If you copy your other pad and then change to npth then the pad number is still there. At least it was this way last time i manually made a footprint. (might have been as long ago as late nightlies before v5 came out.)
I really didn’t take this too far. After the OP raised the question I wanted to see what could be done with the default editor. One pad on each layer and the NPTH to get the drill hole. That made it a ‘footprint’ without having to get the drill strike from another procedure. I then dropped it onto an existing board to see if the DRC would complain. Other than the footprint wasn’t connected to anything else the DRC didn’t seem to mind. I know home board makers have trouble tearing up copper when doing something like this and that would be my only concern if using a cheap board house. Not something I’ve needed to think about in my limited experience though.
I think the best option with kicad, to be DRC compliant, would be a geometry with an annular pad…
op600-fp-v5.kicad_mod (3.0 KB)
and here the FreeCAD fp (done with StepUp) & 3d model
op600-fp-v5.FCStd (124.2 KB)
2 Likes
This looks pretty good, but I’m not sure how a manufacturer would interpret the copper which touches the edge of the hole (in this case it seems to overlap a bit).
In any case copper near a NPTH may be problematic. The manufacturer could without asking remove some copper up to their NPTH/copper clearance value if they have one. If it’s for example 0.2mm you have to bridge it with solder in the bottom side. The top side shouldn’t be a problem because there are pins.
If there’s no clearance and they just drill through copper you have to be careful that there’s no copper chips left in the hole.
1 Like
If you open the fp I posted, you can see that there is not copper touching the edge of the hole.
You probably have just looked at the pictures and not went through the real kicad fp.
It is also possible to reduce the annular crown, to give the pad a NPTH clearance, in case is needed by the manufacturer.
1 Like
I did go through it, and it looks like it overlaps.
Green is back copper, light brownish is the hole, bright green is the overlapping part.
You are right, when I replaced the first pad, I simply calculate the crown to reach the drill.
The margin is instead present on top pads.
I don’t think this is an issue for the manufacturer, but as I said, it is possible to edit the crown to give the pad a NPTH clearance, in case is needed.
I would do some careful analysis when using this design approach, and co-ordinate my design with the supplier’s capabilities. Board fabricators seem to have a list of preferred hole sizes, and a process for mapping hole sizes from the design drawings into the bit sizes available on their machines. For example, the footprint design may be beautifully crafted based on a 1.7mm hole size, but the board fabricator is likely to create the hole with, say, a 1.5mm or 1.8mm drill. (He may not advise you beforehand because the difference falls within his published tolerances for NPTH hole sizes.) And that is BEFORE factoring in allowances for tool wear, and positional accuracy of the hole’s center point. When you populate a board with typical through-hole components the tolerance requirements are simply not as tight as what this footprint seems to require.
Dale
Wow I didn’t think my little fun component will interest so many people!
It’s sure that it has to be discuss with the PCB vendor, but I think can live with some of the last footprint posted
Thanks
Well, that should be the default behavior along with the supplier doing a revue and giving feedback. Also a good reason to do a trail run before committing to thousands of boards.
Engineering is about puzzle solving and this one was a bit different and interested people. Now you won’t have to try and do a half drill out on you PTH. 
It is a package I don’t recall ever encountering. I have a current application where its mechanical design would actually be quite useful, except that the devices available in that package (as well as a long list of discontinued devices using that package) don’t have the electrical characteristics I need.
Dale
Just to be clear, when I said that I don’t think this could be an issue, that didn’t mean that before producing a board with new footprints, one can forget to check the manufacturer for possible issues…
I know that some cheap factory sets a pad as PTH if the drill touches the pad itself, instead of getting the info from the drill files. At the same time other manufacturers will set a pad without copper on both sides as unplated.
Anyway I posted the fp and the source file for the fp in FC, so the OP can easily change the fp in case of need.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.