Hi 
I use kicad every day
But I need to create circular PCB with this footprint :
Now, I don’t know exactly the size (a circle around 70mm).
I hope it’s possible with kicad
Do you have an idea to create “circular extern/reverse hole” (by portion) ?
Thank you a lot for your help
I guess you want to create a board outline, not a footprint. I also guess you want a board outline matching the dark/gray portion of the image? I would not call that circular. Clearly, at some point you will need to know the size…
Anyway, you can draw any shape you want using KiCad. You might find it easier to create a DXF outside of KiCad and import it. Personally, I would write a script.
Edit : I wonder if you have the design already in a CAD package, you can export a DXF from there? Anyway, I wrote an OpenSCAD script:
$fs=1;
$fn=0;
$fa=0.01;
r1 = 65; // inner radius
r2 = 70; // outer radius
num_teeth = 18;
da=360/num_teeth/2;
module wedge(r,ang)
{
difference ()
{
circle (r/2);
translate ([-r,-r,0]) square([r*2,r]);
translate ([-r*2,0,0]) square([r*2,r]);
rotate ([0,0,-90+ang+0.1]) translate ([-r*2,0,0]) square([r*2,r*2]);
}
}
for (ang=[0:da*2:360])
{
rotate ([0,0,ang]) wedge (r2, da);
rotate ([0,0,ang-da]) wedge (r1, da);
}
Do you want copper on the edge? Not all fabs can do it the way you showed. Most fabs need a plated through hole at the edge that will get partly milled away. These are called Castellations.
My impression is that the white areas are the pads/footprint on the PCB. Do they have to wrap around or be exposed on the sides? Are they solid? I think we need more information.
Especially - what’s the aim.
Many ways lead to Rome and maybe we get a better idea HOW we and KiCAD can achieve the desired outcome, by knowing what it goes into…
Ah, that might make more sense! Creating a a pad in the shape of an arc segment is possible, a little tricky. Again I would script it. When we get support for arbitrary shaped pads it will be easy.
Plating the edge is a manufacturer option, I guess that would be specified by notes on the drawing. A compromise might be a series of through holes around the edge which will be milled, similar to current castellation technique.
Sorry. So this is more informations :
I have solidworkd to create DXF. I used this software to create the form of the pcb
I want to create a circular PCB around 70mm of diam.
But before to create this I would like to know how to create my footprint.
Each white part on my circle is in gold effect and represent the footprint also on the EDGE (yes for the copper)
I would like to create capacitive touch on each footprint and I need to keep a circule PCB.
I don’t know the best way to create this. But know I don’t know how to create this forme on the footprint editor.
In the end we will see only the edge. (The pcb will be sandwiched by two blocks of marble.
The user could slide the finger only on the edge of the PCB to activate features of the product.
So, I would like to keep a smooth appearance and no a series of through holes
Talk with the fabricator… example from Eurocircuits on their website:
To manufacture a board with round-edge plating we rout the board profile where the edge plating is required before the through-hole plating process. This involves extra process steps so round-edge plating is a cost option.
From here: http://www.eurocircuits.com/blog/copper-and-the-board-edge/
They will tell you how you need to communicate this and then you can decide (or ask us) how to get the layout/footprint/gerbers into a state to make this work.
I asked my PCB factory about this. And this is not a problem.
This is a 3D picture of an exemple of the final result :
I think the footprint need to be like a through hole (for the gerber document)
Thats something you need to ask your fab. They know how they want it communicated. (Through hole would be wrong. You do not need something in the drill file for this.)
Ok, I think that is simpler, if you place pads overlapping the edge in KiCad, they will be chopped to the board edge by the manufacturer. KiCad does not display the final effect correctly in the 3D view, but that does not matter.
I would use a through-hole pad, then copper appears both sides, and you get a hole, but you can always create a pad as a combination of SMD, connector, through hole as required.
If you put instructions on a drawing layer, eg. ECO1, you can instruct the manufacturer which areas need edge plating.
As an aside, if the board is sandwiched in marble, are there components on the board?
As @bobc writes, SMD pads (top/bottom) over the edge. Then telling the boardhouse those should be edge plated. They should be able to take it from there.
If you got no other copper ares than those going over the outline, they should know what to do, if you told them that those are edge plated (and yeah, putting this info also on an extra layer should help).
My approach would be to place pads on both sides of the board, at the appropriate spacing, like bobc’s depiction, and then place arc shaped slots in the pads, with the slots being 0.8mm wide or greater to allow them to be milled by the fab.
In effect, you would be using multiples copies of a footprint with a slot, with slot being an arc rather than a straight line.
The arcs defining these slots would typically go in the outline layer for the fab I deal with. The gerber file for plated through holes may need to have these slots in it too, depending on your fab.
The inner radius of the arc defined slots would need to be slightly under your final marble circumference, to allow for the plating thickness.
This would allow you to sandwich the final board between the marble pieces, and turn/grind/polish the non plated FR4 intervals between pads down to the level of the marble surface, without affecting the plating in the slots.
You may prefer to leave the plated slots as slight depressions below the level of the marble and/or fill the resulting slots with a conductive epoxy or similar, which could be coloured appropriately.
Simplest of all, if you opt for recessed plated slots for later filling with something like conductive epoxy, would be to use straight slots in your footprint, which kicad should be able to handle with no extra hacking/hand crafting required for the gerber layers.
An interesting challenge.
Regards,
Erich
