Hoping this isn’t a difficult want. Sometimes an alligator-clip-friendly hole/pad at the edge of a board would be useful. Of course, just a large hole would “do”, but, human nature being what it is “I want it all”, and was trying to create something along the lines of what is found on the BBC Micro:Bit. Guidance on the best approach would be welcome. I can probably get myself from that to the result I want without too much “click-by-click” hand-holding.
A circular PTH pad with some extra rectangular pads that you then place at the edge of your board.
z_BBC-BIT.kicad_mod (1023 Bytes)
The expensive bit is the edge plating with some hard-gold to make it durable.
I think @Joan_Sparky has the right approach for what you are asking. If you want stranger shapes I would recommend svg2mod. I used it to create this thing:
I can’t tell from the photo whether the text numerals on each pad are done in silkscreen, or etched in the pad’s copper.
The KiCAD DRC will allow silkscreen to overlay exposed copper; many other layout programs do NOT permit that. And, many fab houses will either put the job on “Hold” when they detect silkscreen on a pad, or else remove the silkscreen from the pad (perhaps without notifying you that they did so).
I don’t know whether KiCAD will permit numerals etched into the copper pads or not, much less how to do it.
Dale
Looks as it’s in the copper (or better there is no copper where the numbers/letters are):
And you’re right, to recreate those numbers/letters as well will be a little more complicated and @kasbah s suggestion the best way forward.
One thing to watch out for when doing this sort of thing with inkscape and svg2mod is that you have to convert everything to separate enclosed paths. Because of this there is an extra step when doing a shape like the zero. The attached files were done by:
Creating a square, converting that to a path.
Making a text object with “0”, converting that to a path, then un-grouping the result.
Subtracting the paths from each other. You are then left with one path that includes the hole of the zero, svg2mod won’t be able to cope with that and will leave out the hole.
You have to break the that path apart which will give you this:
You then have to subtract the outer two paths from each other to which will leave you with two distinct paths
I then converted this with svg2mod.py -i zero.svg -o zero.kicad_mod --format pretty -p 0.1
zero.svg
zero.kicad_mod (55.8 KB)
And you must do this for each individual character? I sincerely thank you for posting these detailed instructions, but it seems like a lot of work, and 3 programs (including KiCAD), to do what seems like a rather straight-forward task.
Dale
Well, it’s not exactly a standard thing to do. The 3 programs pretty much allow you to turn arbitrary shapes into PCBs so it’s pretty powerful. I am not saying it’s straight-forward.
For the task at hand, you can do it in KiCad alone currently if you just want the pad like @Joan_Sparky describes and you can add text to copper layers. But I don’t think there is a way to have negative text i.e. cut out of copper like what I did above.
The negative text is the impressive thing, and looks sexy on a finished board when it’s done well. I can perhaps justify the effort if the production run will go to thousands or tens of thousands, or if the board will spend much of its life “on display” on the desk or workbench. But many of us in the KiCAD world are doing prototypes, product feasibility demos, or small firms with production runs of a few hundred units. (If we were doing high-volume, long-run products we would be working for big companies that have spent big bucks on the big programs which integrate board layout with configuration control, MRP, etc.)
Is it practical to create a footprint library containing a pre-made, negative character, footprint for each character in a standard alphabet? (In the English-speaking Western world that’s around 50-ish footprints: 26 letters, 10 numerals, and a dozen punctuation or special symbols.) The character footprints can then be dropped onto a board similar to how we put mounting-hole footprints onto a board as needed.
We would have to agree on a usable size for the characters - perhaps 50 -100 mils (1.5 - 2.5 mm) high. This choice is constrained by the minimum copper width that can be routinely rendered by a typical board fab house (currently about 6 mils (0.15 mm)). And of course, it must be easy to embed the character footprints into a copper pour region so you get the desired effect of the negative characters!
Dale
