited to mass production, as the tooling is expensive.
It’s one of the reasons FR-2 board can be mass produced cheap. It’s not just the cost of the base material, but the holes in these tend to be punched with a punch that does all the holes for a PCB in a single operation.
Having a look at: https://en.wikipedia.org/wiki/FR-2
suggest that the boards may be heated before punching to soften them up a bit, which makes much sense. Less hard and brittle FR-2 would mean cleaner edges and also less tool wear. This is all speculation though, I have not seen this in production.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.